30i/31i/32i A USER'S MANUAL (Common To Lathe System/Machining Center System) FANUC Series 31 User
User Manual: Pdf
Open the PDF directly: View PDF 
.
Page Count: 2458 [warning: Documents this large are best viewed by clicking the View PDF Link!]
- B-63944EN/03
- SAFETY PRECAUTIONS
- TABLE OF CONTENTS
- I. GENERAL
- II. PROGRAMMING
- 1 GENERAL
- 1.1 TOOL MOVEMENT ALONG WORKPIECE PARTS FIGURE-INTERPOLATION
- 1.2 FEED-FEED FUNCTION
- 1.3 PART DRAWING AND TOOL MOVEMENT
- 1.4 CUTTING SPEED - SPINDLE FUNCTION
- 1.5 SELECTION OF TOOL USED FOR VARIOUS MACHINING - TOOL FUNCTION
- 1.6 COMMAND FOR MACHINE OPERATIONS - AUXILIARY FUNCTION
- 1.7 PROGRAM CONFIGURATION
- 1.8 TOOL MOVEMENT RANGE - STROKE
- 2 CONTROLLED AXES
- 3 PREPARATORY FUNCTION (G FUNCTION)
- 4 INTERPOLATION FUNCTIONS
- 4.1 POSITIONING (G00)
- 4.2 SINGLE DIRECTION POSITIONING (G60)
- 4.3 LINEAR INTERPOLATION (G01)
- 4.4 CIRCULAR INTERPOLATION (G02, G03)
- 4.5 HELICAL INTERPOLATION (G02, G03)
- 4.6 HELICAL INTERPOLATION B (G02, G03)
- 4.7 SPIRAL INTERPOLATION, CONICAL INTERPOLATION (G02, G03)
- 4.8 POLAR COORDINATE INTERPOLATION (G12.1, G13.1)
- 4.9 CYLINDRICAL INTERPOLATION (G07.1)
- 4.10 CUTTING POINT INTERPOLATION FOR CYLINDRICAL INTERPOLATION (G07.1)
- 4.11 EXPONENTIAL INTERPOLATION (G02.3, G03.3)
- 4.12 SMOOTH INTERPOLATION (G05.1)
- 4.13 NANO SMOOTHING
- 4.14 NURBS INTERPOLATION (G06.2)
- 4.15 HYPOTHETICAL AXIS INTERPOLATION (G07)
- 4.16 VARIABLE LEAD THREADING (G34)
- 4.17 CIRCULAR THREADING (G35, G36)
- 4.18 SKIP FUNCTION (G31)
- 4.19 MULTI-STEP SKIP (G31)
- 4.20 HIGH-SPEED SKIP SIGNAL (G31)
- 4.21 CONTINUOUS HIGH-SPEED SKIP FUNCTION
- 4.22 TORQUE LIMIT SKIP
- 4.23 THREE-DIMENSIONAL CIRCULAR INTERPOLATION
- 5 FEED FUNCTIONS
- 6 REFERENCE POSITION
- 7 COORDINATE SYSTEM
- 7.1 MACHINE COORDINATE SYSTEM
- 7.2 WORKPIECE COORDINATE SYSTEM
- 7.2.1 Setting a Workpiece Coordinate System
- 7.2.2 Selecting a Workpiece Coordinate System
- 7.2.3 Changing Workpiece Coordinate System
- 7.2.4 Workpiece Coordinate System Preset (G92.1)
- 7.2.5 Addition of Workpiece Coordinate System Pair (G54.1 or G54)
- 7.2.6 Automatic Coordinate System Setting
- 7.2.7 Workpiece Coordinate System Shift
- 7.3 LOCAL COORDINATE SYSTEM
- 7.4 PLANE SELECTION
- 8 COORDINATE VALUE AND DIMENSION
- 9 SPINDLE SPEED FUNCTION (S FUNCTION)
- 10 TOOL FUNCTION (T FUNCTION)
- 10.1 TOOL SELECTION FUNCTION
- 10.2 TOOL MANAGEMENT FUNCTION
- 10.3 TOOL MANAGEMENT EXTENSION FUNCTION
- 10.3.1 Customization of Tool Management Data Display
- 10.3.2 Setting of Spindle Position / Standby Position Display
- 10.3.3 Input of Customize Data with the Decimal Point
- 10.3.4 Protection of Various Tool Information Items with the KEY Signal
- 10.3.5 Selection of a Tool Life Count Period
- 10.3.6 Each tool Data Screen
- 10.3.7 Total Life Time Display for Tools of The Same Type
- 10.4 TOOL MANAGEMENT FUNCTION FOR OVERSIZE TOOLS
- 10.5 TOOL LIFE MANAGEMENT
- 11 AUXILIARY FUNCTION
- 12 PROGRAM MANAGEMENT
- 13 PROGRAM CONFIGURATION
- 14 FUNCTIONS TO SIMPLIFY PROGRAMMING
- 15 COMPENSATION FUNCTION
- 16 CUSTOM MACRO
- 16.1 VARIABLES
- 16.2 SYSTEM VARIABLES
- List of system variables and constants
- - Interface signals
- - Tool compensation value
- - Tool compensation value
- - Workpiece coordinate system shift amount
- - Automatic operation or the like
- - Time
- - Number of parts
- - Tool compensation memory
- - Main program number
- - Modal information
- - Position information
- - Tool length compensation value
- - Tool offset value
- - Servo position deviation
- - Manual handle interruption
- - Distance to go
- - Workpiece origin offset value, extended workpiece origin offset value
- - Skip position (detection unit)
- - Rotary table dynamic fixture offset value
- - Second geometry tool offset value
- - Dynamic standard tool compensation value
- - Feedrate reduction ratio for rapid traverse overlap
- - System constant
- Explanation
- - Interface signal #1000-#1031, #1032, #1033-#1035 (Attribute: R), #1100-#1115, #1132, #1133-#1135 (Attribute: R/W)
- - Tool compensation value #2001-#2800, #10001-#13999 (Attribute: R/W)
- - Tool compensation value #2001-#2964, #10001-#19999 (Attribute: R/W)
- - Alarm #3000 (Attribute: W)
- - Clock #3001, #3002 (Attribute: R/W)
- - Controlling of single block stop and waiting for the auxiliary function completion signal #3003 (Attribute: R/W)
- - Enabling of feed hold, feedrate override, and exact stop check #3004 (Attribute: R/W)
- - Settings #3005 (Attribute: R/W)
- - Stop with a message #3006 (Attribute: W)
- - Status of a mirror image #3007 (Attribute: R)
- - Status during restart of a program #3008 (Attribute: R)
- - Time #3011, #3012 (Attribute: R)
- - Total number of parts and the number of required parts #3901 and #3902 (Attribute: R/W)
- - Type of tool compensation memory #3980 (Attribute: R)
- - Main program number #4000 (Attribute: R)
- - Modal information #4001-#4130, #4201-#4330, #4401-#4530 (Attribute: R)
- - Position information #5001-#5080, #100001-#100200 (Attribute: R)
- - Tool length compensation value #5081-#5100, #100201-#100250 (Attribute: R)
- - Tool offset #5081-#5083, #5121-#5123 (Attribute: R), #100201-#100250, #100901-#100950
- - Servo position deviation #5101-#5120, #100251-#100300 (Attribute: R)
- - Manual handle interruption #5121-#5140, #100651-#100700 (Attribute: R)
- - Distance to go #5181-#5200, #100801-#100850 (Attribute: R)
- - Workpiece coordinate system shift value #2501, #2601 (Attribute: R/W)
- - Workpiece origin offset value #5201-#5340, #100301-#100650 (Attribute: R/W)
- - Workpiece origin offset value of the additional workpiece coordinate system
- - Skip position (detection unit) #5421-#5440, #100701-#100750 (Attribute: R)
- - Reference fixture offset number being selected #5500 (Attribute: R)
- - Reference fixture offset value being selected #5501-#5520, #117001-#117050 (Attribute: R)
- - Reference fixture offset value #5521-#5680, #117051-#117450 (Attribute: R/W)
- - Second geometry tool offset value #5801-#5896, #27001-#29999 (Attribute: R/W)
- - Dynamic reference tool compensation value #118051-#118450 (Attribute: R/W)
- - Feedrate reduction ratio for rapid traverse overlap #100851-#100900 (Attribute: R/W)
- - Switching between P-CODE variables and system variables (#10000 or later) #8570 (Attribute: R/W)
- List of system variables and constants
- 16.3 ARITHMETIC AND LOGIC OPERATION
- 16.4 INDIRECT AXIS ADDRESS SPECIFICATION
- 16.5 MACRO STATEMENTS AND NC STATEMENTS
- 16.6 BRANCH AND REPETITION
- 16.7 MACRO CALL
- 16.7.1 Simple Call (G65)
- 16.7.2 Modal Call: Call After the Move Command (G66)
- 16.7.3 Modal Call: Each Block Call (G66.1)
- 16.7.4 Macro Call Using a G Code
- 16.7.5 Macro Call Using a G Code (Specification of Multiple Definitions)
- 16.7.6 Macro Call Using a G Code with a Decimal Point (Specification of Multiple Definitions)
- 16.7.7 Macro Call Using an M Code
- 16.7.8 Macro Call Using an M Code (Specification of Multiple Definitions)
- 16.7.9 Subprogram Call Using an M Code
- 16.7.10 Subprogram Call Using an M Code (Specification of Multiple Definitions)
- 16.7.11 Subprogram Calls Using a T Code
- 16.7.12 Subprogram Calls Using an S Code
- 16.7.13 Subprogram Calls Using a Secondary Auxiliary Function
- 16.7.14 Subprogram Call Using a Specific Address
- 16.8 PROCESSING MACRO STATEMENTS
- 16.9 REGISTERING CUSTOM MACRO PROGRAMS
- 16.10 CODES AND RESERVED WORDS USED IN CUSTOM MACROS
- 16.11 EXTERNAL OUTPUT COMMANDS
- 16.12 RESTRICTIONS
- 16.13 INTERRUPTION TYPE CUSTOM MACRO
- 17 REAL-TIME CUSTOM MACRO
- 18 PROGRAMMABLE PARAMETER INPUT (G10)
- 19 PATTERN DATA INPUT
- 20 HIGH-SPEED CUTTING FUNCTIONS
- 21 AXIS CONTROL FUNCTIONS
- 21.1 AXIS SYNCHRONOUS CONTROL
- 21.1.1 Axis Configuration for Axis Synchronous Control
- 21.1.2 Synchronous Error Compensation
- 21.1.3 Synchronous Establishment
- 21.1.4 Automatic Setting for Grid Position Matching
- 21.1.5 Synchronous Error Check
- 21.1.6 Methods of Alarm Recovery by Synchronous Error Check
- 21.1.7 Axis Synchronous Control Torque Difference Alarm
- 21.2 POLYGON TURNING (G50.2, G51.2)
- 21.3 SYNCHRONOUS, COMPOSITE AND SUPERIMPOSED CONTROL BY PROGRAM COMMAND (G50.4, G51.4, G50.5, G51.5, G50.6, AND G51.6)
- 21.4 ROTARY AXIS ROLL-OVER
- 21.5 ARBITRARY ANGULAR AXIS CONTROL
- 21.6 TOOL RETRACT AND RECOVER
- 21.7 ELECTRONIC GEAR BOX
- 21.8 TANDEM CONTROL
- 21.1 AXIS SYNCHRONOUS CONTROL
- 22 5-AXIS MACHINING FUNCTION
- 22.1 TOOL CENTER POINT CONTROL
- 22.2 TOOL POSTURE CONTROL
- 22.3 TILTED WORKING PLANE COMMAND
- 22.3.1 Tilted Working Plane Command
- 22.3.2 Tilted Working Plane Command by Tool Axis Direction
- 22.3.3 Tilted Working Plane command with Guidance
- 22.3.3.1 Tilted working plane command based on roll-pitch-yaw
- 22.3.3.2 Tilted working plane command based on three points
- 22.3.3.3 Tilted working plane command based on two vectors
- 22.3.3.4 Tilted working plane command based on projection angles
- 22.3.3.5 Absolute multiple command
- 22.3.3.6 Incremental multiple command
- 22.4 INCLINED ROTARY AXIS CONTROL
- 22.5 3-DIMENSIONAL CUTTER COMPENSATION
- 23 MUITI-PATH CONTROL FUNCTION
- 1 GENERAL
- III. OPERATION
- 1 GENERAL
- 2 OPERATIONAL DEVICES
- 3 MANUAL OPERATION
- 3.1 MANUAL REFERENCE POSITION RETURN
- 3.2 JOG FEED (JOG)
- 3.3 INCREMENTAL FEED
- 3.4 MANUAL HANDLE FEED
- 3.5 MANUAL ABSOLUTE ON AND OFF
- 3.6 MANUAL LINEAR/CIRCULAR INTERPOLATION
- 3.7 RIGID TAPPING BY MANUAL HANDLE
- 3.8 MANUAL NUMERICAL COMMAND
- 3.9 THREE-DIMENSIONAL MANUAL FEED
- 3.9.1 Tool Axis Direction Handle Feed / Tool Axis Direction JOG Feed / Tool Axis Direction Incremental Feed
- 3.9.2 Tool Axis Right-Angle Direction Handle Feed / Tool Axis Right-Angle Direction JOG Feed / Tool Axis Right-Angle Direction Incremental Feed
- 3.9.3 Tool Tip Center Rotation Handle Feed / Tool Tip Center Rotation JOG Feed / Tool Tip Center Rotation Incremental Feed
- 3.9.4 Table Vertical Direction Handle Feed / Table Vertical Direction JOG Feed / Table Vertical Direction Incremental Feed
- 3.9.5 Table Horizontal Direction Handle Feed / Table Horizontal Direction JOG Feed / Table Horizontal Direction Incremental Feed
- 3.10 DISTANCE CODED LINEAR SCALE INTERFACE
- 3.11 LINEAR SCALE WITH DISTANCE-CODED REFERENCE MARKS (SERIAL)
- 3.12 MANUAL HANDLE RETRACE
- 3.13 AUXILIARY FUNCTION OUTPUT BLOCK REVERSE MOVEMENT FOR MANUAL HANDLE RETRACE
- 4 AUTOMATIC OPERATION
- 5 TEST OPERATION
- 6 SAFETY FUNCTIONS
- 7 ALARM AND SELF-DIAGNOSIS FUNCTIONS
- 8 DATA INPUT/OUTPUT
- 8.1 OVERWRITING FILES ON A MEMORY CARD
- 8.2 INPUT/OUTPUT ON EACH SCREEN
- 8.2.1 Inputting and Outputting a Program
- 8.2.2 Inputting and Outputting Parameters
- 8.2.3 Inputting and Outputting Offset Data
- 8.2.4 Inputting and Outputting Pitch Error Compensation Data
- 8.2.5 Inputting and Outputting Three-dimensional Error Compensation Data
- 8.2.6 Inputting and Outputting Custom Macro Common Variables
- 8.2.7 Inputting and Outputting Workpiece Coordinates System Data
- 8.2.8 Inputting and Outputting Operation History Data
- 8.2.9 Inputting and Outputting Tool Management Data
- 8.2.9.1 Inputting tool management data
- 8.2.9.2 Outputting tool management data
- 8.2.9.3 Inputting magazine data
- 8.2.9.4 Outputting magazine data
- 8.2.9.5 Inputting tool life status name data
- 8.2.9.6 Outputting tool life status name data
- 8.2.9.7 Inputting name data of customize data
- 8.2.9.8 Outputting name data of customize data
- 8.2.9.9 Inputting customize data displayed as tool management data
- 8.2.9.10 Outputting customize data displayed as tool management data
- 8.2.9.11 Inputting spindle waiting position name data
- 8.2.9.12 Outputting spindle waiting position name data
- 8.2.9.13 Inputting decimal point position data of customize data
- 8.2.9.14 Outputting decimal point position data of customize data
- 8.2.9.15 Inputting tool geometry data
- 8.2.9.16 Outputting tool geometry data
- 8.3 INPUT/OUTPUT ON THE ALL IO SCREEN
- 8.3.1 Inputting/Outputting a Program
- 8.3.2 Inputting and Outputting Parameters
- 8.3.3 Inputting and Outputting Offset Data
- 8.3.4 Inputting/Outputting Pitch Error Compensation Data
- 8.3.5 Inputting/Outputting Custom Macro Common Variables
- 8.3.6 Inputting and Outputting Workpiece Coordinates System Data
- 8.3.7 Inputting and Outputting Operation History Data
- 8.3.8 Inputting and Outputting Tool Management Data
- 8.3.9 File Format and Error Messages
- 8.4 EMBEDDED ETHERNET OPERATIONS
- 8.5 SCREEN HARD COPY FUNCTION
- 9 CREATING PROGRAMS
- 10 EDITING PROGRAMS
- 10.1 EDIT DISABLE ATTRIBUTE
- 10.2 INSERTING, ALTERING AND DELETING A WORD
- 10.3 DELETING BLOCKS
- 10.4 PROGRAM SEARCH
- 10.5 SEQUENCE NUMBER SEARCH
- 10.6 DELETING PROGRAMS
- 10.7 EDITING OF CUSTOM MACROS
- 10.8 CURSOR MOVEMENT LIMITATIONS ON PROGRAM EDITING
- 10.9 PASSWORD FUNCTION
- 10.10 EDITING PROGRAM CHARACTERS
- 10.11 PROGRAM COPY FUNCTION
- 10.12 KEYS AND PROGRAM ENCRYPTION
- 10.13 SIMULTANEOUS EDITING OF MULTIPATH PROGRAMS
- 11 PROGRAM MANAGEMENT
- 11.1 SELECTING A DEVICE
- 11.2 CREATING A FOLDER
- 11.3 RENAMING A FOLDER
- 11.4 CHANGING FOLDER ATTRIBUTES
- 11.5 DELETING A FOLDER
- 11.6 SELECTING A DEFAULT FOLDER
- 11.7 RENAMING A FILE
- 11.8 DELETING A FILE
- 11.9 CHANGING FILE ATTRIBUTES
- 11.10 SELECTING A MAIN PROGRAM
- 11.11 MAKING A PROGRAM COMPACT
- 11.12 PROGRAM COPY FUNCTION
- 12 SETTING AND DISPLAYING DATA
- 12.1 SCREENS DISPLAYED BY FUNCTION KEY <POS>
- Screens of a 7.2/8.4/10.4-inch display unit
- 12.1.1 Position Display in the Workpiece Coordinate System
- 12.1.2 Position Display in the Relative Coordinate System
- 12.1.3 Overall Position Display
- 12.1.4 Workpiece Coordinate System Preset
- 12.1.5 Actual Feedrate Display
- 12.1.6 Display of Run Time and Parts Count
- 12.1.7 Setting the Floating Reference Position
- 12.1.8 Operating Monitor Display
- 12.1.9 Display of Three-dimensional Manual Feed (Tool Tip Coordinates, Number of Pulses, Machine Axis Move Amount)
- Screens of a 15-inch display unit
- 12.1.10 Overall Position Display (15-inch Display Unit)
- 12.1.11 Workpiece Coordinate System Preset (15-inch Display Unit)
- 12.1.12 Actual Feedrate Display (15-inch Display Unit)
- 12.1.13 Display of Run Time and Parts Count (15-inch Display Unit)
- 12.1.14 Setting the Floating Reference Position (15-inch Display Unit)
- 12.1.15 Operating Monitor Display (15-inch Display Unit)
- 12.1.16 Display of Three-dimensional Manual Feed (Tool Tip Coordinates, Number of Pulses, Machine Axis Move Amount) (15-inch Display Unit)
- Screens of a 7.2/8.4/10.4-inch display unit
- 12.2 SCREENS DISPLAYED BY FUNCTION KEY <PROG>
- Screens of a 7.2/8.4/10.4-inch display unit
- 12.2.1 Program Contents Display
- 12.2.2 Editing a Program
- 12.2.3 Program Screen for MDI Operation
- 12.2.4 Program Folder Screen
- 12.2.5 Next Block Display Screen
- 12.2.6 Program Check Screen
- 12.2.7 Background Editing
- 12.2.8 Stamping the Machining Time
- 12.2.9 Screen for Assistance in Entering Tilted Working Plane Command
- Screens of a 15-inch display unit
- 12.2.10 Program Contents Display (15-inch Display Unit)
- 12.2.11 Editing a Program (15-inch Display Unit)
- 12.2.12 Program Screen for MDI Operation (15-inch Display Unit)
- 12.2.13 Program Folder Screen (15-inch Display Unit)
- 12.2.14 Next Block Display Screen (15-inch Display Unit)
- 12.2.15 Program Check Screen (15-inch Display Unit)
- 12.2.16 Background Editing (15-inch Display Unit)
- 12.2.17 Stamping the Machining Time (15-inch Display Unit)
- 12.2.18 Screen for Assistance in Entering Tilted Working Plane Command (15-inch Display Unit)
- Screens of a 7.2/8.4/10.4-inch display unit
- 12.3 SCREENS DISPLAYED BY FUNCTION KEY <OFS/SET>
- Screens of a 7.2/8.4/10.4-inch display unit
- 12.3.1 Displaying and Entering Setting Data
- 12.3.2 Sequence Number Comparison and Stop
- 12.3.3 Displaying and Setting Run Time, Parts Count, and Time
- 12.3.4 Displaying and Setting the Workpiece Origin Offset Value
- 12.3.5 Direct Input of Workpiece Origin Offset Value Measured
- 12.3.6 Displaying and Setting Custom Macro Common Variables
- 12.3.7 Displaying and Setting Real Time Custom Macro Data
- 12.3.8 Displaying and Setting the Software Operator’s Panel
- 12.3.9 Setting and Displaying Tool Management Data
- 12.3.9.1 Displaying and setting magazine screen
- 12.3.9.2 Displaying and setting tool management screen
- 12.3.9.3 Each tool data screen
- 12.3.9.4 Displaying the total life of tools of the same type
- 12.3.9.5 Tool geometry data screen
- 12.3.10 Displaying and Switching the Display Language
- 12.3.11 Protection of Data at Eight Levels
- 12.3.11.1 Operation level setting
- 12.3.11.2 Password modification
- 12.3.11.3 Protection level setting
- 12.3.11.4 Setting the change protection level and output protection level of a program
- 12.3.12 Precision Level Selection
- 12.3.13 Displaying and Setting Tool Life Management Data
- 12.3.13.1 Tool life management (list screen)
- 12.3.13.2 Tool life management (group editing screen)
- 12.3.14 Displaying and Setting Workpiece Setting Error Compensation Data
- 12.3.15 Displaying and Setting Pattern Data Inputs
- Screens of a 15-inch display unit
- 12.3.16 Displaying and Entering Setting Data (15-inch Display Unit)
- 12.3.17 Sequence Number Comparison and Stop (15-inch Display Unit)
- 12.3.18 Displaying and Setting Run Time, Parts Count, and Time (15-inch Display Unit)
- 12.3.19 Displaying and Setting the Workpiece Origin Offset Value (15-inch Display Unit)
- 12.3.20 Direct Input of Workpiece Origin Offset Value Measured (15-inch Display Unit)
- 12.3.21 Displaying and Setting Custom Macro Common Variables (15-inch Display Unit)
- 12.3.22 Displaying and Setting Real Time Custom Macro Data (15-inch Display Unit)
- 12.3.23 Displaying and Setting the Software Operator’s Panel (15-inch Display Unit)
- 12.3.24 Setting and Displaying Tool Management Data (15-inch Display Unit)
- 12.3.24.1 Displaying and setting magazine screen (15-inch display unit)
- 12.3.24.2 Displaying and setting tool management screen (15-inch display unit)
- 12.3.24.3 Each tool data screen (15-inch display unit)
- 12.3.24.4 Displaying the total life of tools of the same type (15-inch display unit)
- 12.3.24.5 Tool geometry data screen (15-inch display unit)
- 12.3.25 Displaying and Switching the Display Language (15-inch Display Unit)
- 12.3.26 Protection of Data at Eight Levels (15-inch Display Unit)
- 12.3.27 Precision Level Selection (15-inch Display Unit)
- 12.3.28 Displaying and Setting Tool Life Management Data (15-inch Display Unit)
- 12.3.29 Displaying and Setting Workpiece Setting Error Compensation Data (15-inch Display Unit)
- 12.3.30 Displaying and Setting Pattern Data Inputs (15-inch Display Unit)
- Screens of a 7.2/8.4/10.4-inch display unit
- 12.4 SCREENS DISPLAYED BY FUNCTION KEY <SYSTEM>
- Screens of a 7.2/8.4/10.4-inch display unit
- 12.4.1 Displaying and Setting Parameters
- 12.4.2 Displaying and Setting Pitch Error Compensation Data
- 12.4.3 Displaying and Setting Three-Dimensional Error Compensation Data
- 12.4.4 Servo Parameters
- 12.4.5 Servo Tuning
- 12.4.6 Spindle Setting
- 12.4.7 Spindle Tuning
- 12.4.8 Spindle Monitor
- 12.4.9 Color Setting Screen
- 12.4.10 Machining Parameter Tuning
- 12.4.11 Displaying Memory Data
- 12.4.12 Parameter Tuning Screen
- 12.4.12.1 Displaying the menu screen and selecting a menu item
- 12.4.12.2 Parameter tuning screen (system setting)
- 12.4.12.3 Parameter tuning screen (axis setting)
- 12.4.12.4 Displaying and setting the FSSB amplifier setting screen
- 12.4.12.5 Displaying and setting the FSSB axis setting screen
- 12.4.12.6 Displaying and setting the servo setting screen
- 12.4.12.7 Parameter tuning screen (spindle setting)
- 12.4.12.8 Parameter tuning screen (miscellaneous settings)
- 12.4.12.9 Displaying and setting the servo tuning screen
- 12.4.12.10 Displaying and setting the spindle tuning screen
- 12.4.12.11 Displaying and setting the machining parameter tuning screen
- 12.4.13 Periodic Maintenance Screen
- 12.4.14 System Configuration Screen
- 12.4.15 Overview of the History Function
- Screens of a 15-inch display unit
- 12.4.16 Displaying and Setting Parameters (15-inch Display Unit)
- 12.4.17 Displaying and Setting Pitch Error Compensation Data (15-inch Display Unit)
- 12.4.18 Displaying and Setting Three-Dimensional Error Compensation Data (15-inch Display Unit)
- 12.4.19 Servo Parameters (15-inch Display Unit)
- 12.4.20 Servo Tuning (15-inch Display Unit)
- 12.4.21 Spindle Setting (15-inch Display Unit)
- 12.4.22 Spindle Tuning (15-inch Display Unit)
- 12.4.23 Spindle Monitor (15-inch Display Unit)
- 12.4.24 Color Setting Screen (15-inch Display Unit)
- 12.4.25 Machining Parameter Tuning (15-inch Display Unit)
- 12.4.26 Displaying Memory Data (15-inch Display Unit)
- 12.4.27 Parameter Tuning Screen (15-inch Display Unit)
- 12.4.27.1 Displaying the menu screen and selecting a menu item (15-inch display unit)
- 12.4.27.2 Parameter tuning screen (system setting) (15-inch display unit)
- 12.4.27.3 Parameter tuning screen (axis setting) (15-inch display unit)
- 12.4.27.4 Displaying and setting the FSSB amplifier setting screen (15-inch display unit)
- 12.4.27.5 Displaying and setting the FSSB axis setting screen (15-inch display unit)
- 12.4.27.6 Displaying and setting the servo setting screen (15-inch display unit)
- 12.4.27.7 Parameter tuning screen (spindle setting) (15-inch display unit)
- 12.4.27.8 Parameter tuning screen (miscellaneous settings) (15-inch display unit)
- 12.4.27.9 Displaying and setting the servo tuning screen (15-inch display unit)
- 12.4.27.10 Displaying and setting the spindle tuning screen (15-inch display unit)
- 12.4.27.11 Displaying and setting the machining parameter tuning screen (15-inch display unit)
- 12.4.28 Periodic Maintenance Screen (15-inch Display Unit)
- 12.4.29 System Configuration Screen (15-inch Display Unit)
- 12.4.30 Overview of the History Function (15-inch Display Unit)
- Screens of a 7.2/8.4/10.4-inch display unit
- 12.5 SCREENS DISPLAYED BY FUNCTION KEY <MESSAGE>
- 12.6 DISPLAYING THE PROGRAM NUMBER/NAME, SEQUENCE NUMBER, AND STATUS, AND WARNING MESSAGES FOR DATA SETTING OR INPUT/OUTPUT OPERATION
- 12.7 SCREEN ERASURE FUNCTION AND AUTOMATIC SCREEN ERASURE FUNCTION
- 12.8 LOAD METER SCREEN
- 12.1 SCREENS DISPLAYED BY FUNCTION KEY <POS>
- 13 GRAPHIC FUNCTION
- 14 VIRTUAL MDI KEY FUNCTION
- IV. MAINTENANCE
- APPENDIX
- A PARAMETERS
- B PROGRAM CODE LIST
- C LIST OF FUNCTIONS AND PROGRAM FORMAT
- D RANGE OF COMMAND VALUE
- E NOMOGRAPHS
- F SETTINGS AT POWER-ON, IN THE CLEAR STATE, OR IN THE RESET STATE
- G CHARACTER-TO-CODES CORRESPONDENCE TABLE
- H ALARM LIST
- (1) Alarms on program and operation (PS alarm)
- (2) Background edit alarms (BG alarm)
- (3) Communication alarms (SR alarm)
- (4) Parameter writing alarm (SW alarm)
- (5) Servo alarms (SV alarm)
- (6) Overtravel alarms (OT alarm)
- (7) Memory file alarms (IO alarm)
- (8) Alarms requiring power to be turned off (PW alarm)
- (9) Spindle alarms (SP alarm)
- (10) Alarm list (serial spindle)
- (11) Overheat alarms (OH alarm)
- (12) Other alarms (DS alarm)
- (13) Malfunction prevention function alarms (IE alarm)
- I PC TOOL FOR MEMORY CARD PROGRAM OPERATION/EDITING
- INDEX
- Revision Record
USER’S MANUAL
B-63944EN/03
Common to Lathe System/Machining Center System
FANU
C
Series 30*
/
300*
/
300*
s
-
MODEL A
FANUC Series 31*/310*/310*s-MODEL A
FANUC Series 32*/320*/320*s-MODEL A
• No part of this manual may be reproduced in any form.
• All specifications and designs are subject to change without notice.
The products in this manual are controlled based on Japan’s “Foreign Exchange and
Foreign Trade Law”. The export of Series 30i/300i/300is-MODEL A, Series
31i/310i/310is-MODEL A5 from Japan is subject to an export license by the government of
Japan. Other models in this manual may also be subject to export controls.
Further, re-export to another country may be subject to the license of the government of
the country from where the product is re-exported. Furthermore, the product may also be
controlled by re-export regulations of the United States government.
Should you wish to export or re-export these products, please contact FANUC for advice.
In this manual we have tried as much as possible to describe all the various matters.
However, we cannot describe all the matters which must not be done, or which cannot be
done, because there are so many possibilities.
Therefore, matters which are not especially described as possible in this manual should be
regarded as ”impossible”.
B-63944EN/03 SAFETY PRECAUTIONS
s-1
SAFETY PRECAUTIONS
This section describes the safety precautions related to the use of CNC
units.
It is essential that these precautions be observed by users to ensure the
safe operation of machines equipped with a CNC unit (all descriptions
in this section assume this configuration). Note that some precautions
are related only to specific functions, and thus may not be applicable
to certain CNC units.
Users must also observe the safety precautions related to the machine,
as described in the relevant manual supplied by the machine tool
builder. Before attempting to operate the machine or create a program
to control the operation of the machine, the operator must become
fully familiar with the contents of this manual and relevant manual
supplied by the machine tool builder.
CONTENTS
DEFINITION OF WARNING, CAUTION, AND NOTE ................s-2
GENERAL WARNINGS AND CAUTIONS....................................s-3
WARNINGS AND CAUTIONS RELATED TO
PROGRAMMING .............................................................................s-6
WARNINGS AND CAUTIONS RELATED TO HANDLING........s-9
WARNINGS RELATED TO DAILY MAINTENANCE...............s-12
SAFETY PRECAUTIONS B-63944EN/03
s-2
DEFINITION OF WARNING, CAUTION, AND NOTE
This manual includes safety precautions for protecting the user and
preventing damage to the machine. Precautions are classified into
Warning and Caution according to their bearing on safety. Also,
supplementary information is described as a Note. Read the
Warning, Caution, and Note thoroughly before attempting to use
the machine.
WARNING
Applied when there is a danger of the user being
injured or when there is a danger of both the user
being injured and the equipment being damaged if
the approved procedure is not observed.
CAUTION
Applied when there is a danger of the equipment
being damaged, if the approved procedure is not
observed.
NOTE
The Note is used to indicate supplementary
information other than Warning and Caution.
• Read this manual carefully, and store it in a safe place.
B-63944EN/03 SAFETY PRECAUTIONS
s-3
GENERAL WARNINGS AND CAUTIONS
WARNING
1 Never attempt to machine a workpiece without first
checking the operation of the machine. Before
starting a production run, ensure that the machine
is operating correctly by performing a trial run
using, for example, the single block, feedrate
override, or machine lock function or by operating
the machine with neither a tool nor workpiece
mounted. Failure to confirm the correct operation
of the machine may result in the machine behaving
unexpectedly, possibly causing damage to the
workpiece and/or machine itself, or injury to the
user.
2 Before operating the machine, thoroughly check
the entered data.
Operating the machine with incorrectly specified
data may result in the machine behaving
unexpectedly, possibly causing damage to the
workpiece and/or machine itself, or injury to the
user.
3 Ensure that the specified feedrate is appropriate
for the intended operation. Generally, for each
machine, there is a maximum allowable feedrate.
The appropriate feedrate varies with the intended
operation. Refer to the manual provided with the
machine to determine the maximum allowable
feedrate.
If a machine is run at other than the correct speed,
it may behave unexpectedly, possibly causing
damage to the workpiece and/or machine itself, or
injury to the user.
4 When using a tool compensation function,
thoroughly check the direction and amount of
compensation.
Operating the machine with incorrectly specified
data may result in the machine behaving
unexpectedly, possibly causing damage to the
workpiece and/or machine itself, or injury to the
user.
SAFETY PRECAUTIONS B-63944EN/03
s-4
WARNING
5 The parameters for the CNC and PMC are
factory-set. Usually, there is not need to change
them. When, however, there is not alternative other
than to change a parameter, ensure that you fully
understand the function of the parameter before
making any change.
Failure to set a parameter correctly may result in
the machine behaving unexpectedly, possibly
causing damage to the workpiece and/or machine
itself, or injury to the user.
6 Immediately after switching on the power, do not
touch any of the keys on the MDI panel until the
position display or alarm screen appears on the
CNC unit.
Some of the keys on the MDI panel are dedicated
to maintenance or other special operations.
Pressing any of these keys may place the CNC
unit in other than its normal state. Starting the
machine in this state may cause it to behave
unexpectedly.
7 The User’s Manual and programming manual
supplied with a CNC unit provide an overall
description of the machine's functions, including
any optional functions. Note that the optional
functions will vary from one machine model to
another. Therefore, some functions described in
the manuals may not actually be available for a
particular model. Check the specification of the
machine if in doubt.
8 Some functions may have been implemented at
the request of the machine-tool builder. When
using such functions, refer to the manual supplied
by the machine-tool builder for details of their use
and any related cautions.
CAUTION
The liquid-crystal display is manufactured with very
precise fabrication technology. Some pixels may
not be turned on or may remain on. This
phenomenon is a common attribute of LCDs and is
not a defect.
B-63944EN/03 SAFETY PRECAUTIONS
s-5
NOTE
Programs, parameters, and macro variables are
stored in nonvolatile memory in the CNC unit.
Usually, they are retained even if the power is
turned off.
Such data may be deleted inadvertently, however,
or it may prove necessary to delete all data from
nonvolatile memory as part of error recovery.
To guard against the occurrence of the above, and
assure quick restoration of deleted data, backup all
vital data, and keep the backup copy in a safe
place.
SAFETY PRECAUTIONS B-63944EN/03
s-6
WARNINGS AND CAUTIONS RELATED TO PROGRAMMING
This section covers the major safety precautions related to
programming. Before attempting to perform programming, read the
supplied User’s Manual carefully such that you are fully familiar with
their contents.
WARNING
1 Coordinate system setting
If a coordinate system is established incorrectly,
the machine may behave unexpectedly as a result
of the program issuing an otherwise valid move
command. Such an unexpected operation may
damage the tool, the machine itself, the workpiece,
or cause injury to the user.
2 Positioning by nonlinear interpolation
When performing positioning by nonlinear
interpolation (positioning by nonlinear movement
between the start and end points), the tool path
must be carefully confirmed before performing
programming. Positioning involves rapid traverse. If
the tool collides with the workpiece, it may damage
the tool, the machine itself, the workpiece, or
cause injury to the user.
3 Function involving a rotation axis
When programming polar coordinate interpolation
or normal-direction (perpendicular) control, pay
careful attention to the speed of the rotation axis.
Incorrect programming may result in the rotation
axis speed becoming excessively high, such that
centrifugal force causes the chuck to lose its grip
on the workpiece if the latter is not mounted
securely. Such mishap is likely to damage the tool,
the machine itself, the workpiece, or cause injury to
the user.
4 Inch/metric conversion
Switching between inch and metric inputs does not
convert the measurement units of data such as the
workpiece origin offset, parameter, and current
position. Before starting the machine, therefore,
determine which measurement units are being
used. Attempting to perform an operation with
invalid data specified may damage the tool, the
machine itself, the workpiece, or cause injury to the
user.
B-63944EN/03 SAFETY PRECAUTIONS
s-7
WARNING
5 Constant surface speed control
When an axis subject to constant surface speed
control approaches the origin of the workpiece
coordinate system, the spindle speed may become
excessively high. Therefore, it is necessary to
specify a maximum allowable speed. Specifying
the maximum allowable speed incorrectly may
damage the tool, the machine itself, the workpiece,
or cause injury to the user.
6 Stroke check
After switching on the power, perform a manual
reference position return as required. Stroke check
is not possible before manual reference position
return is performed. Note that when stroke check is
disabled, an alarm is not issued even if a stroke
limit is exceeded, possibly damaging the tool, the
machine itself, the workpiece, or causing injury to
the user.
7 Tool post interference check
A tool post interference check is performed based
on the tool data specified during automatic
operation. If the tool specification does not match
the tool actually being used, the interference check
cannot be made correctly, possibly damaging the
tool or the machine itself, or causing injury to the
user. After switching on the power, or after
selecting a tool post manually, always start
automatic operation and specify the tool number of
the tool to be used.
8 Absolute/incremental mode
If a program created with absolute values is run in
incremental mode, or vice versa, the machine may
behave unexpectedly.
9 Plane selection
If an incorrect plane is specified for circular
interpolation, helical interpolation, or a canned
cycle, the machine may behave unexpectedly.
Refer to the descriptions of the respective
functions for details.
10 Torque limit skip
Before attempting a torque limit skip, apply the
torque limit. If a torque limit skip is specified
without the torque limit actually being applied, a
move command will be executed without
performing a skip.
SAFETY PRECAUTIONS B-63944EN/03
s-8
WARNING
11 Programmable mirror image
Note that programmed operations vary
considerably when a programmable mirror image is
enabled.
12 Compensation function
If a command based on the machine coordinate
system or a reference position return command is
issued in compensation function mode,
compensation is temporarily canceled, resulting in
the unexpected behavior of the machine.
Before issuing any of the above commands,
therefore, always cancel compensation function
mode.
B-63944EN/03 SAFETY PRECAUTIONS
s-9
WARNINGS AND CAUTIONS RELATED TO HANDLING
This section presents safety precautions related to the handling of
machine tools. Before attempting to operate your machine, read the
supplied User’s Manual carefully, such that you are fully familiar with
their contents.
WARNING
1 Manual operation
When operating the machine manually, determine
the current position of the tool and workpiece, and
ensure that the movement axis, direction, and
feedrate have been specified correctly. Incorrect
operation of the machine may damage the tool, the
machine itself, the workpiece, or cause injury to the
operator.
2 Manual reference position return
After switching on the power, perform manual
reference position return as required.
If the machine is operated without first performing
manual reference position return, it may behave
unexpectedly. Stroke check is not possible before
manual reference position return is performed.
An unexpected operation of the machine may
damage the tool, the machine itself, the workpiece,
or cause injury to the user.
3 Manual numeric command
When issuing a manual numeric command,
determine the current position of the tool and
workpiece, and ensure that the movement axis,
direction, and command have been specified
correctly, and that the entered values are valid.
Attempting to operate the machine with an invalid
command specified may damage the tool, the
machine itself, the workpiece, or cause injury to the
operator.
4 Manual handle feed
In manual handle feed, rotating the handle with a
large scale factor, such as 100, applied causes the
tool and table to move rapidly. Careless handling
may damage the tool and/or machine, or cause
injury to the user.
SAFETY PRECAUTIONS B-63944EN/03
s-10
WARNING
5 Disabled override
If override is disabled (according to the
specification in a macro variable) during threading,
rigid tapping, or other tapping, the speed cannot be
predicted, possibly damaging the tool, the machine
itself, the workpiece, or causing injury to the
operator.
6 Origin/preset operation
Basically, never attempt an origin/preset operation
when the machine is operating under the control of
a program. Otherwise, the machine may behave
unexpectedly, possibly damaging the tool, the
machine itself, the tool, or causing injury to the
user.
7 Workpiece coordinate system shift
Manual intervention, machine lock, or mirror
imaging may shift the workpiece coordinate
system. Before attempting to operate the machine
under the control of a program, confirm the
coordinate system carefully.
If the machine is operated under the control of a
program without making allowances for any shift in
the workpiece coordinate system, the machine
may behave unexpectedly, possibly damaging the
tool, the machine itself, the workpiece, or causing
injury to the operator.
8 Software operator's panel and menu switches
Using the software operator's panel and menu
switches, in combination with the MDI panel, it is
possible to specify operations not supported by the
machine operator's panel, such as mode change,
override value change, and jog feed commands.
Note, however, that if the MDI panel keys are
operated inadvertently, the machine may behave
unexpectedly, possibly damaging the tool, the
machine itself, the workpiece, or causing injury to
the user.
9 RESET key
Pressing the RESET key stops the currently
running program. As a result, the servo axes are
stopped. However, the RESET key may fail to
function for reasons such as an MDI panel
problem. So, when the motors must be stopped,
use the emergency stop button instead of the
RESET key to ensure security.
B-63944EN/03 SAFETY PRECAUTIONS
s-11
WARNING
10 Manual intervention
If manual intervention is performed during
programmed operation of the machine, the tool
path may vary when the machine is restarted.
Before restarting the machine after manual
intervention, therefore, confirm the settings of the
manual absolute switches, parameters, and
absolute/incremental command mode.
11 Feed hold, override, and single block
The feed hold, feedrate override, and single block
functions can be disabled using custom macro
system variable #3004. Be careful when operating
the machine in this case.
12 Dry run
Usually, a dry run is used to confirm the operation
of the machine. During a dry run, the machine
operates at dry run speed, which differs from the
corresponding programmed feedrate. Note that the
dry run speed may sometimes be higher than the
programmed feed rate.
13 Cutter and tool nose radius compensation in
MDI mode
Pay careful attention to a tool path specified by a
command in MDI mode, because cutter or tool
nose radius compensation is not applied. When a
command is entered from the MDI to interrupt in
automatic operation in cutter or tool nose radius
compensation mode, pay particular attention to the
tool path when automatic operation is subsequently
resumed. Refer to the descriptions of the
corresponding functions for details.
14 Program editing
If the machine is stopped, after which the
machining program is edited (modification,
insertion, or deletion), the machine may behave
unexpectedly if machining is resumed under the
control of that program. Basically, do not modify,
insert, or delete commands from a machining
program while it is in use.
SAFETY PRECAUTIONS B-63944EN/03
s-12
WARNINGS RELATED TO DAILY MAINTENANCE
WARNING
1 Memory backup battery replacement
When replacing the memory backup batteries,
keep the power to the machine (CNC) turned on,
and apply an emergency stop to the machine.
Because this work is performed with the power on
and the cabinet open, only those personnel who
have received approved safety and maintenance
training may perform this work.
When replacing the batteries, be careful not to
touch the high-voltage circuits (marked and
fitted with an insulating cover).
Touching the uncovered high-voltage circuits
presents an extremely dangerous electric shock
hazard.
NOTE
The CNC uses batteries to preserve the contents
of its memory, because it must retain data such as
programs, offsets, and parameters even while
external power is not applied.
If the battery voltage drops, a low battery voltage
alarm is displayed on the machine operator's panel
or screen.
When a low battery voltage alarm is displayed,
replace the batteries within a week. Otherwise, the
contents of the CNC's memory will be lost.
Refer to the Section “Method of replacing battery”
in the User’s Manual (Common to T/M series) for
details of the battery replacement procedure.
B-63944EN/03 SAFETY PRECAUTIONS
s-13
WARNING
2 Absolute pulse coder battery replacement
When replacing the memory backup batteries,
keep the power to the machine (CNC) turned on,
and apply an emergency stop to the machine.
Because this work is performed with the power on
and the cabinet open, only those personnel who
have received approved safety and maintenance
training may perform this work.
When replacing the batteries, be careful not to
touch the high-voltage circuits (marked and
fitted with an insulating cover).
Touching the uncovered high-voltage circuits
presents an extremely dangerous electric shock
hazard.
NOTE
The absolute pulse coder uses batteries to
preserve its absolute position.
If the battery voltage drops, a low battery voltage
alarm is displayed on the machine operator's panel
or screen.
When a low battery voltage alarm is displayed,
replace the batteries within a week. Otherwise, the
absolute position data held by the pulse coder will
be lost.
Refer to the FANUC SERVO MOTOR αi series
Maintenance Manual for details of the battery
replacement procedure.
SAFETY PRECAUTIONS B-63944EN/03
s-14
WARNING
3 Fuse replacement
Before replacing a blown fuse, however, it is
necessary to locate and remove the cause of the
blown fuse.
For this reason, only those personnel who have
received approved safety and maintenance training
may perform this work.
When replacing a fuse with the cabinet open, be
careful not to touch the high-voltage circuits
(marked and fitted with an insulating cover).
Touching an uncovered high-voltage circuit
presents an extremely dangerous electric shock
hazard.
B-63944EN/03 TABLE OF CONTENTS
c-1
TABLE OF CONTENTS
SAFETY PRECAUTIONS............................................................................s-1
DEFINITION OF WARNING, CAUTION, AND NOTE ............................................. s-2
GENERAL WARNINGS AND CAUTIONS............................................................... s-3
WARNINGS AND CAUTIONS RELATED TO PROGRAMMING ............................ s-6
WARNINGS AND CAUTIONS RELATED TO HANDLING...................................... s-9
WARNINGS RELATED TO DAILY MAINTENANCE............................................. s-12
I. GENERAL
1 GENERAL ...............................................................................................3
1.1 NOTES ON READING THIS MANUAL.......................................................... 8
1.2 NOTES ON VARIOUS KINDS OF DATA ...................................................... 9
II. PROGRAMMING
1 GENERAL .............................................................................................13
1.1 TOOL MOVEMENT ALONG WORKPIECE PARTS
FIGURE-INTERPOLATION ......................................................................... 14
1.2 FEED-FEED FUNCTION............................................................................. 16
1.3 PART DRAWING AND TOOL MOVEMENT................................................ 17
1.3.1 Reference Position (Machine-specific Position) ....................................................17
1.3.2 Coordinate System on Part Drawing and Coordinate System Specified by CNC -
Coordinate System .................................................................................................18
1.3.3 How to Indicate Command Dimensions for Moving the Tool
(Absolute, Incremental Commands).......................................................................24
1.4 CUTTING SPEED - SPINDLE FUNCTION.................................................. 27
1.5 SELECTION OF TOOL USED FOR VARIOUS MACHINING - TOOL
FUNCTION .................................................................................................. 28
1.6 COMMAND FOR MACHINE OPERATIONS - AUXILIARY FUNCTION ...... 29
1.7 PROGRAM CONFIGURATION ................................................................... 30
1.8 TOOL MOVEMENT RANGE - STROKE...................................................... 33
2 CONTROLLED AXES ...........................................................................34
2.1 NUMBER OF CONTROLLED AXES ........................................................... 35
2.2 NAMES OF AXES ....................................................................................... 36
2.3 INCREMENT SYSTEM................................................................................ 37
2.4 MAXIMUM STROKE.................................................................................... 38
TABLE OF CONTENTS B-63944EN/03
c-2
3 PREPARATORY FUNCTION (G FUNCTION) .....................................39
3.1 G CODE LIST IN THE MACHINING CENTER SYSTEM ............................ 41
3.2 G CODE LIST IN THE LATHE SYSTEM .................................................... 45
4 INTERPOLATION FUNCTIONS............................................................ 50
4.1 POSITIONING (G00) ................................................................................... 51
4.2 SINGLE DIRECTION POSITIONING (G60) ................................................ 53
4.3 LINEAR INTERPOLATION (G01)................................................................ 56
4.4 CIRCULAR INTERPOLATION (G02, G03).................................................. 59
4.5 HELICAL INTERPOLATION (G02, G03) ..................................................... 65
4.6 HELICAL INTERPOLATION B (G02, G03).................................................. 67
4.7 SPIRAL INTERPOLATION, CONICAL INTERPOLATION (G02, G03)........ 68
4.8 POLAR COORDINATE INTERPOLATION (G12.1, G13.1) ......................... 76
4.9 CYLINDRICAL INTERPOLATION (G07.1) .................................................. 85
4.10 CUTTING POINT INTERPOLATION FOR CYLINDRICAL
INTERPOLATION (G07.1)........................................................................... 90
4.11 EXPONENTIAL INTERPOLATION (G02.3, G03.3) ................................... 102
4.12 SMOOTH INTERPOLATION (G05.1) ........................................................ 109
4.13 NANO SMOOTHING ................................................................................. 113
4.14 NURBS INTERPOLATION (G06.2) ........................................................... 121
4.14.1 NURBS Interpolation Additional Functions ........................................................127
4.15 HYPOTHETICAL AXIS INTERPOLATION (G07) ...................................... 131
4.16 VARIABLE LEAD THREADING (G34)....................................................... 133
4.17 CIRCULAR THREADING (G35, G36) ....................................................... 134
4.18 SKIP FUNCTION (G31)............................................................................. 139
4.19 MULTI-STEP SKIP (G31) .......................................................................... 141
4.20 HIGH-SPEED SKIP SIGNAL (G31) ........................................................... 142
4.21 CONTINUOUS HIGH-SPEED SKIP FUNCTION....................................... 143
4.22 TORQUE LIMIT SKIP ................................................................................ 145
4.23 THREE-DIMENSIONAL CIRCULAR INTERPOLATION............................ 149
5 FEED FUNCTIONS ............................................................................. 154
5.1 OVERVIEW ............................................................................................... 155
5.2 RAPID TRAVERSE ................................................................................... 157
5.3 CUTTING FEED ........................................................................................ 158
5.4 CUTTING FEEDRATE CONTROL ............................................................ 164
5.4.1 Exact Stop (G09, G61), Cutting Mode (G64), Tapping Mode (G63) ..................165
5.4.2 Automatic Corner Override..................................................................................166
B-63944EN/03 TABLE OF CONTENTS
c-3
5.4.2.1 Automatic override for inner corners (G62) .............................................. 166
5.4.2.2 Internal circular cutting feedrate change.................................................... 168
5.5 FEEDRATE INSTRUCTION ON IMAGINARY CIRCLE FOR A ROTARY
AXIS .......................................................................................................... 169
5.6 DWELL ...................................................................................................... 174
6 REFERENCE POSITION.....................................................................176
6.1 REFERENCE POSITION RETURN........................................................... 177
6.2 FLOATING REFERENCE POSITION RETURN (G30.1)........................... 184
7 COORDINATE SYSTEM.....................................................................186
7.1 MACHINE COORDINATE SYSTEM.......................................................... 187
7.2 WORKPIECE COORDINATE SYSTEM .................................................... 190
7.2.1 Setting a Workpiece Coordinate System..............................................................190
7.2.2 Selecting a Workpiece Coordinate System ..........................................................193
7.2.3 Changing Workpiece Coordinate System ............................................................194
7.2.4 Workpiece Coordinate System Preset (G92.1).....................................................198
7.2.5 Addition of Workpiece Coordinate System Pair (G54.1 or G54) ........................201
7.2.6 Automatic Coordinate System Setting .................................................................203
7.2.7 Workpiece Coordinate System Shift ....................................................................204
7.3 LOCAL COORDINATE SYSTEM .............................................................. 206
7.4 PLANE SELECTION.................................................................................. 208
8 COORDINATE VALUE AND DIMENSION .........................................209
8.1 ABSOLUTE AND INCREMENTAL PROGRAMMING................................ 210
8.2 INCH/METRIC CONVERSION (G20, G21) ............................................... 212
8.3 DECIMAL POINT PROGRAMMING .......................................................... 216
8.4 DIAMETER AND RADIUS PROGRAMMING ............................................ 218
8.5 DIAMETER AND RADIUS SETTING SWITCHING FUNCTION................ 219
9 SPINDLE SPEED FUNCTION (S FUNCTION) ...................................223
9.1 SPECIFYING THE SPINDLE SPEED WITH A CODE............................... 224
9.2 SPECIFYING THE SPINDLE SPEED VALUE DIRECTLY
(S5-DIGIT COMMAND) ............................................................................. 224
9.3 CONSTANT SURFACE SPEED CONTROL (G96, G97) .......................... 225
9.4 SPINDLE POSITIONING FUNCTION ....................................................... 230
9.4.1 Spindle Orientation...............................................................................................231
9.4.2 Spindle Positioning ..............................................................................................232
9.4.3 Canceling Spindle Positioning .............................................................................234
9.5 SPINDLE SPEED FLUCTUATION DETECTION....................................... 236
TABLE OF CONTENTS B-63944EN/03
c-4
9.6 SPINDLE CONTROL WITH SERVO MOTOR........................................... 241
9.6.1 Spindle Control with Servo Motor .......................................................................241
9.6.2 Spindle Indexing Function ...................................................................................242
10 TOOL FUNCTION (T FUNCTION) ...................................................... 244
10.1 TOOL SELECTION FUNCTION ................................................................ 245
10.2 TOOL MANAGEMENT FUNCTION........................................................... 247
10.3 TOOL MANAGEMENT EXTENSION FUNCTION ..................................... 265
10.3.1 Customization of Tool Management Data Display ..............................................265
10.3.2 Setting of Spindle Position / Standby Position Display .......................................270
10.3.3 Input of Customize Data with the Decimal Point.................................................272
10.3.4 Protection of Various Tool Information Items with the KEY Signal...................275
10.3.5 Selection of a Tool Life Count Period..................................................................275
10.3.6 Each tool Data Screen ..........................................................................................276
10.3.7 Total Life Time Display for Tools of The Same Type.........................................276
10.4 TOOL MANAGEMENT FUNCTION FOR OVERSIZE TOOLS .................. 277
10.5 TOOL LIFE MANAGEMENT...................................................................... 279
10.5.1 Tool Life Management Data ................................................................................281
10.5.2 Registering, Changing, and Deleting Tool Life Management Data .....................284
10.5.3 Tool Life Management Commands in Machining Program.................................290
10.5.4 Tool Life Counting and Tool Selection................................................................299
10.5.5 Tool Life Count Restart M Code..........................................................................303
10.5.6 Disabling Life Count ............................................................................................305
11 AUXILIARY FUNCTION......................................................................306
11.1 AUXILIARY FUNCTION (M FUNCTION)................................................... 307
11.2 MULTIPLE M COMMANDS IN A SINGLE BLOCK.................................... 308
11.3 M CODE GROUPING FUNCTION ............................................................ 309
11.3.1 Setting an M Code Group Number Using the Setting Screen ..............................309
11.3.2 Setting an M Code Group Number Using a Program...........................................312
11.3.3 M Code Group Check Function ...........................................................................313
11.4 SECOND AUXILIARY FUNCTIONS (B CODES) ...................................... 314
12 PROGRAM MANAGEMENT ............................................................... 317
12.1 FOLDERS.................................................................................................. 318
12.1.1 Folder Configuration ............................................................................................318
12.1.2 Folder Attributes...................................................................................................321
12.1.3 Default Folders .....................................................................................................322
12.2 FILES......................................................................................................... 323
B-63944EN/03 TABLE OF CONTENTS
c-5
12.2.1 File Name .............................................................................................................323
12.2.2 File Attributes.......................................................................................................325
12.3 RELATION WITH CONVENTIONAL FUNCTIONS.................................... 326
12.3.1 Relation with Folders ...........................................................................................326
12.3.2 Relation with File Names .....................................................................................328
12.3.3 Related Parameters ...............................................................................................329
12.3.4 Part Program Storage Size / Number of Registerable Programs ..........................330
13 PROGRAM CONFIGURATION...........................................................331
13.1 PROGRAM COMPONENTS OTHER THAN PROGRAM SECTIONS....... 333
13.2 PROGRAM SECTION CONFIGURATION ................................................ 336
13.3 SUBPROGRAM (M98, M99) ..................................................................... 344
14 FUNCTIONS TO SIMPLIFY PROGRAMMING ...................................350
14.1 FIGURE COPYING (G72.1, G72.2)........................................................... 351
14.2 THREE-DIMENSIONAL COORDINATE SYSTEM CONVERSION ........... 359
15 COMPENSATION FUNCTION ............................................................370
15.1 TOOL LENGTH COMPENSATION (G43, G44, G49)................................ 371
15.1.1 Overview ..............................................................................................................371
15.1.2 G53, G28, G30, and G30.1 Commands in Tool Length Compensation Mode ....377
15.2 SCALING (G50, G51) ................................................................................ 379
15.3 PROGRAMMABLE MIRROR IMAGE (G50.1, G51.1) ............................... 389
15.4 NORMAL DIRECTION CONTROL (G40.1,G41.1,G42.1).......................... 391
15.5 WORKPIECE SETTING ERROR COMPENSATION ................................ 397
16 CUSTOM MACRO...............................................................................437
16.1 VARIABLES............................................................................................... 438
16.2 SYSTEM VARIABLES ............................................................................... 445
16.3 ARITHMETIC AND LOGIC OPERATION .................................................. 502
16.4 INDIRECT AXIS ADDRESS SPECIFICATION .......................................... 509
16.5 MACRO STATEMENTS AND NC STATEMENTS..................................... 511
16.6 BRANCH AND REPETITION..................................................................... 512
16.6.1 Unconditional Branch (GOTO Statement)...........................................................512
16.6.2 GOTO Statement Using Stored Sequence Numbers ............................................513
16.6.3 Conditional Branch (IF Statement) ......................................................................515
16.6.4 Repetition (WHILE Statement)............................................................................517
16.7 MACRO CALL ........................................................................................... 520
16.7.1 Simple Call (G65) ................................................................................................521
16.7.2 Modal Call: Call After the Move Command (G66) .............................................532
TABLE OF CONTENTS B-63944EN/03
c-6
16.7.3 Modal Call: Each Block Call (G66.1) .................................................................537
16.7.4 Macro Call Using a G Code .................................................................................540
16.7.5 Macro Call Using a G Code (Specification of Multiple Definitions)...................542
16.7.6 Macro Call Using a G Code with a Decimal Point (Specification of Multiple
Definitions)...........................................................................................................543
16.7.7 Macro Call Using an M Code...............................................................................544
16.7.8 Macro Call Using an M Code (Specification of Multiple Definitions)................545
16.7.9 Subprogram Call Using an M Code .....................................................................546
16.7.10 Subprogram Call Using an M Code (Specification of Multiple Definitions).......547
16.7.11 Subprogram Calls Using a T Code.......................................................................548
16.7.12 Subprogram Calls Using an S Code .....................................................................549
16.7.13 Subprogram Calls Using a Secondary Auxiliary Function ..................................550
16.7.14 Subprogram Call Using a Specific Address .........................................................551
16.8 PROCESSING MACRO STATEMENTS ................................................... 555
16.9 REGISTERING CUSTOM MACRO PROGRAMS ..................................... 557
16.10 CODES AND RESERVED WORDS USED IN CUSTOM MACROS ......... 558
16.11 EXTERNAL OUTPUT COMMANDS.......................................................... 559
16.12 RESTRICTIONS ........................................................................................ 563
16.13 INTERRUPTION TYPE CUSTOM MACRO............................................... 565
16.13.1 Specification Method ...........................................................................................566
16.13.2 Details of Functions..............................................................................................567
17 REAL-TIME CUSTOM MACRO ..........................................................577
17.1 TYPES OF REAL TIME MACRO COMMANDS......................................... 581
17.1.1 Modal Real Time Macro Command / One-shot Real Time Macro Command.....581
17.2 VARIABLES............................................................................................... 588
17.2.1 Variables Dedicated To Real Time Custom Macros ............................................589
17.2.1.1 System variables......................................................................................... 589
17.2.1.2 Real time macro variables (RTM variables) ............................................. 592
17.2.2 Custom Macro Variables......................................................................................594
17.2.2.1 System variables......................................................................................... 594
17.2.2.2 Local variables ........................................................................................... 595
17.3 ARITHMETIC AND LOGICAL OPERATION.............................................. 596
17.4 CONTROL ON REAL TIME MACRO COMMANDS .................................. 598
17.4.1 Conditional Branch (ZONCE Statement).............................................................599
17.4.2 Condition Transition (ZEDGE Statement)...........................................................600
17.4.3 Repetition (ZWHILE Statement) .........................................................................601
17.4.4 Multi-statement (ZDO...ZEND Statement) ..........................................................602
B-63944EN/03 TABLE OF CONTENTS
c-7
17.5 MACRO CALL ........................................................................................... 605
17.6 OTHERS.................................................................................................... 607
17.7 AXIS CONTROL COMMAND .................................................................... 608
17.8 NOTES ...................................................................................................... 622
17.9 LIMITATION .............................................................................................. 624
18 PROGRAMMABLE PARAMETER INPUT (G10)................................626
19 PATTERN DATA INPUT ..................................................................... 629
19.1 OVERVIEW ............................................................................................... 630
19.2 EXPLANATION.......................................................................................... 631
19.3 EXPLANATION OF OPERATION.............................................................. 634
19.4 DEFINITION OF THE SCREEN ................................................................ 638
19.4.1 Definition of the Pattern Menu Screen.................................................................639
19.4.2 Definition of the Custom Macro Screen...............................................................641
19.4.3 Setting the Character-codes..................................................................................645
20 HIGH-SPEED CUTTING FUNCTIONS................................................652
20.1 AI CONTOUR CONTROL FUNCTION I AND AI CONTOUR CONTROL
FUNCTION II (G05.1) ................................................................................ 653
20.2 MACHINING CONDITION SELECTING FUNCTION ................................ 670
20.3 JERK CONTROL ....................................................................................... 671
20.3.1 Speed Control with Change of Acceleration on Each Axis..................................671
20.3.2 Look-Ahead Smooth Bell-Shaped Acceleration/Deceleration before
Interpolation .........................................................................................................674
20.4 OPTIMUM TORQUE ACCELERATION/DECELERATION........................ 676
20.5 HIGH-SPEED CYCLE MACHINING .......................................................... 689
21 AXIS CONTROL FUNCTIONS............................................................691
21.1 AXIS SYNCHRONOUS CONTROL........................................................... 692
21.1.1 Axis Configuration for Axis Synchronous Control..............................................693
21.1.2 Synchronous Error Compensation........................................................................696
21.1.3 Synchronous Establishment .................................................................................698
21.1.4 Automatic Setting for Grid Position Matching ....................................................701
21.1.5 Synchronous Error Check ....................................................................................702
21.1.6 Methods of Alarm Recovery by Synchronous Error Check.................................704
21.1.7 Axis Synchronous Control Torque Difference Alarm..........................................706
21.2 POLYGON TURNING (G50.2, G51.2)....................................................... 709
TABLE OF CONTENTS B-63944EN/03
c-8
21.3 SYNCHRONOUS, COMPOSITE AND SUPERIMPOSED CONTROL BY
PROGRAM COMMAND (G50.4, G51.4, G50.5, G51.5, G50.6, AND
G51.6)........................................................................................................ 715
21.4 ROTARY AXIS ROLL-OVER..................................................................... 719
21.4.1 Rotary Axis Roll-over ..........................................................................................719
21.4.2 Rotary Axis Control .............................................................................................720
21.5 ARBITRARY ANGULAR AXIS CONTROL ................................................ 721
21.6 TOOL RETRACT AND RECOVER............................................................ 732
21.7 ELECTRONIC GEAR BOX........................................................................ 736
21.7.1 Electronic Gear Box .............................................................................................736
21.7.2 Electronic Gear Box Automatic Phase Synchronization......................................746
21.7.3 Skip Function for EGB Axis ................................................................................751
21.7.4 Electronic Gear Box 2 Pair...................................................................................753
21.7.4.1 Specification method (G80.5, G81.5) ........................................................ 753
21.7.4.2 Description of commands compatible with those for a hobbing machine
(G80, G81) ................................................................................................. 756
21.7.4.3 Controlled axis configuration example ...................................................... 761
21.7.4.4 Sample programs........................................................................................ 762
21.7.4.5 Synchronization ratio specification range .................................................. 766
21.7.4.6 Retract function.......................................................................................... 770
21.8 TANDEM CONTROL ................................................................................. 771
22 5-AXIS MACHINING FUNCTION ........................................................ 772
22.1 TOOL CENTER POINT CONTROL........................................................... 773
22.2 TOOL POSTURE CONTROL .................................................................... 828
22.3 TILTED WORKING PLANE COMMAND ................................................... 838
22.3.1 Tilted Working Plane Command..........................................................................838
22.3.2 Tilted Working Plane Command by Tool Axis Direction....................................862
22.3.3 Tilted Working Plane command with Guidance ..................................................870
22.3.3.1 Tilted working plane command based on roll-pitch-yaw........................... 871
22.3.3.2 Tilted working plane command based on three points............................... 875
22.3.3.3 Tilted working plane command based on two vectors............................... 879
22.3.3.4 Tilted working plane command based on projection angles ...................... 882
22.3.3.5 Absolute multiple command ...................................................................... 885
22.3.3.6 Incremental multiple command.................................................................. 888
22.4 INCLINED ROTARY AXIS CONTROL ...................................................... 894
22.5 3-DIMENSIONAL CUTTER COMPENSATION ......................................... 897
22.5.1 Cutter Compensation in Tool Rotation Type Machine ........................................900
22.5.1.1 Tool side offset........................................................................................... 901
22.5.1.2 Leading edge offset.................................................................................... 921
B-63944EN/03 TABLE OF CONTENTS
c-9
22.5.1.3 Tool tip position (cutting point) command ................................................ 927
22.5.2 Cutter Compensation in Table Rotation Type Machine.......................................931
22.5.3 Cutter Compensation in Composite Type Machine .............................................939
22.5.4 Interference Check and Interference Avoidance ..................................................946
22.5.5 Restrictions...........................................................................................................950
22.5.5.1 Restrictions common to machine configurations ....................................... 950
22.5.5.2 Restriction on tool rotation type................................................................. 953
22.5.5.3 Restriction on machine configurations having table rotation axes
(table rotation type and composite type).................................................... 954
22.5.6 Examples ..............................................................................................................958
23 MUITI-PATH CONTROL FUNCTION..................................................963
23.1 OVERVIEW ............................................................................................... 964
23.2 WAITING FUNCTION FOR PATHS .......................................................... 966
23.3 COMMON MEMORY BETWEEN EACH PATH......................................... 972
23.4 SPINDLE CONTROL BETWEEN EACH PATH......................................... 974
23.5 SYNCHRONOUS/COMPOSITE/SUPERIMPOSED CONTROL................ 975
III. OPERATION
1 GENERAL ...........................................................................................981
1.1 MANUAL OPERATION.............................................................................. 982
1.2 TOOL MOVEMENT BY PROGRAMING - AUTOMATIC OPERATION ..... 984
1.3 AUTOMATIC OPERATION ....................................................................... 986
1.4 TESTING A PROGRAM ............................................................................ 988
1.4.1 Check by Running the Machine ...........................................................................988
1.4.2 How to View the Position Display Change without Running the Machine .........989
1.5 EDITING A PROGRAM ............................................................................. 990
1.6 DISPLAYING AND SETTING DATA.......................................................... 991
1.7 DISPLAY ................................................................................................... 994
1.7.1 Program Display...................................................................................................994
1.7.2 Current Position Display ......................................................................................995
1.7.3 Alarm Display ......................................................................................................996
1.7.4 Parts Count Display, Run Time Display ..............................................................996
1.8 ADJUSTMENT OF THE BRIGHTNESS OF THE MONOCHROME LCD .. 997
2 OPERATIONAL DEVICES..................................................................998
2.1 SETTING AND DISPLAY UNITS............................................................... 999
2.1.1 7.2" LCD CNC Display Panel............................................................................1000
2.1.2 8.4" LCD CNC Display Panel............................................................................1000
TABLE OF CONTENTS B-63944EN/03
c-10
2.1.3 10.4" LCD CNC Display Panel..........................................................................1001
2.1.4 12.1" LCD CNC Display Panel..........................................................................1001
2.1.5 15" LCD CNC Display Panel.............................................................................1002
2.1.6 Standard MDI Unit (ONG Key) .........................................................................1003
2.1.7 Standard MDI Unit (QWERTY Key).................................................................1004
2.1.8 Small MDI Unit (ONG Key)..............................................................................1005
2.2 OPERATIONAL DEVICES....................................................................... 1006
2.3 FUNCTION KEYS AND SOFT KEYS ...................................................... 1009
2.3.1 General Screen Operations .................................................................................1010
2.3.2 Function Keys ....................................................................................................1012
2.3.3 Soft Keys ............................................................................................................1013
2.3.4 Key Input and Input Buffer ................................................................................1023
2.3.5 Warning Messages .............................................................................................1024
2.4 EXTERNAL I/O DEVICES ....................................................................... 1025
2.5 POWER ON/OFF..................................................................................... 1027
2.5.1 Turning on the Power .........................................................................................1027
2.5.2 Power Disconnection..........................................................................................1028
3 MANUAL OPERATION.....................................................................1029
3.1 MANUAL REFERENCE POSITION RETURN......................................... 1030
3.2 JOG FEED (JOG).................................................................................... 1032
3.3 INCREMENTAL FEED ............................................................................ 1034
3.4 MANUAL HANDLE FEED........................................................................ 1036
3.5 MANUAL ABSOLUTE ON AND OFF....................................................... 1040
3.6 MANUAL LINEAR/CIRCULAR INTERPOLATION................................... 1046
3.7 RIGID TAPPING BY MANUAL HANDLE................................................. 1052
3.8 MANUAL NUMERICAL COMMAND........................................................ 1055
3.9 THREE-DIMENSIONAL MANUAL FEED ................................................ 1064
3.9.1 Tool Axis Direction Handle Feed / Tool Axis Direction JOG Feed /
Tool Axis Direction Incremental Feed ...............................................................1065
3.9.2 Tool Axis Right-Angle Direction Handle Feed / Tool Axis Right-Angle
Direction JOG Feed / Tool Axis Right-Angle Direction Incremental Feed.......1067
3.9.3 Tool Tip Center Rotation Handle Feed / Tool Tip Center Rotation JOG Feed /
Tool Tip Center Rotation Incremental Feed.......................................................1071
3.9.4 Table Vertical Direction Handle Feed / Table Vertical Direction JOG Feed /
Table Vertical Direction Incremental Feed ........................................................1074
3.9.5 Table Horizontal Direction Handle Feed / Table Horizontal Direction JOG
Feed / Table Horizontal Direction Incremental Feed .........................................1076
B-63944EN/03 TABLE OF CONTENTS
c-11
3.10 DISTANCE CODED LINEAR SCALE INTERFACE................................. 1080
3.10.1 Procedure for Reference Position Establishment ...............................................1080
3.10.2 Reference Position Return..................................................................................1082
3.10.3 Distance Coded Rotary Encoder ........................................................................1082
3.10.4 Axis Synchronization Control ............................................................................1083
3.10.5 Axis Control by PMC.........................................................................................1084
3.10.6 Angular Axis Control .........................................................................................1085
3.10.7 Note ....................................................................................................................1085
3.11 LINEAR SCALE WITH DISTANCE-CODED REFERENCE MARKS
(SERIAL) ................................................................................................. 1087
3.12 MANUAL HANDLE RETRACE ................................................................ 1093
3.13 AUXILIARY FUNCTION OUTPUT BLOCK REVERSE MOVEMENT
FOR MANUAL HANDLE RETRACE........................................................ 1108
4 AUTOMATIC OPERATION ............................................................... 1110
4.1 MEMORY OPERATION .......................................................................... 1111
4.2 MDI OPERATION .................................................................................... 1114
4.3 DNC OPERATION................................................................................... 1118
4.4 SCHEDULE OPERATION ....................................................................... 1121
4.5 EXTERNAL SUBPROGRAM CALL (M198)............................................. 1124
4.6 MANUAL HANDLE INTERRUPTION ...................................................... 1127
4.7 MIRROR IMAGE...................................................................................... 1134
4.8 PROGRAM RESTART ............................................................................ 1136
4.9 TOOL RETRACT AND RECOVER.......................................................... 1149
4.9.1 Retract ................................................................................................................1153
4.9.2 Withdrawal .........................................................................................................1154
4.9.3 Return .................................................................................................................1154
4.9.4 Repositioning .....................................................................................................1155
4.9.5 Tool Retract and Recover for Threading............................................................1156
4.9.6 Operation Procedure for a Canned Cycle for Drilling........................................1159
4.10 RETRACE................................................................................................ 1161
4.11 ACTIVE BLOCK CANCEL FUNCTION.................................................... 1172
5 TEST OPERATION ...........................................................................1177
5.1 MACHINE LOCK AND AUXILIARY FUNCTION LOCK ........................... 1178
5.2 FEEDRATE OVERRIDE.......................................................................... 1180
5.3 RAPID TRAVERSE OVERRIDE.............................................................. 1181
5.4 DWELL/AUXILIARY FUNCTION TIME OVERRIDE ................................ 1182
TABLE OF CONTENTS B-63944EN/03
c-12
5.5 DRY RUN ................................................................................................ 1184
5.6 SINGLE BLOCK ...................................................................................... 1185
5.7 HIGH SPEED PROGRAM CHECK FUNCTION ...................................... 1187
6 SAFETY FUNCTIONS.......................................................................1190
6.1 EMERGENCY STOP............................................................................... 1191
6.2 OVERTRAVEL......................................................................................... 1192
6.3 STORED STROKE CHECK..................................................................... 1193
6.4 STROKE LIMIT CHECK BEFORE MOVE ............................................... 1198
6.5 WRONG OPERATION PREVENTION FUNCTIONS .............................. 1201
6.5.1 Functions that are Used When Data is Set .........................................................1202
6.5.1.1 Input data range check ............................................................................. 1203
6.5.1.2 Confirmation of incremental input........................................................... 1205
6.5.1.3 Prohibition of the absolute input by the soft key ..................................... 1206
6.5.1.4 Confirmation of the deletion of the program ........................................... 1207
6.5.1.5 Confirmation of the deletion of all data ................................................... 1208
6.5.1.6 Confirmation of a data update during the data setting process ................ 1209
6.5.2 Functions that are Used when the Program is Executed ....................................1210
6.5.2.1 Display of updated modal information..................................................... 1210
6.5.2.2 Start check signal ..................................................................................... 1211
6.5.2.3 Axis status display ................................................................................... 1212
6.5.2.4 Confirmation of the start from a middle block......................................... 1213
6.5.2.5 Data range check...................................................................................... 1214
6.5.2.6 Maximum incremental value check ......................................................... 1215
6.5.3 Setting Screen.....................................................................................................1216
6.5.3.1 Operation confirmation function setting screen....................................... 1217
6.5.3.2 Tool offset range setting screen ............................................................... 1219
6.5.3.3 Workpiece origin offset range setting screen........................................... 1224
6.5.3.4 Y-axis tool offset range setting screen ..................................................... 1226
6.5.3.5 Workpiece shift range setting screen ....................................................... 1228
7 ALARM AND SELF-DIAGNOSIS FUNCTIONS................................1230
7.1 ALARM DISPLAY .................................................................................... 1231
7.2 ALARM HISTORY DISPLAY ................................................................... 1233
7.3 CHECKING BY DIAGNOSTIC DISPLAY................................................. 1234
7.4 RETURN FROM THE ALARM SCREEN................................................. 1235
7.4.1 Return from the Alarm Screen ...........................................................................1235
7.4.2 Relationship with Other Functions.....................................................................1237
8 DATA INPUT/OUTPUT .....................................................................1239
8.1 OVERWRITING FILES ON A MEMORY CARD ...................................... 1241
8.2 INPUT/OUTPUT ON EACH SCREEN ..................................................... 1244
B-63944EN/03 TABLE OF CONTENTS
c-13
8.2.1 Inputting and Outputting a Program...................................................................1246
8.2.1.1 Inputting a program.................................................................................. 1246
8.2.1.2 Outputting a program............................................................................... 1248
8.2.2 Inputting and Outputting Parameters..................................................................1250
8.2.2.1 Inputting parameters ................................................................................ 1250
8.2.2.2 Outputting parameters.............................................................................. 1252
8.2.3 Inputting and Outputting Offset Data.................................................................1254
8.2.3.1 Inputting offset data ................................................................................. 1254
8.2.3.2 Outputting offset data............................................................................... 1256
8.2.4 Inputting and Outputting Pitch Error Compensation Data .................................1261
8.2.4.1 Inputting pitch error compensation data .................................................. 1261
8.2.4.2 Outputting pitch error compensation data................................................ 1263
8.2.4.3 Input/output format of pitch error compensation data ............................. 1264
8.2.5 Inputting and Outputting Three-dimensional Error Compensation Data ...........1265
8.2.5.1 Inputting three-dimensional error compensation data.............................. 1265
8.2.5.2 Outputting three-dimensional error compensation data ........................... 1267
8.2.5.3 Input/output format of three-dimensional error compensation data......... 1268
8.2.6 Inputting and Outputting Custom Macro Common Variables ...........................1270
8.2.6.1 Inputting custom macro common variables ............................................. 1270
8.2.6.2 Outputting custom macro common variables........................................... 1272
8.2.7 Inputting and Outputting Workpiece Coordinates System Data ........................1274
8.2.7.1 Inputting workpiece coordinate system data............................................ 1274
8.2.7.2 Outputting workpiece coordinate system data ......................................... 1276
8.2.8 Inputting and Outputting Operation History Data..............................................1277
8.2.8.1 Outputting operation history data............................................................. 1277
8.2.9 Inputting and Outputting Tool Management Data .............................................1279
8.2.9.1 Inputting tool management data............................................................... 1279
8.2.9.2 Outputting tool management data ............................................................ 1281
8.2.9.3 Inputting magazine data ........................................................................... 1282
8.2.9.4 Outputting magazine data ........................................................................ 1284
8.2.9.5 Inputting tool life status name data .......................................................... 1285
8.2.9.6 Outputting tool life status name data........................................................ 1287
8.2.9.7 Inputting name data of customize data..................................................... 1288
8.2.9.8 Outputting name data of customize data .................................................. 1290
8.2.9.9 Inputting customize data displayed as tool management data.................. 1291
8.2.9.10 Outputting customize data displayed as tool management data............... 1293
8.2.9.11 Inputting spindle waiting position name data .......................................... 1294
8.2.9.12 Outputting spindle waiting position name data........................................ 1296
8.2.9.13 Inputting decimal point position data of customize data.......................... 1297
8.2.9.14 Outputting decimal point position data of customize data ....................... 1299
8.2.9.15 Inputting tool geometry data .................................................................... 1300
8.2.9.16 Outputting tool geometry data ................................................................. 1302
TABLE OF CONTENTS B-63944EN/03
c-14
8.3 INPUT/OUTPUT ON THE ALL IO SCREEN............................................ 1303
8.3.1 Inputting/Outputting a Program .........................................................................1304
8.3.2 Inputting and Outputting Parameters..................................................................1308
8.3.3 Inputting and Outputting Offset Data.................................................................1311
8.3.4 Inputting/Outputting Pitch Error Compensation Data........................................1313
8.3.5 Inputting/Outputting Custom Macro Common Variables ..................................1316
8.3.6 Inputting and Outputting Workpiece Coordinates System Data ........................1318
8.3.7 Inputting and Outputting Operation History Data..............................................1320
8.3.8 Inputting and Outputting Tool Management Data .............................................1321
8.3.9 File Format and Error Messages.........................................................................1329
8.4 EMBEDDED ETHERNET OPERATIONS................................................ 1330
8.4.1 FTP File Transfer Function ................................................................................1330
8.5 SCREEN HARD COPY FUNCTION ........................................................ 1339
9 CREATING PROGRAMS..................................................................1341
9.1 CREATING PROGRAMS USING THE MDI PANEL................................ 1342
9.2 AUTOMATIC INSERTION OF SEQUENCE NUMBERS ......................... 1343
9.3 CREATING PROGRAMS IN TEACH IN MODE (PLAYBACK) ................ 1345
10 EDITING PROGRAMS ......................................................................1348
10.1 EDIT DISABLE ATTRIBUTE.................................................................... 1349
10.2 INSERTING, ALTERING AND DELETING A WORD .............................. 1350
10.2.1 Word Search .......................................................................................................1351
10.2.2 Heading a Program.............................................................................................1353
10.2.3 Inserting a Word.................................................................................................1354
10.2.4 Altering a Word..................................................................................................1355
10.2.5 Deleting a Word .................................................................................................1356
10.3 DELETING BLOCKS ............................................................................... 1357
10.3.1 Deleting a Block.................................................................................................1357
10.3.2 Deleting Multiple Blocks ...................................................................................1358
10.4 PROGRAM SEARCH .............................................................................. 1359
10.5 SEQUENCE NUMBER SEARCH ............................................................ 1361
10.6 DELETING PROGRAMS......................................................................... 1363
10.6.1 Deleting One Program........................................................................................1363
10.6.2 Deleting All Programs........................................................................................1363
10.7 EDITING OF CUSTOM MACROS ........................................................... 1364
10.8 CURSOR MOVEMENT LIMITATIONS ON PROGRAM EDITING........... 1365
10.9 PASSWORD FUNCTION ........................................................................ 1367
B-63944EN/03 TABLE OF CONTENTS
c-15
10.10 EDITING PROGRAM CHARACTERS ..................................................... 1370
10.10.1 Available Keys ...................................................................................................1374
10.10.2 Input Mode .........................................................................................................1374
10.10.3 Line Number Display .........................................................................................1375
10.10.4 Search .................................................................................................................1375
10.10.5 Replacement .......................................................................................................1376
10.10.6 Reversing Edit Operations (Undo Function)......................................................1377
10.10.7 Copy ...................................................................................................................1377
10.10.8 Cut ......................................................................................................................1377
10.10.9 Paste ...................................................................................................................1378
10.10.10 Saving.................................................................................................................1378
10.10.11 Creation ..............................................................................................................1378
10.10.12 Line Search.........................................................................................................1379
10.11 PROGRAM COPY FUNCTION................................................................ 1380
10.11.1 Copying and Moving Files between Devices.....................................................1382
10.12 KEYS AND PROGRAM ENCRYPTION................................................... 1386
10.13 SIMULTANEOUS EDITING OF MULTIPATH PROGRAMS.................... 1391
11 PROGRAM MANAGEMENT ............................................................. 1395
11.1 SELECTING A DEVICE........................................................................... 1396
11.1.1 Selecting a Memory Card Program as a Device.................................................1397
11.2 CREATING A FOLDER ........................................................................... 1402
11.3 RENAMING A FOLDER .......................................................................... 1403
11.4 CHANGING FOLDER ATTRIBUTES....................................................... 1404
11.5 DELETING A FOLDER............................................................................ 1405
11.6 SELECTING A DEFAULT FOLDER ........................................................ 1406
11.7 RENAMING A FILE ................................................................................. 1407
11.8 DELETING A FILE................................................................................... 1408
11.9 CHANGING FILE ATTRIBUTES.............................................................. 1409
11.10 SELECTING A MAIN PROGRAM............................................................ 1410
11.11 MAKING A PROGRAM COMPACT......................................................... 1411
11.12 PROGRAM COPY FUNCTION................................................................ 1412
12 SETTING AND DISPLAYING DATA.................................................1414
12.1 SCREENS DISPLAYED BY FUNCTION KEY ................................. 1429
12.1.1 Position Display in the Workpiece Coordinate System .....................................1431
12.1.2 Position Display in the Relative Coordinate System..........................................1433
12.1.3 Overall Position Display ....................................................................................1436
TABLE OF CONTENTS B-63944EN/03
c-16
12.1.4 Workpiece Coordinate System Preset ................................................................1438
12.1.5 Actual Feedrate Display .....................................................................................1439
12.1.6 Display of Run Time and Parts Count................................................................1441
12.1.7 Setting the Floating Reference Position .............................................................1443
12.1.8 Operating Monitor Display ................................................................................1444
12.1.9 Display of Three-dimensional Manual Feed (Tool Tip Coordinates, Number
of Pulses, Machine Axis Move Amount) ...........................................................1447
12.1.10 Overall Position Display (15-inch Display Unit) ...............................................1451
12.1.11 Workpiece Coordinate System Preset (15-inch Display Unit)...........................1454
12.1.12 Actual Feedrate Display (15-inch Display Unit)................................................1455
12.1.13 Display of Run Time and Parts Count (15-inch Display Unit) ..........................1457
12.1.14 Setting the Floating Reference Position (15-inch Display Unit)........................1459
12.1.15 Operating Monitor Display (15-inch Display Unit) ...........................................1460
12.1.16 Display of Three-dimensional Manual Feed (Tool Tip Coordinates, Number
of Pulses, Machine Axis Move Amount) (15-inch Display Unit)......................1463
12.2 SCREENS DISPLAYED BY FUNCTION KEY ................................. 1466
12.2.1 Program Contents Display..................................................................................1467
12.2.1.1 Displaying the executed block ................................................................. 1468
12.2.2 Editing a Program...............................................................................................1470
12.2.3 Program Screen for MDI Operation ...................................................................1472
12.2.4 Program Folder Screen.......................................................................................1473
12.2.4.1 Split display on the program folder screen............................................... 1474
12.2.5 Next Block Display Screen ................................................................................1481
12.2.6 Program Check Screen .......................................................................................1482
12.2.7 Background Editing............................................................................................1483
12.2.8 Stamping the Machining Time ...........................................................................1489
12.2.9 Screen for Assistance in Entering Tilted Working Plane Command .................1499
12.2.9.1 Command type selection screen............................................................... 1506
12.2.9.2 Tilted working plane data setting screen.................................................. 1507
12.2.9.3 Details of the tilted working plane data setting screen............................. 1512
12.2.9.4 Limitation................................................................................................. 1519
12.2.10 Program Contents Display (15-inch Display Unit) ............................................1521
12.2.10.1 Displaying the executed block ................................................................. 1521
12.2.11 Editing a Program (15-inch Display Unit) .........................................................1522
12.2.12 Program Screen for MDI Operation (15-inch Display Unit)..............................1524
12.2.13 Program Folder Screen (15-inch Display Unit)..................................................1525
12.2.13.1 Split display on the program folder screen............................................... 1526
12.2.14 Next Block Display Screen (15-inch Display Unit) ...........................................1532
B-63944EN/03 TABLE OF CONTENTS
c-17
12.2.15 Program Check Screen (15-inch Display Unit)..................................................1533
12.2.16 Background Editing (15-inch Display Unit) ......................................................1534
12.2.17 Stamping the Machining Time (15-inch Display Unit)......................................1540
12.2.18 Screen for Assistance in Entering Tilted Working Plane Command
(15-inch Display Unit)........................................................................................1550
12.2.18.1 Command type selection screen............................................................... 1557
12.2.18.2 Tilted working plane data setting screen.................................................. 1558
12.2.18.3 Details of the tilted working plane data setting screen............................. 1563
12.2.18.4 Limitation................................................................................................. 1570
12.3 SCREENS DISPLAYED BY FUNCTION KEY ................................. 1571
12.3.1 Displaying and Entering Setting Data ................................................................1573
12.3.2 Sequence Number Comparison and Stop ...........................................................1576
12.3.3 Displaying and Setting Run Time, Parts Count, and Time ................................1578
12.3.4 Displaying and Setting the Workpiece Origin Offset Value ..............................1581
12.3.5 Direct Input of Workpiece Origin Offset Value Measured ................................1582
12.3.6 Displaying and Setting Custom Macro Common Variables...............................1584
12.3.7 Displaying and Setting Real Time Custom Macro Data ....................................1586
12.3.8 Displaying and Setting the Software Operator’s Panel ......................................1588
12.3.9 Setting and Displaying Tool Management Data ................................................1591
12.3.9.1 Displaying and setting magazine screen .................................................. 1591
12.3.9.2 Displaying and setting tool management screen ...................................... 1593
12.3.9.3 Each tool data screen................................................................................ 1599
12.3.9.4 Displaying the total life of tools of the same type.................................... 1602
12.3.9.5 Tool geometry data screen ....................................................................... 1607
12.3.10 Displaying and Switching the Display Language ..............................................1612
12.3.11 Protection of Data at Eight Levels......................................................................1614
12.3.11.1 Operation level setting ............................................................................. 1614
12.3.11.2 Password modification............................................................................. 1616
12.3.11.3 Protection level setting............................................................................. 1618
12.3.11.4 Setting the change protection level and output protection level of
a program ................................................................................................. 1621
12.3.12 Precision Level Selection ...................................................................................1623
12.3.13 Displaying and Setting Tool Life Management Data.........................................1625
12.3.13.1 Tool life management (list screen)........................................................... 1627
12.3.13.2 Tool life management (group editing screen) .......................................... 1632
12.3.14 Displaying and Setting Workpiece Setting Error Compensation Data...............1640
12.3.15 Displaying and Setting Pattern Data Inputs........................................................1642
12.3.16 Displaying and Entering Setting Data (15-inch Display Unit)...........................1645
12.3.17 Sequence Number Comparison and Stop (15-inch Display Unit)......................1648
TABLE OF CONTENTS B-63944EN/03
c-18
12.3.18 Displaying and Setting Run Time, Parts Count, and Time
(15-inch Display Unit)........................................................................................1650
12.3.19 Displaying and Setting the Workpiece Origin Offset Value
(15-inch Display Unit)........................................................................................1653
12.3.20 Direct Input of Workpiece Origin Offset Value Measured
(15-inch Display Unit)........................................................................................1655
12.3.21 Displaying and Setting Custom Macro Common Variables
(15-inch Display Unit)........................................................................................1657
12.3.22 Displaying and Setting Real Time Custom Macro Data (15-inch Display Unit)1659
12.3.23 Displaying and Setting the Software Operator’s Panel (15-inch Display Unit).1662
12.3.24 Setting and Displaying Tool Management Data (15-inch Display Unit) ...........1665
12.3.24.1 Displaying and setting magazine screen (15-inch display unit)............... 1665
12.3.24.2 Displaying and setting tool management screen (15-inch display unit)... 1667
12.3.24.3 Each tool data screen (15-inch display unit) ............................................ 1674
12.3.24.4 Displaying the total life of tools of the same type (15-inch display unit) 1677
12.3.24.5 Tool geometry data screen (15-inch display unit).................................... 1683
12.3.25 Displaying and Switching the Display Language (15-inch Display Unit) .........1688
12.3.26 Protection of Data at Eight Levels (15-inch Display Unit) ................................1690
12.3.26.1 Operation level setting (15-inch display unit).......................................... 1690
12.3.26.2 Password modification (15-inch display unit) ......................................... 1692
12.3.26.3 Protection level setting (15-inch display unit) ......................................... 1694
12.3.26.4 Setting the change protection level and output protection level of
a program (15-inch display unit).............................................................. 1697
12.3.27 Precision Level Selection (15-inch Display Unit)..............................................1699
12.3.28 Displaying and Setting Tool Life Management Data (15-inch Display Unit)....1701
12.3.28.1 Tool life management (list screen) (15-inch display unit) ....................... 1703
12.3.28.2 Tool life management (group editing screen) (15-inch display unit)....... 1708
12.3.29 Displaying and Setting Workpiece Setting Error Compensation Data
(15-inch Display Unit)........................................................................................1716
12.3.30 Displaying and Setting Pattern Data Inputs (15-inch Display Unit) .................1718
12.4 SCREENS DISPLAYED BY FUNCTION KEY ................................. 1721
12.4.1 Displaying and Setting Parameters.....................................................................1723
12.4.2 Displaying and Setting Pitch Error Compensation Data ....................................1726
12.4.3 Displaying and Setting Three-Dimensional Error Compensation Data .............1729
12.4.4 Servo Parameters................................................................................................1733
12.4.5 Servo Tuning ......................................................................................................1734
12.4.6 Spindle Setting ...................................................................................................1735
12.4.7 Spindle Tuning ...................................................................................................1736
12.4.8 Spindle Monitor..................................................................................................1737
B-63944EN/03 TABLE OF CONTENTS
c-19
12.4.9 Color Setting Screen...........................................................................................1738
12.4.10 Machining Parameter Tuning.............................................................................1741
12.4.11 Displaying Memory Data ...................................................................................1749
12.4.12 Parameter Tuning Screen ...................................................................................1751
12.4.12.1 Displaying the menu screen and selecting a menu item........................... 1751
12.4.12.2 Parameter tuning screen (system setting)................................................. 1755
12.4.12.3 Parameter tuning screen (axis setting) ..................................................... 1757
12.4.12.4 Displaying and setting the FSSB amplifier setting screen ....................... 1758
12.4.12.5 Displaying and setting the FSSB axis setting screen ............................... 1759
12.4.12.6 Displaying and setting the servo setting screen ....................................... 1759
12.4.12.7 Parameter tuning screen (spindle setting) ................................................ 1760
12.4.12.8 Parameter tuning screen (miscellaneous settings).................................... 1761
12.4.12.9 Displaying and setting the servo tuning screen........................................ 1762
12.4.12.10 Displaying and setting the spindle tuning screen..................................... 1762
12.4.12.11 Displaying and setting the machining parameter tuning screen............... 1763
12.4.13 Periodic Maintenance Screen .............................................................................1768
12.4.14 System Configuration Screen.............................................................................1776
12.4.15 Overview of the History Function......................................................................1779
12.4.15.1 Alarm history ........................................................................................... 1781
12.4.15.2 External operator message history ........................................................... 1784
12.4.15.3 Operation history...................................................................................... 1786
12.4.15.4 Selecting operation history signals........................................................... 1796
12.4.15.5 Outputting all history data........................................................................ 1798
12.4.16 Displaying and Setting Parameters (15-inch Display Unit) ...............................1802
12.4.17 Displaying and Setting Pitch Error Compensation Data (15-inch Display Unit)1805
12.4.18 Displaying and Setting Three-Dimensional Error Compensation Data
(15-inch Display Unit)........................................................................................1808
12.4.19 Servo Parameters (15-inch Display Unit)...........................................................1812
12.4.20 Servo Tuning (15-inch Display Unit).................................................................1813
12.4.21 Spindle Setting (15-inch Display Unit) ..............................................................1814
12.4.22 Spindle Tuning (15-inch Display Unit)..............................................................1815
12.4.23 Spindle Monitor (15-inch Display Unit) ............................................................1816
12.4.24 Color Setting Screen (15-inch Display Unit) .....................................................1817
12.4.25 Machining Parameter Tuning (15-inch Display Unit)........................................1820
12.4.26 Displaying Memory Data (15-inch Display Unit)..............................................1828
12.4.27 Parameter Tuning Screen (15-inch Display Unit) ..............................................1830
12.4.27.1 Displaying the menu screen and selecting a menu item
(15-inch Display Unit) ............................................................................. 1830
12.4.27.2 Parameter tuning screen (system setting) (15-inch Display Unit)............ 1834
12.4.27.3 Parameter tuning screen (axis setting) (15-inch Display Unit) ................ 1836
TABLE OF CONTENTS B-63944EN/03
c-20
12.4.27.4 Displaying and setting the FSSB amplifier setting screen
(15-inch Display Unit) ............................................................................. 1837
12.4.27.5 Displaying and setting the FSSB axis setting screen
(15-inch Display Unit) ............................................................................. 1838
12.4.27.6 Displaying and setting the servo setting screen (15-inch Display Unit) .. 1839
12.4.27.7 Parameter tuning screen (spindle setting) (15-inch Display Unit)........... 1840
12.4.27.8 Parameter tuning screen (miscellaneous settings) (15-inch Display Unit)1841
12.4.27.9 Displaying and setting the servo tuning screen (15-inch Display Unit)... 1842
12.4.27.10 Displaying and setting the spindle tuning screen (15-inch Display Unit) 1842
12.4.27.11 Displaying and setting the machining parameter tuning screen
(15-inch Display Unit) ............................................................................. 1843
12.4.28 Periodic Maintenance Screen (15-inch Display Unit)........................................1847
12.4.29 System Configuration Screen (15-inch Display Unit)........................................1855
12.4.30 Overview of the History Function (15-inch Display Unit) ................................1858
12.4.30.1 Alarm history ........................................................................................... 1860
12.4.30.2 External operator message history ........................................................... 1863
12.4.30.3 Operation history...................................................................................... 1865
12.4.30.4 Selecting operation history signals........................................................... 1875
12.4.30.5 Outputting all history data........................................................................ 1877
12.5 SCREENS DISPLAYED BY FUNCTION KEY ................................. 1881
12.6 DISPLAYING THE PROGRAM NUMBER/NAME, SEQUENCE NUMBER,
AND STATUS, AND WARNING MESSAGES FOR DATA SETTING OR
INPUT/OUTPUT OPERATION ................................................................ 1882
12.6.1 Displaying the Program Number, Program Name, and Sequence Number........1882
12.6.2 Displaying the Status and Warning for Data Setting or Input/Output
Operation............................................................................................................1883
12.6.3 Displaying the Program Number, Program Name, and Sequence Number
(15-inch Display Unit)........................................................................................1887
12.6.4 Displaying the Status and Warning for Data Setting or Input/Output Operation
(15-inch Display Unit)........................................................................................1888
12.7 SCREEN ERASURE FUNCTION AND AUTOMATIC SCREEN
ERASURE FUNCTION............................................................................ 1892
12.8 LOAD METER SCREEN ......................................................................... 1894
12.8.1 Single-Path Display............................................................................................1894
12.8.2 Two-Path Display and Three-Path Display........................................................1896
13 GRAPHIC FUNCTION.......................................................................1899
13.1 GRAPHIC DISPLAY ................................................................................ 1900
13.2 DYNAMIC GRAPHIC DISPLAY............................................................... 1913
13.2.1 Path Drawing......................................................................................................1914
B-63944EN/03 TABLE OF CONTENTS
c-21
13.2.1.1 GRAPHIC PARAMETER (DYNAMIC GRAPHIC) screen................... 1915
13.2.1.2 PATH GRAPHIC screen ......................................................................... 1922
13.2.1.3 PATH GRAPHIC (TOOL POSITION) screen ........................................ 1930
13.2.2 Animation...........................................................................................................1933
13.2.2.1 GRAPHIC PARAMETER (DYNAMIC GRAPHIC) SCREEN.............. 1934
13.2.2.2 ANIMATION GRAPHIC screen............................................................. 1939
13.2.3 Programmable Data Input (G10) for Blank Figure Drawing Parameters...........1946
13.2.4 Warning Messages .............................................................................................1948
13.2.5 Note ....................................................................................................................1948
13.2.6 Restrictions.........................................................................................................1949
14 VIRTUAL MDI KEY FUNCTION........................................................1956
14.1 VIRTUAL MDI KEY.................................................................................. 1957
14.1.1 Limitations..........................................................................................................1960
IV. MAINTENANCE
1 ROUTINE MAINTENANCE ............................................................... 1963
1.1 ACTION TO BE TAKEN WHEN A PROBLEM OCCURRED ................... 1964
1.2 BACKING UP VARIOUS DATA ITEMS ................................................... 1965
1.3 METHOD OF REPLACING BATTERY .................................................... 1967
1.3.1 Replacing Battery for LCD-mounted Type CNC Control Unit .........................1968
1.3.2 Replacing the Battery for Stand-alone Type CNC Control Unit........................1971
1.3.3 Battery in the PANEL i (3 VDC) .......................................................................1973
1.3.4 Battery for Absolute Pulsecoders .......................................................................1975
APPENDIX
A PARAMETERS.................................................................................. 1983
A.1 DESCRIPTION OF PARAMETERS......................................................... 1984
A.2 DATA TYPE............................................................................................. 2280
A.3 STANDARD PARAMETER SETTING TABLES....................................... 2281
B PROGRAM CODE LIST....................................................................2283
C LIST OF FUNCTIONS AND PROGRAM FORMAT ..........................2286
D RANGE OF COMMAND VALUE.......................................................2298
E NOMOGRAPHS ................................................................................ 2301
E.1 INCORRECT THREADED LENGTH ....................................................... 2302
E.2 SIMPLE CALCULATION OF INCORRECT THREAD LENGTH .............. 2304
E.3 TOOL PATH AT CORNER ...................................................................... 2306
TABLE OF CONTENTS B-63944EN/03
c-22
E.4 RADIUS DIRECTION ERROR AT CIRCLE CUTTING ............................ 2309
F SETTINGS AT POWER-ON, IN THE CLEAR STATE, OR IN
THE RESET STATE..........................................................................2310
G CHARACTER-TO-CODES CORRESPONDENCE TABLE ..............2313
G.1 CHARACTER-TO-CODES CORRESPONDENCE TABLE...................... 2314
G.2 FANUC DOUBLE-BYTE CHARACTER CODE TABLE ........................... 2315
H ALARM LIST .....................................................................................2321
I PC TOOL FOR MEMORY CARD PROGRAM
OPERATION/EDITING......................................................................2389
I.1 PC TOOL FOR MEMORY CARD PROGRAM OPERATION/EDITING ... 2390
I.1.1 Usage Notes........................................................................................................2390
I.1.2 List of Functions of PC Tool..............................................................................2390
I.1.3 Explanation Of Operations.................................................................................2391
I.2 NAMING RULES ..................................................................................... 2401
I.2.1 Naming Rules of Program File...........................................................................2401
I.2.2 Naming Rules Of Folder ....................................................................................2402
I.3 RULES OF CHARACTERS IN PROGRAM FILE..................................... 2403
I.3.1 Usable Characters in Program File.....................................................................2404
I.4 ERROR MESSAGE AND NOTE.............................................................. 2406
I.4.1 List of Error Message .........................................................................................2406
I.4.2 Note ....................................................................................................................2406
I. GENERAL
B-63944EN/03 GENERAL 1.GENERAL
- 3 -
1 GENERAL
This manual consists of the following parts:
About this manual
I. GENERAL
Describes chapter organization, applicable models, related
manuals, and notes for reading this manual.
II. PROGRAMMING
Describes each function: Format used to program functions in the
NC language, explanations, and limitations.
III. OPERATION
Describes the manual operation and automatic operation of a
machine, procedures for inputting and outputting data, and
procedures for editing a program.
IV. MAINTENANCE
Describes procedures for daily maintenance and replacing
batteries.
APPENDIX
Lists parameters, valid data ranges, and alarms.
NOTE
1 This manual describes the functions common to
the lathe system and machining center system.
For the functions specific to the lathe system or
machining center system, refer to the User's
Manual (Lathe System) (B-63944EN-1) or the
User's Manual (Machining Center System)
(B-63944EN-2).
2 Some functions described in this manual may not
be applied to some products. For detail, refer to the
Descriptions manual (B-63942EN).
3 This manual does not detail the parameters not
mentioned in the text. For details of those
parameters, refer to the Parameter Manual
(B-63950EN).
Parameters are used to set functions and operating
conditions of a CNC machine tool, and frequently-
used values in advance. Usually, the machine tool
builder factory-sets parameters so that the user
can use the machine tool easily.
4 This manual describes not only basic functions but
also optional functions. Look up the options
incorporated into your system in the manual written
by the machine tool builder.
1.GENERAL GENERAL B-63944EN/03
- 4 -
Applicable models
This manual describes the models indicated in the table below.
In the text, the abbreviations indicated below may be used.
Model name Abbreviation
FANUC Series 30i-MODEL A 30i –A Series 30i
FANUC Series 300i-MODEL A 300i–A Series 300i
FANUC Series 300is-MODEL A 300is–A Series 300is
FANUC Series 31i-MODEL A 31i –A
FANUC Series 31i-MODEL A5 31i –A5 Series 31i
FANUC Series 310i-MODEL A 310i–A
FANUC Series 310i-MODEL A5 310i–A5 Series 310i
FANUC Series 310is-MODEL A 310is–A
FANUC Series 310is-MODEL A5 310is–A5 Series 310is
FANUC Series 32i-MODEL A 32i –A Series 32i
FANUC Series 320i-MODEL A 320i–A Series 320i
FANUC Series 320is-MODEL A 320is–A Series 320is
NOTE
1 For an explanatory purpose, the following
descriptions may be used according to the types of
path control used:
- T series: For the lathe system
- M series: For the machining center system
2 Unless otherwise noted, the model names
31i/310i/310is-A, 31i/310i/310is-A5, and
32i/320i/320is-A are collectively referred to as
30i/300i/300is. However, this convention is not
necessarily observed when item 3 below is
applicable.
3 Some functions described in this manual may not
be applied to some products.
For details, refer to the Descriptions (B-63942EN).
B-63944EN/03 GENERAL 1.GENERAL
- 5 -
Special symbols
This manual uses the following symbols:
- M
Indicates a description that is valid only for the machine center system
set as system control type (in parameter No. 0983).
In a general description of the method of machining, a machining
center system operation is identified by a phase such as "for milling
machining".
- T
Indicates a description that is valid only for the lathe system set as
system control type (in parameter No. 0983).
In a general description of the method of machining, a lathe system
operation is identified by a phrase such as "for lathe cutting".
-
Indicates the end of a description of a system control type.
When a system control type mark mentioned above is not followed by
this mark, the description of the system control type is assumed to
continue until the next item or paragraph begins. In this case, the next
item or paragraph provides a description common to the control types.
- IP
Indicates a combination of axes such as X_ Y_ Z_
In the underlined position following each address, a numeric value
such as a coordinate value is placed (used in PROGRAMMING.).
- ;
Indicates the end of a block. It actually corresponds to the ISO code
LF or EIA code CR.
1.GENERAL GENERAL B-63944EN/03
- 6 -
Related manuals of
Series 30i/300i/300is- MODEL A
Series 31i/310i/310is- MODEL A
Series 32i/320i/320is- MODEL A
The following table lists the manuals related to Series 30i/300i /300is-
A, Series 31i/310i /310is-A, Series 32i/320i /320is-A. This manual is
indicated by an asterisk(*).
Table 1 Related manuals
Manual name Specification
number
DESCRIPTIONS B-63942EN
CONNECTION MANUAL (HARDWARE) B-63943EN
CONNECTION MANUAL (FUNCTION) B-63943EN-1
USER’S MANUAL
(Common to Lathe System/Machining Center System)
B-63944EN *
USER’S MANUAL (For Lathe System) B-63944EN-1
USER’S MANUAL (For Machining Center System) B-63944EN-2
MAINTENANCE MANUAL B-63945EN
PARAMETER MANUAL B-65950EN
Programming
Macro Compiler / Macro Executor PROGRAMMING
MANUAL
B-63943EN-2
Macro Compiler OPERATOR’S MANUAL B-66264EN
C Language Executor OPERATOR’S MANUAL B-63944EN-3
PMC
PMC PROGRAMMING MANUAL B-63983EN
Network
PROFIBUS-DP Board OPERATOR’S MANUAL B-63994EN
Fast Ethernet / Fast Data Server OPERATOR’S MANUAL B-64014EN
DeviceNet Board OPERATOR’S MANUAL B-64044EN
FL-net Board OPERATOR’S MANUAL B-64164EN
Operation guidance function
MANUAL GUIDE i
(Common to Lathe System/Machining Center System)
OPERATOR’S MANUAL
B-63874EN
MANUAL GUIDE i (For Machining Center System)
OPERATOR’S MANUAL
B-63874EN-2
MANUAL GUIDE i (Set-up Guidance Functions)
OPERATOR’S MANUAL
B-63874EN-1
B-63944EN/03 GENERAL 1.GENERAL
- 7 -
Related manuals of SERVO MOTOR αi/βi series
The following table lists the manuals related to SERVO MOTOR
αi/βi series
Table 2 Related manuals
Manual name Specification
number
FANUC AC SERVO MOTOR αi series
DESCRIPTIONS B-65262EN
FANUC AC SPINDLE MOTOR αi series
DESCRIPTIONS B-65272EN
FANUC AC SERVO MOTOR βi series
DESCRIPTIONS B-65302EN
FANUC AC SPINDLE MOTOR βi series
DESCRIPTIONS B-65312EN
FANUC SERVO AMPLIFIER αi series
DESCRIPTIONS B-65282EN
FANUC SERVO AMPLIFIER βi series
DESCRIPTIONS B-65322EN
FANUC SERVO MOTOR αis series
FANUC SERVO MOTOR αi series
FANUC AC SPINDLE MOTOR αi series
FANUC SERVO AMPLIFIER αi series
MAINTENANCE MANUAL
B-65285EN
FANUC SERVO MOTOR βis series
FANUC AC SPINDLE MOTOR βi series
FANUC SERVO AMPLIFIER βi series
MAINTENANCE MANUAL
B-65325EN
FANUC AC SERVO MOTOR αi series
FANUC AC SERVO MOTOR βi series
FANUC LINEAR MOTOR LiS series
FANUC SYNCHRONOUS BUILT-IN SERVO MOTOR DiS
series PARAMETER MANUAL
B-65270EN
FANUC AC SPINDLE MOTOR αi/βi series,
BUILT-IN SPINDLE MOTOR Bi series
PARAMETER MANUAL
B-65280EN
The above servo motors and the corresponding spindles can be
connected to the CNC covered in this manual. In the αi SV series,
they can be connected only to upgrade versions. In the βi SVSP series,
they cannot be connected.
This manual mainly assumes that the FANUC SERVO MOTOR αi
series of servo motor is used. For servo motor and spindle information,
refer to the manuals for the servo motor and spindle that are actually
connected.
1.GENERAL GENERAL B-63944EN/03
- 8 -
1.1 NOTES ON READING THIS MANUAL
CAUTION
1 The function of an CNC machine tool system
depends not only on the CNC, but on the
combination of the machine tool, its magnetic
cabinet, the servo system, the CNC, the operator's
panels, etc. It is too difficult to describe the function,
programming, and operation relating to all
combinations. This manual generally describes these
from the stand-point of the CNC. So, for details on a
particular CNC machine tool, refer to the manual
issued by the machine tool builder, which should take
precedence over this manual.
2 In the header field of each page of this manual, a
chapter title is indicated so that the reader can
reference necessary information easily.
By finding a desired title first, the reader can
reference necessary parts only.
3 This manual describes as many reasonable variations
in equipment usage as possible. It cannot address
every combination of features, options and commands
that should not be attempted.
If a particular combination of operations is not
described, it should not be attempted.
B-63944EN/03 GENERAL 1.GENERAL
- 9 -
1.2 NOTES ON VARIOUS KINDS OF DATA
CAUTION
Machining programs, parameters, offset data, etc.
are stored in the CNC unit internal non-volatile
memory. In general, these contents are not lost by
the switching ON/OFF of the power. However, it is
possible that a state can occur where precious data
stored in the non-volatile memory has to be deleted,
because of deletions from a maloperation, or by a
failure restoration. In order to restore rapidly when
this kind of mishap occurs, it is recommended that
you create a copy of the various kinds of data
beforehand.
II. PROGRAMMING
B-63944EN/03 PROGRAMMING 1.GENERAL
- 13 -
1 GENERAL
Chapter 1, "GENERAL", consists of the following sections:
1.1 TOOL MOVEMENT ALONG WORKPIECE PARTS FIGURE-
INTERPOLATION .....................................................................14
1.2 FEED-FEED FUNCTION ..........................................................16
1.3 PART DRAWING AND TOOL MOVEMENT.........................17
1.4 CUTTING SPEED - SPINDLE FUNCTION .............................27
1.5 SELECTION OF TOOL USED FOR VARIOUS MACHINING -
TOOL FUNCTION.....................................................................28
1.6 COMMAND FOR MACHINE OPERATIONS - AUXILIARY
FUNCTION ................................................................................29
1.7 PROGRAM CONFIGURATION ...............................................30
1.8 TOOL MOVEMENT RANGE - STROKE ................................33
1.GENERAL PROGRAMMING B-63944EN/03
- 14 -
1.1 TOOL MOVEMENT ALONG WORKPIECE PARTS FIGURE-
INTERPOLATION
The tool moves along straight lines and arcs constituting the
workpiece parts figure (See II-4).
Explanation
The function of moving the tool along straight lines and arcs is called
the interpolation.
- Tool movement along a straight line
• For milling machining
Workpiece
Program
G01X_Y_ ;
X_ ;
Tool
• For lathe cutting
Program
G01Z_ ;
Tool
Workpiece Z
X
G01X_Z_ ;
Fig. 1.1 (a) Tool movement along a straight line
B-63944EN/03 PROGRAMMING 1.GENERAL
- 15 -
- Tool movement along an arc
• For milling machining
Workpiece Tool
Program
G03 X_ Y_ R_ ;
• For lathe cutting
Program
G02 X_ Z_ R_ ;
or
G03 X_ Z_ R_ ;
Workpiece Z
X
Fig. 1.1 (b) Tool movement along an arc
The term interpolation refers to an operation in which the tool moves
along a straight line or arc in the way described above.
Symbols of the programmed commands G01, G02, ... are called the
preparatory function and specify the type of interpolation conducted in
the control unit.
(a) Movement along straight line
G01 Y_ ;
X_ Y_ ;
(b) Movement along arc
G03X_ Y_ R_ ;
CNC
X axis
Y axis
Tool
movement
Interpolation
a)Movement
along straight
line
b)Movement
along arc
Fig. 1.1 (c) Interpolation function
NOTE
Some machines move tables instead of tools but
this manual assumes that tools are moved against
workpieces.
1.GENERAL PROGRAMMING B-63944EN/03
- 16 -
1.2 FEED-FEED FUNCTION
Movement of the tool at a specified speed for cutting a workpiece is
called the feed.
• For milling machining
Tool
Workpiece
Table
F
mm/min
• For lathe cutting
To o l
Workpiece
Chuck
F
mm/min
Fig. 1.2 (a) Feed function
Feedrates can be specified by using actual numerics. For example, to
feed the tool at a rate of 150 mm/min, specify the following in the
program:
F150.0
The function of deciding the feed rate is called the feed function (See
II-5).
B-63944EN/03 PROGRAMMING 1.GENERAL
- 17 -
1.3 PART DRAWING AND TOOL MOVEMENT
1.3.1 Reference Position (Machine-specific Position)
A CNC machine tool is provided with a fixed position. Normally, tool
change and programming of absolute zero point as described later are
performed at this position. This position is called the reference
position.
• For milling machining
Reference position
Tool
Workpiece
Table
• For lathe cutting
Tool post
Reference
position
Chuck
Fig. 1.3.1 (a) Reference position
Explanation
The tool can be moved to the reference position in two ways:
1. Manual reference position return (See III-3.1)
Reference position return is performed by manual button
operation.
2. Automatic reference position return (See II-6)
In general, manual reference position return is performed first
after the power is turned on. In order to move the tool to the
reference position for tool change thereafter, the function of
automatic reference position return is used.
1.GENERAL PROGRAMMING B-63944EN/03
- 18 -
1.3.2 Coordinate System on Part Drawing and Coordinate System
Specified by CNC - Coordinate System
• For milling machining
Z
Y
X
Part drawing
Z
Y
X
Coordinate system
Z
Y
X
Tool
Workpiece
Machine tool
Program
Command
CNC
Tool
• For lathe cutting
Part drawing
Machine tool
Program
Command
CNC
X
Z
X
Z
Coordinate system
Workpiece
X
Z
Fig. 1.3.2 (a) Coordinate system
B-63944EN/03 PROGRAMMING 1.GENERAL
- 19 -
Explanation
- Coordinate system
The following two coordinate systems are specified at different
locations: (See II-7)
1 Coordinate system on part drawing
The coordinate system is written on the part drawing. As the
program data, the coordinate values on this coordinate system are
used.
2. Coordinate system specified by the CNC
The coordinate system is prepared on the actual machine tool
table. This can be achieved by programming the distance from
the current position of the tool to the zero point of the coordinate
system to be set.
230
300
Program
origin
Distance to the zero point of a coor-
dinate system to be set
Present tool position
X
X
Y
Fig. 1.3.2 (b) Coordinate system specified by the CNC
Concrete programming methods for setting coordinate systems
specified by the CNC are explained in II-7, "COORDINATE
SYSTEM".
1.GENERAL PROGRAMMING B-63944EN/03
- 20 -
The positional relation between these two coordinate systems is
determined when a workpiece is set on the table.
• For milling machining
YY
Table
Workpiece
X
X
Coordinate system
specified by the CNC
established on the table
Coordinate system on
part drawing estab
lished on the workpiece
• For lathe cutting
Z
Workpiece
X
X
Z
Coordinate system on part drawing
established on the workpiece
Coordinate system specified by the
CNC established on the chuck
Chuck
Fig. 1.3.2 (c) Coordinate system specified by CNC and coordinate
system on part drawing
The tool moves on the coordinate system specified by the CNC in
accordance with the command program generated with respect to the
coordinate system on the part drawing, and cuts a workpiece into a
shape on the drawing.
Therefore, in order to correctly cut the workpiece as specified on the
drawing, the two coordinate systems must be set at the same position.
B-63944EN/03 PROGRAMMING 1.GENERAL
- 21 -
- Methods of setting the two coordinate systems in the same position
M
To set the two coordinate systems at the same position, simple
methods shall be used according to workpiece shape, the number of
machinings.
1. Using a standard plane and point of the workpiece.
Program
origin
Y
X
Workpiece's
standard point
Fixed distance
Bring the tool center to the workpiece standard point.
A
nd set the coordinate system specified by CNC at this position.
Fixed distance
2. Mounting a workpiece directly against the jig
Jig
Program origin
Meet the tool center to the reference position. And set the coordinate
specified by CNC at this position. (Jig shall be mounted on the
point from the reference
3. Mounting a workpiece on a pallet, then mounting the workpiece
and pallet on the jig
Pallet
(Jig and coordinate system shall be specified by the same as (2)).
Jig
Workpiece
1.GENERAL PROGRAMMING B-63944EN/03
- 22 -
T
The following method is usually used to define two coordinate
systems at the same location.
1 When coordinate zero point is set at chuck face
Workpiece
X
150
40
Z
60 40
Workpiece
X
Z
Chuck
- Coordinates and
dimensions on part drawing
- Coordinate system on
lathe as s
p
ecified b
y
CNC
Program origin
When the coordinate system on the part drawing and the coordinate
system specified by the CNC are set at the same position, the program
origin can be set on the chuck face.
B-63944EN/03 PROGRAMMING 1.GENERAL
- 23 -
2. When coordinate zero point is set at workpiece end face.
X
Z
60 30
100
80
30
X
Z
Workpiece
Workpiece
Chuck
- Coordinates and
dimensions on part drawing
- Coordinate system on
lathe as s
p
ecified b
y
CNC
Program origin
When the coordinate system on the part drawing and the coordinate
system specified by the CNC are set at the same position, the program
origin can be set on the end face of the workpiece.
1.GENERAL PROGRAMMING B-63944EN/03
- 24 -
1.3.3 How to Indicate Command Dimensions for Moving the Tool
(Absolute, Incremental Commands)
Explanation
Command for moving the tool can be indicated by absolute command
or incremental command (See II-8.1).
- Absolute command
The tool moves to a point at "the distance from zero point of the
coordinate system" that is to the position of the coordinate values.
• For milling machining
B(10.0,30.0,5.0)
Y
X
Tool
A
Command specifying movement from
point A to point B
Z
G90 X10.0 Y30.0 Z5.0 ;
Coordinates of point B
• For lathe cutting
Command specifying movement from point A to
point B
X
30.0Z70.0;
Tool
φ
30
A
B
Z
X
70
110
Coordinates of point B
Workpiece
B-63944EN/03 PROGRAMMING 1.GENERAL
- 25 -
- Incremental command
Specify the distance from the previous tool position to the next tool
position.
• For milling machining
Y
Z
A
X=40.0
Z=-10.0
Y-3 0 . 0
XB
G91 X40.0 Y-30.0 Z-10.0 ;
Distance and direction for
movement along each axis
Tool
Command specifying movement from
point A to point B
• For lathe cutting
φ
30
A
B
X
-40.0
φ60 Z
-30.0 (diameter value)
Tool
Workpiece
Command specifying movement from point
A
to point B
U-30.0 W-40.0
Distance and direction for movement along each axis
1.GENERAL PROGRAMMING B-63944EN/03
- 26 -
- Diameter programming / radius programming
Dimensions of the X axis can be set in diameter or in radius. Diameter
programming or radius programming is employed independently in
each machine.
1. Diameter programming
In diameter programming, specify the diameter value indicated
on the drawing as the value of the X axis.
Coordinate values of points A and B
A
(30.0, 80.0), B(40.0, 60.0)
Workpiece
Z
X
60
80
φ
30
A
B
φ
40
2. Radius programming
In radius programming, specify the distance from the center of
the workpiece, i.e. the radius value as the value of the X axis.
Coordinate values of points A and B A(15.0, 80.0), B(20.0, 60.0)
Workpiece
Z
X
60
80
A
B
20 15
B-63944EN/03 PROGRAMMING 1.GENERAL
- 27 -
1.4 CUTTING SPEED - SPINDLE FUNCTION
The speed of the tool with respect to the workpiece when the
workpiece is cut is called the cutting speed.
As for the CNC, the cutting speed can be specified by the spindle
speed in min-1 unit.
• For milling machining
min-1
φ
D mm
m/min
Tool
V: Cutting speed
Workpiece
Spindle speed N Tool diameter
<When a workpiece should be machined with a tool 100 mm in
diameter at a cutting speed of 80 m/min.>
The spindle speed is approximately 250 min-1, which is obtained from
N=1000v/πD. Hence the following command is required:
S250;
Commands related to the spindle speed are called the spindle speed
function (See II-9).
• For lathe cutting
φD
Tool
v m/min
N min-
1
Workpiece
Cutting speed
Spindle speed
<When a workpiece 200 mm in diameter should be machined at a
cutting speed of 300 m/min.>
The spindle speed is approximately 478 min-1, which is obtained from
N=1000v/πD. Hence the following command is required:
S478;
Commands related to the spindle speed are called the spindle speed
function (See II-9).
The cutting speed v (m/min) can also be specified directly by the
speed value. Even when the workpiece diameter is changed, the CNC
changes the spindle speed so that the cutting speed remains constant.
This function is called the constant surface speed control function (See
II-9.3).
1.GENERAL PROGRAMMING B-63944EN/03
- 28 -
1.5 SELECTION OF TOOL USED FOR VARIOUS MACHINING -
TOOL FUNCTION
Overview
For each of various types of machining (such as drilling, tapping,
boring, and milling for milling machining, or rough machining,
semifinish machining, finish machining, threading, and grooving for
lathe cutting), a necessary tool is to be selected. When a number is
assigned to each tool and the number is specified in the program, the
corresponding tool is selected.
Examples
M
01
02
Tool number
A
TC magazine
Fig. 1.5 (a) Tool used for various machining
<When No.01 is assigned to a drilling tool>
When the tool is stored at location 01 in the ATC magazine, the tool
can be selected by specifying T01. This is called the tool function (See
II-10).
T
Tool number
Tool post
01 06
02 05
04
03
Fig. 1.5 (b) Tool used for various machining
<When No.01 is assigned to a roughing tool>
When the tool is stored at location 01 of the tool post, the tool can be
selected by specifying T0101. This is called the tool function (See II-
10).
B-63944EN/03 PROGRAMMING 1.GENERAL
- 29 -
1.6 COMMAND FOR MACHINE OPERATIONS - AUXILIARY
FUNCTION
When a workpiece is actually machined with a tool, the spindle is
rotated, coolant is supplied, and the chuck is opened/closed. So,
control needs to be exercised on the spindle motor of the machine,
coolant valve on/off operation, and chuck open/close operation.
• For milling machining
Workpiece
Tool
Coolant on/off
Spindle
rotation
• For lathe cutting
Workpiece
Chuck open/close
Spindle rotation
Coolant on/off
Fig. 1.6 (a) Auxiliary function
The function of specifying the on-off operations of the components of
the machine is called the auxiliary function. In general, the function is
specified by an M code (See II-11).
For example, when M03 is specified, the spindle is rotated clockwise
at the specified spindle speed.
1.GENERAL PROGRAMMING B-63944EN/03
- 30 -
1.7 PROGRAM CONFIGURATION
A group of commands given to the CNC for operating the machine is
called the program. By specifying the commands, the tool is moved
along a straight line or an arc, or the spindle motor is turned on and off.
In the program, specify the commands in the sequence of actual tool
movements.
Block
Block
Block
Block
:
:
:
:
Block
Program
Tool movement
sequence
Fig. 1.7 (a) Program configuration
A group of commands at each step of the sequence is called the block.
The program consists of a group of blocks for a series of machining.
The number for discriminating each block is called the sequence
number, and the number for discriminating each program is called the
program number (See II-13).
B-63944EN/03 PROGRAMMING 1.GENERAL
- 31 -
Explanation
The block and the program have the following configurations.
- Block
End of block
Nxxxxx Gxx Xxxx.x Yxxx.x Mxx Sxx Txx ;
1 block
Sequence
number
Preparatory
function
A
uxiliary
function
Spindle
function
Tool
function
Dimension word
Fig. 1.7 (b) Block configuration
A block starts with a sequence number to identify the block and ends
with an end-of-block code.
This manual indicates the end-of-block code by; (LF in the ISO code
and CR in the EIA code).
The contents of the dimension word depend on the preparatory
function. In this manual, the portion of the dimension word may be
represent as IP_.
- Program
;
Oxxxxx ; Program number
Block
Block
Block
:
:
:
M30 ; End of program
:
:
:
Fig. 1.7 (c) Program configuration
Normally, a program number is specified after the end-of-block (;)
code at the beginning of the program, and a program end code (M02
or M30) is specified at the end of the program.
1.GENERAL PROGRAMMING B-63944EN/03
- 32 -
- Main program and subprogram
When machining of the same pattern appears at many portions of a
program, a program for the pattern is created. This is called the
subprogram. On the other hand, the original program is called the
main program. When a subprogram execution command appears
during execution of the main program, commands of the subprogram
are executed. When execution of the subprogram is finished, the
sequence returns to the main program.
Main program
M98P1001
:
:
M98P1002
:
:
:
:
:
:
:
:
Subprogram #1
Subprogram #2
O1001
M99
O1002
M99
M98P1001
Fig. 1.7 (d) Subprogram execution
B-63944EN/03 PROGRAMMING 1.GENERAL
- 33 -
1.8 TOOL MOVEMENT RANGE - STROKE
Limit switches are installed at the ends of each axis on the machine to
prevent tools from moving beyond the ends. The range in which tools
can move is called the stroke.
Stroke area
Motor
Limit
switch
Machine zero point
Besides strokes defined with limit switches, the operator can define an
area which the tool cannot enter using a program or data in memory.
This function is called stroke check (see III-6.3).
Motor
Limit
switch
Specif
y
these distances.
Machine zero point
Tools cannot enter this area. The area is
specified by data in memory or a program.
2.CONTROLLED AXES PROGRAMMING B-63944EN/03
- 34 -
2 CONTROLLED AXES
Chapter 2, "CONTROLLED AXES", consists of the following
sections:
2.1 NUMBER OF CONTROLLED AXES.......................................35
2.2 NAMES OF AXES .....................................................................36
2.3 INCREMENT SYSTEM.............................................................37
2.4 MAXIMUM STROKE................................................................38
B-63944EN/03 PROGRAMMING 2.CONTROLLED AXES
- 35 -
2.1 NUMBER OF CONTROLLED AXES
Explanation
The number of controlled axes used with this NC system depends on
the model and system control type as indicated below.
NOTE
1 The maximum number of controlled axes that can
be used is limited depending on the option
configuration. Refer to the manual provided by the
machine tool builder for details.
2 The number of simultaneously controllable axes for
manual operation (jog feed, manual reference
position return, or manual rapid traverse) is 1 or 3
(1 when bit 0 (JAX) of parameter No. 1002 is set to
0 and 3 when it is set to 1).
Series 30i-A
Series 300i-A
Series 300is-A
Series 31i-A5
Series 310i-A5
Series 310is-A5
Series 31i-A
Series 310i-A
Series 310is-A
Series 32i-A
Series 320i-A
Series 320is-A
Lathe system 2 axes 2 axes 2 axes 2 axes Number of basic
controlled axes Machining
center system 3 axes 3 axes 3 axes 3 axes
Controlled axes expansion (total)
(including Cs axes and PMC axes) Max. 32 axes Max. 20 axes Max. 20 axes Max. 9 axes
Basic simultaneously controlled axes
(each path) 2 axes 2 axes 2 axes 2 axes
Simultaneously controlled axes
expansion (total / each path) Max. 24 axes Max. 12 axes Max. 12 axes Max. 5 axes
2.CONTROLLED AXES PROGRAMMING B-63944EN/03
- 36 -
2.2 NAMES OF AXES
Explanation
The move axes of machine tools are assigned names. These names are
referred to as addresses or axis names. Axis names are determined
according to the machine tool. The naming rules comply with
standards such as the ISO standards.
With complex machines, one character would become insufficient for
representing axis names. So, up to three characters can be used for
axis names. A move axis may be named "X", "X1", or "XA1". The
first character of the three characters is called the first axis name
character, the second character is called the second axis name
character, and third character is called the third axis name character.
Example)
X A 1
3rd axis name character
2nd axis name character
1st axis name character
NOTE
1 Axis names are predetermined according to the
machine used. Refer to the manual supplied by the
machine tool builder.
2 Since many ordinary machines use one character
to represent each address, one-character
addresses are used in the description in this
manual.
B-63944EN/03 PROGRAMMING 2.CONTROLLED AXES
- 37 -
2.3 INCREMENT SYSTEM
Explanation
The increment system consists of the least input increment (for input)
and least command increment (for output). The least input increment
is the least increment for programming the travel distance. The least
command increment is the least increment for moving the tool on the
machine. Both increments are represented in mm, inches, or deg.
Five types of increment systems are available as indicated in Table 2.3
(a). For each axis, an increment system can be set using a bit from bit
0 to bit 3 (ISA, ISC, ISD, or ISE) of parameter No. 1013.
IS-C, IS-D, and IS-E are optional functions.
Table 2.3 (a) Increment system
Name of increment
system Least input increment Least command
increment
0.01 mm 0.01 mm
0.001 inch 0.001 inch
IS-A
0.01 deg 0.01 deg
0.001 mm 0.001 mm
0.0001 inch 0.0001 inch
IS-B
0.001 deg 0.001 deg
0.0001 mm 0.0001 mm
0.00001 inch 0.00001 inch
IS-C
0.0001 deg 0.0001 deg
0.00001 mm 0.00001 mm
0.000001 inch 0.000001 inch
IS-D
0.00001 deg 0.00001 deg
0.000001 mm 0.000001 mm
0.0000001 inch 0.0000001 inch
IS-E
0.000001 deg 0.000001 deg
The least command increment is either metric or inch depending on
the machine tool. Set metric or inch to the parameter INM
(No.0100#0).
For selection between metric and inch for the least input increment, G
code (G20 or G21) or a setting parameter selects it.
Combined use of the inch system and the metric system is not allowed.
There are functions that cannot be used between axes with different
unit systems (circular interpolation, cutter compensation, etc.). For the
increment system, see the machine tool builder's manual.
NOTE
1 The unit (mm or inch) in the table is used for
indicating a diameter value for diameter programming
(when bit 3 (DIA) of parameter No. 1006 is set to 1)
or a radius value for radius programming.
2 Some increment systems are unavailable depending
on the model. For details, refer to “Descriptions” (B-
63942EN).
2.CONTROLLED AXES PROGRAMMING B-63944EN/03
- 38 -
2.4 MAXIMUM STROKE
Explanation
The maximum stroke controlled by this CNC is shown in the table
below:
Maximum stroke = Least command increment × 999999999
(99999999 for IS-A)
Commands that exceed the maximum stroke are not permitted.
Table 2.4 (a) Maximum strokes
Name of increment
system Least input increment Maximum stroke
0.01 mm ±999999.99 mm
0.001 inch ±99999.999 inch
IS-A
0.01 deg ±999999.99 deg
0.001 mm ±999999.999 mm
0.0001 inch ±99999.9999 inch
IS-B
0.001 deg ±999999.999 deg
0.0001 mm ±99999.9999 mm
0.00001 inch ±9999.99999 inch
IS-C
0.0001 deg ±99999.9999 deg
0.00001 mm ±9999.99999 mm
0.000001 inch ±999.999999 inch
IS-D
0.00001 deg ±9999.99999 deg
0.000001 mm ±999.999999 mm
0.0000001 inch ±99.9999999 inch
IS-E
0.000001 deg ±999.999999 deg
NOTE
1 The actual stroke depends on the machine tool.
2 The unit (mm or inch) in the table is used for
indicating a diameter value for diameter
programming (when bit 3 (DIA) of parameter No.
1006 is set to 1) or a radius value for radius
programming.
3 Some increment systems are unavailable
depending on the model. For details, refer to
"Descriptions" (B-63942EN).
B-63944EN/03 PROGRAMMING
- 39 -
3.PREPARATORY FUNCTION
(G FUNCTION)
3 PREPARATORY FUNCTION
(G FUNCTION)
A number following address G determines the meaning of the
command for the concerned block.
G codes are divided into the following two types.
Type Meaning
One-shot G code The G code is effective only in the block in which it
is specified.
Modal G code The G code is effective until another G code of the
same group is specified.
(Example)
G01 and G00 are modal G codes in group 01.
G01 X_ ;
Z_ ; G01 is effective in this range.
X_ ;
G00 Z_ ; G00 is effective in this range.
X_ ;
G01 X_ ;
:
T
There are three G code systems in the lathe system: A, B, and C
(Table 3.1(a)). Select a G code system using bits 6 (GSB) and 7
(GSC) of parameter No. 3401. To use G code system B or C, the
corresponding option is needed. Generally, User’s Manual describes
the use of G code system A, except when the described item can use
only G code system B or C. In such cases, the use of G code system B
or C is described.
PROGRAMMING B-63944EN/03
- 40 -
3. PREPARATORY FUNCTION
(G FUNCTION)
Explanation
1. When the clear state (bit 6 (CLR) of parameter No. 3402) is set at
power-up or reset, the modal G codes are placed in the states
described below.
(1) The modal G codes are placed in the states marked with
as indicated in Table.
(2) G20 and G21 remain unchanged when the clear state is set
at power-up or reset.
(3) Which status G22 or G23 at power on is set by bit 7 (G23)
of parameter No. 3402. However, G22 and G23 remain
unchanged when the clear state is set at reset.
(4) The user can select G00 or G01 by setting parameter G01
(No. 3402#0).
(5) The user can select G90 or G91 by setting parameter G91
(No. 3402#3).
When G code system B or C is used in the lathe system,
setting bit 3 (G91) of parameter No. 3402 determines which
code, either G90 or G91, is effective.
(6) In the machining center system, the user can select G17,
G18, or G19 by setting bits 1 (G18) and 2 (G19) of
parameter No. 3401.
2. G codes other than G10 and G11 are one-shot G codes.
3. When a G code not listed in the G code list is specified, or a G
code that has no corresponding option is specified, alarm PS0010
occurs.
4. Multiple G codes can be specified in the same block if each G
code belongs to a different group. If multiple G codes that belong
to the same group are specified in the same block, only the last G
code specified is valid.
5. If a G code belonging to group 01 is specified in a canned cycle
for drilling, the canned cycle for drilling is cancelled. This means
that the same state set by specifying G80 is set. Note that the G
codes in group 01 are not affected by a G code specifying a
canned cycle for drilling.
6. G codes are indicated by group.
7. The group of G60 is switched according to the setting of bit 0
(MDL) of parameter No. 5431. (When the MDL bit is set to 0,
the 00 group is selected. When the MDL bit is set to 1, the 01
group is selected.)
T
8. When G code system A is used, absolute or incremental
programming is specified not by a G code (G90/G91) but by an
address word (X/U, Z/W, C/H, Y/V). Only the initial level is
provided at the return point of the canned cycle for drilling..
B-63944EN/03 PROGRAMMING
- 41 -
3.PREPARATORY FUNCTION
(G FUNCTION)
3.1 G CODE LIST IN THE MACHINING CENTER SYSTEM
M
Table 3.1 (a) G code list
G code Group Function
G00 Positioning (rapid traverse)
G01 Linear interpolation (cutting feed)
G02 Circular interpolation CW or helical interpolation CW
G03 Circular interpolation CCW or helical interpolation CCW
G02.2, G03.2 Involute interpolation CW/CCW
G02.3, G03.3 Exponential interpolation CW/CCW
G02.4, G03.4
01
Three-dimensional coordinate system conversion CW/CCW
G04 Dwell
G05 AI contour control (high-precision contour control compatible command),
High-speed cycle machining
G05.1 AI contour control / Nano smoothing / Smooth interpolation
G05.4
00
HRV3, 4 on/off
G06.2 01 NURBS interpolation
G07 Hypothetical axis interpolation
G07.1 (G107) Cylindrical interpolation
G08 AI contour control (advanced preview control compatible command)
G09 Exact stop
G10 Programmable data input
G10.6 Tool retract and recover
G10.9 Programmable switching of diameter/radius specification
G11
00
Programmable data input mode cancel
G12.1 Polar coordinate interpolation mode
G13.1 21 Polar coordinate interpolation cancel mode
G15 Polar coordinates command cancel
G16 17 Polar coordinates command
G17 XpYp plane selection
G18 ZpXp plane selection
G19
02
YpZp plane selection
Xp: X axis or its parallel axis
Yp: Y axis or its parallel axis
Zp: Z axis or its parallel axis
G20 (G70) Input in inch
G21 (G71) 06 Input in mm
G22 Stored stroke check function on
G23 04 Stored stroke check function off
G25 Spindle speed fluctuation detection off
G26 19 Spindle speed fluctuation detection on
G27 Reference position return check
G28 Automatic return to reference position
G29 Movement from reference position
G30 2nd, 3rd and 4th reference position return
G30.1 Floating reference position return
G31 Skip function
G31.8
00
EGB-axis skip
G33 Threading
G34 Variable lead threading
G35 Circular threading CW
G36
01
Circular threading CCW
PROGRAMMING B-63944EN/03
- 42 -
3. PREPARATORY FUNCTION
(G FUNCTION)
Table 3.1 (a) G code list
G code Group Function
G37 Automatic tool length measurement
G38 Tool radius/tool nose radius compensation : preserve vector
G39
00
Tool radius/tool nose radius compensation : corner circular interpolation
G40 Tool radius/tool nose radius compensation : cancel
3-dimensional cutter compensation : cancel
G41 Tool radius/tool nose radius compensation : left
3-dimensional cutter compensation : left
G42 Tool radius/tool nose radius compensation : right
3-dimensional cutter compensation : right
G41.2 3-dimensional cutter compensation : left (type 1)
G41.3 3-dimensional cutter compensation : leading edge offset
G41.4 3-dimensional cutter compensation : left (type 1) (FS16i-compatible command)
G41.5 3-dimensional cutter compensation : left (type 1) (FS16i-compatible command)
G41.6 3-dimensional cutter compensation : left (type 2)
G42.2 3-dimensional cutter compensation : right (type 1)
G42.4 3-dimensional cutter compensation : right (type 1) (FS16i-compatible command)
G42.5 3-dimensional cutter compensation : right (type 1) (FS16i-compatible command)
G42.6
07
3-dimensional cutter compensation : right (type 2)
G40.1 Normal direction control cancel mode
G41.1 Normal direction control on : left
G42.1
19
Normal direction control on : right
G43 Tool length compensation +
G44 Tool length compensation -
G43.1 Tool length compensation in tool axis direction
G43.4 Tool center point control (type 1)
G43.5
08
Tool center point control (type 2)
G45 Tool offset : increase
G46 Tool offset : decrease
G47 Tool offset : double increase
G48
00
Tool offset : double decrease
G49 (G49.1) 08 Tool length compensation cancel
G50 Scaling cancel
G51 11 Scaling
G50.1 Programmable mirror image cancel
G51.1 22 Programmable mirror image
G50.2 Polygon turning cancel
G51.2 31 Polygon turning
G50.4 Cancel synchronous control
G50.5 Cancel composite control
G50.6 Cancel superimposed control
G51.4 Start synchronous control
G51.5 Start composite control
G51.6
00
Start superimposed control
G52 Local coordinate system setting
G53 Machine coordinate system setting
G53.1
00
Tool axis direction control
B-63944EN/03 PROGRAMMING
- 43 -
3.PREPARATORY FUNCTION
(G FUNCTION)
Table 3.1 (a) G code list
G code Group Function
G54 (G54.1) Workpiece coordinate system 1 selection
G55 Workpiece coordinate system 2 selection
G56 Workpiece coordinate system 3 selection
G57 Workpiece coordinate system 4 selection
G58 Workpiece coordinate system 5 selection
G59
14
Workpiece coordinate system 6 selection
G54.2 23 Rotary table dynamic fixture offset
G54.4 33 Workpiece setting error compensation
G60 00 Single direction positioning
G61 Exact stop mode
G62 Automatic corner override
G63 Tapping mode
G64
15
Cutting mode
G65 00 Macro call
G66 Macro modal call A
G66.1 Macro modal call B
G67
12
Macro modal call A/B cancel
G68 Coordinate system rotation start or three-dimensional coordinate conversion mode on
G69 Coordinate system rotation cancel or three-dimensional coordinate conversion mode off
G68.2 Tilted working plane command
G68.3 Tilted working plane command by tool axis direction
G68.4
16
Tilted working plane command (incremental multi-command)
G70.7 Finishing cycle
G71.7 Outer surface rough machining cycle
G72.7 End rough machining cycle
G73.7 Closed loop cutting cycle
G74.7 End cutting off cycle
G75.7 Outer or inner cutting off cycle
G76.7 Multiple threading cycle
G72.1 Figure copying (rotary copy)
G72.2
00
Figure copying (linear copy)
G73 Peck drilling cycle
G74 09 Left-handed tapping cycle
G75 01 Plunge grinding cycle
G76 09 Fine boring cycle
G77 Plunge direct sizing/grinding cycle
G78 Continuous-feed surface grinding cycle
G79
01
Intermittent-feed surface grinding cycle
G80 09
Canned cycle cancel
Electronic gear box : synchronization cancellation
G80.4 Electronic gear box: synchronization cancellation
G81.4 34 Electronic gear box: synchronization start
G80.5 Electronic gear box 2 pair: synchronization cancellation
G81.5 24 Electronic gear box 2 pair: synchronization start
G81 09
Drilling cycle or spot boring cycle
Electronic gear box : synchronization start
G81.1 00 Chopping
PROGRAMMING B-63944EN/03
- 44 -
3. PREPARATORY FUNCTION
(G FUNCTION)
Table 3.1 (a) G code list
G code Group Function
G82 Drilling cycle or counter boring cycle
G83 Peck drilling cycle
G84 Tapping cycle
G84.2 Rigid tapping cycle (FS15 format)
G84.3 Left-handed rigid tapping cycle (FS15 format)
G85 Boring cycle
G86 Boring cycle
G87 Back boring cycle
G88 Boring cycle
G89
09
Boring cycle
G90 Absolute programming
G91 03 Incremental programming
G91.1 Checking the maximum incremental amount specified
G92 Setting for workpiece coordinate system or clamp at maximum spindle speed
G92.1
00
Workpiece coordinate system preset
G93 Inverse time feed
G94 Feed per minute
G95
05
Feed per revolution
G96 Constant surface speed control
G97 13 Constant surface speed control cancel
G96.1 Spindle indexing execution (waiting for completion)
G96.2 Spindle indexing execution (not waiting for completion)
G96.3 Spindle indexing completion check
G96.4
00
SV speed control mode ON
G98 Canned cycle : return to initial level
G99 10 Canned cycle : return to R point level
G107 00 Cylindrical interpolation
G112 Polar coordinate interpolation mode
G113 21 Polar coordinate interpolation mode cancel
G160 Infeed control cancel
G161 20 Infeed control
B-63944EN/03 PROGRAMMING
- 45 -
3.PREPARATORY FUNCTION
(G FUNCTION)
3.2 G CODE LIST IN THE LATHE SYSTEM
T
Table 3.2 (a) G code list
G code system
A B C
Group Function
G00 G00 G00 Positioning (Rapid traverse)
G01 G01 G01 Linear interpolation (Cutting feed)
G02 G02 G02 Circular interpolation CW or helical interpolation CW
G03 G03 G03 Circular interpolation CCW or helical interpolation CCW
G02.2 G02.2 G02.2 Involute interpolation CW
G02.3 G02.3 G02.3 Exponential interpolation CW
G02.4 G02.4 G02.4 Three-dimensional coordinate system conversion CW
G03.2 G03.2 G03.2 Involute interpolation CCW
G03.3 G03.3 G03.3 Exponential interpolation CCW
G03.4 G03.4 G03.4
01
Three-dimensional coordinate system conversion CCW
G04 G04 G04 Dwell
G05 G05 G05 AI contour control (command compatible with high precision
contour control), High-speed cycle machining
G05.1 G05.1 G05.1 AI contour control / Nano smoothing / Smooth interpolation
G05.4 G05.4 G05.4
00
HRV3, 4 on/off
G06.2 G06.2 G06.2 01 NURBS interpolation
G07 G07 G07 Hypothetical axis interpolation
G07.1
(G107)
G07.1
(G107)
G07.1
(G107) Cylindrical interpolation
G08 G08 G08 Advanced preview control
G09 G09 G09 Exact stop
G10 G10 G10 Programmable data input
G10.6 G10.6 G10.6 Tool retract and recover
G10.9 G10.9 G10.9 Programmable switching of diameter/radius specification
G11 G11 G11
00
Programmable data input mode cancel
G12.1
(G112)
G12.1
(G112)
G12.1
(G112) Polar coordinate interpolation mode
G13.1
(G113)
G13.1
(G113)
G13.1
(G113)
21
Polar coordinate interpolation cancel mode
G17 G17 G17 XpYp plane selection
G18 G18 G18 ZpXp plane selection
G19 G19 G19
16
YpZp plane selection
G20 G20 G70 Input in inch
G21 G21 G71 06 Input in mm
G22 G22 G22 Stored stroke check function on
G23 G23 G23 09 Stored stroke check function off
G25 G25 G25 Spindle speed fluctuation detection off
G26 G26 G26
08 Spindle speed fluctuation detection on
PROGRAMMING B-63944EN/03
- 46 -
3. PREPARATORY FUNCTION
(G FUNCTION)
Table 3.2 (a) G code list
G code system
A B C
Group Function
G27 G27 G27 Reference position return check
G28 G28 G28 Return to reference position
G29 G29 G29 Movement from reference position
G30 G30 G30 2nd, 3rd and 4th reference position return
G30.1 G30.1 G30.1 Floating reference point return
G31 G31 G31 Skip function
G31.8 G31.8 G31.8
00
EGB-axis skip
G32 G33 G33 Threading
G34 G34 G34 Variable lead threading
G35 G35 G35 Circular threading CW
G36 G36 G36
Circular threading CCW (When bit 3 (G36) of parameter No.
3405 is set to 1) or Automatic tool offset (X axis) (When bit 3
(G36) of parameter No. 3405 is set to 0)
G37 G37 G37 Automatic tool offset (Z axis) (When bit 3 (G36) of parameter No.
3405 is set to 0)
G37.1 G37.1 G37.1 Automatic tool offset (X axis) (When bit 3 (G36) of parameter No.
3405 is set to 1)
G37.2 G37.2 G37.2 Automatic tool offset (Z axis) (When bit 3 (G36) of parameter No.
3405 is set to 1)
G38 G38 G38 Tool radius/tool nose radius compensation: with vector held
G39 G39 G39
01
Tool radius/tool nose radius compensation: corner rounding
interpolation
G40 G40 G40 Tool radius/tool nose radius compensation : cancel
G41 G41 G41 Tool radius/tool nose radius compensation : left
G42 G42 G42 Tool radius/tool nose radius compensation : right
G41.2 G41.2 G41.2 3-dimensional cutter compensation : left (type 1)
G41.3 G41.3 G41.3 3-dimensional cutter compensation :
(leading edge offset)
G41.4 G41.4 G41.4 3-dimensional cutter compensation : left (type 1) (FS16i-
compatible command)
G41.5 G41.5 G41.5 3-dimensional cutter compensation : left (type 1) (FS16i-
compatible command)
G41.6 G41.6 G41.6 3-dimensional cutter compensation : left (type 2)
G42.2 G42.2 G42.2 3-dimensional cutter compensation : right (type 1)
G42.4 G42.4 G42.4 3-dimensional cutter compensation : right (type 1) (FS16i-
compatible command)
G42.5 G42.5 G42.5 3-dimensional cutter compensation : right (type 1) (FS16i-
compatible command)
G42.6 G42.6 G42.6
07
3-dimensional cutter compensation : right (type 2)
G40.1 G40.1 G40.1 Normal direction control cancel mode
G41.1 G41.1 G41.1 Normal direction control left on
G42 .1 G42 .1 G42 .1
19
Normal direction control right on
B-63944EN/03 PROGRAMMING
- 47 -
3.PREPARATORY FUNCTION
(G FUNCTION)
Table 3.2 (a) G code list
G code system
A B C
Group Function
G43 G43 G43 Tool length compensation +
(Parameter TCT (No.5040#3) must be "1".)
G44 G44 G44 Tool length compensation -
(Parameter TCT (No.5040#3) must be "1".)
G43.1 G43.1 G43.1 Tool length compensation in tool axis direction
(Parameter TCT (No.5040#3) must be "1".)
G43.4 G43.4 G43.4 Tool center point control (type 1)
(Parameter TCT (No.5040#3) must be "1".)
G43.5 G43.5 G43.5 Tool center point control (type 2)
(Parameter TCT (No.5040#3) must be "1".)
G43.7
(G44.7)
G43.7
(G44.7)
G43.7
(G44.7)
Tool offset
(Parameter TCT (No.5040#3) must be "1".)
G49
(G49.1)
G49
(G49.1)
G49
(G49.1)
23
Tool length compensation cancel
(Parameter TCT (No.5040#3) must be "1".)
G50 G92 G92 Coordinate system setting or max spindle speed clamp
G50.3 G92.1 G92.1 00 Workpiece coordinate system preset
- G50 G50 Scaling cancel
- G51 G51 18 Scaling
G50.1 G50.1 G50.1 Programmable mirror image cancel
G51.1 G51.1 G51.1 22 Programmable mirror image
G50.2
(G250)
G50.2
(G250)
G50.2
(G250) Polygon turning cancel
G51.2
(G251)
G51.2
(G251)
G51.2
(G251)
20
Polygon turning
G50.4 G50.4 G50.4 Cancel synchronous control
G50.5 G50.5 G50.5 Cancel composite control
G50.6 G50.6 G50.6 Cancel superimposed control
G51.4 G51.4 G51.4 Start synchronous control
G51.5 G51.5 G51.5 Start composite control
G51.6 G51.6 G51.6 Start superimposed control
G52 G52 G52 Local coordinate system setting
G53 G53 G53 Machine coordinate system setting
G53.1 G53.1 G53.1
00
Tool axis direction control
G54
(G54.1)
G54
(G54.1)
G54
(G54.1) Workpiece coordinate system 1 selection
G55 G55 G55 Workpiece coordinate system 2 selection
G56 G56 G56 Workpiece coordinate system 3 selection
G57 G57 G57 Workpiece coordinate system 4 selection
G58 G58 G58 Workpiece coordinate system 5 selection
G59 G59 G59
14
Workpiece coordinate system 6 selection
G54.4 G54.4 G54.4 26 Workpiece setting error compensation
G60 G60 G60 00 Single direction positioning
G61 G61 G61 Exact stop mode
G62 G62 G62 Automatic corner override mode
G63 G63 G63 Tapping mode
G64 G64 G64
15
Cutting mode
G65 G65 G65 00 Macro call
G66 G66 G66 Macro modal call A
G66.1 G66.1 G66.1 Macro modal call B
G67 G67 G67
12
Macro modal call A/B cancel
PROGRAMMING B-63944EN/03
- 48 -
3. PREPARATORY FUNCTION
(G FUNCTION)
Table 3.2 (a) G code list
G code system
A B C
Group Function
G68 G68 G68 04 Mirror image on for double turret or balance cutting mode
G68.1 G68.1 G68.1 Coordinate system rotation start or three-dimensional coordinate
system conversion mode on
G68.2 G68.2 G68.2 Tilted working plane command
G68.3 G68.3 G68.3 Tilted working plane command by tool axis direction
G68.4 G68.4 G68.4
17
Tilted working plane command (incremental multi-command)
G69 G69 G69 04 Mirror image off for double turret or balance cutting mode cancel
G69.1 G69.1 G69.1 17 Coordinate system rotation cancel or three-dimensional
coordinate system conversion mode off
G70 G70 G72 Finishing cycle
G71 G71 G73 Stock removal in turning
G72 G72 G74 Stock removal in facing
G73 G73 G75 Pattern repeating cycle
G74 G74 G76 End face peck drilling cycle
G75 G75 G77 Outer diameter/internal diameter drilling cycle
G76 G76 G78
00
Multiple-thread cutting cycle
G71 G71 G72 Traverse grinding cycle
G72 G72 G73 Traverse direct sizing/grinding cycle
G73 G73 G74 Oscillation grinding cycle
G74 G74 G75
01
Oscillation direct sizing/grinding cycle
G80 G80 G80 10
Canned cycle cancel for drilling
Electronic gear box : synchronization cancellation
G80.4 G80.4 G80.4 Electronic gear box: synchronization cancellation
G81.4 G81.4 G81.4 28 Electronic gear box: synchronization start
G80.5 G80.5 G80.5 Electronic gear box 2 pair: synchronization cancellation
G81.5 G81.5 G81.5 27 Electronic gear box 2 pair: synchronization start
G81 G81 G81 Spot drilling (FS15-T format)
Electronic gear box : synchronization start
G82 G82 G82 Counter boring (FS15-T format)
G83 G83 G83 Cycle for face drilling
G83.1 G83.1 G83.1 High-speed peck drilling cycle (FS15-T format)
G83.5 G83.5 G83.5 High-speed peck drilling cycle
G83.6 G83.6 G83.6 Peck drilling cycle
G84 G84 G84 Cycle for face tapping
G84.2 G84.2 G84.2 Rigid tapping cycle (FS15-T format)
G85 G85 G85 Cycle for face boring
G87 G87 G87 Cycle for side drilling
G87.5 G87.5 G87.5 High-speed peck drilling cycle
G87.6 G87.6 G87.6 Peck drilling cycle
G88 G88 G88 Cycle for side tapping
G89 G89 G89
10
Cycle for side boring
G90 G77 G20 Outer diameter/internal diameter cutting cycle
G92 G78 G21 Threading cycle
G94 G79 G24
01
End face turning cycle
G91.1 G91.1 G91.1 00 Maximum specified incremental amount check
G96 G96 G96 Constant surface speed control
G97 G97 G97 02 Constant surface speed control cancel
B-63944EN/03 PROGRAMMING
- 49 -
3.PREPARATORY FUNCTION
(G FUNCTION)
Table 3.2 (a) G code list
G code system
A B C
Group Function
G96.1 G96.1 G96.1 Spindle indexing execution (waiting for completion)
G96.2 G96.2 G96.2 Spindle indexing execution (not waiting for completion)
G96.3 G96.3 G96.3 Spindle indexing completion check
G96.4 G96.4 G96.4
00
SV speed control mode ON
G93 G93 G93 Inverse time feed
G98 G94 G94 Feed per minute
G99 G95 G95
05
Feed per revolution
- G90 G90 Absolute programming
- G91 G91 03 Incremental programming
- G98 G98 Canned cycle : return to initial level
- G99 G99 11 Canned cycle : return to R point level
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 50 -
4 INTERPOLATION FUNCTIONS
Interpolation functions specify the way to make an axis movement (in
other words, a movement of the tool with respect to the workpiece or
table).
Chapter 4, "INTERPOLATION FUNCTIONS", consists of the
following sections:
4.1 POSITIONING (G00) ..............................................................51
4.2 SINGLE DIRECTION POSITIONING (G60).........................53
4.3 LINEAR INTERPOLATION (G01) ........................................56
4.4 CIRCULAR INTERPOLATION (G02, G03) ..........................59
4.5 HELICAL INTERPOLATION (G02, G03) .............................65
4.6 HELICAL INTERPOLATION B (G02, G03) .........................67
4.7 SPIRAL INTERPOLATION, CONICAL
INTERPOLATION (G02, G03) ...............................................68
4.8 POLAR COORDINATE INTERPOLATION (G12.1, G13.1) 76
4.9 CYLINDRICAL INTERPOLATION (G07.1) .........................85
4.10 CUTTING POINT INTERPOLATION FOR
CYLINDRICAL INTERPOLATION (G07.1) .........................90
4.11 EXPONENTIAL INTERPOLATION (G02.3, G03.3) ..........102
4.12 SMOOTH INTERPOLATION (G05.1) .................................109
4.13 NANO SMOOTHING............................................................113
4.14 NURBS INTERPOLATION (G06.2).....................................121
4.15 HYPOTHETICAL AXIS INTERPOLATION (G07) ............131
4.16 VARIABLE LEAD THREADING (G34)..............................133
4.17 CIRCULAR THREADING (G35, G36) ................................134
4.18 SKIP FUNCTION (G31)........................................................139
4.19 MULTI-STEP SKIP (G31).....................................................141
4.20 HIGH-SPEED SKIP SIGNAL (G31).....................................142
4.21 CONTINUOUS HIGH-SPEED SKIP FUNCTION ...............143
4.22 TORQUE LIMIT SKIP ..........................................................145
4.23 THREE-DIMENSIONAL CIRCULAR INTERPOLATION.149
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 51 -
4.1 POSITIONING (G00)
The G00 command moves a tool to the position in the workpiece
system specified with an absolute or an incremental programming at a
rapid traverse rate.
In the absolute programming, coordinate value of the end point is
programmed.
In the incremental programming the distance the tool moves is
programmed.
Format
G00 IP_ ;
IP_ : For an absolute programming, the coordinates of an
end point, and for an incremental programming, the
distance the tool moves.
Explanation
Either of the following tool paths can be selected according to bit 1
(LRP) of parameter No. 1401.
• Nonlinear interpolation type positioning
The tool is positioned with the rapid traverse rate for each axis
separately. The tool path is normally straight.
• Linear interpolation type positioning
The tool is positioned within the shortest possible time at a speed
that is not more than the rapid traverse rate for each axis.
End position Non linear interpolation type positioning
Start position
Linear interpolation type positioning
The rapid traverse rate in G00 command is set to the parameter No.
1420 for each axis independently by the machine tool builder. In the
positioning mode actuated by G00, the tool is accelerated to a
predetermined speed at the start of a block and is decelerated at the
end of a block. Execution proceeds to the next block after confirming
the in-position.
"In-position " means that the feed motor is within the specified range.
This range is determined by the machine tool builder by setting to
parameter (No. 1826).
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 52 -
Limitation
The rapid traverse rate cannot be specified in the address F.
Even if linear interpolation type positioning is specified, nonlinear
type interpolation positioning is used in the following cases. Therefore,
be careful to ensure that the tool does not foul the workpiece.
• G28 specifying positioning between the reference and
intermediate positions.
• G53
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 53 -
4.2 SINGLE DIRECTION POSITIONING (G60)
For accurate positioning without play of the machine (backlash), final
positioning from one direction is available.
Start point
Temporary stop
End point
Overrun
Start point
Format
G60 IP_ ;
IP_ : For an absolute programming, the coordinates of an
end point, and for an incremental programming, the
distance the tool moves.
Explanation
An overrun and a positioning direction are set by the parameter No.
5440. Even when a commanded positioning direction coincides with
that set by the parameter, the tool stops once before the end point.
G60, which is a one-shot G-code, can be used as a modal G-code in
group 01 by setting 1 to the bit 0 (MDL) of parameter No. 5431.
This setting can eliminate specifying a G60 command for every block.
Other specifications are the same as those for a one-shot G60
command. When a one-shot G code is specified in the single direction
positioning mode, the one-shot G command is effective like G codes
in group 01.
(Example)
When one-shot G60 commands are used.
G90;
G60 X0Y0;
G60 X100;
G60 Y100;
G04 X10;
G00 X0Y0;
Single direction positioning
When modal G60 command is used.
G90G60;
X0Y0;
X100;
Y100;
G04X10;
G00X0 Y0;
Single direction positioning mode start
Single direction positioning
Single direction positioning mode cancel
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 54 -
- Overview of operation
• In the case of positioning of non-linear interpolation type (bit
1 (LRP) of parameter No. 1401 = 0)
As shown below, single direction positioning is performed
independently along each axis.
Programmed end point
Programmed start point
Overrun distance in the
X-axis direction
Overrun distance in the Z-axis direction
Z
X
• In the case of positioning of linear interpolation type (bit 1
(LRP) of parameter No. 1401 = 1)
Positioning of interpolation type is performed until the tool once
stops before or after a specified end point. Then, the tool is
positioned independently along each axis until the end point is
reached.
Programmed end point
Programmed start point
Overrun distance in the
X-axis direction
Overrun distance in the Z-axis direction
Z
X
Limitation
• Single direction positioning is not performed along an axis for
which no overrun distance is set in parameter No. 5440.
• Single direction positioning is not performed along an axis for
which travel distance 0 is specified.
• The mirror image function is not applied in a parameter-set
direction. Even in the mirror image mode, the direction of single
direction positioning remains unchanged. If positioning of linear
interpolation type is used, and the state of mirror image when a
single direction positioning block is looked ahead differs from
the state of mirror image when the execution of the block is
started, an alarm is issued. When switching mirror image in the
middle of a program, disable looking ahead by specifying a
non-buffering M code. Then, switch mirror image when there is
no look-ahead block.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 55 -
• In the cylindrical interpolation mode (G07.1), single direction
positioning cannot be used.
• In the polar coordinate interpolation mode (G12.1), single
direction positioning cannot be used.
• When specifying single direction positioning on a machine that
uses arbitrary angular axis control, first position the angular axis
then specify the positioning of the Cartesian axis. If the reverse
specification order is used, or the angular axis and Cartesian axis
are specified in the same block, an incorrect positioning direction
can result.
• In positioning at a restart position by program restart function,
single direction positioning is not performed.
M
• During canned cycle for drilling, no single direction positioning
is effected in drilling axis.
• The single direction positioning does not apply to the shift
motion in the canned cycles of G76 and G87.
T
• The G-code for single direction positioning is always G60, if
G-code system is A or B or C in all case.
• The single direction positioning can not be commanded during
the multiple repetitive cycle (G70-G76).
• No single direction positioning is effected in the drilling or
patting axis, during canned cycle for drilling (G83-G89) and the
rigid tapping (G84, G88). However, it can be commanded for
positioning.
• The single direction positioning can not be commanded during
the canned cycle (G90, G92, G94).
• During the single direction positioning mode (G60), the
following G-code can not be commanded.
G07.1, G12.1, G70-G76, G90-G94.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 56 -
4.3 LINEAR INTERPOLATION (G01)
Tools can move along a line.
Format
G01 IP_ F_ ;
IP_ : For an absolute programming, the coordinates of an
end point, and for an incremental programming, the
distance the tool moves.
F_ : Speed of tool feed (Feedrate)
Explanation
A tools move along a line to the specified position at the feedrate
specified in F.
The feedrate specified in F is effective until a new value is specified.
It need not be specified for each block.
The feedrate commanded by the F code is measured along the tool
path. If the F code is not commanded, the feedrate is regarded as zero.
The feedrate of each axis direction is as follows.
G01 αα ββ γγ ζζ Ff ;
Feed rate of α axis direction : f
L
F×=
α
α
Feed rate of β axis direction : f
L
F×=
β
β
Feed rate of γ axis direction : f
L
F×=
γ
γ
Feed rate of ζ axis direction : f
L
F×=
ζ
ζ
2222
ζγβα
+++=L
The feedrate of the rotary axis is commanded in the unit of deg/min
(the unit is decimal point position).
When the straight line axis α (such as X, Y, or Z) and the rotating axis
β (such as A, B, or C) are linearly interpolated, the feedrate is that in
which the tangential feedrate in the α and β cartesian coordinate
system is commanded by F (mm/min).
β-axis feedrate is obtained ; at first, the time required for distribution
is calculated by using the above formula, then the β-axis feedrate unit
is changed to deg/min.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 57 -
A calculation example is as follows.
G91 G01 X20.0B40.0 F300.0 ;
This changes the unit of the C axis from 40.0 deg to 40mm
with metric input. The time required for distribution is
calculated as follows:
300
4020 22 +)(14907.0 mm
The feedrate for the C axis is
14907.0
40 mindeg/3.268
In simultaneous 3 axes control, the feedrate is calculated the same way
as in 2 axes control.
Example
- Linear interpolation
• For milling machining
(G91) G01X200.0Y100.0F200.0;
Y axis
100.0
200.0
0 (Start point)
(End point)
X axis
• For lathe cutting
(Diameter programming)
G01X40.0Z20.1F20; (Absolute programming)
or
G01U20.0W-25.9F20; (Incremental programming)
Z
20.1
46.0
φ20.0
X
φ40.0
Start
point
End
point
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 58 -
- Feedrate for the rotary axis
90°
(Start point)
(End point)
Feedrate is 300 deg/min
G91G01C-90.0 F300.0 ;Feed rate of 300deg/min
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 59 -
4.4 CIRCULAR INTERPOLATION (G02, G03)
The command below will move a tool along a circular arc.
Format
Arc in the XpYp plane
G02 I_ J_
G17 G03 Xp_ Yp_ R_ F_ ;
Arc in the ZpXp plane
G02 I_ K_G18
G03 Zp_ Xp_ R_ F_ ;
Arc in the YpZp plane
G02 J_ K_
G19 G03 Yp_ Zp_ R_ F_ ;
Command Description
G17 Specification of arc on XpYp plane
G18 Specification of arc on ZpXp plane
G19 Specification of arc on YpZp plane
G02 Circular Interpolation : Clockwise direction (CW)
G03 Circular Interpolation : Counterclockwise direction (CCW)
Xp_ Command values of X axis or its parallel axis
(set by parameter No. 1022)
Yp_
Command values of Y axis or its parallel axis
(set by parameter No. 1022)
Zp_
Command values of Z axis or its parallel axis
(set by parameter No. 1022)
I_ Xp axis distance from the start point to the center of an arc
with sign
J_ Yp axis distance from the start point to the center of an arc
with sign
K_ Zp axis distance from the start point to the center of an arc
with sign
R_ Arc radius (with sign, radius value for lathe cutting)
F_ Feedrate along the arc
T
NOTE
The U-, V-, and W-axes can be used with G-codes
B and C.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 60 -
Explanation
- Direction of the circular interpolation
"Clockwise"(G02) and "counterclockwise"(G03) on the XpYp plane
(ZpXp plane or YpZp plane) are defined when the XpYp plane is
viewed in the positive-to-negative direction of the Zp axis (Yp axis or
Xp axis, respectively) in the Cartesian coordinate system. See the
figure below.
G02
G03
X
G17 G18 G19
G02
G03
Z
G02
G03
Y
YZ
X
- Distance moved on an arc
The end point of an arc is specified by address Xp, Yp or Zp, and is
expressed as an absolute or incremental value according to G90 or
G91. For the incremental value, the distance of the end point which is
viewed from the start point of the arc is specified with sign.
- Distance from the start point to the center of arc
The arc center is specified by addresses I, J, and K for the Xp, Yp, and
Zp axes, respectively. The numerical value following I, J, or K,
however, is a vector component in which the arc center is seen from
the start point, and is always specified as an incremental value
irrespective of G90 and G91, as shown below.
I, J, and K must be signed according to the direction.
End point (x,y)
Center
Start
point
End point (z,x) End point (y,z)
Start
point
Start
point
Center Center
i
x
yx
z
k
z
y
j
j
ik
I0, J0, and K0 can be omitted.
If the difference between the radius at the start point and that at the
end point exceeds the permitted value in a parameter (No.3410), an
alarm PS0020 occurs.
- Command for a circle
When Xp, Yp, and Zp are omitted (the end point is the same as the
start point) and the center is specified with I, J, and K, a 360° arc
(circle) is specified.
G02 I_ ; Command for a circle
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 61 -
- Arc radius
The distance between an arc and the center of a circle that contains the
arc can be specified using the radius, R, of the circle instead of I, J,
and K.
In this case, one arc is less than 180°, and the other is more than 180°
are considered. When an arc exceeding 180° is commanded, the radius
must be specified with a negative value. If Xp, Yp, and Zp are all
omitted, if the end point is located at the same position as the start
point and when R is used, an arc of 0° is programmed
G02R_ ; (The cutter does not move.)
r=50mm
End point
Start point r=50mm
<1>
<2>
For arc <1> (less than 180°)
G91 G02 XP60.0 YP55.0 R50.0 F300.0 ;
For arc <2> (greater than 180°)
G91 G02 XP60.0 YP55.0 R-50.0 F300.0 ;
Y
X
- Feedrate
The feedrate in circular interpolation is equal to the feedrate specified
by the F code, and the feedrate along the arc (the tangential feedrate of
the arc) is controlled to be the specified feedrate.
The error between the specified feedrate and the actual tool feedrate is
±2% or less. However, this feedrate is measured along the arc after the
tool radius compensation is applied
Limitation
- Simultaneously specifying R with I, J, and K
If I, J, K, and R addresses are specified simultaneously, the arc
specified by address R takes precedence and the other are ignored.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 62 -
- Specifying an axis that is not contained in the specified plane
If an axis not comprising the specified plane is commanded, an alarm
PS0028 occurs.
For example,
For milling machining:
If the X-axis and a U-axis parallel to the X-axis are specified when the
XY plane is specified
For lathe cutting:
If the X-axis and a U-axis parallel to the X-axis are specified when the
ZX plane is specified with G code system B or C
- Specifying a semicircle with R
When an arc having a center angle approaching 180° is specified, the
calculated center coordinates may contain an error. In such a case,
specify the center of the arc with I, J, and K.
- Difference in the radius between the start and end points
If the difference in the radius between the start and end points of the
arc exceeds the value specified in parameter No. 3410, alarm PS0020
is generated.
When an end point does not lie on the arc, a spiral results, as shown
below.
γe
γ(t)
γs
Start point
Center
End point
θ(t) θ
Start point
End point
Center θ
θ
γs
γe
Radius
θ
ts)e(
s(t)
)(θγγ
γγ −
+=
The arc radius changes linearly with the center angle θ(t). Spiral
interpolation is performed using a circular command that specifies one
arc radius for the start point and another arc radius for the end point.
To use spiral interpolation, set a large value in parameter No. 3410,
used to specify the limit on the arc radius error.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 63 -
Example
M
100
60
40
090 120 140 200
60
50
Y axis
X axis
The above tool path can be programmed as follows;
(1) In absolute programming
G92X200.0 Y40.0 Z0 ;
G90 G03 X140.0 Y100.0 R60.0 F300. ;
G02 X120.0 Y60.0 R50.0 ;
or
G92X200.0 Y40.0Z0 ;
G90 G03 X140.0 Y100.0I-60.0 F300. ;
G02 X120.0 Y60.0I-50.0 ;
(2) In incremental programming
G91 G03 X-60.0 Y60.0 R60.0 F300. ;
G02 X-20.0 Y-40.0 R50.0 ;
or
G91 G03 X-60.0 Y60.0 I-60.0 F300. ;
G02 X-20.0 Y-40.0 I-50.0 ;
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 64 -
T
- Command of circular interpolation X, Z
Start point
X
Z-axis
X-axis
Center of arc
End point
ZK
X
Z-axis
X-axis
(Diameter
programming)
K
Z
Start point
X
Z-axis
X-axis
Center of arc
End point
Z
R
(Diameter
programming)
(Absolute programming) (Absolute programming) (Absolute programming)
G02X_Z_I_K_F_; G03X_Z_I_K_F_; G02X_Z_R_F_;
(Diameter programming)
I
I
Start point
End point
(Diameter programming)
G02X50.0Z30.0I25.0F0.3; or
G02U20.0W-20.0I25.0F0.3; or
G02X50.0Z30.0R25.0F0.3 or
G02U20.0W-20.0R25.F0.3;
Z
φ50.0
X
10.0 15.0
30.0
50.0
R25.0
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 65 -
4.5 HELICAL INTERPOLATION (G02, G03)
Helical interpolation which moved helically is enabled by specifying
up to two other axes which move synchronously with the circular
interpolation by circular commands.
Format
Arc in the XpYp plane
G02 I_ J_
G17 G03 Xp_ Yp_ R_ α_ (β_) F_ ;
Arc in the ZpXp plane
G02 K_ I_
G18 G03 Zp_ Xp_ R_ α_ (β_) F_ ;
Arc in the YpZp plane
G02 J_ K_
G19 G03 Yp_ Zp_ R_ α_ (β_) F_ ;
α, β : Any one axis where circular interpolation is not
applied.
Up to two other axes can be specified.
Explanation
A tangential velocity of an arc in a specified plane or a tangential
velocity about the linear axis can be specified as the feedrate,
depending on the setting of bit 5 (HTG) of parameter No.1403.
An F command specifies a feedrate along a circular arc, when HTG is
specified to 0. Therefore, the feedrate of the linear axis is as follows:
Length of linear axis
F ×
Length of circular arc
Determine the feedrate so the linear axis feedrate does not exceed any
of the various limit values.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 66 -
The feedrate along the circumference of two circular
interpolated axes is the specified feedrate.
Z
XY
Tool path
If HTG is set to 1, specify a feedrate along the tool path about the
linear axis. Therefore, the tangential velocity of the arc is expressed as
follows:
Length of arc
F ×
(Length of arc)2 + (Length of linear axis)2
The velocity along the linear axis is expressed as follows:
Length of linear axis
F ×
(Length of arc)2 + (Length of linear axis)2
Z
Y
X
The feedrate along the tool path is specified.
Tool path
Limitation
• Tool radius/tool nose radius compensation is applied only for a
circular arc.
• Tool offset and tool length compensation cannot be used in a block
in which a helical interpolation is commanded.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 67 -
4.6 HELICAL INTERPOLATION B (G02, G03)
The helical interpolation B function differs from the helical
interpolation function just in that circular interpolation and a
movement on four axes outside the specified plane can be
simultaneously performed.
For the restrictions and parameters, see the description of the helical
interpolation function.
Format
Arc in the XpYp plane
G02 I_ J_ G17
G03 Xp_ Yp_ R_ α_ β_ γ_ δ_ F_ ;
Arc in the ZpXp plane
G02 K_ I_
G18 G03 Zp_ Xp_ R_ α_ β_ γ_ δ_ F_ ;
Arc in the YpZp plane
G02 J_ K_
G19 G03 Yp_ Zp_ R_ α_ β_ γ_ δ_ F_ ;
α, β, γ, δ : Any axis to which circular interpolation is not
applied.
Up to four axes can be specified.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 68 -
4.7 SPIRAL INTERPOLATION, CONICAL INTERPOLATION
(G02, G03)
Spiral interpolation is enabled by specifying the circular interpolation
command together with a desired number of revolutions or a desired
increment (decrement) for the radius per revolution.
Conical interpolation is enabled by specifying the spiral interpolation
command together with an additional axis of movement, as well as a
desired increment (decrement) for the position along the additional
axes per spiral revolution.
Format
- Spiral interpolation
XpYp plane
G02
G17 G03 X_Y_I_J_Q_L_F_;
ZpXp plane
G02
G18 G03 Z_X_K_I_Q_L_F_;
YpZp plane
G02
G19 G03 Y_Z_J_K_Q_L_F_;
X, Y, Z : Coordinates of the end point
L : Number of revolutions (positive value without a decimal point) (*1)
Q : Radius increment or decrement per spiral revolution (*1, *2)
I, J, K : Signed distance from the start point to the center (same as the distance
specified for circular interpolation)
F : Feedrate
(*1) Either the number of revolutions (L) or the radius increment or decrement (Q)
can be omitted. When L is omitted, the number of revolutions is automatically
calculated from the distance between the current position and the center, the
position of the end point, and the radius increment or decrement. When Q is
omitted, the radius increment or decrement is automatically calculated from the
distance between the current position and the center, the position of the end
point, and the number of revolutions. If both L and Q are specified but their
values contradict, Q takes precedence. Generally, either L or Q should be
specified. The L value must be a positive value without a decimal point. To
specify four revolutions plus 90°, for example, round the number of revolutions
up to five and specify L5.
(*2) The increment system for Q depends on the reference axis.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 69 -
- Conical interpolation
XpYp plane
G02
G17 G03 X_ Y_ I_ J_ Z_ Q_ L_ F_ ;
ZpXp plane
G02
G18 G03 Z_ X_ K_ I_ Y_ Q_ L_ F_ ;
YpZp plane
G02
G19 G03 Y_ Z_ J_ K_ X_ Q_ L_ F_ ;
X, Y, Z : Coordinates of the end point
L : Number of revolutions (positive value without a decimal point) (*1)
Q : Radius increment or decrement per spiral revolution (*1, *2)
I, J, K : Two of the three values represent a signed vector from the start point to
the center. The remaining value is a height increment or decrement per
spiral revolution in conical interpolation. (*1)
When the XpYp plane is selected:
The I and J values represent a signed vector from the start point to the
center. The K value represents a height increment or decrement per
spiral revolution.
When the ZpXp plane is selected:
The K and I values represent a signed vector from the start point to the
center. The J value represents a height increment or decrement per
spiral revolution.
When the YpZp plane is selected:
The J and K values represent a signed vector from the start point to the
center. The I value represents a height increment or decrement per
spiral revolution.
F : Feedrate (The tangential velocity about the linear axis is specified.)
(*1) One of the height increment/decrement (I, J, K), radius increment/decrement
(Q), and the number of revolutions (L) must be specified. The other two items
can be omitted.
• Sample command for the XpYp plane
G02 K_
Q_ G18 G03 X_ Y_ I_ J_ Z_
L_
F_ ;
If both L and Q are specified, but their values contradict, Q takes precedence.
If both L and a height increment or decrement are specified, but their values
contradict, the height increment or decrement takes precedence. If both Q
and a height increment or decrement are specified, but their values
contradict, Q takes precedence. The L value must be a positive value without
a decimal point. To specify four revolutions plus 90°, for example, round the
number of revolutions up to five and specify L5.
(*2) The increment system for Q depends on the reference axis.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 70 -
Explanation
- Function of spiral interpolation
Spiral interpolation in the XY plane is defined as follows:
22
0
2
0)Q'(R)Y(Y)X(X
+
=
−
+
−
X0 : X coordinate of the center
Y0 : Y coordinate of the center
R : Radius at the beginning of spiral interpolation
Q' : Variation in radius
When the programmed command is assigned to this function, the
following expression is obtained:
222 )Q)
360
(L'(RJ)Y(YI)X(X SS
θ
++=−−+−−
where
XS : X coordinate of the start point
YS : Y coordinate of the start point
I : X coordinate of the vector from the start point to the
center
J : Y coordinate of the vector from the start point to the
center
R : Radius at the beginning of spiral interpolation
Q : Radius increment or decrement per spiral revolution
L' : (Current number of revolutions) - 1
θ : Angle between the start point and the current position
(degrees)
- Controlled axes
For conical interpolation, two axes of a plane and two additional axes,
that is, four axes in total, can be specified. A rotary axis can be
specified as the additional axis.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 71 -
- Difference between end points
If the difference between the programmed end point and the calculated
end point of a spiral exceeds a value specified in parameter No. 3471
about any axis of a selected plane, an alarm PS5123 will be issued.
If the difference between the programmed height and calculated height
of the end point a cone exceeds a value specified in parameter No.
3471, an alarm PS5123 will be issued. The figure below illustrates
details.
G90 G02 X0 Y-33.5 I0 J-100. F300;
Q-20.
L4
The coordinates of the programmed end point are (0, -33.5) while the coordinates of
the calculated end point are (0, -30.0). A value greater than the difference (α:
Tolerance) is specified in parameter No. 3471. If the end point is exceeded, an alarm
PS5123 will be issued. The same is specified for the height of conical interpolation.
-33.5
-30.0
100.0
Y
X
20.0
20.0
20.0
α
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 72 -
- Tool radius compensation
M
The spiral or conical interpolation command can be programmed in
tool radius compensation mode. This compensation is performed in
the same way as described in "When it is exceptional" in "Tool
Movement in Offset Mode" section. A virtual circle centered on the
center of spiral interpolation is thought at the end of a block. The tool
path is obtained by performing tool radius compensation along the
virtual circle and the blocks before and after the spiral interpolation.
When the end point of the block is at the center of the spiral
interpolation, no virtual circle can be drawn. If drawing is attempted,
an alarm PS5124 is issued.
Programmed spiral
interpolation
Virtual circle
Tool center path
r
r
Center
After cutter
compensation
- Actual cutting feedrate
A constant speed is maintained in spiral interpolation or conical
interpolation. The angular velocity near the center, however, may
increase because of the small radius of the spiral. This can be avoided
by maintaining the angular velocity after the radius of the spiral
reaches a value specified in parameter No. 3472. Consequently, the
actual cutting feedrate decreases.
An example is illustrated below.
Specified feedrate: F100.
Parameter 3472 (r) = 1.000
IS-B
While the radius of the spiral shown
at the left is greater than the value
specified in parameter No. 3472, the
actual cutting feedrate is F100. As
the radius decreases, the actual
feedrate also decreases, the actual
feedrate near the end point being
about F65.
r
1.5
-0.5
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 73 -
- Deceleration by acceleration
During spiral interpolation, the function of deceleration by
acceleration is enabled. The feedrate may decrease as the tool
approaches the center of the spiral.
- Dry run
When the dry run signal is inverted from 0 to 1 or from 1 to 0 during
movement along an axis, the movement is accelerated or decelerated
to the desired speed without first reducing the speed to zero.
Limitation
- Radius
During spiral interpolation and conical interplation, the addresses "C",
"R", ",C", or ",R" cannot be specified.
- Feed functions
The functions of feed per rotation, inverse time feed, F command with
one digit, and automatic corner override cannot be used.
- Retrace
A program including spiral or conical interpolation cannot be retraced.
- Polar coordinate interpolation, scaling, and normal direction control
Spiral interpolation and conical interpolation cannot be specified in
these modes.
- Optional function
To use the conical interpolation function, the optional function for
helical interpolation is also necessary.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 74 -
Example
- Spiral interpolation
The path indicated below is programmed with absolute and
incremental values as follows:
-120 -100 -80 -60 -40
–
20 20 40 60 80 100 120
20
Y axis
X axis
40
60
80
100
20. 20.
-20
-40
-60
-80
-100
-120
120
This sample path has the following values:
• Start point : (0, 100.0)
• End point (X, Y) : (0, -30.0)
• Distance to the center (I, J) : (0, -100.0)
• Radius increment or decrement (Q) : -20.0
• Number of revolutions (L) : 4
(1) With absolute values, the path is programmed as follows:
Q-20.0
G90 G02 X0 Y-30.0 I0 J-100.0 L4 F300.0 ;
(2) With incremental values, the path is programmed as follows:
Q-20.0
G91 G02 X0 Y-130.0 I0 J-100.0 L4 F300.0 ;
(Either the Q or L setting can be omitted.)
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 75 -
- Conical interpolation
The sample path shown below is programmed with absolute and
incremental values as follows:
+Z
+Y
+X
(0,-37.5,62.5)
25.0 25.0
25.0
25.0
100.0
-100.0
This sample path has the following values:
• Start point : (0, 100.0, 0)
• End point (X, Y, Z) : (0, -37.5, 62.5)
• Distance to the center (I, J) : (0, -100.0)
• Radius increment or decrement (Q) : -25.0
• Height increment or decrement (K) : 25.0
• Number of revolutions (L) : 3
(1) With absolute values, the path is programmed as follows:
G90 G02 X0 Y-37.5 Z62.5 I0 J-100.0 K25.0
Q-25.0
L3
F300.0 ;
(2) With incremental values, the path is programmed as follows:
G91 G02 X0 Y-137.5 Z62.5 I0 J-100.0
K25.0
Q-25.0
L3
F300.0;
(Either the Q or L setting can be omitted.)
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 76 -
4.8 POLAR COORDINATE INTERPOLATION (G12.1, G13.1)
Overview
Polar coordinate interpolation is a function that exercises contour
control in converting a command programmed in a Cartesian
coordinate system to the movement of a linear axis (movement of a
tool) and the movement of a rotary axis (rotation of a workpiece).
This function is useful for grinding a cam shaft.
Format
G12.1; Starts polar coordinate interpolation mode
(enables polar coordinate interpolation).
Specify linear or circular interpolation using
coordinates in a Cartesian coordinate system
consisting of a linear axis and rotary axis
(hypothetical axis).
G13.1; Polar coordinate interpolation mode is
cancelled (for not performing polar coordinate
interpolation).
Specify G12.1 and G13.1 in Separate Blocks.
Explanation
- Polar coordinate interpolation mode (G12.1)
The axes of polar coordinate interpolation (linear axis and rotary axis)
should be specified in advance, with corresponding parameters.
Specifying G12.1 places the system in the polar coordinate
interpolation mode, and selects a plane (called the polar coordinate
interpolation plane) formed by one linear axis and a hypothetical axis
intersecting the linear axis at right angles. The linear axis is called the
first axis of the plane, and the hypothetical axis is called the second
axis of the plane. Polar coordinate interpolation is performed in this
plane.
In the polar coordinate interpolation mode, both linear interpolation
and circular interpolation can be specified by absolute or incremental
programming.
Tool radius compensation can also be performed. The polar coordinate
interpolation is performed for a path obtained after tool radius
compensation.
The tangential velocity in the polar coordinate interpolation plane
(Cartesian coordinate system) is specified as the feedrate, using F.
- Polar coordinate interpolation cancel mode (G13.1)
Specifying G13.1 cancels the polar coordinate interpolation mode.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 77 -
- Polar coordinate interpolation plane
G12.1 starts the polar coordinate interpolation mode and selects a
polar coordinate interpolation plane (Fig. 4.8 (a)). Polar coordinate
interpolation is performed on this plane.
Rotary axis (hypothetical axis)
(unit: mm or inch)
Linear axis
(unit: mm or inch)
Origin of the local coordinate system (G52 command)
(Or origin of the workpiece coordinate system)
Fig. 4.8 (a) Polar coordinate interpolation plane
When the power is turned on or the system is reset, polar coordinate
interpolation is canceled (G13.1).
The linear and rotation axes for polar coordinate interpolation must be
set in parameters Nos. 5460 and 5461 beforehand.
CAUTION
The plane used before G12.1 is specified (plane
selected by G17, G18, or G19) is canceled. It is
restored when G13.1 (canceling polar coordinate
interpolation) is specified.
When the system is reset, polar coordinate
interpolation is canceled and the plane specified by
G17, G18, or G19 is used.
- Distance moved and feedrate for polar coordinate interpolation
• The unit for coordinates on the hypothetical axis is the same as
the unit for the linear axis (mm/inch).
In the polar coordinate interpolation mode, program commands
are specified with Cartesian coordinates on the polar coordinate
interpolation plane. The axis address for the rotary axis is used as
the axis address for the second axis (hypothetical axis) in the
plane. Whether a diameter or radius is specified for the first axis
in the plane is the same as for the rotary axis regardless of the
specification for the first axis in the plane.
The hypothetical axis is at coordinate 0 immediately after G12.1
is specified. Polar interpolation is started assuming the rotation
angle of 0 for the position of the tool when G12.1 is specified.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 78 -
Example)
When a value on the X-axis (linear axis) is input in
millimeters
G12.1;
G01 X10. F1000. ;.... A 10-mm movement is made on the
Cartesian coordinate system.
C20. ; ........................ A 20-mm movement is made on the
Cartesian coordinate system.
G13.1;
When a value on the X-axis (linear axis) is input in inches
G12.1;
G01 X10. F1000. ; .. A 10-inch movement is made on the
Cartesian coordinate system.
C20. ; ........................ A 20-inch movement is made on the
Cartesian coordinate system.
G13.1;
• The unit for the feedrate is mm/min or inch/min.
Specify the feedrate as a speed (relative speed between the
workpiece and tool) tangential to the polar coordinate
interpolation plane (Cartesian coordinate system) using F.
- G codes which can be specified in the polar coordinate interpolation mode
G01 .......................Linear interpolation
G02, G03...............Circular interpolation
G02.2, G03.2.........Involute interpolation
G04 .......................Dwell, Exact stop
G40, G41, G42......Tool radius compensation
(Polar coordinate interpolation is applied to the
path after tool radius compensation.)
G65, G66, G67......Custom macro command
G90, G91...............Absolute programming, incremental programming
G94, G95...............Feed per minute, feed per revolution
- Circular interpolation in the polar coordinate plane
The addresses for specifying the radius of an arc for circular
interpolation (G02 or G03) in the polar coordinate interpolation plane
depend on the first axis in the plane (linear axis).
• I and J in the Xp-Yp plane when the linear axis is the X-axis or
an axis parallel to the X-axis.
• J and K in the Yp-Zp plane when the linear axis is the Y-axis or
an axis parallel to the Y-axis.
• K and I in the Zp-Xp plane when the linear axis is the Z-axis or
an axis parallel to the Z-axis.
The radius of an arc can be specified also with an R command.
NOTE
In a lathe system, the parallel axes U, V, and W
can be used in the G code system B or C.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 79 -
- Movement along axes not in the polar coordinate interpolation plane in the polar
coordinate interpolation mode
The tool moves along such axes normally, independent of polar
coordinate interpolation.
- Current position display in the polar coordinate interpolation mode
Actual coordinates are displayed. However, the remaining distance to
move in a block is displayed based on the coordinates in the polar
coordinate interpolation plane (Cartesian coordinates).
- Coordinate system for the polar coordinate interpolation
Basically, before G12.1 is specified, a local coordinate system (or
workpiece coordinate system) where the center of the rotary axis is the
origin of the coordinate system must be set.
- Compensation in the direction of the hypothetical axis in polar coordinate
interpolation
If the first axis of the plane has an error from the center of the rotary
axis in the hypothetical axis direction, in other words, if the rotary
axis center is not on the X-axis, the hypothetical axis direction
compensation function in the polar coordinate interpolation mode is
used. With the function, the error is considered in polar coordinate
interpolation. The amount of error is specified in parameter No. 5464.
(X, C)
Hypothetical axis (C-axis)
Error in the direction of
hypothetical axis (P)
Center of rotary axis
X-axis
Rotary axis
(X, C) Point in the X-C plane (The center of the rotary axis is
considered to be the origin of the X-C plane.)
X X coordinate in the X-C plane
C Hypothetical axis coordinate in the X-C plane
P Error in the direction of the hypothetical axis
(specified in parameter No. 5464)
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 80 -
- Shifting the coordinate system in polar coordinate interpolation
In the polar coordinate interpolation mode, the workpiece coordinate
system can be shifted. The current position display function shows the
position viewed from the workpiece coordinate system before the shift.
The function to shift the coordinate system is enabled when bit 2
(PLS) of parameter No. 5450 is specified accordingly.
The shift can be specified in the polar coordinate interpolation mode,
by specifying the position of the center of the rotary axis C (A, B) in
the X-C (Y-A, Z-B) interpolation plane with reference to the origin of
the workpiece coordinate system, in the following format.
G12.1 X_ C_ ; (Polar coordinate interpolation for the X-axis and C-axis)
G12.1 Y_ A_ ; (Polar coordinate interpolation for the Y-axis and A-axis)
G12.1 Z_ B_ ; (Polar coordinate interpolation for the Z-axis and B-axis)
X
C
x
c
Center of C-axis
G12.1 Xx Cc ;
Origin of workpiece
coordinate system
Limitation
- Changing the coordinate system during polar coordinate interpolation
In the G12.1 mode, the coordinate system must not be changed (G92,
G52, G53, relative coordinate reset, G54 through G59, etc.).
- Tool radius/tool nose radius compensation
The polar coordinate interpolation mode (G12.1 or G13.1) cannot be
started or terminated in the tool radius/tool nose radius compensation
mode (G41 or G42). G12.1 or G13.1 must be specified in the tool
radius/tool nose radius compensation canceled mode (G40).
- Tool length offset command
Tool length offset must be specified in the polar coordinate
interpolation cancel mode before G12.1 is specified. It cannot be
specified in the polar coordinate interpolation mode. Furthermore, no
offset values can be changed in the polar coordinate interpolation
mode.
- Tool offset command
A tool offset must be specified before the G12.1 mode is set. No offset
can be changed in the G12.1 mode.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 81 -
- Program restart
For a block in the G12.1 mode, the program and the block cannot be
restarted.
- Cutting feedrate for the rotary axis
Polar coordinate interpolation converts the tool movement for a figure
programmed in a Cartesian coordinate system to the tool movement in
the rotary axis (C-axis) and the linear axis (X-axis). When the tool
comes close to the center of the workpiece, the C-axis velocity
component increases. If the maximum cutting feedrate for the C-axis
(parameter No. 1430) is exceeded, the automatic feedrate override
function and automatic speed clamp function are enabled.
If the maximum cutting feedrate for the X-axis is exceeded, the
automatic feedrate override function and automatic speed clamp
function are enabled.
WARNING
1 Consider lines L1, L2, and L3. ∆X is the distance the tool moves per time unit at the
feedrate specified with address F in the Cartesian coordinate system. As the tool
moves from L1 to L2 to L3, the angle at which the tool moves per time unit
corresponding to ∆X in the Cartesian coordinate system increases from θ1 to θ2 to
θ3. In other words, the C-axis component of the feedrate becomes larger as the
tool moves closer to the center of the workpiece. The C component of the feedrate
may exceed the maximum cutting feedrate for the C-axis because the tool
movement in the Cartesian coordinate system has been converted to the tool
movement for the C-axis and the X-axis.
L1
L2
L3
θ
3
θ
2
θ
1
∆X
L: Distance (in mm) between the tool center and workpiece center when the tool
center is the nearest to the workpiece center
R: Maximum cutting feedrate (deg/min) of the C axis
Then, a speed specifiable with address F in polar coordinate interpolation can be
given by the formula below. If the maximum cutting feedrate for the C-axis is
exceeded, the automatic speed control function for polar coordinate interpolation
automatically controls the feedrate.
F < L × R × 180
π
(mm/min)
2 The following function cannot be used for the rotary axis of polar coordinate
interpolation.
• Index table indexing function
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 82 -
- Automatic speed control for polar coordinate interpolation
If the velocity component of the rotary axis exceeds the maximum
cutting feedrate in the polar coordinate interpolation mode, the speed
is automatically controlled.
- Automatic override
If the velocity component of the rotary axis exceeds the permissible
velocity (maximum cutting feedrate multiplied by the permission
factor specified in parameter No. 5463), the feedrate is automatically
overridden as indicated below.
Override = (Permissible velocity) ÷ (Velocity component of rotary
axis) × 100(%)
- Automatic speed clamp
If the velocity component of the rotary axis after automatic override
still exceeds the maximum cutting feedrate, the speed of the rotary
axis is automatically clamped. As a result, the velocity component of
the rotary axis will not exceed the maximum cutting feedrate.
The automatic speed clamp function works only when the center of
the tool is very close to the center of the rotary axis.
C-axis
A
B C D
X-axis
-10. +10.
[Example]
G90 G00 X10.0 C0. ;
G12.1 ;
G01 C0.1 F1000 ;
X-10.0 :
G13.1 ;
Automatic speed control for polar coordinate interpolation
Suppose that the maximum cutting feedrate of the rotary axis is 360
(3600 deg/min) and that the permission factor of automatic override
for polar coordinate interpolation (parameter No. 5463) is 0 (90%).
If the program indicated above is executed, the automatic override
function starts working when the X coordinate becomes 2.273 (point
A). The automatic speed clamp function starts working when the X
coordinate becomes 0.524 (point B).
The minimum value of automatic override for this example is 3%.
The automatic speed clamp function continues working until the X
coordinate becomes -0.524 (point C). Then, the automatic override
function works until the X coordinate becomes -2.273 (point D).
(The coordinates indicated above are the values in the Cartesian
coordinate system.)
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 83 -
NOTE
1 While the automatic speed clamp function is
working, the machine lock or interlock function may
not be enabled immediately.
2 If a feed hold stop is made while the automatic
speed clamp function is working, the automatic
operation halt signal is output. However, the
operation may not stop immediately.
3 The clamped speed may exceed the clamp value
by a few percent.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 84 -
Example
Sample program for polar coordinate interpolation in a Cartesian
coordinate system consisting of the X-axis (a linear axis) and a
hypothetical axis
N204
N205
N206
N203
N202 N201
N208
N207
N200
Tool
C axis
Hypothetical axis
Path after cutter compensation
Program path
X axis
Z axis
O001;
.
No10 T0101
.
N0100 G90 G00 X60.0 C0 Z ; Positioning to start point
N0200 G12.1;
N0201 G42 G01 X20.0F ;
N0202 C10.0;
N0203 G03 X10.0 C20.0 R10.0;
N0204 G01 X-20.0;
N0205 C-10.0;
N0206 G03 X-10.0 C-20.0 I10.0 J0;
N0207 G01 X20.0;
N0208 C0;
N0209 G40 X60.0;
N0210 G13.1;
N0300 Z ;
N0400 X C ;
.
N0900M30;
Start of polar coordinate interpolation
Geometry program
(program based on cartesian
coordinates on X
axis-hypothetical axis plane)
Cancellation of polar coordinate
interpolation
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 85 -
4.9 CYLINDRICAL INTERPOLATION (G07.1)
In cylindrical interpolation function, the amount of movement of a
rotary axis specified by angle is converted to the amount of movement
on the circumference to allow linear interpolation and circular
interpolation with another axis.
Since programming is enabled with the cylinder side face expanded,
programs such as a program for grooving cylindrical cams can be
created very easily.
Format
G07.1 IP r; Starts the cylindrical interpolation mode
(enables cylindrical interpolation).
:
:
:
G07.1 IP 0; The cylindrical interpolation mode is
cancelled.
IP : An address for the rotary axis
r : The radius of the workpiece
Specify G07.1 IPr; and G07.1 IP0; in separate blocks.
G107 can be used instead of G07.1.
Explanation
- Plane selection (G17, G18, G19)
To specify a G code for plane selection, set the rotary axis in
parameter No. 1022 as a linear axis that is one of the basic three axes
of the basic coordinate system or an axis parallel to one of the basic
axes. For example, when rotary axis C-axis is assumed to be parallel
to the X-axis, specifying G17, axis address C, and Y at the same time
can select a plane formed by the C-axis and Y-axis (the Xp-Yp plane).
T
NOTE
The U-, V-, and W-axes can be used with G-codes
B and C.
- Feedrate
A feedrate specified in the cylindrical interpolation mode is the
feedrate on the circumference.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 86 -
- Circular interpolation (G02, G03)
Circular interpolation can be performed between the rotary axis set for
cylindrical interpolation and another linear axis. Radius R is used in
commands in the same way as described.
The unit for a radius is not degrees but millimeters (for metric input)
or inches (for inch input).
<Example Circular interpolation between the Z axis and C axis>
For the C axis of parameter (No.1022), 5 (axis parallel with the X
axis) is to be set. In this case, the command for circular
interpolation is
G18 Z_C_;
G02 (G03) Z_C_R_;
For the C axis of parameter (No.1022), 6 (axis parallel with the Y
axis) may be specified instead. In this case, however, the
command for circular interpolation is
G19 C_Z_;
G02 (G03) Z_C_R_;
- Tool radius/tool nose radius compensation
To perform tool radius/tool nose radius compensation in the
cylindrical interpolation mode, cancel any ongoing tool radius/tool
nose radius compensation mode before entering the cylindrical
interpolation mode. Then, start and terminate tool radius/tool nose
radius compensation within the cylindrical interpolation mode.
- Cylindrical interpolation accuracy
In the cylindrical interpolation mode, the amount of travel of a rotary
axis specified by an angle is once internally converted to a distance of
a linear axis on the outer surface so that linear interpolation or circular
interpolation can be performed with another axis. After interpolation,
such a distance is converted back to an angle. For this conversion, the
amount of travel is rounded to a least input increment.
So when the radius of a cylinder is small, the actual amount of travel
can differ from a specified amount of travel. Note, however, that such
an error is not accumulative.
If manual operation is performed in the cylindrical interpolation mode
with manual absolute on, an error can occur for the reason described
above.
=
travelofamount actual The
×
××
×REV MOTION
R22
valueSpecified
R22
REV MOTION
π
π
MOTION REV : The amount of travel per rotation of the rotary axis
(360°)
R : Workpiece radius
[]
: Rounded to the least input increment
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 87 -
Limitation
- Arc radius specification in the circular interpolation
In the cylindrical interpolation mode, an arc radius cannot be specified
with word address I, J, or K.
- Positioning
In the cylindrical interpolation mode, positioning operations
(including those that produce rapid traverse cycles such as G28, G53,
G73, G74, G76, G80 to G89) cannot be specified. Before positioning
can be specified, the cylindrical interpolation mode must be cancelled.
Cylindrical interpolation (G07.1) cannot be performed in the
positioning mode (G00).
- Cylindrical interpolation mode setting
In the cylindrical interpolation mode, the cylindrical interpolation
mode cannot be reset. The cylindrical interpolation mode must be
cancelled before the cylindrical interpolation mode can be reset.
- Rotary axis
Only one rotary axis can be set for cylindrical interpolation.
Therefore, it is impossible to specify more than one rotary axis in the
G07.1 command.
- Rotary axis roll-over
If a rotary axis using the roll-over function is specified at the start of
the cylindrical interpolation mode, the roll-over function is
automatically disabled in the cylindrical interpolation mode. After the
cylindrical interpolation mode is canceled, the roll-over function is
enabled automatically.
- Rotary axis control function
If a rotary axis using the multiple rotary axis control function is
specified at the start of the cylindrical interpolation mode, the rotary
axis control function is automatically disabled in the cylindrical
interpolation mode. After the cylindrical interpolation mode is
canceled, the rotary axis control function is enabled automatically.
- Tool radius/tool nose radius compensation
If the cylindrical interpolation mode is specified when tool radius/tool
nose radius compensation is already being applied, correct
compensation is not performed. Specify compensation in the
cylindrical interpolation mode.
- Canned cycle for drilling
Canned cycles (G73, G74, and G81 to G89 for M series / G80 to G89
for T series) for drilling, cannot be specified during cylindrical
interpolation mode.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 88 -
M
- Coordinate system setting
In the cylindrical interpolation mode, a workpiece coordinate system
(G92, G54 to G59) or local coordinate system (G52) cannot be
specified.
- Tool offset
A tool offset must be specified before the cylindrical interpolation
mode is set. No offset can be changed in the cylindrical interpolation
mode.
- Index table indexing function
Cylindrical interpolation cannot be specified when the index table
indexing function is being used.
- Parallel axis
The rotary axis specified for cylindrical interpolation must not be a
parallel axis.
T
- Coordinate system setting
In the cylindrical interpolation mode, a workpiece coordinate system
G50 cannot be specified.
- Mirror image for double turret
Mirror image for double turret, G68 and G69, cannot be specified
during cylindrical interpolation mode.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 89 -
Example
Z
C
R
C
230190
150
0
mm
Z
deg
110
90
70
120
30 60 70 270
N05
N06
N07
N08 N09 N10
N11
N12 N13
360
60
Example of a Cylindrical Interpolation
O0001 (CYLINDRICAL INTERPOLATION );
N01 G00 G90 Z100.0 C0 ;
N02 G01 G91 G18 Z0 C0 ;
N03 G07.1 C57299 ;*
N04 G90 G01 G42 Z120.0 D01 F250. ;
N05 C30.0 ;
N06 G03 Z90.0 C60.0 R30.0 ;
N07 G01 Z70.0 ;
N08 G02 Z60.0 C70.0 R10.0 ;
N09 G01 C150.0 ;
N10 G02 Z70.0 C190.0 R75.0 ;
N11 G01 Z110.0 C230.0 ;
N12 G03 Z120.0 C270.0 R75.0 ;
N13 G01 C360.0 ;
N14 G40 Z100.0 ;
N15 G07.1 C0 ;
N16 M30 ;
(* A command with a decimal point can also be used.)
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 90 -
4.10 CUTTING POINT INTERPOLATION FOR CYLINDRICAL
INTERPOLATION (G07.1)
The conventional cylindrical interpolation function controls the tool
center so that the tool axis always moves along a specified path on the
cylindrical surface, towards the rotary axis (cylindrical axis) of the
workpiece. The cutting point interpolation for cylindrical interpolation
function controls the tool so that the tangent of the tool and the cutting
surface of a contour always passes the rotation center of the workpiece.
This means that the cutting surface of the contour is always
perpendicular to the cylinder. With this function, the figure on the
cutting surface can always be kept constant regardless of the tool
radius compensation value of the tool used.
Format
This command is specified in the same way as for the
conventional cylindrical interpolation function.
G07.1 IPr ; Circular interpolation mode on start
(enabling cylindrical interpolation)
:
G07.1 IP0 ; Circular interpolation mode cancel
IP : One rotary axis address
r : Cylinder radius of rotary axis
Specify each of G07.1 IPr; and G07.1 IP0; singly in a block.
G107 can also be specified.
Explanation
- Comparison with conventional circular interpolation
As shown in Fig. 4.10 (a), the tool is controlled in the offset axis
(Y-axis) direction that is perpendicular to the tool center and
workpiece rotation center.
Workpiece
Rotation
axis
Rotation
axis
Tool
Center of
tool
Y-axis
Conventional cylindrical interpolation Cylindrical interpolation with this function
Y-axis
Fig. 4.10 (a) Comparison with conventional circular interpolation
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 91 -
- Cutting point compensation
(1) Cutting point compensation between blocks
As shown in Fig. 4.10 (b), cutting point compensation is
achieved by moving between blocks N1 and N2.
(a) Let C1 and C2 be the heads of the vectors normal to N1 and
N2 from S1, which is the intersection of the tool center
paths of blocks N1 and N2
(b) After the tool moves to S1 according to the command of N1,
the tool moves through V on the C-axis as a result of cutting
point compensation, then through rV ××−
180
π
along the
Y-axis.
Z-axis
C-axis on the
cylindrical surface
Y-a xis
S1
C1
C2
N1
N2
V
Tool center path
Programmed path
V : C-axis component of C1 - C2
C1 : Cutting surface of block N1
C2 : Cutting surface of block N2
Fig.4.10 (b) Cutting point compensation between blocks
(2) Cutting point compensation in a circular command block
As shown in Fig. 4.10 (c), the movement required for cutting
point compensation is made simultaneously with circular
interpolation in block N1.
(a) Let C0 be the head of the vector normal to N1 from S0,
which is the tool center position at the start point of circular
block N1. Let C1 be the head of the similar vector at the end
point.
(b) As the tool moves from S0 to S1, a superimposed
movement is made by the C-axis component of (C1 - C2)
(V in the figure) on the C-axis, and a superimposed
movement is made by rV ××−
180
π
along the Y-axis.
along the Y-axis.
That is, the following expressions are valid. As movement
is made through L as shown in Fig. 4.10 (c), the
superimposed movements are made on the C-axis and
Y-axis as follows:
VC
∆
=
∆
rVY )(
180 ∆−=∆
π
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 92 -
∆V : Cutting point compensation value (∆V2 - ∆V1) for
movement of ∆L
∆V1 : C-axis component of the vector normal to N1 from
the tool center of the start point of ∆L
∆V2 : C-axis component of the vector normal to N1 from
the tool center of the end point of ∆L
R : Arc radius
Z-axis
C-axis on the
cylindrical surface
Y-axis
C0
N1
O
C1
V
Tool center path
Programmed path
V : C-axis component of C1 - C0
C0 : Cutting surface at the start point of block N1
C1 : Cutting surface at the end point of block N1
R
S0
∆V2
∆V1
∆L
C0
S1
Fig.4.10 (c) Cutting point compensation in a circular command block
(3) When cutting point compensation is not applied between blocks
When, as shown in Fig. 4.10 (d) and Fig. 4.10 (e), the cutting
point compensation value (V in the figures) is less than the value
set in parameter No. 19534, one of the operations below is
performed. (The operation that is performed depends on the
setting of bit 6 (CYS) of parameter No.19530.
(a) When bit 6 (CYS) of parameter No.19530 is set to 1
Cutting point compensation is not applied between blocks
N1 and N2, but is applied when block N2 is executed.
Z-axis
C-axis on the
cylindrical surface
Y-axis
S2
C2
C2
V
Tool center path
Programmed path
V : C-axis component of C2 - C1
C1 : Cutting surface of block N1
C2 : Cutting surface after the end of block N1
S1
C1
N1 N2
N3
Fig.4.10 (d) When bit 6 (CYS) of parameter No.19530 is set to 1
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 93 -
(b) When bit 6 (CYS) of parameter No.19530 is set to 0
Cutting point compensation is not performed between
blocks N1 and N2. Whether to apply cutting point
compensation between block N2 and N3 is determined by
taking the cutting point compensation value between blocks
N2 and N3 (V in the figure) into consideration.
Z-axis
C-axis on the
cylindrical surface
Y-axis
S2
C1
C2
V
Tool center path
Programmed path
V : C-axis component of C2 - C1
C1 : Cutting surface of blocks N1 and N2
C2 : Cutting surface at the end of block N3
S1
C1
N1 N2
N3
Fig.4.10 (e) When bit 6 (CYS) of parameter No.19530 is 0
(b) When the amount of travel (L1) of block N2 is less than the
value set in parameter No. 19535, as shown in Fig. 4.10 (f),
cutting point compensation is not applied between blocks
N1 and N2. Instead, block N2 is executed with the cutting
point compensation of the previous block. When the amount
of travel (L2) of block N3 is greater than the value set in
parameter No. 19535, cutting point compensation is applied
between blocks N2 and N3.
Z-axis
C-axis on the
cylindrical surface
Y-axis
C1
C2
V
Tool center path
Programmed path
V : C-axis component of C2 - C1
C1 : Cutting surface of blocks N1 and N2
C2 : Cutting surface at the end of block N3
C1
N1
N2
N3
L1
L2
Fig.4.10 (f) When the amount of travel (L1) of block N2 is less than the
parameter value
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 94 -
(d) When, as shown in Fig. 4.10 (g), the diameter of an arc (R
in the figure) is less than the value set in parameter No.
19535, cutting point compensation is not applied
simultaneously with circular interpolation
Z-axis
C-axis on the
cylindrical surface
Y-axis
C1
C2
V
Tool center path
Programmed path
V : Cutting point compensation between blocks N2 and N3
C1 : Cutting surface of blocks N1 and N2
C2 : Cutting surface of block N3
C1
N1
N2
N3
L1
S2
S1
D
Fig.4.10 (g) When the diameter of an arc is less than the parameter
value
- When cutting point compensation is used with normal direction control
When cutting point compensation is used with normal direction
control, cutting point compensation between specified blocks is
performed regardless of the method described in "Cutting point
compensation" above, but is performed simultaneously with the
movement of the normal direction control axis (C-axis).
Z axis
A
axis
Y axis
X axis
C axis
Fig. 4.10 (h) When used with normal direction control
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 95 -
(1) When the normal direction changes between blocks N1 and N2,
cutting point compensation is also performed between blocks N1
and N2.
As shown in Fig. 4.10 (i), cutting point compensation described
in (1) in "Cutting point compensation" is performed
simultaneously with the movement made by normal direction
control between blocks N1 and N2.
Y axis
X axis
C1
C2
V
Tool center path
Programmed path
V : A-axis component of C2-C1
C1 : Cutting surface of block N1
C2 : Cutting surface of block N2
N1
N2
S0
A
-axis on the
cylindrical surface
Normal direction vector (G41.1)
Tool
Fig. 4.10 (i) When the normal direction changes between blocks N1 and
N2
(2) When gentle normal direction control changes the normal
direction as a specified block is executed, cutting point
compensation is performed simultaneously with the movement
made by the block. When the normal direction control axis
rotates by θ1 simultaneously with the movement made by blocks
N1 to N2 as shown in Fig. 4.10 (j), cutting point compensation
by the movement of vector V1 is also performed simultaneously
with the movement in N2.
Y-axis
X-axis
C1
C2
V1
Tool center path (G42)
Programmed path
V1 : A-axis component of C2-C1
C1 : Cutting surface of block N1
C2’ : Cutting surface at the end point of
block N2
N1
N2
S1
A
-axis on the
cylindrical surface
Normal direction vector (G41.1)
Tool
C2’ S2
N3
θ1
Fig. 4.10 (j) Gentle normal direction control
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 96 -
(3) When a specified block is executed while the normal direction
control axis is held in the normal direction set at the end point of
the previous block, cutting point compensation is not performed,
and cutting point compensation applied in the previous block is
maintained. As shown in Fig. 4.10 (k), when the movement
amount in N2 (L1 in the figure) is smaller than the setting of
parameter No. 5483, so the normal direction control axis does not
rotate at S1 while the movement amount in N3 (L2 in the figure)
is greater than the setting of parameter No. 5483, so the normal
direction axis rotates at S2, cutting point compensation is not
performed at S1 but is performed by the movement for vector V2
at S2.
Y-axis
X-axis
C1
C2
V1
Tool center path (G42)
Programmed path
V2 : A-axis component of C3-C1'
C1 : Cutting surface of block N1
C1’ : Cutting surface of block N2
C3 : Cutting surface of block N3
Vector S2 C1 = vector S2 C1'
N1
N2
S1
A
-axis on the
cylindrical surface
Normal direction vector (G41.1)
Tool
C3
S2
N3 V2
L1
C1’
L2
Fig. 4.10 (k) When the normal direction is the same as in the previous
block
- Feedrate during cutting point compensation
(1) The tool moves at a specified feedrate while cutting point
compensation is being applied between blocks.
(2) The actual speed indication and feedrate during circular
interpolation are as described below.
Actual speed indication
The speed component of each axis after cutting point
compensation at a point in time during circular interpolation is as
follows:
FzFz'
=
: Speed component of linear axis
Vcs)-(VceFcFc'
+
=
: Speed component of rotary axis
180
r
Vcs)-(Vce-Fy' π
= : Speed component of offset axis
Fz : Speed component of a cylindrical interpolation linear
axis before cutting point compensation
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 97 -
Fc : Speed component of cylindrical interpolation rotation
axis before cutting point compensation
Vcs: Rotation axis component of a tool contact point vector
(Vs in the figure) at the start point at a point in time
Vce: Rotation axis component of tool contact point vector
(Ve in the figure) at the end point at a point in time
r : Radius of the cylinder of a rotary axis
Accordingly, the actual speed indication during circular
interpolation is greater than the specified value when |Fc’| >
|Fc|(inner offset of the arc). Conversely, the actual speed
indication during circular interpolation is less than the
specified value when |Fc’| < |Fc|(outer offset of the arc).
Z-axis
C-axis
Y-axis
Programmed path
Vs
Fc
Vce
Ve
Vcs
Tool
Fz = Fz’
Fc’
Tool center path
Fig.4.10 (l) Actual speed indication during circular interpolation
- Usable G codes
(1) In any of the following G code modes, cutting point interpolation
for cylindrical interpolation can be specified:
G01, G02, G03: Linear interpolation, circular interpolation
G17, G18, G19: Plane selection
G22 : Stored stroke check function on
G64 : Cutting mode
G90, G91 : Absolute programming, incremental
programming
G94 : Feed per minute
(2) Any of the following G codes can be specified in cutting point
interpolation for cylindrical interpolation mode:
G01, G02, G03 : Linear interpolation, circular interpolation
G04 : Dwell
G40, G41, G42 : Tool radius compensation
G40.1 to G42.1 : Normal direction control
G64 : Cutting mode
G65 to G67 : Macro call
G90, G91 : Absolute programming, incremental
programming
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 98 -
- Parameter
To enable this function, set bit 5 (CYA) of parameter No. 19530 to 1.
Limitation
- Overcutting during inner corner cutting
Theoretically, when the inner area of a corner is cut using linear
interpolation as shown in Fig. 4.10 (m), this function slightly overcuts
the inner walls of the corner. This overcutting can be avoided by
specifying a value of R that is slightly greater than the radius of the
tool at the corner.
Tool Tool
Overcut portion
Fig.4.10 (m) Overcutting
- Setting the minimum input increment for an offset axis (Y-axis)
Set the same minimum input increment for an offset axis and linear
axis when cylindrical interpolation is performed.
- Workpiece radius specification
When specifying the radius of a workpiece, use the minimum input
increment (with no decimal point) for the linear axis used in
cylindrical interpolation.
- Reference axis setting (parameter No. 1031)
When different increment systems are used for a linear axis and a
rotary axis in cylindrical interpolation, specify the number of the
linear axis in cylindrical interpolation to set the axis as the reference
axis.
- Rotary axis roll-over function
When a rotary axis for which the rollover function is used is specified
as a rotary axis to be used for cylindrical interpolation, the roll-over
function is disabled in the cylindrical interpolation mode.
When the cylindrical interpolation is canceled, the rollover function is
automatically enabled.
- Program restart
In a program restart operation, G07.1 for the cylindrical interpolation
mode must not be specified.
Otherwise, PS0175 is issued.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 99 -
Example
- Example of cutting point interpolation for cylindrical interpolation
The sample program below indicates the positional relationships
between a workpiece and tool.
O0001 (CYLINDRICAL INTERPOLATION1) ;
N01 G00 G90 Z100.0 C0 ;
N02 G01 G91 G19 Z0 C0 ;
N03 G07.1 C57299 ;
N04 G01 G42 G90 Z120.0 D01 F250. ; .......... (1)
N05 C20.0 ; ..................................................... (2)
N06 G02 Z110.0 C60.0 R10.0 ;....................... (3)
N07 G01 Z100.0 ; ............................................ (4)
N08 G03 Z60.0 C70.0 R40.0 ;......................... (5)
N09 G01 C100.0 ;
:
M30 ;
Z-axis
C-axis on the Cylindrical surface
Tool center path
Programmed path
Tool
20 30 60 70 (deg)
30
60
70
80
90
120
(mm)
C-axis on the
Cylindrical
surface
Z-axis
Tool
(1) (2) (3)
(4)
(5)
Fig. 4.10 (n) Path of sample program for cutting point interpolation for
cylindrical interpolation
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 100 -
Workpiece
Rotary axis Rotary axis
Tool
Tool center
Y-axis Y-axis
Positional relationship between the
workpiece and tool of (1)
Positional relationship between the
workpiece and tool of (2)
Cutting surface 20°
0°
0°
Workpiece
Rotary axis Rotary axis
Tool
Tool center
Y-axis Y-axis
Positional relationship between the
workpiece and tool of (3) and (4)
Positional relationship between the
workpiece and tool of (5)
Cutting surface 70°
60° 60°
20°
Fig. 4.10 (o) Positional relationships between workpiece and tool of
sample program
The cutting surface in the rotary axis direction in (3) and (4) are
uniform even if the tool radius compensation amount is modified.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 101 -
- Example of specifying cutting point interpolation for cylindrical interpolation and
normal direction control at the same time
Tool radius compensation No.01 is 30 mm.
O0002 (CYLINDRICAL INTERPOLATION2) ;
N01 G00 G90 X100.0 A0 ;
N02 G01 G91 G17 X0 A0 ;
N03 G07.1 C57299 ;
N04 G01 G41 G42.1 G90 X120.0 D01 F250. ;
N05 A20.0 ;
N06 G03 X80.0 A60.0 R40.0 ;
N07 G01 X70.0 ;
N08 G02 X70.0 A70.0 R10.0 ;
N09 G01 A150.0 ;
N10 G02 X70.0 A190.0 R85.0 ;
N11 G01 X110.0 A265.0 ;
N12 G03 X120.0 A305.0 R85.0 ;
N13 G01 A360.0 ;
N14 G40 G40.1 X100.0 ;
N15 G07.1 A0 ;
N16 M30 ;
Z axis
A
axis
Y axis
X axis
C axis
Fig. 4.10 (p) Example of specifying normal direction control at the
same time
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 102 -
4.11 EXPONENTIAL INTERPOLATION (G02.3, G03.3)
Exponential interpolation exponentially changes the rotation of a
workpiece with respect to movement on the rotary axis. Furthermore,
exponential interpolation performs linear interpolation with respect to
another axis. This enables tapered groove machining with a constant
helix angle (constant helix taper machining). This function is best
suited for grooving and grinding tools such as taper end mills.
Helix angle
β
1 = β2 = β3
Z
A
X
β1
β
3
β
2
A
(Rotary axis)
X (Linear axis)
∆
X
∆
A
Relationship between X-axis and A-axis
Fig. 4.11 (a) Exponential interpolation
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 103 -
Format
Positive rotation (ω = 0)
G02. 3 X_ Y_ Z_ I_ J_ K_ R_ F_ Q_ ;
Negative rotation (ω = 1)
G03. 3 X_ Y_ Z_ I_ J_ K_ R_ F_ Q_ ;
X_ : Specifies an end point with an absolute or incremental value.
Y_ : Specifies an end point with an absolute or incremental value.
Z_ : Specifies an end point with an absolute or incremental value.
I_ : Specifies angle I (from ±1 to ±89 deg in units of 0.001 deg).
J_ : Specifies angle J (from ±1 to ±89 deg in units of 0.001 deg).
K_ : Specifies the amount to divide the linear axis for exponential
interpolation (span value). The specification unit depends on
the reference axis. Specify a positive value.
The span value is specified in the manner specified in bit 0
(SPN) of parameter No. 5630. If SPN is set to 0, the division
amount is specified in parameter No. 5643. If SPN is set to
1, the value specified with K becomes valid.
R_ : Specifies constant R for exponential interpolation. (See
Explanations below.)
F_ : Specifies the initial feedrate.
Specified in the same way as an ordinary F code. Specify a
composite feedrate including a feedrate on the rotary axis.
Q_ : Specifies the feedrate at the end point.
The same unit used for F is used. The CNC internally
performs interpolation between the initial feedrate (F) and
final feedrate (Q), depending on the travel distance on the
linear axis.
Explanation
Z
A
X
I
B
r
J
U
X
Z(0)
r : Diameter of left end
U : Excess length
X : Amount of travel along the linear axis
I : Taper angle
B : Groove bottom taper angle
J : Helix angle
Fig. 4.11 (b) Constant helix machining for producing a tapered figure
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 104 -
In Fig. 4.11 (b) an absolute value on the X-axis, Z-axis, or A-axis is
expressed as a function of workpiece rotation angle θ, such as X(θ),
Z(θ), and A(θ).
Linear interpolation with the X-axis is performed for an axis other
than the X-axis or A-axis. When X(θ) = 0, A(θ) = 0.
The relationship is expressed as follows.
{ }
(0)
)tan(
)tan(
*1)(*)tan(*
2
)( Z
I
B
eIU
r
θZK
θ
+−−= ................. (1)
{ }
)tan(
1
*1)(*)tan(*
2
)( I
eIU
r
θXK
θ
−−= ........................... (2)
θ
π
θAω*
2
360
*1)()( −=
Where
I
J
Ktan
tan
=
ω
: Helix direction (0: Positive, 1: Negative)
From Expressions (1) and (2), the following is obtained ;
(0))(*)tan()( ZθXBθZ
+
=
.................................................. (3)
From Expression (3), the Z-axis position is determined from a groove
bottom taper angle (B) and X-axis position.
From Expression (1) and exponential definition expression (described
later), the following is determined:
)tan(*/2 IUrR
−
=
.............................................................. (4)
Constant R is determined from the left end diameter (r), excess length
(U), and taper angle (I) according to Expression (4). Specify a taper
angle (I) in address I, and specify a helix angle (J) in address J.
Select a helix direction with G02.3 or G03.3.
- Exponential definition expressions
Exponential relational expressions for a linear axis and rotary axis are
defined as follows:
)tan(
1
*1)(*)( I
eRθXK
θ
−= .................................................. (5)
π
θ
θAω
2
*360*1)()( −= ........................................................ (6)
Where,
)tan(
)tan(
I
J
K=
0/1
=
ω
R, I, and J are constants, and θ represents an angle (radian).
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 105 -
- Span value K
A movement on an axis is carried out as linear interpolation in units of
values obtained by dividing the movement on the X-axis by the span
value (address K).
The following is obtained from Expression (5)
1)
)tan(*
ln(*)( += R
IX
KXθ................................................ (7)
When there is movement from X1 to X2 on the linear axis, the amount
of movement on the rotary axis is determined by:
1)}
)tan(*
ln(1)
)tan(*
{ln(*∆12 +−+= R
IX
R
IX
Kθ
X (linear axis)
Rotation angle
θ
∆
θ
K
X2
X1
Fig. 4.11 (c) Span value K
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 106 -
- Rotation axis θ
In exponential interpolation, Expression (7) indicates the relationship
between the X coordinate and the rotation angle θ about the A-axis.
The expression in the parentheses of the natural logarithm ln in
Expression (7) must satisfy Expression (8) indicated below, because
of the condition of ln (the value in the parentheses is positive).
1
)tan(* −>
R
IX ................................................................... (8)
If the value of X*tan(I)/R becomes -1 or less, the position comes to
the right of point (A) in Fig. 4.11 (d). Because the resultant figure is
unfeasible, an alarm PS5062 will be issued.
In exponential interpolation, the X, Y, Z, and U values are handled as
coordinates in the workpiece coordinate system. If a positive value
specified in incremental programming corresponds to a negative value
in the workpiece coordinate system, the negative value is used in the
calculation.
X
x
U
x*tan(I)
I
r
R
Origin of
workpiece
coordinate
system
x*tan(I)/R
≤
-1
(A)
x*tan(I)/R > -1
Fig. 4.11 (d) Rotation angle θ
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 107 -
- Taper angle I
The machining profile and the sign of taper angle I have the following
relationships:
• If the profile tapers up toward the right, the I value is positive.
• If the profile tapers down toward the right, the I value is negative.
X
Y
I > 0
I > 0
I < 0
I < 0
Y
YY
X
XX
Example)
Fig. 4.11 (e) Taper angle I
- Helix angle J
The sign of the helix angle J is assigned as illustrated below.
X
J > 0 J > 0
X
Example)
X
J < 0 J < 0
X
J
J
J
J
Fig. 4.11 (f) Helix angle J
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 108 -
Example
N10 G90 G01 X5.0 Z1.575 ;
N20 G02.3 X25.0 Z2.273 I3.0 J-45.0 K1.0 R1.238
F1000 Q1000 ;
Z
A
X
r = 3.0
Z(0) = 1.4
J = 45°
I = 3.0°
U = 5.0
X = 25.0
B = 2.0°
Xe
Xs
Xs: Start point on the
X-axis
Xe: End point on the
X-axis
The start point and end point of the Z-axis and the constant R are
obtained from the following expressions:
Start point on the Z-axis (0)*)tan( ZXsB
+
=
End point on the Z-axis (0)*)tan( ZXeB
+
=
)tan(*/2 IUrR
−
=
Limitation
- Cases where linear interpolation is performed
Even when the G02.3 or G03.3 mode is set, linear interpolation is
performed in the following cases:
• When the linear axis specified in parameter No. 5641 is not
specified, or the amount of movement on the linear axis is 0
• When the rotary axis specified in parameter No. 5642 is specified
• When the amount for dividing the linear axis (span value) is 0
- Tool compensation
The tool compensation functions (tool length compensation, tool
radius/tool nose radius compensation, and 3-dimensional cutter
compensation) cannot be used in the G02.3 or G03.3 mode.
CAUTION
The amount for dividing the linear axis for
exponential interpolation (span value) affects figure
precision. However, if an excessively small value is
set, the machine may stop during interpolation. Try
to specify an optimal span value depending on the
machine being used.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 109 -
4.12 SMOOTH INTERPOLATION (G05.1)
Either of two types of machining can be selected, depending on the
program command.
• For those portions where the accuracy of the figure is critical,
such as at corners, machining is performed exactly as specified
by the program command.
• For those portions having a large radius of curvature where a
smooth figure must be created, points along the machining path
are interpolated with a smooth curve, calculated from the
polygonal lines specified with the program command (smooth
interpolation).
In this manner, high-speed, high-precision machining can be
performed.
Format
G05.1Q2X0Y0Z0 ; Starting of smooth interpolation mode
:
G05.1Q0 ; Cancellation of smooth interpolation mode
Explanation
- Characteristics of smooth interpolation
To machine a part having sculptured surfaces, such as metal moldings
used in automobiles and airplanes, a part program usually
approximates the sculptured surfaces with minute line segments. As
shown in the following figure, a sculptured curve is normally
approximated using line segments with a tolerance of about 10 µm.
Enlarged
10
µ
m
: Specified point
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 110 -
When a program approximates a sculptured curve with line segments,
the length of each segment differs between those portions that have
mainly a small radius of curvature and those that have mainly a large
radius of curvature. The length of the line segments is short in those
portions having a small radius of curvature, while it is long in those
portions having a large radius of curvature. Because linear
interpolation controls the tool movement exactly as programmed so as
not to let the tool depart from the path specified by a part program,
machining is performed exactly along line segments with which a
sculptured curve is approximated. Consequently, when a curve with a
large radius of curvature and a moderate curvature change is machined,
the corners of line segments may become apparent. Such concave and
convex portions, produced as a result of machining performed exactly
as specified, are found troublesome when a smooth surface must be
obtained by finishing.
Profile
Portions having mainly
a small radius of
curvature
Portions having mainly
a large radius of
curvature
Example of machined
parts Automobile parts Decorative parts, such
as body side moldings
Length of line segment Short Long
Resulting surfaces
produced using
high-precision contour
control
Smooth surface even
when machining is
performed exactly as
specified by a program
Uneven surfaces may
result when machining
is performed exactly as
specified by a program
Example of uneven surfaces (polygon) resulting from machining that precisely follows the line segments.
In smooth interpolation mode, the CNC automatically determines,
according to the program command, whether an accurate figure is
required, such as at corners, or a smooth figure is required where the
radius of curvature is large. If a block specifies a travel distance or
direction which differs greatly from that in the preceding block,
smooth interpolation is not performed for that block. Linear
interpolation is performed exactly as specified by the program
command. Programming is thus very simple.
Specifying G5.1 Q2 also enables AI contour control to be turned on at
the same time. The automatic velocity control by AI contour control
reduces impacts on the machanical system. Specifying G5.1 Q0
cancels the smooth interpolation mode. The AI contour control mode
is also canceled at the same time.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 111 -
Interpolated by smooth curve
Interpolated by smooth curve
(Example)
N17
N16
N1
N2
N15 N14 N13 N12 N11
N10
N9
N3 N4 N5 N6 N7
N8
Linear interpolation
Linear interpolation
N17
N16
N1
N2
N15 N14 N13 N12 N11
N10
N9
N3 N4 N5 N6 N7
N8
- Conditions for performing smooth interpolation
Smooth interpolation is performed when all the following conditions
are satisfied. If any of the following conditions is not satisfied for a
block, that block is executed without smooth interpolation then the
conditions are checked for the next block.
(1) The machining length specified in the block is shorter than the
length specified with parameter No. 8486.
(2) The machining length is other than 0.
(3) The modes are:
G01 : Linear interpolation
G13.1 : Polar coordinate interpolation cancel
G15 : Polar coordinate command cancel
G40 : Tool radius/tool nose radius compensation cancel
(except for 3-dimensional cutter compensation)
G64 : Cutting mode
G80 : Canned cycle cancel
G94 : Feed per minute
(4) Machining is specified only along the axes specified with
G05.1Q2.
(5) The block is judged to be unsuitable for smooth interpolation, as
performed with the internal algorithm of the CNC.
- Commands which cancel smooth interpolation
(1) Auxiliary and second auxiliary functions
(2) M98, M99 : Subprogram call
M198 : Calling a subprogram in external memory
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 112 -
- Checking the smooth interpolation mode
Diagnostic data (No. 5000#0) indicates whether the smooth
interpolation mode is enabled in the current block.
If the smooth interpolation mode is enabled, "smooth interpolation on"
bit is set to 1.
Limitation
- Controlled axes
Smooth interpolation can be specified only for the X-, Y-, and Z-axes
and any axes parallel to these axes (up to three axes at one time).
Example
<Example program for smooth interpolation>
N10 X-1000 Z350 ;
. N11 X-1000 Z175 ;
. N12 X-1000 Z25 ;
G91 ; N13 X-1000 Z- 50 ;
G05. 1 Q2 X0 Y0 Z0 ; N14 X-1000 Z- 50 ;
N01 G01 X1000 Z-300 ; N15 X-1000 Z50 ;
N02 X1000 Z-200 ; N16 X-1000 Z200 ;
N03 X1000 Z-50 ; N17 X-1000 Z300 ;
N04 X1000 Z50 ; G05. 1 Q0 ;
N05 X1000 Z50 ; .
N06 X1000 Z-25 ; .
N07 X1000 Z-175 ;
N08 X1000 Z-350 ;
N09 Y1000 ;
Interpolated by smooth curve
Interpolated by smooth curve
(Example)
N17
N16
N1
N2
N15 N14 N13 N12 N11
N10
N9
N3 N4 N5 N6 N7
N8
Linear interpolation
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 113 -
4.13 NANO SMOOTHING
Overview
When a desired sculptured surface is approximated by minute
segments, the nano smoothing function generates a smooth curve
inferred from the programmed segments and performs necessary
interpolation.
The nano smoothing function infers a curve from a programmed
figure approximated with segments within tolerance. If the spacing
between adjacent inflection points or programmed points is not
constant, this function can generate a smoother curve than the
conventional smooth interpolation function.
The interpolation of the curve reduces the segment approximation
error, and the nano-interpolation makes the cutting surface smoother.
The interpolation of the curve reduces the segment approximation
error, and the nano interpolation makes the cutting surface smoother.
Nano smoothing 2 allows the basic three axes (X, Y, and Z) or their
parallel axes as well as two rotation axes to be specified. This enables
five-axis machining (including rotation axes) to produce very smooth
finished surfaces and so finds applications such as machining of
smooth workpiece side faces.
In addition, this function can be used with tool center point control
(type 1 (G43.4)). This eliminates the necessity of modifying a
program when the tool length is changed.
For this function, the AI contour control option is required.
For nano smoothing 2, the nano smoothing option is required.
Format
G5.1 Q3 Xp0 Yp0 Zp0 [α0] [β0] ; : Nano smoothing mode on
G5.1 Q0 ; : Nano smoothing mode off
Xp : X-axis or an axis parallel to the X-axis
Yp : Y-axis or an axis parallel to the Y-axis
Zp : Z-axis or an axis parallel to the Z-axis
α, β : Rotary axis
NOTE
1 Specify G5.1 alone in a block. (Avoid specifying
any other G code in the same block.)
2 Specify position 0 for the axis programmed in the
nano smoothing mode on block. The specified axis
is subjected to nano smoothing, but no movement
is made even in the absolute programming mode.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 114 -
Nano smoothing 2 enables specification of the basic three axes (X-, Y-,
and Z-axes) or their parallel axes as axes on which to perform nano
smoothing, as well as two rotary axes.
If executing nano smoothing 2 simultaneously with tool center point
control (type 1 (G43.4)), enable tool center point control (G43.4) first
and then enable nano smoothing 2 (G5.1 Q3). To cancel them, cancel
nano smoothing 2 (G5.1 Q0) first and then cancel tool center point
control (G49).
Example :
O0010
…
G43.4 H1 P0;
G5.1 Q3 X0 Y0 Z0 B0 C0;
…
G5.1 Q0;
G49;
…
M30; Nano smoothing 2
Tool center point control
- Nano smoothing mode
Specifying G5.1 Q3 selects the nano smoothing mode. An axis of
nano smoothing is specified in the same block. The basic three axes
(X, Y, and Z) and their parallel axes can be specified as the axis of
nano smoothing. In the nano smoothing mode, nano smoothing is
performed in a block which satisfies the conditions described below.
Nano smoothing is cancelled in a block which does not satisfy the
conditions.
Specifying G5.1 Q3 also enables AI contour control. The automatic
velocity control by AI contour control reduces impacts on the
mechanical system.
Specifying G5.1 Q0 cancels the nano smoothing mode. The AI
contour control mode is also cancelled at the same time.
Making a reset also cancels the nano smoothing mode.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 115 -
- Conditions to enable nano smoothing
Nano smoothing is enabled when the following conditions are
satisfied. Nano smoothing is cancelled in a block which does not
satisfy the conditions. A decision is made to perform nano smoothing
from the next block.
In the programmed block length and the difference in angle between
adjacent programmed blocks in the conditions listed below, only the
basic three axes (or their parallel axes) are considered, and the rotation
axes are excluded. When the nano smoothing mode is canceled in a
block when these conditions are satisfied, nano smoothing for the
rotation axes is not performed, either.
<1> The programmed block length is shorter than the length specified
in parameter No. 8486.
<2> The programmed block length is longer than the length specified
in parameter No. 8490.
<3> The difference in angle between adjacent programmed blocks is
smaller than the value specified in parameter No. 8487.
<4> The current mode is one of the following:
• Linear interpolation
• Feed per minute
• Tool radius compensation cancel
• Canned cycle cancel
• Scaling cancel
• Macro modal call cancel
• Constant surface speed control cancel
• Cutting mode
• Coordinate system rotation / 3-dimensional coordinate system
conversion cancel
• Polar coordinate cancel
• Normal-direction control cancel
• Polar coordinate interpolation cancel
• Programmable mirror image cancel
• Polygon turning cancel
<5> No one-shot G code is specified in the block.
<6> Buffering is not suppressed in the block.
<7> A movement just on the axis of nano smoothing is specified in
the block.
- Checking the nano smoothing mode
Diagnostic data (No. 5000) indicates whether the nano smoothing
mode is enabled in the current block.
If the nano smoothing mode is enabled, the "smoothing on" bit is set
to 1.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 116 -
Explanation
Generally, a program approximates a sculptured surface with minute
segments with a tolerance of about 10 µm.
To l e r a nc e
Programmed point
Desired curve
Many programmed points are placed on the boundary of tolerance.
The programmed points also have a rounding error owing to the least
input increment of the CNC. The nano smoothing function creates
multiple insertion points between adjacent programmed points so that
a smooth curve can be created from the approximation segments.
The desired curve is inferred from the insertion points of multiple
blocks including buffered blocks.
Many insertion points are closer to the desired curve than the
programmed points. A stable curve can be inferred with the insertion
points created from multiple blocks including buffered blocks.
Because the position of each insertion point is corrected in a unit
smaller than the least input increment of the CNC within tolerance, the
impact of rounding error is reduced.
Nano-interpolation is performed for the curve inferred from the
corrected insertion points, so the resultant cutting surface becomes
smooth.
Programmed point
Insertion point
Corrected insertion point Inferred curve
To l e r a nc e
- Specifying the tolerance
The tolerance of the program of nano smoothing is specified in
parameter No. 19581.
The insertion points are corrected within tolerance, and a curve is
inferred accordingly.
If 0 is specified in parameter No. 19581, the minimum travel distance
in the increment system is considered to be the tolerance.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 117 -
- Nano smoothing 2
Nano smoothing 2 performs smooth interpolation for the basic three
axes (or their parallel axes) and two rotation axes independently.
: Command point
Smoothing on XYZ space
: Command point
Smoothing on BC space
X
Y
Z
B
C
G5.1 Q3 X0 Y0 Z0 B0 C0;
X_ Y_ Z_ B_ C_;
X_ Y_ Z_ B_ C_;
…
G5.1 Q0;
Insertion points for the rotation axes are corrected so that each axis
element of the distance between an insertion point and the corrected
insertion point for both axes does not exceed the tolerance set for each
axis in parameter No. 19587.
Tolerance
for C-axis
Tolerance for
B-axis
Insertion point should be
corrected within
tolerance for each axis
Insertion point
Corrected insertion point
B
C
Inferred curve
- Making a decision on the basis of the spacing between adjacent programmed
points
If the spacing between adjacent programmed points (block length)
exceeds the value specified in parameter No. 8486 or falls below the
value specified in parameter No. 8490 in the nano smoothing mode,
the nano smoothing mode is cancelled at the start point of the block.
Linear interpolation can be performed in the block.
When a decision is made on the basis of the spacing between adjacent
programmed points, only the basic three axes (or their parallel axes)
are considered, and the rotation axes are excluded. When the nano
smoothing mode is canceled in a block, nano smoothing for the
rotation axes is not performed, either.
If the values specified in the parameters are 0, no decision is made on
the basis of the spacing between adjacent programmed points.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 118 -
- Making a decision at a corner
If the difference in angle (see the following figure) between adjacent
programmed blocks exceeds the value specified in parameter No.
8487 in the nano smoothing mode, the nano smoothing mode is
cancelled at the corner.
The decision at the corner is made by considering the basic three axes
(or their parallel axes) only; the rotation axes are not considered.
When the nano smoothing mode is canceled in a block, nano
smoothing for the rotation axes is not performed, either.
N1
N2
N3
θ1
θ2
θ1: Difference in angle between blocks N1 and N2
θ2: Difference in angle between blocks N2 and N3
If the value specified in the parameter is 0, no decision is made at the
corner on the basis of the difference in angle.
Very minute blocks created for some reasons such as a calculation
error of CAM can be ignored, and a smooth connection can be made
at a corner. To do this, specify parameter No. 19582 to the minimum
travel distance with which a decision is made on the basis of
difference in angle. Then, the decision at a corner is disabled for a
block of which distance is less than the specified minimum travel
distance.
However, a decision based on the spacing between adjacent
programmed points specified in parameter No. 8490 has higher
priority than the decision at a corner. Therefore, the value specified in
parameter No. 19582 must be greater than the value specified in
parameter No. 8490.
If parameter No. 19582 is specified, a very minute block is not
considered to be a corner, and a smooth connection can be made.
Limitation
- Single-block operation
When single-block operation is carried out in the nano smoothing
mode, the operation stops at a corrected insertion point not at a
programmed point.
Even in the nano smoothing mode, normal single-block operation is
carried out for a block that does not satisfy the conditions of nano
smoothing mode.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 119 -
- Tool length compensation
To carry out tool length compensation, specify the command before
specifying nano smoothing. Avoid changing the amount of
compensation in the nano smoothing mode.
If G43, G44, or G49 is specified in a block between the block in
which the command of nano smoothing mode on (G5.1 Q3) is
specified and the block in which the command of nano smoothing
mode off (G5.1 Q0) is specified, an alarm PS0343 will be issued.
- Tool radius/tool nose radius compensation
If tool radius/tool nose radius compensation is specified in the nano
smoothing mode, the nano smoothing mode is cancelled. Then, when
the command of tool radius/tool nose radius compensation cancel
(G40) is specified, a decision is made whether to start nano smoothing
from the next block. The startup and cancel operations of type C are
always carried out for the tool radius/tool nose radius compensation
specified in the nano smoothing mode, irrespective of the parameter
setting.
A command related to tool radius/tool nose radius compensation
should not be specified in the nano smoothing mode unless it is
absolutely necessary.
- Interruption type custom macro
No interruption type custom macro can be used in the nano smoothing
mode.
If the nano smoothing mode is specified while an interruption type
custom macro is enabled or if an interruption type custom macro is
enabled in the nano smoothing mode, an alarm PS0342 will be issued.
- Manual intervention
Manual intervention by specifying the manual absolute on command
cannot be performed in the nano smoothing mode. If this is attempted,
an alarm PS0340 will be issued at the cycle start after manual
intervention.
- Rotary table dynamic fixture offset
The command of rotary table dynamic fixture offset (G54.2) must be
cancelled before specifying the nano smoothing mode. These
commands cannot be used in the nano smoothing mode. If an attempt
is made to use one of these commands, an alarm PS0343 will be
issued.
- Number of blocks that can be specified successively
Up to about 300,000,000 blocks can be specified successively in the
nano smoothing mode. If more blocks are specified, an alarm PS0341
will be issued.
However, when a block which does not satisfy the conditions of the
nano smoothing mode is encountered, the mode is canceled and the
counted number of successive blocks is reset to 0.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 120 -
- Continuity of a program
Curve interpolation is carried out for multiple programmed blocks
including buffered blocks in the nano smoothing mode.
Therefore, the programmed commands must be executed continuously
in the nano smoothing mode.
The continuity of a program may be lost, and continuous execution
may not be performed, in some cases such as the following: A
single-block stop is made in the nano smoothing mode; and another
program is executed in the MDI mode. If this occurs, an alarm PS0344
will be issued.
- Restrictions on resumption of automatic operation
(1) Program restart
Curve interpolation is performed for corrected insertion points
not for programmed points in the nano smoothing mode.
Accordingly, when a sequence number is specified to restart the
program, the operation cannot be restart from a programmed
point in a block.
To restart a program, specify a block number, using the block
counter displayed in the program screen.
(2) Block restart
A block cannot be restarted in the nano smoothing mode. When
an attempt is made to restart a block, an alarm PS0344 will be
issued.
(3) Tool retract and recover
The tool cannot be retracted or recovered in the nano smoothing
mode.
(4) Retracing
Retracing cannot be performed in the nano smoothing mode.
(5) Active block cancel
The active block cancel function is temporarily disabled in the
nano smoothing mode.
- Functions that cannot be used simultaneously
The nano smoothing function cannot be used simultaneously with the
following functions.
• Parallel axis control
• Twin table control
- Tool center point control
Nano smoothing 2 can be used with tool center point control (type 1
(G43.4)). However, when it is used with tool center point control (type
2 (G43.5)) or tool posture control, alarm PS5421 (ILLEGAL
COMMAND IN G43.4/G43.5) is issued.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 121 -
4.14 NURBS INTERPOLATION (G06.2)
Many computer-aided design (CAD) systems used to design metal
dies for automobiles and airplanes utilize non-uniform rational
B-spline (NURBS) to express a sculptured surface or curve for the
metal dies.
This function enables NURBS curve expression to be directly
specified to the CNC. This eliminates the need for approximating the
NURBS curve with minute line segments. This offers the following
advantages:
1. No error due to approximation of a NURBS curve by small line
segments
2. Short part program
3. No break between blocks when small blocks are executed at high
speed
4. No need for high-speed transfer from the host computer to the
CNC
When this function is used, a computer-aided machining (CAM)
system creates a NURBS curve according to the NURBS expression
output from the CAD system, after compensating for the length of the
tool holder, tool diameter, and other tool elements. The NURBS curve
is programmed in the NC format by using these three defining
parameters: control point, weight, and knot.
CAM (Creating an NC part program)
CAD(Designing a metal die)
Generating a metal die surface
(NURBS surface or curve)
Studying the machining
method and others
Tool compensation file
NC part program after tool compensation
(NURBS curve)
CNC equipment Machine tool
NURBS curve (control point, weight, knot)
Fig. 4.14 (a) NC part program for machining a metal die according to a
NURBS curve
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 122 -
NURBS interpolation can be performed for up to five axes (including
two rotation axes). Therefore, NURBS interpolation can be performed
for the basic three axes (X, Y, and Z) and two rotation axes at the
same time. This enables five-axis machining to produce very smooth
finished surfaces and so finds applications such as machining of
smooth workpiece side faces.
In addition, NURBS interpolation can be used with tool center point
control (type 1 (G43.4)). This eliminates the necessity of modifying a
program when the tool length is changed.
Format
G06.2[P ] K X Y Z [α ] [β ][R ] [F ];
K X Y Z [α ] [β ][R ];
K X Y Z [α ] [β ][R ];
K X Y Z [α ] [β ][R ];
:
K X Y Z [α ] [β ][R ];
K ;
:
K ;
G01 . . .
G06.2 : Start NURBS interpolation mode
P : Rank of NURBS curve
X Y Z : Control point
α β : Control point (rotary axes)
R : Weight
K : Knot
F : Feedrate
If executing NURBS interpolation simultaneously with tool center
point control (type 1 (G43.4)), enable tool center point control (G43.4)
first and then enable NURBS interpolation (G06.2). To cancel them,
end NURBS interpolation (G code command in group 01 other than
G06.2) first and then cancel tool center point control (G49).
Example :
O0010
…
G43.4 H1 P0;
G06.2 K_ X_ Y_ Z_ B_ C_;
…
K_
G01 X_ Y_ Z_ B_ C_;
G49;
…
M30; NURBS interpolation
Tool center point control
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 123 -
Explanation
- NURBS interpolation mode
NURBS interpolation mode is selected when G06.2 is programmed.
G06.2 is a modal G code of group 01. NURBS interpolation mode
ends when a G code of group 01 other than G06.2 (G00, G01, G02,
G03, etc.) is specified.
- Rank of NURBS
A rank of NURBS can be specified with address P. The rank setting, if
any, must be specified in the first block. If the rank setting is omitted,
a rank of four (degree of three) is assumed for NURBS. The valid
data range for P is 2 to 4. The P values have the following meanings:
P2: NURBS having a rank of two (degree of one)
P3: NURBS having a rank of three (degree of two)
P4: NURBS having a rank of four (degree of three) (default)
This rank is represented by k in the defining expression indicated in
the description of NURBS curve below. For example, a NURBS curve
having a rank of four has a degree of three. The NURBS curve can be
expressed by the constants t3, t2, and t1.
- Weight
The weight of a control point programmed in a single block can be
defined. When the weight setting is omitted, a weight of 1.0 is
assumed.
- Knot
The number of specified knots must equal the number of control
points plus the rank value. In the blocks specifying the first to last
control points, each control point and a knot are specified in an
identical block. After these blocks, as many blocks (including only a
knot) as the rank value are specified. The NURBS curve programmed
for NURBS interpolation must start from the first control point and
end at the last control point. The first k knots (where k is the rank)
must have the same values as the last k knots (multiple knots). If the
absolute coordinates of the start point of NURBS interpolation do not
match the position of the first control point, alarm PS5117 is issued.
(To specify incremental values, G06.2 X0 Y0 Z0 K_ must be
programmed.)
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 124 -
- NURBS curve
Using these variables:
k : Rank
Pi : Control point
Wi : Weight
Xi : Knot (Xi < Xi+1)
Knot vector [X0, X1, . . . , Xm] (m = n+ k)
t : Spline parameter,
the spline basis function N can be expressed with the de Boor-Cox
recursive formula, as indicated below:
<
+
<+
<<
=)
1
,(0
)
1
1(1
)(
1, t
i
x
i
xt
i
xt
i
x
t
i
N
1
)(
1,1
)(
1
)(
1,
)(
)(
,+
−
+
−+
−
+
+
−
−+
−
−
=
i
x
ki
x
t
ki
Nt
ki
x
i
x
ki
x
t
ki
N
i
xt
t
ki
N
The NURBS curve P(t) of interpolation can be expressed as follows:
∑
∑
=
=
=n
0i
1k,i
n
0i
iik,i
w)t(N
pw)t(N
)t(P
(X0<t<Xm)
- Reset
A reset during NURBS interpolation results in the clear state. The
modal code of group 1 enters the state specified in bit 0 (G01) of
parameter No. 3402.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 125 -
Limitation
- Controlled axes
NURBS interpolation can be performed on up to five axes (including
two rotary axes). The axes of NURBS interpolation must be specified
in the first block. A new axis cannot be specified before the beginning
of the next NURBS curve or before NURBS interpolation mode ends.
- Command in NURBS interpolation mode
In NURBS interpolation mode, any command other than the NURBS
interpolation command (miscellaneous function and others) cannot be
specified.
- Manual intervention
If manual intervention is attempted while manual absolute mode is set,
alarm PS5118 is issued.
- Tool radius compensation
Tool radius compensation cannot be simultaneously executed.
NURBS interpolation can only be specified after tool radius
compensation has been canceled.
- 3-dimensional cutter compensation
3-dimensional cutter compensation cannot be simultaneously executed.
NURBS interpolation can only be specified after 3-dimensional cutter
compensation has been canceled.
- Tool centerpoint control
Tool center point control (type 1 (G43.4)) can be simultaneously
executed, but tool center point control (type 2 (G43.5)) and tool
posture control cannot be simultaneously executed. If an attempt is
made to execute tool center point control (type 2 (G43.5) or tool
posture control simultaneously with NURBS interpolation, alarm
PS5421 is issued.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 126 -
Example
<Sample NURBS interpolation program>
G90;
...
G06.2 K0. X0. Z0.;
K0. X300. Z100.;
K0. X700. Z100.;
K0. X1300. Z-100.;
K0.5 X1700. Z-100.;
K0.5 X2000. Z0.;
K1.0;
K1.0;
K1.0;
K1.0;
G01 Y0.5;
G06.2 K0. X2000. Z0.;
K0. X1700. Z-100.;
K0. X1300. Z-100.;
K0. X700. Z100.;
K0.5 X300. Z100.;
K0.5 X0. Z0.;
K1.0;
K1.0;
K1.0;
K1.0;
G01 Y0.5;
G06.2 ...
...
G01 ...
Y
Z
X
1000.
2000.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 127 -
4.14.1 NURBS Interpolation Additional Functions
In the FANUC Series 30i/31i, NURBS interpolation provides the
following additional functions:
- Parametric feedrate control
The maximum feedrate of each segment is determined according to a
specified feedrate and acceleration. For a series of segments, the
feedrates at the start point and end point of the segments are
determined as described below. During a movement from the start
point to end point, the feedrate changes continuously. This function
can be used only for NURBS interpolation when bit 5 (FDI) of
parameter No. 8412 is set to 1.
1. Start point speed
(1) At the start of NURBS interpolation
If the amount of travel in the previous block is 0, the
maximum speed in the first segment is regarded as the start
point speed. If the amount of travel in the previous block is
not 0, whichever is smaller of the specified speed in the
previous block and the maximum speed in the first segment
is regarded as the start point speed.
Previous block: Block immediately preceding the block in
which NURBS interpolation is specified.
(2) Second and subsequent segments
Whichever is smaller of the maximum speed in the previous
segment and the maximum speed in this segment is
regarded as the start point speed.
2. End point speed
(1) In a segment other than the last
Whichever is smaller of the maximum speed in this segment
and the maximum speed in the next segment is regarded as
the end point speed.
(2) At the end of NURBS interpolation
If the amount of travel in the next block is 0, the maximum
speed in this segment is regarded as the end point speed. If
the amount of travel in the next block is not 0, whichever is
smaller of the maximum speed in this segment and the
specified speed in the next block is regarded as the end
point speed.
After the stop of a single block, the start point speed at a restart will be
the maximum speed in this segment.
After the stop of a feed hold, the speed at a restart will be the same as
the speed at the stop of the feed hold.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 128 -
Example
1. Specified program
G90 G06.2 X0. Y0. K0. F2000 ;
X10. Y10. K0. F1500 ;
X20. Y20. K0. F1800 ;
X30. Y30. K0. ;
X40. Y40. K1.
X50. Y50. K2.
K3.
K3.
K3.
K3.
2. Specified speed
Speed
Time
1500
1800
2000
3. Parametric speed control
Speed
Time
1500
1800
2000
4. Because of the addition of acceleration/deceleration before
interpolation, the actual cutting feedrate is as shown below.
Speed
Time
1500
1800
2000
NOTE
The actual acceleration/deceleration method is
bell-shaped acceleration/deceleration.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 129 -
- High-precision knot command
If bit 1 (HIK) of parameter No. 8412 is set to 1, knot commands with a
whole number of up to 12 digits and a decimal fraction of up to 12
digits can be specified. This function can be used only for knot
commands (address K) with a decimal point which are specified
during NURBS interpolation.
If a high precision knot command is used, the knot command format is
as shown below.
K (Number of A digits) . (Number of B digits)
where A + B must be 12 or less. The address K and the
numbers including the decimal point must be 14 characters
or less.
(Example)
Valid
K.999999999999
K1234.56789012
K999999999999.
Invalid (causing alarm PS0012 to be issued)
K0.999999999999
K1234.567891230
K1234.567891234
K999999999999.0
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 130 -
- Simple start command
If bit 0 (EST) of parameter No. 8412 is set to 1, a control command
may be omitted at the first control point. Because the same value is set
for the knot in the first block and the knot in the second block, the
knot command may also be omitted in the first bock.
The format of a NURBS interpolation command using this function is
as shown below.
G06.2 [P ] [K ] [IP ] [R ] [F ] ;
K IP [R ] ;
K IP [R ] ;
K IP [R ] ;
…
K IP [R ] ;
K ;
…
K ;
G01…
…
G06.2 : NURBS interpolation mode ON
P : Rank of the NURBS curve
IP : Control point
R : Weight
K : Knot
F : Speed
Words enclosed in [ ] are optional.
If a control point command is omitted in the first block, the current
position as determined when NURBS interpolation is started is
regarded as the first control point. Also, only the axis specified for the
control point in the second block is handled as a NURBS interpolation
axis and, therefore, in the second block, specify all axes subject to
NURBS interpolation.
If a knot command is omitted in the first block, the knot is regarded as
the same as the knot specified in the second block.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 131 -
4.15 HYPOTHETICAL AXIS INTERPOLATION (G07)
In helical interpolation, when pulses are distributed with one of the
circular interpolation axes set to a hypothetical axis, sine interpolation
is enabled.
When one of the circular interpolation axes is set to a hypothetical
axis, pulse distribution causes the speed of movement along the
remaining axis to change sinusoidally. If the major axis for threading
(the axis along which the machine travels the longest distance) is set
to a hypothetical axis, threading with a fractional lead is enabled. The
axis to be set as the hypothetical axis is specified with G07.
Format
G07 α0 ; : Hypothetical axis setting
:
G07 α1 ; : Hypothetical axis cancel
Where, α is any one of the addresses of the controlled axes.
Explanation
- Sine interpolation
The a axis is regarded as a hypothetical axis for the period of time
from the G07 α0 command until the G07 α1 command appears.
Suppose sine interpolation is performed for one cycle in the YZ plane.
The hypothetical axis is then the X axis.
X2+Y2 = r2 (r is the radius of an arc.)
Y = rSIN ( 1
2
π
Z) (1 is the distance traveled along the Z-axis in one
cycle.)
Y
r
OZ
1
π
2
2π
π
- Interlock, stroke limit, and external deceleration
Interlock, stroke limit, and external deceleration can also apply to the
hypothetical axis.
- Handle interruption
An interrupt caused by the handle also applies to the hypothetical axis.
This means that movement for a handle interrupt is performed.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 132 -
Limitation
- Manual operation
The hypothetical axis can be used only in automatic operation. In
manual operation, it is not used, and movement takes place.
- Move command
Specify hypothetical axis interpolation only in the incremental mode.
- Coordinate rotation
Hypothetical axis interpolation does not support coordinate rotation.
Example
- Sine interpolation
Y
Z
20.0
0
10.0
N001 G07 X0 ;
N002 G91 G17 G03 X-20.0 Y0.0 I-10.0 Z20.0 F100 ;
N003 G01 X10.0 ;
N004 G07 X1 ;
From the N002 to N003 blocks, the X-axis is set to a hypothetical axis.
The N002 block specifies helical cutting in which the Z-axis is the
linear axis. Since no movement takes place along the X axis,
movement along the Y-axis is performed while performing sine
interpolation along the Z-axis.
In the N003 block, there is no movement along the X-axis, and so the
machine dwells until interpolation terminates.
- Changing the feedrate to form a sine curve
(Sample program)
G07Z0 ; The Z-axis is set to a hypothetical axis.
G02X0Z0I10.0F4. ; The feedrate on the X-axis changes sinusoidally.
G07Z1 ; The use of the Z-axis as a hypothetical axis is
canceled.
F
4.0
Xt
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 133 -
4.16 VARIABLE LEAD THREADING (G34)
Specifying an increment or a decrement value for a lead per screw
revolution enables variable lead threading to be performed.
Fig. 4.16 (a) Variable lead screw
Format
G34 IP_ F_ K_ Q_ ;
IP_ : End point
F_ : Lead in longitudinal axis direction at the start point
K_ : Increment and decrement of lead per spindle revolution
Q_ : Shift amount of starting angle of thread cutting
Explanation
Address other than K are the same as in straight/taper thread cutting
with G32.
The K value depends on the increment system of the reference axis, as
indicated in Table 4.16 (a).
If the specified K value exceeds the range indicated in Table 4.16 (a),
if the maximum lead is exceeded after a change due to the K value, or
if the lead value is negative, an alarm PS0313 will be issued.
Table 4.16 (a) Range of valid K values
Increment system
of reference axis Metric input (mm/rev) Inch input (inch/rev)
IS-A ±0.001 to ±500.000 ±0.00001 to ±50.00000
IS-B ±0.0001 to ±500.0000 ±0.000001 to ±50.000000
IS-C ±0.00001 to ±50.00000 ±0.0000001 to ±5.0000000
IS-D ±0.000001 to ±5.000000 ±0.00000001 to ±0.50000000
IS-E ±0.0000001 to ±0.5000000 ±0.000000001 to ±0.050000000
CAUTION
The "thread cutting cycle retract" is not effective for
G34.
Example
Lead at the start point: 8.0 mm
Lead increment: 0.3 mm/rev
G34 Z-72.0 F8.0 K0.3 ;
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 134 -
4.17 CIRCULAR THREADING (G35, G36)
Using the G35 and G36 commands, a circular thread, having the
specified lead in the direction of the major axis, can be machined.
L
L: Lead
Fig. 4.17 (a) Circular threading
Format
A sample format for the G18 plane (Z-X plane) is indicated below.
When using the format for the G17 plane (X-Y plane), change the
addresses Z, X, K, and I to X, Y, I, and J respectively. When using the
format for the G19 plane (Y-Z plane), change the addresses Z, X, K,
and I to Y, Z, J, and K respectively.
M
G35 I_ K_
G36 X_ Z_ R_ F_ Q_ ;
G35 : Clockwise circular threading command
G36 : Counterclockwise circular threading command
X, Z : Specify the arc end point (in the same way as for
G02, G03).
I, K : Specify the arc center relative to the start point, using
relative coordinates (in the same way as for G02,
G03).
R : Specify the arc radius.
F : Specify the lead in the direction of the major axis.
Q : Specify the shift of the threading start angle
(0° to 360°, with least input increment of 0.001)
(The value can be programmed with a decimal point.)
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 135 -
T
G35 I_ K_
G36 X(U)_ Z(W)_ R_ F_ Q_ ;
G35 : Clockwise circular threading command
G36 : Counterclockwise circular threading command
X(U), Z(W) : Specify the arc end point (in the same way as
for G02, G03).
I, K : Specify the arc center relative to the start point, using
relative coordinates (in the same way as for G02,
G03).
R : Specify the arc radius.
F : Specify the lead in the direction of the major axis.
Q : Specify the shift of the threading start angle
(0° to 360°, with least input increment of 0.001)
(The value cannot be programmed with a decimal
point.)
F
X
Z
K
R
I
End point (Z, X)
A
rc center
Start point
Explanation
- Specifying the arc radius
If R is specified with I and K, only R is effective.
- Shift angle
If an angle greater than 360° is programmed, it is set to 360°.
M
- Specifying shift angle Q
To specify the shift angle Q, set bit 0 (GQS) of parameter No. 3451 to
1.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 136 -
T
- Automatic tool compensation
The G36 command is used to specify the following two functions:
Automatic tool compensation X and counterclockwise circular
threading. The function for which G36 is to be used depends on bit 3
(G36) of parameter No. 3405.
• When parameter G36 is set to 0, the G36 command is used for
automatic tool compensation X.
• When parameter G36 is set to 1, the G36 command is used for
counterclockwise circular threading.
G37.1 can be used to specify automatic tool compensation X and
G37.2 can be used to specify automatic tool compensation Z.
(Specification method)
G37.1 X_
G37.2 Z_
• G code when parameter G36 (bit 3 of No. 3405) is set to 1
G code G code group Function
G35 Clockwise circular threading
G36 01 Counterclockwise circular threading
G37 Automatic tool compensation Z
G37.1 Automatic tool compensation X
G37.2
00
Automatic tool compensation Z
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 137 -
Limitation
- Range of specifiable arc
An arc must be specified such that it falls within a range in which the
major axis of the arc is always the Z-axis or always the X-axis, as
shown in Fig. 4.17 (b), and (c). If the arc includes a point at which
the major axis changes from the X-axis to Z-axis, or vice versa, as
shown in Fig. 4.17 (d), an alarm PS5058 is issued.
X
45°
Z
Start point End point
Fig. 4.17 (b) Range in which the Z-axis is the major axis
X
45°
Z
Start point
End point
Fig. 4.17 (c) Range in which the X-axis is the major axis
X
45°
Z
Start point
End point
The major axis changes at this point.
Fig. 4.17 (d) Example of arc specification which causes an alarm
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 138 -
- End point not on an arc
If the end point is not on an arc, a movement on an axis is made to a
position of which coordinate matches the corresponding coordinate of
the end point. Then, a movement is made on another axis to reach the
end point.
Start point
Center
End point
r
Center
End point
r
Start point
Fig. 4.17 (e) Movement when the end point is not on an arc
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 139 -
4.18 SKIP FUNCTION (G31)
Linear interpolation can be commanded by specifying axial move
following the G31 command, like G01. If an external skip signal is
input during the execution of this command, execution of the
command is interrupted and the next block is executed.
The skip function is used when the end of machining is not
programmed but specified with a signal from the machine, for
example, in grinding. It is used also for measuring the dimensions of a
workpiece.
Format
G31 IP ;
G31 : One-shot G code (If is effective only in the block in
which it is specified)
Explanation
The coordinate values when the skip signal is turned on can be used in
a custom macro because they are stored in the custom macro system
variable #100151 to #100182, as follows. For systems with up to 20
axes, FS16-compatible system variables (#5061 to #5080) may also be
used.
#100151 (#5061) : First axis coordinate value
#100151 (#5062) : Second axis coordinate value
:
#100170 (#5080) : 20th axis coordinate value
#100171 : 21st axis coordinate value
#100172 : 22nd axis coordinate value
:
#100182 : 32nd axis coordinate value
CAUTION
Disable feedrate override, dry run, and automatic
acceleration/deceleration (however, these become
available by setting bit 7 (SKF) of parameter
No.6200 to 1.) when the feedrate per minute is
specified, allowing for an error in the position of the
tool when a skip signal is input. These functions are
enabled when the feedrate per rotation is specified.
NOTE
If G31 command is issued while tool radius/tool
nose radius compensation is applied, an alarm
PS0035 is displayed. Cancel the tool radius
compensation with the G40 command before the
G31 command is specified.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 140 -
Example
- The next block to G31 is an incremental programming
G31 G91 X100.0 F100;
Y50.0;
50.0
100.0
Skip signal is input here
A
ctual motion
Motion without skip signal
Y
X
Fig. 4.18 (a) The next block is an incremental programming
- The next block to G31 is an absolute programming for 1 axis
G31 G90 X200.0 F100;
Y100.0; Y100.0
Skip signal is input here
A
ctual motion
Motion without skip signal
X200.0
Fig. 4.18 (b) The next block is an absolute programming for 1 axis
- The next block to G31 is an absolute programming for 2 axes
100 200 300
A
ctual motion
Motion without skip signal
Skip signal is input here
(300,100)
Y
X
100
G31 G90 X200.0 F100;
X300.0 Y100.0;
Fig. 4.18 (c) The next block is an absolute programming for 2 axes
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 141 -
4.19 MULTI-STEP SKIP (G31)
In a block specifying P1 to P4 after G31, the multi-step skip function
stores coordinates in a custom macro variable when a skip signal
(4-point or 8-point ; 8-point when a high-speed skip signal is used) is
turned on. In the block where Q1 to Q4 are specified after G04, dwell
can be skipped when skip signals (four or eight signals, or eight
signals when high-speed skip signals are used) are input.
A skip signal from equipment such as a fixed-dimension size
measuring instrument can be used to skip programs being executed.
In plunge grinding, for example, a series of operations from rough
machining to spark-out can be performed automatically by applying a
skip signal each time rough machining, semi-fine machining,
fine-machining, or spark-out operation is completed.
Format
Move command
G31 IP_ F_ P_ ;
IP_ : End point
F_ : Feedrate
P_ : P1 to P4
Dwell
G04X(U,P)_ (Q_ );
X(U,P)_ : Dwell time
Q_ : Q1 to Q4
Explanation
Multi-step skip is caused by specifying P1, P2, P3, or P4 in a G31
block. For an explanation of selecting (P1, P2, P3, or P4), refer to the
manual supplied by the machine tool builder.
Specifying Q1, Q2, Q3, or Q4 in G04 (dwell command) enables dwell
skip in a similar way to specifying G31. A skip may occur even if Q is
not specified. For an explanation of selecting (Q1, Q2, Q3, or Q4),
refer to the manual supplied by the machine tool builder.
- Correspondence to skip signals
Parameter Nos. 6202 to 6205 can be used to specify whether the
4-point or 8-point skip signal is used (when a high-speed skip signal is
used). Specification is not limited to one-to-one correspondence. It is
possible to specify that one skip signal correspond to two or more Pn's
or Qn's (n=1, 2, 3, 4). Also, bits 0 (DS1) and 7 (DS8) parameter
No.6206 can be used to specify dwell.
CAUTION
Dwell is not skipped when Qn is not specified and
bits 0 (DS1) and 7 (DS8) parameter No.6206 are
not set.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 142 -
4.20 HIGH-SPEED SKIP SIGNAL (G31)
The skip function operates based on a high-speed skip signal
(connected directly to the NC; not via the PMC) instead of an ordinary
skip signal. In this case, up to eight signals can be input.
Delay and error of skip signal input is 0 - 2 msec at the NC side (not
considering those at the PMC side).
This high-speed skip signal input function keeps this value to 0.1 msec
or less, thus allowing high precision measurement.
For details, refer to the appropriate manual supplied from the machine
tool builder.
Format
G31 IP ;
G31; One-shot G code (If is effective only in the block in
which it is specified)
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 143 -
4.21 CONTINUOUS HIGH-SPEED SKIP FUNCTION
Overview
The continuous high-speed skip function is used to read absolute
coordinates using high-speed skip signals HDI0 to HDI7. Inputting a
high-speed skip signal in a G31P90 block causes absolute coordinates
to be stored in custom macro variables #5061 to #5080. For a system
with more than 20 axes, they are stored in variables #100151 to
#100182. An axis movement does not stop even if a signal is input, so
that the coordinates of multiple points can be read.
Using bit 5 (CSE) of parameter No. 6201, it is possible to enable both
the rising and falling edges of a high-speed skip signal.
For details, refer to the manual supplied by the machine tool builder.
Format
G31 P90 IP ;
G31; One-shot G code (If is effective only in the block in
which it is specified)
Explanation
- Custom macro variables
If a high-speed skip signal is input when G31P90 is issued, absolute
coordinates are stored in custom macro variables #5061 to #5080. For
a system exceeding 20 axes, they are stored in variables #100151 to
#100182.
These variables are updated as soon as the axis reaches a new skip
position. It is, therefore, necessary to specify a speed so that the axis
reaches the next skip position in a period of time longer than it takes
for the application to read the variable values.
System with 20 or less axes System with more than 20 axes
#5061 Coordinates on the first
axis
#100151 Coordinates on the first
axis
#5062 Coordinates on the
second axis
#100152 Coordinates on the
second axis
#5063 Coordinates on the third
axis
#100153 Coordinates on the third
axis
: :
#5079 Coordinates on the 19th
axis
#100181 Coordinates on the 31st
axis
#5080 Coordinates on the 20th
axis
#100182 Coordinates on the
32nd axis
- High-speed skip signal
This function works with a high-speed skip signal only.
Select a high-speed skip signal with bits 0 to 7 (9S1 to 9S8) of
parameter No. 6208.
- Ending a block
A G31P90 block is ended when the axis reaches the end point.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 144 -
Limitation
The continuous high-speed skip function (G31P90) block must be a
command for a single axis only. If an attempt is made to specify two
or more axes, P/S alarm No. 5068 is issued.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 145 -
4.22 TORQUE LIMIT SKIP
Overview
Executing the move command following G31P99 (or G31P98) while
overriding the torque limit*1 on the servo motor enables cutting feed in
to be performed in the same way as in linear interpolation (G01). If,
during the movement with this command, the torque of the servo
motor reaches the torque limit value (torque limit on the servo motor
multiplied by the override) due to pressing or other causes or a skip
signal (including a high-speed skip signal) is input, any remaining
move commands will be canceled, and the next block is executed.
(The operation of canceling any remaining move commands and
executing the next block is called a skip operation in the remainder of
this document.)
It is possible to override the torque limit on the servo motor with the
following command methods:
(1) Execute the torque limit override command in the PMC window.
(2) Execute an address Q command in the same block as that
containing a G31P99 (or G31P98) command.
*1 : The torque limit on the servo motor is automatically set to a
value conforming to the motor type setting.
Format
G31 P98 Q_ α_ F_
G31 P99 Q_ α_ F_
G31 : Skip command (one-shot G code)
P98 : Performs a skip operation if the torque of the servo motor
reaches the limit value.
P99 : Performs a skip operation if the torque of the servo motor
reaches the limit value or if a skip signal is input.
Q : Override value for the torque limit
Range of valid settings: 1 to 254 (%)
0 to 255 correspond to 0% to 100%.
The Q command is optional. If omitting it, specify the torque
limit command in the PMC window beforehand. If it is
omitted, and no torque limit override is set beforehand,
alarm PS0035 is issued.
If an attempt is made to specify a value out of range, alarm
PS0366 is issued.
The specified override value is effective only to the block in
which it is specified.
At the end of the skip operation, the override value returns to
the one assumed immediately before the G31 command.
α : Axis address on any one axis
F : Feedrate
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 146 -
- Conditions for performing a skip operation
Command
Condition G31P98 G31P99
The torque limit value is reached. A skip operation is
performed.
A skip operation
is performed.
A skip signal is input. No skip operation
is performed.
A skip operation
is performed.
- Operation during a torque limit skip
A torque limit skip presses a specified axis against a previously
prepared part or other item while the torque limit command is being
executed on the servo motor, and then performs a skip operation when
the servo motor reaches the torque limit value. A skip operation is
performed with the fact that the torque limit value as detected in the
servo motor is reached. It is, therefore, not necessary to input a skip
signal using a separate sensor or other device unlike with normal skip
functions.
(1) At point A, the machine comes in contact with the object under
measurement and stops. At this time, because the torque limit
value is not reached, no skip operation is performed, move
commands are continuously output, and the current position of
the CNC is updated.
(2) Because move commands are output but the machine remains
stopped, there occurs a difference (error amount) between the
current position of the CNC and the machine position, and torque
is applied to the servo motor.
(3) When the torque limit value is reached, a skip operation is
performed at machine stop position, point A, and the N2
command is executed. Assuming that the current position of the
CNC when the torque limit is reached is point B, the error
amount during the torque limit skip is (A - B).
(Example)
N1 G31 P99 Q50 Z400.0 F100.0 ;
N2 G01 X300.0 F500.0 ;
100.0 200.0 300.0 400.0
100.0
200.0
300.0
N1
N2
B
A
C
Error amount
X
Z
A
: Machine stop position
B : Current position of the CNC when the
torque limit is reached
C : N1 command end point position
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 147 -
- Torque limit command
If, with the torque limit skip command, no torque limit override value
is specified with address Q and no torque limit command is issued
from the PMC window, etc., alarm PS0035 is issued.
When no toque limit command is issued, the torque limit override
value is either 0% or 100%.
If, in a torque limit skip command block, no torque limit override
value is specified with address Q, a torque limit is to be specified as in
the program example below.
(Program example)
O0012
:
Mxx (Specify a torque limit from the PMC via the window)
:
G31 P99 X200. F100.（Torque limit skip command）
:
G01 X100. F500.
（Move command with the torque limit being still
effective）
:
Myy (Cancel the torque limit from the PMC)
:
M30
- Positional deviation limit during the torque limit command
While the torque limit skip command is being executed, the positional
deviation limit check with the settings of parameters Nos. 1828 and
1829 is not performed. Instead, the positional deviation limit check
with the settings of parameter No. 6287 is performed. If the positional
deviation exceeds the limit, alarm SV0004 is issued and an
instantaneous stop occurs.
- Custom macro variables
When the torque limit skip command is executed, the custom macro
system variables #5061 to #5080 (skip signal position; for a system
with more than 20 axes, variables #100151 to #100182 are used) store
the coordinate position assumed at the end of the skip. In reality, there
is a deviation due to the delay of the servo system between the
machine position and the current position of the CNC when a skip
operation is executed. This deviation can be determined from the
positional deviation of the servo. By setting bit 2 (TSE) of parameter
No. 6201, it is possible to select whether or not the skip signal
position to be stored in system variables should be compensated for
with the error (positional deviation) of the servo system.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 148 -
Position during a skip operation
Current position of the CNC
Machine position Error
Position compensated for by
reflecting the delay
Position not reflecting the dela
y
Coordinate origin Stop point
NOTE
1 Specify only a single axis with the torque limit skip
command. If no axis is specified or an attempt is
made to specify more than one, alarm PS0369 is
issued.
2 Do not issue the torque limit skip command in
3-dimensional coordinate conversion mode or to a
parallel axis. Otherwise, alarm PS0035 is issued.
3 Do not issue the torque limit skip command in G41 or
G42 mode. Otherwise, alarm PS0035 is issued.
4 A torque limit arrival signal is output regardless of the
torque limit skip command.
5 Do not issue the torque limit skip command for an
axis being synchronized with synchronization control
(such as synchronization control, twin table control,
or electronic gear box).
6 Do not specify the torque limit skip command in a
continuous block.
7 The higher the movement speed, the larger the error
between the position at which the machine stops and
the position at which a skip is actually detected. Also,
the error increases as the speed is varied during
movement. Do not vary the speed with override and
so on.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 149 -
4.23 THREE-DIMENSIONAL CIRCULAR INTERPOLATION
Overview
Specifying an intermediate and end point on an arc enables circular
interpolation in a 3-dimensional space.
Format
The command format is as follows:
G02.4 XX1 YY1 ZZ1 αα1 ββ1 ; First block (mid-point of the
arc)
X
X2 YY2 ZZ2 αα2 ββ2 ; Second block (end point of
the arc)
α,β : Arbitrary axes other than the 3-dimensional circular
interpolation axis (up to two axes)
To be specified if necessary.
G03.4 can also be specified instead of G02.4.
G03.4 performs the same operation as G02.4.
Explanation
- G code group
G02.4 and G03.4 are modal G codes of group 01. They therefore
remain effective until another G code in group 01 is specified.
- Start point, mid-point, and end point
An arc in a 3-dimensional space is uniquely defined with its start point
(current position) and a specified intermediate point and end point, as
shown below. Two command blocks are used to define this arc. The
first command block specifies the tool path between the start point and
intermediate point. The second command block specifies the tool path
between the intermediate point and end point.
X
Y
Z
Start point
Mid-point
(X1,Y1,Z1)
End point
(X2,Y2,Z2)
Fig. 4.23 (a) Start, Mid, and End Points
If the modal code is changed by specifying a code such as G01 with
the end point not specified, the arc cannot be obtained, and alarm
PS5432 is issued. During MDI operation, alarm PS5432 is also issued
if a cycle start is applied with only the mid-point specified.
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 150 -
- Movement along axes other than the three-dimensional circular interpolation axis
In addition to the three-dimensional circular interpolation axis
(X/Y/Z), up to two arbitrary axes (α/β) can be specified at a time. If /
are omitted from the first block (mid-point specification) and are
specified only in the second block (end point specification), the tool
moves to the specified point along the α/β axes during movement
from the mid-point of the arc to the end point. If α/β are omitted from
the second block (end point specification) and are specified only in the
first block (mid-point specification), the tool moves to the specified
point along the α/β axes during movement from the start point of the
arc to the mid-point.
- Incremental programming
With an incremental programming, the position of the mid-point
relative to the start point must be specified in the first block, and the
position of the end point relative to the mid-point must be specified in
the second block.
- Direction of rotation
The direction of rotation cannot be specified. The movement is the
same regardless of whether G02.4 or G03.4 is specified.
- Single block
When operation is performed using a single block, one cycle start
causes movement from the start point to the end point. A single-block
stop is not performed between the first block (mid-point specification)
and the second block (end point specification).
- Start point assumed if three-dimensional circular interpolations are specified
consecutively
If three-dimensional circular interpolations are specified consecutively,
the end point in one interpolation is assumed to be the start point in
the next interpolation.
- Velocity commands
As the velocity command, specify the tangential velocity along the arc
in the three-dimensional space.
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 151 -
Limitation
- Cases in which linear interpolation is performed
• f the start point, mid-point, and end-point are on the same line,
linear interpolation is performed.
• If the start point coincides with the mid-point, the mid-point
coincides with the end point, or the end point coincides with the
start point, linear interpolation is performed up to the end point.
• If the start point, mid-point, and end-point are on the same line
and the end point lies between the start point and the mid-point,
the tool first moves with linear interpolation from the start point
to the mid-point, then returns from the mid-point to the end point
with linear interpolation. Thus, the tool always passes through
the specified point.
Start point Mid-pointEnd
p
oint
- Whole circles
A whole circle (360° arc) cannot be specified. (This corresponds to the
case in which linear interpolation is performed, as described earlier.)
- Compensation functions
Before using this function, cancel the compensation functions of
group 07, such as cutter radius compensation.
- Manual absolute
While this function is in use, manual intervention is not possible with
the manual absolute switch set to the ON position. If intervention is
performed, alarm PS5433 is issued when operation restarts.
- Restrictions on commands
In the three-dimensional circular interpolation mode, the functions
listed below can be used, but the states of these functions must not be
modified.
• Inch input/metric input (An alarm is issued if a state
modification is made with G20 or G21.)
• Mirror image (The state of a signal must not be changed.)
• One-digit F code feed (No feedrate change must be made using
the manual handle.)
- Unusable commands
In the three-dimensional circular interpolation mode, the functions
listed below must not be specified. Otherwise, an alarm is issued.
• Exponential interpolation.............................................. G02.3,G03.3
• Dwell ..........................................................................................G04
• High-speed machining ................................................................G05
(Excluding G05P10000 and G05P0)
• AI contour control ................................................ G05.1Q1,G5.1Q0
4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/03
- 152 -
• Hypothetical axis interpolation...................................................G07
• Cylindrical interpolation..........................................................G07.1
• Advanced preview control..........................................................G08
(Use AI high-precision contour control.)
• Polar coordinate interpolation.......................................G12.1,G13.1
• Polar coordinate command ................................................. G15,G16
• Reference position return check .................................................G27
• Reference position return............................................................G28
• 2nd reference position return......................................................G30
• 3rd, 4th reference position return................................................G30
• Skip.............................................................................................G31
• Threading....................................................................................G33
• Automatic tool length measurement ...........................................G37
• 3-dimensional cutter compensation ............................................G41
• Tool offset........................................................... G45,G46,G47,G48
• Programmable mirror image......................................... G50.1,G51.1
• Local coordinate system .............................................................G52
• Machine coordinate system ........................................................G53
• Single direction positioning........................................................G60
• Tapping mode .............................................................................G63
• Macro call (Subprogram call is possible.) .................. G65,G66,G67
• Figure copying .............................................................. G72.1,G72.2
• Canned cycle............................... G73-G79,G80,G81-G89,G98,G99
• Workpiece coordinate system setting .........................................G92
• Workpiece coordinate system preset .......................................G92.1
• Feed per revolution.....................................................................G95
• Constant surface speed control ........................................... G96,G97
• NURBS interpolation...............................................................G06.2
• Workpiece coordinate system setting ......................G54-G59,G54.1
• 3-dimensional coordinate system conversion .............................G68
• Coordinate system rotation.........................................................G68
• Scaling ................................................................................ G50,G51
• Programmable mirror image......................................... G50.1,G51.1
• Exact stop mode..........................................................................G61
• Tool radius/tool nose radius compensation G38,G39,G40,G41,G42
• 3-dimensional cutter compensation ....... G40, G41.2, G41.3, G41.4,
..................................... G41.5, G41.6, G42.2, G42.4, G42.5, G42.6
• Data setting .................................................................................G10
• Exact stop ...................................................................................G09
• Auxiliary function
• 2nd auxiliary function
• Spindle function
• Tool function
B-63944EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS
- 153 -
- Unusable functions
If the following function is specified in the three-dimensional circular
interpolation mode, a warning is output:
• MDI intervention
If any of the following functions is specified in the three-dimensional
circular interpolation mode, the alarm (PS5196) is issued:
• Manual operation interrupt
• Tool retract and recover
In the three-dimensional circular interpolation mode, the following
functions cannot be used:
• Sequence number comparison and stop (Stop operation cannot be
performed with a sequence number in the three-dimensional
circular interpolation mode.)
• Index table indexing
• Rotary axis control
• Macro executor (Execution macro)
• Manual handle interruption
• Optional chamfering/corner R
- Other limitations
When the following function is used, three-dimensional circular
interpolation cannot be used:
• Arbitrary angular axis control
A limitation may be imposed on other NC command combinations.
See the description of each function.
5.FEED FUNCTIONS PROGRAMMING B-63944EN/03
- 154 -
5 FEED FUNCTIONS
Chapter 5, "FEED FUNCTIONS", consists of the following sections:
5.1 OVERVIEW .............................................................................155
5.2 RAPID TRAVERSE .................................................................157
5.3 CUTTING FEED ......................................................................158
5.4 CUTTING FEEDRATE CONTROL ........................................164
5.5 FEEDRATE INSTRUCTION ON IMAGINARY CIRCLE
FOR A ROTARY AXIS ...........................................................169
5.6 DWELL.....................................................................................174
B-63944EN/03 PROGRAMMING 5.FEED FUNCTIONS
- 155 -
5.1 OVERVIEW
The feed functions control the feedrate of the tool. The following two
feed functions are available:
- Feed functions
1. Rapid traverse
When the positioning command (G00) is specified, the tool
moves at a rapid traverse feedrate set in the CNC (parameter No.
1420).
2. Cutting feed
The tool moves at a programmed cutting feedrate.
- Override
Override can be applied to a rapid traverse rate or cutting feedrate
using the switch on the machine operator's panel.
- Automatic acceleration/deceleration
To prevent a mechanical shock, acceleration/deceleration is
automatically applied when the tool starts and ends its movement (Fig.
5.1(a)).
Rapid traverse rate
FR : Rapid traverse
rate
TR : Deceleration time
constant for rapid
traverse rate
0
Time
0
Feedrate
FR
TRTR
FC
TCTC
FC : Feedrate
TC : Acceleration/
deceleration time
constant for a
cutting feedrate
Time
Fig. 5.1 (a) Automatic acceleration/deceleration (example)
5.FEED FUNCTIONS PROGRAMMING B-63944EN/03
- 156 -
- Tool path in a cutting feed
When the movement direction changes between a specified block and
the next block during cutting feed, the tool path may be rounded
because of the relationship between the time constant and feedrate
(Fig. 5.1(b)).
0
Programmed path
A
ctual tool path
Y
X
Fig. 5.1 (b) Example of tool path between two blocks
In circular interpolation, a radial error occurs (Fig. 5.1(c)).
0
Y
X
r
∆
r : Error
Programmed path
A
ctual tool path
Fig. 5.1 (c) Example of radial error in circular interpolation
The rounded-corner path shown in Fig. 5.1(b) and the error shown in
Fig. 5.1 (c) depend on the feedrate. So, the feedrate needs to be
controlled for the tool to move as programmed.
B-63944EN/03 PROGRAMMING 5.FEED FUNCTIONS
- 157 -
5.2 RAPID TRAVERSE
Format
G00 IP_ ;
G00 : G code (group 01) for positioning (rapid traverse)
IP_ : Dimension word for the end point
Explanation
The positioning command (G00) positions the tool by rapid traverse.
In rapid traverse, the next block is executed after the specified feedrate
becomes 0 and the servo motor reaches a certain range set by the
machine tool builder (in-position check).
A rapid traverse rate is set for each axis by parameter No. 1420, so no
rapid traverse feedrate need be programmed.
The following overrides can be applied to a rapid traverse rate with
the switch on the machine operator's panel:F0, 25%, 50%, 100%
F0: Allows a fixed feedrate to be set for each axis by parameter No.
1421.
For detailed information, refer to the appropriate manual of the
machine tool builder.
5.FEED FUNCTIONS PROGRAMMING B-63944EN/03
- 158 -
5.3 CUTTING FEED
Overview
Feedrate of linear interpolation (G01), circular interpolation (G02,
G03), etc. are commanded with numbers after the F code.
In cutting feed, the next block is executed so that the feedrate change
from the previous block is minimized.
M
Four modes of specification are available:
1. Feed per minute (G94)
After F, specify the amount of feed of the tool per minute.
2. Feed per revolution (G95)
After F, specify the amount of feed of the tool per spindle
revolution.
3. Inverse time feed (G93)
Specify the inverse time (FRN) after F.
4. One-digit F code feed
Specify a desired one-digit number after F. Then, the feedrate set
with the CNC for that number is set.
T
Two modes of specification are available:
1. Feed per minute (G98)
After F, specify the amount of feed of the tool per minute.
2. Feed per revolution (G99)
After F, specify the amount of feed of the tool per spindle
revolution.
3. Inverse time feed (G93)
Specify the inverse time (FRN) after F.
Format
M
Feed per minute
G94 ; G code (group 05) for feed per minute
F_ ; Feedrate command (mm/min or inch/min)
Feed per revolution
G95 ; G code (group 05) for feed per revolution
F_ ; Feedrate command (mm/rev or inch/rev)
Inverse time feed (G93)
G93 ; Inverse time feed command G code (05 group)
F_ ; Feedrate command (1/min)
One-digit F code feed
Fn ;
n : Number from 1 to 9
B-63944EN/03 PROGRAMMING 5.FEED FUNCTIONS
- 159 -
T
Feed per minute
G98 ; G code (group 05) for feed per minute
F_ ; Feedrate command (mm/min or inch/min)
Feed per revolution
G99 ; G code (group 05) for feed per revolution
F_ ; Feedrate command (mm/rev or inch/rev)
Inverse time feed (G93)
G93 ; Inverse time feed command G code (05 group)
F_ ; Feedrate command (1/min)
Explanation
- Direction of the cutting feedrate
Cutting feed is controlled so that the tangential feedrate is always set
at a specified feedrate.
X
End point Start
point
X
F
F
Center End
Start
point
Linear interpolation Circular interpolation
YY
Fig. 5.3 (a) Tangential feedrate (F)
- Feed per minute
After specifying G code for feed per minute (in the feed per minute
mode), the amount of feed of the tool per minute is to be directly
specified by setting a number after F. G code for feed per minute is a
modal code. Once a G code for feed per minute is specified, it is valid
until G code for feed per revolution (feed per revolution) is specified.
M
At power-on, the feed per minute mode is set.
T
At power-on, the feed per revolution mode is set.
An override from 0% to 254% (in 1% steps) can be applied to feed per
minute with the switch on the machine operator's panel. For detailed
information, see the appropriate manual of the machine tool builder.
5.FEED FUNCTIONS PROGRAMMING B-63944EN/03
- 160 -
• For milling machining
Workpiece
Table
Tool
Feed amount per minute
(mm/min or inch/min)
• For lathe cutting
Feed amount per minute
(mm/min or Íinch/min)
F
Fig. 5.3 (b) Feed per minute
CAUTION
No override can be used for some commands such
as for threading.
- Feed per revolution
After specifying G code for feed per revolution (in the feed per
revolution mode), the amount of feed of the tool per spindle revolution
is to be directly specified by setting a number after F. G code for
feed per revolution is a modal code. Once a G code for feed per
revolution is specified, it is valid until G code for feed per minute
(feed per minute) is specified.
An override from 0% to 254% (in 1% steps) can be applied to feed per
revolution with the switch on the machine operator's panel. For
detailed information, see the appropriate manual of the machine tool
builder.
T
If bit 0 (NPC) of parameter No. 1402 has been set to 1, feed per
revolution commands can be specified even when a position coder is
not being used. (The CNC converts feed per revolution commands to
feed per minute commands.)
B-63944EN/03 PROGRAMMING 5.FEED FUNCTIONS
- 161 -
• For milling machining
F
Feed amount per spindle
revolution (mm/rev or inch/rev)
• For lathe cutting
Feed amount per spindle revolution
(mm/rev or inch/rev)
F
Fig. 5.3 (c) Feed per revolution
CAUTION
When the speed of the spindle is low, feedrate
fluctuation may occur.
The slower the spindle rotates, the more frequently
feedrate fluctuation occurs.
- Inverse time feed
When G code for inverse time feed is specified, the inverse time
specification mode (G93 mode) is set. Specify the inverse time
(FRN) with an F code.
A value from 0.001 to 9999.999 can be specified as FRN, regardless
of whether the input mode is inches or metric, or the increment system
is IS-B or IS-C.
F code specification value FRN
F1 0.001
F1 (*1) 1.000
F1.0 1.000
F9999999 9999.999
F9999 (*1) 9999.000
F9999.999 9999.999
NOTE
*1 Value specified in fixed-point format with bit 0 (DPI)
of parameter No. 3401 set to 1
5.FEED FUNCTIONS PROGRAMMING B-63944EN/03
- 162 -
G code for inverse time feed is a modal G code and belongs to group
05 (includes G code for feed per revolution and G code for feed per
minute).
When an F value is specified in inverse time specification mode and
the feedrate exceeds the maximum cutting feedrate, the feedrate is
clamped to the maximum cutting feedrate.
In the case of circular interpolation, the feedrate is calculated not from
the actual amount of movement in the block but from the arc radius.
This means that actual machining time is longer when the arc radius is
longer than the arc distance and shorter when the arc radius is shorter
than the arc distance. Inverse time feed can also be used for cutting
feed in a canned cycle.
NOTE
1 In the inverse time specification mode, an F code is
not handled as a modal code and therefore needs
to be specified in each block. If an F code is not
specified, alarm PS0011 (FEED ZERO
(COMMAND)) is issued.
2 When F0 is specified in inverse time specification
mode, alarm PS0011 (FEED ZERO (COMMAND))
is issued.
3 Inverse time feed cannot be used when PMC axis
control is in effect.
4 If the calculated cutting feedrate is smaller than the
allowable range, alarm PS0011 (FEED ZERO
(COMMAND)) is issued.
Example
• For linear interpolation (G01)
distance
feedrate
time(min)
1
FRN ==
Feedrate: mm/min (for metric input)
inch/min (for inch input)
Distance: mm (for metric input)
inch (for inch input)
- To end a block in 1 (min)
1
(min)1
1
(min)
1=== time
FRN
Specify F1.0.
- To end a block in 10 (sec)
6
(sec)60/10
1
60/(sec)
1=== time
FRN
Specify F6.0.
- To find the movement time required when F0.5 is specified
2
5.0
11
(min) === FRN
TIME
2 (min) is required.
B-63944EN/03 PROGRAMMING 5.FEED FUNCTIONS
- 163 -
- To find the movement time required when F10.0 is
specified
6
10
60601
(min) ==
×
=FRN
TIME
6 (sec) is required.
• For circular interpolation (G02, G03)
arcradius
feedrate
time
FRN == (min)
1
Feedrate: mm/min (for metric input)
inch/min (for inch input)
Arc radius: mm (for metric input)
inch (for inch input)
NOTE
In the case of circular interpolation, the feedrate is
calculated not from the actual amount of movement
in the block but from the arcadias.
- One-digit F code feed
M
When a one-digit number from 1 to 9 is specified after F, the feedrate
set for that number in a parameter Nos. 1451 to 1459 is used. When
F0 is specified, the rapid traverse rate is applied.
The feedrate corresponding to the number currently selected can be
increased or decreased by turning on the switch for changing one-digit
F feedrate on the machine operator's panel, then by rotating the
manual pulse generator.
The increment/decrement, ∆F, in feedrate per scale of the manual
pulse generator is as follows:
X
F
F100
max
=∆
Fmax : Feedrate upper limit for F1-F4 set by parameter
(No.1460), or feedrate upper limit for F5-F9 set by
parameter (No.1461)
X : Any value of 1-127 set by parameter No.1450
The feedrate set or altered is kept even while the power is off. The
current feed rate is displayed on the LCD screen.
- Cutting feedrate clamp
Parameter No. 1430 can be used to specify the maximum cutting
feedrate for each axis. When the cutting feedrate along an axis
exceeds the maximum feedrate for the axis as a result of interpolation,
the cutting feedrate is clamped to the maximum feedrate.
Reference
See Appendix D for range of feedrate command value.
5.FEED FUNCTIONS PROGRAMMING B-63944EN/03
- 164 -
5.4 CUTTING FEEDRATE CONTROL
Cutting feedrate can be controlled, as indicated in Table 5.4 (a).
Table 5.4 (a) Cutting Feedrate Control
Function name G code Validity of G code Description
Exact stop G09 This function is valid for
specified blocks only.
The tool is decelerated at the end point of a
block, then an in-position check is made.
Then the next block is executed.
Exact stop mode G61
Once specified, this function is
valid until G62, G63, or G64 is
specified.
The tool is decelerated at the end point of a
block, then an in-position check is made.
Then the next block is executed.
Cutting mode G64
Once specified, this function is
valid until G61, G62, or G63 is
specified.
The tool is not decelerated at the end point of
a block, but the next block is executed.
Tapping mode G63
Once specified, this function is
valid until G61, G62, or G64 is
specified.
The tool is not decelerated at the end point of
a block, but the next block is executed.
When G63 is specified, feedrate override and
feed hold are invalid.
Automatic
override for inner
corners
G62
Once specified, this function is
valid until G61, G63, or G64 is
specified.
When the tool moves along an inner corner
during tool radius compensation, override is
applied to the cutting feedrate to suppress the
amount of cutting per unit of time so that a
good surface finish can be produced.
Automatic
corner
override Internal circular
cutting feedrate
change
-
This function is valid in the tool
radius compensation mode,
regardless of the G code.
The internal circular cutting feedrate is
changed.
NOTE
1 The purpose of in-position check is to check that
the servo motor has reached within a specified
range (specified with a parameter by the machine
tool builder).
In-position check is not performed when bit 5 (NCI)
of parameter No. 1601 is set to 1.
2 Inner corner angle θ: 2° < θ ≤ α ≤ 178°
(α is a set value)
Workpiece
θ
Tool
Format
Exact stop G09 IP_ ;
Exact stop mode G61 ;
Cutting mode G64 ;
Tapping mode G63 ;
Automatic corner override G62 ;
B-63944EN/03 PROGRAMMING 5.FEED FUNCTIONS
- 165 -
5.4.1 Exact Stop (G09, G61), Cutting Mode (G64), Tapping Mode
(G63)
Explanation
The inter-block paths followed by the tool in the exact stop mode,
cutting mode, and tapping mode are different (Fig. 5.4.1 (a)).
Tool
p
ath in the exact sto
p
mode
Tool path in the cutting mode or tapping mode
In-position check
(1)
(2)
Y
0 X
Fig. 5.4.1 (a) Example of tool paths from block (1) to block (2)
CAUTION
The cutting mode (G64 mode) is set at power-on or
system clear.
5.FEED FUNCTIONS PROGRAMMING B-63944EN/03
- 166 -
5.4.2 Automatic Corner Override
When tool radius compensation is performed, the movement of the
tool is automatically decelerated at an inner corner and internal
circular area. This reduces the load on the tool and produces a
smoothly machined surface.
5.4.2.1 Automatic override for inner corners (G62)
Explanation
- Override condition
When G62 is specified, and the tool path with tool radius
compensation applied forms an inner corner, the feedrate is
automatically overridden at both ends of the corner.
There are four types of inner corners (Fig. 5.4.2(a)).
2°≤θ≤θp≤178° in Fig. 5.4.2(a)qp is a value set with parameter No.
1711. When θ is approximately equal to θp, the inner corner is
determined with an error of 0.001° or less.
θ
θ θ
θ
: Tool
: Programmed path
: Tool center path
1. Straight line-straight line 2. Straight line-arc
3. Arc-straight line 4. Arc-arc
Fig. 5.4.2(a) Inner corner
B-63944EN/03 PROGRAMMING 5.FEED FUNCTIONS
- 167 -
- Override range
When a corner is determined to be an inner corner, the feedrate is
overridden before and after the inner corner. The distances Ls and Le,
where the feedrate is overridden, are distances from points on the tool
center path to the corner (Fig. 5.4.2(b), Fig. 5.4.2(c), Fig. 5.4.2(d)). Ls
and Le are set with parameter Nos. 1713 and 1714.
Programmed path
Le
ab
Ls
Tool center path
The feedrate is overridden from point a to point b.
FIg. 5.4.2.1 (b) Override Range (Straight Line to Straight Line)
When a programmed path consists of two arcs, the feedrate is
overridden if the start and end points are in the same quadrant or in
adjacent quadrants (Fig. 5.4.2(c)).
Programmed path
The feedrate is overridden from
p
oint a to b.
Tool center path
Fig. 5.4.2(c) Override Range (Arc to Arc)
Regarding program (2) of an arc, the feedrate is overridden from point
a to point b and from point c to point d (Fig. 5.4.2(d)).
c
d
a
LsLe
b
Ls Le
(2)
Pro
g
rammed
p
ath
Tool center path
Tool
Fig. 5.4.2(d) Override Range (Straight Line to Arc, Arc to Straight Line)
- Override value
An override value is set with parameter No. 1712. An override value
is valid even for dry run and one-digit F code feed specification.
In the feed per minute mode, the actual feedrate is as follows:
override) (feedratecorners)inner for override (automatic ×=F
5.FEED FUNCTIONS PROGRAMMING B-63944EN/03
- 168 -
Limitation
- Acceleration/deceleration before interpolation
Override for inner corners is disabled during acceleration/deceleration
before interpolation.
- Start-up/G41, G42
Override for inner corners is disabled if the corner is preceded by a
start-up block or followed by a block including G41 or G42.
- Offset
Override for inner corners is not performed if the offset is zero.
5.4.2.2 Internal circular cutting feedrate change
For internally offset circular cutting, the feedrate on a programmed
path is set to a specified feedrate (F) by specifying the circular cutting
feedrate with respect to F, as indicated below (Fig. 5.4.2(e)). This
function is valid in the tool radius compensation mode, regardless of
the G62 code.
Rp
Rc
F=
Rc : Tool center path radius
Rp : Programmed radius
It is also valid for the dry run and the one-digit F code feed command.
Rc
Rp
Programmed
Tool center
path
Fig. 5.4.2(e) Internal circular cutting feedrate change
If Rc is much smaller than Rp, Rc/Rp
0; the tool stops. A minimum
deceleration ratio (MDR) is to be specified with parameter No. 1710.
When Rc/Rp≤MDR, the feedrate of the tool is (F×MDR).
CAUTION
When internal circular cutting must be performed
together with override for inner corners, the
feedrate of the tool is as follows:
override) (feedratecorners)inner for the (override ××× Rp
Rc
F
B-63944EN/03 PROGRAMMING 5.FEED FUNCTIONS
- 169 -
5.5 FEEDRATE INSTRUCTION ON IMAGINARY CIRCLE FOR
A ROTARY AXIS
Overview
This function acquires movement feedrate on imaginary circle by
synthetic movement distance is calculated from movement distance of
a rotary axis by using instruction angle and the parameter of an
imaginary radius (No.1465).
Then, movement feedrate on imaginary circle is feedrate of a rotary
axis.
Explanation
Cutting feedrate
- Conventional method
In linear interpolation of a linear axis and a rotary axis, 1deg in
movement angle of a rotary axis is interpolated as 1mm in movement
distance (1inch at inch input).
Program example
N1G91G01X10.F10.;
N2C10.F10.;
It instructs in a instruction feedrate
of a rotary axis at a feedrate of a
rotary axis.
Instruction speed
(deg/min)
X
Y
N2
N1
C
Feedrate of liner axis(X axis)
()
minmmX L
X
FF /
∆
×=
Feedrate of rotary axis(C axis)
()
mindegC L
C
FF /
∆
×=
Synthetic movement distance
()
mm
CBZYXL 22222 ∆+∆+∆+∆+∆=
Movement time )(min
F
L
T=
- Feedrate instruction on imaginary circle of a rotary axis
In this function, synthetic movement distance is obtained based on
movement distance of a rotary axis requested from instruction angle
and the parameter of an imaginary radius(parameter No.1465).
5.FEED FUNCTIONS PROGRAMMING B-63944EN/03
- 170 -
Instruction
feedrate(mm/min)
Imaginary
radius
半径
X
Y
Program example
N1G91G01X10.F10.
N2C10.
Instruction feedrate is feedrate of
a rotary axis on imaginary circle in
a radius specified by the
parameter.
Then, feedrate element of a rotary
axis can be excluded by setting 0
in imaginary radius
N2
N1
C
Feedrate of liner axis(X axis)
()
minmmX L
X
FF /
′
∆
×=
Feedrate of rotary axis(C axis)
()
mindegC L
C
FF /
′
∆
×=
Synthetic movement distance
()
mm
C
BCl
Bl
ZYXL
2
2
222
180180
∆××
+
∆××
+∆+∆+∆=
′
π
π
Movement time
()
min
F
L
T
′
=
′
lB ，lC : imaginary radius(parameter No.1465)
It becomes feedrate from which movement feedrate on imaginary
circle is instructed by this. <Example 1 reference>
In this function, feedrate of a axis becomes LL ′
/ times for the
feedrate displayed on the NC screen from difference of the method of
obtaining movement distance. Especially, a movement of a axis
quickens when small value is set to an imaginary radius. Note input of
the parameter enough.
Cutting feedrate is clamped based on the maximum cutting feedrate
parameter (No.1430) and feedrate of an actual axis (data before this
function is converted). Therefore, it is possible to instruct at feedrate
more than setting the maximum cutting feedrate by setting big value in
an imaginary radius (parameter No.1465). When small value is set in
an imaginary radius, it is clamped at the feedrate following setting the
maximum cutting feedrate.
Moreover, dry run becomes effective as for this function, too.
AI Contour Control
AI contour control is done to movement feedrate on imaginary circle.
Therefore, It is likely not to become feedrate in the calculation in this
function by feedrate control of AI contour control. Then, feedrate of
AI contour Control is clamped at parameter(No.1432). Moreover, it is
clamped at parameter(No.8465), When the parameter(No.8465) is not
0.
B-63944EN/03 PROGRAMMING 5.FEED FUNCTIONS
- 171 -
0mm in imaginary radius
When an imaginary radius is assumed 0mm, synthesized distance is as
follows because the movement distance of a rotary axis becomes
0mm.
222 ZYXL ∆+∆+∆=
′
A movement feedrate of a linear axis can be instruction feedrate F by
excluding feedrate element of a rotary axis.<Example 2 reference>
Moreover, it moves at the maximum cutting feedrate in case of this
setting and instruction only in a rotary axis.
Examples
- Example 1
When the follwing block is instructed on IS-B,
G91 G01 C10. F10. ;
The calculation is as follows, when 10.000(10mm) is set in an
imaginary radius(parameter No.1465).
()
)()(
)/(
)(
)/(
)(
)(
min/
)(
2
)()(
2
4719755.1017453292.0
10
7453292.1
2957795.57
7453292.1
10
10
7453292.1
180
1010
180
secmin
minmm
mm
mindeg
mm
deg
mmC
mm
degmm
C
F
L
T
F
Bl
L
⋅⋅⋅=⋅⋅⋅=
⋅⋅⋅
=
′
=
′
⋅⋅⋅=
⋅⋅⋅
×=
⋅⋅⋅=
××
=
∆××
=
′
π
π
Therefor, the movement time becomes about 10.472(sec), and the
rotation feedrate becomes about 57.296(deg/min). The feedrate on
10.000mm in an imaginary radius becomes 10.000mm/min at
instruction feedrate in Fig.5.5(a).
The calclation is as follows, when 36.000(36mm) is set in an
imaginary radius(parameter No.1465).
()
)()(
)/(
)(
)/(
)(
)(
/
)(
2
)()(
2
6991118.37628318530.0
10
28318530.6
9154943.15
28318530.6
10
10
28318530.6
180
1036
180
secmin
minmm
mm
mindeg
mm
deg
minmmC
mm
degmm
C
F
L
T
F
Bl
L
⋅⋅⋅=⋅⋅⋅=
⋅⋅⋅
=
′
=
′
⋅⋅⋅=
⋅⋅⋅
×=
⋅⋅⋅=
××
=
∆××
=
′
π
π
Therefor, the movement time becomes about 37.700(sec), and the
rotation feedrate becomes about 15.915(deg/min). The feedrate on
36.000mm in an imaginary radius becomes 10.000mm/min at
instruction feedrate in Fig.5.5(a).
5.FEED FUNCTIONS PROGRAMMING B-63944EN/03
- 172 -
10mm
36mm
Instruction feedrate
F=10mm/min
Rotation feedrate when
36mm setting.:(2)
Rotation feedrate when
10mm setting.:(1)
Fig. 5.5 (a)
- Example 2
When a machine into which direction of a tool changes by a rotary
axis like Fig2, movement feedrate of a standard point can be assumed
to be instruction feedrate F by making this function effective and
setting 0 in imaginary radius(parameter No.1465) .
The feedrate element of a rotary
axis is excluded.
The movement feedrate of a
standard point becomes
instruction feedrate F.
Standard point
Fig. 5.5 (b)
B-63944EN/03 PROGRAMMING 5.FEED FUNCTIONS
- 173 -
Limitation
This function corresponds only the linear interpolation(G01).
However, it doesn't correspond to the following functions.
• Inverse time feed
• Feed per revolution
• Normal direction control
• High-speed cycle cutting
• Cylindrical interpolation
• Polar coordinate interpolation
• Tool center point control for 5-axis machining
• Axis control by PMC
• Manual numerical command
In this function, in case of using the parallel axis control and the twin
table control, an imaginary radius parameter(No.1465) specifies the
same value with a master axis and a slave axis.
NOTE
1 When the parameter ROTx (No.1006#0) and the
parameter RFDx (No.1408#0) are 1, this function
becomes effective.
2 The parameter RFDx (No.1408#0) and an
imaginary radius (parameter No.1465) of this
function can be rewriting by the programable
parameter input(G10).
3 It moves at the maximum cutting feedrate when
this function effectively and sets 0 in an imaginary
radius (parameter No.1465) and it instructs only a
rotary axis.
4 Note setting RFDx (No.1408#0) and an imaginary
radius (parameter No.1465) enough. Especially, a
movement of axis quickens compared with this
function unused when small value is set to an
imaginary radius.
5 In this function, the same value as the parameter
value (No.1408, No.1465) of a master axis is used
with a slave axis, when it uses axis synchronous
control.
5.FEED FUNCTIONS PROGRAMMING B-63944EN/03
- 174 -
5.6 DWELL
Format
M
G04 X_; or G04 P_;
X_ : Specify a time or spindle speed (decimal point permitted)
P_ : Specify a time or spindle speed (decimal point not
permitted)
T
G04 X_ ; or G04 U_ ; or G04 P_ ;
X_ : Specify a time or spindle speed (decimal point permitted)
U_ : Specify a time or spindle speed (decimal point permitted)
P_ : Specify a time or spindle speed (decimal point not
permitted)
Explanation
By specifying a dwell, the execution of the next block is delayed by
the specified time. (Dwell per second)
By setting bit 1 (DWL) of parameter No. 3405 in the feed per
revolution mode, the execution of the next block is delayed until the
rotation count of the spindle reaches the specified number. (Dwell
per revolution)
Table 5.6 (a) Command value range of the dwell time (Command by X or U)
Increment system Command value range Dwell time unit
IS-A 0.01 to 999999.99
IS-B 0.001 to 99999.999
IS-C 0.0001 to 9999.9999
IS-D 0.00001 to 999.99999
IS-E 0.000001 to 99.999999
s or rev
Table 5.6 (b) Command value range of the dwell time (Command by P)
Increment system Command value range Dwell time unit
IS-A 1 to 99999999 0.01 s or rev
IS-B 1 to 99999999 0.001 s or rev
IS-C 1 to 99999999 0.0001 s or rev
IS-D 1 to 99999999 0.00001 s or rev
IS-E 1 to 99999999 0.000001 s or rev
B-63944EN/03 PROGRAMMING 5.FEED FUNCTIONS
- 175 -
In the case of dwell per second, the specification unit for dwell time
specified with P can be fixed at 0.001 second by setting bit 7 (DWT)
of parameter No. 1015 to 1.
NOTE
1 When X, U, or P is specified without a decimal
point, the specification unit does not depend on
inch/metric input. Depending on whether the
X-axis is present, the following increment system is
used:
• When the X-axis is present
The increment system of the X-axis is used.
• When the X-axis is not present
The increment system of the reference axis is
used.
2 When P is specified, bit 7 (IPR) of parameter No.
1004 exercises no influence.
M
Specify dwell also to make an exact check in the cutting mode (G64
mode).
If the specification of P and X is omitted, an exact stop occurs.
6.REFERENCE POSITION PROGRAMMING B-63944EN/03
- 176 -
6 REFERENCE POSITION
A CNC machine tool has a special position where, generally, the tool
is exchanged or the coordinate system is set, as described later. This
position is referred to as a reference position.
Chapter 6, "REFERENCE POSITION", consists of the following
sections:
6.1 REFERENCE POSITION RETURN........................................177
6.2 FLOATING REFERENCE POSITION RETURN (G30.1) .....184
B-63944EN/03 PROGRAMMING 6.REFERENCE POSITION
- 177 -
6.1 REFERENCE POSITION RETURN
Overview
- Reference position
The reference position is a fixed position on a machine tool to which
the tool can easily be moved by the reference position return function.
For example, the reference position is used as a position at which tools
are automatically changed. Up to four reference positions can be
specified by setting coordinates in the machine coordinate system in
parameters (No. 1240 to 1243).
Reference position
Machine zero point
3rd reference position
2nd reference position
4th reference
position
Y
X
Fig. 6.1 (a) Machine zero point and reference positions
- Automatic reference position return (G28) and movement from the reference
position (G29)
The automatic reference position return (G28) function returns tools
automatically to the reference position via an intermediate position
along a specified axis. When reference position return is completed,
the lamp for indicating the completion of reference position return
goes on. The return from reference position (G29) function moves
tools from the reference position to a specified position via an
intermediate position along a specified axis.
A
(Start position for reference
position return)
C (Destination of return from
the reference position)
R (Reference position)
A
utomatic reference position return (G28)
A
→ B → R
Movement from the reference position (G29)
R
→ B → C
B (Intermediate
position)
Fig. 6.1 (b) Reference position return and return form the reference
position
6.REFERENCE POSITION PROGRAMMING B-63944EN/03
- 178 -
- Reference position return check (G27)
The reference position return check (G27) is the function which
checks whether the tool has correctly returned to the reference
position as specified in the program. If the tool has correctly
returned to the reference position along a specified axis, the lamp for
the axis for indicating the completion of reference position return goes
on.
If the tool has not reached the reference position, an alarm (PS0092)
"ZERO RETURN CHECK (G27) ERROR" is issued.
When no movement was made along the axis, whether the current
position is the reference position is checked.
Format
- Automatic reference position return and 2nd/3rd/4th reference position return
G28 IP_; Reference position return
G30 P2 IP_; 2nd reference position return (P2 can be
omitted.)
G30 P3 IP_; 3rd reference position return
G30 P4 IP_; 4th reference position return
IP : Specify the intermediate position in the absolute
coordinate system.
(absolute/incremental programming)
There is no need to calculate an actual travel distance
between the intermediate position and the reference
position.
- Movement from reference position
G29 IP_;
IP : Specify the destination of return from the reference
position in the absolute coordinate system.
(absolute/incremental programming)
The intermediate position is determined by G28, G30, or
G30.1 specified immediately before this command.
- Reference position return check
G27 IP_;
IP : Specify positioning to the reference position in the
absolute coordinate system so as to return to the
reference position. (absolute/incremental programming)
B-63944EN/03 PROGRAMMING 6.REFERENCE POSITION
- 179 -
Explanation
- Automatic reference position return (G28)
Positioning to the intermediate or reference positions are performed at
the rapid traverse rate of each axis.
Therefore, for safety, the compensation functions, such as the tool
radius compensation and tool length compensation, should be
cancelled before executing this command.
The coordinates for the intermediate position are stored in the CNC
for the axes for which a value is specified in a G28 block. For the
other axes, the previously specified coordinates are used.
(Example)
N1 G28 X40.0 ;
(The tool moves to the reference position along the X-axis and
the intermediate position (X40.0) is stored.)
N2 G28 Y60.0 ;
(The tool moves to the reference position along the Y-axis and
the intermediate position (Y60.0) is stored.)
N3 G29 X10.0 Y20.0 ;
(The tool moves to the position specified with G29 via the
intermediate position (X40.0 Y60.0) previously specified with
G28 along the X-axis and Y-axis.)
- 2nd, 3rd, and 4th reference position return (G30)
The 2nd, 3rd, and 4th reference position return (G30) function can be
used after the reference positions are established.
The G30 command is generally used when the automatic tool changer
(ATC) position differs from the reference position.
- Movement from the reference position (G29)
This function is executed after the tool is returned to the reference
position by G28 or G30.
For incremental programming, the command value specifies the
incremental value from the intermediate point.
The tool moves to the intermediate and specified positions at the
feedrate specified with a parameter.
When the workpiece coordinate system is changed after the tool
reaches the reference position through the intermediate point by the
G28 command, the intermediate point also shifts to a new coordinate
system. If G29 is then commanded, the tool moves to the
commanded position through the intermediate point which has been
shifted to the new coordinate system.
The same operations are performed also for G30 and G30.1
commands.
After the power is turned on, an alarm (PS0305) is issued if an attempt
is made to execute G29 (movement from the reference position)
before G28 (automatic reference position return), G30 (2nd, 3rd, and
4th reference position return), or G30.1 (floating reference position
return) is executed.
6.REFERENCE POSITION PROGRAMMING B-63944EN/03
- 180 -
- Reference position return check (G27)
G27 command positions the tool at rapid traverse rate. If the tool
reaches the reference position, the lamp for indicating the completion
of reference position return lights up.
When the tool returns to the reference position along only one axis,
the lamp for the axis for indicating the completion of reference
position return lights up.
After positioning, if the tool has not reached the reference position
along a specified axis, an alarm (PS0092) "ZERO RETURN CHECK
(G27) ERROR" is issued.
When no movement was made along the axis, whether the current
position is the reference position is checked.
B-63944EN/03 PROGRAMMING 6.REFERENCE POSITION
- 181 -
- Setting of the reference position return feedrate
Before a coordinate system is established with the first reference
position return after power-on, the manual and automatic reference
position return feedrates and automatic rapid traverse rate conform to
the setting of parameter No. 1428 for each axis.
After a reference position is established upon the completion of
reference position return, the manual reference position return feedrate
conforms to the setting of the parameter No. 1428 for each axis.
NOTE
1 To this feedrate, a rapid traverse override (F0,25,50,100%) is applied, for which
the setting is 100%.
2 After a reference position has been established upon the completion of reference
position return, the automatic reference position return feedrate will conform to the
ordinary rapid traverse rate.
3 When a value is set for parameter No. 1428, the feedrates conform to the
parameter settings shown below.
Before a coordinate system
is established
After a coordinate system is
established
Automatic reference position return (G28) No. 1428 No.1420
Automatic rapid traverse (G00) No.1428 No.1420
Manual reference position return (*1) No.1428 No.1428 (*3)
Manual rapid traverse rate No.1423 (*2) No.1424
1420: Rapid traverse rate
1423: Jog feedrate
1424: Manual rapid traverse rate
1428: Reference position return feedrate
When parameter No. 1428 is set to 0, the feedrates conform to the parameter settings
shown below.
Before a coordinate system
is established
After a coordinate system is
established
Automatic reference position return (G28) No. 1420 No.1420
Automatic rapid traverse (G00) No.1420 No.1420
Manual reference position return (*1) No.1424 No.1424 (*3)
Manual rapid traverse rate No.1423 (*2) No.1424
*1 By using JZR (bit 2 of parameter No. 1401), the manual reference position
return feedrate can always be set as a jog feedrate.
*2 When RPD (bit 0 of parameter No. 1401) is 1, the setting of parameter No.
1424 (manual rapid traverse rate) is used.
When the setting of parameter No. 1424 (manual rapid traverse rate) is 0,
parameter No. 1420 (rapid traverse rate) is used.
*3 When reference position return without dogs is performed in rapid traverse
mode, or when manual reference position return is performed in rapid
traverse mode regardless of deceleration dogs after a reference position is
established, the reference position return feedrate for each of these functions
(setting of DLF (bit 1 of parameter No. 1404)) is used.
6.REFERENCE POSITION PROGRAMMING B-63944EN/03
- 182 -
Limitation
- Status the machine lock being turned on
The lamp for indicating the completion of reference position return
does not go on when the machine lock is turned on, even when the
tool has automatically returned to the reference position. In this case,
it is not checked whether the tool has returned to the reference
position even when a reference position return check command is
specified.
- When automatic reference position return (G28) is executed if no reference
position is established
When automatic reference position return (G28) is executed if no
reference position is established, movement from the intermediate
position in a reference position direction is the same as that in manual
reference position return.
(This movement is referred to as a low-speed type of automatic
reference position return (G28).)
In this case, the tool moves in the direction for reference position
return specified in parameter ZMIx (bit 5 of No. 1006). Therefore
the specified intermediate position must be a position to which
reference position return is possible.
NOTE
When automatic reference position return (G28) is
executed after a reference position is established,
positioning is performed from the intermediate
position to the reference position. This movement
is referred to as a high-speed type of automatic
reference position return (G28).
- Reference position return check in an offset mode
In an offset mode, the position to be reached by the reference position
return check is the position obtained by adding the offset value.
Therefore, if the position with the offset value added is not the
reference position, the lamp for indicating the completion of reference
position return does not light up, but an alarm is displayed instead.
Usually, cancel offsets before G27 is commanded.
- Lighting the lamp when the programmed position does not coincide with the
reference position
When the machine tool system is an inch system with metric input, the
lamp for indicating the completion of reference position return may
also light up even if the programmed position is shifted from the
reference position by the least setting increment. This is because the
least setting increment of the machine tool system is smaller than its
least command increment.
B-63944EN/03 PROGRAMMING 6.REFERENCE POSITION
- 183 -
Example
G28G90X1000.0Y500.0 ;
(Programs movement from A to B. The tool moves to
reference position R via intermediate position B.)
T1111 ;
(Changing the tool at the reference position)
G29X1300.0Y200.0 ;
(Programs movement from B to C. The tool moves from
reference position R to C specified with G29 via intermediate
position B.)
200
300
500
200 1000 1300
Y
X
A
utomatic reference position return (G28)
A → B → R
Movement from the reference position (G29)
R → B → C
A
(Start position for reference
position return)
B (Intermediate
position)
C (Destination of return from the
reference position)
R (Reference position)
Fig. 6.1 (c) Reference position return and movement from the reference position
6.REFERENCE POSITION PROGRAMMING B-63944EN/03
- 184 -
6.2 FLOATING REFERENCE POSITION RETURN (G30.1)
Tools ca be returned to the floating reference position.
A floating reference point is a position on a machine tool, and serves
as a reference point for machine tool operation.
A floating reference point need not always be fixed, but can be moved
as required.
Format
G30.1 IP_;
IP_ : Specify the intermediate position to the floating
reference position in the absolute coordinate system.
(absolute/incremental programming)
Explanation
Generally speaking, on a machining center or milling machine, cutting
tools can be replaced only at specific positions. A position where tools
can be replaced is defined as the second or third reference point. Using
G30 can easily move the cutting tools back to these points.
On some machine tools, the cutting tools can be replaced at any
position unless they interfere with the workpiece. With these
machines, the cutting tools should be replaced at a position as close to
the workpiece as possible so as to minimize the machine cycle time.
For this purpose, the tool change position is to be changed, depending
on the figure of the workpiece. This operation can easily be
performed using this function.
That is, a tool change position suitable for the workpiece is
memorized as a floating reference point. Then command G30.1 can
easily cause return to the tool change position.
A floating reference point becomes a machine coordinate position
memorized by pressing the soft key [SETFRP] on the current
positions display screen. The coordinates of the floating reference
position are stored with parameter No. 1244.
The G30.1 block first positions the tool at the intermediate point along
the specified axes at rapid traverse rate, then further moves the tool
from the intermediate point to the floating reference point at rapid
traverse rate. Before using G30.1, cancel the compensation functions,
such as tool radius compensation and tool length compensation.
A floating reference point is not lost even if power is turned off.
The function for movement from the reference position (G29) can be
specified for moving the tool from the floating reference position.
B-63944EN/03 PROGRAMMING 6.REFERENCE POSITION
- 185 -
Example
Y
X
Workpiece
Intermediate position (50,40)
Floating reference
position
G30.1 G90 X50.0 Y40.0 ;
7.COORDINATE SYSTEM PROGRAMMING B-63944EN/03
- 186 -
7 COORDINATE SYSTEM
By teaching the CNC a desired tool position, the tool can be moved to
the position. Such a tool position is represented by coordinates in a
coordinate system. Coordinates are specified using program axes.
When three program axes, the X-axis, Y-axis, and Z-axis, are used,
coordinates are specified as follows:
X_Y_Z_
This command is referred to as a dimension word.
• For milling machining (Tool position specified by
X40.0Y50.0Z25.0 )
Z
Y
X
40.0
50.0
25.0
• For lathe cutting (Tool position specified by X50.0 Z40.0)
X
Zero point
40.0
Z
50.0
Coordinates are specified in one of following three coordinate
systems:
(1) Machine coordinate system
(2) Workpiece coordinate system
(3) Local coordinate system
The number of the axes of a coordinate system varies from one
machine to another. So, in this manual, a dimension word is
represented as IP_.
B-63944EN/03 PROGRAMMING 7.COORDINATE SYSTEM
- 187 -
7.1 MACHINE COORDINATE SYSTEM
The point that is specific to a machine and serves as the reference of
the machine is referred to as the machine zero point. A machine tool
builder sets a machine zero point for each machine.
A coordinate system with a machine zero point set as its origin is
referred to as a machine coordinate system.
A machine coordinate system is set by performing manual reference
position return after power-on (see III-3.1). A machine coordinate
system, once set, remains unchanged until the power is turned off.
The reference position is not always the origin of the machine
coordinate system.
(See "Setting a machine coordinate system" described later.)
Format
M
(G90) G53 IP_ P1;
IP_: Absolute dimension word
P1: Enables the high-speed G53 function.
T
G53 IP_ P1;
IP_: Absolute dimension word
P1: Enables the high-speed G53 function.
Explanation
- Selecting a machine coordinate system (G53)
When a command is specified the position on a machine coordinate
system, the tool moves to the position by rapid traverse. G53, which
is used to select a machine coordinate system, is a one-shot G code;
that is, it is valid only in the block in which it is specified on a
machine coordinate system. Specify an absolute command for G53.
When an incremental command is specified, the G53 command is
ignored. When the tool is to be moved to a machine-specific position
such as a tool change position, program the movement in a machine
coordinate system based on G53.
- High-speed G53 function
This function enables the inter-rapid traverse block overlap function
between machine coordinate selection command (G53) and
positioning (rapid traverse) command (G00) blocks, thus making it
possible to execute the next rapid traverse command (G00) without
decelerating to a stop at the end of the machine coordinate selection
command (G53). Therefore, high-speed positioning is available even
when the machine coordinate selection command (G53) is used.
Specifying P1 in a G53 block enables the high-speed G53 function.
7.COORDINATE SYSTEM PROGRAMMING B-63944EN/03
- 188 -
Limitation
- Cancel of the compensation function
When the G53 command is specified, cancel the compensation
functions such as the cutter compensation, tool length compensation,
tool nose radius compensation, and tool offset.
- G53 specification immediately after power-on
Since the machine coordinate system must be set before the G53
command is specified, at least one manual reference position return or
automatic reference position return by the G28 command must be
performed after the power is turned on. This is not necessary when
an absolute-position detector is attached.
- Blocks in which the high-speed G53 function is usable
The high-speed G53 function is usable in the following combinations
of commands:
• G53 → G00
• G53 → G53
The high-speed G53 function is unusable in the following
combination of commands:
• G00 → G53
- Specification in the same block
M
Commands G50/G51, G50.1/G51.1, and G68/G69 cannot be specified
in the same block where the G53 command is specified.
T
Commands G50/G51 (except for G code system A), G50.1/G51.1, and
G68.1/G69.1 cannot be specified in the same block where the G53
command is specified.
Note
NOTE
G53 is a G code for disabling buffering.
Reference
- Setting a machine coordinate system
When manual reference position return is performed after power-on, a
machine coordinate system is set so that the reference position is at the
coordinate values of (α, β) set using parameter No.1240.
B-63944EN/03 PROGRAMMING 7.COORDINATE SYSTEM
- 189 -
β
Reference position
Machine coordinate system
Machine zero point
α
7.COORDINATE SYSTEM PROGRAMMING B-63944EN/03
- 190 -
7.2 WORKPIECE COORDINATE SYSTEM
Overview
A coordinate system used for machining a workpiece is referred to as
a workpiece coordinate system. A workpiece coordinate system is to
be set with the CNC beforehand (setting a workpiece coordinate
system).
A machining program sets a workpiece coordinate system (selecting a
workpiece coordinate system).
A set workpiece coordinate system can be changed by shifting its
origin (changing a workpiece coordinate system).
7.2.1 Setting a Workpiece Coordinate System
A workpiece coordinate system can be set using one of three methods:
(1) Method using a workpiece coordinate system setting G code
A workpiece coordinate system is set by specifying a value in the
program after a workpiece coordinate system setting G code.
(2) Automatic setting
If bit 0 of parameter ZPR No. 1201 is set to 1, a workpiece
coordinate system is automatically set when manual reference
position return is performed (see III-3.1.).
This function is, however, disabled when the workpiece
coordinate system option is being used.
(3) Method using a workpiece coordinate system selection G code
Six workpiece coordinate systems can be set beforehand using
the MDI panel. Program commands G54 to G59 can be used to
select the workpiece axis to be used. (see III-12.3.4.)
When using an absolute command, establish the workpiece coordinate
system in any of the above ways.
Format
- Setting a workpiece coordinate system
M
(G90) G92 IP_
T
G50 IP_
B-63944EN/03 PROGRAMMING 7.COORDINATE SYSTEM
- 191 -
Explanation
A workpiece coordinate system is set so that a point on the tool, such
as the tool tip, is at specified coordinates.
M
If a coordinate system is set using G92 during tool length offset, a
coordinate system in which the position before offset matches the
position specified in G92 is set. Cutter compensation is cancelled
temporarily with G92.
T
If IP_ is an incremental command value, the workpiece coordinate
system is defined so that the current tool position coincides with the
result of adding the specified incremental value to the coordinates of
the previous tool position. If a coordinate system is set using G50
during offset, a coordinate system in which the position before offset
matches the position specified in G50 is set.
Example
M
25.2 X
Z
23.0
0
X
Z
600.0
IIf an absolute command is issued, the
base point moves to the commanded
position. In order to move the tool tip to
the commanded position, the difference
from the tool tip to the base point is
compensated by tool length offset (see II-
14.1).
(Example 2)
Setting the coordinate system by the G92X600.0Z1200.0; command (The
base point on the tool holder is the start point for the program.)
0
Base point
1200.0
(Example 1)
Setting the coordinate system by the
G92X25.2Z23.0; command (The tool tip is the start
point for the program.)
7.COORDINATE SYSTEM PROGRAMMING B-63944EN/03
- 192 -
T
(Example 1)
Setting the coordinate system by the G50X128.7Z375.1;
command (Diameter designation) (The tool nose is the
start point for the program.)
(Example 2)
Setting the coordinate system by the G50X1200.0Z700.0;
command (Diameter designation) (The base point on the turret is
the start point for the program.)
Z
X
Origin
375.1 Start point
φ128.7
Z
X
700.0
Start point
(base point)
φ
1200.0
CAUTION
The set workpiece coordinate system depends on
diameter programming or radius programming.
Notes
- Command for setting a workpiece coordinate system in the tool length
compensation mode
Executing a workpiece coordinate system setting G code command
(G92 or, for G code system A in the lathe system, G50) presets a
coordinate system in such a way that the specified position will be a
pre-compensation position.
However, this G code cannot be used together with a block where tool
length compensation vectors vary. For example, it cannot be used
together with the following blocks.
EXAMPLE
1 Block in which G43/G44 is issued
2 Block which is in the G43 or G44 mode and in
which an H code is issued
3 Block which is in the G43 or G44 mode and in
which G49 is issued
4 Block in which, in the G43 or G44 mode,
compensation vectors are canceled using a G code
such as G28 or G53 and then resumed again
When presetting a workpiece coordinate system, using the workpiece
coordinate system setting G code, do not stop in the previous block to
change a tool length compensation offset selected, for example, with
the MDI.
B-63944EN/03 PROGRAMMING 7.COORDINATE SYSTEM
- 193 -
7.2.2 Selecting a Workpiece Coordinate System
The user can choose from set workpiece coordinate systems as
described below. (For information about the methods of setting, see
II-7.2.1.)
(1) Once a workpiece coordinate system is set by a workpiece
coordinate system setting G code or by automatic workpiece
coordinate system setting, absolute commands indicate positions
in the workpiece coordinate system.
(2) Choosing from six workpiece coordinate systems set using the
MDI panel
By specifying a G code from G54 to G59, one of the workpiece
coordinate systems 1 to 6 can be selected.
G54 : Workpiece coordinate system 1
G55 : Workpiece coordinate system 2
G56 : Workpiece coordinate system 3
G57 : Workpiece coordinate system 4
G58 : Workpiece coordinate system 5
G59 : Workpiece coordinate system 6
Workpiece coordinate system 1 to 6 are established after
reference position return after the power is turned on. When the
power is turned on, G54 coordinate system is selected.
When bit 2 (G92) of parameter No. 1202 is set to 1, executing the
workpiece coordinate system setting G92 code command results in the
issue of an alarm PS0010. This is designed to prevent the user from
confusing coordinate systems.
CAUTION
The set workpiece origin offset value depends on
diameter programming or radius programming.
Example
X
Y
100.0
40.
Workpiece coordinate system 2 (G55)
In this example, positioning is made to
positions (X=40.0, Y=100.0) in workpiece
coordinate system 2.
G90 G55 G00 X40.0 Y100.0 ;
Fig. 7.2.2 (a)
7.COORDINATE SYSTEM PROGRAMMING B-63944EN/03
- 194 -
7.2.3 Changing Workpiece Coordinate System
The six workpiece coordinate systems specified with G54 to G59 can
be changed by changing an external workpiece origin offset value or
workpiece origin offset value.
Three methods are available to change an external workpiece origin
offset value or workpiece origin offset value.
(1) Inputting from the MDI panel (see III-12.3.4)
(2) Programming (using a programmable data input G code or a
workpiece coordinate system setting G code)
(3) Using the external data input function
An external workpiece origin offset value can be changed by
input signal to CNC. Refer to machine tool builder's manual for
details.
Workpiece
coordinate system 1
(G54)
Workpiece
coordinate system 2
(G55)
Workpiece
coordinate system 3
(G56)
Workpiece
coordinate system 4
(G57)
Workpiece coordinate
system 5 (G58)
Workpiece coordinate
system 6 (G59)
ZOFS2 ZOFS3 ZOFS4
ZOFS5
ZOFS1
ZOFS6
Machine zero point
EXOFS : External workpiece origin offset value
ZOFS1 to ZOFS6 : Workpiece origin offset value
EXOFS
Fig. 7.2.3 (a) Changing an external workpiece origin offset value or workpiece origin offset value
Format
- Changing by inputting programmable data
G10 L2 Pp IP_;
p=0 : External workpiece origin offset value
p=1 to 6 : Workpiece origin offset value correspond to
workpiece coordinate system 1 to 6
IP_ : For an absolute command, workpiece origin offset for
each axis.
For an incremental command, value to be added to
the set workpiece origin offset for each axis (the result
of addition becomes the new workpiece origin offset).
B-63944EN/03 PROGRAMMING 7.COORDINATE SYSTEM
- 195 -
- Changing by setting a workpiece coordinate system
M
G92 IP_ ;
T
G50 IP_ ;
Explanation
- Changing by inputting programmable data
By specifying a programmable data input G code, the workpiece
origin offset value can be changed for each workpiece coordinate
system.
- Changing by setting a workpiece coordinate system
By specifying a workpiece coordinate system setting G code, the
workpiece coordinate system (selected with a code from G54 to G59)
is shifted to set a new workpiece coordinate system so that the current
tool position matches the specified coordinates (IP_).
Then, the amount of coordinate system shift is added to all the
workpiece origin offset values. This means that all the workpiece
coordinate systems are shifted by the same amount.
CAUTION
When a coordinate system is set with workpiece
coordinate system setting G92 code command
after an external workpiece origin offset value is
set, the coordinate system is not affected by the
external workpiece origin offset value. When
G92X100.0Z80.0; is specified, for example, the
coordinate system having its current tool reference
position at X = 100.0 and Z = 80.0 is set.
T
If IP is an incremental command value, the workpiece coordinate
system is defined so that the current tool position coincides with the
result of adding the specified incremental value to the coordinates of
the previous tool position. (Coordinate system shift)
7.COORDINATE SYSTEM PROGRAMMING B-63944EN/03
- 196 -
Example
M
X
X’
Y’
Y
Tool position
A
160 100
100
100
200
If G92X100Y100; is commanded when the tool is positioned
at (200, 160) in G54 mode, workpiece coordinate system 1
(X' - Y') shifted by vector A is created.
New workpiece coordinate system
Original workpiece coordinate system
G54 workpiece coordinate system
60
Suppose that a G54 workpiece coordinate
system is specified. Then, a G55 workpiece
coordinate system where the black circle on
the tool (figure at the left) is at (600.0,1200.0)
can be set with the following command if the
relative relationship between the G54
workpiece coordinate system and G55
workpiece coordinate system is set correctly:
G92X600.0Z1200.0;
A
lso, suppose that pallets are loaded at two
different positions. If the relative relationship
of the coordinate systems of the pallets at the
two positions is correctly set by handling the
coordinate systems as the G54 workpiece
coordinate system and G55 workpiece
coordinate system, a coordinate system shift
with G92 in one pallet causes the same
coordinate system shift in the other pallet.
This means that workpieces on two pallets
can be machined with the same program just
by specifying G54 or G55.
G54 workpiece coordinate system
1200.0
Z
Z
X'
600.0
600.0
1200.0
G55 workpiece coordinate system
Z'
Z'
X
X
X' - Z' ...........New workpiece coordinate system
X - Z .............Original workpiece coordinate system
A
: Offset value created by G92
B : Workpiece origin offset value in the G54
C : Workpiece origin offset value in the G55
A
B
C
A
X'
A
B-63944EN/03 PROGRAMMING 7.COORDINATE SYSTEM
- 197 -
Example
T
XX'
Tool position
A
160 100
100
100
200
If G50X100Z100; is commanded when the tool is
positioned at (200, 160) in G54 mode, workpiece
coordinate system 1 (X' - Z') shifted by vector A is
created.
New workpiece coordinate system
Original workpiece coordinate system
G54 workpiece coordinate system
60
Z
Z'
G54 workpiece coordinate system
Z
Z
X'
600.0
Z'
Z'
X
X
Suppose that a G54 workpiece coordinate
system is specified. Then, a G55
workpiece coordinate system where the
black tool nose point on the tool (figure at
the left) is at (600.0,1200.0) can be set
with the following command if the relative
relationship between the G54 workpiece
coordinate system and G55 workpiece
coordinate system is set correctly:
G50X600.0Z1200.0;
A
lso, suppose that loading is performed at
two different places and that the G54 and
G55 workpiece coordinate systems are
set for these two places. If the relative
relationship between the coordinate
systems in the two places is correctly set,
a coordinate system shift with G50 in one
loading place causes the same
coordinate system shift in the other
loading place. This means that
workpieces on the two loading positions
can be machined with the same program
j
ust by specifying G54 or G55.
X' - Z'............ New workpiece coordinate system
X - Z ............. Original workpiece coordinate system
A
: Offset value created by G50
B : Workpiece origin offset value in G54
C : Workpiece origin offset value in G55
A
B
C
A
X'
1200.0
1200.0
600.0
G55 workpiece coordinate system
7.COORDINATE SYSTEM PROGRAMMING B-63944EN/03
- 198 -
7.2.4 Workpiece Coordinate System Preset (G92.1)
The workpiece coordinate system preset function presets a workpiece
coordinate system shifted by manual intervention to the pre-shift
workpiece coordinate system. The latter system is displaced from
the machine zero point by a workpiece origin offset value.
There are two methods for using the workpiece coordinate system
preset function. One method uses a programmed command. The
other uses MDI operations on the absolute position display screen,
relative position display screen, and overall position display screen
(see III-12.1.4).
Format
M
G92.1 IP 0 ;
IP 0 : Specifies axis addresses subject to the workpiece
coordinate system preset operation. Axes that are
not specified are not subject to the preset operation.
T
G50.3 IP0 ; (G92.1 IP 0; for G code system B or C)
IP 0 : Specifies axis addresses subject to the workpiece
coordinate system preset operation. Axes that are
not specified are not subject to the preset operation.
Explanation
When manual reference position return operation is performed in the
reset state, a workpiece coordinate system is shifted by the workpiece
origin offset value from the machine coordinate system zero point.
Suppose that the manual reference position return operation is
performed when a workpiece coordinate system is selected with G54.
In this case, a workpiece coordinate system is automatically set which
has its origin displaced from the machine zero point by the G54
workpiece origin offset value; the distance from the origin of the
workpiece coordinate system to the reference position represents the
current position in the workpiece coordinate system.
Reference position
G54 workpiece coordinate system
Workpiece origin
Manual reference position return
Machine zero point
G54 workpiece
origin offset value
B-63944EN/03 PROGRAMMING 7.COORDINATE SYSTEM
- 199 -
If an absolute position detector is provided, the workpiece coordinate
system automatically set at power-up has its origin displaced from the
machine zero point by the G54 workpiece origin offset value. The
machine position at the time of power-up is read from the absolute
position detector and the current position in the workpiece coordinate
system is set by subtracting the G54 workpiece origin offset value
from this machine position. The workpiece coordinate system set by
these operations is shifted from the machine coordinate system using
the commands and operations listed below.
(a) Manual intervention performed when the manual absolute signal
is off
(b) Move command executed in the machine lock state
(c) Movement by handle interruption
(d) Operation using the mirror image function
(e) Shifting the workpiece coordinate system by setting the local
coordinate system or workpiece coordinate system
In the case of (a) above, the workpiece coordinate system is shifted by
the amount of movement during manual intervention.
WZn-
Machine zero point
Workpiece origin
offset value
WZo
G54 workpiece
coordinate system before
manual intervention
G54 workpiece coordinate
system after manual
intervention
Po
Pn
A
mount of
movement during
manual intervention
In the operation above, a workpiece coordinate system once shifted
can be preset using G code (G92.1) specification or MDI operation to
a workpiece coordinate system displaced by a workpiece origin offset
value from the machine zero point.
Bit 3 (PPD) of parameter No. 3104 specifies whether to preset relative
coordinates (RELATIVE) as well as absolute coordinates.
When no workpiece coordinate system option (G54 to G59) is
selected, the workpiece coordinate system is preset to the coordinate
system with its origin placed at the reference position.
7.COORDINATE SYSTEM PROGRAMMING B-63944EN/03
- 200 -
Limitation
- Tool radius ⋅ tool nose radius compensation, tool length compensation, tool
offset
When using the workpiece coordinate system preset function, cancel
compensation modes: Tool radius ⋅ tool nose radius compensation,
tool length compensation, and tool offset. If the function is executed
without canceling these modes, compensation vectors are cancelled.
M
- Tool length compensation
When using the workpiece coordinate system preset function, cancel
tool length compensation. If the function is executed without
canceling these modes, compensation vectors are cancelled.
- Program restart
The workpiece coordinate system preset function is not executed
during program restart.
- Prohibited modes
Do not use the workpiece coordinate system preset function when the
scaling, coordinate system rotation, programmable image, or figure
copy mode is set.
B-63944EN/03 PROGRAMMING 7.COORDINATE SYSTEM
- 201 -
7.2.5 Addition of Workpiece Coordinate System Pair (G54.1 or G54)
Besides the six workpiece coordinate systems (standard workpiece
coordinate systems) selectable with G54 to G59, 48 or 300 additional
workpiece coordinate systems (additional workpiece coordinate
systems) can be used.
Format
- Selecting the additional workpiece coordinate systems
G54.1Pn ; or G54Pn ;
Pn : Codes specifying the additional workpiece coordinate
systems
n : 1 to 48 or 1 to 300
- Setting the workpiece origin offset value in the additional workpiece coordinate
systems (G10)
G10L20Pn IP_;
Pn : Codes specifying the workpiece coordinate system for
setting the workpiece origin offset value
n : 1 to 48 or 1 to 300
IP_ : Axis addresses and a value set as the workpiece
origin offset
Explanation
- Selecting the additional workpiece coordinate systems
When a P code is specified together with G54.1 (G54), the
corresponding coordinate system is selected from the additional
workpiece coordinate systems (1 to 48 or 1 to 300).
A workpiece coordinate system, once selected, is valid until another
workpiece coordinate system is selected. Standard workpiece
coordinate system 1 (selectable with G54) is selected at power-on.
G54.1 P1 ......... Additional workpiece coordinate system 1
G54.1 P2 ......... Additional workpiece coordinate system 2
:
G54.1 P48 ....... Additional workpiece coordinate system 48
:
G54.1 P300 ..... Additional workpiece coordinate system 300
7.COORDINATE SYSTEM PROGRAMMING B-63944EN/03
- 202 -
As with the standard workpiece coordinate systems, the following
operations can be performed for a workpiece origin offset in an
additional workpiece coordinate system:
(1) The workpiece origin offset value setting screen can be used to
display and set a workpiece origin offset value.
(2) The G10 function enables a workpiece origin offset value to be
set by programming (refer to II-7.2.3).
(3) A custom macro allows a workpiece origin offset value to be
handled as a system variable.
(4) Workpiece origin offset data can be entered or output as external
data.
(5) The PMC window function enables workpiece origin offset data
to be read as program command modal data.
- Setting the workpiece origin offset value in the additional coordinate systems
(G10)
When a workpiece origin offset value is specified using an absolute
value, the specified value is the new offset value. When it is
specified using an incremental value, the specified value is added to
the current offset value to obtain a new offset value.
Limitation
- Specifying P codes
A P code must be specified after G54.1 (G54). If G54.1 is not
followed by a P code in the same block, additional workpiece
coordinate system 1 (G54.1P1) is assumed.
If a value not within the specifiable range is specified in a P code, an
alarm PS0030 is issued.
P codes other than workpiece offset numbers cannot be specified in a
G54.1 (G54) block.
Example 1) G54.1G04P1000;
Example 2) G54.1M98P48;
B-63944EN/03 PROGRAMMING 7.COORDINATE SYSTEM
- 203 -
7.2.6 Automatic Coordinate System Setting
When bit 0 (ZPR) of parameter No. 1201 for automatic coordinate
system setting is 1, a coordinate system is automatically determined
when manual reference position return is performed.
Once α, β, and γ are set with parameter No. 1250, a workpiece
coordinate system is set upon reference position return so that the base
point on the tool holder or the tip of the basic tool is positioned at X =
α, Y = β, and Z = γ.
This processing occurs as if the following are specified at the
reference position:
M
G92XαYβZγ;
T
G50XαZγ;
This function cannot be used, however, when the workpiece
coordinate system option is selected.
T
When the setting of a workpiece coordinate system shift amount is
other than 0, a workpiece coordinate system shifted by the amount is
set.
7.COORDINATE SYSTEM PROGRAMMING B-63944EN/03
- 204 -
7.2.7 Workpiece Coordinate System Shift
T
Explanation
When the coordinate system actually set by the G50 command or the
automatic system setting deviates from the programmed workpiece
system, the set coordinate system can be shifted (see III-3.1).
Set the desired shift amount in the workpiece coordinate system shift
memory.
Z
X
z
xX-Z : Coordinate system in programming
x-z : Current set coordinate system with shift amount 0
(coordinate system to be modified by shifting)
O
O’
Set the shift amount from O' to O in the workpiece coordinate system shift memory.
Shift
Fig. 7.2.7 (a) Workpiece coordinate system shift
Format
- Changing the workpiece coordinate system shift amount
G10 P0 IP_;
IP : Settings of an axis address and a workpiece coordinate
system shift amount
CAUTION
A single block can contain a combination of X, Y, Z,
C, U, V, W, and H (in G code system A). In this
case, if commands are specified for the same axis,
whichever appears later becomes valid.
B-63944EN/03 PROGRAMMING 7.COORDINATE SYSTEM
- 205 -
Limitation
- Shift amount and coordinate system setting command
Specifying a coordinate system setting command (G50 or G92)
invalidates the shift amount that has already been set.
Example)
When G50X100.0Z80.0; is specified, a coordinate system is set
so that the current base position of the tool is at X =100.0 and Z
= 80.0, regardless of which value has been set for the workpiece
coordinate system shift amount.
- Shift amount and coordinate system setting
After a shift amount is set, when automatic coordinate system setting
is performed upon manual reference position return, the set coordinate
system is immediately shifted by the set amount.
- Diameter and radius values
The workpiece coordinate system shift amount depends on diameter
programming or radius programming.
Example)
Although the base point should be positioned at X = φ120.0
(diameter value) and Z = 70.0 from the workpiece origin, the
actual position is at X = φ121.0 and Z = 69.0 from the origin.
Set a shift amount as shown below:
X=1.0, Z=-1.0
Z
X69.0
Start point = base
point
φ121.0
7.COORDINATE SYSTEM PROGRAMMING B-63944EN/03
- 206 -
7.3 LOCAL COORDINATE SYSTEM
When a program is created in a workpiece coordinate system, a child
workpiece coordinate system can be set for easier programming.
Such a child coordinate system is referred to as a local coordinate
system.
Format
G52 IP_; Setting the local coordinate system
:
G52 IP 0 ; Canceling of the local coordinate system
IP_ : Origin of the local coordinate system
Explanation
By specifying G52 IP_;, a local coordinate system can be set in all the
workpiece coordinate systems (G54 to G59). The origin of each
local coordinate system is set at the position specified by IP_ in the
workpiece coordinate system.
Once a local coordinate system is established, the coordinates in the
local coordinate system are used in an axis shift command. The local
coordinate system can be changed by specifying the G52 command
with the origin of a new local coordinate system in the workpiece
coordinate system.
To cancel the local coordinate system or specify the coordinate value
in the workpiece coordinate system, match the origin of the local
coordinate system with that of the workpiece coordinate system.
(Local coordinate system)
(Local coordinate system)
(Machine coordinate system)
Machine coordinate system zero point
Reference position
(G59: Workpiece coordinate
system 6)
(G54: Workpiece coordinate system 1)
G55 G56 G57
G58
IP_
IP_
Fig. 7.3 (a) Setting the local coordinate system
B-63944EN/03 PROGRAMMING 7.COORDINATE SYSTEM
- 207 -
CAUTION
1 When ZCL (bit 2 of parameter No.1201) is set to 1
and an axis returns to the reference position by the
manual reference position return function, the
origin of the local coordinate system of the axis
matches that of the workpiece coordinate system.
The same is true when the following command is
issued:
G52α0;
α: Axis which returns to the reference position
2 The local coordinate system setting does not
change the workpiece and machine coordinate
systems.
3 Whether the local coordinate system is canceled at
reset depends on the parameter setting. The local
coordinate system is canceled when either bit 6
(CLR) of parameter No.3402 or bit 3 (RLC) of
parameter No.1202 is set to 1. In
three-dimensional coordinate conversion mode,
however, the local coordinate system is not
canceled when bit 2 (D3R) of parameter No. 5400
is set to 1.
4 When a workpiece coordinate system is set with
the G92 (G50 for G code system A in the T series)
command, the local coordinate system is canceled.
However, the local coordinate system of an axis for
which no coordinate system is specified in a G92
(G50 for G code system A in the T series) block
remains unchanged.
5 G52 cancels the offset temporarily in tool radius ⋅
tool nose radius compensation.
6 Command a move command immediately after the
G52 block in the absolute mode.
7.COORDINATE SYSTEM PROGRAMMING B-63944EN/03
- 208 -
7.4 PLANE SELECTION
Select the planes for circular interpolation, cutter compensation, and
drilling by G-code.
The following table lists G-codes and the planes selected by them.
Explanation
Table 7.4 (a) Plane selected by G code
G code Selected plane Xp Yp Zp
G17 Xp Yp plane
G18 Zp Xp plane
G19 Yp Zp plane
X-axis or an
axis parallel to
it
Y-axis or an
axis parallel to
it
Z-axis or an
axis parallel to
it
Xp, Yp, Zp are determined by the axis address appeared in the block
in which G17, G18 or G19 is commanded.
When an axis address is omitted in G17, G18 or G19 block, it is
assumed that the addresses of basic three axes are omitted.
Parameter No. 1022 is used to specify that an optional axis be parallel
to the each axis of the X-, Y-, and Z-axes as the basic three axes.
The plane is unchanged in the block in which G17, G18 or G19 is not
commanded.
The movement instruction is irrelevant to the plane selection.
M
When the power is turned on or the CNC is reset, G17 (XY plane),
G18 (ZX plane), or G19 (YZ plane) is selected by bits 1 (G18) and 2
(G19) of parameter No. 3402).
T
When the power is turned on, G18 (ZX plane) is selected.
NOTE
U-, V-, and W-axes can be used with G-codes B
and C.
Example
Plane selection when the X-axis is parallel with the U-axis.
G17X_Y_ XY plane,
G17U_Y_ UY plane
G18X_Z_ ZX plane
X_Y_ Plane is unchanged (ZX plane)
G17 XY plane
G18 ZX plane
G17 U_ UY plane
G18Y_ ; ZX plane, Y axis moves regardless without any
relation to the plane.
B-63944EN/03 PROGRAMMING 8.COORDINATE VALUE AND DIMENSION
- 209 -
8 COORDINATE VALUE AND DIMENSION
Chapter 8, "COORDINATE VALUE AND DIMENSION", consists
of the following sections:
8.1 ABSOLUTE AND INCREMENTAL PROGRAMMING .......210
8.2 INCH/METRIC CONVERSION (G20, G21)...........................212
8.3 DECIMAL POINT PROGRAMMING ....................................216
8.4 DIAMETER AND RADIUS PROGRAMMING .....................218
8.5 DYNAMIC SWITCHING OF DIAMETER/RADIUS
SPECIFICATION .....................................................................219
8.COORDINATE VALUE AND DIMENSION PROGRAMMING B-63944EN/03
- 210 -
8.1 ABSOLUTE AND INCREMENTAL PROGRAMMING
There are two ways to command travels of the tool; the absolute
programming, and the incremental programming. In the absolute
programming, coordinate value of the end position is programmed.
The incremental programming is used to program the amount of a tool
movement.
M
G90 and G91 are used to programming absolute or incremental
programming, respectively.
T
Absolute programming or incremental programming is used
depending on the programming used. See following tables.
G code system A B or C
Command method Address word G90, G91
Format
M
Absolute programming G90 IP_ ;
Incremental programming G91 IP_ ;
T
- G code system A
Absolute
programming
Incremental
programming
X axis move command X U
Z axis move command Z W
Y axis move command Y V
C axis move command C H
- G code system B or C
Absolute programming G90 IP_ ;
Incremental programming G91 IP_ ;
B-63944EN/03 PROGRAMMING 8.COORDINATE VALUE AND DIMENSION
- 211 -
Example
M
A
bsolute programming
Incremental programming
G90 X40.0 Y70.0 ;
G91 X-60.0 Y40.0 ;
Y
X
70.0
30.0
40.0 100.0
End point
Start point
T
Tool movement from point P to point Q (diameter programming is
used for the X-axis)
G code system A G code system B or C
Absolute programming X400.0 Z50.0 ; G90 X400.0 Z50.0 ;
Incremental
programming U200.0 W-400.0 ; G91 X200.0 Z-400.0 ;
φ400
φ
200
50
450
P
(
200, 450
)
Q
(
400, 50
)
Z
X
NOTE
1 Absolute programming and incremental
programming can be used together in a block.
In the above example, the following command can
be specified : X400.0 W-400.0 ; (in the G code
system A)
2 When both X and U or Z and W are used together
in a block, the one specified later is effective.
3 Incremental programming cannot be used when
names of the axes are A and B during G code
system A is selected.
8.COORDINATE VALUE AND DIMENSION PROGRAMMING B-63944EN/03
- 212 -
8.2 INCH/METRIC CONVERSION (G20, G21)
Either inch or metric input (least input increment) can be selected by
G code.
Format
G20 ; Inch input
G21 ; Metric input
This G code must be specified in an independent block before setting
the coordinate system at the beginning of the program. After the G
code for inch/metric conversion is specified, the unit of input data is
switched to the least inch or metric input increment of increment
system (II-2.3). The unit of data input for degrees remains unchanged.
The unit systems for the following values are changed after
inch/metric conversion:
• Feedrate commanded by F code
• Positional command
• Workpiece origin offset value
• Tool compensation value
• Unit of scale for manual pulse generator
• Movement distance in incremental feed
• Some parameters
When the power is turned on, the G code is the same as that held
before the power was turned off.
WARNING
G20 and G21 must not be switched during a
program.
NOTE
1 When the least input increment and the least
command increment systems are different, the
maximum error is half of the least command
increment. This error is not accumulated.
2 The inch and metric input can also be switched
using settings (see III-12.3.1).
3 If a function selected using bit 2 (IRF) of parameter
No. 14000 or bit 0 (NIM) of parameter No. 11222 is
not used, be sure to perform inch/metric conversion
at the reference position (machine coordinate
system origin).
B-63944EN/03 PROGRAMMING 8.COORDINATE VALUE AND DIMENSION
- 213 -
Performing inch/metric conversion in the reference position (parameter No. 1240 is
not 0)
Conventionally, inch/metric conversion must be performed at the
machine coordinate system origin. However, setting bit 2 (IRF) of
parameter No. 14000 to 1 enables inch/metric conversion to be
performed in the reference position (parameter No. 1240).
If an attempt is made to perform inch/metric conversion when an axis
with this function enabled is not in the reference position, alarm
PS5362 is issued to cancel the attempt.
Before trying to perform inch/metric conversion, be sure to set the
axis of interest to the reference position, using the G28 command, for
example.
In addition, if the workpiece coordinate system has been shifted from
the machine coordinate system, using the following commands or
operations, bit 1 (CIM) of parameter No. 11222 can be used to select
whether to issue alarm PS1298 or to clear the offset.
• Manual intervention performed with the manual absolute signal
being off
• Move command issued with the machine locked
• Move command issued using a handle interrupt
• Mirror image-based operation
• Workpiece coordinate system shift caused by local coordinate
system setting (G52) or workpiece coordinate system setting
(G92)
Switching conditions
Performing inch/metric conversion in any position other than the
reference position requires satisfying all of the following conditions.
Failing to satisfy any of the conditions results in alarm PS1298 being
issued. For electronic gear box 2 pair synchronization or electronic
gear box synchronization, alarm PS1595 is issued.
• Positioning or linear interpolation
• Polar coordinate interpolation cancel mode
• Polar coordinate command cancel
• Spindle Speed fluctuation detection off
• Tool radius ⋅ tool nose radius compensation cancel /
3-dimensional tool compensation cancel
• Normal direction control cancel
• Tool length offset cancel
• Scaling cancel
• Programmable mirror image cancel
• Polygon turning cancel
• Macro modal call A/B cancel
• Coordinate system rotation or 3-dimensional coordinate system
conversion mode off
• Mirror image for double turret or balanced cutting mode cancel
(T series only)
• Canned cycle cancel
8.COORDINATE VALUE AND DIMENSION PROGRAMMING B-63944EN/03
- 214 -
• Electronic gear box 2 pair synchronization cancel
• Electronic gear box synchronization cancel
• Constant surface speed control cancel
In addition, performing inch/metric conversion in any position other
than the reference position requires the following options.
• Inch/metric conversion
• Workpiece coordinate system
Restrictions
When performing the following operations, make sure that the axis of
interest is in the reference position (machine coordinate system
origin).
• Inch/metric conversion based on bit 2 (INI) of setting parameter
No. 0
• Inch/metric conversion based on programmable parameter input
(G10)
• Inch/metric conversion based on custom macro variable No.
3005
Performing inch/metric conversion in positions other than the reference position
Setting bit 0 (NIM) of parameter No. 11222 enables inch/metric
conversion to be performed even in positions other than the reference
position.
In addition, if the workpiece coordinate system has been shifted from
the machine coordinate system, using the following commands or
operations, bit 1 (CIM) of parameter No. 11222 can be used to select
whether to issue alarm PS1298 or to clear the offset.
• Manual intervention performed with the manual absolute signal
being off
• Move command issued with the machine locked
• Move command issued using a handle interrupt
• Mirror image-based operation
• Workpiece coordinate system shift caused by local coordinate
system setting (G52) or workpiece coordinate system setting
(G92)
If an axis is under any of the following controls, however, no
automatic coordinate system conversion based on this function can be
carried out for the axis.
• Axis control by PMC
• Axis synchronous control (for slave axes when the master axis is
a PMC axis)
• Flexible synchronous control (for slave axes when the master
axis is a PMC axis)
• Chopping
• Spindle control with servo motor
• Spindle control with Cs contour control
• Servo/spindle synchronous control
B-63944EN/03 PROGRAMMING 8.COORDINATE VALUE AND DIMENSION
- 215 -
Switching conditions
Performing inch/metric conversion in any position other than the
reference position requires satisfying all of the following conditions.
Failing to satisfy any of the conditions results in alarm PS1298 being
issued. For electronic gear box 2 pair synchronization or electronic
gear box synchronization, alarm PS1595 is issued.
• Positioning or linear interpolation
• Polar coordinate interpolation cancel mode
• Polar coordinate command cancel
• Spindle Speed fluctuation detection off
• Tool radius ⋅ tool nose radius compensation cancel /
3-dimensional tool compensation cancel
• Normal direction control cancel
• Tool length offset cancel
• Scaling cancel
• Programmable mirror image cancel
• Polygon turning cancel
• Macro modal call A/B cancel
• Coordinate system rotation or 3-dimensional coordinate system
conversion mode off
• Mirror image for double turret or balanced cutting mode cancel
(T series only)
• Canned cycle cancel
• Electronic gear box 2 pair synchronization cancel
• Electronic gear box synchronization cancel
• Constant surface speed control cancel
In addition, performing inch/metric conversion in any position other
than the reference position requires the following options.
• Inch/metric conversion
• Workpiece coordinate system
• Workpiece coordinate system preset
Restrictions
When performing the following operations, make sure that the axis of
interest is in the reference position (machine coordinate system
origin).
• Inch/metric conversion based on bit 2 (INI) of setting parameter
No. 0
• Inch/metric conversion based on programmable parameter input
(G10)
• Inch/metric conversion based on custom macro variable No.
3005
8.COORDINATE VALUE AND DIMENSION PROGRAMMING B-63944EN/03
- 216 -
8.3 DECIMAL POINT PROGRAMMING
Numerical values can be entered with a decimal point. A decimal
point can be used when entering a distance, time, or speed. Decimal
points can be specified with the following addresses:
M
X, Y, Z, U, V, W, A, B, C, I, J, K, Q, R, F
T
X, Y, Z, U, V, W, A, B, C, I, J, K, R, F
Explanation
There are two types of decimal point notation: calculator-type notation
and standard notation.
When calculator-type decimal notation is used, a value without
decimal point is considered to be specified in millimeters inch, or deg.
When standard decimal notation is used, such a value is considered to
be specified in least input increments. Select either calculator-type
or standard decimal notation by using the bit 0 (DPI) of parameter
No.3401.Values can be specified both with and without decimal point
in a single program.
Example
Program command
Pocket calculator
type decimal point
programming
Standard type decimal point
programming
X1000
Command value
without decimal point
1000mm
Unit :mm
1mm
Unit : Least input increment
(0.001mm)
X1000.0
Command value with
decimal point
1000mm
Unit :mm
1000mm
Unit :mm
CAUTION
When specifying a dimension word for a command
G code in a block, be sure to place the dimension
word after the command G code.
B-63944EN/03 PROGRAMMING 8.COORDINATE VALUE AND DIMENSION
- 217 -
NOTE
1 A specified value less than the minimum unit is
treated as described below.
Example 1)
When a value is specified directly at an address
(in the case of IS-B)
X1.2345 ; Treated as X1.235
X-1.2345 ; Treated as X-1.234
Example 2)
When a value is assigned to a macro variable (in
the case of IS-B)
#100=1.2345;
X#100 ; Treated as X1.235
#100=-1.2345;
X#100 ; Treated as X-1.234
2 When more than eight digits are specified, an
alarm occurs. If a value is entered with a decimal
point, the number of digits is also checked after the
value is converted to an integer according to the
least input increment.
Examples:
X1.23456789;
Alarm PS0003 occurs because more than
eight digits are specified.
X123456.7;
If the least input increment is 0.001 mm, the
value is converted to integer 123456700.
Because the integer has more than eight
digits, an alarm occurs.
8.COORDINATE VALUE AND DIMENSION PROGRAMMING B-63944EN/03
- 218 -
8.4 DIAMETER AND RADIUS PROGRAMMING
Since the workpiece cross section is usually circular in CNC lathe
control programming, its dimensions can be specified in two ways :
Diameter and Radius
Zaxis
A
B
D1
X axis
D2
R1
R2
D1, D2 : Diameter programming
R1, R2 : Radius programming
When the diameter is specified, it is called diameter programming and
when the radius is specified, it is called radius programming.
Explanation
- Notes on diameter programming/radius programming for each command
Radius programming or diameter programming can be specified by bit
3 (DIA) of parameter No.1006. When using diameter programming,
note the conditions listed in the Table 8.4 (a).
Table 8.4 (a) Notes on specifying diameter value
Item Notes
X axis command Specified with a diameter value
Incremental command
Specified with a diameter value
In the above figure, specifies D2
minus D1 for tool path B to A.
Coordinate system setting (G50) Specifies a coordinate value with a
diameter value
Component of tool offset value
Bit 1 of parameter No.5004
determines either diameter or radius
value
Parameters in canned cycle, such
as cutting depth along X axis. (R) Specifies a radius value
Radius designation in circular
interpolation (R, I, K, and etc.) Specifies a radius value
Feedrate along axis Specifies change of radius/rev. or
change of radius/min.
Display of axis position Displayed as diameter value
B-63944EN/03 PROGRAMMING 8.COORDINATE VALUE AND DIMENSION
- 219 -
8.5 DIAMETER AND RADIUS SETTING SWITCHING
FUNCTION
Overview
Usually, whether to use diameter specification or radius specification
to specify a travel distance on each axis is uniquely determined by the
setting of bit 3 (DIAx) of parameter No. 1006. However, this
function enables switching between diameter specification and radius
specification by using a signal or G code.
Thus, a coordinate, program, and so forth can be specified by
switching between diameter specification and radius specification for
each controlled axis.
Explanation
- Selection of a diameter/radius specification switching method
Two methods are available for switching between diameter
specification and radius specification:
1) Signal
2) G code
Use bit 5 (PGD) of parameter No. 3400 to determine which method to
use.
- Switching method using a signal
For switching between diameter specification and radius specification,
set the diameter/radius specification switch signal from DI1 to DI8
(input signals) corresponding to a desired axis, from 0 to 1.
If an input signal is set from 0 to 1, and radius specification is selected
(with bit 3 (DIAx) of parameter No. 1006 = 0) for the axis
corresponding to the input signal, the specification method switches to
diameter specification; the specification method switches to radius
specification if diameter specification is selected (with bit 3 (DIAx) of
parameter No. 1006 = 1).
During switching, the diameter/radius specification switching
in-progress signal from DM1 to DM8 (output signals) corresponding
to a switched axis is output.
To return the diameter/radius specification of an axis to the original
state, set the setting of the corresponding diameter/radius specification
switch signal from DI1 to DI8, from 1 to 0.
8.COORDINATE VALUE AND DIMENSION PROGRAMMING B-63944EN/03
- 220 -
NOTE
1 When operating an input signal by using an M
code, for example, during automatic operation,
perform a switching operation according to the
method below to reflect the state of diameter/radius
specification switching in the execution block
correctly.
As an auxiliary function for switching, use an
unbuffered M code (parameter No. 3411 and up).
Use the following sequences for a specified M
code:
- When switching is performed
Ｍ code → Input signal ON → Confirmation of
output signal ON → FIN
- When switching is cancelled
Ｍ code → Input signal OFF → Confirmation of
output signal OFF → FIN
If a diameter/radius specification switch signal is
operated during automatic operation without
following the sequences above, alarm PS5320 is
issued.
2 If a diameter/radius specification switch signal is
operated while a movement is made on an axis
subject to switching, alarm PS5320 is issued.
- Switching method using a G code (programmable diameter/radius specification
switching)
The format of a G code for diameter/radius specification switching is
as follows:
Format
G10.9 IP_ ;
IP_ : Address and command value of an specified axis
subject to diameter/radius specification switching
Specify 0 or 1 as the command value.
0: Radius specification
1: Diameter specification
NOTE
1 Specify G10.9 in a single block specifying no other
codes.
2 After an axis address, specify a command value
without using the decimal point.
B-63944EN/03 PROGRAMMING 8.COORDINATE VALUE AND DIMENSION
- 221 -
- Switching operation
According to the switching methods above, diameter/radius
specification is internally switched as described below.
1) Switching using a signal
• When parameter DIAx = 0 (radius specification) →
Operation is performed with diameter specification.
• When parameter DIAx = 1 (diameter specification) →
Operation is performed with radius specification.
2) Switching using a G code
• When the specified address value = 0 (radius specification)
→ Operation is performed with radius specification.
• When the specified address value = 1 (diameter
specification) → Operation is performed with diameter
specification.
NOTE
1 When the diameter/radius specification switching
state is to be cancelled using a reset or mode
switching at the time of signal-based switching, the
input signal needs to be operated.
2 Switching using a G code is cancelled by a reset.
CAUTION
When switching is performed from diameter
specification to radius specification, the travel
distance based on the same move command is
doubled when compared with diameter
specification. So, when switching from diameter
specification to radius specification, ensure safety
in machine operation.
- Selecting the machine coordinate system
When diameter and radius setting switching is taking place as directed
with the diameter and radius setting switching function, the
coordinates specified by a machine coordinate system select command
(G53) vary depending on the value of bit 7 (PDM) of parameter No.
11222. If the parameter PDM is 0, diameter and radius switching
occurs. If the parameter PDM is 1, the coordinates vary according to
the value of bit 3 (DIAx) of parameter No. 1006.
Limitation
- Feedrate
A radius-based feedrate is specified in both of diameter specification
and radius specification at all times.
8.COORDINATE VALUE AND DIMENSION PROGRAMMING B-63944EN/03
- 222 -
- Data not switchable
The following data follows the setting of parameter DIAx, so that
diameter and radius switching is not performed:
• Parameter
• Offset
• Workpiece coordinate system
• Scale display on the graphic screen
NOTE
For offset data, the settings of bit 1 (ORC) of
parameter No. 5004 and bit 2 (ODI) of parameter
No. 5004 have priority.
- Switchable data and commands
For the following data and commands, diameter and radius switching
is performed according to the specified specification method:
• Programmed move command
• Current position display
• Workpiece coordinate system preset
• Movement based on the manual numeric command G00 or G01
- Use with other functions
Diameter/radius specification switching cannot be performed for an
axis on which a movement is being made with any of the functions
indicated below.
Moreover, none of the functions indicated below can be performed
during diameter and radius switching.
• Synchronous/composite control
• Superimposed Control
• Axis synchronous control
• PMC axis control
B-63944EN/03 PROGRAMMING
- 223 -
9.SPINDLE SPEED FUNCTION
(S FUNCTION)
9 SPINDLE SPEED FUNCTION
(S FUNCTION)
The spindle speed can be controlled by specifying a value following
address S.
Chapter 9, "SPINDLE SPEED FUNCTION (S FUNCTION)",
consists of the following sections:
9.1 SPECIFYING THE SPINDLE SPEED WITH A CODE .........224
9.2 SPECIFYING THE SPINDLE SPEED VALUE DIRECTLY
(S5-DIGIT COMMAND) .........................................................224
9.3 CONSTANT SURFACE SPEED CONTROL (G96, G97) ......225
9.4 SPINDLE POSITIONING FUNCTION...................................230
9.5 SPINDLE SPEED FLUCTUATION DETECTION.................236
9.6 SPINDLE CONTROL WITH SERVO MOTOR......................241
PROGRAMMING B-63944EN/03
- 224 -
9. SPINDLE SPEED FUNCTION
(S FUNCTION)
9.1 SPECIFYING THE SPINDLE SPEED WITH A CODE
When a value is specified after address S, the code signal and strobe
signal are sent to the machine to control the spindle rotation speed.
A block can contain only one S code. Refer to the appropriate manual
provided by the machine tool builder for details such as the number of
digits in an S code or the execution order when a move command and
an S code command are in the same block.
9.2 SPECIFYING THE SPINDLE SPEED VALUE DIRECTLY
(S5-DIGIT COMMAND)
The spindle speed can be specified directly by address S followed by a
max. five-digit value (min-1). The unit for specifying the spindle speed
may vary depending on the machine tool builder. Refer to the
appropriate manual provided by the machine tool builder for details.
B-63944EN/03 PROGRAMMING
- 225 -
9.SPINDLE SPEED FUNCTION
(S FUNCTION)
9.3 CONSTANT SURFACE SPEED CONTROL (G96, G97)
Specify the surface speed (relative speed between the tool and
workpiece) following S. The spindle is rotated so that the surface
speed is constant regardless of the position of the tool.
Format
- Constant surface speed control command
G96Sxxxxx ;
↑ Surface speed (m/min or feet/min)
This surface speed unit may change according to machine
tool builder's specification.
- Constant surface speed control cancel command
G97Sxxxxx ;
↑ Spindle speed (min-1)
This surface speed unit may change according to machine
tool builder's specification.
- Constant surface speed controlled axis command
G96Pα ;
P0 : Axis set in the parameter (No. 3770)
P1 : X axis, P2 : Y axis, P3 : Z axis, P4 : 4th axis
P5 : 5th axis, P6 : 6th axis, P7 : 7th axis, P8 : 8th axis
NOTE
If multi-spindle control (spindle selecting based on
address P or spindle name expansion) is enabled,
axis specification based on address P is disabled.
Use parameter No. 3770 for axis specification.
- Clamp of maximum spindle speed
G92 S_ ;
The maximum spindle speed (min-1) follows S.
T
G50 S_ ;
The maximum spindle speed (min-1) follows S.
NOTE
G50 can be used with G code system A.
PROGRAMMING B-63944EN/03
- 226 -
9. SPINDLE SPEED FUNCTION
(S FUNCTION)
Explanation
- Constant surface speed control command (G96)
G96 (constant surface speed control command) is a modal G code.
After a G96 command is specified, the program enters the constant
surface speed control mode (G96 mode) and specified S values are
assumed as a surface speed. A G96 command must specify the axis
along which constant surface speed control is applied. A G97
command cancels the G96 mode. When constant surface speed
control is applied, a spindle speed higher than the value specified in
G92S_; or G50S_; (maximum spindle speed) is clamped at the
maximum spindle speed. When the power is turned on, the maximum
spindle speed is not yet set and the speed is not clamped. S (surface
speed) commands in the G96 mode are assumed as S = 0 (the surface
speed is 0) until M03 (rotating the spindle in the positive direction) or
M04 (rotating the spindle in the negative direction) appears in the
program.
The spindle speed (min-1) almost coincides
with the surface speed (m/min) at approx.
160 mm (radius).
Spindle speed (min-1)
Relation between workpiece radius,
s
p
indle s
p
eed and surface s
p
eed Radius (mm)
Surface speed S is 600 m/min.
Fig. 9.3 (a) Relation between workpiece radius, spindle speed and
surface speed
B-63944EN/03 PROGRAMMING
- 227 -
9.SPINDLE SPEED FUNCTION
(S FUNCTION)
- Setting the workpiece coordinate system for constant surface speed control
To execute the constant surface speed control, it is necessary to set the
workpiece coordinate system , and so the coordinate value at the
center of the rotary axis, for example, Z axis, (axis to which the
constant surface speed control applies) becomes zero.
X
Z
0
Fig. 9.3 (b) Example of the workpiece coordinate system for constant
surface speed control
- Surface speed specified in the G96 mode
G96 mode G97 mode
Specify the surface speed in m/min
(or feet/min)
G97 command
Store the surface speed in m/min
(or feet/min)
Command for
the spindle
speed
Specified
The specified
spindle speed
(min-1) is used
Not specified
The surface speed (m/min or
feet/min) is converted to the
spindle speed (min-1)
Commands other than G96
G96 command
The specified
surface
speed is used
Command
for the surface
speed
The stored surface speed (m/min or
feet/min) is used. If no surface
is stored, 0 is assumed.
Specified
Not specified
PROGRAMMING B-63944EN/03
- 228 -
9. SPINDLE SPEED FUNCTION
(S FUNCTION)
Limitation
- Constant surface speed control for threading
The constant surface speed control is also effective during threading.
Accordingly, it is recommended that the constant surface speed
control be invalidated with G97 command before starting the scroll
threading and taper threading, because the response problem in the
servo system may not be considered when the spindle speed changes.
- Constant surface speed control for rapid traverse (G00)
In a rapid traverse block specified by G00, the constant surface speed
control is not made by calculating the surface speed to a transient
change of the tool position, but is made by calculating the surface
speed based on the position at the end point of the rapid traverse block,
on the condition that cutting is not executed at rapid traverse.
B-63944EN/03 PROGRAMMING
- 229 -
9.SPINDLE SPEED FUNCTION
(S FUNCTION)
Example
T
300 400 500 600 700 800 900 1000 1100
1200
1300 14001500
1050
1475
200
375
500
300
400
700
X
Z
1
2
3
4
N16
N16
N15
N15
N14
N14 N11
N11
100
675
600
Programmed path
Tool path after offset
Radius value
φ600
φ
400
N8 G00 X1000.0Z1400.0 ;
N9 T33;
N11 X400.0Z1050.0;
N12 G50S3000 ; (Designation of max. spindle speed)
N13 G96S200 ; (Surface speed 200 m/min)
N14 G01 Z 700.0F1000 ;
N15 X600.0Z 400.0;
N16 Z_ ;
The CNC calculates the spindle speed which is proportional to the
specified surface speed at the position of the programmed coordinate
value on the X axis. This is not the value calculated according to the X
axis coordinate after offset when offset is valid. At the end point N15
in the example above, the speed at 600 dia. (Which is not the turret
center but the tool nose) is 200 m/min. If X axis coordinate value is
negative, the CNC uses the absolute value.
PROGRAMMING B-63944EN/03
- 230 -
9. SPINDLE SPEED FUNCTION
(S FUNCTION)
9.4 SPINDLE POSITIONING FUNCTION
Overview
In turning, the spindle connected to the spindle motor is rotated at a
certain speed to rotate the workpiece mounted on the spindle. This
spindle control status is referred to as spindle rotation mode.
The spindle positioning function turns the spindle connected to the
spindle motor by a certain angle to position the workpiece mounted on
the spindle at a certain angle. This spindle control status is referred
to as spindle positioning mode.
The spindle positioning function involves the following three
operations:
1. Canceling the spindle rotation mode and entering the spindle
positioning mode
Place the spindle in the spindle positioning mode and establish a
reference position by specifying a given M code (set with a
parameter). (Spindle orientation)
2. Positioning the spindle in the spindle positioning mode
The spindle is positioned in either of the two methods:
1) Positioning with an arbitrary angle by an axis address
2) Positioning with a semi-fixed angle by a given M code (set
with a parameter)
3. Canceling the spindle positioning mode, and entering the spindle
rotation mode
Place the spindle in the spindle rotation mode by specifying a
given M code (set with a parameter).
The least command increment, least input increment, and maximum
value for the spindle positioning axis are as follows:
• Least command increment
• Least input increment
0.001 deg (IS-B)
• Maximum value
±999999.999 deg
360
4096 = 0.088 deg (when the gear ratio of the spindle to the position coder
•
•
B-63944EN/03 PROGRAMMING
- 231 -
9.SPINDLE SPEED FUNCTION
(S FUNCTION)
9.4.1 Spindle Orientation
When spindle positioning is first performed after the spindle motor is
used for normal spindle operation, or when spindle positioning is
interrupted, the spindle orientation is required.
Orientation permits the spindle to stop at a predetermined position.
Orientation is directed by the M code set in parameter No. 4960. The
direction of orientation can be set with a parameter.
For the serial spindle, it is set in bit 4 (RETSV) of parameter No. 4000.
With the grid shift function, the orientation position can be shifted in a
range of 0 to 360 deg with parameter No. 4073 for a serial spindle.
- Feedrate during spindle orientation
An orientation feedrate for a serial spindle is determined by a spindle
parameter setting.
In orientation, the serial spindle stops at the orientation position after
several rotations of the spindle motor.
- Omission of orientation
By using bit 2 (ISZ) of parameter No. 4950, orientation upon
switching to spindle positioning mode can be omitted if it is
unnecessary (for example, when no start position is specified and
incremental positioning from the current position is only required).
More specifically, when an M code for switching to spindle
positioning mode is specified, the spindle control mode is simply
switched to spindle positioning mode and then the processing is
completed without orientation.
- Program reference position
The position at which orientation is completed is assumed to be a
program reference position. However, the program reference
position can be changed through coordinate system setting (G92 or
G50) or automatic coordinate system setting (bit 0 (ZPR) of parameter
No. 1201).
When a setting is made to omit orientation, a program reference
position is not established, and operation by an absolute command is
unpredictable during spindle positioning with an axis address.
PROGRAMMING B-63944EN/03
- 232 -
9. SPINDLE SPEED FUNCTION
(S FUNCTION)
9.4.2 Spindle Positioning
The spindle can be positioned with a semi-fixed angle or arbitrary
angle.
- Positioning with a semi-fixed angle
Use an M code to specify a positioning angle. The specifiable M
code value may be one of the six values from Mα to M (α+5). Value
α must be set in parameter No. 4962 beforehand. The positioning
angles corresponding to Mα to M (α+5) are listed below. Value β
must be set in parameter No. 4963 beforehand.
M-code
(Ex.) β = α + 5 Positioning angle (Ex.) β = 30°
Mα β 30°
M (α + 1) 2β 60°
M (α + 2) 3β 90°
M (α + 3) 4β 120°
M (α + 4) 5β 150°
M (α + 5) 6β 180°
When the number of M codes to be used, value γ, is specified in
parameter No. 4964, a specifiable M code value may be in a range of
values from Mα to M (α + (γ - 1)), up to 255 values from Mα to M (α
+ (255 - 1)).
M code
(Ex.) γ = 11 Positioning angle (Ex.) β = 30°
Mα β 30°
M (α + 1) 2β 60°
M (α + 2) 3β 90°
M (α + 3) 4β 120°
... ... ...
M (α + 11 - 1) 11β 330°
The direction of rotation can be specified in IDM (bit 1 of parameter
4950).
- Positioning with an arbitrary angle
Specify the position with an arbitrary angle using the axis address
followed by a signed numeric value or numeric values. The axis
address must be specified in the G00 mode.
(The explanation below is given assuming that a C axis address is set.)
(Example) C-45000
C180.000
A numeric with the decimal point can be entered. The value must be
specified in degrees.
(Example) C36.0=C36 degrees
B-63944EN/03 PROGRAMMING
- 233 -
9.SPINDLE SPEED FUNCTION
(S FUNCTION)
- Absolute commands and incremental commands
Incremental commands are always used for positioning with a
semi-fixed angle (using M codes).
The direction of rotation can be specified with bit 1 (IDM) of
parameter No. 4950.
Absolute and incremental commands can be used for positioning with
an arbitrary angle.
With absolute commands for positioning with an arbitrary angle, when
the rotation axis rollover function is used (bit 0 (ROA) of parameter
No. 1008 is 1), shortcut control is also enabled (bit 1 (RAB) of
parameter No. 1008 is 0).
Program reference position
A
B
180°
90°
G-code system A in
lathe system
G-code system B or C in
lathe system, and
machining center system
Command format
Address
used
Command
A-B in the
above
figure
Address
used and G
code
Command
A-B in the
above
figure
Absolute
command
Specify the end
point with a
distance from the
program reference
position.
C C180.0 ; G90, C G90 C180 .;
Incremental
command
Specify a
distance from
the start point to
the end point.
H H90.0 ; G91, C G91 C90 .;
- Feedrate during positioning
The feedrate during positioning equals the rapid traverse speed
specified in parameter No. 1420.
For the specified speed, an override of 100%, 50%, 25%, and F0
(parameter No. 1421) can be applied.
PROGRAMMING B-63944EN/03
- 234 -
9. SPINDLE SPEED FUNCTION
(S FUNCTION)
9.4.3 Canceling Spindle Positioning
When modes are to be switched from spindle positioning to normal
spindle rotation, the M code set in parameter No. 4961 must be
specified.
Also, the spindle positioning mode is canceled and the spindle rotation
mode is set in the following cases:
<1> A reset operation (including an emergency stop) occurs when a
servo alarm is issued.
<2> A reset operation (including an emergency stop) occurs when a
spindle alarm is issued.
<3> An orientation operation in progress is stopped due to a reset or
alarm, or for some other reason.
<4> A reset operation (including an emergency stop) occurs when bit
(IOR) 0 of parameter No. 4950 is 1.
CAUTION
1 During execution of spindle positioning sequences
(canceling the spindle rotation mode and entering
the spindle positioning mode, positioning the spindle
in the spindle positioning mode, and canceling the
spindle positioning mode and entering the spindle
rotation mode), the automatic operation stop signal
*SP is invalid. This means that automatic operation
does not stop until all the sequences are completed,
even when the *SP signal becomes 0.
2 Dry run and machine lock cannot be performed
during spindle positioning.
3 Auxiliary function lock is disabled for M codes for the
spindle positioning function.
4 The serial spindle Cs-axis contour control function
and the spindle positioning function cannot be used
at a time. If both options are specified, the spindle
positioning function has priority.
5 The spindle positioning axis is handled as a
controlled axis. Therefore, controlled axis-related
signals (such as the overtravel signal) must be set.
6 When using the rigid tapping function and the
spindle positioning function concurrently, do not
specify rigid tapping in spindle positioning mode or
spindle positioning in rigid tapping mode.
B-63944EN/03 PROGRAMMING
- 235 -
9.SPINDLE SPEED FUNCTION
(S FUNCTION)
NOTE
1 M code commands for positioning of a spindle must
be specified in a single block. Other commands must
not be contained in the same block. (Also, M code
commands for positioning of another spindle must
not be contained in the same block.)
Even when the single-block, multiple-M code
command function is also used, related M codes
must be specified in a single block.
2 Even when the single-block, multiple-M code
command function is also used, related M codes
must be specified in a single block.
3 Axis address commands for positioning of a spindle
must be specified in a single block. Other commands
must not be contained in the same block. However,
the following commands can be contained in the
same block where axis address commands are
specified:
G00, G90, G91, G92 (G-code systems B and C in
the T series, M series)
G00, G50 (G-code system A in the T series)
4 M code commands for spindle positioning specify M
codes that are not buffered.
5 Spindle positioning cannot be performed by manual
operation (in jog feed, manual handle feed, manual
numeric command, or other mode).
6 Spindle positioning cannot be performed by PMC
axis control.
7 For spindle positioning, program restart and block
restart operations cannot be performed. Use the
MDI for these operations.
8 The stored stroke limit check is disabled for the
spindle positioning axis.
9 The axis removal function is disabled for the spindle
positioning axis.
10 The pitch error compensation function is disabled for
the spindle positioning axis.
11 When a setting is made to omit spindle orientation,
the reference position return completion signal does
not become 1.
12 In spindle orientation, all-axis interlock and
axis-specific interlock are checked only when a block
is started. A signal is ignored if input during the
execution of the block.
13 A difference between a specified travel distance and
an actual travel distance is maintained until spindle
positioning mode is canceled.
PROGRAMMING B-63944EN/03
- 236 -
9. SPINDLE SPEED FUNCTION
(S FUNCTION)
9.5 SPINDLE SPEED FLUCTUATION DETECTION
Overview
With this function, an overheat alarm (OH0704) is raised and the
spindle speed fluctuation detection alarm signal SPAL is issued when
the spindle speed deviates from the specified speed due to machine
conditions.
This function is useful, for example, for preventing the seizure of the
guide bushing.
G26 enables spindle speed fluctuation detection.
G25 disables spindle speed fluctuation detection.
Format
- Spindle fluctuation detection on
G26 Pp Qq Rr Ii；
P: Time (in ms) from the issue of a new spindle rotation
command (S command) to the start of checking whether
the actual spindle speed is so fast that an overheat can
occur.
When a specified speed is reached within the time period
of P, a check is started at that time.
Q: Tolerance (%) of a specified spindle speed
100
1 ×
−
=speedspndlespecified
speedspindleactual
q
If a specified spindle speed lies within this range, it is
regarded as having reached the specified value. Then,
the checking of an actual spindle speed is started.
R: Spindle speed fluctuation (%) at which the actual spindle
speed is so fast that an overheat can occur
100
1 ×
−
=speedspndlespeciofied
overheatcausecanthatspeed
r
If the fluctuation of the actual spindle speed to the
specified spindle speed exceeds the spindle speed
fluctuation of R, the actual spindle speed is regarded as
being so fast that an overheat can occur.
I: Spindle speed fluctuation width at which the actual
spindle speed (min-1) is so fast that an overheat can
occur
If the fluctuation (width) between the specified and
actual spindle speeds exceeds the spindle speed
fluctuation width of I, the actual spindle speed is
regarded as being so fast that an overheat can occur.
B-63944EN/03 PROGRAMMING
- 237 -
9.SPINDLE SPEED FUNCTION
(S FUNCTION)
G26 enables the spindle speed fluctuation detection function. The
values specified for P, Q, R, and I are set in the following parameters:
No. 4914, No. 4911, No. 4912, and No. 4913, respectively. Each
command address corresponds to a parameter number as listed below.
Command address Parameter number
Q No.4911
R No.4912
I No.4913
P No.4914
If the P, Q, R, or I command address is omitted, the function detects
the fluctuation of the actual spindle speed according to the value set in
the corresponding parameter (No. 4914, No. 4911, No. 4912, or No.
4913).
The parameters (No. 4914, No. 4911, No. 4912, and No. 4913) for the
spindle on which the currently selected position coder is mounted are
used for the setting and spindle speed fluctuation detection check.
- Spindle fluctuation detection off
G25;
G25 disables the spindle speed fluctuation detection function.
When G25 is specified, the parameters (No. 4914, No. 4911, No. 4912,
and No. 4913) are unchanged. When the power is turned on or after
a reset (clear state (bit 6 (CLR) of parameter No. 3402 = 1)) is
executed, the spindle speed fluctuation detection function is disabled
(G25). For the clear state, also check the setting of bit 3 (C19) of
parameter No. 3408 for the M series or bit 0 (C08) of parameter No.
3407 for the T series.
Explanation
The function for detecting spindle speed fluctuation checks whether
the actual speed varies for the specified speed or not. Si or Sr,
whichever is greater, is taken as the allowable fluctuation speed (Sm).
An alarm (OH0704) is activated when the actual spindle speed varies
for the commanded speed (Sc) under the condition that the variation
width exceeds the allowable variation width (Sm).
|Sc – Sa| > Sm
Sc : Specified spindle speed
Sa : Actual spindle speed
Si : The allowable constant variation width which is
independent of the specified spindle speed (parameter
(No.4913))
Sr : The allowable variation width which is obtained by
multiplying Sc (commanded spindle speed) by r (constant
ratio). (r = parameter (No.4912))
Parameter FLR(No.4900#0)= 0 Parameter FLR(No.4900#0)= 1
100
r
ScSr ×= 1000
r
ScSr ×=
Sm: Si or Sr, whichever is greater
PROGRAMMING B-63944EN/03
- 238 -
9. SPINDLE SPEED FUNCTION
(S FUNCTION)
- Conditions to start spindle speed fluctuation detection
If the specified spindle speed Sc changes, spindle speed fluctuation
detection starts when one of the conditions below is met:
<1> The actual spindle speed falls in a range of (Sc - Sq) to (Sc + Sq)
Sc : Specified spindle speed
Sq : Tolerance within which the spindle is assumed to attain the
programmed speed
(parameter (No.4911))
Parameter FLR= 0 Parameter FLR= 1
100
q
ScSq ×= 1000
q
ScSq ×=
<2> When time p specified in parameter No. 4914 elapses after the
specified speed Sc changes.
- Examples of spindle speed fluctuation detection
(Example 1)
When an alarm (OH0704) is issued after a specified spindle
speed is reached
Spindle
speed
Specified
speed
A
ctual
speed
Time
A
larm
Start of check
Specification of
another speed
CHECK
NO CHECK
CHECK
Sq
Sq
Si
Si
S
r
S
r
G26 mode
P
B-63944EN/03 PROGRAMMING
- 239 -
9.SPINDLE SPEED FUNCTION
(S FUNCTION)
(Example 2)
When an alarm OH0704 is issued before a specified spindle
speed is reached
Spindle
speed
Specified
speed
A
ctual
speed
Time
A
larm
Start of
check
Specification o
f
another speed
CHECK
NO CHECK
CHECK
Sq
Sq
Si
Si
S
r
S
r
P
G26 mode
Specified speed :
(Speed specified by address S and five-digit value) × (spindle
override)
Actual speed : Speed detected with a position coder
p : Period after a change occurs in the actual spindle speed until
detection starts
Parameter No.4914, address P
Sq : (Specified spindle speed) × (Detection start tolerance (q))
Parameter No.4911, address Q
Parameter FLR = 0 Parameter FLR = 1
100
q 1000
q
Sr : (Specified spindle speed) × (Allowable variation (r))
Parameter No.4912, address R
Parameter FLR = 0 Parameter FLR = 1
100
r 1000
r
Si : Allowable variation width
Parameter No.4913, address I
If the difference between the specified speed and actual speed exceeds
both Sr and Si, an alarm OH0704 is raised.
- Relationship between spindle speed control and each spindle
Serial spindle Spindle
Function 1st spindle 2nd spindle 3rd spindle 4th spindle
Spindle speed
fluctuation detection Possible Possible(*1) Possible(*1) Possible(*1)
PROGRAMMING B-63944EN/03
- 240 -
9. SPINDLE SPEED FUNCTION
(S FUNCTION)
NOTE
1 An optional function of multi spindle control is
necessary.
2 The spindle speed fluctuation detection function is
effective for a single spindle. The function cannot be
executed for two or more spindles.
The spindle speed fluctuation detection function is
effective for a spindle on which the currently selected
position coder is mounted. Just a single position
coder can be selected. Multiple position coders
cannot be selected. For the selection of a position
coder, see the section of "Multi spindle."
* Position coder selection signals
(PC2SLC<Gn028.7>, PC3SLC<Gn026.0>,
PC4SLC<Gn026.1>)
3 The parameters that become valid are the parameters
of the spindle speed fluctuation detection function
(No.4911, No.4912, No.4913, No.4914) for the
spindle on which the currently selected position coder
is mounted.
- Spindle for which to detect the spindle speed fluctuation
For the spindle for which to detect the spindle speed fluctuation, refer
to the appropriate manual provided by the machine tool builder.
B-63944EN/03 PROGRAMMING
- 241 -
9.SPINDLE SPEED FUNCTION
(S FUNCTION)
9.6 SPINDLE CONTROL WITH SERVO MOTOR
9.6.1 Spindle Control with Servo Motor
- Command with a program
This function provides SV speed control mode in which spindle
rotation commands, S commands, are effective to a rotation axis with
a servo motor and position control mode in which normal positioning
can be performed. To place a servo motor under speed control, you
must turn SV speed control mode ON (G96.4). Once SV speed
control mode is turned ON,
S commands are effective to the servo motor until it is canceled.
You cannot specify positioning commands while SV speed control
mode is ON. To perform positioning, you must cancel SV speed
control mode.
To cancel SV speed control mode (turn position control mode ON),
you must specify a spindle indexing command, G96.1/G96.2.
In position control mode, S commands are invalid as in the normal
servo axis state. Note, however, S command information is stored;
when SV speed control mode is ON, rotation starts at the already
specified speed.
- Command with a signal
You can also turn SV speed control mode ON/OFF with the SV speed
control mode signal (Gn521). When you turn SV speed control
mode ON with the signal, and if you turn SV speed control mode OFF
with a program command, you must specify the SV speed control
mode signal or specify G96.4 to turn SV speed control mode ON
again. You can check the state of SV speed control mode with the
SV speed control mode in-progress signal (Fn521). When you turn
SV speed control mode signal OFF while rotating, spindle indexing is
executed. Then SV speed control mode is turned off. Spindle
indexing is executed with R0(absolute position 0).
Format
G96.4 P_ ; SV speed control mode ON
M03 (M04) S_ P_ ; Rotation command
S: Spindle speed [min-1] (numeric value of up to five digits)
P: Spindle selection with multi-spindle control
Using G96.4 and a spindle selection command P can turn the SV
speed control mode ON for each axis separately. Likewise, using a
spindle indexing command (G96.1/G96.2) and a spindle selection
command P can cancel the SV speed control mode, that is, turn on the
position control mode ON, for each axis separately.
To specify “G96.4 P_ ;”, use an independent block.
However, it is possible to specify "G96.4 P_ S_ ;".
PROGRAMMING B-63944EN/03
- 242 -
9. SPINDLE SPEED FUNCTION
(S FUNCTION)
9.6.2 Spindle Indexing Function
Format
G96.1 P_ R_ ; After spindle indexing is completed, the
operation of the next block is started.
G96.2 P_ R_ ; Before spindle indexing is completed,
the operation of the next block is
started.
G96.3 P_ ; After it is confirmed that spindle
indexing is completed, the operation of
the next block is started.
P: Spindle selection with multi-spindle control
R: Stoppage angle [deg] (0 to (parameter No. 1260))
To specify address P, use parameter No. 3781 (P code for selecting a
spindle in multi-spindle control).
To turn the position control mode ON without performing spindle
indexing, do so after canceling the SV speed control mode by issuing
a G96.1 command with no R specified when the motor is at a halt.
When the motor is rotating, issuing a G96.1 (or G96.2) command with
no R specified results in the motor coming to a halt by behaving in the
same manner as for R0.
NOTE
1 When using G96.2, issue G96.3 before another
spindle move command, to make sure that the
spindle is at a complete halt.
2 To issue G96.1, G96.2, or G96.3, use an
independent block.
Spindle indexing command
- Move command
(1) Command waiting for spindle indexing to be completed
If G96.1 is issued, the next block is executed after spindle
indexing is completed.
(2) Command not waiting for spindle indexing to be completed
If G96.2 is issued, the next block can be executed before spindle
indexing is completed.
- Movement completion check command
G96.3 is used to check to see if spindle indexing is completed. If it
has not been completed, the next block waits for spindle indexing to
be completed. If it is completed, the next block is executed.
B-63944EN/03 PROGRAMMING
- 243 -
9.SPINDLE SPEED FUNCTION
(S FUNCTION)
- SV speed control mode cancellation
If G96.1 is used to perform spindle indexing, the SV speed control
mode is canceled when spindle indexing is completed.
If G96.2 is used to perform spindle indexing, G96.3 can be used to
check to see if spindle indexing is completed and, if completed, cancel
the SV speed control mode. Issuing G96.2 not followed by G96.3
cannot cancel the SV speed control mode even if spindle indexing is
completed.
Start SV speed control mode cancellation at a path to which the axis of
interest belongs.
- Spindle indexing command during spindle rotation
Issuing G96.1 or G96.2 with a position specified during spindle
rotation causes the spindle to stop at the specified position.
Example)
M03 S1000 ; ............. Rotation at S1000
G96.1 P1 R180. ; ...... Stoppage of rotation at the 180deg position
- Spindle indexing speed
Issuing G96.1 or G96.2 causes a move speed to be dedicated to
spindle indexing. Specify the move speed for spindle indexing,
using parameter No. 11012.
Spindle indexing command (absolute coordinate/machine coordinate)
Using bit 0 (SIC) of parameter No. 11005 can select which coordinate
system, absolute or machine, is to be used in spindle indexing.
Example:
If the difference between the machine and absolute coordinates
(machine coordinate – absolute coordinate) is 100.000:
• Spindle indexing performed by turning the SV speed
control mode signal (Gn521) OFF (1 to 0) or issuing a
spindle indexing G code (with no R specified)
1. If bit 0 (SIC) of parameter No. 11005 = 0:
Spindle indexing is performed with a machine coordinate
of 100.000 and an absolute coordinate of 0.000.
2. If bit 0 (SIC) of parameter No. 11005 = 1:
Spindle indexing is performed with a machine coordinate
of 0.000 and an absolute coordinate of 260.000.
• G code-based spindle indexing (with R specified)
Assuming that spindle indexing is specified with R100.000:
1. If bit 0 (SIC) of parameter No. 11005 = 0:
Spindle indexing is performed with a machine coordinate
of 200.000 and an absolute coordinate of 100.000.
2. If bit 0 (SIC) of parameter No. 11005 = 1:
Spindle indexing is performed with a machine coordinate
of 100.000 and an absolute coordinate of 0.000.
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 244 -
10 TOOL FUNCTION (T FUNCTION)
Chapter 10, "TOOL FUNCTION (T FUNCTION)", consists of the
following sections:
10.1 TOOL SELECTION FUNCTION..........................................245
10.2 TOOL MANAGEMENT FUNCTION...................................247
10.3 TOOL MANAGEMENT EXTENSION FUNCTION ...........265
10.4 TOOL MANAGEMENT FUNCTION FOR OVERSIZE
TOOLS ...................................................................................277
10.5 TOOL LIFE MANAGEMENT ..............................................279
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 245 -
10.1 TOOL SELECTION FUNCTION
By specifying an up to 8-digit numerical value following address T, a
code signal and a strobe signal are transmitted to the machine tool.
This is used to select tools on the machine.
One T code can be commanded in a block. Refer to the machine tool
builder's manual for the number of digits commendable with address T
and the correspondence between the T codes and machine operations.
When a move command and a T code are specified in the same block,
the commands are executed in one of the following two ways:
(i) Simultaneous execution of the move command and T function
commands.
(ii) Executing T function commands upon completion of move
command execution.
The selection of either (i) or (ii) depends on the machine tool builder's
specifications. Refer to the manual issued by the machine tool
builder for details.
Explanations
T
The value after the T code indicates the desired tool. Part of the
value is also used as a tool offset number that specifies the amount of
tool offset or the like. The tool can be selected as follows according
to the specification method and parameter settings.
Description of a T code (Note 1)
LGN (No.5002#1) = 0 LGN (No.5002#1) = 1
How to specify the offset number for each
parameter setting (Note 2)
The tool wear offset number is specified using
the low-order one digit of a T code.
T{{{{{{{ {
↑ ↑
Tool selection Tool geometry
tool wear
offset
T{{{{{{{ {
↑ ↑
Tool selection Tool wear
tool geometry offset
offset
When parameter (No.5028) is set to 1
The tool wear offset number is specified using
the low-order two digits of a T code.
T{{{{{{ {{
↑ ↑
Tool selection Tool geometry
tool wear
offset
T{{{{{{ {{
↑ ↑
Tool selection Tool wear
tool geometry offset
offset
When parameter (No.5028) is set to 2
The tool wear offset number is specified using
the low-order three digits of a T code.
T{{{{{ {{{
↑ ↑
Tool selection Tool geometry
tool wear
offset
T{{{{{ {{{
↑ ↑
Tool selection Tool wear
tool geometry offset
offset
When parameter (No.5028) is set to 3
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 246 -
NOTE
1 The maximum number of digits of a T code can be
specified by parameter (No.3032) as 1 to 8.
2 When parameter (No.5028) is set to 0, the number
of digits used to specify the offset number in a T
code depends on the number of tool offsets.
Example)
When the number of tool offsets is 1 to 9:
Low-order one digit
When the number of tool offsets is 10 to 99:
Low-order two digits
When the number of tool offsets is 100 to 999:
Low-order three digits
Refer to the machine tool builder's manual for correspondence
between the T-code and the tool and the number of digit to specify
tool selection.
Example (T2+2)
N1G00X1000Z1400;
N2T0313; (Select tool No. 3 and tool offset value No. 13)
N3X400Z1050;
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 247 -
10.2 TOOL MANAGEMENT FUNCTION
Overview
The tool management function totally manages tool information
including information about tool offset and tool life.
Explanation
A tool type number is specified with a T code. The tool type number
is any number the user can define freely. With tool type numbers,
tools can be grouped by various conditions such as life, compensation
value, and cutting conditions. When each type is assumed to have a
single tool, tool type numbers are equivalent to unique tool numbers.
For each tool, an information storage area is prepared in the CNC
(SRAM). This area contains information such as a tool type number,
tool life, tool status (such as a breakage condition), tool compensation
number (H, D, G, or W), spindle speed (S), cutting feedrate (F), and
freely-definable customize data. Such data is called tool
management data.
A cartridge management table that links cartridge information and tool
management data is provided so that the CNC can manage the
cartridges of the machine and tool change operations. In addition,
areas for managing the tools in the spindle and tool standby positions
are prepared.
When a tool type number is specified using a T code command, a tool
that has the tool type number and the shortest life is searched for, and
the cartridge number and pot number of the location where the tool is
stored are output to the PMC. Then, a tool change operation using
the cartridge number and pot number is enabled by the PMC ladder
sequence.
Tool information in the CNC is managed by the tool management data
and cartridge management table (including the spindle management
table and standby position table).
- Tool management data
As tool management data, information about each tool is registered
with a tool management data number.
The following number of sets of tool management data can be used:
Tool management function 64 sets 64 sets in total
Tool management function 240 sets 240 sets in total
Tool management function 1000 sets 1000 sets in total
NOTE
For the number of tool management data sets,
refer to the relevant manual issued by the machine
tool builder.
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 248 -
- Details of data
The following details the tool management data registered for each
data number:
• Tool type number (T code)
Item Description
Data length 4byte
Valid data range 0,1 to 99,999,999
• Tool life counter
Item Description
Data length 4byte
Unit of data When the number of use times is specified: Times
When time is specified: Seconds
Valid data range When the number of use times is specified: 0 to
99,999,999 times
When time is specified: 0 to 3,599,999 s (999 hours
59 minutes 59 seconds)
The value of an increment counter, that is, the number of use times
(time) is indicated. The remaining life value is [the maximum tool
life value minus tool life counter value].
• Maximum tool life value
Item Description
Data length 4byte
Unit of data When the number of use times is specified: Times
When time is specified: Seconds
Valid data range When the number of use times is specified: 0 to
99,999,999 times
When time is specified: 0 to 3,599,999 s (999 hours
59 minutes 59 seconds)
• Notice life value
Item Description
Data length 4byte
Unit of data When the number of use times is specified: Times
When time is specified: Seconds
Valid data range When the number of use times is specified: 0 to
99,999,999 times
When time is specified: 0 to 3,599,999 s (999 hours
59 minutes 59 seconds)
If a value other than 0 is set, the tool life expiration notice signal
TLCHB <F064.3> or TLCHBx <F329.4 to 7> is output when the
remaining life value of the tool (= maximum tool life value minus tool
life counter value) has reached the set value.
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 249 -
• Tool life status
Item Description
Data length 1byte
Detail data 0: Life management is not performed.
1: Tool not yet used
2: Life remains.
3: Life expired.
4: Tool breakage (skip)
The machine (PMC) determines tool breakage and stores
corresponding information through the window. In tool management
of the CNC, a broken tool is regarded as being equivalent to tools
whose lives have expired.
• Tool information
Item Description
Data length 1 byte (flag data)
#0 RGS
0: Tool management data is invalid. (-)
1: Tool management data is valid. (R)
#1 TIM
0: Type for counting the number of use times (C)
1: Type for counting time (T)
#2 BDT 0: Normal tool (N)
1: Oversize tool (B)
#3 LOC 0: Data accessible (U)
1: Data not accessible (L)
#4 SEN When the tool life status indicates that tool
management is not performed:
0: This tool is not searched. (-).
1: This tool is searched. (S)
#5 to #7 Reserved
When RGS is set to 0 in tool management data, the tool management
data is regarded as not being registered even when values are set for
other items.
NOTE
Make sure you specify the same life count type for
all tools of the same type. You can check tools of
the same type for any difference in life count type,
using the "check function."
M
• Tool length compensation number (H)
Item Description
Data length 2byte
Valid data range 0 to 999
• Cutter compensation number (D)
Item Description
Data length 2byte
Valid data range 0 to 999
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 250 -
T
• Tool geometry compensation number (G)
Item Description
Data length 2byte
Valid data range 0 to 999
• Tool wear compensation number (W)
Item Description
Data length 2byte
Valid data range 0 to 999
NOTE
When the machine control type is the combined
system type, tool length compensation and cutter
compensation numbers are used for paths for the
machining center system, and for paths for the
lathe system, tool geometry compensation and tool
wear compensation numbers are used.
• Spindle speed (S)
Item Description
Data length 4byte
Unit of data min-1
Valid data range 1 to 99,999
• Feedrate (F)
Item Description
Data length 4byte
Unit of data mm/min, inch/min, deg/min, mm/rev, inch/rev
Valid data range 0 to 99,999,999
As additional tool management data, areas for setting customize data
(5 data items including customize data 0 and customize data 1 to 4)
are provided without defining specific usage. The user can use these
customize data areas freely to set a warning life value, cutting
resistance, override value, spindle current value, maximum and
minimum S/F, and other items according to the targeted application.
• Customize data 0
Item Description
Data length 1 byte (bit type)
Valid data range 0 or 1 on a bit-by-bit basis
• Customize data 1 to 4 (to 20) (to 40)
Item Description
Data length 4byte
Valid data range -99,999,999 to 99,999,999
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 251 -
NOTE
For the maximum number of tool management
function customization data items, refer to the
relevant manual issued by the machine tool builder.
- Cartridge management table
The storage status of tools in cartridges is managed with the cartridge
management table.
• Multiple cartridge numbers can be defined. (Numbers from 1 to
4, up to four cartridges)
• The maximum number of pots for all cartridges is 64, 240, or
1000, which depends on whether a tool management data option
is selected.
• Cartridge numbers and pot numbers can be assigned freely
within cartridge management data by parameter setting
(described later).
• The tool management data number adjacent to a pot number is
linked with tool data defined in the tool management table.
Therefore, the tool attached to the pot is indicated.
• Zero set as a data number indicates that no tool is attached.
• The cartridge management table can be read from and written to
through the PMC window and FOCAS2.
• The spindle management table and standby position table are
provided to indicate special cartridge positions.
• Spindle positions and standby positions, regarded as special
cartridge positions, have fixed cartridge numbers 11 to 14 (the
positions of the first to fourth spindles) and 21 to 24 (the first to
fourth standby positions).
• With the PMC window, the spindle position table and standby
position table can be read from and written to.
• Tool life counting is performed only for the tools at the spindle
positions.
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 252 -
- Multi-path system
The tool management data and cartridge management table are
common data among the paths. The spindle management table and
standby position table, however, are treated as independent data for
each path.
When the spindle table or standby position table is specified as a
cartridge from the PMC window, specify the following, in which the
path number is set in the hundred’s place:
Spindle position
First Second Third Fourth
First path 111(11) 112(12) 113(13) 114(14)
Second path 211 212 213 214
Third path 311 312 313 314
Fourth path 411 412 413 414
Fifth path 511 512 513 514
Sixth path 611 612 613 614
Seventh path 711 712 713 714
Eighth path 811 812 813 814
Ninth path 911 912 913 914
Tenth path 1011 1012 1013 1014
Standby position
First Second Third Fourth
First path 121(21) 122(22) 123(23) 124(24)
Second path 221 222 223 224
Third path 321 322 323 324
Fourth path 421 422 423 424
Fifth path 521 522 523 524
Sixth path 621 622 623 624
Seventh path 721 722 723 724
Eighth path 821 822 823 824
Ninth path 921 922 923 924
Tenth path 1021 1022 1023 1024
NOTE
When specifying 111, 121, and so on to specify the
first path, you may specify just 11, 21, and so on.
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 253 -
Tool management data
- Data of each tool such as type number, life status, and compensation number
- The number of sets of data is 64, 240, or 1000.
Cartridge management table
- This table indicates the cartridge and pot to which each set of tool management
data is assigned.
- Up to four cartridges are used.
Path 1 Path 10
Path 2
Standby position table
121 to 124 (21 to 24)
Spindle position table
111 to 114 (11 to 14)
Standby position table
221 to 224
Spindle position table
211 to 214
Standby position table
1021 to 1024
Spindle position table
1011 to 1014
. . . . . . . . . . .
- M/T series
The tool management data and cartridge management table are data
common to the M and T series.
- Tool life management and tool change
The CNC performs tool life management, regarding tools having the
same tool type number as a group. When a tool type number (T
code) is specified by an NC program, the tool management data
registered in the CNC is searched to find a tool having the shortest life
among the tools with the same tool type number.
The cartridge number and pot number corresponding to the searched
tool are output as a T code signal to the PMC. Based on the output
cartridge number and pot number, the PMC performs preparation for a
tool change (to the next tool). A different tool can also be selected
on the PMC side.
The CNC performs tool life counting for each tool that is at a spindle
position in the spindle management table.
When the lives of all tools having the tool type number specified by
the T code have expired, alarm PS5317 is issued. If there is a tool in
the spindle position or standby position, that tool is selected to
continue machining.
As the T code signal, a specified tool type number instead of the
cartridge number and pot number can also be output directly by
parameter setting.
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 254 -
There are two types of tool life management counting methods:
counting the number of use times and counting cutting time. One of
the counting methods is set in tool information of tool management
data.
Other major specifications related to tool life management are as
follows:
Tool type number (T code): Up to 8 digits (1 to 99,999,999)
Maximum tool life value:
99,999,999 times when the number of use times is specified
999 hours 59 minutes 59 seconds when time is specified
Life count interval when time is specified: 1 second
Tool life management count restart M code: Enabled
Tool life count override: Enabled
To specify a certain tool directly without performing tool life
management by tool type number, use the following format:
M (value in parameter No. 13252) T (cartridge number) (pot
number) ;
When parameter No. 13252 is set to 333, the cartridge number is 2,
and the pot number is 27, for example, the following command is
specified:
M333 T20027;
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 255 -
- Tool search order
Tools having a tool type number (T) specified by a program are
searched sequentially from tool management data number 1 while
registered data contents are checked. The following shows how a
search operation is made within the NC:
Is tool management data valid (is bit 0 (RGS) of tool information set to 1)?
Is tool being edited?
Does tool type number (T) match with specified number?
Is tool registered in cartridge (is cartridge number non-zero value)?
Is cartridge targeted for search (are bits 0 to 3 of parameter No. 13203 set to 0)?
Is tool registered at spindle position or standby position of another path?
Does tool life status indicate that tool management is not performed (0)?
Is tool excluded from management target a search target (is bit 4 (SEN) of tool information 1)?
Search end
Does tool life status indicate that life expired (3)?
Does tool life status indicate tool breakage (4)?
Regard tool with smallest remaining life or customize data value as candidate.
Bit 6 (SWC) of parameter No. 13203 (0: Check remaining life, 1: Check customize data)
Check of next tool?
Search end
Yes
No
No
Yes
Yes
No
Yes
No
Yes
No
No
Yes
Yes
No
No
Yes
No
No
Yes
Yes
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 256 -
- System variables
The following tool management data of the tool being used as a
spindle after a tool change by M06 and the tool to be used next which
is specified by a T code can be read through custom macro variables:
Being
used Item
#8401 Tool management data number
#8402 Tool type number (T)
#8403 Tool life counter
#8404 Maximum tool life value
#8405 Tool notice life value
#8406 Tool life status
#8407 Customize data 0 (bit)
#8408 Tool information
#8409 Tool length compensation number (H)
#8410 Cutter compensation number (D)
#8411 Spindle speed (S)
#8412 Cutting feedrate (F)
#8413 Tool geometry compensation number (G)
#8414 Tool wear compensation number (W)
#8431 Customize data 1
#8432 Customize data 2
#8433 Customize data 3
#8434 Customize data 4
#8435 Customize data 5
#8436 Customize data 6
#8437 Customize data 7
#8438 Customize data 8
#8439 Customize data 9
#8440 Customize data 10
#8441 Customize data 11
#8442 Customize data 12
#8443 Customize data 13
#8444 Customize data 14
#8445 Customize data 15
#8446 Customize data 16
#8447 Customize data 17
#8448 Customize data 18
#8449 Customize data 19
#8450 Customize data 20
#8451 Customize data 21
#8452 Customize data 22
#8453 Customize data 23
#8454 Customize data 24
#8455 Customize data 25
#8456 Customize data 26
#8457 Customize data 27
#8458 Customize data 28
#8459 Customize data 29
#8460 Customize data 30
#8461 Customize data 31
#8462 Customize data 32
#8463 Customize data 33
For machining
center systems
For lathe systems
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 257 -
Being
used Item
#8464 Customize data 34
#8465 Customize data 35
#8466 Customize data 36
#8467 Customize data 37
#8468 Customize data 38
#8469 Customize data 39
#8470 Customize data 40
When a cartridge number of a spindle position (11 to 14) or standby
position (21 to 24) is specified in #8400, information about the
corresponding position can be read.
If the spindle position table or standby position table has an empty pot,
<empty> is read from #8402 to #8470.
Value 0 is read from #8401 (data number).
Therefore, machining conditions registered in tool management data
can be specified directly by coding, for example, D#8410, H#8409,
S#8411, and F#8412 with a tool change macro (such as M06).
Similarly, customize data can be referenced by a custom macro, and
machining programs can be customized according to the tool used.
NOTE
For the maximum number of tool management
function customization data items, refer to the
relevant manual issued by the machine tool builder.
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 258 -
- Specifying a tool compensation number
M
When parameter No. 13265 is 0, a compensation number registered as
tool management data of a tool attached at a spindle position can be
selected by specifying H99 or D99.
(99 is treated as a special number, so 99 cannot be specified directly as
a compensation number.)
When other than 0 is set in parameter No. 13265, the number set in the
parameter can be specified instead of 99. For example, if parameter
No. 13265 is 3, specifying H3 specifies the tool length compensation
number registered for the tool at the spindle position.
T
When the tool management function is not used, a tool compensation
number is specified also with a T code; when the tool management
function is used, the T code is used only to specify a tool type number,
so a tool compensation number must be specified with address D.
Except the specifications for addresses, the specifications for the
number of permissible digits (parameter No. 3032) and the number of
digits consisting of a compensation number (parameter No. 5028),
separation of geometry compensation numbers and wear
compensation numbers (bit 1 (LGN) of parameter No. 5002), and so
on are the same as for T.
If parameter No. 13265 is set to 0, when a compensation number
registered for a tool attached at a spindle position is specified, the
specification format varies according to the number of digits as
follows, which is the same as for conventional T:
When the compensation number is 1 digit long: D9
When the compensation number is 2 digits long: D99
When the compensation number is 3 digits long: D999
Because 9, 99, or 999 is treated as a special number, it cannot be
specified directly as a compensation number.
Unless parameter No. 13265 is set to 0, the number set in the
parameter can be specified instead of 9, 99, or 999. When parameter
No. 13265 is set to 3, specifying D3 specifies the tool geometry
compensation number and tool wear compensation number registered
for a tool attached at the spindle position.
Multi-path system
Depending on whether the local path is a machining center system or a
lathe system, tool compensation numbers are specified by using one of
the above methods.
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 259 -
Spindle selection
When specifying compensation numbers of a tool attached to a spindle
other than the first spindle, specify the spindle number with address P
within the same block that contains H/D. When specifying the first
spindle, you can omit P.
D99 P3; Specifying compensation numbers registered for the tool
attached at the third spindle
D99 ; Specifying compensation numbers registered for the tool
attached at the first spindle
- Read/write operations for tool management data and cartridge management table
The tool management data and cartridge management table can be
read from and written to by using the CNC/PMC data window library
(FOCAS2). Therefore, a specific tool management system including
all available tool data not registered in the CNC can be built easily by
using the OPEN CNC.
Similarly, the tool management data and cartridge management table
can also be read from and written to using the PMC window.
Tool management data of the tool being used as a spindle after a tool
change operation performed by M06 and the tool being selected by
specifying a T code can be read using a custom macro.
The user can modify tool management data by MDI from the tool
management function screen of the CNC. Addition, modification,
and deletion of the above tool management data can be made from a
part program (G10). Such data can also be input to and output from
external I/O equipment by using the ALL I/O screen and tool
management function screen.
- G10 format
Addition, modification, and deletion are performed for the tool
management data and cartridge management table from programs.
For use of this function, the programmable data input option function
is required.
If a format error is found in the commands from G10 L75/L76/L77 to
G11, or if a value beyond the valid data range is specified, alarm
PS5312 is issued. In such a case, correct the program. Within the
range from G10 to G11, no decimal point can be specified with any
address. If a decimal point is specified, alarm PS0007 results.
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 260 -
- Registering new tool management data
Tool management data can be registered. When data is punched out
to an external device from the tool management data screen, this
format is used. The specification of those items that are not
registered may be omitted.
G10 L75 P1;
N_ ; Tool management data number specification
T_ C_ L_ I_ B_ Q_ H_ D_ S_ F_ J_ K_ ;
P0 R_ ; Customization data 0
P1 R_ ; Customization data 1
P2 R_ ; Customization data 2
P3 R_ ; Customization data 3
P4 R_ ; Customization data 4
N_ ; Tool management data number
:
G11;
N_ Tool management data No. 1 to 64 (1 to 240, 1 to 1000)
T_ Tool type No. (T) 0 to 99,999,999
C_ Tool life counter 0 to 99,999,999
L_ Maximum tool life 0 to 99,999,999
I_ Noticed life 0 to 99,999,999
B_ Tool life state 0 to 4
Q_ Tool information Bit format (8 bits)
H_ Tool length compensation No. (H) 0 to 999 (M series)
D_ Cutter compensation No. (D) 0 to 999 (M series)
S_ Spindle speed (S) 0 to 99,999
F_ Cutting feedrate (F) 0 to 99,999,999
J_ Tool geometry compensation No. (G) 0 to 999 (T series)
K_ Tool geometry compensation No. (W) 0 to 999 (T series)
P_ Customization data No. 0 to 4 (0 to 20, 0 to 40)
R_ Customization data value -99,999,999 to 99,999,999
Specify customization data in the following format:
P (customization-number) R (value)
Use the bit format only when specifying the customization data 0 (P0).
Specify other data in the binary format. The specification of
customization data that need not be set may be omitted.
Example)
G10 L75 P1;
N1 ; Tool management data No.1
T10000001 C0 L1000 B1 Q00000001 H1 D1 S4000 F10000 ;
P0 R11101101 ; Customization data 0
P4 R99999999 ; Customization data 4
N2 ; Tool management data No.2
:
G11 ;
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 261 -
Modifying tool management data
Tool management data can be modified.
The specification of those items that are not modified may be omitted.
G10 L75 P2 ;
N_ ;
T_ C_ L_ I_ B_ Q_ H_ D_ S_ F_ J_ K_ ;
P_ R_ ;
N_ ;
:
G11 ;
Deleting tool management data
The data of a specified data number can be deleted from tool
management data.
The cartridge management table data corresponding to a deleted tool
management data number is also deleted. (The tool management
data number in the cartridge management table is cleared to 0.)
G10 L75 P3 ;
N_ ;
N_ ;
:
N_ ;
G11 ;
Registering new cartridge management table data
A tool management data number can be registered with a free pot in
the cartridge management table.
G10 L76 P1 ;
N cartridge-number P pot-number R tool-management-data-number ;
N cartridge-number P pot-number R tool-management-data-number ;
N cartridge-number P pot-number R tool-management-data-number ;
N cartridge-number P pot-number R tool-management-data-number ;
G11 ;
For a spindle position table and standby position table, only cartridge
number data is specified.
Example)
G10 L76 P2 ;
N11 R1; Changes the tool management data number of the spindle
position to No. 1.
N21 R29; Changes the tool management data number of the standby
position to No. 29.
G11 ;
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 262 -
Modifying the cartridge management table
Tool management data numbers in the cartridge management table can
be modified.
G10 L76 P2 ;
N cartridge-number P pot-number R tool-management-data-number ;
N cartridge-number P pot-number R tool-management-data-number ;
N cartridge-number P pot-number R tool-management-data-number ;
N cartridge-number P pot-number R tool-management-data-number ;
G11 ;
For a spindle position table and standby position table, only cartridge
number data is specified.
Example)
G10 L76 P2 ;
N11 R1; Changes the tool management data number of the spindle
position to No. 1.
N21 R29; Changes the tool management data number of the standby
position to No. 29.
G11 ;
Deleting cartridge management table data
Tool management data numbers can be deleted from the cartridge
management table.
G10 L76 P3 ;
N cartridge-number P pot-number R tool-management-data-number ;
N cartridge-number P pot-number R tool-management-data-number ;
N cartridge-number P pot-number R tool-management-data-number ;
N cartridge-number P pot-number R tool-management-data-number ;
G11 ;
For a spindle position table and standby position table, only cartridge
number data is specified.
Example)
G10 L76 P3 ;
N11 ; Deletes the tool management data number of the spindle
position (clears the number to 0).
N21 ; Deletes the tool management data number of the standby
position (clears the number to 0).
G11 ;
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 263 -
Naming customization data
The display name of customization data (0 to 40) can be set.
G10 L77 P1 ;
N_ ;
P_ R_ ;
P_ R_ ;
;
N_ ;
P_ R_ ;
P_ R_ ;
G11 ;
N_: Customization data No. (0 to 40)
P_: Character No. (1 to 16)
R_: Character code (ANK or shifted JIS)
- When a shifted JIS code is used, an area for
two characters is used.
- Specify 0 to clear data.
• A set display name can be checked on the tool management data
screen only.
• When no name is registered, a name such as the default
"Customize 3" is displayed.
• A name consisting of up to 16 characters is displayed. For a
name shorter than 16 characters, register 0 in the empty area.
Those characters that are registered immediately before 0 are
displayed.
• To clear data, set 0 as a character code.
• No character code data check is made.
When the name of customization data 3 is set as "MEASURE5", for
example, specify the following:
Example)
G10 L77 P1 ;
N3 ; Specifies customization data 3.
P1 R32 ; character ‘space’ ASCII code 20h
P2 R77 ; character “M” ASCII code 4Dh
P3 R69 ; character “E” ASCII code 45h
P4 R65 ; character “A” ASCII code 41h
P5 R83 ; character “S” ASCII code 53h
P6 R85 ; character “U” ASCII code 55h
P7 R82 ; character “R” ASCII code 54h
P8 R69 ; character “E” ASCII code 45h
P9 R53 ; character “5” ASCII code 35h
P10 R0 ; Clears data. (Not displayed. End)
G11 ;
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 264 -
Naming tool life states
The display name of a tool life state (0 to 4) can be set.
G10 L77 P2 ;
N_ ;
P_ R_ ;
P_ R_ ;
N_ ;
P_ R_ ;
P_ R_ ;
G11 ;
N_: Tool life state (0 to 4)
P_: Character No. (1 to 12)
R_: Character code (ANK or shifted JIS)
- When a shifted JIS code is used, an area for
two characters is used.
- Specify 0 to clear data.
• A set display name can be checked on the tool management data
screen only.
• If no name is registered, a default such as "Remaining" and
"Unremaining" is displayed.
• A name consisting of up to 12 characters is displayed. For a
name shorter than 12 characters, register 0 in the empty area.
Those characters that are registered immediately before 0 are
displayed.
• To clear data, set 0 as a character code.
• No character code data check is made.
• The defaults are as follows:
- 0: Invalid
- 1: Remaining
- 2: Remaining
- 3: Unremaining
- 4: Broken
To set "NORMAL" as the name of tool life state 2 (Remaining),
specify the following:
Example)
G10 L77 P2 ;
N2 ; Specifies tool life state 2.
P1 R78 ; character “N” ASCII code 4Eh
P2 R79 ; character “O” ASCII code 4Fh
P3 R82 ; character “R” ASCII code 52h
P4 R77 ; character “M” ASCII code 4Dh
P5 R65 ; character “A” ASCII code 41h
P6 R76 ; character “L” ASCII code 4Ch
P7 R0 ; Clears data. (Not displayed. End)
G11 ;
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 265 -
10.3 TOOL MANAGEMENT EXTENSION FUNCTION
Overview
The following functions have been added to the tool management
function:
1. Customization of tool management data display
2. Setting of spindle position/standby position display
3. Input of customize data with the decimal point
4. Protection of various tool information items with the KEY signal
5. Selection of a tool life count period
6. Each tool data screen
7. Total life time display for tools of the same type
They will be explained in detail below.
10.3.1 Customization of Tool Management Data Display
With the tool management data screen display customization function,
the display positions of screen elements (type number, tool
information, life counter, and so forth) on the tool management screen
can be changed and whether to display or hide such screen elements
can be chosen using the G10 format. This function enables a
customized tool management screen to be configured.
Format
G10L77P3;
N_ R_;
G11;
N_: Tool management data screen display position number
R_: Tool management data display item
Explanation
- number (N_)
• A display position number represents an ordinal number from the
leftmost position on the tool management data screen.
• As N, a number from 1 to 200 can be specified.
- Tool management data display item (R_)
• For a value to be set (in R_), see the table below.
• For actual setting, consider a display width plus 1.
Items common to machining center systems and lathe systems
R Item Display width Remarks
-1 End of setting -
0 Blank column 10
1 No. 4 For spindle/standby
positions for 10 paths
2 TYPE-NO. 8
3 MG 4
4 POT 5
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 266 -
R Item Display width Remarks
5 T-INFORMATION 10
6 L-COUNT 10
7 MAX-LIFE 10
8 NOTICE-L 10
9 L-STATE 6 or 12
The display width is
switched by bit 1 of
parameter No. 13201.
10 S (Spindle speed) 10
11 F (Feedrate) 10
12 Tool figure number (A) 3
Offset-related items for machining center systems
R Item Display width Remarks
20 H (Tool length
compensation number)
4
21 D (Cutter compensation
number)
4
22 OFFSET－M 10 Tool offset memory A
23 GEOMETRY－M 10
24 WEAR－M 10
Tool offset memory B
25 GEOMETRY（H） 10
26 WEAR（H） 10
27 GEOMETRY（D） 10
28 WEAR（D） 10
Tool offset memory C
Offset-related items for lathe systems
R Item Display width Remarks
40 TG (Tool geometry
compensation number)
4
41 TW (Tool wear
compensation number)
4
42 OFFSET－X 10
43 OFFSET－Z 10
44 OFFSET－R 10
45 TIP 10
Tool nose radius
compensation
46 OFFSET－Y 10 Y-axis offset
47 OFFSET－B 10 B-axis control
48 GEOMETRY (X) 10
49 WEAR (X) 10
50 GEOMETRY (Z) 10
51 WEAR (Z) 10
Tool geometry/wear
compensation
52 GEOMETRY (R) 10
53 GEOMETRY TIP 10
54 WEAR (R) 10
55 WEAR TIP 10
Tool nose radius
compensation, Tool
geometry/wear
compensation
56 GEOMETRY (Y) 10
57 WEAR (Y) 10
Y-axis offset, Tool geometry/
wear compensation
58 GEOMETRY (B) 10
59 WEAR (B) 10
B-axis control, Tool
geometry/ wear
compensation
60 GEOMETRY (X2) 10
61 GEOMETRY (Z2) 10
62 GEOMETRY (Y2) 10
2nd geometry tool offset
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 267 -
Items related to customize data
R Item Display width Remarks
80 CUSTOM 0 10
81 CUSTOM 1 10
82 CUSTOM 2 10
83 CUSTOM 3 10
84 CUSTOM 4 10
85 CUSTOM 5 10
86 CUSTOM 6 10
87 CUSTOM 7 10
88 CUSTOM 8 10
89 CUSTOM 9 10
90 CUSTOM 10 10
91 CUSTOM 11 10
92 CUSTOM 12 10
93 CUSTOM 13 10
94 CUSTOM 14 10
95 CUSTOM 15 10
96 CUSTOM 16 10
97 CUSTOM 17 10
98 CUSTOM 18 10
99 CUSTOM 19 10
100 CUSTOM 20 10
Tool management function
customize data extension
(5 to 20) or tool
management function
customize data extension
(5 to 40)
101 CUSTOM 21 10
102 CUSTOM 22 10
103 CUSTOM 23 10
104 CUSTOM 24 10
105 CUSTOM 25 10
106 CUSTOM 26 10
107 CUSTOM 27 10
108 CUSTOM 28 10
109 CUSTOM 29 10
110 CUSTOM 30 10
111 CUSTOM 31 10
112 CUSTOM 32 10
113 CUSTOM 33 10
114 CUSTOM 34 10
115 CUSTOM 35 10
116 CUSTOM 36 10
117 CUSTOM 37 10
118 CUSTOM 38 10
119 CUSTOM 39 10
120 CUSTOM 40 10
Tool management function
customize data extension
(5 to 40)
NOTE
1 If G10 L77 P3 is terminated normally, the power
must be turned off before operation is continued.
2 The setting becomes effective after the power is
turned off then back on.
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 268 -
Example
Example of setting tool offset memory A
G10L77P3; Set tool management data screen display
customization
N1 R1; Set No. as number 1
N2 R2; Set TYPE-NO. as number 2
N3 R3; Set MG as number 3
N4 R4; Set POT as number 4
N5 R5; Set T-INFORMATION as number 5
N6 R6; Set L-COUNT as number 6
N7 R7; Set MAX-LIFE as number 7
N8 R8; Set NOTICE-L as number 8
N9 R9; Set L-STATE as number 9
N10 R11; Set F (Feedrate) as number 10
N11 R21; Set D as number 11
N12 R22; Set OFFSET-M as number 12
N13 R80; Set CUSTOM 0 as number 13
N14 R81; Set CUSTOM 1 as number 14
N15 R-1; End
G11; Cancel the setting mode
On the tool management data screen, the first page displays "No.,
Type Number, MG, Pot, Tool Information, Life Counter, Maximum
Life, Noticed Life, and Life State".
The second page displays "F (Feedrate), D (Cutter Compensation
Number), Tool Offset-M, Customize Data 0, and Customize Data 1".
Example 1: Page 1
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 269 -
Example 1: Page 2
NOTE
1 This setting is enabled when bit 0 (TDC) of
parameter No. 13201 is set to 1.
2 Up to 20 pages can be set.
3 Be sure to specify an end.
4 If an item that requires the corresponding option is
specified without specifying the option, the item is
displayed as a blank field.
5 No items after an end are displayed.
(Example) In the case of N1 → R1 (No.), N2 → R2
(Type Number), N 3 → R3 (MG), N4 →
R-1 (End), N5 → R4 (Pot), only the items
"No., Type Number, and MG" are
displayed on the screen.
6 If G10 L77 P3 is specified, the setting immediately
before is initialized.
7 If an invalid value is set in R (tool management data
display item), a blank field is displayed.
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 270 -
10.3.2 Setting of Spindle Position / Standby Position Display
In MG on the tool management data screen, a spindle position or
standby position is displayed as a number such as 11, 12, and 13.
With the spindle position/standby position display setting function,
three arbitrary characters can be displayed using the G10 format.
Format
G10L77P4;
N_;
P_R_;
G11;
N_: Spindle position/standby position setting
P_: Character number
R_: Character code
Explanation
- Spindle position/standby position setting (N_)
Specify a spindle position or standby position to be renamed. The
table below indicates the values to be specified.
Spindle position
First Second Third Fourth
1st path 111 112 113 114
2nd path 211 212 213 214
3rd path 311 312 313 314
4th path 411 412 413 414
5th path 511 512 513 514
6th path 611 612 613 614
7th path 711 712 713 714
8th path 811 812 813 814
9th path 911 912 913 914
10th path 1011 1012 1013 1014
Standby position
First Second Third Fourth
1st path 121 122 123 124
2nd path 221 222 223 224
3rd path 321 322 323 324
4th path 421 422 423 424
5th path 521 522 523 524
6th path 621 622 623 624
7th path 721 722 723 724
8th path 821 822 823 824
9th path 921 922 923 924
10th path 1021 1022 1023 1024
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 271 -
- Character number (P_)
Specify a character number (1 to 3). Up to three characters are
displayed. If a character string to be specified is shorter than three
characters, specify 0 in the leading blank character position(s). A
character string immediately before 0 is displayed.
- Character code (R_)
Set the name of a spindle position/standby position by using a
character code (ASCII code or Shift JIS code).
- For a character code, use ASCII code or Shift JIS code.
- No character code data check is made.
Example
When spindle 1 is named "SP1", and standby 1 is named "WT1"
G10L77P4; Set spindle position/standby position
N111; Specify spindle 1
P1 R83; 53h as ASCII code for "S"
P2 R80; 50h as ASCII code for "P"
P3 R49; 31h as ASCII code for "1"
N121; Specify standby 1
P1 R87; 57h as ASCII code for "W"
P2 R84; 54h as ASCII code for "T"
P3 R49; 31h as ASCII code for "1"
G11; Cancel the setting mode
In the MG item on the tool management data screen, spindle 1 is
displayed as "SP1", and standby 1 is displayed as "WT1".
NOTE
Data registered becomes effective after the screen
display is switched to the tool management screen.
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 272 -
10.3.3 Input of Customize Data with the Decimal Point
With the function for input of customize data with the decimal point,
the number of decimal places can be set using the G10 format for each
customize data item (customize data 1, ..., 40) to enable data input
with the decimal point.
Format
G10L77P5;
N_R_;
G11;
N_: Customize data number
R_: Decimal point position
Explanation
- Customize data number (N_)
- A value of 1 to 4 can be specified for N.
- When tool management function customize data extension (5 to
20) is available, a value of 1 to 20 can be specified.
- When tool management function customize data extension (5 to
40) is available, a value of 1 to 40 can be specified.
- Decimal point position (R_)
Specify a decimal point position (0 to 7). When 0 is set, the number
of decimal places of customize data cannot be input.
NOTE
1 If G10 L77 P5 is terminated normally, the power
must be turned off before operation is continued.
2 The setting becomes effective after the power is
turned off then back on.
3 When the number of decimal places is set for
customize data, the number of decimal places can
be input only through the MDI keys.
4 To set the number of decimal places for customize
data 5 to 20, the customize data extension (5 to 20)
option for the tool management function or the
customize data extension (5 to 40) option for the
tool management function is required.
5 To set the number of decimal places for customize
data 21 to 40, the customize data extension (5 to
40) option for the tool management function is
required.
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 273 -
Example 1
When customize data 1 and customize data 2 are input with three
decimal places
G10L77P5; Set the number of decimal places for
customize data
N1 R3; Set the number of decimal places to 3 for
customize data 1
N2 R3; Set the number of decimal places to 3 for
customize data 2
G11; Cancel the setting mode
- Use in the G10 format
Between G10 and G11, the decimal point cannot be specified at any
address. So, if decimal point input for customize data is enabled
with this function, a G10 L75/L76/L77 command using a custom
macro variable (#8431 to #8450) reads and sets the value of the
integer part.
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 274 -
Example 2
(Example 1)
Condition:
"3" is set as the decimal point position of customize data 1.
"1" is set as the decimal point position of customize data 2.
Operation:
Data is transferred from customize data 1 to customize data
2 by using a custom macro variable.
G10L77P5; <1> Set customize data decimal point position
N1 R3; <2> Set 3 as decimal point position of customize data 1
N2 R1; <3> Set 1 as decimal point position of customize data 2
G11; <4> Cancel the setting mode
;
G10 L75 P1; <5> Register tool management data
N01; <6> Register with No. 1
P1 R12345; <7> Set ”12.345” for customize data 1
P2 R#8431; <8> Set ”1.2” for customize data 2
G11; <9> Cancel the setting mode
In Example 1, customize data 1 is directly set in customize data 2
by using a custom macro variable.
Customize data 1 holds "12.345". In step <8>, only the integer
part is read and processed as "P2 R12".
So, "1.2" is set in customize data 2.
(Example 2)
Condition:
"3" is set as the decimal point position of customize data 1.
"1" is set as the decimal point position of customize data 2.
Operation:
By using the custom macro variable of customize data 1, the
data is transferred to customize data 2 after being multiplied
by 1000.
G10L77P5; <1> Set customize data decimal point position
N1 R3; <2> Set 3 as decimal point position of customize data 1
N2 R1; <3> Set 1 as decimal point position of customize data 2
G11; <4> Cancel the setting mode
;
G10 L75 P1; <5> Register tool management data
N01; <6> Register with No. 1
P1 R12345; <7> Set ”12.345” for customize data 1
P2 R[#8431*1000]; <8> Set ”1234.5” for customize data 2
G11; <9> Cancel the setting mode
In Example 2, customize data 1 is directly set in customize data 2
by using a custom macro variable.
Customize data 1 holds "12.345". In step <8>, the data is
multiplied by 1000 to eliminate the fractional part.
So, this command is equivalent to "P2 R12345", so that "1234.5"
is set in customize data 2.
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 275 -
10.3.4 Protection of Various Tool Information Items with the KEY
Signal
When tool management data is in the edit state, various information
items can be modified. By setting bit 0 of parameter No. 13204 to 1,
tool management data can be protected with the KEY signal so that
various information items are not registered, modified, and deleted.
10.3.5 Selection of a Tool Life Count Period
A tool life count period can be chosen between 1 sec and 8 msec on a
tool-by-tool basis.
- Tool life count period selection
Bit 5 of tool information is used to make a life count period selection.
Item Description
Data length 1 byte (flag data)
#5 REV 0: A life count period of 1 sec is used.
1: A life count period of 8 msec is used.
Range of count is as follows.
1sec: 0 to 3,599,999 seconds (999 hours 59 minutes 59 seconds)
8msec: 0 to 3,599,992 ms (59 minutes 59 seconds 992 milliseconds)
NOTE
This function is valid when the tool information TIM
(#1) is set to 1.
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 276 -
10.3.6 Each tool Data Screen
All data for a specified tool can be extracted and displayed.
10.3.7 Total Life Time Display for Tools of The Same Type
The remaining lives of tools with the same type numbers are totaled,
and totals are displayed in order by tool type number or by remaining
life. Also, data of tools with the same tool type numbers are
displayed in a list.
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 277 -
10.4 TOOL MANAGEMENT FUNCTION FOR OVERSIZE TOOLS
Overview
Tool management function for oversize tools is added to the tool
management function.
The figure of an oversize tool can be defined freely, and the figure of
each oversize tool is registered. When an oversize tool is stored in a
cartridge, interference with tools stored in other pots is considered.
This function is usable with cartridges of chain type and matrix type.
Format
By G10 data input, an oversize tool number can be set in the tool
management data. Moreover, tool figure data can be set.
<Registration of new tool management data>
G10 L75 P1 ;
N_;
A_;
G11 ;
N_: Tool management data number
A_: Specify tool figure number (0 to 20).
<Modification of tool management data>
G10 L75 P2;
N_;
A_;
G11 ;
N_: Tool management data number
A_: Specify tool figure number (0 to 20).
<Registration of tool figure data>
G10 L77 P6 ;
N_P_Q_R_S_T_;
G11 ;
N_: Tool figure number
P_: Number of pots to be occupied in left direction (in steps
of 0.5 pot)
Q_: Number of pots to be occupied in right direction (in
steps of 0.5 pot)
R_: Number of pots to be occupied in upper direction (in
steps of 0.5 pot)
S_: Number of pots to be occupied in lower direction (in
steps of 0.5 pot)
T_: 0 for figure A, or 1 for figure B
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 278 -
NOTE
1 If a target tool is registered in a cartridge and
interferes with other tools in registration or
modification of tool figure data of the tool
management data, alarm PS5360 is issued. (The
data is not input.)
2 If a tool interferes with other tools in registration or
modification to the cartridge management table,
alarm PS5360 is issued. (The data is not input.)
3 If an attempt is made to modify tool figure data,
and the tool for which the tool figure data number
subject to modification is set is registered in the
cartridge, alarm PS5360 is issued. (The data is
not input.)
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 279 -
10.5 TOOL LIFE MANAGEMENT
Tools are classified into several groups, and a tool life (use count or
use duration) is specified for each group in advance. Each time a
tool is used, its life is counted, and when the tool life expires, a new
tool that is sequenced next within the same group is selected
automatically. With this function, the tool life can be managed while
machining is being performed continuously. Data for tool life
management consists of tool group numbers, tool life values, tool
numbers, and codes for specifying a tool offset value. These data
items are registered in the CNC.
Tool group number m
Tool life value l
1 Tool number (T) Code for specifying tool offset
value (H/D)
1st-tool management data
2 : : 2nd-tool management data
:
:
:
:
:
:
:
:
n : : nth-tool management data
Fig. 10.5 (a) Tool selection from machining program
M
A group is selected by a T code, and tool life counting is started by the
M06 command.
T
The T series has two tool change types (the turret type and the ATC
type). The turret type uses only a T code to select a group, specify a
tool offset value, and start tool life counting, whereas the ATC type,
like the M series, uses a T code to select a group and the M06
command to start tool life counting. With the ATC type, only a D
code is used for specifying a tool offset value. The tool change type
is selected by bit 3 (TCT) of parameter No. 5040.
CAUTION
This function cannot be used if bit 1 (LGN) of
parameter No. 5002 is set to 1 to use the same
number as the tool selection number to specify a
geometric offset number.
Machine and CNC operations
Machine CNC
Places a
selected tool
in the wait
state.
Automatically
selects, from tool
group m, a tool
whose life has not
expired.
Attaches the
tool in the
wait state to
the spindle
(tool
change).
Starts counting the
life of the tool
attached to the
spindle.
Tool life
management data
Tool group number 1
:
:
Tool group number m
:
:
Tool group number p
Machining program
:
:
:
Command for selecting
tool group m
:
:
Tool change command
(M06)
:
:
Select
tool.
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 280 -
- Life management B function
If the tool life management B function is enabled, the maximum tool
life value can be extended, and the tool life expiration prior notice
signal can be output to post tool life expiration in advance when the
remaining life (the life value minus the life counter value) has reached
the remaining life setting. The remaining life setting is registered as
tool life management data in the CNC in advance.
The tool life management B function is enabled by setting bit 4 (LFB)
of parameter No. 6805 to 1.
M
If the tool life management B function is enabled, the function for
selecting a tool group by an arbitrary group number can be used.
T
The tool life management B function can be used. However, the
function for selecting a tool group by an arbitrary group number can
be used only if the tool change type is the ATC type (bit 3 (TCT) of
parameter No. 5040 = 1).
- Maximum number of tool life management groups and multipath system
Up to 256 tool life management groups can be used in the entire CNC
system.
For each path, set a maximum number of groups to be used in
parameter No. 6813.
The maximum number of groups must be a multiple of the minimum
number of groups (eight groups). If the maximum number of groups
is 0, the tool life management function is disabled.
The total number of groups in the entire CNC system can be expanded
to 1024 groups by using an option for additional tool life management
groups.
Fig. 10.5 (b) Group allocation in entire system
CAUTION
Re-setting this parameter results in the tool life
management data file being cleared at power-on.
Once the parameter is re-set, register tool life
management data for each path again.
Multipath system (when tool life management is performed for three paths)
Suppose that, of the total groups in the system (256 groups), 128 groups are
allocated to path 1, 64 groups to path 2, and 64 groups to path 3. Then, set
parameter No. 6813 as follows:
Tool life management data file
(256 groups in total in system)
Path 1
Up to 128 groups
Path 2
Up to 64 groups
Path 3
Up to 64 groups
Parameter No. 6813
Path 1
Set 128 in parameter
Path 2
Set 64 in parameter
Path 3
Set 64 in parameter
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 281 -
10.5.1 Tool Life Management Data
Tool life management data consists of tool group numbers, tool
numbers, codes for specifying a tool offset value, tool life values,
arbitrary group numbers, and remaining life settings.
Whether to use arbitrary group numbers and remaining life settings
can be specified by setting bit 5 (TGN) and bit 3 (GRP) of parameter
No. 6802.
Explanation
- Tool group number
Up to 256 tool life management groups can be used in the entire CNC
system.
In parameter No. 6813, set a maximum number of groups to be used.
With the set maximum number of groups, up to four tools can be
registered per group. The combination of the maximum number of
registrable groups and the maximum number of tools can be changed
by setting bit 0 (GS1) and bit 1 (GS2) of parameter No. 6800 as
follows.
Table 10.5.1 Maximum numbers of registrable groups and tools
GS2
(No. 6800#1)
GS1
(No. 6800#0) Number of groups Number of
tools
0 0 1/8 of maximum number of groups
(parameter No. 6813)
32
0 1 1/4 of maximum number of groups
(parameter No. 6813)
16
1 0 1/2 of maximum number of groups
(parameter No. 6813)
8
1 1 Maximum number of groups
(parameter No. 6813)
4
CAUTION
After changing the setting of bit 0 (GS1) and bit 1
(GS2) of parameter No. 6800, re-register tool life
management data by issuing the G10L3
(registration after deletion of data for all groups).
Otherwise, the newly set combination does not
become valid.
NOTE
The total number of groups in the entire CNC system
can be expanded to up to 1024 groups, using an
option for additional tool life management groups.
- Tool number
A tool number is specified with a T code. A number consisting of up
to eight digits (99999999) can be specified.
NOTE
The maximum number of digits usable in the T
code is specified in parameter No. 3032.
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 282 -
- Codes for specifying a tool offset value
M
Codes for specifying a tool offset value include an H code (for tool
length offset) and a D code (for cutter compensation). Numbers up
to 999 (up to three digits long) can be registered as codes for
specifying tool offset values. However, the number of registered
codes must not exceed the number of tool offsets the CNC can use.
NOTE
If codes for specifying tool offset values are not
used, the registration of these codes can be
omitted.
T
If the tool change type is the turret type (bit 3 (TCT) of parameter No.
5040 = 0), neither the H code nor D code is used to specify a tool
offset value. The T code includes a compensation code. If the tool
change type is the ATC type (bit 3 (TCT) of parameter No. 5040 = 1),
only the D code is used.
- Tool life value
A tool life value can be registered in terms of use duration or use
count. The maximum value is as follows:
Up to 4300 minutes can be registered if duration specification is
selected, or up to 65535 times can be registered if use count
specification is selected.
When the tool life management B function is enabled, up to 100000
minutes (or 60000 minutes if the life is counted every 0.1 second) can
be registered if duration specification is selected, or up to 99999999
times can be registered if use count specification is selected.
- Arbitrary group number
M
If a function for allowing specification of arbitrary group numbers is
used (bit 5 (TGN) of parameter No. 6802 = 1), an arbitrary group
number can be specified with a T code to select a tool life
management group.
An arbitrary group number ranging from 1 to 99999999 can be
specified.
T
Arbitrary group numbers can be used only if the tool change type is
the ATC type (bit 3 (TCT) of parameter No. 5040 = 1).
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 283 -
- Remaining life setting
Bit 3 (GRP) of parameter No. 6802 is used to specify which value, a
value set for each group or a parameter-set value (parameters No.
6844 and 6845), is to be used as the remaining life setting until a new
tool is selected.
If a value set for each group is used (bit 3 (GRP) of parameter No.
6802 = 1), the value is registered as tool life management data.
A value ranging from 1 to 100000 minutes (or 60000 minutes if the
life is counted every 0.1 second) can be specified if duration
specification is selected, or a value up to 99999999 times can be
specified if use count specification is selected.
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 284 -
10.5.2 Registering, Changing, and Deleting Tool Life Management
Data
By programming, tool life management data can be registered in the
CNC, and registered tool life management data can be changed or
deleted.
Explanation
The program format varies depending on the following four types of
operation:
- Registration after deletion of all groups
After all registered tool life management data is deleted, programmed
tool life management data is registered.
- Change of tool life management data
Tool life management data can be set for a group for which no tool
life management data is registered, and already registered tool life
management data can be changed.
- Deletion of tool life management data
Tool life management data can be deleted.
- Setting of tool life count type
A count type (use duration or use count) can be set for each group
separately.
Format
- Registration after deletion of all groups
M
Format Meaning
G10L3;
P-L-;
T-H-D-;
T-H-D-;
:
P-L-;
T-H-D-;
T-H-D-;
:
G11;
M02(M30);
G10L3: Register data after deleting data of all groups.
P-: Group number
L-: Tool life value
T-: Tool number
H-: Code for specifying tool offset value (H code)
D-: Code for specifying tool offset value (D code)
G11: End of registration
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 285 -
T
Format Meaning
G10L3;
P-L-;
T-(D-);
T-(D-);
:
P-L-;
T-(D-);
T-(D-);
:
G11;
M02(M30);
G10L3: Register data after deleting data of all groups.
P-: Group number
L-: Tool life value
T-: For turret type (bit 3 (TCT) of parameter No. 5040 =
0), tool number and tool offset number
For ATC type (bit 3 (TCT) of parameter No. 5040 =
1), tool number
G11: End of registration
(D-): For ATC type (bit 3 (TCT) of parameter No. 5040 =
1), code for specifying tool offset value
NOTE
No H code is used even if the tool change type is
the ATC type (bit 3 (TCT) of parameter No. 5040 =
1).
If more than one offset value is to be used for the same tool within one
process, specify the command as shown below (on the assumption that
tool offset numbers are two digits long).
Format Meaning
G10L3;
P-L-;
T0101;
T0102;
T0103;
:
G11;
M02(M30);
Tool number 01, tool offset number 01
Tool number 01, tool offset number 02
Tool number 01, tool offset number 03
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 286 -
- Change of tool life management data
M
Format Meaning
G10L3P1;
P-L-;
T-H-D-;
T-H-D-;
:
P-L-;
T-H-D-;
T-H-D-;
:
G11;
M02(M30);
G10L3P1: Start changing group data.
P-: Group number
L-: Tool life value
T-: Tool number
H-: Code for specifying tool offset value (H code)
D-: Code for specifying tool offset value (D code)
G11: End of change of group
T
Format Meaning
G10L3P1;
P-L-;
T-(D-);
T-(D-);
:
P-L-;
T-(D-);
T-(D-);
:
G11;
M02(M30);
G10L3P1: Start changing group data.
P-: Group number
L-: Tool life value
T-: For turret type (bit 3 (TCT) of parameter No. 5040 =
0), tool number and tool offset number
For ATC type (bit 3 (TCT) of parameter No. 5040 = 1),
tool number
G11: End of registration
(D-): For ATC type (bit 3 (TCT) of parameter No. 5040 =
1), code for specifying tool offset value
NOTE
No H code is used even if the tool change type is
the ATC type (bit 3 (TCT) of parameter No. 5040 =
1).
- Deletion of tool life management data
Format Meaning
G10L3P2;
P-;
P-;
P-;
P-;
:
G11;
M02(M30);
G10L3P2: Start deleting group data.
P-: Group number
G11: End of deletion
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 287 -
- Setting of tool life count type
Format Meaning
G10L3
(or G10L3P1);
P-L-Q-;
T-H-D-;
T-H-D-;
:
G11;
M02(M30);
Q: Life count type
(1: Use count. 2: Duration.)
CAUTION
If the Q command is omitted, the life count type is
set according to the setting of bit 2 (LTM) of
parameter No. 6800.
- Arbitrary group number
M
If the tool life management B function is enabled (bit 4 (LFB) of
parameter No. 6805 = 1), and use of the function for specifying an
arbitrary group number is set (bit 5 (TGN) of parameter No. 6802 = 1),
an arbitrary group number can be registered by programming a
command.
Format Meaning
G10L3;
(or G10L3P1);
P-L-T-;
T-H-D-;
T-H-D-;
:
G11;
M02(M30);
T-: Arbitrary group number (1 to 99999999)
NOTE
1 A group number that is the same as the group
number of another group cannot be registered.
An attempt to register such a group number results
in alarm PS0431.
2 If an arbitrary group number (T) is 0, alarm PS0431
is issued.
3 If ever an arbitrary group number is specified, the T
command must be specified. If the T command is
omitted, alarm PS0149 is issued.
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 288 -
T
The function for specifying an arbitrary group number is available
only if the tool change type is the ATC type (bit 3 (TCT) of parameter
No. 5040 = 1).
If the tool change type is the ATC type, the format used for setting an
arbitrary group number is the same as for the M series.
Remaining life setting
If the tool life management B function is enabled (bit 4 (LFB) of
parameter No. 6805 = 1), and a remaining life value is to be set for
each group separately (bit 3 (GRP) of parameter No. 6802 = 1), a
remaining life value can be set as tool life management data by
programming a command.
Format Meaning
G10L3;
(or G10L3P1);
P-L-R-;
T-H-D-;
T-H-D-;
:
G11;
M02(M30);
R-: Remaining life setting (remaining life until a new tool
is selected)
NOTE
1 If the remaining life setting (R) is 0 or omitted, the
remaining life is assumed to be 0. In this case,
the tool life expiration prior notice function is
disabled.
2 The remaining life setting (R) cannot exceed the
life value (L). If an attempt is made to specify a
value greater than the life value, alarm PS0431 is
issued.
3 The remaining life setting (R) must be an unsigned
value having no decimal point.
4 The unit of the remaining life setting (R) depends
on the setting of bit 1 (FGL) of parameter No. 6805,
which selects the unit of the tool life value.
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 289 -
Tool life value
- If the life management B function is disabled
If the tool life management B function is disabled (bit 4 (LFB) of
parameter No. 6805 = 0), a tool life value is registered as a duration or
a use count according to the setting of bit 2 (LTM) of parameter No.
6800 or the setting of a count type (Q command). The maximum
values are listed below.
Table 10.5.2 (a) Life count types and maximum life values
LFB
(No.6805#4)
LTM
(No.6800#2) Life count type Maximum life value
0 Use count specification 65535 times
0 1 Duration specification 4300 minutes
If the count type is duration specification, the unit of a life value
specified with address L in a program may be one minute or 0.1
second, which is determined by the setting of bit 1 (FGL) of parameter
No. 6805.
Table 10.5.2 (b) Life value unit and maximum value in L command
LFB
(No.6805#4)
FGL
(No.6805#1)
Life value
unit
Maximum
value in L
command
Example
0 1 minute 4300 L100:
Life value is 100 minutes.
0
1 0.1 second 2580000 L1000:
Life value is 100 seconds.
- If the life management B function is enabled
If the tool life management B function is enabled (bit 4 (LFB) of
parameter No. 6805 = 1)
Table 10.5.2 (c) Life count types and maximum life values
LFB
(No.6805#4)
LTM
(No.6800#2) Life count type Maximum life value
0 Use count specification 99999999 times
100000 minutes
1 1 Duration specification 60000 minutes(Note)
Table 10.5.2 (d) Life value unit and maximum value in L command
LFB
(No.6805#4)
FGL
(No.6805#1)
Life value
unit
Maximum value
in L command Example
100000 L100:
0 1 minute
60000(Note) Life value is 100 minutes.
60000000 L1000:
1
1 0.1 second 36000000(Note) Life value is 100 seconds.
NOTE
If the life is counted every 0.1 second (bit 0 (FCO)
of parameter No. 6805 = 1), the maximum value
specified by duration is 60000 minutes.
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 290 -
10.5.3 Tool Life Management Commands in Machining Program
Explanation
M
- Commands
The following commands are used for tool life management:
T○○○○○○○○;
Specifies a tool group number.
The tool life management function selects, from a specified group, a
tool whose life has not expired, and outputs its T code signal.
In {{{{{{{{, specify the sum of the tool life management
ignore number specified in parameter No. 6810 and a desired group
number.
Example: To specify tool group number 1 when the tool life
management ignore number is 100, specify “T101;”.
NOTE
If {{{{{{{{ is not greater than a tool life
management ignore number, the T code is treated
as an ordinary T code.
If an arbitrary group number is used (bit 4 (LFB) of parameter No.
6805 = 1, and bit 5 (TGN) of parameter No. 6802 = 1), it must be a
preset arbitrary group number rather than a tool group number
specified in {{{{{{{{.
Example: To specify tool group number 1 when arbitrary group
number 1234 is set for tool group number 1, specify T1234.
NOTE
1 If an arbitrary group number is used, the tool life
management ignore number specified in parameter
No. 6810 is not used.
2 If the group specified by {{{{{{{{ is not
present, the CNC assumes that a tool not controlled
under the tool life management function is selected.
M06;
Terminates life management for the previously used tools, and begins
counting the life of a new tool selected with the T code.
NOTE
1 M06 is treated as an M code not involving buffering.
2 If more than one M code is to be specified within the
same block, specify M06 first among these M
codes.
H99;
Selects the H code registered in tool life management data for the
currently used tool to enable tool length offset. Parameter No. 13265
can be used to enable compensation according to an H code other than
H99.
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 291 -
H00;
Cancels tool length offset.
D99;
Selects the D code registered in tool life management data for the
currently used tool to perform cutter compensation.
Parameter No. 13266 can be used to enable compensation according to
a D code other than D99.
D00;
Cancels cutter compensation.
NOTE
H99 and D99 must be specified after the M06
command. If a code other than H99 or D99 or a
code other than the H or D code set, respectively, in
parameter No. 13265 or 13266 is specified following
M06, no H code or D code is selected for tool life
management data.
- Types
For tool life management, the four tool change types (types A to D)
listed below are used. Which type to use varies from one machine to
another. For details, refer to the relevant manual of each machine
tool builder.
Table 10.5.3 Differences among tool change types
Tool change type Ａ Ｂ Ｃ Ｄ
M6T M6E M6T M6E M6T M6E M6T M6E
Parameters M6T and
M6E
M6T (No.6800#7)
M6E (No.6801#7)
0 0
1 0 1 0 1
Tool group number
specified in the same
block as the tool change
command (M06)
Tool group already
used Tool group to be used next
Time when tool life is
counted
Life counting is performed for a tool in the specified tool group if M06 is
specified next.
Life counting is
performed if a tool in
the tool group
specified in the
same block as M06
is specified.
Remarks
If the T command (retract tool
group) following the M06
command is not the currently
used tool group, alarm PS0155
is issued (if bit 6 (IGI) of
parameter No. 6800 = 0).
Normally, if a tool group number
command is specified alone, type B is
used. However, even if a tool group
number command is specified alone with
type C, no alarm is issued. (This means
that there is no difference in operation
between types B and C.)
If M06 is specified
alone, alarm PS0153
is raised.
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 292 -
NOTE
If a tool group number is specified and a new tool
is selected, the new tool selection signal is output.
- Tool length compensation in tool axis direction
- Tool center point control
For these functions, a compensation value selected in tool life
management is used for compensation.
T
If the tool change type is the ATC type (bit 3 (TCT) of parameter No.
5040 = 1), commands are specified in the same manner as for the M
series except that neither H99 nor H00 is used for the T series. See
the description for the M series. For details on the tool compensation
types applied when the tool change type is the ATC type, refer to
Section 5.7, “Extended Tool Selection,” in II “Programming,” of the
lathe system user's manual (B-63944EN-1).
The command specification method for the turret type (bit 3 (TCT) of
parameter No. 5040 = 0) is explained below.
CAUTION
This function cannot be used if the same number
as the tool selection number is to be used to
specify geometry offset number (bit 1 (LGN) of
parameter No. 5002 = 1).
- Commands
T{{{{{{99;
The tool life management function ends counting the life of the tool
used so far, selects, from the group specified by {{{{{{, a tool
whose life has not expired, outputs the T code signal for the tool, and
starts counting the life of the tool.
Example:
Suppose that a T199 command (with a tool offset specified with
the lower two digits) is issued to cause the life management
function to select T10001 of tool group 1. Then, T code 100 is
output, and the tool offset number 1 is selected.
If the condition that a new tool be selected is not met, and the second
or subsequent selection of the same group is made since the entry of
the control unit into the automatic operation start state from the reset
state, the next to the currently selected T code is selected if more than
one offset is registered.
If the third selection is made, for example, the third offset is selected
from among multiple offsets registered for the same tool.
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 293 -
Example:
Suppose that the tool offset is specified with the lower two digits,
and that two offset numbers are set for the same tool number in
group 1 with the following two T codes:
T10001 T10002
The first T199 command issued since the entry of the control unit
into the automatic operation start state from the reset state selects
the first T code, T10001. Then, if T199 is issued again before
the control unit is reset, the second T code, T10002, is selected.
Furthermore, if T199 is issued again before the control unit is
reset, the second T code, T10002, is selected because no third
offset is present.
Setting bit 1 (TSM) of parameter No. 6801 set to 1 enables life
counting to be performed for each T code separately even if T
codes specifying multiple offsets for the same number are
registered.
T{{{{{{88;
The offset of the tool whose life is currently counted by tool life
management is canceled. The tool offset code is set to 00, and the
tool number is output as a T code signal.
Example:
Suppose that the tool number of the tool currently used by the
life management function is 100. Then, issuing a T188
command (with a tool offset specified with the lower two digits)
outputs T code 100 and selects offset number 0, canceling the
offset.
NOTE
If life counting is not performed, or if the specified
tool does not belong to the group for which life
counting is being performed, alarm PS0155 is
issued.
The numbers of digits in {{{{{{ and 99/88 vary as follows:
No.5028 99 88
1 T{{{{{{{ 9
↑ ↑
Select group Start life counting
T{{{{{{{ 8
↑ ↑
Select group Cancel tool offset
2 T{{{{{{ 99
↑ ↑
Select group Start life counting
T{{{{{{ 88
↑ ↑
Select group Cancel tool offset
3 T{{{{{ 999
↑ ↑
Select group Start life counting
T{{{{{ 888
↑ ↑
Select group Cancel tool offset
The maximum number of digits in T codes is set in parameter No.
3032.
The number of digits used for specifying an offset number is selected
by parameter No. 5028. If 0 is selected, the number of digits
depends on the number of tool offsets.
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 294 -
Example:
If there are one to nine tool offsets: Lowest digit
If there are 10 to 99 tool offsets: Lower two digits
If there are 100 to 999 tool offsets: Lower three digits
NOTE
Offset start and cancel operations involve
compensation by moving a tool or by shifting the
coordinate system. Using bit 6 (LWM) of
parameter No. 5002 can select whether to perform a
compensation operation if a T code is specified or if
an axis move command is specified.
For details, refer to Subsection 5.1.5, “Offset
Operation,” of the lathe system User's Manual
(B-63944EN-1).
T{{{{{{∆∆;
If the tool offset number in ∆∆ is neither 99 nor 88, the T code is
treated as an ordinary T code. If life counting is being currently
performed, it is ended.
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 295 -
Examples
M
- Tool change type A
If a block specifying a tool change command (M06) also contains a
tool group command (T code), the T code is used as a command for
returning the tool to its cartridge. By specifying a tool group number
with a T code, the number of the tool used so far is output as a T code
signal. If the specified tool number is not a tool number of the tool
group of the tool being used, alarm PS0155 is issued. The alarm,
however, can be suppressed by setting bit 6 (IGI) of parameter No.
6800 to 1.
Example: Suppose that the tool life management ignore number is 100.
T101 ;
:
:
M06 ;
:
:
T102 ;
:
:
M06 T101 ;
:
:
:
T103 ;
:
:
M06 T102 ;
:
:
G43 H99 ;
:
G41 D99 ;
:
D00 ;
:
H00 ;
A tool whose life has not expired is selected from group 1.
(Suppose that tool number 010 is selected.)
Tool life counting is performed for the tool in group 1.
(The life of tool number 010 is counted.)
A tool whose life has not expired is selected from group 2.
(Suppose that tool number 100 is selected.)
Tool life counting is performed for the tool in group 2.
(The life of tool number 100 is counted.)
The number of the tool currently used (in group 1) is output
with a T code signal. (Tool number 010 is output.)
A tool whose life has not expired is selected from group 3.
(Suppose that tool number 200 is selected.)
Tool life counting is performed for the tool in group 3.
(The life of tool number 200 is counted.)
Tool length offset for the tool selected from group 3 is used.
Cutter compensation for the tool selected from group 3 is
used.
Cutter compensation is canceled.
Tool length offset is canceled.
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 296 -
- Tool change types B and C
If a block specifying a tool change command (M06) also contains a
tool group command (T code), the T code is used to specify a tool
group number for which life counting is to be performed by the next
tool change command.
Example: Suppose that the tool life management ignore number is 100.
T101 ;
:
:
M06 T102 ;
:
:
:
M06 T103 ;
:
:
:
G43 H99 ;
:
:
G41 D99 ;
:
:
D00 ;
:
:
H00 ;
:
:
M06 T104 ;
:
A tool whose life has not expired is selected from group 1.
(Suppose that tool number 010 is selected.)
Tool life counting is performed for the tool in group 1.
(The life of tool number 010 is counted.)
A tool whose life has not expired is selected from group 2.
(Suppose that tool number 100 is selected.)
Tool life counting is performed for the tool in group 2.
(The life of tool number 100 is counted.)
A tool whose life has not expired is selected from group 3.
(Suppose that tool number 200 is selected.)
Tool length offset for the tool selected from group 2 is used.
Cutter compensation for the tool selected from group 2 is
used.
Cutter compensation is canceled.
Tool length offset is canceled.
Tool life counting is performed for the tool in group 3.
(The life of tool number 200 is counted.)
A tool whose life has not expired is selected from group 4.
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 297 -
- Tool change type D
For a tool selected by a tool group command (T code), life counting is
performed by a tool change command (M06) specified in the same
block as the tool group command. Specifying a T code alone does
not results in an alarm; however, specifying an M06 command alone
results in alarm PS0153. However, the alarm can be suppressed by
setting bit 7 (TAD) of parameter No. 6805 to 1.
Example: Suppose that the tool life management ignore number is 100.
T101 M06 ;
:
:
:
:
T102 M06 ;
:
:
:
G43 H99 ;
:
:
G41 D99 ;
:
:
D00 ;
:
:
H00 ;
:
:
T103 M06 ;
:
:
A tool whose life has not expired is selected from group 1.
(Suppose that tool number 010 is selected.)
Tool life counting is performed for the tool in group 1.
(The life of tool number 010 is counted.)
A tool whose life has not expired is selected from group 2.
(Suppose that tool number 100 is selected.)
Tool life counting is performed for the tool in group 2.
(The life of tool number 100 is counted.)
Tool length offset for the tool selected from group 2 is used.
Cutter compensation for the tool selected from group 2 is
used.
Cutter compensation is canceled.
Tool length offset is canceled.
A tool whose life has not expired is selected from group 3.
Tool life counting is performed for the tool in group 3.
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 298 -
T
For the ATC type (bit 3 (TCT) of parameter No. 5040 = 1), commands
are specified in the same manner as for the M series except that D99
rather than H99 is used. For the ATC type, see the description for
the M series.
The following shows how commands are specified if the turret type is
used (bit 3 (TCT) of parameter No. 5040 = 0):
Example: Suppose that offset numbers are two digits long.
T0199 ;
:
:
:
:
:
:
T0188 ;
:
:
:
:
T0299 ;
:
:
:
:
:
T0299 ;
:
:
:
:
:
:
T0301 ;
:
:
A tool whose life has not expired is selected from group 1.
(Suppose that T1001 is selected. The tool number is 10,
and the offset number is 01.)
Tool life counting is performed for the tool in group 1.
(The life of tool number 10 is counted.)
The offset of the tool being used in group 1 is canceled.
(Since the tool being used is T1001, the tool number is 10,
and the offset number is 00.)
A tool whose life has not expired is selected from group 2.
(Suppose that T2002 is selected. The tool number is 20,
and the offset number is 02.)
Tool life counting is performed for the tool in group 2.
(The life of tool number 20 is counted.)
If more than one offset number is specified for the currently
used tool in group 2, the next offset number is selected.
(Suppose that T2002 and T2003 are registered with tool
number 20. In this case, T2003 is selected. The tool
number is 20, and the offset number is 03.)
Life counting for the tool in group 2 ends, and this command
is treated as an ordinary T code.
(The tool number is 03, and the offset number is 01.)
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 299 -
10.5.4 Tool Life Counting and Tool Selection
Either use count specification or duration specification is selected as
the tool life count type according to the state of bit 2 (LTM) of
parameter No. 6800. Life counting is performed for each group
separately, and the life counter contents are preserved even after the
power is turned off.
Table 10.5.4 Tool life management count types and intervals
Tool life count type Use count specification Time specification
Bit 2 (LTM) of
parameter No. 6800 0 1
Life count interval
Incremented by one for tools
used in one program
Counting can be resumed by
using tool life count restart M
code (parameter No. 6811).
Bit 0 (FCO) of parameter
No. 6805
0: Every second
1: Every 0.1 second
Can be changed by
override.
Explanation
M
- Use count specification (LTM=0)
If a tool group (T code) is specified, a tool whose life has not expired
is selected from the specified tool group. The life counter for the
selected tool is then incremented by one by a tool change command
(M06). Unless a tool life count restart M code is specified, selection
of a new tool and the increment operation can be performed only if a
tool group number command and a tool change command are issued
for the first time since the entry of the control unit into the automatic
operation start state from the reset state.
CAUTION
No matter how many times the same tool group
number is specified in a program, the use count is
not incremented, and no new tool is selected.
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 300 -
- Duration specification (LTM=1)
After all registered tool life management data is deleted, programmed
tool life management data is registered.
If a tool group command (T code) is specified, a tool whose life has
not expired is selected from the specified tool group. Then, life
management for the selected tool is started by a tool change command
(M06). Life management (counting) is performed by measuring the
time during which the tool is actually used in the cutting mode at
regular intervals (every second or 0.1 second). The life count
interval is specified by bit 0 (FCO) of parameter No. 6805. The time
required for single block stop, feed hold, rapid traverse, dwell,
machine lock, and interlock operations is not counted.
Setting bit 2 (LFV) of parameter No. 6801 enables the life count to be
overridden as directed by tool life count override signals. An
override from 0 times to 99.9 times can be applied. If 0 times is
specified, counting is not performed.
T
If the tool change type is the ATC type (bit 3 (TCT) of parameter No.
5040 = 1), the same specification method as for the M series applies.
See the description for the M series.
The following explains the specification method for the turret type (bit
3 (TCT) of parameter No. 5040 = 0):
- Use count specification (LTM=0)
If a tool group command (T○○99 code) is issued, a tool whose life
has not expired is selected from the specified tool group, and the life
counter for the selected tool is incremented by one. Unless a tool life
count restart M code is specified, selection of a new tool and the
increment operation can be performed only if a tool group number
command and a tool change command are issued for the first time
since the entry of the control unit into the automatic operation start
state from the reset state.
CAUTION
No matter how many times the same tool group
number is specified in a program, the use count is
not incremented, and no new tool is selected.
- Duration specification (LTM=1)
If a tool group command (T○○99 code) is specified, a tool whose
life has not expired is selected from the specified tool group, and tool
management for the selected tool starts.
Life management (counting) is performed by measuring the time
during which the tool is actually used in the cutting mode at regular
intervals (every second or 0.1 second). The life count interval is
specified by bit 0 (FCO) of parameter No. 6805. The time required
for single block stop, feed hold, rapid traverse, dwell, machine lock,
and interlock operations is not counted.
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 301 -
Setting bit 2 (LFV) of parameter No. 6801 enables the life count to be
overridden according tool life count override signals. An override
from 0 times to 99.9 times can be applied. If 0 times is specified,
counting is not performed.
M
T
NOTE
1 When a tool is selected, tools are searched starting
from the current tool toward the last tool to find a
tool whose life has not expired. When the last tool
is reached during this search, the search restarts
from the first tool. If the search does find any tool
whose life has not expired, the last tool is selected.
When the tool currently used is changed by the tool
skip signal, the next new tool is selected using the
method described here.
2 If tool life counting indicates that the life of the last
tool in a group has expired, the tool change signal
is output. If the life count type is duration
specification, the signal is output as soon as the life
of the last tool in the group has expired. If the life
count type is use count specification, the signal is
output when the CNC is reset by a command such
as M02 or M30 or when the tool life count restart M
code is specified after the life of the last tool in the
group has expired.
3 If a T command is specified, a group and a tool in
the group are selected while the T command is
buffered. This means that if a block to be buffered
contains a T command specifying a group while
machining is being performed with that group
selected, the next T command is already buffered
even if the tool life expires during machining, so the
next tool is not selected. To prevent this, if the life
count type is duration specification and a T
command is to be specified to select the same
group successively, insert an M code for
suppressing buffering into a place immediately
before the T command.
4 When the tool life is counted, the remaining life of a
group (the life value minus the life counter value) is
compared with the remaining life setting, and the
status of the tool life expiration prior notice signal is
changed according to the result of the comparison.
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 302 -
- M99
If the life count is specified by use count and bit 0 (T99) of parameter
No. 6802 is 1, the tool change signal TLCH<Fn064.0> is output and
the automatic operation is stopped if the life of at least one tool group
has expired when the M99 command is executed. If the life count
type is duration specification, the tool change signal is output
immediately when the life of at least one tool group has expired; when
the M99 command is specified, the automatic operation is stopped, but
no more tool change signal is output.
M
If the life count is specified by use count, a tool group command (T
code) issued after the M99 command selects, from a specified group,
a tool whose life has not expired, and the next tool change command
(M06) increments the tool life counter by one.
T
If the life count is specified by use count, when a tool group command
(T code) is specified after the M99 command is specified, a tool
whose life has not expired is selected from a specified group, and the
tool life counter is incremented by one.
If the tool change type is the ATC type (bit 3 (TCT) of parameter No.
5040 = 1), the same specifications as for the M series apply.
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 303 -
10.5.5 Tool Life Count Restart M Code
Explanation
M
If the life count is specified by use count, the tool change signal is
output if the life of at least one tool group has expired when a tool life
count restart M code is issued. A tool group command (T code)
issued after the tool life count restart M code selects, from a specified
group, a tool whose life has not expired, and the next tool change
command (M06) increments the tool life counter by one. This
enables the tool life to be counted by a tool change command (M06)
even if the command is not the first tool change command (M06)
issued since the entry of the CNC into the automatic operation start
state from the reset state. The tool life count restart M code is
specified in parameter No. 6811.
Example:
Suppose that M16 is a tool life count restart M code and that the
tool life management ignore number is 100.
Also suppose that the life count is specified by use count.
T101 ; A tool whose life has not expired is selected from group 1.
:
:
M06 ; Tool life management is performed for group 1.
: (The tool life counter is incremented by one.)
:
T102 ; A tool whose life has not expired is selected from group 2.
:
:
M06 ; Tool life management is performed for group 2.
: (The tool life counter is incremented by one.)
:
M16 ; Tool life counting is restarted.
T101 ; A tool whose life has not expired is selected from group 1.
:
:
M06 ; Tool life management is performed for group 1.
: (The tool life counter is incremented by one.)
10.TOOL FUNCTION (T FUNCTION) PROGRAMMING B-63944EN/03
- 304 -
T
If the tool change type is the ATC type (bit 3 (TCT) of parameter No.
5040 = 1), the same specifications as for the M series apply. See the
description for the M series.
The following explanation assumes that the tool change type is the
turret type (bit 3 (TCT) of parameter No. 5040 = 0).
If the life count is specified by use count, the tool change signal is
output if the life of at least one tool group has expired when a tool life
count restart M code is specified. A tool group command (T code)
issued after the tool life count restart M code selects a tool whose life
has not expired from a specified group, and the tool life counter is
incremented by one. This enables the tool life to be counted by a
tool group command (T code) even if the command is not the first tool
group command issued since the entry of the CNC into the automatic
operation start state from the reset state. The tool life count restart M
code is specified in parameter No. 6811.
Example:
Suppose that M16 is a tool life count restart M code.
Also suppose that the life count is specified by use count.
T199 ; A tool whose life has not expired is selected from group 1.
: Tool life management is performed for group 1.
: (The tool life counter is incremented by one.)
:
T299 ; A tool whose life has not expired is selected from group 2.
: Tool life management is performed for group 2.
: (The tool life counter is incremented by one.)
:
M16 ; Tool life counting is restarted.
T199 ; A tool whose life has not expired is selected from group 1.
: Tool life management is performed for group 1.
: (The tool life counter is incremented by one.)
M
T
NOTE
1 The tool life count restart M code is treated as an M
code not involved in buffering.
2 If the life count type is use count specification, the
tool change signal is output if the life of at least one
tool group has expired when the tool life count
restart M code is specified. If the life count type is
duration specification, specifying the tool life count
restart M code causes nothing.
B-63944EN/03 PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)
- 305 -
10.5.6 Disabling Life Count
Explanation
M
T
If bit 6 (LFI) of parameter No. 6804 is “1”, the tool life count disable
signal LFCIV can be used to select whether to cancel the tool life
count.
If the tool life count disable signal LFCIV is “1”, the tool life count
disabled signal LFCIF becomes “1”, and the tool life count is
disabled.
If the tool life count disable signal LFCIV is “0”, the tool life count
disabled signal LFCIF becomes “0”, and the tool life count is enabled.
NOTE
No buffering should occur when the state of the
tool life count disable signal LFCIV is changed.
So, use, for example, M codes not involved in
buffering to change the signal state. If M06 (for
the M series) or a tool change T code (for the T
series) is issued in a block that follows directly a
block in which an auxiliary function code with
buffering enabled is used to turn on or off the tool
life count disable signal LFCIV, it is likely that a
command for specifying whether to count may
become incorrect.
11.AUXILIARY FUNCTION PROGRAMMING B-63944EN/03
- 306 -
11 AUXILIARY FUNCTION
Overview
There are two types of auxiliary functions ; auxiliary function (M
code) for specifying spindle start, spindle stop, program end, and so
on, and secondary auxiliary function (B code) for specifying index
table positioning.
When a move command and auxiliary function are specified in the
same block, the commands are executed in one of the following two
ways:
(1) Simultaneous execution of the move command and auxiliary
function commands.
(2) Executing auxiliary function commands upon completion of
move command execution.
The selection of either sequence depends on the machine tool builder's
specification. Refer to the manual issued by the machine tool builder
for details.
Chapter 11, "AUXILIARY FUNCTION", consists of the following
sections:
11.1 AUXILIARY FUNCTION (M FUNCTION).........................307
11.2 MULTIPLE M COMMANDS IN A SINGLE BLOCK.........308
11.3 M CODE GROUPING FUNCTION ......................................309
11.4 SECOND AUXILIARY FUNCTIONS (B CODES) .............314
B-63944EN/03 PROGRAMMING 11.AUXILIARY FUNCTION
- 307 -
11.1 AUXILIARY FUNCTION (M FUNCTION)
When a numeral is specified following address M, code signal and a
strobe signal are sent to the machine. The machine uses these signals
to turn on or off its functions.
Usually, only one M code can be specified in one block. Depending
on the setting of bit 7 (M3B) of parameter No. 3404, up to three M
codes can be specified.
Which M code corresponds to which machine function is determined
by the machine tool builder. The machine processes all operations
specified by M codes except those specified by M98, M99,M198 or
called subprogram(Parameter No.6071 to 6079), or called custom
macro (Parameter No.6080 to 6089). Refer to the machine tool
builder's instruction manual for details.
Explanation
The following M codes have special meanings.
- M02,M30 (End of program)
This indicates the end of the main program.
Automatic operation is stopped and the CNC unit is reset. (This differs
with the machine tool builder.)
After a block specifying the end of the program is executed, control
returns to the start of the program.
Bits 5 (M02) and 4 (M30) of parameter No. 3404 can be used to
disable M02, M30 from returning control to the start of the program.
- M00 (Program stop)
Automatic operation is stopped after a block containing M00 is
executed. When the program is stopped, all existing modal
information remains unchanged. The automatic operation can be
restarted by actuating the cycle operation. (This differs with the
machine tool builder.)
- M01 (Optional stop)
Similarly to M00, automatic operation is stopped after a block
containing M01 is executed. This code is only effective when the
Optional Stop switch on the machine operator's panel has been
pressed.
- M98 (Calling of subprogram)
This code is used to call a subprogram. The code and strobe signals
are not sent. See the subprogram II-13.3 for details.
- M99 (End of subprogram)
This code indicates the end of a subprogram.
M99 execution returns control to the main program. The code and
strobe signals are not sent. See the subprogram section II-13.3 for
details.
11.AUXILIARY FUNCTION PROGRAMMING B-63944EN/03
- 308 -
11.2 MULTIPLE M COMMANDS IN A SINGLE BLOCK
Usually, only one M code can be specified in one block. By setting
bit 7 (M3B) of parameter No. 3404 to 1, however, up to three M codes
can be specified simultaneously in one block.
Up to three M codes specified in one block are output to the machine
at the same time. So, when compared with a case where a single M
code is specified in one block, a reduced machining cycle time can be
achieved.
Explanation
CNC allows up to three M codes to be specified in one block.
However, some M codes cannot be specified at the same time due to
mechanical operation restrictions. For detailed information about the
mechanical operation restrictions on simultaneous specification of
multiple M codes in one block, refer to the manual of each machine
tool builder.
M00, M01, M02, M30, M98, M99, or M198 must not be specified
together with another M code.
Some M codes other than M00, M01, M02, M30, M98, M99, and
M198 cannot be specified together with other M codes; each of those
M codes must be specified in a single block.
Such M codes include these which direct the CNC to perform internal
operations in addition to sending the M codes themselves to the
machine. To be specified, such M codes are M codes for calling
program numbers 9001 to 9009 and M codes for disabling advance
reading (buffering) of subsequent blocks. Meanwhile, multiple of M
codes that direct the CNC only to send the M codes themselves
(without performing internal operations ) can be specified in a single
block.
However, it is possible to specify multiple M codes that are sent to the
machine in the same block unless they direct the CNC to perform
internal operations. (Since the processing method depends on the
machine, refer to the manual of the machine tool builder.)
Example
One M command in a single block Multiple M commands in a single
block
M40;
M50;
M60;
G28G91X0Y0Z0;
:
:
:
M40M50M60;
G28G91X0Y0Z0;
:
:
:
:
:
B-63944EN/03 PROGRAMMING 11.AUXILIARY FUNCTION
- 309 -
11.3 M CODE GROUPING FUNCTION
Overview
Classifying a maximum of 500 M codes into a maximum of 127
groups allows the user:
• To receive an alarm if an M code that must be specified alone is
included when multiple M codes are specified in a block.
• To receive an alarm if M codes belonging to the same group are
specified in the same block when multiple M codes are specified in
a block.
11.3.1 Setting an M Code Group Number Using the Setting Screen
- Procedure for displaying the M code group setting screen
Fig. 11.3 (a) M code group setting screen
You can use the “M code group setting screen (Fig. 11.3 (a))” to set a
group number for each M code.
Display the “M code group setting screen” using the following
procedure:
(1) Press function key and the continuous menu key several
times. Soft key [M CODE GROUP] appears.
(2) Press soft key [M CODE GROUP].
In the “NO.” field, M codes for which an M code group can be set are
displayed.
An M code group can be set for the following M codes: M00 to M99,
and any 400 M codes selected from M100 and subsequent M codes.
For details of how to add the 100th and subsequent M codes, see the
explanation of parameters Nos. 3441 to 3444.
11.AUXILIARY FUNCTION PROGRAMMING B-63944EN/03
- 310 -
In the “DATA” field, the M code group number corresponding to each
M code is displayed.
- Setting a group number
To set an M code group number on the “M code group setting screen
(Fig. 11.3 (a)),” use he following procedure:
1 Select the MDI mode.
2 Set “PARAMETER WRITE” on the setting screen to 1.
3 Display the “M code group setting screen”.
4 Move the cursor to the M code to be set using page keys and
cursor keys. You can also enter the number of the M code to be
set and press soft key [NO.SRH] to move the cursor to the M
code.
5 Enter a group number and press soft key [INPUT] or the
key.
The valid range of M code group numbers is from 1 to 127 (127
groups). If a value of 0 is input, it is not registered as an M code
group.
- Examples of setting parameters Nos. 3441 to 3444
In the following examples, the number of digits of an M code is 4.
<1> to <4> indicate parameters Nos. 3441 to 3444.
(1) When <1> = 300, <2> = 400, <3> = 500, and <4> = 900 are set
M code groups can be set for M0000 to
M0099, M0300 to M0599, and M0900
to M999.
M codes M0300 to M0599 and M0900
to M999 are added to the M code group
setting screen.
N
umbe
r
0000
: 100 codes
0099
0300
: 100 codes
0399
0400
: 100 codes
0499
0500
: 100 codes
0599
0900
: 100 codes
0999
B-63944EN/03 PROGRAMMING 11.AUXILIARY FUNCTION
- 311 -
(2) When <1> = 200, <2> = 0, <3> = 550, and <4> = 800 are set
M code groups can be set for M0000 to M0099,
M0200 to M0299, M0550 to M0649, and
M0800 to M0899.
(The setting of parameter <2> is invalid because
it is 0.)
In this case, M codes M0200 to M0299, M0550
to M0649, and M0800 to M0899 are added to
the M code group setting screen.
N
umbe
r
0000
:
0099
0200
:
0299
0550
:
0649
0800
:
0899
11.AUXILIARY FUNCTION PROGRAMMING B-63944EN/03
- 312 -
11.3.2 Setting an M Code Group Number Using a Program
You can execute a program to set an M code group number and M
code name. The command format is shown below.
Format
G10 L40 Pn Rg ;
Pn: “n” specifies an M code.
Rg: “g” specifies an M code group number.
NOTE
1 If the format is invalid, an alarm PS1144 is issued.
2 If an M code group cannot be set for the M code
specified for the P command or if the group number
specified for the R command is not within the range
between 0 and 127, an alarm PS1305 is issued.
(Example)
Executing the following program sets M code group “1” to M03:
G10 L40 P03 R1 ;
B-63944EN/03 PROGRAMMING 11.AUXILIARY FUNCTION
- 313 -
11.3.3 M Code Group Check Function
When multiple M commands in a single block (enabled when bit 7
(M3B) of parameter No. 3404 is set to 1) are used, you can check the
following items. You can also select whether to check the items
using bit 1 (MGC) of parameter No. 3400.
(1) M code to be specified in a single block containing no other M
codes
If an M code which must be specified in a single block containing
no other M codes is specified together with another M code, an
alarm PS5016 is issued.
(2) M codes in the same group
If multiple M codes in the same group are specified together, an
alarm PS5016 is issued.
The valid range of group numbers is from 0 to 127 (128 groups).
Group numbers 0 and 1 have special meaning. Note the following
points:
• Each M code with group number 1 is assumed to be an M code to
be specified in a single block containing no other M codes.
• For each M code with group number 0, the “same group M code
check” is ignored. That is, when multiple M codes with group
number 0 are specified in a single block, the alarm is not issued.
• For each M code with group number 0, the “check for an M code
to be specified in a single block containing no other M codes” is
not ignored. That is, if an M code with group number 1 and an
M code with group number 0 are specified in a single block, the
alarm is issued.
• For M codes that are not to be output to the machine such as M98,
M99, M198, and M codes for subprogram and macro calls (set in
parameters Nos. 6071 to 6079 and Nos. 6080 to 6089 and with
the macro executor), be sure to set 0 as the group number.
• For M00, M01, M02, M30, and M codes for which buffering is
suppressed (set in parameters Nos. 3411 to 3432), be sure to set 1
as the group number.
11.AUXILIARY FUNCTION PROGRAMMING B-63944EN/03
- 314 -
11.4 SECOND AUXILIARY FUNCTIONS (B CODES)
Overview
If a value with a maximum of eight digits is specified after address B,
the code signal and strobe signal are transferred for calculation of the
rotation axis. The code signal is retained until the next B code is
specified.
Only one B code can be specified for each block. When the
maximum number of digits are specified by parameter No.3033, an
alarm is issued if the number of digits of a command exceeds the
specified number.
In addition, the address used for specifying the second auxiliary
function can be changed to an address other than address B (address A,
C, U, V, or W) by setting parameter No.3460.
However, the address used for the second auxiliary function cannot
also be used as the address of the controlled axis. For details, refer to
the manual available from the machine tool builder.
Explanation
- Range of specification
-99999999 to 99999999
- Output value
The value specified after the address of the second auxiliary function
is output on the code signals B00 to B31. Note the following about a
output value.
1. When a command with a decimal point or a negative command is
disabled
(When bit 0 (AUP) of parameter No.3450 is set to 0)
When the second auxiliary function with no decimal point is
specified, the specified value is output on the code signals as is,
regardless of the desktop calculator decimal point setting (bit 0
(DPI) of parameter No.3401).
Example:
Specified value Output value
B10 10
When the second auxiliary function with a decimal point is
specified, alarm PS0007 is issued.
When the second auxiliary function is specified with a negative
value, alarm PS0006 is issued.
B-63944EN/03 PROGRAMMING 11.AUXILIARY FUNCTION
- 315 -
2. When a command with a decimal point or a negative command is
enabled
(When bit 0 (AUP) of parameter No.3450 is set to 1)
When the desktop calculator decimal point setting is not
specified (when bit 0 (DPI) of parameter No.3401 is set to 0), if
the second auxiliary function with no decimal point is specified,
the specified value is output on the code signals as is.
Example:
Specified value Output value
B10 10
When desktop calculator decimal point input is specified (when
bit 0 (DPI) of parameter No.3401 is set to 1), if the second
auxiliary function with no decimal point is specified, the
specified value multiplied by a magnification is output on the
code signals. (Magnifications are shown in Table 11.4 (a).)
Example:
Specified value Output value
B10 10000 (When metric input is used and
the reference axis is IS-B. The
magnification is 1000.)
When the second auxiliary function with a decimal point is
specified, the specified value multiplied by a magnification is
output to the code signals. (Magnifications are shown in Table
11.4 (a).)
Example:
Specified value Output value
B10. 10000 (When metric input is used and
the reference axis is IS-B. The
magnification is 1000.)
B0.123 1230 (When inch input is used, the
reference axis is IS-B, and
parameter AUX is set to 1. The
magnification is 10000.)
11.AUXILIARY FUNCTION PROGRAMMING B-63944EN/03
- 316 -
The magnification is determined as shown below according to
the setting unit of the reference axis (specified by parameter
No.1031) and bit 0 (AUX) of parameter No.3405.
Table 11.4 (a) Magnifications for an output value when the second
auxiliary function with a decimal point is specified for
desktop calculator decimal point input
Setting unit Parameter
AUX = 0
Parameter
AUX = 1
Reference axis: IS-A 100× 100×
Reference axis: IS-B 1000× 1000×
Reference axis: IS-C 10000× 10000×
Reference axis: IS-D 100000× 100000×
Metric input system
Reference axis: IS-E 1000000× 1000000×
Reference axis: IS-A 100× 1000×
Reference axis: IS-B 1000× 10000×
Reference axis: IS-C 10000× 100000×
Reference axis: IS-D 100000× 1000000×
Inch input system
Reference axis: IS-E 1000000× 10000000×
CAUTION
If a decimal fraction remains after multiplying the
specified value with a decimal point by a magnitude
in Table 11.4 (a), the fraction is truncated.
Example:
Specified value Output value
B0.12345 1234 (When inch input is used,
the reference axis is IS-B, and
parameter AUX is set to 1. The
magnification is 10000.)
NOTE
If the number of digits of the specified value
exceeds the allowable number of digits (set by
parameter No.3033), alarm PS0003 is issued.
When the specified value is multiplied by a
magnitude in Table 11.4 (a), the allowable number
of digits must be set for the resultant value.
Limitation
Addresses used for the second auxiliary functions (addresses specified
with B or parameter No. 3460) cannot be used as the addresses used
for controlled axis names.
B-63944EN/03 PROGRAMMING 12.PROGRAM MANAGEMENT
- 317 -
12 PROGRAM MANAGEMENT
Chapter 12, "PROGRAM MANAGEMENT", consists of the
following sections:
12.1 FOLDERS ..............................................................................318
12.2 FILES .....................................................................................323
12.3 RELATION WITH CONVENTIONAL FUNCTIONS .........326
12.PROGRAM MANAGEMENT PROGRAMMING B-63944EN/03
- 318 -
12.1 FOLDERS
Overview
Folders can be created in program memory.
12.1.1 Folder Configuration
The following folders can be created:
• Folder names are up to 32 characters long.
• The following characters can be used in folder names:
Alphabetical characters (uppercase and lowercase letters),
numeric characters, and the symbols below:
− + _ .
Because "." and ".." are reserved folder names, they cannot be
used.
- Initial folders
When program memory is initialized, folders having predefined
structures and names are created. These folders are called initial
folders.
(1) Root folder
The parent folder of all folders
(2) System folder (SYSTEM)
Contains subprograms and macro programs of the system.
(3) MTB dedicated folder 1 (MTB1)
Contains subprograms and macro programs created by the
machine tool builder.
(4) MTB dedicated folder 2 (MTB2)
Contains subprograms and macro programs created by the
machine tool builder.
(5) User folder
Contains programs created by the user.
The following folders are further created in this folder:
(a) Path folders (PATHn: As many folders as the number of
paths are created.)
Each contains main programs, subprograms, and macro
programs used for the corresponding path.
(b) Common program folder (LIBRARY)
Contains subprograms and macro programs used
commonly.
NOTE
The initial folders can neither be deleted nor
renamed.
B-63944EN/03 PROGRAMMING 12.PROGRAM MANAGEMENT
- 319 -
[Initial folder configuration]
/
SYSTEM/
//CNC_MEM
MTB1/
USER/
PATH1/
PATH2/
LIBRARY/
(1) Root folder
(2) System folder (SYSTEM)
(3) MTB dedicated folder 1 (MTB1)
(5) User folder
(b) Common program folder (LIBRARY)
(a) Path folders (PATHn)
The device that used to contain
programs is called CNC_MEM.
PATHn/
MTB2/
(4) MTB dedicated folder 2 (MTB2)
12.PROGRAM MANAGEMENT PROGRAMMING B-63944EN/03
- 320 -
- User created folders
Folders other than the initial folders are called user created folders.
User created folders can be created in the following initial folders:
• User folder
• Path folders
User created folders can contain user created main programs,
subprograms, and macro programs.
NOTE
1 Folder names must each be unique in the same
folder.
2 Each time a user created folder is created, the
number of programs that can be registered
decreases by one.
3 Folder hierarchical levels of user created folders
are limited.
Up to three hierarchical levels starting from the
user folder (USER/) are permitted.
/
SYSTEM/
[Sample folder configuration]
//CNC_MEM
MTB1/
USER/
PATH1/
PATH2/
LIBRARY
/
User created folders
Programs are grouped by
part to be machined, and the
program groups are stored in
individual folders.
CYLINDER/
PISTON/
GEAR1/
GEAR2/
MTB2/
B-63944EN/03 PROGRAMMING 12.PROGRAM MANAGEMENT
- 321 -
12.1.2 Folder Attributes
The following attributes can be set for folders except the root folder:
• Edit disable
• Edit/display disable
- Edit disable
Editing of the programs and folders in a folder can be disabled.
A program in the folder can be output to an external device.
A program cannot be input (registered) from an external device to the
folder.
- Edit/display disable
Editing and display of the programs and folders in a folder can be
disabled.
When this attribute is set for a folder, the programs and folders in the
folder become invisible. (The folder appears to contain nothing.)
A program in the folder cannot be output to an external device and a
program cannot be input (registered) from an external device to a
folder.
12.PROGRAM MANAGEMENT PROGRAMMING B-63944EN/03
- 322 -
12.1.3 Default Folders
Default folders are folders on which operations are performed when
no folder is specified. There are two types of default folders as
follows:
• Foreground default folder
• Background default folder
- Foreground default folder
A folder used for foreground operations except automatic operations
and program editing is set.
The target operations include:
• Program input/output
• External data input
• External workpiece number search
- Background default folder
A folder used for background operations is set.
The target operations include:
• Program input/output
• External I/O device control
NOTE
1 When the foreground or background default folder
is not set, a path folder, which is an initial folder, is
assumed.
2 Foreground and background default folder settings
are stored in default folder setting files.
3 When a program file, program folder, or program
folder management file is cleared, the default folder
setting file is cleared at the same time.
B-63944EN/03 PROGRAMMING 12.PROGRAM MANAGEMENT
- 323 -
12.2 FILES
Overview
Desired file names can be given to part programs in program memory.
12.2.1 File Name
File names can be set as follows:
• File names are up to 32 characters long.
• The following characters can be used in file names:
Alphabetical characters (uppercase and lowercase letters),
numeric characters, and the symbols below:
− + _ .
Because "." and ".." are reserved file names, they cannot be used.
- File names and program numbers
File names are associated with program numbers as explained below.
When the file name of a program consists of "O" plus a numeric with
the following limitation, the program can be handled also by program
number.
• The numeric must be a leading zero suppressed value from 1 to
9999.
When the file name of a program does not have the above format, the
program cannot be handled by program number.
When a file name consisting of "O" plus a numeric does not satisfy the
above limitation, the file cannot be created.
Example)
File names that can be treated as program numbers
O123 Program number 123
O1 Program number 1
O3000 Program number 3000
O9999 Program number 9999
File names that cannot be treated as program numbers
ABC
o123
O123.4
NOTE
1 File names must each be unique in the same
folder.
2 When the file name of a program is not treated as a
program number, the program is restricted as
follows:
- The program cannot be specified by program
number.
- Information output by program number is
impossible..
12.PROGRAM MANAGEMENT PROGRAMMING B-63944EN/03
- 324 -
- Displaying File Names and Program Numbers
The file name of the program selected or being executed as the main
program is displayed as shown in Figs. 12.2.1 (a) to 12.2.2 (c).
• For file names that can be handled as program numbers, the
program number is displayed.
Fig. 12.2.1 (a) File name display 1
• For file names that cannot be handled as program numbers, the
file name is displayed.
The display layout varies as shown below, depending on the
length of a file name.
Fig. 12.2.1 (b) File name display 2
Fig. 12.2.1 (c) File name display 3
B-63944EN/03 PROGRAMMING 12.PROGRAM MANAGEMENT
- 325 -
12.2.2 File Attributes
The following attributes can be set for files:
• Edit disable
• Edit/display disable
• Encoding
• Change protection level/output protection level
- Edit disable
Editing of a specified program can be disabled.
A program cannot be input (registered) from an external device to the
folder.
- Edit/display disable
Editing and display of a specified program can be disabled.
When this attribute is set, the program becomes invisible.
(The folder appears not to contain this program.)
An output to an external device and an input from an external device
(program registration) cannot be made.
- Encoding
A specified program can be encoded.
For details of encoding, see the description of the “Program
encryption” function.
An output to an external device and an input from an external device
(program registration) cannot be made.
- Change protection level/output protection level
With the 8-level data protection function, change and output
protection can be provided for a specified program.
For details of the 8-level data protection function, see the description
of the “Protection of data at eight levels” function.
12.PROGRAM MANAGEMENT PROGRAMMING B-63944EN/03
- 326 -
12.3 RELATION WITH CONVENTIONAL FUNCTIONS
This section explains relation with conventional functions when folder
names and file names are used.
12.3.1 Relation with Folders
This subsection explains how folders are used for operations and
editing.
- Automatic operation
Main program
As the main program running for an automatic operation, a program in
a desired folder can be selected.
Subprogram (called by M98/G72.1/G72.2)
Macro program (called by G65/G66/G66.1/M96)
• Subprogram call (M98)
• Macro call (simple call G65/modal call G66, G66.1)
• Macro interrupt (M96)
• Figure copying (G72.1, G72.2)
When a call listed above is made, folders are searched in the following
order, and the program found first is called:
<1> Folders containing the main program
<2> Common program folder, which is an initial folder (LIBRARY)
Bit 7 (SCF) of parameter No. 3457 can be used to add the following
search folders. (The folders are searched in the order listed below.)
The folder to be actually enabled is separately set by bits 1 to 3 of
parameters No. 3457.
<3> MTB dedicated folder 2, which is an initial folder (MTB2)
<4> MTB dedicated folder 1, which is an initial folder (MTB1)
<5> System folder, which is an initial folder (SYSTEM)
Subprogram (called by M code/specific address/2nd auxiliary function)
Macro program (called by G code/M code/T code/one touch macro)
• Subprogram call by M code/specific address/2nd auxiliary
function code
• Macro call by G code/M code/T code
• One touch macro call
For programs called as listed above, the folders to be searched are set
in bits 0 to 3 of parameter No.3457 in advance. (The search order is
described below.)
The folders set as the search targets are searched, and the program
found first is called.
<1> Common program folder, which is an initial folder (LIBRARY)
<2> MTB dedicated folder 2, which is an initial folder (MTB2)
<3> MTB dedicated folder 1, which is an initial folder (MTB1)
<4> System folder, which is an initial folder (SYSTEM)
B-63944EN/03 PROGRAMMING 12.PROGRAM MANAGEMENT
- 327 -
- Program editing
A program in any folder can be edited.
- Program I/O
The following functions are performed for default folders:
• Program input from external devices
• Program output to external devices
(Except the format with folder names)
The following functions are performed for a set background default
folder:
• External I/O device control
- External data input
A set foreground default folder is searched for an external program.
- External workpiece number search
A set foreground default folder is searched for an external workpiece
number.
- Macro executor
Programs called by execution macros, conversational macros, and
auxiliary macros are programs in P-Code files regardless of the default
folder.
For programs on the macro executor, the folder function and file name
function are unavailable.
12.PROGRAM MANAGEMENT PROGRAMMING B-63944EN/03
- 328 -
12.3.2 Relation with File Names
File names can be used with the following functions:
• Subprogram call (M98)
• Macro call (simple call G65/modal call G66, G66.1)
• Interruption type macro call (M96)
• Subprogram call in figure copying (G72.1, G72.2)
• Program I/O with external devices
- Subprogram call by file name
- Macro call by file name
• Subprogram call (M98)
• Macro call (G65/G66/G66.1)
• Interruption type macro call (M96)
• Figure copying (G72.1, G72.2)
When a program is called in the above functions, a subprogram call by
file name and a macro call by file name can be used.
• Subprogram call by file name
M98 <file-name> Lxx ;
• Macro call by file name
G65 <file-name> Lxx argument-specification ;
G66 <file-name> Lxx argument-specification ;
G66.1 <file-name> Lxx argument-specification ;
• Interruption type macro call
M96 <file-name> ;
• Subprogram call by file name in figure copying (G72.1, G72.2)
G72.1 <file-name> Lxx Xxx Yxx Rxx ;
G72.2 <file-name> Lxx Ixx Jxx ;
In the above subprogram and macro calls, the program having the file
name indicated by <file-name> is called.
Format examples:
• Subprogram call
M98 <R50> L1 ;
• Macro call
G65 <R50> L1 A0 ;
G66 <R50> L1 A1 ;
G66.1 <R50> L1 A2 ;
• Interruption type macro call
M96 <R50> ;
• Subprogram call in figure copy
G72.1 <R50> L1 X0 Y0 R0 ;
G72.2 <R50> L1 I0 J0 ;
B-63944EN/03 PROGRAMMING 12.PROGRAM MANAGEMENT
- 329 -
NOTE
1 When characters in <> are read, they are treated in
the same way as for characters in comments. So,
note that these characters are treated differently
from other significant information portions.
Refer to Appendix B “PROGRAM CODE LIST” for
details.
2 The <file-name> word must be placed immediately
after each word for calling (M98, G65, and so forth).
12.3.3 Related Parameters
This subsection lists the meanings of parameters related to program
numbers and the folders and programs to be manipulated or executed.
Parameter
No. Bit No. Description Manipulation/execution target
0 (NE8) Disables or enables editing of programs O8000
to O8999. Corresponding programs in all folders
3202
4 (NE9) Disables or enables editing of programs O9000
to O9999. Same as above
3 (P8E) Disables or enables editing of programs
O80000000 to O8999999. Same as above
4 (P9E) Disables or enables editing of programs
O90000000 to O99999999. Same as above
3204
5 (SPR)
Assumes or does not assume a particular
program number in the nine thousands to be a
number obtained by adding 90000000.
Same as above
3210/3211 -
Password/keyword for protecting programs in the
nine thousands Same as above
3222/3223 -
Program protection range (minimum
value)/(maximum value) Same as above
3404 2 (SBP)
In the subprogram call function, address P in the
M198 block specifies a file/program number.
(Not dependent on the folder function
and file name function)
6001 5 (TCS) Calls or does not call a custom macro by T code.
The following initial folders can be
selected by parameter setting:
- Common program folder (LIBRARY)
- MTB dedicated folder 2 (MTB2)
- MTB dedicated folder 1 (MTB1)
- System folder (SYSTEM)
6050 to 6059 - G code for calling a custom macro with program
No. 9010 to 9019 Same as above
6071 to 6079 - M code for calling a subprogram with program
No. 9001 to 9009 Same as above
6080 to 6089 - M code for calling a custom macro with program
No. 9020 to 9029 Same as above
6090/6091 -
ASCII code for calling a subprogram with
program No. 9004/9005 Same as above
8341/8343 -
Target program number (for 4- and 8-digit O
number) for sequence number comparison and
stop
Foreground or background default
folder depending on the mode
12.PROGRAM MANAGEMENT PROGRAMMING B-63944EN/03
- 330 -
12.3.4 Part Program Storage Size / Number of Registerable
Programs
The following table lists the combinations of program storage sizes
and the total number of registrable programs.
Part
program
storage size
Number of
registerable
programs
Number of
registerable
programs
expansion 1
Number of
registerable
programs
expansion 2 *2
32Kbyte *1 63 - -
64Kbyte 63 125 -
128Kbyte 63 250 -
256Kbyte 63 500 -
512Kbyte 63 1000 -
1Mbyte 63 1000 2000
2Mbyte 63 1000 4000
4Mbyte *2 63 1000 4000
8Mbyte *2 63 1000 4000
*1) For Series 32i-A only
*2) For Series 30i/31i-A, For Series 31i-A5 only
NOTE
1 Creating one folder results in the number of
programs yet to be registerable decreasing one.
2 The program storage size means the maximum
size of a program if the program is the one and
only program registered.
3 If more than one program is registered, the total
size of registerable programs reduces for the
following reason.
The Series 30i/31i/32i-A and Series 31i-A5
manage programs in page units. The unit of
program storage is managed also in page units.
When a program is created, as many pages as
necessary to store the program are secured, and
the program is stored on these pages. Generally,
the last program storage page has an unused area
(left figure). This unused area cannot be used to
store any other program. For the sake of program
management, it is regarded as an area in use.
The Series 16i/18i/21i uses a similar way of
management, but the unit of pages in it differs from
that in the Series 30i/31i/32i-A and FS31i-A5. So,
if more than one program is registered in the Series
30i/31i/32i-A or FS31i-A5, the total program size of
registerable programs in the Series 30i/31i/32i-A or
Series 31i-A5 differs from that in the Series
16i/18i/21i.
Example of creating program O0001
O0001 ;
N1 G01 ;
M30 ;
First page
Second page
Last page
Program O0001
Unusable for any other
p
ro
g
ram
(
Area in use
)
N100 … ;
(
Area in use
)
(
Area in use
)
(Unused area)
B-63944EN/03 PROGRAMMING 13.PROGRAM CONFIGURATION
- 331 -
13 PROGRAM CONFIGURATION
Overview
- Main program and subprogram
There are two program types, main program and subprogram.
Normally, the CNC operates according to the main program.
However, when a command calling a subprogram is encountered in
the main program, control is passed to the subprogram. When a
command specifying a return to the main program is encountered in a
subprogram, control is returned to the main program.
Follow the direction of the
subprogram
Main program Subprogram
Instruction 1
Instruction 2
Instruction n
Instruction 1’
Instruction 2’
Instruction n+1
Return to the main program
Fig. 13 (a) Main program and Subprogram
The CNC memory can hold up to 4000 main programs and
subprograms (63 as standard). A main program can be selected from
the stored main programs to operate the machine. See III-9 or III-10.4
for the methods of registering and selecting programs.
13.PROGRAM CONFIGURATION PROGRAMMING B-63944EN/03
- 332 -
- Program components
A program consists of the following components:
Table 13 (a) Program components
Components Descriptions
Program code start Symbol indicating the start of a program file
Leader section Used for the title of a program file, etc.
Program start Symbol indicating the start of a program
Program section Commands for machining
Comment section Comments or directions for the operator
Program code end Symbol indicating the end of a program file
Program code start %TITLE ;
O0001 ;
M30 ;
%
(COMMENT)
Program section
Leader section
Program start
Comment section
Program code end
Fig. 13 (b) Program configuration
- Program section configuration
A program section consists of several blocks. A program section starts
with a program number or file name and ends with a program end
code.
Program section Program section
configuration
Program number O0001 ;
Block 1 N1 G91 G00 X120.0 Y80.0 ;
Block 2 N2 G43 Z-32.0 H01 ;
: :
Block n Nn Z0 ;
Program end M30 ;
A block contains information necessary for machining, such as a move
command or coolant on/off command. Specifying a slash (/) at the
start of a block disables the execution of some blocks (see "optional
block skip" in II-13.2).
B-63944EN/03 PROGRAMMING 13.PROGRAM CONFIGURATION
- 333 -
13.1 PROGRAM COMPONENTS OTHER THAN PROGRAM
SECTIONS
This section describes program components other than program
sections. See II-13.2 for a program section.
%TITLE;
O0001 ;
M30 ;
%
(COMMENT)
Pro
g
ram code start
Program section
Leader section
Program start
Comment section
Program code end
Fig. 13.1 (a) Program configuration
Explanation
- Program code start
The program code start indicates the start of a file that contains NC
programs.
The mark is not required when programs are entered using SYSTEM
P or ordinary personal computers. The mark is not displayed on the
screen. However, if the file is output, the mark is automatically output
at the start of the file.
Table 13.1 (a) Code of a program code start
Name ISO code EIA code Notation in this
manual
Program code start % ER %
- Leader section
Data entered before the programs in a file constitutes a leader section.
When machining is started, the label skip state is usually set by
turning on the power or resetting the system. In the label skip state, all
information is ignored until the first end-of-block code is read.
When a file is read into the CNC unit from an I/O device, leader
sections are skipped by the label skip function.
A leader section generally contains information such as a file header.
When a leader section is skipped, even a TV parity check is not made.
So a leader section can contain any codes except the EOB code.
13.PROGRAM CONFIGURATION PROGRAMMING B-63944EN/03
- 334 -
- Program start
The program start code is to be entered immediately after a leader
section, that is, immediately before a program section.
This code indicates the start of a program, and is always required to
disable the label skip function.
With SYSTEM P or ordinary personal computers, this code can be
entered by pressing the return key.
Table 13.1 (b) Code of a program start
Name ISO code EIA code Notation in this
manual
Program start LF CR ;
NOTE
If one file contains multiple programs, the EOB code
for label skip operation must not appear before a
second or subsequent program number.
- Comment section
Any information enclosed by the control-out and control-in codes is
regarded as a comment.
The user can enter a header, comments, directions to the operator, etc.
in a comment section.
Table 13.1 (c) Codes of a control-in and a control-out
Name ISO code EIA code Notation in this
manual Meaning
Control-out ( 2-4-5 (
Start of comment
section
Control-in ) 2-4-7 )
End of comment
section
When a program is read into memory for memory operation, comment
sections, if any, are not ignored but are also read into memory. Note,
however, that codes other than those listed in the code table in
Appendix A are ignored, and thus are not read into memory.
When data in memory is output on external I/O device (See III-8), the
comment sections are also output.
When a program is displayed on the screen, its comment sections are
also displayed. However, those codes that were ignored when read
into memory are not output or displayed.
During memory operation or DNC operation, all comment sections are
ignored.
The TV check function can be used for a comment section by setting
bit 1 (CTV) of parameter No. 0100.
B-63944EN/03 PROGRAMMING 13.PROGRAM CONFIGURATION
- 335 -
CAUTION
If a long comment section appears in the middle of
a program section, a move along an axis may be
suspended for a long time because of such a
comment section. So a comment section should be
placed where movement suspension may occur or
no movement is involved.
NOTE
1 If only a control-in code is read with no matching
control-out code, the read control-in code is
ignored.
2 The following codes cannot be used in the
comment section:
- EOB
- % (ER for EIA)
- Program code end
A program code end is to be placed at the end of a file containing NC
programs.
If programs are entered using the automatic programming system, the
mark need not be entered.
The mark is not displayed on the screen. However, when a file is
output, the mark is automatically output at the end of the file.
If an attempt is made to execute % when M02 or M30 is not placed at
the end of the program, the alarm PS5010 is occurred.
Table 13.1 (d) Code of a program code end
Name ISO code EIA code Notation in this
manual
Program code end % ER %
13.PROGRAM CONFIGURATION PROGRAMMING B-63944EN/03
- 336 -
13.2 PROGRAM SECTION CONFIGURATION
This section describes elements of a program section. See II-13.1 for
program components other than program sections.
%
(COMMENT)
%TITLE ;
O0001 ;
N1 ... ;
M30 ;
Program section
Program number
Sequence number
Program end
Fig. 13.2 (a) Program configuration
- Program number
A program number consisting of address O followed by a four-digit
number is assigned to each program at the beginning registered in
memory to identify the program. When the 8-digit number function
is selected, the program number consists of eight digits.
In ISO code, the colon ( : ) can be used instead of O.
When no program number is specified at the start of a program, the
sequence number (N....) at the start of the program is regarded as its
program number. If a five-digit sequence number is used, the lower
four digits are registered as a program number. If the lower four digits
are all 0, the program number registered immediately before added to
1 is registered as a program number. Note, however, that N0 cannot
be used for a program number.
If there is no program number or sequence number at the start of a
program, a program number must be specified using the MDI panel
when the program is stored in memory (See III-8.2 or III-9.1)
NOTE
Program numbers 8000 to 9999 may be used by
machine tool builders, and the user may not be able
to use these numbers.
B-63944EN/03 PROGRAMMING 13.PROGRAM CONFIGURATION
- 337 -
- File name
A file name can be assigned instead of a program number.
When coding a file name, be sure to place the file name enclosed in
"<" and ">" at the beginning of a program.
Example) % ;
<PARTS_1> ;
N1 ...
:
M30 ;
%
NOTE
A file name can be coded:
- At the beginning of a program
- Immediately after M98, G65, G66, G66.1, M96,
G72.1, or G72.2
Do not code a file name in other than the above.
- Sequence number and block
A program consists of several commands. One command unit is called
a block. One block is separated from another with an EOB of end of
block code.
Table 13.2 (a) EOB code
Name ISO code EIA code Notation in this manual
End of block (EOB) LF CR ;
At the head of a block, a sequence number consisting of address N
followed by a number not longer than eight digits (1 to 99999999) can
be placed. Sequence numbers can be specified in a random order, and
any numbers can be skipped. Sequence numbers may be specified
for all blocks or only for desired blocks of the program. In general,
however, it is convenient to assign sequence numbers in ascending
order in phase with the machining steps (for example, when a new tool
is used by tool replacement, and machining proceeds to a new surface
with table indexing.)
N300X200.0Z300.0 ; A sequence number is underlined.
Fig. 13.2 (b) Sequence number and block (example)
NOTE
N0 must not be used for the reason of file
compatibility with other CNC systems.
Program number 0 cannot be used. So 0 must
not be used for a sequence number regarded as a
program number.
13.PROGRAM CONFIGURATION PROGRAMMING B-63944EN/03
- 338 -
- TV check (Vertical parity check)
A parity check is made for each block of input data. If the number of
characters in one block (starting with the code immediately after an
EOB and ending with the next EOB) is odd, a P/S alarm (No.002) is
output.
No TV check is made only for those parts that are skipped by the label
skip function. Bit 1 (CTV) of parameter No. 0100 is used to specify
whether comments enclosed in parentheses are counted as characters
during TV check. The TV check function can be enabled or disabled
by setting on the MDI unit (See III-12.3.1.).
- Block configuration (word and address)
A block consists of one or more words. A word consists of an
address followed by a number some digits long. (The plus sign (+) or
minus sign (-) may be prefixed to a number.)
For an address, one of the letters (A to Z) is used ; an address defines
the meaning of a number that follows the address.
Word = Address + number (Example : X-1000)
Table 13.2 (b) indicates the usable addresses and their meanings.
The same address may have different meanings, depending on the
preparatory function specification.
Table 13.2 (b) Major functions and addresses
Function Address Meaning
Program number O(*) Program number
Sequence number N Sequence number
Preparatory function G Specifies a motion mode (linear,
arc, etc.)
X, Y, Z, U, V,
W, A, B, C Coordinate axis move command
I, J, K Coordinate of the arc center
Dimension word
R Arc radius
Feed function F Rate of feed per minute,
Rate of feed per revolution
Spindle speed function S Spindle speed
Tool function T Tool number
M On/off control on the machine tool
Auxiliary function B Table indexing, etc.
Program number
designation P Subprogram number
Number of repetitions P, L Number of subprogram repetitions
Parameter P, Q Canned cycle parameter
M
Offset number D, H Offset number
Dwell P, X Dwell time
T
Dwell P, X, U Dwell time
B-63944EN/03 PROGRAMMING 13.PROGRAM CONFIGURATION
- 339 -
NOTE
(*) In ISO code, the colon ( : ) can also be used as the
address of a program number.
N_ G_ X_ Y_ F_ S_ T_ M_ ;
Sequence
number
Preparatory
function
Dimension
word
Feed-functi
on
Spindle
speed
function
Tool
function
Auxiliary
function
Fig. 13.2 (c) 1 block (example)
- Major addresses and ranges of command values
Major addresses and the ranges of values specified for the addresses
are shown below. Note that these figures represent limits on the CNC
side, which are totally different from limits on the machine tool side.
For example, the CNC allows a tool to traverse up to about 100 m (in
millimeter input) along the X axis.
However, an actual stroke along the X axis may be limited to 2 m for
a specific machine tool.
Similarly, the CNC may be able to control a cutting feedrate of up to
240 m/min, but the machine tool may not allow more than 3 m/min.
When developing a program, the user should carefully read the
manuals of the machine tool as well as this manual to be familiar with
the restrictions on programming.
Table 13.2 (c) Major addresses and ranges of command values
Function Address Input in mm Input in inch
Program number O (*1)
1 to 99999999 1 to 99999999
Sequence number N
1 to 99999999 1 to 99999999
Preparatory function G
0 to 99.9 0 to 99.9
Increment system IS-A
±
999999.99 mm
±
999999.99 deg.
±
99999.999 inch
*3
±
999999.99 deg.
Increment system IS-B
±
999999.999 mm
±
999999.999 deg.
±
99999.9999 inch
*3
±
999999.999 deg.
Increment system IS-C
±
99999.9999 mm
±
99999.9999 deg.
±
9999.99999 inch
*3
±
99999.9999 deg.
Increment system IS-D
±
9999.99999 mm
±
9999.99999 deg.
±
999.999999 inch
*3
±
9999.99999 deg.
Dimension
word
Increment system IS-E
X,Y,Z,U,V,
W,A,B,C,I,J
,K,R (*2)
±
999.999999 mm
±
999.999999 deg.
±
99.9999999 inch
*3
±
999.999999 deg.
Increment system IS-A
0.01 to 999000.00mm/min 0.001 to 96000.000inch/min
Increment system IS-B
0.001 to 999000.000mm/min 0.0001 to 9600.0000inch/min
Increment system IS-C
0.0001 to 99999.9999mm/min 0.00001 to 4000.00000inch/min
Increment system IS-D
0.00001 to 9999.99999mm/min 0.000001 to 400.000000inch/min
Feed per
minute
Increment system IS-E
F
0.000001 to 999.999999mm/min 0.0000001 to 40.0000000inch/min
Feed per revolution F
0.001 to 50000mm/rev 0.0001 to 50.0000inch/rev
Spindle speed function S (*4)
0 to 99999999 0 to 99999999
Tool function T (*4)
0 to 99999999 0 to 99999999
M (*4)
0 to 99999999 0 to 99999999
Auxiliary function B (*4)
0 to 99999999 0 to 99999999
Offset number (M series only) H, D
0 to 999 0 to 999
13.PROGRAM CONFIGURATION PROGRAMMING B-63944EN/03
- 340 -
Function Address Input in mm Input in inch
Increment system IS-A
0 to 999999.99 sec 0 to 999999.99 sec
Increment system IS-B
0 to 99999.999 sec 0 to 99999.999 sec
Increment system IS-C
0 to 9999.9999 sec 0 to 9999.9999 sec
Increment system IS-D
0 to 999.99999 sec 0 to 999.99999 sec
Dwell
Increment system IS-E
X,
U (T series
only)
0 to 99.999999 sec 0 to 99.999999 sec
Dwell P
1 to 99999999
1 to 99999999
Designation of a program number P
1 to 99999999 1 to 99999999
L
1 to 99999999 1 to 99999999
Number of subprogram repetitions P
0 to 9999 0 to 9999
*1 In ISO code, the colon ( : ) can also be used as the address of a
program number.
*2 When address I, J, K, or R is used to specify the radius for
circular interpolation, the specifiable range is as follows:
Increment system Input in mm Input in inch
IS-A
±
999999999.99 mm
±
99999999.999 inch
IS-B
±
999999999.999 mm
±
99999999.9999 inch
IS-C
±
99999999.9999 mm
±
9999999.99999 inch
IS-D
±
9999999.99999 mm
±
999999.999999 inch
IS-E
±
999999.999999 mm
±
99999.9999999 inch
*3 For inch input/millimeter machines, the maximum specifiable
range of dimension words is as follows:
Increment system Maximum specifiable range
IS-A
±
39370.078 inch
IS-B
±
39370.0787 inch
IS-C
±
3937.00787 inch
IS-D
±
393.700787 inch
IS-E
±
39.3700787 inch
*4 The maximum value of addresses M, S, T, and B is 99999999.
Note that, however, values longer than the permissible number of
digits set in parameter No. 3030 to 3033 cannot be specified. The
values and uses for some codes are limited by parameter setting.
(For example, some M codes are not buffered.) For details, refer
to the parameter manual.
- Optional block skip
When a slash followed by a number (/n (n=1 to 9)) is specified at the
head of a block, and optional block skip signals BDT1 to BDT9 are
set to 1 during automatic operation, the information (/n to the end of
the block (EOB)) contained in the block for which /n corresponding to
signal BDTn is specified is ignored.
Example 1)
/2 N123 X100.0 Y200.0 ;
Example 2)
//3 N123 X100.0 Y200.0 ; → Incorrect
/1 /3 N123 X100.0 Y200.0 ; → Correct
B-63944EN/03 PROGRAMMING 13.PROGRAM CONFIGURATION
- 341 -
Input signal and program code
Input signal Start code to be ignored
BDT1 / or /1(NOTE)
BDT2 /2
BDT3 /3
BDT4 /4
BDT5 /5
BDT6 /6
BDT7 /7
BDT8 /8
BDT9 /9
NOTE
1 Number 1 for /1 can be omitted. However, when
two or more optional block skips are specified for
one block, number 1 for /1 cannot be omitted.
2 Depending on the machine tool, all optional block
skip signals (1 to 9) may not be usable. Refer to
manuals of the machine tool builder to find which
switches are usable.
The following shows the relationship between the timing at which
optional block skip signals BDT1 to BDT9 are set to 1 and the range
of information to be ignored.
1. When the signal BDTn is set to 1 before the CNC starts reading a
block that contains /n, the block is ignored.
BDTn "1"
"0"
Read by CNC → . . . ; /n N123 X100. Y200. ;N234 . . . .
This range of information is ignored.
2. When the signal BDTn is set to 1 while the CNC is reading a
block that contains /n, the block is not ignored.
BDTn "1"
"0"
Read by CNC → . . . ; /n N123 X100. Y200. ; N234 . . . .
This range of information is not ignored.
13.PROGRAM CONFIGURATION PROGRAMMING B-63944EN/03
- 342 -
3. When the signal BDTn is set to 0 while the CNC is reading a
block that contains /n, the block is ignored.
BDTn "1"
"0"
Read by CNC → . . . ; /n N123 X100. Y200.; N234 . . . .
This range of information is ignored.
4. Two or more optional block skips can be specified in one block.
When the signal corresponding to any of the specified skips is set
to 1, the block is ignored.
BDT3 "1"
"0"
Read by CNC → . . . ; /1 /3 /5 N123 X100. Y200. ; N234 . . . .
This range of information is ignored.
NOTE
1 This function is not used when a program is
registered in memory. A block containing / is
registered in memory regardless of the statuses of
optional block skip signals. When a program in
memory is also output regardless of the statuses of
optional block skip signals.
In addition, the optional block skip function is
enabled during a search for a sequence number.
2 Position of a slash
A slash (/) must be specified at the head of a block.
If a slash is placed elsewhere, the information from
the slash to immediately before the EOB code is
ignored.
3 TV and TH check
When the optional block skip signal is set to 1, TH
and TV checks are made for the skipped portions
in the same way as when the optional block skip
signal is set to 0.
B-63944EN/03 PROGRAMMING 13.PROGRAM CONFIGURATION
- 343 -
- Program end
The end of a program is indicated by programming one of the
following codes at the end of the program:
Table 13.2 (d) Code of a program end
Code Meaning usage
M02
M03 For main program
M99 For subprogram
If one of the program end codes is executed in program execution, the
CNC terminates the execution of the program, and the reset state is set.
When the subprogram end code is executed, control returns to the
program that called the subprogram.
CAUTION
A block containing an optional block skip code such
as /M02 ; , /M30 ; , or /M99 ; is not regarded as the
end of a program. (see "Optional block skip".)
13.PROGRAM CONFIGURATION PROGRAMMING B-63944EN/03
- 344 -
13.3 SUBPROGRAM (M98, M99)
If a program contains a fixed sequence or frequently repeated pattern,
such a sequence or pattern can be stored as a subprogram in memory
to simplify the program.
A subprogram can be called from the main program.
A called subprogram can also call another subprogram.
Format
- Subprogram configuration
One subprogram
Subprogram number or subprogram file name (or
the colon (:) optionally in the case of ISO)
Program end
M99 need not constitute a separate block as indicated below.
Example) X100.0Y100.0M99;
- Subprogram call
- When a subprogram with a 4-digit or shorter
program number is called
M98 Pxxxx xxxx ;
Subprogram number
Number of times the subprogram is called repeatedly
or
M98 Pxxxx Lxxxxxxxx ;
Number of times the subprogram is called repeatedly
Subprogram number
- When a subprogram with a 5-digit or longer
program number is called
M98 Pxxxxxxxx Lxxxxxxxx ;
Subprogram number
Number of times the subprogram is called repeatedly
- When a subprogram is called by file name
M98 <xxxx> Lxxxxxxxx ;
Subprogram file name
Number of times the subprogram is called repeatedly
Oxxxx ;
:
M99;
B-63944EN/03 PROGRAMMING 13.PROGRAM CONFIGURATION
- 345 -
- Called program and folders to be searched
The order in which folders are searched depends on the method of
calling a subprogram. Folders are searched in sequence and the
program found first is called. For details, see the "Managing
Programs" chapter.
NOTE
1 When calling a subprogram of a 4-digit or shorter
subprogram number repeatedly (P8 digit), make
the subprogram number 4 digits by prefixing it with
“0” if the subprogram number is shorter than 4
digits.
Example)
P100100: Call subprogram No. 100 ten times.
P50001: Call subprogram No. 1 five times.
2 If the number of times the subprogram is called
repeatedly is omitted when a subprogram with a
4-digit or shorter program number is called, the
subprogram is called just once.
In this case, it is not necessary to adjust the
subprogram number length to 4 digits as described
in Item 1 above.
3 When calling a subprogram of a 4-digit or shorter
program number repeatedly (P8 digit), do not
specify address L in the same block.
4 When calling a subprogram with a 5-digit or longer
program number, do not omit the specification of
the number of repeats.
5 When calling a subprogram by file name, be sure
to specify the file name immediately after M98.
13.PROGRAM CONFIGURATION PROGRAMMING B-63944EN/03
- 346 -
Explanation
When the main program calls a subprogram, it is regarded as a
one-level subprogram call. Thus, subprogram calls can be nested up to
ten levels as shown below.
O0001 ;
M98P0010 ;
M30 ;
Main program
O0090 ;
M99 ;
O0010 ;
M98P0020 ;
M99 ;
O0020 ;
M98P0030 ;
M99 ;
Subprogram
(One-level
nesting)
(Two-level
nesting)
(Nine-level
nesting)
Subprogram Subprogram
O0100 ;
M99 ;
(Ten-level
nesting)
Subprogram
M98P0100 ;
A single call command can repeatedly call a subprogram up to
99999999 times. For compatibility with automatic programming
systems, in the first block, Nxxxxxxxx can be used instead of a
subprogram number that follows O (or :). A sequence number after N
is registered as a subprogram number.
NOTE
1 The M98 and M99 code signal and strobe signal
are not output to the machine tool.
2 If the subprogram number specified by address P
cannot be found, an alarm PS0078 is output.
3 When an attempt is made to call a subprogram by
file name, but the specified file cannot be found,
alarm PS0310 is issued.
Example
- M98 P51002 ;
- X1000.0 M98 P1200 ;
- Execution sequence of subprograms called from a main program
A
subprogram can call another subprogram in the same way as a main
program calls a subprogram.
This command specifies "Call the subprogram (number 1002) five times in
succession." A subprogram call command (M98P_) can be specified in the
same block as a move command.
This example calls the subprogram (number 1200) after an X movement.
123
Main program
N0010 . . . ;
N0020 . . . ;
N0030 M98 P21010 ;
N0040 . . . ;
N0050 M98 P1010 ;
N0060 . . . ;
Subprogram
O1010 . . . ;
N1020 . . . ;
N1030 . . . ;
N1040 . . . ;
N1050 . . . ;
N1060 . . . M99 ;
B-63944EN/03 PROGRAMMING 13.PROGRAM CONFIGURATION
- 347 -
Special usage
- Specifying the sequence number for the return destination in the main program
If P is used to specify a sequence number when a subprogram is
terminated, control does not return to the block after the calling block,
but returns to the block with the sequence number specified by P.
Note, however, that P is ignored if the main program is operating in a
mode other than memory operation mode.
This method consumes a much longer time than the normal return
method to return to the main program.
Subprogram
O0010 . . . ;
N1020 . . . ;
N1030 . . . ;
N1040 . . . ;
N1050 . . . ;
N1060 . . . M99 P0060 ;
Main program
N0010 . . . ;
N0020 . . . ;
N0030 M98 P1010 ;
N0040 . . . ;
N0050 . . . ;
N0060 . . . ;
- Using M99 in the main program
If M99 is executed in a main program, control returns to the start of
the main program. For example, M99 can be executed by placing
/M99 ; at an appropriate location of the main program and setting the
optional block skip function to off when executing the main program.
When M99 is executed, control returns to the start of the main
program, then execution is repeated starting at the head of the main
program.
Execution is repeated while the optional block skip function is set to
off.
If the optional block skip function is set to on, the /M99 ; block is
skipped ; control is passed to the next block for continued execution.
If/M99Pn ; is specified, control returns not to the start of the main
program, but to sequence number n. In this case, a longer time is
required to return to sequence number n.
N0010 . . . ;
N0020 . . . ;
N0030 . . . ;
N0040 . . . ;
N0050 . . . ;
N0060 . . . M99 P0030 ;
N0070 . . . ;
N0080 M02 ;
/Optional block skip
ON
Optional block skip
OFF
13.PROGRAM CONFIGURATION PROGRAMMING B-63944EN/03
- 348 -
- Using a subprogram only
A subprogram can be executed just like a main program by searching
for the start of the subprogram with the MDI.
(See III-10.4 for information about search operation.)
In this case, if a block containing M99 is executed, control returns to
the start of the subprogram for repeated execution. If a block
containing M99Pn is executed, control returns to the block with
sequence number n in the subprogram for repeated execution. To
terminate this program, a block containing /M02 ; or /M30 ; must be
placed at an appropriate location, and the optional block switch must
be set to off ; this switch is to be set to on first.
N1010 . . . ;
N1020 . . . ;
N1030 . . . ;
N1040 . . . M02 ;
N1050 M99 P1020 ;
/Optional block skip ON
- Subprogram call with sequence number
Setting bit 0 (SQC) of parameter No. 6005 to 1 can call a specified
sequence number in the subprogram for execution.
In a subprogram call command, specify the letter Q followed by a
sequence number to be called after the letter P for specifying a
program number.
M98 Pxxxx Qxxxxx ;
Sequence number
Program number
This command causes program execution to start at the called
sequence number in the subprogram. If a repetition count is
specified, program execution is repeated from the specified sequence
number.
Main program
N0010…;
N0020…;
N0030 M98 P1010 Q1030 ;
N0040…;
N0050…;
N0060…;
Sub program
O1010…;
N1020…;
N1030…;
N1040…;
N1050…;
N1060…M99 ;
This function enables a sequence number in the same program to be
called for execution as shown below.
This method, however, requests the programmer to be aware of an
allowable call nesting level. If an attempt is made to exceed the
allowable nesting level, alarm PS0077 meaning “TOO MANY
SUB,MACRO NESTING” is issued.
B-63944EN/03 PROGRAMMING 13.PROGRAM CONFIGURATION
- 349 -
O0001 ;
N0010…;
N0020 M98 (P0001) Q0050 ;
N0030…;
N0040…;
N0050…;
N0060…;
N0070…M99;
For a call within the same program, specification of Pxxxx in a block
can be omitted when the block includes M98.
This function is usable only for subprogram calls by M98; it is
unusable for non-M98 calls, such as macro calls or external
subprogram calls based on M198.
PROGRAMMING B-63944EN/03
- 350 -
14. FUNCTIONS TO SIMPLIFY
PROGRAMMING
14 FUNCTIONS TO SIMPLIFY
PROGRAMMING
Chapter 14, "FUNCTIONS TO SIMPLIFY PROGRAMMING",
consists of the following sections:
14.1 FIGURE COPYING (G72.1, G72.2)......................................351
14.2 THREE-DIMENSIONAL COORDINATE SYSTEM
CONVERSION ......................................................................359
B-63944EN/03 PROGRAMMING
- 351 -
14.FUNCTIONS TO SIMPLIFY
PROGRAMMING
14.1 FIGURE COPYING (G72.1, G72.2)
Machining can be repeated after moving or rotating the figure using a
subprogram.
Format
- Rotational copying
Xp-Yp plane (specified by G17) :
G72.1 P_ L_ Xp_Yp_R_ ;
Zp-Xp plane (specified by G18) :
G72.1 P_ L_ Zp_Xp_R_ ;
Yp-Zp plane (specified by G19) :
G72.1 P_ L_ Yp_Zp_R _;
P :Subprogram number
L :Number of times the operation is repeated
Xp :Center of rotation on the Xp axis
(Xp : X-axis or an axis parallel to the X-axis)
Yp :Center of rotation on the Yp axis
(Yp: Y-axis or an axis parallel to the Y-axis)
Zp :Center of rotation on the Zp axis
(Zp: Z-axis or an axis parallel to the Z-axis)
R :Angular displacement
(A positive value indicates a counterclockwise angular
displacement. Specify an incremental value.)
Specify a plane selection command (G17, G18, or G19) to
select the plane on which the rotational copying is made.
- Linear copying
Xp-Yp plane (specified by G17) :
G72.2 P_ L_ I_ J_ ;
Zp-Xp plane (specified by G18) :
G72.2 P_ L_ K_ I_ ;
Yp-Zp plane (specified by G19) :
G72.2 P_ L_ J_ K_;
P :Subprogram number
L :Number of times the operation is repeated
I :Shift along the Xp axis
J :Shift along the Yp axis
K :Shift along the Zp axis
Specify a plane selection command (G17, G18, or G19) to
select the plane on which the linear copying is made.
PROGRAMMING B-63944EN/03
- 352 -
14. FUNCTIONS TO SIMPLIFY
PROGRAMMING
Explanation
- First block of the subprogram
Always specify a move command in the first block of a subprogram
that performs a rotational or linear copying. If the first block
contains only the program number such as O1234; and does not have a
move command, movement may stop at the start point of the figure
made by the n-th (n = 1, 2, 3, ...) copying.
Specify the first move command in the absolute mode.
(Example of an incorrect program)
O1234 ;
G00 G90 X100.0 Y200.0 ;
. . . . . ;
. . . . . ;
M99 ;
(Example of a correct program)
O1000 G00 G90 X100.0 Y200.0 ;
. . . . . ;
. . . . . ;
M99 ;
- Combination of rotational and linear copying
The linear copying command can be specified in a subprogram for a
rotational copying. Also, the rotational copying command can be
specified in a subprogram for a linear copying.
- Subprogram call
In a subprogram for rotational or linear copying, M98 for calling
another subprogram or G65 for calling a macro can be specified.
- Specifying the center of rotation
The center of rotation specified with G72.1 is processed as an absolute
position even in the incremental mode.
- Specifying address
In a block with G72.1, addresses other than P, L, Xp, Yp, Zp, or R are
ignored. The subprogram number (P), coordinates of the center of
rotation (Xp, Yp, Zp), and angular displacement (R) must be
specified.
In a block with G72.2, addresses other than P, L, I, J, or K are ignored.
The subprogram number (P) and shift (I, J, K) must be specified.
- Address P
If the subprogram number specified with P is not found, alarm PS0078
occurs. If P is not specified, alarm PS0076 occurs.
- Address L
If L is omitted, the repetition count is assumed to be 1 and the
subprogram is called only once.
B-63944EN/03 PROGRAMMING
- 353 -
14.FUNCTIONS TO SIMPLIFY
PROGRAMMING
- Increment in angular displacement or shift
In a block with G72.1, an increment in angular displacement is
specified with address R. The angular displacement of the figure made
by the n-th rotation is calculated as follows : R × (n - 1).
In a block with G72.2, an increment in shift is specified with
addresses I, J, and K. The shift of the figure made by the n-th
movement is calculated as follows : (Programmed shift) × (n - 1).
- Nesting level of a subprogram
If a subprogram is called by G72.1 or G72.2, the nesting level is
increased by one in the same manner as when M98 is specified.
- Block end position
The coordinates of a figure moved rotationally or linearly (block end
position) can be read from #5001 and subsequent system variables of
the custom macro of rotational or linear copying.
PROGRAMMING B-63944EN/03
- 354 -
14. FUNCTIONS TO SIMPLIFY
PROGRAMMING
- Disagreement between end point and start point
If the end point of the figure made by the n-th copy does not agree
with the start point of the figure to be made by the next (n + 1) copy,
the figure is moved from the end point to the start point, then copying
is started. (Generally, this disagreement occurs if an incorrect angular
displacement or shift is specified.)
Start point
End point of the first copy
Start point of the second copy
Y
70
P0
P1 P2
P3
P4 P5
P6 P7
X
30 20
Main program
O1000 ;
N10 G92 X-20.0 Y0 ;
N20 G00 G90 X0 Y0 ;
N30 G01 G17 G41 X20. Y0 D01 F10 ; (P0)
N40 Y20. ; (P1)
N50 X30. ; (P2)
N60 G72.2 P2000 L3 I90. J0 ;
Although a shift of 70 mm was
required, I90.0 was specified instead
of I70.0. Since an incorrect shift was
specified, the end point of the figure
made by the n-th copy disagrees
with the start point of the figure to be
made by the next (n + 1) copy.
Subprogram
O2000 G90 G01 X40. ; (P3)
N100 Y40. ; (P4)
N200 G01 X80. ; (P5)
N300 G01 Y20. ; (P6)
N400 X100. ; (P7)
N500 M99;
B-63944EN/03 PROGRAMMING
- 355 -
14.FUNCTIONS TO SIMPLIFY
PROGRAMMING
Limitation
- Specifying two or more commands to copy a figure
G72.1 cannot be specified more than once in a subprogram for making
a rotational copying (If this is attempted, alarm PS0160 will occur).
G72.2 cannot be specified more than once in a subprogram for making
a linear copying (If this is attempted, alarm PS0161 will occur).
- Commands that must not be specified
Within a program that performs a rotational or linear copying, the
following must not be specified:
• Command for changing the selected plane (G17 to G19)
• Command for specifying polar coordinates
• Reference position return command
• Coordinate system rotation, scaling, programmable mirror image
The command for rotational or linear copying can be specified after a
command for coordinate system rotation, scaling, or programmable
mirror image is executed.
- Modes that must not be selected
The figure cannot be copied during chamfering, corner rounding, or
tool offset.
- Unit system
The two axes of the plane for copying a figure must have an identical
unit system.
- Single block
Single-block stops are not performed in a block with G72.1 or G72.2.
- Specifying tool radius compensation and the workpiece coordinate system
In a subprogram for copying a figure, the G code for tool radius / tool
nose radius compensation or compensation amount (H or D code)
cannot be changed. G92 and G54 to G59 cannot be changed either.
Those codes must be specified before figure copying is started.
PROGRAMMING B-63944EN/03
- 356 -
14. FUNCTIONS TO SIMPLIFY
PROGRAMMING
Example
- Rotational copying
Start point
Main program
O1000 ;
N10 G92 X40.0 Y50.0 ;
N20 G00 G90 X_ Y_ ; (P0)
N30 G01 G17 G41 X_ Y_ D01 F10 ; (P1)
N40 G72.1 P2000 L3 X0 Y0 R120.0 ;
N50 G40 G01 X_ Y_ I_ J_ ; (P0)
N60 G00 X40.0 Y50.0 ;
N70 M30 ;
Sub program
O2000 G03 X_ Y_ R30.0 ; (P2)
N100 G01 X_ Y_ ; (P3)
N200 G03 X_ Y_ R10.0 ; (P4)
N300 G01 X_ Y_ ; (P5)
N400 G03 X_ Y_ R30.0 ; (P6)
N500 M99;
120°
Y
P3
P0
P1 X
P6
P5
P4
P2
B-63944EN/03 PROGRAMMING
- 357 -
14.FUNCTIONS TO SIMPLIFY
PROGRAMMING
- Rotational copying (spot boring)
Main program
O3000 ;
N10 G92 G17 X80.0 Y50.0 ; (P0)
N20 G72.1 P4000 L6 X0 Y0 R60.0 ;
N30 G80 G00 X80.0 Y50.0 ; (P0)
N40 M30 ;
Subprogram
O4000 N100 G90 G81 X_ Y_ R_ Z_ F_ ; (P1)
N200 M99 ;
Y
P1
P0
Start point
60°
X
- Linear copying
Main
p
ro
g
ram
O1000 ;
N10 G92 X-20.0 Y0 ;
N20 G00 G90 X0 Y0 ;
N30 G01 G17 G41 X20. Y0 D01 F10 ; (P0)
N40 Y20. ; (P1)
N50 X30. ; (P2)
N60 G72.2 P2000 L3 I70.0 J0 ;
N70 X_ Y_ ; (P8)
N80 X0 ;
N90 G00 G40 X-20.0 Y0 ;
N100 M30 ;
Subprogram
O2000 G90 G01 X_ ; (P3)
N100 Y_ ; (P4)
N200 G02 X_ I_ ; (P5)
N300 G01 Y_ ; (P6)
N400 X_ ; (P7)
N500 M99 ;
Start
point
P8
P0
P1
P2
P4
P3
70 70 70 X
P5
P7
Y
P6
PROGRAMMING B-63944EN/03
- 358 -
14. FUNCTIONS TO SIMPLIFY
PROGRAMMING
- Combination of rotational copying and linear copying (bolt hole circle)
Main program
O1000 ;
N10 G92 G17 X100.0 Y80.0 ; (P0)
N20 G72.1 P2000 X0 Y0 L8 R45.0 ;
N30 G80 G00 X100.0 Y80.0 ; (P0)
N40 M30 ;
Subprogram (rotational copy)
O2000 N100 G72.2 P3000 I0 J_ L3 ;
N200 M99 ;
Y
X
45°
P1
P0 Start point
Subprogram (linear copy)
O3000 N110 G90 G81 X_ Y_ R_ Z_ F_ ; (P1)
N210 M99 ;
B-63944EN/03 PROGRAMMING
- 359 -
14.FUNCTIONS TO SIMPLIFY
PROGRAMMING
14.2 THREE-DIMENSIONAL COORDINATE SYSTEM
CONVERSION
Coordinate system conversion about an axis can be carried out if the
center of rotation, direction of the axis of rotation, and angular
displacement are specified. This function is very useful in
three-dimensional machining by a die-sinking machine or similar
machine. For example, if a program specifying machining on the
XY plane is converted by the three-dimensional coordinate system
conversion function, the identical machining can be executed on a
desired plane in three-dimensional space.
• For milling machining
X
Y
Z
ZY
X
Three-dimensional coordinate system conversion
• For lathe cutting
X
X'
Z'
Z
Surface to be
machined
B
#3#2
#1 #4
Y
Z
Machinin
g
such as millin
g
, pocketin
g
, and drillin
g
is performed.
PROGRAMMING B-63944EN/03
- 360 -
14. FUNCTIONS TO SIMPLIFY
PROGRAMMING
Format
M
G68 XpX1 Ypy1 Zpz1 Ii1 Jj1 Kk1 Rα ; Starting three-dimensional coordinate system
: conversion
: Three-dimensional coordinate system conversion
mode
G69 ; Canceling three-dimensional coordinate system
conversion
Xp, Yp, Zp : Center of rotation (absolute coordinates) on the X, Y, and Z axis or parallel
axes
I, J, K : Direction of the axis of rotation
R : Angular displacement
T
G68.1 XpX1 Ypy1 Zpz1 Ii1 Jj1 Kk1 Rα ; Starting three-dimensional coordinate system
: conversion
: Three-dimensional coordinate system conversion
mode
G69.1 ; Canceling three-dimensional coordinate system
conversion
Xp, Yp, Zp : Center of rotation (absolute coordinates) on the X, Y, and Z axis or parallel
axes
I, J, K : Direction of the axis of rotation
R : Angular displacement
NOTE
The G code of this function is hereinafter described
using the format (G68/G69) for the machining center
system in this section.
Explanation
- Command for three-dimensional coordinate system conversion (program
coordinate system)
N1 G68 Xp x1 Yp y1 Zp z1 I i1 J j1 K k1 R α ;
N2 G68 Xp x2 Yp y2 Zp z2 I i2 J j2 K k2 R β ;
N3
:
Nn G69 ;
Three-dimensional coordinate system conversion can be executed
twice.
In the N1 block, specify the center, direction of the axis of rotation,
and angular displacement of the first rotation.
B-63944EN/03 PROGRAMMING
- 361 -
14.FUNCTIONS TO SIMPLIFY
PROGRAMMING
When this block is executed, the center of the original coordinate
system is shifted to (x1, y1, z1), then rotated around the vector (i1, j1,
k1) by angular displacement α. The new coordinate system is called
X'Y'Z'. In the N2 block, specify the center, direction of the axis of
rotation, and angular displacement of the second rotation. In the N2
block, specify coordinates and the angle with the coordinate system
formed after the N1 block in Xp, Yp, Zp, I, J, K, and R. When the N2
block is executed, the X'Y'Z' coordinate system is shifted to (x2, y2, z2),
then rotated around the vector (i2, j2, k2) by angular displacement β.
The newest coordinate system is called X''Y''Z''. In the subsequent N3
block, coordinates in the X''Y''Z'' coordinate system are specified with
Xp, Yp, and Zp. The X''Y''Z'' coordinate system is called the program
coordinate system.
If (Xp, Yp, Zp) is not specified in the N2 block, (Xp, Yp, Zp) in the
N1 block is assumed to be the center of the second rotation (the N1
and N2 blocks have a common center of rotation). If the coordinate
system is to be rotated only once, the N2 block need not be specified.
y
Example) G68 Xx0 Yy0 Zz0 I0 J0 K1 Rα ;
G68 I1 J0 K0 R
β
;
Z
Y
X
O (x0, y0, z0)
Z" Z'
Y"
Y'
α
P (x, y, z)
z
β
β
X, Y, Z : Workpiece coordinate system
X', Y', Z' : Coordinate system formed after the first conversion
X", Y", Z" : Coordinate system formed after the second conversion
α : Angular displacement of the first rotation
β : Angular displacement of the second rotation
O (x0, y0, z0) : Center of rotation
P (x, y, z) : Coordinates in the X''Y''Z'' coordinate system (program
coordinate system)
x
α
PROGRAMMING B-63944EN/03
- 362 -
14. FUNCTIONS TO SIMPLIFY
PROGRAMMING
- Format error
If one of the following format errors is detected, alarm PS5044 occurs:
1. When I, J, or K is not specified in a block with G68
(a parameter of coordinate system rotation is not specified)
2. When I, J, and K are all set to 0 in a block with G68
3. When R is not specified in a block with G68
- Center of rotation
Specify absolute coordinates with Xp, Yp, and Zp in the G68 block.
- Equation for three-dimensional coordinate system conversion
The following equation shows the general relationship between (x, y,
z) in the program coordinate system and (X, Y, Z) in the original
coordinate system (workpiece coordinate system).
()
+
=
1
1
1
1
z
y
x
z
y
x
M
Z
Y
X
When conversion is carried out twice, the relationship is expressed as
follows:
()() ()
+
+
=
1
1
1
2
2
2
121
z
y
x
z
y
x
M
z
y
x
MM
Z
Y
X
X, Y, Z : Coordinates in the original coordinate system
(workpiece coordinate system)
x, y, z : Programmed value
(coordinates in the program coordinate system)
x1, y1, z1 : Center of rotation of the first conversion
x2, y2, z2 : Center of rotation of the second conversion
(coordinates in the coordinate system formed after the
first conversion)
M1 : First conversion matrix
M2 : Second conversion matrix
M1 and M2 are conversion matrices determined by an angular
displacement and rotation axis. Generally, the matrices are expressed
as shown below.
−++−−−
−−−++−
+−−−−+
θθθθθ
θθθθθ
θθθθθ
cos)1(sin)cos1(sin)cos1(
sin)cos1(cos)1(sin)cos1(
sin)cos1(sin)cos1(cos)1(
2
3
2
3132231
132
2
2
2
2321
231321
2
1
2
1
nnnnnnnn
nnnnnnnn
nnnnnnnn
n1 : Cosine of the angle made by the rotation axis and X-axis i/p
n2 : Cosine of the angle made by the rotation axis and Y-axis j/p
n3 : Cosine of the angle made by the rotation axis and Z-axis k/p
θ : Angular displacement
Value p is obtained by the following:
222 kjip ++=
B-63944EN/03 PROGRAMMING
- 363 -
14.FUNCTIONS TO SIMPLIFY
PROGRAMMING
Conversion matrices for rotation on two-dimensional planes are
shown below:
(1) Coordinate system conversion on the XY plane
−
=
100
0cossin
0sincos
θθ
θθ
M
(2) Coordinate system conversion on the YZ plane
−=
θθ
θθ
cossin0
sincos0
001
M
(3) Coordinate system conversion on the ZX plane
−
=
θθ
θθ
cos0sin
010
sin0cos
M
- Three basic axes and their parallel axes
Three-dimensional coordinate system conversion can be applied to a
desired combination of three axes selected out of the basic three axes
(X, Y, Z) and their parallel axes. The three-dimensional coordinate
system subjected to three-dimensional coordinate system conversion is
determined by axis addresses specified in the G68 block. If Xp, Yp, or
Zp is not specified, X, Y, or Z of the basic three axes is assumed.
However, if the basic three axes are not specified in parameter 1022,
alarm PS0048 occurs.
In a single G68 block, both a basic axis and a parallel axis cannot be
specified.
If this is attempted, alarm PS0047 occurs.
(Example)
When U-axis, V-axis, and W-axis are parallel to the X-axis,
Y-axis, and Z-axis respectively
G68 X_ I_ J_ K_ R_ ; XYZ coordinate system
G68 U_V_ Z_ I_ J_ K_ R_ ; UVZ coordinate system
G68 W_ I_ J_ K_ R_ ; XYW coordinate system
- Specifying the second conversion
Three-dimensional coordinate system conversion can be executed
twice. The center of rotation of the second conversion must be
specified with the axis addresses specified for the first conversion. If
the axis addresses of the second conversion are different from the axis
addresses of the first conversion, the different axis addresses are
ignored. An attempt to execute three-dimensional coordinate system
conversion three or more times causes alarm PS5043.
PROGRAMMING B-63944EN/03
- 364 -
14. FUNCTIONS TO SIMPLIFY
PROGRAMMING
- Angular displacement R
A positive angular displacement R indicates a clockwise rotation
along the axis of rotation. Specify angular displacement R in 0.001
degrees within the range of -360000 to 360000.
To specify angular displacement R in 0.00001 degrees (one
hundred-thousandth), set bit 0 (FRD) of parameter No. 11630 to 1.
In this case, angular displacement R is specified within the range of
-36000000 to 36000000.
- G codes that can be specified
The following G codes can be specified in the three-dimensional
coordinate system conversion mode:
G00 Positioning
G01 Linear interpolation
G02 Circular interpolation (clockwise)
G03 Circular interpolation (counterclockwise)
G04 Dwell
G10 Data setting
G17 Plane selection (XY)
G18 Plane selection (ZX)
G19 Plane selection (YZ)
G28 Reference position return
G29 Movement from the reference position
G30 Second, third, or fourth reference position return
G53 Selecting the machine coordinate system
G65 Custom macro call
G66 Custom macro modal call
G67 Custom macro modal call cancel
G40 Canceling tool radius / tool nose radius compensation
G41 Tool radius / tool nose radius compensation to the left
G42 Tool radius / tool nose radius compensation to the right
G73, G74, G76, G80 to G89 Canned cycle for drilling
M
G43 Increasing tool length compensation
G44 Decreasing tool length compensation
G45 Increasing the tool offset
G46 Decreasing the tool offset
G47 Doubling the tool offset
G48 Halving the tool offset
G49 Canceling tool length compensation
G50.1 Canceling programmable mirror image
G51.1 Programmable mirror image
G90 Absolute programming
G91 Incremental programming
G94 Feed per minute
G95 Feed per revolution
G98 Canned cycle (return to the initial level)
G99 Canned cycle (return to the level of point R)
B-63944EN/03 PROGRAMMING
- 365 -
14.FUNCTIONS TO SIMPLIFY
PROGRAMMING
T
G90 Absolute programming (when G code system B or C is used.)
G91 Incremental programming (when G code system B or C is
used.)
G94 Feed per minute (when G code system B or C is used.)
G95 Feed per revolution(when G code system B or C is used.)
G98 Canned cycle (return to the initial level) (when G code system
B or C is used.)
G99 Canned cycle (return to the level of point R) (when G code
system B or C is used.)
- Rapid traverse rate in drilling of a canned cycle for drilling
In three-dimensional coordinate system conversion mode, rapid
traverse rate in drilling by a canned cycle for drilling equals the
cutting feedrate specified in parameter No. 5412. If the parameter is
set to 0, the rapid traverse rate equals the maximum cutting feedrate.
- Compensation functions
M
If tool length compensation, tool radius / tool nose radius
compensation, or tool offset is specified with three-dimensional
coordinate system conversion, compensation is performed first,
followed by three-dimensional coordinate system conversion.
T
If tool radius / tool nose radius compensation is specified with
three-dimensional coordinate system conversion, compensation is
performed first, followed by three-dimensional coordinate system
conversion.
- Relationship between three-dimensional and two-dimensional coordinate system
conversion
Three-dimensional and two-dimensional coordinate system conversion
use identical G codes (G68 and G69). A G code specified with I, J,
and K is processed as the command for three-dimensional coordinate
system conversion. A G code not specified with I, J, and K is
processed as the command for two-dimensional coordinate system
conversion.
- Custom macro system variables
Coordinates on the workpiece coordinate system are assigned to
system variables #5041 to #5048 (current position on each axis).
PROGRAMMING B-63944EN/03
- 366 -
14. FUNCTIONS TO SIMPLIFY
PROGRAMMING
- Reset
If a reset occurs during three-dimensional coordinate system
conversion mode, the mode is canceled and the continuous-state G
code is changed to G69.
Bit 2 (D3R) of parameter No. 5400 determines whether just the G69.1
code is used to cancel the three-dimensional coordinate system
conversion mode (G68.1). When this setting is selected, a CNC reset
by a reset operation or by an input signal from the PMC will not
cancel the three-dimensional coordinate system conversion mode.
- Absolute position display
The absolute coordinates based on the program or workpiece
coordinate system can be displayed in the three-dimensional
coordinate system conversion mode. Specify a desired coordinate
system in bit 6 (DAK) of parameter No. 3106.
- Three-dimensional rigid tapping
By specifying the rigid tapping command in three-dimensional
coordinate system conversion mode, tapping can be executed in the
direction of the angle programmed by the three-dimensional
coordinate system conversion command.
In three-dimensional coordinate system conversion mode, "Position
Error Z", displayed on the spindle adjustment screen, is taken from the
longitudinal tapping axis after three-dimensional conversion.
Positioning in three-dimensional coordinate system conversion mode
must be linear interpolation positioning (bit 1 (LRP) of parameter
No.1401 is set to 1).
Limitation
- Manual intervention
Three-dimensional coordinate system conversion does not affect the
degree of manual intervention or manual handle interrupt.
- Positioning in the machine coordinate system
Three-dimensional coordinate system conversion does not affect
positioning in the machine coordinate system (e.g. specified with G28,
G30, or G53).
- Specifying rapid traverse
Specify linear rapid traverse when three-dimensional coordinate
system conversion is executed. (Set bit 1 (LRP) of parameter No.1401
to 1.)
- Block with G68 or G69
In a block with G68 or G69, other G codes must not be specified.
G68 must be specified with I, J, and K.
- Position display and compensation
To display the absolute position when three-dimensional coordinate
system conversion is executed, set bits 4 to 7 (DRL, DRC, DAL, and
DAC) of parameters No. 3104 to 0.
B-63944EN/03 PROGRAMMING
- 367 -
14.FUNCTIONS TO SIMPLIFY
PROGRAMMING
- Mirror image
M
Programmable mirror image can be specified, but external mirror
image (mirror image by the mirror image signal or setting) cannot be
specified. Three-dimensional coordinate system conversion is carried
out after the programmable mirror image function is executed.
T
External mirror image (mirror image by the mirror image signal or
setting) cannot be specified.
- Three-dimensional coordinate system conversion and other continuous-state
commands
M
Canned cycles, G41, G42, or G51.1 must be nested between G68 and
G69.
(Example)
G68 X100. Y100. Z100. I0. J0. K1. R45. ;
:
G41 D01 ;
:
G40 ;
:
G69 ;
T
Canned cycles, G41 or G42 must be nested between G68.1 and G69.1.
(Example)
G68.1 X100. Y100. Z100. I0. J0. K1. R45. ;
:
G41 X_ Z_ I_ K_ ;
:
G40 ;
:
G69.1 ;
T
- Relationship between three-dimensional coordinate system conversion and tool
offset
When using a tool offset command, nest the tool offset command
within the three-dimensional coordinate system conversion mode.
(Example)
G68.1 X100. Y100. Z100. I0. J0. K1. R45. ;
:
T0101;
:
T0100;
:
G69.1 ;
PROGRAMMING B-63944EN/03
- 368 -
14. FUNCTIONS TO SIMPLIFY
PROGRAMMING
- PMC axis control
In the three-dimensional coordinate system conversion mode, PMC
axis control cannot be performed for the three axes related to the
conversion (alarm).
- Manual operation
When manual feeding is performed during a three-dimensional
coordinate system conversion, the tangent velocity in the coordinate
system after conversion (program coordinate system) equals the
lowest feedrate of those on the selected axes.
- Workpiece coordinate system
Avoid changing the workpiece coordinate system in the
three-dimensional coordinate system conversion mode.
- Manual reference position return
Avoid making a manual reference position return in the
three-dimensional coordinate system conversion mode.
- Cs contour axis
When specifying the Cs contour axis and rapid traverse at the same
time in the three-dimensional coordinate system conversion mode,
make a reference position return on the Cs contour axis in advance. If
a reference position return is made in the first rapid traverse after the
Cs contour axis is selected (bit 1 (NRF) of parameter No.3700 is set to
0), avoid specifying the reference position return command in the
three-dimensional coordinate system conversion mode.
B-63944EN/03 PROGRAMMING
- 369 -
14.FUNCTIONS TO SIMPLIFY
PROGRAMMING
Example
N1 G90 X0 Y0 Z0 ; Carries out positioning to zero
point H.
N2 G68 X10. Y0 Z0 I0 J1 K0 R30. ; Forms new coordinate system
X'Y'Z'.
N3 G68 X0 Y-10. Z0 I0 J0 K1 R-90. ; Forms other coordinate system
X''Y''Z''.
The origin agrees with (0, -10,
0) in coordinate system X'Y'Z.
N4 G90 X0 Y0 Z0 ; Carries out positioning to zero
point H'' on coordinate system
X''Y''Z''.
N5 X10. Y10. Z0 ; Carries out positioning to (10,
10, 0) on coordinate system
X''Y''Z''.
YY'
H
Z
N4
H'
X'
Y"
N5
Z"
Z'
H"
(10, 10, 0)
10
-10
30°
30°
X"
-90°
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 370 -
15 COMPENSATION FUNCTION
Chapter 15, "COMPENSATION FUNCTION", consists of the
following sections:
15.1 TOOL LENGTH COMPENSATION (G43, G44, G49) ........371
15.2 SCALING (G50, G51) ...........................................................379
15.3 PROGRAMMABLE MIRROR IMAGE (G50.1, G51.1) ......389
15.4 NORMAL DIRECTION CONTROL (G40.1,G41.1,G42.1) .391
15.5 WORKPIECE SETTING ERROR COMPENSATION.........397
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 371 -
15.1 TOOL LENGTH COMPENSATION (G43, G44, G49)
This function can be used by setting the difference between the tool
length assumed during programming and the actual tool length of the
tool used into the offset memory. It is possible to compensate the
difference without changing the program.
Specify the direction of offset with G43 or G44. Select a tool length
compensation value from the offset memory by entering the
corresponding address and number (H code).
To o l a s s um e d
during programming Actual tool
Specify this distance as
the value of tool length
compensation.
Fig. 15.1 (a) Tool length compensation
15.1.1 Overview
The following three methods of tool length compensation can be used,
depending on the axis along which tool length compensation can be
made.
- Tool length compensation A
Compensates for the difference in tool length along the basic Z-axis.
- Tool length compensation B
Compensates for the difference in tool length in the direction normal
to a selected plane.
- Tool length compensation C
Compensates for the difference in tool length along a specified axis.
Format
Type Format Description
Tool length compensation A G43 Z_ H_ ;
G44 Z_ H_ ;
Tool length compensation B
G17 G43 Z_ H_ ;
G17 G44 Z_ H_ ;
G18 G43 Y_ H_ ;
G18 G44 Y_ H_ ;
G19 G43 X_ H_ ;
G19 G44 X_ H_ ;
Tool length compensation C G43 α_H_ ;
G44 α_H_ ;
Tool length compensation cancel G49 ; or H0 ;
G43 : Positive offset
G44 : Negative offset
G17 : XY plane selection
G18 : ZX plane selection
G19 : YZ plane selection
α : Address of a specified axis
H : Address for specifying the
tool length compensation
value
X, Y, Z : Offset move command
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 372 -
Explanation
- Selection of tool length compensation
Select tool length compensation A, B, or C, by setting bits 0 (TLC)
and 1 (TLB) of parameter No.5001 .
Parameter No.5001
Bit 1 (TLB) Bit 0 (TLC) Type
0 0 Tool length compensation A
1 0 Tool length compensation B
0/1 1 Tool length compensation C
- Direction of the offset
When G43 is specified, the tool length compensation value (stored in
offset memory) specified with the H code is added to the coordinates
of the end position specified by a command in the program. When
G44 is specified, the same value is subtracted from the coordinates of
the end position. The resulting coordinates indicate the end position
after compensation, regardless of whether the absolute or incremental
mode is selected.
When the specification of an axis is omitted, a movement is made by
the tool length compensation value.
G43 and G44 are modal G codes. They are valid until another G code
belonging to the same group is used.
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 373 -
- Specification of the tool length compensation value
The tool length compensation value assigned to the number (offset
number) specified in the H code is selected from offset memory and
added to or subtracted from the moving command in the program.
Example
:
H1 ; The offset value of offset number 1 is
selected.
:
G43 Z_ ; Offset is applied according to the offset
value of offset number 1.
:
H2 ; Offset is applied according to the offset
value of offset number 2.
:
H0 ; Offset is applied according to the offset
value 0.
:
H3 ; Offset is applied according to the offset
value of offset number 3.
:
G49 ; Offset is canceled.
:
H4 ; The offset value of offset number 4 is
selected.
:
A tool length compensation value is to be set in the offset memory
corresponding to an offset number.
WARNING
When another offset number is specified, the tool
length compensation value just changes to a new
value. The new tool length compensation value
is not added to the old tool length compensation
value.
H1 : Tool length compensation value 20.0
H2 : Tool length compensation value 30.0
G90 G43 Z100.0 H1 ; Z will move to 120.0
G90 G43 Z100.0 H2 ; Z will move to 130.0
NOTE
The tool length compensation value corresponding
to offset No. 0, that is, H0 always means 0. It is
impossible to set any other tool length
compensation value to H0.
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 374 -
- Performing tool length compensation along two or more axes
Tool length compensation B can be executed along two or more axes
when the axes are specified in two or more blocks.
By setting bit 3 (TAL) of parameter No. 5001 to 1, tool length
compensation C can also can be executed along two or more axes
when the axes are specified in two or more blocks. If no axis is
specified in the same block, the alarm PS0027 is issued. If two or
more axes are specified in the same block, the alarm PS0336 is issued.
Example 1
When tool length compensation B is executed
along the X-axis and Y-axis
G19 G43 H_ ; Offset in X axis
G18 G43 H_ ; Offset in Y axis
Example 2
When tool length compensation C is executed
along the X-axis and Y-axis
G43 X_ H_ ; Offset in X axis
G43 Y_ H_ ; Offset in Y axis
Example 3
When an alarm is issued with tool length
compensation C
G43 X_ Y_ H_ ; An alarm (PS0336) occurs
- Tool length compensation cancel
To cancel tool length compensation, specify G49 or H0. After G49 or
H0 is specified, the system immediately cancels the offset mode.
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 375 -
NOTE
1 If offset is executed along two or more axes, offset
along all axes is canceled by specifying G49. If H0
is used to specify cancellation, offset along only the
axis normal to a selected plane is canceled in the
case of tool length compensation B, or offset along
only the last axis specified by G43 or G44 is
canceled in the case of tool length compensation C.
2 If offset is executed along three or more axes, and
offset along all axes is canceled using G49, the
alarm PS0015 (TOO MANY SIMULTANEOUS
AXES) may be issued. By using H0 together, for
example, cancel offset so that the number of
simultaneously controlled axes (the number of axes
along which movements are made simultaneously)
does not exceed the allowable range of the system.
3 If tool length compensation and three-dimensional
coordinate system conversion are canceled by a
reset with three-dimensional coordinate system
conversion performed during tool length
compensation, the direction of tool length
compensation vector cancellation becomes
incorrect. By setting bit 6 (LVK) of parameter No.
5003 to 1 and setting bit 2 (D3R) of parameter No.
5400 to 1, ensure that the tool length compensation
vector and three-dimensional coordinate system
conversion are not canceled by a reset.
Example)
G43 H1 ;
G68 X_ Y_ Z_ I_ J_ K_ R_ ;
:
: Ensure that tool length compensation and three-dimensional
: coordinate conversion are not canceled by a reset in this range.
G69 ;
G49 ;
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 376 -
Example
A
ctual position
Programmed
position
Offset value
=4mm
#1
20
30
30
120
#3
#2
+Y
+X
30 50 +Z
3
35
30
18 22
8
Tool length compensation (in boring holes #1, #2, and #3)
(
1
)
(2)
(3)
(4)
(5)
(6)
(7) (8)
(9)
(13)
(10)
(11)
(12)
Program
H1=-4.0 (Tool length compensation value)
N1 G91 G00 X120.0 Y80.0 ;........................................................... (1)
N2 G43 Z-32.0 H1 ; ....................................................................... (2)
N3 G01 Z-21.0 F1000 ; ................................................................. (3)
N4 G04 P2000 ;............................................................................... (4)
N5 G00 Z21.0 ;................................................................................ (5)
N6 X30.0 Y-50.0 ;........................................................................... (6)
N7 G01 Z-41.0 ; .............................................................................. (7)
N8 G00 Z41.0 ;................................................................................ (8)
N9 X50.0 Y30.0 ; ............................................................................ (9)
N10 G01 Z-25.0 ; ............................................................................ (10)
N11 G04 P2000 ; ........................................................................... (11)
N12 G00 Z57.0 H0 ; ...................................................................... (12)
N13 X-200.0 Y-60.0 ;...................................................................... (13)
N14 M2 ;
Notes
- Command for setting a workpiece coordinate system in the tool length
compensation mode
Executing a workpiece coordinate system setting G code command
(G92 or, for G code system A in the lathe system, G50) presets a
coordinate system in such a way that the specified position will be a
pre-compensation position.
However, this G code cannot be used together with a block where tool
length compensation vectors vary. For details, see “Notes” in
Subsection 7.2.1, “Setting a Workpiece Coordinate System.”
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 377 -
15.1.2 G53, G28, G30, and G30.1 Commands in Tool Length
Compensation Mode
This section describes the tool length compensation cancellation and
restoration performed when G53, G28, G30, or G31 is specified in
tool length compensation mode. Also described is the timing of tool
length compensation.
Explanation
- Tool length compensation vector cancellation
When G53, G28, G30, or G30.1 is specified in tool length
compensation mode, tool length compensation vectors are canceled as
described below. However, the previously specified modal G code
remains displayed; modal code display is not switched to G49.
(1) When G53 is specified
Command Specified axis Operation
Tool length compensation
axis
Canceled upon movement
being performed
G53 IP_ Other than tool length
compensation axis Not canceled
Tool length compensation
axis
Canceled upon movement
being performed
G49 G53 IP_Other than tool length
compensation axis Canceled
(IP_ : Dimension word)
CAUTION
If tool length compensation is applied along
multiple axes, the offset vector along the axis
specified by G53 is canceled.
(2) When G28, G30, or G30.1 is specified
Command Specified axis Operation
Tool length compensation
axis
Not canceled at an
intermediate point.
Canceled at the reference
position.
G28 IP_ Other than tool length
compensation axis
Not canceled at an
intermediate point.
Canceled at the reference
position.
Tool length compensation
axis
Canceled when a movement is
made to an intermediate point.
G49 G28 IP_Other than tool length
compensation axis
Canceled when a movement is
made to an intermediate point.
(IP_ : Dimension word)
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 378 -
CAUTION
If tool length compensation is applied along
multiple axes, the offset vector along the axis on
which a reference position return operation has
been performed is canceled.
- Tool length compensation vector restoration
Tool length compensation vectors, canceled by specifying G53, G28,
G30, or G30.1 in tool length compensation mode, are restored as
described below.
Type Parameter EVO
(No.5001#6) Restoration condition
0 The H command or G43 (G44) is
specified.
A/B
1 Restored by the next buffered block.
C The H command or G43 (G44)IP_ is
specified.
(IP_ : Dimension word)
CAUTION
If a tool length compensation vector is restored
only with H_, G43, or G44 when tool length
compensation is applied along multiple axes, the
tool length compensation vector along only the
axis normal to a selected plane is restored in the
case of tool length compensation B, or the tool
length compensation vector along only the last
axis for which tool length compensation is
specified is restored in the case of tool length
compensation C. The tool length compensation
vector along any other axes is not restored.
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 379 -
15.2 SCALING (G50, G51)
Overview
A programmed figure can be magnified or reduced (scaling).
Two types of scaling are available, one in which the same
magnification rate is applied to each axis and the other in which
different magnification rates are applied to different axes.
The magnification rate can be specified in the program.
Unless specified in the program, the magnification rate specified in the
parameter is applied.
Y
X
P4
P4’
P1
P1’
P3’
P2’
P2
P3
P0
P0 : Scaling center
P1 to P4: Programmed figure
P1’ to P4’ : Scaled figure
0
Fig. 15.2 (a) Scaling
Format
Scaling up or down along all axes
at the same rate of magnification
(When parameter XSC (No. 5400#6) = 0)
Format Meaning of command
G51 IP_P_ ; Scaling start
Scaling is effective.
(Scaling mode)
G50 ; Scaling cancel
IP_ : Absolute command for
center coordinate value
of scaling
P_ : Scaling magnification
Scaling up or down along each axes at
a different rate of magnification (mirror image)
(When parameter XSC (No. 5400#6) = 1)
Format Meaning of command
G51 IP_I_J_K_; Scaling start
Scaling is effective.
(Scaling mode)
G50 ; Scaling cancel
IP_ : Absolute command for
center coordinate value
of scaling
I_J_K_ : Scaling magnification for
basic 3 axes (X, Y, and Z
axes) respectively
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 380 -
T
NOTE
This function is available when the G-code system
B or C is set.
CAUTION
1 Specify G51 in a separate block.
2 After the figure is enlarged or reduced, specify G50
to cancel the scaling mode.
NOTE
1 Entering electronic calculator decimal point input
mode (bit 0 (DPI) of parameter No. 3401 = 1) does
not cause the units of the magnification rates P, I, J,
and K to change.
2 Setting the least input increment equal to 10 times
the least command increment (bit 7 (IPR) of
parameter No. 1004 = 1) does not cause the units
of the magnification rates P, I, J, and K to change.
3 An attempt to specify 0 as a magnification rate
causes alarm PS0142 to occur in a G51 block.
Explanation
- Axis for which scaling is to be enabled
For the axis for which scaling is to be enabled, set bit 0 (SCL) of
parameter No. 5401 to 1.
- Minimum unit of scaling magnification
Least input increment of scaling magnification is: 0.001 or 0.00001.
It is 0.00001 (one hundred thousandth) if bit 7 (SCR) of parameter No.
5400 is 0 and 0.001 if it is 1.
- Scaling center
Even in incremental command (G91) mode, the scaling center
coordinates IP_ specified in the G51 block are assumed those of an
absolute position.
If the scaling center coordinates are omitted, the position assumed
when G51 is specified is assumed the scaling center.
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 381 -
CAUTION
With the move command subsequent to the G51
block, execute an absolute (G90 mode) position
command.
If no absolute position command is executed after
the G51 block, the position assumed when G51 is
specified is assumed the scaling center; once an
absolute position command is executed, the scaling
center assumes the coordinates specified in the
G51 block, after that block.
- Scaling along each axis at the same rate of magnification
Set bit 6 (XSC) of parameter No. 5400 to 0.
If the scaling magnification P is not specified, the magnification set in
parameter No. 5411 is used.
Decimal point input is not accepted as the magnification P. If decimal
point input is made, alarm PS0007 will occur.
A negative value cannot be specified as the magnification P. If a
negative value is specified, alarm PS0006 will occur.
The allowable magnification range is from 0.00001 to 9999.99999.
- Scaling of each axis, programmable mirror image (negative magnification)
Each axis can be scaled by different magnifications. Also when a
negative magnification is specified, a mirror image is applied. The
axis subject to the mirror image is the one that contains the scaling
center.
Set bit 6 (XSC) of parameter No. 5400to 1 to validate each axis
scaling (mirror image).
Using I, J, and K, specify the scaling magnifications for the basic 3
axes (X to Z axes). Use parameter No. 1022 to specify which axes to
use as the basic 3 axes. For those of the X to Z axes for which I, J,
and K are not specified and for axes other than the basic 3 axes, the
magnification set with parameter No. 5421 is used.
A value other than 0 must be set to parameter No. 5421.
Decimal point programming can not be used to specify the rate of
magnification (I, J, K).
Magnification can be set within the range of ±0.00001 to
±9999.99999.
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 382 -
Y axis
X axis
b
a
d
a/b : Scaling magnification of X axis
c/d : Scaling magnification of Y axis
o : Scaling center
Programmed figure
Scaled figure
o
c
Fig. 15.2 (b) Scaling of each axis
CAUTION
Specifying the following commands at the same
time causes them to be executed in the order
indicated below:
<1> Programmable mirror image (G51.1)
<2> Scaling (G51) (including a mirror image with a
negative magnification)
<3> Mirror image due to the external switch of the
CNC or the settings of the CNC
In this case, the programmable mirror image is
effective to the scaling center and magnification as
well.
To specify G51.1 and G51 at the same time,
specify them in this order; to cancel them, specify
them in the reverse order.
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 383 -
- Scaling of circular interpolation
Even if different magnifications are applied to each axis in circular
interpolation, the tool will not trace an ellipse.
G90 G00 X0.0 Y100.0 Z0.0;
G51 X0.0 Y0.0 Z0.0 I2000 J1000;
(A magnification of 2 is applied to the X-component and a
magnification of 1 is applied to the Y-component.)
G02 X100.0 Y0.0 I0 J–100.0 F500;
Above commands are equivalent to the following command:
G90 G00 X0.0 Y100.0 Z0.0;
G02 X200.0 Y0.0 I0 J–100.0 F500;
(Because the end point is not on an arc, spiral interpolation is
assumed.)
(0,0) (100.0) (200.0)
Y
X
Scaled shape
Fig. 15.2 (c) Scaling for circular interpolation1
Even for an R-specified arc, scaling is applied to each of I, J, and K
after the radius value (R) is converted into a vector in the center
direction of each axis.
If, therefore, the above G02 block contains the following R-specified
arc, the operation will be same as that in which I and J are specified.
G02 X100.0 Y0.0 R100.0 F500 ;
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 384 -
- Scaling and coordinate system rotation
If both scaling and coordinate system rotation are specified at the
same time, scaling is performed first, followed by coordinate system
rotation. In this case, scaling is effective to the rotation center as
well.
To specify both of them, specify scaling first and then coordinate
system rotation. To cancel them, specify them in the reverse order.
Example
Main program
O1
G90 G00 X20.0 Y10.0 ;
M98 P1000 ;
G51 X20.0 Y10.0 I3000 J2000 ; (x 3 in the X direction and x 2
in the Y direction)
M98 P1000 ;
G17 G68 X35.0 Y20.0 R30. ;
M98 P1000 ;
G69 ;
G50 ;
M30 ;
Subprogram
O1000 ;
G01 X20.0 Y10.0 F500 ;
G01 X50.0 ;
G01 Y30.0 ;
G01 X20.0 ;
G01 Y10.0 ;
M99 ;
Y
X
Scaling center
Original program
Shape after
coordinate system
rotation Scaled shape
Rotation center of
coordinate system
after scaling
Rotation center
of coordinate
system before
scalin
g
Fig. 15.2 (d) Scaling and coordinate system rotation
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 385 -
- Scaling and optional chamfering/corner R
Chamfering
Scaling
x 2 in the X direction
x 1 in the Y direction
Corner R
If different magnifications are applied to the individual axes, corner R results in
a spiral, not an arc, because scaling is applied to the end point and radius of
the arc.
Scaling
x 2 in the X direction
x 1 in the Y direction
Fig. 15.2 (e) Scaling and optional chamfering/corner R
Limitation
- Tool compensation
This scaling is not applicable to tool radius ⋅ tool nose radius
compensation values, tool length compensation values, and tool offset
values (Fig. 15.2 (f) ).
Cutter compensation values are not scaled.
Programmed figure
Scaled figure
Fig. 15.2 (f) Scaling during cutter compensation
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 386 -
- Invalid scaling
M
Scaling is not applied to the travel distance during canned cycle
shown below.
• Cut-in value Q and retraction value d of peck drilling cycle (G83,
G73).
• Fine boring cycle (G76)
• Shift value Q of X and Y axes in back boring cycle (G87).
In manual operation, the travel distance cannot be increased or
decreased using the scaling.
T
This function is available to G code systems B and C only; it is not
available to G code system A.
During scaling, the following functions cannot be used. If any of
them is specified, alarm PS0300 will occur.
• Finishing cycle (G70, G72)
• Outer surface rough cutting cycle (G71, G73)
• End rough cutting cycle (G72, G74)
• Closed loop cutting cycle (G73, G75)
• End cutting off cycle (G74, G76)
• Outer/inner surface cutting off cycle (G75, G77)
• Multiple threading cycle (G76, G78)
• Traverse grinding cycle (for grinding machines) (G71, G72)
• Traverse direct constant-size grinding cycle (for grinding
machines) (G72, G73)
• Oscillation grinding cycle (for grinding machines) (G73, G74)
• Oscillation direct constant-size grinding cycle (for grinding
machines) (G74, G75)
• Face drilling cycle (G83, G83)
• Face tapping cycle (G84, G84)
• Face boring cycle (G85, G85)
• Side drilling cycle (G87, G87)
• Side tapping cycle (G88, G88)
• Side boring cycle (G89, G89)
• Outer/inner surface turning cycle (G77, G20)
• Threading cycle (G78, G21)
• End turning cycle (G79, G24)
(The G code in system B is given first, followed by that of system C.)
In manual operation, the travel distance cannot be increased or
decreased using the scaling.
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 387 -
CAUTION
1 If a parameter setting value is employed as a
scaling magnification without specifying P, the
setting value at G51 command time is employed as
the scaling magnification, and a change of this
value, if any, is not effective.
2 Before specifying the G code for reference position
return (G27, G28, G29, G30, etc.) or coordinate
system setting (G52 to G59, G92, etc.), cancel the
scaling mode.
3 If scaling results are rounded by counting fractions
of 5 and over as a unit and disregarding the rest,
the move amount may become zero. In this case,
the block is regarded as a no movement block, and
therefore, it may affect the tool movement by cutter
compensation. See the description of cutter
compensation.
4 Refrain from scaling on a rotation axis for which the
rollover function is enabled. Otherwise, the tool
may rotate in a short-cut manner, possibly resulting
in unexpected movement.
NOTE
1 The position display represents the coordinate
value after scaling.
2 When a mirror image was applied to one axis of the
specified plane, the following results:
(1) Circular command
......................... Direction of rotation is reversed.
(2) Tool radius ⋅ tool nose radius compensation
................................ Offset direction is reversed.
(3) Coordinate system rotation
................................. Rotation angle is reversed.
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 388 -
Example
Sample program of a scaling in each axis
O1;
G51 X20.0 Y10.0 I750 J250; (× 0.75 in the X direction, × 0.25 in
the Y direction)
G00 G90 X60.0 Y50.0;
G01 X120.0 F100;
G01 Y90;
G01 X60;
G01 Y50;
G50;
M30;
Y axis
X axis
100
75
Programmed figure
Scaled figure
Scaling center
80
20
90
10
20 95 120
30
(60,50)
Fig. 15.2 (g) Program example of scaling in each axis
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 389 -
15.3 PROGRAMMABLE MIRROR IMAGE (G50.1, G51.1)
A mirror image of a programmed command can be produced with
respect to a programmed axis of symmetry (Fig. 15.3 (a)).
Y
100
60
50
50 X
60
100
(1)
(2)
(3) (4)
(1) Original image of a programmed command
(2) Image symmetrical about a line parallel to the Y-axis and crossing the
X-axis at 50
(3) Image symmetrical about point (50, 50)
(4) Image symmetrical about a line parallel to the X-axis and crossing the
Y-axis at 50
A
xis of symmetry (X=50)
A
xis of symmetry
(Y=50)
40
0
40
0
Fig. 15.3 (a) Programmable mirror image
Format
G51.1 IP_ ; Setting a programmable image
: A mirror image of a command specified in
: these blocks is produced with respect to
: the axis of symmetry specified by G51.1
: IP_;.
G50.1 IP_ ; Canceling a programmable mirror image
IP_ : Point (position) and axis of symmetry for producing a
mirror image when specified with G51.1.
Axis of symmetry for producing a mirror image when
specified with G50.1. Point of symmetry is not
specified.
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 390 -
Explanation
- Mirror image by setting
If the programmable mirror image function is specified when the
command for producing a mirror image is also selected by a CNC
external switch or CNC setting (see III-4.5), the programmable mirror
image function is executed first.
- Mirror image on a single axis in a specified plane
Applying a mirror image to one of the axes on a specified plane
changes the following commands as follows :
Command Explanation
Circular command G02 and G03 are interchanged.
Tool radius ⋅ tool nose radius
compensation G41 and G42 are interchanged.
Coordinate system rotation CW and CCW (directions of rotation)
are interchanged.
Limitation
- Scaling and coordinate system rotation
Processing proceeds from program mirror image to scaling and
coordinate system rotation in the stated order. The commands should
be specified in this order, and, for cancellation, in the reverse order.
Do not specify G50.1 or G51.1 during scaling or coordinate system
rotation mode.
- Commands related to reference position return and coordinate system
In programmable mirror image mode, G codes related to reference
position return (G27, G28, G29, G30, etc.) and those for changing the
coordinate system (G52 to G59, G92, etc.) must not be specified. If
any of these G codes is necessary, specify it only after canceling the
programmable mirror image mode.
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 391 -
15.4 NORMAL DIRECTION CONTROL (G40.1,G41.1,G42.1)
Overview
When a tool with a rotation axis (C-axis) is moved in the XY plane
during cutting, the normal direction control function can control the
tool so that the C-axis is always perpendicular to the tool path (Fig.
15.4 (a)).
Tool
Tool
Programmed tool path
Normal direction (in
which the tool moves)
C-axis
C-axis
Fig. 15.4 (a) Sample Movement of the tool
Format
G41.1 ; Normal direction control, left
G42.1 ; Normal direction control, right
G40.1 ; Cancel normal direction control
The normal direction control, left (G41.1) command is
used when the workpiece is on the right side of the tool as
viewed while you are looking into the tool’s way.
Once either G41.1 or G42.1 is issued, normal direction
control is enabled (normal direction control mode).
Issuing G40.1 cancels the normal direction control mode.
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 392 -
Center of the arc
Programmed tool path
Tool center path Tool center path
Programmed tool path
Fig. 15.4 (b) Normal direction control, left (G41.1) Fig. 15.4 (c) Normal direction control, right (G42.1)
Explanation
- Angle of the C axis
When viewed from the center of rotation around the C-axis, the
angular displacement about the C-axis is determined as shown in Fig.
15.4 (d). The positive side of the X-axis is assumed to be 0, the
positive side of the Y-axis is 90°, the negative side of the X-axis is
180°, and the negative side of the Y-axis is 270°.
Center of rotation
+Y
180°+X
270°
0°
90°
Fig. 15.4 (d) Angle of the C axis
- Normal direction control of the C axis
When the cancel mode is switched to the normal direction control
mode, the C-axis becomes perpendicular to the tool path at the
beginning of the block containing G41.1 or G42.1.
In the interface between blocks in the normal direction control mode,
a command to move the tool is automatically inserted so that the
C-axis becomes perpendicular to the tool path at the beginning of each
block. The tool is first oriented so that the C-axis becomes
perpendicular to the tool path specified by the move command, then it
is moved along the X- and Y axes.
In the cutter compensation mode, the tool is oriented so that the C-axis
becomes perpendicular to the tool path created after compensation.
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 393 -
In single-block operation, the tool is not stopped between a command
for rotation of the tool and a command for movement along the X- and
Y-axes. A single-block stop always occurs after the tool is moved
along the X- and Y-axes.
S
N1
N2
S
N3
S
Programmed tool path
S : Single block stop point
Tool center path
S
S
Fig. 15.4 (e) Point at which a single-block stop occurs in the normal
direction control mode
Before circular interpolation is started, the C-axis is rotated so that the
C-axis becomes normal to the arc at the start point. During circular
interpolation, the tool is controlled so that the C-axis is always
perpendicular to the tool path determined by circular interpolation.
Center of the arc
Programmed tool path
Tool center path
The tool is controlled so that the C-axis
is always normal to the tool path
determined by circular interpolation.
A
rotation command is inserted so
that the C-axis becomes normal to
the arc at the start point.
Fig. 15.4 (f) Normal direction control of the circular interpolation
NOTE
During normal direction control, the C axis always
rotates through an angle less than 180 deg. I.e., it
rotates in whichever direction provides the shorter
route.
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 394 -
- C axis feedrate
Movement of the tool inserted at the beginning of each block is
executed at the feedrate set in parameter 5481. If dry run mode is on at
that time, the dry run feedrate is applied. If the tool is to be moved
along the X-and Y-axes in rapid traverse (G00) mode, the rapid
traverse feedrate is applied.
The feedrate of the C axis during circular interpolation is defined by
the following formula.
Amount of movement of the C axis (deg)
F × Length of arc (mm or inch) (deg/min)
F : Feedrate (mm/min or inch/min) specified by the corresponding
block of the arc
Amount of movement of the C axis :
The difference in angles at the beginning and the end of the
block.
NOTE
If the feedrate of the C axis exceeds the maximum
cutting speed of the C axis specified to parameter
No. 1430, the feedrate of each of the other axes is
clamped to keep the feedrate of the C axis below
the maximum cutting speed of the C axis.
- Normal direction control axis
A C-axis to which normal-direction control is applied can be assigned
to any axis with parameter No. 5480.
- Angle for which figure insertion is ignored
When the rotation angle to be inserted, calculated by normal-direction
control, is smaller than the value set with parameter No. 5482, the
corresponding rotation block is not inserted for the axis to which
normal-direction control is applied. This ignored rotation angle is
added to the next rotation angle to be inserted, the total angle being
subject to the same check at the next block.
If an angle of 360 degrees or more is specified, the corresponding
rotation block is not inserted.
If an angle of 180 degrees or more is specified in a block other than
that for circular interpolation with a C-axis rotation angle of 180
degrees or more, the corresponding rotation block is not inserted.
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 395 -
- Movement for which arc insertion is ignored
Specify the maximum distance for which machining is performed with
the same normal direction as that of the preceding block.
• Linear movement
When distance N2, shown below, is smaller than the set value,
machining for block N2 is performed using the same direction as
that for block N1.
N1
N2
N3
Tool center path
Distance
Programmed tool path
• Circular movement
When the diameter of block N2, shown below, is smaller than the
set value, machining for block N2 is performed using the same
normal direction as that for block N1. And control as
compensation along the circular arc is not performed.
N1
N2
N3
Tool center path
Programmed tool path
Diameter
NOTE
1 Do not specify any command to the C axis during
normal direction control. Any command specified at
this time is ignored.
2 Before processing starts, it is necessary to
correlate the workpiece coordinate of the C axis
with the actual position of the C axis on the
machine using the coordinate system setting (G92)
or the like.
3 The helical cutting option is required to use this
function. Helical cutting cannot be specified in the
normal direction control mode.
4 Normal direction control cannot be performed by
the G53 move command.
5 The C-axis must be a rotation axis.
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 396 -
T
NOTE
1 In the normal direction control mode, the following
commands cannot be issued. An attempt to issue
any of them results in alarm PS1471 being raised.
- Plane selection command (G17, G18, G19)
- Automatic reference position return(G28)
- 2nd/3rd/4th reference position return(G30)
- Move from the reference position (G29)
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 397 -
15.5 WORKPIECE SETTING ERROR COMPENSATION
When a workpiece is placed on the machine, the workpiece is not
always placed at an ideal position.
With this function, a displaced workpiece can be machined according
to the program.
This function can compensate for a workpiece setting error on a
rotation axis used with a function involving rotation axis operation
such as a function for tool center point control, function for
3-dimensional cutter compensation, and a tilted working plane
command. So, a workpiece can be machined according to the
program even during tool center point control, 3-dimensional cutter
compensation, and tilted working plane command.
Workpiece setting error
Rotary tool
The coordinates system and the tool automatically
rotate in accordance with the Workpiece setting error.
Workpiece
Fig. 15.5 (a) Outline of workpiece setting error
Format
G54.4 Pn ; Start workpiece setting error compensation
:
:
G54.4 P0 ; Cancel workpiece setting error compensation
Pn : Workpiece setting error specification code
n : 1 to 7
A start block and cancellation block for workpiece setting error
compensation suppress buffering.
Workpiece setting error compensation mode
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 398 -
Explanation
- Workpiece setting error
A workpiece setting error is defined by the following eight variables:
• X direction error ∆x
• Y direction error ∆y
• Z direction error ∆z
• Rotation direction error ∆a (rotation error on the X-axis in
degrees)
• Rotation direction error ∆b (rotation error on the Y-axis in
degrees)
• Rotation direction error ∆c (rotation error on the Z-axis in
degrees)
• Table rotation axis position 1
• Table rotation axis position 2
[About ∆x, ∆y, and ∆z]
∆x, ∆y, and ∆z represent the coordinate values of the origin of the
workpiece coordinate system (X'Y'Z' in the figure below, which is
hereinafter referred to as the "workpiece setting coordinate system")
based on a displaced workpiece, as viewed from the original
workpiece coordinate system (XYZ in the figure below).
Coordinate system X'Y'Z'
(workpiece setting coordinate
system) based on the
displaced workpiece
X'
Y'
X
Y
Workpiece coordinate
system XYZ
∆
x
∆
y
Workpiece
Correct workpiece position Displace workpiece
-
∆
c degrees
Fig. 15.5 (b) Errors in X, Y, and Z directions
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 399 -
[About ∆a, ∆b, and ∆c]
∆a, ∆b, and ∆c are defined as described below.
The workpiece coordinate system obtained by rotating a workpiece
coordinate system about the X-axis by angle ∆a, about the Y-axis by
angle ∆b, and about the Z-axis by angle ∆c then shifting that
workpiece coordinate system by (∆x, ∆y, ∆z) from the origin of that
workpiece coordinate system is supposed to match the "workpiece
setting coordinate system".
(Note: In determination of positive/negative rotation, clockwise
rotation is defined to be positive rotation.)
X (= X')
Z
Y
Z’
Y’
∆
a
X
Z
Y
Z’
Y’
∆
b
X'
X
Z
Y
Z’
Y’
∆
c
X'
X
Z
Y
Z’ Y’
X'
(
∆
x,
∆
y, ∆z )
The workpiece coordinate
system (X,Y,Z) is rotated
about the X-axis by ∆a.
Further rotated about the
Y-axis by ∆b.
Further rotated about the
Z-axis by ∆c.
Workpiece setting
coordinate system
Fig. 15.5 (c) Errors in rotation directions
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 400 -
The example of Fig. 15.5 (b) assumes that ∆a = ∆b = 0 and ∆c
represents a nonzero value.
[About table rotation axis position 1 and table rotation axis position 2]
The table rotation axis position means the machine coordinate on the
table rotation axis of a 5-axis machine with a table rotation axis
(machine of table rotation type or composite type) when a workpiece
setting error (displacement from the correct workpiece position to the
actual workpiece position) is measured.
When two table rotation axes are used, set table rotation axis position
1 for the master rotation axis, and set table rotation axis position 2 for
the slave rotation axis. (As for master rotation axis and slave rotation
axis, refer to the Table 1 described later.)
When only one table rotation axis is used, set table rotation axis
position 1 for the axis.
When no table rotation axis is used, or the machine used is not a
5-axis machine, table rotation axis position 1 and table rotation axis
position 2 need not be set.
No setting can be made for a hypothetical axis.
In the descriptions above, X, Y, and Z represent the three basic axes,
X, Y, and Z, specified by parameter No. 1022.
If the specification of any of the three basic axes, X, Y, and Z, is
missing, alarm PS0436 is issued.
- Setting of a workpiece setting error on the workpiece setting error setting screen
A workpiece setting error is set on the workpiece setting error setting
screen.
For explanations about the setting method, see Chapter 12, "SETTING
AND DISPLAYING DATA," of Part III.
- Workpiece setting error of No. 00 (COMMON)
Each of the values set in No. 00 (COMMON) is added to the
corresponding value of each of No. 01 through No. 07.
Note that rotation direction errors for No.00(COMMON) are not
available.
Example:
Suppose that workpiece setting errors are set as follows:
No. 00 (COMMON) No. 01 No. 02
X 10.000 x 0.500 x 0.800
Y 0.000 y 0.000 y 0.000
Z 0.000 z 0.000 z 0.000
a 1.500 a 1.800
b 0.000 b 0.000
c 0.000 c 0.000
When the workpiece setting error of No. 01 is selected,
workpiece setting error compensation is performed based on the
following:
∆x = 10.000+0.500 = 10.500
∆a = 1.500
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 401 -
When the workpiece setting error of No. 02 is selected,
workpiece setting error compensation is performed based on the
following:
∆x = 10.000+0.800 = 10.800
∆a = 1.800
If the setting of table rotation axis position 1/table rotation axis
position 2 differs between the workpiece setting error of No. 00 and
each workpiece setting error when a 5-axis machine (machine of table
rotation type or composite type) with table rotation axes is used, no
simple additions are made. Instead, before additions are made,
conversion is made to values based on the machine coordinate on a
table rotation axis being 0.
Example:
Suppose that workpiece setting errors are set as follows on a
5-axis machine with table rotation axis C about the Z-axis.
No. 00 (COMMON) No. 01
X 0.000 x 5.000
y 10.000 y 0.000
z 0.000 z 0.000
a 0.000
b 0.000
c 2.000
C -90.000 C 90.000
First, the error values of No. 00 are converted to those based on C
= 0.000.
Next, the error values of No. 01 are converted to those based on C
= 0.000.
X
Y
X'
Y'
∆y = 5.000, ∆c = 2.000
5
C = 0
2°
C positive direction
5 X
Y
X'
Y'
2°
∆x = 5.000, ∆c = 2.000
C = 90
∆c positive direction
C positive direction
X
Y
X'
Y'
10
∆y = 10.000
C = -90 C = 0
X
Y
X'
Y'
10
∆x = 10.000
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 402 -
When the workpiece setting error of No. 01 is selected, workpiece
setting error compensation is performed as follows based on the
converted error values based on C = 0.000:
∆x = 10.000+0.000 = 10.000
∆y = 0.000+5.000 = 5.000
∆c = 2.000
- Least input increment of data and valid data range
[About errors ∆x, ∆y, and ∆z]
The unit of data is the unit of input, and follows the least input
increment for the reference axis specified by parameter No. 1031.
- For metric input
Unit system of reference axis IS-A IS-B IS-C IS-D IS-E
Least input increment (mm) 0.01 0.001 0.0001 0.00001 0.000001
Maximum settable value (mm) ±999,999.99 ±999,999.999 ±99,999.9999 ±9,999.99999 ±999.999999
- For inch input
Unit system of reference axis IS-A IS-B IS-C IS-D IS-E
Least input increment (inch) 0.001 0.0001 0.00001 0.000001 0.0000001
Maximum settable value (inch) ±99,999.999 ±99,999.9999 ±9,999.99999 ±999.999999 ±99.9999999
[About errors ∆a, ∆b, and ∆c]
With parameter No. 11201, the number of decimal places of the least
input increment can be specified.
Parameter No. 11201 1 2 3 4
Least input increment (deg) 0.1 0.01 0.001 0.0001
Maximum settable value (deg) ±99,999,999.9 ±9999,999.99 ±999,999.999 ±99,999.9999
Parameter No. 11201 5 6 7 8
Least input increment (deg) 0.00001 0.000001 0.0000001 0.00000001
Maximum settable value (deg) ±9,999.99999 ±999.999999 ±99.9999999 ±9.99999999
Note, however, that a value from 1 to 8 can be specified in parameter
No. 11201.
If a value not within the specifiable range is specified in parameter No.
11201, the least input increment of the reference axis is followed.
Unit system of reference axis IS-A IS-B IS-C IS-D IS-E
Least input increment (deg) 0.01 0.001 0.0001 0.00001 0.000001
Maximum settable value (deg) ±999,999.99 ±999,999.999 ±99,999.9999 ±9,999.99999 ±999.999999
X'
Y'
5
X
Y
2°
Δx = 10.000, Δy = 5.000, Δc = 2.000
C = 0
∆c positive direction
10
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 403 -
[About table rotation axis position 1 and table rotation axis position 2]
The unit of data follows the least input increment of each
corresponding rotation axis.
Unit system of rotation axis IS-A IS-B IS-C IS-D IS-E
Least input increment (deg) 0.01 0.001 0.0001 0.00001 0.000001
Maximum settable value (deg) ±999,999.99 ±999,999.999 ±99,999.9999 ±9,999.99999 ±999.999999
- "Active workpiece setting error"
In the workpiece setting error compensation mode, "Active workpiece
setting error" on the workpiece setting error setting screen displays the
currently selected workpiece setting error number and workpiece
setting error (sum of the data of the currently selected workpiece
setting error number and the data of No. 00).
If the workpiece setting error compensation mode is not set, "MODE
OFF" is indicated, and 0 is displayed in each data field.
If a 5-axis machine (machine of table rotation type or composite type)
with table rotation axes is used, and a nonzero value is set for table
rotation axis position 1/table rotation axis position 2, error values
obtained by conversion based on the machine coordinates on the table
rotation axes being 0 are displayed.
- Setting of workpiece setting errors with custom macro variables
By using custom macro variables #26000 to #26077, workpiece
setting errors can be read and written.
(The custom macro option is required.)
The numbers of macro variables correspond to Errors as follows :
Error
No.00
(COMMON)
Error
No.01
Error
No.02
Error
No.03
Error
No.04
Error
No.05
Error
No.06
Error
No.07
X direction error ∆x #26000 #26010 #26020 #26030 #26040 #26050 #26060 #26070
Y direction error ∆y #26001 #26011 #26021 #26031 #26041 #26051 #26061 #26071
Z direction error ∆z #26002 #26012 #26022 #26032 #26042 #26052 #26062 #26072
Rotation direction error ∆a - #26013 #26023 #26033 #26043 #26053 #26063 #26073
Rotation direction error ∆b - #26014 #26024 #26034 #26044 #26054 #26064 #26074
Rotation direction error ∆c - #26015 #26025 #26035 #26045 #26055 #26065 #26075
Table rotation axis position 1 #26006 #26016 #26026 #26036 #26046 #26056 #26066 #26076
Table rotation axis position 2 #26007 #26017 #26027 #26037 #26047 #26057 #26067 #26077
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 404 -
- Workpiece setting error compensation mode
By specifying G54.4 Pn (n: 1 to 7), the workpiece setting error
compensation mode is set.
With Pn, select a workpiece setting error from No. 01 to No. 07.
In the workpiece setting error compensation mode, the program is
executed in a "workpiece setting coordinate system" defined by
shifting the workpiece coordinate system.
G54.4 is a modal G code that belongs to group 33 with the M series or
group 26 with the T series.
By specifying G54.4 P0, the workpiece setting error compensation
mode is canceled.
In a block for starting workpiece setting error compensation, the
machine is not moved, but the absolute coordinates are changed by the
error. So, the next absolute command makes a movement to a
specified position in the workpiece setting coordinate system. This
means that an absolute command is needed after a block for starting
workpiece setting error compensation.
NOTE
1 Be sure to specify Pn in a block specifying G54.4.
If P is not specified, or a number (n) not within the
specifiable range is specified after P, alarm
PS0437 is issued.
2 Specify G54.4 singly. If another G code or axis
command is specified together, alarm PS0437 is
issued.
3 Workpiece setting error compensation is valid for
movement in automatic operation.
4 Any workpiece setting error between starting
blocks remains valid until the workpiece setting
error compensation mode is canceled.
5 Workpiece setting error compensation may not be
specified doubly. If G54.4 Pn (n 0) is specified in
the workpiece setting error compensation mode,
alarm PS0437 is issued.
6 No absolute coordinate is changed in a block for
starting workpiece setting error compensation
unless the two angles stated below exceed the
value specified in parameter No. 11204.
(1) Angle made by the current absolute coordinate
point and a singular point posture
(2) Angle made by a point sifted by a workpiece
setting error from the absolute coordinate point
and a singular point posture
7 If all the errors are 0, issuing the G54.4 command
cannot put the workpiece setting error
compensation mode in effect.
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 405 -
- Tool direction compensation on a 5-axis machine
With a 5-axis machine, tool direction compensation must be
performed by setting bit 0 (RCM) of parameter No. 11200 to 1. This
means that rotation axis position compensation is performed to direct
the tool as programmed relative to the workpiece.
For tool direction compensation, the following parameters must be set:
Parameter No. Description
19680 Type of mechanical section
19681 Controlled axis number of the first rotation axis
19682 Axis direction of the first rotation axis
19683 Inclination angle when the first rotation axis is inclined
19684 Rotation direction of the first rotation axis
19685 Rotation angle when the first rotation axis is a hypothetical axis
19686 Controlled axis number of the second rotation axis
19687 Axis direction of the second rotation axis
19688 Inclination angle when the second rotation axis is inclined
19689 Rotation direction of the second rotation axis
19690 Rotation angle when the second rotation axis is a hypothetical axis
19696#0 Whether the first rotation axis is an ordinary rotation axis/hypothetical
axis
19696#1 Whether the second rotation axis is an ordinary rotation
axis/hypothetical axis
19697 Tool axis direction
19698 Reference angle RA
19699 Reference angle RB
19700 Rotary table position (X-axis of the basic three axes)
19701 Rotary table position (Y-axis of the basic three axes)
19702 Rotary table position (Z-axis of the basic three axes)
19703 Intersection offset vector between the first and second rotation axes of
the table (X-axis of the basic three axes)
19704 Intersection offset vector between the first and second rotation axes of
the table (Y-axis of the basic three axes)
19705 Intersection offset vector between the first and second rotation axes of
the table (Z-axis of the basic three axes)
With a 5-axis machine, it is recommended that Workpiece setting
error compensation is commanded after AICC(AI contouring control)
is already active.(G05.1 Q1 is commanded or bit 0 (SHP) of
parameter No.1604 is 1.) And, the following parameters for
Acc/Deceleration are needed.
Parameter No. Description
1432 Maximum cutting feedrate in the acceleration/deceleration before
interpolation mode
1660 Maximum allowable acceleration rate in acceleration/deceleration
before interpolation
1671 Maximum allowable acceleration rate for rapid traverse in
acceleration/deceleration before interpolation
1672 Acceleration/deceleration change time for rapid traverse in
bell-shaped acceleration/deceleration before interpolation
1737 Allowable acceleration rate for each axis when the deceleration
function based on acceleration/deceleration under AI contour control.
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 406 -
Parameter No. Description
1769 Time constant for acceleration/deceleration after cutting feed
interpolation in the acceleration/deceleration before interpolation mode
1772 Acceleration/deceleration change time in bell-shaped
acceleration/deceleration before interpolation
1783 Allowable speed difference in speed determination based on a corner
speed difference
NOTE
1 If any of the parameters above is set incorrectly, alarm
PS0438 is issued.
2 Depending on the machine configuration, it may be
physically impossible to orient the tool in the compensation
direction. In such a case, alarm DS0030 is issued.
3 In a block for starting workpiece setting error compensation,
the absolute coordinate on a rotation axis is changed
considering the workpiece setting error. At this time,
depending on the machine configuration, a rotation axis for
orienting the tool in the tool direction as viewed from the
workpiece setting coordinate system may be absent. In
such a case, alarm PS0438 is issued.
4 In the workpiece setting error compensation mode,
look-ahead acceleration/deceleration before interpolation is
automatically valid. Moreover, be sure to set the following
parameters:
(1) Bit 1 (LRP) of parameter No. 1401=1:
Linear rapid traverse
(2) Bit 5 (FRP) of parameter No. 19501=1:
Use acceleration/deceleration before interpolation for
rapid traverse.
(3) Parameter No. 1671:
Maximum allowable acceleration rate for rapid traverse
in acceleration/deceleration before interpolation
(4) Parameter No. 1660:
Maximum allowable acceleration rate in
acceleration/deceleration before interpolationIf the
parameters above are not set, alarm PS0438 is issued.
5 When TCP(Tool center point control) or G53.1 of TWP(Tilted
working plane command) is used during Workpiece setting
error compensation, Tool direction compensation is needed
(Bit 0 (RCM) of parameter No.11200 is 1. ) Otherwise, in
the case of TCP, the alarm PS5421, in the case of G53.1 of
TWP, the alarm PS5458 occurs.
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 407 -
If linear interpolation or circular interpolation is specified on a
machine of table rotation type or composite type, linear interpolation
or circular interpolation is performed as viewed from the workpiece
on the table.
<Example>
The machine is a table rotation type with A axis(master axis)
around X axis and C axis (slave axis) around Z axis (when A=0).
Firstly, suppose that Workpiece setting error is 0 and the
following program is commanded.
O1
N10 G55 (G55 is X50.0 Y0.0 Z0.0.)
N20 X0 Y0 Z0 A0 C0
N30 G01 X－50.0 Y150.0 C－90.0 F100.0
Next, suppose that Workpiece setting error has ∆c=5.0, which is
the error around Z axis, and N15,N16 are added to O2 as follows :
When Tool direction compensation is available (Bit 0 (RCM) of
parameter No.11200 is 1), the path will be as follows :
O2
N10 G55
N15 G05.1 Q1
N16 G54.4 P1
N20 X0 Y0 Z0 A0 C0
N30 G01 X－50.0 Y150.0 C－90.0 F100.0
The path looked from the workpiece in the middle of the block is
linear.
C -90
N20 end
N30 end Path in the middle
of the block
Path looked from the
workpiece in the middle of
the block
X
Y
C -90 N20 end
N30 and
Path in the middle
of the block
Path looked from the
workpiece in the middle of
the block
X
Y
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 408 -
- "Rotation axis closer to the tool" and "rotation axis closer to the workpiece" on a
5-axis machine
When tool direction compensation is performed on a 5-axis machine, a
singular point and singular point posture need to be considered. Here,
a "rotation axis closer to the tool" and "rotation axis closer to the
workpiece", which are used in a description of a singular point and
singular point posture provided later, are explained.
On a 5-axis machine with two rotation axes, one rotation axis
functions to tilt the tool toward the workpiece. This rotation axis is
referred to as a "rotation axis closer to the tool".
The other rotation axis is referred to as a "rotation axis closer to the
workpiece".
Depending on the type of mechanical section, the rotation axis closer
to the tool and rotation axis closer to the workpiece are determined as
indicated in Table 1.
Table 15.5 "Rotation axis closer to the tool" and "rotation axis closer to
the workpiece"
Type of mechanical
section (No. 19680)
Rotation axis closer
to the tool
Rotation axis closer
to the workpiece
Tool rotation type (2) Slave axis Master axis
Table rotation type (12) Master axis Slave axis
Composite type (21) Tool rotation axis Table rotation axis
Tool rotation type Table rotation type Composite type
Rotation axis closer to the tool
Rotation axis closer to the workpiece
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 409 -
- Singular point and singular point posture on a 5-axis machine
A tool posture is uniquely determined when the angles of the two
rotation axes are determined. Usually, however, a combination of
the angles of the two rotation axes for achieving a certain tool posture
is not determined uniquely.
In particular, such a tool posture that the angle of the rotation axis
closer to the tool is arbitrary is referred to as a "singular point posture".
Moreover, such an angle of the rotation axis closer the tool that the
tool posture becomes a singular point posture is referred to as a
"singular point (or singular point angle)". When the angle of the
rotation axis closer to the tool is a singular point, the center of the
rotation axis closer to the workpiece and the tool posture (tool
direction) are parallel with each other.
Example:
When the C-axis (about the Z-axis) is the master axis, the B-axis
is the slave axis (about the Y-axis), and the reference tool axis
direction is along the Z-axis on a 5-axis machine of tool rotation
type, the singular point is B = …, 0 deg, 180 deg, .... At this
time, an arbitrary C-axis angle represents a singular point posture
(in the same direction as the Z-axis or in the direction opposite to
the Z-axis).
If the angle of the B-axis is B = 0 (singular point) as shown in
Fig. 4, for example, an arbitrary C-axis angle represents the same
tool posture (singular point posture).
Fig. 15.5 (d) Singular point and singular point attitude
When the reference tool axis direction is inclined (parameter No.
19698, No. 19699), or the rotation axis is an angular axis (parameter
No. 19682, No. 19683, No. 19687, No. 19688), for example, no
singular point and singular point posture exist on some machines.
B=0
(Singular
point)
C=0 C=60
B=0
(Singular
point)
X
Z
Singular point
p
osture
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 410 -
- Conditions to decide that Tool is in singular posture
When the angle between the tool and the singular posture is less than
the parameter No.11204, it is decided that the tool is in singular
posture.
In the descriptions below, the description ‘when the tool is in
singular…’ means that ‘when it is decided that the tool is in singular
posture….’.
In addition, whether the tool is in singular point posture is decided at
each end point of tool paths calculated in the NC. If the parameter
No. 11204 value is very small and the feedrate and the override value
are large, it is likely that the tool may pass by a singular point without
deciding that the tool is in a singular point posture at each end point
even when the tool path crosses the singular point. In this case, the
tool will not be able to go beyond the singular point. To avoid this
problem, set parameter No. 11204 with a value slightly larger than the
quotient of the division of the highest rotation axis move speed (the
highest cutting feedrate (parameter No. 1432) among the rotation axes
or the rapid traverse rate (parameter No. 1420) whichever is higher)
by 15000.
- Movement in the case that Tool direction is compensated
In the case that the tool direction is compensated (bit 0 (RCM) of
parameter No.11200=1) on a 5 axis machine, the compensation is
performed in every interpolation, and the rotation axes may move to
positions which are different from the commanded positions.
In general, there are two pairs of rotation axes positions in the region
between 0 degree to 360 degree to turn the tool in a certain direction.
And in the case that the tool is in singular point posture, the position
of the rotation axis closer to the workpiece is not determined uniquely.
How the positions are determined is described as follows :
(1) In the case that the current machine position is singular and the
position after movement in real time is also singular.
(a) When the absolute position after movement in real time is
not singular, the rotation axis closer to the workpiece does
not move.
Example:
The rotation axis about the Z-axis is the master axis,
the rotation axis about the Y-axis is the slave axis, and
the reference tool axis direction is along the Z-axis on
a 5-axis machine of tool rotation type.
X
Y
The tool posture before movement
The tool posture after movement
(Not singular)
The tool posture in the
absolute coordinate system
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 411 -
Assume that the workpiece setting error around the
Y-axis exists, and the tool posture after the
compensation of tool direction becomes like following
figure. (The tools before and after movement are in
singular point posture.)
In this case, the rotation axis about the Z-axis (the
rotation axis closer to the workpiece) does not move.
(Only the rotation axis closer to the tool moves.)
If the parameter No.11204 is set to the value except 0,
the tools both before and after movement may be in
singular point posture like the above example.
In this case, the rotation axis closer to the workpiece
does not move. The rotation axis closer to the tool
moves in the move direction in which the tool in the
machine system (machine coordinate system) is
decided to be in a singular point posture, but not move
in the opposite direction.
X
Y
The tool posture in the
machine coordinate system The calculated tool
posture after movement
(Singular)
The tool posture before movement
(Singular)
X
The actual tool posture after
movement
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 412 -
(b) When the absolute position after movement in real time is
singular, the rotation axis closer to the workpiece moves as
commanded.
Example:
The rotation axis about the Z-axis is the master axis,
the rotation axis about the Y-axis is the slave axis, and
the reference tool axis direction is along the Z-axis on
a 5-axis machine of tool rotation type.
Assume that the workpiece setting error around the
Z-axis exists, and the tool posture after the
compensation of tool direction becomes like following
figure.
In this case, the rotation axis about Z-axis (the rotaion
axis closer to the workpiece) moves as commanded.
X
Y
The tool posture in the
absolute coordinate system The tool posture after movement
(Singular)
The tool posture before movement
X
Y
The tool posture in the
machine coordinate system
The tool posture after movement
(Singular)
The tool posture before movement
(Singular)
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 413 -
(2) In the case that the current machine position is not singular and
the position after movement in real time is singular.
: The rotation axis closer to workpiece does not move.
Example:
The rotation axis about the Z-axis is the master axis, the
rotation axis about the Y-axis is the slave axis, and the
reference tool axis direction is along the Z-axis on a 5-axis
machine of tool rotation type.
Assume that the tool posture after the compensation of tool
direction becomes like following figure.
In this case, the rotation axis about the Z-axis (the rotation
axis closer to the workpiece) does not move. (Only the
rotation axis closer to the tool moves.)
X
Y
The tool posture in the
machine coordinate system
The calculated tool posture
after movement
(Singular)
The tool posture before movement
(Not singular)
X
Y
The actual tool posture
after movement
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 414 -
(3) In the case that the current machine position is singular and the
position after movement in real time is not singular.
: In order to position the tool to the correct direction, there are
two pairs of solutions of rotation axes angles within 0 – 360deg.
A solution with which the rotation axis closer to workpiece
moves shorter is selected.
Example:
The rotation axis about the Z-axis is the master axis, the
rotation axis about the Y-axis is the slave axis, and the
reference tool axis direction is along the Z-axis on a 5-axis
machine of tool rotation type.
Assume that the tool posture after the compensation of tool
direction becomes like following figure.
In this case, the rotation axes move to the positions with
which the rotation axis about the Z-axis (the rotation axis
closer to workpiece) moves shorter. (The tool moves in the
direction of the arrow in the above figure.)
The tool does not move in the direction of the arrow in the
following figure.
The tool posture in the
machine coordinate system
The tool posture before movement
(Singular)
The tool posture after movement
(Not singular)
X
Y
X
Y
The tool posture
before movement
The tool posture
after movement
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 415 -
(4) In the case that the current machine position is not singular and
the position after movement in real time is not singular.
: In order to position the tool to the correct direction, there are
two pairs of solutions of rotation axes angles within 0 – 360deg.
One solution with which the rotation axes don’t pass the singular
point is selected. And, the rotation axes move to the positions of
the selected solution.
Example:
The rotation axis about the Z-axis is the master axis, the
rotation axis about the Y-axis is the slave axis, and the
reference tool axis direction is along the Z-axis on a 5-axis
machine of tool rotation type.
Assume that the tool posture after the compensation of tool
direction becomes like following figure.
In this case, the rotation axes move to the positions with
which the rotation axes don’t pass the singular point. (The
tool moves in the direction of the arrow in the above
figure.)
The tool does not move in the direction of the arrow in the
following figure.
X
Y The tool posture after movement
The tool posture
before movement
X
Y
The tool posture in the
machine coordinate system
The tool posture after movement
(Not singular)
The tool posture before movement
(Not singular)
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 416 -
- When the tool posture is closer to a singular point posture on a 5-axis machine
If tool direction compensation is performed on a 5-axis machine, and
the tool posture gets closer to a singular point posture during
execution of a block, the rotation axis closer to the workpiece may
make a large motion.
In addition, if parameter No. 11204 (angle for deciding on a singular
point posture) is set with a value, it is likely that the tool direction and
tool tip position may be incorrect while the tool is decided to be in a
singular point posture. Furthermore, it is likely that the rotation axis
closer to the tool may abruptly move by the parameter-set angle. So,
do not set parameter No. 11204 with a value larger than necessary.
- Notes in the case that rotary axes have movable range
When the tool direction is compensated on a 5-axis machine, there can
be the case that the machine position does not pass the singular
posture during a progress of work at all.
In this case, in accordance with 4) described above, the solution with
which the rotary axes don’t pass the singular point is always selected.
Therefore, in this case, the movement direction(area) depends on
where the tool exists in comparison with the singular point, because
the tool position is always selected so that the rotary axes don’t pass
the singular point.
In the case that rotary axes have movable range and a singular point
exists in that range, Workpiece setting error compensation must be
activated after the rotary axes have been moved to the range where the
rotary axes should move, that is, the range (A) between the lower limit
and the singular point or the range(B) between the upper limit and the
singular point.
Generally speaking, if (A) and (B) are different, it is recommended
that the larger one is selected.
Movable range of
rotary axis
Lower limit of
movable range
Upper limit of
movable range
Singular position
0de
g
(A) (B)
Workpiece setting error compensation must be activated after the rotary
axes have been moved to the range where the rotary axes should move
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 417 -
The following is an example that the movement direction(area)
depends on position of the rotary axes before starting workpiece
setting error compensation.
The Master axis is C axis around Z axis, and the Slave axis is B axis
around Y axis(when C=0). Tool direction is +Z when B=C=0.
Here, suppose B axis’ movable range is –45 deg to +100 deg.
When B=0, the tool posture does not change even if C axis moves.
That means the position B=0 is singular point.
Firstly, suppose the following program without Workpiece setting
error.
Program without Workpiece setting error
O1
N10 G5.1 Q1
N20 G90 G01 B-1.0 C0 F1000
N30 G43.4 H1
N40 X0 Y0 Z0
N50 B90.0 C90.0
X
Y
Z
C axis rotates around Z axis.
B axis rotates around Y axis.
Figure when B = C = 0
B axis movable range
- 45deg 100deg
Singular position
0de
g
X
Y
Z
N40 end
B C
Absolute -1.0 0.0
Machine -1.0 0.0
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 418 -
At N50, machine position moves to B90.0 and C90.0, as commanded.
Next, suppose there is the error -2.0deg around Y axis and Workpiece
setting error ∆b=-2.000 is set, and the block N25 is added as follows :
On O2, B axis position is –1.0 before Workpiece setting error
compensation is activated, which is between the lower limit of
movable range and the singular point of B axis.
X
Y
Z
In the middle of N50
X
Y
Z
N50 end
B C
Absolute 90.0 90.0
Machine 90.0 90.0
B axis movable
range
-45deg 100deg
B axis position of N20 before Workpiece
setting error compensation is activated
Singular point 0deg
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 419 -
O2
N10 G5.1 Q1
N20 G90 G01 B-1.0 C0 F1000 ; B axis machine position is between
the lower limit and the singular
point
N25 G54.4 P1
N30 G43.4 H1
N40 X0 Y0 Z0
N50 B90.0 C90.0
During N50, Machine position does not pass the singular point at all.
So, B axis moves from the starting position(–1.0) to the
position(B–90.0,C–90.0). As the result, B axis moves over the lower
limit of B axis movable range.
Therefore, suppose the program O3 in which B axis position is
changed to 1.0, which is between the singular point and the upper
limit, before Workpiece setting error compensation is activated.
Then, the range between the singular point and the upper limit of B
axis movable range is the range where B axis should move.
X
Y
Z
N40 end
B C
Absolute 1.0 0.0
Machine -1.0 0.0
X
Y
Z
In the middle of N50
B axis movable
range
-45deg 100deg
Singular point 0deg
B axis position of N20 before Workpiece
setting error compensation is activated
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 420 -
O3
N10 G5.1 Q1
N20 G90 G01 B1.0 C0 F1000 ; B axis machine position is between
the upper limit and the singular
point
N25 G54.4 P1
N30 G43.4 H1
N40 X0 Y0 Z0
N50 B90.0 C90.0
X
Y
Z
N40 end
B C
Absolute 3.0 0.0
Machine 1.0 0.0
X
Y
Z
In the middle of N50
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 421 -
This time, machine position moves to B90.0,C90.0 during N50. As the
result, B axis does not move over the lower limit of B axis movable
range.
In O2, the case that B axis moves over the limit of movable range is
the case that machine position does not make the singular point
posture during N50.
When parameter No.11204 has 0, whether the tool posture is a
singular point posture or not is judged strictly. So when the tool
posture is almost a singular point posture, the tool posture is not
regarded as a singular point posture.
When parameter No.11204 has a proper value and the tool posture in
the machine coordinate system is regarded as a singular point posture,
there is the possibility that the position passes the singular point.
In the above example, when parameter No.11204 has 0.1, the machine
position come to make the singular point posture during N50 in O2,
and B axis passes the singular point and moves to B90.0,C90.0 during
N50.
O2
N10 G5.1 Q1
N20 G90 G01 B-1.0 C0 F1000 ; B axis is between the lower limit
and the singular point.
N25 G54.4 P1
N30 G43.4 H1
N40 X0 Y0 Z0
N50 B90.0 C90.0
O2 is executed with the parameter No.11204=0.1.
X
Y
Z
N50 end
B C
Absolute 90.0 90.0
Machine 90.0 90.0
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 422 -
At N50, the machine position moves to B90.0,C90.0. As the result, B
axis does not move over the lower limit of B axis movable range.
X
Y
Z
N40 end
B C
Absolute 1.0 0.0
Machine -1.0 0.0
X
Y
Z
N50 end
B C
Absolute 90.0 90.0
Machine 90.0 90.0
X
Y
Z In the middle of N50
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 423 -
- Error for which the singular point processing is unnecessary
Even if tool direction compensation must be performed in a 5-axis
machine, the above mentioned singular point processing becomes
unnecessary if all workpiece setting errors in rotation directions are 0
(only X, Y, and Z directions) or there is only an error about the
rotation axis closer to the workpiece.
In this case, rotation axis compensation is performed simply by
shifting the rotation axis closer to the workpiece by a distance
corresponding to the error; the above mentioned singular point
processing is not carried out.
[Tool rotation type example]
In a tool rotation type, specify the C-axis (rotating about the
Z-axis) and B-axis (rotating about the Y-axis), respectively, as
the master and slave rotation axes.
The C-axis is a rotation axis closer to the workpiece.
No singular point posture processing is carried out if the
workpiece setting errors in rotation directions are:
Rotation direction error ∆a (rotation error about the X-axis): 0°
Rotation direction error ∆b (rotation error about the Y-axis): 0°
Rotation direction error ∆c (rotation error about the Z-axis): α°
The B-axis will move as directed. The C-axis will move to a
position compensated by α° with respect to the specified
position.
[Table rotation type example]
In a table rotation type, specify the A-axis (rotating about the
X-axis) and C-axis (rotating about the Z-axis), respectively, as
the master and slave rotation axes.
The C-axis is a rotation axis closer to the workpiece.
No singular point posture processing is carried out if the
workpiece setting errors in rotation directions are:
Rotation direction error ∆a (rotation error about the X-axis): 0°
Rotation direction error ∆b (rotation error about the Y-axis): 0°
Rotation direction error ∆c (rotation error about the Z-axis): α°
The A-axis will move as directed. The C-axis will move to a
position compensated by α° with respect to the specified
position.
[Composite type example]
In a composite type, specify the B-axis (rotating about the
Y-axis) and C-axis (rotating about the Z-axis), respectively, as
the tool and table rotation axes.
The C-axis is a rotation axis closer to the workpiece.
No singular point posture processing is carried out if the
workpiece setting errors in rotation directions are:
Rotation direction error ∆a (rotation error about the X-axis): 0°
Rotation direction error ∆b (rotation error about the Y-axis): 0°
Rotation direction error ∆c (rotation error about the Z-axis): α°
The B-axis will move as directed. The C-axis will move to a
position compensated by α° with respect to the specified
position.
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 424 -
- Absolute position display
Whether absolute coordinates in the workpiece setting error mode are
to be displayed in the workpiece coordinate system or workpiece
setting coordinate system can be chosen by using bit 6 (DAK) of
parameter No. 3106.
- Custom macro variables
To system variables #5041 through #5048 (current position on each
axis), the coordinates in the workpiece coordinate system are assigned.
- Range of rotary axes movements
In the case that Tilted working plane command or Type II of Tool
center point control or Type II of Tool radius compensation for 5-axis
machining is used, there are the parameters No.19741 to No.19744 to
limit the range of rotary axes movements. When tool direction is
compensated (bit 0 (RCM) of parameter No.11200=1), the rotary axes
are compensated after the range of rotary axes movements are limited.
Therefore, when the rotary axes are compensated, the rotary axes
positions may be out of the range of rotary axes movements.
Therefore, in the case that the rotary axes have the range of
movements, set the stored stroke limit check to prevent a movement
over the range.
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 425 -
Examples
- Example 1
O1 represents a program that cuts each side of a square.
Fig. 15.5 (e) Operation when there is no workpiece setting error
Suppose that the workpiece is displaced from the "correct workpiece
setting position" as shown in Fig. 15.5 (f).
Fig. 15.5 (f) Operation when there is a workpiece setting error
X
Y
Workpiece coordinate system G55 (XYZ)
Correct workpiece setting position
N50
N60
N70
N80 Workpiece
Workpiece setting coordinate system (X'Y'Z')
X
Y
Workpiece coordinate system G55 (XYZ)
Correct workpiece setting position
Displaced workpiece.
Operation is performed to cut four sides.
X'
Y'
N50
N60
N70
N80
Δx
=10.000
∆y
=20.000
∆c
=-20.000
Workpiece
O1 ;
N10 G55 ; Set coordinate system
N20 G90 G00 X0 Y0 Z300.0 B0 C0 ; Move to initial position
N30 G01 G43 H01 Z40.0 F500. ; Start tool length compensation
H01 is tool length compensation number.
N40 X50.0 Y50.0 Z20.0 ; Z-axis height of machining plane is 20.0.
N50 X150.0 ;
N60 Y150.0 ;
N70 X50.0 ;
N80 Y50.0 ;
N90 X0 Y0 Z40.0 ;
N100 G49 Z300.0 ; Cancel tool length compensation
Move to initial position on Z-axis
N110 M30;
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 426 -
The workpiece coordinate system, when rotated by -20.000 deg about
the Z-axis, shifted by 10.000 in the X direction, and shifted by 20.000
in the Y direction, is to match the workpiece setting coordinate
system.
At this time, set the following workpiece setting error values:
(Workpiece setting error No. 01)
x 10.000
y 20.000
z 0.000
a 0.000
b 0.000
c -20.000
To validate the workpiece setting error, add N15 and N115 to O1 as
indicated below.
When O1 is executed, the tool moves to cut each side of the displaced
workpiece as shown by the solid lines in Fig. 15.5 (f) .
O1 ;
N10 G55 ; Set coordinate system
N15 G54.4 P1 Workpiece setting error compensation mode ON
N20 G90 G00 X0 Y0 Z300.0 B0 C0 ; Move to initial position
N30 G01 G43 H01 Z40.0 F500. ; Start tool length compensation
H01 is tool length compensation number.
N40 X50.0 Y50.0 Z20.0 ; Z-axis height of machining plane is 20.0.
N50 X150.0 ;
N60 Y150.0 ;
N70 X50.0 ;
N80 Y50.0 ;
N90 X0 Y0 Z40.0 ;
N100 G49 Z300.0 ; Cancel tool length compensation
Move to initial position on Z-axis
N115 G54.4 P0 ; Workpiece setting error compensation mode OFF
N110 M30;
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 427 -
- Example 2
O2 is a program for cutting each side of a square by using tool center
point control.
The machine is of tool rotation type, the C-axis is the master rotation
axis and rotates about the Z-axis, and the B-axis is the slave axis and
rotates about the Y-axis. For cutting on the plane normal to the
movement direction, the tool is tilted 45 deg relative to the +Z
direction.
Fig. 15.5 (g) Operation of tool center point control when there is no
workpiece setting error
X
Workpiece coordinate system XYZ
Correct workpiece setting position
N50
N70
N110 Workpiece
N90
O2 ;
N10 G55 ; Set coordinate system
N20 G90 G00 X0 Y0 Z300.0 B0 C0 ; Move to initial position
N30 G01 G43.4 H01 Z40.0 F500. ; Start tool center point control
H01 is tool length compensation number.
N40 X50.0 Y50.0 Z20.0 B45.0 C-90.0 ; Z-axis height of machining plane is 20.0.
N50 X150.0 ;
N60 C0.0 ;
N70 Y150.0 ;
N80 C90.0 ;
N90 X50.0 ;
N100 C180.0 ;
N110 Y50.0 ;
N120 X0 Y0 Z40.0 B0.0 C0.0 ;
N130 G49 Z300.0 ; Cancel tool length compensation
Move to initial position on Z- axis
N140 M30;
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 428 -
Suppose that the workpiece is displaced from the correct workpiece
setting position as with example 1, and set a workpiece setting error in
the same was as in Example 1.
Moreover, add N15,N16,N135 and N136 to O2 as indicated below to
validate the workpiece setting error as in the case of Example 1.
Set bit 0 (RCM) of parameter No. 11200 to 1 to perform tool direction
compensation, then execute O2. When the tool moves to cut each
side of the workpiece with the tool tip, the tool is tilted 45 deg relative
to the +Z direction on the plane normal to the movement direction as
shown in Fig. 15.5 (h).
O2 ;
N10 G55 ; Set coordinate system
N15 G05.1 Q1 AI contour control mode ON
N16 G54.4 P1 Workpiece setting error compensation mode ON
N20 G90 G00 X0 Y0 Z300.0 B0 C0 ; Move to initial position
N30 G01 G43.4 H01 Z40.0 F500. ; Start tool center point control
H01 is tool length compensation number.
N40 X50.0 Y50.0 Z20.0 B45.0 C-90.0 ; Z-axis height of machining plane is 20.0.
N50 X150.0 ;
N60 C0.0 ;
N70 Y150.0 ;
N80 C90.0 ;
N90 X50.0 ;
N100 C180.0 ;
N110 Y50.0 ;
N120 X0 Y0 Z40.0 B0.0 C0.0 ;
N130 G49 Z300.0 ; Cancel tool length compensation
Move to initial position on Z- axis
N135 G54.4 P0 ; Workpiece setting error compensation mode OFF
N136 G05.1 Q0 ; AI contour control mode OFF
N140 M30;
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 429 -
Fig. 15.5 (h) Operation of tool center point control when there is a workpiece
setting error
Restrictions (general)
Described below is the restriction related to workpiece setting
compensation errors.
Note that, for 5-axis machines of tool rotation or composite type, the
restriction, “Restrictions (only with a 5-axis machine of table rotation
or composite type),” described later, in addition to the above, is
applied.
- Specifiable G codes
When workpiece setting error compensation is enabled, the G codes
listed below can be specified.
G00 Positioning
G01 Linear interpolation
G04 Dwell
G05.1 Q0/Q1 AI contour control mode OFF/ON
G10 Programmable data input
G11 Programmable data input mode cancel
G17 Plane selection (XY)
G18 Plane selection (ZX)
G19 Plane selection (YZ)
G40 Tool radius ⋅ tool nose radius compensation / 3-dimensional
cutter compensation cancel
G41.2/G41.4/G41.5 3-dimensional cutter compensation left (type 1)
(only if also tool center point control is used)
N50
N70
N110
N90
Workpiece setting coordinate system X'Y'Z'
Displaced workpiece.
Operation is performed to
cut four sides.
X'
Y'
X
Y
Workpiece coordinate system XYZ
Correct workpiece
setting position
Workpiece
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 430 -
G41.6 3-dimensional cutter compensation left (type 2)
(only if also tool center point control is used)
G42.2/G42.4/G42.5 3-dimensional cutter compensation right (type 1)
(only if also tool center point control is used)
G42.6 3-dimensional cutter compensation right (type 2)
(only if also tool center point control is used)
G43 Tool length compensation +
G43.4 Tool center point control (type 1)
G43.5 Tool center point control (type 2)
G49 (G49.1) Tool length compensation cancel
G53.1 Tool axis direction control
G65 Custom macro call
G66 Custom macro modal call
G67 Custom macro modal call cancel
G68.2 Tilted working plane command
G69 Coordinate system rotation/three-dimensional coordinate
system conversion/tilted working plane command cancel
G90 Absolute programming
G91 Incremental programming
G94 Feed per minute
G95 Feed per revolution
G69.1 Coordinate system rotation/three-dimensional coordinate
system conversion/tilted working plane command cancel
G90 Absolute programming (for G code system B and C)
G91 Incremental programming (for G code system B and C)
G94 Feed per minute (for G code system B and C)
G95 Feed per revolution (for G code system B and C)
- Modal G codes usable when workpiece setting error compensation is specified
In a modal G code state listed below, workpiece setting error
compensation can be specified.
G00 Positioning
G01 Linear interpolation
G13.1 Polar coordinate interpolation mode cancel
G15 Polar coordinate command cancel
G17 Plane selection (XY)
G18 Plane selection (ZX)
G19 Plane selection (YZ)
G21 Metric input
G23 Stored stroke check function OFF
G25 Spindle speed fluctuation detection OFF
M
T
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 431 -
G40 Tool radius ⋅ tool nose radius compensation / 3-dimensional
cutter compensation cancel
G49 (G49.1) Tool length compensation cancel
G50 Scaling cancel
G50.1 Programmable mirror image cancel
G50.2 Polygon turning cancel
G54 to G59, G54.1 Workpiece coordinate system selection
G64 Cutting mode
G67 Custom macro modal call cancel
G80 Canned cycle cancel
G80.5 (G80.8) Electronic gear box synchronization cancel
G97 Constant surface speed control cancel
G40.1 Normal direction control cancel
G54.2 P0 Rotary table dynamic fixture offset cancel
G69 Coordinate system rotation/three-dimensional coordinate
system conversion/tilted working plane command cancel
G90 Absolute programming
G91 Incremental programming
G94 Feed per minute
G95 Feed per revolution
G98 Canned cycle initial level return
G99 Canned cycle R point level return
G69 Mirror image for double turret OFF/balanced cutting mode
cancel
G69.1 Coordinate system rotation/three-dimensional coordinate
system conversion/tilted working plane command cancel
G90 Absolute programming (for G code system B and C)
G91 Incremental programming (for G code system B and C)
G94 Feed per minute (for G code system B and C)
G95 Feed per revolution (for G code system B and C)
G98 Canned cycle initial level return (for G code system B and C)
G99 Canned cycle R point level return (for G code system B and C)
- Manual intervention and handle interruption
In the workpiece setting error compensation mode, do not perform
manual intervention and handle interruption.
- Positioning in the machine coordinate system
In the workpiece setting error compensation mode, do not perform
positioning in the machine coordinate system (such as G28, G30, or
G53 command).
M
T
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 432 -
- Rapid traverse command
When using workpiece setting error compensation, specify linear
rapid traverse (by setting set bit 1 (LRP) of parameter No. 1401 to 1).
- Relationships with other modal commands
The commands for the functions listed below must be nested with a
workpiece setting error compensation command and must be placed
between G54.4 P_ and G54.4 P0.
Namely, specify G54.4 P_ when the mode of a desired function below
is off. Next, turn on then off the mode of the function, then specify
G54.4 P0.
• Cutter compensation (G40, G41.2, G41.4, G41.5, G41.6, G42.2,
G42.4, G42.5, G42.6)
• Tool length compensation (G43, G43.4, G43.5, G49)
• Tilted working plane command (G68.2, G69)
- PMC axis control
In the workpiece setting error compensation mode, do not perform
PMC axis control to the axes which are for workpiece setting error
compensation.
- Movement of start-up and cancel of Tool length offset
To perform tool length compensation (including tool center point
control) in the workpiece setting error compensation mode, set bit 6
(TOS) of parameter No. 5006 to 1 (perform tool length compensation
by shifting a coordinate system). If parameter TOS = 0, alarm
PS0438 is issued.
- Mirror image
Do not use programmable mirror imaging or external mirror imaging
(based on a mirror image signal or setting) during workpiece setting
error compensation.
- Stroke limit check before movement
In the mode of Workpiece setting error compensation, Stroke limit
check before movement is not available.
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 433 -
- Feedrate override
When tool direction is compensated (bit 0 (RCM) of parameter
No.11200=1), the rotation axis compensation is performed to the
movement which is modified by the override signals. If a large
movement of rotary axis occurs for the compensation, the feedrate of
the rotary axis is clamped by the speed which is generated by
calculation that the parameters No.11202,No.11203 override the
maximum cutting feedrate/rapid traverse.
While rotary axes move with this override, even when the override
signals change, the actual feedrate may not change, and, even when
feed hold or the like is done, the actual rotary axes movements may
not stop immediately because automatic operation stops after the
movement caused by rotation axis compensation has been completed.
WARNING
Rotation axis compensation near a singular point
causes a rotation axis to move largely, thus
resulting in a symptom that it is impossible to
change override or to reset feed hold during the
axis movement being likely to occur. If it is
necessary to stop the axis immediately during this
symptom, use the emergency stop function.
- In the case that Tool posture control is used with Type-2 of Tool center point
control
In the case that Tool posture control is used with Type-2 of Tool
center point control, when the angle between a tool posture and the
singular posture is less than the parameter No.19738, the tool posture
at the end of the block is changed so that the tool posture passes the
singular posture.
But, when tool direction is compensated (bit 0 (RCM) of parameter
No.11200 = 1), the tool posture may not pass the singular posture
because of the compensation after tool posture control.
- Distance-to-go display
The distance-to-go display is one before workpiece setting error
compensation is performed.
It is not the actual machine’s distance to go.
- Program restart
Do not restart a program if workpiece setting error compensation is
being performed for it.
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 434 -
- Reset
To cancel the workpiece setting error compensation mode, be sure to
use a reset by resetting bit 2 (D3R) of parameter No. 5400 to 0.
Performing tool length compensation (including tool center point
control) in the workpiece setting error compensation mode causes the
tool length compensation mode and tool length compensation vector
to be canceled by a reset no matter what the setting of the following
parameters:
• Bit 6 (CLR) of parameter No.3402
• Bit 0 (C08) of parameter No.3407
• Bit 6 (LVK) of parameter No.5003
- Setting not involving tool direction compensation
For 5-axis machines, be sure to select tool direction compensation (set
bit 0 (RCM) of parameter No. 11200 to 1).
For machines other than 5-axis machines, workpiece setting error
compensation is carried out with no tool direction compensation
selected (bit 0 (RCM) of parameter No. 11200 is 0). However, do
not specify rotation errors other than those about the tool direction.
Otherwise, machining will not be performed properly. (Example:
If the tool is in the Z direction, do not specify rotation errors about the
X- or Y-axis.
- Synchronous slave axis absolute coordinates
If feed axis synchronization is in effect, no slave axis absolute
coordinate is displayed properly.
- Workpiece coordinate system shift
Do not perform workpiece setting error compensation with G52 (local
coordinate system setting) or G92/G50 (T series) (workpiece
coordinate system shift) executed.
Once the workpiece coordinate system has been shifted, preset it using
G92.1 or axis-specific workpiece coordinate system preset functions
before starting workpiece setting error compensation.
- Canned cycle
In the workpiece setting error compensation mode, do not carry out
canned cycles.
Restrictions (only with a 5-axis machine of table rotation or composite type)
For 5-axis machines of table rotation or composite type in particular,
this restriction, in addition to "Restrictions (general)" above, is
applied.
- Hypothetical axis used for a table rotation axis
If a hypothetical axis is used as a table rotation axis, compensation is
performed with the angle of the table rotation axis set to 0 degree.
B-63944EN/03 PROGRAMMING 15.COMPENSATION FUNCTION
- 435 -
- Acceleration/deceleration at a corner
When a command for linear interpolation is specified, linear
interpolation is performed as viewed from the workpiece on the table.
So, even when the command specifies a linear interpolation, the
control point may make a curved motion. This means that a corner
operation may be performed with some commands.
So, if a small value is set as an allowable feedrate difference
(parameter No. 1783) or as an allowable acceleration/deceleration rate
(parameter No. 1660 and No. 1737) for a corner, the tool may be
decelerated.
- G codes that must not be specified
Among the "Specifiable G codes" in "Restrictions (general)" above,
the G codes listed below must not be specified when tool direction
compensation is performed with a 5-axis machine of table rotation
type or composite type.
G95 Feed per revolution
G95 Feed per revolution (for G code system B and C)
- Modal G codes not usable when workpiece setting error compensation is
specified
Among the "Modal G codes usable when workpiece setting error
compensation is specified" in "Restrictions (general)" above, the G
codes listed below must not be specified with a 5-axis machine of
table rotation type or composite type in the modal G code state
indicated below.
G95 Feed per revolution
G95 Feed per revolution (for G code system B and C)
- Command for an axis not related to 5-axis machining
Those axes that are not related to 5-axis machining must not be
specified. Otherwise, alarm PS0439 is issued.
M
T
M
T
15.COMPENSATION FUNCTION PROGRAMMING B-63944EN/03
- 436 -
- Combination with tool center point control
If bit 5 (WKP) of parameter No. 19696 = 0 (table coordinate system
command), starting tool center point control with the table rotation
axis position not set at 0 usually causes the workpiece coordinate
system to be fixed at the table with it in the startup state, thus making
it the table coordinate system.
If tool center point control is carried out in the workpiece setting error
compensation mode, this specification becomes ineffective, and the
table coordinate system is set up on the assumption that the workpiece
coordinate system is fixed at the table with the table rotation axis
position being at 0.
- Speed in the workpiece setting error compensation mode
When workpiece setting error compensation is performed in a
machine of table rotation or composite type, processing equivalent to
tool center point control is carried out so that tool movement as
viewed from the table can be controlled.
In this case, control point movement is calculated by assuming that the
tool tip moves at the specified speed. If the resulting control point
speed exceeds the specified speed, the feedrate is clamped at the
specified speed.
Conversely, if the control point speed is lower than the specified speed,
it is likely that the tool may move at a speed lower than the specified
speed.
Center point movement (at specified speed F) viewed
from the table
Control point movement as viewed from the table
Workpiece setting error
compensation
(Rotation axis position
is also compensated)
Table rotation
A
ctual control point
m
o
v
e
m
e
n
t
If this speed is about to exceed the specified speed,
the feedrate is clam
p
ed at the s
p
ecified s
p
eed.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 437 -
16 CUSTOM MACRO
Although subprograms are useful for repeating the same operation, the
custom macro function also allows use of variables, arithmetic and
logic operations, and conditional branches for easy development of
general programs such as pocketing and user-defined canned cycles.
A machining program can call a custom macro with a simple
command, just like a subprogram.
O0001 ;
:
:
:
G65 P9010 R50.0 L2 ;
:
:
M30 ;
Machining program Custom macro
O9010 ;
#1=#18/2 ;
G01 G42 X#1 Y#1 F300 ;
02 X#1 Y-#1 R#1 ;
:
:
:
M99 ;
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 438 -
16.1 VARIABLES
An ordinary machining program specifies a G code and the travel
distance directly with a numeric value; examples are G100 and
X100.0.
With a custom macro, numeric values can be specified directly or
using a variable number. When a variable number is used, the
variable value can be changed by a program or using operations on the
MDI panel.
#1=#2+100 ;
G01 X#1 F300 ;
Explanation
- Variable representation
When specifying a variable, specify a number sign (#) followed by a
variable number.
#i (i = 1, 2, 3, 4, .....)
[Example] #5
#109
#1005
A variable can also be represented as follows using <expression>
described in the section about arithmetic and logic operation
commands.
#[<expression>]
[Example] #[#100]
#[#1001-1]
#[#6/2]
Variable #i shown in the following can be replaced with a variable of
#[<expression>].
- Types of variables
Variables can be classified as local variables, common variables, and
system variables according to the variable number. Each of those
variables has its own usage and characteristics. Read-only system
constants are also provided.
- Range of variable values
Local and common variables can have a value in the following ranges.
If the result of calculation exceeds the range, an alarm PS0111 is
issued.
When bit 0 (F16) of parameter No.6008 = 0
Maximum value: approx. ±10308
Minimum value: approx. ±10-308
Numeric data handled by a custom macro conforms to the IEEE
standard and is handled as a double-precision real number. An
error resulting from operation depends on the precision.
When bit 0 (F16) of parameter No.6008 = 1
Maximum value: approx. ±1047
Minimum value: approx. ±10-29
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 439 -
- Local variable (#1-#33)
A local variable is a variable that is used locally in a macro. That is,
local variable #i used by a macro called at a certain time is different
from that used by a macro called at another time, regardless of
whether the two macros are the same. Therefore, for example, when
macro A calls macro B during multiple calls or the like, it is
impossible for macro B to corrupt a local variable used by macro A by
erroneously using the variable.
A local variable is used to pass arguments. For information on
correspondence between arguments and addresses, see the section
about macro calling commands. The initial state of a local variable
to which no arguments are passed is <null> and the user can freely use
the variable. The attribute of a local variable is READ/WRITE
enabled.
- Common variable (#100-#199, #500-#999)
A common variable is shared among the main program, subprograms
called by the main program, and macros while a local variable is used
locally in a macro. That is, #i used by a macro is the same as that used
by another macro. Therefore, a resultant common variable obtained by
using a macro can be used by another macro. The attribute of a
common variable is basically READ/WRITE enabled. However, the
common variable can be protected (its attribute is set to READ only) by
specifying its variable number using parameters No.6031 and No.6032.
A common variable can be freely used by the user even when its usage
is not defined by the system. The number of common variables can be
specified by selecting one of the following options.
(a) 100 common variables (specified only with the custom macro
option)
The common variables #100 to #149 and #500 to #549 can be
used. The variables #100 to #149 are cleared during
power-down, but the variables #500 to #549 are retained during
power-down.
(b) 600 common variables (specified with the custom macro
option or custom macro common variable addition option)
The common variables #100 to #199 and #500 to #999 can be
used. The variables #100 to #199 are cleared during
power-down, but the variables #500 to #999 are retained during
power-down.
- Write protection of a common variable
Multiple common variables (#500 to #999) can be protected (their
attributes are set to READ only) by setting variable numbers in
parameters No.6031 and No.6032. This protection is enabled for
both Input/All Clear by MDI on the macro screen and write operation
by a macro program. If the NC program specifies WRITE operation
(used in the left side) for a common program in the set range, an alarm
PS0116 is issued.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 440 -
- System variable
A variable whose usage does not vary in the system. The attribute of
a system variable is READ only, WRITE only, or READ/WRITE
enabled depending on the nature of a system variable.
- System constant
A system constant can be referenced as with a variable even though its
value is fixed. The attribute of a system constant is READ only.
- Omission of the decimal point
When a variable value is defined in a program, the decimal point can
be omitted.
[Example]
When #1 = 123; is defined, the actual value of variable #1 is 123.000.
- Referencing variables
The value following an address can be replaced with a variable.
When programming as <address>#i or <address>-#i, the variable
value or the complement of it is used as the specified value of the
address.
[Example] F#33 is the same as F1.5 when #33 = 1.5.
Z-#18 is the same as Z-20.0 when #18 = 20.0.
G#130 is the same as G3 when #130 = 3.0.
A variable cannot be referenced using address/, :, or O and N.
[Example] Programming such as O#27 or N#1 is not allowed.
n (n = 1 to 9) in the optional block skip /n cannot be a variable.
A variable number cannot be specified by a direct variable.
[Example] When replacing 5 in #5 with #30, specify #[#30] instead of ##30.
No values exceeding the maximum allowable value for each
address can be specified.
[Example] When #140 = 120, G#140 exceeds the maximum allowable
value.
When a variable is used as address data, the variable is
automatically rounded off to the number of significant figures of
each address or less.
[Example] For a machine with an increment system of 1/1000 mm (IS-B),
when #1 = 12.3456, G00 X#1; becomes G00 X12.346;.
If <expression>, described later, is used, the value following an
address can be replaced with <expression>.
<address>[<expression>] or <address>-[<expression>]
The program code shown above indicates the value of <expression> or
the complement of the value is used as an address value. Note that a
constant with no decimal point, enclosed in brackets ([ ]), is assumed
to have a decimal point at the end.
[Example] X[#24+#18*COS[#1]]
Z-[#18+#26]
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 441 -
- Undefined variable
When the value of a variable is not defined, such a variable is referred
to as a "null" variable. Variables #0 and #3100 are always null
variables. They cannot be written to, but they can be read.
(a) Quotation
When an undefined variable is quotated, the address itself is also
ignored.
Original command G90 X100 Y#1
Equivalent command when #1 = <null> G90 X100
Equivalent command when #1 = 0 G90 X100 Y0
(b) Definition/replacement, addition, multiplication
When a local variable or common variable is directly replaced
with <null>, the result is <null>. When a system variable is
directly replaced with <null> or the result of calculation
including <null> is replaced, a variable value of 0 is assumed.
Original expression
(local variable) #2=#1 #2=#1*5 #2=#1+#1
Replacement result
(when #1 = <null>) <null> 0 0
Replacement result (when #1 = 0) 0 0 0
Original expression
(common variable) #100=#1 #100=#1*5 #100=#1+#1
Replacement result
(when #1 = <null>) <null> 0 0
Replacement result (when #1 = 0) 0 0 0
Original expression
(system variable) #2001=#1 #2001=#1*5 #2001=#1+#1
Replacement result
(when #1 = <null>) 0 0 0
Replacement result (when #1 = 0) 0 0 0
(c) Comparison
<null> differs from 0 only for EQ and NE.
<null> is equal to 0 for GE, GT, LE, and LT.
• When <null> is assigned to #1
Conditional
expression #1 EQ #0 #1 NE 0 #1 GE #0 #1 GT 0 #1 LE #0 #1 LT 0
Evaluation
result
Established
(true)
Established
(true)
Established
(true)
Not
established
(false)
Established
(true)
Not
established
(false)
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 442 -
• When 0 is assigned to #1
Conditional
expression #1 EQ #0 #1 NE 0 #1 GE #0 #1 GT 0 #1 LE #0 #1 LT 0
Evaluation
result
Not
established
(false)
Not
established
(false)
Established
(true)
Not
established
(false)
Established
(true)
Not
established
(false)
- Specifying a system variable (constant) by its name
A system variable (constant) is specified by its variable number, but it
can also be specified by its predetermined system variable (constant)
name. A system variable (constant) name begins with an underscore
(_), followed by up to seven uppercase letters, numerics, or
underscores. For axis-dependent variables (such as coordinates) or
variables having a lot of data of similar types (such as tool
compensation), subscript [n] (n: integer) can be used to specify values.
In this case, n can be specified in <expression> format (calculation
format).
The command format must be specified in [#system-variable-name]
format, as shown below.
[#_DATE]
[Example]
[#_DATE]=20040117 ; : 2004.01.17 is assigned to #3011 (year
month date).
[#_TIME]=161705 ; : 16:17:05 is assigned to #3012 (time
minute second).
#101=[#_ABSMT[1]] ; : #5021 (machine coordinate value of
the 1st axis) is read off and assigned
to #101.
#102=[#_ABSKP[#500*2]] ; : #506x (skip position of [#500*2]th axis)
is read off and assigned to #102.
If a value other than an integer is specified for subscript n, a variable
value is referenced, assuming that the fractional portion is rounded
off.
[Example]
[#_ABSIO[1.4999999]] : This value is assumed to be [#_ABSIO[1]],
that is, #5001.
[#_ABSIO[1.5000000]] : This value is assumed to be [#_ABSIO[2]],
that is, #5002.
NOTE
1 When the specified variable name is not registered,
an alarm PS1098 is issued.
2 When a negative or other invalid subscript is
specified, an alarm PS1099 is issued.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 443 -
- System constant #0, #3100-#3102 (Attribute: R)
Constants used as fixed values in the system can be used as system
variables. Such constants are called system constants. The system
constants provided are shown below.
Constant
number
Constant
name Description
#0, #3100 [#_EMPTY] Null
#3101 [#_PI] Circular constant π
= 3.14159265358979323846
#3102 [#_E] Base of natural logarithm e
= 2.71828182845904523536
- Specifying a common variable by its name
Specifying a variable name set by the SETVN command described
later allows reading from or writing to a common variable.
The command must be specified in the form
[#common-variable-name] such as [#VAR500].
[Example]
X[#POS1] Y[#POS2] ; : Specifying a position by the variable
name
[#POS1] = #100+#101 ; : Executing a assignment statement
by the variable name
#[100+[#ABS]] = 500 ; : Same as above (by a variable
number)
#500 = [1000+[#POS2]*10] ; : Reading a variable by a variable
name
- Setting and specifying the name of a common variable (SETVN)
For the 50 common variables, #500 to #549, a name of up to eight
characters can be specified by using a command as shown below.
SETVN n [VAR500, VAR501, VAR502,......] ;
n represents the starting number of a common variable for which the
name is specified.
VAR500 is the variable name of variable n, VAR501 is the variable
name of variable n+1, and VAR502 is the variable name of variable
number n+2, and so on. Each string is delimited by a comma (,).
All codes that can be used as meaningful information in a program
except control in, control out, [, ], EOB, EOR, and : (colon in a
program number) can be used. However, each name must begin with
an alphabetical character. Variable names are not cleared on
switch-off.
Specifying a set variable name allows reading from or writing to the
common variable. The command must be specified in the form
[#common-variable-name] such as [#VAR500].
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 444 -
[Example] SETVN 510[TOOL_NO, WORK_NO, COUNTER1, COUNTER2];
The command above names the variables as follows.
Variable Name
#510 TOOL_NO
#511 WORK_NO
#512 COUNTER1
#513 COUNTER2
The names specified by the command can be used in a
program. For example, when 10 is assigned to #510, the
expression [#TOOL_NO]=10; can be used instead #510=10;.
NOTE
If the same name was specified for different
common variables, only the variable which has the
smaller variable number can be referenced with the
specified name.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 445 -
16.2 SYSTEM VARIABLES
System variables can be used to read and write internal CNC data such
as tool compensation values and current position data. System
variables are essential for automation and general-purpose program
development.
List of system variables and constants
n represents a subscript.
R, W, and R/W are attributes of a variable and indicate read-only,
write-only, and read/write enabled, respectively.
- Interface signals
System
variable
number
System
variable
name
Attribute Description
#1000-#1031 [#_UI[n]] R Interface input signals (BIT), UI000-UI031
NOTE) Subscript n represents a BIT position (0-31).
#1032-#1035 [#_UIL[n]] R Interface input signals (LONG), UI000-UI031/ UI100-UI131/
UI200-UI231/UI300-UI331
NOTE) Subscript n (0-3): 0 = UI000-UI031, 1 = UI100-UI131,
2 = UI200-231, 3 = UI300-UI331
#1100-#1131 [#_UO[n]] R/W Interface output signals (BIT), UO000-UO031
NOTE) Subscript n represents a BIT position (0-31).
#1132-#1135 [#_UOL[n]] R/W Interface output signals (LONG), UO000-UO031/
UO100-UO131/UO200-UO231/UO300-UO331
NOTE) Subscript n (0-3): 0 = UO000-UO031, 1 = UO100-UO131,
2 = UO200-231, 3 = UO300-UO331
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 446 -
- Tool compensation value
M
Tool compensation memory A
System variable
number
System
variable name Attribute Description
#2001-#2200
#10001-#10999
[#_OFS[n]] R/W Tool compensation value
Note) Subscript n represents a compensation
number (1 to 200).
When the number of sets is larger than 200,
the numbers to the left can also be used.
Note) Subscript n represents a compensation
number (1 to 999).
Tool compensation memory B when bit 3 (V15) of parameter No.6000 = 0
System variable
number
System
variable name Attribute Description
#2001-#2200 Tool compensation value (wear)
Note) Subscript n represents a compensation
number (1 to 200).
#10001-#10999
[#_OFSW[n]] R/W
The numbers to the left can also be used.
Note) Subscript n represents a compensation
number (1 to 999).
#2201-#2400 Tool compensation value (H code, geometry)
Note) Subscript n represents a compensation
number (1 to 200).
#11001-#11999
[#_OFSG[n]] R/W
The numbers to the left can also be used.
Note) Subscript n represents a compensation
number (1 to 999).
Tool compensation memory B when bit 3 (V15) of parameter No.6000 = 1
System variable
number
System
variable name Attribute Description
#2001-#2200 Tool compensation value (geometry)
Note) Subscript n represents a compensation
number (1 to 200).
#10001-#10999
[#_OFSG[n]] R/W
The numbers to the left can also be used.
Note) Subscript n represents a compensation
number (1 to 999).
#2201-#2400 Tool compensation value (H code, wear)
Note) Subscript n represents a compensation
number (1 to 200).
#11001-#11999
[#_OFSW[n]] R/W
The numbers to the left can also be used.
Note) Subscript n represents a compensation
number (1 to 999).
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 447 -
Tool compensation memory C when bit 3 (V15) of parameter No.6000 = 0
System variable
number
System
variable name Attribute Description
#2001-#2200 Tool compensation value (H code, wear)
Note) Subscript n represents a compensation
number (1 to 200).
#10001-#10999
[#_OFSHW[n]] R/W
The numbers to the left can also be used.
Note) Subscript n represents a compensation
number (1 to 999).
#2201-#2400 Tool compensation value (H code, geometry)
Note) Subscript n represents a compensation
number (1 to 200).
#11001-#11999
[#_OFSHG[n]] R/W
The numbers to the left can also be used.
Note) Subscript n represents a compensation
number (1 to 999).
#12001-#12999 [#_OFSDW[n]] R/W Tool compensation value (D code, wear)
Note) Subscript n represents a compensation
number (1 to 999).
# 13001-#13999 [#_OFSDG[n]] R/W Tool compensation (D code, geometry)
Note) Subscript n represents a compensation
number (1 to 999).
Tool compensation memory C when bit 3 (V15) of parameter No.6000 = 1
System variable
number
System
variable name Attribute Description
#2001-#2200 Tool compensation value (H code, geometry)
Note) Subscript n represents a compensation
number (1 to 200).
#10001-#10999
[#_OFSHG[n]] R/W
The numbers to the left can also be used.
Note) Subscript n represents a compensation
number (1 to 999).
#2201-#2400 Tool compensation value (H code, wear)
Note) Subscript n represents a compensation
number (1 to 200).
#11001-#11999
[#_OFSHW[n]] R/W
The numbers to the left can also be used.
Note) Subscript n represents a compensation
number (1 to 999).
#2401-#2600 Tool compensation value (D code, geometry)
(Note 2)
Note 1) Subscript n represents a
compensation number (1 to 200).
Note 2) Enabled when bit 5 (D15) of
parameter No.6004 = 1.
#12001-#12999
[#_OFSDG[n]] R/W
The numbers to the left can also be used.
Note) Subscript n represents a compensation
number (1 to 999).
#2601-#2800 Tool compensation value (D code, wear) (Note 2)
Note 1) Subscript n represents a
compensation number (1 to 200).
Note 2) Enabled when bit 5 (D15) of
parameter No.6004 = 1.
#13001-#13999
[#_OFSDW[n]] R/W
The numbers to the left can also be used.
Note) Subscript n represents a compensation
number (1 to 999).
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 448 -
- Tool compensation value
T
Without tool geometry/wear compensation memory
System variable
number
System
variable name Attribute Description
#2001-#2064
#10001-#10999
[#_OFSX[n]] R/W X-axis compensation value (*1)
Note) Subscript n represents a compensation
number (1 to 64).
When the number of sets is larger than 64, the
numbers to the left can be used.
Note) Subscript n represents a compensation
number (1 to 999).
#2101-#2164
#11001-#11999
[#_OFSZ[n]] R/W Z-axis compensation value (*1)
Note) Subscript n represents a compensation
number (1 to 64).
When the number of sets is larger than 64, the
numbers to the left can be used.
Note) Subscript n represents a compensation
number (1 to 999).
#2201-#2264
#12001-#12999
[#_OFSR[n]] R/W Tool nose radius compensation value
Note) Subscript n represents a compensation
number (1 to 64).
When the number of sets is larger than 64, the
numbers to the left can be used.
Note) Subscript n represents a compensation
number (1 to 999).
#2301-#2364
#13001-#13999
[#_OFST[n]] R/W Virtual tool tip T position
Note) Subscript n represents a compensation
number (1 to 64).
When the number of sets is larger than 64, the
numbers to the left can be used.
Note) Subscript n represents a compensation
number (1 to 999).
#2401-#2449
#14001-#14999
[#_OFSY[n]] R/W Y-axis compensation value (*1)
Note) Subscript n represents a compensation
number (1 to 49).
When the number of sets is larger than 49,
the numbers to the left can be used.
Note) Subscript n represents a compensation
number (1 to 999).
(*1) X-axis: X-axis of basic three axes, Z-axis: Z-axis of basic three
axes, Y-axis: Y-axis of basic three axes
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 449 -
With tool geometry/wear compensation memory
System variable
number
System
variable name Attribute Description
#2001-#2064
#10001-#10999
[#_OFSXW[n]] R/W X-axis compensation value (wear) (*1)
Note) Subscript n represents a compensation
number (1 to 64).
When the number of sets is larger than 64,
the numbers to the left can be used.
Note) Subscript n represents a compensation
number (1 to 999).
#2101-#2164
#11001-#11999
[#_OFSZW[n]] R/W Z-axis compensation value (wear) (*1)
Note) Subscript n represents a compensation
number (1 to 64).
When the number of sets is larger than 64,
the numbers to the left can be used.
Note) Subscript n represents a compensation
number (1 to 999).
#2201-#2264
#12001-#12999
[#_OFSRW[n]] R/W Tool nose radius compensation value (wear)
Note) Subscript n represents a compensation
number (1 to 64).
When the number of sets is larger than 64,
the numbers to the left can be used.
Note) Subscript n represents a compensation
number (1 to 999).
#2301-#2364
#13001-#13999
[#_OFST[n]] R/W Virtual tool tip T position
Note) Subscript n represents a compensation
number (1 to 64).
When the number of sets is larger than 64,
the numbers to the left can be used.
Note) Subscript n represents a compensation
number (1 to 999).
#2401-#2449
#14001-#14999
[#_OFSYW[n]] R/W Y-axis compensation value (wear) (*1)
Note) Subscript n represents a compensation
number (1 to 49).
When the number of sets is larger than 49,
the numbers to the left can be used.
Note) Subscript n represents a compensation
number (1 to 999).
#2451-#2499
#19001-#19999
[#_OFSYG[n]] R/W Y-axis compensation value (geometry) (*1)
Note) Subscript n represents a compensation
number (1 to 49).
When the number of sets is larger than 49,
the numbers to the left can be used.
Note) Subscript n represents a compensation
number (1 to 999).
#2701-#2749
#15001-#15999
[#_OFSXG[n]] R/W X-axis compensation value (geometry) (*1)
Note) Subscript n represents a compensation
number (1 to 49).
When the number of sets is larger than 49,
the numbers to the left can be used.
Note) Subscript n represents a compensation
number (1 to 49).
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 450 -
System variable
number
System
variable name Attribute Description
#2801-#2849
#16001-#16999
[#_OFSZG[n]] R/W Z-axis compensation value (geometry) (*1)
Note) Subscript n represents a compensation
number (1 to 49).
When the number of sets is larger than 49,
the numbers to the left can be used.
Note) Subscript n represents a compensation
number (1 to 999).
#2901-#2964
#17001-#17999
[#_OFSRG[n]] R/W Tool nose radius compensation value
(geometry)
Note) Subscript n represents a compensation
number (1 to 64).
When the number of sets is larger than 64,
the numbers to the left can be used.
Note) Subscript n represents a compensation
number (1 to 999).
(*1) X-axis: X-axis of basic three axes, Z-axis: Z-axis of basic three
axes, Y-axis: Y-axis of basic three axes
- Workpiece coordinate system shift amount
T
System variable
number
System
variable name Attribute Description
#2501 [#_WKSFTX] R/W X-axis workpiece shift amount
#2601 [#_WKSFTZ] R/W Z-axis workpiece shift amount
#100751 to
#100800
[#_WZ_SFT [n]] R/W nth axis workpiece shift amount
Note) Subscript n represents an axis number
(1 to 50).
X-axis: X-axis of basic three axes, Z-axis: Z-axis of basic three axes
- Automatic operation or the like
System variable
number
System
variable name Attribute Description
#3000 [#_ALM] W Macro alarm
#3001 [#_CLOCK1] R/W Clock 1 (ms)
#3002 [#_CLOCK2] R/W Clock 2 (hr)
#3003 [#_CNTL1] R/W Enable or disable the suppression of single
block stop.
Enable or disable the waiting of the auxiliary
function completion signal.
#3003 bit 0 [#_M_SBK] R/W Enable or disable the suppression of single
block stop.
#3003 bit 1 [#_M_FIN] R/W Enable or disable waiting for the auxiliary
function completion signal.
#3004 [#_CNTL2] R/W Enable or disable feed hold.
Enable or disable feedrate override.
Enable or disable exact stop check.
#3004 bit 0 [#_M_FHD] R/W Enable or disable feed hold.
#3004 bit 1 [#_M_OV] R/W Enable or disable feedrate override.
#3004 bit 2 [#_M_EST] R/W Enable or disable exact stop check.
#3005 [#_SETDT] R/W Read/write setting data.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 451 -
System variable
number
System
variable name Attribute Description
#3006 [#_MSGSTP] W Stop with a message.
#3007 [#_MRIMG] R Status of a mirror image (DI and setting)
#3008 [#_PRSTR] R Restarting/not restarting a program
- Time
System variable
number
System
variable name Attribute Description
#3011 [#_DATE] R Year/Month/Date
#3012 [#_TIME] R Hour/Minute/Second
- Number of parts
System variable
number
System
variable name Attribute Description
#3901 [#_PRTSA] R/W Total number of parts
#3902 [#_PRTSN] R/W Number of required parts
- Tool compensation memory
M
System variable
number
System
variable name Attribute Description
#3980 [#_OFSMEM] R Tool compensation memory information
- Main program number
System variable
number
System
variable name Attribute Description
#4000 [#_MAINO] R Main program number
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 452 -
- Modal information
M
System variable
number
System
variable name Attribute Description
#4001-#4030 [#_BUFG[n]] R Modal information on blocks that have been
specified by last minute (G code)
Note) Subscript n represents a G code group
number.
#4102 [#_BUFB] R Modal information on blocks that have been
specified by last minute (B code)
#4107 [#_BUFD] R Modal information on blocks that have been
specified by last minute (D code)
#4108 [#_BUFE] R Modal information on blocks that have been
specified by last minute (E code)
#4109 [#_BUFF] R Modal information on blocks that have been
specified by last minute (F code)
#4111 [#_BUFH] R Modal information on blocks that have been
specified by last minute (H code)
#4113 [#_BUFM] R Modal information on blocks that have been
specified by last minute (M code)
#4114 [#_BUFN] R Modal information on blocks that have been
specified by last minute (sequence number)
#4115 [#_BUFO] R Modal information on blocks that have been
specified by last minute (program number)
#4119 [#_BUFS] R Modal information on blocks that have been
specified by last minute (S code)
#4120 [#_BUFT] R Modal information on blocks that have been
specified by last minute (T code)
#4130 [#_BUFWZP] R Modal information on blocks that have been
specified by last minute (additional workpiece
coordinate system number)
#4201-#4230 [#_ACTG[n]] R Modal information on the block currently being
executed (G code)
Note) Subscript n represents a G code group
number.
#4302 [#_ACTB] R Modal information on the block currently being
executed (B code)
#4307 [#_ACTD] R Modal information on the block currently being
executed (D code)
#4308 [#_ACTE] R Modal information on the block currently being
executed (E code)
#4309 [#_ACTF] R Modal information on the block currently being
executed (F code)
#4311 [#_ACTH] R Modal information on the block currently being
executed (H code)
#4313 [#_ACTM] R Modal information on the block currently being
executed (M code)
#4314 [#_ACTN] R Modal information on the block currently being
executed (sequence number)
#4315 [#_ACTO] R Modal information on the block currently being
executed (program number)
#4319 [#_ACTS] R Modal information on the block currently being
executed (S code)
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 453 -
System variable
number
System
variable name Attribute Description
#4320 [#_ACTT] R Modal information on the block currently being
executed (T code)
#4330 [#_ACTWZP] R Modal information on the block currently being
executed (additional workpiece coordinate
system number)
#4401-#4430 [#_INTG[n]] R Modal information on interrupted blocks (G
code)
Note) Subscript n represents a G code group
number.
#4502 [#_INTB] R Modal information on interrupted blocks (B
code)
#4507 [#_INTD] R Modal information on interrupted blocks (D
code)
#4508 [#_INTE] R Modal information on interrupted blocks (E
code)
#4509 [#_INTF] R Modal information on interrupted blocks (F
code)
#4511 [#_INTH] R Modal information on interrupted blocks (H
code)
#4513 [#_INTM] R Modal information on interrupted blocks (M
code)
#4514 [#_INTN] R Modal information on interrupted blocks
(sequence number)
#4515 [#_INTO] R Modal information on interrupted blocks
(program number)
#4519 [#_INTS] R Modal information on interrupted blocks (S
code)
#4520 [#_INTT] R Modal information on interrupted blocks (T
code)
#4530 [#_INTWZP] R Modal information on interrupted blocks
(additional workpiece coordinate system
number)
T
System variable
number
System
variable name Attribute Description
#4001-#4030 [#_BUFG[n]] R Modal information on blocks that have been
specified by last minute (G code)
Note) Subscript n represents a G code group
number.
#4108 [#_BUFE] R Modal information on blocks that have been
specified by last minute (E code)
#4109 [#_BUFF] R Modal information on blocks that have been
specified by last minute (F code)
#4113 [#_BUFM] R Modal information on blocks that have been
specified by last minute (M code)
#4114 [#_BUFN] R Modal information on blocks that have been
specified by last minute (sequence number)
#4115 [#_BUFO] R Modal information on blocks that have been
specified by last minute (program number)
#4119 [#_BUFS] R Modal information on blocks that have been
specified by last minute (S code)
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 454 -
System variable
number
System
variable name Attribute Description
#4120 [#_BUFT] R Modal information on blocks that have been
specified by last minute (T code)
#4130 [#_BUFWZP] R Modal information on blocks that have been
specified by last minute (additional workpiece
coordinate system number)
#4201-#4230 [#_ACTG[n]] R Modal information on the block currently being
executed (G code)
Note) Subscript n represents a G code group
number.
#4308 [#_ACTE] R Modal information on the block currently being
executed (E code)
#4309 [#_ACTF] R Modal information on the block currently being
executed (F code)
#4313 [#_ACTM] R Modal information on the block currently being
executed (M code)
#4314 [#_ACTN] R Modal information on the block currently being
executed (sequence number)
#4315 [#_ACTO] R Modal information on the block currently being
executed (program number)
#4319 [#_ACTS] R Modal information on the block currently being
executed (S code)
#4320 [#_ACTT] R Modal information on the block currently being
executed (T code)
#4330 [#_ACTWZP] R Modal information on the block currently being
executed (additional workpiece coordinate
system number)
#4401-#4430 [#_INTG[n]] R Modal information on interrupted blocks (G
code)
Note) Subscript n represents a G code group
number.
#4508 [#_INTE] R Modal information on interrupted blocks (E
code)
#4509 [#_INTF] R Modal information on interrupted blocks (F
code)
#4513 [#_INTM] R Modal information on interrupted blocks (M
code)
#4514 [#_INTN] R Modal information on interrupted blocks
(sequence number)
#4515 [#_INTO] R Modal information on interrupted blocks
(program number)
#4519 [#_INTS] R Modal information on interrupted blocks (S
code)
#4520 [#_INTT] R Modal information on interrupted blocks (T
code)
#4530 [#_INTWZP] R Modal information on interrupted blocks
(additional workpiece coordinate system
number)
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 455 -
- Position information
System variable
number
System
variable name Attribute Description
#5001-#5020 End point position of the previous block
(workpiece coordinate system)
Note) Subscript n represents an axis number
(1 to 20)
#100001-#100050
[#_ABSIO[n]] R
The numbers to the left can also be used.
Note) Subscript n represents an axis number
(1 to 50).
#5021-#5040 Specified current position (machine coordinate
system)
Note) Subscript n represents an axis number
(1 to 20).
#100051-#100100
[#_ABSMT[n]] R
The numbers to the left can also be used.
Note) Subscript n represents an axis number
(1 to 50).
#5041-#5060 Specified current position (workpiece
coordinate system)
Note) Subscript n represents an axis number
(1 to 20).
#100101-#100150
[#_ABSOT[n]] R
The numbers to the left can also be used.
Note) Subscript n represents an axis number
(1 to 50).
#5061-#5080 Skip position (workpiece coordinate system)
Note) Subscript n represents an axis number
(1 to 20).
#100151-#100200
[#_ABSKP[n]] R
The numbers to the left can also be used.
Note) Subscript n represents an axis number
(1 to 50).
- Tool length compensation value
M
System variable
number
System
variable name Attribute Description
#5081-#5100 Tool length compensation value
Note) Subscript n represents an axis number
(1 to 20).
#100201-#100250
[#_TOFS[n]] R
The numbers to the left can also be used.
Note) Subscript n represents an axis number
(1 to 50).
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 456 -
- Tool offset value
T
System variable
number
System
variable name Attribute Description
#5081, #100201 [#_TOFSWX] X-axis tool offset (wear)
#5082, #100202 [#_TOFSWZ] Z-axis tool offset (wear)
#5083, #100203 [#_TOFSWY] Y-axis tool offset (wear)
#5084 - #5100 Tool offset (wear) for an arbitrary axis
Note) Subscript n represents an axis number
(4 to 20).
#100204 -
#100250
[#_TOFS[n]]
R
Tool offset (wear) for an arbitrary axis
Note) Subscript n represents an axis number
(4 to 50).
#5121, #100901 [#_TOFSGX] X-axis tool offset (geometry)
#5122, #100902 [#_TOFSGZ] Y-axis tool offset (geometry)
#5123, #100903 [#_TOFSGY] Z-axis tool offset (geometry)
#5124 - #5140 Tool offset (geometry) for an arbitrary axis
Note) Subscript n represents an axis number
(4 to 20).
#100904 -
#100950
[#_TOFSG[n]]
R
Tool offset (geometry) for an arbitrary axis
Note) Subscript n represents an axis number
(4 to 50).
X-axis: X-axis of basic three axes, Z-axis: Z-axis of basic three axes,
Y-axis: Y-axis of basic three axes
- Servo position deviation
System variable
number
System
variable name Attribute Description
#5101-#5120 Servo positional deviation
Note) Subscript n represents an axis number
(1 to 20).
#100251-#100300
[#_SVERR[n]] R
The numbers to the left can also be used.
Note) Subscript n represents an axis number
(1 to 50).
- Manual handle interruption
System variable
number
System
variable name Attribute Description
#5121-#5140 Manual handle interruption
Note) Subscript n represents an axis number
(1 to 20).
#100651-#100700
[#_MIRTP[n]] R
The numbers to the left can also be used.
Note) Subscript n represents an axis number
(1 to 50).
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 457 -
- Distance to go
System variable
number
System
variable name Attribute Description
#5181-#5200 Distance to go
Note) Subscript n represents an axis number
(1 to 20).
#100801-#100850
[#_DIST[n]] R
The numbers to the left can also be used.
Note) Subscript n represents an axis number
(1 to 50).
- Workpiece origin offset value, extended workpiece origin offset value
M
System variable
number
System
variable name Attribute Description
#5201-#5220 [#_WZCMN[n]] R/W External workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
#5221-#5240 [#_WZG54[n]] R/W G54 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
#5241-#5260 [#_WZG55[n]] R/W G55 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
#5261-#5280 [#_WZG56[n]] R/W G56 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
#5281-#5300 [#_WZG57[n]] R/W G57 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
#5301-#5320 [#_WZG58[n]] R/W G58 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
#5321-#5340 [#_WZG59[n]] R/W G59 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
#100301-#100350 [#_WZCMN[n]] R/W External workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 50).
#100351-#100400 [#_WZG54[n]] R/W G54 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 50).
#100401-#100450 [#_WZG55[n]] R/W G55 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 50).
#100451-#100500 [#_WZG56[n]] R/W G56 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 50).
#100501-#100550 [#_WZG57[n]] R/W G57 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 50).
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 458 -
System variable
number
System
variable name Attribute Description
#100551-#100600 [#_WZG58[n]] R/W G58 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 50).
#100601-#100650 [#_WZG59[n]] R/W G59 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 50).
Extended workpiece origin offset value
#7001-#7020 [#_WZP1[n]] R/W G54.1P1 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
#7021-#7040 [#_WZP2[n]] R/W G54.1P2 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
:
:
:
:
:
:
:
:
#7941-#7960 [#_WZP48[n]] R/W G54.1P48 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
#14001-#14020 [#_WZP1[n]] R/W G54.1P1 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
#14021-#14040 [#_WZP2[n]] R/W G54.1P2 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
:
:
:
:
:
:
:
:
#19981-#20000 [#_WZP300[n]] R/W G54.1P300 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
#101001-#101050 [#_WZP1[n]] R/W G54.1P1 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 50).
#101051-#101100 [#_WZP2[n]] R/W G54.1P2 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 50).
:
:
:
:
:
:
:
:
#115901-#115950 [#_WZP299[n]] R/W G54.1P299 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 50).
#115951-#116000 [#_WZP300[n]] R/W G54.1P300 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 50).
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 459 -
T
System variable
number
System
variable name Attribute Description
#5201-#5220 [#_WZCMN[n]] R/W External workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
#5221-#5240 [#_WZG54[n]] R/W G54 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
#5241-#5260 [#_WZG55[n]] R/W G55 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
#5261-#5280 [#_WZG56[n]] R/W G56 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
#5281-#5300 [#_WZG57[n]] R/W G57 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
#5301-#5320 [#_WZG58[n]] R/W G58 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
#5321-#5340 [#_WZG59[n]] R/W G59 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
#100301-#100350 [#_WZCMN[n]] R/W External workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 50).
#100351-#100400 [#_WZG54[n]] R/W G54 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 50).
#100401-#100450 [#_WZG55[n]] R/W G55 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 50).
#100451-#100500 [#_WZG56[n]] R/W G56 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 50).
#100501-#100550 [#_WZG57[n]] R/W G57 workpiece origin offset value
Note)
(1 to 50).
#100551-#100600 [#_WZG58[n]] R/W G58 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 50).
#100601-#100650 [#_WZG59[n]] R/W G59 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 50).
Extended workpiece origin offset value
#7001-#7020 [#_WZP1[n]] R/W G54.1P1 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
#7021-#7040 [#_WZP2[n]] R/W G54.1P2 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
:
:
:
:
:
:
:
:
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 460 -
System variable
number
System
variable name Attribute Description
#7941-#7960 [#_WZP48[n]] R/W G54.1P48 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 20).
#101001-#101050 [#_WZP1[n]] R/W G54.1P1 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 50).
#101051-#101100 [#_WZP2[n]] R/W G54.1P2 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 50).
:
:
:
:
:
:
:
:
#115901-#115950 [#_WZP299[n]] R/W G54.1P299 workpiece origin offset value
Note)
(1 to 50).
#115951-#116000 [#_WZP300[n]] R/W G54.1P300 workpiece origin offset value
Note) Subscript n represents an axis number
(1 to 50).
- Skip position (detection unit)
System variable
number
System
variable name Attribute Description
#5421-#5440 Skip position (detection unit)
Note) Subscript n represents an axis number
(1 to 20).
#100701-#100750
[#_SKPDTC[n]] R
The numbers to the left can also be used.
Note) Subscript n represents an axis number
(1 to 50).
- Rotary table dynamic fixture offset value
M
System variable
number
System
variable name Attribute Description
#5500 [#_FOFSP] R Number of the standard fixture offset being
selected (P)
#5501-#5520 Offset value of the standard fixture offset being
selected
Note) Subscript n represents an axis number
(1 to 20).
#117001-#117050
[#_FOFSVAL[n]] R
The numbers to the left can also be used.
Note) Subscript n represents an axis number
(1 to 50).
#5521-#5540 Standard fixture offset value (first set)
Note) Subscript n represents an axis number
(1 to 20).
#117051-#117100
[#_FOFS1[n]] R/W
The numbers to the left can also be used.
Note) Subscript n represents an axis number
(1 to 50).
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 461 -
System variable
number
System
variable name Attribute Description
#5541-#5560 Standard fixture offset value (second set)
Note) Subscript n represents an axis number
(1 to 20).
#117101-#117150
[#_FOFS2[n]] R/W
The numbers to the left can also be used.
Note) Subscript n represents an axis number
(1 to 50).
#5561-#5580 Standard fixture offset value (third set)
Note) Subscript n represents an axis number
(1 to 20).
#117151-#117200
[#_FOFS3[n]] R/W
The numbers to the left can also be used.
Note) Subscript n represents an axis number
(1 to 50).
#5581-#5600 Standard fixture offset value (fourth set)
Note) Subscript n represents an axis number
(1 to 20).
#117201-#117250
[#_FOFS4[n]] R/W
The numbers to the left can also be used.
Note) Subscript n represents an axis number
(1 to 50).
#5601-#5620 Standard fixture offset value (fifth set)
Note) Subscript n represents an axis number
(1 to 20).
#117251-#117300
[#_FOFS5[n]] R/W
The numbers to the left can also be used.
Note) Subscript n represents an axis number
(1 to 50).
#5621-#5640 Standard fixture offset value (sixth set)
Note) Subscript n represents an axis number
(1 to 20).
#117301-#117350
[#_FOFS6[n]] R/W
The numbers to the left can also be used.
Note) Subscript n represents an axis number
(1 to 50).
#5641-#5660 Standard fixture offset value (seventh set)
Note) Subscript n represents an axis number
(1 to 20).
#117351-#117400
[#_FOFS7[n]] R/W
The numbers to the left can also be used.
Note) Subscript n represents an axis number
(1 to 50).
#5661-#5680 Standard fixture offset value (eighth set)
Note) Subscript n represents an axis number
(1 to 20).
#117401-#117450
[#_FOFS8[n]] R/W
The numbers to the left can also be used.
Note) Subscript n represents an axis number
(1 to 50).
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 462 -
- Second geometry tool offset value
T
System variable
number
System
variable name Attribute Description
#5801-#5832
#27001-#27999
[#_OFSX2G[n]] R/W Second geometry tool offset X-axis
compensation value
Note) Subscript n represents a compensation
number (1 to 32).
If the number of pairs is greater than 32, the
numbers on the left are also permitted.
Note) Subscript n represents a compensation
number (1 to 999).
#5833-#5864
#28001-#28999
[#_OFSZ2G[n]] R/W Second geometry tool offset Z-axis
compensation value
Note) Subscript n represents a compensation
number (1 to 32).
If the number of pairs is greater than 32, the
numbers on the left are also permitted.
Note) Subscript n represents a compensation
number (1 to 999).
#5865-#5896
#29001-#29999
[#_OFSY2G[n]] R/W Second geometry tool offset Y-axis
compensation value
Note) Subscript n represents a compensation
number (1 to 32).
If the number of pairs is greater than 32, the
numbers on the left are also permitted.
Note) Subscript n represents a compensation
number (1 to 999).
- Dynamic standard tool compensation value
M
System variable
number
System
variable name Attribute Description
#118051-#118100 [#_DOFS1[n]] R/W Dynamic standard tool compensation value
(first set)
Note) Subscript n represents an axis number
(1 to 50).
#118101-#118150 [#_DOFS2[n]] R/W Dynamic standard tool compensation value
(second set)
Note) Subscript n represents an axis number
(1 to 50).
#118151-#118200 [#_DOFS3[n]] R/W Dynamic standard tool compensation value
(third set)
Note) Subscript n represents an axis number
(1 to 50).
#118201-#118250 [#_DOFS4[n]] R/W Dynamic standard tool compensation value
(fourth set)
Note) Subscript n represents an axis number
(1 to 50).
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 463 -
System variable
number
System
variable name Attribute Description
#118251-#118300 [#_DOFS5[n]] R/W Dynamic standard tool compensation value
(fifth set)
Note) Subscript n represents an axis number
(1 to 50).
#118301-#118350 [#_DOFS6[n]] R/W Dynamic standard tool compensation value
(sixth set)
Note) Subscript n represents an axis number
(1 to 50).
#118351-#118400 [#_DOFS7[n]] R/W Dynamic standard tool compensation value
(seventh set)
Note) Subscript n represents an axis number
(1 to 50).
#118401-#118450 [#_DOFS8[n]] R/W Dynamic standard tool compensation value
(eighth set)
Note) Subscript n represents an axis number
(1 to 50).
- Feedrate reduction ratio for rapid traverse overlap
System variable
number
System
variable name Attribute Description
#100851-
#100900
[#_ROVLP [n]] R/W Feedrate reduction ratio for rapid traverse
overlap
Note) Subscript n represents an axis number
(1 to 50).
- System constant
System constant
number
System
constant name Attribute Description
#0, #3100 [#_EMPTY] R Null
#3101 [#_PI] R Circular constant π
= 3.14159265358979323846
#3102 [#_E] R Base of natural logarithm e
= 2.71828182845904523536
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 464 -
Explanation
R, W, and R/W are attributes of a variable and represents read-only,
write-only, and read/write enabled, respectively.
- Interface signal #1000-#1031, #1032, #1033-#1035 (Attribute: R)
#1100-#1115, #1132, #1133-#1135 (Attribute: R/W)
[Input signal]
The status of interface input signals can be obtained by reading the
value of system variables #1000 to #1032.
Variable
number
Variable
name Point Interface input signal
#1000 [#_UI[0]] 1 UI000 (20)
#1001 [#_UI[1]] 1 UI001 (21)
#1002 [#_UI[2]] 1 UI002 (22)
#1003 [#_UI[3]] 1 UI003 (23)
#1004 [#_UI[4]] 1 UI004 (24)
#1005 [#_UI[5]] 1 UI005 (25)
#1006 [#_UI[6]] 1 UI006 (26)
#1007 [#_UI[7]] 1 UI007 (27)
#1008 [#_UI[8]] 1 UI008 (28)
#1009 [#_UI[9]] 1 UI009 (29)
#1010 [#_UI[10]] 1 UI010 (210)
#1011 [#_UI[11]] 1 UI011 (211)
#1012 [#_UI[12]] 1 UI012 (212)
#1013 [#_UI[13]] 1 UI013 (213)
#1014 [#_UI[14]] 1 UI014 (214)
#1015 [#_UI[15]] 1 UI015 (215)
#1016 [#_UI[16]] 1 UI016 (216)
#1017 [#_UI[17]] 1 UI017 (217)
#1018 [#_UI[18]] 1 UI018 (218)
#1019 [#_UI[19]] 1 UI019 (219)
#1020 [#_UI[20]] 1 UI020 (220)
#1021 [#_UI[21]] 1 UI021 (221)
#1022 [#_UI[22]] 1 UI022 (222)
#1023 [#_UI[23]] 1 UI023 (223)
#1024 [#_UI[24]] 1 UI024 (224)
#1025 [#_UI[25]] 1 UI025 (225)
#1026 [#_UI[26]] 1 UI026 (226)
#1027 [#_UI[27]] 1 UI027 (227)
#1028 [#_UI[28]] 1 UI028 (228)
#1029 [#_UI[29]] 1 UI029 (229)
#1030 [#_UI[30]] 1 UI030 (230)
#1031 [#_UI[31]] 1 UI031 (231)
#1032 [#_UIL[0]] 32 UI000-UI031
#1033 [#_UIL[1]] 32 UI100-UI131
#1034 [#_UIL[2]] 32 UI200-UI231
#1035 [#_UIL[3]] 32 UI300-UI331
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 465 -
Variable value Input signal
1.0 Contact closed
0.0 Contact opened
Since the read value is 1.0 or 0.0 regardless of the unit system, the unit
system must be considered when a macro is created.
The input signals at 32 points can be read at a time by reading from
system variables #1032 to #1035.
31
30
0
21031#2]1000[#1032# ×−×+= ∑
=
i
i
i
{}
∑
=
×−×=+
30
0
31
31
22]1032[#
i
i
iVVn
When UIni = 0, Vi = 0.
When UIni = 1, Vi = 1.
n = 0-3
[Output signal]
Interface output signals can be sent by assigning values to system
variables #1100 to #1132 for sending interface signals.
Variable
number
Variable
name Point Interface input signal
#1100 [#_UO[0]] 1 UO000 (20)
#1101 [#_UO[1]] 1 UO001 (21)
#1102 [#_UO[2]] 1 UO002 (22)
#1103 [#_UO[3]] 1 UO003 (23)
#1104 [#_UO[4]] 1 UO004 (24)
#1105 [#_UO[5]] 1 UO005 (25)
#1106 [#_UO[6]] 1 UO006 (26)
#1107 [#_UO[7]] 1 UO007 (27)
#1108 [#_UO[8]] 1 UO008 (28)
#1109 [#_UO[9]] 1 UO009 (29)
#1110 [#_UO[10]] 1 UO010 (210)
#1111 [#_UO[11]] 1 UO011 (211)
#1112 [#_UO[12]] 1 UO012 (212)
#1113 [#_UO[13]] 1 UO013 (213)
#1114 [#_UO[14]] 1 UO014 (214)
#1115 [#_UO[15]] 1 UO015 (215)
#1116 [#_UO[16]] 1 UO016 (216)
#1117 [#_UO[17]] 1 UO017 (217)
#1118 [#_UO[18]] 1 UO018 (218)
#1119 [#_UO[19]] 1 UO019 (219)
#1120 [#_UO[20]] 1 UO020 (220)
#1121 [#_UO[21]] 1 UO021 (221)
#1122 [#_UO[22]] 1 UO022 (222)
#1123 [#_UO[23]] 1 UO023 (223)
#1124 [#_UO[24]] 1 UO024 (224)
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 466 -
Variable
number
Variable
name Point Interface input signal
#1125 [#_UO[25]] 1 UO025 (225)
#1126 [#_UO[26]] 1 UO026 (226)
#1127 [#_UO[27]] 1 UO027 (227)
#1128 [#_UO[28]] 1 UO028 (228)
#1129 [#_UO[29]] 1 UO029 (229)
#1130 [#_UO[30]] 1 UO030 (230)
#1131 [#_UO[31]] 1 UO031 (231)
#1132 [#_UOL[0]] 32 UO000-UO031
#1133 [#_UOL[1]] 32 UO100-UO131
#1134 [#_UOL[2]] 32 UO200-UO231
#1135 [#_UOL[3]] 32 UO300-UO331
Variable value Input signal
1.0 Contact closed
0.0 Contact opened
The output signals at 32 points can be written at a time by writing to
system variables #1132 to #1135. The signals can also be read.
31
30
0
21131#2]1000[#1132# ×−×+= ∑
=
i
i
i
{}
∑
=
×−×=+
30
0
31
31
22]1132[#
i
i
iVVn
When UIni = 0, Vi = 0.
When UIni = 1, Vi = 1.
n = 0-3
NOTE
1 When a value other than 1.0 or 0.0 is assigned to
variables #1100 to #1131, it is assumed as follows.
<null> is assumed to be 0.
A value other than <null> or 0 is assumed to be 1.
Where, a value less than 0.00000001 is undefined.
2 When any of UI016 to UI031, UI100 to UI131,
UI200 to UI231, UI300 to UI331, UO016 to UO031,
UO200 to UO231, and UO300 to UO331 are used,
parameter MIF (No.6001#0) must be set to 1.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 467 -
Example
Structure of DI
215 2
14 213 212 211 210 2928272625 2
4 2
3 2
22120
Used for other
purposes
Sign 102 101 100
Structure of DO
2
8272625 2
4 2
3 2
22120
Not used Used for other purposes Address
<1> Address switching signed BCD 3 digits are read.
Macro calling instruction
G65 P9100 D (address);
A custom macro body is created as follows.
O9100 ;
#1132 = #1132 AND 496 OR#7 ; : Address sending
G65 P9101 T60 ; : Timer macro
#100 = BIN[#1032 AND 4095] ; : BCD 3 digits are read.
IF [#1012 EQ 0] GOTO 9100 ; : A sign is attached.
#100 = -#100
N9100 M99
<2> Eight types of address switching signed BCD 6 digits (3-digit
integer part + 3-digit fractional part) are read into #101.
Structure on the machine side
When DO 20 = 0: Data with 3 decimal places
When DO 20 = 1: Data with 3-digit integer part
When DO 23 to 21 = 000: No1 data when #1 = 0
When DO 23 to 21 = 001: No2 data when #2 = 0
:
When DO 23 to 21 = 111: No8 data when #8 = 0
Macro calling instruction
G65 P9101 D (data number);
A custom macro body is created as follows.
O9101 ;
G65 P9101 D[#1*2+1] ;
#101 = #100 ;
G65 P9100 D[#1*2] ;
#101 = #101 + #100/1000 ;
M99 ;
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 468 -
- Tool compensation value #2001-#2800, #10001-#13999 (Attribute: R/W)
M
The compensation values can be obtained by reading system variables
#2001 to #2800 or #10001 to #13999 for tool compensation. The
compensation values can also be changed by assigning values to the
system variables.
<1> Tool compensation memory A
• When the number of compensations is 200 or less
Compensation
number Variable number Variable name
1 #2001 [#_OFS[1]]
2 #2002 [#_OFS[2]]
3 #2003 [#_OFS[3]]
: : :
199 #2199 [#_OFS[199]]
200 #2200 [#_OFS[200]]
• When the number of compensations is more than 200 (For
compensation with a compensation number of 200 or less,
#2001 to #2200 can also be used.)
Compensation
number Variable number Variable name
1 #10001 [#_OFS[1]]
2 #10002 [#_OFS[2]]
3 #10003 [#_OFS[3]]
: : :
998 #10998 [#_OFS[998]]
999 #10999 [#_OFS[999]]
<2> Tool compensation memory B
• When the number of compensations is 200 or less
When bit 3 (V15) of parameter No.6000 = 0
Wear Geometry
Compensation
number Variable
number Variable name Variable
number Variable name
1 #2001 [#_OFSW[1]] #2201 [#_OFSG[1]]
2 #2002 [#_OFSW[2]] #2202 [#_OFSG[2]]
3 #2003 [#_OFSW[3]] #2203 [#_OFSG[3]]
: : : : :
199 #2199 [#_OFSW[199]] #2399 [#_OFSG[199]]
200 #2200 [#_OFSW[200]] #2400 [#_OFSG[200]]
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 469 -
When bit 3 (V15) of parameter No.6000 = 1
Wear Geometry
Compensation
number Variable
number Variable name Variable
number Variable name
1 #2201 [#_OFSW[1]] #2001 [#_OFSG[1]]
2 #2202 [#_OFSW[2]] #2002 [#_OFSG[2]]
3 #2203 [#_OFSW[3]] #2003 [#_OFSG[3]]
: : : : :
199 #2399 [#_OFSW[199]] #2199 [#_OFSG[199]]
200 #2400 [#_OFSW[200]] #2200 [#_OFSG[200]]
• When the number of compensations is more than 200 (For
compensation with a compensation number of 200 or less,
#2001 to #2400 can also be used.)
When bit 3 (V15) of parameter No.6000 = 0
Geometry Wear
Compensation
number Variable
number Variable name Variable
number Variable name
1 #11001 [#_OFSG[1]] #10001 [#_OFSW[1]]
2 #11002 [#_OFSG[2]] #10002 [#_OFSW[2]]
3 #11003 [#_OFSG[3]] #10003 [#_OFSW[3]]
: : : : :
998 #11998 [#_OFSG[998]] #10998 [#_OFSW[998]]
999 #11999 [#_OFSG[999]] #10999 [#_OFSW[999]]
When bit 3 (V15) of parameter No.6000 = 1
Geometry Wear
Compensation
number Variable
number Variable name Variable
number Variable name
1 #10001 [#_OFSG[1]] #11001 [#_OFSW[1]]
2 #10002 [#_OFSG[2]] #11002 [#_OFSW[2]]
3 #10003 [#_OFSG[3]] #11003 [#_OFSW[3]]
: : : : :
998 #10998 [#_OFSG[998]] #11998 [#_OFSW[998]]
999 #10999 [#_OFSG[999]] #11999 [#_OFSW[999]]
<3> Tool offset memory C
• When the number of compensations is 200 or less
When bit 3 (V15) of parameter No.6000 = 0
H code
Geometry Wear
Compensation
number Variable
number Variable name Variable
number Variable name
1 #2201 [#_OFSHG[1]] #2001 [#_OFSHW[1]]
2 #2202 [#_OFSHG[2]] #2002 [#_OFSHW[2]]
3 #2203 [#_OFSHG[3]] #2003 [#_OFSHW[3]]
: : : : :
199 #2399 [#_OFSHG[199]] #2199 [#_OFSHW[199]]
200 #2400 [#_OFSHG[200]] #2200 [#_OFSHW[200]]
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 470 -
When bit 3 (V15) of parameter No.6000 = 1
H code
Geometry Wear
Compensation
number Variable
number Variable name Variable
number Variable name
1 #2001 [#_OFSHG[1]] #2201 [#_OFSHW[1]]
2 #2002 [#_OFSHG[2]] #2202 [#_OFSHW[2]]
3 #2003 [#_OFSHG[3]] #2203 [#_OFSHW[3]]
: : : : :
199 #2199 [#_OFSHG[199]] #2399 [#_OFSHW[199]]
200 #2200 [#_OFSHG[200]] #2400 [#_OFSHW[200]]
D code
Geometry Wear
Compensation
number Variable
number Variable name Variable
number Variable name
1 #2401 [#_OFSDG[1]] #2601 [#_OFSDW[1]]
2 #2402 [#_OFSDG[2]] #2602 [#_OFSDW[2]]
3 #2403 [#_OFSDG[3]] #2603 [#_OFSDW[3]]
: : : : :
199 #2599 [#_OFSDG[199]] #2799 [#_OFSDW[199]]
200 #2600 [#_OFSDG[200]] #2800 [#_OFSDW[200]]
NOTE
1 When #2401 to #2800 are used for reading or
writing of D codes, bit 5 (D15) of parameter
No.6004 must be set to 1.
2 When bit 5 (D15) of parameter No.6004 is set to 1,
system variables #2500 to #2806 for workpiece
origin offset cannot be used. Use system
variables #5201 to #5324.
• When the number of compensations is more than 200 (For
compensation with a compensation number of 200 or less,
#2001 to #2800 can also be used.)
When bit 3 (V15) of parameter No.6000 = 0
H code
Geometry Wear
Compensation
number Variable
number Variable name Variable
number Variable name
1 #11001 [#_OFSHG[1]] #10001 [#_OFSHW[1]]
2 #11002 [#_OFSHG[2]] #10002 [#_OFSHW[2]]
3 #11003 [#_OFSHG[3]] #10003 [#_OFSHW[3]]
: : : : :
998 #11998 [#_OFSHG[998]] #10998 [#_OFSHW[998]]
999 #11999 [#_OFSHG[999]] #10999 [#_OFSHW[999]]
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 471 -
D code
Geometry Wear
Compensation
number Variable
number Variable name Variable
number Variable name
1 #13001 [#_OFSDG[1]] #12001 [#_OFSDW[1]]
2 #13002 [#_OFSDG[2]] #12002 [#_OFSDW[2]]
3 #13003 [#_OFSDG[3]] #12003 [#_OFSDW[3]]
: : : : :
998 #13998 [#_OFSDG[998]] #12998 [#_OFSDW[99
8]]
999 #13999 [#_OFSDG[999]] #12999 [#_OFSDW[99
9]]
When bit 3 (V15) of parameter No.6000 = 1
H code
Geometry Wear
Compensation
number Variable
number Variable name Variable
number Variable name
1 #10001 [#_OFSHG[1]] #11001 [#_OFSHW[1]]
2 #10002 [#_OFSHG[2]] #11002 [#_OFSHW[2]]
3 #10003 [#_OFSHG[3]] #11003 [#_OFSHW[3]]
: : : : :
998 #10998 [#_OFSHG[998]] #11998 [#_OFSHW[998]]
999 #10999 [#_OFSHG[999]] #11999 [#_OFSHW[999]]
D code
Geometry Wear
Compensation
number Variable
number Variable name Variable
number Variable name
1 #12001 [#_OFSDG[1]] #13001 [#_OFSDW[1]]
2 #12002 [#_OFSDG[2]] #13002 [#_OFSDW[2]]
3 #12003 [#_OFSDG[3]] #13003 [#_OFSDW[3]]
: : : :
998 #12998 [#_OFSDG[998]] #13998 [#_OFSDW[998]]
999 #12999 [#_OFSDG[999]] #13999 [#_OFSDW[999]]
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 472 -
- Tool compensation value #2001-#2964, #10001-#19999 (Attribute: R/W)
T
The compensation values can be obtained by reading system variables
#2001 to #2964 or #10001 to #19999 for tool compensation. The
compensation values can also be changed by assigning values to the
system variables.
<1> Without tool geometry/wear compensation memory
• When the number of compensations is 64 or less
Compensation
number
Variable
number Variable name Description
1 #2001 [#_OFSX[1]]
2 #2002 [#_OFSX[2]]
3 #2003 [#_OFSX[3]]
: : :
63 #2063 [#_OFSX[63]]
64 #2064 [#_OFSX[64]]
X-axis compensation value
(*1)
1 #2101 [#_OFSZ[1]]
2 #2102 [#_OFSZ[2]]
3 #2103 [#_OFSZ[3]]
: : :
63 #2163 [#_OFSZ[63]]
64 #2164 [#_OFSZ[64]]
Z-axis compensation value
(*1)
1 #2201 [#_OFSR[1]]
2 #2202 [#_OFSR[2]]
3 #2203 [#_OFSR[3]]
: : :
63 #2263 [#_OFSR[63]]
64 #2264 [#_OFSR[64]]
Tool nose radius
compensation value
1 #2301 [#_OFST[1]]
2 #2302 [#_OFST[2]]
3 #2303 [#_OFST[3]]
: : :
63 #2363 [#_OFST[63]]
64 #2364 [#_OFST[64]]
Virtual tool tipT position
1 #2401 [#_OFSY[1]]
2 #2402 [#_OFSY[2]]
3 #2403 [#_OFSY[3]]
: : :
48 #2448 [#_OFSY[48]]
49 #2449 [#_OFSY[49]]
Y-axis compensation value
(*1)
(*1) X-axis: X-axis of basic three axes, Z-axis: Z-axis of basic three
axes, Y-axis: Y-axis of basic three axes
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 473 -
• When the number of compensations is more than 64 (For
compensation with a compensation number of 64 or less,
#2001 to #2449 can also be used.)
Compensation
number
Variable
number Variable name Description
1 #10001 [#_OFSX[1]]
2 #10002 [#_OFSX[2]]
3 #10003 [#_OFSX[3]]
: : :
998 #10998 [#_OFSX[998]]
999 #10999 [#_OFSX[999]]
X-axis compensation value
(*1)
1 #11001 [#_OFSZ[1]]
2 #11002 [#_OFSZ[2]]
3 #11003 [#_OFSZ[3]]
: : :
998 #11998 [#_OFSZ[998]]
999 #11999 [#_OFSZ[999]]
Z-axis compensation value
(*1)
1 #12001 [#_OFSR[1]]
2 #12002 [#_OFSR[2]]
3 #12003 [#_OFSR[3]]
: : :
998 #12998 [#_OFSR[998]]
999 #12999 [#_OFSR[999]]
Tool nose radius
compensation value
1 #13001 [#_OFST[1]]
2 #13002 [#_OFST[2]]
3 #13003 [#_OFST[3]]
: : :
998 #13998 [#_OFST[998]]
999 #13999 [#_OFST[999]]
Virtual tool tip T position
1 #14001 [#_OFSY[1]]
2 #14002 [#_OFSY[2]]
3 #14003 [#_OFSY[3]]
: : :
998 #14998 [#_OFSY[998]]
999 #14999 [#_OFSY[999]]
Y-axis compensation value
(*1)
(*1) X-axis: X-axis of basic three axes, Z-axis: Z-axis of basic three
axes, Y-axis: Y-axis of basic three axes
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 474 -
<2> With tool geometry/wear compensation memory
• When the number of compensations is 64 or less
Compensation
number
Variable
number Variable name Description
1 #2001 [#_OFSXW[1]]
2 #2002 [#_OFSXW[2]]
3 #2003 [#_OFSXW[3]]
: : :
63 #2063 [#_OFSXW[63]]
64 #2064 [#_OFSXW[64]]
X-axis compensation value
(wear) (*1)
1 #2101 [#_OFSZW[1]]
2 #2102 [#_OFSZW[2]]
3 #2103 [#_OFSZW[3]]
: : :
63 #2163 [#_OFSZW[63]]
64 #2164 [#_OFSZW[64]]
Z-axis compensation value
(wear) (*1)
1 #2201 [#_OFSRW[1]]
2 #2202 [#_OFSRW [2]]
3 #2203 [#_OFSRW [3]]
: : :
63 #2263 [#_OFSRW [63]]
64 #2264 [#_OFSRW [64]]
Tool nose radius
compensation value (wear)
1 #2301 [#_OFST[1]]
2 #2302 [#_OFST[2]]
3 #2303 [#_OFST[3]]
: : :
63 #2363 [#_OFST[63]]
64 #2364 [#_OFST[64]]
Virtual tool tip T position
1 #2401 [#_OFSYW[1]]
2 #2402 [#_OFSYW [2]]
3 #2403 [#_OFSYW [3]]
: : :
48 #2448 [#_OFSYW [48]]
49 #2449 [#_OFSYW [49]]
Y-axis compensation value
(wear) (*1)
1 #2451 [#_OFSYG[1]]
2 #2452 [#_OFSYG [2]]
3 #2453 [#_OFSYG [3]]
: : :
48 #2498 [#_OFSYG [48]]
49 #2499 [#_OFSYG [49]]
Y-axis compensation value
(geometry) (*1)
1 #2701 [#_OFSXG[1]]
2 #2702 [#_OFSXG[2]]
3 #2703 [#_OFSXG [3]]
: : :
48 #2748 [#_OFSXG [48]]
49 #2749 [#_OFSXG [49]]
X-axis compensation value
(geometry) (*1)
1 #2801 [#_OFSZG[1]]
2 #2802 [#_OFSZG[2]]
3 #2803 [#_OFSZG[3]]
: : :
48 #2848 [#_OFSZG[48]]
49 #2849 [#_OFSZG[49]]
Z-axis compensation value
(geometry) (*1)
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 475 -
Compensation
number
Variable
number Variable name Description
1 #2901 [#_OFSRG[1]]
2 #2902 [#_OFSRG[2]]
3 #2903 [#_OFSRG[3]]
: : :
63 #2963 [#_OFSRG[63]]
64 #2964 [#_OFSRG[64]]
Tool nose radius
compensation value
(geometry)
1 #19001 [#_OFSYG[1]]
2 #19002 [#_OFSYG[2]]
3 #19003 [#_OFSYG[3]]
: : :
998 #19998 [#_OFSYG[998]]
999 #19999 [#_OFSYG[999]]
Y-axis compensation value
(geometry) (*1)
(*1) X-axis: X-axis of basic three axes, Z-axis: Z-axis of basic three
axes, Y-axis: Y-axis of basic three axes
• When the number of compensations is more than 64 (For
compensation with a compensation number of 64 or less,
#2001 to #2964 or #10001 to #19999 can also be used.)
Compensation
number
Variable
number Variable name Description
1 #10001 [#_OFSXW[1]]
2 #10002 [#_OFSXW[2]]
3 #10003 [#_OFSXW[3]]
: : :
998 #10998 [#_OFSXW[998]]
999 #10999 [#_OFSXW[999]]
X-axis compensation value
(wear) (*1)
1 #11001 [#_OFSZW[1]]
2 #11002 [#_OFSZW[2]]
3 #11003 [#_OFSZW[3]]
: : :
998 #11998 [#_OFSZW[998]]
999 #11999 [#_OFSZW[999]]
Z-axis compensation value
(wear) (*1)
1 #12001 [#_OFSRW[1]]
2 #12002 [#_OFSRW [2]]
3 #12003 [#_OFSRW [3]]
: : :
998 #12998 [#_OFSRW [998]]
999 #12999 [#_OFSRW [999]]
Tool nose radius
compensation value (wear)
1 #13001 [#_OFST[1]]
2 #13002 [#_OFST[2]]
3 #13003 [#_OFST[3]]
: : :
998 #13998 [#_OFST[998]]
999 #13999 [#_OFST[999]]
Virtual tool tip T position
1 #14001 [#_OFSYW[1]]
2 #14002 [#_OFSYW [2]]
3 #14003 [#_OFSYW [3]]
: : :
998 #14998 [#_OFSYW [998]]
999 #14999 [#_OFSYW [999]]
Y-axis compensation value
(wear) (*1)
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 476 -
Compensation
number
Variable
number Variable name Description
1 #15001 [#_OFSXG[1]]
2 #15002 [#_OFSXG[2]]
3 #15003 [#_OFSXG [3]]
: : :
998 #15998 [#_OFSXG [998]]
999 #15999 [#_OFSXG [999]]
X-axis compensation value
(geometry) (*1)
1 #16001 [#_OFSZG[1]]
2 #16002 [#_OFSZG[2]]
3 #16003 [#_OFSZG[3]]
: : :
998 #16998 [#_OFSZG[998]]
999 #16999 [#_OFSZG[999]]
Z-axis compensation value
(geometry) (*1)
1 #17001 [#_OFSRG[1]]
2 #17002 [#_OFSRG[2]]
3 #17003 [#_OFSRG[3]]
: : :
998 #17998 [#_OFSRG[998]]
999 #17999 [#_OFSRG[999]]
Tool nose radius
compensation value
(geometry)
1 #19001 [#_OFSYG[1]]
2 #19002 [#_OFSYG[2]]
3 #19003 [#_OFSYG[3]]
: : :
998 #19998 [#_OFSYG[998]]
999 #19999 [#_OFSYG[999]]
Y-axis compensation value
(geometry) (*1)
(*1) X-axis: X-axis of basic three axes, Z-axis: Z-axis of basic three
axes, Y-axis: Y-axis of basic three axes
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 477 -
- Alarm #3000 (Attribute: W)
When an error is detected in a macro, an unit can enter the alarm state.
In addition, an alarm message of up to 60 characters with alphabet and
numerals can be specified between a control-out and a control-in after
the expression. When an alarm message is not specified, a macro
alarm is used instead.
Variable
number Variable name Description
#3000 [#_ALM] Macro alarm
When bit 1 (MCA) of parameter No.6008 = 0
#3000 = n (ALARM MESSAGE); (n: 0-200)
On the screen, the alarm number obtained by adding the value of
#3000 to 3000 and alarm message appear.
(Example) #3000 = 1 (ALARM MESSAGE);
→ "3001 ALARM MESSAGE" appears on the alarm
screen.
When bit 1 (MCA) of parameter No.6008 = 1
#3000 = n (ALARM MESSAGE); (n: 0-4095)
On the screen, the alarm number of #3000 and alarm message
appear after MC.
(Example) #3000=1 (ALARM MESSAGE);
→ "MC0001 ALARM MESSAGE" appears on the alarm
screen.
- Clock #3001, #3002 (Attribute: R/W)
The clock time can be obtained by reading system variables #3001
and #3002 for clocks. The time can be preset by entering a value in
the system variables.
Type Variable
number
Variable
name Unit At power-on Count
condition
Clock 1 #3001 [#_CLOCK1] 1 ms Reset to 0 Anytime
Clock 2 #3002 [#_CLOCK2] 1 hour Same as at
power-down
When the STL
signal is on
The clock accuracy is 16 ms. Clock 1 returns to 0 after a lapse of
2147483648 ms. Clock 2 returns to 0 after a lapse of 9544.37176
hours.
[Example]
Timer
Macro calling command
G65 P9101 T (wait time) ms ;
A macro is created as follows.
O9101;
#3001 = 0; Initial setting
WHILE [#3001 LE #20] DO1: Wait for a specified time
END1 ;
M99 ;
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 478 -
- Controlling of single block stop and waiting for the auxiliary function completion
signal #3003 (Attribute: R/W)
Assigning the following values in system variable #3003 allows the
specification of whether single block stop is disabled in the following
blocks or whether a wait for the completion signal (FIN) of the
auxiliary function (M, S, T, or B) before going to the next block is
enabled. When a wait for completion signal is disabled, the
distribution end signal (DEN) is not sent. Be careful not to specify
the next auxiliary function without waiting for the completion signal.
Variable number and
variable name Value Single block stop Auxiliary function
completion signal
0 Enabled Waiting
1 Disabled Waiting
2 Enabled Not waiting
#3003
[#_CNTL1]
3 Disabled Not waiting
In addition, the following variable names can be used to enable or
disable single block stop and a wait for the auxiliary function
completion signal, individually.
Variable name Value Single block stop Auxiliary function
completion
0 Enabled -
[#_M_SBK] 1 Disabled -
0 - Waiting
[#_M_FIN] 1 - Not waiting
[Example]
Drill cycle (for incremental programming)
(G81 equivalent)
Macro calling command
G65 P9081 L Iterations R R point Z Z point;
A custom macro body is created as follows.
O9081 ;
#3003 = 1 ;
G00 Z#18 ;
G01 Z#26 ;
G00 Z-[ ROUND[#18] + ROUND[#26] ] ;
#3003 = 0 ;
M99 ;
NOTE
#3003 is cleared by a reset.
Disable single block stop.
#18 corresponds to R and
#26 to Z.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 479 -
- Enabling of feed hold, feedrate override, and exact stop check #3004
(Attribute: R/W)
Assigning the following values in system variable #3004 allows the
specification of whether feed hold and feedrate override are enabled in
the following blocks or whether exact stop in G61 mode or by G09
command is disabled.
Variable number and
variable name Value Field hold Feedrate
override Exact stop
0 Enabled Enabled Enabled
1 Disabled Enabled Enabled
2 Enabled Disabled Enabled
3 Disabled Disabled Enabled
4 Enabled Enabled Disabled
5 Disabled Enabled Disabled
6 Enabled Disabled Disabled
#3004
[#_CNTL2]
7 Disabled Disabled Disabled
In addition, the following variable names can be used to enable or
disable feed hold, feedrate override, and exact stop in G61 mode or by
the G09 command, individually.
Variable number and
variable name Value Feed hold Feedrate
override Exact stop
0 Enabled - -
[#_M_FHD] 1 Disabled - -
0 - Enabled -
[#_M_OV] 1 - Disabled -
0 - - Enabled
[#_M_EST] 1 - - Disabled
NOTE
1 These system variables are provided to maintain
compatibility with conventional NC programs. It is
recommended that functions provided by G63, G09,
G61, and other G codes be used to enable or
disable feed hold, feedrate override, and exact stop.
2 When the feed hold button is pressed during
execution of a block for which feed hold is disabled:
<1> If the feed hold button is kept pressed,
operation stops after execution of the block.
When single block stop is disabled, however,
operation does not stop.
<2> If the pressed feed hold button is released, the
feed hold lamp lights, but operation does not
stop until the end of the first block that was
enabled.
3 #3004 is cleared by a reset.
4 If exact stop is disabled by #3004, the original exact
stop position between cutting feed and positioning
block is not affected. #3004 can temporarily
disable exact stop in G61 mode or by the G09
command between cutting feed and cutting feed.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 480 -
- Settings #3005 (Attribute: R/W)
Settings can be read and written.
Binary values are converted to decimals.
#3005
#15 #14 #13 #12 #11 #10 #9 #8
Setting
FCV
#7 #6 #5 #4 #3 #2 #1 #0
Setting
SEQ
INI ISO TVC
#9 (FCV) : Whether to use the FANUC Series 15 program format
conversion capability
#5 (SEQ) : Whether to automatically insert sequence numbers
#2 (INI) : Millimeter input or inch input
#1 (ISO) : Whether to use EIA or ISO as the output code
#0 (TVC) : Whether to make a TV check
- Stop with a message #3006 (Attribute: W)
When "#3006=1 (MESSAGE);" is commanded in the macro, the
program executes blocks up to the immediately previous one and then
stops. When a message of up to 60 characters with alphabet and
numerals, which is enclosed by a control-in character and control-out
character, is programmed in the same block, the message is displayed
on the external operator message screen.
Variable number Variable name Description
#3006 [#_MSGSTP] Stop with a message
- Status of a mirror image #3007 (Attribute: R)
The status of an mirror image (setting or DI) at that point in time can
be obtained for each axis by reading #3007.
Variable number Variable name Description
#3007 [#_MRIMG] Status of a mirror image
When the status is indicated in binary, each bit corresponds with an
axis as follows.
Bit 31 30 29 28 27 26 25 24 23 22 21 20 19 18 17 16
nth axis 32 31 30 29 28 27 26 25 24 23 22 21 20 19 18 17
Bit 15 14 13 12 11 10 9 8 7 6 5 4 3 2 1 0
nth axis 16 15 14 13 12 11 10 9 8 7 6 5 4 3 2 1
For the 32 bits, 0 indicates that a mirror image is disabled and 1
indicates that a mirror image is enabled.
[Example] When #3007 is 3, a mirror image is enabled for the 1st and 2nd
axes.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 481 -
NOTE
1 The status of a programmable mirror image is not
reflected on this variable.
2 When the mirror image function is set for the same
axis by the mirror image signal and setting, the
signal value and setting value are ORed and then
output.
3 When mirror image signals for axes other than the
controlled axes are turned on, they are not read
into system variable #3007.
- Status during restart of a program #3008 (Attribute: R)
Whether a program is restarting can be determined by reading #3008.
Variable number Variable name Description
#3008 [#_PRSTR] 0: Program is not restarting.
1: Program is restarting.
- Time #3011, #3012 (Attribute: R)
Year/month/date and hour/minute/second can be obtained by reading
system variables #3011 and #3012. This variable is read-only. To
change year/month/date and hour/minute/second, use the timer screen.
[Example] May 20, 2004, PM 04:17:05
#3011 = 20040520
#3012 = 161705
- Total number of parts and the number of required parts #3901 and #3902
(Attribute: R/W)
The number of required parts and the number of machined parts can
be displayed on the screen by using the operation time and part
number displaying function. When the (total) number of machined
parts reaches the number of required parts, a signal indicating the fact
is sent to the machine (PMC side).
The system variables can be used to read or write the total number of
parts and the number of required parts.
Variable number Variable name Description
#3901 [#_PRTSA] Total number of parts
#3902 [#_PRTSN] Number of required parts
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 482 -
- Type of tool compensation memory #3980 (Attribute: R)
M
System variable #3980 can be used to read the type of compensation
memory.
Variable number Variable name Description
#3980 [#_OFSMEM] Types of tool compensation memory
0: Tool compensation memory A
1: Tool compensation memory B
2: Tool compensation memory C
- Main program number #4000 (Attribute: R)
System variable #4000 can be used to read the main program number
regardless of the level of a subprogram.
Variable number Variable name Description
#4000 [#_MAINO] Main program number
NOTE
1 The main program number indicates the number of
the program that is first started.
2 When an O number is specified by MDI during
execution of the main program or when the second
O number is specified in DNC mode, the value of
#4000 changes to the specified O number. In
addition, when no programs are registered or when
no O numbers are specified in DNC mode, the
value of #4000 changes to 0.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 483 -
- Modal information #4001-#4130, #4201-#4330, #4401-#4530 (Attribute: R)
The modal information specified before the previous block of the
macro statement that reads system variables #4001 to #4130 can be
obtained in the block currently being looked ahead, by reading system
variables #4001 to #4130.
The modal information of the block currently being executed can be
obtained by reading system variables #4201 to #4330.
The modal information specified before the block interrupted by an
interruption type custom macro by reading system variables #4401 to
#4530.
The unit used when it was specified is applied.
M
(Category: <1> Previous block, <2> Running block, <3>
Interrupted block)
Category Variable
number
Variable
name Description
<1>
<2>
<3>
#4001
#4201
#4401
[#_BUFG[1]]
[#_ACTG[1]]
[#_INTG[1]]
Modal information (G code: group 1)
<1>
<2>
<3>
#4002
#4202
#4402
[#_BUFG[2]]
[#_ACTG[2]]
[#_INTG[2]]
Modal information (G code: group 2)
:
:
:
:
:
:
:
:
<1>
<2>
<3>
#4030
#4230
#4430
[#_BUFG[30]]
[#_ACTG[30]]
[#_INTG[30]]
Modal information
(G code: group 30)
<1>
<2>
<3>
#4102
#4302
#4502
[#_BUFB]
[#_ACTB]
[#_INTB]
Modal information (B code)
<1>
<2>
<3>
#4107
#4307
#4507
[#_BUFD]
[#_ACTD]
[#_INTD]
Modal information (D code)
<1>
<2>
<3>
#4108
#4308
#4508
[#_BUFE]
[#_ACTE]
[#_INTE]
Modal information (E code)
<1>
<2>
<3>
#4109
#4309
#4509
[#_BUFF]
[#_ACTF]
[#_INTF]
Modal information (F code)
<1>
<2>
<3>
#4111
#4311
#4511
[#_BUFH]
[#_ACTH]
[#_INTH]
Modal information (H code)
<1>
<2>
<3>
#4113
#4313
#4513
[#_BUFM]
[#_ACTM]
[#_INTM]
Modal information (M code)
<1>
<2>
<3>
#4114
#4314
#4514
[#_BUFN]
[#_ACTN]
[#_INTN]
Modal information
(sequence number N)
<1>
<2>
<3>
#4115
#4315
#4515
[#_BUFO]
[#_ACTO]
[#_INTO]
Modal information
(program number O)
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 484 -
Category Variable
number
Variable
name Description
<1>
<2>
<3>
#4119
#4319
#4519
[#_BUFS]
[#_ACTS]
[#_INTS]
Modal information (S code)
<1>
<2>
<3>
#4120
#4320
#4520
[#_BUFT]
[#_ACTT]
[#_INTT]
Modal information (T code)
<1>
<2>
<3>
#4130
#4330
#4530
[#_BUFWZP]
[#_ACTWZP]
[#_INTWZP]
Modal information
(additional workpiece coordinate
system number P)
T
(Category: <1> Previous block, <2> Running block, <3>
Interrupted block)
Category Variable
number
Variable
name Description
<1>
<2>
<3>
#4001
#4201
#4401
[#_BUFG[1]]
[#_ACTG[1]]
[#_INTG[1]]
Modal information (G code: group 1)
<1>
<2>
<3>
#4002
#4202
#4402
[#_BUFG[2]]
[#_ACTG[2]]
[#_INTG[2]]
Modal information (G code: group 2)
:
:
:
:
:
:
:
:
<1>
<2>
<3>
#4030
#4230
#4430
[#_BUFG[30]]
[#_ACTG[30]]
[#_INTG[30]]
Modal information
(G code: group 30)
<1>
<2>
<3>
#4108
#4308
#4508
[#_BUFE]
[#_ACTE]
[#_INTE]
Modal information (E code)
<1>
<2>
<3>
#4109
#4309
#4509
[#_BUFF]
[#_ACTF]
[#_INTF]
Modal information (F code)
<1>
<2>
<3>
#4113
#4313
#4513
[#_BUFM]
[#_ACTM]
[#_INTM]
Modal information (M code)
<1>
<2>
<3>
#4114
#4314
#4514
[#_BUFN]
[#_ACTN]
[#_INTN]
Modal information
(sequence number N)
<1>
<2>
<3>
#4115
#4315
#4515
[#_BUFO]
[#_ACTO]
[#_INTO]
Modal information
(program number O)
<1>
<2>
<3>
#4119
#4319
#4519
[#_BUFS]
[#_ACTS]
[#_INTS]
Modal information (S code)
<1>
<2>
<3>
#4120
#4320
#4520
[#_BUFT]
[#_ACTT]
[#_INTT]
Modal information (T code)
<1>
<2>
<3>
#4130
#4330
#4530
[#_BUFWZP]
[#_ACTWZP]
[#_INTWZP]
Modal information
(additional workpiece coordinate
system number P)
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 485 -
NOTE
1 Previous block and running block
Since the CNC reads the block that is ahead of the
block currently being executed by the machining
program, the block being retrieved by the CNC is
normally different from that currently being
executed. The previous block indicates the block
that is ahead of the block being retrieved by the
CNC, that is, the block that is ahead of the program
block in which #4001 to #4130 are specified.
2 When variables exceeding the number of control
axes are specified, the alarm PS0115, “VARIABLE
NO. OUT OF RANGE” occurs.
[Example] O1234 ;
N10 G00 X200. Y200. ;
N20 G01 X1000. Y1000. F10. ;
:
:
N50 G00 X500. Y500. ;
N60 #1 = #4001 ;
Assume that the CNC is currently executing N20. If the CNC retrieved and
processed the blocks up to N60 as shown above, the running block is N20 and
the previous block is N50. Therefore, group 1 modal information in the
running block is G01 and group 1 modal information in the previous block is
G00.
When N60 #1 = #4201, #1 = 1.
When N60 #1 = #4001, #1 = 0.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 486 -
- Position information #5001-#5080, #100001-#100200 (Attribute: R)
The end position of the previous block, the specified current position
(for the machine coordinate system and workpiece coordinate system),
and the skip signal position can be obtained by reading the values of
system variables #5001 to #5080 or #100001 to -#100200.
Variable
number Variable name Position information Coordinate
system
Tool position/tool
length/cutter
compensation
Reading
operation during
movement
#5001
#5002
:
#5020
[#_ABSIO[1]]
[#_ABSIO[2]]
:
[#_ABSIO[20]]
1st axis block end point position
2nd axis block end point position
:
20th axis block end point position
#100001
#100002
:
#100050
[#_ABSIO[1]]
[#_ABSIO[2]]
:
[#_ABSIO[50]]
1st axis block end point position
2nd axis block end point position
:
50th axis block end point position
Workpiece
coordinate
system
Not included Enabled
#5021
#5022
:
#5040
[#_ABSMT[1]]
[#_ABSMT[2]]
:
[#_ABSMT[20]]
1st axis current position
2nd axis current position
:
20th axis current position
#100051
#100052
:
#100100
[#_ABSMT[1]]
[#_ABSMT[2]]
:
[#_ABSMT[50]]
1st axis current position
2nd axis current position
:
50th axis current position
Machine
coordinate
system
Included Disabled
#5041
#5042
:
#5060
[#_ABSOT[1]]
[#_ABSOT[2]]
:
[#_ABSOT[20]]
1st axis current position
2nd axis current position
:
20th axis current position
#100101
#100102
:
#100150
[#_ABSOT[1]]
[#_ABSOT[2]]
:
[#_ABSOT[50]]
1st axis current position
2nd axis current position
:
50th axis current position
Workpiece
coordinate
system
Included Disabled
#5061
#5062
:
#5080
[#_ABSKP[1]]
[#_ABSKP[2]]
:
[#_ABSKP[20]]
1st axis skip position
2nd axis skip position
:
20th axis skip position
#100151
#100152
:
#100200
[#_ABSKP[1]]
[#_ABSKP[2]]
:
[#_ABSKP[50]]
1st axis skip position
2nd axis skip position
:
50th axis skip position
Workpiece
coordinate
system
Included Enabled
NOTE
1 When variables exceeding the number of control axes are specified, the alarm
PS0115, “VARIABLE NO. OUT OF RANGE” occurs.
2 The position information for 20th or earlier axis can be used with #5001 to #5080.
3 The block end point position (ABSIO) of the skip (G31) is the position where the
skip signal is turned on. If the skip signal is not turned on, the position is the end
position of the block.
4 "Read operation during movement is disabled" means that the accurate reading of
values during movement is not guaranteed.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 487 -
- Tool length compensation value #5081-#5100, #100201-#100250 (Attribute: R)
M
Tool length compensation in the block currently being executed can
be obtained for each axis by reading system variables #5081 to #5100
or #100201 to #100250.
Variable
number
Variable
name Position information
Read operation
during
movement
#5081
#5082
:
#5100
[#_TOFS[1]]
[#_TOFS[2]]
:
[#_TOFS[20]]
1st axis tool length compensation value
2nd axis tool length compensation value
:
20th axis tool length compensation value
#100201
#100202
:
#100250
[#_TOFS[1]]
[#_TOFS[2]]
:
[#_TOFS[50]]
1st axis tool length compensation value
2nd axis tool length compensation value
:
50th axis tool length compensation value
Disabled
NOTE
1 When variables exceeding the number of control
axes are specified, the alarm PS0115, “VARIABLE
NO. OUT OF RANGE” occurs.
2 The tool length compensation for 20th or earlier
axis can also be used with #5081 to #5100.
- Tool offset #5081-#5083, #5121-#5123 (Attribute: R)
#100201-#100250, #100901-#100950
T
Tool offset in the block currently being executed can be obtained for
each axis by reading system variables #5081 to #5083 or #5121 to
#5123. (X-axis: X-axis of basic three axes, Z-axis: Z-axis of basic
three axes, Y-axis: Y-axis of basic three axes)
<1> Without tool geometry/wear compensation memory
Variable
number Variable name Position information
Read operation
during
movement
#5081
#5082
#5083
#5084
:
#5100
[#_TOFSWX]
[#_TOFSWZ]
[#_TOFSWY]
[#_TOFS[4]]
:
[#_TOFS[20]]
X-axis tool offset value
Z-axis tool offset value
Y-axis tool offset value
4th axis tool offset value
:
20th axis tool offset value
#100201
#100202
#100203
#100204
:
#100250
[#_TOFSWX]
[#_TOFSWZ]
[#_TOFSWY]
[#_TOFS[4]]
:
[#_TOFS[50]]
X-axis tool offset value
Z-axis tool offset value
Y-axis tool offset value
4th axis tool offset value
:
50th axis tool offset value
Disabled
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 488 -
<2> With tool geometry/wear compensation memory
Variable
number Variable name Position information
Read operation
during
movement
#5081
#5082
#5083
#5084
:
#5100
[#_TOFSWX]
[#_TOFSWZ]
[#_TOFSWY]
[#_TOFS[4]]
:
[#_TOFS[20]]
X-axis tool offset value (geometry)
Z-axis tool offset value (geometry)
Y-axis tool offset value (geometry)
4th axis tool offset value (geometry)
:
20th axis tool offset value (geometry)
#100201
#100202
#100203
#100204
:
#100250
[#_TOFSWX]
[#_TOFSWZ]
[#_TOFSWY]
[#_TOFS[4]]
:
[#_TOFS[50]]
X-axis tool offset value (geometry)
Z-axis tool offset value (geometry)
Y-axis tool offset value (geometry)
4th axis tool offset value (geometry)
:
50th axis tool offset value (geometry)
#5121
#5122
#5123
#5124
:
#5140
[#_TOFSGX]
[#_TOFSGZ]
[#_TOFSGY]
[#_TOFSG[4]]
:
[#_TOFSG[20]]
X-axis tool offset value (geometry)
Z-axis tool offset value (geometry)
Y-axis tool offset value (geometry)
4th axis tool offset value (geometry)
:
20th axis tool offset value (geometry)
#100901
#100902
#100903
#100904
:
#100950
[#_TOFSGX]
[#_TOFSGZ]
[#_TOFSGY]
[#_TOFSG[4]]
:
[#_TOFSG[50]]
X-axis tool offset value (geometry)
Z-axis tool offset value (geometry)
Y-axis tool offset value (geometry)
4th axis tool offset value (geometry)
:
50th axis tool offset value (geometry)
Disabled
When tool geometry/wear compensation memory exists, the system
variable values vary as follows depending on parameter LWT
(No.5002#2) and parameter LGT (No.5002#4).
Variable
number
LWT=0
LGT=0
LWT=1
LGT=0
LWT=0
LGT=1
LWT=1
LGT=1
#5081
#5082
#5083
Wear
compensation 0 Wear
compensation
Wear
compensation
#5121
#5122
#5123
Geometry
compensation
Wear
compensation +
Geometry
compensation
Geometry
compensation
Geometry
compensation
NOTE
1 The set value is read as the tool offset regardless
of bit 1 (ORC) of parameter No.5004 and bit 0
(OWD) of parameter No.5040.
2 To read the tool offset (geometry) using #5121 to
#5123, set bit 2 (VHD) of parameter No.6004 to 0.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 489 -
- Servo position deviation #5101-#5120, #100251-#100300 (Attribute: R)
The servo position deviation for each axis can be obtained by reading
system variables #5101 to #5120 or #100251 to #100300.
Variable
number Variable name Position information
Read operation
during
movement
#5101
#5102
:
#5120
[#_SVERR[1]]
[#_SVERR[2]]
:
[#_SVERR[20]]
1st axis servo position deviation
2nd axis servo position deviation
:
20th axis servo position deviation
#100251
#100252
:
#100300
[#_SVERR[1]]
[#_SVERR[2]]
:
[#_SVERR[50]]
1st axis servo position deviation
2nd axis servo position deviation
:
50th axis servo position deviation
Disabled
NOTE
1 When variables exceeding the number of control
axes are specified, the alarm PS0115, “VARIABLE
NO. OUT OF RANGE” occurs.
2 The servo position deviation for 20th or earlier axis
can be used with #5101 to #5120.
- Manual handle interruption #5121-#5140, #100651-#100700 (Attribute: R)
The manual handle interruption for each axis can be obtained by
reading system variables #5121 to #5140 or #100651 to #100700.
Variable
number
Variable
name Position information
Read operation
during
movement
#5121
#5122
:
#5140
[#_MIRTP[1]]
[#_MIRTP[2]]
:
[#_MIRTP[20]]
1st axis manual handle interruption
2nd axis manual handle interruption
:
20th axis manual handle interruption
#100651
#100652
:
#100700
[#_MIRTP[1]]
[#_MIRTP[2]]
:
[#_MIRTP[50]]
1st axis manual handle interruption
2nd axis manual handle interruption
:
50th axis manual handle interruption
Disabled
NOTE
1 When variables exceeding the number of control
axes are specified, the alarm PS0115, “VARIABLE
NO. OUT OF RANGE” occurs.
2 The manual handle interruption for 20th or earlier
axis can be used with #5121 to #5140.
T
NOTE
#5121 to #5140 are enabled only when bit 2 (VHD)
of parameter No.6004 is set to 1.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 490 -
- Distance to go #5181-#5200, #100801-#100850 (Attribute: R)
The distance to go value for each axis can be obtained by reading
system variables #5181 to #5200 or #100801 to #100850.
Variable
number
Variable
name Position information Read operation
during movement
#5181
#5182
:
#5200
[#_DIST[1]]
[#_DIST[2]]
:
[#_DIST[20]]
1st axis distance to go value
2nd axis distance to go value
:
20th axis distance to go value
#100801
#100802
:
#100850
[#_DIST[1]]
[#_DIST[2]]
:
[#_DIST[50]]
1st axis distance to go value
2nd axis distance to go value
:
50th axis distance to go value
Disabled
NOTE
1 When variables exceeding the number of control
axes are specified, the alarm PS0115, “VARIABLE
NO. OUT OF RANGE” occurs.
2 The distance to go values for 20th or earlier axis
can be used with #5181 to #5200.
- Workpiece coordinate system shift value #2501, #2601 (Attribute: R/W)
T
The X-axis workpiece coordinate system shift value can be obtained
by system variable #2501 while Z-axis workpiece coordinate system
shift value by system variable #2601. Each workpiece coordinate
system shift value can be obtained by system variable
#100751-#100800. The X-axis or Z-axis workpiece coordinate
system shift value can be changed by assigning values to the system
variables. (X-axis: X-axis of basic three axes, Z-axis: Z-axis of basic
three axes, Y-axis: Y-axis of basic three axes)
Variable number Variable name Description
#2501 [#_WZ_SFTX] X-axis workpiece shift value
#2601 [#_WZ_SFTZ] Z-axis workpiece shift value
#100751
#100752
:
#100800
[#_WZ_SFT[1]]
[#_WZ_SFT [2]]
:
[#_WZ_SFT [50]]
1st axis workpiece shift value
2nd axis workpiece shift value
:
50th axis workpiece shift value
NOTE
1 The value of a variable with a number greater than
the number of controlled axes is undefined.
2 The X-axis of three basic axes can also be used in
system variable #2501, and the Z-axis of three basic
axes can also be used in system variable #2601.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 491 -
- Workpiece origin offset value #5201-#5340, #100301-#100650 (Attribute: R/W)
The workpiece origin offset value can be obtained by reading system
variables #5201 to #5340 or #100301 to #100650. The offset value
can also be changed by assigning values to the system variables.
Variable
number Variable name Controlled axis Workpiece
coordinate system
#5201
#5202
:
#5220
[#_WZCMN[1]]
[#_WZCMN[2]]
:
[#_WZCMN[20]]
1st axis external workpiece origin offset value
2nd axis external workpiece origin offset value
:
20th axis external workpiece origin offset value
External workpiece
origin offset value
(applied to all
coordinate systems)
#5221
#5222
:
#5240
[#_WZG54[1]]
[#_WZG54[2]]
:
[#_WZG54[20]]
1st axis workpiece origin offset value
2nd axis workpiece origin offset value
:
20th axis workpiece origin offset value
G54
#5241
#5242
:
#5260
[#_WZG55[1]]
[#_WZG55[2]]
:
[#_WZG55[20]]
1st axis workpiece origin offset value
2nd axis workpiece origin offset value
:
20th axis workpiece origin offset value
G55
#5261
#5262
:
#5280
[#_WZG56[1]]
[#_WZG56[2]]
:
[#_WZG56[20]]
1st axis workpiece origin offset value
2nd axis workpiece origin offset value
:
20th axis workpiece origin offset value
G56
#5281
#5282
:
#5300
[#_WZG57[1]]
[#_WZG57[2]]
:
[#_WZG57[20]]
1st axis workpiece origin offset value
2nd axis workpiece origin offset value
:
20th axis workpiece origin offset value
G57
#5301
#5302
:
#5320
[#_WZG58[1]]
[#_WZG58[2]]
:
[#_WZG58[20]]
1st axis workpiece origin offset value
2nd axis workpiece origin offset value
:
20th axis workpiece origin offset value
G58
#5321
#5322
:
#5340
[#_WZG59[1]]
[#_WZG59[2]]
:
[#_WZG59[20]]
1st axis workpiece origin offset value
2nd axis workpiece origin offset value
:
20th axis workpiece origin offset value
G59
#100301
#100302
:
#100350
[#_WZCMN[1]]
[#_WZCMN[2]]
:
[#_WZCMN[50]]
1st axis external workpiece origin offset value
2nd axis external workpiece origin offset value
:
50th axis external workpiece origin offset value
External workpiece
origin offset value
(applied to all
coordinate systems)
#100351
#100352
:
#100400
[#_WZG54[1]]
[#_WZG54[2]]
:
[#_WZG54[50]]
1st axis workpiece origin offset value
2nd axis workpiece origin offset value
:
50th axis workpiece origin offset value
G54
#100401
#100402
:
#100450
[#_WZG55[1]]
[#_WZG55[2]]
:
[#_WZG55[50]]
1st axis workpiece origin offset value
2nd axis workpiece origin offset value
:
50th axis workpiece origin offset value
G55
#100451
#100452
:
#100500
[#_WZG56[1]]
[#_WZG56[2]]
:
[#_WZG56[50]]
1st axis workpiece origin offset
2nd axis workpiece origin offset
:
50th axis workpiece origin offset
G56
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 492 -
Variable
number Variable name Controlled axis Workpiece
coordinate system
#100501
#100502
:
#100550
[#_WZG57[1]]
[#_WZG57[2]]
:
[#_WZG57[50]]
1st axis workpiece origin offset
2nd axis workpiece origin offset
:
50th axis workpiece origin offset
G57
#100551
#100552
:
#100600
[#_WZG58[1]]
[#_WZG58[2]]
:
[#_WZG58[50]]
1st axis workpiece origin offset
2nd axis workpiece origin offset
:
50th axis workpiece origin offset
G58
#100601
#100602
:
#100650
[#_WZG59[1]]
[#_WZG59[2]]
:
[#_WZG59[50]]
1st axis workpiece origin offset
2nd axis workpiece origin offset
:
50th axis workpiece origin offset
G59
M
The following variables can also be used when bit 5 (D15) of
parameter No. 6004 is set to 0:
Axis Function
Variable
number
1st axis External workpiece origin offset value #2500
G54 workpiece origin offset value #2501
G55 workpiece origin offset value #2502
G56 workpiece origin offset value #2503
G57 workpiece origin offset value #2504
G58 workpiece origin offset value #2505
G59 workpiece origin offset value #2506
2nd axis External workpiece origin offset value #2600
G54 workpiece origin offset value #2601
G55 workpiece origin offset value #2602
G56 workpiece origin offset value #2603
G57 workpiece origin offset value #2604
G58 workpiece origin offset value #2605
G59 workpiece origin offset value #2606
3rd axis External workpiece origin offset value #2700
G54 workpiece origin offset value #2701
G55 workpiece origin offset value #2702
G56 workpiece origin offset value #2703
G57 workpiece origin offset value #2704
G58 workpiece origin offset value #2705
G59 workpiece origin offset value #2706
4th axis External workpiece origin offset value #2800
G54 workpiece origin offset value #2801
G55 workpiece origin offset value #2802
G56 workpiece origin offset value #2803
G57 workpiece origin offset value #2804
G58 workpiece origin offset value #2805
G59 workpiece origin offset value #2806
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 493 -
T
The following variables can be used to maintain compatibility with
conventional models.
Axis Function
Variable
number
1st axis External workpiece origin offset value #2550
G54 workpiece origin offset value #2551
G55 workpiece origin offset value #2552
G56 workpiece origin offset value #2553
G57 workpiece origin offset value #2554
G58 workpiece origin offset value #2555
G59 workpiece origin offset value #2556
2nd axis External workpiece origin offset value #2650
G54 workpiece origin offset value #2651
G55 workpiece origin offset value #2652
G56 workpiece origin offset value #2653
G57 workpiece origin offset value #2654
G58 workpiece origin offset value #2655
G59 workpiece origin offset value #2656
3rd axis External workpiece origin offset value #2750
G54 workpiece origin offset value #2751
G55 workpiece origin offset value #2752
G56 workpiece origin offset value #2753
G57 workpiece origin offset value #2754
G58 workpiece origin offset value #2755
G59 workpiece origin offset value #2756
4th axis External workpiece origin offset value #2850
G54 workpiece origin offset value #2851
G55 workpiece origin offset value #2852
G56 workpiece origin offset value #2853
G57 workpiece origin offset value #2854
G58 workpiece origin offset value #2855
G59 workpiece origin offset value #2856
NOTE
1 When variables exceeding the number of control
axes are specified, the alarm PS0115, “VARIABLE
NO. OUT OF RANGE” occurs.
2 The workpiece origin offset value for 20th or earlier
axis can be used with #5201 to #5340.
M
NOTE
To use variables #2500 to #2806, #5201 to #5340,
and #100301 to #100650, optional variables for the
workpiece coordinate systems are necessary.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 494 -
T
NOTE
To use variables #2550 to #2856, #5201 to #5340,
and #100301 to #100650, optional variables for the
workpiece coordinate systems are necessary.
- Workpiece origin offset value of the additional workpiece coordinate system
#7001-#7960, #101001-#116000 (Attribute: R/W)
M
#14001-#20000 (Attribute: R/W)
The workpiece origin offset value of the additional workpiece
coordinate system can be obtained by reading system variables #7001
to #7960, #14001 to #20000, #101001 to #116000. The offset value
can also be changed by assigning values to the system variables.
Variable
number Variable name Controlled axis
Additional
workpiece
system number
#7001
#7002
:
#7020
[#_WZP1[1]]
[#_WZP1[2]]
:
[#_WZP1[20]]
1st axis workpiece origin offset value
2nd axis workpiece origin offset value
:
20th axis workpiece origin offset value
1
(G54.1 P1)
#7021
#7022
:
#7040
[#_WZP2[1]]
[#_WZP2[2]]
:
[#_WZP2[20]]
1st axis workpiece origin offset value
2nd axis workpiece origin offset value
:
20th axis workpiece origin offset value
2
(G54.1 P2)
#7041
#7042
:
#7060
[#_WZP3[1]]
[#_WZP3[2]]
:
[#_WZP3[20]]
1st axis workpiece origin offset value
2nd axis workpiece origin offset value
:
20th axis workpiece origin offset value
3
(G54.1 P3)
: : : :
#7941
#7942
:
#7960
[#_WZP48[1]]
[#_WZP48[2]]
:
[#_WZP48[20]]
1st axis workpiece origin offset value
2nd axis workpiece origin offset value
:
20th axis workpiece origin offset value
48
(G54.1 P48)
System variable number = 7000 + (Coordinate system number -1) ×
20 + Axis number
Coordinate number: 1 to 48
Axis number: 1 to 20
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 495 -
M
Variable
number Variable name Controlled axis
Additional
workpiece
system number
#14001
#14002
:
#14020
[#_WZP1[1]]
[#_WZP1[2]]
:
[#_WZP1[20]]
1st axis workpiece origin offset value
2nd axis workpiece origin offset value
:
20th axis workpiece origin offset value
1
(G54.1 P1)
#14021
#14022
:
#14040
[#_WZP2[1]]
[#_WZP2[2]]
:
[#_WZP2[20]]
1st axis workpiece origin offset value
2nd axis workpiece origin offset value
:
20th axis workpiece origin offset value
2
(G54.1 P2)
#14041
#14042
:
#14060
[#_WZP3[1]]
[#_WZP3[2]]
:
[#_WZP3[20]]
1st axis workpiece origin offset value
2nd axis workpiece origin offset value
:
20th axis workpiece origin offset value
3
(G54.1 P3)
: : : :
#19981
#19982
:
#20000
[#_WZP300[1]]
[#_WZP300[2]]
:
[#_WZP300[20]]
1st axis workpiece origin offset value
2nd axis workpiece origin offset value
:
20th axis workpiece origin offset value
300
(G54.1 P300)
System variable number = 14000 + (Coordinate system number -1) ×
20 + Axis number
Coordinate number: 1 to 300
Axis number: 1 to 20
Variable
number Variable name Controlled axis
Additional
workpiece
system number
#101001
#101002
:
#101050
[#_WZP1[1]]
[#_WZP1[2]]
:
[#_WZP1[50]]
1st axis workpiece origin offset value
2nd axis workpiece origin offset value
:
50th axis workpiece origin offset value
1
(G54.1 P1)
#101051
#101052
:
#101100
[#_WZP2[1]]
[#_WZP2[2]]
:
[#_WZP2[50]]
1st axis workpiece origin offset value
2nd axis workpiece origin offset value
:
50th axis workpiece origin offset value
2
(G54.1 P2)
#101101
#101102
:
#101150
[#_WZP3[1]]
[#_WZP3[2]]
:
[#_WZP3[50]]
1st axis workpiece origin offset value
2nd axis workpiece origin offset value
:
50th axis workpiece origin offset value
3
(G54.1 P3)
: : : :
#115951
#115952
:
#116000
[#_WZP300[1]]
[#_WZP300[2]]
:
[#_WZP300[50]]
1st axis workpiece origin offset value
2nd axis workpiece origin offset value
:
50th axis workpiece origin offset value
300
(G54.1 P300)
System variable number = 101000 + (Coordinate system number -1) ×
50 + Axis number
Coordinate number: 1 to 300
Axis number: 1 to 50
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 496 -
M
NOTE
1 When variables exceeding the number of control
axes are specified, the alarm PS0115, “VARIABLE
NO. OUT OF RANGE” occurs.
2 The workpiece origin offset of additional workpiece
coordinate system for 20th or earlier axis can be
used with #7001 to #7960 or #14001 to #20000.
3 Optional variables for 48 additional workpiece
coordinate systems are #7001 to #7960 (G54.1 P1
to G54.1 P48). Optional variables for 300
additional workpiece coordinate systems are
#14001 to #20000, and #101001 to #116000
(G54.1 P1 to G54.1 P300). With these variables,
#7001 to #7960 can also be used.
T
NOTE
1 When variables exceeding the number of control
axes are specified, the alarm PS0115, “VARIABLE
NO. OUT OF RANGE” occurs.
2 Optional variables for 48 additional workpiece
coordinate systems are #7001 to #7960 (G54.1 P1
to G54.1 P48).
3 Optional variables for 300 additional workpiece
coordinate systems are #101001 to #116000
(G54.1 P1 to G54.1 P300). With these variables,
#7001 to #7960 can also be used.
- Skip position (detection unit) #5421-#5440, #100701-#100750 (Attribute: R)
The skip position with the detection unit can be obtained by reading
system variables #5421 to #5440 or #100701 to #100750. The
values of these variables are integers, and values in the workpiece
coordinate system.
Variable
number Variable name Position information
Read operation
during
movement
#5421
#5422
:
#5440
[#_SKPDTC[1]]
[#_SKPDTC[2]]
:
[#_SKPDTC[20]]
1st axis skip position (detection unit)
2nd axis skip position (detection unit)
:
20th axis skip position (detection unit)
#100151
#100152
:
#100200
[#_SKPDTC[1]]
[#_SKPDTC[2]]
:
[#_SKPDTC[50]]
1st axis skip position (detection unit)
2nd axis skip position (detection unit)
:
50th axis skip position (detection unit)
Disabled
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 497 -
NOTE
1 When variables exceeding the number of control
axes are specified, the alarm PS0115, “VARIABLE
NO. OUT OF RANGE” occurs.
2 The skip position (detection unit) for 20th or earlier
axis can be used with #5421 to #5440.
3 To specify these variables, set bit 2 (DSK) of
parameter No. 6210 to 1. (If an attempt is made to
specify them when DSK is 0, alarm PS0115 is
issued.)
- Reference fixture offset number being selected #5500 (Attribute: R)
M
The reference fixture offset number being selected can be read by
reading system variables #5500.
Variable
number Variable name Description
#5500 [#_FOFSP] Reference fixture offset number being selected
- Reference fixture offset value being selected #5501-#5520, #117001-#117050
(Attribute: R)
M
The reference fixture offset being selected can be read by reading
system variables #5501 to #5520 or #117001# to 117050.
Variable
number Variable name Description
#5501
#5502
:
#5520
[#_FOFSVAL[1]]
[#_FOFSVAL[2]]
:
[#_FOFSVAL[20]]
1st axis reference fixture offset value being selected
2nd axis reference fixture offset value being selected
:
20th axis reference fixture offset value being selected
#117001
#117002
:
#117050
[#_FOFSVAL[1]]
[#_FOFSVAL[2]]
:
[#_FOFSVAL[50]]
1st axis reference fixture offset value being selected
2nd axis reference fixture offset value being selected
:
50th axis reference fixture offset value being selected
NOTE
1 When variables exceeding the number of control
axes are specified, the alarm PS0115, “VARIABLE
NO. OUT OF RANGE” occurs.
2 The reference fixture offset for 20th or earlier axis
can be used with #5501 to #5520.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 498 -
- Reference fixture offset value #5521-#5680, #117051-#117450 (Attribute: R/W)
M
The reference fixture offset values in the rotary table dynamic fixture
offset function can be obtained by reading system variables #5521 to
#5680 or #117051 to #117450. The reference fixture offset values
can also be changed by assigning values to the system values.
Variable
number
Variable
name Controlled axis Fixture offset
number
#5521
#5522
:
#5540
[#_FOFS1[1]]
[#_FOFS1[2]]
:
[#_FOFS1[20]]
1st axis reference fixture offset value being selected
2nd axis reference fixture offset value being selected
:
20th axis reference fixture offset value being selected
1
(G54.2 P1)
#5541
#5542
:
#5560
[#_FOFS2[1]]
[#_FOFS2[2]]
:
[#_FOFS2[20]]
1st axis reference fixture offset value being selected
2nd axis reference fixture offset value being selected
:
20th axis reference fixture offset value being selected
2
(G54.2 P2)
: : : :
#5661
#5662
:
#5680
[#_FOFS8[1]]
[#_FOFS8[2]]
:
[#_FOFS8[20]]
1st axis reference fixture offset value being selected
2nd axis reference fixture offset value being selected
:
20th axis reference fixture offset value being selected
8
(G54.2 P8)
#117051
#117052
:
#117100
[#_FOFS1[1]]
[#_FOFS1[2]]
:
[#_FOFS1[50]]
1st axis reference fixture offset value being selected
2nd axis reference fixture offset value being selected
:
50th axis reference fixture offset value being selected
1
(G54.2 P1)
#117101
#117102
:
#117150
[#_FOFS2[1]]
[#_FOFS2[2]]
:
[#_FOFS2[50]]
1st axis reference fixture offset value being selected
2nd axis reference fixture offset value being selected
:
50th axis reference fixture offset value being selected
2
(G54.2 P2)
: : : :
#117401
#117402
:
#117450
[#_FOFS8[1]]
[#_FOFS8[2]]
:
[#_FOFS8[50]]
1st axis reference fixture offset value being selected
2nd axis reference fixture offset value being selected
:
50th axis reference fixture offset value being selected
8
(G54.2 P8)
NOTE
1 When variables exceeding the number of control
axes are specified, the alarm PS0115, “VARIABLE
NO. OUT OF RANGE” occurs.
2 The reference fixture offset values for 20th or
earlier axis can be used with #5521 to #5580.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 499 -
- Second geometry tool offset value #5801-#5896, #27001-#29999 (Attribute: R/W)
T
By reading the values of system variables #5801 to #5896 and #27001
to #29999, it is possible to determine the second geometry tool offset
value, and by assigning values to the system variables, it is possible to
change the second geometry tool offset value.
• For compensation numbers up to 32
Compensation
number
Variable
number Variable name Attribute Description
1 #5801 [#_OFSX2G[1]] R/W
: : : :
32 #5832 [#_OFSX2G[32]] R/W
Second geometry tool offset X-axis
compensation value
1 #5833 [#_OFSZ2G[1]] R/W
: : : :
32 #5864 [#_OFSZ2G[32]] R/W
Second geometry tool offset Z-axis
compensation value
1 #5865 [#_OFSY2G[1]] R/W
: : : :
32 #5896 [#_OFSY2G[32]] R/W
Second geometry tool offset Y-axis
compensation value
• For compensation numbers greater than 32 (Compensation values
with compensation numbers of up to 32 can also be used in
variables #5801 to #5896.)
Compensation
number
Variable
number Variable name Attribute Description
1 #27001 [#_OFSX2G[1]] R/W
: : : :
999 #27999 [#_OFSX2G[999]] R/W
Second geometry tool offset X-axis
compensation value
1 #28001 [#_OFSZ2G[1]] R/W
: : : :
999 #28999 [#_OFSZ2G[999]] R/W
Second geometry tool offset Z-axis
compensation value
1 #29001 [#_OFSY2G[1]] R/W
: : : :
999 #29999 [#_OFSY2G[999]] R/W
Second geometry tool offset Y-axis
compensation value
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 500 -
- Dynamic reference tool compensation value #118051-#118450 (Attribute: R/W)
M
The dynamic reference tool compensation value in the rotary head
dynamic tool compensation function can be obtained by reading
system variables #118051 to #118450. The dynamic reference tool
compensation value can also be obtained by assigning values to the
system variables.
Variable
number Variable name Controlled axis Dynamic tool
offset number
#118051
#118052
:
#118100
[#_DOFS1[1]]
[#_DOFS1[2]]
:
[#_DOFS1[50]]
1st axis dynamic reference tool compensation value
2nd axis dynamic reference tool compensation value
:
50th axis dynamic reference tool compensation value
1
(G43.2H1)
#118101
#118102
:
#118150
[#_DOFS2[1]]
[#_DOFS2[2]]
:
[#_DOFS2[50]]
1st axis dynamic reference tool compensation value
2nd axis dynamic reference tool compensation value
:
50th axis dynamic reference tool compensation value
2
(G43.2H2)
#118151
#118152
:
#118200
[#_DOFS3[1]]
[#_DOFS3[2]]
:
[#_DOFS3[50]]
1st axis dynamic reference tool compensation value
2nd axis dynamic reference tool compensation value
:
50th axis dynamic reference tool compensation value
3
(G43.2H3)
#118201
#118202
:
#118250
[#_DOFS4[1]]
[#_DOFS4[2]]
:
[#_DOFS4[50]]
1st axis dynamic reference tool compensation value
2nd axis dynamic reference tool compensation value
:
50th axis dynamic reference tool compensation value
4
(G43.2H4)
#118251
#118252
:
#118300
[#_DOFS5[1]]
[#_DOFS5[2]]
:
[#_DOFS5[50]]
1st axis dynamic reference tool compensation value
2nd axis dynamic reference tool compensation value
:
50th axis dynamic reference tool compensation value
5
(G43.2H5)
: : : :
#118401
#118402
:
#118450
[#_DOFS8[1]]
[#_DOFS8[2]]
:
[#_DOFS8[50]]
1st axis dynamic reference tool compensation value
2nd axis dynamic reference tool compensation value
:
50th axis dynamic reference tool compensation value
8
(G43.2H8)
NOTE
When variables exceeding the number of control
axes are specified, the alarm PS0115, “VARIABLE
NO. OUT OF RANGE” occurs.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 501 -
- Feedrate reduction ratio for rapid traverse overlap #100851-#100900 (Attribute:
R/W)
The feedrate reduction ratio for rapid traverse overlap can also be
changed by setting values to the system variables #100851 to
#100900.
Variable number Variable name Controlled axis
#100851
#100852
:
#100900
[#_ROVLP[1]]
[#_ROVLP[2]]
:
[#_ROVLP[50]]
1st axis feedrate reduction ratio for rapid
traverse overlap
2nd axis feedrate reduction ratio for rapid
traverse overlap
:
50th axis feedrate reduction ratio for rapid
traverse overlap
- Switching between P-CODE variables and system variables (#10000 or later)
#8570 (Attribute: R/W)
This system variable allows read/write operations of P-CODE
variables (#10000 to #89999) for the macro executor function. For
details on P-CODE variables, refer to the Macro Compiler / Macro
Executor Programming Manual (B-63943EN-2).
System variable #8570 can be used to make variables #10000 or later
correspond to either P-CODE variables or system variables.
#8570 setting Specified variable Corresponding variable
#8570 = 1
#10000
:
#89999
P-CODE variables (#10000)
:
P-CODE variables (#89999)
#8570 = 0
#10000
:
#89999
System variables (#10000)
:
System variables (#89999)
Example
#8570 = 0 ;
#10001 = 123 ; → Writing to system variable
#10001 (tool compensation)
#8570 = 1 ;
#10001 = 456 ; → Writing to P-CODE variable
#10001 (tool compensation)
NOTE
1 Variable #8570 can be used only when the macro
executor function is enabled.
2 System variables (#10000 or later) always
correspond to system variables specified by their
variable names even when #8570 is 1.
3 When an attempt is made to access a variable that
cannot be used with P-CODE variables (#10000 or
later), an alarm PS0115 occurs.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 502 -
16.3 ARITHMETIC AND LOGIC OPERATION
Various operations can be performed on variables. Program an
arithmetic and logic operation in the same way as for a general
arithmetic expression.
#i=<expression>
<Expression>
The expression to the right of the arithmetic and logic operation
contains constants and/or variables combined by a function or
operator. Variables #j and #k below can be replaced with a constant.
If a constant used in an expression has no decimal point, it is assumed
to end with a decimal point.
Table 16.3 (a) Arithmetic and logic operation
Type of operation Operation Description
<1> Definition or
replacement
#i=#j Definition or replacement of a variable
<2> Addition-type
operations
#i=#j+#k
#i=#j-#k
#i=#j OR #k
#i=#j XOR #k
Addition
Subtraction
Logical OR (bit by bit of 32 bits)
Exclusive OR (bit by bit of 32 bits)
<3> Multiplication-type
operations
#i=#j*#k
#i=#j/#k
#i=#j AND #k
#i=#j MOD #k
Multiplication
Division
Logical AND (bit by bit of 32 bits)
Remainder (A remainder is obtained after #j and #k
are rounded to their nearest whole numbers. When
#j is a negative value, #i is assumed to be a negative
value.)
<4> Functions #i=SIN[#j]
#i=COS[#j]
#i=TAN[#j]
#i=ASIN[#j]
#i=ACOS[#j]
#i=ATAN[#j]
#i=ATAN[#j]/[#k]
#i=ATAN[#j,#k]
#i=SQRT[#j]
#i=ABS[#j]
#i=BIN[#j]
#i=BCD[#j]
#i=ROUND[#j]
#i=FIX[#j]
#i=FUP[#j]
#i=LN[#j]
#i=EXP[#j]
#i=POW[#j,#k]
#i=ADP[#j]
Sine (in degrees)
Cosine (in degrees)
Tangent (in degrees)
Arc sine
Arc cosine
Arc tangent (one argument), ATN can also be used.
Arc tangent (two arguments), ATN can also be used.
Arc tangent (two arguments), ATN can also be used.
Square root, SQR can also be used.
Absolute value
Conversion from BCD to binary
Conversion from binary to BCD
Rounding off, RND can also be used.
Rounding down to an integer
Rounding up to an integer
Natural logarithm
Exponent using base e (2.718...)
Power (#j to the #kth power)
Addition of a decimal point
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 503 -
Explanation
- Angle units
The units of angles used with the SIN, COS, ASIN, ACOS, TAN, and
ATAN functions are degrees. For example, 90 degrees and 30
minutes is represented as 90.5 degrees.
- ARCSIN #i = ASIN[#j];
• The solution ranges are as indicated below:
When the NAT bit (bit 0 of parameter 6004) is set to 0: 270° to
90°
When the NAT bit (bit 0 of parameter 6004) is set to 1: -90° to
90°
• When #j is beyond the range of -1 to 1, an alarm PS0119 is issued.
• A constant can be used instead of the #j variable.
- ARCCOS #i = ACOS[#j];
• The solution ranges from 180° to 0°.
• When #j is beyond the range of -1 to 1, an alarm PS0119 is issued.
• A constant can be used instead of the #j variable.
- ARCTAN #i = ATAN[#j]/[#k]; (two arguments)
• ATAN[#j,#k] is equivalent to ATAN[#j]/[#k].
• When point (#k,#j) on plane X-Y is given, this function returns the
value of the arc tangent for the angle made by the point.
• A constant can be used instead of the #j variable.
• The solution ranges are as follows:
When the NAT bit (bit 0 of parameter 6004) is set to 0: 0° to
360°
Example:
When #1 = ATAN[-1]/[-1]; is specified, #1 is 225.0.
When the NAT bit (bit 0 of parameter 6004) is set to 1: -180° to
180°
Example:
When #1 = ATAN[-1]/[-1]; is specified, #1 is -135.0.
- ARCTAN #i = ATAN[#j]; (one argument)
• When ATAN is specified with one argument, this function returns
the main value of arc tangent (-90° ≤ ATAN[#j] ≤ 90°). In other
word, this function returns the same value as ATAN in calculator
specifications.
• To use this function as the dividend of a division, be sure to
enclose it with brackets ([]). If this function is not enclosed,
ATAN[#j]/[#k] is assumed.
Example:
#100 = [ATAN[1]]/10 ; : Divides ATAN with one argument by 10.
#100 = ATAN[1]/[10] ; : Executes ATAN with two arguments.
#100 = ATAN[1]/10 ; : Assumes ATAN with two arguments, but issues
an alarm PS1131 because the X coordinate
specification is not enclosed with brackets ([]).
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 504 -
- Natural logarithm #i = LN[#j];
• When the antilogarithm (#j) is zero or smaller, an alarm PS0119 is
issued.
• A constant can be used instead of the #j variable.
- Exponential function #i = EXP[#j];
• When the result of the operation overflows, an alarm PS0119 is
issued.
• A constant can be used instead of the #j variable.
- ROUND function
• When the ROUND function is included in an arithmetic or logic
operation command, IF statement, or WHILE statement, the
ROUND function rounds off at the first decimal place.
Example:
When #1=ROUND[#2]; is executed where #2 holds 1.2345, the value of
variable #1 is 1.0.
• When the ROUND function is used in NC statement addresses, the
ROUND function rounds off the specified value according to the
least input increment of the address.
Example:
Creation of a drilling program that cuts according to the values of variables
#1 and #2, then returns to the original position
Suppose that the increment system is 1/1000 mm, variable #1 holds
1.2345, and variable #2 holds 2.3456. Then,
G00 G91 X-#1; Moves 1.235 mm in negative direction.
G01 X-#2 F300; Moves 2.346 mm in negative direction.
G00 X[#1+#2]; Since 1.2345 + 2.3456 = 3.5801 in positive direction, the
travel distance is 3.580, which does not return the tool to
the original position.
This difference comes from whether addition is performed before
or after rounding off. G00X-[ROUND[#1]+ROUND[#2]]; must
be specified to return the tool to the original position.
- Add decimal point (ADP) function
• ADP[#n] (n = 1 to 33) can be executed to add a decimal point to an
argument passed with no decimal point, in the subprogram.
Example:
In the subprogram called with G65 P_X10;, the value of ADP[#24] is a
value to which a decimal point is added at its end (that is, 10.). Use this
function when you do not want to consider the increment system in the
subprogram. When bit 4 (CVA) of parameter No. 6007 is set to 1,
however, the ADP function cannot be used because any argument is
converted to 0.01 the moment it is passed.
NOTE
For compatibility among programs, it is
recommended that the ADP function be not used,
and decimal points be added in the argument
specification for a macro call.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 505 -
- Rounding up and down to an integer (FUP and FIX)
With CNC, when the absolute value of the integer produced by an
operation on a number is greater than the absolute value of the original
number, such an operation is referred to as rounding up to an integer.
Conversely, when the absolute value of the integer produced by an
operation on a number is less than the absolute value of the original
number, such an operation is referred to as rounding down to an
integer. Be particularly careful when handling negative numbers.
Example:
Suppose that #1=1.2 and #2=-1.2.
When #3=FUP[#1] is executed, 2.0 is assigned to #3.
When #3=FIX[#1] is executed, 1.0 is assigned to #3.
When #3=FUP[#2] is executed, -2.0 is assigned to #3.
When #3=FIX[#2] is executed, -1.0 is assigned to #3.
- Abbreviations of arithmetic and logic operation commands
When a function is specified in a program, the first two characters of
the function name can be used to specify the function.
Example:
ROUND → RO
FIX → FI
NOTE
POW cannot be abbreviated.
- Priority of operations
<1> Functions
<2> Operations such as multiplication and division (*, /, AND)
<3> Operations such as addition and subtraction (+, -, OR, XOR)
Example) #1=#2+#3*SIN[#4];
<1>, <2> and <3> indicate the order of
operations.
<1>
<2>
<3>
- Bracket nesting
Brackets are used to change the order of operations. Brackets can be
used to a depth of five levels including the brackets used to enclose a
function. When a depth of five levels is exceeded, an alarm PS0118
occurs.
Example) #1=SIN [ [ [#2+#3] *#4 +#5] *#6];
<1> to <5> indicate the order of operations.
<1>
<2>
<3>
<4>
<5>
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 506 -
Limitation
• Caution concerning decreased precision
When bit 0 (F16) of parameter No. 6008 is set to 0
• Addition and subtraction
Note that when an absolute value is subtracted from another
absolute value in addition or subtraction, the relative error may
become 10-15 or greater.
For example, assume that #1 and #2 have the following true values
in the process of operation.
(The following values are examples in the process of operation and
cannot actually be specified from any program.)
#1=9876543210.987654321
#2=9876543210.987657777
You cannot obtain the following result with operation #2-#1:
#2-#1=0.000003456
This is because the precision of custom macro variables is 15
decimal digits. With this precision, the values of #1 and #2
become:
#1=9876543210.987650000
#2=9876543210.987660000
(Precisely, the actual values are slightly different from the above
values because they are internally processed in binary.) Therefore,
the result is:
#2-1=0.000010000
A large error occurs.
• Logical expressions
Be aware of errors that can result from conditional expressions
using EQ, NE, GT, LT, GE, and LE because they are processed
basically in the same way as addition and subtraction. For
example, if the following statement is used to decide whether #1 is
equal to #2 in the above example, a correct decision may not be
resulted because errors may occur:
IF [#1 EQ #2]
Evaluate the difference between #1 and #2 with:
IF [ABS [#1-#2]LT 0.1]
Then, assume that the values are equal when the difference does
not exceed the allowable error range.
• Trigonometric functions
The absolute error is guaranteed for trigonometric functions.
However, the relative error is 10-15 or greater. Carefully perform
multiplication or division after executing a trigonometric function.
• FIX function
When using the FIX function for the result of an operation, be
careful with the precision. For example, when the following
operations are performed, the value of #3 may not always be 2.
N10 #1=0.002;
N20 #2=#1*1000;
N30 #3=FIX[#2];
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 507 -
This is because an error may occur in operation N20 and the result
may not be
#2=2.0000000000000000
but a value a little smaller than 2 such as the following:
#2=1.9999999999999997
To prevent this, specify N30 as follows:
N30 #3=FIX[#2+0.001];
Generally, specify the FIX function as follows:
FIX[expression] → FIX[expression ±ε]
(Specify +ε when the value of the expression is positive or -ε when
it is negative, and 0.1, 0.01, 0.001, ... for ε as required.)
NOTE
The operation result of exponential function
#i=EXP[#j]; overflows when #j exceeds about 790.
When bit 0 (F16) of parameter No. 6008 is set to 1
Errors may occur when operations are performed.
Table 16.3 (b) Errors involved in operations
Operation Average
error
Maximum
error Type of error
a = b*c 1.55×10-10 4.66×10-10
a = b / c 4.66×10-10 1.88×10-9
a = b 1.24×10-9 3.73×10-9
Relative error(*1)
a = b + c
a = b – c
2.33×10-10 5.32×10-10 (*2)
a = SIN [ b ]
a = COS [ b ]
5.0×10-9 1.0×10-8
a = ATAN [ b ] / [ c ] 1.8×10-6 3.6×10-6
Absolute error(*3)
degrees
NOTE
1 The relative error depends on the result of the
operation.
2 Smaller of the two types of errors is used.
3 The absolute error is constant, regardless of the
result of the operation.
4 Function TAN performs SIN/COS.
5 Note that, in the case of natural logarithm #i=LN[#j];
and exponential function #i=EXP[#j];, the relative
error may become 10-8 or greater.
6 The operation result of exponential function
#i=EXP[#j]; overflows when #j exceeds about 110.
• The precision of variable values is about 8 decimal digits. When
very large numbers are handled in an addition or subtraction, the
expected results may not be obtained.
ε
a
ε ε
MIN b c
ε
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 508 -
Example:
When an attempt is made to assign the following values to variables #1
and #2:
#1=9876543210123.456
#2=9876543277777.777
the values of the variables become:
#1=9876543200000.000
#2=9876543300000.000
In this case, when #3=#2-#1; is calculated, #3=100000.000 results. (The
actual result of this calculation is slightly different because it is performed
in binary.)
• Also be aware of errors that can result from conditional
expressions using EQ, NE, GE, GT, LE, and LT.
Example:
IF[#1 EQ #2] is effected by errors in both #1 and #2, possibly resulting in
an incorrect decision.
Therefore, instead find the difference between the two variables with
IF[ABS[#1-#2]LT0.001].
Then, assume that the values of the two variables are equal when the
difference does not exceed an allowable limit (0.001 in this case).
• Also, be careful when rounding down a value.
Example:
When #2=#1*1000; is calculated where #1=0.002;, the resulting value of
variable #2 is not exactly 2 but 1.99999997.
Here, when #3=FIX[#2]; is specified, the resulting value of variable #3 is
not 2.0 but 1.0.
In this case, round down the value after correcting the error so that the
result is greater than the expected number, or round it off as follows:
#3=FIX[#2+0.001]
#3=ROUND[#2]
- Brackets
Brackets ([ ]) are used to enclose an expression.
Note that parentheses ( ) are used for comments.
- Divisor
When a divisor of zero is specified in a division, an alarm PS0112
occurs.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 509 -
16.4 INDIRECT AXIS ADDRESS SPECIFICATION
Overview
When the custom macro function is enabled, you can use
AX[(axis-number)] in an axis address specification to indirectly
specify an axis with its axis number and not to directly specify it with
its axis name.
You can also use AXNUM[(axis-name)] to obtain the axis number for
an axis name.
Explanation
- Indirect axis address
You can use indirect axis address AX[ ] to specify an axis with its axis
number. (An equal sign (=) is always required following AX[ ].)
AX[(axis-number)] = (numeric-value) ;
(axis-number): 1 to the number of controlled axes (number of
controlled axes for each path in a multipath system)
(numeric-value): Value specified for the axis specified with its axis
number
If an invalid axis number is specified, an alarm PS0331 occurs. If a
value is put in a decimal place, the number is rounded off to an integer
and the result is treated as the axis number.
You can also specify a variable (local, common, or system variable)
for (axis-number). To specify an operation using a variable name in
(axis-number), however, enclose the variable name with brackets ([ ]).
1. AX[1]=100.0;
Specifies a value of 100.000 for the first axis.
2. AX[#500]=200.0;
Specifies a value of 200.000 for the axis having the axis number
indicated by the value stored in #500.
3. AX[#500+1]=300.0;
Specifies a value of 300.000 for the axis having the axis number
obtained by adding 1 to the value stored in #500.
4. SETVN 500 [ABC];
AX[#ABC]=400.0;
Specifies a value of 400.000 for the axis having the axis number
indicated by the value stored in #ABC (#500).
5. SETVN 500 [ABC];
AX[[#ABC]+1]=500.0;
Specifies a value of 400.000 for the axis having the axis number
obtained by adding 1 to the value stored in #ABC (#500).
6. SETVN 500 [ABC];
AX[#ABC+1]=500.0;
Alarm PS0331 occurs.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 510 -
- AXNUM function
You can use AXNUM[ ] to obtain an axis number.
AXNUM[(axis-name)];
If an invalid axis name is specified, an alarm PS0332 occurs.
When the number of controlled axes is 3, the name of the first axis
is X, that of the second axis is Y, and that of the third axis is Z
1. #500=AXNUM[X];
A value of 1 is stored in #500.
2. #501=AXNUM[Y];
A value of 2 is stored in #501.
3. #502=AXNUM[Z];
A value of 3 is stored in #502.
4. #503=AXNUM[A];
Alarm PS0332 occurs.
Example
Examples when the name of the first axis is X, that of the second axis
is Y, and that of the third axis is Z1
N10 SETVN 500[AXIS1,AXIS2,AXIS3] ;
N20 [#AXIS1]=AXNUM[X] ;
N30 [#AXIS2]=AXNUM[Y] ;
N40 [#AXIS3]=AXNUM[Z1] ;
N50 G92 AX[#AXIS1]=0 AX[#AXIS2]=0 AX[#AXIS3]=0 ;
N60 G90G01F1000. ;
N70 AX[#AXIS1]=100.0 AX[#AXIS2]=100.0 AX[#AXIS3]=100.0 ;
N80 G02 AX[#AXIS1]=100. 0 AX[#AXIS2]= 0.0 R50.0 ;
N90 M02;
Limitation
When the custom macro function is enabled, AX and AXN cannot be
used as an extended axis name. AX is assumed to be AX[ ] and
AXN is assumed to be AXNUM[ ].
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 511 -
16.5 MACRO STATEMENTS AND NC STATEMENTS
The following blocks are referred to as macro statements:
• Blocks containing an arithmetic or logic operation (=)
• Blocks containing a control statement (such as GOTO, DO, END)
• Blocks containing a macro call command (such as macro calls by
G65, G66, G66.1, G67, or other G codes, or by M codes)
Any block other than a macro statement is referred to as an NC
statement.
Explanation
- Differences from NC statements
• Even when single block mode is on, the machine does not stop.
Note, however, that the machine stops in the single block mode
when bit 5 of parameter SBM No. 6000 is 1.
• Macro blocks are not regarded as blocks that involve no movement
in the cutter compensation mode.
- NC statements that have the same property as macro statements
• NC statements that include a subprogram call command (such as
subprogram calls by M98 or other M codes, or by T codes) and not
include other command addresses except an O, file name, N, P, or
L address have the same property as macro statements.
• NC statements that include M99 and those do not include other
command addresses except an O, file name, N, P, or L address
have the same property as macro statements.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 512 -
16.6 BRANCH AND REPETITION
In a program, the flow of control can be changed using the GOTO
statement and IF statement. Three types of branch and repetition
operations are used:
Branch and GOTO (unconditional branch)
repetition IF (conditional branch: if ..., then...)
WHILE (repetition while ...)
16.6.1 Unconditional Branch (GOTO Statement)
A branch to sequence number n occurs. When a sequence number
outside of the range 1 to 99999999 is specified, an alarm PS1128
occurs. A sequence number can also be specified using an
expression.
GOTOn ; n: Sequence number (1 to 99999999)
Example:
GOTO 1;
GOTO #10;
WARNING
Do not specify multiple blocks with the same
sequence number in a single program. It is very
dangerous to specify such blocks because the
destination of a branch from the GOTO statement is
undefined.
NOTE
1 A backward branch takes more time as compared
with a forward branch.
2 In the destination of GOTOn, that is, the block with
sequence number n, the sequence number must
appear at the beginning of the block. If the
sequence number is not at the beginning of the
block, a branch cannot be made.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 513 -
16.6.2 GOTO Statement Using Stored Sequence Numbers
When the GOTO statement is executed in a custom macro control
command, a sequence number search is made for sequence numbers
stored at previous execution of the corresponding blocks at a high
speed.
As a "sequence number stored at previous execution of the
corresponding block", a unique sequence number within the same
program or the sequence number of a subprogram call with which the
block was executed is stored.
The storage type differs depending on the values of the following
parameters.
(1) When bit 1 (MGO) of parameter No. 6000 is set to 1
• Fixed type: Up to 20 sequence numbers stored at execution
of the corresponding blocks from the start of
operation
(2) When bit 4 (HGO) of parameter No. 6000 is set to 1
• Variable type: Up to 30 sequence numbers stored at execution
of the corresponding blocks before execution of
the GOTO statement
• History type: Up to 10 sequence numbers stored by a
sequence number search previously made using
the GOTO statement
The stored sequence numbers are canceled in the following cases:
• Immediately after power-on
• After a reset
• Operation after program registration or editing (including
background editing and MDI program editing)
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 514 -
A
branch to
N10 before
the GOTO
statement
occurs.
A
branch to
N10 after the
GOTO
statement
occurs.
WARNING
Do not specify multiple blocks with the same
sequence number in a single program.
It is very dangerous to specify the sequence number
of the branch destination before and after the GOTO
statement and execute the GOTO statement because
the branch destination changes according to the
values of the parameters as shown below:
When bit 1 (MGO) or 4 (HGO) of
parameter No. 6000 is set to 1
When both bits 1 (MGO) and 4
(HGO) of parameter No. 6000
are set to 0
:
N10;
:
GOTO10;
:
N10;
:
N10;
:
GOTO10;
:
N10;
When bit 1 (MGO) or 4 (HGO) of parameter No. 6000
is set to 1 and the GOTO statement is executed, the
sequence number of the branch destination may not be
contained in the sequence numbers stored at previous
execution of the corresponding blocks. In this case, a
branch to the sequence number in a block following the
GOTO statement occurs (the destination is the same
as when both bits are set to 0).
NOTE
When an external program is read and executed by
DNC operation, the executed sequence numbers are
not stored.
When a program registered in memory is executed by
a subprogram call, the sequence numbers are stored.
CAUTION
According to the restrictions on the GOTO statement,
no branch to a sequence number within a DO-END
loop cannot be made. If a program in which a
branch to a sequence number within a loop occurs is
executed, operation may differ depending on whether
the GOTO statement using stored sequence numbers
is used.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 515 -
16.6.3 Conditional Branch (IF Statement)
Specify a <conditional expression> after IF.
IF[<conditional expression>]GOTOn
If the specified <conditional expression> is satisfied (true), a branch to
sequence number n occurs. If the specified condition is not satisfied,
the next block is executed.
If the value of variable #1 is greater than 10, a branch to sequence number
N2 occurs.
IF[<conditional expression>]THEN
If the specified <conditional expression> is satisfied (true), a macro
statement specified after THEN is executed.
Only a single macro statement is executed.
If the values of #1 and #2 are the same, 0 is assigned to #3.
IF[#1 EQ #2] THEN#3=0 ;
If the values of #1 and #2 are the same and those of #3 and #4 are also
the same, 0 is assigned to #5.
IF[[#1 EQ #2] AND [#3 EQ #4]] THEN#5=0 ;
If the values of #1 and #2 are the same or those of #3 and #4 are the
same, 0 is assigned to #5.
IF[[#1 EQ #2] OR [#3 EQ #4]] THEN#5=0 ;
Explanation
- <Conditional expression>
<Conditional expressions> are divided into <simple conditional
expressions> and <complex conditional expressions>. In a <simple
conditional expression>, a relational operator described in Table 16.6
(a) is specified between two variables or between a variable and
constant to be compared. An <expression> can be used instead of a
variable. With a <complex conditional expression>, an AND
(logical AND), OR (logical OR), or XOR (exclusive OR) operation is
performed for the results (true or false) of multiple <simple
conditional expressions>.
If the condition
is not satisfied
IF [#1 GT 10] GOTO 2 ;
N2 G00 G91 X10.0 ;
:
Processing If the condition is satisfied
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 516 -
- Relational operators
Relational operators each consist of two letters and are used to
compare two values to determine whether they are equal or one value
is smaller or greater than the other value. Note that the equal sign (=)
and inequality sign (>, <) cannot be used as a relational operator.
Table 16.6 (a) Relational operators
Operator Meaning
EQ Equal to(=)
NE Not equal to(≠)
GT Greater than(>)
GE Greater than or equal to(≥)
LT Less than(<)
LE Less than or equal to(≤)
Sample program
The sample program below finds the total of numbers 1 to 10.
O9500;
#1=0;................................ Initial value of the variable to hold the sum
#2=1;................................ Initial value of the variable as an addend
N1 IF[#2 GT 10] GOTO 2; ... Branch to N2 when the addend is greater than
10
#1=#1+#2;........................ Calculation to find the sum
#2=#2+1;.......................... Next addend
GOTO 1; .......................... Branch to N1
N2 M30;............................... End of program
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 517 -
16.6.4 Repetition (WHILE Statement)
Specify a conditional expression after WHILE. While the specified
condition is satisfied, the program from DO to END is executed. If
the specified condition is not satisfied, program execution proceeds to
the block after END.
If the
condition
is not
satisfied
WHILE
[
conditional ex
p
ression
]
DO m ;
(
m=1,2,3
)
END m ;
:
Processing
If the
condition
is satisfied
Explanation
While the specified condition is satisfied, the program from DO to
END after WHILE is executed. If the specified condition is not
satisfied, program execution proceeds to the block after END. The
same format as for the IF statement applies. A number after DO and
a number after END are identification numbers for specifying the
range of execution. The numbers 1, 2, and 3 can be used. When a
number other than 1, 2, and 3 is used, an alarm PS0126 occurs.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 518 -
- Nesting
The identification numbers (1 to 3) in a DO-END loop can be used as
many times as desired. Note, however, when a program includes
crossing repetition loops (overlapped DO ranges), an alarm PS0124
occurs.
Processing
1. The identification numbers (1 to
3) can be used as many times
as required.
WHILE [ … ] DO 1 ;
END 1 ;
:
Processing
WHILE [ … ] DO 1 ;
END 1 ;
:
2. DO ranges cannot
overlap.
Processing
WHILE [ … ] DO 1 ;
END 1 ;
Processing
WHILE [ … ] DO 2 ;
:
END 2 ;
3. DO loops can be nested to a
maximum depth of three levels.
WHILE [ … ] DO 1 ;
:
WHILE [ … ] DO 2 ;
:
WHILE [ … ] DO 3 ;
Processing
END 3 ;
:
END 2 ;
:
END 1 ;
4. Control can be transferred
to the outside of a loop.
WHILE [ … ] DO 1 ;
END 1 ;
IF [ … ] GOTO n ;
Nn
5. Branches cannot be made to a
location within a loop.
WHILE [ … ] DO 1 ;
:
END 1 ;
IF [ … ] GOTO n ;
:
Nn … ;
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 519 -
Limitation
- Infinite loops
When DO m is specified without specifying the WHILE statement, an
infinite loop ranging from DO to END is produced.
- Processing time
When a branch to the sequence number specified in a GOTO
statement occurs, the sequence number is searched for. For this
reason, processing in the reverse direction takes a longer time than
processing in the forward direction. Therefore, in the case of
processing in the reverse direction, use the WHILE statement for
repetition to reduce processing time.
- Undefined variable
In a conditional expression that uses EQ or NE, a <null> and zero
have different effects. In other types of conditional expressions, a
<null> is regarded as zero.
Sample program
The sample program below finds the total of numbers 1 to 10.
O0001;
#1=0;
#2=1;
WHILE[#2 LE 10]DO 1;
#1=#1+#2;
#2=#2+1;
END 1;
M30;
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 520 -
16.7 MACRO CALL
A macro program can be called using the following methods. The
calling methods can roughly be divided into two types: macro calls
and subprogram calls.
A macro program can also be called during MDI operation in the same
way.
Macro call Simple call (G65)
Modal call (G66, G66.1, G67)
Macro call using a G code
Macro call using an M code
Subprogram call using an M code
Subprogram call using a T code
Subprogram call using an S code
Subprogram call using a second auxiliary function code
Subprogram call using a specific code
Limitation
- Call nesting
Macro calls can be nested to a depth of up to five levels and
subprogram calls can be nested to a depth of up to ten levels; calls can
be nested to a depth of up to 15 levels in total.
- Differences between macro calls and subprogram calls
Macro call (G66, G66.1, Ggg, or Mmm) differs from subprogram call
(for example M98, Mmm, or Ttt) as described below.
• With a macro call, an argument (data passed to a macro) can be
specified. A subprogram call does not have this capability.
• If a macro call block contains another NC command (such as G01
X100.0 G65 Pp), an alarm PS0127 occurs.
• If a subprogram call block contains another NC command (such as
G01 X100.0 M98 Pp), the subprogram is called after the command
is executed.
• In any macro call block, the machine does not stop in the single
block mode.
If a subprogram call block contains another NC command (such as
G01 X100.0 M98 Pp), the machine stops in the single block mode.
• With a macro call, the level of local variables changes. With a
subprogram call, the level of local variables does not change.
(See "Local variable levels" in Limitation of Subsection 16.7.1.)
- Called program and folders to be searched
The order in which folders are called depends on the method of calling
a macro or subprogram.
Folders are searched in sequence and the program found first is called.
For details, see the "Managing Programs" chapter.
Subprogram call
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 521 -
16.7.1 Simple Call (G65)
When G65 is specified, the custom macro specified at address P is
called. Data (argument) can be passed to the custom macro program.
P : Number of the program to call
l: Repetition count (1 by default)
A
rgument : Data passed to the macro
O0001 ;
:
G65 P9010 L2 A1.0 B2.0 ;
:
M30 ;
O9010 ;
#3=#1+#2 ;
IF [#3 GT 360] GOTO 9 ;
G00 G91 X#3 ;
N9 M99 ;
G65 P p L
l <argument-
specification> ;
Explanation
- Call
• After G65, specify at address P the program number of the custom
macro to call.
• When a number of repetitions is required, specify a number from 1
to 999999999 after address L. When L is omitted, 1 is assumed.
• By using argument specification, values are assigned to
corresponding local variables.
- Argument specification
Two types of argument specification are available. Argument
specification I uses letters other than G, L, O, N, and P once each.
Argument specification II uses A, B, and C once each and also uses I,
J, and K up to ten times. The type of argument specification is
determined automatically according to the letters used.
• Argument specification I
Add
ress
V
ar
i
a
bl
e
number
A
B
C
D
E
F
H
#1
#2
#3
#7
#8
#9
#11
I
J
K
M
Q
R
S
#4
#5
#6
#13
#17
#18
#19
T
U
V
W
X
Y
Z
#20
#21
#22
#23
#24
#25
#26
Add
ress
V
ar
i
a
bl
e
number
Add
ress
V
ar
i
a
bl
e
number
• Addresses G, L, N, O, and P cannot be used in arguments.
• Addresses that need not be specified can be omitted. Local
variables corresponding to an omitted address are set to null.
• Addresses do not need to be specified alphabetically. They
conform to word address format.
I, J, and K need to be specified alphabetically, however.
Argument specification I is always used for I, J, and K by setting
bit 7 (IJK) of parameter No. 6008 to 1
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 522 -
Example
- When bit 7 (IJK) of parameter No. 6008 is 0,
I_J_K_ means that I = #4, J = #5, and K = #6 while
K_J_I_ means K = #6, J = #8, and I= #10 because
argument specification II is used.
- When bit 7 (IJK) of parameter No. 6008 is 1,
K_J_I_ means that I = #4, J = #5, and K = #6,
which is the same as with I_J_K_, because
argument specification I is used.
• Argument specification II
Argument specification II uses A, B, and C once each and uses I, J,
and K up to ten times. Argument specification II is used to pass
values such as three-dimensional coordinates as arguments.
Add
ress
V
ar
i
a
bl
e
number
A
B
C
I1
J1
K1
I2
J2
K2
I3
J3
#1
#2
#3
#4
#5
#6
#7
#8
#9
#10
#11
IK3
I4
J4
K4
I5
J5
K5
I6
J6
K6
I7
#12
#13
#14
#15
#16
#17
#18
#19
#20
#21
#22
J7
K7
I8
J8
K8
I9
J9
K9
I10
J10
K10
#23
#24
#25
#26
#27
#28
#29
#30
#31
#32
#33
Add
ress
V
ar
i
a
bl
e
number
Add
ress
V
ar
i
a
bl
e
number
• Subscripts of I, J, and K for indicating the order of argument
specification are not written in the actual program.
NOTE
When bit 7 (IJK) of parameter No. 6008 is 1,
argument II cannot be used.
Limitation
- Format
G65 must be specified before any argument.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 523 -
- Mixture of argument specifications I and II
The CNC internally identifies argument specification I and argument
specification II. If a mixture of argument specification I and
argument specification II is specified, the type of argument
specification specified later takes precedence.
[Example]
G65 A1.0 B2.0 I-3.0 I4.0 D5.0 P1000 ;
(Variables)
#1:1.0
#2:2.0
#3:
#4:-3.0
#5:
#6:
#7:4.0 5.0
When both the I4.0 and D5.0 arguments are commanded for variable
#7 in this example, the latter, D5.0, is valid.
- Position of the decimal point
The units used for argument data passed without a decimal point
correspond to the least input increment of each address.
CAUTION
The value of an argument passed without a
decimal point may vary according to the system
configuration of the machine. It is good practice to
use decimal points in macro call arguments to
maintain program compatibility.
- Extended axis name
The axis address of an extended axis name cannot be specified as an
argument. If an attempt is made to specify it, alarm PS0129 is issued.
M
When a value is specified with no decimal point, the number of
decimal places is determined as follows.
Address For a non-axis
address
For an axis
address
D, E, H, M, S, or T 0
Q or R α (NOTE 2)
A, C, I, J, K, X, Y, or Z α (NOTE 2) β (NOTE 3)
B, U, V(NOTE 1), or W 0 β (NOTE 3)
Second auxiliary function γ (NOTE 4)
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 524 -
Address Metric input Inch input
F (G93 mode) 3
F (G94 mode) 0 2
F (G95 mode) 2 (NOTE 5) 4
(NOTE 5)
NOTE
1 When V is used in a call using a specific code, the number of
decimal places is determined according to the setting for the
reference axis.
2 α is determined according to the increment system for the
reference axis (axis specified with parameter No. 1031) as
listed in the table in NOTE 3.
3 β is determined according to the increment system for the
corresponding axis address as listed in the following table.
Increment system Linear axis
(metric input)
Linear axis
(inch input) Rotation axis
IS-A 2 3 2
IS-B 3 4 3
IS-C 4 5 4
IS-D 5 6 5
IS-E 6 7 6
When bit 7 (IPR) of parameter No. 1004 is set to 1, the above
values from which 1 is subtracted are used. When the
increment system for an axis is IS-A, however, the setting of
bit 7 (IPR) of parameter No. 1004 is not effective.
When calculator-type decimal notation for each axis is used
(bit 0 (ADX) of parameter No. 3455 is set to 1), the number of
decimal places is 0. When bit 7 (EAP) of parameter No. 3452
is set to 1, however, calculator-type decimal notation is not
effective and the number of decimal places is determined as
listed in the above table.
4 γ is determined according to the increment system for the
reference axis (axis specified with parameter No. 1031) as
listed in the following table. (When bit 7 (BDX) of parameter
No. 3450 is set to 1, γ is also determined in the same way.)
AUP(3450#0) = 1
AUX (No.3405#0) = 0 AUX (No.3405#0) = 1
Increment system
for the reference
axis
AUP
(No.3450#0)
= 0 Metric Inch Metric Inch
IS-A 2 2 3
IS-B 3 3 4
IS-C 4 4 5
IS-D 5 5 6
IS-E
0
6 6 7
5 When bit 1 (FR3) of parameter No. 1405 is 1, the values in the
table need to be incremented by 1.
6 When calculator-type decimal notation is used (bit 0 (DPI) of
parameter No. 3401 is set to 1), the number of decimal places
is 0.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 525 -
T
When a value is specified with no decimal point, the number of
decimal places is determined as follows.
Address For a non-axis
address
For an axis
address
H, M, Q, S, or T 0
D or R α (NOTE 1)
A, B, C, I, J, K, U, V, W, X, Y, or Z α (NOTE 1) β (NOTE 2)
Second auxiliary function γ (NOTE 3)
Address Metric input Inch input
E, F (G98 mode) 0 (NOTE 4) 2
(NOTE 4)
E, F (G99 mode) 4 6
NOTE
1 α is determined according to the increment system for the
reference axis (axis specified with parameter No. 1031) as
listed in the table in NOTE 2.
2 β is determined according to the increment system for the
corresponding axis address as listed in the following table.
Increment system Linear axis
(metric input)
Linear axis
(inch input) Rotation axis
IS-A 2 3 2
IS-B 3 4 3
IS-C 4 5 4
IS-D 5 6 5
IS-E 6 7 6
When bit 7 (IPR) of parameter No. 1004 is set to 1, the above
values from which 1 is subtracted are used. When the
increment system for an axis is IS-A, however, the setting of
bit 7 (IPR) of parameter No. 1004 is not effective.
When calculator-type decimal notation for each axis is used
(bit 0 (ADX) of parameter No. 3455 is set to 1), the number of
decimal places is 0. When bit 7 (EAP) of parameter No.
3452 is set to 1, however, calculator-type decimal notation is
not effective and the number of decimal places is determined
as listed in the above table.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 526 -
NOTE
3 γ is determined according to the increment system for the
reference axis (axis specified with parameter No. 1031) as
listed in the following table. (When bit 7 (BDX) of parameter
No. 3450 is set to 1, γ is also determined in the same way.)
AUP(3450#0) = 1
AUX (No.3405#0) = 0 AUX (No.3405#0) = 1
Increment system
for the reference
axis
AUP
(No.3450#0)
= 0 Metric Inch Metric Inch
IS-A 2 2 3
IS-B 3 3 4
IS-C 4 4 5
IS-D 5 5 6
IS-E
0
6 6 7
4 When bit 2 (FM3) of parameter No. 1404 is 1, the values in the
table need to be incremented by 3.
5 When calculator-type decimal notation is used (bit 0 (DPI) of
parameter No. 3401 is set to 1), the number of decimal places
is 0.
- Call nesting
Macro calls can be nested to a depth of up to five levels including
simple calls (G65) and modal calls (G66/G66.1). Subprogram calls
can be nested to a depth of up to 15 levels including macro calls.
A macro program can also be called during MDI operation in the same
way.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 527 -
- Local variable levels
• Local variables from level 0 to 5 are provided for nesting.
• The level of the main program is 0.
• Each time a macro is called (with G66, G66.1, Ggg, or Mmm), the
local variable level is incremented by one. The values of the local
variables at the previous level are saved in the CNC.
• When M99 is executed in a macro program, control returns to the
calling program. At that time, the local variable level is
decremented by one; the values of the local variables saved when
the macro was called are restored.
Macro
(level 4)
O0006
:
:
:
:
:
M99 ;
Local variables
(level 0) (Level 1)
#1
:
:
#33
1
:
#1
:
:
#33
2
:
(Level 2)
#1
:
:
#33
3
:
(Level 3)
#1
:
:
#33
4
:
(Level 4)
#1
:
:
#33
5
:
Common variables
#100-, #500- Variables that can be read from and written to by macros at different levels
O0001 ;
:
#1=1 ;
G65 P2 A2 ;
:
:
M30 ;
Main program
(level 0)
Macro
(level 1)
Macro
(level 2)
Macro
(level 3)
O0002 ;
:
:
G65 P3 A 3;
:
:
M99 ;
O0003 ;
:
:
G65 P4 A4 ;
:
:
M99 ;
O0004 ;
:
:
G65 P5 A5 ;
:
:
M99 ;
O0005 ;
:
:
G65 P6 A6 ;
:
:
M99 ;
(Level 5)
#1
:
:
#33
:
6
Macro
(level 5)
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 528 -
Sample program (bolt hole circle)
M
A macro is created which drills H holes at intervals of B degrees after
a start angle of A degrees along the periphery of a circle with radius I.
The center of the circle is (X,Y). Commands can be specified in
either the absolute or incremental programming.
To drill in the clockwise direction, specify a negative value for B.
- Calling format
G65 P9100 Xx Yy Zz Rr Ff Ii Aa Bb Hh ;
X : X coordinate of the center of the circle
(absolute or incremental programming) ................................ (#24)
Y : Y coordinate of the center of the circle
(absolute or incremental programming) ................................ (#25)
Z : Hole depth.............................................................................. (#26)
R : Coordinates of an approach point.......................................... (#18)
F : Cutting feedrate ....................................................................... (#9)
I : Radius of the circle .................................................................. (#4)
A : Drilling start angle ................................................................... (#1)
B : Incremental angle
(clockwise when a negative value is specified) ....................... (#2)
H : Number of holes .................................................................... (#11)
- Program calling a macro program
O0002;
G90 G92 X0 Y0 Z100.0;
G65 P9100 X100.0 Y50.0 R30.0 Z-50.0 F500 I100.0 A0 B45.0 H5;
M30;
H=
H=
H=
H=
A
B
B
Center
Radius
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 529 -
- Macro program (called program)
O9100;
#3=#4003; ................................ Stores G code of group 3.
G81 Z#26 R#18 F#9 K0; (Note)... Drilling cycle.
.................................................. Note: L0 can also be used.
IF[#3 EQ 90]GOTO 1; .............. Branches to N1 in the G90 mode.
#24=#5001+#24; ...................... Calculates the X coordinate of the center.
#25=#5002+#25; ..................... Calculates the Y coordinate of the center.
N1 WHILE[#11 GT 0]DO 1;...... Until the number of remaining holes reaches 0
#5=#24+#4*COS[#1];............... Calculates a drilling position on the X-axis.
#6=#25+#4*SIN[#1];................. Calculates a drilling position on the Y-axis.
G90 X#5 Y#6; ........................... Performs drilling after moving to the target
position.
#1=#1+#2; ................................ Updates the angle.
#11=#11-1; ............................... Decrements the number of holes.
END 1;
G#3 G80;.................................. Returns the G code to the original state.
M99;
Meaning of variables:
#3: Stores the G code of group 3.
#5: X coordinate of the next hole to drill
#6: Y coordinate of the next hole to drill
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 530 -
Sample program (Drill cycle)
T
Move the tool beforehand along the X- and Z-axes to the position
where a drilling cycle starts. Specify Z or W for the depth of a hole,
K for the depth of a cut, and F for the cutting feedrate to drill the hole.
ZW
K
Cutting
Rapid traverse
- Calling format
G65 P9100 Kk Ff ;
Z : Hole depth (absolute programming)
W : Hole depth (incremental programming)
K : Cutting amount per cycle
F : Cutting feedrate
- Program calling a macro program
O0002;
G50 X100.0 Z200.0 ;
G00 X0 Z102.0 S1000 M03 ;
G65 P9100 Z50.0 K20.0 F0.3 ;
G00 X100.0 Z200.0 M05 ;
M30
Zz
Ww
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 531 -
- Macro program (called program)
O9100;
#1=0 ;............................... Clear the data for the depth of the current hole.
#2=0 ;............................... Clear the data for the depth of the preceding
hole.
IF [#23 NE #0] GOTO 1 ;. If incremental programming, specifies the jump
to N1.
IF [#26 EQ #0] GOTO 8 ;. If neither Z nor W is specified, an error occurs.
#23=#5002-#26 ;.............. Calculates the depth of a hole.
N1 #1=#1+#6 ;....................... Calculates the depth of the current hole.
IF [#1 LE #23] GOTO 2 ; . Determines whether the hole to be cut is too
deep?
#1=#23 ;........................... Clamps at the depth of the current hole.
N2 G00 W-#2 ; ...................... Moves the tool to the depth of the preceding
hole at the cutting feedrate.
G01 W- [#1-#2] F#9 ;....... Drills the hole.
G00 W#1 ;........................ Moves the tool to the drilling start point.
IF [#1 GE #23] GOTO 9 ;. Checks whether drilling is completed.
#2=#1 ;............................. Stores the depth of the current hole.
GOTO 1 ;
N9 M99
N8 #3000=1 (NOT Z OR W COMMAND) Issues an alarm.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 532 -
16.7.2 Modal Call: Call After the Move Command (G66)
Once G66 is issued to specify a modal call a macro is called after a
block specifying movement along axes is executed. This continues
until G67 is issued to cancel a modal call.
G66 P p L l <argument-specification> ; P : Number of the program to call
l : Repetition count (1 by default)
A
rgument : Data passed to the macro
O0001 ;
:
G66 P9100 L2 A1.0 B2.0 ;
G00 G90 X100.0 ;
Y200.0 ;
X150.0 Y300.0 ;
G67 ;
:
M30 ;
O9100 ;
:
G00 Z-#1 ;
G01 Z-#2 F300 ;
:
:
:
:
M99 ;
Explanation
- Call
• After G66, specify at address P a program number subject to a
modal call.
• When a number of repetitions is required, a number from 1 to
999999999 can be specified at address L.
• As with a simple call (G65), data passed to a macro program is
specified in arguments.
• In the G66 mode, a macro or subprogram can be called.
- Cancellation
When a G67 code is specified, modal macro calls are no longer
performed in subsequent blocks.
- Call nesting
Macro calls can be nested to a depth of up to five levels including
simple calls (G65) and modal calls (G66/G66.1). Subprogram calls
can be nested to a depth of up to 15 levels including macro calls.
- Modal call nesting
For a single modal call (when G66 is specified only once), each time
the move command is executed, the specified macro is called. When
nested modal macro calls are specified, the macro at the next higher
level is called each time the move command for a macro call is
executed.
Macros are called in reverse order in which they are specified. Each
time G67 is issued, the macros are canceled one by one in reverse
order in which they are specified.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 533 -
[Example]
G66 P9100 ; O9100 ; O9200 ;
X10.0 ; (1-1) Z50.0 ; (2-1) X60.0 ; (3-1)
G66 P9200 ; M99 ; Y70.0 ; (3-2)
X15.0 ; (1-2) M99;
G67 ; Cancels P9200.
G67 ; Cancels P9100.
X-25.0 ; (1-3)
Execution order of the above program (blocks not containing the
move command omitted)
(1-1) (1-2) (1-3)
(2-1) (3-1) (3-2)
(2-1) (2-1)
* No modal call is performed after (1-3) because the mode is not
the macro call mode.
Limitation
• G66 and G67 blocks are specified in pairs in the same program.
If a G67 code is specified not in the G66 mode, an alarm PS1100
occurs. Bit 0 (G67) of parameter No. 6000 can be set to 1 to
specify that the alarm does not occur in this case.
• In a G66 block, no macros can be called. Local variables
(arguments) are set, however.
• G66 needs to be specified before any arguments.
• No macros can be called in a block which contains a code such as a
auxiliary function that does not involve movement along an axis.
• Local variables (arguments) can only be set in G66 blocks. Note
that local variables are not set each time a modal call is performed.
NOTE
If M99 is specified in a block in which a call is
performed, it is executed after the call is
performed.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 534 -
Sample program
M
The same operation as the drilling canned cycle G81 is created using a
custom macro and the machining program makes a modal macro call.
For program simplicity, all drilling data is specified using absolute
values.
Operation 1
Operation 3
Operation 2
Point I
Point R
Z=0
Point Z
Operation 4
The canned cycle consists of the following
basic operations:
Operation 1: Positioning along the X-axis
and Y-axis
Operation 2: Rapid traverse to point R
Operation 3: Cutting feed to point Z
Operation 4: Rapid traverse to point R or I
R
Z
Rapid traverse
Cutting feed
- Calling format
G66 P9110 Zz Rr Ff Ll ;
Z : Coordinates of position Z (absolute programming only) ....... (#26)
R : Coordinates of position R (absolute programming only)....... (#18)
F : Cutting feedrate........................................................................ (#9)
L : Repetition count
- Program that calls a macro program
O0001;
G28 G91 X0 Y0 Z0;
G92 X0 Y0 Z50.0;
G00 G90 X100.0 Y50.0;
G66 P9110 Z-20.0 R5.0 F500;
G90 X20.0 Y20.0;
X50.0;
Y50.0;
X70.0 Y80.0;
G67;
M30;
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 535 -
- Macro program (program called)
O9110;
#1=#4001; .......................Stores G00/G01.
#3=#4003;.........................Stores G90/G91.
#4=#4109;.........................Stores the cutting feedrate.
#5=#5003;.........................Stores the Z coordinate at the start of drilling.
G00 G90 Z#18; .................Positioning at position R
G01 Z#26 F#9;..................Cutting feed to position Z
IF[#4010 EQ 98]GOTO 1; Return to position I
G00 Z#18;.........................Positioning at position R
GOTO 2;
N1 G00 Z#5;........................Positioning at position I
N2 G#1 G#3 F#4; ................Restores modal information.
M99;
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 536 -
Sample program
T
This program makes a groove at a specified position.
U
- Calling format
G66 P9110 Uu Ff
U : Groove depth (incremental programming)
F : Cutting feed of grooving
- Program that calls a macro program
O0003 ;
G50 X100.0 Z200.0 ;
S1000 M03 ;
G66 P9110 U5.0 F0.5 ;
G00 X60.0 Z80.0 ;
Z50.0 ;
Z30.0 ;
G67 ;
G00 X00.0 Z200.0 M05 ;
M30;
- Macro program (program called)
O9110 ;
G01 U - #21 F#9 ;....... Cuts the workpiece.
G00 U#21 ; ................. Retracts the tool.
M99 ;
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 537 -
16.7.3 Modal Call: Each Block Call (G66.1)
In this macro call mode, the specified macro is unconditionally called
for each NC command block. All data other than O, file name, N,
and G codes that is specified in each block is not executed and is used
as arguments. (The G code in the block in which G66.1 is specified
is not used as an argument. Only the last G code specified in
subsequent blocks is used as an argument.)
The NC command blocks having O or file name N have the same
effect as when G65P is specified in the next position, the other NC
command blocks have the same effect as when G65P is specified at
the beginning.
G66.1 P p L l <argument-specification> ; P : Number of the program to call
l : Repetition count (1 by default)
A
rgument : Data passed to the macro
O0001 ;
:
G66.1 P9100 L2 A1.0
B2.0 ;
A
10.0 B20.0 F300 ;
A
0 B-30.0 ;
F1000 ;
G67 ;
:
O9100 ;
:
G00 Z-#1 ;
G01 Z-#2 F#9 ;
:
:
:
:
M99 ;
[Example]
In the G66.1 P100 ; mode,
N001 G01 G91 X100 Y200 D1 R1000 ;
is the same as
N001 G65 P100 G01 G91 X100 Y200 D1 R1000 ;
Explanation
- Call
• After G66.1, specify at address P a program number subject to a
modal call.
• When a number of repetitions is required, a number from 1 to
999999999 can be specified at address L.
• As with a simple call (G65), data passed to a macro program is
specified in arguments.
• In the G66.1 mode, a macro or subprogram can be called.
- Cancellation
When a G67 code is specified, modal macro calls are no longer
performed in subsequent blocks.
- Call nesting
Macro calls can be nested to a depth of up to five levels including
simple calls (G65) and modal calls (G66/G66.1). Subprogram calls
can be nested to a depth of up to 15 levels including macro calls.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 538 -
- Modal call nesting
For a single modal call (when G66.1 is specified only once), the
specified macro is called for each NC command block. When nested
modal macro calls are specified, the macro at the next higher level is
also called in a block within a called macro in which an NC command
is specified.
Macros are called in reverse order in which they are specified. Each
time G67 is issued, the macros are canceled one by one in reverse
order in which they are specified.
[Example] Axis specification switching
N1 G66.1 P1000 X10.0 ; →Calls O1000 and executes Y10.0.
N2 X20.0 ; →Calls O1000 and executes Y20.0.
N3 G66.1 P2000 Y10.0 Z20.0 ; →Calls O2000 and executes Y20.0
Z10.0. Then, calls O1000 and
executes X20.0 Z10.0.
N4 X10.0 Y20.0 Z30.0 ; →Calls O2000 and executes X10.0
Y30.0 Z20.0. Then, calls O1000
and executes X30.0 Y10.0 Z20.0.
N5 G67 ; →Cancels P2000.
N6 G67 ;
→Cancels P1000.
O1000 X#25 Y#24 Z#26 ;
M99 ;
(X-Y switching)
O2000 X#24 Y#26 Z#25 ;
M99 ;
(Y-Z switching)
Execution order of the above program (blocks not containing the
move command omitted)
Calling program N1 N2 N3 N4 N5 N6
O1000
Called
programs
O2000
In N1 and N2 blocks, O1000 is called and the X and Y specifications
are made to change places.
In N3 and N4 blocks, O2000 is called first and the Y and Z
specifications are made to change places. For the switched
specification, O1000 is called and the X and Y specifications are made
to change places. Therefore, the X, Y, and Z specifications are
switched to the Z, X, and Y specifications.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 539 -
Limitation
• G66.1 and G67 blocks are specified in pairs in the same program.
If a G67 code is specified not in the G66.1 mode, an alarm PS1100
occurs. Bit 0 (G67) of parameter No. 6000 can be set to 1 to
specify that the alarm does not occur in this case.
• G66.1 block
(a) In a G66.1 block, a macro is called.
(b) The correspondence between addresses specified as arguments
and variables is the same as for simple calls.
• Block following a G66.1 block in which a call is performed (not
including G66.1 blocks)
(a) Addresses G, P, and L can also be used as arguments.
Address G corresponds to #10; address L to #12; address P to
#16. However, the restrictions on the input format of normal
NC commands are put on the data. For example, ;G1000.
P0.12 L-4 cannot be specified.
(b) When multiple G codes are specified, only the last G code is
used as an argument. O, file name, and N codes and G codes
not in group 00 are passed to the next and subsequent blocks.
NOTE
1 In a block in which only an O number, file name,
sequence number, EOB, macro statement, or M99
command is specified, a macro is not called for
each block.
2 In each block, when an address other than O, file
name, or N is specified, it is assumed to be an NC
command and a macro is called for each block.
When N is specified following an address other
than O, file name, or N, it is used as an argument.
In this case, N corresponds to variable #14 and the
number of decimal places is 0.
3 If M99 is specified in a block in which a macro is
called, it is executed after the call is performed.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 540 -
16.7.4 Macro Call Using a G Code
By setting a G code number used to call a macro program in a
parameter, the macro program can be called in the same way as for a
simple call (G65).
O0001 ;
:
G81 X10.0 Y20.0 Z-10.0 ;
:
M30 ;
O9010 ;
:
:
:
N9 M99 ;
Parameter No.6050=81
Explanation
By setting a G code number from -9999 to 9999 used to call a custom
macro program (O9010 to O9019) in the corresponding parameter
(No.6050 to No.6059), the macro program can be called in the same
way as with G65. To call custom macro program O9040 to O9049
using a G code with a decimal point, set bit 0 (DPG) of parameter No.
6007 to 1 and set the G code number in the corresponding parameter
(Nos. 6060 to 6069).
The number of decimal places of a G code is 1. Set the value
obtained by multiplying a desired G code number by 10 in the
corresponding parameter.
[Example] When parameter No. 6060 is set to 234, custom macro program
O9040 is called using G23.4.
When a negative G code is set, a modal call is performed. In this
case, bit 3 (MGE) of parameter No. 6007 can be set to select the G66
or G66.1 mode.
For example, when a parameter is set so that macro program O9010
can be called with G81, a user-specific cycle created using a custom
macro can be called without modifying the machining program.
- Correspondence between parameter numbers and program numbers
G code with no decimal point G code with a decimal point
Parameter number Program number Parameter number Program number
6050
6051
6052
6053
6054
6055
6056
6057
6058
6059
O9010
O9011
O9012
O9013
O9014
O9015
O9016
O9017
O9018
O9019
6060
6061
6062
6063
6064
6065
6066
6067
6068
6069
O9040
O9041
O9042
O9043
O9044
O9045
O9046
O9047
O9048
O9049
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 541 -
- Repetition
As with a simple call, a number of repetitions from 1 to 999999999
can be specified at address L.
- Argument specification
As with a simple call, two types of argument specification are
available: Argument specification I and argument specification II.
The type of argument specification is determined automatically
according to the addresses used.
Limitation
- Nesting of calls using G codes
• To call another program in a program called using a G code, only
G65, M98, G66, or G66.1 can be used normally.
• When bit 6 (GMP) of parameter No. 6008 is set to 1, a call using
an M, T, or S code, second auxiliary function, or specific code can
be performed in a program called using a G code.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 542 -
16.7.5 Macro Call Using a G Code (Specification of Multiple
Definitions)
By setting the starting G code number used to call a macro program,
the number of the starting program to be called, and the number of
definitions, macro calls using multiple G codes can be defined.
Explanation
As many custom macros as the number specified in parameter No.
6040 can be called using as many G codes as the number specified in
parameter No. 6040. The numeric value set in parameter No. 6038
indicates the starting G code number and the program number set in
parameter No. 6039 indicates the starting program number. To
disable this type of call, set 0 in parameter No. 6040.
When a negative G code is set in parameter No. 6038, modal calls are
performed. In this case, bit 3 (MGE) of parameter No. 6007 can be
set to select the G66 or G66.1 mode.
The number of repetitions and argument specification are set in the
same way as with a macro call using a G code.
[Example]
Set parameter No. 6038 to 900, parameter No. 6039 to 10000000, and
parameter No. 6040 to 100.
G900 → O1000
G901 → O1001
G902 → O1002
:
G999 → O1099
Custom macro calls (simple calls) for 100 combinations are defined as
shown above. When parameter No. 6038 is changed to -900, custom
macro calls (modal calls) for the same combinations are defined.
NOTE
1 The calls defined by this setting become all invalid
in the following cases:
<1> A value outside the valid data range is set in
one of the above parameters.
<2> (No. 6039 + No. 6040 - 1) > 99999999
2 Simple and modal calls cannot be mixed in the
specification.
3 If the G code set in parameter Nos. 6050 to 6059
to call the corresponding macro program is within
the G code range for calling programs using
multiple G codes, the macro program
corresponding to the G code set in parameter Nos.
6050 to 6059 is called.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 543 -
16.7.6 Macro Call Using a G Code with a Decimal Point
(Specification of Multiple Definitions)
When bit 0 (DPG) of parameter No. 6007, by setting the starting G
code number with a decimal point used to call a macro program, the
number of the starting program to be called, and the number of
definitions, multiple macro calls using multiple G codes with a
decimal point can be defined.
Explanation
As many custom macros as the number specified in parameter No.
6043 can be called using as many G codes with a decimal point as the
number specified in parameter No. 6043. The numeric value set in
parameter No. 6041 indicates the starting G code number with a
decimal point and the program number set in parameter No. 6042
indicates the starting program number. To disable this type of call,
set 0 in parameter No. 6043.
When a negative G code is set in parameter No. 6041, modal calls are
performed. In this case, bit 3 (MGE) of parameter No. 6007 can be
set to select the G66 or G66.1 mode.
The number of repetitions and argument specification are set in the
same way as with a macro call using a G code.
[Example]
Set parameter No. 6041 to 900, parameter No. 6042 to 2000, and
parameter No. 6043 to 100.
G90.0 → O2000
G90.1 → O2001
G90.2 → O2002
:
G99.9 → O2099
Custom macro calls (simple calls) for 100 combinations are defined as
shown above. When parameter No. 6041 is changed to -900, custom
macro calls (modal calls) for the same combinations are defined.
NOTE
1 The calls defined by this setting become all invalid in
the following cases:
<1> A value outside the valid data range is set in
one of the above parameters.
<2> (No. 6042 + No. 6043 - 1) > 99999999
<3> Bit 0 (DPG) of parameter No. 6007 is set to 0
(this setting invalidates a macro call using a G
code with a decimal point).
2 Simple and modal calls cannot be mixed in the
specification.
3 If the G code set in parameter Nos. 6060 to 6069 to
call the corresponding macro program is within the
G code range for calling programs using multiple G
codes, the macro program corresponding to the G
code set in parameter Nos. 6060 to 6069 is called.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 544 -
16.7.7 Macro Call Using an M Code
By setting an M code number used to call a macro program in a
parameter, the macro program can be called in the same way as with a
simple call (G65).
O0001 ;
:
M50 A1.0 B2.0 ;
:
M30 ;
O9020 ;
:
:
:
M99 ;
Parameter No.6080=50
Explanation
By setting an M code number from 3 to 99999999 used to call custom
macro program O9020 to O9029 in the corresponding parameter (Nos.
6080 to 6089), the macro program can be called in the same way as
with G65.
- Correspondence between parameter numbers and program numbers
Parameter number Corresponding program number
6080
6081
6082
6083
6084
6085
6086
6087
6088
6089
O9020
O9021
O9022
O9023
O9024
O9025
O9026
O9027
O9028
O9029
Example)
When parameter No. 6080 is set to 990, O9020 is called using
M990.
- Repetition
As with a simple call, a number of repetitions from 1 to 99999999 can
be specified at address L.
- Argument specification
As with a simple call, two types of argument specification are
available: Argument specification I and argument specification II.
The type of argument specification is determined automatically
according to the addresses used.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 545 -
Limitation
• An M code used to call a macro program must be specified at the
start of a block.
• To call another program in a program called using an M code, only
G65, M98, G66, or G66.1 can be used normally.
• When bit 6 (GMP) of parameter No. 6008 is set to 1, a call using a
G code can be performed in a program called using an M code.
16.7.8 Macro Call Using an M Code (Specification of Multiple
Definitions)
By setting the starting M code number used to call a macro program,
the number of the starting program to be called, and the number of
definitions, macro calls using multiple M codes can be defined.
Explanation
As many custom macros as the number specified in parameter No.
6049 can be called using as many M codes as the number specified in
parameter No. 6049. The numeric value set in parameter No. 6047
indicates the starting M code number and the program number set in
parameter No. 6048 indicates the starting program number. To
disable this type of call, set 0 in parameter No. 6049.
The number of repetitions and argument specification are set in the
same way as with a macro call using a M code.
[Example]
Set parameter No. 6047 to 9000, parameter No. 6048 to 4000, and
parameter No. 6049 to 100.
M90000000 → O4000
M90000001 → O4001
M90000002 → O4002
:
M90000099 → O4099
Custom macro calls (simple calls) for 100 combinations are defined as
shown above.
NOTE
1 The calls defined by this setting become all invalid
in the following cases:
<1> A value outside the valid data range is set in
one of the above parameters.
<2> (No. 6048 + No. 6049 - 1) > 99999999
2 If the M code set in parameter Nos. 6080 to 6089
to call the corresponding macro program is within
the M code range for calling programs using multiple
M codes, the macro program corresponding to the M
code set in parameter Nos. 6080 to 6089 is called.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 546 -
16.7.9 Subprogram Call Using an M Code
By setting an M code number used to call a subprogram (macro
program) in a parameter, the macro program can be called in the same
way as with a subprogram call (M98).
Explanation
By setting an M code number from 3 to 99999999 used to call
subprogram O9001 to O9009 in the corresponding parameters Nos.
6071 to 6079, the subprogram can be called in the same way as with
M98.
- Correspondence between parameter numbers and program numbers
Parameter number Program number
6071
6072
6073
6074
6075
6076
6077
6078
6079
O9001
O9002
O9003
O9004
O9005
O9006
O9007
O9008
O9009
- Repetition
As with a simple call, a number of repetitions from 1 to 99999999 can
be specified at address L.
- Argument specification
Argument specification is not allowed.
- M code
An M code in a macro program that has been called is treated as an
ordinary M code.
Limitation
• To call another program in a program called using an M code, only
G65, M98, G66, or G66.1 can be used normally.
• When bit 6 (GMP) of parameter No. 6008 is set to 1, a call using a
G code can be performed in a program called using an M code.
O0001
;
:
M03 ;
:
O9001
;
:
:
:
Parameter No.6071=03
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 547 -
16.7.10 Subprogram Call Using an M Code (Specification of Multiple
Definitions)
By setting the starting M code number used to call a subprogram, the
number of the starting subprogram to be called, and the number of
definitions, subprogram calls using multiple M codes can be defined.
Explanation
As many subprograms as the number specified in parameter No. 6046
can be called using as many M codes as the number specified in
parameter No. 6046. The numeric value set in parameter No. 6044
indicates the starting M code number and the numeric value set in
parameter No. 6045 indicates the starting subprogram number. To
disable this type of call, set 0 in parameter No. 6046.
[Example]
Set parameter No. 6044 to 80000000, parameter No. 6045 to 30000000,
and parameter No. 6046 to 100.
M80000000 → O3000
M80000001 → O3001
M80000002 → O3002
:
M80000099 → O3099
Subprogram calls for 100 combinations are defined as shown above.
NOTE
1 The calls defined by this setting become all invalid in
the following cases:
<1> A value outside the valid data range is set in
one of the above parameters.
<2> (No. 6045 + No. 6046 - 1) > 99999999
2 If the M code set in parameter Nos. 6071 to 6079 to
call the corresponding subprogram is within the M
code range for calling subprograms using multiple M
codes, the subprogram corresponding to the M code
set in parameter Nos. 6071 to 6079 is called.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 548 -
16.7.11 Subprogram Calls Using a T Code
By enabling subprograms to be called with a T code in a parameter, a
subprogram can be called each time the T code is specified in the
machining program.
O0001 ;
:
T23 ;
:
M30 ;
O9000 ;
:
:
:
M99 ;
Bit 5 (TCS) of parameter No. 6001 = 1
Explanation
- Call
By setting bit 5 (TCS) of parameter No. 6001 to 1, subprogram O9000
can be called each time a T code is specified in a machining program.
A T code specified in a machining program is assigned to common
variable #149.
- Repetition
As with a simple call, a number of repetitions from 1 to 99999999 can
be specified at address L.
- Argument specification
Argument specification is not allowed.
Limitation
• To call another program in a program called using a T code, only
G65, M98, G66, or G66.1 can be used normally.
• When bit 6 (GMP) of parameter No. 6008 is set to 1, a call using a
G code can be performed in a program called using a T code.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 549 -
16.7.12 Subprogram Calls Using an S Code
By enabling subprograms to be called with an S code in a parameter, a
subprogram can be called each time the S code is specified in the
machining program.
O0001 ;
:
S23 ;
:
M30 ;
O9029 ;
:
:
:
M99 ;
Bit 1 (SCS) of parameter No. 6007 = 1
Explanation
- Call
By setting bit 1 (SCS) of parameter No. 6007 to 1, subprogram O9029
can be called each time a S code is specified in a machining program.
An S code specified in a machining program is assigned to common
variable #147.
- Repetition
As with a simple call, a number of repetitions from 1 to 99999999 can
be specified at address L.
- Argument specification
Argument specification is not allowed.
Limitation
• To call another program in a program called using an S code, only
G65, M98, G66, or G66.1 can be used normally.
• When bit 6 (GMP) of parameter No. 6008 is set to 1, a call using a
G code can be performed in a program called using an S code.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 550 -
16.7.13 Subprogram Calls Using a Secondary Auxiliary Function
By enabling subprograms to be called with a secondary auxiliary
function in a parameter, a subprogram can be called each time the
secondary auxiliary function is specified in the machining program.
O0001 ;
:
B23 ;
:
M30 ;
O9028 ;
:
:
:
M99 ;
Bit 2 (BCS) of parameter No. 6007 = 1
Explanation
- Call
By setting bit 2 (BCS) of parameter No. 6007 to 1, subprogram O9028
can be called each time a secondary auxiliary function code is
specified in a machining program. A secondary auxiliary function
specified in a machining program is assigned to common variable
#146.
- Repetition
As with a simple call, a number of repetitions from 1 to 99999999 can
be specified at address L.
- Argument specification
Argument specification is not allowed.
Limitation
• To call another program in a program called using a second
auxiliary function, only G65, M98, G66, or G66.1 can be used
normally.
• When bit 6 (GMP) of parameter No. 6008 is set to 1, a call using a
G code can be performed in a program called using a second
auxiliary function.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 551 -
16.7.14 Subprogram Call Using a Specific Address
By enabling subprograms to be called with a specific address in a
parameter, a subprogram can be called each time the specific address
is specified in the machining program.
O0001 ;
:
B100. ;
:
M30 ;
O9004 ;(#146=100.)
:
:
:
M99 ;
Parameter No.6090=66(B)
Explanation
- Call
By setting the code (ASCII code converted to decimal) corresponding
to a specific address in parameter No. 6090 or No. 6091, the custom
macro program, O9004 or O9005, corresponding to each parameter
can be called when the specific address is specified in a machining
program. The code value corresponding to a specific address
specified in a machining program is assigned to the common variables
(#146, #147). The table below indicates the addresses that can be
set.
M
Address Parameter setting
A 65
B 66
D 68
F 70
H 72
I 73
J 74
K 75
L 76
M 77
P 80
Q 81
R 82
S 83
T 84
V 86
X 88
Y 89
Z 90
NOTE
When address L is set, the number of repetitions
cannot be set.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 552 -
T
Address Parameter setting
A 65
B 66
F 70
H 72
I 73
J 74
K 75
L 76
M 77
P 80
Q 81
R 82
S 83
T 84
NOTE
When address L is set, the number of repetitions
cannot be set.
- Correspondence between parameter numbers and program numbers and
between the parameter numbers and common variables
Parameter number Program number Common variable
6090
6091
O9004
O9005
#146
#147
- Repetition
As with a simple call, a number of repetitions from 1 to 99999999 can
be specified at address L.
- Argument specification
Argument specification is not allowed.
Limitation
• To call another program in a program called using a specific code,
only G65, M98, G66, or G66.1 can be used normally.
• When bit 6 (GMP) of parameter No. 6008 is set to 1, a call using a
G code can be performed in a program called using a specific code.
Sample program
By using the subprogram call function that uses M codes, the
cumulative usage time of each tool is measured.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 553 -
Conditions
• The cumulative usage time of each of tools T01 to T05 is
measured.
No measurement is made for tools with numbers greater than T05.
• The following variables are used to store the tool numbers and
measured times:
#501 Cumulative usage time of tool number 1
#502 Cumulative usage time of tool number 2
#503 Cumulative usage time of tool number 3
#504 Cumulative usage time of tool number 4
#505 Cumulative usage time of tool number 5
• Usage time starts being counted when the M03 command is
specified and stops when M05 is specified. System variable
#3002 is used to measure the time during which the cycle start
lamp is on. The time during which the machine is stopped by
feed hold and single block stop operation is not counted, but the
time used to change tools and pallets is included.
Operation check
- Parameter setting
Set 3 in parameter No.6071, and set 5 in parameter No.6072.
- Variable value setting
Set 0 in variables #501 to #505.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 554 -
- Program that calls a macro program
O0001;
T01 M06;
M03;
:
M05; ......................................... Changes #501.
T02 M06;
M03;
:
M05; ......................................... Changes #502.
T03 M06;
M03;
:
M05; ......................................... Changes #503.
T04 M06;
M03;
:
M05; ......................................... Changes #504.
T05 M06;
M03;
:
M05; ......................................... Changes #505.
M30;
- Macro program (program called)
O9001(M03); ...................................................Macro to start counting
M01;
IF[#4120 EQ 0]GOTO 9; ..............................No tool specified
IF[#4120 GT 5]GOTO 9;...............................Out-of-range tool number
#3002=0;.......................................................Clears the timer.
N9 M03;...........................................................Rotates the spindle in the
M99; forward direction.
O9002(M05); ...................................................Macro to end counting
M01;
IF[#4120 EQ 0]GOTO 9; ..............................No tool specified
IF[#4120 GT 5]GOTO 9;...............................Out-of-range tool number
#[500+#4120]=#3002+#[500+#4120]; ..........Calculates cumulative time.
N9 M05;...........................................................Stops the spindle.
M99;
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 555 -
16.8 PROCESSING MACRO STATEMENTS
For smooth machining, the CNC prereads the NC statement to be
performed next. This operation is referred to as buffering. For
example, many NC statements are buffered during look-ahead by AI
contour control and so forth.
In the cutter compensation mode (G41 or G42), the CNC prereads the
NC statements at least three blocks ahead to find intersections even if
look-ahead by AI contour control and so forth is not applied.
Macro statements for arithmetic expressions and conditional branches
are processed as soon as they are read into the buffer. Therefore, the
timing of the macro statement execution is not always the specified
order.
At the blocks containing M00, M01, M02 or M30, blocks containing
M-codes for which buffering is suppressed by setting parameters Nos.
3411 to 3420 and No.3421 to 3432, and blocks containing prevention
buffering G codes such as G31 or G53, the CNC stops to preread the
NC statement after that. Then, the stop of the macro statement
execution is guaranteed until such M codes or G codes complete its
execution.
Explanation
- When the next block is not buffered (M codes that are not buffered, G31, etc.)
> N1 G31 X100.0 ;
N2 #100=1
:
> :Block being executed
NC statement
execution
Macro statement execution
Buffer
N1
N2
CAUTION
In case that you need to execute the macro
statement after completing the block just before the
macro statement, specify M code or G code that is
not buffered just before the macro statement.
Specially, in case of reading/writing the system
variables to control signals, coordinates, offset
value, etc., it may different system variable data by
the timing of the NC statement execution. To avoid
this phenomenon, specify such M codes or G
codes before the macro statement, if necessary.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 556 -
- Buffering the next block in other than cutter compensation mode (G41, G42)
N1
N2 N3
N4
N4
> N1 X100.0 ;
> : Block being executed
: Block read into the buffer
NC statement
execution
Macro statement
execution
Buffer
N2 #1=100 ;
N3 #2=200 ;
N4 Y200.0 ;
When N1 is being executed, the next NC statement (N4) is read into
the buffer. The macro statements (N2, N3) between N1 and N4 are
processed during execution of N1.
- In cutter compensation mode (G41, G42)
> N1 G01 G41 X100.0 F100 Dd ;
> : Block being executed
: Blocks read into the buffer
NC statement
execution
Macro statement
execution
Buffer
N1
N2
N3
N2 #1=100 ;
N3 Y100.0 ;
N4 #2=200 ;
N5 Y150.0 ;
N6 #3=300 ;
N7 X200.0 ;
:
N4
N3
N5
N6
N7
When N1 is being executed, the NC statements in the next three
blocks (up to N7) are read into the buffer. The macro statements (N1,
N4, N6) between N1 and N7 are processed during execution of N1.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 557 -
16.9 REGISTERING CUSTOM MACRO PROGRAMS
Custom macro programs are similar to subprograms. They can be
registered and edited in the same way as subprograms. The storage
capacity is determined by the total length of tape used to store both
custom macros and subprograms.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 558 -
16.10 CODES AND RESERVED WORDS USED IN CUSTOM
MACROS
In addition to the codes used in ordinary programs, the following
codes are used in custom macro programs.
Explanation
- Codes
(1) When the ISO code is used or when bit 4 (ISO) of parameter No.
6008 is set to 0
(The codes are represented in hexadecimal.)
Meaning Code
* 0AAh
= 0BDh
# 0A3h
[ 0DBh
] 0DDh
? 03Fh
@ 0C0h
& 0A6h
_ 05Fh
O 0CFh
(2) When the EIA code is used or when the ISO code is used with bit
4 (ISO) of parameter No. 6008 set to 1
Meaning Code
* Code set in parameter No. 6010
= Code set in parameter No. 6011
# Code set in parameter No. 6012
[ Code set in parameter No. 6013
] Code set in parameter No. 6014
? Code set in parameter No. 6015
@ Code set in parameter No. 6016
& Code set in parameter No. 6017
_ Code set in parameter No. 6018
For O, the same code as for O indicating a program number is used.
Set a hole pattern for each of *, =, #, [, ], ?, @, &, and _ in the ISO or
EIA code in the corresponding parameter (Nos. 6010 to 6018).
The code 00h cannot be used. The code indicating an alphabetic
character can be used for the code indicating a character listed above,
but the code can be no longer used to indicate the original character.
- Reserved words
The following reserved words are used in custom macros:
AND, OR, XOR, MOD, EQ, NE, GT, LT, GE, LE,
SIN, COS, TAN, ASIN, ACOS, ATAN, ATN, SQRT, SQR, ABS,
BIN, BCD, ROUND, RND, FIX, FUP, LN, EXP, POW, ADP, IF,
GOTO, WHILE, DO, END, BPRNT, DPRNT, POPEN, PCLOS,
SETVN, AX, AXNUM
System variable (constant) names and registered common variable
names are also used as reserved words.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 559 -
16.11 EXTERNAL OUTPUT COMMANDS
In addition to the standard custom macro commands, the following
macro commands are available. They are referred to as external
output commands.
• BPRNT
• DPRNT
• POPEN
• PCLOS
These commands are provided to output variable values and characters
through the reader/puncher interface.
Explanation
Specify these commands in the following order:
Open command: POPEN
Before specifying a sequence of data output commands, specify
this command to establish a connection to an external input/output
device.
Data output command: BPRNT or DPRNT
Specify necessary data output.
Close command: PCLOS
When all data output commands have completed, specify PCLOS
to release a connection to an external input/output device.
- Open command POPEN
The POPEN command establishes a connection to an external
input/output device. It must be specified before a sequence of data
output commands. The CNC outputs a DC2 control code.
- Data output command BPRNT
The BPRNT command outputs characters and variable values in
binary.
Number of significant decimal places
BPRNT [ a #b [c] … ]
Variable
Character
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 560 -
(i) Specified characters are converted to the codes according to the
setting data (ISO) that is output at that time.
Specifiable characters are as follows:
• Letters (A to Z)
• Numbers
• Special characters (*, /, +, -, ?, @, &, _)
NOTE
1 An asterisk (*) is output by a space code.
2 When using ?, @, &, and/or _, use the ISO code as
the punch code (setting data (ISO) = 1).
(ii) All variables are stored with a decimal point. Specify a variable
followed by the number of significant decimal places enclosed in
brackets. A variable value is treated as 2-word (32-bit) data,
including the decimal digits. It is output as binary data starting
from the highest byte.
(iii) When specified data has been output, an EOB code is output
according to the setting code (ISO).
(iv) <Null> variables are regarded as 0.
Example
BPRNT [ C** X#100 [3] Y#101 [3] M#10 [0] ]
Variable value
#100=0.40956
#101=-1638.4
#10=12.34
are output as follows:
- Data output command DPRNT
DPRNT [ a #b [c d] … ]
Character
Number of significant digits in the integer part
Number of significant decimal places
Variable
The DPRNT command outputs characters and each digit in the value
of a variable according to the code set in the settings (ISO).
↓ ↓
C sp sp X0000019A YFFE70000 M0000000C LF
( * * ) (410) (-1638400) (12) ( ; )
C3 A0 A0 D8 00 00 01 9A 59 FF E7 00 00 4D 00 00 00 0C 0A
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 561 -
(i) For an explanation of the DPRNT command, see Items (i), (iii),
and (iv) for the BPRNT command.
(ii) When outputting a variable, specify # followed by the variable
number, then specify the number of digits in the integer part and
the number of decimal places enclosed in brackets.
For the value of a variable, as many codes as the specified
number of digits are output according to the settings one by one,
starting with the highest digit. The decimal point is also output
using the set code.
Each variable must be a numeric value consisting of up to nine
digits. When high-order digits are zeros, these zeros are not
output if bit 1 (PRT) of parameter No. 6001 is 1. If parameter
PRT is 0, a space code is output each time a zero is encountered.
When the number of decimal places is not zero, digits in the
decimal part are always output. If the number of decimal places
is zero, no decimal point is output.
When bit 1 (PRT) of parameter No. 6001 is 0, a space code is
output to indicate a positive number instead of +; if parameter
PRT is 1, no code is output.
Example
DPRNT [ X#2 [53] Y#5 [53] T#30 [20] ]
Variable value
#2=128.47398
#5=-91.2
#30=123.456
are output as follows:
(1) Parameter PRT (No.6001#1) = 0
(2) Parameter PRT (No.6001#1) = 1
D8 B1 B2 B8 2E B4 B7 B4 59 2D 39 B1 2E B2 30 30 D4 A0 B2 33 0A
↓
X128.474 Y-91.200 T023 LF
X sp sp sp 128.474 Y- sp sp sp 91.200 T sp 023 LF
D8 A0 A0 A0 B1 B2 B8 2E B4 B7 B4 59 2D A0 A0 A0 39 B1 2E B2 30 30 D4 A0 B2 33 0A
↓ ↓ ↓ ↓
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 562 -
- Close command PCLOS
The PCLOS command releases a connection to an external
input/output device. Specify this command when all data output
commands have terminated. DC4 control code is output from the
CNC.
- Required setting
Specify the specification number of an input/output device to be used
for the I/O device specification number.
According to the above settings, set data items (such as the baud rate)
for the reader/puncher interface.
Never specify the output device FANUC Cassette or Floppy for
punching.
When specifying a DPRNT command to output data, specify whether
leading zeros are output as spaces (by setting bit 1 (PRT) of parameter
No. 6001 to 1 or 0).
To indicate the end of a line of data in ISO code, specify whether to
use only an LF (bit 4 (CRO) of parameter 6001 is 0) or an LF and CR
bit 4 (CRO) of parameter 6001 is 1).
NOTE
1 It is not necessary to always specify the open
command (POPEN), data output command
(BPRNT, DPRNT), and close command (PCLOS)
together. Once an open command is specified at
the beginning of a program, it does not need to be
specified again except after a close command was
specified.
2 Be sure to specify open commands and close
commands in pairs. Specify the close command
at the end of the program. However, do not
specify a close command if no open command has
been specified.
3 When a reset operation is performed while
commands are being output by a data output
command, output is stopped and subsequent data
is erased. Therefore, when a reset operation is
performed by a code such as M30 at the end of a
program that performs data output, specify a close
command at the end of the program so that
processing such as M30 is not performed until all
data is output.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 563 -
16.12 RESTRICTIONS
- Sequence number search
A custom macro program cannot be searched for a sequence number.
- Single block
Even while a macro program is being executed, blocks can be stopped
in the single block mode.
A block containing a macro call command (G66, G66.1, Ggg, Mmm,
or G67) does not stop even when the single block mode is on.
Whether blocks containing arithmetic and logic operation commands
and control commands are stopped depends on the settings of bits 5
(SBM) and 7 (SBV) of parameter No. 6000 as shown in the following
table.
Bit 5 (SBM) of parameter No. 6000
0 1
0Not stopped when the
single block mode is on.
Bit 7 (SBV)
of
parameter
No. 6000 1
Can be stopped in the
single bock mode.
(Variable #3003 can be
used to enable or disable
single block stop.)
Can be stopped in the
single block mode.
(Variable #3003 cannot be
used to disable single
block stop. Single block
stop is always enabled.)
Note that when a single block stop occurs at a macro statement in
cutter compensation mode, the statement is assumed to be a block that
does not involve movement, and proper compensation cannot be
performed in some cases. (Strictly speaking, the block is regarded as
specifying a movement with a travel distance 0.)
- Optional block skip
A / appearing in the middle of an <expression> (enclosed in brackets
[ ] on the right-hand side of an arithmetic expression) is regarded as
a division operator; it is not regarded as the specifier for an optional
block skip code.
- Operation in EDIT mode
By setting bit 0 (NE8) of parameter No.3202 and bit 4 (NE9) of
parameter No.3202 to 1, deletion and editing are disabled for custom
macro programs and subprograms with program numbers 8000 to
8999 and 9000 to 9999. This prevents registered custom macro
programs and subprograms from being destroyed by accident. When
the entire memory is cleared, the contents of memory such as custom
macro programs are deleted.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 564 -
- Reset
With a reset operation, local variables and common variables #100 to
#199 are cleared to null values. They can be prevented from clearing
by setting bit 6 (CCV) of parameter No.6001. System variables #100
to #199 are not cleared.
A reset operation clears any called states of custom macro programs
and subprograms, and any DO states, and returns control to the main
program.
- Display of the PROGRAM RESTART
As with M98, the M and T codes used for subprogram calls are not
displayed.
- Feed hold
When a feed hold is enabled during execution of a macro statement,
the machine stops after execution of the macro statement. The
machine also stops when a reset or alarm occurs.
- DNC operation
The control commands (such as GOTO and WHILE-DO) cannot be
executed during DNC operation.
However, this restriction is removed when a program registered in
program memory is called during DNC operation.
- Constant values that can be used in <expression>
+0.00000000001 to +999999999999
-999999999999 to -0.00000000001
The number of significant digits is 12 (decimal).
If this range is exceeded, an alarm PS0012 occurs.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 565 -
16.13 INTERRUPTION TYPE CUSTOM MACRO
When a program is being executed, another program can be called by
inputting an interrupt signal (UINT) from the machine.
This function is referred to as an interruption type custom macro
function. Program an interrupt command in the following format:
Format
M96Pxxxxxxxx ; Enables custom macro interrupt
M97 ; Disables custom macro interrupt
Explanation
Use of the interruption type custom macro function allows the user to
call a program during execution of an arbitrary block of another
program. This allows programs to be operated to match situations
which vary from time to time.
(1) When a tool abnormality is detected, processing to handle the
abnormality is started by an external signal.
(2) A sequence of machining operations is interrupted by another
machining operation without the cancellation of the current
operation.
(3) At regular intervals, information on current machining is read.
Listed above are examples like adaptive control applications of
the interruption type custom macro function.
Interrupt signal
(UINT) **
Interrupt signal
(UINT) *
Interrupt signal
(UINT) *
M96 Pxxxxxxxx;
Nxxxxxxxx ;
M97 ;
M99 (Pxxxxxxxx) ;
O xxxxxxxx;
Fig 16.13 (a) Interruption type custom macro function
When M96Pxxxx is specified in a program, subsequent program
operation can be interrupted by an interrupt signal (UINT) input to
execute the program specified by Pxxxx. When the interrupt signal
(UINT, marked with an asterisk (*) in Fig 16.13 (a)) is input during
execution of the interrupt program or after M97, it is ignored.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 566 -
16.13.1 Specification Method
Explanation
- Interrupt conditions
A custom macro interrupt is available only during program execution.
It is enabled under the following conditions
• When memory operation, DNC operation, or MDI operation is
selected
• When STL (start lamp) is on
• When a custom macro interrupt is not currently being processed
A macro interrupt cannot be performed during manual operation.
- Specification
Generally, the custom macro interrupt function is used by specifying
M96 to enable the interrupt signal (UINT) and M97 to disable the
signal.
Once M96 is specified, a custom macro interrupt can be initiated by
the input of the interrupt signal (UINT) until M97 is specified or the
CNC is reset. After M97 is specified or the CNC is reset, no custom
macro interrupts are initiated even when the interrupt signal (UINT) is
input. The interrupt signal (UINT) is ignored until another M96
command is specified.
The interrupt signal (UINT) becomes valid after M96 is specified.
Even when the signal is input in M97 mode, it is ignored. When the
signal input in M97 mode is kept on until M96 is specified, a custom
macro interrupt is initiated as soon as M96 is specified (only when the
status-triggered scheme is employed); when the edge-triggered
scheme is employed, the custom macro interrupt is not initiated even
when M96 is specified.
NOTE
For the status-triggered and edge-triggered
schemes, see Item "Custom macro interrupt signal
(UINT)" of II-16.13.2.
Interrupt signal
(UINT)
Effective interrupt
input signal When UINT is kept on
1
0
M96 M97 M96
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 567 -
16.13.2 Details of Functions
Explanation
- Subprogram-type interrupt and macro-type interrupt
There are two types of custom macro interrupts: Subprogram-type
interrupts and macro-type interrupts. The interrupt type used is
selected by bit 5 (MSB) of parameter No.6003.
(a) Subprogram-type interrupt: When bit 5 (MSB) of parameter
No.6003 is set to 1
An interrupt program is called as a subprogram.
This means that the levels of local variables remain unchanged
before and after the interrupt.
This interrupt is not included in the nesting level of subprogram
calls.
(b) Macro-type interrupt: When bit 5 (MSB) of parameter No.6003
is set to 0
An interrupt program is called as a custom macro.
This means that the levels of local variables change before and
after the interrupt.
The interrupt is not included in the nesting level of custom macro
calls.
When a subprogram call or a custom macro call is performed
within the interrupt program, this call is included in the nesting
level of subprogram calls or custom macro calls.
Arguments cannot be passed from the current program even
when the custom macro interrupt is a macro-type interrupt. The
local variables immediately after interruption are all cleared to
null.
- M codes for custom macro interrupt control
In general, custom macro interrupts are controlled by M96 and M97.
However, these M codes, may already being used for other purposes
(such as an M function or macro M code call) by some machine tool
builders.
For this reason, bit 4 (MPR) of parameter No.6003 is provided to set
M codes for custom macro interrupt control.
When specifying this parameter to use the custom macro interrupt
control M codes set by parameters, set parameters Nos.6033 and 6034
as follows:
Set the M code to enable custom macro interrupts in parameters
Nos.6033, and set the M code to disable custom macro interrupts in
parameter 6034.
When specifying that parameter-set M codes are not used, M96 and
M97 are used as the custom macro control M codes regardless of the
settings of parameters Nos.6033 and 6034.
The M codes used for custom macro interrupt control are processed
internally (they are not output to external units). However, in terms
of program compatibility, it is undesirable to use M codes other than
M96 and M97 to control custom macro interrupts.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 568 -
- Custom macro interrupts and NC statements
When performing a custom macro interrupt, the user may want to
interrupt the NC statement being executed, or the user may not want to
perform the interrupt until the execution of the current block is
completed. Bit 2 (MIN) of parameter No.6003)is used to select
whether to perform interrupts even in the middle of a block or to wait
until the end of the block. The type of interrupt performed even in
the middle of a block is called type I and the type of interrupt
performed at the end of the block is called type II.
CAUTION
For interrupt type I, operation after control is
returned differs depending on whether the interrupt
program contains an NC statement.
When the program number block contains EOB (;),
it is assumed to contain an NC statement.
(Program containing an
NC statement)
O0013;
#101=#5041;
#102=#5042;
#103=#5043;
M99;
(Program containing no
NC statement)
O0013#101=#5041;
#102=#5042;
#103=#5043;
M99;
Type I (when an interrupt is performed even in the middle of a block)
(i) When the interrupt signal (UINT) is input, any movement or
dwell being performed is stopped immediately and the interrupt
program is executed.
(ii) If there are NC statements in the interrupt program, the command
in the interrupted block is lost and the NC statement in the
interrupt program is executed. When control is returned to the
interrupted program, the program is restarted from the next block
after the interrupted block.
(iii) If there are no NC statements in the interrupt program, control is
returned to the interrupted program by M99, then the program is
restarted from the command in the interrupted block.
Interrupt signal
(UINT) input
Custom macro interrupt
Execution in progress
Execution in progress
Normal program
CNC command restart;
when there are no NC statements
in the interrupt program
Interrupted by macro interrupt
Fig. 16.13 (b) Custom macro interrupt and NC command (type I)
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 569 -
Type II (when an interrupt is performed at the end of the block)
(i) If the block being executed is not a block that consists of several
cycle operations such as a drilling canned cycle and automatic
reference position return (G28), an interrupt is performed as
follows:
When an interrupt signal (UINT) is input, macro statements in
the interrupt program are executed immediately unless an NC
statement is encountered in the interrupt program. NC
statements are not executed until the current block is completed.
(ii) If the block being executed consists of several cycle operations,
an interrupt is performed as follows:
When the last movement in the cycle operations is started, macro
statements in the interrupt program are executed unless an NC
statement is encountered. NC statements are executed after all
cycle operations are completed.
Custom macro interrupt
Execution in progress
Execution in progress
Normal program
NC statement in the interrupt
program
Interrupt signal (UINT) input
Fig. 16.13 (c) Custom macro interrupt and NC command (type II)
M
NOTE
During execution of a program for cycle operations,
interrupt type II is performed regardless of whether
bit 2 (MIN) of parameter No. 6003 is set to 0 or 1.
Cycle operations are available for the following
functions:
<1> Automatic reference position return
<2> Tool radius ⋅ tool nose radius compensation
(generating multiple blocks using the specified
block such as when the tool moves around the
outside of an acute angle)
<3> Canned cycle
<4> Automatic tool length measurement
<5> Optional chamfering/corner R
<6> Exponential interpolation
<7> Normal direction control
<8> Cutting point interpolation for cylindrical
interpolation
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 570 -
T
NOTE
During execution of a program for cycle operations,
interrupt type II is performed regardless of whether
bit 2 (MIN) of parameter No. 6003 is set to 0 or 1.
Cycle operations are available for the following
functions:
<1> Automatic reference position return
<2> Tool radius ⋅ tool nose radius compensation
(generating multiple blocks using the specified
block such as when the tool moves around the
outside of an acute angle)
<3> Canned cycle (No interruption type custom
macro can be used during execution of a
multiple repetitive canned turning cycle,
however.)
<4> Automatic tool length measurement
<5> Chamfering/corner R
<6> Exponential interpolation
<7> Cutting point interpolation for cylindrical
interpolation
- Conditions for enabling and disabling the custom macro interrupt signal
The interrupt signal becomes valid after execution starts of a block
that contains M96 for enabling custom macro interrupts. The signal
becomes invalid when execution starts of a block that contains M97.
While an interrupt program is being executed, the interrupt signal
becomes invalid. The signal become valid when the execution of the
block that immediately follows the interrupted block in the main
program is started after control returns from the interrupt program.
In type I, if the interrupt program consists of only macro statements,
the interrupt signal becomes valid when execution of the interrupted
block is started after control returns from the interrupt program.
- Custom macro interrupt signal (UINT)
There are two schemes for custom macro interrupt signal (UINT)
input: The status-triggered scheme and edge-triggered scheme.
When the status-triggered scheme is used, the signal is valid when it is
on. When the edge triggered scheme is used, the signal becomes
valid on the rising edge when it switches from off to on status.
One of the two schemes is selected with bit 3 (TSE) of parameter
No.6003.
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 571 -
When the status-triggered scheme is selected by this parameter, a
custom macro interrupt is generated if the interrupt signal (UINT) is
on at the time the signal becomes valid. By keeping the interrupt
signal (UINT) on, the interrupt program can be executed repeatedly.
When the edge-triggered scheme is selected, the interrupt signal
(UINT) becomes valid only on its rising edge. Therefore, the
interrupt program is executed only momentarily (in cases when the
program consists of only macro statements). When the
status-triggered scheme is inappropriate, or when a custom macro
interrupt is to be performed just once for the entire program (in this
case, the interrupt signal may be kept on), the edge-triggered scheme
is useful.
Except for the specific applications mentioned above, use of either
scheme results in the same effects. The time from signal input until a
custom macro interrupt is executed does not vary between the two
schemes.
In the example shown in Fig 16.13 (d), an interrupt is executed four
times when the status-triggered scheme is used; when the
edge-triggered scheme is used, the interrupt is executed just once.
Interrupt signal (UINT)
1
0
Status-triggered scheme
Edge-triggered scheme
Interrupt
execution
Interrupt
execution
Interrupt
execution Interrupt
execution
Interrupt execution
Fig. 16.13 (d) Custom macro interrupt signal
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 572 -
- Return from a custom macro interrupt
To return control from a custom macro interrupt to the interrupted
program, specify M99. A sequence number in the interrupted
program can also be specified using address P. If this is specified,
the program is searched from the beginning for the specified sequence
number. Control is returned to the first sequence number found.
NOTE
When an M99 block consists only of address O, N,
P, L, or M, this block is regarded as belonging to
the previous block in the program. Therefore, a
single-block stop does not occur for this block. In
terms of programming, the following <1> and <2>
are basically the same. (The difference is whether
Gxx is executed before M99 is recognized.)
<1> Gxx Xxxx ;
M99 ;
<2> Gxx Xxxx M99 ;
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 573 -
- Custom macro interrupt and modal information
A custom macro interrupt is different from a normal program call. It
is initiated by an interrupt signal (UINT) during program execution.
In general, any modifications of modal information made by the
interrupt program should not affect the interrupted program.
For this reason, even when modal information is modified by the
interrupt program, the modal information before the interrupt is
restored when control is returned to the interrupted program by M99.
When control is returned from the interrupt program to the interrupted
program by M99 Pxxxxxxxx, however, modal information can again
be controlled by the program. In this case, the new continuous
information modified by the interrupt program is passed to the
interrupted program.
In this case, take the following action as required:
<1> The interrupt program provides modal information to be used
after control is returned to the interrupted program.
<2> After control is returned to the interrupted program, modal
information is specified again as necessary.
{∆∆∆∆
M96 Pxxxxxxxx ; {xxxxxxxx ;
Interrupt signal (UINT)
Modify modal information
(Without P specification)
Modal information remains
unchanged before and after
the interrupt.
M99 (Pxxxxxxxx) ;
(With P specification)
The new modal information modified by the interrupt program is present.
Nxxxxxxxx ;
Fig. 16.13 (e) Custom macro interrupt and modal information
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 574 -
Modal information when control is returned by M99
The modal information present before the interrupt becomes valid.
The new modal information modified by the interrupt program is
made invalid.
Modal information when control is returned by M99 Pxxxxxxxx
The new modal information modified by the interrupt program
remains valid even after control is returned.
Modal information which was valid in the interrupted block
The old modal information which was valid in the interrupted block
can be read using custom macro system variables #4401 to #4530.
M
System variable Modal information which was valid when a custom
macro interrupt was generated
#4401
:
#4421
#4502
#4507
#4508
#4509
#4511
#4513
#4514
#4515
#4519
#4520
#4530
G code (group 01)
:
G code (group 21)
B code
D code
E code
F code
H code
M code
Sequence number
Program number
S code
T code
Additional workpiece coordinate system number
T
System variable Modal information which was valid when a custom
macro interrupt was generated
#4401
:
#4421
#4508
#4509
#4513
#4514
#4515
#4519
#4520
#4530
G code (group 01)
:
G code (group 21)
E code
F code
M code
Sequence number
Program number
S code
T code
Additional workpiece coordinate system number
B-63944EN/03 PROGRAMMING 16.CUSTOM MACRO
- 575 -
- System variables (position information values) for the interrupt program
Position information can be read as follows.
Macro
variable Condition Position information
value
Until the first NC statement appears Coordinates of point A
After an NC statement with no move
command appears
Coordinates of point A'
#5001 or
above
After an NC statement with a move
command appears
Coordinates of the end
point of the move
command
#5021 or
above
Machine coordinates of
point B'
#5041 or
above
Workpiece coordinates
of point B'
B
B
A
’
A
Interrupt generated
Programmed tool path
Offset vector
Tool center path
- Custom macro interrupt and custom macro modal call
When the interrupt signal (UINT) is input and an interrupt program is
called, the custom macro modal call is canceled (G67). However,
when G66 is specified in the interrupt program, the custom macro
modal call becomes valid. When control is returned from the
interrupt program by M99, the modal call is restored to the state it was
in before the interrupt was generated. When control is returned by
M99 Pxxxxxxxx;, the modal call in the interrupt program remains
valid.
16.CUSTOM MACRO PROGRAMMING B-63944EN/03
- 576 -
- Custom macro interrupt and program restart
In program restart, when the interrupt signal (UINT) is input during
dry run recovery after a search, the interrupt program is called after
restart of all axes is completed.
That is, interrupt type II is assumed regardless of the parameter
setting.
M
NOTE
1 Alarm PS1101 occurs in the following cases:
<1> An interrupt is generated in the programmable
mirror image (G51.1) mode and another G51.1
is specified in the interrupt program.
<2> An interrupt is generated in the coordinate
system rotation (G68) mode and another G68
is specified in the interrupt program.
<3> An interrupt is generated in the scaling (G51)
mode and another G51 is specified in the
interrupt program.
2 In program restart, do not input the interrupt signal
(UINT) during dry run recovery after a search.
T
NOTE
1 Alarm PS1101 occurs in the following cases:
<1> An interrupt is generated in the programmable
mirror image (G51.1) mode and another G51.1
is specified in the interrupt program.
<2> An interrupt is generated in the coordinate
system rotation (G68.1) mode and another
G68.1 is specified in the interrupt program.
<3> An interrupt is generated in the scaling (G51)
mode and another G51 is specified in the
interrupt program.
2 No interruption type custom macro can be used
during execution of a multiple repetitive canned
turning cycle.
3 In program restart, do not input the interrupt signal
(UINT) during dry run recovery after a search.
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 577 -
17 REAL-TIME CUSTOM MACRO
Chapter 17, "REAL-TIME CUSTOM MACRO", consists of the
following sections:
17.1 TYPES OF REAL TIME MACRO COMMANDS................581
17.2 VARIABLES..........................................................................588
17.3 ARITHMETIC AND LOGICAL OPERATION....................596
17.4 CONTROL ON REAL TIME MACRO COMMANDS ........598
17.5 MACRO CALL ......................................................................605
17.6 OTHERS.................................................................................607
17.7 AXIS CONTROL COMMAND.............................................608
17.8 NOTES ...................................................................................622
17.9 LIMITATION.........................................................................624
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 578 -
Overview
Used with an NC program, the real time custom macro function
controls peripheral axes and signals.
If a macro statement is used together with an NC statement, a program
using the conventional custom macro function executes the macro
statement immediately when the macro statement is read. So, the
macro statement cannot be executed independently of the NC
statement.
On the other hand, the real time custom macro function enables the
following control operations when a real time macro command (RTM
command) is coded in an NC program.
• A real time macro command starts operation in synchronism with
the NC statement and is executed independently. During NC
program execution, a real time macro command can be executed
at the same time.
• PMC interface signals can be read and written (with a restriction).
In an NC program, a motion using a signal as a trigger can be
coded.
• Variables dedicated to a real time macro command can be read
and written.
• A real time macro command can exercise axis control. (The
option is required.)
• Multiple real time macro commands can be executed at the same
time. Multiple real time custom macro statements can be coded
in an NC program and can be controlled independently of each
other.
By using a real time custom macro, control on signals and peripheral
axes can be programmed.
The example below turns on and off a signal and performs operation
on a peripheral axis when machining points are passed.
During movement for machining along the X-axis in the figure above:
<1> When point Xa is passed, the G99.5 signal is set to 1.
→ Real time macro command 1
<2> When point Xb is passed, positioning is started on peripheral axis
Y. → Real time macro command 2
<3> When point Xc is passed, the G99.5 signal is set to 0.
→ Real time macro command 3
Signal
ON OFF
Peri
p
heral axis Y
X-axis machining direction
Xa=30 Xb=50 Xc=80
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 579 -
The operation above is programmed using real time macro commands.
Program
O0001 ;
G92 X0 ;
//1 ZEDGE [#100101 GE 30. ] #IOG[99,5] = 1 ;
//2 ZEDGE [#100101 GE 50.] ZDO ;
G91 G00 Y100 ;
ZEND ;
//3 ZEDGE [#100101GE 80. ] #IOG[99,5] = 0 ;
G90 G01 X200. F150 ;
M30 ;
The timing is as follows. (‘**’ represents the satisfaction of the
condition.)
X coordinate 30 50 80
Peripheral axis Y operation
G99.5 signal
NC statement (machining)
G90 G01 X200. F150
Real time macro command 1
//1 ZEDGE [#100101 GE 30.]
#IOG[99,5] = 1 ;
**
Real time macro command 2
//2 ZEDGE [#100101 GE 50. ]
ZDO ;
G91 G00 Y100 ;
ZEND ;
**
Real time macro command 3
//3 ZEDGE [#100101 GE 80. ]
#IOG[99,5] = 0 ;
**
Explanation
To use the real time custom macro function, a real time macro
command (RTM command) is coded in an NC program.
- Real time macro command (RTM command)
The real time macro command (RTM command) is a macro command
that starts execution in phase with an NC statement in the program.
After the execution of a real time macro command starts, the RTM
command operates independently of the NC statement.
An RTM command is a statement dedicated to the real time custom
macro function.
An RTM command consists of a set of one or more real time macro
statements (RTM statements).
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 580 -
- Real time macro statement (RTM statement)
The real time macro statement (RTM statement) is a statement
included in an RTM command.
One or more RTM statements make up an RTM command.
An RTM statement consists of a macro command and axis control
command dedicated to the real time custom macro function.
The axis control command of an RTM statement is an RTM statement
including an address. This command is used to exercise axis control.
Example
// ZDO ;
G90 G00 X100 ;
ZEND ;
(ZDO and ZEND are reserved words required for the axis control
command of an RTM statement, and are detailed later.)
The macro command of an RTM statement is a macro statement used
with an RTM statement for arithmetic/logical operation and signal
control. (In the example below, #RV[1] and #RV[2] are variables
dedicated to the real time macro command.)
Example
// #IOG[124, 5] = 1 ;
// #RV[1] = #RV[2] * 10 ;
Format
The real time macro command format is shown below.
The RTM command is a command with two slashes (//) prefixed at the
start of a block.
//n <real-time-macro-statement>
or
//n ZDO ;
<real-time-macro-statement>
:
ZEND ;
N: Modal ID (1 to 10) (Omissible)
When a proper number is coded in n, a modal real time
macro command is specified. When n is omitted, a
one-shot real time macro command is specified.
ZDO to ZEND are detailed later.
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 581 -
17.1 TYPES OF REAL TIME MACRO COMMANDS
17.1.1 Modal Real Time Macro Command / One-shot Real Time
Macro Command
Explanation
A command with ’//’ followed by an RTM statement is referred to as a
one-shot real time macro command (one-shot RTM command).
Example:
// #RV[1] = 30 ;
On the other hand, a command with ’//’ followed by number n (1 to
10) then an RTM statement is referred to as a modal real time macro
command (modal RTM command).
Example:
//3 #RV[1] = 30 ;
A one-shot RTM command starts when the execution of the first
following NC command starts. A started one-shot RTM command is
valid until the end of the NC command.
A modal RTM command starts when the execution of the first
following NC command starts, as in the case of a one-shot RTM
command.
Unlike a one-shot RTM command, however, a started modal RTM
command is valid until the automatic operation is completed.
- Start of a real time macro command
An RTM command starts when the execution of the first following
NC command starts.
Example:
When NC command (1) starts execution in the program below, macro
commands (2) and (4) are executed in succession without waiting for
the end of (1).
On the other hand, RTM command (3)starts execution when NC
command (5) starts execution after the end of NC command (1).
O0001 ;
G90 G00 X30. ; (1) NC command
#100=0 ; (2) Macro command
// #RV[0]=1 ; (3) RTM command
#102=2; (4) Macro command
G90 G00 X100. ; (5) NC command
M30 ;
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 582 -
- End of a real time macro command
When one of the following conditions is satisfied, the RTM command
is terminated.
Termination conditions common to one-shot RTM and modal RTM
commands
• When RTM command processing is completed
• When a reset occurs
Termination condition specific to a one-shot RTM command
• When the execution of the NC command that started at the same
time has ended
However, if the RTM statement being executed is an axis control
command, the command is terminated when the execution of the block
is completed.
If the execution of the Y10. block is completed before the X100. block
in the command below, and the execution of the Y20. block starts, for
example, the X100. command of the RTM statement is executed until
the end.
// ZDO ;
X100 ;
ZEND ;
Y10. ;
Y20. ;
NOTE
1 No one-shot RTM command can be specified using
any of the commands indicated below as a trigger.
When using any of these commands as a trigger,
use a modal RTM command.
- Command related to reference position return
- Command related to AI contour control
- Command related to canned cycles (rigid tapping,
drilling cycle, etc.)
- Command related to cutter compensation
- Command related to tool length compensation
- Command related to automatic tool length
measurement
- Command related to coordinate system rotation
Command related to scaling
- Command related to programmable mirror image
2 If an RTM command is specified using, as a trigger,
a block such as a block specifying NURBS
interpolation or a T series multiple repetitive canned
cycle that does not necessarily pass the start point
or end point of the command, operation can start or
end at a point other than the start point and end
point. Do not use such a block as a trigger.
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 583 -
NOTE
3 Do not restart a program that includes an RTM
command.
4 When an NC statement used as a trigger for an
RTM command represents an auxiliary function,
execution continues even if the FIN signal is
awaited.
If the following program is executed, for example,
the count-up operation of #RV[0] continues until the
FIN signal of M55 is returned:
O0001 ;
// ZWHILE [1] #RV[0] = #RV[0]+1 ;
M55 ;
G91 X200. ;
:
5 If M02 follows an RTM command, execution
continues until a reset occurs, even when the
program itself is terminated.
If the following program is executed, for example,
the count-up operation of #RV[0] continues until a
reset occurs:
O0001 ;
// ZWHILE [1] #RV[0] = #RV[0]+1 ;
M02 ;
- Priority of commands
If a modal RTM command and one-shot RTM command are specified
at the same time, the modal RTM command is executed first.
If multiple modal RTM commands are specified at the same time, the
commands are executed in ascending order of ID values.
No priority is applicable to one-shot RTM commands.
The order of execution is as follows:
Modal RTM command with ID value being 1
Modal RTM command with ID value being 2
:
:
Modal RTM command with ID value being 10
One-shot RTM command
:
One-shot RTM command
Example 1)
Priority of modal RTM commands
O0001 ;
//1 #RV[0]=1 ;
//3 #RV[0]=3 ;
//2 #RV[0]=2 ;
M02 ;
High
Low
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 584 -
When the program above is executed, the RTM commands are
executed in the following order:
#RV[0]=1
#RV[0]=2
#RV[0]=3
So, the value of #RV[0] is 3.
Example 2)
Priority of modal RTM commands and a one-shot RTM
command
O0001 ;
//3 #RV[0]=3 ;
//1 #RV[0]=1 ;
// #RV[0]=10 ;
//5 #RV[0]=5 ;
M02 ;
When the program above is executed, the RTM commands are
executed in the following order:
//1 #RV[0]=1
//3 #RV[0]=3
//5 #RV[0]=5
// #RV[0]=10
So, the value of #RV[0] is 10.
Example 3)
Priority of one-shot RTM commands
When the following program is executed, the value of #RV[0] is
undefined, that is, 1, 2, or 3.
O0001 ;
//#RV[0]=1 ;
//#RV[0]=2 ;
//#RV[0]=3 ;
G04P10 ;
M30 ;
Even if a priority is applicable, the order of execution or the order of
termination can change when an RTM statement includes a control
code, ZWHILE or ZEDGE, or axis control command.
Example 4)
The RTM command priority of #RV[0]=1 in a modal command
with its ID value being 1 is higher than the priority of #RV[1]=1
in a modal command with its ID value being 2. However,
#RV[0]=1 is executed after the end of the execution of the block
specifying the axis control command G91 G00 X10., so that
#RV[1]=1 is actually executed earlier than #RV[0]=1.
O0001 ;
//1 ZDO ;
G91 G00 X10. ;
#RV[0]=1 ;
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 585 -
ZEND ;
//2 #RV[1]=1 ;
G04 P10 ;
M30 ;
Example 5)
In the RTM command priority, ZEDGE in a modal command
with its ID value being 1 is always a false control code (detailed
later). The RTM command priority of #RV[0]=1 in a modal
command with its ID value being 1 is higher than the priority of
#RV[1]=1 and #RV[2]=1 in a modal command with their ID
values being 2. However, #RV[0]=1 is executed after the
condition of ZEDGE becomes true (that is, at the second time or
later), so that #RV[1]=1 and #RV[2]=1 are executed earlier than
#RV[0]=1.
O0001 ;
//1 ZEDGE [ #IOG[234.0] EQ 1 ] #RV[0]=1 ;
//2 ZDO ;
#RV[1]=1 ;
#RV[2]=1 ;
ZEND ;
G04 P10 ;
M30 ;
- Number of real time macro commands
A program can have multiple RTM commands coded.
Up to six one-shot RTM commands can be specified.
If one-shot RTM commands more than the maximum allowable
number are specified, an alarm is issued.
Up to ten modal RTM commands can be specified. When specifying
modal RTM commands, ensure that there is no duplicate ID.
If there is a duplicate ID, or an incorrect ID is specified, an alarm is
issued.
In all paths, up to 16 RTM commands can be executed
simultaneously.
When an axis control command is included, up to four commands can
be executed simultaneously.
NOTE
1 In a block specifying an RTM statement, no NC
command can be coded.
2 If the maximum specifiable number of commands or
the maximum number of simultaneously executable
commands is exceeded, a PS alarm is issued.
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 586 -
NOTE
3 If an NC statement to be used to trigger an RTM
command is specified in a block (e.g., small block) that
ends in a very short time, an RTM statement
programmed to start at a different timing may be
executed simultaneously. If the following is specified,
for example, #RV[0]=1 and #RV[1]=2 may be executed
simultaneously:
// #RV[0]=1 ;
G91 G01 X0.002 ; F5000
// #RV[1]=2 ;
X0.001 ;
4 When a function for reading multiple blocks in advance
is used, the same ID must not be coded in the scope of
blocks read in advance. In the following program, for
example, while //1 #RV[0]=#100101 is being executed
during AI contour control, //1 #RV[1]=#100101 and //1
#RV[2]=#100101 are also read in advance. So, an
alarm may be issued.
//1 #RV[0]=#100101 ;
X#100 ;
//1 #RV[1]=#100101 ;
X#100 ;
//1 #RV[2]=#100101 ;
X#100 ;
5 When a function for reading multiple blocks in advance
is used, up to three blocks among the blocks read in
advance can trigger an RTM command.
For example, if the blocks up to the block of (2) are
read in advance during execution of (1) in the program
below, up to three blocks can trigger an RTM
command. In the program below, the number of NC
blocks that trigger an RTM command exceeds 3, so
that the RTM command of (a) must not be coded.
X30. Y50. ; ......................................................(1)
// Z-30. ;
// #RV[0]=#RV[0]+1 ;
X3. Y16. ; → NC block 1 triggering an RTM command
X-23. Y4. ;
// #RV[1]=#RV[1]+1 ;
//2 Z30. ;
X-2. Y9. ; → NC block 2 triggering an RTM command
X17. Y5. ;
// #RV[2]=#RV[2]+1 ;
X-2. Y9. ; → NC block 3 triggering an RTM command
// #RV[3]=#RV[3]+1 ; ..........................................(a)
X-12. Y-3. ;
X-100. Y200. ; ....................................................(2)
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 587 -
- Reserved words
The following reserved words are used with real time custom macros:
- Reserved words dedicated to real time custom macros
ZDO, ZEND, ZONCE, ZWHILE, ZEDGE
- Reserved words shared with custom macros
AND, OR, XOR, MOD, EQ, NE, GT, LT, GE, LE, SIN, COS,
TAN, ASIN, ACOS, ATAN, ATN, SQRT, SQR, ABS, BIN,
BCD, ROUND, RND, FIX, FUP, LN, EXP, POW
Be sure to fully spell out the reserved words for real time custom
macros. For example, ’ZONCE’ must not be coded as ’ZON’
or ’ZONC’.
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 588 -
17.2 VARIABLES
Overview
With real time custom macros, the following variables can be handled:
- System variables dedicated to real time custom macros
- Variables (RTM variables) dedicated to real time custom macros
- System variables for some custom macros
The RTM variables mean the variables dedicated to real time custom
macros.
List of usable variables
Real time
custom macro
Custom
macro
System variables Usable Unusable Real time custom
macro variables RTM variables Usable Unusable
System variables Partially usable Usable
Common variables Unusable Usable
Custom macro
variables Local variables Unusable Usable
The variables (system variables and RTM variables) dedicated to real
time custom macros are the variables specific to the real time custom
macro function. Those variables cannot be used with the custom
macro function.
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 589 -
17.2.1 Variables Dedicated To Real Time Custom Macros
These variables are dedicated to real time custom macros. The
variables are classified as system variables and RTM variables.
17.2.1.1 System variables
System variables dedicated to real time custom macros
Format
#IOp [m, n] Bit-by-bit read/write
#IOpB [m] Byte-by-byte read/write
#IOpW [m] Word-by-word read/write
#IOpD [m] Double word-by-double word read/write
p : Signal type (X, G, F, Y, D, R)
m : Signal byte address
n : (Used for bit-by-bit read/write only) Signal address bit
number (0 to 7)
PMC interface signals are read and written. Bit-by-bit and
byte-by-byte read/write operations are possible.
The following signals can be used:
Variable name Signal type Read Write
#IOX
#IOXB
#IOXW
#IOXD
X Possible Impossible
#IOG
#IOGB
#IOGW
#IOGD
G Impossible Possible
#IOF
#IOFB
#IOFW
#IOFD
F Possible Impossible
#IOY
#IOYB
#IOYW
#IOYD
Y Impossible Possible
#IOD
#IODB
#IODW
#IODD
D Possible Possible
#IOR
#IORB
#IORW
#IORD
R Possible Possible
For the valid signal address range, see the specifications of the PMC
as well.
When writing to a signal, make the variable unprotected on the PMC
signal protection screen (described later) beforehand.
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 590 -
Specify an address by using m and n.
Example:
#IOF[1, 3] F1.3 bit type
#IOG[1, 5] G1.5 bit type
#IOFB[32] F32 byte type
#IOGB[12] G12 byte type
Read/write operations are performed in the same as for an ordinary
macro statement.
Example:
#RV[0]=#IOFB[32] Assigns F32 to #RV[0].
#IOG[99.3] = 1 Sets G99.3 to 1.
If a signal at a nonexistent address is specified, a PS alarm is issued.
CAUTION
1 Controls handling other signals, such as a ladder
or macro executor, must not write to a signal
address being written to by an RTM statement.
Ensure that a single control writes to the same byte
signal address.
For example, when the G000.0 signal is written to
by an RTM statement, do not write to the G000.7
signal from a ladder.
2 Ensure that the same F signal is not read from by
an RTM statement and written to by the NC
simultaneously.
3 Ensure that the same G signal is not written to by
an RTM statement and read from by the NC
simultaneously.
4 For word-by-word read/write, specify an
even-numbered address and for double
word-by-double word read/write, specify an
address that is a multiple of four.
NOTE
The system variables described above are not
supported for a multi-path PMC.
- PMC signal protection
Whether to enable a write to a signal handled by an RTM statement
can be set. This function protects against a malfunction due to
incorrect coding.
On the PMC signal protection screen, set whether to enable a write to
a signal.
If an RTM statement makes an attempt to write to a signal
write-protected on the PMC signal protection screen, a PS alarm is
issued at the time of execution.
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 591 -
Set whether to enable a write to each address of Y and G on a
byte-by-byte basis.
For each of addresses D and R, set a write-enabled range.
For the unwritable signals (X, F), the screen is not displayed.
Before changing an address on the PMC signal protection range
specification screen, perform a clear operation first and then input a
new address.
- Input/output
A value set for PMC signal protection can be input/output.
- Input/output format
After punching PMC signal protection, one file(DIDOENBL.TXT) is
created.
Please execute input/output operation in EDIT mode.
The output format is as follows:
L Specification method
0: Byte specification
1: Range specification
Q Alphabetic signal address
0: G, 2: Y, 5: R, 9: D
K (for use in range specification only) Index number (0 to 9)
R Address number for byte specification
Start address number for range specification
P Protection value for byte specification
0: Not writable
1: Writable
End address number
for range specification
Example of output
%
L0Q2R0000P0
L0Q2R0001P1
:
L0Q2R0127P1
:
L0Q0R0000P1
L0Q0R0001P1
:
L0Q0R0767P0
L0Q0R1000P1
:
L0Q0R1767P0
:
L1Q5K0R0002P0014
:
L1Q9K9R0032P0127
M02
%
Byte
specification
G0 to G767 protect
information
G1000 to G1767 protect
information
Y0 to Y127 protect
information
R2 to R14 are writable
(Index 0)
D32 to D127 are writable
(Index 9)
Range
specification
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 592 -
17.2.1.2 Real time macro variables (RTM variables)
The real time macro variables (RTM variables) are variables dedicated
to real time custom macros.
The RTM variables are classified as volatile real time macro variables
(volatile RTM variables) and nonvolatile real time macro variables
(nonvolatile RTM variables).
The data of a nonvolatile RTM variable is preserved even when the
power is turned off.
The data of a volatile RTM variable is cleared to 0 when the power is
turned off.
Format
#RV [ m ] Volatile RTM variable
m: Volatile RTM variable number (0 to 99)
#RVS [ n ] Nonvolatile RTM variable
n: Nonvolatile RTM variable number (0 to 31)
NOTE
1 RTM variables can be used with an RTM statement
only. RTM variables cannot be used with an NC
statement and macro statement.
2 No RTM variable assumes a "null" value.
3 Volatile RTM variables are cleared to 0 by a reset.
On the other hand, nonvolatile RTM variables are
not cleared to 0 by a reset.
Explanation
- Input/output
RTM variables can be input/output in a specified format.
Both nonvolatile RTM variables and volatile RTM variables can be
input/output.
- Input/output format
After punching RTM variables, one file(RTMMACRO.TXT) is
created.
The output format is described below.
The value of an RTM variable is output in hexadecimal as a
double-precision floating-point data bit image.
When a nonvolatile RTM variable is output, G10L87 is followed by
an RTM variable number and a variable value.
When a volatile RTM variable is output, G10L88 is followed by an
RTM variable number and a variable value.
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 593 -
Example of output
%
G10L87P0(3FE0000000000000)
G10L87P1(4000000000000000)
:
G10L87P30(4010000000000000)
G10L87P31(4014000000000000)
G10L88P0(4008000000000000)
G10L88P1(3FD9999999800000)
:
G10L88P98(3FF0000000000000)
G10L88P99(4010000000000000)
M02
%
Execute input/output operation in EDIT mode.
Nonvolatile RTM variable
Volatile RTM variable
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 594 -
17.2.2 Custom Macro Variables
With real time custom macros, a part of the custom macro variables
(part of the system variables) can be handled.
17.2.2.1 System variables
With real time custom macros, position-related information among the
system variables of the custom macros can be handled.
- Position information #100001 to #100182 (Attribute: Read only)
Block end position #100001 to #100032
Current position (machine coordinate system) #100051 to #100082
Current position (workpiece coordinate system) #100101 to #100132
Skip position #100151 to #100182
By readying the values of system variables #100001 to #100182, the
end position of the previous block, the current positions (machine
coordinate system and workpiece coordinate system), and skip signal
position can be found.
Variable No. Position information Coordinate system
#100001
#100002
:
#100032
Block end position on 1st axis
Block end position on 2nd axis
:
Block end position on 32nd axis
Workpiece coordinate
system
#100051
#100052
:
#100082
Current position on 1st axis
Current position on 2nd axis
:
Current position on 32nd axis
Machine coordinate
system
#100101
#100102
:
#100132
Current position on 1st axis
Current position on 2nd axis
:
Current position on 32nd axis
Workpiece coordinate
system
#100151
#100152
:
#100182
Skip position on 1st axis
Skip position on 2nd axis
:
Skip position on 32nd axis
Workpiece coordinate
system
NOTE
1 The value of a variable with a number greater than
the number of controlled axes is undefined.
2 The end position (ABSIO) of a skip (G31) block is
the skip signal ON position if the skip signal is
turned on. If the skip signal is not turned on, the
block end point is undefined.
3 As block end position information #100001 to
#100032, the end positions read in advance are
obtained instead of the end positions of the block
currently being executed.
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 595 -
- Servo positional deviation #100251 to #100282 (Attribute: Read only)
By reading the values of system variables #100251 to #100282, the
servo positional deviation on each axis can be found.
Variable No. Position information
#100251
#100252
:
#100282
Servo positional deviation on 1st axis
Servo positional deviation on 2nd axis
:
Servo positional deviation on 32nd axis
NOTE
The value of a variable with a number greater than
the number of controlled axes is undefined.
- Remaining travel distance #100801 to #100832 (Attribute: Read only)
By reading the values of system variables #100801 to #100832, the
remaining travel distance on each axis can be read.
Variable No. Position information
#100801
#100802
:
#100832
Travel distance on 1st axis
Travel distance on 2nd axis
:
Travel distance on 32nd axis
NOTE
1 The value of a variable with a number greater than
the number of controlled axes is undefined.
2 System variables not described here are unusable.
3 The name of a system variable cannot be
specified.
Do not specify a command as indicated below.
//1 #RV[0]=[#_ABSOT[1]] ;
17.2.2.2 Local variables
The local variables(#1 to #33) cannot be used.
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 596 -
17.3 ARITHMETIC AND LOGICAL OPERATION
With the real time custom macros, the following arithmetic and logical
operations can be specified:
Table 1.3 Arithmetic and logical operation
Type of operation Operation Description
(1) Definition, substitution #i=#j Definition or substitution of a variable
(2) Additive operation #i=#j+#k
#i=#j-#k
#i=#j OR #k
#i=#j XOR #k
Addition
Subtraction
Logical OR (Bit by bit for 32 bits)
Exclusive OR (Bit by bit for 32 bits)
(3) Multiplicative operation #i=#j*#k
#i=#j/#k
#i=#j AND #k
#i=#j MOD #k
Multiplication
Division
Logical AND (Bit by bit for 32 bits)
Remainder (#j and #k are rounded to an integer to
find a remainder. When #j is negative, #i is also
negative.)
(4) Function #i=SIN[#j]
#i=COS[#j]
#i=TAN[#j]
#i=ASIN[#j]
#i=ACOS[#j]
#i=ATAN[#j]
#i=ATAN[#j]/[#k]
#i=ATAN[#j,#k]
#i=SQRT[#j]
#i=ABS[#j]
#i=BIN[#j]
#i=BCD[#j]
#i=ROUND[#j]
#i=FIX[#j]
#i=FUP[#j]
#i=LN[#j]
#i=EXP[#j]
#i=POW[#j,#k]
Sine (in deg)
Cosine (in deg)
Tangent (in deg)
Arcsine
Arccosine
Arctangent (1 argument). ATN is acceptable.
Arctangent (2 arguments). ATN is acceptable.
Ditto
Square root. SQR is acceptable.
Absolute value
Binary conversion from BCD
BCD conversion from binary
Rounding. RND is acceptable.
Discarding fractional digits
Rounding fractional digits upward to an integer
Natural logarithm
Exponent with e (2.718……) used as the base
Power (#j to #k power)
- Constant specifiable in <expression>
+0.00000000001 to +999999999999
-999999999999 to -0.00000000001
Up to 12 decimal digits can be specified.
If the maximum allowable number of digits is exceeded, P/S0012
alarm is issued.
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 597 -
NOTE
1 The ADP function is not available.
2 With an RTM statement, the external output
commands (BPRNT, DPRNT, POPEN, and
PCLOS) are unavailable.
3 The FS16i compatibility specifications are not
applicable. Bit 0 (F16) of parameter No. 6008 = 1
(with the operation result precision based on the
FS16i compatibility specifications) is invalid.
4 For information on decreased precision, see
"When bit 0 (F16) of parameter No. 6008 is set to
0" in "Caution concerning decreased precision" in
the CUSTOM MACRO chapter.
5 Bit 0 (NAT) of parameter No. 6004 is valid in an
RTM command.
6 The setting of bit 5 (SBM) of parameter No. 6000
and bit 7 (SBV) of parameter No. 6000 is invalid.
For the single block specifications, see the
separate item.
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 598 -
17.4 CONTROL ON REAL TIME MACRO COMMANDS
Explanation
By using a reserved word for controlling statements in an RTM
command, the flow of the RTM command can be changed or multiple
statements can be controlled as a set of statements. Four reserved
words are used to control an RTM command as indicated below.
Reserved
word name Syntax Meaning
ZONCE // ZONCE A B If A is true, B is executed.
ZEDGE // ZEDGE A B If A becomes true, B is
executed.
ZWHILE // ZWHILE A B While A is true, B is executed
repeatedly.
ZDO...ZEND // ZDO B1 B2 B3 ZEND (Multiple statements) B1, B2,
and B3 are sequentially
executed.
The timing chart of an RTM command using these reserved words is
indicated below. (Multi-statement control ZDO...ZEND is
excluded.)
When the condition of a each reserved word is True, it shows ‘*’.
When condition A makes transitions from True to False to True
True
False
ZONCE *
ZEDGE
*
ZWHILE * * *
When condition A makes transitions from False to True to False
True
False
ZONCE
*
ZEDGE
*
ZWHILE
* * * * * * *
Time
Time
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 599 -
17.4.1 Conditional Branch (ZONCE Statement)
After ZONCE, <conditional-expression> and
<real-time-macro-statement> are coded.
- //(n) ZONCE [<conditional-expression>] <real-time-macro-statement>
If <conditional-expression> is true, <real-time-macro-statement> is
executed. If <conditional-expression> is false,
<real-time-macro-statement> is not executed, but control exits from
the ZONCE command to terminate the execution.
<conditional-expression> conforms to the custom macro
specifications.
// ZONCE A B (If A is true, B is executed.)
If A is true, the command is terminated after executing B.
If A is false, the command is terminated without executing B.
If the workpiece coordinate on the first axis is greater than 30, the Y1.0 signal
is output.
// ZONCE [#100101 GT 30.] #IOY[1,0] = 1 ;
If the workpiece coordinate on the first axis is greater than 30 and #RV[0]
matches #RV[3], the Y1.0 signal is output.
// ZONCE[[#100101 GT 30.] AND [#RV[0] EQ #RV[3]]] #IOY[1,0]=1 ;
In <real-time-macro-statement>, multiple RTM statements can be
coded.
In this case, code the following by using ZDO...ZEND of
multi-statement structure:
// ZONCE [<conditional-expression>] ZDO ;
<real-time-macro-statement-1> ;
<real-time-macro-statement-2> ;
:
ZEND ;
If the workpiece coordinate on the second axis is equal to or less than 10, the
rapid traverse override value is changed.
// ZONCE [#100102 LE 10.] ZDO ;
#IOG[14,0]=0 ;
#IOG[14,1]=1 ;
ZEND ;
However, if <conditional-expression-1> specifies an axis control
command, be sure to use ZDO...ZEND even when a single statement
is used.
If the workpiece coordinate on the first axis is greater than 30 and #RV[0]
matches #RV[3], a movement on the A-axis starts.
//1 ZONCE [[#100101 GT 30.] AND [#RV[0] EQ #RV[3]]] ZDO ;
G91 G00 A20. ;
ZEND ;
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 600 -
Similarly, use ZDO...ZEND for a multi-statement including an axis
control command.
If the workpiece coordinate on the second axis is equal to or less than 10, a
movement on the V-axis starts and the Y1.0 signal is set to 1.
//1 ZONCE [#100102 LE 10.] ZDO ;
G91 G00 V10. ;
#IOY[1,0] = 1 ;
ZEND ;
17.4.2 Condition Transition (ZEDGE Statement)
After ZEDGE, <conditional-expression> and
<real-time-macro-statement> are coded.
// ZEDGE A B (If A becomes true, B is executed.)
- //(n) ZEDGE [<conditional-expression>] <real-time-macro-statement>
When <conditional-expression> makes a transition from false to true,
an RTM statement specified after <conditional-expression> is
executed. <conditional-expression> conforms to the custom macro
specifications.
With the ZEDGE command, the result of the first evaluation of
<conditional-expression> is always false.
Explanation
The difference between the ZONCE command and ZEDGE command
is that if <conditional-expression> is false, the RTM statement itself is
terminated in the case of ZONCE, while the evaluation of
<conditional-expression> continues until <conditional-expression>
becomes true in the case of ZEDGE. (With a one-shot real time
macro command, the evaluation of <conditional-expression>
continues until the execution of the NC statement that started
operation simultaneously with the command ends.)
On the rising edge of the G address signal 4.3, the workpiece coordinate on
the third axis is read.
// ZEDGE [#IOG[4,3] EQ 1] #RV[0]=#100103 ;
In the example above, even if the [#IOG[4,3] EQ 1] is true from the
beginning, #RV[0]=#100103 of the RTM statement is not executed.
#RV[0]=#100103 is executed when the result of evaluation of
[#IOG[4,3] EQ 1] changes from false to true.
As in the case of ZONCE, multiple RTM statements can be coded in
<real-time-macro-statement>.
If <conditional-expression-1> specifies an axis control command, be
sure to use ZDO...ZEND even when a single statement is used.
Code the following by using ZDO...ZEND of multi-statement
structure:
// ZEDGE [<conditional-expression>] ZDO ;
<real-time-macro-statement-1> ;
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 601 -
<real-time-macro-statement-2> ;
:
ZEND ;
On the falling edge of the X address signal, a movement on the B-axis is
started and the Y1.0 signal is set to 1.
// ZEDGE [#IOX[1,3] EQ 0] ZDO ;
G91 G00 B10. ;
#IOY[1,0] = 1 ;
ZEND ;
On the rising edge of the Ｇ address signal, a movement on the U-axis is
started.
// ZEDGE [#IOG[4,3] EQ 1] ZDO ;
G91 G00 U25. ;
ZEND ;
If the remaining travel distance on the second axis is equal to or less than 10,
the rapid traverse override value is changed.
// ZEDGE [#100802 LE 10.] ZDO ;
#IOG[14,0]=0 ;
#IOG[14,1]=1 ;
ZEND ;
17.4.3 Repetition (ZWHILE Statement)
After ZWHILE, a <conditional statement> is coded.
// ZWHILE A B (While A is true, B is executed repeatedly.)
- //(n) ZWHILE [<conditional-expression>] <real-time-macro-statement>
While <conditional-expression> is true, the RTM statement specified
after <conditional-expression> is executed.
If <conditional-expression> is not satisfied, the ZWHILE statement is
terminated, and the next block is processed.
ZEND ;
:
<Real time macro
statement>
When
condition
is true
* When the <real time macro statement> is a single statement and is not
an axis control statement, ZDO and ZEND are not required.
* When “conditional-expression” is fulfilled and “Real time macro
statement” is complete, interpolation cycle time has passed before the
next evaluation of "ZWHILE conditional-expression".
ZWHILE
<conditional-expression> ZDO ; When condition is
false
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 602 -
Explanation
While <conditional-expression> is true, the command or commands
between ZDO and ZEND after ZWHILE are executed.
If <conditional-expression> is not satisfied, the command after ZEND
is processed.
The same <conditional-expression> and operators as for the ZONCE
statement are used.
While the F address 234.1 signal is 1, an incremental movement on the
U-axis is repeatedly performed, and #RV[0] is incremented by 1 each time.
//1 ZWHILE [#IOF[234,1] EQ 1] ZDO ;
G91 G00 U10. ;
#RV[0] = #RV[0]+1 ;
ZEND ;
17.4.4 Multi-statement (ZDO...ZEND Statement)
- //(n) ZDO ;
<real-time-macro-statement-1> <real-time-macro-statement-2>
<real-time-macro-statement-3> …
ZEND ;
One or multiple statements enclosed in ZDO...ZEND are regarded as a
one RTM statement (multiple-statement structure).
Explanation
The maximum number of RTM statements in one multi-statement
(between ZDO...ZEND) is roughly five, but it is subject to change
(Because it depends on the contents of RTM statements).
ZDO...ZEND is used in the following cases:
• When multiple <real time macro statements> are handled as a
series of commands
If the workpiece coordinate on the first axis exceeds 30, the rapid traverse
override value is changed.
// ZEDGE [#100101 GT 30.] ZDO ;
#IOG[14,0]=1 ;
#IOG[14,1]=0 ;
ZEND ;
• When an axis control command is specified
On the rising edge of the X signal 7.0, a movement on the V-axis is started.
// ZEDGE [#IOX[7,0] EQ 1] ZDO ;
G91 G00 V35. ;
ZEND ;
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 603 -
- Nesting
ZONCE, ZEDGE, ZWHILE, and ZDO...ZEND cannot be nested and
overlapped.
For details, see the following:
- Endless loop
An endless loop is formed if the conditional expression enclosed in
brackets after the ZWHILE statement is always satisfied.
Example)
In the example below, #RV[0] is counted up unconditionally.
// ZWHILE [1] #RV[1]=#RV[1]+1 ;
Processing
1. ZONCE, ZEDGE, ZWHILE, and
ZDO...ZEND may be used any
number times.
// ZWHILE […] ZDO ;
ZEND ;
:
Processing
// ZONCE[…] ZDO ;
ZEND ;
:
2. One ZDO...ZEND range must not
overlap another ZDO...ZEND range.
Processing
// ZONCE […] ZDO ;
ZEND ;
Processing
// ZWHILE […] ZDO ;
:
ZEND ;
3. ZONCE, ZEDGE, ZWHILE, and
ZDO...ZEND must not be
nested.
// ZWHILE […] ZDO ;
:
ZONCE […] ZDO ;
:
ZEDGE […] ZDO ;
Processin
g
ZEND ;
:
ZEND ;
:
ZEND ;
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 604 -
Sample program
The sample program below exercises the following three control
operations at the same time.
(1) A cutting operation is performed on the X-axis and Z-axis.
(2) On each rising edge of the X signal 5.2, 20 is fed on the
peripheral axis A.
(3) When the workpiece coordinate on the X-axis (#100101) is equal
to or less than 50, the Y signal 2.3 is set to 1.
The operation of (1) is coded in the main NC statement.
The operation of (2) is coded in the first modal RTM command (//1).
The operation of (3) is coded in the second modal RTM command
(//2).
O0001 ;
G90 G00 X100 Z100;
//1 ZWHILE[1] ZDO ;
ZEDGE [#IOX[5,2] EQ 1 ] ZDO ;
G91 G00 A20. ;
ZEND ;
ZEND ;
//2 ZWHILE[1] ZDO ;
ZEDGE [ #100101 LE 50.0 ] #IOY[2,3] = 1 ;
ZEND ;
#100=100 ;
WHILE [ #100 GT 0 ]) DO1
G91 G01 Z-#100 F200. ;
Z#100. ;
#100 = #100 - 10 ;
X-10. F100;
END1
M02 ;
Workpiece
50
(Y signal is
turned on
when tool
enters this
range.)
X
Z
RTM command (2)
operation
(On each rising edge of
X5.2, 20 is fed on peripheral
axis A.)
RTM command (3)
operation
(When X coordinate is 50 or
less, Y signal 2.3 is set to 1.)
Command for cutting on
X-axis and Z-axis
Peripheral axis A
Signal switch
(Address X5.2)
Signal lamp
(Address
Y2.3)
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 605 -
17.5 MACRO CALL
A series of RTM statements can be formed into a subprogram, which
can be called from the main program.
When G65 is specified in an RTM command, the real time macro
specified in address P is called.
Explanation
- Calling
In address P after G65, specify the program number of a real time
custom macro to be called.
NOTE
1 In argument P of G65, only a constant value can
be used. No value can be specified through a
variable.
Example:
// G65 P9010 ; Correct
// G65 P#RV[0] ; Incorrect
2 The inclusion of another NC command (such as
G01 X100.0 G65 Pp) is not allowed. If another
NC command is included, PS0127 alarm is issued.
3 The G65 block for calling a real time macro does
not make a single block stop.
4 On the other hand, a real time macro program
called by real time macro calling makes a single
block stop.
P : Number of real time macro program to be called
O0001 ;
:
:
//1 G65 P9010 ;
G04 P2000 ;
:
:
M30 ;
O9010 ;
:
:
:
:
:
:
M99 ;
G65 P p ;
The execution of real time macro //1 including O9010 starts simultaneously
with the G04 block of main program O0001.
Code real time macro
statements.
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 606 -
- Call destination real time program
In a called real time macro program, only an RTM statement can be
coded.
In a called real time macro program, no additional RTM command
may be executed. (The RTM command symbol ‘//’ may not be
coded.) For example, do not execute the following program:
O0001 ; O9010 ;
// G65 P9010 ; // #RV[0]=1 ;
M02 ; M99 ;
Code M99 in the last block only.
For example, do not execute the following program:
O0001 ; O9010 ;
// G65 P9010 ; ZEDGE [#RV[0] EQ 1] M99 ;
M02 ; G91 G00 X50. ;
M99 ;
When executing an RTM statement in a subprogram, code an NC
statement before the M99 block for returning to the calling program.
O0001 ; O9010 ;
G65 P9010 ; // #RV[0] = 20 ; Real time macro statement
M02 ; G04 ; NC statement
M99 ;
- Format
Specify G65 at the start of a block.
- Call nesting level
Macro call nesting is not allowed.
- Differences from macro call using a custom macro
Macro call using a real time custom macro and macro call using a
custom macro differs as described below.
• In macro call using a custom macro, an argument (data to be
passed to a macro) and the number of repetitions can be specified.
In macro call using a real time custom macro, such information
cannot be specified.
• With a real time custom macro, other types of macro call (macro
call using G66, G66.1, G, and M code) and subprogram call are
not allowed.
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 607 -
17.6 OTHERS
If an axis control command is followed by a macro command in an
RTM command, the execution of the macro command starts when the
axis control command is completed or deceleration starts.
If deceleration on the X-axis starts upon completion of distribution
according to the axis control command of (1), for example, the macro
command of (2) is executed. If acceleration/deceleration is not
applied on the X-axis, (2) is executed upon completion of distribution
on the X-axis.
// ZDO ;
G91 G00 X30 ; (1) Axis control command of the RTM statement
#RV[0] = 1 ; (2) Macro command of the RTM statement
ZEND ;
If an RTM command is executed in a custom macro WHILE DO to
END loop, and the same RTM is looked ahead while the RTM
command is being executed, a PS alarm may be issued.
For example, if the command below is executed, a PS alarm is issued.
WHILE [1] DO1 ;
// #RV[0] = #RV[0] + 1 ;
#100=#100+1 ;
END1 ;
In this example, insert G04 ; block between a #100=#100+1; and
END1;.
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 608 -
17.7 AXIS CONTROL COMMAND
In an RTM statement, a G code for specifying a movement can be
specified. For axis control, the PMC axis control interface is used.
The specifications differ from the specifications for the G code used
with an NC statement.
Format
// ZDO ;
G_ IP _ F_ ;
:
ZEND ;
For an axis control command, ZDO...ZEND of multi-statement
structure is used for coding even if a single statement (single RTM
statement) is used.
CAUTION
Do not specify an NC statement for an axis to be
controlled with an RTM statement. Moreover, do
not exercise axis control with an RTM statement on
an axis to be controlled with an NC statement.
NOTE
1 In one block, only one axis may be specified. Do
not specify two or more axes in the same block.
2 In the three-dimensional coordinate conversion
mode, the polygon mode, etc., an RTM statement
concerning that axis cannot be specified.
Explanation
- Setting
For an axis control command in an RTM statement, the interface of a
PMC axis control group set by a parameter beforehand is used.
For an axis to be controlled with an RTM statement, set a group to be
used with parameter No. 8010. Then, set bit 0 (XRT) of parameter
No. 8011 for the axis to 1.
NOTE
An axis for which bit 0 (XRT) of parameter No.
8011 is set to 1 is dedicated to real time custom
macros, so that such an axis cannot be used with
PMC axis control.
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 609 -
- Relationship with PMC axis control
Axis control based on an RTM statement uses the PMC axis control
interface. So, the specifications for a move command in each block
within an RTM statement are generally equivalent to the specifications
for the PMC axis control command.
For the detailed specifications and restrictions related to axis control,
refer to the specifications of PMC axis control as well.
NOTE
1 An axis used with an RTM statement must not be
specified from PMC axis control.
2 A PMC axis control group used with an RTM
statement must not be specified from PMC axis
control.
- Operation command code
The table below indicates the G codes that can be specified in an RTM
statement.
The mark in the table indicates modal G codes when an RTM
command starts.
Code Group Meaning
G00 Positioning
G01 01 Feed at specified feedrate
G28 Reference position return
G53 00 Machine coordinate system selection
G90 Absolute command
NOTE 1
G91 03 Incremental command NOTE 2
G94 Feed per minute
G95 05 Feed per revolution
NOTE
1 The absolute command (G90) is valid for machine
coordinate system selection (G53) only.
2 The incremental command (G91) is valid for
positioning (G00), linear interpolation (G01), and
reference position return (G28) only.
3 In T series G code system A as well, not G98/G99
but G90/G91 are valid with an RTM command.
- Modal information
Basically, modal information such as F and modal G codes in an RTM
statement is independent in an NC statement and each RTM statement.
Modal information in an RTM statement is initialized when the
execution of the RTM statement is started (when a block specified
with // is executed).
The initial value of modal information in an RTM statement is as
follows:
State of the G codes marked with in the operation command
code list
F code : F0
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 610 -
CAUTION
With the G codes (inch input/metric input) of group
06, the same information as the modal information
of an NC statement is used in an RTM statement.
Do not change the modal information of group 06
with an NC statement in a block after the first RTM
statement coded in a program.
NOTE
With an RTM command, bit 0 (G01), bit 3 (G91),
and bit 4 (FPM) of parameter No. 3402 are invalid
when the power is turned on or in the cleared
state.
Example 1)
Modal information can be controlled independently in an NC
statement and each RTM statement.
O0001 ;
G90 G01 X100. Y100. F500. ; (1)
//1 ZDO ;
Z50. ; (2)
G01 Z100. F100. ; (3)
ZEND ;
//2 ZDO ;
G01 A30. F200. ; (4)
A50. ; (5)
ZEND ;
X200. ; (6)
:
The modal information of command (2) is G00, G91, and G94,
regardless of the modal information (G90 G01 set in (1)) of the
NC statement.
The modal information of command (5) is G01, G91, G94, and
F200.. This modal information is not affected by the modal
information (command (1)) of the NC statement and the modal
information (commands (2) and (3)) in the RTM statement with
modal ID=1.
The modal information of command (6) is not affected by the
modal information (commands (2) to (5)) in the RTM statement,
so that the modal information is G01, G90, and F500..
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 611 -
Example 2)
Modal information is initialized when the execution of each
RTM command is started. Even if the same program includes
RTM commands with the same ID, the modal information of the
RTM command executed first is not inherited by the RTM
command executed next.
O0001 ;
G90 G01 X100. Y100. F500. ;
//1 ZDO ;
G01 Z100. F3000. ; (1)
ZEND ;
X200. ;
//1 ZDO ;
Z200. ; (2)
ZEND ;
X300. ;
:
The modal information of command (2) is G91 and G00,
regardless of command (1).
- Single block stop
If an NC statement is placed in the single block stop state, for example,
by the single block stop signal SBK, the axis control command of an
RTM statement also comes to a single block stop.
However, the automatic operation start signal STL is turned off when
all conditions on the NC statement side are satisfied, even if the axis
control command of an RTM statement is not terminated.
If an RTM command consists of multiple statements and an axis
control command is coded in multiple blocks, only the block of the
RTM statement that is currently executing an axis command can be
brought to a single block stop by setting the group-by-group single
block stop signal (ESBKg) for PMC axis control corresponding to the
axis to 1.
- Feed hold
Even when an NC statement enters the automatic operation halt state,
the axis control command of an RTM statement does not stop
immediately but stops at the time of termination of the block currently
being executed. To stop also the axis control command of an RTM
statement immediately when the NC statement enters the automatic
operation halt state, control the temporary stop signal (ESTPg) for
PMC axis control of the related group by monitoring the automatic
operation halt in-progress signal (SPL).
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 612 -
- Reset
Even when the CNC is reset by an MDI reset, the external reset signal
(ERS), or the reset and rewind signal (RRW), the axis control
command of an RTM statement does not stop immediately but stops at
the time of termination of the block currently being executed. When
the emergency stop state is set, however, the RTM statement also
stops immediately.
During execution of the axis control command of an RTM statement,
the real time macro being executed can be stopped independently of
the NC statement by setting the group-by-group reset signal (ECLRg)
for PMC axis control corresponding to the axis to 1. To stop also the
axis control command of an RTM statement when the CNC is reset,
control the reset signal (ECLRg) for PMC axis control of the related
group by monitoring the reset signal (RST).
- Alarm stop
Even when a PS alarm is issued with an NC statement, the axis control
command of the RTM statement being executed does not stop
immediately but stops at the time of termination of the block currently
being executed. Moreover, even when an overtravel alarm is issued
for an axis other than the axis controlled by the RTM statement being
executed, the RTM statement being executed does not stop
immediately but stops at the time of termination of the block currently
being executed.
- Alarm reset
When the group-by-group alarm signal (EIALg) for PMC axis control
corresponding to the axis specified by an RTM statement is set to 1,
correct the cause of the alarm, then reset the CNC, and reset PMC axis
control with the reset signal (ECLRg) for PMC axis control of the
related group.
(Tip)
In the following cases, the alarm signal (EIALg) is set to 1:
(1) When a servo alarm is issued
(2) When an overtravel alarm is issued
(3) When P/S0130 alarm is issued
(4) When P/S0139 alarm is issued
- Interlock
In an RTM statement, the interlock signal (*IT) for an NC statement,
interlock signal for each axis (*ITn), interlock signal for each axis
direction (+ITn/-ITn) are invalid. Instead, the axis control temporary
stop signal (ESTPg) for PMC axis control is valid in an RTM
statement. When temporarily stopping the axis controlled by an
RTM statement, control the corresponding axis control temporary stop
signal (ESTPg) for PMC axis control.
The cutting block start interlock signal *CSL (G8.1) and the block
start interlock signal *BSL (G8.3) are invalid.
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 613 -
- Machine lock
The same machine lock signals (all axes/each axis) as used with an
NC statement are used. However, by disabling machine lock for
PMC axis control with the following parameters, machine lock can be
disabled for the axis being controlled by an RTM statement:
Bit 0 (MLE) of parameter No. 8001
Bit 1 (MLS) of parameter No. 8006
- Dry run
With bit 2 (OVE) of parameter No. 8001, whether to use the dry run
signal (DRN) for an NC statement or the dry run signal (EDRN) for a
PMC axis can be chosen. When enabling a dry run feedrate for rapid
traverse in an RTM statement, set bit 3 (RDE) of parameter No. 8001
to 1. If a feed command specifying a feedrate is specified when the
manual rapid traverse selection signal (RT or ERT) is set to 1, the
cutting feedrate is used as the feedrate during dry run. ("Dry run
feedrate × maximum manual feedrate override value" is not
applicable.)
- In-position check
In the in-position state, the in-position signal (EINPg) is set to 1.
When bit 6 (NCI) of parameter No. 8004 is set to 1, no in-position
check is made during axis control based on an RTM statement. The
setting of bit 5 (NCI) of parameter No. 1601 for an NC statement is
invalid. (However, the in-position signal (INPx) for an NC statement
is affected by the value of NCI.)
- Manual absolute
The manual absolute signal (*ABSM) is invalid.
- External deceleration
By setting bit 0 (EDC) of parameter No. 8005 to 1, the external
deceleration function can be used also for the axis being controlled by
an RTM statement. Note, however, that the external deceleration
function is unusable for feed with a specified feedrate (feed per
revolution). For an external deceleration rate, the external
deceleration rate setting for rapid traverse (parameter No. 1427, No.
1441, and No. 1444) is valid, regardless of the type of feed.
The external deceleration function for the axis being controlled by an
RTM statement is also valid for feed with a specified feedrate (feed
per minute), regardless of the settings of bit 4 (EDP) of parameter No.
1005 and bit 5 (EDM) of parameter No. 1005. (The enabling of rapid
traverse only is impossible.)
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 614 -
- Mirror image
At enabling mirror image for the axis being controlled by an RTM
statement, set bit 0 (EMR) of parameter No. 8008 to 1, and set either
bit 0 (MIRx) of parameter No.0012 or mirror image signal MIx to '1'.
Programmable mirror image is not available.
NOTE
1 The same group as the PMC axis control group
used for axis control cannot be executed with an
RTM statement.
2 No NC statement can specify an axis being
controlled by an RTM statement.
3 An alarm is issued if, during execution of an RTM
statement, an attempt is made to execute another
RTM statement with the same ID. In the program
below, for example, the RTM statement of (1)
operates using the NC statement of (2) as a
trigger, and the RTM statement of (3) operates
using the NC statement of (4) as a trigger. An
alarm is issued if (1) is still operating when (4) is
started after completion of the interpolation of (2).
//1 ZDO ;
G91 G00 A100. ; (1) RTM statement
ZEND ;
G01 X30. Y20. ; (2) NC statement
//1 ZDO ;
G91 G00 B100. ; (3) RTM statement
ZEND ;
X40. Y50. ; (4) NC statement
4 When T series G code system A is used, address
words (such as U, W, H, and V) for incremental
commands must not be coded. Otherwise, alarm
PS0413 is issued.
5 An RTM statement for performing axis control
proceeds to the next command at the end of
distribution. For example, in the program below,
#RV[0] counts up at the time X50. distribution ends
and deceleration starts.
// ZDO ;
G00 X50. ;
#RV[0]=#RV[0]+1 ;
ZEND ;
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 615 -
Command details
- Rapid traverse
A movement is made at a rapid traverse rate on an axis from the
current position to the point separated by a specified value.
Format
// ZDO ;
G91 G00 IP _ ;
ZEND ;
G91 : G code for incremental command
IP _ : Travel distance
NOTE
1 Only one axis can be specified in one block.
2 The absolute command (G90) cannot be specified.
3 The rapid traverse overlap function cannot be
used.
4 When using this function, be sure to set bit 0
(RPD) of parameter No. 8002 to 0.
• Rapid traverse override
With bit 2 (OVE) of parameter No. 8001, whether to use the
rapid traverse override signal (ROV) for an NC statement or the
rapid traverse override signal (EROV) dedicated to PMC axis
control can be chosen.
NOTE
Even if bit 4 (RF0) of parameter No. 1401 is set to
1, rapid traverse does not stop with a cutting feed
override of 0%.
- Feed with a specified feedrate (feed per minute)
A movement is made at a feedrate specified in F on an axis from the
current position to the point separated by a specified value.
Format
// ZDO ;
G94 G91 G01 IP _ F_ ;
ZEND ;
G94 : G code for feed per minute
G91 : G code for incremental command
IP __: Travel distance
F__ : Feedrate command (mm/min or inch/min)
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 616 -
NOTE
1 Only one axis can be specified in one block.
2 The absolute command (G90) cannot be specified.
3 The block overlap function cannot be used.
4 When IS-A is used, a feedrate below 10 mm/min is
discarded.
5 The feedrate cannot be clamped to a
parameter-set maximum cutting feedrate.
6 No time is added to the cumulative cutting time.
7 Even if this command is executed, the cutting
in-progress signal is not output.
8 The operation between blocks for feed with a
specified feedrate is performed in the cutting
mode.
9 For this command, the feedrate arrival signal SAR
(G029.4) cannot be used.
• Feedrate specification range
The table below indicates the feedrate specification range.
Linear axis
Metric input
(mm/min)
Inch input
(inch/min)
Rotation axis
(deg/min)
IS-A 10. to 240000. 0.1 to 6553.5 10. to 240000.
IS-B 1. to 65535. 0.01 to 655.35 1. to 65535.
IS-C 0.1 to 6553.5 0.001 to 65.535 0.1 to 6553.5
IS-D 0.01 to 655.35 0.0001 to 6.5535 0.01 to 655.35
IS-E 0.001 to 65.535 0.00001 to 0.65535 0.001 to 65.535
NOTE
1 Be sure to set the following parameters to 0:
Bit 3 (F10) of parameter No. 8002
Bit 4 (EFD) of parameter No. 8006
Bit 4 (PF1) of parameter No. 8002
Bit 5 (PF2) of parameter No. 8002
When a value other than 0 is set, the feedrate
specification range changes, depending on the set
parameter.
2 A value less than the lowest feedrates indicated
above is discarded.
• Feedrate override
With bit 2 (OVE) of parameter No. 8001, whether to use the
feedrate override signal (*FV) for an NC statement or the
feedrate override signal (*EFOV) dedicated to PMC axis control
can be chosen.
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 617 -
NOTE
1 The second feedrate override function cannot be
used.
2 The feedrate override function cannot be disabled
using #3004.
• Override cancel
With bit 2 (OVE) of parameter No. 8001, whether to use the
feedrate override cancel signal (OVC) for an NC statement or the
feedrate override cancel signal (EOVC) dedicated to PMC axis
control can be chosen.
• Operation between blocks
If feed with a specified feedrate is performed in succession in
RTM statements, no stop occurs between blocks, but the next
block is executed. With the accumulated pulse zero check
signal (ELCKZg) for PMC axis control, an accumulated pulse
zero check can be made between blocks specifying feed with a
specified feedrate.
NOTE
1 The error detect signal (SMZ) cannot be used.
2 With the accumulated pulse zero check signal
(ELCKZg) for PMC axis control, an accumulated
pulse zero check can be made between blocks
specifying feed with a specified feedrate for feed on
the same axis only.
• Acceleration/deceleration time constant
For an acceleration/deceleration time constant to be used for feed
with a specified feedrate in an RTM statement when exponential
acceleration/deceleration is used, whether to use the time
constant for an NC statement or the time constant dedicated to
PMC axis control can be chosen using parameter No. 8030.
NOTE
Look-ahead acceleration/deceleration before
interpolation cannot be used.
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 618 -
- Feed with a specified feedrate (feed per revolution)
A movement is made at a feedrate specified in F on an axis from the
current position to the point separated by a specified value.
Format
// ZDO ;
G95 G91 G01 IP _ F_ ;
ZEND ;
G95 : G code for feed per revolution
G91 : G code for incremental command
IP _ : Travel distance
F_ : Feedrate command (mm/rev or inch/rev)
NOTE
1 Only one axis can be specified in one block.
2 The absolute command (G90) cannot be specified.
3 The block overlap function cannot be used.
4 Be sure to set the parameters below to 0. If a
value other than 0 is set, the feedrate specification
range changes, depending on the set parameter.
FR1 (bit 6 of parameter No. 8002)
FR2 (bit 7 of parameter No. 8002)
5 The feedrate is clamped to the maximum cutting
feedrate set in parameter No. 8022. (Parameter
No. 1430 for an NC statement is not valid for this
command.)
6 To use feed per revolution, a position coder is
required at all times. (Bit 0 (NPC) of parameter
No. 1402 is not applicable to this command.)
7 No time is added to the cumulative cutting time.
8 Even if this command is executed, the cutting
in-progress signal is not output.
9 The operation between blocks for feed with a
specified feedrate is performed in the cutting mode
at all times.
10 For this command, the feedrate arrival signal SAR
(G029.4) cannot be used.
• Feedrate specification range
The table below indicates the feedrate specification range.
Linear axis
Metric input
(mm/rev)
Inch input
(inch/rev)
Rotation axis
(deg/rev)
T series 0.001 to 65.535 0.000001 to 0.65535 0.001 to 65.535
M series 0.01 to 500.00 0.0001 to 6.5535 0.01 to 500.00
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 619 -
• Feedrate override
With bit 2 (OVE) of parameter No. 8001, whether to use the
feedrate override signal (*FV) for an NC statement or the
feedrate override signal (*EFV) dedicated to PMC axis control
can be chosen.
NOTE
1 The second feedrate override function cannot be
used.
2 The feedrate override function cannot be disabled
using #3004.
• Override cancel
With bit 2 (OVE) of parameter No. 8001, whether to use the
feedrate override cancel signal (OVC) for an NC statement or the
feedrate override cancel signal (EOVC) dedicated to PMC axis
control can be chosen.
• Operation between blocks
If feed with a specified feedrate is performed in succession in
RTM statements, no stop occurs between blocks, but the next
block is executed. With the accumulated pulse zero check
signal (ELCKZg) for PMC axis control, an accumulated pulse
zero check can be made between blocks specifying feed with a
specified feedrate.
NOTE
1 The error detect signal (SMZ) cannot be used.
2 With the accumulated pulse zero check signal
(ELCKZg) for PMC axis control, an accumulated
pulse zero check can be made between blocks
specifying feed with a specified feedrate for feed on
the same axis only.
• Acceleration/deceleration time constant
For an acceleration/deceleration time constant to be used for feed
with a specified feedrate in an RTM statement when exponential
acceleration/deceleration is used, whether to use the time
constant for an NC statement or the time constant dedicated to
PMC axis control can be chosen using parameter No. 8030.
NOTE
Look-ahead acceleration/deceleration before
interpolation cannot be used.
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 620 -
- Reference position return
A movement is made at the rapid traverse rate to the first reference
position on a specified axis. Upon completion of reference position
return, the return completion lamp is turned on.
Format
// ZDO ;
G91 G28 IP 0 ;
ZEND ;
G91 : G code for incremental command
IP 0 : Specify an axis on which reference position return is to
be performed.
Be sure to specify 0 as the travel distance.
NOTE
1 Only one axis can be specified in one block.
2 No intermediate point may be specified. (Be sure
to specify 0 as the travel distance. Otherwise,
alarm PS0410 is issued.) If a movement needs to
be once made to an intermediate point, specify
positioning with rapid traverse (G00)/machine
coordinate system selection (G53) then specify this
command.
3 The absolute command (G90) cannot be specified.
4 When using this function, be sure to set bit 0 (RPD)
of parameter No. 8002 to 0.
5 Before this command can be specified, a reference
position must be established. (With this command,
do not specify an axis on which a reference position
is not established.)
6 Before specifying this command with the T series,
cancel tool offset and tool-nose radius
compensation. Before specifying this command
with the M series, cancel cutter compensation, tool
length compensation, and tool offset.
• Rapid traverse override
With bit 2 (OVE) of parameter No. 8001, whether to use the
rapid traverse override signal for an NC statement or the rapid
traverse override signal dedicated to PMC axis control can be
chosen.
NOTE
Even if bit 4 (RF0) of parameter No. 1401 is set to
1, rapid traverse does not stop with a cutting feed
override of 0%.
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 621 -
- Machine coordinate system selection
When a position in the machine coordinate system is specified, a
movement is made to the position on the axis by rapid traverse. The
G53 code for machine coordinate system selection is a one-shot G
code, so that a command in the machine coordinate system is valid in
the block that specifies G53. When moving the tool to a
machine-specific position such as a tool change position, perform
programming in the machine coordinate system based on G53.
Format
// ZDO ;
G90 G53 IP _ ;
ZEND ;
G90 : G code for absolute command
IP _ : Position in machine coordinate system
NOTE
1 Only one axis can be specified in one block.
2 The incremental command (G91) cannot be
specified.
3 When using this function, be sure to set bit 0 (RPD)
of parameter No. 8002 to 0.
4 Before this command can be specified, a reference
position must be established. (With this command,
do not specify an axis on which a reference position
is not established.)
5 Before specifying this command with the T series,
cancel tool offset and tool-nose radius
compensation. Before specifying this command
with the M series, cancel cutter compensation, tool
length compensation, and tool offset.
• Rapid traverse override
With bit 2 (OVE) of parameter No. 8001, whether to use the
rapid traverse override signal for an NC statement or the rapid
traverse override signal dedicated to PMC axis control can be
chosen.
NOTE
Even if bit 4 (RF0) of parameter No. 1401 is set to
1, rapid traverse does not stop with a cutting feed
override of 0%.
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 622 -
17.8 NOTES
- Address without the decimal point
In general, an NC address without the decimal point is subject to
calculator-type decimal point input when bit 0 (DPI) of parameter No.
3401 or bit 0 (AXDx) of parameter No. 3455 is set to 1. In other
cases, an NC address without the decimal point is regarded as a least
input increment.
- Indirect axis address specification
When indirect axis address specification is used, use a direct reference
argument. No indirect reference may be used.
Example)
AX[1] Correct
AX[#RV[0]] Incorrect
- Diameter specification/radius specification
For an axis to be controlled with an RTM statement, select radius
specification. (Set bit 3 (DIA) of parameter No. 1006 to 0.)
- Alarm PS0224
If bit 0 (ZRN) of parameter No. 1005 is set to 0, and an axis control
command is specified in an NC statement before a reference position
return operation is not performed even once after power-up, alarm
PS0224, “ZERO RETURN NOT FINISHED.” is issued. In axis
control using an RTM statement, the alarm is not issued even when bit
0 (ZRN) of parameter No. 1005 is set to 0, unless bit 6 (EZR) of
parameter No. 8006 is set to 1.
- Axis removal
Even when axes are removed, interlock is not applied to the axis being
controlled by an RTM statement.
- Stroke limit check before movement
No stroke limit check before movement is made with a block in an
RTM statement.
- Others
For the axis being controlled by an RTM statement, the functions
disabled for PMC axis control cannot be used.
- Other disabled functions
For the axis being controlled by an RTM statement, the functions
listed below as examples are disabled.
Do not specify these functions for the axis being controlled by an
RTM statement.
- Feed-forward
- Advanced preview feed-forward
- Fine acceleration/deceleration
- Automatic corner deceleration
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 623 -
- One-digit F code feed
- Scaling
- Coordinate system rotation
- Polar coordinate interpolation
- Balance cutting
- Feed stop
- Constant surface speed control
- Positioning function based on optimal acceleration, etc.
CAUTION
In an RTM statement, do not specify an axis used
with any of the following functions:
- Axis synchronous control
Be sure to set the axis synchronous control
selection signal (SYNCn) and axis synchronous
control manual feed selection signal (SYNCJn) of
the axis to 0.
- Synchronous/composite control, superimposed
control
- Index table indexing
- Three-dimensional coordinate system conversion
- Rigid tapping
- Compound machining
- Polygon turning
- Cs contour control
- AI contour control I/II
17.REAL-TIME CUSTOM MACRO PROGRAMMING B-63944EN/03
- 624 -
17.9 LIMITATION
Major general notes on RTM commands are provided below.
- Background drawing
The RTM command has no effect in background drawing. Do not
specify an RTM command during background drawing.
- Interrupt-type custom macro
In an interrupt-type custom macro, no RTM command can be coded.
- Macro executor
In a macro executor, no RTM command can be coded.
Moreover, no macro executor can be coded from an RTM command.
In a series of programs, do not code a macro executor (execution
macro) and RTM command at the same time.
In addition, observe the following:
• Do not code an RTM command in a program that uses an
execution macro.
• Do not call an execution macro from a program with an RTM
command coded.
• Do not code an RTM command in an execution macro.
• Do not use an execution macro as an RTM command trigger.
- Sequence number
No sequence number can be coded in an RTM command. No RTM
command can be searched for a sequence number.
- Optional block skip
Optional block skip is unusable.
A slash (/) that appears in the middle of <expression> (enclosed in [ ]
on the right-hand side of an arithmetic/logical expression) is regarded
as a division operator; it is not regarded as an optional block skip
code.
- Single block
When an RTM command is used, a single block stop generally occurs
according to an NC statement, regardless of the values of bit 5 (SBM)
of parameter No. 6000 and bit 7 (SBV) of parameter No. 6000.
However, no single block stop occurs according to G65 for real time
macro call.
- Processing
If there are many RTM statements between NC statements, the
command flow may break.
- DNC operation
DNC operation is disabled.
B-63944EN/03 PROGRAMMING 17.REAL-TIME CUSTOM MACRO
- 625 -
- Operation in each event
If an event such as an emergency stop or alarm occurs during
execution of an RTM command, the NC command and RTM
command generally operate as indicated below.
Event NC command
RTM command consisting of
a macro command
RTM command including an axis
control command
PS alarm issued in
NC command
execution
Operation stops
when the block
involving the PS
alarm cause starts.
The RTM command stops
when the NC command stops.
If the RTM statement being executed
when the NC command stops is an axis
control command, operation on the axis
stops when the block stops.
Alarm issued in
RTM command
execution
Operation stops with
the alarm.
The RTM statement stops at
that point. Other RTM
commands stop when the NC
command stops.
The RTM statement stops at that point.
Other RTM commands stop operation
on the axis when axis control by the
RTM statement being executed when
the NC statement stops ends.
Single block (SBK
signal)
Operation stops
when the command
being executed
ends.
The RTM command is
suspended when the NC
command stops.
When the NC command
restarts, the RTM command
restarts.
If the RTM statement being executed
when the NC command stops is an axis
control statement, operation on the axis
stops when the block ends.
Feed hold (*SP
signal)
A gradual stop
occurs.
The RTM command stops
when the NC command stops.
When the NC command
restarts, the RTM command
restarts.
If the RTM statement being executed
when the NC command stops is an axis
control statement, operation on the axis
stops when the block ends.
NC command
stopped by a reset
(ERS signal)
A gradual stop
occurs, and the
command also
ends.
The RTM command stops
when the NC command stops.
If the RTM statement being executed
when the NC command stops is an axis
control command, operation on the axis
stops when the block ends.
Emergency stop An immediate stop
occurs, and the
command also
ends.
The command immediately
ends.
Operation on the axis immediately
stops, and the command also
immediately ends.
End of the NC
command
- If the RTM command being
executed is a one-shot RTM
command, the command ends.
If the RTM command being
executed is a modal RTM
command, the command
continues execution.
If the one-shot RTM command being
executed when the NC command ends
is an axis control command, operation
on the axis stops when the block ends.
Machine lock
(MLK signal)
The NC command is
valid.
The RTM command operates. The RTM command can be enabled.
For details, see the description of the
axis control command.
Dry run (DRN
signal)
The NC command is
valid.
The RTM command operates. The RTM command can be enabled.
For details, see the description of the
axis control command.
Interlock (*IT
signal)
The NC command is
valid.
The RTM command operates. The RTM command can be enabled.
For details, see the description of the
axis control command.
PROGRAMMING B-63944EN/03
- 626 -
18. PROGRAMMABLE
PARAMETER INPUT (G10)
18 PROGRAMMABLE PARAMETER INPUT
(G10)
Overview
The values of parameters and pitch error compensation data can be
entered in a program. This function is used for setting pitch error
compensation data when attachments are changed or the maximum
cutting feedrate or cutting time constants are changed to meet
changing machining conditions.
Format
- Prameter entry mode
G10L52 ; Parameter entry mode setting
N_R_ ; For parameters other than the axis type or spindle type
N_P_R_ ; For axis type or spindle type parameters
:
G11 ; Parameter entry mode cancel
N_ : Parameter number
R_ : Parameter setting value (Leading zeros can be omitted.)
P_ : Axis number 1 to maximum controlled axis number (to be
specified when an axis type parameter or spindle type parameter
is specified)
NOTE
G10L52 cannot be used to enter pitch error compensation
data.
- Pitch error compensation data entry mode
G10L50 ; Pitch error compensation data entry mode setting
N_R_ ; Pitch error compensation data entry
N_P_R_ ; For axis type parameters
:
G11 ; Pitch error compensation data entry mode cancel
N_ : Compensation position number for pitch errors compensation
+10,000
R_ : Pitch error compensation data
NOTE
G10L50 cannot be used to enter parameter.
B-63944EN/03 PROGRAMMING
- 627 -
18.PROGRAMMABLE
PARAMETER INPUT (G10)
Explanation
- Setting value (R_)
Do not use a decimal point in the setting (R_) of a parameter or pitch
error compensation data. As the value of R, a custom macro variable
can be used.
When a parameter of real type is used, set an integer value in (R_)
according to the increment system of the parameter.
- Axis number (P_)
As the axis number (P_), specify the order of a controlled axis to be
displayed on the CNC display screen, by using an axis type parameter.
For example, specify P2 for the control axis which is displayed
second.
For a spindle type also, specify the order of an axis to be display on
the CNC display screen.
WARNING
1 Do not fail to perform reference position return
manually after changing the pitch error
compensation data or backlash compensation
data. Without this, the machine position can
deviate from the correct position.
2 The canned cycle mode must be cancelled before
entering of parameters. When not cancelled, the
drilling motion may be activated.
CAUTION
Compatibility with the Series 16i/18i/21i:
This model has parameters that are not compatible
with the Series 16i/18i/21i. So, before using this
function, make a check according to the Parameter
Manual (B-63950EN) of this model.
NOTE
Other NC statements cannot be specified while in
parameter input mode.
PROGRAMMING B-63944EN/03
- 628 -
18. PROGRAMMABLE
PARAMETER INPUT (G10)
Example
1. Set bit 2 (SBP) of bit type parameter No. 3404
G10L52 ; Parameter entry mode
N3404 R 00000100 ; SBP setting
G11 ; Cancel parameter entry mode
2. Change the values for the Z-axis (3rd axis) and A-axis (4th axis)
in axis type parameter No. 1322 (the coordinates of stored stroke
limit 2 in the positive direction for each axis).
(When the increment systems for the 3rd and 4th axes are IS-B
and millimeter machine, respectively)
G10L52 ; Parameter entry mode
N1322P3R4500 ; Change the value for the Z-axis to 4.500
N1322PP4R12000 ; Change the value for the A-axis to
12.000
G11 ; Cancel parameter entry mode
3. Change compensation point numbers 10 and 20 of pitch error
compensation.
G10L50 ; Pitch error compensation data entry
mode
N10010R1 ; Change the compensation point number
from 10 to 1
N10020R5 ; Change the compensation point number
from 20 to 5
G11 ; Pitch error compensation data entry
mode
B-63944EN/03 PROGRAMMING 19.PATTERN DATA INPUT
- 629 -
19 PATTERN DATA INPUT
Chapter 19, "PATTERN DATA INPUT", consists of the following
sections:
19.1 OVERVIEW...........................................................................630
19.2 EXPLANATION ....................................................................631
19.3 EXPLANATION OF OPERATION ......................................634
19.4 DEFINITION OF THE SCREEN ..........................................638
19.PATTERN DATA INPUT PROGRAMMING B-63944EN/03
- 630 -
19.1 OVERVIEW
In the program of the fixed form processing with the custom macro,
the operator select the processing pattern on the menu screen and
specified the size, number and so on to the variable on the custom
macro screen. As above mentioned, this function enables users to
perform programming simply without programming using an existing
NC language.
With the aid of this function, a machine tool builder can prepare the
program of a hole machining cycle (such as a boring cycle or tapping
cycle) using the custom macro function, and can store it into the
program memory.
This cycle is assigned pattern names, such as BOR1, TAP3, and
DRL2.
An operator can select a pattern from the menu of pattern names
displayed on the screen.
Data (pattern data) which is to be specified by the operator should be
created in advance with variables in a drilling cycle.
The operator can identify these variables using names such as DEPTH,
RETURN RELIEF, FEED, MATERIAL or other pattern data names.
The operator assigns values (pattern data) to these names.
The operator selects the pattern on the menu screen, and the selected
pattern number is assigned to the system variable. The custom macro
of the selected pattern can be started by starting a program then
referring to the system variable in the program.
B-63944EN/03 PROGRAMMING 19.PATTERN DATA INPUT
- 631 -
19.2 EXPLANATION
This function is consist of Pattern menu screen and Custom macro
screen.
The process pattern is selected on the pattern menu screen.
Then the process pattern is selected, the custom macro screen is
displayed.
On this custom macro screen, the variable with the name and coment
is displayed according to the selected process pattern.
The process data can be input by referring to the variable name with
the numerical value on the drawing.
The following is the example for the pattern menu and the custom
macro.
(1) Pattern menu screen
Fig. 19.2 (a) Pattern data menu screen (10.4-inch)
19.PATTERN DATA INPUT PROGRAMMING B-63944EN/03
- 632 -
Fig. 19.2 (b) Pattern data menu screen (15-inch)
(2) Custom macro screen
The name of varialbe and comment can be displayed on the usual
custom macro screen.
The menu title and pattern name on the pattern menu screen and
the variable name on the custom macro screen can be defined
The position of the comment displayed on the custom macro
screen can be selected by setting bit 0 (POC) of parameter No.
11318.
On 15-inch display unit, the comment is displayed at only bottom
of the custom macro screen.
Fig. 19.2 (c) Custom macro screen (No. 11318#0=0) (10.4-inch)
B-63944EN/03 PROGRAMMING 19.PATTERN DATA INPUT
- 633 -
Fig. 19.2 (d) Custom macro screen (parameter No. 11318#0=1) (10.4-inch)
Fig. 19.2 (e) Custom macro screen (15-inch)
19.PATTERN DATA INPUT PROGRAMMING B-63944EN/03
- 634 -
19.3 EXPLANATION OF OPERATION
The following explains how to display the pattern menu screen.
For 7.2-, 8.4-, and 10.4-inch LCDs
1 Press function key .
2 Press continous menu key .
3 Press soft key [PATTERN MENU].
For a 15-inch LCD
1 Press function key .
2 Press vertical soft key [NEXT PAGE] several times.
3 Press vertical soft key [PATTERN MENU].
Pattern menu screen
The following pattern menu is displayed.
Fig. 19.3 (f) Pattern menu screen (10.4-inch)
B-63944EN/03 PROGRAMMING 19.PATTERN DATA INPUT
- 635 -
Fig. 19.3 (g) Pattern menu screen (15-inch)
Select the pattern on this screen
The following two methods are effective.
• Selection by cursor
Move the cursor to the pattern name with the cursor move keys
, and press the softkey [SELECT] or .
• Selection by setting of pattern number
The number that is displayed in the left side of the pattern name
is input and press the softkey [select] or .
The selected pattern number is registered to system variable #5900.
The custom macro of the selected pattern can be started by starting a
fixed program (external program No. search) with an external signal.
This program refers to the system variable #5900 in the program. This
system variable #5900 is kept after power-off.
19.PATTERN DATA INPUT PROGRAMMING B-63944EN/03
- 636 -
Custom macro variable screen
The following custom macro screen is displayed.
Fig. 19.3 (h) Custom macro screen when the pattern data is input
(10.4-inch)
Fig. 19.3 (i) Custom macro screen when the pattern data is input
(15-inch)
When the screen is changed to the custom macro screen, the macro
variable number that is selected first is specifiied with the parameters
Nos.6101 to 6110. The macro variables that variable name is not
defined can be input, too.
B-63944EN/03 PROGRAMMING 19.PATTERN DATA INPUT
- 637 -
NOTE
1 The variable name that is displayed cannot be used
as the common variable name of the NC program.
2 When the common varialbe name is defined by
SETVN command, the varialbe name defined by
pattern data input function is given priority.
3 When bit 0 (POC) of parameter No.11318 is set to
“1”, The variable number is three digit display.
And the value of 12 digits or more is input, 11 digits
from head of value are displayed.
Example)
Input: -123456789.123 → Display: -123456789.1
19.PATTERN DATA INPUT PROGRAMMING B-63944EN/03
- 638 -
19.4 DEFINITION OF THE SCREEN
The definition of the screen is performed by NC program.
Program configuration
This function is consist of one program for the definition of pattern
menu screen and maximum ten programs for the definition of custom
macro screen.
Register the macro program for the pattern data input function to the
following folder.
//CNC_MEM/USER/LIBRARY/PATH1 to PATH[n]
* [n] is the maximum path number of the system
* The PATH1 to PATH[n] should be made by the machine tool
builder.
The program number is as follows
Table 19.4 (a) Numbers of subprograms employed in the pattern data
input function
Sub program No. Screen
O9500 Specifies character strings displayed on the pattern
data menu.
O9501 Specifies a character string of the pattern data
corresponding to pattern No.1
O9502 Specifies a character string of the pattern data
corresponding to pattern No.2
O9503 Specifies a character string of the pattern data
corresponding to pattern No.3
O9504 Specifies a character string of the pattern data
corresponding to pattern No.4
O9505 Specifies a character string of the pattern data
corresponding to pattern No.5
O9506 Specifies a character string of the pattern data
corresponding to pattern No.6
O9507 Specifies a character string of the pattern data
corresponding to pattern No.7
O9508 Specifies a character string of the pattern data
corresponding to pattern No.8
O9509 Specifies a character string of the pattern data
corresponding to pattern No.9
O9510 Specifies a character string of the pattern data
corresponding to pattern No.10
Table 19.4 (b) Macro commands used in the pattern data input function
G code H code Function
G65 H90 Specifies the menu title.
G65 H91 Specifies the pattern name.
G65 H92 Specifies the pattern data title.
G65 H93 Specifies the variable name.
G65 H94 Specifies the comment.
Table 19.4 (c) System variables employed in the pattern data input
function
System variable Function
#5900 Pattern No. selected by user.
B-63944EN/03 PROGRAMMING 19.PATTERN DATA INPUT
- 639 -
19.4.1 Definition of the Pattern Menu Screen
Menu title and pattern name are defined as follows.
Fig. 19.4.1 (a) Pattern menu screen
Definition of menu title
The character string displayed in the menu title of the pattern menu
screen is defined.
The menu title is specified up to 12 characters in a half size letter and
up to 6 characters in a full size letter such as kanji character.
- Format
G65 H90 P_ Q_ R_ I_ J_ K_ ;
H90 : Specifies the menu title
P_ : The code of 1st and 2nd characters of title
Q_ : The code of 3rd and 4th characters of title
R_ : The code of 5th and 6th characters of title
I_ : The code of 7th and 8th characters of title
J_ : The code of 9th and 10th characters of title
K_ : The code of 11th and 12th characters of title
As for the way of setting the character-code, refer to the
Subsection 19.4.3, "Setting the Character-codes".
Menu title
Pattern name
19.PATTERN DATA INPUT PROGRAMMING B-63944EN/03
- 640 -
Definition of pattern name
The character string displayed in the pattern name which becomes a
menu item is defined.
The pattern name is specified up to 10 characters in a half size letter
and up to 5 characters in a full size letter.
- Format
G65 H91 P_ Q_ R_ I_ J_ K_ ;
H91 : Specifies the pattern name
P_ : Specifies the menu number of the pattern name
The menu number = 1 to 10
Q_ : The code of 1st and 2nd characters of pattern name
R_ : The code of 3rd and 4th characters of pattern name
I_ : The code of 5th and 6th characters of pattern name
J_ : The code of 7th and 8th characters of pattern name
K_ : The code of 9thd and 10th characters of pattern nam
e
As for the way of setting the character-code, refer to the
Subsection 19.4.3, "Setting the Character-codes".
Example
The following is example for pattern menu screen.
Fig. 19.4.1 (b) Pattern menu screen
O9500
N1 G65 H90 P072079 Q076069 R032080 I065084 J084069 K082078; .. "HOLE PATTERN"
N2 G65 H91 P1 Q066079 R076084 I032072 J079076 K069032; ............ "BOLT HOLE"
N3 G65 H91 P2 Q071082 R073068; ........................................................ "GRID"
N4 G65 H91 P3 Q076073 R078069 I032065 J078071 K076069; ............ "LINE ANGLE"
N5 G65 H91 P4 Q084065 R080080 I073078 J071032; .......................... "TAPPING"
N6 G65 H91 P5 Q068082 R073076 I076073 J078071;............................ "DORILLING"
N7 G65 H91 P6 Q066079 R082073 I078071; .......................................... "BORING"
N8 G65 H91 P7 Q080079 R067075 I069084; .......................................... "POCKET"
N9 G65 H91 P8 Q080069 R067075; ........................................................ "PECK"
N10 G65 H91 P9 Q084069 R083084; ...................................................... "TEST"
N11 G65 H91 P10 Q066065 R067075; .................................................... "BACK"
N12 M99;
B-63944EN/03 PROGRAMMING 19.PATTERN DATA INPUT
- 641 -
19.4.2 Definition of the Custom Macro Screen
The title, variable name and comment are defined as follows.
Fig. 19.4.2 (a) Custom macro screen
Definition of title
The character string displayed in the title of the custom macro screen
is defined.
The title is specified up to 12 characters in a half size letter and up to 6
characters in a full size letter.
- Format
G65 H92 P_ Q_ R_ I_ J_ K_ ;
H92 : Specifies the menu title
P_ : The code of 1st and 2nd characters of the menu title
Q_ : The code of 3rd and 4th characters of the menu title
R_ : The code of 5th and 6th characters of the menu title
I_ : The code of 7th and 8th characters of the menu title
J_ : The code of 9th and 10th characters of the menu title
K_ : The code of 11th and 12th characters of the menu title
As for the way of setting the character-code, refer to the
Subsection 19.4.3, "Setting the Character-codes".
Macro variable name Title
Comment
19.PATTERN DATA INPUT PROGRAMMING B-63944EN/03
- 642 -
Definition of macro variable
The character string displayed in the macro variable name is defined.
The macro variable is specified up to 10 characters in a half size letter
and up to 5 characters in a full size letter.
The variable which can be used is as follows
#100 to 199 (100 variables)
#500 to 999 (500 variables), 600 variables in total
- Format
G65 H93 P_ Q_ R_ I_ J_ K_ ;
H93 : Specifies the variable name
P_ : Specifies the variable number
Specifies 100 to 199 or 500 to 999
Q_ : The code of 1st and 2nd characters of the variable name
R_ : The code of 3rd and 4th characters of the variable name
I_ : The code of 5th and 6th characters of the variable name
J_ : The code of 7th and 8th characters of the variable name
K_ : The code of 9th and 10th characters of the variable name
As for the way of setting the character-code, refer to the
Subsection 19.4.3, "Setting the Character-codes".
B-63944EN/03 PROGRAMMING 19.PATTERN DATA INPUT
- 643 -
Definition of a comment
The character string of the comment displayed on the custom macro
screen is defined.
The comment is specified by up to 12 characters in a half size letter
and up to 6 characters in a full size letter per one block.
• When the comment is displayed at the bottom(bit 0 (POC) of
parameter No.11318=0)
The number of blocks is defined up to maximum 9 blocks.
One line is composition of 3 blocks and maximum 3 lines can be
displayed.
The comment is displayed in the order specified by program as
the following figure.
The block is arranged in defined order.
Block 1 Block 2 Block 3
Block 4 Block 5 Block 6
Block 7 Block 8 Block 9
Fig.19.4.2 (b) Block reyout of comment
• When the comment is displayed at the right(bit 0 (POC) of
parameter No.11318=1)
1 line is composed by 1 blocks, the maximum number of lines is
8 on the 7.2-inch and 8.4-inch display unit or 12 on the 10.4-inch
display unit.
- Format
G65 H94 P_ Q_ R_ I_ J_ K_ ;
H94 : Specifies the comment
P_ : The code of 1st and 2nd characters of comment
Q_ : The code of 3rd and 4th characters of comment
R_ : The code of 5th and 6th characters of comment
I_ : The code of 7th and 8th characters of comment
J_ : The code of 9th and 10th characters of comment
K_ : The code of 11th and 12th characters of comment
As for the way of setting the character-code, refer to the
Subsection 19.4.3, "Setting the Character-codes".
19.PATTERN DATA INPUT PROGRAMMING B-63944EN/03
- 644 -
Example
The following is example of the custom macro screen.
Fig. 19.4.2 (c) Custom macro screen (No. 11318#0=0)
Fig. 19.4.2 (d) Custom macro screen (No. 11318#0=1)
O9501;
N1 G65 H92 P066079 Q076084 R032072 I079076 J069032; ...................."BOLT HOLE"
N2 G65 H93 P500 Q084079 R079076; ......................................................"TOOL"
N3 G65 H93 P501 Q079082 R071032 I08832;..........................................."ORG X"
N4 G65 H93 P502 Q079082 R071032 I08932;..........................................."ORG Y"
N5 G65 H93 P503 Q082065 R068073 I085803;........................................."RADIUS"
N6 G65 H93 P504 Q083046 R032065 I078071 J076032 ..........................."S. ANGL"
N7 G65 H93 P505 Q072079 R076079 I083032 J078079 K046032............"HOLES NO."
N8 G65 H94 P032042 Q066079 R076084 I032072 J079076 K069032;....." *BOLT HOLE"
N9 G65 H94 P067073 Q082067 R076069 I042032;..................................."CIRCLE*"
N10 G65 H94 P083069 Q084032 R080065 I084084 J069082 K078032;..."SET PATTERN"
N11 G65 H94 P068065 Q084065 R032084 I079032 J086065 K082046;..."DATA NO VAR."
N12 G65 H94 P078079 Q046053 R048048 I045053 J048053 K046032;..."NO500-505"
N13 M99;
B-63944EN/03 PROGRAMMING 19.PATTERN DATA INPUT
- 645 -
19.4.3 Setting the Character-codes
The character cannot be used to specify the NC program.
Therefor, the code corresponding to the character is specified.
One character is consist of three figures in a half size letter and six
figures in a full size letter.
The character code is specified for each address of the G65 instruction
by six digits.
Refer to the table for the character code.
Example）
When "ABCDEFGH" is specified, the description of the code is
as follows.
Encoded character string : 065 066 067 068 069 070 071 072
P065066 Q067068 R069070 I071072;
AB CD EF GH
NOTE
1 Space (032) is added ahead of the character-code,
when the character-code of three digits or less is
specified.
Example)
P065066 Q067; → " AB C "
032(space) is put at the end, when "ABC" is
displayed.
P065066 Q067032; → " ABC "
2 It is assumed in that the space of two characters was
defined in the address when there is an address not
defined.
Example)
P065066 I067068; → "AB CD"
19.PATTERN DATA INPUT PROGRAMMING B-63944EN/03
- 646 -
Characters and codes to be used for the patterndata input function
Character Code Comment Character Code Comment
A 065 6 054
B 066 7 055
C 067 8 056
D 068 9 057
E 069 032 Space
F 070 ! 033 Exclamation mark
G 071 ” 034 Quotation mark
H 072 # 035 Hash sign
I 073 $ 036 Dollar sign
J 074 % 037 Percent
K 075 & 038 Ampersand
L 076 ’ 039 Apostrophe
M 077 * 042 Asterisk
N 078 + 043 Plus sign
O 079 , 044 Comma
P 080 - 045 Minus sign
Q 081 . 046 Period
R 082 / 047 Slash
S 083 : 058 Colon
T 084 ; 059 Semicolon
U 085 < 060 Left angle bracket
V 086 = 061 Equal sign
W 087 > 062 Right angle bracket
X 088 ? 063 Question mark
Y 089 @ 064 HAt”mark
Z 090 [ 091 Left square bracket
0 048 ¥ 092 Yen sign
1 049 ] 093 Right squar bracket
2 050 ^ 094
3 051 _ 095 Underscore
4 052
5 053
B-63944EN/03 PROGRAMMING 19.PATTERN DATA INPUT
- 647 -
The characters and the codes of the katakana is as follows.
Character Code Comment Character Code Comment
ア 177 ム 209
イ 178 メ 210
ウ 179 モ 211
エ 180 ヤ 212
オ 181 ユ 213
カ 182 ヨ 214
キ 183 ラ 215
ク 184 リ 216
ケ 185 ル 217
コ 186 レ 218
サ 187 ロ 219
シ 188 ワ 220
ス 189 ヲ 166
セ 190 ン 221
ソ 191 ァ 167
タ 192 ィ 168
チ 193 ゥ 169
ツ 194 ェ 170
テ 195 ォ 171
ト 196 ャ 172
ナ 197 ュ 173
ニ 198 ョ 174
ヌ 199 ッ 175
ネ 200 ″ 222 Diacritical mark
ノ 201 ° 223 Diacritical mark
ハ 202 。 161 Punctuation
ヒ 203 「 162 Left quotation mark
フ 204 」 163 Right quotation mark
ヘ 205 、 164 Comma
ホ 206 ・ 165 Point
マ 207 000 Space
ミ 208
NOTE
Diacritical mark is one character.
19.PATTERN DATA INPUT PROGRAMMING B-63944EN/03
- 648 -
The characters and the codes of the hiragana and the kanji are as
follows. The following hiraganas and kanjis use two characters of the
alphanumeric character.
ぁ あ ぃ い う う ぇ え ぉ お
002 000 002 002 002 004 002 006 002 008 002 010 002 012 002 014 002 016 002 018
か が き ぎ く ぐ け げ こ ご
002 020 002 022 002 024 002 026 002 028 002 030 002 032 002 034 002 036 002 038
さ ざ し じ す ず せ ぜ そ ぞ
002 040 002 042 002 044 002 046 002 048 002 050 002 052 002 054 002 056 002 058
た だ ち ぢ っ つ づ て で と
002 060 002 062 002 064 002 066 002 068 002 070 002 072 002 074 002 076 002 078
ど な に ぬ ね の は ば ぱ ひ
002 080 002 082 002 084 002 086 002 088 002 090 002 092 002 094 002 096 002 098
び ぴ ふ ぶ ぷ へ べ ぺ ほ ぼ
002 100 002 102 002 104 002 106 002 108 002 110 002 112 002 114 002 116 002 118
ぽ ま み む め も ゃ や ゅ ゆ
002 120 002 122 002 124 002 126 002 128 002 130 002 132 002 134 002 136 002 138
ょ よ ら り る れ ろ わ わ 素
002 140 002 142 002 144 002 146 002 148 002 150 002 152 002 154 002 156 002 158
材 を ん 種 類 棒 穴 成 形 質
002 160 002 162 002 164 002 166 002 168 002 170 002 172 002 174 002 176 002 178
寸 法 外 径 長 端 面 最 小 内
002 180 002 182 002 184 002 186 002 188 002 190 002 192 002 194 002 196 002 198
大 加 工 切 削 倣 正 途 中 荒
002 200 002 202 002 204 002 206 002 208 002 210 002 212 002 214 002 216 002 218
具 番 号 仕 上 込 点 方 向 速
002 220 002 222 002 224 002 226 002 228 002 230 002 232 002 234 002 236 002 238
度 送 量 開 始 深 主 軸
002 240 002 242 002 244 002 246 002 248 002 250 002 252 002 254
回 転 数 位 置 決 直 線 時 円
003 000 003 002 003 004 003 006 003 008 003 010 003 012 003 014 003 016 003 018
反 現 在 指 令 値 領 域 診 断
003 020 003 022 003 024 003 026 003 028 003 030 003 032 003 034 003 036 003 038
操 作 手 引 機 械 残 移 動 次
003 040 003 042 003 044 003 046 003 048 003 050 003 052 003 054 003 056 003 058
早 電 源 投 入 間 分 秒 自 運
003 060 003 062 003 064 003 066 003 068 003 070 003 072 003 074 003 076 003 078
負 荷 実 使 用 寿 命 新 規 除
003 080 003 082 003 084 003 086 003 088 003 090 003 092 003 094 003 096 003 098
隅 取 単 補 能 独 終 了 記 角
003 100 003 102 003 104 003 106 003 108 003 110 003 112 003 114 003 116 003 118
溝 刃 幅 広 設 定 一 覧 表 部
003 120 003 122 003 124 003 126 003 128 003 130 003 132 003 134 003 136 003 138
炭 合 金 鋼 超 硬 先 付 摩 耗
003 140 003 142 003 144 003 146 003 148 003 150 003 152 003 154 003 156 003 158
仮 想 副 行 挿 消 去 山 高 準
003 160 003 162 003 164 003 166 003 168 003 170 003 172 003 174 003 176 003 178
備 完 後 弧 助 択 無 視 器 原
003 180 003 182 003 184 003 186 003 188 003 190 003 192 003 194 003 196 003 198
B-63944EN/03 PROGRAMMING 19.PATTERN DATA INPUT
- 649 -
登 録 再 処 理 描 画 過 容 編
003 200 003 202 003 204 003 206 003 208 003 210 003 212 003 214 003 216 003 218
集 未 対 相 座 標 示 名 歯 変
003 220 003 222 003 224 003 226 003 228 003 230 003 232 003 234 003 236 003 238
呼 推 馬 力 系 選 達 閉
003 240 003 242 003 244 003 246 003 248 003 250 003 252 003 254
禁 復 帰 書 個 桁 稼 由 両 半
004 000 004 002 004 004 004 006 004 008 004 010 004 012 004 014 004 016 004 018
逃 底 逆 下 空 四 触 平 代 辺
004 020 004 022 004 024 004 026 004 028 004 030 004 032 004 034 004 036 004 038
格 子 周 心 本 群 停 止 巾 微
004 040 004 042 004 044 004 046 004 048 004 050 004 052 004 054 004 056 004 058
状 路 範 囲 倍 率 注 側 特 殊
004 060 004 062 004 064 004 066 004 068 004 070 004 072 004 074 004 076 004 078
距 離 連 続 増 隔 件 初 期 条
004 080 004 082 004 084 004 086 004 088 004 090 004 092 004 094 004 096 004 098
経 握 圧 扱 陰 隠 右 押 横 黄
004 100 004 102 004 104 004 106 004 108 004 110 004 112 004 114 004 116 004 118
億 屋 化 何 絵 階 概 該 巻 換
004 120 004 122 004 124 004 126 004 128 004 130 004 132 004 134 004 136 004 138
気 起 軌 技 疑 供 共 境 強 教
004 140 004 142 004 144 004 146 004 148 004 150 004 152 004 154 004 156 004 158
掘 繰 係 傾 型 検 権 研 肩 見
004 160 004 162 004 164 004 166 004 168 004 170 004 172 004 174 004 176 004 178
験 元 弦 減 孔 巧 控 更 校 構
004 180 004 182 004 184 004 186 004 188 004 190 004 192 004 194 004 196 004 198
根 左 差 雑 参 散 産 算 治 耳
004 200 004 202 004 204 004 206 004 208 004 210 004 212 004 214 004 216 004 218
式 失 修 十 従 勝 商 少 尚 昇
004 220 004 222 004 224 004 226 004 228 004 230 004 232 004 234 004 236 004 238
植 色 食 伸 信 侵 振 浸
004 240 004 242 004 244 004 246 004 248 004 250 004 252 004 254
真 暗 以 意 異 影 鋭 越 価 可
005 000 005 002 005 004 005 006 005 008 005 010 005 012 005 014 005 016 005 018
科 果 箇 課 各 拡 核 学 掛 漢
005 020 005 022 005 024 005 026 005 028 005 030 005 032 005 034 005 036 005 038
簡 観 関 含 却 客 休 急 業 曲
005 040 005 042 005 044 005 046 005 048 005 050 005 052 005 054 005 056 005 058
均 筋 継 計 軽 言 限 互 降 採
005 060 005 062 005 064 005 066 005 068 005 070 005 072 005 074 005 076 005 078
済 細 姿 思 写 射 斜 者 車 借
005 080 005 082 005 084 005 086 005 088 005 090 005 092 005 094 005 096 005 098
縦 重 出 述 術 渉 照 省 章 証
005 100 005 102 005 104 005 106 005 108 005 110 005 112 005 114 005 116 005 118
象 身 進 人 図 違 印 沿 遠 央
005 120 005 122 005 124 005 126 005 128 005 130 005 132 005 134 005 136 005 138
奥 往 応 会 解 改 割 活 願 基
005 140 005 142 005 144 005 146 005 148 005 150 005 152 005 154 005 156 005 158
奇 寄 岐 既 近 区 矩 駆 偶 旧
005 160 005 162 005 164 005 166 005 168 005 170 005 172 005 174 005 176 005 178
19.PATTERN DATA INPUT PROGRAMMING B-63944EN/03
- 650 -
求 球 究 級 欠 結 口 語 誤 交
005 180 005 182 005 184 005 186 005 188 005 190 005 192 005 194 005 196 005 198
厚 項 刻 告 黒 財 策 糸 試 資
005 200 005 202 005 204 005 206 005 208 005 210 005 212 005 214 005 216 005 218
事 持 似 釈 弱 受 収 純 順 所
005 220 005 222 005 224 005 226 005 228 005 230 005 232 005 234 005 236 005 238
序 剰 場 常 飾 水 錐 据
005 240 005 242 005 244 005 246 005 248 005 250 005 252 005 254
制 整 製 前 全 然 則 属 即 他
006 000 006 002 006 004 006 006 006 008 006 010 006 012 006 014 006 016 006 018
多 存 谷 探 短 徴 鎮 調 頂 鉄
006 020 006 022 006 024 006 026 006 028 006 030 006 032 006 034 006 036 006 038
添 頭 同 導 道 熱 年 濃 箱 発
006 040 006 042 006 044 006 046 006 048 006 050 006 052 006 054 006 056 006 058
抜 伴 必 百 複 物 文 聞 併 忘
006 060 006 062 006 064 006 066 006 068 006 070 006 072 006 074 006 076 006 078
末 密 有 余 与 裏 立 略 青 席
006 080 006 082 006 084 006 086 006 088 006 090 006 092 006 094 006 096 006 098
石 積 赤 接 折 粗 創 双 捜 太
006 100 006 102 006 104 006 106 006 108 006 110 006 112 006 114 006 116 006 118
打 体 待 態 替 段 知 地 致 遅
006 120 006 122 006 124 006 126 006 128 006 130 006 132 006 134 006 136 006 138
追 通 伝 得 読 凸 凹 突 鈍 敗
006 140 006 142 006 144 006 146 006 148 006 150 006 152 006 154 006 156 006 158
杯 背 配 品 不 布 並 頁 別 片
006 160 006 162 006 164 006 166 006 168 006 170 006 172 006 174 006 176 006 178
返 勉 弁 保 明 滅 木 目 歪 揺
006 180 006 182 006 184 006 186 006 188 006 190 006 192 006 194 006 196 006 198
様 溶 要 抑 良 輪 和 話 枠 節
006 200 006 202 006 204 006 206 006 208 006 210 006 212 006 214 006 216 006 218
説 絶 千 専 浅 旋 総 走 退 台
006 220 006 222 006 224 006 226 006 228 006 230 006 232 006 234 006 236 006 238
第 題 卓 室 着 柱 鋳 丁
006 240 006 242 006 244 006 246 006 248 006 250 006 252 006 254
低 訂 肉 日 白 薄 比 皮 被 非
007 000 007 002 007 004 007 006 007 008 007 010 007 012 007 014 007 016 007 018
美 普 伏 歩 包 門 問 絡 列 万
007 020 007 022 007 024 007 026 007 028 007 030 007 032 007 034 007 036 007 038
利 訳 礼 乱 放 枚 約 練 油 劣
007 040 007 042 007 044 007 046 007 048 007 050 007 052 007 054 007 056 007 058
例 郭 戻 冷 垂 緑 紫 許 測 精
007 060 007 062 007 064 007 066 007 068 007 070 007 072 007 074 007 076 007 078
効 → ↑ ← ↓
007 080 007 082 007 084 007 086 007 088 007 090 007 092 007 094 007 096 007 098
板 予 〃 家 装 管
007 100 007 102 007 104 007 106 007 108 007 110 007 112 007 114 007 116 007 118
粉 等
貫 安 α β
007 120 007 122 007 124 007 126 007 128 007 130 007 132 007 134 007 136 007 138
程 抗 張 任 破 損 御 足 守 般
007 140 007 142 007 144 007 146 007 148 007 150 007 152 007 154 007 156 007 158
B-63944EN/03 PROGRAMMING 19.PATTERN DATA INPUT
- 651 -
納 義 丸 汎 固 毎 当 的 詳 鳥
007 160 007 162 007 164 007 166 007 168 007 170 007 172 007 174 007 176 007 178
適 論 額 縁 温 給 界 混 監 締
007 180 007 182 007 184 007 186 007 188 007 190 007 192 007 194 007 196 007 198
護 己 称 樹 脂 料 落 確 認 報
007 200 007 202 007 204 007 206 007 208 007 210 007 212 007 214 007 216 007 218
排 性 生 績 判 搬 砥 θ 島 壁
007 220 007 222 007 224 007 226 007 228 007 230 007 232 007 234 007 236 007 238
] [ ■
007 240 007 242 007 244 007 246 007 248 007 250 007 252 007 254
PROGRAMMING B-63944EN/03
- 652 -
20. HIGH-SPEED CUTTING
FUNCTIONS
20 HIGH-SPEED CUTTING FUNCTIONS
Chapter 20, "HIGH-SPEED CUTTING FUNCTIONS", consists of the
following sections:
20.1 AI CONTOUR CONTROL FUNCTION I AND AI
CONTOUR CONTROL FUNCTION II (G05.1)...................653
20.2 MACHINING CONDITION SELECTING FUNCTION ......670
20.3 JERK CONTROL...................................................................671
20.4 OPTIMUM TORQUE ACCELERATION/
DECELERATION..................................................................676
20.5 HIGH-SPEED CYCLE MACHINING ..................................689
B-63944EN/03 PROGRAMMING
- 653 -
20.HIGH-SPEED CUTTING
FUNCTIONS
20.1 AI CONTOUR CONTROL FUNCTION I AND AI CONTOUR
CONTROL FUNCTION II (G05.1)
Overview
The AI contour control I and AI contour control II functions are
provided for high-speed, high-precision machining. This function
enables suppression of acceleration/deceleration delays and servo
delays that become larger with increases in the feedrate and reduction
of machining profile errors.
There are two types of AI contour control; these two types are referred
to temporarily as AI contour control I and AI contour control II. AI
contour control I is designed mainly for part machining, and AI
contour control II is for machining of successive minute straight lines
such as mold machining and for machining by curve commands in
NURBS and so on.
When a high-speed processing option is used with AI contour control
II, high-speed operation processing is enabled, which reduces the
interpolation cycle, therefore, faster and more precise machining is
enabled. In addition, an option to expand read-ahead blocks to up to
1000 blocks is available.
In the descriptions below that are common to AI contour control I and
AI contour control II, the term "AI contour control" is used.
Format
G05.1 Q_ ;
Q1 : AI contour control mode on
Q0 : AI contour control mode off
NOTE
1 Always specify G05.1 in an independent block.
2 The AI contour control mode is also canceled by a
reset.
3 The AI contour control mode can be turned on at
the start of automatic operation by setting bit 0
(SHP) of parameter No. 1604.
The AI contour control mode can be controlled also with the formats
that have been used for the conventional advanced preview control,
high-precision contour control, and AI high-precision contour control
functions.
G08 P_ ;
P1 : AI contour control mode on
P0 : AI contour control mode off
G05 P_ ;
P10000 : AI contour control mode on
P0 : AI contour control mode off
PROGRAMMING B-63944EN/03
- 654 -
20. HIGH-SPEED CUTTING
FUNCTIONS
NOTE
1 Always specify G08 and G05 in an independent
block.
2 G05 can be specified only for AI contour control II.
3 The AI contour control mode is also canceled by a
reset.
4 Valid functions are limited depending on the
command format. For details, see the description
of "Valid functions".
Valid functions
The functions listed below are valid in the AI contour control mode.
Valid functions are limited depending on the command format and
whether AI contour control I or II is used.
Function AI contour control I AI contour control II AI contour control II with
high-speed processing
Number of blocks read
ahead
30
(When G8 is specified: 1)
200
(When G8 is specified: 1)
600 (*1)
(When G8 is specified: 1)
Look-ahead
acceleration/deceleration
before interpolation
Linear or bell-shaped
acceleration/deceleration
Linear or bell-shaped
acceleration/deceleration
Linear or bell-shaped
acceleration/deceleration
Speed control with feedrate
difference on each axis Enabled Enabled Enabled
Speed control with
acceleration in circular
interpolation
Enabled Enabled Enabled
Speed control with
acceleration on each axis
Enabled
(When G8 is specified:
Not enabled)
Enabled
(When G8 is specified:
Not enabled)
Enabled
(When G8 is specified:
Not enabled)
Smooth speed control Not enabled
Enabled
(When G8 is specified:
Not enabled)
Enabled
(When G8 is specified:
Not enabled)
Speed control with cutting
load Not enabled Enabled Enabled
Disregard of feedrate
command Not enabled Enabled Enabled
*1 The number of blocks can optionally be expanded to 1000
blocks.
Explanation
- Look-ahead acceleration/deceleration before interpolation
There are two types of look-ahead acceleration/deceleration before
interpolation, the linear acceleration/deceleration type and the
bell-shaped acceleration/deceleration type.
Look-ahead bell-shaped acceleration/deceleration before interpolation
produces smoother acceleration/deceleration.
B-63944EN/03 PROGRAMMING
- 655 -
20.HIGH-SPEED CUTTING
FUNCTIONS
- Setting an acceleration
A permissible acceleration for the linear acceleration/deceleration of
each axis is set in parameter No.1660. For bell-shaped
acceleration/deceleration, acceleration change time (B) (period of
transition from constant speed state (A) to constant acceleration/
deceleration state (C)) is set in parameter No.1772. In the constant
acceleration/deceleration state (C), acceleration/deceleration is
performed with the maximum tangential acceleration not exceeding
the permissible acceleration of each axis specified in parameter
No.1660.
The acceleration change time specified in parameter No.1772 is held
constant, regardless of the tangential acceleration.
Tangential feedrate
A
n optimum gradient is
automatically calculated from the
setting made in parameter
No.1660.
Time set in parameter No.1772
(A) (B) (B) (B) (B) (A) (A) (C) (C)
PROGRAMMING B-63944EN/03
- 656 -
20. HIGH-SPEED CUTTING
FUNCTIONS
- Method of determining the tangent acceleration
Acceleration/deceleration is performed with the largest tangent
acceleration/deceleration that does not exceed the acceleration set for
each axis.
(Example)
X-axis permissible acceleration: 1000 mm/sec2
Y-axis permissible acceleration: 1200 mm/sec2
Acceleration change time: 20 msec
Program:
N1 G01 G91 X20. F6000 ..Move on the X-axis.
G04 X0.01
N2 Y20............................Move on the Y-axis.
G04 X0.01
N3 X20. Y20. ...................Move in the XY direction (at 45 degrees).
The acceleration in N3 is 1414 mm/sec2. At this point, the
acceleration on the X-axis is equal to the set value (1000 mm/sec2).
20ms
20ms20ms 20ms
1000mm/sec2
gradient
Tangent feedrate
1200mm/sec2
gradient
1414mm/sec2
gradient
- Acceleration
Acceleration is performed so that the feedrate programmed for a block
is attained at the beginning of the block.
Acceleration can be performed over several blocks.
Speed control by look-ahead
acceleration/deceleration before
Programmed speed
N2N1
Feedrate
Time
N4N3 N5
B-63944EN/03 PROGRAMMING
- 657 -
20.HIGH-SPEED CUTTING
FUNCTIONS
- Deceleration
Deceleration starts in advance so that the feedrate programmed for a
block is attained at the beginning of the block.
Deceleration can be performed over several blocks.
Feedrate
Time
Deceleration
start point
Deceleration
start point
Speed control by look-ahead
acceleration/deceleration before
interpolation
Programmed speed
- Deceleration based on a distance
If the total distance of the blocks read ahead becomes shorter than or
equal to the deceleration distance obtained from the current feedrate,
deceleration starts.
If the total distance of the blocks read ahead during deceleration
increases, acceleration is performed.
If the blocks of a small amount of travel are successively specified,
deceleration and acceleration may be performed alternately, making
the feedrate inconsistent.
To avoid this, decrease the programmed feedrate.
- Function for changing time constant of bell-shaped acceleration/deceleration
Bell-shaped acceleration/deceleration before interpolation is
performed using the parameter-set acceleration and acceleration
change time. If a low feedrate is specified, a linear acceleration/
deceleration may not achieve the specified acceleration as shown:
Linear acceleration/deceleration not achieving
specified acceleration/deceleration
Specified
feedrate
T1
Feedrate
T1
T2
Time
T1 : Time obtained from specified feedrate and specified acceleration (specified
feedrate/acceleration (parameter No. 1660))
T2 : Acceleration change time (parameter No. 1772)
PROGRAMMING B-63944EN/03
- 658 -
20. HIGH-SPEED CUTTING
FUNCTIONS
In such a case, set bit 3 (BCG) of parameter No. 7055 to 1. Then, the
internal acceleration and vector time constant of
acceleration/deceleration before interpolation are changed to make the
acceleration/deceleration pattern as close as possible to the optimum
bell-shaped acceleration/deceleration before interpolation based on a
specified acceleration/deceleration reference speed, and so
acceleration/deceleration time is reduced.
A
cceleration/deceleration curve
Specified
feedrate
Feedrate
T1'
T2' T2'
There are three methods for specifying the acceleration/deceleration
reference speed.
(1) Specifying the speed using an F in a G05.1 Q1 block
(2) Setting the speed on parameter No.7066
(3) Setting the speed specified with the F command issued at the
start of cutting as the reference speed
When F is specified in a G05.1Q1 block, the specified feedrate is
assumed to be the acceleration/deceleration reference speed. This
command can be used only in the feed per minute mode.
If no F command is specified in a G05.1Q1 block, the feedrate
specified in parameter No. 7066 is assumed to be the
acceleration/deceleration reference speed. If 0 is set in parameter No.
7066, the F command specified in the cutting start block is assumed to
be the acceleration/deceleration reference speed.
B-63944EN/03 PROGRAMMING
- 659 -
20.HIGH-SPEED CUTTING
FUNCTIONS
- Automatic feedrate control function
In AI contour control mode, the feedrate is automatically controlled
by the reading-ahead of blocks.
The feedrate is determined using the following conditions. If the
specified feedrate exceeds the determined feedrate, acceleration/
deceleration before interpolation is performed to achieve the
determined feedrate.
<1> Feedrate changes on each axis at a corner and the permissible
feedrate change that has been set
<2> Expected acceleration on each axis and the permissible
acceleration that has been set
<3> Cutting load that is expected from the travel direction on the
Z-axis
Specified tool path
Tool path assumed when
A
l contour control is not
used
Tool path assumed when Al
contour control is used
The machining error is decreased
because of the deceleration with
the acceleration.
The machining error is decreased
because of the deceleration by
difference in feedrate.
For details, see the explanation of each function.
PROGRAMMING B-63944EN/03
- 660 -
20. HIGH-SPEED CUTTING
FUNCTIONS
- Speed control based on the feedrate difference on each axis at a corner
By using the speed control based on the feedrate difference on each
axis at a corner, if a feedrate change occurs on an axis on each axis at
a corner, the feedrate is determined so that any feedrate difference
exceeding the permissible feedrate difference on that axis that has
been set for parameter No. 1783 does not occur, and deceleration is
automatically performed.
(Example)
Program
N1 G01 G91 X100. F5000
N2 Y100.
N1
N2
Tangent feedrate
X-axis feedrate
Y-axis feedrate
The deceleration
based on the feedrate
difference is used.
Tan
g
ent feedrate
X-axis feedrate
Y-axis feedrate
The feedrate difference becomes
small, and the feedrate on each
axis becomes smooth.
The tangent feedrate is
smooth, but the feedrate
on each axis is not.
N1 N2 N1 N2
N1 N2 N1 N2
The method of deceleration based on the feedrate difference differs
depending on the setting made for bit 6 (FNW) of parameter No.
19500.
If "0" is set, the largest feedrate that does not exceed the permissible
feedrate difference set for parameter No. 1783 is assumed to be the
deceleration feedrate.
B-63944EN/03 PROGRAMMING
- 661 -
20.HIGH-SPEED CUTTING
FUNCTIONS
In this case, the deceleration feedrate differs if the travel direction
differs, even if the shape is the same.
Deceleration to
500 mm/min
Deceleration to
354 mm/min
(Example)
If parameter FNW (bit 6 of No. 19500) = 0 and the
permissible feedrate difference = 500 mm/min (on all axes)
If "1" is set, the feedrate is determined not only with the condition that
the permissible feedrate difference and permissible acceleration on
each axis are not exceeded, but also that the deceleration feedrate is
constant regardless of the travel direction if the shape is the same.
If 1 is set for this parameter, the deceleration feedrate determined with
the feedrate difference may be up to 30% lower than that determined
if 0 is set.
Deceleration to
354 mm/min
Deceleration to
354 mm/min
(Example)
If parameter FNW (bit 6 of No. 19500) = 1 and
permissible feedrate difference = 500 mm/min (on all axes)
PROGRAMMING B-63944EN/03
- 662 -
20. HIGH-SPEED CUTTING
FUNCTIONS
- Speed control with acceleration in circular interpolation
When high-speed cutting is performed in circular interpolation, helical
interpolation, or spiral interpolation, the actual tool path has an error
with respect to the programmed path. In circular interpolation, this
error can be approximated from the equation given below.
Specified path
A
ctual path
∆
r : Maximum radius error (mm)
v : Feedrate (mm/sec)
r : Arc radius (mm)
a : Acceleration (mm/sec2)
T1: Time constant of
acceleration/deceleration after
interpolation at cutting (sec)
T2: Time constant of servo motor (sec)
∆
r : Error
0
Y
X
r
a)
2
2
T
2
1
T(
2
1
r
2
v
)
2
2
T
2
1
T(
2
1
r⋅+=+=∆ ................................ (Equation 1)
In actual machining, permissible error ∆r is given, so the maximum
permissible acceleration a (mm/sec2) in equation 1 is determined.
When a specified feedrate causes the radial error from an arc having a
programmed radius to exceed the permissible error, speed control with
acceleration in circular interpolation automatically clamps the
arc-cutting feedrate by using parameter settings.
Let the permissible acceleration calculated from the permissible
acceleration set for each axis be A. Then, maximum permissible
feedrate v with programmed radius r is expressed as follows:
rAv ⋅= ........................................................................... (Equation 2)
If a specified feedrate exceeds feedrate v obtained from equation 2,
the feedrate is clamped at feedrate v automatically.
The permissible acceleration is specified in parameter No. 1735. If
there is a difference in permissible acceleration between two axes for
circular interpolation, the lower acceleration is regarded as the
permissible acceleration.
If the radius of an arc is small, too small value can be calculated as
deceleration v. In such a case, the lower feedrate limit can be set in
parameter No. 1732 to prevent the feedrate from being decreased too
much.
B-63944EN/03 PROGRAMMING
- 663 -
20.HIGH-SPEED CUTTING
FUNCTIONS
- Speed control with the acceleration on each axis
When consecutive small lines are used to form a curve, as in the
example shown in the figure below, the feedrate differences on each
axis at the individual corners are not very large. Thus, deceleration
with the feedrate differences is not effective. Consecutive small
feedrate differences, however, cause a large acceleration on each axis,
as a whole.
In such a case, deceleration can be performed to reduce the impact on
the machine and the machining error caused by too large an
acceleration. The deceleration feedrate is determined to be the feedrate
that does not cause the acceleration on each axis to exceed the
permissible acceleration set for parameter No. 1737.
The deceleration feedrate is determined for each corner. The actual
feedrate is the smaller of the deceleration feedrate determined at the
start point of the block and that determined at the end point.
Depending on the specified figure, a very low deceleration feedrate
may be calculated. In such a case, the lower feedrate limit can be set in
parameter No. 1738 to prevent the feedrate from being decreased too
much.
In the following example, the acceleration (gradient of the broken line
in the feedrate graph) at too large at corners N2 to N4 and N6 to N8
and, therefore, deceleration is performed.
X-axis
feedrate
N1
N2
Y
X
N3
N4
N6
N7
N8
Y-axis
feedrate
Tangent
feedrate
N1 N5 N9 N1 N5 N9
N9
N5
PROGRAMMING B-63944EN/03
- 664 -
20. HIGH-SPEED CUTTING
FUNCTIONS
The method of determining the feedrate with the acceleration differs
depending on the setting of bit 6 (FNW) of parameter No. 19500.
If "0" is set, the highest feedrate that does not cause the permissible
acceleration set for parameter No. 1737 to be exceeded is assumed to
be the deceleration feedrate. In this case, the deceleration feedrate
differs depending on the travel direction even if the shape is the same,
as shown in the figure below.
(Example) If a circular shape with a radius of 10 mm is specified with small
line blocks
Parameter FNW (bit 6 of No. 19500) = 0
Permissible acceleration = 1000 mm/s2 (on all axes)
The feedrate is
higher in these
directions.
Tangent feedrate
Time
F6000
If "1" is set, the feedrate is determined with not only the condition that
the permissible acceleration on each axis is not exceeded but also the
condition that the deceleration feedrate is constant regardless of the
travel direction if the shape is the same.
If 1 is set for this parameter, the deceleration feedrate determined with
the feedrate difference or acceleration may be up to 30% lower than
that determined if 0 is set.
(Example) If a circular shape with a radius of 10 mm is specified with small
line blocks
Parameter FNW (bit 6 of No. 19500) = 1,
radius = 10 mm, permissible acceleration = 1000 mm/s2 (on all axes)
The tangent
feedrate is
constant.
Tangent feedrate
Time
F6000
NOTE
In circular interpolation, the tangent feedrate is
constant regardless of the setting of the parameter.
B-63944EN/03 PROGRAMMING
- 665 -
20.HIGH-SPEED CUTTING
FUNCTIONS
- Smooth speed control
In speed control with acceleration, the smooth speed control function
recognizes the entire figure from preceding and following blocks
including blocks read ahead to make a smooth feedrate determination.
When a curve is specified with successive minute straight lines,
programmed values are rounded to the least input increment before
issued, so the machining profile is approximated with a broken line.
When the feedrate is determined with acceleration in an ordinary
manner, an optimum feedrate is automatically calculated exactly for a
programmed figure, so a large acceleration may result depending on
the command, which can lead to deceleration.
In such a case, the use of smooth speed control enables speed control
by recognizing the entire figure, which provides smooth speed control
while suppressing local deceleration, therefore increasing the feedrate.
Large acceleration
: Programmed path
: Recognized figure
Also for a part of a programmed figure in which a large acceleration
would be required, the acceleration is obtained based on the figure
recognized from multiple blocks, and the feedrate is determined so
that the acceleration is within the permissible acceleration set in
parameter No. 1737.
Tangential feedrate Deceleration with acceleration
in ordinar
y
manner
Smooth speed control
Time
Command with large acceleration
PROGRAMMING B-63944EN/03
- 666 -
20. HIGH-SPEED CUTTING
FUNCTIONS
Smooth speed control obtains the acceleration by using the figure
recognized from the preceding and following blocks including blocks
read ahead, so smooth speed control is enabled even in parts in which
the acceleration increases.
Smooth speed control is enabled under the following conditions:
<1> Speed control with acceleration is enabled in the AI contour
control mode.
<2> Successive linear interpolation commands are specified.
<3> Bit 0 (HPF) of parameter No. 19503 is set to 1.
CAUTION
When smooth speed control is used, the feedrate in
a certain figure such as a corner may become
larger than the feedrate obtained by ordinary speed
control with acceleration. For corners, set
parameter No. 1783, which is the permissible
feedrate difference parameter for speed control with
the feedrate difference at corners, to perform
appropriate deceleration by speed control with the
corner feedrate difference.
- Speed control with the cutting load
Usually, the cutting resistance produced when machining is performed
with the bottom of the cutter as the tool lowers along the Z-axis is
greater than the cutting resistance produced when machining is
performed with the side of the cutter as the tool rises along the Z-axis.
Therefore, deceleration is required.
In AI contour control, the tool travel direction on the Z-axis is used as
a condition for calculating the machining feedrate.
This function is enabled when bit 4 (ZAG) of parameter No. 8451 is
set to 1.
During ascent on the Z-axis
θ
During descent on the Z-axis
B-63944EN/03 PROGRAMMING
- 667 -
20.HIGH-SPEED CUTTING
FUNCTIONS
The descent angle
θ
during descent on the Z-axis (angle formed by the
XY plane and the tool center path) is as shown in the figure. The
descent angle is divided into four areas, and the override values for the
individual areas are set for the following parameters:
Parameter No. 8456 for area 2
Parameter No. 8457 for area 3
Parameter No. 8458 for area 4
For area 1, however, no parameter is available, and an override of
100% is used at all times. The feedrate obtained according to other
feedrate control is multiplied by the override value of the area to
which descent angle
θ
belongs.
Area1 0º ≤
θ
< 30º
Area2 30º ≤
θ
< 45º
Area3 45º ≤
θ
< 60º
Area4 60º ≤
θ
< 90º
The feedrate can be overridden with an inclination by setting bit 1
(ZG2) of parameter No. 19515 to 1. In this case, specify the override
value for area 1 in parameter No. 19516.
XY plane
Z
30°
45°
60°
90°
A
rea1
A
rea2
A
rea3
A
rea4
PROGRAMMING B-63944EN/03
- 668 -
20. HIGH-SPEED CUTTING
FUNCTIONS
CAUTION
1 The speed control with the cutting feed is effective
only when the tool is parallel with the Z-axis.
Thus, it may not be possible to apply this function,
depending on the structure of the machine used.
2 In the speed control with the cutting feed, the travel
direction on the Z-axis is determined with the
appropriate NC command. If, therefore, manual
intervention is performed on the Z-axis with manual
absolute on, or if a mirror image is applied on the
Z-axis, the direction on the Z-axis cannot be
determined. When using the speed control with
the cutting load, do not use these functions.
3 When performing three-dimensional coordinate
conversion, determine the descent angle on the
Z-axis using the converted coordinate system.
4 Speed control with the cutting load is enabled for
all interpolations in the AI contour control mode.
This function, however, can be made valid only for
linear interpolations by setting bit 4 (ZOL) of
parameter No. 19503 to 1.
- Ignoring feedrate commands
In a block in which AI contour control is enabled, all feedrate
commands (F commands) can be ignored by setting bit 7 (NOF) of
parameter No. 8451.
The term feedrate commands, as used here, refer to the following
commands:
<1> Modal F commands before the block in which AI contour control
is enabled
<2> F commands and modal F commands in the block in which AI
contour control is enabled
When the feedrate commands are ignored, it is assumed that the upper
feedrate limit specified for parameter No. 8465 is specified.
Note, however, that any issued F commands and modal F commands
are stored within the CNC.
Thus, in a block in which AI contour control changes from the
enabled state to the disabled state, the modal values of the F
commands described in <1> and <2> described above are used as
modal F commands, instead of the modal values of the F commands
calculated by AI contour control.
- Another example of determining the feedrate
If a specified feedrate exceeds the upper feedrate limit of AI contour
control (in parameter No. 8465), the feedrate is clamped at the upper
feedrate. The upper feedrate limit is clamped at the maximum
cutting feedrate (parameter No. 1432).
B-63944EN/03 PROGRAMMING
- 669 -
20.HIGH-SPEED CUTTING
FUNCTIONS
Limitation
- Conditions for temporarily canceling the AI contour control mode
If one of the commands listed below is issued in the AI contour
control mode, the AI contour control mode is canceled temporarily.
If the system becomes ready for AI contour control after it is canceled,
the AI contour control mode is restored automatically.
• Positioning (rapid traverse)
• Single direction positioning
• Spindle positioning
• Rigid tapping
• Hypothetical axis interpolation
• Threading (single type, combined type)
• Electronic gear box
• Superimposed control
• When no move command is specified
• One-shot G code other than the following:
Tool offset
Cutter compensation vector retention
Cutter compensation corner rounding
Exact stop
- Functions that cannot be specified in the AI contour control mode
In the AI contour control mode, the functions listed below cannot be
specified. Before specifying these functions, turn off the AI contour
control mode; after the command ends, turn on the mode again.
• Threading
• Circular threading
• Variable lead threading
Threading, circular threading, and variable lead threading can be
specified in the AI contour control mode by setting bit 1 (THA) of
parameter No. 1611. However, the AI contour control mode is
automatically canceled.
Notes
- About processing macro statements
In AI contour control mode, the NC statements of multiple blocks are
looked ahead. Macro statements such as arithmetic expressions and
conditional branches are processed as soon as they are read into the
buffer. Therefore, the timing of the macro statement execution is not
always the specified order.
In case that you need to execute the macro statement after completing
the NC block just before the macro statement, specify M code or G
code that is not buffered just before the macro statement. Specially, in
case of reading/writing the system variables to control signals,
coordinates, offset value, etc., it may be different system variable data
by the timing of the NC statement execution. To avoid this
phenomenon, specify such M codes or G codes before the macro
statement, if necessary.
PROGRAMMING B-63944EN/03
- 670 -
20. HIGH-SPEED CUTTING
FUNCTIONS
20.2 MACHINING CONDITION SELECTING FUNCTION
Overview
By setting a speed- or precision-focused parameter set in an AI
contour control function and specifying a precision level in
accordance with the machining conditions during machining,
parameters suitable to the conditions can be automatically calculated
so that machining can be performed.
This function is an optional one.
Format
- Changing the precision level using a program
In addition to being switched on the precision level selection screen,
the precision level can be changed using a program in the format
below.
G05.1 Q1 Rx ;
x .......Level (1 to 10)
The precision level can also be changed in the format used with
conventional "advanced preview control", "high precision contour
control", and "AI high precision contour control".
G05 P10000 Rx ;
x .......Level (1 to 10)
G08 P1 Rx ;
x .......Level (1 to 10)
CAUTION
Once specified, a level remains effective even if the
AI contour control mode is canceled.
B-63944EN/03 PROGRAMMING
- 671 -
20.HIGH-SPEED CUTTING
FUNCTIONS
20.3 JERK CONTROL
20.3.1 Speed Control with Change of Acceleration on Each Axis
Overview
In portions in which acceleration changes largely, such as a portion
where a programmed figure changes from a straight line to curve,
vibration or shock on the machine may occur. Speed control with
change of acceleration on each axis is a function to suppress
machining errors due to vibration and machine shock generated by
change of acceleration. This function obtains a feedrate so that
change of acceleration is within the parameter-set permissible accel-
eration change amount for each axis, and performs deceleration by
using acceleration/deceleration before interpolation.
CAUTION
Before speed control with change of acceleration
on each axis can be used, the options for jerk
control and AI contour control are required.
Explanation
In the following example, the Y-axis acceleration changes largely at
the contact point between a linear interpolation and circular interpo-
lation, so deceleration is performed.
From linear interpolation (N1) to circular interpolation (N2)
Y
X
Vibration due to change
of acceleration
N1
N2
Tangential
feedrate
Y-axis
acceleration
Feedrate
Time
N1
N2
Time
Feedrate
A
cceleration
Time
A
cceleration
Time
PROGRAMMING B-63944EN/03
- 672 -
20. HIGH-SPEED CUTTING
FUNCTIONS
- Setting the permissible acceleration change amount
The permissible acceleration change amount for each axis is set in
parameter No. 1788. When 0 is set in this parameter for a certain
axis, speed control with change of acceleration is not performed for
that axis.
• Parameter setting example
Suppose a figure shown below in which a straight line is followed by
an arc. Let the specified feedrate and the arc radius be 6000 mm/min
and 10 mm, respectively. Then, the Y-axis acceleration change
amount at the contact point of the linear and arc portions is obtained
as follows:
Y
X
Y-axis
acceleration
A
cceleration
Time
From straight line to arc
Specified feedrate: 6000 mm/min
A
cceleration
change amount:
1000 mm/s2
A
rc radius: 10 mm
To suppress the change of acceleration to 300 mm/s2, set 300 mm/s2
for the Y-axis in parameter No. 1788.
Note that the change of acceleration is determined from the
interpolation data of the CNC, so it may differ from the theoretical
value.
The actual machine is affected by acceleration/deceleration and other
factors, so the value to be set in the parameter should be determined
after adjustments are made.
2
2
/1000 smm
r
v=
B-63944EN/03 PROGRAMMING
- 673 -
20.HIGH-SPEED CUTTING
FUNCTIONS
- For successive linear interpolations
When there are successive linear interpolations, speed control with
change of acceleration obtains the deceleration feedrate from the
change in acceleration between the start point and end point of a
specified block.
When a curve is specified using successive minute straight lines,
programmed values are rounded to the least input increment before
issued, so the machining profile is approximated with a broken line.
The error due to rounding may increase change of acceleration, and
especially when the line segments specified by blocks are short,
deceleration is performed frequently. As a result, the machining
speed cannot increase enough. In such a case, a relatively large
value should be set in parameter No. 1789 as the permissible
acceleration change amount for each axis in successive linear
interpolations to improve the machining speed.
When a value other than 0 is set in parameter No. 1789 for an axis for
which deceleration with change of acceleration is enabled, this setting
is regarded as the permissible acceleration change amount at corners
in which linear interpolations meet. (For portions where a linear
interpolation and circular interpolation meet and where circular
interpolations meet, the setting in parameter No. 1788 is used.)
When 0 is set in parameter No. 1789 for an axis, the setting in
parameter No. 1788 specifying the ordinary permissible acceleration
change amount is used even at a corner in which linear interpolations
meet.
When smooth speed control is used in speed control with permissible
acceleration in AI contour control (named temporarily), the
deceleration feedrate is obtained from the change of acceleration
calculated by smooth speed control.
Therefore, the deceleration feedrate may be higher than the ordinary
deceleration feedrate.
When linear interpolation is followed
by circular interpolation, speed
control is performed using the
permissible acceleration change
amount set in parameter No. 1788.
Linear
interpolation Circular
interpolation
For successive linear interpolations,
speed control is performed using the
permissible acceleration change
amount set in parameter No. 1789.
Linear
interpolation
PROGRAMMING B-63944EN/03
- 674 -
20. HIGH-SPEED CUTTING
FUNCTIONS
20.3.2 Look-Ahead Smooth Bell-Shaped Acceleration/Deceleration
before Interpolation
Overview
In look-ahead bell-shaped acceleration/deceleration before interpo-
lation performs smooth acceleration/deceleration by changing the
acceleration at a constant rate in specified acceleration change time.
In look-ahead smooth bell-shaped acceleration/deceleration before
interpolation, the jerk change time is specified in parameter No. 1790
by using the percentage to the acceleration change time for look-ahead
bell-shaped acceleration/deceleration before interpolation, and change
of acceleration is also controlled so that the change is bell-shaped.
This enables smoother acceleration/deceleration, therefore reducing
machine vibration and shock due to acceleration/ deceleration.
(Look-ahead bell-shaped
acceleration/deceleration before interpolation)
(Look-ahead smooth bell-shaped
acceleration/deceleration before interpolation)
Time
Tangential feedrate
A
cceleration
Jerk
acceleration
Jerk
acceleration
A
cceleration change time
Time set in parameter No.
1772
Jerk change time
Time set in parameter No.
1790 by using the
percentage to the
acceleration change time
Tangential feedrate
Time
Time Time
Time Time
A
cceleration
CAUTION
Before look-ahead smooth bell-shaped acceleration/deceleration before interpolation
can be used, the option for jerk control and AI contour control II is required.
B-63944EN/03 PROGRAMMING
- 675 -
20.HIGH-SPEED CUTTING
FUNCTIONS
Explanation
- Setting the jerk change time
The jerk change time is set in parameter No. 1790 by using the
percentage to the acceleration change time.
The actual jerk change time is represented by the percentage to the
acceleration change time set in parameter No. 1772.
The jerk change time must be within a half of the acceleration change
time, so the value to be set in the parameter ranges 0 to 50 (percent).
If 0 or a value beyond the specifiable range is specified in parameter
No. 1790, look-ahead smooth bell-shaped acceleration/deceleration
before interpolation is not enabled.
- Acceleration/deceleration before interpolation for linear type rapid traverse
When bell-shaped acceleration/deceleration is used in acceleration/
deceleration before interpolation for linear type rapid traverse,
enabling look-ahead smooth bell-shaped acceleration/deceleration
before interpolation applies smooth bell-shaped acceleration/decel-
eration to acceleration/deceleration before interpolation for linear type
rapid traverse.
In this case, the jerk change time is represented by the percentage set
in parameter No. 1790 to the acceleration change time set in parameter
No. 1672.
- Optimum torque acceleration/deceleration
When bell-shaped acceleration/deceleration is used in optimum torque
acceleration/deceleration, enabling look-ahead smooth bell-shaped
acceleration/deceleration before interpolation applies smooth
bell-shaped acceleration/deceleration to optimum torque acceleration/
deceleration.
In this case, the jerk change time is represented by the percentage set
in parameter No. 1790 to the acceleration change time set in parameter
No. 1672.
PROGRAMMING B-63944EN/03
- 676 -
20. HIGH-SPEED CUTTING
FUNCTIONS
20.4 OPTIMUM TORQUE ACCELERATION/DECELERATION
Overview
This function enables execution of acceleration/deceleration adapted
to the torque characteristics of the motor and the characteristics of the
machine due to the friction and gravity of the machine.
Usually, because of the friction of the machine, gravity, the torque
characteristics of the motor, and other factors, the acceleration/
deceleration performance (torque for acceleration/deceleration) is
different with direction of movement, acceleration or deceleration. In
this function, acceleration pattern of rapid traverse for the following
situations, plus movement and acceleration, plus movement and
deceleration, minus movement and acceleration, minus movement and
deceleration can be set into parameters according to the torque for
acceleration/deceleration of each situation.
Acceleration/deceleration can be performed according to these
parameter setting, so that the most of the capability of the motor can
be used and positioning time can be reduced.
Tim e
Tim e
Acceleration
A
cc/Dec pattern is the sam e way in each condition.
Speed
A
cceleration
and
+ move
Deceleration
and
+ move
A
cceleration
and
-move
Deceleration
and
- m ove
Fig. 20.4 (a) Conventional acceleration/declaration
Tim e
Speed
Tim e
Acceleration
A
cceleration
and
+ move
Deceleration
and
+ m ove
A
cc/Dec pattern can be changed in each condition.
A
cceleration
and
- m ov e
Deceleration
and
- m ov e
Fig. 20.4 (b) Acceleration/deceleration with this function
B-63944EN/03 PROGRAMMING
- 677 -
20.HIGH-SPEED CUTTING
FUNCTIONS
Explanation
Optimum torque acceleration/deceleration selects the acceleration
pattern set with parameters on the basis of the axial movement
direction and the acceleration/deceleration state, determines the
acceleration for each axis from the current speed, and controls the
tangential acceleration/deceleration for rapid traverse.
- Setting optimum torque acceleration/deceleration
When bit 0 (FAP) of parameter No. 19540 and bit 1 (LRP) of
parameter No. 1401 are set to 1, and a value other than 0 is set for any
one of the axes as the reference acceleration in parameter No. 1671 as
shown below, rapid traverse is accelerated/decelerated by optimum
torque acceleration/deceleration.
Table 20.4 (a) Optimum torque acceleration/deceleration
Parameter
FAP
(Optimum
torque
acc/dec)
Parameter
LRP
(Linear type
positioning)
Reference
acceleration
Bell-shaped
acceleration
change time
Acceleration
pattern
1 1
Parameter
No.1671
Parameter
No.1672
See "Setting an
acceleration
pattern".
To enable bell-shaped acceleration/deceleration in addition to
optimum torque acceleration/declaration, set the bell-shaped accel-
eration change time with parameter No.1672.
- Required conditions in addition to parameter setting
If the conditions for performing AI contour control and for
acceleration/deceleration before interpolation are satisfied, optimum
torque acceleration/deceleration is performed for accelerating and
decelerating rapid traverse. Note, however, that if 1 is set to bit 0
(FAE) of parameter No. 11240, optimum torque
acceleration/deceleration is enabled even if AI contour control is
disabled. If rapid traverse is subject to optimum torque
acceleration/deceleration, after-interpolation acceleration/deceleration
does not apply to rapid traverse.
- Cases in which optimum torque acceleration/ deceleration is disabled
If optimum torque acceleration/deceleration is disabled by parameter
settings, or the required conditions other than parameter settings are
not satisfied, acceleration/deceleration after interpolation is used to
accelerate and decelerate rapid traverse.
PROGRAMMING B-63944EN/03
- 678 -
20. HIGH-SPEED CUTTING
FUNCTIONS
- Setting acceleration pattern data
A
cceleration
Speed
Fb Fa
A
a
P1 P
2
P3
P4 P
5
Ab
A
cceleration patter
n
P0
Fig. 20.4 (c) Setting acceleration pattern
Set the speed and the acceleration at each of the acceleration setting
points P0 to P5 for each condition, plus movement and acceleration,
plus movement and deceleration, minus movement and acceleration,
minus movement and deceleration, and for each axis.
The line joining the acceleration setting points is regarded a
acceleration pattern.
For example, while the speed is between Fa and Fb in the previous
figure, the acceleration is calculated with Aa and Ab. Tangential
acceleration is controlled not to exceed the calculated acceleration for
each axis.
CAUTION
It is not desirable to set an acceleration pattern in
which a large acceleration is set right at a speed of
0, because this will shock the machine. For this
reason, be sure to set a low acceleration at a
speed of 0, as in the figure above.
Table 20.4 (b) Parameters for acceleration pattern
Acceleration parameter
During acceleration During deceleration
Acceleration
setting point
Speed
parameter
During
movement in
plus
direction
During
movement in
minus
direction
During
movement in
plus
direction
During
movement in
minus
direction
P0 (Speed 0) No.19545 No.19551 No.19557 No.19563
P1 No.19541 No.19546 No.19552 No.19558 No.19564
P2 No.19542 No.19547 No.19553 No.19559 No.19565
P3 No.19543 No.19548 No.19554 No.19560 No.19566
P4 No.19544 No.19549 No.19555 No.19561 No.19567
P5 No.1420 No.19550 No.19556 No.19562 No.19568
B-63944EN/03 PROGRAMMING
- 679 -
20.HIGH-SPEED CUTTING
FUNCTIONS
The speed at P0 is 0, and the speed at P5 is the rapid traverse rate
specified with parameter No. 1420. The speeds at P1 to P4 are to be
set into speed parameters Nos. 19541 to 19544 as ratio to the rapid
traverse speed (parameter No. 1420).
Any acceleration setting point for which the speed parameters Nos.
19541 to 19544 is set to 0 will be skipped, and the next point whose
speed parameter is set to a non-zero value will be joined together as
acceleration pattern.
The accelerations at P0 to P5 are to be set into acceleration parameters
Nos. 19545 to 19568 as ratio to the reference acceleration. If any of
the acceleration parameters Nos. 19545 to 19568 is set to 0, the
acceleration is assumed 100% (Reference acceleration). Acceleration
parameters should be set to 0 at the acceleration setting point whose
speed parameter is set to 0.
If this function is enabled and parameter No.1671 for an axis are set to
0, the following values are assumed as the reference acceleration for
that axis:
1000.0mm/sec2, 100.0inch/sec2, 100.0 deg/sec2
- Example of setting acceleration pattern data
In this example, the machine is equipped with the αiS 30/4000.
Motor speed at rapid traverse is 3000 (min-1).
0
50
100
150
0 1000 2000 3000 4000
Speed(min-1)
Torque(Nm)
Fig. 20.4 (d) Speed-torque characteristics of model αiS 30/4000
Specifications of the motor model αiS 30/4000
Rotor inertia :0.0099(Kgm2)
Maximum torque :100(Nm) Speed 0 to 2000(min-1)
Torque at rapid traverse :79(Nm) Speed 3000(min-1)
Minimum torque :58(Nm) Speed 4000(min-1)
It assumes that 10 (Nm) is needed for the friction torque, so that the
torque for acceleration/deceleration is shown as the following figure.
Because the friction torque is different on each machine, it is
necessary to observe the actual torque output on the machine.
Maximum torque :90(=100-10)(Nm) Speed 0 to 2000(min-1)
Torque at rapid traverse :69(=79-10)(Nm) Speed 3000(min-1)
Minimum torque :48(=58-10)(Nm) Speed 4000(min-1)
PROGRAMMING B-63944EN/03
- 680 -
20. HIGH-SPEED CUTTING
FUNCTIONS
0
20
40
60
80
100
0 1000 2000 3000 4000
Speed(min-1)
Torque(Nm)
Fig. 20.4 (e) Torque for Acc/Dec with consideration of friction
Let the torque be x (Nm), the inertia be y (Kgm2), and the ball screw
pitch p (mm), then the acceleration A is calculated as follows:
]sec/[
2
][
2
][
])][sec/([
][
2
][
][
2
2
2
2
mm
y
px
mm
p
mkgy
mmkgx
mm
p
mkgy
mNx
A
×
×
=
×
⋅
⋅
=×
⋅
⋅
=
π
ππ
Machine specification is assumed as follows,
Ball screw pitch : 16 (mm)
Inertia : The machine inertia is to be 2.0 times higher than
that of the rotor.
(Rotor inertia: 0.0099 (Kgm2))
The acceleration at maximum torque 90 (Nm) is,
]sec/[7717
0099.00.32
1690 2
mm=
××
×
π
The acceleration at torque 69 (Nm) in rapid traverse 3000 (min-1) is,
]sec/[5916
0099.00.32
1669 2
mm=
××
×
π
From the above data, the parameters related to acceleration pattern is
given in the table below.
The example assumes that the acceleration is the same regardless of
whether acceleration or deceleration is in progress or whether the
movement is in the plus or minus direction.
• When setting the speed at P1, use the following value as a rough
guide:
If a bell-shaped acceleration change time (parameter No. 1672) is
set, use as a rough guide the ratio of the following speed to the
rapid traverse rate:
Reference acceleration × T2/4
where T2 is the bell-shaped acceleration change time (msec).
For example, assume T2 to be 40 msec, then the speed at P1
should be approximately
4124 [mm/sec2]×40 [msec]/4
=4124 [mm/sec2]×602×40 [msec]/60000/4
=2474 [mm/min]
• If no bell-shaped acceleration change time (parameter No. 1672)
is set, use about 5% of the rapid traverse rate as a rough guide.
B-63944EN/03 PROGRAMMING
- 681 -
20.HIGH-SPEED CUTTING
FUNCTIONS
Table 20.4 (c) Example of setting parameters related to acceleration pattern
Parameter No. Setting Unit Remarks
Rapid
traverse rate
1420 48000. mm/
min
The ball screw pitch is assumed 16
mm, so that the rapid traverse rate is
48000 mm/min at the maximum speed
3000 (min-1).
Reference
acceleration
1671
4124. msec Reference acceleration is
4124mm/sec2.
Speed at P1 19541 515 0.01% - Assuming that parameter No. 1672
(bell-shaped acceleration change
time) is set to 40 (msec), the speed
at P1 will be 2474 mm/min from the
calculation described on the
previous page. Set its ratio to the
rapid traverse rate, or 5.15%.
0.0515=2474/48000
- If parameter No. 1672 (bell-shaped
acceleration change time) is not
set, set about 5.00%.
Speed at P2 19542 6666 0.01% Since the torque characteristic is
constant (90 Nm) in speeds reaching
2000 min-1, set P2 to the ratio of the
speed (32000 mm/min) at 2000 min-1
to the rapid traverse rate (48000
mm/min).
0.6666=32000 / 48000
Speeds at P3
to P4
19543 to 19544 0 0.01% P3 to P4 are skipped because the
torque drops almost linearly from the
speed
2000 (min-1) to 3000 (min-1).
Acceleration
at P0
19545,19551,
19557,19563
9356 0.01% Set half the acceleration at P1, or
9356.
Acceleration
at P1
19546,19552,
19558,19564
18712 0.01% At P1, 90(Nm) can be used for the
acceleration/deceleration, so set the
ratio 7717 (mm/sec2) to 4124
(mm/sec2).
(1.8712 = 7717/4124)
Acceleration
at P2
19547,19553
19559,19565
18712 0.01% At P2, set the same speed as that at
P1.
Acceleration
at P3 to P4
19548 to 19549,
19554 to 19555,
19560 to 19561
19566 to 19567
0 0.01% 0 is set because P3 to P4 are
skipped.
Acceleration
at P5
19550,19556
19562,19568
14345 0.01% At P5, 69(Nm) can be used for the
acceleration/deceleration, so set the
ratio 5916 (mm/sec2) to 4124
(mm/sec2).
(1.4345 = 5916 / 4124)
PROGRAMMING B-63944EN/03
- 682 -
20. HIGH-SPEED CUTTING
FUNCTIONS
With the above parameter settings, the acceleration pattern will be
shown as the following figure. From speeds from 0 mm/min to 2474
mm/min, the acceleration as calculated in accordance with the
acceleration pattern is applied; from speeds from 2474 mm/min to
32000 mm/min, an acceleration of 7716 mm/sec2; and from speeds
from 32000 mm/min to 48000 mm/min, the acceleration as calculated
in accordance with the acceleration pattern.
P2P1
P0
0
1000
2000
3000
4000
5000
6000
7000
8000
9000
0 8000 16000 24000 32000 40000 48000
Speed mm/min
Acceleration mm/sec2
P5
Fig. 20.4 (f) Acceleration pattern with consideration of friction
NOTE
The values in the model αiS 30/4000 speed-torque
characteristic diagram are just typical ones. The
values will change depending on the digital servo
software, parameters, input voltage, and other
factors.
The optimum acceleration will, therefore, change
due to the characteristics of the machine.
- Examples of setting if the acceleration pattern differs depending on whether
acceleration or deceleration is in progress and whether the movement is in the
minus or plus direction
From the effect of gravity and friction, torque for
acceleration/deceleration is different on each condition, such as
acceleration, deceleration or plus move (up), minus move (down).
The following example is for the vertical axis and gravity and friction
torque are assumed as follows.
Torque of gravity : 20 (Nm)
Torque of friction : 10 (Nm)
Because these value are different on each machine, it is necessary to
observe the output torque on the actual machine for deciding
acceleration pattern. The conditions are the same as the previous
example.
(Condition)
Motor speed at rapid traverse : 3000(min-1)
Ball screw pitch : 16(mm)
Inertia : The machine inertia is to be 2.0 times higher than
that of the rotor.
Rotor inertia : 0.0099(Kgm2)
B-63944EN/03 PROGRAMMING
- 683 -
20.HIGH-SPEED CUTTING
FUNCTIONS
Maximum torque : 100(Nm) Speed 0 to 2000(min-1)
Torque at rapid traverse : 79(Nm) Speed 3000(min-1)
Minimum torque : 58(Nm) Speed 4000(min-1)
(1) In case of plus move (up) and acceleration
Because torque of Gravity and friction work against the output
torque of motor, the torque for acceleration/deceleration is as
follows.
Maximum torque : 70(=100-20-10) (Nm)
Speed 0 to 2000(min-1)
Torque at rapid traverse : 49(=79-20-10) (Nm)
Speed 3000(min-1)
Minimum torque : 28(=58-20-10) (Nm)
Speed 4000(min-1)
0
20
40
60
80
0 1000 2000 3000 4000
Speed(min-1)
Torque(Nm)
P0 P1
P5
Fig. 20.4 (g) Torque for Acc/Dec in case of + move and acceleration
Parameter setting is as follows,
Parameter No. Setting Unit Remarks
Acceleration
at P0 19545 7277 0.01%
Set half the acceleration at P1, or
7277.
Acceleration
at P1-P2 19546,19547 14554 0.01%
At P1 and P2, 70(Nm) can be used for
the acceleration/ deceleration, so set
the ratio 6002 (mm/sec2) to 4124
(mm/sec2).
(1.4554 = 6002 / 4124)
Acceleration
at P3-P4 19548 to 19549 0 0.01% 0 is set because P3 to P4 are
skipped.
Acceleration
at P5 19550 10187 0.01%
At P5, 49(Nm) can be used for the
acceleration/deceleration, so set the
ratio 4201 (mm/sec2) to 4124
(mm/sec2).
(1.0187 = 4201 / 4124)
PROGRAMMING B-63944EN/03
- 684 -
20. HIGH-SPEED CUTTING
FUNCTIONS
P0
P1 P2
0
1000
2000
3000
4000
5000
6000
7000
0 8000 16000 24000 32000 40000 48000
Speed mm/min
Acceleration mm/sec2
P5
Fig. 20.4 (h) Acceleration pattern in case of + move and acceleration
(2) In case of plus move (up) and deceleration
Because torque of Gravity and friction work forward to the
output torque of motor, the torque for acceleration/deceleration is
as follows.
Maximum torque : 130(=100+20+10) (Nm)
Speed 0 to 2000(min-1)
Torque at rapid traverse : 109(=79+20+10) (Nm)
Speed 3000(min-1)
Minimum torque : 88(=58+20+10) (Nm)
Speed 4000(min-1)
0
50
100
150
0 1000 2000 3000 4000
Speed(min-1)
Torque(Nm)
P0 P1
P5
Fig. 20.4 (i) Torque for Acc/Dec in case of + move and deceleration
Parameter setting is as follows,
Parameter No. Setting Unit Remarks
Acceleration
at P0 19557 13514 0.01% Set half the acceleration at P1, or 13514.
Acceleration
at P1-P2 19558, 19559 27027 0.01%
At P1 and P2, 130(Nm) can be used for
the acceleration/ deceleration, so set the
ratio 11146 (mm/sec2) to 4124 (mm/sec2).
(2.7027 = 11146 / 4124)
Acceleration
at P3-P4 19560 to 19561 0 0.01% 0 is set because P3 to P4 are skipped.
Acceleration
at P5 19562 22662 0.01%
At P5, 109(Nm) can be used for the
acceleration/deceleration, so set the ratio
9346 (mm/sec2) to 4124 (mm/sec2).
(2.2662 = 9346 / 4124)
B-63944EN/03 PROGRAMMING
- 685 -
20.HIGH-SPEED CUTTING
FUNCTIONS
P0
P1 P2
0
2000
4000
6000
8000
10000
12000
0 8000 16000 24000 32000 40000 48000
Speed mm/min
Acceleration mm/sec2
P5
Fig. 20.4 (j) Acceleration pattern in case of + move and deceleration
(3) In case of minus move (down) and acceleration
Because torque of Gravity works forward to the output torque of
motor and torque of friction works against the output torque of
motor, torque for acceleration/deceleration is as follows.
Maximum torque : 110(=100+20-10) (Nm)
Speed 0 to 2000(min-1)
Torque at rapid traverse : 89(=79+20-10) (Nm)
Speed 3000(min-1)
Minimum torque : 68(=58+20-10) (Nm)
Speed 4000(min-1)
0
50
100
150
0 1000 2000 3000 4000
Speed(min-1)
Torque(Nm)
P0 P1 P5
Fig. 20.4 (k) Torque for Acc/Dec in case of - move and acceleration
Parameter setting is as follows,
Parameter No. Setting Unit Remarks
Acceleration at
P0 19551 11435 0.01%
Set half the acceleration at P1, or
11435.
Acceleration at
P1-P2 19552,19553 22869 0.01%
At P1 and P2, 110(Nm) can be used
for the acceleration/ deceleration, so
set the ratio 9431 (mm/sec2) to 4124
(mm/sec2).
(2.2869 = 9431 / 4124)
Acceleration at
P3-P4 19554 to 19555 0 0.01% 0 is set because P3 to P4 are
skipped.
Acceleration at
P5 19556 18504 0.01%
At P5, 89(Nm) can be used for the
acceleration/deceleration, so set the
ratio 7631 (mm/sec2) to 4124
(mm/sec2).
(1.8504 = 7631 / 4124)
PROGRAMMING B-63944EN/03
- 686 -
20. HIGH-SPEED CUTTING
FUNCTIONS
P0
P1 P2
0
1000
2000
3000
4000
5000
6000
7000
8000
9000
10000
0 8000 16000 24000 32000 40000 48000
Speed mm/min
Acceleration mm/sec2
P5
Fig. 20.4 (l) Acceleration pattern in case of - move and acceleration
(4) In case of minus move (down) and deceleration
Because torque of Gravity works against the output torque of
motor and torque of friction works forward to the output torque
of motor, torque for acceleration/deceleration is as follows.
Maximum torque : 90(=100-20+10) (Nm)
Speed 0 to 2000(min-1)
Torque at rapid traverse : 69(=79-20+10) (Nm)
Speed 3000(min-1)
Minimum torque : 48(=58-20+10) (Nm)
Speed 4000(min-1)
0
20
40
60
80
100
0 1000 2000 3000 4000
Speed(min-1)
Torque(Nm)
P0 P1
P5
Fig. 20.4 (m) Torque for Acc/Dec in case of - move and deceleration
Parameter setting is as follows,
Parameter No. Setting Unit Remarks
Acceleration at
P0 19563 9356 0.01% Set half the acceleration at P1, or 9356.
Acceleration at
P1-P2 19564,19565 18712 0.01%
At P1 and P2, 90(Nm) can be used for
the acceleration/ deceleration, so set the
ratio 7717 (mm/sec2) to 4124 (mm/sec2).
(1.8712 = 7717 / 4124)
Acceleration at
P3-P4
19566 to
19567 0 0.01% 0 is set because P3 to P4 are skipped.
Acceleration at
P5 19568 14345 0.01%
At P5, 69(Nm) can be used for the
acceleration/deceleration, so set the ratio
5916 (mm/sec2) to 4124 (mm/sec2).
(1.4345 = 5916 / 4124)
B-63944EN/03 PROGRAMMING
- 687 -
20.HIGH-SPEED CUTTING
FUNCTIONS
P0
P1 P2
0
1000
2000
3000
4000
5000
6000
7000
8000
9000
0 8000 16000 24000 32000 40000 48000
Speed mm/min
Acceleration mm/sec2
P5
Fig. 20.4 (n) Acceleration pattern in case of - move and deceleration
Limitation
- Linear type positioning
Optimum torque acceleration/deceleration is not enabled unless
linear-type positioning is set (bit 1 (LRP) of parameter No. 1401 is set
to 1).
- Modes and conditions
Optimum torque acceleration/deceleration is enabled when AI contour
control mode is active and the conditions under which look-ahead
acceleration/deceleration before interpolation is performed are
satisfied. Note, however, that if 1 is set to bit 0 (FAE) of parameter No.
11240, optimum torque acceleration/deceleration is enabled even if AI
contour control is disabled.
- Target axes
Optimum torque acceleration/deceleration cannot be performed for a
specific axis only. All axes operated by programmed commands are
targeted for optimum torque acceleration/deceleration. This means
that the PMC axes are excluded.
- Acceleration pattern
In the same direction move, it is necessary that the acceleration during
deceleration is set 1/3 of one during acceleration at least.
Also, the acceleration pattern data must be set so that the time required
for the deceleration from the rapid traverse rate to a speed of 0 does
not exceed 4000 (msec). This does not include the acceleration change
time of bell-shaped acceleration/deceleration.
If the deceleration acceleration ratio or the time required for the
deceleration to a speed of 0 exceeds the above range, alarm (DS1710)
will be issued at the time rapid traverse is executed.
A slight error will occur between the specified acceleration and the
actual acceleration.
PROGRAMMING B-63944EN/03
- 688 -
20. HIGH-SPEED CUTTING
FUNCTIONS
- Relationship with the customer board
Optimum torque acceleration/deceleration cannot be used from the
customer board.
- Tool center point control
Optimum torque acceleration/deceleration is disabled in the tool
center point control mode (except startup and cancellation). In this
case, positioning is accelerated/decelerated with the reference
acceleration.
B-63944EN/03 PROGRAMMING
- 689 -
20.HIGH-SPEED CUTTING
FUNCTIONS
20.5 HIGH-SPEED CYCLE MACHINING
This function converts the shape to be machined into a data group that
can be subject to high-speed pulse distribution, using the macro
executor, calls the data group with a CNC command (G05 command),
and executes it.
Format
G05 P10xxx Lxxx ;
P10001 to P10999 : Start number of the machining cycle to
call
L1 to L999 : Repeat count of the machining cycle
(assumed to be L1 if omitted).
Cycle data for up to 999 cycles can be created. Use address "P" to
specify which cycle to use for machining. It is possible to call multiple
cycles in succession using connection information (in a header) and
execute them.
Use address "L" to specify the repeat count of the machining cycle. It
is possible to specify the repeat count (in a header) for each cycle.
Connection of cycles and the repeat count are explained with the
following example.
Example)
If
Cycle 1 Connection information 2 Repeat count 1
Cycle 2 Connection information 3 Repeat count 3
Cycle 3 Connection information 0 Repeat count 1
G05 P10001 L2;
the following cycles are executed in succession:
1,2,2,2,3,1,2,2,2,3
PROGRAMMING B-63944EN/03
- 690 -
20. HIGH-SPEED CUTTING
FUNCTIONS
NOTE
1 If an attempt is made to issue the function in the
modes below, an alarm is issued.
• Hypothetical axis interpolation (G07)
• Cylindrical interpolation (G07.1)
• Polar coordinate interpolation (G12.1)
• Polar coordinate command (G16)
• Spindle speed fluctuation detection (G26)
• Tool radius⋅Tool nose radius compensation
(G41/G42)
• Normal direction control (G41.1/G42.1)
• Scaling (G51)
• Programmable mirror image (G51.1)
• Coordinate system rotation (G68)
• Canned cycle (G81 to G89)
• Constant surface speed control (G96)
• Macro interrupt (M96)
2 During high-speed cycle machining, single block
stop is disabled.
3 During high-speed cycle machining, handle
interruption is disabled.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 691 -
21 AXIS CONTROL FUNCTIONS
Chapter 21, "AXIS CONTROL FUNCTIONS", consists of the
following sections:
21.1 AXIS SYNCHRONOUS CONTROL ....................................692
21.2 POLYGON TURNING (G50.2, G51.2).................................709
21.3 SYNCHRONOUS, COMPOSITE AND SUPERIMPOSED
CONTROL BY PROGRAM COMMAND (G50.4, G51.4,
G50.5, G51.5, G50.6, AND G51.6)........................................715
21.4 ROTARY AXIS ROLL-OVER..............................................719
21.5 ARBITRARY ANGULAR AXIS CONTROL.......................721
21.6 TOOL RETRACT AND RECOVER .....................................732
21.7 ELECTRONIC GEAR BOX ..................................................736
21.8 TANDEM CONTROL ...........................................................771
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 692 -
21.1 AXIS SYNCHRONOUS CONTROL
Overview
When a movement is made along one axis by using two servo motors
as in the case of a large gantry machine, a command for one axis can
drive the two motors by synchronizing one motor with the other.
Moreover, by using a feedback signal from each motor, a positional
difference (synchronous error) between the two motors is detected to
compensate for the synchronous error. When a synchronous error
exceeding a set value occurs, a synchronous error check can be made
to issue an alarm and stop a movement along the axis.
An axis used as the reference for axis synchronous control is referred
to as a master axis (M-axis), and an axis along which a movement is
made in synchronism with the master axis is referred to as a slave axis
(S-axis).
Y
Z
A
(Slave axis)
X
(Master axis)
Fig. 21.1 (a) Example of machine with X and A being synchronous axes
Even when synchronous error compensation is not used, the
synchronous establishment function can be used for automatic
compensation to eliminate a machine coordinate error in cases such as
emergency stop cancellation.
An external signal can be used to turn synchronization on and off.
When synchronization is turned on and off using an external signal,
synchronous error compensation cannot be used.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 693 -
21.1.1 Axis Configuration for Axis Synchronous Control
Explanation
- Master axis and slave axis for axis synchronous control
An axis used as the reference for axis synchronous control is referred
to as a master axis (M-axis), and an axis along which a movement is
made in synchronism with the master axis is referred to as a slave axis
(S-axis).
By setting the axis number of a master axis in the parameter No. 8311
of the slave axis, the axis configuration for axis synchronous control is
determined.
- Synchronous operation and normal operation
Operation where axis synchronous control is turned on (enabled) to
make a movement along the slave axis in synchronism with the master
axis is referred to as synchronous operation. Operation where axis
synchronous control is turned off (disabled) to make movements along
the master axis and slave axis independently of each other is referred
to as normal operation.
(Example)
Automatic operation when the master axis is the X-axis and the slave
axis is the A-axis
In synchronous operation, movements are made along the X-axis
and A-axis according to the programmed command Xxxxx for
the master axis.
In normal operation, movements are made along the master axis
and slave axis independently of each other as in the case of
normal CNC control. The programmed command Xxxxx
makes a movement along the X-axis. The programmed
command Aaaaa makes a movement along the A-axis. The
programmed command Xxxxx Aaaaa makes movements along
the X-axis and A-axis at the same time.
The mode of operation can be switched between synchronous
operation and normal operation by an input signal, or synchronous
operation can be performed at all times. Which mode to use can be
set using bit 5 (SCA) of parameter No. 8304.
- Switching between synchronous operation and normal operation by using an
input signal
When bit 5 (SCA) of parameter No. 8304 is set to 0 for the slave axis,
the signal SYNCx/SYNCJx (with x representing a slave axis number)
is used to switch between synchronous operation and normal
operation. When SYNCx/SYNCJx = 1, synchronous operation is
selected. When SYNCx/SYNCJx = 0, normal operation is selected.
Synchronous error compensation cannot be used when the mode of
operation is switched between synchronous operation and normal
operation.
During feed axis synchronization control, the output signal SYNOx is
set to "1".
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 694 -
- Setting for using synchronous operation at all times
When bit 5 (SCA) of parameter No. 8304 for the slave axis is set to 1,
synchronous operation is performed at all times, regardless of the
setting of the signal SYNCx/SYNCJx.
- Synchronous control axis name
The name of a master axis and the name of a slave axis may be the
same or may be different from each other.
- Restrictions on using the same name for the master axis and slave axis
If the same axis name is assigned to the master axis and slave axis,
manual operation only is allowed in normal operation. Automatic
operation and manual numeric command cannot be performed.
- Setting of an axis name subscript
A subscript can be attached to an axis name like X1, X2, XM, and XS.
If the same axis name is used for multiple axes, and a unique subscript
is assigned to each of those axes, the axes can be distinguished from
each other on the screen display, or which of those axes issued an
alarm can be identified.
Set a subscript in parameter No. 3131.
- Setting of multiple slave axes
One master axis can have multiple slave axes.
(Example)
In the example below, movements along the X1-axis and X2-axis
are made in synchronism with the XM-axis.
Axis name
indication
Controlled
axis number
Axis name
Parameter
(No. 1020)
Subscript
Parameter
(No.3131)
Master axis
number
Parameter
(No.8311)
Operation
XM 1 88 77 0
Y 2 89 0 0
X1 3 88 49 1
A movement is made
in synchronism with
the XM-axis.
X2 4 88 50 1
A movement is made
in synchronism with
the XM-axis.
When one master axis has multiple slave axes, synchronous error
compensation, synchronous establishment, and synchronous error
check are performed for each slave axis independently.
- Combination with tandem control
Tandem control can be used with each of the master and slave axes.
The same restriction on axis arrangement as imposed in the case of
normal tandem control is imposed. No particular restriction is
imposed on axis synchronous control.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 695 -
- Axis selection on the screen display
On a screen such as the current position display screen, a slave axis is
also displayed. The display of a slave axis can be disabled by setting
bit 0 (NDP) of parameter No. 3115 to 1 and setting bit 1 (NDA) of
parameter No. 3115 to 1.
- Axis selection in actual cutting feedrate display
By setting bit 2 (SAF) of parameter No. 8303 to 1 for a slave axis, the
slave axis can be included in an actual cutting feedrate display
calculation during synchronous operation.
- Axis synchronous control with an absolute-position detector
When bit 7 (SMA) of parameter No. 8302 is set to 1 to attach an
absolute-position detector, and bit 4 (APZ) of parameter No. 1815 for
an axis placed in synchronous operation is turned off, APZ for the axis
(axes) placed together in synchronous operation is also turned off.
- Slave axis mirror image
By setting parameter No. 8312, a mirror image can be applied to a
slave axis placed in synchronous operation. When the mirror image
function is enabled, the direction in which the absolute and relative
coordinates change is the same as for the machine coordinates.
At this time, synchronization error compensation, synchronization
establishment, synchronization error check, and correction mode
cannot be used.
The mirror image set by bit 0 (MIR) of parameter No. 0012 cannot be
applied to the slave axis. Because this mirror image differs from the
mirror image set by parameter MIR, it does not affect input signal MIx
<G106> or output signal MMIx <F108>.
- External machine coordinate system shift
Bit 7 (SYE) of parameter No. 8304 can be set to 1 for the slave axis to
shift the slave axis by the same amount as specified for the master axis
when external machine coordinate system shift is specified by external
data input/output for the master axis in synchronous control.
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 696 -
21.1.2 Synchronous Error Compensation
Explanation
When a synchronous error value exceeding the zero width set in
parameter No. 8333 is detected, compensation pulses for synchronous
error reduction are calculated and added onto the command pulses
output for the slave axis. This compensation is not performed in
servo-off state, servo alarm state, follow-up operation, and
modification mode.
Compensation pulses are calculated by multiplying the synchronous
error value between master and slave axes by a compensation gain.
Compensation pulses = synchronous error × (Ci/1024)
Ci: Compensation gain (parameter No. 8334)
Before synchronous error compensation can be performed, bit 5
(SCA) of parameter No. 8304 must be set to 1 to perform synchronous
operation at all times. Furthermore, the first synchronous
establishment after power-up must already be performed by a manual
reference position return or another operation.
K1
Compensation
pulse counter
A
dded to command for
slave axis
Master axis
machine position
Slave axis machine
position
Compensation gain
Compensation pulses
+
-
Synchronous
error counter
- Synchronous error compensation smooth suppress function
When bit 6 (SMS) of parameter No. 8304 is set to 1, the synchronous
error compensation smooth suppress function is enabled. With this
function, another set of parameters for a synchronous error zero width
and synchronous error compensation gain (B and Ks in the figure
below) can be set. So, even a small synchronous error can be
reduced smoothly as shown below.
Synchronous error compensation gain
Synchronous error value
Kd
0
A
Ks
B
A: Synchronous error zero width (parameter No. 8333)
B: Synchronous error zero width 2 (parameter No. 8335)
(0 < B < A)
Kd: Synchronous error compensation gain (parameter No. 8334)
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 697 -
Ks: Synchronous error compensation gain 2 (parameter No.
8336) (0 < Ks < Kd)
Er: Synchronous error value between the current master axis
and slave axis
K: Current synchronous error compensation gain for Er
1. When Er < B, compensation is not performed. (K = 0)
2. When B < Er < A
Ks +K(Er - B)(Kd - Ks)
=A - B
Compensation is performed with the above gain:
3. When Er > A, compensation is performed with a gain of K = Kd.
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 698 -
21.1.3 Synchronous Establishment
Explanation
Upon power-up or after emergency stop cancellation, the machine
positions on the master axis and slave axis under axis synchronous
control are not always the same. In such a case, the synchronous
establishment function matches the machine position on the master
with that on the slave axis.
- Synchronous establishment method
The method of synchronous establishment used when synchronous
error compensation is performed differs from that used when
synchronous error is not performed.
- Synchronous establishment based on synchronous error compensation
When synchronous error compensation is performed (when bit 3
(CLP) of parameter No. 8304 for the slave axis is set to 1),
synchronous establishment is performed in the same way as
synchronous error compensation. This means that the positional
difference between the master axis and slave axis is regarded as a
synchronous error, and pulses produced by multiplying the positional
difference by a synchronous error compensation gain are output for
the slave axis. So, the parameter No. 8334 for specifying a
synchronous error compensation gain must be set before synchronous
establishment can be performed.
If the parameter No. 8333 for specifying a synchronous error
compensation zero width is set, no further synchronous establishment
is performed after the positional difference between the master axis
and slave axis becomes the zero width or below.
- Synchronous establishment based on machine coordinates
To perform synchronous establishment when synchronous error
compensation is disabled (when bit 3 (CLP) of parameter No. 8304 for
the slave axis is set to 0), enable synchronous establishment based on
machine coordinates by setting bit 7 (SOF) of parameter No. 8303 to 1.
This method of synchronous establishment outputs the machine
coordinate difference between the master axis and slave axis as
command pulses for the slave axis to establish synchronization. A
machine coordinate difference is output at a time as command pulses.
So, if the compensation value is large, the machine abruptly makes a
large movement. Taking this into consideration, set a maximum
allowable compensation value to be used for synchronous
establishment in parameter No. 8325. As a maximum allowable
compensation value, set a maximum allowable value by which the
machine may move abruptly. If a compensation value is larger than
the value set in this parameter, an alarm SV0001 is issued, and
synchronous establishment is not performed. Moreover, when
parameter No. 8325 is set to 0, synchronous establishment is not
performed.
The result of comparing the positional difference between the master
axis and slave axis with a maximum allowable compensation value for
synchronous establishment can be checked using the synchronous
establishment enable state output signal SYNOF <F0211>.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 699 -
- First synchronous establishment after power-up
Two methods of performing the first synchronous establishment after
power-up are available. One method is based on manual reference
position return operation, and the other is based on absolute position
detection.
Until this synchronous establishment is completed, synchronous error
compensation is disabled. However, a synchronous error check is
made.
- Synchronous establishment based on manual reference position return operation
When manual reference position return operation is performed along
axes under axis synchronous control, the machine is placed at the
reference position on the master axis and slave axis according to the
same sequence as for normal reference position return operation.
When synchronous error compensation is used, the synchronous error
counter is reset and synchronous error compensation is started upon
completion of reference position return along both axes.
The sequence is the same as the grid method for one axis only.
However, only the deceleration signal for the master axis is used.
When the deceleration signal is set to 0, the machine gradually stops
along the master axis and slave axis, then an FL feedrate is set.
When the deceleration signal is set to 1, the machine moves to a grid
point along each of the master axis and slave axis, then stops.
NOTE
When the grid position difference between the master axis and
slave axis is large, a reference position shift can occur,
depending on the timing of the *DEC signal set to 1. In the
example below, the shift along the slave axis is so large that
the position shifted one grid point from the actual reference
position is regarded as the reference position.
*DEC
Master axis feedrate
Master axis grid
Slave axis feedrate
Slave axis grid
A
ctual reference position
Stop at position shifted one
grid point
(Example) When the reference position on the slave axis is shifted one grid point
A
ctual reference position
In such a case, match the grid position according to Subsection
21.1.4, "Automatic Setting for Grid Position Matching."
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 700 -
- Synchronous establishment based on absolute position detection
When an absolute-position detector is used as the position detector,
the machine positions on the master axis and slave axis are found at
power-up time for automatic establish synchronization.
- Synchronous establishment after emergency stop cancellation, etc.
Synchronous establishment is also performed when servo position
control is turned on, for example, at emergency stop cancellation,
servo alarm cancellation, or servo-off cancellation time.
However, synchronous establishment is not performed at the time of
axis removal cancellation. So, synchronous establishment based on
manual reference position return operation is required as in the case of
power-up time.
- One-direction synchronous establishment
When synchronous error compensation is disabled, synchronous
establishment can be performed by setting bit 0 (SSO) of parameter
No. 8305 to 1 to move the machine in one direction along the master
axis and slave axis. The move direction depends on the reference
position setting based on bit 0 (SSA) of parameter No. 8304. When
SSA = 0, for example, the machine coordinate on the master axis or
slave axis, whichever larger, is used as the reference point. So, the
machine moves in the + direction along the axes.
When bit 1 (SSE) of parameter No. 8305 is set to 1, normal
synchronous establishment is performed instead of one-direction
synchronous establishment after an emergency stop.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 701 -
21.1.4 Automatic Setting for Grid Position Matching
Explanation
Before axis synchronous control can be performed, the reference
position on the master axis must be matched with the reference
position on the slave axis. With this function, the CNC
automatically matches the reference positions (grid positions) on the
master axis and slave axis under axis synchronous control.
[Operation procedure]
The procedure below is usable when bit 0 (ATE) of parameter No.
8303 is set to 1.
1. Set bit 1 (ATS) of parameter No. 8303 to 1.
2. Turn off the power then turn on the power.
3. Set the REF mode (or JOG mode in the case of reference position
setting without dogs) when synchronous operation is ready, and
make movements in the reference position return direction along
the master axis and slave axis.
4. The movements along the master axis and slave axis
automatically stop, and a grid difference value is set in parameter
No. 8326. At this time, bit 1 (ATS) of parameter No. 8303 is
set to 0, and the power-off request alarm PW0000 is issued.
5. Turn off the power then turn on the power again.
6. Perform normal reference position return operation.
NOTE
1 Parameter setting
When bit 1 (ATS) of parameter No. 8303 is set, bit
4 (APZ) of parameter No. 1815 and parameter No.
8326 for the master axis and slave axis are set to
0.
When the operator sets parameter No. 8326 (MDI,
G10L50), bit 0 (ATE) of parameter No. 8303 is set
to 0.
2 This function cannot be used together with the
reference position shift function.
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 702 -
21.1.5 Synchronous Error Check
Explanation
A synchronous error value is monitored at all times. If an error
exceeding a certain limit is detected, an alarm is issued and the
movement along the axis is stopped.
When synchronous error compensation is performed, a check
considering a positional deviation as well is made.
When synchronous error compensation is not performed, a
synchronous error check based on machine coordinates is made.
- Check made when synchronous error compensation is performed
When synchronous error compensation is performed, a check
considering a positional deviation is made. The actual machine
position shift considering a servo positional deviation as well is
checked. Depending on the value of a synchronous error, one of two
alarms is issued: an alarm (DS alarm) for deceleration stop, and an
alarm (SV alarm) for turning off the servo system immediately. This
check is enabled when a value other than 0 is set in the parameters
Nos. 8331 and 8332 for specifying a maximum allowable synchronous
error. When using this method of checking a synchronous error
value, disable "synchronous error check based on machine
coordinates" described later by setting parameter No. 8314 to 0.
- Synchronous error excessive alarm 1 (DS0002)
When a synchronous error exceeding the value set in parameter No.
8331 is detected, synchronous error excessive alarm 1 is issued.
When synchronous error excessive alarm 1 is issued, the motor
gradually stops. At this time, synchronous error compensation
remains enabled, so that the synchronous error is reduced by
compensation. Accordingly, as the synchronous error value becomes
smaller than the maximum allowable value, the alarm can be reset. If
the alarm cannot be reset, the synchronous error needs to be manually
corrected by selecting the correction mode described later.
- Synchronous error excessive alarm 2 (SV0002)
When a synchronous error exceeding the value set in parameter No.
8332 is detected, synchronous error excessive alarm 2 is issued.
Before synchronous establishment is performed at power-up time, a
value obtained by multiplying the value set in parameter No. 8332 by
the coefficient set in parameter No. 8330 is used for judgement.
When synchronous error excessive alarm 2 is issued, the motor
immediately stops as in the case of other servo alarms. Accordingly,
the positional difference between the master axis and slave axis
remains uncorrected, so that the alarm cannot be reset usually. In
this case, the synchronous error needs to be manually corrected by
selecting the correction mode described later.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 703 -
- Synchronous error check based on machine coordinates
When synchronous error compensation is not performed, a
synchronous error check based on machine coordinates is made.
The machine coordinate on the master axis is compared with that on
the slave axis. When the error between the machine coordinates
exceeds the value set in parameter No. 8314, the SV0005 alarm is
issued, and the motor is stopped immediately.
A check can be made even in the emergency stop, servo off, and servo
alarm states.
If a synchronous error check is made when the mode of operation is
switched between synchronous operation and normal operation with
an input signal, an error check is made even in normal operation. So,
even if the axis synchronous control selection signal (SYNCx) or the
axis synchronous control manual feed selection signal (SYNCJx) is set
to 0 by mistake during synchronous operation, damage to the machine
can be prevented.
The machine coordinates on the master axis and slave axis can be
checked using the machine coordinate match state output signal
SYNMT <F0210>.
- Synchronous error check based on a positional deviation value
The servo positional deviation value of the master axis and slave axis
is monitored during axis synchronous control. When the positional
deviation value exceeds the limit value set in parameter No. 8323, the
DS0001 alarm is issued, and the axis synchronous control positional
deviation error alarm signal <F403.0> is output.
The DS0001 alarm is issued to the master axis and slave axis.
When bit 4 (SYA) of parameter No. 8301 is set to 1, the positional
deviation limit value of the master axis and slave axis is checked even
if a servo-off occurs during axis synchronous control.
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 704 -
21.1.6 Methods of Alarm Recovery by Synchronous Error Check
Explanation
To recover from an alarm issued as a result of synchronous error
check, two methods are available. One method uses the correction
mode, and the other uses normal operation.
If the mode of operation is switched between synchronous operation
and normal operation by using an input signal, only the method using
normal operation can be used.
If synchronous operation is used at all times, only the method using
the correction mode can be used.
- Procedure for correcting a synchronous error by using the correction mode
Use this method if synchronous operation is used at all times without
using an input signal (when bit 5 (SCA) of parameter No. 8304 is set
to 1).
When the correction mode is used, synchronous error check can be
temporarily disabled, and a movement can be made along the master
axis or slave axis to correct a synchronous error.
In the correction mode, synchronous error compensation and error
check are not performed, so that an alarm DS0003 is issued as a
warning.
1. Select the correction mode, and select an axis along which a
movement is to be made by manual master axis feed. Set bit 2
(ADJ) of parameter No. 8304 of the master axis or slave axis to 1
to set the correction mode. Thus, by manual master axis feed, a
movement can be made along the axis with this parameter set to
1.
When this parameter is set to 1, the DS0003 (axis synchronous
control correction mode) alarm is issued.
2. Reset the synchronous error excessive alarm.
In this state, synchronous error compensation and error check are
not performed. Be careful.
3. Select the manual mode (jog, incremental feed, or handle).
4. While checking the synchronous error value, make a movement
along the master axis or slave axis in the direction that reduces
the error.
If one master axis has multiple slave axes, an attempt to reduce
the synchronous error of one slave axis by master axis movement
may increase the synchronous error of another slave axis, thus
disabling a movement in any direction. In such a case, by
setting bit 4 (MVB) of parameter No. 8304 to 1, a movement can
be made in a direction that increases the synchronous error.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 705 -
5. When the synchronous error is reduced to within the allowable
value for suppressing the alarm, reset the value of bit 2 (ADJ) of
parameter No. 8304 to the original value to switch from the
correction mode to the normal synchronization mode.
Synchronous error compensation and synchronous error check
are restarted.
6. Reset the correction mode alarm.
- Method of recovery using normal operation
Use this method when switching between synchronous operation and
normal operation by using an input signal.
Use the procedure below for recovery from alarm SV0005.
1. Set SYNCx/SYNCJx (with x representing a slave axis number)
to 0 to select normal operation.
2. Set a value greater than the current value in the parameter No.
8314 for specifying a maximum allowable synchronous error,
then reset the alarm.
3. Make a movement along the master axis or slave axis by using
the manual handle so that the machine coordinates of the master
axis and slave axis match to a maximum possible extent.
4. Return the value of parameter No. 8314 for specifying a
maximum allowable synchronous error to the original value.
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 706 -
21.1.7 Axis Synchronous Control Torque Difference Alarm
Explanation
If a movement made along the master axis differs from a movement
made along the slave axis during axis synchronous control, the
machine can be damaged. To prevent such damage, the torque
command difference between the two axes is observed. If the
difference is abnormal, a servo alarm SV0420 can be issued.
Kp
+
Slave axis
position
command
A
larm detection
Master axis
position
command
Position gain
Feedrate
control
Master axis
torque command
Master axis
position feedback
-
+
-
Torque command
difference
+
-
Kp
Compare absolute
value with threshold
Feedrate
control Slave axis torque
command
Slave axis
position feedback
Position gain
Fig. 21.1.7 (a) System configuration
[Method of use]
Specify the threshold parameter No. 2031 according to the procedure
below.
1. Set 0 in parameter No. 2031, and disable the torque difference
alarm detection function.
2. To check the absolute value of the torque difference between the
synchronous axes, set the parameters below. Set the same value
for the two axes placed under axis synchronous control.
Parameter No. 2115 = 0
Parameter No. 2151 is as described below.
• For the servo software 90E0 series, set it to 434 if the
setting of parameter No. 1023 is 1, 2, 5, 6, 9, 10… and
to 6578 if it is 3, 4, 7, 8, 11, 12…
• For the servo software 90D0 series, set it to 434.
3. Display the diagnostic screen by pressing the function key
then the [DGNOS] soft key.
Diagnose No. 0353 indicates the absolute value of the torque
difference between the two axes.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 707 -
4. Read the absolute torque difference value presented when normal
operation is being performed. In the threshold parameter No.
2031, set a value obtained by adding some margin to the read
absolute value.
The absolute torque difference value can be observed with the
Servo Guide Mate.
- Enabling/disabling of alarm detection
Alarm detection is enabled when the time set in parameter No. 8327
has elapsed after the servo ready signal SA <F000.6> is set to 1.
When the input signal NSYNCA <G059.7> is set to 1, alarm detection
is disabled.
SA<F000#6> 1
0
A
larm detection function Enabled
Setting of parameter No. 8327
(512 msec when this parameter is not set)
Disabled
Fig. 21.1.7 (b) Timing chart
When the servo ready signal SA <F000.6> is set to 0, torque
difference alarm detection is disabled.
NOTE
The servo axis number combination of the master
axis and slave axis synchronized with each other
must be such that an odd servo axis number is
assigned to the master axis and the next servo axis
number is assigned to the slave axis like (1,2) and
(3,4).
CAUTION
1 When making a synchronous error check, ensure
that the reference position on the master axis and
the reference position on the slave axis must be at
the same position.
2 In manual reference position return operation, the
same operation is performed along the master axis
and slave axis until a deceleration operation starts.
After a deceleration operation starts, grid detection
is performed for the master axis and slave axis
independently of each other.
3 Pitch error compensation and backlash
compensation are performed for the master axis
and slave axis independently of each other.
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 708 -
NOTE
1 During axis synchronous control, a movement based
on the reference position return check (G27), automatic
reference position return (G28), 2nd/3rd/4th reference
position return (G30), or machine coordinate system
selection (G53) command is made as described below
according to the setting of bit 7 (SRF) of parameter No.
8304.
<1> When SRF = 0, the same movement as made
along the master axis is made along the slave
axis.
<2> When SRF = 1, a movement is made along the
slave axis to the specified position independently
of a movement made along the master axis to the
specified position.
2 A command not involving a movement along an axis
such as the workpiece coordinate system setting
command (G92) and local coordinate system setting
command (G52) is set with the master axis according
to the master axis programming.
3 During synchronous operation, the axis-by-axis signals
such as for external deceleration, interlock, and
machine lock are enabled for the master axis only.
During synchronous operation, those signals for the
slave axis are ignored.
4 When switching the synchronization state in a program,
be sure to specify M codes (parameter No. 8337 and
No. 8338) for turning synchronization on and off. By
switching between the input signals SYNCx <G138>
and SYNCJx <G140> from the PMC with the M codes,
the synchronization state can be switched in the
program.
5 When controlled axis removal is performed, the
synchronization state is cancelled. When performing
controlled axis removal, perform removal for the master
axis and slave axis at the same time.
6 If a programmed command is specified for the slave
axis during synchronous operation, an alarm PS0213 is
issued.
A programmed command can be specified for the slave
axis when switching between synchronous operation
and normal operation is set to 0 (with bit 5 (SCA) of
parameter No. 8304 set to 0) to select normal
operation.
7 Axis synchronous control and PMC axis control cannot
be used at the same time.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 709 -
21.2 POLYGON TURNING (G50.2, G51.2)
Polygon turning means machining a workpiece to a polygonal figure
by rotating the workpiece and tool at a certain ratio.
Workpiece Workpiece Tool
Fig. 21.2 (a) Polygon turning
By changing conditions which are rotation ratio of workpiece and tool
and number of cutters, the workpiece can be machined to a square or
hexagon. The machining time can be reduced as compared with
polygonal figure machining using the polar coordinate interpolation.
The machined figure, however, is not exactly polygonal. Generally,
polygon turning is used for the heads of square and/or hexagon bolts
or hexagon nuts.
As the tool rotary axis, one of the following can be used:
• CNC controlled axis (servo axis)
• Second spindle (Two serial spindles are connected.)
Polygonal machining performed using a servo axis as the tool rotary
axis is referred to as polygon turning. Polygonal machining
performed using the second spindle as the tool rotary axis is referred
to as polygon turning with two spindles.
Function name Workpiece axis Tool rotary axis
Polygon turning
Spindle
(Either an analog spindle or
serial spindle is usable.
However, a detector
equivalent to a position
coder is required.)
Servo axis
Polygon turning with
two spindles
Spindle
(Serial spindle)
Spindle
(Serial spindle)
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 710 -
Explanation
A CNC controlled axis (servo axis) is assigned to the tool rotary axis.
This rotary axis of tool is called Y-axis in the following description.
As the workpiece axis (spindle), either a serial spindle or analog
spindle can be used.
The Y-axis is controlled by the G51.2 command, so that the ratio of
the rotation speeds of the spindle (previously specified by
S-command) and the tool becomes the specified ratio.
When simultaneous start is specified by G51.2, the one-rotation signal
sent from the position codes set on the spindle is detected. After
one-rotation signal detection, the Y-axis is controlled using the
rotation ratio of the spindle and Y-axis specified by P and Q. So, a
position coder needs to be attached to the spindle. This control will
be maintained until the polygon turning cancel command is executed
(G50.2). Polygon turning is cancelled by any of the following in
addition to the G50.2 command:
(1) Power off
(2) Emergency stop
(3) Servo alarm
(4) Reset (external reset signal ERS, reset/rewind signal RRW, and
RESET key on the MDI panel)
(5) Occurrence of alarms PS0217 to PS0221, PS0314, and PS05018
NOTE
1 Before polygon turning, reference position return
operation on the Y-axis needs to be specified to
determine the rotation start position of the tool.
This reference position return operation is
performed by detecting a deceleration limit as in the
case of manual reference position return operation.
(By setting bit 7 (PLZ) of parameter No. 7600,
reference position return operation can be
performed without detecting a deceleration limit.)
2 The rotation direction on the Y-axis is determined
by the sign of Q, and is not affected by the rotation
direction of the position coder.
3 Among Y-axis position indications, the indication of
a machine coordinate (MACHINE) changes within
the amount of movement for 0 to 1 revolution as a
movement is made on the Y-axis. The absolute
coordinate and relative coordinate are not updated.
So, when specifying an absolute-position command
for the Y-axis after polygon turning mode
cancellation, set a workpiece coordinate system
after reference position return operation.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 711 -
NOTE
4 For the Y-axis engaged in polygon turning, jog feed
and handle feed are disabled.
5 For the Y-axis not engaged in polygon turning, a
move command can be specified as in the case of
other controlled axes.
6 The Y-axis engaged in polygon turning is not
counted in the number of simultaneously controlled
axes.
7 One workpiece must be machined using a fixed
spindle speed until the workpiece is finished.
8 Polygon turning with two spindles cannot be used at
the same time.
9 G50.2 is the G code for suppressing buffering.
CAUTION
1 During polygon turning, threading cannot be
performed.
2 For the Y-axis engaged in synchronous operation,
the signals below are valid or invalid:
Signals valid for the Y-axis
• Machine lock
• Servo-off
Signals invalid for the Y-axis
• Feed hold
• Interlock
• Override
• Dry run
(At dry run time, however, the one-rotation
signal is not awaited in a G51.2 block.)
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 712 -
Format
G50.2 Polygon turning cancel
G51.2 P_ Q_ ;
P,Q: Rotation ratio of spindle and Y-axis
Specify range:
P: Integer from 1 to 999
Q: Integer from -999 to -1 or from 1 to 999
When Q is a positive value, Y-axis makes positive
rotation.
When Q is a negative value, Y-axis makes
negative rotation.
NOTE
Specify G50.2 and G51.2 in a single block.
Example
G00 X100. 0 Z20.0 S1000.0 M03 ;
(Workpiece rotation speed 1000 (min-1))
G51.2 P1 Q2 ; (Tool rotation start (tool rotation speed
2000 (min-1))
G01 X80.0 F10.0 ; (X-axis infeed)
G04 X2.0 ; (Waiting 2 seconds)
G00 X100.0 ; (X-axis escape)
G50.2 ; (Tool rotation stop)
M05 S0 ; (Spindle stop )
- Principle of polygon turning
The principle of polygon turning is explained below. In the figure
below the radius of tool and workpiece are A and B, and the angular
speeds of tool and workpiece are α and β. The origin of XY
Cartesian coordinates is assumed to be the center of the workpiece.
Simplifying the explanation, consider that the tool center exists at the
position
Po (A, 0) on the workpiece periphery, and the tool nose starts from
position Pto (A-B, 0).
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 713 -
Y
X
A
(0,0)
Pto
Po
B
A
ngular speed
α
A
: Workpiece radius
B : Rool radius
A
ngular
speed β Workpiece
Tool
α : Workpiece angular speed
β : Tool angular speed
Po (A, 0)
Pto (A-B, 0)
Fig. 21.2 (b) Principle of polygon turning
(0, 0)
α
t
β
t
A
P
Start point
B
Pt (Xt, Yt)
Fig. 21.2 (c) Tool nose position
In this case, the tool nose position Pt (Xt, Yt) after time t is expressed
by equations 1 and 2:
Xt=Acos
α
t-Bcos(
β
-
α
)t (Equation 1)
Yt=Asin
α
t+Bsin(
β
-
α
)t (Equation 2)
Assuming that the rotation ration of workpiece to tool is 1:2, namely,
β=2α, equations 1 and 2 are modified as follows:
Xt=Acos
α
t-Bcos
α
t=(A-B)cos
α
t (Equation 1)'
Xt=Asin
α
t+Bsin
α
t=(A+B)sin
α
t (Equation 2)'
These equations indicate that the tool nose path draws an ellipse with
longer diameter A+B and shorter diameter A-B.
Then consider the case when one tool is set at 180° symmetrical
positions, for a total of two. A square can be machined with these
tools as shown below.
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 714 -
If three tools are set at every 120°, the machining figure will be a
hexagon as shown below.
WARNING
For the maximum rotation speed of the tool, see
the instruction manual supplied with the machine.
Do not specify a spindle speed higher than the
maximum tool speed or a ratio to the spindle speed
that results in a speed higher than the maximum
tool speed.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 715 -
21.3 SYNCHRONOUS, COMPOSITE AND SUPERIMPOSED
CONTROL BY PROGRAM COMMAND (G50.4, G51.4,
G50.5, G51.5, G50.6, AND G51.6)
Synchronous control, composite control, and superimposed control
can be started or canceled using a program command instead of a DI
signal. Synchronous control, composite control, and superimposed
control based on a DI signal is also possible.
For the basic operations of synchronous control, composite control,
and superimposed control, see Section 8.5, "SYNCHRONOUS
CONTROL AND COMPOSITE CONTROL", and Section 8.6,
"SUPERIMPOSED CONTROL" in the CONNECTION MANUAL
(FUNCTION) (B-63943EN-1).
Format
G51.4 P_ Q_ (L_) ; Synchronous control start (L is omissible.)
G50.4 Q_ ; Synchronous control cancel
P: Synchronous master axis ID number
Q: Synchronous slave axis ID number
L: Parking command
1: Master parking (slave parking cancel)
2: Slave parking (master parking cancel)
0: No parking (parking cancel)
(When L is omitted, the specification of L0 is assumed.)
G51.5 P_ Q_ ; Composite control start
G50.5 P_ Q_ ; Composite control cancel
P: Composite axis 1 ID number
Q: Composite axis 2 ID number
G51.6 P_ Q_ ; Superimposed control start
G50.6 Q_ ; Superimposed control cancel
P: Superimposed master axis ID number
Q: Superimposed slave axis ID number
As an ID number, set a unique value for identifying each axis in parameter
No. 12600 for both of P and Q.
G51.4/G50.4, G51.5/G50.5, and G51.6/G50.6 are one-shot G codes of
group 00.
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 716 -
Explanation
Synchronous control
Synchronous control is performed with the G51.4/G50.4 commands,
instead of simultaneously controlled axis selection signals.
Parameter setting examples for a 3-path system
• Parameter No.12600
Path 1 Path 2 Path 3
X 101 201 301
Z 102 202 302
• Parameter No.8180
Path 1 Path 2 Path 3
X 0 0 0
Z 0 102 102
• Program example (M100 to M103 are synchronization M codes.)
Path 1 Path 2 Path 3 Operation
N10 M100 P123 ; M100 P123 ; M100 P123 ; Synchronization between paths 1, 2, and 3
N20 G51.4 P102 Q202 ;
N30 G51.4 P102 Q302 ;
Start of Z1-Z2 synchronous control
Start of Z1-Z3 synchronous control
N40 M101 P123 ; M101 P123 ; M101 P123 ; Synchronization between paths 1, 2, and 3
N50 G00 Z100.; Synchronous
slave movement
Synchronous
slave movement
Z1-Z2 and Z1-Z3 synchronous control
N60 M102 P123 ; M102 P123 ; M102 P123 ; Synchronization between paths 1, 2, and 3
N70 G50.4 Q202 ;
N80 G50.4 Q302 ;
Cancellation of Z1-Z2 synchronous control
Cancellation of Z1-Z3 synchronous control
N90 M103 P123 ; M103 P123 ; M103 P123 ; Synchronization between paths 1, 2, and 3
- Start of synchronous control
N20 G51.4 P102 Q202 : Start of synchronous control with the Z1-axis
being a master axis and the Z2-axis being a slave axis
N30 G51.4 P102 Q302 : Start of synchronous control with the Z1-axis
being a master axis and the Z3-axis being a slave axis
- Cancellation of synchronous control
N70 G50.4 Q202 : Cancellation of synchronous control with the
Z1-axis being a master axis and the Z2-axis being a slave axis
N80 G50.4 Q302 : Cancellation of synchronous control with the
Z1-axis being a master axis and the Z3-axis being a slave axis
- Parking
Use the L command to specify the start and cancellation of the parking
of synchronous axes.
If the L command is omitted or if the L0 command is issued, the
parking of both synchronous master axis and synchronous slave axis is
canceled.
- Parameter check
If the axis number corresponding to the P specified with G51.4 is not
set in slave axis parameter No. 8180, alarm PS5339 is issued.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 717 -
Composite control
Composite control is performed with the G51.5/G50.5 commands,
instead of composite control axis selection signals.
Parameter setting examples for a 3-path system
• Parameter No.12600
Path 1 Path 2 Path 3
X 101 201 301
Z 102 202 302
• Parameter No.8183
Path 1 Path 2 Path 3
X 0 101 0
Z 0 102 0
• Program example (M100 to M103 are synchronization M codes.)
Path 1 Path 2 Path 3 Operation
N10 M100 P12 ; M100 P12 ; Synchronization between paths 1 and 2
N20 G51.5 P101 Q201 ;
N30 G51.5 P102 Q202 ;
Start of X1-X2 composite control
Start of Z1-Z2 composite control
N40 M101 P12 ; M101 P12 ; Synchronization between paths 1 and 2
N50 G00 X 100. Z100.; Composite
movement
X1-X2 and Z1-Z2 composite control
N60 M102 P12 ; M102 P12 ; Synchronization between paths 1 and 2
N70 G50.5 P101 Q201 ;
N80 G50.5 P102 Q202 ;
Cancellation of X1-X2 composite control
Cancellation of Z1-Z2 composite control
N90 M103 P12 ; M103 P12 ;
Independent
operation
Synchronization between paths 1 and 2
- Start of composite control
N20 G51.5 P101 Q201 : Start of composite control on the X1- and
X2-axes
N30 G51.5 P102 Q202 : Start of composite control on the Z1- and
Z2-axes
- Cancellation of composite control
N70 G50.5 P101 Q201 : Cancellation of composite control on the X1-
and X2-axes
N80 G50.5 P102 Q202 : Cancellation of composite control on the Z1-
and Z2-axes
- Parameter check
If the composite control axis corresponding to the P or Q specified
with G51.5/G50.5 is not set in parameter No. 8183, alarm PS5339 is
issued.
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 718 -
Superimposed control
Superimposed control is performed with the G51.6/G50.6 commands,
instead of superimposed control axis selection signals.
Parameter setting examples for a 3-path system
• Parameter No.12600
Path 1 Path 2 Path 3
X 101 201 301
Z 102 202 302
• Parameter No.8186
Path 1 Path 2 Path 3
X 0 0 0
Z 0 0 102
• Program example (M100 to M103 are synchronization M codes.)
Path 1 Path 2 Path 3 Operation
N10 M100 P13 ; M100 P13 ; Synchronization between paths 1 and 3
N20 G51.6 P102 Q302 ; Start of Z1-Z3 superimposed control
N30 M101 P13 ; M101 P13 ; Synchronization between paths 1 and 3
N40 G00 Z100.; G00 Z-200.;
Z1-Z3 superimposed control
(Z+100 superimposed on Z3)
N50 M102 P13 ; M102 P13 ; Synchronization between paths 1 and 3
N60 G50.6 Q302 ; Cancellation of Z1-Z3 superimposed control
N70 M103 P13 ;
Independent
operation
M103 P13 ; Synchronization between paths 1 and 3
- Start of superimposed control
N20 G51.6 P102 Q302 : Start of superimposed control with the
Z1-axis being a master axis and the Z3-axis being a slave axis
- Cancellation of superimposed control
N60 G50.6 Q302 : Cancellation of superimposed control with the
Z1-axis being a master axis and the Z3-axis being a slave axis
- Parameter check
If the axis number corresponding to the P specified with G51.6 is not
set in superimposed slave axis parameter No. 8186, alarm PS5339 is
issued.
NOTE
1 If G codes (G50.4/G50.5/G50.6) for canceling synchronous,
composite, and superimposed control with program commands
are issued for axes under synchronous, composite, and
superimposed control with DI signals, synchronous, composite,
and superimposed control is canceled.
2 If the synchronous control axis selection signal, composite
control axis selection signal, and superimposed control axis
selection signal are changed from '1' to '0' for axes under
synchronous, composite, and superimposed control with
program commands, synchronous, composite, and
superimposed control is canceled.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 719 -
21.4 ROTARY AXIS ROLL-OVER
The roll-over function prevents coordinates for the rotary axis from
overflowing. The roll-over function is enabled by setting bit 0 (ROAx)
of parameter No. 1008 to 1.
21.4.1 Rotary Axis Roll-over
Explanation
For an incremental programming, the tool moves the angle specified
in the command. For an absolute programming, the coordinates after
the tool has moved are values set in parameter No. 1260, and rounded
by the angle corresponding to one rotation. The tool moves in the
direction in which the final coordinates are closest when bit 1 (RABx)
of parameter No. 1008 is set to 0. Displayed values for relative
coordinates are also rounded by the angle corresponding to one
rotation when bit 2 (RRLx) of parameter No. 1008 is set to 1.
Example
Assume that axis A is the rotary axis and that the amount of
movement per rotation is 360.000 (parameter No. 1260 = 360000).
When the following program is executed using the roll-over function
of the rotary axis, the axis moves as shown below.
G90 A0 ;
Sequence
number
Actual
movement value
Absolute coordinate
value after
movement end
N1 G90 A-150.0 ; N1 -150 210
N2 G90 A540.0 ; N2 -30 180
N3 G90 A-620.0 ; N3 -80 100
N4 G91 A380.0 ; N4 +380 120
N5 G91 A-840.0 ; N5 -840 0
Relative
coordinate value
A
bsolute
coordinate value
-720°
-0°
-360°
-0°-0°
-0°360°
-0°
N1
N2
N3
N4
N5
210° (Absolute)
180°
100°
120°
M
NOTE
This function cannot be used together with the
index table indexing function.
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 720 -
21.4.2 Rotary Axis Control
This function controls a rotary axis as specified by an absolute
command.
With this function, the sign of the value specified in the command is
interpreted as the direction of rotation, and the absolute value of the
specified value is interpreted as the coordinates of the target end
position.
Explanation
This function is valid when rotary axis roll-over is enabled (bit 0
(ROAx) of parameter No. 1008 is set to 1).
If bit 3 (RAAx) of parameter No.1007 is set to 1, an absolute
command specified for the roll-over rotary axis is interpreted as
follows: The sign and absolute value of the value specified in the
command represent the direction of rotation and the end position of
movement respectively.
If bit 3 (RAAx) of parameter No.1007 is set to 0, the setting by bit 1
(RABx) of parameter No.1008 becomes significant.
NOTE
1 This function can be used only when the
corresponding option is provided. (When a
machining center system is used, this function
cannot be used together with the index table
indexing function.)
2 This function is valid for a roll-over rotary axis.
3 If bit 3 (RAAx) of parameter No.1007 is set to 1, bit
1 (RABx) of parameter No.1008 is ignored. To
select a rotary motion of a shorter travel distance,
set both RAAx and RABx to 0.
4 This function is not supported when the machine
coordinate system of the PMC axis control function
is selected.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 721 -
21.5 ARBITRARY ANGULAR AXIS CONTROL
Overview
When the angular axis installed makes an angle other than 90° with
the perpendicular axis, the Arbitrary angular axis control function
controls the distance traveled along each axis according to the
inclination angle as in the case where the angular axis makes 90° with
the perpendicular axis.
Arbitrary axes can be specified as a set of an angular axis and
perpendicular axis by parameter setting.
The actual distance traveled is controlled according to an inclination
angle. However, a program, when created, assumes that the angular
axis and perpendicular axis intersect at right angles. The coordinate
system used at this time is referred to as the program coordinate
system. (The program coordinate system may be referred to as the
Cartesian coordinate system, and the actual move coordinate system
may be referred to as the angular coordinate system or machine
coordinate system.)
θ
+Y'(Hypothetical axis)
+Y'(Angular axis)
θ: Inclination angle
+X(Perpendicular axis)
Program coordinate system
(Cartesian coordinates)
Machine coordinate system
(Angular coordinates)
+Y'
+
X
+
X
+Y
Fig. 21.5 (a)
Explanation
When the amounts of travel along the angular axis and the
perpendicular axis are Ya and Xa, respectively, the amounts are
controlled according to the formulas shown below.
Ya = Yp
cos
θ
Xa,Ya: Actual distance
Xp,Yp: Programmed distance
The amount of travel along the perpendicular axis is corrected by the
influence of travel along the angular axis, and is determined by the
following formula:
Xa = Xp – C × Yp × tan
θ
NOTE
The coefficient C is 2 in the case of diameter
specification for the perpendicular axis (X) or 1 in
the case of radius specification.
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 722 -
+Y (Angular axis)
+Y' (Hypothetical axis)
θ
Yp tan
θ
(perpendicular axis
component produced by
travel along the angular axis)
Xp and Yp
Xa and Ya
A
ctual tool travel
+X (Perpendicular axis)
Fig. 21.5 (b)
- Feedrate
When the Y-axis is an angular axis, and the X-axis is a perpendicular
axis, the feedrate along each axis is controlled as described below so
that the feedrate in the tangent direction becomes Fp.
The feedrate component along the Y-axis is determined by the
following expressions:
Fay = Fp
cos
θ
Fa represents the actual feedrate.
Fp represents a programmed feedrate.
Fax = Fp – Fp × tan
θ
- Absolute and relative position display
An absolute and a relative position are indicated in the programmed
Cartesian coordinate system.
- Machine position display
A machine position indication is provided in the machine coordinate
system where an actual movement is taking place according to an
inclination angle.
Method of use
The angular and perpendicular axes for which arbitrary angular axis
control is to be applied must be specified beforehand, using
parameters Nos. 8211 and 8212. When 0 is set in one of the
parameters, the same number is specified in the parameters, or a
number other than the controlled axis numbers is specified in a
parameter, however, an angular axis and perpendicular axis are
selected according to the table below.
Angular axis Perpendicular axis
M series
Y-axis of the basic three axes
(axis with 2 set in parameter
No. 1022)
Z-axis of the basic three axes
(axis with 3 set in parameter
No. 1022)
T series
X-axis of the basic three axes
(axis with 1 set in parameter
No. 1022)
Z-axis of the basic three axes
(axis with 3 set in parameter
No. 1022)
• Bit 0 (AAC) of parameter No. 8200 enables or disables the
arbitrary angular axis control. If the function is enabled, the
distance traveled along each axis is controlled according to an
angular angle parameter No. 8210.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 723 -
• By using bit 2 (AZR) of parameter No. 8200, whether to make a
movement along the perpendicular axis by a movement made along
the angular axis when a manual reference position return operation
is performed along the angular axis can be chosen. When a
movement along the perpendicular axis is enabled (AZR = 1), a
reference position return operation along the perpendicular axis can
be performed by a movement made along the angular axis.
• By setting the normal axis/angular axis control invalid signal
NOZAGC to 1, angular axis control only for the angular axis can
be available. In this time the angular axis are converted to those
along the angular coordinate system without affecting commands
to normal axis.
Use this signal when operating each axis independently.
- Manual reference position return operation
A movement is made to the reference position (machine position) set
in parameter No. 1240. By using bit 2 (AZR) of parameter No. 8200,
whether to make a movement along the perpendicular axis when a
reference position return operation is performed along the angular axis
can be chosen.
- Automatic reference position return operation and floating reference position
return operation (G28, G30, G30.1)
A movement to the middle point along the angular axis affects a
movement along the perpendicular axis. As a movement from the
middle point to the reference position along the angular axis, a
selection can be made with bit 0 (ARF) of parameter No. 8209
between a Cartesian coordinate system operation (FS16i
compatibility) and an angular coordinate system operation. If manual
reference position return operation is not performed even once after
the power is turned on, operation is performed in the same sequence as
for manual reference position return operation. So, specify
commands first for the angular axis then for the perpendicular axis.
Example 1)
When the Y-axis is an angular axis and the X-axis is a
perpendicular axis
(1) If the angular axis is first specified then the perpendicular
axis is specified, reference position return operation is
performed normally.
G28Y_;
G28X_;
(2) If the perpendicular axis is first specified then the angular
axis is specified, or if the perpendicular axis and the angular
axis are specified at the same time, alarm PS0372 is issued
when a movement is made along the perpendicular axis.
G28X_; or G28X_ Y_;
G28Y_;
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 724 -
Example 2)
Automatic reference position return examples
(If the Y-axis is an angular axis, the X-axis is a perpendicular
axis, and the inclination angle is -30°)
<1> Command for automatic reference position return along the
Y-axis from point P2
>G91G28X200.
<2> Command for automatic reference position return along the
X-axis from point P1
>G91G28Y100.
(1) If bit 0 (ARF) of parameter No. 8209 is 1 (FS16i
compatibility)
<1> Coordinates of P1
(Absolute coordinates) (Machine coordinates)
X 0.000 X 57.735
Y 100.000 Y 115.470
<2> Coordinates of P0
(Absolute coordinates) (Machine coordinates)
X 0.000 X 0.000
Y 0.000 Y 0.000
30°
+X
(Perpendicular
axis)
+Y' (Hypothetical axis)
+Y (Angular axis)
P1
P0(0,0)
P2
257.735 200 57.735
115.470
(2) If bit 0 (ARF) of parameter No. 8209 is 0
<1> Coordinates of P1
(Absolute coordinates) (Machine coordinates)
X 0.000 X 0.000
Y 100.000 Y 115.470
<2> Coordinates of P0
(Absolute coordinates) (Machine coordinates)
X 0.000 X 0.000
Y 0.000 Y 0.000
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 725 -
30°
+X(Perpendicular
axis)
+Y’(Hypothetical axis)
+Y(Angular axis)
P1
P0(0,0)
P2
200
115.470
- Reference position return operation of high-speed type
When a reference position is already established and a reference
position return operation of high-speed type is to be performed, the
reference position return operation need not be performed in the order
from the angular axis to the perpendicular axis.
- Machine coordinate selection (G53)
By specifying (G90)G53X_Y_: (when the Y-axis is an angular axis,
the X-axis is a perpendicular axis, and the inclination angle is -30°), a
movement is made by rapid traverse.
However, a movement along the angular axis (G53 command) does
not affect a movement along the perpendicular axis, regardless of
whether the perpendicular axis/angular axis control disable signal
(NOZAGC) is turned on or off.
Example)
1 Move command for movement from point P0 to point P1
>G90G53Y100.
2 Move command for movement from point P1 to point P2
>G90G53X200.
<1> Coordinates of P1
(Absolute coordinates) (Machine coordinates)
X -50.000 X 0.000
Y 86.603 Y 100.000
<2> Coordinates of P2
(Absolute coordinates) (Machine coordinates)
X 150.000 X 200.000
Y 86.603 Y 100.000
+Y (Angular axis) +Y' (Hypothetical axis)
P1(0,100) P2(200,100)
+X
(Perpendicular
axis)
P0(0,0)
30°
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 726 -
- Commands for linear interpolation and linear interpolation type positioning (G01,
G00)
The tool moves to a specified position in the Cartesian coordinate
system when the following is specified:
(G90)G00X_Y_; (when the Y-axis is an angular axis, the X-axis is a
perpendicular axis, and the inclination angle is -30°)
or
(G90)G01X_Y_F_; (when the Y-axis is an angular axis, the X-axis is
a perpendicular axis, and the inclination angle is -30°)
Example) Examples of positioning
1 Move command for movement from point P0 to point P1
>G90G00Y100.
2 Move command for movement from P1 to P2
G90G00X200.
(1) When the perpendicular axis/angular axis control disable
signal (NOZAGC) is set to 0
<1> Coordinates of P1
(Absolute coordinates) (Machine coordinates)
X 0.000 X 57.735
Y 100.000 Y 115.470
<2> Coordinates of P2
(Absolute coordinates) (Machine coordinates)
X 200.000 X 257.735
Y 100.000 Y 115.470
30°
+Y (Angular axis)
P1
P0(0,0)
P2
257.73520057.735
115.470
+Y' (Hypothetical axis)
+X (Perpen-
dicular axis)
(2) When the perpendicular axis/angular axis control disable
signal (NOZAGC) is set to 1
<1> Coordinates of P1
(Absolute coordinates) (Machine coordinates)
X 0.000 X 0.000
Y 100.000 Y 115.470
<2> Coordinates of P2
(Absolute coordinates) (Machine coordinates)
X 200.000 X 200.000
Y 100.000 Y 115.470
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 727 -
30°
P1
P0(0,0)
P2
200
115.470
+Y (Angular axis) +Y' (Hypothetical axis)
+X (Perpendicular
axis)
- Three-dimensional coordinate conversion
In the three-dimensional coordinate conversion mode, angular
coordinate system conversion is applied to the workpiece coordinate
system that has undergone three-dimensional coordinate conversion.
- Stored stroke limit
Stored stroke limits under arbitrary angular axis control can be set not
in a angular coordinate system but in the Cartesian coordinate system
by setting bits 0, 1, and 2 (AOT, AO2, and AO3) of parameter No.
8201.
X
YY'
X
Y
Y'
Fig. 21.5 (c) OT area in a angular coordinate system Fig. 21.5 (d) OT area in a Cartesian coordinate system
Machine coordinates include a value converted for the angular axis
and a compensation value for the perpendicular axis, so that a angular
machine coordinate system as shown in Fig. 21.5 (c) results.
A stored stroke limit is checked in the machine coordinate system, so
that the limit area is slanted to form a rhombus as shown in Fig. 21.5
(c). In this case, the area cannot be identified intuitively. So, stroke
limits are checked not in an actual angular machine coordinate system
but in a virtual Cartesian machine coordinate system as shown in Fig.
21.5 (d).
The functions that operate in the Cartesian coordinate system are:
• Stored stroke check 1 (Both of I and II)
• Stored stroke check 2 (G22/G23)
• Stored stroke check 3
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 728 -
• Stored stroke check before move
The stored stroke check function before move does not work in a
angular coordinate system. Unless this function is enabled, and the
coordinate system is converted to the Cartesian coordinate system, no
stroke check is made.
• Stroke limit external setting (function specific to the M series only
and valid only for OT1)
• Bit 7 (BFA) of parameter No. 1300 for specifying whether to issue
an alarm before or after a stroke limit is exceeded (valid for OT1
and OT3)
The stored stroke limit functions other than the above work in a
angular coordinate system.
- Relationships between this function and axis-by-axis input/output signals
The table below indicates the relationships between this function and
the meaning of each controlled axis signal.
The input/output signals are classified as signals valid for the program
coordinate system (Cartesian coordinate system) and signals valid for
the machine coordinate system (angular coordinate system). In the
"Classification" column, "Cartesian" is indicated for a signal that is
valid for the Cartesian coordinate system, and "Angular" is indicated
for a signal that is valid for the angular coordinate system.
A signal valid for the Cartesian coordinate system means a signal
valid for a specified axis, and a signal valid for the angular coordinate
system is a signal valid for actual machine movement.
This means that when a movement is made along the perpendicular
axis by a movement along the angular axis alone:
A signal valid for the Cartesian coordinate system is affected by
a movement along the angular axis.
A signal valid for the angular coordinate system is not affected
by a movement along the angular axis.
Input signal
Signal name Address Classification Remarks
Interlock for each axis *ITx G130 Cartesian
When a movement is made along the angular axis
only, interlocking the perpendicular axis does not
interlock a movement along the perpendicular axis
made by a movement along the angular axis.
Caution) When using the interlock signal for each
axis, make both of the angular axis and
perpendicular axis high.
Overtravel *+Lx
*-Lx
G114
G116 Angular
This signal is applied to each axis independently.
(If the perpendicular axis is made high, no alarm is
issued for the perpendicular axis even when an OT
alarm is issued for the angular axis.)
Deceleration signal for
reference position return *DECx X009 Angular This signal is applied to each axis independently.
Servo-off signal SVFx G126 Angular This signal is applied to each axis independently.
Control axis detach signal DTCHx G124 Angular This signal is applied to each axis independently.
Feed axis direction
selection signal
+Jx
-Jx
G100
G102 Cartesian
A movement is made in the Cartesian coordinate
system. (When the +J/-J signal for the angular
axis is made high, a movement is made also along
the perpendicular axis.)
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 729 -
Input signal
Signal name Address Classification Remarks
Mirror image MIx G106 Angular
Mirror image is applied to the angular coordinate
system for each axis independently.
Caution) Be sure to turn off the mirror image
signal for the angular axis and
perpendicular axis engaged in manual
operation.
Manual feed interlock
signal for each axis
direction, tool
compensation value write
signal
+MIT1,
+MIT2
X004.2,
4 Cartesian Set the tool compensation parameter in the
Cartesian coordinate system.
Machine lock for each
axis MLKx G108 Angular This signal is applied to each axis independently.
Output signal
Signal name Address Classification Remarks
In-position signal INPx F104 Angular Applied to each axis independently.
Mirror image check signal MMIx F108 Angular Applied to each axis independently.
Controlled axis removal
in-progress signal
MDTC
Hx F110 Angular Applied to each axis independently.
Travel in-progress signal MVx F102 Angular Applied to each axis independently.
Reference position return
completion signal ZPx F094 Cartesian
Applied to each axis independently. (A manual
reference position return operation and the first
automatic reference position return operation after
power-up need to be performed first for the angular
axis.)
2nd reference position
return completion signal ZP2x F096 Cartesian Applied to each axis independently.
3rd reference position
return completion signal ZP3x F098 Cartesian Applied to each axis independently.
4th reference position
return completion signal ZP4x F100 Cartesian Applied to each axis independently.
Limitation
- Three-dimensional coordinate conversion
If the basic three axes in the three-dimensional coordinate conversion
mode do no include a perpendicular axis and angular axis for arbitrary
angular axis control, operation cannot be performed normally in a
correct angular coordinate system.
- Linear scale with absolute address reference mark
• For both of the angular axis and perpendicular axis, a linear scale
with an absolute address reference mark must be used.
• Reference position return operation must be first completed along
the angular axis.
• Return operation cannot be performed along the perpendicular axis
while return operation is being performed along the angular axis.
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 730 -
- Synchronous control
For synchronous control on axes related to arbitrary angular axis
control, the angular axis and Cartesian axis on the master axis side and
the angular axis and Cartesian axis on the slave axis side must be
placed under synchronous control at the same time. Moreover,
synchronous control can be exercised between angular axes only or
between Cartesian axes only.
If an attempt is made to perform operation under a condition other
than the above, the alarm PS0375 is issued.
Example)
Path 1 Path 2
X1 (Cartesian axis) ←Synchronous→ X2 (Cartesian axis)
Y1 (angular axis) ←Synchronous→ Y2 (angular axis)
- Composite control
For composite control on axes related to arbitrary angular axis control,
the angular axis and Cartesian axis on the master axis side and the
angular axis and Cartesian axis on the slave axis side must be placed
under composite control at the same time. Moreover, composite
control can be exercised between angular axes only or between
Cartesian axes only.
If an attempt is made to perform operation under a condition other
than the above, the alarm PS0375 is issued.
Example)
Path 1 Path 2
X1 (Cartesian axis) ←composite→ X2 (Cartesian axis)
Y1 (angular axis) ←composite→ Y2 (angular axis)
- Rigid tapping
As a rigid tapping axis, no angular axis can be used.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 731 -
- Functions that cannot be used simultaneously
• Axis synchronous control, twin table control, parallel axis control,
polygon turning, rigid tapping, hypothetical axis control, EGB
function, PMC axis control, superimposed control
CAUTION
1 After arbitrary angular axis control parameter setting,
be sure to perform manual reference position return
operation.
2 Before manual reference position return operation is
performed along the perpendicular axis, reference
position return operation along the angular axis must
be completed (with the reference position return
completion signal for the angular axis (ZPx) set to 1).
If reference position return operation is performed
along the perpendicular axis first, an alarm PS0372 is
issued.
3 When the setting is made so that the tool moves
along the perpendicular axis during manual reference
position return along the angular axis (bit 2 (AZK) of
parameter No. 8200 is set to 0), if once manual
reference position return has been performed along
the angular axis, also perform manual reference
position return along the perpendicular axis
immediately after the operation.
4 Before attempting to manually move the tool along the
angular and perpendicular axes simultaneously, set
perpendicular/angular axis control disable signal
NOZAGC to 1.
5 Once the tool has been moved along the angular axis
when perpendicular/angular axis control disable signal
NOZAGC has been set to 1, manual reference
position return must be performed.
6 The same increment system must be used with the
angular axis and perpendicular axis.
7 Before a perpendicular axis reference position return
check can be made, angular axis reference position
return operation must be completed.
8 No rotary axis must be set for the angular axis and
perpendicular axis. A rotary axis may be specified
only for a linear axis.
9 Set a position switch operation range (parameter Nos.
6930 to 6965) in a angular coordinate system.
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 732 -
21.6 TOOL RETRACT AND RECOVER
Overview
To replace the tool damaged during machining or to check the status
of machining, the tool can be withdrawn from a workpiece. The tool
can then be advanced again to restart machining efficiently.
The tool retract and recover operation consists of the following four
steps:
• Retract
The tool is retracted to a predefined position using the TOOL
WITHDRAW switch.
• Withdrawal
The tool is moved to the tool-change position manually.
• Return
The tool returns to the retract position.
• Repositioning
The tool returns to the interrupted position.
For the tool retract and recover operations, see “Tool retract and
recover ” in the Part III.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 733 -
: Position at which tool retract switch is turned on
: Programmed position
: Position at which tool is retracted by manual operation
: Retract path
: Manual operation (retract path)
: Return path
: Re-positioning
X
Y
Z
Z
X
Format
Specify a retraction axis and distance in the following format:
Specify the amount of retraction, using G10.6.
G10.6 IP_ ;
IP: In incremental mode, retraction distance from the
position where the retract signal is turned on
In the absolute mode, retraction distance to an absolute
position
The specified amount of retraction is effective until G10.6
is next executed. To cancel the retraction, specify the
following:
G10.6 ; (as a single block containing no other commands)
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 734 -
Explanation
- Retraction
When the TOOL WITHDRAW switch on the machine operator's
panel is turned on during automatic operation or in the automatic
operation stop or hold state, the tool is retracted the length of the
programmed retraction distance. This operation is called retraction.
The position at which retraction is completed is called the retraction
position. The tool is retracted to the retraction position in linear
interpolation at the dry run feedrate. When retraction is completed,
the RETRACTIONS POSITION LED on the machine operator’s
panel goes on.
When the TOOL WITHDRAW switch is turned on during execution
of a block in automatic operation, execution of the block is interrupted
immediately and the tool is retracted. After retraction is completed,
the system enters the automatic operation hold state.
If the retraction distance and direction are not programmed, retraction
is not performed. In this state, the tool can be withdrawn and
returned.
When the TOOL WITHDRAW switch is turned on in the automatic
operation stop or hold state, the tool is retracted, then the automatic
operation stop or hold state is entered again.
When the TOOL WITHDRAW switch is turned on, the tool withdraw
mode is set. When the tool withdraw mode is set, the TOOL BEING
WITHDRAWN LED on the machine operator's panel goes on.
- Withdrawal
When the manual mode is set, the tool can be moved manually (jog
feed, incremental feed, handle feed, or manual numeral command) to
replace the tool or measure a machined workpiece. This operation is
called a withdrawal. The tool withdrawal path is automatically
memorized by the CNC.
- Return
When the mode is returned to automatic operation mode and the
TOOL RETURN switch on the machine operator's panel is turned off,
the CNC automatically moves the tool to the retraction position by
tracing the manually-moved tool path backwards. This operation is
called a return. Upon completion of a return to the retraction
position, the RETRACTIONS POSITION LED comes on.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 735 -
- Repositioning
When the cycle start button is pressed while the tool is in the
retraction position, the tool moves to the position where the TOOL
WITHDRAW switch was turned on. This operation is called
repositioning. Upon completion of repositioning, the TOOL BEING
WITHDRAWN LED is turned off, indicating that the tool withdrawal
mode has terminated. Operation after completion of repositioning
depends on the automatic operation state when the tool withdrawal
mode is set.
(1) When the tool withdrawal mode is set during automatic operation,
operation is resumed after completion of repositioning.
(2) When the tool withdrawal mode is set when automatic operation
is held or stopped, the original automatic operation hold or stop
state is set after completion of repositioning. When the cycle
start button is pressed again, automatic operation is resumed.
Limitation
- Offset
If the origin, presetting, or workpiece origin offset value (or External
workpiece origin offset value) is changed after retraction is specified
with G10.6 in absolute mode, the change is not reflected in the
retraction position. After such changes are made, the retraction
position must be respecified with G10.6.
When the tool is damaged, automatic operation can be interrupted
with a tool withdrawal and return operation in order to replace the tool.
Note that if the tool offset value is changed after tool replacement, the
change is ignored when automatic operation is resumed from the start
point or other point in the interrupted block.
- Machine lock, mirror image, and scaling
When withdrawing the tool manually in the tool withdrawal mode,
never use the machine lock, mirror-image, or scaling function.
- Reset
Upon reset, the retraction data specified in G10.6 is cleared.
Retraction data needs to be specified again.
- Retraction command
The tool withdrawal and return function is enabled even when the
retraction command is not specified. In this case, retraction and
repositioning are not performed.
WARNING
The retraction axis and retraction distance
specified in G10.6 need to be changed in an
appropriate block according to the figure being
machined. Be very careful when specifying the
retraction distance; an incorrect retraction distance
may damage the workpiece, machine, or tool.
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 736 -
21.7 ELECTRONIC GEAR BOX
21.7.1 Electronic Gear Box
Overview
This function enables fabrication of high-precision gears, screws, and
other components by rotating the workpiece in synchronization with a
rotating tool or by moving the tool in synchronization with a rotating
workpiece. The rate of synchronization can be specified with a
program. The synchronization of tool and workpiece axes with this
function adopts a system in which the synchronization is directly
controlled by digital servo, so that the workpiece axis can follow up
the speed fluctuations on the tool axis with no error, thereby allowing
fabrication of high-precision cogwheels. In the subsequent
explanation, the Electronic Gear Box is called the EGB.
There are several conditions in the setting and so on of the workpiece
axis and the tool axis, and refer to the appropriate manual provided by
the machine tool builder.
- Example of controlled axis configuration
Spindle : EGB master axis : Tool axis
1st axis : X axis
2nd axis : Y axis
3rd axis : C axis (EGB slave axis : Workpiece axis)
4th axis : C axis (EGB dummy axis : Cannot be used as a normal
controlled axis.)
Spindle amp. Motor
Spindle (master axis)
1st axis X (omitted)
2nd axis Y (omitted)
Tool axis
3rd axis C
slave axis
4th axis
dummy axis
EGB
-
+
+
-
K1: Sync coefficient
K1
Error counter
Sync switch
Motor
Detector
Velocity/current control Servo amp.
Position control
Workpiece axis
C axis
Separate detector
FFG
+
Follow-up
Spindle Detector
CNC
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 737 -
Format
Parameter EFX(No.7731#0)=1
Parameter EFX
(No.7731#0)=0 Parameter HBR
(No.7731#5)=1
Parameter HBR
(No.7731#5)=0
Start of synchronization G81 T＿ ( L＿ )
( Q＿ P＿ ) ;
G81.4 R＿ ( L＿ )
( Q＿ P＿ ) ;
G81.4 T＿ ( L＿ )
( Q＿ P＿ ) ;
Cancellation of synchronization G80 ; G80.4 ; G80.4 ;
(*1) (*2) (*3)
T(or R) : Number of teeth (Specifiable range: 1 to 1000)
L : Number of hob threads (Specifiable range: -200 to +200)
The sign of L determines the direction of rotation for the workpiece axis.
When L is positive, the direction of rotation for the workpiece axis is
positive (+ direction).
When L is negative, the direction of rotation for the workpiece axis is
negative (- direction).
When L is 0, it follows the setting of bit 3 (LZR) of parameter No.7701.
If L is not specified, the number of hob threads is assumed 1.
Q : Module or diametral pitch
Specify a module in the case of metric input.
(Unit: 0.00001mm, Specifiable range: 0.01 to 25.0mm)
Specify a diametral pitch in the case of inch input.
(Unit: 0.00001inch-1, Specifiable range: 0.01 to 254.0 inch-1)
P : Gear helix angle
(Unit: 0.0001deg, Specifiable range: -90.0 to 90.0deg)
*1 Use it for machining centers.
*2 Use it for lathes.
*3 Use it for machining centers.
This format enables specification of the same G codes as those for lathes.
*4 When specifying Q and P, the user can use a decimal point.
NOTE
Specify G81, G80, G81.4, and G80.4 in a single
block.
Explanation
- Master axis, slave axis, and dummy axis
The synchronization reference axis is called the master axis, while the
axis along which movement is performed in synchronization with the
master axis is called the slave axis. For example, if the workpiece
moves in synchronization with the rotating tool as in a hobbing
machine, the tool axis is the master axis and the workpiece axis is the
slave axis.
Which axes to become the master and slave axes depends on the
configuration of the machine. For details, refer to the manual issued
by the machine tool builder.
A single servo axis is used exclusively so that digital servo can
directly read the rotation position of the master axis. (This axis is
called the EGB dummy axis.)
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 738 -
- Synchronization control
(1) Start of synchronization
If G81 is issued so that the machine enters synchronization mode,
the synch switch of the EGB function is closed, and the
synchronization of the tool and workpiece axes is started.
During synchronization, the rotation about the tool and
workpiece axes is controlled so that the relationship between T
(number of teeth) and L (number of hob threads) is maintained.
During synchronization, the synchronization relationship is
maintained regardless of whether the operation is automatic or
manual.
Specify P and Q to use helical gear compensation.
If only either P or Q is issued, alarm PS1594 is generated.
If, during synchronization, G81 is issued again without
synchronization cancelation, alarm PS1595 is generated if ECN,
bit 3 of parameter No. 7731, is 0. If ECN, bit 3 of parameter No.
7731, is 1, helical gear compensation is conducted with the
synchronization coefficient being changed to the one newly
specified with T and L commands if T and L commands are
issued, and if T and L commands are not issued and only P and Q
commands are issued, helical gear compensation is conducted
with the synchronization coefficient kept intact. This allows
consecutive fabrication of helical gears and super gears.
(2) Start of tool axis rotation
When the rotation of the tool axis starts, the rotation of the
workpiece axis starts so that the synchronous relationship
specified in the G81 block can be maintained.
The rotation direction of the workpiece axis depends on the
rotation direction of the tool axis. That is, when the rotation
direction of the tool axis is positive, the rotation direction of the
workpiece axis is also positive; when the rotation direction of the
tool axis is negative, the rotation direction of the workpiece axis
is also negative. However, by specifying a negative value for L,
the rotation direction of the workpiece axis can be made opposite
to the rotation direction of the tool axis.
During synchronization, the machine coordinates of the
workpiece axis and EGB axis are updated as synchronous motion
proceeds. On the other hand, a synchronous move command
has no effect on the absolute and relative coordinates.
(3) Termination of tool axis rotation
In synchronism with gradual stop of the tool axis, the workpiece
axis is decelerated and stopped. By specifying the command
below after the spindle stops, synchronization is canceled, and
the EGB synchronization switch is opened.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 739 -
(4) Cancellation of synchronization
When cancellation of synchronization is issued, the absolute
coordinate on the workpiece axis is updated in accordance with
the amount of travel during synchronization. Subsequently,
absolute commands for the workpiece axis will be enabled.
For a rotation axis, the amount of travel during synchronization,
as rounded to 360-degree units is added to the absolute
coordinate.
In the G80 block, only O and N addresses can be specified.
By setting HBR, bit 0 of parameter No. 7700, to 0, it is possible
to cancel synchronization with a reset. If the manual absolute
signal is ON, the absolute coordinate is updated.
Synchronization is automatically canceled under the following
conditions:
<1> An emergency stop is applied.
<2> A servo alarm is generated.
<3> Alarm PW0000 (POWER MUST BE OFF) is generated.
<4> An IO alarm is generated.
CAUTION
1 Feed hold, interlock, and machine lock are invalid
to a slave axis in EGB synchronization.
2 Even if an OT alarm is issued for a slave axis in
EGB synchronization, synchronization will not be
canceled.
3 During synchronization, it is possible to execute a
move command for a slave axis and other axes,
using a program. The move command for a slave
command must be an incremental one.
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 740 -
NOTE
1 If bit 0 (HBR) of parameter No. 7700 is set to 1,
EGB synchronization will not be canceled due to a
reset. Usually, set this parameter bit to 1.
2 In synchronous mode, it is not possible to specify
G27, G28, G29, G30, G30.1, and G53 for a slave
axis.
3 It is not possible to use controled axis detach for a
slave axis.
4 During synchronization, manual handle interruption
can be performed on the slave and other axes.
5 In synchronization mode, no inch/metric conversion
commands (G20 and G21) cannot be issued.
6 In synchronous mode, only the machine
coordinates on a slave axis are updated.
7 If bit 0 (EFX) of parameter No. 7731 is 0, no drilling
canned cycle can be used. To use a drilling canned
cycle, set bit 0 (EFX) of parameter No. 7731 to 1
and use G81.4 instead of G81 and G80.4 instead
of G80.
8 If TDP, bit 0 of parameter No. 7702, is 1, the
permissible range of T is 0.1 to 100 (1/10 of the
specified value).
9 If, at the start of EGB synchronization (G81), L is
specified as 0, synchronization starts with L
assumed to be 1 if bit 3 (LZR) of parameter
No.7701, is 0; if bit 3 (LZR) of parameter No.7701,
is 1, synchronization is not started with L assumed
to be 0. At this time, helical gear compensation is
performed.
10 Feed per revolution is performed on the feedback
pulses on the spindle. By setting ERV, bit 0 of
parameter No. 7703, to 1, feed per revolution can
be performed based on the speed on the
synchronous slave axis.
11 Actual cutting feedrate display does not take
synchronization pulses into consideration.
12 For an EGB slave axis, synchronous and
cpmposite control cannot be executed.
13 In EGB synchronization mode, AI contour control
mode is temporarily canceled.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 741 -
- Helical gear compensation
For a helical gear, the workpiece axis is compensated for the
movement along the Z-axis (axial feed axis) based on the torsion angle
of the gear.
Helical gear compensation is performed with the following formulas:
Compensation angle = × 360 (for metric input)
Compensation angle = × 360 (for inch input)
where
Compensation angle: Signed absolute value (deg)
Z : Amount of travel on the Z-axis after the specification of G81
P : Signed gear helix angle (deg)
π : Circular constant
T : Number of teeth
Q : Module (mm) or diametral pitch (inch-1)
Use P, T, and Q specified in the G81 block.
In helical compensation, the machine coordinates on the workpiece
axis and the absolute coordinates are updated with helical
compensation.
QT
sin(P)
××
×
π
Z
T
sin(P)QZ
×
××
π
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 742 -
- Direction of helical gear compensation
The direction depends on HDR, bit 2 of parameter No. 7700.
When HDR is set to 1.
+C
C:+, Z:+, P:+
Compensation direction : +
(a)
-Z
+Z +C
C:+, Z:+, P:-
Compensation direction : -
(b)
+C
C:+, Z:-, P:+
Compensation direction : -
(c)
+C
C:+, Z:-, P:-
Compensation direction : +
(d)
-Z
+Z
C:-, Z:+, P:+
Compensation direction : -
(e)
-C
C:-, Z:+, P:-
Compensation direction : +
(f)
-C
C:-, Z:-, P:+
Compensation direction : +
(g)
-C
C:-, Z:-, P:-
Compensation direction : -
(h)
-C
When HDR is set to 0. (In (a), (b), (c), and (d), the same as that if HDR is 1)
-Z
+Z
C:-, Z:+, P:+
Compensation direction : +
(e)
-C
C:-, Z:+, P:-
Compensation direction : -
(f)
-C
C:-, Z:-, P:+
Compensation direction : -
(g)
-C
C:-, Z:-, P:-
Compensation direction : +
(h)
-C
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 743 -
- Synchronization coefficient
A synchronization coefficient is internally represented using a fraction
(Kn/Kd) to eliminate an error. The formula below is used for
calculation.
α
β
T
L
K
K
=t coefficienation Synchroniz
d
n×=
where
L : Number of hob threads
T : Number of teeth
α : Number of pulses of the position detector per rotation about the
master axis (parameter No. 7772)
β : Number of pulses of the position detector per rotation about the
slave axis (parameter No. 7773)
Kn / Kd is a value resulting from reducing the right side of the above
formula, but the result of reduction is subject to the following
restrictions:
-2147483648≤Kn≤2147483647
1≤Kd≤65535
When this restriction is not satisfied, the alarm PS1596 is issued when
G81 is specified.
Example
O1000 ;
N0010 M19 ; Tool axis orientation
N0020 G28 G91 C0 ; Reference position return on the
workpiece axis
N0030 G81 T20 L1 ; Synchronous start on tool and
workpiece axes
(Rotation about the workpiece axis by
18° per rotation about the tool axis)
N0040 S300 M03 ; Rotation about the tool axis at 300min-1
N0050 G01 X F ; Movement along the X-axis (cut)
N0060 G01 Z F ; Movement along the Z-axis
(machining)
-----------------------------; If necessary, axis commands such as C,
X, and Z commands are allowed.
N0100 G01 X F ; Movement along the X-axis (escape)
N0110 M05 ; Stop on the tool axis
N0120 G80 ; Synchronous cancellation on tool and
workpiece axes
N0130 M30 ;
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 744 -
- Retract function
(1) Retract function with an external signal
When the retract switch on the machine operator’s panel is
turned on, retraction is performed with the retract amount set in
parameter No. 7741 and the feedrate set in parameter No. 7740.
No movement is performed along an axis for which 0 is set as the
retract amount.
For the retract switch, refer to the relevant manual provided by
the machine tool builder.
(2) Retract function with an alarm
If, during EGB synchronization or automatic operation, a CNC
alarm is issued, retraction is performed with the retract amount
set in parameter No. 7741 and the speed set in parameter No.
7740.
This can prevent the tool and the object being machined from
damage if a servo alarm is generated.
No movement is performed along an axis for which 0 is set as the
retract amount.
For the retract switch, refer to the relevant manual provided by
the machine tool builder.
Conditions under the retract function with an alarm can be
executed
The conditions under which the retract function with an alarm
can be executed can be changed using the settings of ARE, bit 1
of parameter No. 7703, and bit 2 (ARO) of parameter No. 7703.
The table below lists parameter settings and corresponding
conditions.
ARE ARO Condition
1 0 EGB synchronization is in progress.
1 1
Both EGB synchronization and
automatic operation are in progress.
0 0
0 1
Either EGB synchronization or
automatic operation is in progress.
CAUTION
1 Retraction is performed at the speed specified in
parameter No. 7740.
2 Feed hold is not effective to movement during
retraction.
3 Feedrate override is not effective to movement
during retraction.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 745 -
NOTE
1 During a retract operation, an interlock is effective
to the retract axis.
2 During a retract operation, a machine lock is
effective to the retract axis.
3 The retraction direction depends on the movement
direction of the machine, regardless of whether an
mirror image (signal and setting) is enabled or
disabled. (No mirror image can be applied to the
updating of absolute coordinates.)
4 If retraction is performed during automatic
operation, automatic operation is halted
simultaneously with a retract operation, but it is at
the end of the retract operation that the operation
state switches to the automatic operation halt state.
5 It is not possible to perform automatic operation
during retraction.
6 The acceleration/deceleration of a retract operation
is in the acceleration/deceleration state at the start
of retraction.
7 Retract movement is performed with non-linear
type positioning.
8 If, during a retract operation, a reset or an
emergency stop is made, the operation is
interrupted.
9 If, during a retract operation on multiple axes, an
OT alarm or a malfunction prevention alarm is
issued for a retract axis, the operation stops only
on the axis for which the alarm is issued if bit 4
(RTS) of parameter No. 7731 is 0. If bit 4 (RTS) of
parameter No. 7731 is 1, the retract operation is
interrupted on all axes. If a servo alarm or non-axis
malfunction prevention alarm is issued, the retract
operation is interrupted on all axes regardless of
the setting of bit 4 (RTS) of parameter No. 7731.
10 To enable the retract function with an alarm, bit 3
(ART) of parameter No.7702, must be set.
11 The retract function with an alarm does not perform
a retract operation on the retract axis if an overtravel
alarm or a servo alarm is geneated on the retract
axis.
12 If a new alarm is issued during retraction with the
retract function with an alarm, a retract operation is
not performed.
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 746 -
21.7.2 Electronic Gear Box Automatic Phase Synchronization
Overview
In the electronic gear box (EGB), when synchronization start or
cancellation is specified, synchronization is not started or canceled
immediately. Instead, acceleration/deceleration is executed first.
Therefore, synchronization can be started or canceled while the
spindle is rotating. Also, synchronization ratio can be changed while
the spindle is rotating.
At synchronization start, automatic phase synchronization is
performed such that the workpiece axis position matches the position
corresponding to the spindle one-rotation signal. With this
synchronization, the same operation is performed as synchronization
start caused by a one-rotation signal in hobbing synchronization when
using the functions of a hobbing machine.
The spindle corresponds to the EGB master axis and the workpiece
axis corresponds to an EGB slave axis.
Format
- Acceleration/deceleration type
G81 T _ L _ R1 ; Synchronization start
G80 R1 ; Synchronization cancellation
T : Number of teeth (range of valid settings: 1-1000)
L : Number of hob threads (range of valid settings: -200 to
+200, excluding 0)
When L is positive, the direction of rotation about the
workpiece axis is positive (+ direction).
When L is negative, the direction of rotation about the
workpiece axis is negative (- direction).
- Acceleration/deceleration plus automatic phase synchronization type
G81 T _ L _ R2 ; Synchronization start
G80 R1 ; Synchronization cancellation
T : Number of teeth (range of valid settings: 1-1000)
L : Number of hob threads (range of valid settings: -200 to
+200, excluding 0)
When L is positive, the direction of rotation about the
workpiece axis is positive (+ direction).
When L is negative, the direction of rotation about the
workpiece axis is negative (- direction).
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 747 -
Explanation
- Acceleration/deceleration type
Synchronization
cancellation command
Synchronization
start command
Workpiece-
axis speed
Synchronization state
Acceleration Deceleration
Spindle
speed
1. Specify G81R1 to start synchronization.
When G81R1 is specified, the workpiece axis (slave axis) is
subject to acceleration at the acceleration rate set in parameter No.
7778. When the synchronization speed is reached, the G81R1
block is terminated.
2. For cancellation, specify G80R1 while the tool is moved away
from the workpiece.
3. When G80R1 is specified, deceleration is started immediately at
the acceleration rate set in parameter No. 7778.
When the speed is reduced to 0, the G80R1 block is terminated.
NOTE
1 During synchronization start/cancellation,
acceleration/deceleration is linear.
2 In the automatic cancellation of synchronization due
to one of the following causes, deceleration is
performed and synchronization is canceled:
<1> Reset
<2> PW0000 (POWER MUST BE OFF)
<3> IO alarm
3 If EFX, bit 0 of parameter No. 7731, is 0, the
canned cycle for drilling cannot be used. To use
the canned cycle for drilling, set EFX, bit 0 of
parameter No. 7731, to 1 and use G81.4 instead of
G81 and G80.4 instead of G80.
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 748 -
- Acceleration/deceleration plus automatic phase synchronization type
Automatic phase
synchronization
Synchronization
cancellation command
Synchronization
start command
Workpiece-
axis speed
Synchronization
state
Acceleration Deceleration
Spindle
speed
1. Move the workpiece axis to the position that corresponds to that
of the one-rotation signal of the spindle.
2. Specify G81R2 to start synchronization.
When G81R2 is specified, the workpiece axis is accelerated with
the acceleration according to the acceleration rate set in the
parameter No.7778. Upon completion of phase synchronization,
the G81R2 block terminates.
3. For cancellation, specify G80R2 while the tool is moved away
from the workpiece.
4. When G80R2 is issued, deceleration is started immediately
according to the acceleration rate set in parameter No. 7778.
When the speed reaches 0, the G80R2 block terminates.
CAUTION
1 Set the automatic phase synchronization speed in
parameter No. 7776 and the movement direction in
PHD, bit 7 of parameter No. 7702.
2 Phase synchronization acceleration/deceleration is
performed with the rapid traverse linear
acceleration/deceleration rate (time constant
specified in parameter No. 1620).
3 The workpiece axis speed is the speed
synchronized with spindle rotation with automatic
phase synchronization speed being superposed.
When setting the position deviation limit parameter
No. 1828, take the superposition into consideration.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 749 -
NOTE
1 The one-rotation signal used for automatic phase synchronization is issued not by
the spindle position coder but by the separate pulse coder attached to the spindle
and used to collect EGB feedback information. This means that the orientation
position based on the one-rotation signal issued by the spindle position coder does
not match the position used as the reference for the workpiece axis when
establishing phase synchronization for automatic phase synchronization based on
G81R2.
Moreover, the one-rotation signal of the separate pulse coder must be turned on
for each rotation of the spindle.
2 With the use of parameter No.7777, the position at which the phase of the
workpiece axis is matched can be shifted from the position corresponding to the
one-rotation signal in automatic phase matching.
3 In automatic phase synchronization, when a synchronization command is issued
again in a synchronization state, movement about the workpiece axis is performed
such that the position corresponding to the one-rotation signal of the spindle
matches the position about the workpiece axis specified in the G81R2
synchronization start command executed first.
4 In automatic phase synchronization, movement is performed about the workpiece
axis from the current position to the nearest phase position in the phase
synchronization movement direction specified by the parameter.
5 Linear acceleration/deceleration applies to synchronization start/cancellation.
6 The acceleration/deceleration plus automatic phase synchronization type can be
executed by the PHS parameter, bit 6 of No.7702, without specifying an R2
command in a G81 or G80 block.
7 In the automatic cancellation of synchronization due to one of the following causes,
deceleration is performed and synchronization canceled:
<1> Reset
<2> PW0000 (POWER MUST BE OFF)
<3> IO alarm
8 The acceleration rate parameter No.7778 must not be changed in the
synchronization mode.
9 If the acceleration/deceleration parameter No. 7778 is 0, alarm PS1598 is issued
when G81 is issued.
10 For the FS16i series, the acceleration/deceleration for automatic phase
synchronization is divided into acceleration/deceleration and time constant, which
are set in parameters Nos. 2135 and 2136. For the FS30i series,
acceleration/deceleration is directly set in parameter No. 7778.
11 If EFX, bit 0 of parameter No. 7731, is 0, the canned cycle for drilling cannot be
used. To use the canned cycle for drilling, set EFX, bit 0 of parameter No. 7731,
to 1 and use G81.4 instead of G81 and G80.4 instead of G80.
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 750 -
Program example
- Acceleration/deceleration type
M03 ; Clockwise spindle rotation command
G81 T_ L_ R1 ; Synchronization start command
G00 X_ ; Positions the workpiece at the machining
position.
Machining in the synchronous state
G00 X_ ; Retract the workpiece from the tool.
G81 T_ L_ R1 ; Synchronization ratio change.
G00 X_ ; Positions the workpiece at the machining
position.
Machining in the synchronous state
G00 X_ ; Retract the workpiece from the tool.
G80 R1 ; Synchronization cancel command
- Acceleration/deceleration plus automatic phase synchronization type
M03 ; Clockwise spindle rotation command
G00 G90 C_ ; C-axis positioning
G81 T_ L_ R2 ; Synchronization start command
G00 X_ ; Positions the workpiece at the machining
position.
Machining in the synchronous state
G00 X_ ; Retract the workpiece from the tool.
G81 T_ L_ R2 ; Synchronization ratio change.
G00 X_ ; Positions the workpiece at the machining
position.
Machining in the synchronous state
G00 X_ ; Retract the workpiece from the tool.
G80 R2 ; Synchronization cancel command
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 751 -
21.7.3 Skip Function for EGB Axis
Overview
This function enables the skip or high-speed skip signal (these signals
are collectively called skip signals in the remainder of this manual) for
the EBG slave axis in synchronization mode with the EGB (electronic
gear box ).
This function has features such as the following:
1 If a skip signal is input while an EGB axis skip command block
is being executed, this block does not terminate until the
specified number of skip signals have been input.
2 If a skip signal is input while an EGB axis skip command block
is being executed, the tool remains in synchronous mode and
moves, not stopping on the EGB slave axis.
3 The machine coordinates assumed when skip signals are input
and the number of input skip signals are stored in specified
custom macro variables.
Format
G81 T_ L_ ; EGB mode ON
G31.8 G91 α0 P_ Q_ ( R_ ) ; EGB skip command
α: Specify an EGB slave axis. The specified value
must always be "0".
P: Number of the first one of the custom macro
variables used to store the machine coordinates
assumed when skip signals are input.
Q: Number of skip signals that can be input during the
execution of G31.8
(permissible range: 1 to 200).
R: Number of the custom macro variable used to store
the number of input skip signals.
Specify it to check the number of input signals.
Explanation
G31.8 is a one-shot G code.
When G31.8 is executed, the machine coordinates assumed when skip
signals are input are written in as many custom macro variables as the
number specified in Q, starting with the one having the number
specified in P, when the skip command block terminates.
Also, the number of input skip signals is written to the custom macro
variable specified in R each time a skip signal is input.
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 752 -
Example
G81 T200 L2 ; EGB mode ON
X ;
Z ;
G31.8 G91 C0 P500 Q200 R1 ; EGB skip command
After 200 skip signals have been input, the 200 skip positions on the
C-axis that correspond to the respective skip signals are stored in
custom macro variables #500 to #699.
Also, the number of input skip signals is stored in custom macro
variable #1.
NOTE
1 When specifying this function, specify only a single
EGB slave axis. If no axis is specified for two or
more axes are specified, alarm PS1152 is
generated.
2 If P is not specified, alarm PS1152 is generated.
3 If R is not specified, the number of input skip
signals is not written to a custom macro variable.
4 The custom macro variable numbers specified in P
and R must be existing ones. If a non-existent
variable number is specified, alarm PS0115 is
generated.
If a variable shortage occurs, alarm PS0115 is
generated.
5 Whether to use conventional skip signals or
high-speed skip signals with this function can be
specified with HSS, bit 4 of parameter No. 6200.
If deciding to use high-speed skip signals, specify
which high-speed signals to enable with 9S1 to
9S8, bits 0 to 7 of parameter No. 6208).
6 Skip positions are calculated from feedback pulses
from the machine. Thus, they are free from errors
due to delay in acceleration/deceleration and the
servo system
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 753 -
21.7.4 Electronic Gear Box 2 Pair
Overview
The Electronic Gear Box is a function for rotating a workpiece in sync
with a rotating tool, or to move a tool in sync with a rotating
workpiece. With this function, the high-precision machining of gears,
threads, and the like can be implemented. A desired synchronization
ratio can be programmed.
Up to two sets of axes can be synchronized. A gear grinding machine
can be controlled, for instance, by using one axis for rotating the
workpiece in sync with the tool and another axis for performing
dressing in sync with the tool.
The specification method differs depending on the configuration of
the machine. For details, refer to the relevant manual provided by
the machine tool builder.
The electronic gear box is hereinafter called an EGB function.
21.7.4.1 Specification method (G80.5, G81.5)
Format
G81.5
p P
t T
l L 0
j
β
β ; Synchronization start
↑ ↑
Amount of travel Amount of travel
along the master along the slave axis
axis
G80.5 β0 ; Synchronization end
Explanation
- Master axis, slave axis, and dummy axis
The synchronization reference axis is called the master axis, while the
axis along which movement is performed in synchronization with the
master axis is called the slave axis. For example, if the workpiece
moves in synchronization with the rotating tool as in a hobbing
machine, the tool axis is the master axis and the workpiece axis is the
slave axis.
Which axes to become the master and slave axes depends on the
configuration of the machine. For details, refer to the manual issued
by the machine tool builder.
A single servo axis is used exclusively so that digital servo can
directly read the rotation position of the master axis. (This axis is
called the EGB dummy axis.)
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 754 -
- Synchronization start
When the ratio of the master-axis travel to the slave-axis travel is
specified, synchronization starts.
Specify the master-axis travel in either of the following ways.
1 Master-axis speed
T t: Master-axis speed (1≤ t ≤1000)
2 Master-axis pulse count
P p : Master-axis pulse count (1≤ p ≤999999999)
Specify a pulse count on the condition that four pulses
correspond to one period in the A and B phases.
Specify the slave-axis travel in either of the following ways.
1 Slave-axis travel
βj : Slave-axis address
j : Slave-axis travel indicated in units of the minimum travel
increments(the range of valid settings for usual axis
movement applies)
When j = 0, the specified command is regarded as being a
command for the slave-axis speed, described below. In this
case, if L is not specified, an alarm is output.
2 Slave-axis speed
β0 L±l
β : Slave-axis address
l : Slave axis speed(1≤ l ≤200)
- Synchronization end
1 Canceling synchronization for each axis by issuing a command
With a G80.5 β0 command, synchronization is canceled.
β is the address of the slave axis. Synchronization of the slave
axis specified by β is canceled.
A cancellation command can be issued only for one axis in one
block.
When β0 is not specified, the synchronization of all currently
synchronized axes is canceled.
When a synchronization cancellation command is issued, the
absolute coordinates for the slave axis are updated according to
the amount of travel during synchronization. For a rotation axis,
the value obtained by rounding off the amount of travel during
synchronization to the nearest 360 degrees is added to the
absolute coordinates.
2 Canceling synchronization by a reset
By setting HBR, bit 0 of parameter No. 7700, to 0,
synchronization is canceled with a reset. If the manual absolute
signal is ON, the absolute coordinates are updated.
3 Others
Synchronization is automatically canceled under the following
conditions.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 755 -
<1> Emergency stop
<2> Servo alarm
<3> Alarm PW0000 (indicating that the power should be turned
off)
<4> An IO alarm is generated
CAUTION
1 Feed hold, interlock, and machine lock are invalid
to a slave axis in EGB synchronization.
2 Even if an OT alarm is issued for a slave axis in
EGB synchronization, synchronization will not be
canceled.
3 During synchronization, it is possible to execute a
move command for a slave axis and other axes,
using a program. The move command for a slave
command must be an incremental one.
NOTE
1 If bit 0 (HBR) of parameter No. 7700 is set to 1,
EGB synchronization will not be canceled due to a
reset. Usually, set this parameter bit to 1.
2 In synchronous mode, it is not possible to specify
G27, G28, G29, G30, G30.1, and G53 for a slave
axis.
3 It is not possible to use controled axis detach for a
slave axis.
4 During synchronization, manual handle interruption
can be performed on the slave and other axes.
5 In synchronization mode, no inch/metric conversion
commands (G20 and G21) cannot be issued.
6 In synchronous mode, only the machine
coordinates on a slave axis are updated.
7 If bit 0 (EFX) of parameter No. 7731 is 0, no drilling
canned cycle can be used. To use a drilling canned
cycle, set bit 0 (EFX) of parameter No. 7731 to 1.
8 If, during synchronization, G81.5 is issued again,
alarm PS1594 is issued if bit 3 (ECN) of parameter
No. 7731 is 0. If bit 3 (ECN) of parameter No. 7731
is 1, the synchronization coefficient can be
changed to a newly specified one.
9 Actual cutting feedrate display does not take
synchronization pulses into consideration.
10 For an EGB slave axis, synchronous and
cpmposite control cannot be executed.
11 In EGB synchronization mode, AI contour control
mode is temporarily canceled.
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 756 -
21.7.4.2 Description of commands compatible with those for a
hobbing machine (G80, G81)
A command compatible with that for a hobbing machine can be used
as a synchronization command.
Usually, a hobbing machine performs machining by synchronizing the
workpiece axis (usually, the C-axis) to the hobbing axis (spindle).
If there are two synchronization sets with the EGB, which
synchronization set to start with this specification method can be
specified with parameter No. 7710.
Format
Parameter EFX(No.7731#0)=1 Parameter EFX
(No.7731#0)=0 Parameter HBR
(No.7731#5)=1
Parameter HBR
(No.7731#5)=0
Start of synchronization G81 T＿ ( L＿ )
( Q＿ P＿ ) ;
G81.4 R＿ ( L＿ )
( Q＿ P＿ ) ;
G81.4 T＿ ( L＿ )
( Q＿ P＿ ) ;
Cancellation of
synchronization G80 ; G80.4 ; G80.4 ;
(*1) (*2) (*3)
T(or R) : Number of teeth (Specifiable range: 1 to 1000)
L : Number of hob threads (Specifiable range: -200 to +200)
The sign of L determines the direction of rotation for the workpiece
axis.
When L is positive, the direction of rotation for the workpiece axis
is positive (+ direction).
When L is negative, the direction of rotation for the workpiece axis
is negative (- direction).
When L is 0, it follows the setting of bit 3 (LZR) of parameter
No.7701.
If L is not specified, the number of hob threads is assumed 1.
Q : Module or diametral pitch
Specify a module in the case of metric input.
(Unit: 0.00001mm, Specifiable range: 0.01 to 25.0mm)
Specify a diametral pitch in the case of inch input.
(Unit: 0.00001inch-1, Specifiable range: 0.01 to 254.0 inch-1)
P : Gear helix angle
(Unit: 0.0001deg, Specifiable range: -90.0 to 90.0deg)
*1 Use it for machining centers.
*2 Use it for lathes.
*3 Use it for machining centers.
This format enables specification of the same G codes as those
for lathes.
*4 When specifying Q and P, the user can use a decimal point.
NOTE
Specify G81, G80, G81.4, and G80.4 in a single block.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 757 -
Explanation
- Synchronization start
Specify P and Q to use helical gear compensation. In this case, if only
one of P and Q is specified, alarm PS1594 is generated.
When G81 is issued so that the machine enters synchronization mode,
the synchronization of the workpiece axis to the spindle is started.
During synchronization, control is performed such that the ratio of the
spindle speed to the workpiece-axis speed is the same as that of T
(number of teeth) to L (number of hob threads).
If, during synchronization, G81 is issued again without
synchronization cancellation, alarm PS1595 is generated if ECN, bit 3
of parameter No. 7731, is 0. If ECN, bit 3 of parameter No. 7731, is
1, helical gear compensation is conducted with the synchronization
coefficient being changed to the one newly specified with T and L
commands if T and L commands are issued, and if T and L commands
are not issued and only P and Q commands are issued, helical gear
compensation is conducted with the synchronization coefficient kept
intact. This allows consecutive fabrication of helical gears and super
gears.
- Synchronization end
Synchronization of all synchronized axes is canceled.
When a synchronization cancellation command is issued, the absolute
coordinates for the slave axis are updated according to the amount of
travel during synchronization.
For a rotation axis, the value obtained by rounding off the amount of
travel during synchronization to the nearest 360 degrees is added to
the absolute coordinates.
In a G80 block, do not specify addresses other than O or N.
CAUTION
1 Feed hold, interlock, and machine lock are invalid
to a slave axis in EGB synchronization.
2 Even if an OT alarm is issued for a slave axis in
EGB synchronization, synchronization will not be
canceled.
3 During synchronization, it is possible to execute a
move command for a slave axis and other axes,
using a program. The move command for a slave
command must be an incremental one.
NOTE
1 If bit 0 (HBR) of parameter No. 7700 is set to 1,
EGB synchronization will not be canceled due to a
reset. Usually, set this parameter bit to 1.
2 In synchronous mode, it is not possible to specify
G27, G28, G29, G30, G30.1, and G53 for a slave
axis.
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 758 -
NOTE
3 It is not possible to use controled axis detach for a
slave axis
4 During synchronization, manual handle interruption
can be performed on the slave and other axes.
5 In synchronization mode, no inch/metric conversion
commands (G20 and G21) cannot be issued.
6 In synchronous mode, only the machine
coordinates on a slave axis are updated.
7 If bit 0 (EFX) of parameter No. 7731 is 0, no drilling
canned cycle can be used. To use a drilling canned
cycle, set bit 0 (EFX) of parameter No. 7731 to 1
and use G81.4 instead of G81 and G80.4 instead
of G80.
8 If bit 0 (TDP) of parameter No. 7702, is 1, the
permissible range of T is 0.1 to 100 (1/10 of the
specified value).
9 If, at the start of EGB synchronization (G81), L is
specified as 0, synchronization starts with L
assumed to be 1 if bit 3 (LZR) of parameter
No.7701, is 0; if bit 3 (LZR) of parameter No.7701,
is 1, synchronization is not started with L assumed
to be 0. At this time, helical gear compensation is
performed.
10 Feed per revolution is performed on the feedback
pulses on the spindle. By setting bit 0 (ERV) of
parameter No. 7703, to 1, feed per revolution can
be performed based on the speed on the
synchronous slave axis.
11 Actual cutting feedrate display does not take
synchronization pulses into consideration.
12 For an EGB slave axis, synchronous and
cpmposite control cannot be executed.
13 In EGB synchronization mode, AI contour control
mode is temporarily canceled.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 759 -
- Helical gear compensation
For a helical gear, the workpiece axis is subjected to compensation for
movement along the Z axis (axial feed axis) according to the twisted
angle of the gear.
Helical gear compensation is performed with the following data.
Compensation angle = ×360 (for metric input)
Compensation angle = ×360 (for inch input)
where
Compensation angle: Absolute value with sign (degrees)
Z : Amount of travel along the Z axis after a G81 command is
issued (mm or inch)
P : Twisted angle of the gear with sign (degrees)
π : Circular constant
T : Number of teeth
Q : Module (mm) or diametral pitch (inch-1)
Use P, T, and Q specified in the G81 block.
In helical compensation, the machine coordinates on the workpiece
axis and the absolute coordinates are updated with helical
compensation.
QT
sin(P)
××
×
π
Z
T
sin(P)QZ
×
××
π
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 760 -
- Direction of helical gear compensation
The direction depends on bit 2 (HDR) of parameter No. 7700.
When HDR is set to 1.
+C
C:+, Z:+, P:+
Compensation direction : +
(a)
-Z
+Z +C
C:+, Z:+, P:-
Compensation direction : -
(b)
+C
C:+, Z:-, P:+
Compensation direction : -
(c)
+C
C:+, Z:-, P:-
Compensation direction : +
(d)
-Z
+Z
C:-, Z:+, P:+
Compensation direction : -
(e)
-C
C:-, Z:+, P:-
Compensation direction : +
(f)
-C
C:-, Z:-, P:+
Compensation direction : +
(g)
-C
C:-, Z:-, P:-
Compensation direction : -
(h)
-C
When HDR is set to 0. (In (a), (b), (c), and (d), the same as that if HDR is 1)
-Z
+Z
C:-, Z:+, P:+
Compensation direction : +
(e)
-C
C:-, Z:+, P:-
Compensation direction : -
(f)
-C
C:-, Z:-, P:+
Compensation direction : -
(g)
-C
C:-, Z:-, P:-
Compensation direction : +
(h)
-C
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 761 -
21.7.4.3 Controlled axis configuration example
- For gear grinders
Spindle : EGB master axis : Tool axis
1st axis : X axis
2nd axis : Y axis
3rd axis : C axis (EGB slave axis : Workpiece axis)
4th axis : C axis (EGB dummy axis : Cannot be used as a normal
controlled axis)
5th axis : V axis (EGB slave axis : Dressing axis)
6th axis : V axis (EGB dummy axis : Cannot be used as a normal
controlled axis)
Cannot be used as a normal controlled axis)
Spindle amp. Motor
Spindle (master axis)
1st axis X (omitted)
2nd axis Y (omitted)
Tool axis
3rd axis C
slave axis
4th axis
dummy axis
EGB
-
+
+
-
K1: Sync coefficient
K1
Error counter
Sync switch
Motor
Detector
Velocity/current control Servo amp.
Position control
Workpiece axis
C axis
Separate detector
FFG
+
Follow-up
Spindle Detector
CNC
5th axis V
slave axis
6th axis
dummy axis
EGB
-
+
+
-
K2: Sync coefficient
K2
Error counter
Sync switch
Motor
Detector
Velocity/current control Servo amp.
Position control
Workpiece axis
V axis
Separate detector
FFG
+
Follow-up
Fig. 21.7.4.3 (a)
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 762 -
21.7.4.4 Sample programs
- When the master axis is the spindle, and the slave axis is the C-axis
(1) G81.5 T10 C0 L1 ;
Synchronization between the master axis and C-axis is
started at the ratio of one rotation about the C-axis to ten
rotations about the master axis.
(2) G81.5 T10 C0 L-1 ;
Synchronization between the master axis and C-axis is
started at the ratio of one rotation about the C-axis to ten
rotations about the master axis.
In this case, however, the direction of rotation is opposite to
that of (1).
(3) G81.5 T1 C3.26 ;
Synchronization between the master axis and C-axis is
started at the ratio of a 3.26-degree rotation about the C-axis
per one rotation about the master axis.
(4) G81.5 P10000 C-0.214 ;
Synchronization between the master axis and C-axis is
started at the ratio of a -0.214 degree rotation about the
C-axis to 10,000 feedback pulses from the pulse coder of
the master axis.
- When the master axis is the spindle, the slave axis is the V-axis (linear axis), and
inch/metric conversion is performed
(1) For a millimeter machine and metric input
G81.5 T1 V1.0 ;
Synchronization between the master axis and V-axis is
started at the ratio of a 1.00 mm movement along the V-axis
per rotation about the master axis.
(2) For a millimeter machine and inch input
G81.5 T1 V1.0 ;
Synchronization between the master axis and V-axis is
started at the ratio of a 1.0 inch movement (25.4 mm) along
the V-axis per rotation about the master axis.
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 763 -
- When two groups of axes are synchronized simultaneously
Based on the controlled axis configuration described in Fig. 21.7.4.3
(a), the sample program below synchronizes the spindle with the
V-axis while the spindle is synchronized with the C-axis.
Grinding
Dressing
Grinding
O0100 ;
...............
N01 M19 ; Performs spindle orientation.
Positions the C-axis.
Starts synchronization at the ratio of one rotation about the
C-axis to ten spindle rotations.
N02 G00 G90 C... ;
N03 G81.5 T10 C0 L1 ;
N04 M03 S300 ; Rotates the spindle.
Makes movements for grinding.
Stops the spindle.
N05 G01 G91 X... Y... F... ;
.......
N06 M05 ;
.......
N10 G00 G90 V... ; Positions the dressing axis.
Starts synchronization at the ratio of a
0.5 mm movement along the V-axis
every 12,000 pulses on the spindle.
Rotates the spindle.
A
subprogram for dressing is called. (Note)
Stops the spindle.
N11 G81.5 P12000 V0.5 ;
N12 M03 S300 ;
N20 M98 P9500 ;
N21 M05 ;
N30 G80.5 V0 ; Cancels V-axis synchronization.
.......
.......
N31 M03 S300 ; Rotates the spindle.
Makes movements for grinding.
N32 G01 G91 X... Y... F... ;
.......
.......
N40 M05 ; Stops the spindle.
Cancels C-axis synchronization.
N41 G80.5 C0 ;
V-axis synchronization mode
C-axis synchronization mode
Thus, the synchronizations of two groups can be started and canceled
independently of each other.
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 764 -
- Example of use of dressing
Gear grinder in the following machine configuration
Limit switch 1 Limit switch 2
V-axis motor
U-axis
V-axis
Rotary whetstone
O9500 ;
N01 G01 G91 U＿ F100 ; Dressing axis approach
N02 M03 S100 ; The M03 command causes the PMC to rotate the
whetstone in the positive direction.
In accordance with this, the tool moves along the V-axis
in the + direction. When the tool reaches the position of
limit switch 2 on the V-axis, the PMC stops the
whetstone and returns FIN.
N02 U＿ V＿ ; Movement to the next dressing position
N03 M04 S100 ; The M04 command causes the PMC to rotate the
whetstone in the negative direction.
In accordance with this, the tool moves along the V-axis
in the - direction. When the tool reaches the position of
limit switch 1 on the V-axis, the PMC stops the
whetstone and returns FIN.
N04 U＿ V＿ ; Movement to the next dressing position
If required, N02 to N04 are repeated to conduct dressing.
..........
..........
M99 ;
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 765 -
NOTE
If the V-axis (linear axis) is synchronized with the
spindle as in dressing, the V-axis travel range is
determined by the rotation of the spindle. To
perform dressing with the tool moving back and
forth along the V-axis in a certain range, therefore,
the PMC must perform an operation in which the
tool is stopped temporarily and is reversed when it
reaches a certain position on the V-axis.
In the above example, limit switches are provided to
determine the range of travel along the V-axis and
the PMC performs control so that the whetstone
rotates until the tool reaches the position of each
limit switch on the V-axis.
By using the position switch function instead of limit
switches, dressing can be performed as in the
following example, without the need to mount limit
switches to the machine. By rewriting the
operating ranges of the position switches
(parameters Nos. 6930 to 6945 and Nos. 6950 to
6965) using the G10 programming Parameter input,
the range of travel along the V-axis can be specified
using a program.
- Command specification for hobbing machines
Based on the controlled axis configuration described in Fig. 21.7.4.3
(a), the sample program below sets the C-axis (in parameter 7710) for
starting synchronization with the spindle according to the command
specification method for hobbing machines.
O1234 ;
N0010 M19 ; Performs tool axis orientation.
N0020 G28 G91 C0 ; Performs reference position return along the workpiece axis.
N0030 G81 T20 L1 ; Starts synchronization with the spindle and C-axis at the ratio of
a 18° rotation about the C-axis to one spindle rotation.
N0040 S300 M03 ; Rotates the spindle at 300 min-1.
N0050 G01 X... F... ; Makes a movement along the X-axis (for cutting).
N0060 G01 Y... F... ; Makes a movement along the Y-axis (for grinding).
Axes such as the C-axis, X-axis, and Y-axis can be specified as
required.
N0100 G01 X... F... ; Makes a movement along the X-axis (for retraction).
N0110 M05 ; Stops the spindle.
N0120 G80 ; Cancels the synchronization between the spindle and C-axis.
N0130 M30 ;
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 766 -
21.7.4.5 Synchronization ratio specification range
The programmed ratio (synchronization ratio) of a movement along
the slave axis to a movement along the master axis is converted to a
detection unit ratio inside the NC. If such converted data (detection
unit ratio) exceeds a certain allowable data range in the NC,
synchronization cannot be established correctly, and an alarm PS1596
is issued.
Even when a programmed master axis movement and a programmed
slave axis movement are within specifiable ranges, a detection unit
ratio obtained by conversion can exceed the allowable range, thus
resulting in an alarm.
Let K be a synchronization ratio. The internal data corresponding K is
the amount of slave axis movement (Kn) represented in the detection
unit divided by the amount of master axis movement (Kd) represented
in the detection unit;
this fraction is represented as Kn/Kd (reduced to its lowest terms) as
indicated below.
unitdetection in the drepresentemovement axismaster ofAmount
unitdetection in the drepresentemovement axis slave ofAmount
Kd
Kn
K==
Kn and Kd must lie within the following ranges:
-2147483648 ≤ Kn ≤ 2147483647
1 ≤ Kd ≤ 65535
When Kn or Kd exceeds its allowable range above, an alarm PS1596
is issued.
In conversion to the detection unit, when the CMR (command
multiplication: parameter 1820) is a fraction or when inch/millimeter
conversion is used, the fraction is directly converted without
modification so that no error can occur in the conversion of specified
amounts of movement.
During conversion, the amount of movement is multiplied by 254/100
for inch input on a millimeter machine, and 100/254 for metric input
on an inch machine. Thus, Kn and Kd can become large numbers. If a
synchronization ratio cannot be reduced to its lowest terms, an alarm
condition is likely to occur.
- Example 1)
Based on the controlled axis configuration described in Fig. 21.7.4.3
(a), suppose that the spindle and V-axis are as follows:
Spindle pulse coder : 72000pulse/rev (4 pulses for one
A/B phase cycle)
C-axis least command increment : 0.001deg
C-axis CMR : 5
V-axis least command increment : 0.001mm
V-axis CMR : 5
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 767 -
Then, the C-axis detection unit is 0.0002 degree. The V-axis detection
unit is 0.0002 mm. In this case, the synchronization ratio (Kn, Kd) is
related with a command as indicated below. Here, let Pm and Ps be
the amounts of movements represented in the detection unit on the
master axis and slave axis specified in a synchronization start
command, respectively.
(1) When the master axis is the spindle, and the slave axis is the
C-axis
(a) Command : G81.5 T10 C0 L1 ;
Operation : Synchronization between the spindle and C-axis
is started at the ratio of one rotation about the
C-axis to ten spindle rotations.
Pm : (Number of pulses per spindle rotation) × (10
rotations) → 72000 × 10
Ps : (Amount of movement per rotation about the
C-axis) × CMR × (one rotation) → 360000 × 5
× 1
Kn
Kd = 360000×5×1
72000×10 = 5
2
Both Kn and Kd are within the allowable range. No alarm is
output.
(b) Command : G81.5 T10 C0 L-1 ;
Operation : Synchronization between the spindle and C-axis
is started at the ratio of one rotation about the
C-axis to ten spindle rotations.
In this case, however, the direction of rotation
is opposite to that of (a) above.
Pm : (Number of pulses per spindle rotation) × (10
rotations) → 72000 × 10
Ps : (Amount of movement per rotation about the
C-axis) × CMR × (one rotation) → -360000 × 5
× 1
Kn
Kd = -360000×5×1
72000×10 = -5
2
Both Kn and Kd are within the allowable range. No alarm is
output.
(c) Command : G81.5 T1 C3.263 ;
Operation : Synchronization between the spindle and C-axis
is started at the ratio of a 3.263-degree rotation
about the C-axis to one spindle rotation.
Pm : (Number of pulses per spindle rotation) × (one
rotation) → 72000 × 1
Ps : (Amount of C-axis movement) × CMR → 3263
× 5
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 768 -
Kn
Kd = 3263×5
72000×1 = 3263
14400
Both Kn and Kd are within the allowable range. No alarm is
output.
In this sample program, when T1 is specified for the master
axis, the synchronization ratio (fraction) of the CMR of the
C-axis to the denominator Kd can always be reduced to
lowest terms, thus Kd falls in the allowable range. So, the
specifiable range of C is as follows:
-99999999 ≤ C ≤ 99999999
(d) Command : G81.5 T10 C3.263 ;
Operation : Synchronization between the spindle and C-axis
is started at the ratio of a 3.263-degree rotation
about the C-axis to ten spindle rotations.
Pm : (Number of pulses per spindle rotation) × (10
rotations) → 72000 × 10
Ps : (Amount of C-axis movement) × CMR → 3263
× 5
Kn
Kd = 3263×5
72000×10 = 3263
144000
In this case, an alarm is issued because Kd exceeds the
specifiable range.
(e) Command : G81.5 P10000 C-0.214 ;
Operation : Synchronization between the spindle and C-axis
is started at the ratio of a -0.214 degree rotation
of the C-axis to 10,000 feedback pulses from
the pulse coder of the spindle.
Pm : (Specified number of feedback pulses from the
pulse coder of the spindle) → 10000
Ps : (Amount of C-axis movement) × CMR → -214
× 5
Kn
Kd = -214×5
10000 = -107
1000
Both Kn and Kd are within the allowable range. No alarm is
output.
(2) When the master axis is the spindle, the slave axis is the V-axis
(linear axis), and inch/metric conversion is performed
(a) For a millimeter machine and metric input
Command : G81.5 T1 V1.0 ;
Operation : Synchronization between the spindle and
V-axis is started at the ratio of a 1.0 inch
movement (25.4 mm) along the V-axis per
spindle rotation.
Pm : (Number of pulses per spindle rotation) × (one
rotation) → 72000 × 1
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 769 -
Ps : (Amount of V-axis movement) × CMR → 1000
× 5
Kn
Kd = 1000×5
72000 = 5
72
Both Kn and Kd are within the allowable range. No alarm is
output.
(b) For a millimeter machine and inch input
Command : G81.5 T1 V1.0 ;
Operation : Synchronization between the spindle and
V-axis is started at the ratio of a 1.0inch
(25.4mm) movement along the V-axis per
spindle rotation.
Pm : (Number of pulses per spindle rotation) × (one
rotation) → 72000 × 1
Ps : (Amount of V-axis movement) × CMR × 254 ÷
100 → 10000 × 5 × 254 ÷ 100
Kn
Kd = 10000×5×254
72000×100 = 127
72
Both Kn and Kd are within the allowable range. No alarm is
output.
(c) For a millimeter machine and inch input
Command : G81.5 T1 V0.0013 ;
Operation : Synchronization between the spindle and
V-axis is started at the ratio of a 0.0013 inch
(0.03302 mm) movement along the V-axis per
spindle rotation.
Pm : (Number of pulses per spindle rotation) × (one
rotation) → 72000 × 1
Ps : (Amount of V-axis movement) × CMR × 254 ÷
100 → 13 × 5 × 254 ÷ 100
Kn
Kd = 13×5×254
72000×100 = 1651
720000
In this case, an alarm is issued because Kd exceeds the
specifiable range.
- Example 2)
Based on the controlled axis configuration described in Fig. 21.7.4.3
(a), suppose that the spindle and V-axis are as follows:
Spindle pulse coder : 72000pulse/rev (4 pulses for one
A/B phase cycle)
C-axis least command increment : 0.001deg
C-axis CMR : 1/2
V-axis least command increment : 0.001mm
V-axis CMR : 1/2
21.AXIS CONTROL FUNCTIONS PROGRAMMING B-63944EN/03
- 770 -
Then, the C-axis detection unit is 0.002 degree. The V-axis detection
unit is 0.002 mm.
In this case, the synchronization ratio (Kn, Kd) is related with a
command as indicated below. Here, let Pm and Ps be the amounts of
movements represented in the detection unit for the master axis and
slave axis specified in a synchronization start command, respectively.
(1) When the master axis is the spindle, and the slave axis is the
C-axis
(a) Command : G81.5 T1 C3.263 ;
Operation : Synchronization between the spindle and C-axis
is started at the ratio of a 3.263-degree rotation
about the C-axis per spindle rotation.
Pm : (Number of pulses per spindle rotation) × (one
rotation) → 72000 × 1
Ps : (Amount of C-axis movement) × CMR →
3263 × 1 ÷ 2
Kn
Kd = 3263×1
72000×2 = 3263
144000
In this case, an alarm is issued because Kd exceeds the
specifiable range.
(b) Command : G81.5 T1 C3.26 ;
The value specified for C slightly differs from
that specified for C in (a).
Operation : Synchronization between the spindle and C-axis
is started at the ratio of a 3.26-degree rotation
about the C-axis per spindle rotation.
Pm : (Number of pulses per spindle rotation) × (one
rotation) → 72000 × 1
Ps : (Amount of C-axis movement) × CMR →
3260 × 1 ÷ 2
Kn
Kd = 3260×1
72000×2 = 163
7200
(a) causes an alarm to be output because the values cannot
be reduced. (b) causes no alarm because the ratio of the
travel distances can be reduced to a simple ratio.
21.7.4.6 Retract function
See "Retract function" in the Subsection 21.7.4, "Electronic Gear
Box".
B-63944EN/03 PROGRAMMING 21.AXIS CONTROL FUNCTIONS
- 771 -
21.8 TANDEM CONTROL
When enough torque for driving a large table cannot be produced by
only one motor, two motors can be used for movement along a single
axis.Positioning is performed by the main motor only. The submotor
is used only to produce torque. With this tandem control function, the
torque produced can be doubled.
Table
Ball screw
Main motor
Sub motor
Fig. 21.8 (a) Example of operation
In general, the NC regards tandem control as being performed for one
axis. However, for servo parameter management and servo alarm
monitoring, tandem control is regarded as being performed for two
axes.
For details, refer to the relevant manual published by the machine tool
builder.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 772 -
22 5-AXIS MACHINING FUNCTION
Chapter 22, "5-AXIS MACHINING FUNCTION", consists of the
following sections:
22.1 TOOL CENTER POINT CONTROL ....................................773
22.2 TOOL POSTURE CONTROL ...............................................828
22.3 TILTED WORKING PLANE COMMAND..........................838
22.4 INCLINED ROTARY AXIS CONTROL..............................894
22.5 3-DIMENSIONAL CUTTER COMPENSATION ................897
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 773 -
22.1 TOOL CENTER POINT CONTROL
Overview
On a 5-axis machine having two rotary axes that turn a tool or table,
this function performs tool length compensation constantly, even in
the middle of a block, and exerts control so that the tool center point
moves along the specified path. (See Fig. 22.1 (a).)
There are three different types of 5-axis machines - <1> those that
rotate the tool only, <2> those that rotate the table only, and <3> those
that rotate both the tool and table. (See Fig. 22.1 (d).)
This function is intended to perform machining on such 5-axis
machines having rotary axes that turn a tool or table as well as three
orthogonal axes (X-, Y-, and Z-axes) by accomplishing tool length
compensation while changing the attitude of the tool. It enables the
tool center point to move along the specified path even if the tool's
direction changes with respect to the workpiece.
A coordinate system used for programming the tool center point
control is called the programming coordinate system.
A coordinate system fixed on the table can be used as the
programming coordinate system, which makes CAM programming
easy. This coordinate system is particularly called the table
coordinate system.
A workpiece coordinate system fixed on a machine coordinate system
can be employed as the programming coordinate system as well.
In any case, the cutting speed can be controlled easily because the tool
center point moves at a specified speed with respect to the table
(workpiece).
The commands that can be issued during tool center point control are
positioning (G00), linear interpolation (G01), circular interpolation
(G02, G03), and helical interpolation (G02, G03).
Program-specified
path
Control
point Tool length
vector
Tool center
point
Fig. 22.1 (a) Path of the tool center point
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 774 -
X'
Y'
Z'
B
A
X'
Y' Z'
Tool center point path
Y'
X'
Z'
Fig. 22.1 (b) Path of the tool center point
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 775 -
When a coordinate system fixed on the table is used as the
programming coordinate system, programming can be performed
without worrying about the rotation of the table because the
programming coordinate system does not move with respect to the
table, although the position and direction of the workpiece fixed on
the table change due to its rotation. When a straight line is specified,
the tool center point moves along a straight path with respect to the
workpiece as instructed. (See Fig. 22.1 (b).)
By setting the relevant parameter, the workpiece coordinate system
can also be employed as the programming coordinate system. In this
case, as the table turns, the position and direction of the workpiece
fixed on the table change with respect to the programming coordinate
system. It is therefore necessary to take into account the rotation of
the table when specifying the end point. In this case, too, when a
straight line is specified, the tool center point moves along a straight
path with respect to the workpiece as instructed.
Fig. 22.1 (c) illustrates how linear interpolation is accomplished with a
composite type machine, showing the relationship between the case
when a table-fixed coordinate system is used as the programming
coordinate system and the case when the workpiece coordinate system
is used. If linear interpolation is specified in this function mode,
speed control is exerted in such a way that the tool center point moves
at a specified speed with respect to the workpiece.
Example)
Machine configuration: The A-axis is the rotation axis for controlling the tool.
The B-axis is the rotation axis for controlling the table.
Program: Created using the programming coordinate system.
X'
Y'
Z'
Workpiece coordinate
system used when tool
center point control starts
B
A
Specified
start point
Specified end-point vector resulting when
a table-fixed coordinate system is used as
the programming coordinate system
The cutting path is straight
Workpiece
coordinate
system (It
doesn’t move
even if the
B-axis rotates.)
Specified end-point vector resulting when
a workpiece coordinate system is used as
the programming coordinate system
X'
Y'
Z'
X”
Y”
Z"
Coordinate system fixed on the table
X”
Z"
Y”
Fig. 22.1 (c) Linear interpolation with a composite type machine
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 776 -
<2> Table rotation type machine
<3> Composite type machine
<1> Tool rotation type machine
X
C
B
Z
Y
B
C
X
Z
Y
B
Y
X
Z
C
Fig. 22.1 (d) Three types of 5-axis machine
Even if the rotary axis that controls the tool does not intersect the one
that controls the table, this function can still be used.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 777 -
There are two types, as described below, one of which is used
depending on how the direction of the tool axis is specified.
(1) Type 1
The block end point of the rotary axes is specified (e.g. A, B, C).
The CNC performs tool length compensation by the specified
amount in the tool axis direction that is calculated from the
specified position of the rotary axes and exerts control so that the
tip of the tool moves along the specified path.
(2) Type 2
The direction of the tool axis (I, J, K) at the block end point, as
seen from the coordinate system fixed on the table, is specified,
instead of the position of the rotary axes.
The CNC calculates an end point of the rotary axes where the
tool will face the specified direction, performs tool length
compensation by the specified amount in the tool axis direction
that is calculated from the position of the rotary axes, and exerts
control so that the tip of the tool moves along the specified path.
Format
- Positioning and linear interpolation for tool center point control (type 1)
G43.4 IP_ α_ β_ H_ ; Starts tool center point control (type 1).
IP_ α_ β_ ;
:
IP : In the case of an absolute programming, the coordinate
value of the end point of the tool tip movement
In the case of an incremental programming, the amount of
the tool tip movement
α, β : In the case of an absolute programming, the coordinate
value of the end point of the rotary axes
In the case of an incremental programming, the amount of
the rotary axis movement
H : Tool offset number
Movement to the position specified by the G43.4 block (startup) does
not constitute tool center point control. Only tool length
compensation is performed.
As for rotary axes, either table rotation axes or tool rotation axes are
specified.
While performing interpolation for the rotary axes, the CNC controls
the control points so that the tool center point moves along a straight
line with respect to the table (workpiece). The end of the tool center
point comes to the point specified on the programming coordinate
system.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 778 -
- Positioning and linear interpolation for tool center point control (type 2)
G43.5 IP_ H_ Q_ ; Starts tool center point control (type 2).
IP_ I_ J_ K_ ;
:
IP : In the case of an absolute programming, the
coordinate value of the end point of the tool tip
movement
In the case of an incremental programming, the
amount of the tool tip movement
I, J, K : Tool axis direction at the block end point as seen from
the programming coordinate system
H : Tool offset number
Q : Inclination angle of the tool (in degrees)
Movement to the position specified by the G43.5 block does not
constitute tool center point control. Only tool length compensation is
performed.
No rotary axes are specified. Instead, the direction of the tool end
point is specified as I, J, K, as seen from the programming coordinate
system (the one fixed on the table when G43.5 is specified).
With a tool rotation type machine, I, J, K can be specified using the
G43.5 block. In the case of a table rotation type or composite type
machine, however, these cannot be specified. Specifying them with
a table rotation type or composite type machine causes alarm PS5421.
While performing interpolation for the rotary axes, the CNC controls
the control points so that the tool center point moves along a straight
line with respect to the table (workpiece). The end of the tool center
point comes to the point specified on the programming coordinate
system.
CAUTION
1 If one or two of the I, J, and K values are omitted, the
omitted value or values are considered to be 0.
2 In a block in which I, J, and K are all omitted, the
compensation vector of the preceding block is used.
3 This block can be used only when the programming
coordinate system is fixed on the table (when the bit 5
(WKP) of parameter No.19696 is set to 0). Specifying
G43.5 when bit 5 (WKP) of parameter No.19696 is set
to 1 causes alarm PS5459.
4 Type 2 cannot be used when there is only one rotary
axis or when any hypothetical axis is used. Specifying
G43.5 in such a case causes alarm PS5459.
5 When using the rotary axis rollover function or the
rotary axis control function, set parameter No.1260
(amount of movement per rotation of the rotary axis) to
360 degrees.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 779 -
- Circular interpolation for tool center point control (type 1)
G43.4 IP_ H_ ; Starts tool center point control (type 1).
:
G17 : X-Y plane of the table coordinate system
G18 : Z-X plane of the table coordinate system
G19 : Y-Z plane of the table coordinate system
G02 : Clockwise (CW) circular interpolation
G03 : Counterclockwise (CCW) circular interpolation
IP : In the case of an absolute programming, the
coordinate value of the end point of the tool tip
movement
In the case of an incremental programming, the
amount of the tool tip movement
(This pertains only to two axes on the plane.)
I, J, K : Specify the distance between the start point in the
rotary axis position of the block start point and the
center of the arc, as seen from the programming
coordinate system.
R : Arc radius R > 0: The center angle of the arc is less
than 180°.
R < 0: The center angle of the arc is
more than 180°.
α, β : In the case of an absolute programming, the
coordinate value of the end point of the rotary axis
In the case of an incremental programming, the
amount of the rotary axis movement
F : Specified speed (speed in the tangent direction of the
arc as seen from the table coordinate system)
H : Tool offset number
Movement to the position specified by the G43.4 block does not
constitute tool center point control. Only tool length compensation is
performed. While performing interpolation for the rotary axes, the
CNC controls the control points so that the tool center point moves
along an arc with respect to the table (workpiece). The end of the
tool center point comes to the point specified on the programming
coordinate system.
CAUTION
Any command that does not move the tool center point
with respect to the workpiece (one that moves the rotary
axes only) must be executed in G00 or G01 mode.
G02 I J K
G17 IP α β F ;
G03 R
G02 I J K
G18 IP α β F ;
G03 R
G02 I J K
G19 IP α β F ;
G03 R
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 780 -
- Circular interpolation for tool center point control (type 2)
G43.5 IP_ H_ Q_ ; Starts tool center point control (type 2).
:
G17 : X-Y plane of the table coordinate system
G18 : Z-X plane of the table coordinate system
G19 : Y-Z plane of the table coordinate system
G02 : Clockwise (CW) circular interpolation
G03 : Counterclockwise (CCW) circular interpolation
IP : In the case of an absolute programming, the
coordinate value of the end point of the tool tip
movement
In the case of an incremental programming, the
amount of the tool tip movement
(This pertains only to two axes on the plane.)
I, J, K : Tool axis direction at the block end point as seen from
the programming coordinate system
R : Arc radius R > 0: The center angle of the arc is less
than 180°.
R < 0: The center angle of the arc is
more than 180°.
F : Specified speed (speed in the tangent direction of the
arc as seen from the table coordinate system)
H : Tool offset number
Q : Inclination angle of the tool (in degrees)
Movement to the position specified by the G43.5 block does not
constitute tool center point control. Only tool length compensation is
performed.
No rotary axes are specified. Instead, the direction of the tool end
point is specified as I, J, K, as seen from the programming coordinate
system (the one fixed on the table when G43.5 is specified).
With a tool rotation type machine, I, J, K can be specified using the
G43.5 block. In the case of a table rotation type or composite type
machine, however, these cannot be specified. Specifying them with
a table rotation type or composite type machine causes alarm PS5421.
While performing interpolation for the rotary axes, the CNC controls
the control points so that the tool center point moves along an arc with
respect to the table (workpiece). The end of the tool center point
comes to the point specified on the programming coordinate system.
G02
G17 IP I J K R F ;
G03
G02
G18 IP I J K R F ;
G03
G02
G19 IP I J K R F ;
G03
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 781 -
CAUTION
1 Only arc radius R can be specified. (The distance
from the start point to the center of the arc cannot
be specified using I, J, and K.)
2 A round circle (the start point and end point are the
same) cannot be specified.
Any command that does not move the tool center
point with respect to the workpiece (one that moves
the rotary axes only) must be executed in G00 or
G01 mode.
3 See the CAUTION box for tool center point control
(type 2).
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 782 -
- Helical interpolation for tool center point control (type 1)
G43.4 IP_ H ; Starts tool center point control (type 1).
:
G17 : X-Y plane of the table coordinate system
G18 : Z-X plane of the table coordinate system
G19 : Y-Z plane of the table coordinate system
G02 : Clockwise (CW) circular interpolation
G03 : Counterclockwise (CCW) circular interpolation
IP : In the case of an absolute programming, the
coordinate value of the end point of the tool tip
movement
In the case of an incremental programming, the
amount of the tool tip movement
(This pertains only to two axes on the plane.)
I, J, K : Specify the distance between the start point in the
rotary axis position of the block start point and the
center of the arc, as seen from the programming
coordinate system.
R : Arc radius R > 0: The center angle of the arc is less
than 180°.
R < 0: The center angle of the arc is
more than 180°.
α, β : In the case of an absolute programming, the
coordinate value of the end point of the rotary axis
In the case of an incremental programming, the
amount of the rotary axis movement
γ : In the case of an absolute programming, the
coordinate value of the end point of the tool tip
movement
In the case of an incremental programming, the
amount of the tool tip movement
(This pertains only to one of the linear axes subject to
tool center point control which does not exist on the
plane. Linear interpolation is performed
simultaneously with circular interpolation.)
F : Specified speed (speed in the tangent direction of the
arc as seen from the table coordinate system)
H : Tool offset number
G02 I
J K
G17 IP α β γ F ;
G03 R
G02 I J K
G18 IP α β γ F ;
G03 R
G02 I J K
G19 IP α β γ F ;
G03 R
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 783 -
Movement to the position specified by the G43.4 block does not
constitute tool center point control. Only tool length compensation is
performed.
Because the specified speed is usually the speed in the tangent
direction of the arc, the speed of the linear axis, when seen from the
table coordinate system, is: arc theofLength
axislinear theofLength
×F.
Depending on bit 5 (HTG) of parameter No.1403, the specified speed
varies as shown in the following table.
Bit 5 (HTG) of parameter No.1403
0 1
Tangential speed of the arc Synthetic speed of the linear axis
speed and tangential speed
While performing interpolation for the rotary axes, the CNC controls
the control points so that the tool center point moves helically with
respect to the table (workpiece). The end of the tool center point
comes to the point specified on the programming coordinate system.
CAUTION
Any command that does not move the tool center
point with respect to the workpiece (one that moves
the rotary axes only) must be executed in G00 or
G01 mode.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 784 -
- Helical interpolation for tool center point control (type 2)
G43.5 IP_ H_ Q_; Starts tool center point control (type 2).
:
G17 : X-Y plane of the table coordinate system
G18 : Z-X plane of the table coordinate system
G19 : Y-Z plane of the table coordinate system
G02 : Clockwise (CW) circular interpolation
G03 : Counterclockwise (CCW) circular interpolation
IP : In the case of an absolute programming, the
coordinate value of the end point of the tool tip
movement
In the case of an incremental programming, the
amount of the tool tip movement
(This pertains only to two axes on the plane.)
I, J, K : Tool axis direction at the block end point as seen from
the programming coordinate system
R : Arc radius R > 0: The center angle of the arc is less
than 180°.
R < 0: The center angle of the arc is
more than 180°.
γ : In the case of an absolute programming, the
coordinate value of the end point of the tool tip
movement
In the case of an incremental programming, the
amount of the tool tip movement
(This pertains only to one of the linear axes subject to
tool center point control which does not exist on the
plane. Linear interpolation is performed
simultaneously with circular interpolation.)
F : Specified speed (speed in the tangent direction of the
arc as seen from the table coordinate system)
H : Tool offset number
Q : Inclination angle of the tool (in degrees)
G02
G17 IP I J K R γ F ;
G03
G02
G18 IP I J K R γ F ;
G03
G02
G19 IP I J K R γ F ;
G03
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 785 -
Movement to the position specified by the G43.5 block does not
constitute tool center point control. Only tool length compensation is
performed.
Because the specified speed is the speed in the tangent direction of the
arc, the speed of the linear axis, when seen from the table coordinate
system, is: arc theofLength
axislinear theofLength
×F.
Depending on bit 5 (HTG) of parameter No.1403, the specified speed
varies as shown in the following table.
Bit 5 (HTG) of parameter No.1403
0 1
Tangential speed of the arc Synthetic speed of the linear axis
speed and tangential speed
No rotary axes are specified. Instead, the direction of the tool end
point is specified as I, J, K, as seen from the programming coordinate
system (the one fixed on the table when G43.5 is specified).
With a tool rotation type machine, I, J, K can be specified using the
G43.5 block. In the case of a table rotation type or composite type
machine, however, these cannot be specified. Specifying them with
a table rotation type or composite type machine causes alarm PS5421.
While performing interpolation for the rotary axes, the CNC controls
the control points so that the tool center point moves helically with
respect to the table (workpiece). The end of the tool center point
comes to the point specified on the programming coordinate system.
CAUTION
1 Only arc radius R can be specified. (The distance
from the start point to the center of the arc cannot
be specified using I, J, and K.)
2 A round circle cannot be specified.
3 Any command that does not move the tool center
point with respect to the workpiece (one that moves
the rotary axes only) must be executed in G00 or
G01 mode.
4 See the CAUTION box for tool center point control
(type 2).
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 786 -
- Tool center point control cancellation command
G49 IP_ α_ β_ ; Cancels tool center point control.
IP : In the case of an absolute programming, the
coordinate value of the end point of the tool control
point movement
In the case of an incremental programming, the
amount of the tool control point movement
α, β : In the case of an absolute programming, the
coordinate value of the end point of the rotary axes
In the case of an incremental programming, the
amount of the rotary axis movement
The cancellation block for tool center point control is the one that
controls buffering.
B
Control point:
Control target on the
machine coordinate system
Tool center point Tool offset value
Fig. 22.1 (e) Control point and tool center point
CAUTION
The G49 command must be executed in G00 or
G01 mode.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 787 -
- Inclination angle of the tool
In the case of tool center point control of type 2, the inclination angle
of the tool can be specified using address Q of G43.5. The
inclination angle of the tool represents how inclined the tool direction
is toward the proceeding direction with respect to the direction
specified by (I, J, K) at the time of machining on the plane produced
by the tool direction specified by (I, J, K) and the proceeding direction
on the programming coordinate system. (See the figure below.)
Overviewly, the normal direction on the machining plane is specified
by (I, J, K). If the tool direction needs to be inclined toward the
proceeding direction with respect to the normal direction at the time of
machining, perform compensation using Q.
If the direction specified by (I, J, K) matches the direction in which
the tool moves at the time of machining, commanding Q is
unnecessary.
Tool direction specified by (I, J, K) Tool direction at the time of machining
Proceeding
direction
Inclination angle of the tool
Example)
To incline the tool by two degrees toward the proceeding
direction at the time of machining, enter the following command:
G43.5 I_ J_ K_ H_ Q2.0
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 788 -
Explanation
- When a coordinate system fixed on the table is used as the programming
coordinate system
The programming coordinate system is used for tool center point
control. When the G43.4 or G43.5 command is specified with bit 5
(WKP) of parameter No.19696 set to 0, the workpiece coordinate
system that is fixed on the table at that point of time becomes the
programming coordinate system. Thereafter, the programming
coordinate system rotates as the table turns around.
It does not rotate with the tool head.
X, Y, and Z mentioned hereinafter are assumed to be commanded on
the programming coordinate system.
When the G43.4 or G43.5 command is specified or when the rotary
axis of the table has moved in a block preceding G43.4 or G43.5, the
angle of the table's rotary axis represents the initial state of the
programming coordinate system.
In the case of type 2, the tool direction seen from the coordinate
system that is fixed on the table is specified by I, J, K.
In the descriptions that follow, the table-fixed coordinate system is
represented by X', Y', and Z'.
When G43.4 or G43.5 is
specified with C = 0
d
Tool center point control
in progress
X'
Y'
Workpiece
coordinate
system
0
45
X'
Y'
C
Programming
coordinate system
45
Tool center point control in
p
ro
g
ress
C-axis reference position
X'
Y'
45
90
Workpiece
coordinate
system
When G43.4 or G43.5 is
specified with C = 45 degrees
X'
C
Programming
coordinate system
90
45
The C-axis reference position is the position where a movement is
made on the C-axis so that a command value for the C-axis is at the
scale position on the table.
Y'
Fig. 22.1 (f) Programming coordinate system fixed on the table
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 789 -
- When the workpiece coordinate system is used as the programming coordinate
system
When the G43.4 command is specified with bit 5 (WKP) of parameter
No.19696 set to 1, the workpiece coordinate system that is in use at
that point of time becomes the programming coordinate system.
In this case, the programming coordinate system does not rotate as the
table turns around but remains fixed on the workpiece coordinate
system.
Hereinafter, when X, Y, and Z are commanded, the tool moves along
a straight line toward the table (workpiece). For X, Y, Z, specify the
end point location after the rotation of the table, as seen from the
programming coordinate system.
Type 2 cannot be used. Specifying G43.5 when bit 5 (WKP) of
parameter No.19696 set to 1 causes alarm PS5459.
In the descriptions that follow, the coordinate values of the workpiece
coordinate system used as the programming coordinate system are
represented by X", Y", and Z".
When G43.4 is specified
with C = 0 degrees Tool center point control
in progress
X"
Y"
Workpiece
coordinate
system
0
45
C
Programming
coordinate
system
45
Tool center point control in
progress
C-axis reference position
45
90
Workpiece
coordinate
system X"
Y"
When G43.4 is specified with
C = 45 degrees
C
Programming
coordinate
system 90
45
X"
Y"
X"
Y"
The C-axis reference position is the position where a movement is made on the
C-axis so that a command value for the C-axis is at the scale position on the
table.
Fig. 22.1 (g) Programming coordinate system identical to the
workpiece coordinate system
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 790 -
- Notes on performing circular interpolation and helical interpolation when using
the workpiece coordinate system as the programming coordinate system
• The start point, end point, and center of an arc change as the
table rotation axis rotates.
• I, J, K commands the vector of the block start point to the center
of the arc from the start point in the rotary axis position.
• Note the following:
<1> Only a table rotation axis normal to a selected plane can be
rotated during circular interpolation.
<2> During circular interpolation, those table rotation axes not
normal to a selected plane must continue to be at the same
position as when tool center point control is started.
If <1> or <2> is not satisfied, the alarm PS5421 is issued.
No restriction is imposed on rotation on a tool rotation axis.
- Program examples
• In the case of a composite type machine
Descriptions are based on the following machine configuration.
C-axis
Center of C-axis rotation
Z-axis
Y- a xi s
X-axis B-axis
Center of B-axis rotation
Tool center point
Workpiece
coordinate system
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 791 -
When the G17 (X-Y plane) command is executed
After the G43.4 command, the X-Y plane is selected using the G17
command and circular interpolation is performed by rotating the
C-axis (table rotation axis) (including those cases where the C-axis
moves before the G43.4 command). → This case corresponds to <1>
and allows circular interpolation.
Example)
:
(G01 C90. ;)
G43.4 H1 ;
G17 G02 IP IR B10. C20. ;
:
IP: Coordinates of the end point
IR: Arc radius
When the G18 (Z-X plane) or G19 (Y-Z plane) command is executed
After the G43.4 command, the Z-X plane is selected using the G18
command and circular interpolation is performed without rotating the
C-axis (including those cases where the C-axis moves before the
G43.4 command). → This case corresponds to <2> and allows
circular interpolation.
The same is also true when the G19 command is used.
Example)
:
(G01 C90. ;)
G43.4 H1 ;
G18 G02 IP IR ;
:
After the G43.4 command, the Z-X plane is selected using the G18
command and the C-axis is rotated during circular interpolation . →
Alarm (violation of <2>)
The same is also true when the G19 command is used.
Example)
:
G43.4 H1 ;
G18 G02 IP IR C20. ;
:
After the G43.4 command, the Z-X plane is selected using the G18
command and circular interpolation is performed after rotating the
C-axis. → Alarm (violation of <2>)
The same is also true when the G19 command is used.
Example)
:
G43.4 H1 ;
G01 C10.
G18 G02 IP IR ;
:
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 792 -
• In the case of a table rotation type machine
Descriptions are based on the following machine configuration.
A table rotation type machine can be considered equivalent to a
composite type machine if any of its two table rotation axes does
not move.
C
Y
Z
A
Workpiece coordinate
system
X
When the G17 (X-Y plane) command is executed
The master axis (A-axis) moves before the G43.4 command and, after
the G43.4 command, circular interpolation is performed without
rotating the A- or C-axis (including those cases where the C-axis
moves before the G43.4 command). → This case corresponds to
<2> and allows circular interpolation.
Example)
:
G01 A90. (C10.);
G43.4 H1 ;
G17 G02 IP IR ;
:
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 793 -
The master axis (A-axis) moves before the G43.4 command and, after
the G43.4 command, circular interpolation is performed using the G17
(X-Y plane) command by rotating the C-axis, or the C-axis is rotated
during circular interpolation. → Alarm (violation of <2>)
Example)
:
G01 A90.;
G43.4 H1 ;
G01 C10. ;
G17 G02 IP IR ;
:
:
G01 A90.;
G43.4 H1 ;
G17 G02 IP IR C10.;
:
After the G43.4 command, the A-axis is moved and circular
interpolation is performed using the G17 command (X-Y plane). →
Alarm (violation of <2>)
Example)
:
G43.4 H1 ;
G01 A10. ;
G17 G02 IP IR C10.;
:
G19 (Y-Z plane) command is executed
The G43.4 command is executed after moving the A-axis and circular
interpolation is performed while rotating the A-axis using the G19
(Y-Z plane) command. → This case corresponds to <1> and
allows circular interpolation.
Example)
:
G01 A90. ;
G43.4 H1 ;
G19 G02 IP IR A10. ;
:
After the G43.4 command, the C-axis is rotated and circular
interpolation is performed using the G19 (Y-Z plane) command. →
Alarm (violation of <2>)
Example)
:
G43.4 H1 ;
G01 C10. ;
G19 G02 IP IR ;
:
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 794 -
When the G18 (Z-X plane) command is executed
The G43.4 command is executed after moving the A- and C-axes, and
circular interpolation is performed using the G18 (Z-X plane)
command without moving any rotary axis. → This case corresponds
to <2> and allows circular interpolation.
Example)
:
G01 A90. C10. ;
G43.4 H1 ;
G18 G02 IP IR;
:
After the G43.4 command, circular interpolation is performed using
the G18 command (Z-X plane) by moving any of the rotary axes. →
Alarm (violation of <2>)
Example)
:
G43.4 H1 ;
G01 A10. (C10.)
G18 G02 IP IR;
:
- Tool center point control command
During tool center point control, the command specifies the location
of each block end point as seen from the programming coordinate
system.
The program specifies the tool center point.
As for the rotary axis, the command specifies the coordinate values of
each block end point in the case of type 1 or the tool direction at each
block end point in the case of type 2.
The feedrate is specified by the tangential speed relative to the
workpiece (the tool's relative speed as opposed to the workpiece),
which is represented by F.
- Commands that can be specified during tool center point control
The commands that can be specified during tool center point control
are linear interpolation (G01), positioning (G00), circular
interpolation (G02, G03), and helical interpolation (G02, G03).
When linear interpolation (G01) is specified during tool center point
control, speed control is exerted so that the tool center point moves at
the specified speed.
The circular interpolation command (G02, G03) controls the
tangential speed of the arc path along which the tool center point
moves.
The helical interpolation command (G02, G03) controls the tangential
speed of the arc path along which the tool center point moves or a
synthetic speed including that of the helical axis. (This is dependent
on the setting of bit 5 (HTG) of parameter No.1403.)
As the actual speed, the speed at the control point is shown.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 795 -
NOTE
When the tool center point control mode is entered,
acceleration/deceleration before look ahead
interpolation is enabled automatically. Be sure to
specify the following parameters:
(1) Bit 1 (LRP) of parameter No.1401=1 :
Linear rapid traverse
(2) Bit 5 (FRP) of parameter No.19501=1 :
Acceleration/deceleration before interpolation
is used for rapid traverse.
(3) Parameter No.1671 :
Acceleration before interpolation for rapid
traverse.
(4) Parameter No.1672 :
Change time for bell-shaped acceleration
before interpolation for rapid traverse.
(5) Parameter No.1660 :
Maximum permissible acceleration for
acceleration/deceleration before interpolation
If they are not specified, alarm PS5420 is
generated.
- Rotary axis command
If a command is specified during tool center point control that
prohibits the tool center point from moving with respect to the
workpiece, the maximum cutting speed (parameter No.1430) is
assumed as the feedrate of the rotary axis when bit 6 (RFC) of
parameter No.19696 is 0, and the speed specified by F is assumed
when bit 6 (RFC) of parameter No.19696 is 1.
The rotary axis command cannot be specified during tool center point
control of type 2. Specifying the command with type 2 causes alarm
PS5421.
- The moving distance of the rotary axis is long compared to that of the linear axis
If the moving distance of the rotary axis is long compared to that of
the linear axis, the rotary axis moves faster so that the tool center
point moves at the specified speed, possibly resulting in the tool
center point traveling on an inadequate path.
In such a case, it is possible to exert control to slow down the speed
and ensure that the tool center point travels on the specified path, by
setting bit 6 (CRS) of parameter No.19746 to 1. When using this
control, specify in parameter No.19751 (for rapid traverse) and
parameter No.19752 (for cutting feed) the extent of deviation of the
path at which the speed is to be slowed down (maximum allowable
deviation of the path). When 0 is specified, the least input increment
is regarded as the maximum allowable deviation of the path.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 796 -
- Tool behavior at startup and cancellation
When tool center point control is started (G43.4/G43.5) or canceled
(G49), the tool moves by a tool offset value.
Compensation vector calculation is performed only at the end of a
block.
- Current position display during tool center point control
During tool center point control, the position of the control point
(rotation center of the tool rotation axis) is displayed as the machine
coordinate.
When bit 5 (WKP) of parameter No.19696 is 0, whether to use
absolute or relative coordinates can be selected using bit 2 (DET) of
parameter No.19608.
If bit 2 (DET) of parameter No.19608 is 0, the position of the tool
center point on the programming coordinate system is displayed.
If bit 2 (DET) of parameter No.19608 is 1, the position of the tool
center point in the workpiece coordinate system is displayed.
- Tool offset
If tool offsets are used based on tool numbers, tool center point
control is carried out using the tool length compensation value
corresponding to the relevant tool number (T code).
If tool life management is used, tool center point control is carried out
using the tool length compensation value corresponding to the tool in
use.
- Function for placing priority on the path rather than on speed
If, in a block specifying a movement on a rotary axis, a high speed
(speed command or rapid traverse rate) is specified or the travel
distance on the rotary axis is larger than the travel distance of the tool
center point, an excessive path deviation can occur in the middle of
the block when a movement is made by the specified speed.
In such a case, priority can be placed on the path instead of the speed
so that the speed can be automatically lowered to prevent a deviation
from the path.
This function is enabled by setting bit 6 (CRS) of parameter No.
19746 to 1.
Set a maximum allowable path deviation in parameter No. 19751 (for
rapid traverse) or in parameter No. 19751 (for cutting feed).
When 0 is set as a maximum allowable path deviation, the
specification of the minimum unit of setting data of the parameter is
assumed.
When a negative value is set, the function for placing priority on the
path is disabled.
When a judgment is made to lower the speed, the speed of the entire
block is lowered.
As a result of speed reduction, the path error may be smaller than a
parameter-set value due to a calculation error.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 797 -
- Canned cycle during tool center point control
When bit 5 (TFA) of parameter No. 5105 is set to 1, if a canned cycle
being subjected to tool center point control is performed when the
position of the rotation axis that determines the tool axis direction is
not ±90° × n (n=0, 1, 2...) on the workpiece coordinate system, alarm
PS5424 (invalid tool axis direction) occurs.
CAUTION
A canned cycle being subjected to tool center point
control operates in the direction of the program
coordinate system. It does not always operates in
the current tool axis direction.
Be extremely careful about programming.
- Tool retract and recover during tool center point control
A tool retract and recover operation can be performed during tool
center point control. A retract operation is performed in the tool axis
direction by setting a tool axis direction retract amount in parameter
No. 11261.
This function is enabled on a machine of head rotation type.
For tool retract and recover operation, refer to "TOOL RETRACT
AND RECOVER" in Part for Operation.
Tool axis direction retract operation is enabled under the following
conditions:
1. The G10.6 command is singly executed (no axis address is
specified in the block specifying G10.6).
2. Bit 2 (RPS) of parameter No. 7040 is set to 1.
3. Tool center point control or workpiece setting error
compensation are being exercised. (However, bit 0 (RCM) of
parameter No. 11200 is set to 1 to perform compensation in the
tool direction.)
4. A nonzero value is set in parameter No. 11261.
If the tool retract signal TRESC is set to 1 under the conditions above,
a retract operation is performed in the tool axis direction. Parameter
No. 11261 is used to specify a retract amount. A retract operation is
performed using the value of parameter No. 11261 as an incremental
retract amount.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 798 -
：Position where tool retract switch is on
：Retract position
：Retract position by manual operation
：Retract path (tool axis direction)
：Manual operation (retract path)
：Recover path
：Repositioning
Y
X
Z
Parameter No.11261
If the tool retract signal TRESC is set to 1 during tool center point
control when the tool axis direction retract conditions mentioned
above are not satisfied, a retract operation of the conventional type is
performed. In such a case, specify the tool center point retract
position in a G10.6 block.
G10.6 alone G10.6 X_ Y_ Z_
Bit 2 (RPS) of parameter No.7040 = 1 = 0
Parameter No.11261 ≠ 0.0 = 0.0
Tool axis direction retract Conventional retract
(Parameter No. 7041)
Retract operation is not
performed.
Conventional
retract
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 799 -
- Angle of the rotary axis for type 2 (when the movement range is not specified)
When the direction of the tool is specified by I, J, K, Q for type 2,
more than two pairs of "computed angles" of the rotary axes usually
exist.
The "computed angle" is the candidate angle at which the rotary axis
is to be controlled in the specified tool axis direction.
The "output angle" is determined from the "computed angle" based on
the "output judgment conditions" described below.
The following descriptions assume that there is no movement range
specification (parameter No.19741 - No.19744 = 0).
"Output judgment conditions"
Tool rotation type or table rotation type machine
<1> The "output angles" are represented by the computed rotary axis
angle pair whose master axis (first rotary axis) moving angle is
smaller.
↓
↓ When the master axis moving angle is the same
↓
<2> The "output angles" are represented by the computed rotary axis
angle pair whose slave axis (second rotary axis) moving angle is
smaller.
↓
↓ When the slave axis moving angle is the same
↓
<3> The "output angles" are represented by the computed rotary axis
angle pair whose master axis (first rotary axis) angle is nearer to 0
degree (multiple of 360 degrees).
↓
↓ When the master axis angle is equally near to 0 degree
↓
<4> The "output angles" are represented by the computed rotary axis
angle pair whose slave axis (second rotary axis) angle is nearer to 0
degree (multiple of 360 degrees).
Composite type machine
<1> The "output angles" are represented by the computed rotary axis
angle pair whose table (second rotary axis) moving angle is smaller.
↓
↓ When the table moving angle is the same
↓
<2> The "output angles" are represented by the computed rotary axis
angle pair whose tool (first rotary axis) moving angle is smaller.
↓
↓ When the tool moving angle is the same
↓
<3> The "output angles" are represented by the computed rotary axis
angle pair whose table (second rotary axis) angle is nearer to 0
degree (multiple of 360 degrees).
↓
↓ When the table angle is equally near to 0 degree
↓
<4> The "output angles" are represented by the computed rotary axis
angle pair whose tool (first rotary axis) angle is nearer to 0 degree
(multiple of 360 degrees).
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 800 -
The process of judging whether the moving angle is smaller or larger
as the output judgement condition is called "movement judgement."
When bit 5 (PRI) of parameter No.19608 is 1, the movement
judgements for the first rotary axis and second rotary axis are made in
reverse order.
The "movement judgement" process is explained below.
When the "computed angle" is within the range between 0 and 360
degrees, it is called the "basic computed angle."
Usually, two pairs of "basic computed angles" exist.
For example, assume that a tool rotation type or table rotation type
machine has rotary axis A (master) and rotary axis B (slave) and that
there are two pairs of basic computed angles as follows:
(A θ1 degree; B φ1 degree)
(A θ2 degrees; B φ2 degrees) where θ1 ≤ θ2.
The "computed angle" is obtained from either of the following
expressions: "basic computed angle" + 360 degrees × N or "basic
computed angle" - 360 degrees × N.
The current position of rotary axis A (master) is PA, and that of rotary
axis B (slave) is 0 degree.
Based on the PA angle, the "movement judgement" process is done as
follows (when bit 5 (PRI) of parameter No.19608 is 0).
-360
×
(N + 1) degrees
θ1 - 360 × N
-360 × N degrees
θ2 - 360 × N
θ2 - 360 × (N + 1) θ1 - 360 × (N - 1)
(*1)
0 degree 360 degrees
θ
1
θ
2
θ
2 - 360 θ1 + 360
(*2)
360 × (N + 1) degrees
θ
1 + 360
×
N
360
×
N degrees
θ
2 + 360
×
N
θ
2 + 360
×
(N - 1) θ1 + 360 × (N + 1)
(*3)
• Computed angle A
"Movement judgment"
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 801 -
When the PA angle is (*1):
The output angle is: (A θ2 - 360 × (N + 1) degrees; B φ2 degrees).
Namely, θ2 - 360 × (N + 1) degrees is adopted that is nearer to the
computed angle of A, and φ2, which is the same group as θ2, is
adopted as the computed angle of B.
When the PA angle is (*2):
The output angle is: (A θ1 degrees; B φ1 degrees).
Namely, θ1 degrees is adopted that is nearer to the computed angle of
A, and φ1, which is the same group as θ1, is adopted as the computed
angle of B.
When the PA angle is (*3):
The output angle is: (A θ + 360 × N degrees; B φ2 degrees).
Namely, θ2 + 360 × N degrees is adopted that is nearer to the
computed angle of A, and φ2, which is the same group as θ2. is
adopted as the computed angle of B.
When the moving angle of rotary axis A (master) is the same, a
"movement judgement" is made for rotary axis B (slave) according to
the "output judgment conditions."
If the "output angle" of rotary axis A is determined by the "movement
judgement" for rotary axis A, the computed angle representing the
"smaller moving angle" is adopted as the "output angle" of rotary axis
B.
Similarly, if the "output angle" of rotary axis B is determined by the
"movement judgement" for rotary axis B, the computed angle
representing the "smaller moving angle" is adopted as the "output
angle" of rotary axis A.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 802 -
The "output angle" is explained below using a tool rotation type
machine as an example.
This example illustrates a machine having a "BC type tool axis Z."
X
Y
Z
C-axis: 1st rotation axis (master)
B-axis: 2nd rotation axis
()
Fig. 22.1 (h) BC type tool axis Z
The following two pairs of "computed basic angles" exist that direct
the tool axis toward the + X axis direction.
(B 90 degrees; C 180 degrees)
(B 270 degrees; C 0 degree)
<1> When the current rotary axis angles are (B -70 degrees; C 30
degrees)
The "output angles" are (B -90 degrees; C 0 degree).
0 degree is adopted because it is nearer to the current
position (30 degrees) of the C-axis that is the master axis.
For the B-axis, 270 degrees is adopted which is the same
group. However, this is changed to -90 degrees (270
degrees - 360 degrees) which is the nearest to the current
position of the B-axis (-70 degrees).
<2> When the current rotary axis angles are (B 80 degrees; C 500
degrees)
The "output angles" are (B 90 degrees; C 540 degrees).
540 degrees (180 degrees + 360 degrees) is adopted because
it is nearer to the current position (500 degrees) of the C-axis
that is the master axis. For the B-axis, 90 degrees is
adopted which is the same group.
<3> When the current rotary axis angles are (B 60 degrees; C 90
degrees)
The "output angles" are (B 90 degrees; C 180 degrees).
Since the two candidates are equally near to the current
position (90 degrees) of the C-axis that is the master axis, a
judgment is made based on the current position of the B-axis.
90 degrees is adopted because it is nearer to the current
position (60 degrees) of the B-axis that is the slave axis.
For the C-axis, 180 degrees is adopted which is the same
group.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 803 -
<4> When the current rotary axis angles are (B 180 degrees; C 90
degrees)
The "output angles" are (B 270 degrees; C 0 degree).
Since the two candidates are equally near to the current
position (90 degrees) of the C-axis that is the master axis, a
judgment is made based on the current position of the B-axis.
In this case, however, the two candidates are also equally
near to the current position of the B-axis (180 degrees).
Therefore, the candidate is adopted in which the C-axis
(master axis) is nearer to 0 degree.
That is, the pair is adopted whose C axis angle is 0 degree
and whose B axis angle is 270 degrees.
When the slave axis angle is 0 degree, the direction of the tool axis
becomes fixed regardless of the master axis angle.
In that case, the master axis does not move from the current angle.
An explanation is shown below using a machine having a "BC type
tool axis Z" as an example.
X
Y
Z
C
Fig. 22.1 (i) BC type tool axis Z
When the current rotary axis angles are (B 45 degrees; C 90 degrees),
the "output angles" are (B 0 degree; C 90 degrees).
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 804 -
- Angle of the rotary axis for type 2 (when the movement range is specified)
If the upper and lower limits of the movement range of the rotary axis
is specified using parameters No.19741 to No.19744, the rotary axis
will move only within the specified range when the direction is
specified using I, J, K, Q command for type 2 control.
Although the procedure for determining the angles is the same as that
used "when the movement range is not specified," the "output angles"
need to be selected from those computed angles that are within the
specified movement range for both axes.
"Output judgment conditions"
Tool rotation type or table rotation type machine
<1> Of the angle pairs whose master and slave axis angles are both within
the specified movement range, the rotary axis angle pair whose
master axis (first rotary axis) moving angle is smaller represents the
"output angles."
↓
↓ When the master axis moving angle is the same
↓
<2> The "output angles" are represented by the computed rotary axis
angle pair whose slave axis (second rotary axis) moving angle is
smaller.
↓
↓ When the slave axis moving angle is the same
↓
<3> The "output angles" are represented by the computed rotary axis
angle pair whose master axis (first rotary axis) angle is nearer to 0
degree (multiple of 360 degrees).
↓
↓ When the master axis angle is equally near to 0 degree
↓
<4> The "output angles" are represented by the computed rotary axis
angle pair whose slave axis (second rotary axis) angle is nearer to 0
degree (multiple of 360 degrees).
Composite type machine
<1> Of the angle pairs whose master and slave axis angles are both within
the specified movement range, the rotary axis angle pair whose table
(second rotary axis) moving angle is smaller represents the "output
angles."
↓
↓ When the table moving angle is the same
↓
<2> The "output angles" are represented by the computed rotary axis
angle pair whose tool (first rotary axis) moving angle is smaller.
↓
↓ When the tool moving angle is the same
↓
<3> The "output angles" are represented by the computed rotary axis
angle pair whose table (second rotary axis) angle is nearer to 0
degree (multiple of 360 degrees).
↓
↓ When the table angle is equally near to 0 degree
↓
<4> The "output angles" are represented by the computed rotary axis
angle pair whose tool (first rotary axis) angle is nearer to 0 degree
(multiple of 360 degrees).
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 805 -
When bit 5 (PRI) of parameter No.19608 is 1, the movement
judgements for the first rotary axis and second rotary axis are made in
reverse order.
CAUTION
1 If the lower limit of the movement range is larger
than the upper limit, alarm PS5459 occurs when
G43.5 is specified.
2 If no "computed angle" is found within the
movement range because the range is too small,
alarm PS5459 occurs.
3 If 0 is set for both parameters that specify the
upper and lower limits of the movement range, the
tool operates assuming that there is no range
specification.
4 When the rotary axis rollover function or rotary axis
control function is used (in which case, set
parameter No.1260 (amount of movement per
rotation of the rotary axis) to 360 degrees), the tool
does not move beyond 0 degree (360 degrees)
(does not take the shortcut) if the movement range
is set between 0 and 360 degrees. Also, do not
specify a negative value or a value larger than 360
degrees for the movement range.
An example of the "movement judgement" process is given below.
Assume that a tool rotation type or table rotation type machine has
rotary axis A (master) and rotary axis B (slave) and that there are two
pairs of basic computed angles as follows:
(A θ1 degree; B φ1 degree)
(A θ2 degrees; B φ2 degrees) where θ1 ≤ θ2.
The "computed angle" is obtained from either of the following
expressions: "basic computed angle" + 360 degrees × N or "basic
computed angle" - 360 degrees × N.
Assume that the current positions and movement ranges of rotary axis
A (master) and rotary axis B (slave) are as shown in the following
figure.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 806 -
360 × (N + 1) degrees
360
×
N degrees
• Computed angle A
Current position A
Movement range A
θ1 + 360 × N θ2 + 360 × N
θ2 + 360 × (N - 1) θ1 + 360 × (N + 1)
"Computed angle of rotary axis A and its current position and movement
range"
360 × (N + 1) degrees
360 × N degrees
• Computed angle B
Current position B
Movement range B
φ2 + 360 × N
φ
1 + 360
×
N
φ1 + 360 × (N - 1) φ2 + 360 × (N + 1)
"Computed angle of rotary axis B and its current position and movement
range"
When the two axes have a positional relationship as shown in the
figure, the output angle of rotary axis A is (θ2 + 360 × N) degrees and
that of rotary axis B is (φ2 + 360 × N) degrees (when bit 5 (PRI) of
parameter No.19608 is set to 0).
More concretely, from the computed angles obtained for rotary axis A,
the nearest angle within the movement range, i.e. θ2 + 360 × N
degrees, is first adopted. Then, from the computed angles obtained
for rotary axis B, the angle belonging to the same group as θ2, i.e. φ2
+ 360 × N, is adopted.
Note that, in this example, the output angles and moving direction
differ depending on whether the movement range is specified or not (0
to 360 degrees), even if N is set to 0 and coordinates are rounded to 0
to 360 degrees.
Namely, if the movement range is not specified, θ1 + 360 degrees
nearest to the current position is adopted as the computed angle for
rotary axis A and, from the computed angles belonging to the same
group as θ1, φ1 degrees nearest to the current position is adopted as
the computed angle for rotary axis B. Rotary axis A moves in the
plus direction. As its coordinate is rounded to 360 degrees, rotary
axis A reaches θ1 degrees while moving in the plus direction.
By contrast, when the movement range is set to 0 to 360 degrees, the
output angles are (A θ2 degrees; B φ2 degrees). Neither rotary axis
A nor B moves in a way that it exceeds 0 degree (360 degrees).
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 807 -
Operation examples
- In the case of a tool rotation type machine
Explanations are given below assuming a machine configuration in
which a tool rotation axis that turns around the Y-axis is located
beneath another tool rotation axis that turns around the Z-axis. (See
Fig. 22.1 (j).)
If linear interpolation is specified for the X-, Y-, and Z-axes when a
workpiece coordinate system is used as the programming coordinate
system, control is exerted in such a way that the tool center point
moves along a specified straight line with respect to the table
(workpiece) as the tool rotates.
Also, speed control is exerted so that the tool center point moves at the
specified speed with respect to the table (workpiece).
In the case of a machine having two tool rotation axes, the table does
not rotate with respect to the workpiece coordinate system even if the
rotary axes move. Therefore, the programming coordinate system
always matches the workpiece coordinate system, regardless of
whether bit 5 (WKP) of parameter No.19696 is set to 0 or 1.
Examples)
For type 1:
O100 (Sample Program1) ;
N1 G00 G90 B0 C0 ;
N2 G55 ; Prepares the programming coordinate
system.
N3 G43.4 H01 ; Starts tool center point control.
H01 is the tool compensation number.
N4 G00 X200.0 Y150.0 Z20.0 ; Moves to the start point.
N5 G01 X5.0 Y5.0 Z5.0 C60.0 B45.0 F500 ; Linear interpolation
N6 G49; Cancels tool center point control.
N7 M30;
For type 2:
O100 (Sample Program1) ;
N1 G00 G90 B0 C0 ;
N2 G55 ; Prepares the programming coordinate system.
N3 G43.5 H01 ; Starts tool center point control.
H01 is the tool compensation number.
N4 G00 X200.0 Y150.0 Z20.0 ; Moves to the start point.
N5 G01 X5.0 Y5.0 Z5.0 I1.0 J1.732 K2.0 F500 ; Linear interpolation
N6 G49; Cancels tool center point control.
N7 M30;
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 808 -
X'
Y'
Z'
C
Control point path (of the machine
coordinate system)
Tool center point path (of the programming coordinate system)
B
X'
Y'
Z'
X'
Y'
Z'
Fig. 22.1 (j) Example for a tool rotation type machine
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 809 -
- In the case of a table rotation type machine
Explanations are given below assuming a machine configuration
(trunnion) in which a rotation table that turns around the Y-axis is
located above another table rotation axis that turns around the X-axis.
(See Fig. 22.1 (k).)
If linear interpolation is specified for the X-, Y-, and Z-axes on the
programming coordinate system and if the rotary axis that moves the
rotation table is specified (in the case of type 1) or the tool direction is
specified (in the case of type 2), control is exerted in such a way that
the tool center point moves along a specified straight line with respect
to the table (workpiece) as the rotation table rotates.
Also, speed control is exerted so that the tool center point moves at the
specified speed with respect to the table (workpiece).
Example)
When type 1 is selected and the coordinate system fixed on the table is
used as the programming coordinate system
(Bit 5 (WKP) of parameter No.19696 = 0):
O200 (Sample Program2) ;
N1 G00 G90 A0 B0 ;
N2 G55 ; Prepares the programming coordinate
system.
N3 G43.4 H01 ; Starts tool center point control.
H01 is the tool compensation number.
N4 G00 X20.0 Y100.0 Z0 ; Moves to the start point.
N5 G01 X10.0 Y20.0 Z30.0 A60.0 B45.0 F500 ; Linear interpolation
N6 G49; Cancels tool center point control.
N7 M30;
When type 1 is selected and the workpiece coordinate system is used
as the programming coordinate system
([Bit 5 (WKP) of parameter No.19696 = 1):
O200 (Sample Program2) ;
N1 G00 G90 A0 B0 ;
N2 G55 ; Prepares the programming coordinate
system.
N3 G43.4 H01 ; Starts tool center point control.
H01 is the tool compensation number.
N4 G00 X20.0 Y100.0 Z0 ; Moves to the start point.
N5 G01 X7.574 Y47.247 Z83.052 A60.0 B45.0 F500 ;
Linear interpolation
N6 G49; Cancels tool center point control.
N7 M30;
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 810 -
For type 2 (when the coordinate system fixed on the table is used as
the programming coordinate system (only when bit 5 (WKP) of
parameter No.19696 is set to 0)):
O200 (Sample Program2) ;
N1 G00 G90 A0 B0 ;
N2 G55 ; Prepares the programming coordinate
system.
N3 G43.5 H01 ; Starts tool center point control.
H01 is the tool compensation number.
N4 G00 X20.0 Y100.0 Z0 ; Moves to the start point.
N5 G01 X10.0 Y20.0 Z30.0 I-1.0 J2.449 K1.0 F500 ;
Linear interpolation
N6 G49; Cancels tool center point control.
N7 M30;
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 811 -
X'
Y'
Z'
B
A
X'
Y'
Z'
Y'
X'
Z'
Tool center point path seen from the table-fixed coordinate system
X
Z'
Y
X
Z'
Y
X
Z'
Y
Tool center point path taken when
the programming coordinate
s
y
stem does not move
Y
X
Z"
Y
XZ"
Y
XZ"
Control point path (of the machine
coordinate system)
Fig. 22.1 (k) Example for a table rotation type machine
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 812 -
- In the case of a composite type machine
Explanations are given below assuming a composite type machine
configuration that has one table rotation axis (which turns around the
X-axis) and one tool rotation axis (which turns around the Y-axis).
(See Fig. 22.1 (l).)
If linear interpolation is specified for the X-, Y-, and Z-axes on the
programming coordinate system and if the rotary axis that moves the
rotation table and the tool rotation axis are specified (in the case of
type 1) or the tool direction is specified (in the case of type 2), control
is exerted in such a way that the tool center point moves along a
specified straight line with respect to the table (workpiece) as the
rotation table and tool rotate.
Also, speed control is exerted so that the tool center point moves at the
specified speed with respect to the table (workpiece).
Example)
When type 1 is selected and the coordinate system fixed on the table is
used as the programming coordinate system
(Bit 5 (WKP) of parameter No.19696 = 0):
O300 (Sample Program3) ;
N1 G00 G90 A0 B0 ;
N2 G55 ; Prepares the programming coordinate
system.
N3 G43.4 H01 ; Starts tool center point control.
H01 is the tool compensation number.
N4 G00 X200.0 Y150.0 Z20.0 ; Moves to the start point.
N5 G01 X5.0 Y5.0 Z5.0 A60.0 B45.0 F500;
Linear interpolation
N6 G49 ; Cancels tool center point control.
N7 M30;
When type 1 is selected and the workpiece coordinate system is used
as the programming coordinate system
(Bit 5 (WKP) of parameter No.19696 = 1):
O300 (Sample Program3) ;
N1 G00 G90 A0 B0 ;
N2 G55 ; Prepares the programming coordinate
system.
N3 G43.4 H01 ; Starts tool center point control.
H01 is the tool compensation number.
N4 G00 X200.0 Y150.0 Z20.0 ; Moves to the start point.
N5 G01 X5.0 Y48.170 Z-79.772 A60.0 B45.0 F500;
Linear interpolation
N6 G49 ; Cancels tool center point control.
N7 M30;
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 813 -
For type 2 (when the coordinate system fixed on the table is used as
the programming coordinate system (only when bit 5 (WKP) of
parameter No.19696 is set to 0)):
O300 (Sample Program3) ;
N1 G00 G90 A0 B0 ;
N2 G55 ; Prepares the programming coordinate
system.
N3 G43.5 H01 ; Starts tool center point control.
H01 is the tool compensation number.
N4 G00 X200.0 Y150.0 Z20.0 ; Moves to the start point.
N5 G01 X5.0 Y5.0 Z5.0 I2.0 J1.732 K1.0 F500;
Linear interpolation
N6 G49 ; Cancels tool center point control.
N7 M30;
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 814 -
X'
Y'
Z'
B
A
X'
Y'
Z'
X'
Y'
Z'
X'
Z'
Y'
X'
Z'
Y'
X'
Z'
Y'
Control point path (of the
machine coordinate system)
Tool center point path seen from the table-fixed coordinate system
Tool center point path taken when
the programming coordinate
system does not move
Z"
Y
X
Z"
Y
X
Z"
Y
X
Fig. 22.1 (l) Example for a composite type machine
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 815 -
- When linear interpolation is performed during tool center point control
Examples are given below in which each 100-mm-long side of an
equilateral triangle is cut at B-axis angles of 0, 30 to 60, and 60
degrees, respectively.
Example)
When type 1 is selected and the table-fixed coordinate system is used
as the programming coordinate system:
O400 (Sample Program4) ;
N10 G55 ; Prepares the programming
coordinate system.
N20 G90 X50.0 Y-70.0 Z300.0 B0 C0 ; Moves to the initial position.
N30 G01 G43.4 H01 Z20.0 F500. ; Starts tool center point control.
Moves to the approaching
position.
H01 is the tool compensation
number.
N40 X28.868 Y-50.0 Z10.0 B30.0 ; The Z-axis height on the
machining plane is 10.0.
N50 Y50.0 ;
N60 B45.0 C120.0 ;
N70 X-57.735 Y0 B60.0 C180.0 ; Moves X and Y while operating
both B- and C-axes.
N80 C240.0 ;
N90 X28.868 Y-50.0 ;
N100 X50.0 Y-70.0 Z20.0 B0 C360.0 ; X, Y, and Z are approaching
positions.
The rotary axes move to their
original positions.
N110 G49 Z300.0 ; Cancels tool center point
control.
Moves the Z-axis to its initial
position.
N120 M30;
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 816 -
When type 1 is selected and the workpiece coordinate system is used
as the programming coordinate system
(Note that the values of N60 to N90 are different from those specified
in the preceding example.):
O400 (Sample Program4) ;
N10 G55 ; Prepares the programming
coordinate system.
N20 G90 X50.0 Y-70.0 Z300.0 B0 C0 ; Moves to the initial position.
N30 G01 G43.4 H01 Z20.0 F500. ; Starts tool center point control.
Moves to the approaching
position.
H01 is the tool compensation
number.
N40 X28.868 Y-50.0 Z10.0 B30.0 ; The Z-axis height on the
machining plane is 10.0.
N50 Y50.0 ;
N60 Y-50.0 B45.0 C120.0 ;
N70 X57.735 Y0 B60.0 C180.0 ; Moves X and Y while operating
both B- and C-axes.
N80 X28.868 Y-50.0 C240.0 ;
N90 Y50.0 ;
N100 X50.0 Y-70.0 Z20.0 B0 C360.0 ; X, Y, and Z are approaching
positions.
The rotary axes move to their
original positions.
N110 G49 Z300.0 ; Cancels tool center point
control.
Moves the Z-axis to its initial
position.
N120 M30;
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 817 -
When type 2 is selected and the table-fixed coordinate system is used
as the programming coordinate system:
O400 (Sample Program4) ;
N10 G55 ; Prepares the programming
coordinate system.
N20 G90 X50.0 Y-70.0 Z300.0 B0 C0 ; Moves to the initial position.
N30 G01 G43.5 H01 Z20.0 F500. ; Starts tool center point control.
Moves to the approaching
position.
H01 is the tool compensation
number.
N40 X28.868 Y-50.0 Z10.0 I1.0 K1.732 ; The Z-axis height on the
machining plane is 10.0.
N50 Y50.0 ;
N60 I-0.5 J0.866 K1.0 ;
N70 X-57.735 Y0 I-1.732 K1.0 ; Moves X and Y while operating
both B- and C-axes.
N80 I-0.866 J1.5 K1.0 ;
N90 X28.868 Y-50.0 ;
N100 X50.0 Y-70.0 Z20.0 K1.0 ; X, Y, and Z are approaching
positions.
The rotary axes move to their
original positions.
N110 G49 Z300.0 ; Cancels tool center point
control.
Moves the Z-axis to its initial
position.
N120 M30;
C
G55 workpiece coordinate system
Center of the B-axis
rotation
X
Z
Y
B
Center of the
C-axis rotation
• Composite type machine (tool rotation axis = B-axis; table rotation
axis = C-axis; tool axis = Z direction)
Machine configuration for the example
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 818 -
The following figure illustrates the position of the workpiece, as well
as the position of the tool head (relative to the workpiece), as seen
from the table-fixed programming coordinate system in the +Z
direction.
• Behavior as seen from the table-fixed programming coordinate system
(X -57.735, Y 0)
(B 30.0)
(B 30.0)
(B 45.0)
(B 60.0)
(B 60.0)
(B 60.0)
(C 0)
(C 120.0)
(C 240.0)
(X 28.868, Y 50.0)
(X 28.868, Y -50.0)
X'
Y'
Illustration of the example (1)
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 819 -
• Detailed diagram of each block
Y"
X" (C 0)
(B 30.0)
(B 0)
Behavior of the tool
center point
Behavior of the control point
(machine coordinate value)
(B 30.0)
C-axis rotates, with C
being 120 degrees. (B 45.0)
(C 0)
(C 120.0) (B 30.0)
B-axis rotates, with
B being 45 degrees.
N60 block
N70 block
(C 120.0)
(B 45.0)
(B 60.0)
C-axis rotates, with C
being 180 degress.
(C 180.0)
Y"
X"
Y"
X"
X'
Y'
X'
Y'
X'
Y'
Detailed diagram of each block (1)
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 820 -
C-axis rotates, with C
being 240 degrees.
(C 120.0)
(B 60.0)
(B 60.0)
(C 240.0)
(C 360.0)
(B 0)
(C-axis rotates, with C being
360 degrees.)
N80 block
N90 block
N100 block
(C 240.0)
(B 60.0)(B 60.0)
Y"
X"
Y"
X"
X' Y'
Y'
X'
X' X"
Y'
Y"
Detailed diagram of each block (2)
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 821 -
- When circular interpolation is performed during tool center point control
In this example, one of the three sides of an equilateral triangle, each
being 100 mm long side, is specified as a straight line and the other
two are specified as arcs, and each side is cut at B-axis angles of -60,
-45 to -30, and -30 degrees, respectively. (For the X-axis, its radius
is specified.)
Example)
The program sample given below assumes that the table-fixed
coordinate system is used as the programming coordinate system.
When the workpiece coordinate system is used as the programming
coordinate system (when bit 5 (WKP) of parameter No.19696 is set to
1), the same shape can be obtained by specifying the values shown in
parentheses.
N001 T0000 ; Cancels the tool offset.
N002 G54 ; Selects the workpiece coordinate system.
N003 G90 X50.0 Y-70.0 Z300.0 B-90.0 C0.0 ; Moves to the initial position.
The tool tip faces the Z- direction at B-axis
angle of -90 degrees.
N020 G01 G43.4 H01 Starts tool center point control.
N021 Z20.0 ; Moves to the approaching position.
N022 X28.868 Y-50.0 Z10.0 B-60.0 ; The Z-axis height on the machining
plane is 10.0.
N031 Y50.0 ;
N032 B-45.0 C90.0 ;
(N032 X50.0 Y-28.868 B-45.0 C90.0 ;)
N033 G17 G03 X-57.735 Y0.0 J-100.0 B-30.0 C150.0 ;
Moves X and Y while operating both B-
and C-axes.
(N033 G17 G03 X50.0 Y28.868 I-100.0 B-30.0 C150.0 ;)
N034 G01 B-30.0 C210.0 ;
(N034 G01 X50.0 Y-28.867 B-30.0 C210.0 ;)
N035 G03 X28.868 Y-50.0 I86.603 J50.0 C270.0 ;
(N035 G03 X50.0 Y28.868 I-100.0 C270.0 ;)
N041 G01 X50.0 Y-70.0 Z20.0 B-90.0 C360.0 ;
X, Y, and Z are approaching positions.
The rotary axes move to their original
positions.
N050 G49 ; Cancels tool center point control.
N051 Z300.0 ; Moves the Z-axis to its initial position.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 822 -
C-axis
Center of the C-
axis rotation
X
Y
Z
Z-axis
Y- a xi s
X-axis
B-axis
Center of the B-axis
rotation
Tool center
point
G54 workpiece
coordinate s
y
stem
Machine configuration for the circular interpolation example
The following figure illustrates the relative positional relationship
between the workpiece and the tool head and their positions, as seen
from the +Z direction. The X and Y coordinate values shown in the
figure are those on the table-fixed programming coordinate system
(which rotates as the C-axis turns).
(X 50.0, Y -70.0, Z 300.0, B -90.0)
(X 28.868, Y -50.0)
(B -60.0)
(B -60.0)
(B -45.0)
(X 28.868, Y 50.0)
(X -57.735, Y 0.0)
(C 0.0)
(C 90.0)
(C 150.0)
(B -30.0)
(B -30.0)
(B -30.0)
Y
X
(C 210.0)
(C 270.0)
• Behavior as seen from the table-fixed programming coordinate system
Illustration of the example
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 823 -
X
Y
[Up to N031]
Y
X
Behavior of the tool
center point
B -60
Behavior of the control point (machine
coordinate system) B -90
X
Y
[N032] B -45
C 90
B -60
[N034]
B -30B -30
Y
X
[N033]
B -45
B -30
C 150
Head path relative
to the workpiece
A
pparent head path
C 210
B -30
[N035]
B -30
X
Y
C 270
X
Y
[N041 and later]
B -30
B -90
Head path
relative to the
workpiece
A
pparent head path
C 360
A
pparent head path
Head path relative to
the workpiece
Detailed diagram of each block
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 824 -
Limitation
- Manual intervention
Manual intervention is impossible during tool center point control.
If manual intervention is performed, alarm PS5421 is issued when
automatic operation is started later.
- Hypothetical axis of a table rotation axis
When a table rotation axis is set as a hypothetical axis, tool center
point control is performed on the assumption that the table rotation
axis is at 0 degrees.
- Look-ahead pre-interpolation acceleration/deceleration
When the tool center point control mode is set, look-ahead
acceleration/deceleration before interpolation is automatically enabled.
Set the parameter for look-ahead acceleration/deceleration before
interpolation. If the parameter is not set correctly, alarm PS5420 is
issued.
Example:
Interpolation
path
Path of tool
center point
In the above example, the feedrate is controlled so that the tool center
point moves at a specified feedrate, so the feedrate on the interpolation
path is equal to or higher than the specified feedrate. At this time,
look-ahead acceleration/deceleration before interpolation allows the
feedrate to be clamped so that the feedrate on the interpolation path
does not exceed the maximum cutting feedrate or maximum rapid
traverse rate.
- Deceleration at a corner
Under tool center point control, the controlled point may move along a
curve even if a straight-line command is issued. Some commands
may cause a corner movement.
When AI contour control is not used, a shock can be applied to the
machine at a corner.
So, it is recommended to use AI contour control as well and set an
allowable speed difference at a corner (parameter No. 1783) and an
allowable acceleration rate (parameter No. 1660, No. 1737).
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 825 -
- 3-dimensional cutter compensation
3-dimensional cutter compensation and tool center point control can
be used at the same time.
For restrictions in such a case, see "Restrictions" of 3-dimensional
cutter compensation.
- Programmable mirror image
Note the following points when making a programmable mirror
image:
• In the case of tool center point control of type 1
Mirroring the linear axis alone does not create a mirror image for
the rotary axis. To make the direction of the tool symmetrical,
it is necessary to make a mirror image for the rotary axis as well.
• In the case of tool center point control of type 2
When bit 6 (MIR) of parameter No.19608 is set to 0, mirroring
the linear axis alone does not create a mirror image for I, J, K.
Note that the inclination direction specified by Q is the
movement direction of the tool center point after mirroring.
When bit 6 (MIR) of parameter No.19608 is set to 1, mirroring
the linear axis automatically creates a mirror image for I, J, K.
A mirror image cannot be put on the rotary axis directly.
- Scaling
Do not apply scaling to a rotary axis.
- Machine coordinate system command
During tool center point control, the machine coordinate system
command (G53) cannot be used.
However, G53 can be specified singly to suppress look-ahead
operation.
- Stored limit check before move
During tool center point control, stored limit check before move is
disabled.
- Type 2
When a type 2 command (G43.5 command) is specified on a machine
of table rotation type or composite type (parameter No. 19680 = 12 or
21), the table coordinate system needs to be set as the programming
coordinate system (by setting bit 5 (WKP) of parameter No. 19696 to
0). If type 2 is specified with a workpiece coordinate system set as
the programming coordinate system, alarm PS5459 is issued.
- Specifiable G codes
The G codes that can be specified in the tool center point control
mode are listed below.
Specifying a G code other than these codes results in alarm PS5421.
• Positioning (G00)
• Linear interpolation (G01)
• Circular interpolation / helical interpolation (G02/G03)
• Dwell (G04)
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 826 -
• Exact stop (G09)
• Programmable data input (G10)
• Tool retract and recover (G10.6)
• Programmable data input mode cancel (G11)
• Plane selection (G17/G18/G19)
• Tool radius compensation cancel (G40)
• 3-dimensional cutter compensation
(G41.2/G42.2/G41.4/G42.4/G41.5/G42.5)
• Tool length compensation cancel (G49)
• Scaling (G50/G51)
• Programmable mirror image (G50.1/G51.1)
• Machine coordinate system command (G53) specified singly
• Cutting mode(G64)
• Macro call (G65)
• Macro modal call A (G66)
• Macro modal call B (G66.1)
• Macro modal call A/B cancel (G67)
• Absolute programming (G90)
• Incremental programming (G91)
• Canned cycle : return to initial level (G98)
• Canned cycle : return to R point level (G99)
- Modal G codes that allow specification of tool center point control
Tool center point control can be specified in the modal G code states
listed below.
Tool center point control cannot be specified in a modal state other
than these.
• Modal G codes included in "Specifiable G codes" described
previously
• Polar coordinate interpolation mode cancel (G13.1)
• Polar coordinates command cancel (G15)
• Input in inch (G20 (G70))
• Input in mm (G21 (G71))
• Polygon turning cancel (G50.2)
• Workpiece coordinate system setting (G54 to G59)
• Canned cycle cancel (G80)
• Constant surface speed control cancel (G97)
M
• Coordinate system rotation cancel or 3-dimensional coordinate
conversion mode off (G69)
• Feed per minute (G94)
• Polar coordinate interpolation mode cancel (G113)
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 827 -
T
• Mirror image for double turret off/balanced cutting mode cancel
(G69)
• Coordinate system rotation cancel or 3-dimensional coordinate
conversion mode off (G69.1)
• Feed per minute (G98 (G94))
- Specification of axes not relating to tool center point control
Axes not relating to tool center point control cannot be specified. If
such an axis is specified, alarm PS5421 is issued.
- Linear axes under tool center point control
The basic three axes set in parameter No. 1022 are regarded as the
three linear axes for tool center point control. Axes parallel to the
basic three axes cannot be used as the linear axes for tool center point
control.
If the basic three axes are not set in parameter No. 1022, alarm
PS5459 is issued.
T
- Extended tool selection
When tool center point control is used with a lathe system, the tool
change method needs to be ATC type (bit 3 (TCT) of parameter No.
5040 = 1).
In this case, only the value set in "Z" on the tool compensation
memory screen is used as a tool length compensation amount. Set
values such as "X", "R", and "Y" axis offset values are not used.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 828 -
22.2 TOOL POSTURE CONTROL
Overview
Under tool center point control, the tool tip moves along a specified
path even when the tool direction relative to the workpiece changes.
Usually, however, the two rotary axes are controlled independently of
each other, and the posture of the tool is not controlled.
Under tool posture control, the tool posture is controlled every
moment for operation on the plane formed by the tool postures (tool
length compensation vectors) at the start point and end point of a
block.
This control method is suitable for machining a plane with the side of
a tool by using tool center point control.
Tool posture control Plane formed b
y
Vs and Ve
Tool length compensation
vector Vs at block start point
Tool length compensation
vector Ve at block end point
Programmed path
Fig. 22.2 (a) Tool posture control
This function is optional. The tool center point control option is also
needed.
Format
Format
G43.4 IP_ α_ β_ H_ P_ ; Tool center point control (type 1)
G43.5 IP_ H_ Q_ P_ ; Tool center point control (type 2)
Description of symbols
IP : For an absolute command, the coordinates of travel end point of the tool
center point
For an incremental command, the travel distance of the tool center point
α, β : For an absolute command, the coordinates of the end point of the rotation axis
For an incremental command, the travel distance of the rotation axis
H : Tool offset number
Q : Tool tilted angle (degree)
P : Tool posture control disabled (P0) or tool posture control enabled (P1)
However, bit 0 (TPC) of setting parameter No. 19604 can be used to select
the behavior taken when the address P command is not present.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 829 -
Tool posture control is enabled when P1 is specified or disabled when
P0 is specified in the G43.4 and G43.5 blocks. The behavior taken
when the address P command is not present can be selected by bit 0
(TPC) of parameter No. 19604. The setting of tool posture control
selected in the G43.4 and G43.5 blocks is kept until the tool center
point control cancellation command (G49) is specified.
Example:
O0010
…
N10 G90 G00 X30.0 Y-30.0 Z0.0;
N20 G43.5 H1 P1;
N30 G42.6 D2;
N40 G01 X20.0 Y-20.0 I-1 J1 K2 F_;
N50 Y20.0 I-1 J-1 K2;
N60 X-20.0 I1 J-1 K2;
N70 Y-20.0 I1 J1 K2;
N80 X20.0 I-1 J1 K2;
…
G40;
G49;
M30;
X
Y
Z
In N20 to N80 in program O0010 to the
left, the sides of a quadrangular pyramid
trapezoid as shown below can be
machined by the side of the tool using
tool posture control. The following figure
illustrates tool movement by N50. The
command in N30 is the three-dimensional
cutter compensation command.
Fig. 22.2 (b) Example of tool posture control
Explanation
In tool posture control, the two rotation axes are controlled so that the
momentary tool posture (tool length compensation vector) satisfies the
following conditions (Fig. 22.2 (c)).
The momentary tool posture (tool length compensation vector) is
present on the plane configured by the tool length compensation
vector at the block start point and that at the block end point.
The angle which the tool length compensation vector at the block start
point makes with the momentary tool length compensation vector
is the angle obtained by proportionally dividing the angle which
the tool length compensation vector at the block start point makes
with the tool length compensation vector at the block end point.
Tool posture control is enabled when P1 is specified or disabled when
P0 is specified in the tool center point control start command
(G43.4/G43.5) blocks. Bit 0 (TPC) of setting parameter No. 19604
can be used to select whether tool posture control is enabled or
disabled when the address P command is not present. The setting of
tool posture control selected in the G43.4 and G43.5 blocks is kept
until the tool center point control cancellation command (G49) is
specified.
This function can be used for positioning (G00) and linear
interpolation (G01) during tool center point control.
Other notes and restrictions are the same as those for tool center point
control.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 830 -
Program specification path
Control
point
V
Tool center
point
Block start point Block end point
Vs
V
Ve
θ
Θ
L
l
Vs
Ve
Plane configured by tool length compensation vectors Vs and Ve
Momentary tool length compensation vector V is controlled so as to
be present on the plane.
=
θ
Θ
L
l
Control is made so that angle
θ
which Vs makes with V
satisfies this expression.
Fig. 22.2 (c) Tool posture control
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 831 -
Singular point
- "Tool-side rotary axis" and "workpiece-side rotary axis"
When tool center point control type 2 is specified, programming needs
to be performed considering a singular point and singular point
posture. The "tool-side rotary axis" and "workpiece-side rotary axis"
used in the descriptions of a singular point and singular point posture
later are explained below.
On a 5-axis machine that has two rotary axes, one rotary axis has a
function for tilting the tool toward a workpiece. This rotary axis is
referred to as a "tool-side rotary axis".
The other rotary axis is referred to as a "workpiece-side rotary axis".
The table below indicates the axes that represent these rotary axes for
each mechanical unit type.
Table 22.2 (a) "Tool-side rotary axis" and "workpiece-side rotary axis"
Mechanical unit type
(parameter No. 19680) Tool-side rotary axis Workpiece-side rotary
axis
Tool rotation type (2) Slave axis Master axis
Table rotation type (12) Master axis Slave axis
Composite type (21) Tool rotary axis Table rotary axis
Tool rotation type Table rotation type Composite type
Tool-side rotary axis
Workpiece-side rotary axis
Fig. 22.2 (d) "Tool-side rotary axis" and "workpiece-side rotary axis"
- Singular point, singular point posture
A tool posture is uniquely determined when the angular displacements
of the two rotary axes are determined. However, a combination of
the angular displacements of the two rotary axes for determining a
particular tool posture is not uniquely determined usually.
In particular, a tool posture with the angular displacement of the
workpiece-side rotary axis being arbitrary is referred to as a "singular
point posture", and the angular displacement of the tool-side rotary
axis that causes the tool posture to assume a singular point posture is
referred to as the "singular point (or singular point angular
displacement)". When the angular displacement of the tool-side
rotary axis is at a singular point, the center of the workpiece-side
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 832 -
rotary axis and the tool posture (tool orientation) are parallel with each
other.
Example)
Suppose that a tool rotation type machine is used, the master axis
is the C-axis (about the Z-axis), the slave axis is the B-axis
(about the Y-axis), and the reference tool axis direction is the
Z-axis direction. In this case, singular point B = ..., 0°, 180°, ...,
and a singular point posture (the same direction as the Z-axis
direction or the direction opposite to the Z-axis direction) results
at an arbitrary C-axis angular displacement.
For example, when the B-axis angular displacement is B = 0 (singular
point) as shown in Fig. 22.2 (e), the same tool posture (singular point
posture) is assumed at an arbitrary C-axis angular displacement.
C=0 C=60
B=0
(Singular point)
X
Z
Singular point
posture
B=0
(Singular point)
Fig. 22.2 (e) Singular point and singular point posture
There is no singular point and singular point posture on some types of
machines as in the case where the reference tool axis direction is tilted
(parameter No. 19698 and No. 19699) or a rotary axis is an angular
axis (parameter No. 19682, No. 19683, No. 19687, and No. 19688).
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 833 -
- When the tool posture is close to a singular point posture
When tool posture control is exercised on a machine that has a
singular point, and the tool posture becomes close to a singular point
posture during execution of a block, the operation of the
workpiece-side rotary axis can become so large, resulting in unstable
machine operation.
In such a case, machine operation can be made stabler, the machining
time can be reduced, and the surface roughness can be improved by
changing the tool posture at the block end point so that the tool
posture passes through a singular point posture.
A
large and abrupt movement is made on
the workpiece-side rotary axis when the tool
posture passes through a singular poin
t
close posture.
A
large and abrupt movement on the workpiece-side
rotary axis can be avoided by passing through a
singular point posture. By passing through a
singular point posture, the tool posture at the block
end is changed within the allowable range.
Fig. 22.2 (f) Changing the tool posture at a block end point
When tool posture control is used, and the angle between a tool
posture and singular point posture is equal to or less than the value of
(parameter No. 19738), the tool posture is determined to be close to a
singular point posture. The tool posture at this time is referred to as a
"singular point close posture". When tool center point control is
specified (G43.5) based on type 2, which specifies the tool posture at
the block end point with tool axis direction (I, J, K), each block is
checked to see if a singular point close posture is assumed. If a
singular point close posture is assumed in a block, the tool posture at
the end point of the block is changed (the rotary axis angular
displacement is changed) to pass through a singular point posture. If
the end points before and after the workpiece-side rotary axis is
changed vary largely from each other as the result of changing the tool
posture at the block end point, the change in the tool posture at the
block end point can be suppressed.
However, if the value of parameter No. 19738 is 0, the tool posture at
the block end point is not changed.
If the tool posture at the start point or end point of a block is a singular
point posture or the tool posture becomes a singular point posture in
the middle of a block, the tool posture is not changed at the block end
point.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 834 -
If this angle is equal to or
less than the value of
parameter No. 19738, a
singular point close
posture is assumed.
Tool posture
Singular
point posture
Fig. 22.2 (g) Singular point close posture
If a singular point close posture is assumed during execution of a
block, change the angular displacements of the rotary axes at the end
point of the block calculated from the tool posture specified by (I, J,
K) so that the tool posture passes through a singular point posture in
the block as indicated below.
Tool-side rotary axis:
Turned reversely relative to the singular point angular
displacement
Example:
When the end point angular displacement before a change is
60°, and the singular point angular displacement is 20°, the
end point angular displacement after a change is -20°.
Workpiece-side rotary axis:
Same as the angular displacement at the start point
Example:
When the end point angular displacement after a change is
30°, and the start point angular displacement is -150°, the
end point angular displacement after a change is -150°.
However, if both of the difference between the end point angular
displacement before a change and (end point angular displacement
after a change + 180°) and the difference between the end point
angular displacement before a change and (end point angular
displacement after a change - 180°) are equal to or greater than the
value of parameter No. 19739, the program is executed according to
the setting of bit 3 (NPC) of parameter No. 19696, suppressing the
change, or alarm PS5421 is issued.
This function is used to avoid unstable machine operation in a block
where a singular point close posture is assumed as shown in Fig. 22.2
(f).
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 835 -
Notes
- When the reference tool axis or a rotary axis is inclined
When tool center point control is used, the inclination of the reference
tool axis can be set in parameter No. 19698 and No. 19699, and the
inclination of a rotary axis can be set in parameter No. 19682, No.
19683, No. 19687 and No. 19688.
On a machine with the reference tool axis or a rotary axis being
inclined, all tool postures cannot be assumed. Some tool postures
can never be assumed by setting the angular displacements of the two
rotary axes in any way. If the tool posture passes through any of
those impossible tool postures during program execution when tool
posture control is enabled, alarm PS0432 is issued before execution of
the block.
Example:
On a tool rotation type machine where the master axis is the
C-axis (about the Z-axis), the slave axis is the B-axis (about the
Y-axis), and the reference tool axis direction is inclined relative
to the positive Z-axis direction (a non-zero value is set in
parameter No. 19698 and No. 19699), no tool posture can be
assumed in the positive or negative direction of the Z-axis. So,
if a block specifies such a tool posture during tool posture control,
alarm PS0432 is issued before execution of the block.
O0010
…
G43.5 H1 P1;
…
N10 X_ Y_ Z_ I1 J0 K2;
N20 X_ Y_ Z_ I-1 J0 K2;
…
G49;
M30;
I1 J0 K2
;
Positive Z-axis direction
I-1 J0 K2
;
X
Y
Z
If O0010 is executed on the machine in
the example above, the tool posture
assumes the positive Z-axis direction
during N20, so alarm PS0432 is issued
before execution of N20.
Fig. 22.2 (h) Example of impossible tool posture
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 836 -
- When the operation range of rotary axes is specified
When tool center point control is used, the operation range of rotary
axes can be set in parameter No. 19741 to No. 19744.
If either of the rotary axes exceeds the set operation range during
program execution when tool posture control is enabled, alarm
DS0029 is issued.
If tool posture control is disabled, rotary axis operation range
specification based on parameter No. 19741 to No. 19744 is enabled
only when the tool center point control type 2 command (G43.5) is
specified. If tool posture control is enabled, the check mentioned
above can be made even when the tool center point control type 1
command (G43.4) is specified.
If the operation range of the first rotary axis is not specified, set 0 in
both of parameter No. 19741 and No. 19742.
If the operation range of the second rotary axis is not specified, set 0
in both of parameter No. 19743 and No. 19744.
- When tool center point control type 1 is used
Tool posture control can also be exercised by using the tool center
point control type 1 command (G43.4), which specifies the tool
posture at the end point of a block with the angular displacements of
the two rotary axes. However, when tool posture control is exercised
using the tool posture at the end point of a block calculated from the
rotary axis angular displacement specified by the program, alarm
PS5421 is issued before execution of the block if the
program-specified rotary axis angular displacement does not result.
Example:
Suppose that a tool rotation type machine where the master axis
is the C-axis (about the Z-axis), the slave axis is the B-axis
(about the Y-axis), the reference tool axis direction is the Z-axis
direction, and the reference tool axis and rotary axes are not
inclined is used. If the rotary axis angular displacements at the
end point of a block are specified as (B, C) = (-90°, -90°) (with
the tool posture being in the positive Y-axis direction) when the
rotary axis angular displacements at the start point of the block
are (B, C) = (90°, 0°) (with the tool posture being in the positive
X-axis direction), tool posture control needs to maintain the tool
posture in parallel with the XY plane. In this state, however,
the specified end point (B, C) = (-90°, -90°) cannot be reached,
so that alarm PS5421 is issued.
If (B, C) = (90°, 90°) for representing the same tool posture in
the positive Y-axis direction at the end point of a block is
specified, tool posture control is possible.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 837 -
O0020
…
G43.4 H1 P1;
…
N10 X_ Y_ Z_ B90.0 C0.0;
N20 X_ Y_ Z_ B-90.0 C-90.0;
…
G49;
M30;
O0021
…
G43.4 H1 P1;
…
N10 X_ Y_ Z_ B90.0 C0.0;
N20 X_ Y_ Z_ B90.0 C90.0;
…
G49;
M30;
X
Y
B=90.0, C=0.0
B=90.0, C=90.0
or B=-90.0, C=-90.0
A
t the N20 end point of both of the programs
O0020 and O0021, the tool posture is in the
positive Y-axis direction. However, the N20
end point (B=-90.0, C=-90.0) of O0020
cannot be reached from the N10 end point
(B=90.0, C=0.0) by tool posture control. So,
alarm PS5421 is issued with O0020.
However, the N20 end point (B=90.0, C-90.0)
of O0021 can be reached by tool posture
control.
Fig. 22.2 (i) Example where tool posture control is impossible when
type 1 is specified
- When the tool posture directions at the start point and end point of a block match
each other
If the direction of the tool posture at the start point of a block matches
the direction of the tool posture at the end point of the block (same
direction or opposite direction), no plane can be determined by these
tool postures. So, tool posture control in that block is temporarily
disabled. However, whether to enable/disable tool posture control is
kept as modal information. So, tool posture control temporarily
disabled for the cause mentioned above is enabled again in the
subsequent blocks.
For other notes, those described for tool center point control are
applicable.
Limitation
This function is enabled for positioning (G00) and linear interpolation
(G01).
For other restrictions, those described for tool center point control are
applicable.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 838 -
22.3 TILTED WORKING PLANE COMMAND
22.3.1 Tilted Working Plane Command
Overview
Programming for creating holes, pockets, and other figures in a datum
plane tilted with respect to the workpiece would be easy if commands
can be specified in a coordinate system fixed to this plane (called a
feature coordinate system). This function enables commands to be
specified in the feature coordinate system. The feature coordinate
system is defined in the workpiece coordinate system.
For explanations about the relationship between the feature coordinate
system and workpiece coordinate system, see Fig. 22.3 (a).
Feature coordinate
system
(G68.2)
Machine coordinate system
Workpiece
coordinate system
(G54)
Fig. 22.3 (a) Feature coordinate system
The G68.2 command causes the programming coordinate system to
switch to the feature coordinate system. The commands in all
subsequent blocks are assumed to be specified in the feature
coordinate system until G69 appears.
If G68.2 specifies the relationship between the feature coordinate
system and the workpiece coordinate system, G53.1 automatically
specifies the +Z direction of the feature coordinate system as the tool
axis direction even if no angle is specified for the rotary axis. (See
Fig. 22.3 (c).)
For explanations about the tool axis direction, see Fig. 22.3 (b).
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 839 -
X
Y
Z
The tool axis direction is the
+Z-axis direction.
The tool axis direction is the
+Y-axis direction.
The tool axis direction is the +X-axis direction.
Fig. 22.3 (b) Tool axis direction
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 840 -
This function regards the direction normal to the machining plane as
the +Z-axis direction of the feature coordinate system. After the
G53.1 command, the tool is controlled so that it remains perpendicular
to the machining plane.
Coordinate system
origin shift
(xo,yo,zo)
Xc
Yc
Zc
Workpiece
coordinate system
X-Y-Z
Feature coordinate
system
Xc-Yc-Zc
X
Y
Z
• Only G68.2 is specified
• G53.1 is specified after G68.2
Xc
Yc
Zc
Control point shift (by
another command)
G53.1 automatically controls
the rotary axis.
X
Y
ZB
C
Feature coordinate
system
Xc-Yc-Zc
Coordinate system
origin shift
(xo,yo,zo)
Workpiece
coordinate system
X-Y-Z
Fig. 22.3 (c) G68.2 and G53.1 commands
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 841 -
This function is applicable to the following machine configurations.
(See Fig. 22.3 (d).)
<1> Tool rotation type machine controlled with two tool rotation
axes
<2> Table rotation type machine controlled with two table rotation
axes
<3> Composite type machine controlled with one tool rotation axis
and one rotary axis
The function can also be used for a machine configuration in which
the rotary axis for controlling the tool does not intersect the rotary axis
for controlling the table.
<2> Table rotation type
machine
<3> Composite type
machine
<1> Tool rotation
type machine
X
C
B
Z
Y
A
C
X
Z
Y
B
Y
X
Z
C
Fig. 22.3 (d) Three types of 5-axis machine
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 842 -
Format
- Tilted working plane command (G68.2)
M
G68.2 X x0 Y y0 Z z0 Iα Jβ Kγ ;
Tilted working plane command
G69 ; Cancels the tilted working plane command.
X, Y, Z : Feature coordinate system origin
The axes specified here are the three axes of the
feature coordinate system. Specify the three
basic axes or parallel axes set by parameter No.
1022. When specification is omitted, the X, Y,
and Z of the basic three axes are assumed to be 0.
I, J, K : Euler's angle for determining the orientation of the
feature coordinate system
T
G68.2 X x0 Y y0 Z z0 Iα Jβ Kγ ;
Tilted working plane command
G69.1 ; Cancels the tilted working plane command.
X, Y, Z : Feature coordinate system origin
The axes specified here are the three axes of the
feature coordinate system. Specify the three
basic axes or parallel axes set by parameter No.
1022. When specification is omitted, the X, Y,
and Z of the basic three axes are assumed to be 0.
I, J, K : Euler's angle for determining the orientation of the
feature coordinate system
- Tool axis direction control (G53.1)
G53.1 ; Controls the tool axis direction.
CAUTION
1 G53.1 must be specified in a block after the block
that contains G68.2.
An alarm occurs if G53.1 is specified without G68.2
being specified in a preceding block.
2 G53.1 must be specified in a block in which there is
no other command.
3 The rotary axis moves at the maximum rapid
traverse federate in the case of rapid traverse and
at the specified federate in the case of cutting feed.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 843 -
Explanation
- Coordinate conversion using an Euler's angle
Coordinate conversion by rotation is assumed to be performed around
the workpiece coordinate system origin.
Let the coordinate system obtained by rotating the workpiece
coordinate system around the Z-axis by an angle of α degrees be
coordinate system 1. Similarly, let the coordinate system obtained
by rotating coordinate system 1 around the X-axis by an angle of β be
coordinate system 2. The feature coordinate system is the coordinate
system obtained by shifting the coordinate system that is obtained by
rotating coordinate system 2 around the Z-axis through an angle of γ
degrees from the workpiece coordinate system origin by (Xo, Yo, Zo).
Fig. 22.3 (e) shows the relationship between the workpiece coordinate
system and the feature coordinate system.
The figure also gives examples of displacement on the X-Y plane.
γ
zc
yc
x
c
x'
y''
γ
Conversion from workpiece
coordinate system X-Y-Z to
coordinate system 1 X'-Y'-Z
x
z
y
x'
y'
α
β
X
'
zy''
z''
y'
β
Conversion from coordinate
system 1 X'-Y'-Z to
coordinate system 2 X'-Y"-Z"
Conversion from coordinate system 2 X'-Y"-Z"
to feature coordinate system Xc-Yc-Zc
Fig. 22.3 (e) Coordinate conversion using an Euler's angle
- I0 J0 K0 command
When I0 J0 K0 is specified as an Euler's angle, the alarm (PS5457)
(G68.2 format error) usually occurs. When bit 1 (ATW) of
parameter No. 13451 is set to 1, the feature coordinate system with a
tilted angle of 0 degree is used.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 844 -
- Constant surface speed control
Constant surface speed control is exercised by using, as the reference,
the machine axis specified in address P in a G96 block or the machine
axis (not in the feature coordinate system but in the actually operating
workpiece coordinate system) set in parameter No. 3770.
- Tool rotation type machine
The following paragraphs describe several cases of the tool rotation
type machine operation.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 845 -
Operation description 1: When G43 (tool length compensation) is specified for a
machine with its axes crossing one another
The G53.1 command, when specified after the G68.2 command,
automatically controls the rotary axis in such a way that the tool axis
will be oriented in the +Z direction of the feature coordinate system.
Example)
O100 (Sample Program1) ;
N1 G55 ;
N2 G90 G01 X0 Y0 Z30.0 F1000 ;
N3 G68.2 X100.0 Y100.0 Z50.0 I30.0 J15.0 K20.0 ;
N4 G01 X0 Y0 Z30.0 F1000 ;
N5 G53.1 ;
N6 G43 H01 X0 Y0 Z0 ;
N7 . . .
In this example, the "BC type tool axis Z-axis" is used as the machine
configuration.
In addition, the tool axis, tool rotation axis B, and tool rotation axis C
cross one another.
B : Second rotation axis (slave)
C : First rotation axis (master)
Control
point
Tool holder offset value =
Parameter No.19666
Tool length offset = H01
BC type tool axis Z-axis
(with the axes crossing
one another)
Tool center
point
Block N3 : Defines a feature coordinate system in the workpiece
coordinate system.
Block N4 : Shifts the control point to point Z30.0 in the feature
coordinate system.
Block N5 : Exerts automatic control over the rotary axes.
Block N6 : Performs tool length compensation in the feature
coordinate system.
The tool center point is shifted to the origin of the feature
coordinate system.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 846 -
Fig. 22.3 (f) shows the behavior of the machine when it runs sample
program 1.
N3 command
Feature coordinate
system
Xc-Yc-Zc
Xc
Yc
Zc
• Sample program 1 (with axes crossing one another)
Xc
Yc
Zc
Xc
Yc
Zc
Xc
Yc
Zc
N4 command
N5 command
N6 command
Workpiece
coordinate
system
X-Y-Z
X
Y
Z
Control
point
Fig. 22.3 (f) Tool axis direction control 1
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 847 -
Operation description 2: When G43 (tool length compensation) is specified for a
machine with no axis crossing
Here is the case where no axis of the machine crosses any other axis.
It is assumed that sample program 1 is used.
In this example, the "BC type tool axis Z-axis" is used as the machine
configuration.
It is assumed, however, that the tool axis does not cross the B-axis
while the B-axis and C-axis cross each other.
C: First rotation axis (master)
Control
point
Tool holder offset value =
Parameter No.19666
Tool length offset = H01
• BC type tool axis Z-axis
(no axis crossing)
Tool center
point
B: Second rotation axis (slave)
Intersection offset vector
between tool axis and
B-axis = Parameters
No.19709 - No.19711
Block N4 : Shifts the control point to point Z30.0 in the feature
coordinate system.
Block N5 : Exerts automatic control over the rotary axes.
Block N6 : An intersection offset vector between the tool axis and
the B-axis with automatic control for rotary axes taken
into consideration is output in the feature coordinate
system.
Performs tool length compensation in the feature
coordinate system.
The tool center point is shifted to the origin of the feature
coordinate system.
This is also true when the B-axis does not cross the C-axis.
For explanations about the offset to be applied when the B-axis does
not cross the C-axis, see the descriptions about parameters No.19712,
No.19713, and No.19714.
Fig. 22.3 (g) shows the behavior of the machine when it runs sample
program 1.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 848 -
N3 command
• Sample program 1 (no axis crossing)
N4 command
N5 command
N6 command
Workpiece
coordinate system
X-Y-Z
X
Y
Z
Control
point
Xc
Yc
Zc
Zc
Feature coordinate
system
Xc-Yc-Zc
Xc
Yc
Xc
Yc
Zc
Xc
Yc
Zc
A
n intersection offset vector
between the tool axis and the B-
axis with automatic control for
rotation axes taken into
consideration is output in the
feature coordinate system. Tool
length compensation is also
performed.
The tool center point is controlled
so that it returns to the Xc-Yc-Zc
origin.
Xc
Yc
Zc
Zc 30.0
Zc 30.0
Fig. 22.3 (g) Tool axis direction control 2
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 849 -
Operation description 3: When no G43 (tool length compensation) command is
specified or if no G53.1 (tool axis direction control)
command is specified
Sample program 2 of O200 is equivalent to sample program 1 except
that sample program 2 has no tool length compensation command
(G43).
Example)
O200 (Sample Program2) ;
N1 G55 ;
N2 G90 G01 X0 Y0 Z30.0 F1000 ;
N3 G68.2 X100.0 Y100.0 Z50.0 I30.0 J15.0 K20.0 ;
N4 G01 X0 Y0 Z0 F1000 ;
N5 G53.1 ;
N6 . . . ;
In this example, the "BC type tool axis Z-axis" is used as the machine
configuration.
The case in which the axes cross one another and the case in which no
axis crosses any other axis are described.
Fig. 22.3 (h) shows the behavior of the machine when it runs sample
program 2.
Sample program 3 of O300 is equivalent to sample program 1 except
that sample program 3 has no tool axis direction control command
(G53.1).
Example)
O300 (Sample Program3) ;
N1 G55 ;
N2 G90 G01 X0 Y0 Z30.0 F1000 ;
N3 G68.2 X100.0 Y100.0 Z50.0 I30.0 J15.0 K20.0 ;
N4 G01 X0 Y0 Z0 F1000 ;
N5 G43 H01 ;
N6 . . . ;
In this example, the "BC type tool axis Z-axis" is used as the machine
configuration.
The case in which the axes cross one another and the case in which no
axis crosses any other axis are described.
Tool length compensation is applied in the +Z-axis direction of the
feature coordinate system.
Fig. 22.3 (i) shows the behavior of the machine when it runs sample
program 3.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 850 -
Feature coordinate
system
Xc-Yc-Zc
N4 command
Xc
Yc
Zc
• Sample program 2 (with axes crossing one another)
Yc
N4 command
Workpiece
coordinate system
X-Y-Z
X
Y
Z
Control
point
Xc
Zc
N4 command
Feature coordinate
system
Xc-Yc-Zc
Xc
Yc
Zc
• Sample program 2 (no axis crossing)
N5 command
Workpiece
coordinate system
X-Y-Z
X
Y
Z
Control
point
Xc
Yc
Zc
Fig. 22.3 (h) When the tool length compensation command is not
specified
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 851 -
N4 command
Feature coordinate
system
Xc-Yc-Zc
Xc
Yc
Zc
• Sample program 3 (with axes crossing one another)
N5 command
Workpiece
coordinate system
X-Y-Z
X
Y
Z
Control
point
Xc
Yc
Zc
N4 command
Z
Feature coordinate
system
Xc-Yc-Zc
Xc
Yc
Zc
• Sample program 3 (no axis crossing)
N5 command
Workpiece
coordinate system
X-Y-Z
X
Y
Control
point
Xc
Yc
Zc
Fig. 22.3 (i) When the tool axis direction control command is not
specified
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 852 -
- Composite type machine
Basic operation
This function is also available for a composite type machine in which
the tool head rotates on the tool rotation axis and the table rotates on
the table rotation axis.
The feature coordinate system Xc-Yc-Zc is set in the workpiece
coordinate system based on the coordinate system origin shift (xo, yo,
zo) and the Euler's angle.
Given the A-axis and B-axis shown in Fig. 22.3 (j), control is
performed in such a way that the A-axis rotates until Zc comes in the
X-Z plane and the B-axis is controlled so that the tool axis is oriented
toward the +Z-axis direction of the feature coordinate system.
X
Y
Z
A
X
Y
Z
A
(xo, yo, zo)
Xc
Yc
Zc
Xc'
Yc'
Zc'
• Tool axis direction control for a composite type machine
B
Fig. 22.3 (j) Composite type machine
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 853 -
- Feature coordinate system with the table rotated by G53.1 (tool axis direction
control)
The composite type machine shown in Fig. 22.3 (j) is explained as an
example.
If the table rotates by the tool axis direction control command (G53.1),
the feature coordinate system (called the first feature coordinate
system), which is set in the workpiece coordinate system by the tilted
working plane command (G68.2), rotates as much as the table rotates.
The feature coordinate system that has rotated is called the second
feature coordinate system.
Once G53.1 is specified, the subsequent machining commands are
assumed to be specified in the second feature coordinate system.
(See Fig. 22.3 (k).)
In the composite type machine, the specified feature coordinate
system (the first feature coordinate system) may differ from the
feature coordinate system to be used for machining (the second feature
coordinate system).
X
Y
Z
Xc'
Yc'
Zc'
• G53.1 command
X
Y
Z
Xc'
Yc'
Zc'
G01 Y10.0 F1000
command after G53.1
Second feature coordinate
system
Xc'-Yc'-Zc'
Second feature coordinate
system
Xc'-Yc'-Zc'
Fig. 22.3 (k) Resetting of the feature coordinate system
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 854 -
- Rotation direction of the table rotation axis
The composite type machine shown in Fig. 22.3 (j) is explained as an
example.
Set parameter No.19684 to 1 if the rotation direction of the rotation
table corresponding to the positive-direction move command is
clockwise when viewed from the positive direction of the rotation
center axis on which the table rotation axis rotates. If the rotation
direction is counterclockwise, set parameter No.19684 to 0.
Let's take sample program 4 of O400 as an example, where the
movement of the table is specified by G53.1.
If parameter No.19684 is set to 1, control is performed in such a way
that the table is rotated to A-45.0.
If parameter No.19684 is set to 0, control is performed in such a way
that the table is rotated to A45.0.
Example)
O400 (Sample Program4) ;
N1 G68.2 X100.0 Y100.0 Z0 I180.0 J45.0 K0 ;
N2 G53.1 ;
N3 . . . ;
X
Y
Z
A
Xc
Yc Zc
Yc
Xc
Zc
CCW CW
Rotation to A-45.0
CCW
Rotation to A45.0
CCW
Yc
Xc
Zc
Positive rotation direction when
parameter No.19684 = 0
Positive rotation direction when
parameter No.19684 = 1
G53.1 command
G53.1 command
Fig. 22.3 (l) Rotation direction of the table rotation axis
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 855 -
- Table rotation type machine
Basic operation
This function is also usable for a table rotation type machine with two
table rotation axes.
The feature coordinate system Xc-Yc-Zc is set in the workpiece
coordinate system based on the coordinate system origin shift (xo, yo,
zo) and the Euler's angle.
Given the A-axis and C-axis shown in Fig. 22.3 (m), the A-axis and
C-axis rotate until Zc comes in the X-Z plane and the tool axis is
directed toward the +Z-axis direction of the feature coordinate system.
A
C
Xc
Yc
Zc
Yc'
Xc'
• Tool axis direction control for a table rotation type machine
X
Y
Z
A
X
Y
Z
Zc'
C
Fig. 22.3 (m) Table rotation type machine
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 856 -
- Feature coordinate system with the table rotated by G53.1 (tool axis direction
control)
The table rotation type machine shown in Fig. 22.3 (m) is explained as
an example.
If the table rotates by the tool axis direction control command (G53.1),
the feature coordinate system (called the first feature coordinate
system), which is set in the workpiece coordinate system by the tilted
working plane command (G68.2), rotates as much as the table rotates.
The feature coordinate system that has rotated is called the second
feature coordinate system.
Once G53.1 is specified, the subsequent machining commands are
assumed to be specified in the second feature coordinate system.
(See Fig. 22.3 (n).)
In the table rotation type machine, the specified feature coordinate
system (the first feature coordinate system) may differ from the
feature coordinate system to be used for machining (the second feature
coordinate system).
• G53.1 command
G01 X10.0 F1000
command after G53.1
Yc'
Xc'
X
Y
Z
Zc'
Yc'
Xc'
X
Y
Z
Zc'
Second feature coordinate
system
Xc'-Yc'-Zc'
Second feature coordinate
system
Xc'-Yc'-Zc'
Fig. 22.3 (n) Resetting of the feature coordinate system
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 857 -
- Angle of the rotary axis
When tool axis direction control (G53.1) has been performed, more
than two pairs of "computed angles" of the rotary axes usually exist.
The "computed angle" is the candidate angle at which the rotary axis
is to be controlled in the tool axis direction specified by G53.1.
The "output angle" is determined from the "computed angle" based on
the "output judgment conditions" described below.
When the upper and lower limits of the movement range of rotary
axes are specified by parameters No. 19741 to No. 19744 at this time,
a calculated angle that makes the two axes fall within the movement
range is selected.
"Output judgment conditions"
Tool rotation type or table rotation type machine
<1> The "output angles" are represented by the computed rotary axis angle
pair whose master axis (first rotary axis) moving angle is smaller.
↓
↓ When the master axis moving angle is the same
↓
<2> The "output angles" are represented by the computed rotary axis angle
pair whose slave axis (second rotary axis) moving angle is smaller.
↓
↓ When the slave axis moving angle is the same
↓
<3> The "output angles" are represented by the computed rotary axis angle
pair whose master axis (first rotary axis) angle is nearer to 0 degree
(multiple of 360 degrees).
↓
↓ When the master axis angle is equally near to 0 degree
↓
<4> The "output angles" are represented by the computed rotary axis angle
pair whose slave axis (second rotary axis) angle is nearer to 0 degree
(multiple of 360 degrees).
Composite type machine
<1> The "output angles" are represented by the computed rotary axis angle
pair whose table (second rotary axis) moving angle is smaller.
↓
↓ When the table moving angle is the same
↓
<2> The "output angles" are represented by the computed rotary axis angle
pair whose tool (first rotary axis) moving angle is smaller.
↓
↓ When the tool moving angle is the same
↓
<3> The "output angles" are represented by the computed rotary axis angle
pair whose table (second rotary axis) angle is nearer to 0 degree (multiple
of 360 degrees).
↓
↓ When the master axis angle is equally near to 0 degree
↓
<4> The "output angles" are represented by the computed rotary axis angle
pair whose tool (first rotary axis) angle is nearer to 0 degree (multiple of
360 degrees).
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 858 -
The process of judging whether the moving angle is smaller or larger
as the output judgement condition is called "movement judgement."
The "movement judgement" process is explained below.
When the "computed angle" is within the range between 0 and 360
degrees, it is called the "basic computed angle."
Usually, two pairs of "basic computed angles" exist.
For example, assume that the machine has rotary axis A (master) and
rotary axis B (slave) and that there are two pairs of basic computed
angles as follows:
(A θ1 degree; B φ1 degree)
(A θ2 degrees; B φ2 degrees) where θ1 ≤ θ2 and φ1 ≤ φ2.
The "computed angle" is obtained from either of the following
expressions: "basic computed angle" + 360 degrees × N or "basic
computed angle" - 360 degrees × N.
The current position of rotary axis A (master) is PA, and that of rotary
axis B (slave) is 0 degree.
Based on the PA angle, the "movement judgement" process is done as
follows.
• Computed angle A
-360
×
(N + 1) degrees
θ
1 - 360
×
N
-360 × N degrees
θ
2 - 360
×
N
θ
2 - 360
×
(N + 1) θ1 - 360 × (N - 1)
(*1)
0 degree 360 degrees
θ
2 - 360
θ
1
θ
2θ1 + 360
(*2)
360 × (N + 1) degrees
θ
1 + 360
×
N
360
×
N degrees
θ
2 + 360 × N
θ
2 + 360
×
(N - 1) θ1 + 360 × (N + 1)
(*3)
"Movement judgment"
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 859 -
When the PA angle is (*1):
The output angle is: (A θ2 - 360 × (N + 1) degrees; B φ2 degrees).
Namely, θ2 - 360 × (N + 1) degrees is adopted that is nearer to the
computed angle of A, and φ2, which is the same group as θ2, is
adopted as the computed angle of B.
When the PA angle is (*2):
The output angle is: (A θ1 degrees; B φ1 degrees).
Namely, θ1 degrees is adopted that is nearer to the computed angle of
A, and φ1, which is the same group as θ1, is adopted as the computed
angle of B.
When the PA angle is (*3):
The output angle is: (A θ2 + 360 × N degrees; B φ2 degrees).
Namely, θ2 + 360 × N degrees is adopted that is nearer to the
computed angle of A, and φ2, which is the same group as θ2. is
adopted as the computed angle of B.
When the moving angle of rotary axis A (master) is the same, a
"movement judgement" is made for rotary axis B (slave) according to
the "output judgment conditions."
If the "output angle" of rotary axis A is determined by the "movement
judgement" for rotary axis A, the computed angle representing the
"smaller moving angle" is adopted as the "output angle" of rotary axis
B.
Similarly, if the "output angle" of rotary axis B is determined by the
"movement judgement" for rotary axis B, the computed angle
representing the "smaller moving angle" is adopted as the "output
angle" of rotary axis A.
CAUTION
1 To use the rotary axis roll-over function, set
parameter No. 1260 (amount of rotary axis
movement per rotation) to 360 degrees.
2 A stroke limit before movement is applied to the
rotary axis subject to tool axis direction control.
3 If the setting of the lower limit (parameters No.
19742 and No. 19744) is greater than that of the
upper limit (parameters No. 19741 and No. 19743),
alarm PS5459 is issued.
4 If there is no calculated angle that falls within the
movement range because the movement range is
too small, alarm PS5459 is issued.
5 When the parameters that specify the upper limit
and lower limit of the movement range are set to 0,
no movement range is assumed to be specified.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 860 -
The "output angle" is explained below using a tool rotation type
machine as an example.
This example illustrates a machine having a "BC type tool axis Z."
• BC type tool axis Z
X
Y
Z
C-axis: First rotation axis
(master)
B-axis: Second rotation axis
(slave)
Fig. 22.3 (o) BC type tool axis Z
The following two pairs of "computed basic angles" exist that direct
the tool axis toward the +X-axis direction.
(B 90 degrees; C 180 degrees)
(B 270 degrees; C 0 degree)
<1> When the current rotary axis angles are (B -70 degrees; C 30
degrees)
The "output angles" are (B -90 degrees; C 0 degree).
0 degree is adopted because it is nearer to the current
position (30 degrees) of the C-axis that is the master axis.
For the B-axis, 270 degrees is adopted which is the same
group. However, this is changed to -90 degrees (270
degrees - 360 degrees) which is the nearest to the current
position of the B-axis (-70 degrees).
<2> When the current rotary axis angles are (B 80 degrees; C 500
degrees)
The "output angles" are (B 90 degrees; C 540 degrees).
540 degrees (180 degrees + 360 degrees) is adopted because
it is nearer to the current position (500 degrees) of the C-axis
that is the master axis. For the B-axis, 90 degrees is
adopted which is the same group.
<3> When the current rotary axis angles are (B 60 degrees; C 90
degrees)
The "output angles" are (B 90 degrees; C 180 degrees).
Since the two candidates are equally near to the current
position (90 degrees) of the C-axis that is the master axis, a
judgment is made based on the current position of the B-axis.
90 degrees is adopted because it is nearer to the current
position (60 degrees) of the B-axis that is the slave axis.
For the C-axis, 180 degrees is adopted which is the same
group.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 861 -
<4> When the current rotary axis angles are (B 180 degrees; C 90
degrees)
The "output angles" are (B 270 degrees; C 0 degree).
Since the two candidates are equally near to the current
position (90 degrees) of the C-axis that is the master axis, a
judgment is made based on the current position of the B-axis.
In this case, however, the two candidates are also equally
near to the current position of the B-axis (180 degrees).
Therefore, the candidate is adopted in which the C-axis
(master axis) is nearer to 0 degree.
That is, the pair is adopted whose C-axis angle is 0 degree
and whose B-axis angle is 270 degrees.
When the slave axis angle is 0 degree, the direction of the tool axis
becomes fixed regardless of the master axis angle.
In that case, the master axis does not move from the current angle.
An explanation is shown below using a machine having a "BC type
tool axis Z" as an example.
• BC type tool axis Z
X
Y
Z
C
Fig. 22.3 (p) BC type tool axis Z
When the current rotary axis angles are (B 45 degrees; C 90 degrees),
the "output angles" are (B 0 degree; C 90 degrees).
- Specification for rotary axes
The tilted working plane command assumes that positioning of a
rotary axis is performed by tool axis direction control (G53.1) and
then machining is performed without the rotary axis being moved.
When movement is made with the rotary axis specified directly, the
movement of the rotary axis is not considered in the movement of the
linear axis. Do not specify the movement of the rotary axis during
execution of the tilted working plane command to ensure correct
machining.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 862 -
22.3.2 Tilted Working Plane Command by Tool Axis Direction
Overview
By specifying G68.3, a coordinate system (feature coordinate system)
where the tool axis direction is the +Z-axis direction can be
automatically specified. When a feature coordinate system is used, a
program for cutting a hole or pocket in a plane tilted relative to the
workpiece coordinate system can be made simpler.
This function can automatically generate a feature coordinate system
that is normal to the tool direction.
Feature coordinate system (G68.3)
Machine coordinate system
Workpiece coordinate system (G54)
Yc
Zc
Xc
Feature coordinate system
When G68.3 is specified in a block, the coordinate system for
programming is changed to a feature coordinate system. All
commands after the block are regarded as commands in the feature
coordinate system until G69 is specified.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 863 -
Format
Format
G68.3 X x0 Y y0 Z z0 Rα ; Tilted working plane command
G69 ; Cancel tilted working plane command (M series).
G69.1; Cancel tilted working plane command (T series).
Explanation of symbols
X,Y,Z : Origin of a feature coordinate system (absolute)
By default, the current position is used as the origin of the
feature coordinate system.
R : Angular displacement about the Z-axis in the feature
coordinate system.
The default is 0°.
Coordinate system
origin shift (xo,yo,zo)
Workpiece
coordinate
s
y
stem
X
-Y-Z
Feature coordinate
system Xc-Yc-Zc
α
X
Y
Z
Zc
Yc
Xc
G68.3 command
Explanation
- Feature coordinate system
By specifying G68.3, a feature coordinate system with the tool axis
direction being the +Z-axis direction can be created. The tool axis
direction means the tool axis direction based on the rotation axis
position reached by automatic operation or manual operation.
- Origin of a feature coordinate system
The origin of a feature coordinate system must be specified using an
absolute command.
Even in the incremental command mode, the specified origin is
regarded as an absolute position.
When 1 address or 2 addresses are omitted in X, Y, Z, alarm PS5457
is issued.
When the origin of a feature coordinate system is not specified, the
position when G68.3 is specified is used as the origin.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 864 -
- Determination of a feature coordinate system
When G68.3 is specified, the tool axis direction vector (
T
) represents
the +Z direction ( Zc ) of the feature coordinate system.
The vector normal to a plane formed by the +Z direction ( Zc ) of the
feature coordinate system and the vertical axis direction vector (
P
)
(parameter No. 12321) represents the +X direction ( Xc ) of the
feature coordinate system.
Expression: ZcPXc
×
=
The vector normal to the +Z direction ( Zc ) of the feature coordinate
system and the +X direction ( Xc ) of the feature coordinate system
represents the +Y direction (Yc ) of the feature coordinate system.
Expression: XcZcYc
×
=
When R is commanded, a coordinate system rotated by R around Zc
from the above-mentioned coordinate system is the feature coordinate
system.
X-axis of feature coordinate
system
Y-axis of feature
coordinate system
Vertical axis direction: P
Z-axis of feature coordinate
system (Tool axis direction:
T)
Xc
Y
c
Zc
Determination of a feature coordinate system
When the tool axis direction vector (
T
) is parallel with the vertical
axis direction vector (
P
) (parameter No. 12321) (when the angle
between the vector (
T
) and the vector (
P
) is equal to or less than the
value of parameter No. 12322), the feature coordinate system
Xc-Yc-Zc is as indicated below. By specifying angular displacement
R, a feature coordinate system rotated about the Z-axis of this
coordinate system can be specified.
Parameter
No. 12321
Z-axis of feature
coordinate system
Zc
X-axis of feature
coordinate system
Xc
Y-axis of feature
coordinate system
Yc
1 +X direction +Y direction +Z direction
2 +Y direction +Z direction +X direction
3 +Z direction +X direction +Y direction
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 865 -
When 0 is set in parameter No. 12321, the vertical axis direction is the
reference tool axis direction (parameter No. 19697).
If a value other than 0 through 3 is set in parameter No. 12321, the
PS5459 alarm is issued.
CAUTION
Tool axis direction is Z-axis direction of feature
coordinate system regardless of the reference tool
axis direction (parameter No. 19697).
- Angular displacement R
Angular displacement R is positive when a rotation is made clockwise
viewed in the Z-axis direction of the feature coordinate system. The
range of angular displacement R is: 0.0° ≤ R ≤ 360.0°.
- Machine of table rotation type
On a machine of table rotation type, the tool direction remains
unchanged. So, a feature coordinate system based on the reference
tool axis direction (parameter No. 19697) is set. However, the origin
specification of the feature coordinate system and angular
displacement R about the Z-axis are valid.
Workpiece coordinate system X-Y-Z
Example: When reference tool axis direction represents +Z-axis
direction (with 3 set in parameter No. 19697)
Feature coordinate system
Xc-Yc-Zc
X
Y
Z
Xc
Yc
Zc
- Use in combination with tool length compensation
The G68.3 command can be specified even during tool length
compensation.
NOTE
Do not specify G68.3 during workpiece setting
error compensation. Otherwise, alarm PS0437 is
issued.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 866 -
- Example of operation
An example of operation on a machine of tool rotation type is given
below.
The machine configuration is "BC type reference tool axis Z-axis".
B: 2nd rotation axis (slave)
C: 1st rotation axis (master)
Control point
Tool holder offset value
= Parameter No. 19666
Tool length offset = H01
BC type tool axis Z-axis
(Axes are intersecting.)
Tool center point
Sample program 1
O0100 ;
N1 G55 ;
N2 G90 G01 X0Y0Z50.0 F1000 ;
N3 G43 H01 X0 Y0 Z0 ;
N4 B-45.0 ;
N5 G68.3 ;
:
N6 G69 ;
:
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 867 -
Xc
Yc
Zc
X
Y
Z
X
Y
Z
X
Y
Z
Machine operation by sample program 1
N3 command
N6 command
N5 command
N4 command
Workpiece coorditate system
X-Y-Z
Workpiece coordinate system
X-Y-Z
Feature coordinate system Xc-Yc-Zc
N3 block: Performs tool length compensation in the workpiece
coordinate system.
The tool center point moves to the origin of the workpiece
coordinate system.
N4 block: Tilts the tool.
N5 block: Sets a feature coordinate system where the tool axis
direction is the Z-axis direction and the tool center point is
placed at the origin.
N6 block: Cancels the feature coordinate system to return to the
workpiece coordinate system.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 868 -
- Multiple G68.3
After the tool axis direction is changed in G68.3 mode, by specifying
G68.3, a new feature coordinate system where the tool axis direction
is the +Z-axis direction can be specified.
Example of operation
An example of operation on a machine of tool rotation type is given
below.
The machine configuration is "AC type reference tool axis Z-axis".
A
: 2nd rotation axis (slave)
C: 1st rotation axis (master)
Control point
Tool holder offset value
= Parameter No. 19666
Tool length offset = H01
AC type tool axis Z-axis
(Axes are intersecting.)
Tool center point
Sample program 2
O0200 ;
N1 G55 ;
N2 G01 A90.0 F1000 ;
N3 G68.3 X0 Y0 Z0 R0;
:
N4 X10.0 Y0 Z0 ;
N5 C90.0;
N6 G68.3 X10.0 Y0 Z0 ;
:
N7 G69 ;
:
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 869 -
N3 command
N4 command
N6 command
N5 command
X
Y
Z
Machine operation by sample program 2
Xc
Yc
Zc
Xc
Yc
Zc
Feature coordinate system Xc-Yc-Zc
X
Y
Z
Xc
Yc
Zc
X
Y
Z
Xc
Yc
Zc
X
Y
Z
N3 block: Sets a feature coordinate system according to the tool
direction.
N4 block: Specifies coordinates in the feature coordinate system.
N5 block: Changes the tool direction.
N6 block: Sets a feature coordinate system according to the tool
direction.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 870 -
22.3.3 Tilted Working Plane command with Guidance
Overview
With the conventional tilted working plane command, a tilted working
plane can be specified based on Eulerian angle and tool axis direction.
This function enables a tilted working plane to be specified based on
the following methods:
• Tilted working plane command based on roll-pitch-yaw
• Tilted working plane command based on three points
• Tilted working plane command based on two vectors
• Tilted working plane command based on projection angles
The user can select most suitable commands for various types of
machining.
With the guidance screen function, a tilted working plane command
block can be created by entering tilted working plane data on the
screen. A complicate tilted working plane command block can be
created easily.
The guidance screen function can be enabled by setting bit 1 (GGD)
of parameter No. 11304 to 1.
The tilted working plane command with guidance is an optional
function.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 871 -
22.3.3.1 Tilted working plane command based on roll-pitch-yaw
Overview
With the tilted working plane command, coordinate system conversion
by rotation about the X-axis, Y-axis, and Z-axis of a workpiece
coordinate system in this order can be used (roll-pitch-yaw).
The order of rotary axes can be specified using address Q.
X
Y
Z
Xc
Zc
Yc
(1)
(2)
(3)
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 872 -
Format
Format
G68.2 P1 Qq X_ Y_ Z_ Iα Jβ Kγ; Tilted working plane command
G69 ; Cancel tilted working plane command (M series).
G69.1; Cancel tilted working plane command (T series).
Explanation of symbols
Q : Order in which axes are rotated
X_ Y_ Z_ : Origin of a feature coordinate system
I : Angle of rotation about the X-axis (roll angle)
J : Angle of rotation about the Y-axis (pitch angle)
K : Angle of rotation about the Z-axis (yaw angle)
The values of address Q and the order in which axes are rotated are
shown below.
First rotation
axis
Second rotation
axis
Third rotation
axis
Q 123 X axis Y axis Z axis
Q 132 X axis Z axis Y axis
Q 213 Y axis X axis Z axis
Q 231 Y axis Z axis X axis
Q 312 Z axis X axis Y axis
Q 321 Z axis Y axis X axis
CAUTION
1 When address Q is omitted, the X-axis, Y-axis, and
Z-axis are rotated in this order.
(equivalent to Q123)
2 When address Q is set to a value other than the
above, alarm PS5457 is issued.
Explanation
Suppose that the coordinate system is rotated about (1) the X-axis, (2)
the Y-axis, and (3) the Z-axis in this order.
A "workpiece coordinate system" rotated by angle α about the X-axis
is "coordinate system 1".
"Coordinate system 1" rotated by angle β about the Y-axis is
"coordinate system 2". "Coordinate system 2" rotated by angle γ
about the Z-axis then shifted by (X0,Y0,Z0) from the workpiece
coordinate system origin is a "feature coordinate system".
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 873 -
Conversion from the workpiece
coordinate system X-Y-Z to
coordinate system 1 X’-Y’-Z’
x
z
y
y’
z’
α
α
x
z
y
y’
z’
x’’
z’’
y’’
β
β
β
γ
x
z
y
x’’
z’’
y’’
γ
γ
xc
yc
zc
Conversion from coordinate system
1 X’-Y’-Z’ to coordinate system 2
X"-Y"-Z"
Conversion from coordinate system 2
X"-Y"-Z" to the feature coordinate
system Xc-Yc-Zc
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 874 -
G68.2 P1 Q123 X200.0 Y0 Z50.0 I30.0 J0 K90.0 ;
G53.1 ;
:
Example
The example of a program when feature coordinate system like the
figure below is used is shown below.
• Feature coordinate system origin : (200.0, 0, 50.0)
• Order in which axes are rotated : X axis → Y axis → Z axis
• Angle of rotation about the X-axis : 30 degrees
• Angle of rotation about the Y-axis : 0 degree
• Angle of rotation about the Z-axis : 90 degrees
Example of a program
X
Y
Z
30°
Xc
Zc
Yc
Workpiece coordinate system
X
-Y-Z
Feature coordinate system
X
c-Yc-Zc
200.0
50.0
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 875 -
22.3.3.2 Tilted working plane command based on three points
Overview
With the tilted working plane command, a tilted working plane can be
specified by specifying three points in a feature coordinate system.
X
Y
Z
P3
P2 P1
X
c
Zc
Y
c
Format
Format
G68.2 P2 Q0 X x0 Y y0 Z z0 Rα ;
G68.2 P2 Q1 X x1 Y y1 Z z1 ;
G68.2 P2 Q2 X x2 Y y2 Z z2 ;
G68.2 P2 Q3 X x3 Y y3 Z z3 ; Tilted working plane command
G69 ; Cancel tilted working plane command (M series).
G69.1; Cancel tilted working plane command (T series).
Explanation of symbols
Q0 X x0 Y y0 Z z0 :
A
mount of shift from the first point to the origin of a
feature coordinate system
By default, this value is 0.
Q1 X x1 Y y1 Z z1 : First point. (origin of a feature coordinate system)
Q2 X x2 Y y2 Z z2 : Second point.
Q3 X x3 Y y3 Z z3 : Third point.
R : Angle of rotation about the Z-axis of a feature coordinate system
By default, this value is 0.
Any block in the G68.2 P2 command can be specified.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 876 -
Coordinate system origin shift
Xc
Y
c
Zc
Workpiece
coordinate system
X-Y-Z
Feature coordinate system Xc-Yc-Zc
X
Y
Z
α
P1
P3
P2
CAUTION
1 Three G68.2P2 commands (Q1, Q2, and Q3)
determine a tilted plane. If the G68.2P2
commands are interrupted, alarm PS5457 is
issued.
2 When any of the following conditions is met or
address Q is set to a value other than the above,
alarm PS5457 is issued.
• When two or more points are duplicate (the
plane is not determined.)
• When three points are placed on a line (the
plane is not determined.)
• When the distance between a line passing two
of the three points and the remaining point is
smaller than the setting of parameter No. 11220
(the plane is unstable.)
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 877 -
Explanation
- Determination of a feature coordinate system
Three entered points are named P1, P2, and P3 in the order of entry.
The P1-to-P2 direction is defined as the X-axis of a feature coordinate
system. Among the directions that are on the plane containing the
three points and are normal to the X-axis of the feature coordinate
system, the direction that makes a smaller angle with the P1→P3
vector is defined as the Y-axis of the feature coordinate system. The
Z-axis of the feature coordinate system is defined according to the
right-handed system.
Feature coordinate
system
Xc－Yc－Zc
Y
X
P1
P3 P2
Xc
Yc
(Yc1)
Zc
Z
Workpiece
coordinate system
X－Y－Z
β
α
Yc2
On the plane containing three points, there are two directions normal to
Xc: Yc1 and Yc2. Angles α and β formed relative to the P1→P3 vector
satisfy
α
<
β
, so that Yc1 is selected as Yc.
- Origin of the feature coordinate system
The origin of the feature coordinate system is the first specified point
P1.
By setting an origin shift amount (G68.2 P2 Q0 X_Y_Z_), the origin
of the feature coordinate system is shifted by (X,Y,Z) from P1.
Specify (X,Y,Z) in the feature coordinate system.
- Angular displacement R
The angular displacement R is positive for clockwise rotation viewed
in the Z-axis direction in the feature coordinate system.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 878 -
G68.2 P2 Q1 X200.0 Y0 Z50.0 ;
G68.2 P2 Q2 X200.0 Y100.0 Z50.0 ;
G68.2 P2 Q3 X26.795 Y0 Z150.0 ;
G53.1 ;
. . .
Example
The example of a program when feature coordinate system like the
figure below is used is shown below.
• First point (origin of a feature coordinate system)
: (200.0, 0, 50.0)
• Second point : (200.0, 100.0, 50.0)
• Third point : (26.795, 0, 150.0)
Example of a program
X
Y
Z
30°
Xc
Zc
Yc
Workpiece coordinate system
X
-Y-Z
Feature coordinate system Xc-Yc-Zc
200.0
50.0 First point
Second point
Third point
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 879 -
22.3.3.3 Tilted working plane command based on two vectors
Overview
With the tilted working plane command, a tilted working plane can be
specified by specifying an X-axis direction vector and a Z-axis
direction vector in the feature coordinate system.
X
Y
Z
X
c
Zc
Yc
V
1
V
2
Format
Format
G68.2 P3 Q1 X_ Y_ Z_ Iα1 Jβ1 Kγ1 ;
G68.2 P3 Q2 Iα2 Jβ2 Kγ2 ; Tilted working plane command
G69 ; Cancel tilted working plane command (M series).
G69.1; Cancel tilted working plane command (T series).
Explanation of symbols
X_ Y_ Z_ : Origin of a feature coordinate system (specifiable in
the Q1 block)
Q1 Iα1 Jβ1 Kγ1 : Feature coordinate system X-axis direction relative to
the workpiece coordinate system (first vector)
Q2 Iα2 Jβ2 Kγ2 : Feature coordinate system Z-axis direction relative to
the workpiece coordinate system (second vector)
CAUTION
1 The two G68.2P3 commands (Q1 and Q2) determine a tilted
plane. The G68.2P3 commands are interrupted, alarm
PS5457 is issued.
2 If the angle between the two vectors is 5 degrees or more off
the 90 degrees, alarm PS5457 is issued.
3 If (I, J, K) is set to a 0 vector, alarm PS5457 is issued.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 880 -
Explanation
- Determination of a feature coordinate system
The first vector is defined as the X-axis of the feature coordinate
system, and the second vector is defined as the Z-axis of the feature
coordinate system. The Y-axis of the feature coordinate system is
defined according to the right-handed system.
Xc
Zc
Yc (Yc1)
V
1
V
2
Yc2
There are two vectors normal to the Xc-axis and Zc-axis.
However, Yc1 is defined as the Yc-axis of the feature
coordinate system according to the right-handed system.
- When the first and second vectors are not normal
When the first vector and second vector are not normal, the
orthographical vector from the second vector to plane P normal to the
first vector is defined as the Z-axis of the feature coordinate system.
Xc (first vector)
Zc Second vector
Plane P normal to the first vector
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 881 -
G68.2 P3 Q1 X200.0 Y0 Z50.0 I0 J1.0 K0 ;
G68.2 P3 Q2 I100.0 J0 K173.205 ;
G53.1 ;
. . .
Example
The example of a program when feature coordinate system like the
figure below is used is shown below.
Origin of a feature coordinate system : (200.0, 0, 50.0)
X-axis direction of a feature coordinate system : (0, 1.0, 0)
(First vector)
Z-axis direction of a feature coordinate system : (100.0, 0, 173.205)
(Second vector )
Example of a program
X
Y
Z
30°
Xc
Zc
Yc
Workpiece coordinate system
X
-Y-Z
Feature coordinate system
Xc-Yc-Zc
200.0
50.0
First vector
Second vector
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 882 -
22.3.3.4 Tilted working plane command based on projection angles
Overview
With the tilted working plane command, a tilted working plane can be
specified based on projection angles.
A plane determined by vector A and vector B produced by rotating the
X-axis vector and Y-axis vector of the workpiece coordinate system is
defined to be a tilted working plane.
X
Y
-α
β
γ
X
c
Yc
A
B
Format
Format
G68.2 P4 X_ Y_ Z_ Iα Jβ Kγ; Tilted working plane command
G69 ; Cancel tilted working plane command (M series).
G69.1; Cancel tilted working plane command (T series).
Explanation of symbols
X_ Y_ Z_ : Origin of a feature coordinate system
α : Angle by which the X-axis vector is rotated about the
Y-axis of the workpiece coordinate system
β : Angle by which the Y-axis vector is rotated about the
X-axis of the workpiece coordinate system
γ : Angle of rotation about the Z-axis of the feature coordinate
system
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 883 -
Explanation
- Determination of a feature coordinate system
The X-axis direction vector of the workpiece coordinate system
rotated by α about the Y-axis of the workpiece coordinate system is
defined as vector A. The Y-axis direction vector of the workpiece
coordinate system rotated by β about the X-axis of the workpiece
coordinate system is defined to be vector B.
The direction normal to plane P containing vector A and vector B
(direction of the outer product of A × B) is defined to be the Z-axis
direction of the feature coordinate system.
Vector A rotated by γ about the Z-axis of the feature coordinate
system is defined to be the X-axis direction of the feature coordinate
system. The Y-axis of the feature coordinate system is defined
according to the right-handed system.
X
Y
Z
-α
β
A
B
Zc
Plane P
By the third command angle α and second command angle β, the
Z-axis of the feature coordinate system are determined.
X
Y
Z
A
B
Yc
γ
Plane P
Zc
Xc
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 884 -
G68.2 P4 X200.0 Y0 Z50.0 I30.0 J0 K90.0 ;
G53.1 ;
:
By the third command angle γ, the X-axis and Y-axis of the feature
coordinate system are determined.
NOTE
When vector A and vector B are considered to be
parallel with each other (when the angle formed by
the two vectors is smaller than 1°), alarm PS5457
is issued.
Example
The example of a program when feature coordinate system like the
figure below is used is shown below.
• Origin of a feature coordinate system :
(200.0, 0, 50.0)
• Angle by which the X-axis vector is rotated about the Y-axis of
the workpiece coordinate system : 30 degrees
• Angle by which the Y-axis vector is rotated about the X-axis of
the workpiece coordinate system : 0 degree
• Angle of rotation about the Z-axis of the feature coordinate
system : 90 degrees
Example of a program
X
Y
Z
30
°
Xc
Zc
Yc
Workpiece coordinate system
X
-Y-Z
Feature coordinate system Xc-Yc-Zc
200.0
50.0
A
B
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 885 -
22.3.3.5 Absolute multiple command
By additionally specifying G68.2 in the tilted working plane
command mode, a feature coordinate system produced by additionally
applying coordinate system conversion to the workpiece coordinate
system can be set. The workpiece coordinate system is resumed by
specifying G69.
This function is enabled by setting bit 0 (MTW) of parameter No.
11221.
Format
The format of the tilted working plane command (G68.2) is
applicable.
Specify the origin of a feature coordinate system in the workpiece
coordinate system.
NOTE
Before specifying G68.2, cancel tool length
compensation and tool radius compensation. If
G68.2 is specified during tool length compensation
or tool radius compensation, alarm PS5462 is
issued.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 886 -
Example of operation
An example of operation on a tool rotation type machine is explained
below.
The machine configuration is "BC type with the reference tool axis
being the Z-axis".
B: 2nd rotation axis (slave)
C: 1st rotation axis (master)
Control point
Tool holder offset value
= Parameter No. 19666
Tool length offset = H01
Machine on which tool rotary
axes cross each other
Tool center point
Sample program 2
O0100 ;
N1 G55 ;
N2 G90 G01 X20.0 Y5.0 Z0 F1000 ;
N3 G68.2 X20.0 Y5.0 Z0 I0 J90.0 K0 ;
N4 G53.1 ;
:
N5 X-15.0 Y0 Z-15.0 ;
N6 G68.2 X5.0 Y20.0 Z0 I90.0 J90.0 K0 ;
N7 G53.1;
:
N8 G69 ;
:
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 887 -
N6 command
X
Y
Z
N4 command
Machine operation by sample program 1
N7 command
N5 command
X
Y
Z
X
Y
Z
Xc
Y
c
Zc
X
Y
Z
Feature coordinate system
Xc-Yc-Zc
Feature coordinate system
Xc-Yc-Zc
Xc
Y
c
Zc
Xc
Y
c
Zc
Xc
Y
c
Zc
G55
Machine
origin
N4 block: Rotates the tool in the Z-axis direction in the feature
coordinate system.
N5 block: Specifies coordinates in the feature coordinate system.
N6 block: Sets a new feature coordinate system.
N7 block: Rotates the tool in the Z-axis direction in the new feature
coordinate system.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 888 -
22.3.3.6 Incremental multiple command
By specifying G68.4, coordinate system conversion can be applied to
the currently set feature coordinate system.
This function is enabled by setting bit 0 (MTW) of parameter No.
11221.
Format
The format of the tilted working plane command (G68.2) is
applicable.
Specify the origin of a feature coordinate system in the immediately
preceding feature coordinate system.
Specification method Incremental multiple command
Eulerian angle G68.4
Roll-pitch-yaw G68.4 P1
Three points G68.4 P2
Two vectors G68.4 P3
Projection angles G68.4 P4
NOTE
1 Before specifying G68.4, cancel tool length
compensation and tool radius compensation. If
G68.4 is specified during tool length compensation
or tool radius compensation, alarm PS5462 is
issued.
2 Do not specify G68.4 during workpiece setting
error compensation. Otherwise, alarm PS0437 is
issued.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 889 -
Example of operation
An example of operation on a tool rotation type machine is explained
below.
Rotary axis C rotates about the Z-axis (master axis).
Rotary axis B rotates about the Y-axis (slave axis).
B: 2nd rotation axis (slave)
C: 1st rotation axis (master)
Control point
Tool holder offset value
= Parameter No. 19666
Tool length offset = H01
BC type tool axis Z-axis
(Axes are intersecting.)
Tool center point
Sample program 3
O0200 ;
N1 G55 ;
N2 G90 G01 X20.0 Y5.0 Z0 F1000 ;
N3 G68.2 X20.0 Y5.0 Z0 I0 J90.0 K0 ;
N4 G53.1 ;
:
N5 X-15.0 Y0 Z-15.0 ;
N6 G68.4 X-15.0 Y0 Z-15.0 I90.0 J90.0 K-90.0 ;
N7 G53.1;
:
N8 G69 ;
:
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 890 -
N6 command
X
Y
Z
N4 command
Machine operation by sample program 2
N7 command
N5 command
Xc1
Y
c1
Zc1
X
Y
Z
X
Y
Z
Xc2
Y
c2
Zc2
X
Y
Z
Feature coordinate system
Xc1-Yc1-Zc1
Feature coordinate system
Xc2-Yc2-Zc2
Xc1
Y
c1
Zc1
Xc2
Y
c2
Zc2
Xc1
Y
c1
Zc1
Xc1
Y
c1
Zc1
N4 block: Rotates the tool in the Z-axis direction in the feature
coordinate system.
N5 block: Specifies coordinates in the feature coordinate system.
N6 block: Applies coordinate system conversion to the feature
coordinate system based on Eulerian angle to set a new
feature coordinate system.
N7 block: Rotates the tool in the Z-axis direction in the new feature
coordinate system.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 891 -
Limitation
- Basic restrictions
The restrictions for this function are similar to those for the
three-dimensional coordinate system conversion function.
- Increment system
The same increment system must be used for the basic three axes used
by this function.
- Rapid traverse command
The rapid traverse command must specify linear rapid traverse (Bit 1
(LRP) of parameter No.1401= 1).
- Feature coordinate system and three-dimensional coordinate system conversion
An alarm occurs if an attempt is made to set a feature coordinate
system in another feature coordinate system.
An alarm also occurs if an attempt is made to set a new coordinate
system by performing three-dimensional coordinate system
conversion in a feature coordinate system.
- Positioning in the machine coordinate system
Positioning commands in the machine coordinate system, such as G28,
G30, and G53, operate in the machine coordinate system rather than in
the feature coordinate system.
- External mirror image
If an attempt is made to use this function and the external mirror
image function simultaneously, this function takes effect before the
external mirror image function.
A
ctual path
Y
X
Yc
Xc
Programmed path
Feature coordinate
system
Workpiece coordinate
system Mirrored position
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 892 -
- Relationships with other modal commands
G41, G42, and G40 (tool radius compensation), G43 and G49 (tool
length compensation), G51.1 and G50.1 (programmable mirror image),
and canned cycle commands must have nesting relationships with
G68.2.
In other words, first issue G68.2 when the modes mentioned above are
off, then turn the modes on and off, and then issue G69.
- Parallel axis control
When a parking signal is applied to an axis during parallel axis control,
conversion to a feature coordinate system occurs for another axis if a
move command is issued for that another axis. For this reason, an
axis may move even if a parking signal has been applied to it.
- Specifiable G codes
The G codes that can be specified in the tilted working plane
command mode are listed below.
Specifying a G code other than these codes results in alarm PS5462.
• Positioning (G00)
• Linear interpolation (G01)
• Circular interpolation / helical interpolation (G02/G03)
• Dwell (G04)
• Programmable data input (G10)
• Programmable data input mode cancel (G11)
• Plane selection (G17/G18/G19)
• Automatic return to reference position (G28)
• Movement from reference position (G29)
• 2nd, 3rd and 4th reference position return (G30)
• Skip function (G31)
• Tool radius compensation : cancel (G40)
• Tool radius ⋅ tool nose radius compensation /
3-dimensional cutter compensation (G41/G42)
• Tool length compensation + (G43)
• Tool length compensation - (G44)
• Tool length compensation cancel (G49)
• Machine coordinate system setting (G53)
• Tool axis direction control (G53.1)
• Macro call (G65)
• Macro modal call A (G66)
• Macro modal call B (G66.1)
• Macro modal call A/B cancel (G67)
• Absolute programming (G90)
• Incremental programming (G91)
• Canned cycle for drilling (G73, G74, G76, G80 to G89)
• Constant surface speed control (G96)
• Constant surface speed control cancel (G97)
• Canned cycle : return to initial level (G98)
• Canned cycle : return to R point level (G99)
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 893 -
M
• Programmable mirror image (G50.1/G51.1)
• Coordinate system rotation cancel or 3-dimensional coordinate
conversion mode off (G69)
• Feed per minute (G94)
• Feed per revolution (G94)
T
• Coordinate system rotation cancel or 3-dimensional coordinate
conversion mode off (G69.1)
• Feed per minute (G98 (G94))
• Feed per revolution (G99 (G94))
- Modal G codes that allow specification of a tilted working plane command
A tilted working plane command can be specified in the modal G code
states listed below.
In a modal state other than the following modal G codes, specifying
the tilted working plane command results in alarm PS5462:
• Modal G codes included in "Specifiable G codes" described
previously
(However, G43/G44 and G41/G42 are excluded.)
• Polar coordinate interpolation mode cancel (G13.1)
• Polar coordinates command cancel (G15)
• Input in inch (G20 (G70))
• Input in mm (G21 (G71))
• Stored stroke check function (G22/G23)
• Scaling cancel (G50)
• Polygon turning cancel (G50.2)
• Workpiece coordinate system 1 selection (G54 to G59)
• Workpiece setting error compensation (G54.4)
• Exact stop mode (G61)
• Automatic corner override (G62)
• Tapping mode (G63)
• Cutting mode (G64)
• Inverse time feed (G93)
• Constant surface speed control cancel (G97)
M
• Polar coordinate interpolation mode cancel (G113)
T
• Programmable mirror image cancel (G50.1)
• Mirror image for double turret off/balanced cutting mode cancel
(G69)
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 894 -
22.4 INCLINED ROTARY AXIS CONTROL
Overview
The conventional tilted working plane command / tool center point
control function / 3-dimensional cutter compensation /
three-dimensional manual feed can be used only for those machines
whose tool rotation axis or table rotation axis is parallel to the basic
axis of the basic coordinate system. (See Fig. 22.4 (a).)
Inclined rotary axis control is intended to allow the tilted working
plane command / tool center point control function / 3-dimensional
cutter compensation / three-dimensional manual handle feed to be
applied even when the tool rotation axis or table rotation axis is
inclined with respect to the X-Z plane, a Y-Z plane or a Z-X plane of
the machine coordinate system.
<2> Table rotation type machine
<3> Composite type machine
<1> Tool rotation type machine
X
Y
Z
B
C
X
Y
Z
A
C
X
C
B
Z
Y
A
C
X
Z
Y
B
Y
X
Z
C
X
Y
Z
C
B
Fig. 22.4 (a) Three types of 5-axis machine
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 895 -
An example of a tool rotation type machine is explained below. (See
Fig. 22.4 (b).)
The machine shown in Fig. 22.4 (b) has rotary axis B (master) that
turns around the Y-axis and rotary axis C (slave) whose Y-axis is
inclined at an angle of 45 degrees on the Y-Z plane.
The tilted working plane command / tool center point control function
/ 3-dimensional cutter compensation / three-dimensional manual feed
can be used even for the machine configuration shown in Fig. 22.4
(b).
B
C
Y
Z
X
C
B
Fig. 22.4 (b) Tool rotation type machine
An example of a table rotation type machine is explained below.
(See Fig. 22.4 (c).)
The machine shown in Fig. 22.4 (c) has rotary axis B (master) whose
Y-axis is inclined at an angle of -45 degrees on the Y-Z plane and
rotary axis C (slave) that turns around the Z-axis.
The tilted working plane command / tool center point control function
/ 3-dimensional cutter compensation / three-dimensional manual feed
can be used even for the machine configuration shown in Fig. 22.4 (c).
B
C
Z
Y
X
C
B
Fig. 22.4 (c) Table rotation type machine
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 896 -
An example of a composite type machine is explained below. (See
Fig. 22.4 (d).)
The machine shown in Fig. 22.4 (d) has table rotation axis B whose
Y-axis is inclined at an angle of -45 degrees on the Y-Z plane and tool
rotation axis C that turns around the Z-axis.
The tilted working plane command / tool center point control function
/ 3-dimensional cutter compensation / three-dimensional manual feed
can be used even for the machine configuration shown in Fig. 22.4
(d).
B
Z
Y
X
A
B
A
Fig. 22.4 (d) Composite type machine
Format and operation
The operation of the tilted working plane command / tool center point
control function / 3-dimensional cutter compensation /
three-dimensional manual feed during the inclined rotary axis control
is similar to the operation performed when the inclined rotary axis
control is not in use.
For details, see the description of each function.
Limitation
The operation of the tilted working plane command / tool center point
control function / 3-dimensional cutter compensation /
three-dimensional manual feed during the inclined rotary axis control
is similar to the operation performed when the inclined rotary axis
control is not in use.
For details, see the description of each function.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 897 -
22.5 3-DIMENSIONAL CUTTER COMPENSATION
Overview
For machines having multiple rotary axes for freely controlling the
orientation of a tool axis, this function calculates a tool vector from
the positions of these rotary axes. The function then calculates a
compensation vector in a plane (compensation plane) perpendicular to
the tool vector and performs 3-dimensional cutter compensation.
The compensation is performed on the block end point.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 898 -
- Machine configuration
This function is applicable to the following machine configurations:
<1> Tool rotation type machine controlled with two tool rotation axes
<2> Table rotation type machine controlled with two table rotation
axes
<3> Composite type machine controlled with one tool rotation axis
and one table rotation axis
<2> Table rotation type machine
<1> Tool rotation type machine
X
C
B
Z
Y
A
C
X
Z
Y
<3> Composite type machine
B
Y
X
Z
C
Fig. 22.5 (a) Three types of machine configuration
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 899 -
The coordinate system in which to execute a program for
3-dimensional cutter compensation is called a programming
coordinate system.
If, in a 5-axis machine having a table rotation axis, 3-dimensional
cutter compensation (tool side offset) is to be performed, the table
coordinate system (coordinate system fixed to the table) can be
selected as a programming coordinate system.
Alternatively, the workpiece coordinate system fixed to the machine
coordinate system can be selected as a programming coordinate
system.
There are two types of 3-dimensional cutter compensation (tool side
offset), which differ in the method of specifying the tool axis
direction.
(1) Type 1
Specify the block end position (for example, A, B, C) of the
rotation axis. The CNC performs cutter compensation on the
plane perpendicular to the tool axis direction calculated from
the specified position on the rotation axis.
(2) Type 2
Instead of specifying a position on the rotation axis, specify the
tool axis direction (I, J, K) at the block end point as viewed
from the table coordinate system. The CNC calculates the end
position on the rotation axis so that the tool points to the
specified direction at the end point, and performs cutter
compensation on the plane perpendicular to the tool axis
direction calculated from the position on the rotation axis.
By using type 2, it is possible to perform the same machining with the
same program regardless of the machine configuration of the 5-axis
machine (tool rotation type, table rotation type, or composite type).
Tool rotation type Table rotation type Composite type
Same program
O0001
:
G41.6 D1
G01 X100. I1.0 K1.0 F1000
:
Fig. 22.5 (b) Type 2 Program
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 900 -
22.5.1 Cutter Compensation in Tool Rotation Type Machine
Overview
In a 5-axis machine having two tool rotation axes as shown in Fig.
22.5.1 (a), this function can perform cutter compensation.
Shown below is a 5-axis machine that has tool rotation axis B on the
Y-axis and tool rotation axis C on the Z-axis.
This machine configuration is used as a sample configuration in the
following explanation unless otherwise noted.
Cutter compensation in tool rotation machines is classified into two
types according to the way of machining: tool side offset and
leading edge offset.
Workpiece coordinate system: A coordinate
system used for creating programs
B
C
Z
Y
X
X
Y
ZWorkpiece coordinate
system
Fig. 22.5.1 (a) Machine having two tool rotation axes
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 901 -
22.5.1.1 Tool side offset
Overview
This type of cutter compensation performs three-dimensional
compensation in a plane (compensation plane) perpendicular to the
tool vector.
Compensation
plane
YZ
X
Tool vector
Cutter compensation
amount
Tool center path
(path after
compensation)
Programmed path
(path before compensation)
Cutter compensation vector
Fig. 22.5.1.1 (a) Tool side offset
Format
- Tool side offset (type 1)
G41.2 (or G42.2) IP_ D_ ;
IP_ ;
:
G41.2: Cutter compensation left (group 07)
G42.2: Cutter compensation right (group 07)
IP_: Value specified for axis movement (including rotary
axis)
D_: Code specifying the cutter compensation amount (1
to 3 digits)
- Tool side offset (type 2)
G41.6 (or G42.6) IP_ I_ J_ K_ D_ Q_ ;
IP_ I_ J_ K_ ;
:
G41.6: Cutter compensation left (group 07)
G42.6: Cutter compensation right (group 07)
IP_: Value specified for axis movement (without rotary
axis)
D_: Code specifying the cutter compensation amount (1
to 3 digits)
Q_: Tool’s angle of gradient (in degrees)
I_ J_ K_: Tool axis direction at the block end point as
viewed from the programming coordinate system
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 902 -
For type 2, do not specify a rotation axis but specify the direction at
the tool end point as viewed from the programming coordinate system
(workpiece coordinate system), with I, J, and K. Specifying a
rotation axis causes alarm PS5460 to be generated.
NOTE
When a movement perpendicular to the next
movement (bit 1 (SUV) of parameter No. 5003 is
set to 1) is specified as the operation performed
at the time of startup or cancellation, a move
command such as X_ Y_ Z_ must not be
specified in the G41.2 and G42.2 block.
The following are the notes on type 2.
NOTE
1 If one or two of I, J, and K are omitted, the omitted
ones of I, J, and K are assumed to be 0.
2 In a block in which all of I, J, and K are omitted,
the values of I, J, and K in the previous block are
used.
3 If there is only one rotation axis (a hypothetical
axis is used), type 2 cannot be used. In this
case, if an attempt is made to issue G41.6/G42.6,
alarm PS5460 is generated.
4 If using the rotation axis rollover function or rotary
axis control function, specify 360 degrees in
parameter No. 1260 (mount of travel per rotation
about the rotation axis).
5 Only tool side offset provides type 2 commands.
Leading edge offset, described later, does not
provide type 2 commands.
- Canceling the tool side offset
G40 IP_ ;
G40: Cancellation of cutter compensation (group 07)
IP_: Value specified for axis movement
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 903 -
Explanation
- Tool’s angle of gradient in type 2
For type 2 of 3-dimensional cutter compensation, the tool's angle of
gradient can be specified with address Q in a G41.6/G42.6 command
block. The tool's angle of gradient refers to the angle by which the
tool direction to be assumed when machining is actually performed is
inclined from the direction specified with (I, J, K) toward the traveling
direction on the plane formed by the tool direction specified with (I, J,
K) and the traveling direction in the programming coordinate system.
(See Fig. 22.5.1.1 (b).)
Because in general, the normal direction of the machining surface is
specified with (I, J, K), if it is desired to incline the tool direction to be
assumed when machining is actually performed from the normal
direction toward the traveling direction, correction may be performed
with a Q command.
If the direction specified with (I, J, K) matches the tool direction to be
assumed when machining is actually performed, no Q command is
necessary.
Tool direction to be assumed when
machining is actually performed
(Plane perpendicular to the "tool direction to be
assumed when machining is actually performed")
Tool direction
specified with (I, J, K)
Traveling
direction of
machinin
g
Tool's angle of gradient (Q)
Compensation plane
Tool center path
(path after compensation)
Programmed path
(path before compensation)
Cutter
compensation
vector
Fig. 22.5.1.1 (b) Tool's angle of gradient in type 2
(Example)
To perform machining by inclining the tool's traveling direction
twice, issue a command such as the following:
G41.6 I_ J_ K_ H_ Q2.0
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 904 -
- Operation at startup and cancellation
<1> Type A
The tool is moved in the same way as for cutter compensation as
shown below.
Tool
G41.2 G40
: Tool center path
: Programmed path
Operation in linear interpolation
: Tool center path
: Pro
g
rammed
p
ath
Tool
G42.2
G40
Operation in circular interpolation
Fig. 22.5.1.1 (c) Operation at startup and cancellation (type A)
When the G40 block contains no movement command, type C
cancellation is performed (see <3> Type C below).
<2> Type B
The tool is moved in the same way as for cutter compensation as
shown below.
Tool
G41.2
G40
: Tool center path
: Programmed path
Operation in linear interpolation
: Tool center path
: Programmed path
Tool
G42.2
G40
Operation in circular interpolation
Fig. 22.5.1.1 (d) Operation at startup and cancellation (type B)
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 905 -
When the G40 block contains no movement command, type C
cancellation is performed (see <3> Type C below).
<3> Type C
When G41.2, G42.2, or G40 is specified as shown below, a linear
block specifying movement by the amount of cutter
compensation in the direction orthogonal to the movement
direction of the block following startup or the block preceding
cancellation is inserted.
Tool
G41.2 G40
: Tool center path
: Programmed path
Operation in linear interpolation
: Tool center path
: Programmed path
Tool
G42.2
G40
Operation in circular interpolation
Fig. 22.5.1.1 (e) Operation at startup and cancellation (type C)
NOTE
For type C (bit 1 (SUV) of parameter No. 5003 is
1), the following conditions need to be satisfied
during startup and cancellation.
1 A block specifying G40, G41.2, or G42.2 must
be in the G00 or G01 mode.
2 A block specifying G40, G41.2, or G42.2 must
contain no move command.
3 The block next to a block specifying G41.2 or
G42.2 must contain move command G00, G01,
G02, or G03.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 906 -
- Operation during compensation
Operations such as change of the offset direction and offset value,
retention of a vector, and interference checks are performed in the
same way as for cutter compensation. However, G39 (corner
rounding) cannot be specified. So, note the following:
<1> When the tool center path goes outside the programmed path at a
corner, a linear movement takes place at the corner without
inserting an arc. When the tool center path goes inside the
programmed path, nothing is inserted.
: Tool center path
: Programmed path
Example <1>-1
Going outside of corner at
acute angle
Example <1>-2
Going inside of corner
Linear block inserted
Tool
Tool
Workpiece Workpiece
: Tool compensation
amount
Nothing inserted
Fig. 22.5.1.1 (f) Operation during compensation <1>-1 and <1>-2
In the above examples, the terms "inside" and "outside" denote
how the tool center path is positioned with respect to the
programmed path. In the figure below, example <1>-3 shows
the same relationship between the tool center path and
programmed path as example <1>-1 and indicates that the tool
center path is outside the programmed path; example <1>-4
shows the same relationship as example <1>-2 and indicates that
the tool center path is inside the programmed path.
: Tool center path
: Programmed path
Example <1>-3 Example <1>-4
A
ctual
tool
Reference
tool
A
ctual
tool
Reference
tool
Workpiece
Workpiec
: Tool compensation
amount
Fig. 22.5.1.1 (g) Operation during compensation <1>-3 and <1>-4
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 907 -
<2> When the tool moves at a corner, the feedrate of the previous
block is used if the corner is positioned before a single-block
stop point; if the corner is after a single-block stop point, the
feedrate of the next block is used.
: Tool center path
: Programmed path
Example <2>-1
F100
Tool Program <2>-1
:
N1 G90 G41.2 Xp Yp Zp Bp Cp D1 ;
N2 G01 Xq Yq Zq F100 ;
N3 Xr Yr Zr F200 ;
:
N2 N3
P' P
Q1'
R'
R
Q
Q2' (single-block stop point)
Fig. 22.5.1.1 (h) Operation during compensation <2>
In the above example, the single-block stop point of N2 is Q2', so
the feedrates along paths P'-Q1' and Q1'-Q2' are both F100.
<3> When a command that makes the tool retrace the path of the
previous block is specified, the tool path can match the locus of
the previous block by changing the G code to change the offset
direction. If the G code is left unchanged, the operation shown
in example <3>-2 results:
: Tool center path
: Programmed path
Example <3>-1
When changing G41.2 to G42.2
(G41.2 mode)
G91 G01 X100.0
G42.2 X-100.0
Example <3>-2
When leaving G code unchanged
(G41.2 mode)
G91 G01 X100.0
X-100.0
Fig. 22.5.1.1 (i) Operation during compensation <3>
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 908 -
- Interference check when the compensation plane changes
An interference check is made when the compensation plane (a plane
perpendicular to the tool vector) has changed.
Example:
If the following program is executed, an alarm PS0041
(INTERFERENCE IN CUTTER COMPENSATION) is issued at N4:
O100 F3000
N1 G90 G00 X0 Y0 Z0 A-46 C180
N2 G41.2 D1
N3 G01 X100
N4 Y-200 Z-200
N5 A45
N6 Y-400 Z0
N7 X0
N8 Y-200 Z-200
N9 A-46
N10 Y0 Z0
N11 G40
M30
X
Y
Z
N3
N4
N6
N5
N7
N8
N10
N9
Fig. 22.5.1.1 (j) Conceptual diagram
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 909 -
Y
Z
VaVb
46°
45°
Va: Tool vector when A=-46
Vb: Tool vector when A=45
A
: End point of N3
B: End point of N4
C: End point of N6
A
B
C
Fig. 22.5.1.1 (k) Tool vector
e3
e2
A
’ C’ B’
V1
V2
A
’: Point A projected onto the compensation plane
B’: Point B projected onto the compensation plane
C’: Point C projected onto the compensation plane
Fig. 22.5.1.1 (l) Compensation vector at the end point (point B) of N4 (in
the compensation plane)
The movement direction of A'B' is opposite to that of B'C', so two
compensation vectors V1 and V2 are produced at point B' (the end
point of N4). In such a case, there is a possibility of overcutting, so
an alarm PS0041 is issued at N4.
<1> Conditions for issuing the interference alarm
Suppose that a move command for a rotary axis makes the tool
vector change significantly from one block to another. In this
case, an interference alarm is assumed because compensation
vectors are regarded as being generated in wrong directions when
the path angle difference in the compensation plane is large, even
though the angle difference between the directions of
compensation vectors to be generated by those blocks is small.
Here, the compensation plane is perpendicular to the tool
direction (Va in the figure below) of the first of the two blocks.
Specifically, the conditions listed below are used for issuing the
alarm.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 910 -
Ua: Vector AB
Ub: Vector BC
Va: Tool vector between A and B
Vb: Tool vector between B and C
Wa: Va × Ua
Wb: Vb × Ub
(Here, × represents an outer product operator.)
Y
Z
Va
Vb
A
B
C
X
Wa
Wb
Ua
Ub
Fig. 22.5.1.1 (m) Conceptual diagram
A
’: Point A projected onto the compensation plane
B’: Point B projected onto the compensation plane
C’: Point C projected onto the compensation plane
Ra: Vector A’B’
Rb: Vector B’C’
e3
e2
A
’ C’ B’
Ra
Rb
Fig. 22.5.1.1 (n) Programmed path before and after the end point (point
B) of N4 (in the compensation plane)
When all the following conditions are satisfied, an alarm
PS0041) is issued:
(1) The tool vector changes significantly.
α: Angle for determination set in parameter No. 19635
(The default is 45°.)
(Va,Vb) ≤ cos(α)(where, (Va,Vb) means an inner product.)
(2) The difference between the directions of the compensation
vectors to be generated is small.
Wa: Direction of a compensation vector to be generated by
block AB
Wb: Direction of a compensation vector to be generated by
block BC
Wa = Va × Ua
Wb = Vb × Ub
(Wa,Wb) ≥ 0
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 911 -
(3) The path angle difference in the compensation plane is
large.
(Ra,Rb) < 0
<2> Suppressing the issue of the alarm with a Q command
By inserting a Q command into a block that resulted in the alarm,
the issue of the alarm can be suppressed.
(1) Q1 command
By inserting a Q1 command, a perpendicular vector is
generated.
Example: N4 Y-200 Z-200 Q1
A
t B', a vector (V) perpendicular to A'B' is generated.
e3
e2
A
’
C’ B’
V
Fig. 22.5.1.1 (o) Q1 command
A perpendicular vector can also be generated by specifying
G41.2 or G42.1 in the next block as follows:
Example: N6 G41.2 Y-400 Z0
(2) Q2 command
With a program specifying a linear-to-linear connection, up
to two compensation vectors are generated. In this case,
the second vector is deleted by inserting a Q2 command.
The Q2 command has no effect on circular interpolation.
Example: N4 Y-200 Z-200 Q2
The second vector (V2) is deleted, and only V1 is used as a compensation vector.
e3 e2
A
’
C’
B’
V1
Fig. 22.5.1.1 (p) Q2 command
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 912 -
(3) Q3 command
By inserting a Q3 command, the issue of the alarm can be
suppressed.
Example: N4 Y-200 Z-200 Q3
The two vectors (V1 and V2) are not deleted.
e3
e2
A
’ C’ B’
V1
V2
Fig. 22.5.1.1 (q) Q3 command
- Others
When the tool movement changes linear to circular (helical), circular
(helical) to linear, or circular (helical) to circular (helical), the start,
end, and center points of a circular (helical) movement are projected
on the compensation plane that is perpendicular to the tool axis, and a
compensation vector is calculated in the plane. The obtained vector
is added to the originally specified position to create a position to be
specified. Then, the tool is moved linearly or circularly (helically) to
the created position.
Z
X
Y
Too l
Tool axis
Start point End point
Too l
Tool center path created in the compensation plane
(Compensation plane = XY plane)
Compensation vector
created in the
compensation plane
A
ctual
compensation
vector
Move command
Pro
j
ected
Fig. 22.5.1.1 (r) Operation during compensation
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 913 -
- Angle of the rotary axis for type 2 (when the movement range is not specified)
When the direction of the tool is specified by I, J, K, Q for type 2,
more than two pairs of "computed angles" of the rotary axes usually
exist.
The "computed angle" is the candidate angle at which the rotary axis
is to be controlled in the specified tool axis direction.
The "output angle" is determined from the "computed angle" based on
the "output judgment conditions" described below.
The following descriptions assume that there is no movement range
specification (parameter No.19741 - No.19744 = 0).
Tool rotation type or table rotation type machine
<1> The "output angles" are represented by the computed rotary axis
angle pair whose master axis (first rotary axis) moving angle is
smaller.
↓
↓ When the master axis moving angle is the same
↓
<2> The "output angles" are represented by the computed rotary axis
angle pair whose slave axis (second rotary axis) moving angle is
smaller.
↓
↓ When the slave axis moving angle is the same
↓
<3> The "output angles" are represented by the computed rotary axis
angle pair whose master axis (first rotary axis) angle is nearer to 0
degree (multiple of 360 degrees).
↓
↓ When the master axis angle is equally near to 0 degree
↓
<4> The "output angles" are represented by the computed rotary axis
angle pair whose slave axis (second rotary axis) angle is nearer to 0
degree (multiple of 360 degrees).
Composite type machine
<1> The "output angles" are represented by the computed rotary axis
angle pair whose table (second rotary axis) moving angle is smaller.
↓
↓ When the table moving angle is the same
↓
<2> The "output angles" are represented by the computed rotary axis
angle pair whose tool (first rotary axis) moving angle is smaller.
↓
↓ When the tool moving angle is the same
↓
<3> The "output angles" are represented by the computed rotary axis
angle pair whose table (second rotary axis) angle is nearer to 0
degree (multiple of 360 degrees).
↓
↓ When the table angle is equally near to 0 degree
↓
<4> The "output angles" are represented by the computed rotary axis
angle pair whose tool (first rotary axis) angle is nearer to 0 degree
(multiple of 360 degrees).
Fig. 22.5.1.1 (s) Output judgment conditions
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 914 -
The process of judging whether the moving angle is smaller or larger
as the output judgement condition is called "movement judgement."
When bit 5 (PRI) of parameter No.19608 is 1, the movement
judgements for the first rotary axis and second rotary axis are made in
reverse order.
The "movement judgement" process is explained below.
When the "computed angle" is within the range between 0 and 360
degrees, it is called the "basic computed angle."
Usually, two pairs of "basic computed angles" exist.
For example, assume that a tool rotation type or table rotation type
machine has rotary axis A (master) and rotary axis B (slave) and that
there are two pairs of basic computed angles as follows:
(A θ1 degree; B φ1 degree)
(A θ2 degrees; B φ2 degrees) where θ1 ≤ θ2.
The "computed angle" is obtained from either of the following
expressions: "basic computed angle" + 360 degrees × N or "basic
computed angle" - 360 degrees × N.
The current position of rotary axis A (master) is PA, and that of rotary
axis B (slave) is 0 degree.
Based on the PA angle, the "movement judgement" process is done as
follows (when bit 5 (PRI) of parameter No.19608 is 0).
• Computed angle A
-360
×
(N + 1) degrees
θ
1 - 360
×
N
-360 × N degrees
θ
2 - 360
×
N
θ
2 - 360
×
(N + 1) θ1 - 360 × (N - 1)
(*1)
0 degree 360 degrees
θ
2 - 360
θ
1
θ
2θ1 + 360
(*2)
360 × (N + 1) degrees
θ
1 + 360
×
N
360
×
N degrees
θ
2 + 360 × N
θ
2 + 360
×
(N - 1) θ1 + 360 × (N + 1)
(*3)
Fig. 22.5.1.1 (t) Movement judgment
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 915 -
When the PA angle is (*1):
The output angle is: (A θ2 - 360 × (N + 1) degrees; B φ2 degrees).
Namely, θ2 - 360 × (N + 1) degrees is adopted that is nearer to the
computed angle of A, and φ2, which is the same group as θ2, is
adopted as the computed angle of B.
When the PA angle is (*2):
The output angle is: (A θ1 degrees; B φ1 degrees).
Namely, θ1 degrees is adopted that is nearer to the computed angle of
A, and φ1, which is the same group as θ1, is adopted as the computed
angle of B.
When the PA angle is (*3):
The output angle is: (A θ2 + 360 × N degrees; B φ2 degrees).
Namely, θ2 + 360 × N degrees is adopted that is nearer to the
computed angle of A, and φ2, which is the same group as θ2, is
adopted as the computed angle of B.
When the moving angle of rotary axis A (master) is the same, a
"movement judgement" is made for rotary axis B (slave) according to
the "output judgment conditions."
If the "output angle" of rotary axis A is determined by the "movement
judgement" for rotary axis A, the computed angle representing the
"smaller moving angle" is adopted as the "output angle" of rotary axis
B.
Similarly, if the "output angle" of rotary axis B is determined by the
"movement judgement" for rotary axis B, the computed angle
representing the "smaller moving angle" is adopted as the "output
angle" of rotary axis A.
The "output angle" is explained below using a tool rotation type
machine as an example.
This example illustrates a machine having a "BC type tool axis Z."
• BC type tool axis Z
X
Y
Z
C-axis: First rotation axis
(master)
B-axis: Second rotation axis
(slave)
Fig. 22.5.1.1 (u) BC type tool axis Z
The following two pairs of "computed basic angles" exist that direct
the tool axis toward the +X-axis direction.
(B 90 degrees; C 180 degrees)
(B 270 degrees; C 0 degree)
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 916 -
<1> When the current rotary axis angles are (B -70 degrees; C 30
degrees)
The "output angles" are (B -90 degrees; C 0 degree).
0 degree is adopted because it is nearer to the current
position (30 degrees) of the C-axis that is the master axis.
For the B-axis, 270 degrees is adopted which is the same
group. However, this is changed to -90 degrees (270
degrees - 360 degrees) which is the nearest to the current
position of the B-axis (-70 degrees).
<2> When the current rotary axis angles are (B 80 degrees; C 500
degrees)
The "output angles" are (B 90 degrees; C 540 degrees).
540 degrees (180 degrees + 360 degrees) is adopted because
it is nearer to the current position (500 degrees) of the C-axis
that is the master axis. For the B-axis, 90 degrees is
adopted which is the same group.
<3> When the current rotary axis angles are (B 60 degrees; C 90
degrees)
The "output angles" are (B 90 degrees; C 180 degrees).
Since the two candidates are equally near to the current
position (90 degrees) of the C-axis that is the master axis, a
judgment is made based on the current position of the B-axis.
90 degrees is adopted because it is nearer to the current
position (60 degrees) of the B-axis that is the slave axis.
For the C-axis, 180 degrees is adopted which is the same
group.
<4> When the current rotary axis angles are (B 180 degrees; C 90
degrees)
The "output angles" are (B 270 degrees; C 0 degree).
Since the two candidates are equally near to the current
position (90 degrees) of the C-axis that is the master axis, a
judgment is made based on the current position of the B-axis.
In this case, however, the two candidates are also equally
near to the current position of the B-axis (180 degrees).
Therefore, the candidate is adopted in which the C-axis
(master axis) is nearer to 0 degree.
That is, the pair is adopted whose C-axis angle is 0 degree
and whose B-axis angle is 270 degrees.
When the slave axis angle is 0 degree, the direction of the
tool axis becomes fixed regardless of the master axis angle.
In that case, the master axis does not move from the current angle.
An explanation is shown below using a machine having a "BC type
tool axis Z" as an example.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 917 -
• BC type tool axis Z
X
Y
Z
C
Fig. 22.5.1.1 (v) BC type tool axis Z
When the current rotary axis angles are (B 45 degrees; C 90 degrees),
the "output angles" are (B 0 degree; C 90 degrees).
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 918 -
- Angle of the rotary axis for type 2 (when the movement range is specified)
If the upper and lower limits of the movement range of the rotary axis
is specified using parameters No.19741 to No.19744, the rotary axis
will move only within the specified range when the direction is
specified using I, J, K, Q command for type 2 control.
Although the procedure for determining the angles is the same as that
used "when the movement range is not specified," the "output angles"
need to be selected from those computed angles that are within the
specified movement range for both axes.
Tool rotation type or table rotation type machine
<1> Of the angle pairs whose master and slave axis angles are both within
the specified movement range, the rotary axis angle pair whose
master axis (first rotary axis) moving angle is smaller represents the
"output angles."
↓
↓ When the master axis moving angle is the same
↓
<2> The "output angles" are represented by the computed rotary axis
angle pair whose slave axis (second rotary axis) moving angle is
smaller.
↓
↓ When the slave axis moving angle is the same
↓
<3> The "output angles" are represented by the computed rotary axis
angle pair whose master axis (first rotary axis) angle is nearer to 0
degree (multiple of 360 degrees).
↓
↓ When the master axis angle is equally near to 0 degree
↓
<4> The "output angles" are represented by the computed rotary axis
angle pair whose slave axis (second rotary axis) angle is nearer to 0
degree (multiple of 360 degrees).
Composite type machine
<1> Of the angle pairs whose master and slave axis angles are both within
the specified movement range, the rotary axis angle pair whose table
(second rotary axis) moving angle is smaller represents the "output
angles."
↓
↓ When the table moving angle is the same
↓
<2> The "output angles" are represented by the computed rotary axis
angle pair whose tool (first rotary axis) moving angle is smaller.
↓
↓ When the tool moving angle is the same
↓
<3> The "output angles" are represented by the computed rotary axis
angle pair whose table (second rotary axis) angle is nearer to 0
degree (multiple of 360 degrees).
↓
↓ When the table angle is equally near to 0 degree
↓
<4> The "output angles" are represented by the computed rotary axis
angle pair whose tool (first rotary axis) angle is nearer to 0 degree
(multiple of 360 degrees).
Fig. 22.5.1.1 (w) Output judgment conditions
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 919 -
When bit 5 (PRI) of parameter No.19608 is 1, the movement
judgements for the first rotary axis and second rotary axis are made in
reverse order.
CAUTION
1 If the lower limit of the movement range is larger
than the upper limit, alarm PS5459 occurs when
G43.5 is specified.
2 If no "computed angle" is found within the
movement range because the range is too small,
alarm PS5459 occurs.
3 If 0 is set for both parameters that specify the
upper and lower limits of the movement range, the
tool operates assuming that there is no range
specification.
4 When the rotary axis rollover function or rotary axis
control function is used (in which case, set
parameter No.1260 (amount of movement per
rotation of the rotary axis) to 360 degrees), the tool
does not move beyond 0 degree (360 degrees)
(does not take the shortcut) if the movement range
is set between 0 and 360 degrees. Also, do not
specify a negative value or a value larger than 360
degrees for the movement range.
An example of the "movement judgement" process is given below.
Assume that a tool rotation type or table rotation type machine has
rotary axis A (master) and rotary axis B (slave) and that there are two
pairs of basic computed angles as follows:
(A θ1 degree; B φ1 degree)
(A θ2 degrees; B φ2 degrees) where θ1 ≤ θ2.
The "computed angle" is obtained from either of the following
expressions: "basic computed angle" + 360 degrees × N or "basic
computed angle" - 360 degrees × N.
Assume that the current positions and movement ranges of rotary axis
A (master) and rotary axis B (slave) are as shown in Fig. 22.5.1.1 (x),
Fig. 22.5.1.1 (y).
360 × (N + 1) degrees
360
×
N degrees
• Computed angle A
Current position A
Movement range A
θ1 + 360 × N θ2 + 360 × N
θ2 + 360 × (N - 1) θ1 + 360 × (N + 1)
Fig. 22.5.1.1 (x) Computed angle of rotary axis A and its current
position and movement range
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 920 -
360 × (N + 1) degrees
360 × N degrees
• Computed angle B
Current position B
Movement range B
φ2 + 360 × N
φ
1 + 360
×
N
φ1 + 360 × (N - 1) φ2 + 360 × (N + 1)
Fig. 22.5.1.1 (y) Computed angle of rotary axis B and its current
position and movement range
When the two axes have a positional relationship as shown in the
figure, the output angle of rotary axis A is (θ2 + 360 × N) degrees and
that of rotary axis B is (φ2 + 360 × N) degrees (when bit 5 (PRI) of
parameter No.19608 is set to 0).
More concretely, from the computed angles obtained for rotary axis A,
the nearest angle within the movement range, i.e. θ2 + 360 × N
degrees, is first adopted. Then, from the computed angles obtained
for rotary axis B, the angle belonging to the same group as θ2, i.e. φ2
+ 360 × N, is adopted.
Note that, in this example, the output angles and moving direction
differ depending on whether the movement range is specified or not (0
to 360 degrees), even if N is set to 0 and coordinates are rounded to 0
to 360 degrees.
Namely, if the movement range is not specified, θ1 + 360 degrees
nearest to the current position is adopted as the computed angle for
rotary axis A and, from the computed angles belonging to the same
group as θ1, φ1 degrees nearest to the current position is adopted as
the computed angle for rotary axis B. Rotary axis A moves in the
plus direction. As its coordinate is rounded to 360 degrees, rotary
axis A reaches θ1 degrees while moving in the plus direction.
By contrast, when the movement range is set to 0 to 360 degrees, the
output angles are (A θ2 degrees; B φ2 degrees). Neither rotary axis
A nor B moves in a way that it exceeds 0 degree (360 degrees).
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 921 -
22.5.1.2 Leading edge offset
Overview
Leading edge offset is a type of cutter compensation used when a
workpiece is machined with the edge of a tool. The tool is
automatically shifted by the amount of cutter compensation on the line
where a plane formed by a tool vector and tool movement direction
meets a plane perpendicular to the tool axis direction.
Tool used
Reference
tool
Cutter
compensation
vector
Cutter compensation
amount
Tool center path
(path after
compensation)
Programmed
path
Too l vec tor
Fig. 22.5.1.2 (a) Leading edge offset
Format
- Leading edge offset
G41.3 D_ ;
- Canceling the leading edge offset
G40 ;
NOTE
1 G41.3 can be specified only in the G00 and G01
modes. In a block containing G41.3 or G40, only
addresses D, O, and N can be specified.
2 The block that follows a block containing a G41.3
command must contain a move command.
In the block after G41.3, however, a tool movement
in the same direction as the tool axis direction or
the opposite direction cannot be specified.
3 No modal G code that belongs to the same group
as G00 and G01 can be specified in the G41.3
mode. If such a modal G code is specified, alarm
PS5460 is issued.
4 Leading edge offset does not provide type 2
commands. It does not allow the tool direction to
be specified with the I, J, and K commands.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 922 -
Explanation
- Operation at startup and cancellation
The operation performed at leading edge offset startup and
cancellation does not vary. When G41.3 is specified, the tool is
moved by the amount of compensation (Vc) in the plane formed by
the movement vector (VM) of the block after the G41.3 block and the
tool vector (VT) obtained at the time of G41.3 specification. The tool
movement is perpendicular to the tool vector. When G40 is specified,
the tool is moved to cancel VC. The following illustrates how the
compensation is performed:
<1> When the tool vector is inclined in the tool movement direction
Tool
Tool compensation vector (VT)
VM
G41.3(VC) G40
: Tool center path
: Programmed path
Fig. 22.5.1.2 (b) When the tool vector is inclined in the tool movement
direction
<2> When the tool vector is inclined in the direction opposite to the
tool movement direction
: Tool center path
: Programmed path
Tool
Tool compensation vector (VT)
VM
G41.3(VC) G40
Fig. 22.5.1.2 (c) When the tool vector is inclined in the direction
opposite to the tool movement direction
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 923 -
- Operation during compensation
The tool center moves so that a compensation vector (VC)
perpendicular to the tool vector (VT) is created in the plane formed by
the tool vector (VT) at the end point of each block and the movement
vector (VM) of the next block.
VMn:Movement vector of block n
VTn: Tool vector at the end of block n
VCn: Compensation vector of block n (that lies in the plane formed by VTn and VMn+1
and is perpendicular to VTn)
Tool center path (path after compensation)
Programmed path VM1 VM2
VT1
VC1 VC2
VT2
VM3
Fig. 22.5.1.2 (d) Operation during compensation
If a G code or M code that suppresses buffering is specified in the
compensation mode, however, the compensation vector created
immediately before the specification is maintained.
When a block specifying no movement (including a block containing
a move command for a rotary axis only) is specified in the
compensation mode, the movement vector of the block after the block
specifying no movement is used to create a compensation vector as
shown below.
Tool center path (path after compensation)
Programmed path VM1 VM2
VT1
VC1
VC2 = VC3
VT2
VM4
There is one block that
specifies no movement
Fig. 22.5.1.2 (e) When there is one block that specifies no movement
If block 3 specifies no movement, the compensation vector of block 2
(VC2) is created in a plane formed by the movement vector of block 4
(VM4) and the tool vector (VT2) at the end of block 2. VC2 is
perpendicular to VT2.
CAUTION
If two or more successive blocks specify no
movement, the previously created compensation
vector is maintained. However, such specification
should be avoided.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 924 -
- Block immediately before the offset cancel command (G40)
In the block immediately before the offset cancel command (G40), a
compensation vector is created from the movement vector of that
block and the tool vector at the end point of the block as shown below.
Tool center path (path after compensation)
Programmed path VM1 VM2
VT1
VC1 VC2
VT2
G40
Fig. 22.5.1.2 (f) Block immediately before G40
The compensation vector (VC2) of block 2 is created in a plane
formed by the tool vector (VT2) at the end point of block 2 and the
movement vector (VM2) of block 2. VC2 is perpendicular to VT2.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 925 -
- Compensation performed when θ is approximately 0°, 90°, or 180°
When the included angle θ between VMn+1 and VTn is regarded as
0°, 180°, or 90°, the compensation vector is created in a different way.
So, when creating a program, note the following points:
<1> Setting a variation range for determining θ to be 0°, 180°, or 90°
When the included angle (θ) between the tool vector (VTn) and
movement vector (VMn+1) becomes approximately 0°, 180°, or
90°, the system regards θ as 0°, 180°, or 90°, respectively, then
creates a compensation vector which is different from the normal
compensation vector. The variation range used for determining
θ to be 0°, 180°, and 90° is set in parameter No. 19631. For
example, let the angle set in this parameter be ∆θ. Then, the
system regards θ as follows:
(1) If 0 ≤ θ ≤ ∆θ , θ is regarded as 0°.
θ
∆
θ
V
Tn
V
Mn+1
Fig. 22.5.1.2 (g) Determination of θ = 0°
(2) If (180 - ∆θ) ≤ θ ≤ 180, θ is regarded as 180°.
θ
∆
θ
V
Tn
V
Mn+1
Fig. 22.5.1.2 (h) Determination of θ = 180°
(3) If (90 − ∆θ) ≤ θ ≤ (90 + ∆θ), θ is regarded as 90°.
θ
∆
θ
V
Tn
V
Mn+1
θ
∆
θ
V
Tn
V
Mn+1
Fig. 22.5.1.2 (i) Determination of θ = 90°
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 926 -
<2> Compensation vector when θ is regarded as 0° or 180°
At startup (when G41.3 is specified), alarm PS5408 is issued.
This means that the tool vector of a block and the movement
vector of the next block must not point in the same direction or in
opposite directions at startup.
At other than startup, the previously created compensation vector
is maintained without change.
If the included angles between VT2 and VM3, VT3 and VM4,
and VT4 and VM5 are regarded as 0°, compensation vector VC1
of block 1 is maintained as compensation vectors VC2, VC3, and
VC4 of blocks 2, 3, and 4, respectively.
Tool center path
(p
ath after com
p
ensation
)
Programmed
path
VMVM
VT1
VCVCVT2
VM
3
VT3
VM
VCVC
VM
VM
VT4
VC
VT5
Fig. 22.5.1.2 (j) When θ = 0° is determined
If the included angles between VT2 and VM3, VT3 and VM4,
and VT4 and VM5 are regarded as 180°, compensation vector
VC1 of block 1 is maintained as compensation vectors VC2,
VC3, and VC4 of blocks 2, 3, and 4, respectively.
Tool center path
(
path after compensation
)
Programmed
path VM
VM
VT1 VCVC
VT2
VM
VT3 VM
VCVC
VM
VM
VT4 VC
VT5
Fig. 22.5.1.2 (k) When θ = 180° is determined
<3> Compensation vector when θ is regarded as 90°
If the previous compensation vector (VCn-1) points in the
opposite direction ((VMn × VTn-1) × VTn-1 direction) to VMn
with respect to VTn-1, the current compensation vector (VCn) is
created so that it also points in the (VMn+1 × VTn) × VTn
direction.
Tool center path
(p
ath after com
p
ensation
)
Programmed
path
VM
VM
VT1
VCVC
VT2
VM
VT3
VM
VCVC
VM
VM
6
VT4
VC
VT5
Fig. 22.5.1.2 (l) When θ = 90° is determined 1
If the previous compensation vector (VCn-1) points in the same
direction (-(VMn × VTn-1) × VTn-1 direction) as VMn with
respect to VTn-1, the current compensation vector (VCn) is
created so that it also points in the -(VMn+1 × VTn) × VTn
direction.
Tool center path
(p
ath after com
p
ensation
)
Programmed
path
VM
VM
VT1 VCVC
VT2
VM
VT3
VM
VCVC
VM
VM
VT4
VC
VT5
Fig. 22.5.1.2 (m) When θ = 90° is determined 2
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 927 -
22.5.1.3 Tool tip position (cutting point) command
Overview
For machines having a rotary axis for rotating a tool, this function
performs 3-dimensional cutter compensation at the tool tip position if
a programmed point is specified with a pivot point.
When this function is used, the programmed point (pivot point) is
converted into a tool tip position (cutting point) and a vector of
3-dimensional cutter compensation is calculated for the position
obtained by the conversion. Then, the programmed point (pivot
point) is compensated for with the vector of 3-dimensional cutter
compensation.
If the tool side offset (G41.2/G42.2) of 3-dimensional cutter
compensation is performed, the operation of this function is as
follows:
(1) If parameter No. 19632 is 0
The vector of 3-dimensional cutter compensation is calculated at
the programmed point (pivot point).
(2) If parameter No. 19632 is not 0 (this function)
The vector of 3-dimensional cutter compensation is calculated at
the tool tip position (cutting point).
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 928 -
Explanation
- Operation explanation
This function calculates a vector at the tool tip position for the
3-dimensional cutter compensation function as described below.
(1) Convert the programmed coordinates from a programmed point
(pivot point) to a tool tip position (cutting point). Parameter No.
19632 is used to store the distance from the programmed point
(pivot point) to the tool tip position (cutting point).
(2) Calculate a vector of 3-dimensional cutter compensation at the
tool tip position (cutting point).
(3) Add the cutter compensation vector to the programmed point
(pivot point).
Programmed point (pivot point)
Workpiece
Tool center
Tool side
Distance from programmed poin
t
(pivot point) to cutting poin
t
(parameter setting)
Vector from programmed point (pivo
t
point) to cutting point
Cutting point
Vector of three-dimensional cutter compensation conforming to this specification
Too l
Vector of conventional three-dimensional
cutter compensation conforming
Vector of
three-dimensional cutter
compensation conforming
to this specification
Fig. 22.5.1.3 (a) Basic operation (for G42.2)
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 929 -
- Operation example
For a machine configuration in which the tool axis direction is along
the Z-axis and the rotary axes are the B and C axes (Fig. 22.5.1.3 (b))
LC: Parameter (No. 19632) specifying the distance from the
programmed point (pivot point) to the tool tip position (cutting
point)
b: Specified B-axis value, c: Specified C-axis value
Q = (Qx,Qy,Qz): Programmed point (pivot point)
P, R: Programmed points (pivot points) in the preceding and
succeeding blocks
QT = (QTx,QTy,QTz): Tool position (tool tip position (cutting point))
resulting from conversion
PT, RT: Tool positions (tool tip positions (cutting positions)) in the
preceding and succeeding blocks
Then,
<1> Convert programmed points (pivot points) P, Q, and R to tool tip
positions (cutting points) PT, QT, and RT.
QTx = LC × sin(b) × cos(c) + Qx
QTy = LC × sin(b) × sin(c) + Qy
QTz LC × cos(b) + Qz
(The same applies to PT and RT.)
<2> Calculate vector VD of 3-dimensional cutter compensation from
tool tip positions (cutting points) PT, QT, and RT and tool
gradient VT.
<3> Add cutter vector VD to programmed point (pivot point) Q and
set the result as the end point position.
Cutter compensation vector (VD') is calculated on a compensation plane perpendicular to
the tool axis direction.
The cutter compensation vector (VD') on the compensation plane is converted to the
original Cartesian coordinate system, and the resulting vector is regarded as the cutte
r
compensation vector (VD).
P’
R’
Q’
VD VD’
e2 e3
e3
e2
V
T
Coordinate system of compensation plane
Tool tip position
LC
Tool radius
e1
Fig. 22.5.1.3 (b) Operation
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 930 -
NOTE
1 This function is disabled for leading edge offset.
2 With a command for a rotary axis only, this function
does not calculate a cutter compensation vector.
3 This function cannot be used in the
three-dimensional coordinate system conversion
mode.
4 In addition to the cautions given here, the cautions
on the 3-dimensional cutter compensation function
apply to this function.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 931 -
22.5.2 Cutter Compensation in Table Rotation Type Machine
Overview
Cutter compensation can be performed for a 5-axis machine having a
rotary table as shown in Fig. 22.5.2 (a).
Shown below is a 5-axis machine that has table rotation axis A on the
X-axis and table rotation axis B on the Y-axis.
This machine configuration is used as a sample configuration in the
following explanation unless otherwise noted:
B
A
Z
X
Y
X
Y
Z
Machine coordinate system
Indicates the direction of machine operation.
This machine configuration is used as a sample
configuration in the explanation.
The table coordinate system is rotated according to the
table rotation. It is possible to specify whether to create
a part program in the workpiece coordinate system or in
the table coordinate system, using an appropriate
parameter.
Table coordinate
system Workpiece
coordinate system
Fig. 22.5.2 (a) Machine having a rotary table
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 932 -
Format
- Startup (start of cutter compensation) (type 1)
When bit 1 (SPG) of parameter No. 19607 is 0
G41.2 (or G42.2) IP_ D_ ;
G41.2: Cutter compensation left (group 07)
G42.2: Cutter compensation right (group 07)
IP_: Value specified for axis moving as viewed from the
programming coordinate system (including rotary
axis)
D_: Code specifying the cutter compensation amount (1
to 3 digits)
When bit 1 (SPG) of parameter No. 19607 is 1
G41.4 (or G42.4) IP_ D_ ;
G41.4: Cutter compensation left (group 07)
G42.4: Cutter compensation right (group 07)
IP_: Value specified for axis moving as viewed from the
programming coordinate system (including rotary
axis)
D_: Code specifying the cutter compensation amount (1
to 3 digits)
NOTE
1 In a table rotation type machine (parameter No.
19680 = 12), if an attempt is made to issue G41.4
or G42.4 with bit 1 (SPG) of parameter No. 19607
equal to 0, alarm PS0010 is generated.
2 In a table rotation type machine, if an attempt is
made to issue G41.2 or G42.2 with bit 1 (SPG) of
parameter No. 19607 equal to 1, alarm PS5460 is
generated.
3 In machine not of the table rotation type machine, if
an attempt is made to issue G41.4 or G42.4 with bit
1 (SPG) of parameter No. 19607 equal to 1, alarm
PS5460 is generated.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 933 -
- Startup (start of cutter compensation) (type 2)
G41.6(or G42.6) IP_ D_ Q_ ;
IP_ I_ J_ K_ ;
:
G41.6: Cutter compensation left (group 07)
G42.6: Cutter compensation right (group 07)
IP_: Value specified for axis moving as viewed from the
programming coordinate system (including rotary
axis)
D_: Code specifying the cutter compensation amount (1
to 3 digits)
Q_: Tool’s angle of gradient (in degrees)
I_ J_ K_: Tool axis direction at the block end point as
viewed from the programming coordinate system
For type 2, do not specify a rotation axis but specify the direction at
the tool end point as viewed from the programming coordinate system
(table coordinate system), with I, J, and K. Specifying a rotation axis
causes alarm PS5460 to be generated.
In a tool rotation type machine, I, J, and K can be specified in a
G41.6/G42.6 command block; in a table rotation type machine,
however, they cannot. If an attempt is made to specify them, alarm
PS5460 is generated.
The following are the notes on type 2.
NOTE
1 If one or two of I, J, and K are omitted, the omitted
ones of I, J, and K are assumed to be 0.
2 In a block in which all of I, J, and K are omitted,
the values of I, J, and K in the previous block are
used.
3 If there is only one rotation axis (a hypothetical
axis is used), type 2 cannot be used. In this
case, if an attempt is made to issue G41.6/G42.6,
alarm PS5460 is generated.
4 If using the rotation axis rollover function or rotary
axis control function, specify 360 degrees in
parameter No. 1260 (mount of travel per rotation
about the rotation axis).
5 They can be used only with the settings that
select the table coordinate system as a
programming coordinate system (bit 5 (WKP) of
parameter No.19696 = 0 and bit 4 (TBP) of
parameter No.19746 = 1). If an attempt is made
to issue G41.6/G42.6 with the settings that select
the workpiece coordinate system as a
programming coordinate system, alarm PS5460 is
generated.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 934 -
- Canceling the cutter compensation
G40 IP_ ;
G40: Cutter compensation cancellation (group 07)
IP_: Value specified for axis movement
- Selecting an offset plane
When bit 1 (PTD) of parameter No. 19746 is 1, compensation is
performed on the selected plane, on the assumption that the tool is
pointing to the direction perpendicular to that plane.
Offset plane Plane selection command IP_
XpYp G17 ; Xp_Yp_
ZpXp G18 ; Xp_Zp_
YpZp G19 ; Yp_Zp_
(Example: In the case of Fig. 22.5.2 (a), the XpYp plane is selected.)
The two axes of a selected plane must be included in the three basic
axes (the axes for which parameter No. 1022 is set to 1 to 3).
When bit 1 (PTD) of parameter No. 19746 is 0, compensation is
performed on the plane perpendicular to the tool direction specified
with parameters Nos. 19697, 19698, and 19699, regardless of which
plane is selected.
NOTE
This function is enabled for tool side offset only. If
leading edge offset is specified, alarm PS5460 is
generated.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 935 -
Explanation
- Tool's angle of gradient in type 2
For type 2 of 3-dimensional cutter compensation, the tool's angle of
gradient can be specified with address Q in a G41.6/G42.6 command
block. The tool's angle of gradient refers to the angle by which the
tool direction to be assumed when machining is actually performed is
inclined from the direction specified with (I, J, K) toward the traveling
direction on the plane formed by the tool direction specified with (I, J,
K) and the traveling direction in the programming coordinate system.
(See Fig. 22.5.2 (b).)
Because in general, the normal direction of the machining surface is
specified with (I, J, K), if it is desired to incline the tool direction to be
assumed when machining is actually performed from the normal
direction toward the traveling direction, correction may be performed
with a Q command.
If the direction specified with (I, J, K) matches the tool direction to be
assumed when machining is actually performed, no Q command is
necessary.
Tool direction to be assumed when
machining is actually performed
(Plane perpendicular to the "tool direction to be
assumed when machining is actually performed")
Tool direction
specified with (I, J, K)
Traveling
direction of
machinin
g
Tool's angle of gradient (Q)
Compensation plane
Tool center path
(path after compensation)
Programmed path
(path before compensation)
Cutter
compensation
vector
Fig. 22.5.2 (b) Tool's angle of gradient in type 2
- Cutter compensation
The function for 3-dimensional cutter compensation in a table rotation
type machine basically performs operations in conformance with
3-dimensional cutter compensation in a tool rotation type machine.
The operations different from those of 3-dimensional cutter
compensation in a tool rotation type machine are mainly described
below.
For the specifications and cautions not mentioned here, see the
description of 3-dimensional cutter compensation in a tool rotation
type machine.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 936 -
- Startup
When cutter compensation for the rotary table is specified (G41.2 or
G42.2, G41.4 or G42.4, a dimension word other than 0 in the offset
plane, or a D code other than D0) in the offset cancel mode, the CNC
enters the offset mode.
Startup is specified with positioning (G00) or linear interpolation
(G01).
NOTE
If a command such as circular interpolation (G02 or
G03) and involute interpolation (G02.2 or G03.2) is
specified at startup, alarm PS0034 is issued.
- Commands in the offset mode
In the offset mode, compensation is performed for positioning (G00)
and linear interpolation (G01).
NOTE
If a command such as circular interpolation (G02 or
G03) and involute interpolation (G02.2 or G03.2) is
specified in the mode for 3-dimensional cutter
compensation in a table rotation type machine,
alarm PS5460 is issued.
- Offset mode cancellation
If a block satisfying either of the following conditions is executed in
the offset mode, the CNC enters the offset cancel mode:
1 G40 is specified.
2 0 is specified as a code specifying the cutter compensation
amount (D code).
When offset cancellation is to be performed, neither circular (G02 or
G03) nor involute (G02.2 or G03.2) command can be specified. If
offset cancellation is specified in such a mode, alarm PS0034 is
issued.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 937 -
- If selecting the table coordinate system as a programming coordinate system
If bit 4 (TBP) of parameter No. 19746 is 1 and bit 5 (WKP) of
parameter No. 19696 is 0, specifying 3-dimensional cutter
compensation causes the table coordinate system to be selected as a
programming coordinate system. The table coordinate system refers
to the workpiece coordinate system fixed to the table when
3-dimensional cutter compensation.
In the blocks subsequent to the one in which 3-dimensional cutter
compensation is specified, the table coordinate system rotates with the
rotation of the table.
A linear axis (X, Y, Z) command is assumed to be issued on the table
coordinate system.
Specifying linear interpolation causes cutter compensation to be
performed on the linear interpolation command on the table coordinate
system.
The table coordinate system does not rotate with the rotation of the
tool head.
The cancel (G40) block becomes a block that suppresses buffering.
It is possible to switch between absolute and relative coordinate
displays, using bit 2 (DET) of parameter No. 19608 as follows:
• When DET is 0, the position in the table coordinate system is
displayed.
• When DET is 1, the position in the workpiece coordinate system
is displayed.
Note, however, the distance to go is always that in the programming
coordinate system.
NOTE
1 If the 3-dimensional cutter compensation mode is entered
when the table coordinate system is used as the
programming coordinate system, look-ahead
acceleration/deceleration before interpolation is
automatically enabled. Be sure to specify the following
parameters:
(1) Bit 1 (LRP) of parameter No.1401 = 1:
Linear rapid traverse
(2) Bit 5 (FRP) of parameter No.19501 = 1:
Acceleration/deceleration before interpolation is used
for rapid traverse.
(3) Parameter No. 1671:
Acceleration of acceleration/deceleration before
interpolation for rapid traverse
(4) Parameter No. 1672:
Change time for bell-shaped acceleration/deceleration
before interpolation for rapid traverse
(5) Parameter No. 1660:
Maximum permissible acceleration for
acceleration/deceleration before interpolation
If they are not specified, alarm PS5463 is generated.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 938 -
NOTE
2 When table rotation axis movement is specified in the start
block of 3-dimensional cutter compensation, after the
movement is completed, the workpiece coordinate system
is fixed to the table and assumed to be a table coordinate
system.
3 In the mode of 3-dimensional cutter compensation, do not
change the workpiece coordinate system or change the
workpiece offset value. If an attempt is made to specify
workpiece coordinate system selection (G54 to G59), alarm
PS5460 is generated.
- If selecting the workpiece coordinate system as a programming coordinate
system
If bit 4 (TBP) of parameter No. 19746 is 0 or if bit 4 (TBP) of
parameter No. 19746 is 1 and bit 5 (WKP) of parameter No. 19696 is
1, the programming coordinate system does not rotate with the
rotation of the table, being fixed to the workpiece coordinate system.
- Angle of the rotation axis in type 2
For an explanation of how the rotation axis end point is determined
when the tool direction is specified with an IJKQ command in type 2,
see the explanations of cutter compensation in a tool rotation type
machine, "Angle of the rotation axis in type 2 (if the operating range
is not specified)" and "Angle of the rotation axis in type 2 (if the
operating range is specified)".
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 939 -
22.5.3 Cutter Compensation in Composite Type Machine
Overview
This function can perform 3-dimensional cutter compensation in a
5-axis machine having a rotary table and a tool axis as shown in Fig.
22.5.3 (a).
Shown below is a 5-axis machine that has tool axis A on the X-axis
(the tool axis direction is along the Z-axis) and table rotation axis B on
the Y-axis.
This machine configuration is used as a sample configuration in the
following explanation unless otherwise noted:
X
Y
Z
Machine
coordinate
system
C
Z
+-
X
+
-
Y
+
-
A
Workpiece
coordinate
system
Table
coordinate
s
y
stem
The table coordinate system is rotated according to the
table rotation. It is possible to specify whether to create
a part program in the workpiece coordinate system or in
the table coordinate system, using an appropriate
parameter.
Fig. 22.5.3 (a) Machine having a tool rotation axis and table rotation
axis
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 940 -
Format
- Startup (start of cutter compensation) (type 1)
When bit 1 (SPG) of parameter No. 19607 is 0
G41.2 (or G42.2) IP_ D_ ;
G41.2: Cutter compensation left (group 07)
G42.2: Cutter compensation right (group 07)
IP_: Value specified for axis moving as viewed from the
programming coordinate system (including rotary axis)
D_: Code specifying the cutter compensation amount (1 to 3 digits)
When bit 1 (SPG) of parameter No. 19607 is 1
G41.5 (or G42.5) IP_ D_ ;
G41.5: Cutter compensation left (group 07)
G42.5: Cutter compensation right (group 07)
IP_: Value specified for axis moving as viewed from the
programming coordinate system (including rotary axis)
D_: Code specifying the cutter compensation amount (1 to 3 digits)
NOTE
1 In a composite type machine (parameter No. 19680 = 21),
if an attempt is made to issue G41.5 or G42.5 with bit 1
(SPG) of parameter No. 19607 equal to 0, alarm PS0010 is
generated.
2 In a composite type machine, if an attempt is made to issue
G41.2 or G42.2 with bit 1 (SPG) of parameter No. 19607
equal to 1, alarm PS5460 is generated.
3 In machine not of the composite type machine, if an
attempt is made to issue G41.5 or G42.5 with bit 1 (SPG)
of parameter No. 19607 equal to 1, alarm PS5460 is
generated.
- Startup (start of cutter compensation) (type 2)
G41.6 (or G42.6) IP_ D_ Q_ ;
IP_ I_ J_ K_ ;
:
G41.6: Cutter compensation left (group 07)
G42.6: Cutter compensation right (group 07)
IP_: Value specified for axis moving as viewed from the
programming coordinate system (including rotary axis)
D_: Code specifying the cutter compensation amount (1 to 3 digits)
Q_: Tool’s angle of gradient (in degrees)
I_ J_ K_: Tool axis direction at the block end point as viewed from the
programming coordinate system
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 941 -
For type 2, do not specify a rotation axis but specify the direction at
the tool end point as viewed from the programming coordinate system
(table coordinate system), with I, J, and K. Specifying a rotation axis
causes alarm PS5460 to be generated.
In a tool rotation type machine, I, J, and K can be specified in a
G41.6/G42.6 command block; in a composite type machine, however,
they cannot. If an attempt is made to specify them, alarm PS5460 is
generated.
The following are the notes on type 2.
NOTE
1 If one or two of I, J, and K are omitted, the omitted
ones of I, J, and K are assumed to be 0.
2 In a block in which all of I, J, and K are omitted,
the values of I, J, and K in the previous block are
used.
3 If there is only one rotation axis (a hypothetical
axis is used), type 2 cannot be used. In this
case, if an attempt is made to issue G41.6/G42.6,
alarm PS5460 is generated.
4 If using the rotation axis rollover function or rotary
axis control function, specify 360 degrees in
parameter No. 1260 (mount of travel per rotation
about the rotation axis).
5 They can be used only with the settings that
select the table coordinate system as a
programming coordinate system (bit 5 (WKP) of
parameter No.19696 = 0 and bit 4 (TBP) of
parameter No.19746 = 1). If an attempt is made
to issue G41.6/G42.6 with the settings that select
the workpiece coordinate system as a
programming coordinate system, alarm PS5460 is
generated.
- Canceling the cutter compensation
G40 IP_ ;
G40: Cutter compensation cancellation (group 07)
IP_: Value specified for axis movement
NOTE
This function is enabled for tool side offset only. If
leading edge offset is specified, alarm PS5460 is
generated.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 942 -
Explanation
- Tool's angle of gradient in type 2
For type 2 of 3-dimensional cutter compensation, the tool's angle of
gradient can be specified with address Q in a G41.6/G42.6 command
block. The tool's angle of gradient refers to the angle by which the
tool direction to be assumed when machining is actually performed is
inclined from the direction specified with (I, J, K) toward the traveling
direction on the plane formed by the tool direction specified with (I, J,
K) and the traveling direction in the programming coordinate system.
(See Fig. 22.5.2 (b).)
Because in general, the normal direction of the machining surface is
specified with (I, J, K), if it is desired to incline the tool direction to be
assumed when machining is actually performed from the normal
direction toward the traveling direction, correction may be performed
with a Q command.
If the direction specified with (I, J, K) matches the tool direction to be
assumed when machining is actually performed, no Q command is
necessary.
Tool direction to be assumed when
machining is actually performed
(Plane perpendicular to the "tool direction to be
assumed when machining is actually performed")
Tool direction
specified with (I, J, K)
Traveling
direction of
machinin
g
Tool's angle of gradient (Q)
Compensation plane
Tool center path
(path after compensation)
Programmed path
(path before compensation)
Cutter
compensation
vector
Fig. 22.5.3 (b) Tool's angle of gradient in type 2
- Cutter compensation
The function for 3-dimensional cutter compensation in a composite
type machine basically performs operations in conformance with
3-dimensional cutter compensation in a tool rotation type machine.
The operations different from those of 3-dimensional cutter
compensation in a tool rotation type machine are mainly described
below.
For the specifications and cautions not mentioned here, see the
description of 3-dimensional cutter compensation in a tool rotation
type machine.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 943 -
- Startup
When 3-dimensional cutter compensation in a composite type
machine (G41.2 or G42.2, G41.5 or G42.5, or a D code other than D0)
is specified in the offset cancel mode, the CNC enters the offset mode.
Startup is specified with positioning (G00) or linear interpolation
(G01).
NOTE
If a command such as circular interpolation (G02 or
G03) and involute interpolation (G02.2 or G03.2) is
specified at startup, alarm PS0034 is issued.
- Commands in the offset mode
In the offset mode, compensation is performed for positioning (G00)
and linear interpolation (G01).
NOTE
If a command such as circular interpolation (G02 or
G03) and involute interpolation (G02.2 or G03.2) is
specified in the mode for 3-dimensional cutter
compensation in a composite type machine, alarm
PS5460 is issued.
- Offset mode cancellation
If a block satisfying either of the following conditions is executed in
the offset mode, the CNC enters the offset cancel mode:
1 G40 is specified.
2 0 is specified as a code specifying the cutter compensation
amount (D code).
When offset cancellation is to be performed, neither circular (G02 or
G03) nor involute (G02.2 or G03.2) command can be specified. If
offset cancellation is specified in such a mode, alarm PS0034 is
issued.
NOTE
1 This function cannot be used in the
three-dimensional coordinate system conversion
mode.
2 In addition to the cautions given here, the cautions
on the 3-dimensional cutter compensation function
apply to this function.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 944 -
- If selecting the table coordinate system as a programming coordinate system
If bit 4 (TBP) of parameter No.19746 is 1 and bit 5 (WKP) of
parameter No.19696 is 0, specifying 3-dimensional cutter
compensation causes the table coordinate system to be selected as a
programming coordinate system. The table coordinate system refers
to the workpiece coordinate system fixed to the table when
3-dimensional cutter compensation.
In the blocks subsequent to the one in which 3-dimensional cutter
compensation is specified, the table coordinate system rotates with the
rotation of the table.
A linear axis (X, Y, Z) command is assumed to be issued on the table
coordinate system.
Specifying linear interpolation causes cutter compensation to be
performed on the linear interpolation command on the table coordinate
system.
The table coordinate system does not rotate with the rotation of the
tool head.
The cancel (G40) block becomes a block that suppresses buffering.
It is possible to switch between absolute and relative coordinate
displays, using bit 2 (DET) of parameter No.19608 as follows:
- When DET is 0, the position in the table coordinate system is
displayed.
- When DET is 1, the position in the workpiece coordinate system
is displayed.
Note, however, the distance to go is always that in the programming
coordinate system.
NOTE
1 If the 3-dimensional cutter compensation mode is entered
when the table coordinate system is used as the
programming coordinate system, look-ahead
acceleration/deceleration before interpolation is
automatically enabled. Be sure to specify the following
parameters:
(1) Bit 1 (LRP) of parameter No.1401 = 1:
Linear rapid traverse
(2) Bit 5 (FRP) of parameter No.19501 = 1:
Acceleration/deceleration before interpolation is used for
rapid traverse.
(3) Parameter No. 1671:
Acceleration of acceleration/deceleration before
interpolation for rapid traverse
(4) Parameter No. 1672:
Change time for bell-shaped acceleration/deceleration
before interpolation for rapid traverse
(5) Parameter No. 1660:
Maximum permissible acceleration for
acceleration/deceleration before interpolation
If they are not specified, alarm PS5463 is generated.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 945 -
NOTE
2 When table rotation axis movement is specified in the start
block of 3-dimensional cutter compensation, after the
movement is completed, the workpiece coordinate system is
fixed to the table and assumed to be a table coordinate
system.
3 In the mode of 3-dimensional cutter compensation, do not
change the workpiece coordinate system or change the
workpiece offset value. If an attempt is made to specify
workpiece coordinate system selection (G54 to G59), alarm
PS5460 is generated.
- If selecting the workpiece coordinate system as a programming coordinate
system
If bit 4 (TBP) of parameter No.19746 is 0 or if bit 4 (TBP) of
parameter No.19746 is 1 and bit 5 (WKP) of parameter No.19696 is 1,
the programming coordinate system does not rotate with the rotation
of the table, being fixed to the workpiece coordinate system.
- Angle of the rotation axis in type 2
For an explanation of how the rotation axis end point is determined
when the tool direction is specified with an IJKQ command in type 2,
see the explanations of cutter compensation in a tool rotation type
machine, "Angle of the rotation axis in type 2 (if the operating range
is not specified)" and "Angle of the rotation axis in type 2 (if the
operating range is specified)".
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 946 -
22.5.4 Interference Check and Interference Avoidance
Overview
By setting bit 1 (NI5) of parameter No. 19608 to 1, this function
performs an interference check on the plane (compensation plane)
perpendicular to the tool axis direction regardless of the machine
configuration.
If bit 5 (CAV) of parameter No. 19607 is set to 1, a vector is generated
to avoid interference on the same plane.
Explanation
- For a tool rotation type machine
An interference check is performed, as well as interference avoidance,
with the tool path as projected from the workpiece coordinate system
(X-Y-Z) onto the compensation plane (X'-Y'-Z') and a compensation
vector.
Z
Y
X
Y’
X’
Z’
Fig. 22.5.4 (a) Tool rotation type
- For a table rotation type machine
An interference check is performed, as well as interference avoidance,
with the tool path as converted from the workpiece coordinate system
(X-Y-Z) into the table coordinate system (X'-Y'-Z') and a
compensation vector.
Z
X
Y
Z’
X’
Y’
Fig. 22.5.4 (b) Table rotation type
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 947 -
- For a composite type machine
An interference check is performed, as well as interference avoidance,
with the tool path as projected from the workpiece coordinate system
(X-Y-Z) onto the table coordinate system (X'-Y'-Z') and then onto the
compensation plane perpendicular to the tool axis direction
(X''-Y''-Z'') and a compensation vector.
Z
Y
X
Z’ Y’
X’
Z’’
Y’’
X’’
Fig. 22.5.4 (c) Composite type
- Interference avoidance
V10
N10
N20
N30
N40
N50
V20 V30
V40
Va
Y
X
Compensation plane
Machining program
N10 X8.010 Y77.91 Z93.345 B21.02 C22.001
N20 X10.221 YY60.932 Z91.265 B24.124 C65.203
N30 X41.579 Y58.223 Z91.736 B23.457 C53.887
N40 X94.631 Y13.767 Z93.769 B20.004 C5.478
N50 X187.513 Y-73.654 Z94.245 B19.534 C-46.336
Fig. 22.5.4 (d) Example of interference avoidance
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 948 -
Fig. 22.4.4(d) shows a tool path in the workpiece coordinate system as
projected onto the compensation plane. This is an example when the
parameter No.19626 is set to 4.
At the start of the execution of the N10 block, the system looks at N20
to N50 ahead and generates V20 to V40.
Then, because the movement direction of N30 greatly differs from the
direction from V20 to V30, V20 and V30 are considered interferences
and eliminated. Similarly, because the movement direction from
N30 to N40 greatly differs from the movement direction from V20 to
V40, V40 is also considered an interference and eliminated.
Then, the interference avoidance vector Va is generated between N20
and N50 and uses it instead of V20, V30, and V40. At this time,
because N20 and N50 generally do not intersect, the plane
perpendicular to the tool axis direction at the N20 end point is
regarded as a compensation plane, N20 and N50 are projected onto
this plane, and Va is determined by calculating the intersection point.
NOTE
Strictly speaking, if the tool axis direction at the
N20 end point differs from the tool axis direction
at the N50 start point, correct intersection point
calculation is not possible. For this reason, the
maximum permissible angle by which the tool axis
directions in the two blocks used to determine the
interference avoidance vector may differ can be
set in parameter No. 19636, and if the change in
tool axis direction is within the range, an
approximate interference avoidance vector is
calculated.
If the maximum angle is exceeded, the
compensation vector is determined but
interference avoidance is not performed.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 949 -
- If interference avoidance is not possible
If there are three consecutive interfering blocks, no interference vector
can be generated.
Example 1 in which interference avoidance is not possible
V40-1
V40-2
V10-1
V10-2
V20 V30
N10
N20
N30
N40
N50
N20 to N40 interfere, so that no interference avoidance vector can be
generated. Too much cutting results.
Example 2 in which interference avoidance is not possible
N10
N20 N30 N40
N50
V10
V20
V30
V40
N10 to N40 interfere, so that no interference avoidance vector can be
generated. V10 causes an interference alarm.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 950 -
22.5.5 Restrictions
22.5.5.1 Restrictions common to machine configurations
- Corner rounding (G39)
In the mode for 3-dimensional cutter compensation, G39 cannot be
specified. Specifying G39 causes an alarm.
- Reset
Whenever a reset is made in the mode for 3-dimensional cutter
compensation (G41.2, G42.2, G41.4, G42.4, G41.5, or G42.5), the
cancel mode (G40) is entered.
- AI contour control I and II
To set the AI contour control I or II mode, the corresponding G code
must be specified. Specifying 3-dimensional cutter compensation
does not automatically place the CNC in the AI contour control I or II
mode.
- Restricted commands
In the mode for 3-dimensional cutter compensation, the following
functions are available, but their statuses cannot be changed:
• Inch/metric input (If an attempt is made to change the status by
using G20 or G21, alarm PS5000 is issued.)
• Mirror image (The signal status cannot be changed.)
• One-digit F code feed (The feedrate cannot be changed by using
the manual handle.)
- When a rotary axis is moved significantly
In 3-dimensional cutter compensation, compensation is performed at
the block end point.
Even when the tool direction relative to the workpiece changes
momentarily as a rotary axis moves, compensation is not performed
momentarily during execution of the block.
Accordingly, when a rotary axis is moved significantly, carry out
programming to divide a block into small movement blocks to prevent
the machining precision from being reduced.
- Operation at cancellation
In a block for canceling 3-dimensional cutter compensation,
compensation accompanying movement is cancelled regardless of
whether the movement command is present.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 951 -
- Unavailable commands
In the mode for 3-dimensional cutter compensation, the functions
listed below cannot be specified. Specifying any of these functions
results in an alarm.
• Hypothetical axis interpolation................................................G07
• Circular interpolation............................................................G07.1
• Polar coordinate interpolation ..................................G12.1, G13.1
• Polar coordinate command .............................................G15, G16
• Reference position return check ..............................................G27
• Reference position return....................................... G28, G29, G30
• Skip..........................................................................................G31
• Threading.................................................................................G33
• Automatic tool length measurement........................................G37
• Normal direction control............................... G40.1, G41.1, G42.1
• Tool radius/tool nose radius compensation ........... G41, G42, G39
• 3-dimensional cutter compensation .........................................G41
• Wheel wear compensation.......................................................G41
• Tool offset..................................................... G45, G46, G47, G48
• Local coordinate system ..........................................................G52
• Machine coordinate system .....................................................G53
• Workpiece coordinate system setting ..................G54-G59, G54.1
• Rotary table dynamic fixture offset ......................................G54.2
• Single direction positioning.....................................................G60
• Automatic corner override.......................................................G62
• Tapping mode ..........................................................................G63
• Three-dimensional coordinate system conversion.......... G68, G69
• Tilted working plane command...................................G68.2, G69
• Figure copy............................................................... G72.1, G72.2
• Canned cycle........................G73-G79, G80, G81-G89, G98, G99
• Electric gear box............................................................. G80, G81
• Hobbling machine function ............................................ G80, G81
• External operation function .....................................................G81
• Chopping ..............................................................................G81.1
• Small hole peck drilling cycle .................................................G83
• Workpiece coordinate system setting ......................................G92
• Workpiece coordinate system presetting ..............................G92.1
• Feed per revolution..................................................................G95
• Constant surface speed control ....................................... G96, G97
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 952 -
- Unavailable functions
If the following function is specified in the 3-dimensional cutter
compensation mode, a warning message is issued:
• MDI interruption
If one of the following functions is specified in the 3-dimensional
cutter compensation mode, a PS alarm is issued:
• Manual interruption operation
• Tool retract and recover
In the 3-dimensional cutter compensation mode, the following
functions cannot be used:
• Twin table control
• Flexible synchronous control
• Sequence number comparison and stop (It is not possible to
cause a stop by sequence number in the 3-dimensional cutter
compensation mode.)
• Index table indexing
• Retrace function (Programs using the 3-dimensional cutter
compensation mode must not use the retrace function.)
• Rotary axis control
• Manual handle interruption
• External deceleration (External deceleration is not performed.)
• Angular axis control
Combinations of other NC commands may be restricted. Refer to the
manual on each function.
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 953 -
22.5.5.2 Restriction on tool rotation type
- Unavailable commands (leading edge offset)
In the G41.3 mode, the following commands cannot be specified:
- G functions of group 01 other than G00 and G01
- Use with tool center point control
If 3-dimensional cutter compensation is specified before tool center
point control when 3-dimensional cutter compensation and tool center
point control are specified together, tool center point control must be
canceled before 3-dimensional cutter compensation is canceled
(Example 1). Contrariwise, if tool center point control is specified
before 3-dimensional cutter compensation, 3-dimensional cutter
compensation must be canceled before tool center point control is
canceled (Example 2).
Example 1
G41.2 D1
:
G43.4 H1
:
G49
:
G40
Example 2
G43.4 H1
:
G41.2 D1
:
G40
:
G49
If the specification sequence of G40 and G49 is reversed, alarm
PS5460 is issued.
When 3-dimensional cutter compensation is specified before tool
center point control, the block for canceling tool center point control
suppresses buffering. Note that, as a result, the block before the G49
block generates a compensation vector for 3-dimensional cutter
compensation, which is perpendicular to the movement.
For each of 3-dimensional cutter compensation and tool center point
control, two commands, type 1 and type 2, are provided. Be sure to
specify commands of the same type. If commands of different types
are specified, alarm PS5460 is issued.
When the tool is tilted by address Q in type 2 command specification,
if Q is specified in both of the block for starting tool center point
control and the block for starting 3-dimensional cutter compensation,
the Q command specified earlier becomes valid.
- Combination with circular interpolation
When circular interpolation is specified in a block, if a rotary axis is
moved in the block, the previous block, or the next block, a cutter
compensation vector may be created in the direction orthogonal to the
plane. In this case, helical interpolation is performed, so the helical
interpolation option is required.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 954 -
22.5.5.3 Restriction on machine configurations having table rotation
axes (table rotation type and composite type)
- Unavailable commands
For machines having table rotation axes, the following commands
cannot be specified during 3-dimensional cutter compensation:
- G functions of group 01 other than G00 and G01
- Use with tool center point control
When the workpiece coordinate system is used as the programming
coordinate system, the same restrictions as for the tool rotation type
apply. See "Use with tool center point control" in the restrictions on
the tool rotation type described previously.
When the table coordinate system is used as the programming
coordinate system, the restrictions to apply will be explained below.
- Type 2
When a type 2 command (G41.6/G42.6 command) is executed, the
table coordinate system needs to be used as the programming
coordinate system (bit 4 (TBP) of parameter No. 19746 = 1 and bit 5
(WKP) of parameter No. 19696 = 0). If a type 2 command
(G41.6/G42.6 command) is executed with the workpiece coordinate
system used as the programming coordinate system, alarm PS5459 is
issued.
- Restrictions when the table coordinate system is used as the programming
coordinate system
Use with tool center point control
When 3-dimensional cutter compensation and tool center point control
are specified together, tool center point control must be specified
before cutter compensation. In addition, tool center point control
must be canceled after 3-dimensional cutter compensation is canceled.
(Example 1)
If tool center point control is specified in the 3-dimensional cutter
compensation mode (Example 2), or if tool center point control is
canceled without canceling 3-dimensional cutter compensation
(Example 3), alarm PS5460 is issued.
Example 1
(Correct
specification)
G43.4 H1
:
G41.2 D1
:
G40
:
G49
Example 2
(Specification
resulting in
alarm)
G41.2 D1
:
G43.4 H1
:
Example 3
(Specification
resulting in
alarm)
G43.4 H1
:
G41.2 D1
:
G49
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 955 -
If the setting of the programming coordinate system differs between
3-dimensional cutter compensation and tool center point control,
specifying both functions together results in alarm PS5460. (See the
following table:)
TBP=0 TBP=1
WKP=0 WKP=1 WKP=0 WKP=1
Tool center point
control
Table
coordinate
system
3-dimensional cutter
compensation
Workpiece
coordinate
system
Both specified
together
Alarm
PS5460
Workpiece
coordinate
system
Table
coordinate
system
Workpiece
coordinate
system
Programming coordinate system determined by bit 4 (TBP) of
parameter No. 19746 and bit 5 (WKP) of parameter No. 19696
The table rotation axis position at the start of tool center point control
and the table rotation axis position at the start of 3-dimensional cutter
compensation must always match.
Each programming coordinate system matches the workpiece
coordinate system used when each function is started.
If these functions are started when their table rotation axis positions
differ, the programming coordinate system for tool center point
control and the programming coordinate system for 3-dimensional
cutter compensation do not match, which results in alarm PS5460.
Example: When the A-axis is the table rotation axis:
(Correct example)
G90 G00 A0.0
G43.4 H1
G01 Z100.0 F1000.
G41.2 D1 ← After G43.4 is specified, G41.2 is specified
without A-axis movement.
:
(Wrong example)
G90 G00 A0.0
G43.4 H1
G01 Z100.0 A30.0 F1000.
G41.2 D1 ← After G43.4 is specified, A-axis movement
is made, then G41.2 is specified.
:
* Furthermore, no A-axis command can be
included in the block specifying G41.2.
For each of 3-dimensional cutter compensation and tool center point
control, two commands, type 1 and type 2, are provided. Be sure to
specify commands of the same type. If commands of different types
are specified, alarm PS5460 is issued.
When the tool is tilted by address Q in type 2 command specification,
if Q is specified in both of the block for starting tool center point
control and the block for starting 3-dimensional cutter compensation,
the Q command specified earlier becomes valid.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 956 -
Look-ahead acceleration/deceleration before interpolation
If the 3-dimensional cutter compensation mode is entered, look-ahead
acceleration/deceleration before interpolation is automatically enabled.
Set the look-ahead acceleration/deceleration parameter. If the
parameter is incorrectly set, an alarm is issued.
Deceleration at a corner
Under 3-dimensional cutter compensation, the controlled point may
move along a curve even if a straight-line command is issued. Some
commands may cause a corner movement.
When AI contour control is not used, there is a possibility that the
machine is shocked at a corner.
Accordingly, it is recommended that AI contour control be used and
the permissible acceleration (parameter No. 1737) and permissible
speed difference at a corner (parameter No. 1783) be set.
Specifiable G codes
When the table coordinate system is used as the programming
coordinate system, the G codes that can be specified in the
3-dimensional cutter compensation mode are listed below.
Specifying a G code other than these codes results in alarm PS5460:
• Positioning (G00)
• Linear interpolation (G01)
• Dwell (G04)
• Exact stop (G09)
• Programmable data input (G10)
• Programmable data input mode cancel (G11)
• Plane selection (G17/G18/G19)
• Cutter compensation : cancel (G40)
• Tool length compensation cancel (G49)
• Programmable mirror image (G50.1/G51.1)
• Macro call (G65)
• Macro modal call A (G66)
• Macro modal call B (G66.1)
• Macro modal call A/B cancel (G67)
• Absolute programming (G90)
• Incremental programming (G91)
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 957 -
Modal G codes that allow specification of 3-dimensional cutter compensation
When the table coordinate system is used as the programming
coordinate system, 3-dimensional cutter compensation can be
specified in the modal G code states listed below.
In a modal state other than the following modal G codes, specifying
tool center point control results in alarm PS5421.
• Modal G codes included in "Specifiable G codes" described
previously
• Polar coordinate interpolation mode cancel (G13.1)
• Polar coordinates command cancel (G15)
• Input in inch (G20 (G70))
• Input in mm (G21 (G71))
• Tool center point control (G43.4/G43.5)
• Polygon turning cancel (G50.2)
• Workpiece coordinate system 1 selection (G54 to G59)
• Canned cycle cancel (G80)
• Constant surface speed control cancel (G97)
• Canned cycle : return to initial level (G98)
• Canned cycle : return to R point level (G99)
M
• Coordinate system rotation start or 3-dimensional coordinate
conversion mode on (G69)
• Feed per minute (G94)
• Polar coordinate interpolation mode cancel (G113)
T
• Mirror image for double turret off/balanced cutting mode cancel
(G69)
• Coordinate system rotation cancel or 3-dimensional coordinate
conversion mode off (G69.1)
• Feed per minute (G98 (G94))
Specification of axes not relating to 3-dimensional cutter compensation
Axes not relating to 3-dimensional cutter compensation cannot be
specified. If such an axis is specified, alarm PS5460 is issued.
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 958 -
22.5.6 Examples
O100 is a sample program.
This is an example in which each side of a square is cut at an angle of
30 degrees on the B-axis in a composite type machine.
Programs 1 to 3 all perform the same machining.
Program 1: Type 1 and the table coordinate system is selected as a
programming coordinate system
O100（Sample Program1）；
N10 G55 ; Preparations for the programming coordinate system
N20 G90 X0 Y0 Z300.0 B0 C0 ; Movement to the initial position
N30 G01 G43.4 H01 Z40.0 F500. ; Start of tool center point control
H01 is a tool length compensation number
N40 G41.2 D01; Start of cutter compensation
D01 is a tool cutter compensation number
N50 X50.0 Y50.0 Z20.0 B30.0 C45.0 ; The Z-axis height on the machining plane is 20.0.
N60 X-50.0 C135.0 ;
N70 X-100.0 Y-100.0 C225.0 ;
N80 X100.0 C315.0 ;
N90 X50.0 Y50.0 C405.0 ;
N100 X0 Y0 Z40.0 B0 C360.0 ;
N110 G40 ; Cutter compensation cancellation
N120 G49 Z300.0 ; Tool center point control cancellation
Movement to the initial position on the Z-axis
N130 M30;
Program 2: Type 1 and the workpiece coordinate system is selected
as a programming coordinate system
(Note that the values specified in N50 to N90 differ from those in
program 1.)
O100（Sample Program2）;
N10 G55 ; Preparations for the programming coordinate system
N20 G90 X0 Y0 Z300.0 B0 C0 ; Movement to the initial position
N30 G01 G43.4 H01 Z40.0 F500. ; Start of tool center point control
H01 is a tool length compensation number
N40 G41.2 D01; Start of cutter compensation
D01 is a tool cutter compensation number
N50 X70.711 Y0 Z20.0 B30.0 C45.0 ; The Z-axis height on the machining plane is 20.0.
N60 C135.0 ;
N70 X141.421 C225.0 ;
N80 C315.0 ;
N90 X70.711 C405.0 ;
N100 X0 Y0 Z40.0 B0 C360.0 ;
N110 G40 ; Cutter compensation cancellation
N120 G49 Z300.0 ; Tool center point control cancellation
Movement to the initial position on the Z-axis
N130 M30;
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 959 -
Program 3: When the type 2 is used:
(The table coordinate system is selected as a
programming coordinate system)
O100（Sample Program3）;
N10 G55 ; Preparations for the programming coordinate system
N20 G90 X0 Y0 Z300.0 B0 C0 ; Movement to the initial position
N30 G01 G43.5 H01 Z40.0 F500. ; Start of tool center point control
H01 is a tool length compensation number
N40 G41.6 D01; Start of cutter compensation
D01 is a tool cutter compensation number
N50 X50.0 Y50.0 Z20.0 I35.355 J35.355 K86.603 ; The Z-axis height on the machining plane is 20.
N60 X-50.0 I-35.355 J35.355 K86.603 ;
N70 X-100.0 Y-100.0 I-35.355 J-35.355 K86.603 ;
N80 X100.0 I35.355 J-35.355 K86.603 ;
N90 X50.0 Y50.0 I35.355 J35.355 K86.603 ;
N100 X0 Y0 Z40.0 K1.0 ;
N110 G40 ; Cutter compensation cancellation
N120 G49 Z300.0 ; Tool center point control cancellation
Movement to the initial position on the Z-axis
N130 M30;
By using type 2 as in program 3, the same program can be used with
machines with different configurations, regardless of whether the
machine configuration is the tool rotation type, table rotation type, or
composite type.
Composite type (tool rotation axis: B-axis - table rotation axis:
C-axis - tool axis: Z direction
C
G55
Workpiece coordinate system
Rotation center of
B-axis
X
Z
Y
B
Rotation center of
C-axis
Fig. 22.5.6 (a) Machine configuration for example
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 960 -
Fig. 22.5.6 (b) shows the attitudes of the workpiece (object to be
machined) and the tool head (relative to the workpiece (object to be
machined)) as viewed in the positive Z direction of the programming
coordinate system fixed to the table (table coordinate system).
Operation as viewed from the table coordinate system
(
X-100.0
,
Y-100.0
)
(
B 30.0
)
(
C 45.0
)
(
C 135.0
)
(
X-50.0
,
Y50.0
)
(
X50.0
,
Y50.0
)
X'
Y'
(
B 30.0
)
(
B 30.0
)
(
B 30.0
)
(
C 225.0
)
(
C 315.0
)
(
X-100.0
,Y
-100.0
)
Fig. 22.5.6 (b) Illustration of example
B-63944EN/03 PROGRAMMING 22.5-AXIS MACHINING FUNCTION
- 961 -
Exploded view of each block
Operation at control point
(machine coordinate values)
Block N70
(
C 45.0
)
(C 135.0)
(
C 135.0
)
X'
Y'
Block N60
Y"
X"
Y"
X"
(
C 225.0
)
X' Y'
X'Y' : Table coordinate system
X"'Y" : Work
p
iece coordinate s
y
stem
Fig. 22.5.6 (c) Exploded View of Each Block (1)
22.5-AXIS MACHINING FUNCTION PROGRAMMING B-63944EN/03
- 962 -
Block N90
X'
Y'
Block N80
Y"
X"
Y"
X"
X'
Y'
(
C 225.0
)
(
C 315.0
)
(
C 315.0
)
(
C 405.0
)
Fig. 22.5.6 (d) Exploded View of Each Block (2)
B-63944EN/03 PROGRAMMING 23.MUITI-PATH CONTROL FUNCTION
- 963 -
23 MUITI-PATH CONTROL FUNCTION
Chapter 23, "MUITI-PATH CONTROL FUNCTION", consists of the
following sections:
23.1 OVERVIEW...........................................................................964
23.2 WAITING FUNCTION FOR PATHS ...................................966
23.3 COMMON MEMORY BETWEEN EACH PATH................972
23.4 SPINDLE CONTROL BETWEEN EACH PATH.................974
23.5 SYNCHRONOUS/COMPOSITE/SUPERIMPOSED
CONTROL .............................................................................975
23.MUITI-PATH CONTROL FUNCTION PROGRAMMING B-63944EN/03
- 964 -
23.1 OVERVIEW
The multi-path control function is designed to enable 10 independent
simultaneous machining with up to 10 paths (10-path control). This
function is applicable to lathes and automatic lathes which perform
cutting simultaneously with multiple tool posts, combined machine
tools which perform turning and milling simultaneously with multiple
paths, and machines which require additional control paths such as a
loader control path.
For multi-path simultaneous machining, each machining program is
stored in a folder in program memory for each path. When automatic
operation is to be performed, each path is activated after selecting a
program for machining with path 1 and programs for machining with
paths 2 to 10 from the programs stored in the respective folders in
program memory. Then the programs selected for the tool posts are
executed independently at the same time. When tool post 1 and tool
post 2 need to wait for each other during machining, the waiting
function is available.
Other available functions specific to multi-path control include
interference check for each path, balance cut, synchronous control,
composite control, spindle control between each path, and common
memory between each path.
Just one LCD/MDI is provided for the all paths. Before operation
and display on the LCD/MDI, the path selection signal is used to
switch between the paths.
B-63944EN/03 PROGRAMMING 23.MUITI-PATH CONTROL FUNCTION
- 965 -
Example) For a system with four paths
Program folder for path
1
Program folder for path
2
Program folder for path
3
Path 1
program
analysis
Path 2
program
analysis
Path 3
program
analysis
Path 1
position
control
Path 2
position
control
Path 3
position
control
Path 1 axis
control
CNC
LCD/MDI
Path 2 axis
control
Path 3 axis
control
Program folder for path
4Path 4
program
analysis
Path 4
position
control
Path 4 axis
control
Program memory
Programs
Programs
Programs
Programs
23.MUITI-PATH CONTROL FUNCTION PROGRAMMING B-63944EN/03
- 966 -
23.2 WAITING FUNCTION FOR PATHS
Overview
Control based on M codes is used to cause one path to wait for the
other during machining. When an M code for waiting is specified in
a block for one path during automatic operation, the other path waits
for the same M code to be specified before staring the execution of the
next block.
A range of M codes used as M codes for waiting is to be set in the
parameters (Nos. 8110 and 8111) beforehand. Waiting can be
ignored using a signal.
Format
M m (Pp) ;
m: Number of an M code for waiting
p: (1) In the binary value specification mode, specify the
sum of the binary values corresponding to the
numbers of paths which are to wait for one another.
(2) In the path number specification mode, specify the
numbers of all paths that are to wait for one another
in combination.
Explanation
The following two methods for specifying paths which are to wait for
one another at address P in the same block in which an M code for
waiting is specified are available and can be selected using bit 1
(MWP) of parameter No. 8103. One method is to specify the paths
with the sum of their corresponding binary values (waiting set for
three or more paths specified with binary values). The other is to
specify them with their path numbers in combination (waiting
specified with path numbers).
When address P is not specified, paths 1 and 2 wait for each other
(waiting set for two paths). Always specify address P in a single
block.
B-63944EN/03 PROGRAMMING 23.MUITI-PATH CONTROL FUNCTION
- 967 -
- Waiting specified with binary values
When bit 1 (MWP) of parameter No. 8103 is set to 0, the value
specified at address P is assumed to be obtained using binary values.
The following table lists the path numbers and corresponding binary
values.
Path number Binary value (decimal number)
1 1
2 2
3 4
4 8
5 16
6 32
7 64
8 128
9 256
10 512
The bit position of each path in binary representation is shown below.
15 14 13 12 11 10 9 8 7 6 5 4 3 2 1 0
To make all of paths 1, 2, and 3 wait for one another, the P value is
obtained as follows:
Binary value of path 1 1 (0000 0000 0000 0001)
Binary value of path 2 2 (0000 0000 0000 0010)
Binary value of path 3 4 (0000 0000 0000 0100)
Sum 7 (0000 0000 0000 0111)
Path 1 (20 = 1)
Path 2 (21 = 2)
Path 3 (22 = 4)
Path 4 (23 = 8)
Path 5 (24 = 16)
Path 6 (25 = 32)
Path 7 (26 = 64)
Path 8 (27 = 128)
Path 9 (28 = 256)
Path 10 (29 = 512)
23.MUITI-PATH CONTROL FUNCTION PROGRAMMING B-63944EN/03
- 968 -
All of the three paths can be made to wait for one another by
specifying P7 together with an M code for waiting.
To make all of paths 1, 3, 5, 7, and 9 wait for one another, the P value
is obtained as follows:
Binary value of path 1 1 (0000 0000 0000 0001)
Binary value of path 3 4 (0000 0000 0000 0100)
Binary value of path 5 16 (0000 0000 0001 0000)
Binary value of path 7 64 (0000 0000 0100 0000)
Binary value of path 9 256 (0000 0001 0000 0000)
Sum 341 (0000 0001 0101 0101)
All of the five paths can be made to wait for one another by specifying
P341 together with an M code for waiting.
- Waiting specified with a combination of path numbers
When bit 1 (MWP) of parameter No. 8103 is set to 1, the value
specified at address P is assumed to be a combination of path numbers.
The following table lists the path numbers and corresponding values.
Path number Value (decimal number)
1 1
2 2
3 3
4 4
5 5
6 6
7 7
8 8
9 9
10 0
To make all of paths 1, 2, and 3 wait for one another, the P value is a
number consisting of 1, 2, and 3.
Example) P123
There are no restrictions on the order in which the numeric characters
are specified, and the following six possible values can be specified:
P123, P132, P213, P231, P312, P321
Path numbers specified in combination in different orders for different
paths are effective as long as the numbers of the relevant paths are
specified.
Example) The following are treated as the same P value and
these paths can be made to wait for one another:
M200P123 for path 1, M200P231 for path 2, and
M200P321 for path 3
To make all of paths 1, 3, 5, 7, and 9 wait for one another, the P value
is a number consisting of 1, 3, 5, 7, and 9.
Example) P13579
B-63944EN/03 PROGRAMMING 23.MUITI-PATH CONTROL FUNCTION
- 969 -
- Waiting for path 10
To make path 10 and another path wait for each other, specify a value
of 0 for the combination.
If a number begins with 0, 0 cannot be recognized. Specify 0 in the
second or subsequent digit from the left.
Incorrect example) P013579
Correct example) P103579
In the incorrect example, the P value is assumed to be the same as
P13579. Path 10 cannot be made to wait for other paths and other
paths cannot be made to wait for path 10.
Example
- When the value specified at P is obtained using binary values
Assume that the waiting ignore signal for path 2 (G1063.7 for a
system with three or more paths) is set to 1 and M101 to M103
(parameter No. 8110 = 101 and parameter No. 8111 = 103) are set as
M codes for waiting. In this case, programs O100, O200, and O300
for individual paths are executed as follows:
O0300;
G50 X Z ;
G00 X Z T0303;
M102 P7; ................. <2>
O0100;
G50 X Z ;
G00 X Z T0101;
M03 S1000;
.
.
M101 P3; .................. <1>
G01 X Z F ;
.
.
M102 P7; .................. <2>
M103 P7; .................. <3>
O0200;
G50 X Z ;
G00 X Z T0202;
M03 S2000;
M101 P3; .................. <1>
G01 X Z F ;
.
.
M102 P7; .................. <2>
M103 P7; .................. <3>
.
.
.
.
.
.
.
.
.
G00 X Z ;
.
.
M103 P7; .................. <3>
G00 X Z ;
.
G01 X Z F ;
.
.
<<Waiting (M102)>>
<<Waiting (M103)>>
Path 1 Path 2 Path 3
<1> M101 P3; (making paths 1 and 2 wait for each other)
When the waiting ignore signal for path 2 is set to 0, paths 1 and
2 wait for each other. Because the signal is set to 1, however,
paths 1 and 2 ignore the M code for waiting and immediately
execute the next block.
<2> M102 P7; (making paths 1, 2, and 3 wait for one another)
In this example, path 3 waits for processing on paths 1 and 2 to
terminate. Because the waiting ignore signal for path 2 is set to
1, however, path 3 assumes that waiting is completed when
processing on path 1 terminates, and executes the next block.
23.MUITI-PATH CONTROL FUNCTION PROGRAMMING B-63944EN/03
- 970 -
<3> M103 P7; (making paths 1, 2, and 3 wait for one another)
In this example, paths 1 and 2 wait for processing on path 3 to
terminate. Because the waiting ignore signal for path 2 is set to
1, however, path 2 does not wait for processing on path 3 to
terminate and executes the next block, but path 1 waits for path
3.
- When the value specified at P is obtained using path numbers in combination
Assume that the waiting ignore signal for path 2 (G1063.7 for a
system with three or more paths) is set to 1 and M101 to M103
(parameter No. 8110 = 101 and parameter No. 8111 = 103) are set as
M codes for waiting. In this case, programs O100, O200, and O300
for individual paths are executed as follows:
O0300;
G50 X Z ;
G00 X Z T0303;
M102 P123; ............. <2>
O0100;
G50 X Z ;
G00 X Z T0101;
M03 S1000;
.
.
M101 P12; ................ <1>
G01 X Z F ;
.
.
M102 P123; .............. <2>
M103 P123; .............. <3>
O0200;
G50 X Z ;
G00 X Z T0202;
M03 S2000;
M101 P12; ................ <1>
G01 X Z F ;
.
.
M102 P123; .............. <2>
M103 P123; .............. <3>
.
.
.
.
.
.
.
.
.
G00 X Z ;
.
.
M103 P123; .............. <3>
G00 X Z ;
.
G01 X Z F ;
.
.
<<Waiting (M102)>>
<<Waiting (M103)>>
Path 1 Path 2 Path 3
<1> M101 P12; (making paths 1 and 2 wait for each other)
When the waiting ignore signal for path 2 is set to 0, paths 1 and
2 wait for each other. Because the signal is set to 1, however,
paths 1 and 2 ignore the M code for waiting and immediately
execute the next block.
<2> M102 P123; (making paths 1, 2, and 3 wait for one another)
In this example, path 3 waits for processing on paths 1 and 2 to
terminate. Because the waiting ignore signal for path 2 is set to
1, however, path 3 assumes that waiting is completed when
processing on path 1 terminates, and executes the next block.
<3> M103 P123; (making paths 1, 2, and 3 wait for one another)
In this example, paths 1 and 2 wait for processing on path 3 to
terminate. Because the waiting ignore signal for path 2 is set to
1, however, path 2 does not wait for processing on path 3 to
terminate and executes the next block, but path 1 waits for path
3.
B-63944EN/03 PROGRAMMING 23.MUITI-PATH CONTROL FUNCTION
- 971 -
CAUTION
1 An M code for waiting must always be specified in a
single block.
2 Unlike other M codes, the M code for waiting is not
output to the PMC.
3 If the operation of a single path is required, the M
code for waiting need not be deleted. By using the
signal to specify that waiting be ignored (NOWT for
the system with two paths, NMWT for the system
with three or more paths), the M code for waiting in
a machining program can be ignored. For details,
refer to the manual supplied by the machine tool
builder.
4 If using a waiting M code in block multiple-M code
command mode, be sure to specify it as the first M
code.
23.MUITI-PATH CONTROL FUNCTION PROGRAMMING B-63944EN/03
- 972 -
23.3 COMMON MEMORY BETWEEN EACH PATH
Overview
In a multi-path system, this function enables data within the specified
range to be accessed as data common to all paths. The data includes
tool compensation memory and custom macro common variables.
Explanation
The path common memory function enables the following operations.
- Tool compensation memory
Part or all of tool compensation memory for individual paths can be
used as common data by setting parameter No. 5029.
Tool
compensation
number 20
Tool
compensation
number 1
50 tool
offset
pairs
30 tool
offset
pairs
Tool offset pairs of path
2 on lathe system
No.5029=20
Tool offset pairs of path
1 on lathe system
NOTE
1 When a combined system including a machining
center system and lathe system is used, data is
made common according to the same path control
type.
2 The same unit for tool compensation (bits 0 to 3 of
parameter No. 5042) must be set for each of the
machining center and lathe systems.
3 Set a value less than the number of tool
compensation values for each path for parameter
No. 5029.
4 If the value set for parameter No. 5029 is greater
than the number of tool compensation values for
each path, the minimum number of tool
compensation values for individual paths is
assumed.
5 For details, refer to the relevant manual of the
machine tool builder.
B-63944EN/03 PROGRAMMING 23.MUITI-PATH CONTROL FUNCTION
- 973 -
- Custom macro common variables
All or part of custom macro common variables #100 to #149 (, #199,
or #499) and #500 to #599 (or #999) can be used as common data by
setting parameters No. 6036 (#100 to #149 (, #199, or #499)) and
6037 (#500 to #599 (or #999)).
50 macro
variables
50 macro
variables
Macro variable number 119
Macro variable number 100
Macro variables
for path 1
No.6036=20
Macro variables
for path 2
NOTE
1 If the value of parameter No. 6036 or 6037 exceeds
the maximum number of macro common variables,
the maximum number of macro common variables
is assumed.
2 Common variables #150 to #199, #150 to #499,
and #600 to #999 are optional functions.
23.MUITI-PATH CONTROL FUNCTION PROGRAMMING B-63944EN/03
- 974 -
23.4 SPINDLE CONTROL BETWEEN EACH PATH
Overview
This function allows a workpiece attached to one spindle to be
machined simultaneously with two tool posts and each of two
workpieces attached to each of two spindles to be machined
simultaneously with each of two tool posts.
Spindle
Tool post 1
Tool post 2
Fig. 23.4 (a) Application to a lathe with one spindle and two tool posts
¥
Tool post 2
Spindle 1
Tool post 1
Spindle 2
Fig. 1.1 (b) Application to a lathe with two spindles and two tool posts
The spindle belonging to each path can generally be controlled by
programmed commands for the path. With path spindle command
selection signals, programmed commands for any path can control the
spindle belonging to any path.
NOTE
For the method of spindle command selection, refer
to the relevant manual of the machine tool builder.
B-63944EN/03 PROGRAMMING 23.MUITI-PATH CONTROL FUNCTION
- 975 -
23.5 SYNCHRONOUS/COMPOSITE/SUPERIMPOSED
CONTROL
Overview
In multi-path control, the synchronous control function, composite
control function, and superimposed control function enable
synchronous control, composite control, and superimposed control in
a single path system or between multi-path systems.
Explanation
- Synchronous control
• Synchronizes movement along an axis of one system with that
along an axis of the other path.
Example)
Synchronizing movement along the Z1 (master) and Z2 (slave)
axes (in the case of turning)
Workpiece
Z2 (Synchronized with
movement along the Z1 axis)
Z1
Turret 1
X1
Machining according to a program for path 1
23.MUITI-PATH CONTROL FUNCTION PROGRAMMING B-63944EN/03
- 976 -
• Synchronizes movement along an axis of one path with that along
another axis of the same path.
Example)
Synchronizing movement along the Z1 (master) and B1 (slave)
axes (in the case of turning)
B1 (Synchronized with
movement along the Z1
axis)
Workpiece 1
Z1
Turret 1
X1
Tail stock
- Composite control
• Exchanges the move commands for different axes of different path.
Example)
Exchanging the commands for the X1 and X2 axes (in the case
of turning)
→ Upon the execution of a command programmed for path 1,
movement is performed along the X2 and Z1 axes.
Upon the execution of a command programmed for path 2,
movement is performed along the X1 and Z2 axes.
Machining according to a program
for path 1
Machining according to
a program for path 2
Workpiece 1
Turret 1
Workpiece 2
Turret 1
Z1
X2
Z2
X1
B-63944EN/03 PROGRAMMING 23.MUITI-PATH CONTROL FUNCTION
- 977 -
- Superimposed control
• Provides a move command of an axis for a different axis in another
path.
Example)
Providing the Z2 (slave) axis with a move command specified
for the Z1 (master) axis (in the case of turning)
Machining according to a program
for path 2
Workpiece 1
Turret 1
Turret 2
Z1 X2
Z2
X1 Machining according to
a program for path 1
NOTE
The method used to specify synchronous,
composite, or superimposed control varies with the
machine tool builder. For details, refer to the
manual supplied by the machine tool builder.
III. OPERATION
B-63944EN/03 OPERATION 1.GENERAL
- 981 -
1 GENERAL
Chapter 1, "GENERAL", consists of the following sections:
1.1 MANUAL OPERATION..........................................................982
1.2 TOOL MOVEMENT BY PROGRAMING - AUTOMATIC
OPERATION ............................................................................984
1.3 AUTOMATIC OPERATION ...................................................986
1.4 TESTING A PROGRAM .........................................................988
1.5 EDITING A PROGRAM..........................................................990
1.6 DISPLAYING AND SETTING DATA....................................991
1.7 DISPLAY..................................................................................994
1.8 ADJUSTMENT OF THE BRIGHTNESS OF THE
MONOCHROME LCD ............................................................997
1.GENERAL OPERATION B-63944EN/03
- 982 -
1.1 MANUAL OPERATION
Explanation
- Manual reference position return
The CNC machine tool has a position used to determine the machine
position.
This position is called the reference position, where the tool is
replaced or the coordinate are set. Ordinarily, after the power is
turned on, the tool is moved to the reference position.
Manual reference position return is to move the tool to the reference
position using switches and pushbuttons located on the operator's
panel. (See Section III-3.1)
Reference position
Tool
Machine operator's panel
Fig. 1.1 (a) Manual reference position return
The tool can be moved to the reference position also with program
commands.
This operation is called automatic reference position return (See
Section II-6).
B-63944EN/03 OPERATION 1.GENERAL
- 983 -
- The tool movement by manual operation
Using machine operator's panel switches, pushbuttons, or the manual
handle, the tool can be moved along each axis.
Tool
Workpiece
Machine operator's panel
Manual pulse
generator
Fig. 1.1 (b) The tool movement by manual operation
The tool can be moved in the following ways:
(i) Jog feed (See Section III-3.2)
The tool moves continuously while a pushbutton remains
pressed.
(ii) Incremental feed (See Section III-3.3)
The tool moves by the predetermined distance each time a button
is pressed.
(iii) Manual handle feed (See Section III-3.4)
By rotating the manual handle, the tool moves by the distance
corresponding to the degree of handle rotation.
1.GENERAL OPERATION B-63944EN/03
- 984 -
1.2 TOOL MOVEMENT BY PROGRAMING - AUTOMATIC
OPERATION
Automatic operation is to operate the machine according to the created
program. It includes memory, MDI and DNC operations. (See Section
III-4).
Program
Tool
01000 ;
M S T ;
G92 X ;
G00 ;
G01 ;
:
:
:
Fig. 1.2 (a) Tool Movement by programming
Explanation
- Memory operation
After the program is once registered in memory of CNC, the machine
can be run according to the program instructions. This operation is
called memory operation.
CNC Machine
Memory
Fig. 1.2 (b) Memory operation
B-63944EN/03 OPERATION 1.GENERAL
- 985 -
- MDI operation
After the program is entered, as an command group, from the MDI
keyboard, the machine can be run according to the program. This
operation is called MDI operation.
CNC MDI keyboard Machine
Manual program
input
Fig. 1.2 (c) MDI operation
- DNC operation
In this mode of operation, the program is not registered in the CNC
memory. It is read from the external input/output devices instead.
This is called DNC operation.
1.GENERAL OPERATION B-63944EN/03
- 986 -
1.3 AUTOMATIC OPERATION
Explanation
- Program selection
Select the program used for the workpiece. Ordinarily, one program
is prepared for one workpiece. If two or more programs are in memory,
select the program to be used, by searching the program number
(Section III-9.3).
Programs in memory
Search for desired program by
file name or program number.
A
utomatic
operation
M30
G92
O1001
Fig. 1.3 (a) Program selection for automatic operation
- Start and stop
Pressing the cycle start pushbutton causes automatic operation to start.
By pressing the feed hold or reset pushbutton, automatic operation
pauses or stops. By specifying the program stop or program
termination command in the program, the running will stop during
automatic operation. When one process machining is completed,
automatic operation stops. (See Section III-4)
Cycle start Start
Feed hold
Reset
A
utomatic
operation
Program stop
Program end
Stop caused
by program
Stop
Fig. 1.3 (b) Start and stop for automatic operation
B-63944EN/03 OPERATION 1.GENERAL
- 987 -
- Handle interruption
While automatic operation is being executed, tool movement can
overlap automatic operation by rotating the manual handle. (See
Section III-4.4)
Z
X
Programmed
depth of cut
Tool position after
handle interru
p
tion
Tool position
during automatic
operation
Depth of cut
by handle
interruption
Fig. 1.3 (c) Handle interruption for automatic operation
1.GENERAL OPERATION B-63944EN/03
- 988 -
1.4 TESTING A PROGRAM
Before machining is started, the automatic running check can be
executed.
It checks whether the created program can operate the machine as
desired.
This check can be accomplished by running the machine actually or
viewing the position display change (without running the machine)
(See Section III-5).
1.4.1 Check by Running the Machine
Explanation
- Dry run
Remove the workpiece, check only movement of the tool. Select the
tool movement rate using the dial on the operator's panel. (See Section
III-5.4)
Tool
Table
Fig. 1.4.1 (a) Dry run
- Feedrate override
Check the program by changing the feedrate specified in the program.
(See Section III-5.2)
Tool
Feedrate specified by program :
100 mm/min.
Feedrate after feed rate
override (20%) : 20 mm/min.
Workpiece
Fig. 1.4.1 (b) Feedrate override
B-63944EN/03 OPERATION 1.GENERAL
- 989 -
- Single block
When the cycle start pushbutton is pressed, the tool executes one
operation then stops. By pressing the cycle start again, the tool
executes the next operation then stops. The program is checked in this
manner. (See Section III-5.5)
Tool
Cycle start Stop Stop
Stop
Workpiece
Cycle
start
Cycle
start
Cycle
start
Fig. 1.4.1 (c) Single Block
1.4.2 How to View the Position Display Change without Running
the Machine
Explanation
- Machine Lock
MDI
X
Y
Z
Tool
The tool remains stopped, and only the
positional displays of the axes change.
Workpiece
Fig. 1.4.2 (a) Machine Lock
- Auxiliary function lock
When automatic running is placed into the auxiliary function lock
mode during the machine lock mode (See Sections III-5.1), all
auxiliary functions (spindle rotation, tool replacement, coolant on/off,
etc.) (See Section III-5.1) are disabled.
1.GENERAL OPERATION B-63944EN/03
- 990 -
1.5 EDITING A PROGRAM
After a created program is once registered in memory, it can be
corrected or modified from the MDI panel (See Section III-10).
This operation can be executed using the program edit function.
B-63944EN/03 OPERATION 1.GENERAL
- 991 -
1.6 DISPLAYING AND SETTING DATA
The operator can display or change a value stored in CNC internal
memory by key operation on the MDI screen (See III-12).
Data setting
Data display
Screen Keys
MDI
CNC memory
Fig. 1.6 (a) Displaying and setting data
Explanation
- Offset value
Setting
Display
Screen Keys
MDI
Geometry Wear
compensation compensation
Tool compensation number 1 12.3 25.0
Tool compensation number 2 20.0 40.0
Tool compensation number 3
CNC memory
Fig. 1.6 (b) Displaying and Setting Offset Values
The tool has the tool dimension (length, diameter). When a workpiece
is machined, the tool movement value depends on the tool dimensions.
By setting tool dimension data in CNC memory beforehand, CNC
automatically generates tool routes that permit any tool to cut the
workpiece specified by the program. Tool dimension data is called the
offset value.
1.GENERAL OPERATION B-63944EN/03
- 992 -
Machined
shape
2nd tool path
1st tool path
Offset value of the 1st tool
Offset value of the 2nd tool
Fig. 1.6 (c) Offset value
- Displaying and setting operator's setting data
Apart from parameters, there is data that is set by the operator in
operation. This data causes machine characteristics to change.
For example, the following data can be set:
• Inch/Metric switching
• Selection of I/O devices
• Mirror image cutting on/off
The above data is called setting data (See Section III-12.3.1).
Setting
Screen Keys
MDI
Displaying
CNC Memory
Program
A
utomatic
operation Movement of
the machine
Operational
characteristics
Setting data
Inch/Metric switching
Ì
Ý
Selection of I/O device
Mirror image ON/OFF setting
:
:
:
Fig. 1.6 (d) Displaying and setting operator's setting data
B-63944EN/03 OPERATION 1.GENERAL
- 993 -
- Displaying and setting parameters
The CNC functions have versatility in order to take action in
characteristics of various machines.
For example, CNC can specify the following:
- Rapid traverse rate of each axis
- Whether increment system is based on metric system or inch
system.
- How to set command multiply/detect multiply (CMR/DMR)
Data to make the above specification is called parameters (See Section
III-12.4.1).
Parameters differ depending on machine tool.
Setting
Screen Keys
MDI
Display
CNC memory
Parameter
Rapid traverse rate
Position control
Reference position return
Backlash compensation data
Pitch error compensation data
:
:
:
Program
A
utomatic
operation Movement o
f
the machine
Operational
characteristics
Fig. 1.6 (e) Displaying and setting parameters
- Data protection key
A key called the data protection key can be defined. It is used to
prevent part programs, offset values, parameters, and setting data from
being registered, modified, or deleted erroneously (See Section
III-12).
Program
Offset value
Parameters
Setting data
Data Setting
Machine
operator's panel
Screen Keys
Data protection key
MDI
Signal
Data
p
rotection ke
y
Registration / modification inhibition
CNC memory
Fig. 1.6 (f) Data protection key
1.GENERAL OPERATION B-63944EN/03
- 994 -
1.7 DISPLAY
1.7.1 Program Display
The contents of the currently active program are displayed.
(See Section III-12.2.1)
Fig. 1.7.1 (a)
A list of the programs held in the currently selected folder is
displayed.
Fig. 1.7.1 (b)
Running sequence number
The line currently being executed
is indicated by the cursor.
Contents of
p
ro
g
ram
Running program number
B-63944EN/03 OPERATION 1.GENERAL
- 995 -
1.7.2 Current Position Display
The current position of the tool is displayed with the coordinate
values.
Moreover, the distance from the current position to a target point can
be displayed as a remaining travel distance.
(See Section III-12.1.1, 12.1.2, 12.1.3.)
Y
X
X
Y
Workpiece coordinate
system
Fig. 1.7.2 (a)
Fig. 1.7.2 (b)
1.GENERAL OPERATION B-63944EN/03
- 996 -
1.7.3 Alarm Display
When a trouble occurs during operation, error code and alarm message
are displayed on the screen. (See Section III-7.1.)
See APPENDIX G for the list of error codes and their meanings.
Fig. 1.7.3 (a)
1.7.4 Parts Count Display, Run Time Display
The position display screen displays a run time, cycle time, and parts
count. (See Section lll-12.3.3.)
Fig. 1.7.4 (a)
B-63944EN/03 OPERATION 1.GENERAL
- 997 -
1.8 ADJUSTMENT OF THE BRIGHTNESS OF THE
MONOCHROME LCD
The brightness of the monochrome LCD can be adjusted.
- Procedure
To adjust the brightness of the monochrome LCD, follow the
procedure below on the SETTING (HANDY) screen.
1 Press function key .
2 Press soft key [SETING] to display the SETTING DATA screen.
Press multiple times until the SETTING (HANDY)
screen appears.
Fig. 1.8 (a) Adjustment of the brightness of the SETTING screen
3 Move the cursor to the CONTRAST item.
4 When soft key [(OPRT)] is pressed, soft keys [ON:1] and
[OFF:0] are displayed.
Each time soft key [ON:1] is pressed, the brightness of the screen
is increased.
Each time soft key [OFF:0] is pressed, the brightness of the
screen is decreased.
NOTE
1 The new brightness of the screen is saved across
power-off.
2 This setting item appears only when the
monochrome LCD is connected.
2.OPERATIONAL DEVICES OPERATION B-63944EN/03
- 998 -
2 OPERATIONAL DEVICES
As operational devices, setting and display devices attached to the
CNC, and machine operator's panels are available.
For machine operator's panels, refer to the relevant manual of the
machine tool builder.
Chapter 2, "OPERATIONAL DEVICES", consists of the following
sections:
2.1 SETTING AND DISPLAY UNITS..........................................999
2.2 OPERATIONAL DEVICES ...................................................1006
2.3 FUNCTION KEYS AND SOFT KEYS .................................1009
2.4 EXTERNAL I/O DEVICES....................................................1025
2.5 POWER ON/OFF....................................................................1027
B-63944EN/03 OPERATION 2.OPERATIONAL DEVICES
- 999 -
2.1 SETTING AND DISPLAY UNITS
The setting and display units are shown in Subsections 2.1.1 to 2.1.8
of Part III.
7.2" LCD CNC Display Panel .................................................. III-2.1.1
8.4" LCD CNC Display Panel .................................................. III-2.1.2
10.4" LCD CNC Display Panel ................................................ III-2.1.3
12.1" LCD CNC Display Panel ................................................ III-2.1.4
15" LCD CNC Display Panel ................................................... III-2.1.5
Standard MDI Unit (ONG Key) ............................................... III-2.1.6
Standard MDI Unit (QWERTY Key) ....................................... III-2.1.7
Small MDI Unit (ONG Key) .................................................... III-2.1.8
2.OPERATIONAL DEVICES OPERATION B-63944EN/03
- 1000 -
2.1.1 7.2" LCD CNC Display Panel
2.1.2 8.4" LCD CNC Display Panel
B-63944EN/03 OPERATION 2.OPERATIONAL DEVICES
- 1001 -
2.1.3 10.4" LCD CNC Display Panel
2.1.4 12.1" LCD CNC Display Panel
2.OPERATIONAL DEVICES OPERATION B-63944EN/03
- 1002 -
2.1.5 15" LCD CNC Display Panel
B-63944EN/03 OPERATION 2.OPERATIONAL DEVICES
- 1003 -
2.1.6 Standard MDI Unit (ONG Key)
Unit with machining center system
Reset keyHelp key
A
ddress/numeric keys
Edit keys
Cancel (CAN) key
Input key
Shift key
Page change keys
(Page key)
Cursor keys Function keys
A
UX key
Uppercase/lowercase
switch key
CTRL key
A
LT key
TAB key
Unit with lathe system
Reset key Help key
A
ddress/numeric keys
Edit keys
Cancel (CAN) key
Input key
Shift key
Page change keys
(Page key)
Cursor keys Function keys
A
UX key
Uppercase/lowercase
switch key
CTRL key
A
LT ke
y
TAB key
2.OPERATIONAL DEVICES OPERATION B-63944EN/03
- 1004 -
2.1.7 Standard MDI Unit (QWERTY Key)
A
ddress keys
Reset key
Help key
Uppercase/lowercase
switch key
Shift key
A
UX key
CTRL key
A
LT key
TAB key
Page change keys
(Page key)
Cursor keys
Function keys
Input key
Cancel (CAN) key
Edit keys
Numeric keys
B-63944EN/03 OPERATION 2.OPERATIONAL DEVICES
- 1005 -
2.1.8 Small MDI Unit (ONG Key)
Unit with machining center system
Reset key
Help key
Shift key
Page change keys
(Page key)
Cursor keys
Function keys
Edit keys
Cancel (CAN) key
Input key
A
ddress/numeric keys
Unit with lathe system
Reset key
Help key
Shift key
Page change keys
(Page key)
Cursor keys
Function keys
Edit keys
Cancel (CAN) key
Input key
A
ddress/numeric keys
2.OPERATIONAL DEVICES OPERATION B-63944EN/03
- 1006 -
2.2 OPERATIONAL DEVICES
Table 2.2 (a) Explanation of the MDI keyboard
Number Name Explanation
1
RESET key
Press this key to reset the CNC, to cancel an alarm, etc.
2
HELP key
Press this key to use the help function when uncertain about the operation
of an MDI key (help function).
3 Soft keys The soft keys have various functions, according to the Applications. The soft key
functions are displayed on the display unit.
4
Address and numeric keys
. . .
Press these keys to input alphabetic, numeric, and other characters.
5
SHIFT key
Some keys have two characters on their keytop. Pressing the <SHIFT> key
switches the characters. Special character ^ is displayed on the screen when a
character indicated at the bottom right corner on the keytop can be entered.
6
INPUT key
When an address or a numerical key is pressed, the data is input to the buffer,
and it is displayed on the screen. To copy the data in the key input buffer to the
offset register, etc., press the key. This key is equivalent to the [INPUT]
key of the soft keys, and either can be pressed to produce the same result. This
key is also used to move to a folder on the program folder screen.
7
CANCEL (CAN) key
Press this key to delete the last character or symbol input to the key input buffer.
Example) When the key input buffer displays
>N001X100Z_
and the cancel key is pressed, Z is canceled and
>N001X100_
is displayed.
8
Edit keys
Press these keys when editing the program.
: ALTER
: INSERT
: IDELETE
9
Function keys
. . .
Press theses keys to switch display screens for each function.
See lll-2.3 for details of the function keys.
10
Cursor keys
There are four different cursor move keys.
: This key is used to move the cursor to the right or in the forward
direction. The cursor is moved in short units in the forward direction.
: This key is used to move the cursor to the left or in the reverse direction.
The cursor is moved in short units in the reverse direction.
: This key is used to move the cursor in a downward or forward direction.
The cursor is moved in large units in the forward direction.
: This key is used to move the cursor in an upward or reverse direction.
The cursor is moved in large units in the reverse direction.
B-63944EN/03 OPERATION 2.OPERATIONAL DEVICES
- 1007 -
Table 2.2 (a) Explanation of the MDI keyboard
Number Name Explanation
11
Page change keys
(Page keys)
Two kinds of page change keys are described below.
12
Uppercase/lowercase
switch key
Press this key to switch between uppercase and lowercase when entering
alphabetic characters.
13
PC function key
These keys are used with the personal computer function of the 300i/300is,
310i/310is, 320i/320is.
Explanation
- 15” LCD/MDI soft key configuration
The 15” LCD panel has 12 soft keys horizontally and 9 soft keys
vertically.
As shown below, the 8 vertical soft keys and the lowermost key are
used as chapter selection soft keys. By pressing each of these keys,
the screen (chapter) belonging to each function can be selected. The
horizontal 12 soft keys are used to perform operations on the screen
selected with a vertical soft key.
For an LCD display with a touch panel, touch a soft key on the screen
to select it.
Vertical soft keys
Horizontal soft keys
Displays operations on selected chapter.
In this manual, the descriptions below assume a 10.4" LCD display
panel with 12 soft keys.
: This key is used to changeover the page on the screen in the forward
direction.
: This key is used to changeover the page on the screen in the reverse
direction.
2.OPERATIONAL DEVICES OPERATION B-63944EN/03
- 1008 -
- Key operation with multi-path control
In the multi-path control, be sure to select the tool post for which data
is specified, using the path selection switch on the machine operator's
panel. Then, perform keyboard operation, such as displaying or
specifying various data items, and editing a program.
B-63944EN/03 OPERATION 2.OPERATIONAL DEVICES
- 1009 -
2.3 FUNCTION KEYS AND SOFT KEYS
The function keys are used to select the type of screen (function) to be
displayed. When a soft key (section select soft key) is pressed
immediately after a function key, the screen (section) corresponding to
the selected function can be selected.
2.OPERATIONAL DEVICES OPERATION B-63944EN/03
- 1010 -
2.3.1 General Screen Operations
- Procedure
1 By pressing a function key on the MDI panel, the chapter
selection soft keys that belong to the function are displayed.
Example 1)
2 When one of the chapter selection soft keys is pressed, the screen
of the chapter is displayed. If the soft key of a desired chapter
is not displayed, press the continuous menu key.
In a chapter, a further choice may be made from multiple
chapters.
3 When the screen of a desired chapter is displayed, press the
operation selection key to display operations to be performed.
4 Select a desired operation with the operation selection soft key.
Depending on the operation to be executed, an auxiliary menu of
soft keys is displayed. Perform an operation according to the
indications on the auxiliary menu.
Example 2)
Example 3)
5 To return to the display of chapter selection soft keys, press the
return menu key.
A general screen display procedure is provided above.
The actual display procedure varies from one screen to another.
For details, see each description of operation.
Operation selection key
Continuous menu key
Chapter selection soft keys
Operation selection soft keys Return menu key
A
uxiliar
y
menu
B-63944EN/03 OPERATION 2.OPERATIONAL DEVICES
- 1011 -
- Button design change depending on soft key state
The soft keys assume one of the following states, depending on the
selection target:
• Chapter selection soft keys
• Operation selection soft keys
• Auxiliary menu of operation selection soft keys
Depending on the state, the button images of the soft keys change.
From the button images, which state the soft keys are assuming can be
known.
Example)
• Chapter selection soft keys
• Operation selection soft keys
• Auxiliary menu of operation selection soft keys
2.OPERATIONAL DEVICES OPERATION B-63944EN/03
- 1012 -
2.3.2 Function Keys
Function keys are provided to select the type of screen to be displayed.
The following function keys are provided on the MDI panel:
Press this key to display the position screen.
Press this key to display the program screen.
Press this key to display the offset/setting screen.
Press this key to display the system screen.
Press this key to display the message screen.
Press this key to display the graphics screen.
Press this key to display the custom screen 1 (conversational macro
screen or C language executor screen).
Press this key to display the custom screen 2 (conversational macro
screen or C language executor screen).
B-63944EN/03 OPERATION 2.OPERATIONAL DEVICES
- 1013 -
2.3.3 Soft Keys
By pressing a soft key after a function key, the corresponding screen
of the function can be displayed.
The chapter selection soft keys of each function are described below.
The horizontal four keys on the right-hand side are assigned to chapter
selection soft keys. When multiple pages are used for chapter
selection soft keys, [+] is displayed on the continuous menu key
(rightmost soft key). Press the continuous menu key to switch
between chapter selection soft keys.
NOTE
1 Press function keys to switch between screens that
are used frequently.
2 Some soft keys are not displayed depending on the
option configuration.
If position indications are provided on the left half of the screen when
a key other than the function key is pressed, the left half of the
soft keys is displayed as follows at all times:
2.OPERATIONAL DEVICES OPERATION B-63944EN/03
- 1014 -
Position display screen
The chapter selection soft keys that belong to the function key
and the function of each screen are described below.
ABS REL ALL HNDL (OPRT)
Page 1 +
(1) (2) (3) (4) (5)
MONI 3-D
MANUAL
(OPRT)
Page 2 +
(6) (7) (8) (9) (10)
Table 2.3.3 (a) Position display screen
No. Chapter menu Description
(1) ABS Selects the absolute coordinate display screen.
(2) REL Selects the relative coordinate display screen.
(3) ALL Selects the overall coordinate display screen.
(4) HNDL
Selects the operation screen for manual handle
operation.
(6) MONI Selects the screen for displaying the servo axis load
meter, serial spindle load meter, and speedometer.
(7) 3-D
MANUAL
Displays a handle pulse interrupt amount in
three-dimensional manual feed.
B-63944EN/03 OPERATION 2.OPERATIONAL DEVICES
- 1015 -
Program screen
The chapter selection soft keys that belong to the function key
and the function of each screen are described below.
PROGRA
M
FOLDER NEXT CHECK (OPRT)
Page 1 +
(1) (2) (3) (4) (5)
TIME JOG RSTR (OPRT)
Page 2 +
(6) (7) (8) (9) (10)
Table 2.3.3 (b) Program
No. Chapter menu Description
(1) PROGRAM Selects the screen for displaying a list of part
programs currently registered.
(2) FOLDER Selects the screen for displaying a list of part
programs currently registered.
(3) NEXT Selects the screen for displaying the command
values of the block currently executed and the next
block to be executed among the command values.
(4) CHECK Selects the screen for displaying programs, position
data, modal information, and so forth
simultaneously.
(6) TIME Selects the screen for displaying executed program
operation time.
(7) JOG Selects the screen for executing, in the JOG mode,
data specified in the program format from the MDI.
(8) RSTR Selects the operation screen for restarting an
interrupted program operation.
2.OPERATIONAL DEVICES OPERATION B-63944EN/03
- 1016 -
Offset/setting screen
The chapter selection soft keys that belong to the function key
and the function of each screen are described below.
OFFSET SETTING WORK (OPRT)
Page 1 +
(1) (2) (3) (4) (5)
MACRO OPR TOOL
MANAGER
(OPRT)
Page 2 +
(6) (7) (8) (9) (10)
OFST.2 W.SHFT GEOM.2 (OPRT)
Page 3 +
(11) (12) (13) (14) (15)
PR-LV EXTEND
OFFSET
(OPRT)
Page 4 +
CHUCK
TAIL LANG. PROTECT GUARD (OPRT)
Page 5 +
(16) (17) (18) (19) (20)
(21) (22) (23) (24) (25)
TOOL
LIFE (OPRT)
Page 6 ＋
(26) (27) (28) (29) (30)
WORK
SET ER (OPRT)
Page 7 ＋
(31) (32) (33) (34) (35)
B-63944EN/03 OPERATION 2.OPERATIONAL DEVICES
- 1017 -
Table 2.3.3 (c) Offset
No. Chapter menu Description
(1) OFFSET Selects the screen for setting tool offset values.
(2) SETTING Selects the screen for setting the setting
parameters.
(3) WORK Selects the screen for setting a workpiece
coordinate system offset.
(6) MACRO Selects the screen for setting macro variables.
(8) OPR Selects the screen for operating some operation
switches on the machine operator's panel as soft
switches.
(9) TOOL
MANAGER
Selects the screen for setting data related to tool
management.
(11) OFST.2 Selects the screen for setting a Y-axis offset.
(12) W.SHFT Selects the screen for setting a workpiece
coordinate system shift value.
(13) GEOM.2 Selects the screen for setting a second geometry
offset.
(17) PR-LV Selects the screen for setting a precision level.
(18) EXTEND
OFFSET
Selects the screen for setting the offsets of the
fourth and fifth axes.
(21) CHUCK TAIL Selects the chuck tail stock barrier screen.
(22) LANG. Selects the screen for setting a display language.
(23) PROTECT Selects the screen for setting data protection.
(24) GUARD Selects the screen for setting wrong operation
prevention.
(29) TOOL LIFE Selects the screen for operations and setting related
to tool life management.
(31) WRK ERR
COMP
Selects the screen for setting errors related to
workpiece mounting position.
2.OPERATIONAL DEVICES OPERATION B-63944EN/03
- 1018 -
System screen
The chapter selection soft keys that belong to the function key
and the function of each screen are described below.
PARAM DGNOS SERVO
GUIDEM SYSTEM (OPRT)
Page 1 +
(1) (2) (3) (4) (5)
MEMORY PITCH SERVO
PARAM SP.SET (OPRT)
Page 2 +
(6) (7) (8) (9) (10)
PMC
MAINTE
PMC
LADDER
PMC
CONFIG
Page 3 +
(11) (12) (13) (14) (15)
MCNG
TUNING
ALL IO OPEHIS (OPRT)
Page 4 +
COLOR MAINTE M-INFO W. DGNS (OPRT)
Page 5 +
(16) (17) (18) (19) (20)
(21) (22) (23) (24) (25)
FSSB PRMTUN P. M AT E
MGR. (OPRT)
Page 6 +
(26) (27) (28) (29) (30)
EMBED
PORT
PCMCIA
LAN
ETHNET
BOARD
PROFI
MASTER (OPRT)
Page 7 +
(31) (32) (33) (34) (35)
B-63944EN/03 OPERATION 2.OPERATIONAL DEVICES
- 1019 -
M CODE 3D ERR
COMP (OPRT)
Page 8 ＋
(36) (37) (38) (39) (40)
(OPRT)
Page 9 ＋
(41) (42) (43) (44) (45)
DUAL
CHECK
R.TIME
MACRO
(OPRT)
Page 10 ＋
(46) (47) (48) (49) (50)
Table 2.3.3 (d) System
No. Chapter menu Description
(1) PARAM Selects the screen for setting parameters.
(2) DGNOS Selects the screen for displaying CNC state.
(3) SERVO GUIDEM Selects the screen for displaying the servo guide mate.
(4) SYSTEM Selects the screen for displaying the current system
status.
(6) MEMORY Selects the screen for displaying the contents of
memory.
(7) PITCH Selects the screen for setting pith error compensation.
(8) SERVO PARAM Selects the screen for setting the servo-related
parameters.
(9) SP.SET Selects the screen for spindle-related setting.
(11) PMC MAINTE Selects the screen related to PMC maintenance such
as PMC signal state monitoring and tracing, and PMC
parameter display/editing.
(12) PMC LADDER Selects the screen related to ladder display/editing.
(13) PMC CONFIG Displays the screen for displaying/editing data other
than ladders that makes up a sequence program and
for setting the PMC function.
(16) MCNG TUNING Displays the screen for setting the parameter set for
emphasis on speed (LV1) or emphasis on precision
(LV10).
(18) ALL IO Selects the screen for data input to and output from the
memory card.
(19) OPEHIS Selects the screen for displaying the history of
operations performed by the operator and issued
alarms.
(21) COLOR Selects the screen for setting colors to be used on the
screen.
(22) MAINTE Selects the screen for setting maintenance items to be
managed periodically.
(23) M-INFO Selects the screen for displaying information about
maintenance performed.
2.OPERATIONAL DEVICES OPERATION B-63944EN/03
- 1020 -
No. Chapter menu Description
(24) W.DGNS Selects the screen for displaying data such as servo
positional deviation values, torque values, machine
signals, and so forth as graphs.
(27) FSSB Selects the screen for making settings related to the
high-speed serial servo bus (FSSB: Fanuc Serial Servo
Bus).
(28) PRMTUN Selects the screen for setting parameters necessary for
start-up and tuning.
(31) EMBED PORT Selects the screen for making settings related to the
embedded Ethernet (embedded port).
(32) PCMCIA LAN Selects the screen for making settings related to the
embedded Ethernet (PCMCIA Ethernet card).
(33) ETHNET BOARD Selects the screen for making settings related to the
fast Ethernet/fast data server.
(34) PROFI MASTER Selects the screen for making settings related to the
profibus master function.
(37) M CODE Selects the screen for setting an M code group.
B-63944EN/03 OPERATION 2.OPERATIONAL DEVICES
- 1021 -
Message screen
The chapter selection soft keys that belong to the function key
and the function of each screen are described below.
ALARM MSG HISTRY MSGHIS (OPRT)
Page 1 +
(1) (2) (3) (4) (5)
EMBED
LOG
PCMCIA
LOG
BOARD
LOG
(OPRT)
Page 2 +
(6) (7) (8) (9) (10)
Table 2.3.3 (e) Message
No. Chapter menu Description
(1) ALARM Selects the alarm message screen.
(2) MSG Selects the operator message screen.
(3) HISTRY Selects the screen for displaying the details of
alarms issued so far.
(4) MSGHIS Selects the external operator message screen.
(6) EMBED LOG Selects the screen for displaying error messages
related to the embedded Ethernet (embedded port).
(7) PCMCIA LOG Selects the screen for displaying error messages
related to the embedded Ethernet (PCMCIA
Ethernet card).
(8) BOARD LOG Selects the screen for displaying error messages
related to the fast Ethernet/fast data server.
2.OPERATIONAL DEVICES OPERATION B-63944EN/03
- 1022 -
Graphic screen
The chapter selection soft keys that belong to the function key
and the function of each screen are described below.
When the graphic display function is enabled:
PARAM GRAPH (OPRT)
Page 1 +
(1) (2) (3) (4) (5)
Table 2.3.3 (f) Graphic
No. Chapter menu Description
(1) PARAM Selects the screen for setting graphic parameters.
(2) GRAPH Selects the screen for graphically displaying the tool
path.
When the dynamic graphic display function is enabled:
DRAW
PARAM
PATH
EXEC
ANIME
EXEC
TOOL
POS
(OPRT)
Page 1
(1) (2) (3) (4) (5)
Table 2.3.3 (g) Graphic
No. Chapter menu Description
(1) DRAW
PARAM
Selects the screen for setting drawing parameters.
(2) PATH EXEC Selects the screen for drawing tool paths.
(3) ANIME
EXEC
Selects the screen for drawing animation.
(4) TOOL POS Selects the screen for displaying tool positions.
B-63944EN/03 OPERATION 2.OPERATIONAL DEVICES
- 1023 -
2.3.4 Key Input and Input Buffer
When an address and a numeric key are pressed, the character
corresponding to that key is input once into the key input buffer. The
contents of the key input buffer is displayed at the bottom of the
screen.
In order to indicate that it is key input data, a ">" symbol is displayed
immediately in front of it. A "_" is displayed at the end of the key
input data indicating the input position of the next character.
Fig. 2.3.4 (a) Key input buffer display
- Switching between upper and lower key characters
To input the lower character of the keys that have two characters
inscribed on them, first press the key and then the key in
question.
When the key is pressed, "_" indicating the next character
input position changes to "^". Now lowercase characters can be
entered (shift state).
When a character is input in shift status the shift status is canceled.
Furthermore, if the key is pressed in shift status, the shift status
is canceled.
It is possible to input up to 128 characters at a time in the key input
buffer.
Press the key to cancel a character or symbol input in the key
input buffer.
(Example)
When the key input buffer displays
>N001X100Z_
and the cancel key is pressed, Z is canceled and
>N001X100_
is displayed.
Key input buffer display
2.OPERATIONAL DEVICES OPERATION B-63944EN/03
- 1024 -
- Switching between uppercase and lowercase alphabetic characters
When entering alphabetic characters, the user can switch between
uppercase and lowercase.
By pressing the uppercase/lowercase switch key , the display of
the key input buffer changes to enable uppercase or lowercase
alphabetic characters to be entered as described below.
Example)
A> A B C _
State enabling uppercase input
a> a b c _
State enabling lowercase input
2.3.5 Warning Messages
After a character or number has been input from the MDI panel, a data
check is executed when key or a soft key is pressed. In the
case of incorrect input data or the wrong operation a flashing warning
message will be displayed on the status display line.
Fig. 2.3.5 (a) Warning message display
Table 2.3.5 (a) Warning Messages
Warning message Content
FORMAT ERROR The format is incorrect.
WRITE PROTECT Key input is invalid because of data protect
key or the parameter is not write enabled.
DATA IS OUT OF RANGE The input value exceeds the permitted range.
TOO MANY DIGITS The input value exceeds the permitted
number of digits.
WRONG MODE Parameter input is not possible in any mode
other than MDI mode.
EDIT REJECTED It is not possible to edit in the current CNC
status.
Key input buffer display
Soft key display
State display
Warning message display
B-63944EN/03 OPERATION 2.OPERATIONAL DEVICES
- 1025 -
2.4 EXTERNAL I/O DEVICES
External I/O devices such as a memory card are available.
By using an external I/O device such as a memory card, the following
data can be input or output:
1. Programs
2. Offset data
3. Parameters
4. Custom macro common variables
For how to input or output data and input data from or output it to a
memory card, see III-8.
- Parameter setting
Before an external input/output device can be used, parameters must
be set as follows.
Main board
Channel 1 Channel 2
JA56A JA36A
RS-232-C RS-232-C
Reader/
puncher
Reader/
puncher
I/O CHANNEL=0
o
r
I/O CHANNEL=1
I/O CHANNEL=2
CNC
This CNC has a total of two channels of reader/puncher interfaces. It
also has a memory card interface. The input/output device to be used
is specified by setting the channel (interface) connected to that device
in setting parameter I/O CHANNEL.
The specified data, such as a baud rate and the number of stop bits, of
an input/output device connected to a specific channel must be set in
parameters for that channel in advance. (These settings are not
required for the memory card interface.)
For channel 1, two combinations of parameters to specify the
input/output device data are provided.
The following shows the interrelation between the reader/puncher
interface parameters for the channels.
2.OPERATIONAL DEVICES OPERATION B-63944EN/03
- 1026 -
I/O CHANNEL
or foreground input
Set channels to be used
for data input/output.
I/O CHANNEL (0 to 5)
=0 : Channel 1
=1 : Channel 1
=2 : Channel 2
=3 : Channel 3
:
:
:
Input/output to and from the memory
card interface, etc. is also possible.
When IO4 is set
Foreground output
Background input
Background input
The channel setting is the same as
No.0020.
Input/output channel number (parameter No.0020)
↓
0101 Stop bit and other data
I/O CHANNEL=0 0102 Number specified for the input/output device
0103 Baud rate
0111 Stop bit and other data
I/O CHANNEL=1 0112 Number specified for the input/output device
0113 Baud rate
0121 Stop bit and other data
I/O CHANNEL=2 0122 Number specified for the input/output device
0123 Baud rate
:
:
:
I/O CHANNEL=5
(Channel 1)
(Channel 1)
(Channel 2)
0020
0021
0022
0023
B-63944EN/03 OPERATION 2.OPERATIONAL DEVICES
- 1027 -
2.5 POWER ON/OFF
2.5.1 Turning on the Power
Procedure of turning on the power
Procedure
1 Check that the appearance of the CNC machine tool is normal.
(For example, check that front door and rear door are closed.)
2 Turn on the power according to the manual issued by the
machine tool builder.
3 After the power is turned on, check that the position screen is
displayed. An alarm screen is displayed if an alarm occurs upon
power-on.
Fig. 2.5.1 (a) Position screen (for machining center system)
4 Check that the fan motor is rotating.
WARNING
Until the positional or alarm screen is displayed at
the power on, do not touch them. Some keys are
used for the maintenance or special operation
purpose. When they are pressed, unexpected
operation may be caused.
2.OPERATIONAL DEVICES OPERATION B-63944EN/03
- 1028 -
2.5.2 Power Disconnection
Procedure of power disconnection
Procedure
1 Check that the LED indicating the cycle start is off on the
operator's panel.
2 Check that all movable parts of the CNC machine tool is
stopping.
3 If an external input/output device such as the Handy File is
connected to the CNC, turn off the external input/output device.
4 Continue to press the <POWER OFF> button for about 5
seconds.
5 Refer to the machine tool builder's manual for turning off the
power to the machine.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1029 -
3 MANUAL OPERATION
MANUAL OPERATION are twelve kinds as follows :
3.1 MANUAL REFERENCE POSITION RETURN...................1030
3.2 JOG FEED (JOG)...................................................................1032
3.3 INCREMENTAL FEED.........................................................1034
3.4 MANUAL HANDLE FEED ..................................................1036
3.5 MANUAL ABSOLUTE ON AND OFF ................................1040
3.6 MANUAL LINEAR/CIRCULAR INTERPOLATION .........1046
3.7 RIGID TAPPING BY MANUAL HANDLE.........................1052
3.8 MANUAL NUMERICAL COMMAND................................1055
3.9 THREE-DIMENSIONAL MANUAL FEED.........................1064
3.10 DISTANCE CODED LINEAR SCALE INTERFACE..........1080
3.11 LINEAR SCALE WITH DISTANCE-CODED REFERENCE
MARKS (SERIAL) ................................................................1087
3.12 MANUAL HANDLE RETRACE ..........................................1093
3.13 AUXILIARY FUNCTION OUTPUT BLOCK REVERSE
MOVEMENT FOR MANUAL HANDLE RETRACE .........1108
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1030 -
3.1 MANUAL REFERENCE POSITION RETURN
The tool is returned to the reference position as follows :
The tool is moved in the direction specified in bit 5 (ZMI) of
parameter No.1006 for each axis with the reference position return
switch on the machine operator's panel. The tool moves to the
deceleration point at the rapid traverse rate, then moves to the
reference position at the FL speed. The rapid traverse rate and FL
speed are specified in parameters Nos. 1424,1421, and 1425.
Four step rapid traverse override is effective during rapid traverse.
When the tool has returned to the reference position, the reference
position return completion LED goes on. The tool generally moves
along only a single axis, but can move along three axes
simultaneously when specified so in bit 0 (JAX) of parameter
No.1002.
Deceleration point Reference position
Rapid traverse motion
Rapid traverse rate
(rapid traverse
override is effective)
Decelerated motion
FL speed
Fig. 3.1 (a) Manual reference position return
Procedure for manual reference position return
Procedure
1 Press the reference position return switch, one of the mode
selection switches.
2 To decrease the feedrate, press a rapid traverse override switch.
3 Press the feed axis and direction selection switch corresponding
to the axis and direction for reference position return. Continue
pressing the switch until the tool returns to the reference position.
The tool can be moved along three axes simultaneously when
specified so in an appropriate parameter setting. The tool moves
to the deceleration point at the rapid traverse rate, then moves to
the reference position at the FL speed set in a parameter. When
the tool has returned to the reference position, the reference
position return completion LED goes on.
4 Perform the same operations for other axes, if necessary.
The above is an example. Refer to the appropriate manual provided by
the machine tool builder for the actual operations.
X
MIRRR
O
R IMA
G
E
Y Z
C
X2 Y2 Z2
X
Y Z
PROGRAM
STOP
M02/
M30
MANU
ABS
SPINDLE
ORI TAP
ATC
READY N
C
?M
C
?
ZERO POSITION
Fig. 3.1 (b)
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1031 -
Explanation
- Automatically setting the coordinate system
Bit 0 (ZPR) of parameter No.1201 is used for automatically setting the
coordinate system. When ZPR is set, the coordinate system is
automatically determined when manual reference position return is
performed.
When α, β and γ are set in parameter 1250, the workpiece coordinate
system is determined so that reference point on the tool holder or the
position of the tip of the reference tool is X= α, Y = β, Z = γ when
reference position return is performed. This has the same effect as
specifying the following command for reference position return:
G92XαYβZγ;
However, when options of the workpiece coordinate system is
selected, it is not able to use.
Limitation
- Moving the tool again
Once the reference position return completion LED lights at the
completion of reference position return, the tool does not move unless
the reference position return switch is turned off.
- Reference position return completion LED
The reference position return completion LED is extinguished by
either of the following operations:
• Moving from the reference position.
• Entering an emergency stop state.
- The distance to return to reference position
For the distance (Not in the deceleration condition) to return the tool
to the reference position, refer to the manual issued by the machine
tool builder.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1032 -
3.2 JOG FEED (JOG)
In the jog mode, pressing a feed axis and direction selection switch on
the machine operator's panel continuously moves the tool along the
selected axis in the selected direction.
The jog feedrate is specified in a parameter No.1423.
The jog feedrate can be adjusted with the jog feedrate override dial.
Pressing the rapid traverse switch moves the tool at the rapid traverse
feedrate No. 1424 regardless of the position of the jog feedrate
override dial. This function is called the manual rapid traverse.
Manual operation is allowed for one axis at a time. 3 axes can be
selected at a time by bit 0 (JAX) of parameter No.1002.
While a switch is pressed, the tool
moves in the direction specified by
the switch.
Z
X
Y
Fig. 3.2 (a) Jog Feed (JOG)
Procedure for JOG feed
Procedure
1 Press the jog switch, one of the mode selection switches.
2 Press the feed axis and direction selection switch corresponding
to the axis and the direction where the tool is to be moved. While
the switch is pressed, the tool moves at the feedrate specified in
the parameter No. 1423. The tool stops when the switch is
released.
3 The jog feedrate can be adjusted with the jog feedrate override
dial.
4 Pressing the rapid traverse switch while pressing a feed axis and
direction selection switch moves the tool at the rapid traverse rate
while the rapid traverse switch is pressed. Rapid traverse
override by the rapid traverse override switches is effective
during rapid traverse.
The above is an example. Refer to the appropriate manual provided
by the machine tool builder for the actual operations.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1033 -
Explanation
- Manual per revolution feed
The manual per revolution feed is enabled for jog feed by setting bit 4
(JRV) of parameter No.1402.
During the manual per revolution feed, the tool is jogged at the
feedrate that is obtained by multiplying the spindle speed by the feed
amount per revolution, which is calculated by multiplying the jog
feedrate override value by the feed amount per revolution specified
with the parameter (No. 1423).
During manual per revolution feed, the tool is jogged at the following
feedrate:
Feed distance per rotation of the spindle (mm/rev) (specified with
parameter No. 1423) × JOG feedrate override × actual spindle speed
(rev/min).
Limitation
- Acceleration/deceleration for rapid traverse
Feedrate, time constant and method of automatic acceleration/
deceleration for manual rapid traverse are the same as G00 in
programmed command.
- Change of modes
Changing the mode to the jog mode while pressing a feed axis and
direction selection switch does not enable jog feed. To enable jog feed,
enter the jog mode at first, then press a feed axis and direction
selection switch.
- Rapid traverse prior to reference position return
If reference position return is not performed after power-on, pushing
rapid traverse button does not actuate the rapid traverse but the
remains at the JOG feedrate. This function can be disabled by setting
bit 0 (RPD) of parameter No.1401.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1034 -
3.3 INCREMENTAL FEED
In the incremental (INC) mode, pressing a feed axis and direction
selection switch on the machine operator's panel moves the tool one
step along the selected axis in the selected direction. The minimum
distance the tool is moved is the least input increment. Each step can
be 10, 100, or 1000 times the least input increment.
With using bit 2 (HNT) of parameter No. 7103, each step can be
additionally 10 times the lest input increment.
The feedrate set in parameter No. 1423 is applied.
By using the manual feedrate override signal, the feedrate can be
increased or decreased.
The tool can also be moved at the rapid traverse rate by using the
manual rapid traverse selection signal, independent of the manual
feedrate override signal.
Y
X
Z
Tool Each time a switch is
pressed, the tool moves one
step in the direction
specified by the switch.
Fig. 3.3 (a) Incremental feed
Procedure for incremental feed
Procedure
1 Press the INC switch, one of the mode selection switches.
2 Select the distance to be moved for each step with the
magnification dial.
3 Press the feed axis and direction selection switch corresponding
to the axis and direction the tool is to be moved. Each time a
switch is pressed, the tool moves one step. The feedrate is the
same as the jog feedrate.
4 Pressing the rapid traverse switch while pressing a feed axis and
direction selection switch moves the tool at the rapid traverse
rate.
Rapid traverse override by the rapid traverse override switch is
effective during rapid traverse.
The above is an example. Refer to the appropriate manual provided by
the machine tool builder for the actual operations.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1035 -
Explanation
- Travel distance specified with a diameter
T
The distance the tool travels along the X-axis can be specified with a
diameter.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1036 -
3.4 MANUAL HANDLE FEED
In the handle mode, the tool can be minutely moved by rotating the
manual pulse generator on the machine operator's panel. Select the
axis along which the tool is to be moved with the handle feed axis
selection switches.
The minimum distance the tool is moved when the manual pulse
generator is rotated by one graduation is equal to the least input
increment. One of four types of magnifiers selected with the manual
handle feed move distance select signal can be applied. With bit 2
(HNT) of parameter No. 7103, the minimum distance can be further
10 times greater.
The number of manual pulse generators depends on the option as
follows:
• Control on 1 manual handle: Up to 1
• Control on 2 or 3 manual handles:
Up to 3 (Up to three manual pulse generators can be moved at a
time.)
• Control on 2 to 5 manual handles:
Up to 5 (Up to five manual pulse generators can be moved at a
time.)
Manual pulse generator
Z
X
Y
Fig. 3.4 (a) Manual handle feed
Procedure for manual handle feed
Procedure
1 Press the handle switch, one of the mode selection switches.
2 Select the axis along which the tool is to be moved by pressing a
handle feed axis selection switch.
3 Select the magnification for the distance the tool is to be moved
by pressing a handle feed magnification switch. The minimum
distance the tool is moved when the manual pulse generator is
rotated by one graduation is equal to the least input increment.
4 Move the tool along the selected axis by rotating the handle.
Rotating the handle 360 degrees moves the tool the distance
equivalent to 100 graduations.
The above is an example. Refer to the appropriate manual provided by
the machine tool builder for the actual operations.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1037 -
Explanation
- Availability of manual pulse generator in Jog mode (JHD)
Bit 0 (JHD) of parameter No.7100 enables or disables the manual
handle feed in the JOG mode.
When bit 0 (JHD) of parameter No.7100 is set 1,both manual handle
feed and incremental feed are enabled.
- Manual handle feed in TEACH IN JOG mode (THD)
By setting bit 1 (THD) of parameter No. 7100, manual handle feed in
TEACH IN JOG mode can be enabled or disabled.
- When manual handle feed exceeding the rapid traverse rate is specified
The amount of pulses exceeding the rapid traverse rate can be saved
by CNC as B. And amount of pulses B will be output as pulses C.
ｔ
Rapid
traverse
rate
A
: Amount of pulses corresponds to value o
f
Rapid Traverse Rate.
B: Amount of pulses accumulated in CNC.
C: Amount of pulses the same as B.
A
B
C
Fig. 3.4 (b) Amount of pulses output by CNC in Manual Handle Feed
Amount of pulses B is calculated in 2 cases as following:
In case of
1) Parameter No.7117 = 0
The feedrate is clamped at the Rapid Traverse Rate and
generated pulses exceeding the Rapid Traverse Rate are
ignored (B=0).
In case of
2) Parameter No.7117 > 0
The feedrate is clamped as the Rapid Traverse Rate, but the
pulses exceeding the Rapid Traverse Rate is not ignored. Amount
of pulses accumulated in CNC is calculated as following.
(Although the rotation of manual pulse generator is stopped, if
there is pulses accumulated in CNC, it will be output and the tool
will move as long as amount of it.)
Magnification set by MP1，MP2<Gn019.4,5> is m, value of
parameter No.7117 is n.
n < m: Clamping is set performed at value of parameter
No.7117.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1038 -
n ≥ m: Amount A+B, shown in figure, which’s value is
multiple of m and small than n. As a result, clamping is
performed as an integral multiple of the selected
magnification.
n
ｍ
A
B
Pulses over (k⋅m) will be ignored
A
: Amount of pulses the same
as Rapid Traverse Rate.
B: Amount of pulses saved in
CNC.
k : Integer number
A＋B=k⋅m
Fig. 3.4 (c) Amount of pulses exceeding the Rapid Traverse Rate
(n ≥ m)
NOTE
Due to change of mode, clamping can be
performed not as an integral multiple of the
selected magnification.
The distance the tool moves may not match the
graduations on the manual pulse generator.
- Upper feedrate limit in manual handle feed
The upper feedrate limit depends on the input signal (maximum
manual handle feedrate switch signal HNDLF) from the PMC as
follows:
• When HNDLF is set to 0, the feedrate is clamped to the manual
rapid traverse rate (parameter No. 1424).
• When HNDLF is set to 1, the feedrate is clamped to the feedrate
set in parameter No. 1434.
- Movement direction of an axis to the rotation of MPG (HNGx)
Bit 0 (HNGx) of parameter No 7102 switches the direction of MPG in
which the tool moves along an axis, corresponding to the direction in
which the handle of the manual pulse generator is rotated.
This parameter is valid only for the following functions:
• Manual handle feed
• Manual handle interruption
Limitation
WARNING
Rotating the handle quickly with a large
magnification such as ×100 moves the tool too fast.
The feedrate is clamped at the rapid traverse
feedrate.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1039 -
NOTE
Rotate the manual pulse generator at a rate of five
rotations per second or lower. If the manual pulse
generator is rotated at a rate higher than five
rotations per second, the tool may not stop
immediately after the handle is no longer rotated or
the distance the tool moves may not match the
graduations on the manual pulse generator.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1040 -
3.5 MANUAL ABSOLUTE ON AND OFF
Whether the distance the tool is moved by manual operation is added
to the coordinates can be selected by turning the manual absolute
switch on or off on the machine operator's panel. When the switch is
turned on, the distance the tool is moved by manual operation is added
to the coordinates. When the switch is turned off, the distance the tool
is moved by manual operation is not added to the coordinates.
O
P1
P2
Y axis
X axis
Manual operation
The coordinates values change by the
amount of manual operation.
Fig. 3.5 (a) Coordinates with the switch ON
The coordinates do not change.
X2
X1
Y1
Y2
P1
P2
O1
O2
Fig. 3.5 (b) Coordinates with the switch OFF
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1041 -
Explanation
The following describes the relation between manual operation and
coordinates when the manual absolute switch is turned on or off, using
a program example.
G01G90 X100.0Y100.0F010 ; <1>
X200.0Y150.0 ; <2>
X300.0Y200.0 ; <3>
Fig. 3.5 (c) Program example
The subsequent figures use the following notation:
Movement of the tool when the switch is on
Movement of the tool when the switch is off
The coordinates after manual operation include the distance the tool is
moved by the manual operation. When the switch is off, therefore,
subtract the distance the tool is moved by the manual operation.
- Manual operation after the end of block
Coordinates when block <1> has been executed after manual
operation (X-axis +20.0, Y-axis +100.0) at the end of movement of
block <2>.
X
Y
Switch ON
Switch OFF
Manual
operation
(100.0 , 100.0)
(200.0 , 150.0)
(120.0 , 200.0)
(220.0 , 250.0)
Fig. 3.5 (d) Manual operation after the end of block
- Manual operation after a feed hold
Coordinates when the feed hold button is pressed while block <2> is
being executed, manual operation (Y-axis + 75.0) is performed, and
the cycle start button is pressed and released.
X
Y
Switch ON
Switch OFF
Manual
operation
(150.0 , 125.0)
(200.0 , 150.0)
(150.0 , 200.0)
(200.0 , 225.0)
(300.0 , 275.0)
(300.0 , 200.0)
Feed hold stop point
Fig. 3.5 (e) Manual operation after a feed hold
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1042 -
- When reset after a manual operation following a feed hold
Coordinates when the feed hold button is pressed while block <2> is
being executed, manual operation (Y-axis +75.0) is performed, the
control unit is reset with the RESET button, and block <2> is read
again.
X
Y
Switch ON
Switch OFF
Manual
operation
(150.0 , 125.0)
(200.0 , 150.0)
(150.0 , 200.0)
(200.0 , 225.0)
(300.0 , 275.0)
(300.0 , 200.0)
Feed hold stop point
Fig. 3.5 (f) When reset after a manual operation following a feed hold
- When a movement command in the next block is only one axis
When there is only one axis in the following command, only the
commanded axis returns.
Program
N1 G90 G01 X100. Y100. F500 ;
N2 X200.0 ;
N3 Y150.0 ;
X
Y
Switch ON
Switch OFF
Manual
operation
(100.0 , 100.0)
(200.0 , 150.0)
(200.0 , 100.0)
N1
N2
N3
Fig. 3.5 (g) When a movement command in the next block is only one
axis
- When the next move block is an incremental
When the following commands are incremental commands, operation
is the same as when the switch is OFF.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1043 -
- Manual operation during cutter or tool nose radius compensation
• When the switch is OFF
After manual operation is performed with the switch OFF during
cutter or tool nose radius compensation, automatic operation is
restarted then the tool moves parallel to the movement that would
have been performed if manual movement had not been
performed.
The amount of separation equals to the amount that was
performed manually.
• When the switch is ON during cutter or tool nose radius
compensation
Operation of the machine upon return to automatic operation
after manual intervention with the switch is ON during execution
with an absolute command program in the cutter or tool nose
radius compensation mode will be described. The vector created
from the remaining part of the current block and the beginning of
the next block is shifted in parallel. A new vector is created
based on the next block, the block following the next block and
the amount of manual movement. This also applies when manual
operation is performed during cornering.
• Manual operation performed in other than cornering
Assume that the feed hold was applied at point PH while moving
from PA to PB of programmed path PA, PB, and PC and that the
tool was manually moved to PH'. The block end point PB moves
to the point PB' by the amount of manual movement, and vectors
VB1 and VB2 at PB also move to VB1' and VB2'. Vectors VC1 and
VC2 between the next two blocks PB - PC and PC - PD are
discarded and new vectors VC1' and VC2' (VC2' = VC2 in this
example) are produced from the relation between PB' - PC and PC
- PD. However, since VB2' is not a newly calculated vector,
correct offset is not performed at block PB' - PC. Offset is
correctly performed after PC.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1044 -
• Manual operation during cornering
This is an example when manual operation is performed during
cornering. VA2', VB1', and VB2' are vectors moved in parallel with
VA2, VB1 and VB2 by the amount of manual movement. The new
vectors are calculated from VC1 and VC2. Then correct cutter or
tool nose radius compensation is performed for the blocks
following PC.
• Manual operation after single block stop
Manual operation was performed when execution of a block was
terminated by single block stop.
Vectors VB1 and VB2 are shifted by the amount of manual
operation. Sub-sequent processing is the same as case a described
above. An MDI operation can also be intervened as well as
manual operation. The movement is the same as that by manual
operation.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1045 -
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1046 -
3.6 MANUAL LINEAR/CIRCULAR INTERPOLATION
In manual handle feed or jog feed, the following types of feed
operations are possible along with the conventional feed operation
with simultaneous single-axis control (for X, Y, Z, or other axis).
• Feed along a tilted straight line in the XY, YZ, or ZX plane
based on simultaneous 2-axis control (linear feed)
• Feed along a circle in the XY, YZ, or ZX plane based on
simultaneous 2-axis control (circular feed)
NOTE
1 Two control axes should be included in the three
standard axes.
2 In the following, only the case of the XY plane is
described. If any other plane is used, replace XY
with YZ or ZX. (Refer to the table below.)
XY plane YZ plane ZX plane
X Y Z
Y Z X
Tool
Workpiece
Tool
Workpiece
<Linear feed> <Circular feed>
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1047 -
Explanations
Procedure
1 For manual handle feed, select the manual handle feed mode.
For jog feed, select the jog feed mode.
2 For manual handle feed, use the handle feed axis selection switch
to select the feed axis (simultaneous 1-axis feed in the X-, Y-, or
Z-axis or simultaneous 2-axes feed of the X- and Y-axes along a
specified line or circle) used when the manual handle is turned.
For jog feed, use the feed axis direction selection switch to select
the feed axis and its direction. The tool moves at the feedrate
(jog feedrate) set in parameter No. 1423 in the specified axis
direction or along the specified line or circle while the feed axis
and its direction are selected.
3 For the manual handle, the tool moves in the specified axis
direction when the manual handle is turned. The feedrate
depends on the rotation speed of the manual handle. The
amount of movement when the manual handle is turned for one
pulse can be selected by the manual handle feed movement scale
switch.
For jog feed, the manual feedrate override dial can be used to
override the feedrate.
The above procedure is an example. For actual operation, refer to
the manual provided by the machine tool builder.
- Line/circle definition
A line or circle definition is not required for axis direction feed. For
linear or circular feed, however, a line or circle must be defined.
(For example, in the case of circular feed, the center and radius of the
circle must be specified.)
Refer to the manual provided by the machine tool builder.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1048 -
- Manual handle feed
In manual handle feed, the tool can be moved along a specified axis
(X-axis, Y-axis, Z-axis, or Nth-axis), along a rotated straight line
(linear feed), or along a circle (circular feed).
(1) Feed along a specified axis (simultaneous 1-axis control)
A single manual handle operation can move the tool along the
desired axis, such as X-axis, Y-axis, or Z-axis, on a simultaneous
1-axis control basis.
Y
X
Path of travel using the Y-axis handle
Path of travel using the X-axis handle
Feed along a specified axis
(2) Linear feed (simultaneous 2-axis control)
A single manual handle operation can move the tool in parallel to
the straight line on a simltaneous 2-axis control basis. This
manual handle is referred to as the "guidance handle". Also, the
tool can be moved at right angles to a specified straight line on a
simultaneous 2-axis control basis. This manual handle is
referred to as the "approach handle". When the guidance handle
or approach handle is turned clockwise or counterclockwise, the
tool travels forward or backward along the respective path.
Y
X
Path of travel using the
approach handle
Path of travel using the
guidance handle
Specified straight line
Tool
Linear feed
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1049 -
(3) Circular feed (simultaneous 2-axis control)
A single manual handle operation can move the tool from the
current position along a concentric circle that has the same center
as a specified circle on a simultaneous 2-axis control basis.
This manual handle is referred to as the guidance handle. Also,
a single manual handle operation can move the tool along a
straight line normal to a specified circle on simultaneous 2-axis
control. This manual handle is refrred to as the approach handle.
When the guidance handle or approach handle is turned
clockwise or counterclockwise, the tool travels forward or
backward along the respective path.
Y
X
Specified circle
Path of travel using the
guidance handle
Path of travel using the
approach handle
Tool
Circular feed
- Feedrate for manual handle feed
The feedrate depends on the speed at which a manual handle is turned.
The distance to be traveled by the tool (along a tangent in the case of
linear or circular feed) per manual handle pulse can be selected using
the manual handle feed travel distance magnification switch.
The approach handle clamp feedrate can be set using parameter No.
7160. The guidance handle clamp feedrate can be set using
parameter No. 7161.
- Manual handle selection
Up to five manual handles to be connected. For information on
specifying the usage of the manual handle connected to each interface
(for feed in the axis direction, use as a guidance handle, or use as an
approach handle), refer to the manual issued by the machine tool
builder.
- Direction of movement using manual handles
When the tool is moved along a straight line or circle using the
guidance handle or approach handle, the direction of the tool
movement (for example, whether to make a clockwise or
counterclockwise movement along a circle) when the handle is turned
clockwise or counterclockwise can be specified.
Refer to the manual provided by the machine tool builder.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1050 -
- Jog feed
In jog feed, the tool can be moved along a specified axis (X-axis,
Y-axis, Z-axis, etc.), along a rotated straight line (linear feed), or
along a circle (circular feed).
(1) Feed along a specified axis (simultaneous 1-axis control)
While a feed axis and its direction are specified with the feed
axis direction selection switch, the tool moves in the specified
axis direction at the feedrate specified in parameter No. 1423.
The feedrate can be overriden using the manual feedrate override
dial.
(2) Linear feed (simultaneous 2-axis control)
By defining a straight line, the tool can be moved as follows:
• While a feed axis and its direction are selected using the
feed axis direction selection switch, the tool moves along a
straight line parallel to the specified straight line on a
simultaneous 2-axis control basis.
• While a feed axis and its direction are selected using the
feed axis direction selection switch, the tool moves along a
straight line perpendicular to the specified staight line on a
simultaneous 2-axis control basis.
The feedrate in the tangential direction is specified in parameter
No. 1410.
The feedrate can be overridden using the manual feedrate
override dial.
(3) Circular feed (simultaneous 2-axis control)
By defining a circle, the tool can be moved as follows:
• While a feed axis and its direction are selected using the
feed axis direction selection switch, the tool moves from the
current position along the concentric circle that has the
same center as the specified circle.
• While a feed axis and its direction are selected using the
feed axis direction selection switch, the tool moves along a
straight line normal to the specified circle.
The feedrate in the tangential direction is specified in parameter
No. 1410. The feedrate can be overridden using the manual
feedrate override dial.
- Manual handle feed in JOG mode
Even in JOG mode, manual handle feed can be enabled using bit 0
(JHD) of parameter No. 7100. In this case, however, manual handle
feed is enabled only when the tool is not moved using jog feed.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1051 -
Limitations
- Mirror image
The mirror image function is not available during the manual
operation. (The manual operation can be executed when the mirror
image switch is off and the mirror image setting is off.)
NOTE
If the tool is operated with the mirror image
function activated, the normal operation will not be
guaranteed.
- Rotation direction
When this function is effective, bit 0 (HNGx) of parameter No. 7102
is invalid which is used to change the axis movement direction with
respect to the rotation direction of the manual pulse generator. (The
rotation direction of the manual pulse generator is always the same as
the axis movement direction; that is, the operation is the same as when
bit 0 of parameter No. 7102 is set to "0".)
- The amount of the shift for manual handle feed
When this function is effective, parameters No. 12350 and No. 12351
used to determine the magnification of manual handle feed for each
axis are invalid and the values of parameter No. 7113 and No. 7114
are used. (Parameters No. 7131 and No. 7132 are used for the
second manual pulse generator, parameters No. 7133 and No. 7134 for
the third, parameters No. 7135 and No. 7136 for the fourth, and
parameters No. 7137 and No. 7138 for fifth.)
- Incremental feed
This function is invalid for the incremental feed.
- Synchronous/composite control
If the axis is set as the synchronous/composite control axis, this
function is invalid.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1052 -
3.7 RIGID TAPPING BY MANUAL HANDLE
For execution of rigid tapping, set rigid mode, then switch to handle
mode and move the tapping axis with a manual handle. For rigid
tapping, refer to Section 4.4 in Part II of the User's Manual (T series)
or Section 5.2 in Part II of the User's Manual (M series) and the
relevant manual of the machine tool builder.
Rigid tapping by manual handle
Procedure
1 Stop the spindle and servo axes, then set MDI mode by pressing
the MDI switch among the mode selection switches.
2 Enter and execute the following program:
Example 1) M series / T series (G code systems B, C)
M29 S100 ;
G91 G84 Z0 F1000 ;
Example 2) T series (G code system A)
M29 S100 ;
G84 W0 F1000 ;
The program above is required to determine a screw lead and set
rigid tapping mode. In this program, a tapping axis must always
be specified. Specify a value that does not operate the tapping
axis. With the M series, specify G84 (G74). With the T series,
specify G84 (G88).
WARNING
In this MDI programming, never specify commands
to position the tool at a drilling position and at point
R. Otherwise, the tool moves along an axis.
3 When the entered program is executed, rigid tapping mode is set.
4 After rigid mode is set upon completion of MDI program
execution, switch to the handle mode by pressing the handle
switch among the mode selection switches.
CAUTION
At this time, never press the reset key. Otherwise,
rigid mode is canceled.
5 To perform rigid tapping, select a tapping axis with the handle
feed axis select switch, and move the tapping axis with the
manual handle.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1053 -
Explanation
- Manual rigid tapping
Manual rigid tapping is enabled by parameter HRG (No. 5203#0) to 1.
- Cancellation of rigid mode
To cancel rigid mode, specify G80 as same the normal rigid tapping.
When the reset key is pressed, rigid mode is canceled, but the canned
cycle is not canceled.
When the rigid mode switch is to be set to off for rigid mode
cancellation (when parameter CRG (No. 5200#2) is set to 0), the G80
command ends after the rigid mode switch is set to off.
- Spindle rotation direction
The rotation direction of the spindle is determined by a specified
tapping cycle G code and the setting of parameter HRM (No. 5203#1).
For example, when the HRM parameter is set to 0 in G84 mode, the
spindle makes forward rotations as the tapping axis moves in the
minus direction. (When the tapping axis moves in the plus direction,
the spindle makes reverse rotations.)
- Arbitrary tapping axis
With the M series, an arbitrary tapping axis can be selected by setting
bit 0 (FXY) of parameter No. 5101 to 1. With the T series, an
arbitrary tapping axis can be selected not by using bit 0 (FXY) of
parameter No. 5101 (but by using bit 0 (FXY) of parameter No. 5101
when the FS15 format is specified). In this case, specify a G code
for plane selection and the address of the tapping axis when setting the
rigid tapping mode in the MDI mode.
- G84 command/same block specifying both M29 and G84
As the MDI program command for setting the rigid mode, G84 can be
specified as a rigid tapping G code (by setting bit 0 (G84) of
parameter No. 5200 to 1), or M29 and G84 can be specified in the
same block.
Example 1: G91 G84 Z0 F1000 S100 ;
Example 2: G91 G84 Z0 F1000 M29 S100 ;
- Specification of manual handle feed faster than the rapid traverse rate
Set parameter (No.7117) to 0 so that when manual handle feed is
specified which is faster than the rapid traverse rate, the handle pulses
beyond the rapid traverse rate are ignored.
- Series 15 format command
By setting bit 1 (FCV) of parameter No. 0001 to 1, the Series15
format can be used for specification.
Example 1: G91 G84.2(G84.3) Z0 F1000 S100; (M series)
Example 2: G84.2 W0 F1000 S100; (T series : G code systems A)
Example 3: G91 G84.2 Z0 F1000 S100; (T series : G code system B,
C)
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1054 -
- Acceleration/deceleration type
When manual rigid tapping is executed, the acceleration/deceleration
type and acceleration/deceleration time constant set in the rigid
tapping parameters are valid.
The same settings are valid also for extraction.
- In the case of multi-spindle operation
In the case of multi-spindle operation, a spindle can be selected by
specifying a P command as well as an S command.
Example : When the 2nd spindle is selected:
M29 S100 P2;
G91 G84 Z0 F1000 ;
Limitation
- Excessive error check
In manual rigid tapping, only an excessive error during movement is
checked.
- Tool axis direction handle feed
Tool axis direction handle feed is disabled.
- Extraction override
In manual rigid tapping, the extraction override function is disabled,
and the use of an acceleration/deceleration time constant for extraction
is disabled.
- Number of repeats
In MDI programming, never specify K0 and L0, which are used to
specify that the number of repeats is 0 and to disable the execution of
a G84 block. If K0 or L0 is specified, rigid mode cannot be set.
- Positioning of the tool to a drilling position
When positioning the tool to a drilling position, select the X-axis or
Y-axis with the axis select switch in handle mode. Never use the
method of positioning to a drilling position in MDI mode or MEM
mode. The method can operate the tapping axis.
- Three-dimensional rigid tapping
Three-dimensional rigid tapping cannot be used in rigid tapping using
the manual handle.
- Interpolation type rigid tapping
Interpolation type rigid tapping cannot be used in rigid tapping using
the manual handle. To perform rigid tapping using the manual
handle, select the conventional type of rigid tapping with bit 3 (CHR)
of parameter No. 5202.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1055 -
3.8 MANUAL NUMERICAL COMMAND
The manual numerical command function allows data programmed
through the MDI to be executed in jog mode. Whenever the system
is ready for jog feed, a manual numerical command can be executed.
The following eight functions are supported:
(1) Positioning (G00)
(2) Linear interpolation (G01)
(3) Automatic reference position return (G28)
(4) 2nd/3rd/4th reference position return (G30)
(5) M codes (miscellaneous functions)
(6) S codes (spindle speed functions)
(7) T codes (tool functions)
(8) B codes (second auxiliary functions)
By setting the following parameters, the commands for axial motion
and the M, S, T, and B functions can be disabled:
(1) Positioning (G00): .........................Parameter JAXx (No. 7010#0)
(2) Linear interpolation (G01):............Parameter JAXx (No. 7010#0)
(3) Automatic reference position return (G28):
.......................................Parameter JAXx (No. 7010#0)
(4) 2nd/3rd/4th reference position return (G30):
.......................................Parameter JAXx (No. 7010#0)
(5) M codes (miscellaneous functions): Parameter JMF (No. 7002#0)
(6) S codes (spindle speed functions):.... Parameter JSF (No. 7002#1)
(7) T codes (tool functions):................... Parameter JSF (No. 7002#2)
(8) B codes (second auxiliary functions):Parameter JBF (No. 7002#3)
Procedure Manual numerical command
Procedure
1 Press the jog switch (one of the mode selection switches).
2 Press function key .
3 Press soft key [JOG] on the screen. The following manual
numerical command screen is displayed.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1056 -
Fig. 3.8 (a) Manual numerical command screen
The remaining portion of the axis information currently not
shown on the screen can be displayed by pressing the or
key.
NOTE
1 The actual feedrate (F) and the actual spindle speed
(S) are displayed only for 9” window.
2 If two or more identical axis names exist for the
same path, they are not displayed.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1057 -
4 Enter the required commands by using address keys and numeric
keys on the MDI panel, then press soft key [INPUT] or the
key to set the entered data.
Fig. 3.8 (b) Example of inputting numerical value
The following data can be set:
1. G00: ................ Positioning
2. G01: ................ Linear interpolation
3. G28: ................ Automatic reference position return
4. G30: ................ 2nd/3rd/4th reference position return
5. M codes: ......... Miscellaneous functions
6. S codes:........... Spindle speed functions
7. T codes:........... Tool functions
8. B codes: .......... Second auxiliary functions
The set data is maintained even when the screen or mode is changed.
NOTE
When an alarm state exists, data cannot be set.
5 Press the cycle start switch on the machine operator's panel to
start command execution. The status is indicated as "MSTR."
The automatic operation signal, STL, can be turned on by setting
bit 2 (JST) of parameter No.7001.
NOTE
If the cycle start switch is pressed while an alarm
state exists, a "START REJECTED (ALARM
EXISTED)" warning is generated, and the entered
data cannot be executed.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1058 -
6 Upon the completion of execution, the "MSTR" status indication
is cleared from the screen, and automatic operation signal STL is
turned off. The set data is cleared entirely. G codes are set to G00
or G01 according to the setting of parameter G01 (No.3402#0).
Explanation
- Positioning
An amount of travel is given as a numeric value, preceded by an
address such as X, Y, or Z. This is always regarded as being an
incremental command, regardless of whether G90 or G91 is specified.
Manual rapid traverse selection switch
Off On
Feedrate
(parameter)
Jog feedrate for each axis
(No.1423)
Rapid traverse rate for each axis
(No.1420)
Automatic
acceleration/
deceleration
(parameter)
Exponential acceleration/
deceleration in jog feed for each axis
(No.1624)
Linear acceleration/deceleration
in rapid traverse for each axis
(No.1620)
Override Manual feed override Rapid traverse override
NOTE
1 When the manual rapid traverse switch is off, the
feedrate is clamped so that the axis-by-axis manual
rapid traverse rate (parameter No. 1424) is not
exceeded.
2 The tool cannot move if linear interpolation type
positioning (where the tool path is linear) has been
performed by setting bit 1 (LRP) of parameter No.
1401.
- Linear interpolation (G01)
An amount of travel is given as a numeric value, preceded by an
address such as X, Y, or Z. This is always regarded as being an
incremental command, regardless of whether G90 or G91 is specified.
Axial movements are always performed in incremental mode even
during scaling or polar coordinate interpolation. In addition,
movement is always performed in feed per minute mode regardless of
the specification of G94 or G95.
Feedrate
(parameter)
Dry run feedrate
(No. 1410)
Automatic acceleration/deceleration
(parameter)
Exponential acceleration/deceleration
in cutting feed for each axis
(No.1622)
Override Manual feed override
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1059 -
NOTE
Since the feedrate is always set to the dry run
feedrate, regardless of the setting of the dry run
switch, the feedrate cannot be specified using F.
The feedrate is clamped such that the maximum
cutting feedrate, set in parameter No. 1430, is not
exceeded.
- Automatic reference position return (G28)
The tool returns directly to the reference position without passing
through any intermediate points, regardless of the specified amount of
travel. For axes for which no move command is specified, however, a
return operation is not performed.
Feedrate
(parameter)
Rapid traverse rate
(No. 1420)
Automatic acceleration/deceleration
(parameter)
Linear acceleration/deceleration in
rapid traverse for each axis
(No. 1620)
Override Rapid traverse override
- 2nd, 3rd, or 4th reference position return (G30)
The tool returns directly to the 2nd, 3rd, or 4th reference position
without passing through any intermediate points, regardless of the
specified amount of travel. To select a reference position, specify 2, 3,
or 4 in address P. If address P is omitted, a return to the second
reference position is performed.
Feedrate
(parameter)
Rapid traverse rate
(No. 1420)
Automatic acceleration/deceleration
(parameter)
Linear acceleration/deceleration in
rapid traverse for each axis
(No. 1620)
Override Rapid traverse override
NOTE
The function for 3rd/4th reference position return is
optional.
1 When the option is not selected
If "P2" is not specified in address P, the alarm
PS0046 is generated and the function cannot be
executed.
2 When the option is selected
If "P2," "P3," or "P4" is not specified in address P,
the alarm PS0046 is generated and the function
cannot be executed.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1060 -
- M codes (Auxiliary functions)
After address M, specify a numeric value of no more than the number
of digits specified by parameter No. 3030. When M98 or M99 is
specified, it is executed but not output to the PMC.
NOTE
Neither subprogram calls nor custom macro calls
can be performed using M codes.
- S codes (spindle speed functions)
After address S, specify a numeric value of no more than the number
of digits specified by parameter No. 3031.
NOTE
Subprogram calls cannot be performed using S
codes.
- T codes (tool functions)
After address T, specify a numeric value of no more than the number
of digits specified by parameter No. 3032.
NOTE
1 Subprogram calls cannot be performed using T
codes.
2 In lathe systems, tool compensation by T code
commands is not performed.
- B codes (second auxiliary functions)
After address B, specify a numeric value of no more than the number
of digits specified by parameter No. 3033.
NOTE
1 B codes can be renamed "U," "V," "W," "A," or "C"
by setting parameter No. 3460. If the new name is
the same as an axis name address, "B" is used.
Note that "U," "V," and "W" can be used for the T
codes only when the G codes are B or C.
2 Subprogram calls cannot be performed using B
codes.
- Data input
(1) When addresses and numeric values of a command are typed,
then soft key [INPUT] is pressed, the entered data is set. In this
case, the input unit is either the least input increment or
calculator-type input format, according to the setting of bit 0
(DPI) of parameter No. 3401.
The key on the MDI panel can be used instead of soft key
[INPUT].
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1061 -
(2) Commands can be typed successively.
(3) Key entry is disabled during execution.
If soft key [INPUT] or the key on the MDI panel is
pressed during execution, an "EXECUTION/MODE
SWITCHING IN PROGRESS" warning is output.
(4) If input data contains an error, the following warnings may
appear:
Warning Description
FORMAT
ERROR
- A G code other than G00, G01, and G28 has been entered.
- An address other than those displayed on the manual
numerical command screen has been entered.
A value that exceeds the following limitations has been
entered.
- Address G:............ 2 digits
- Address P:............ 1 digit
- Axis address: ........ 9 digits
- M, S, T, B: ............ The parameter-set number of digits
NOTE
Even when the memory protection key is set, key
input can nevertheless be performed.
- Erasing data
(1) When soft key [CLEAR] is pressed, followed by soft key
[EXEC], all the set data is cleared. In this case, however, the G
codes are set to G00 or G01, depending on the setting of bit 0
(G01) of parameter No. 3402.
Data can also be cleared by pressing the key on the MDI
panel.
(2) If soft key [CLEAR] is pressed during execution, an
"EXECUTION/MODE SWITCHING IN PROGRESS" warning
is output.
- Scrolling pages
If the whole axis information cannot be displayed on a single page,
you can scroll pages by pressing the or key.
- Halting execution
If one of the following occurs during execution, execution is halted,
and the data is cleared in the same way as when soft key [CLEAR] is
pressed. The remaining distance to be traveled is canceled.
(1) When a feed hold is applied
(2) When the mode is changed to other than jog feed mode
(3) When an alarm is generated
(4) When a reset or emergency stop is applied
The M, S, T, and B functions remain effective even upon the
occurrence of the above events, with the exception of (4).
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1062 -
- Modal information
Modal G codes and addresses used in automatic operation or MDI
operation are not affected by the execution of commands specified
using the manual numerical command function.
- Jog feed
When the tool is moved along an axis using a feed axis and direction
selection switch on the manual numerical command screen, the
remaining amount of travel is always shown as "0".
- Disabling the M, S, T, and B functions
By setting bit 0 to bit 3 (JMF, JSF, JTF, and JBF) of parameter No.
7002, the M, S, T, and B functions can be disabled. If a disabled
function is specified, the warning "THIS COMMAND CANNOT BE
EXECUTED." is issued.
Limitation
- M, S, T, and B functions
While automatic operation is halted, manual numerical commands can
be executed. In the following cases, however, a "START REJECTED
(ALREADY EXECUTING)" warning is output, and command
execution is disabled.
(1) When an M, S, T, or B function is already being executed, a
manual numerical command containing an M, S, T, or B function
cannot be executed.
(2) When an M, S, T, or B function is already being executed, and
that function alone is specified or a block specifying that
function also contains another function (such as a move
command or dwell function) which has already been completed,
a manual numerical command cannot be executed.
- Jog feed
When a manual numerical command is specified while the tool is
being moved along an axis by using a feed axis and direction selection
switch, the axial movement is interrupted, and the manual numerical
command is executed. Therefore, the tool cannot be moved along an
axis by using a feed axis and direction selection switch during
execution of a manual numerical command.
- Mirror image
A mirror image cannot be produced for the direction of a specified
axial movement.
- REF mode
The manual numerical command screen is not displayed in the REF
mode.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1063 -
- Indexing of the index table and chopping
Commands cannot be specified for an axis along which operation is
being performed during indexing or chopping.
If such an axis is specified for execution, a "THIS COMMAND CAN
NOT EXECUTE" warning is output.
- Functions that cannot be specified
Commands cannot be specified for axes that operate using any of the
following functions.
• Index table indexing
• Chopping
• Spindle positioning
• Polygon turning
• Synchronous, composite, and superimposed control
If the commands are executed for any such axis, a "THIS
COMMAND CAN NOT EXECUTE" warning is generated.
- Functions that cannot be used
Commands cannot be specified for the following functions.
• Extended axis name
• Extended spindle name
• Address P command for multi spindle
• Cs contour control function
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1064 -
3.9 THREE-DIMENSIONAL MANUAL FEED
This function enables the use of the following functions.
• Three-dimensional manual feed
- Tool axis direction handle feed/tool axis direction JOG
feed/tool axis direction incremental feed
- Tool axis right-angle direction handle feed/tool axis
right-angle direction JOG feed/tool axis right-angle
direction incremental feed
- Tool tip center rotation handle feed/tool tip center rotation
JOG feed/tool tip center rotation incremental feed
- Table vertical direction handle feed/table vertical direction
JOG feed/table vertical direction incremental feed
- Table horizontal direction handle feed/table horizontal
direction JOG feed/table horizontal direction incremental
feed
A handle interrupt can be generated for each handle feed.
Handle interrupts work according to the corresponding handle
feed specifications described hereinafter unless otherwise noted.
• Screen display functions
- Display of the coordinate of the tool tip
- Display of pulse values
- Display of the amount of machine axes movement
NOTE
1 To execute three-dimensional handle feed requires
the manual handle feed option. Also, to generate
three-dimensional handle interrupts requires the
manual handle interrupt option.
2 A three-dimensional handle interrupt must not be
generated when a rotation axis command is being
executed during automatic operation.
3 Three-dimensional manual feed is disabled when
the manual reference position return mode is
selected.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1065 -
3.9.1 Tool Axis Direction Handle Feed / Tool Axis Direction JOG
Feed / Tool Axis Direction Incremental Feed
Overview
In the tool axis direction handle feed, tool axis direction JOG feed,
and tool axis direction incremental feed, the tool or table is moved in
the tool axis direction.
Explanation
- Tool axis direction
The tool axis direction that is taken when all the rotation axes for
controlling the tool are at an angle of 0 degree is specified in
parameters No.19697, No.19698, and No.19699. As the rotation
axes for controlling the tool rotate, the tool axis direction changes
according to the rotation axis angle.
CB
Z
Y
X
Workpiece
C
B
Tool axis direction
- Tool axis direction feed in the tilted working plane command mode
If bit 0 (TWD) of parameter No. 12320 is set to 1, the feed direction of
the tool axis direction feed in the tilted working plane command mode
is assumed to be the Z direction in the feature coordinate system of the
tilted working plane command.
- Tool axis direction handle feed
The tool axis direction handle feed is enabled when the following four
conditions are satisfied:
<1> Handle mode is selected.
<2> The tool axis direction feed mode signal (ALNGH) is set to "1"
and the table base signal (TB_BASE) is set to "0".
<3> The state of the first manual handle feed axis selection signals
(HS1A - HS1E) to make the tool axis direction handle feed
mode effective is set in parameter No.12310.
<4> The value of parameter No.12310 matches the first manual
handle feed axis selection signals (HS1A - HS1E).
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1066 -
Amount of movement
When the manual pulse generator is rotated, the tool is moved in the
tool axis direction by the amount of rotation.
Feedrate clamp
The feedrate is clamped so that the speed of each moving axis dose
not exceed the manual rapid traverse rate (parameter No.1424).
Handle pulses generated while the clamp feedrate is exceeded are
ignored.
- Tool axis direction JOG feed/tool axis direction incremental feed
The tool axis direction JOG feed or tool axis direction incremental
feed is enabled when the following three conditions are satisfied:
<1> JOG mode or incremental feed mode is selected.
<2> The tool axis direction feed mode signal (ALNGH) is set to "1"
and the table base signal (TB_BASE) is set to "0".
<3> The feed axis direction selection signal (+Jn, -Jn (where n = 1 to
the number of controlled axes)) is set to "1" for the axis
corresponding to the direction specified by parameter No.19697.
(Even when the tool axis direction is slant because of the settings
of parameters No.19698 and No.19699, the signal that activates
the tool axis direction JOG feed or tool axis direction incremental
feed is determined by parameter No.19697 only.)
Ex.) No.19697 = 3 (+Z-axis direction); Z-axis is the 3rd axis.
• +J3 : Tool axis direction +
• -J3 : Tool axis direction -
Feedrate
The feedrate is the dry run rate (parameter No.1410). The manual
feedrate override feature is available.
If bit 2 (JFR) of parameter No. 12320 is set to 1, the feedrate of a
rotation axis is the jog feedrate of the axis to be rotated (parameter No.
1423). The manual feedrate override feature is available.
Feedrate clamp
The feedrate is clamped so that the speed of each moving axis dose
not exceed the manual rapid traverse rate (parameter No.1424).
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1067 -
3.9.2 Tool Axis Right-Angle Direction Handle Feed / Tool Axis
Right-Angle Direction JOG Feed / Tool Axis Right-Angle
Direction Incremental Feed
Overview
In the tool axis right-angle direction handle feed, tool axis direction
JOG feed, or tool axis direction incremental feed, the tool or table is
moved in the tool axis direction.
If bit 1 (FLL) of parameter No. 12320 is set to 1, the tool or table is
moved in the latitude or longitude direction determined by the tool
axis direction vector.
Explanation
- Tool axis right-angle direction
There are two tool axis right-angle directions, which are perpendicular
to the tool axis direction (see the previous section).
Parameter No.19697
Tool axis
right-angle
direction 1
Tool axis
right-angle
direction 2
1 (The reference tool direction is +X.) +Y direction +Z direction
2 (The reference tool direction is +Y.) +Z direction +X direction
3 (The reference tool direction is +Z.) +X direction +Y direction
This table shows the tool axis right-angle directions that may be taken
when the angles of all the rotation axes for controlling the tool are 0
degree and when parameters No.19698 and No.19699 are both set to
0.
When the reference tool axis direction is inclined based on the settings
of parameters No.19698 and No.19699, the tool axis right-angle
direction is also inclined as much.
As the rotation axes for controlling the tool rotate, the tool axis
right-angle direction changes according to the rotation axis angle.
CB
Z
Y
X
Workpiece
C
B
Tool axis
direction
Tool axis right-
angle direction
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1068 -
(Example) When the tool rotation axes are B-axis and C-axis and the tool axis
direction is the Z-axis direction
C B
Z
Y
X
Tool axis right-angle direction 2
Tool axis direction
B
C
Tool axis right-angle direction 1
Y
X
Z
B
C
- Latitude and longitude directions
When bit 1 (FLL) of parameter No. 12320 is set to 1, the feed direction
is defined as follows:
Let a vector perpendicular to a plane formed by the tool axis direction
vector (
T
r
) and normal axis direction vector (
P
r) (parameter No.
12321) be the tool axis right-angle direction 1 (longitude direction)
vector ( 1
r
R
). When tool axis right-angle direction 1 is selected, a
movement in the positive direction means a movement in this vector
direction, and a movement in the negative direction means a movement
in the direction opposite to the vector direction. (Longitude direction
feed)
Equation:
T
P
R
r
r
r
×=1
Let a vector perpendicular to the tool axis direction vector (
T
r
) and
tool axis right-angle direction 1 (longitude direction) vector ( 1
r
R
) be
the tool axis right-angle direction 2 (latitude direction) vector ( 2
R
r
).
When tool axis right-angle direction 2 is selected, a movement in the
positive direction means a movement in this vector direction, and a
movement in the negative direction means a movement in the direction
opposite to the vector direction. (Latitude direction)
Equation: 12
R
T
R
r
r
r
×=
When the tool axis direction vector (
T
r
) is parallel to the normal axis
direction vector (
P
r
) (parameter No. 12321) (when the angle between
them is not greater than the setting of parameter No. 12322), tool axis
right-angle direction 1 and tool axis right-angle direction 2 are
assumed as follows:
Parameter
No.12321
Normal axis
direction
Tool axis
right-angle
direction 1
Tool axis
right-angle
direction 2
1 +X direction +Y direction +Z direction
2 +Y direction +Z direction +X direction
3 +Z direction +X direction +Y direction
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1069 -
If 0 is set in parameter No. 12321, the normal axis direction is set to
the reference tool axis direction (parameter No. 19697).
If a value other than 0 to 3 is specified in parameter No. 12321, alarm
PS5459 is issued.
- Tool axis right-angle direction feed in the tilted working plane command mode
If bit 0 (TWD) of parameter No. 12320 is set to 1, the feed direction of
the tool axis right-angle direction feed in the tilted working plane
command mode is defined as follows:
Tool axis right-angle direction 1: X direction in the feature
coordinate system of the tilted working plane command
Tool axis right-angle direction 2: Y direction in the feature
coordinate system of the tilted working plane command
- Tool axis right-angle direction handle feed
The tool axis right-angle direction handle feed is enabled when the
following four conditions are satisfied:
<1> Handle mode is selected.
<2> The tool axis right-angle direction feed mode signal (RGHTH) is
set to "1" and the table base signal (TB_BASE) is set to "0".
<3> The state of the first manual handle feed axis selection signals
(HS1A - HS1E) to make the tool axis right-angle direction
handle feed mode effective is set in parameter No.12311 or
No.12312.
<4> The value of parameter No.12311 or No.12312 matches the first
manual handle feed axis selection signals (HS1A - HS1E).
Amount of movement
When the manual pulse generator is rotated, the tool is moved in the
tool axis right-angle direction by the amount of rotation.
Tool axis
right-angle direction 1
(longitude direction): R1
Tool axis
right-angle direction 2
(latitude direction): R2
Normal axis direction: P
Tool axis direction: T
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1070 -
Feedrate clamp
The feedrate is clamped so that the speed of each moving axis dose
not exceed the manual rapid traverse rate (parameter No.1424).
Handle pulses generated while the clamp feedrate is exceeded are
ignored.
- Tool axis right-angle direction JOG feed/tool axis right-angle direction
incremental feed
The tool axis right-angle direction JOG feed or tool axis right-angle
direction incremental feed is enabled when the following three
conditions are satisfied:
<1> JOG mode or incremental feed mode is selected.
<2> The tool axis right-angle direction feed mode signal (RGHTH) is
set to "1" and the table base signal (TB_BASE) is set to "0".
<3> The feed axis direction selection signal (+Jn, -Jn (where n = 1 to
the number of controlled axes)) is set to "1" for the axis
corresponding to the direction that is perpendicular to the
direction specified by parameter No.19697. (Even when the
tool axis direction is slant because of the settings of parameters
No.19698 and No.19699, the signal that activates the tool axis
right-angle direction JOG feed or tool axis right-angle direction
incremental feed is determined by parameter No.19697 only.)
Ex.) No.19697=3 (+Z-axis direction); X-, Y-, and Z-axes are the
1st, 2nd, and 3rd axes respectively.
• +J1 : Tool axis right-angle direction 1 +
• -J1 : Tool axis right-angle direction 1 -
• +J2 : Tool axis right-angle direction 2 +
• -J2 : Tool axis right-angle direction 2 -
Feedrate
The feedrate is the dry run rate (parameter No.1410). The manual
feedrate override feature is available.
If bit 2 (JFR) of parameter No. 12320 is set to 1, the feedrate is the jog
feedrate (parameter No. 1423) for a driven feed axis direction
selection signal. The manual feedrate override feature is available.
Feedrate clamp
The feedrate is clamped so that the speed of each moving axis dose
not exceed the manual rapid traverse rate (parameter No.1424).
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1071 -
3.9.3 Tool Tip Center Rotation Handle Feed / Tool Tip Center
Rotation JOG Feed / Tool Tip Center Rotation Incremental
Feed
Overview
In the tool tip center rotation handle feed, tool tip center rotation JOG
feed, and tool tip center rotation incremental feed, when a rotary axis
is rotated by manual feed, the linear axes (X, Y, and Z axes) are
moved so that turning the rotation axis does not change the relative
relationship between the tool tip position and the workpiece (table).
• The following figure shows an example where the tool is rotated on
the rotation axis. In this case, the linear axes are moved so that the
position of the tool tip is not moved with respect to the workpiece.
Workpiece
Tool tip position
• The following figure shows an example where the table is rotated
on the rotation axis. As in the previous case, the linear axes are
moved so that the position of the tool tip is not moved with respect
to the workpiece (table).
B
Z
Y
X
B B
Table Workpiece
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1072 -
- Tool tip center rotation handle feed
The tool tip center rotation handle feed is enabled when the following
four conditions are satisfied:
<1> Handle mode is selected.
<2> The tool tip center rotation feed mode signal (RNDH) is set to
"1".
<3> The state of the first manual handle feed axis selection signals
(HS1A - HS1E) to make the tool tip center rotation handle feed
mode effective is set in parameter No.12313 or No.12314.
<4> The value of parameter No.12313 or No.12314 matches the first
manual handle feed axis selection signals (HS1A - HS1E).
Amount of movement
When the manual pulse generator is rotated, the rotation axis is moved
by the amount of rotation. The linear axes (X, Y, and Z axes) are
moved so that turning the rotation axis does not change the relative
relationship between the tool tip position and the workpiece.
Feedrate clamp
The feedrate is clamped so that the synthetic speed of the linear axes
(in the tangential direction) does not exceed the manual rapid traverse
rate (parameter No.1424) (of any moving linear axis). The feedrate
is also clamped so that the speed of the rotation axis does not exceed
the manual rapid traverse rate (parameter No.1424) (of that particular
axis). Handle pulses generated while the clamp feedrate is exceeded
are ignored.
- Tool tip center rotation JOG feed/tool tip center rotation incremental feed
The tool tip center rotation JOG feed or tool tip center rotation
incremental feed is enabled when the following three conditions are
satisfied:
<1> JOG mode or incremental feed mode is selected.
<2> The tool tip center rotation feed mode signal (RNDH) is set to
"1".
<3> The feed axis direction selection signal (+Jn, -Jn (where n = 1 to
the number of controlled axes)) is set to "1" for the rotation axis
to be rotated.
Ex.) When the B-axis (4th axis) is rotated
• +J4 : Tool tip center rotation feed +
• -J4 : Tool tip center rotation feed -
Feedrate
Control is exerted so that the synthetic speed of the linear axes (in the
tangential direction) is the dry run rate (parameter No.1410). The
manual feedrate override feature is available.
If bit 2 (JFR) of parameter No. 12320 is set to 1, the feedrate of a
rotation axis is the jog feedrate of the axis to be rotated (parameter No.
1423). The manual feedrate override feature is available.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1073 -
Feedrate clamp
The feedrate is clamped so that the synthetic speed of the linear axes
(in the tangential direction) does not exceed the manual rapid traverse
rate (parameter No.1424) (of any moving linear axis). The feedrate
is also clamped so that the speed of the rotation axis does not exceed
the manual rapid traverse rate (parameter No.1424) (of that particular
axis).
- Selection of the tool length offset value
The tool length in three-dimensional manual feed is determined as
explained below. Table 3.9.3 (a))
If bit 2 (LOD) of parameter No. 19746 is set to 0, the value set in
parameter No. 12318 is assumed to be the tool length.
If the LOD parameter is set to 1, and the tool length offset function is
performed, the offset data specified for the tool length offset is
assumed to be the tool length.
If the LOD parameter is set to 1, and the tool length offset function is
not performed, the tool length is determined as follows. If bit 3
(LOZ) of parameter No. 19746 is set to 0, the value set in parameter
No. 12318 is assumed to be the tool length in three-dimensional
manual feed; if LOZ is set to 1, the tool length is assumed to be 0.
Table 3.9.3 (a) Tool length offset value in three-dimensional manual
feed
Parameter No. 19746#2(LOD)
= 1
= 0 Tool length
offset enabled
Tool length offset
canceled
= 0 Parameter No. 12318
Parameter
No. 19746#3
(LOZ) = 1
Parameter
No. 12318
Offset data 0
The tool length offset function is enabled when the following two
conditions are both satisfied:
• The tool length offset function listed below is enabled (modal
code of group 8 except G49)
- G43／G44 : Tool length compensation
- G43.4／G43.5 : Tool center point control
• The H/D code is other than 0.
If bit 6 (CLR) of parameter No. 3402 is set to 0 not to clear the tool
length offset vector, G codes of group 8, and H codes at the time of a
reset, the tool length offset status is maintained when a reset is made
in the tool length offset mode.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1074 -
3.9.4 Table Vertical Direction Handle Feed / Table Vertical Direction
JOG Feed / Table Vertical Direction Incremental Feed
Overview
In the table vertical direction handle feed, table vertical direction JOG
feed, and table vertical direction incremental feed, the tool is moved in
the table vertical direction.
Explanation
- Table vertical direction
The table vertical direction is a direction vertical to the table. It is
equal to the tool axis direction specified in parameter No.19697 when
all of the rotation axes for controlling the table are at a an angle of 0
degree. When the rotation axes for controlling the table rotate, the
table vertical direction changes according to the rotation axis angle.
B
B
Z
Y
X
Table vertical direction
- Table-based vertical direction feed in the tilted working plane command mode
If bit 0 (TWD) of parameter No. 12320 is set to 1, the feed direction of
the table-based vertical direction feed in the tilted working plane
command mode is assumed to be the Z direction in the feature
coordinate system of the tilted working plane command.
- Table vertical direction handle feed
The table vertical direction handle feed is enabled when the following
four conditions are satisfied:
<1> Handle mode is selected.
<2> Both the tool axis direction feed mode signal (ALNGH) and the
table base signal (TB_BASE) are set to "1".
<3> The state of the first manual handle feed axis selection signals
(HS1A - HS1E) to make the table vertical handle feed mode
effective is set in parameter No.12310.
<4> The value of parameter No.12310 matches the first manual
handle feed axis selection signals (HS1A - HS1E).
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1075 -
Amount of movement
When the manual pulse generator is rotated, the tool is moved in the
table vertical direction by the amount of rotation.
Feedrate clamp
The feedrate is clamped so that the speed of each moving axis dose
not exceed the manual rapid traverse rate (parameter No.1424).
Handle pulses generated while the clamp feedrate is exceeded are
ignored.
- Table vertical direction JOG feed/table vertical direction incremental feed
The table vertical direction JOG feed or table vertical direction
incremental feed is enabled when the following three conditions are
satisfied:
<1> JOG mode or incremental feed mode is selected.
<2> Both the tool axis direction feed mode signal (ALNGH) and the
table base signal (TB_BASE) are set to "1".
<3> The feed axis direction selection signal [+Jn,-Jn (where n = 1 to
the number of controlled axes)] is set to "1" for the axis
corresponding to the direction specified by parameter No.19697.
Ex.) No.19697 = 3 (+Z-axis direction); Z-axis is the 3rd axis.
• +J3 : Table vertical direction +
• -J3 : Table vertical direction -
Feedrate
The feedrate is the dry run rate (parameter No.1410). The manual
feedrate override feature is available.
If bit 2 (JFR) of parameter No. 12320 is set to 1, the feedrate is the jog
feedrate (parameter No. 1423) for a driven feed axis direction
selection signal. The manual feedrate override feature is available.
Feedrate clamp
The feedrate is clamped so that the speed of each moving axis dose
not exceed the manual rapid traverse rate (parameter No.1424).
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1076 -
3.9.5 Table Horizontal Direction Handle Feed / Table Horizontal
Direction JOG Feed / Table Horizontal Direction Incremental
Feed
Overview
In the table horizontal direction handle feed, table horizontal direction
JOG feed, and table horizontal direction incremental feed, the tool is
moved in the table horizontal direction.
If bit 1 (FLL) of parameter No. 12320 is set to 1, the tool or table is
moved in the latitude or longitude direction determined by the
table-based vertical direction vector.
Explanation
- Table horizontal direction
There are two table horizontal directions, which are perpendicular to
the table vertical direction (see the previous section).
Parameter No.19697 Table horizontal
direction 1
Table horizontal
direction 2
1 (The reference tool
direction is +X.) +Y direction +Z direction
2 (The reference tool
direction is +Y.) +Z direction +X direction
3 (The reference tool
direction is +Z.) +X direction +Y direction
This table shows the table horizontal directions that may be taken
when the angles of all the rotation axes for controlling the table are 0
degree.
As the rotation axes for controlling the table rotate, the table
horizontal direction changes according to the rotation axis angle.
B
B
Z
Y
X
Table horizontal direction 2
Table horizontal direction 1
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1077 -
(Example) When the table rotation axis is the B-axis, and the table vertical direction
is the Z-axis direction
B
Z
Y
X
Table horizontal direction 2
Table horizontal
direction 1
X
Y
Z
B
BTable vertical di
r
ection
- Latitude and longitude directions
When bit 1 (FLL) of parameter No. 12320 is set to 1, the feed
direction is defined as follows:
Let a vector perpendicular to a plane formed by the table-based
vertical direction vector (
T
r
) and normal axis direction vector (
P
r
)
(parameter No. 12321) be the table-based horizontal direction 1
(longitude direction) vector ( 1
r
R
). When tool axis right-angle
direction 1 is selected, a movement in the positive direction means a
movement in this vector direction, and a movement in the negative
direction means a movement in the direction opposite to the vector
direction. (Longitude direction feed)
Equation:
T
P
R
r
r
r
×=1
Let a vector perpendicular to the table-based vertical direction vector
(
T
r) and table-based horizontal direction 1 (longitude direction) vector
(1
r
R
) be the table-based horizontal direction 2 (latitude direction)
vector ( 2
R
r
). When tool axis right-angle direction 2 is selected, a
movement in the positive direction means a movement in this vector
direction, and a movement in the negative direction means a
movement in the direction opposite to the vector direction. (Latitude
direction)
Equation: 12
R
T
R
r
r
r
×=
When table-based vertical direction vector (
T
r) is parallel to the
normal axis direction vector (
P
r
) (parameter No. 12321) (when the
angle between them is not greater than the setting of parameter No.
12322), tool axis right-angle direction 1 and tool axis right-angle
direction 2 are assumed as follows:
Parameter
No. 12321
Normal axis
direction
Table-based
horizontal direction 1
Table-based
horizontal direction 2
1 +X direction +Y direction +Z direction
2 +Y direction +Z direction +X direction
3 +Z direction +X direction +Y direction
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1078 -
If 0 is set in parameter No. 12321, the normal axis direction is set to
the tool axis direction.
If a value other than 0 to 3 is specified in parameter No. 12321, alarm
PS5459 is issued.
Table-based vertical
direction: T
Table-based horizontal
direction 2 (latitude
direction): R2
Table-based horizontal
direction 1 (longitude
direction): R1
Normal axis direction: P
- Table-based horizontal direction feed in the tilted working plane command mode
If bit 0 (TWD) of parameter No. 12320 is set to 1, the feed direction of
the table-based horizontal direction feed in the tilted working plane
command mode is defined as follows:
Table-based horizontal direction 1: X direction in the feature
coordinate system of the tilted working plane command
Table-based horizontal direction 2: Y direction in the feature
coordinate system of the tilted working plane command
- Table horizontal direction handle feed
The table horizontal direction handle feed is enabled when the
following four conditions are satisfied:
<1> Handle mode is selected.
<2> Both the tool axis right-angle direction feed mode signal
(RGHTH) and the table base signal (TB_BASE) are set to 1.
<3> The state of the first manual handle feed axis selection signals
(HS1A - HS1E) to make the table horizontal direction handle
feed mode effective is set in parameter No.12311 or No.12312.
<4> The value of parameter No.12311 or No.12312 matches the first
manual handle feed axis selection signals (HS1A - HS1E).
Amount of movement
When the manual pulse generator is rotated, the tool is moved in the
table horizontal direction by the amount of rotation.
Feedrate clamp
The feedrate is clamped so that the speed of each moving axis dose
not exceed the manual rapid traverse rate (parameter No.1424).
Handle pulses generated while the clamp feedrate is exceeded are
ignored.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1079 -
- Table horizontal direction JOG feed/table horizontal direction incremental feed
The table horizontal direction JOG feed or table horizontal direction
incremental feed is enabled when the following three conditions are
satisfied:
<1> JOG mode or incremental feed mode is selected.
<2> Both the tool axis right-angle direction feed mode signal
(RGHTH) and the table base signal (TB_BASE) are set to "1".
<3> The feed axis direction selection signal (+Jn, -Jn (where n = 1 to
the number of controlled axes)) is set to "1" for the axis
corresponding to the direction that is perpendicular to the
direction specified by parameter No.19697.
Ex.) No.19697 = 3 (+Z-axis direction); X-, Y-, and Z-axes are
the 1st, 2nd, and 3rd axes respectively.
• +J1 : Table horizontal direction 1 +
• -J1 : Table horizontal direction 1 -
• +J2 : Table horizontal direction 2 +
• -J2 : Table horizontal direction 2 -
Feedrate
The feedrate is the dry run rate (parameter No.1410). The manual
feedrate override feature is available.
If bit 2 (JFR) of parameter No. 12320 is set to 1, the feedrate is the jog
feedrate (parameter No. 1423) of a driven feed axis direction selection
signal. The manual feedrate override feature is available.
Feedrate clamp
The feedrate is clamped so that the speed of each moving axis dose
not exceed the manual rapid traverse rate (parameter No.1424).
Note
1 To perform a three-dimensional handle feed, the manual handle
feed option is required. To perform three-dimensional handle
interrupt, the manual handle interrupt option is required.
2 When a three-dimensional handle interrupt is performed, rotation
axis command execution must not be in progress in automatic
operation.
3 When the manual reference position return mode is selected,
three-dimensional manual feed is not enabled.
4 When the offset value specified for the tool length offset function
is used for tool center point rotation feed (when bit 2 (LOD) of
parameter No. 19746 is set to 1), the controlled point should
generally be shifted. (Set bit 5 (SVC) of parameter No. 19665
to 1.)
In this case, specify the tool length with a radius value.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1080 -
3.10 DISTANCE CODED LINEAR SCALE INTERFACE
Overview
The interval of each reference marks of distance coded linear scale are
variable. Accordingly, if the interval is determined, the absolute
position can be determined. The CNC measures the interval of
reference marks by axis moving of short distance and determines the
absolute position. Consequently the reference position can be
established without moving to reference position.
10.02 10.04
20.02
20.00 20.00
Reference mark 1 Reference mark 2Mark 1 Mark 2 Mark 1
Fig. 3.10 (a) Example of distance coded linear scale
This is an optional function.
3.10.1 Procedure for Reference Position Establishment
Procedure
(1) Select the JOG mode, and set the manual reference position
return selection signal ZRN to "1".
(2) Set a direction selection signal(+J1,-J1,+J2,-J2,…) for a target
axis.
(3) The axis is fed at a constant low speed (reference position return
FL feedrate specified by parameter (No.1425) setting).
(4) When a reference mark is detected, the axis stops, then the axis is
fed at a constant low speed again.
(5) Above (4) is executed repeatedly until two, three or four
reference marks are detected. And absolute position is
determined and reference position establishment signal
(ZRF1,ZRF2,ZRF3, …) turns to "1".
(A number of reference marks is determined by bit 2 (DC2x) and
1 (DC4x) of parameter No.1802.)
Even when the direction selection signal (+J1, -J1, +J2, -J2,...) is set to
"0" while steps (2) to (5) are being performed, the feedrate operation
does not stop, and the operation for establishing a reference position is
carried out continuously.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1081 -
The timing chart for this procedures is given below.
JOG
ZRN
+J1
Reference mark
ZRF1
Feedrate FL rate FL rate FL rate
Fig. 3.10.1 (a) Timing chart for reference position establishment
- Procedure for establishing a reference position through automatic operation
If an automatic reference position return (G28) is specified before a
reference position is not established, steps (3) to (5) above are
performed automatically.
After the reference position is established, the automatic reference
position return is performed.
- Stopping the operation for establishing a reference position
The operation for establishing a reference position is stopped if any of
the following operations is performed in steps (3) to (5), described
above.
• Reset
• Setting the feed axis direction selection signal (+J1, -J1, +J2, -J2,
etc.) to 0
If any of the following operations is performed during the operation of
automatic reference position return (G28) before a reference position
is not established, the operation for establishing a reference position
stops:
• Reset
• Performing feed hold during movement from an intermediate
position
If the operation for establishing a reference position is stopped by an
operation other than a reset, the operation for establishing a reference
position must be reset and resumed.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1082 -
3.10.2 Reference Position Return
(1) When the reference position is not established and the axis
moved by turning the feed axis direction signal
(+J1,-J1,+J2,-J2,...) to "1" in REF mode, the reference position
establishment procedure is executed.
(2) When the reference position is already established and the axis is
moved by turning the feed axis direction signal
(+J1,-J1,+J2,-J2,...) to "1" in REF mode, the axis is moved to the
reference point without executing the reference position
establishment procedure.
(3) When the reference position is not established and the reference
position return command (G28) is executed, the reference
position establishment procedure is executed. The next
movement the axis depends on the setting of parameter RFS
(No.1818#0).
(4) When the reference position is already established and the
reference position command (G28) is executed, the movement of
the axis depends on the setting of bit 1 (RF2) of parameter
No.1818.
3.10.3 Distance Coded Rotary Encoder
In case of setting a rotary axis, if bit 3 (DCRx) of parameter No.1815
is set, the setting axis is regarded as being equipped with a distance
coded rotary encoder.
In case of distance coded rotary encoder, the marker interval may be
different from parameter setting value. (a-b section of the following
figure) When the reference point return is executed through this
section, it is not able to establish the reference point. Therefore, in
case of distance coded rotary encoder, if the reference point return is
started for B point from A point of below figure, the reference point is
not established yet at B point. The reference point return is re-started
for C point. The reference point return procedure is finished at C
point.
9
.
64
9
.
98
9
.
96
19
.
66
20
.
02
20
.
02
20
.
02
9
.
94
20.00 20.00
20.00
A
B
C
b
a
• When the reference point return procedure is executed, the
coordinate value are rounded in 0 to 360 degree, even if Machine
coordinate values are linear axis type.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1083 -
• In case of distance coded rotary encoder, only the measurement
by three points or four points is possible. (bit 2 (DC2) of
parameter No.1802 is disregarded as 0.)
3.10.4 Axis Synchronization Control
Requirements when this function is used with axis synchronization control
axes
When this function is used with axis synchronization control axes, the
distance coded linear scale used for the master axis and that used for
the slave axis must have reference marks placed at identical intervals.
(Set identical values in parameters Nos. 1821 and 1882 for both the
master and slave axes.)
This function does not work unless the use of this function is specified
for both the master and slave axes (bit 2 (DCL) of parameter No. 1815
is 1).
Also, in all parameters related to this function, except parameter No.
1883, 1884 (distance from the scale zero point to reference position 1,
2), set identical values for both the master and slave axes.
If a parameter value for the master axis differs from the corresponding
parameter value for the slave axis, alarm SV1051 is issued.
NOTE
When this function is used with axis
synchronization control axes for which the
operation mode is switched between
synchronization operation and normal operation,
this function is enabled only if the synchronization
select signal (SYNC1, SYNC2, ...<Gn138>) is 1.
(During establishment of a reference position, the
synchronization select signal status must be
maintained.)
Reference position establishment with axis synchronization control axes
With axis synchronization control axes, a reference position is
established as follows. When a reference mark for the master or slave
axis is detected, a stop takes place temporarily. Then, a feed operation
is performed again at the reference position return FL feedrate. This
sequence is repeated until a reference mark is detected three or four
times for both the master and slave axes. Then the absolute position is
calculated for both the master and slave axes, and the reference
position establish signals ZRF1, ZRF2, ... <F120> are set to 1.
After the reference position has been established by the above
operation, a synchronization error is corrected. (Checking for
excessive synchronization error alarm 2 is made even during reference
position establishment.)
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1084 -
Scale end Reference mark
(1) (2) (3)
(a) (b) (c)
Master axis
Slave axis
Start point End Point
(Example of 3 points measurement system)
In the above example, the following sequence is executed.
a. When the reference mark (1) of the master axis is detected, both
master axis and slave axis stop.
b. Both the axes begin to move again at a reference position return
FL feedrate.
c. When the reference mark (a) of the slave axis is detected, both
axes stop again.
d. Both the axes begin to move again at FL feedrate.
e. Both axes repeat the operation until all point ((2) -> (b) ->(3) ->
(c)) are detected.
f. When the slave axis detects the third reference mark (c), both the
axes end the reference position establishment.
NOTE
In case of this function is used with axis
synchronization control axes, if the value of
parameters Nos. 1883 and 1884 for both the master
and slave axes is 0, the reference position is not
established. Also, the reference position establish
signals ZRF1, ZRF2, ... <F120> are set to 0.
3.10.5 Axis Control by PMC
In PMC axis control, if the reference position return command (axis
control command code 05H) is issued for an axis having a distance coded
linear scale, reference position return is performed according to the
reference position return sequence for the distance coded linear scale.
Specifically, the following operations take place:
Before reference
position establishment
The reference position is established by detecting
two, three or four reference marks.
Movement to the reference position is not
performed.
After reference
position establishment
Positioning at the reference position is performed.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1085 -
3.10.6 Angular Axis Control
There are the following limitations when the angular axis control is
used.
(a) It is necessary to use the linear scale with the distance coded
reference mark for both the perpendicular axis and the angular
axis.
(b) When the reference point of the perpendicular axis is established,
it is necessary to establish the reference point of the angular axis
previously. When the reference point of the angular axis is not
previously established, the alarm DS0020 is generated.
(c) During the reference point establishment operation of the angular
axis, the command in the perpendicular axis is invalid in the
manual reference point return.
3.10.7 Note
(1) In the case of the actual interval of reference marks is different
from parameter setting value, the alarm DS1449 occurs.
(2) This function is disabled if any of the following conditions is
satisfied:
• Either parameter No.1821 (mark-1 interval) or parameter
No.1882 (mark-2 interval) is set to 0.
• The setting of parameter No.1821 is greater than or equal to
the setting of parameter No.1882.
• The difference between the settings made for parameters
1821 and 1882 is greater than or equal to twice either
setting.
• The absolute-position detection function is enabled.(Bit 5
(APCx) of parameter No.1815 is set to 1.)
(3) A difference of parameters Nos.1821 and 1882 must be more
than 4.
Example)
When the scale, which is that mark1 interval is 20.000mm
and mark2 interval is 20.004mm, is used on IS-B machine :
When the detection unit of 0.001mm is selected, parameter
No.1821 and No.1882 must be set "20000" and "20004",
and the difference of them is "4".
To use such a scale, please adjust the detection unit by
modification of parameters No.1820 (CMR) and
Nos.2084/2085(flexible feed gear) to make the difference of
parameters Nos.1821 and 1882 more than 4 as following
examples.
(a) Set the detection unit=0.0001mm, and set
No.1821=200000, No.1882=200040
(b) Set the detection unit=0.0005mm, and set
No.1821=40000, No.1882=40008
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1086 -
NOTE
When the detection unit is changed, parameters
relating to the detection unit (such as the effective
area and positional deviation limit) must also be
changed accordingly.
(4) In this procedure, the axis does not stop until two, three or four
reference marks are detected. If this procedure is started at the
position near the scale end, CNC can not detect three or four
reference marks and the axis does not stop until over travel alarm
occurs. Please care to start at the position that has enough
distance from scale end.
Scale end Reference marks
Start point (Bad) Start point (Good)
(5) When the axis used this function, the following function can not
be used.
• Absolute position detection (absolute pulse coder)
• Three-dimensional error correction
(6) If axial movement is made in the direction opposite to that of
reference position return, the movement is reversed to the
direction of reference position return after three or four reference
marks have been detected. Steps (3) to (5) of the basic procedure
for establishing a reference position are carried out to establish
the reference position.
(7) Straightness compensation function
When the reference point establishment of moving axis is
executed after the establishment of compensation axis, the
compensation axis is moved by straightness compensation
amount when the reference point of moving axis is established.
(8) The reference point establishment is not performed during
synchronous control is activated.
(9) The reference point establishment is not performed during
composite control is activated.
(10) The reference point establishment is not performed during
superimposed control is activated.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1087 -
3.11 LINEAR SCALE WITH DISTANCE-CODED REFERENCE
MARKS (SERIAL)
Overview
By using High-resolution serial output circuit for the linear scale with
distance-coded reference marks (serial), the CNC measures the
interval of referenced mark by axis moving of short distance and
determines the absolute position.
This function enables high-speed high-precision detection by using
High-resolution serial output circuit.
It is available that using maximum stroke 30 meters length.
Explanation
The linear scale with distance-coded reference marks (serial) is
combined the irregular reference marked linear scale with the
High-resolution serial output circuit, it can detect the accurate
position.
Reference mark signal
10.02 10.04 10.06
20 40 60
0
The CNC measures the interval of referenced mark by axis moving of
short distance and determines the absolute position, because of the
interval of each reference mark is different with regular interval.
It is not necessary that the axis is moved to the reference position for
establishment of reference position.
This function enables high-speed high-precision detection by using
High-resolution serial output circuit.
It is available that using maximum stroke 30 meters length.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1088 -
- Connection
It is available under linear motor system and full closed system.
CNC Servo
Amp
Separate
Detector
Interface
Unit
Table
High
Resolution
Serial Output
Circuit C
Full Closed System
Linear scale with distance-coded
reference marks (serial)
Max. 30m
Linear motor system
CNC Servo
Amp
Linear motor
Linear Motor
Position Detection
Circuit C
Pole sensor
Linear scale with distance-coded
reference marks (serial)
Max. 30m
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1089 -
- Procedure for reference position establishment through manual operation
(1) Select the JOG mode, and set the manual reference position
return selection signal ZRN to "1".
(2) Set a direction selection signal(+J1,-J1,+J2,-J2,…) for a target
axis.
(3) The axis is fed at a constant low speed (reference position return
FL feedrate specified by parameter No.1425 setting).
(4) When the absolute position of linear scale with distance-coded
reference marks (serial) is detected, the axis stops. Then the
absolute position of CNC is calculated and reference position
establishment signal (ZRF1,ZRF2,ZRF3,…) turns to "1".
The timing chart for this procedures is given below.
FL rate
JOG
ZRN
+J1
Reference mark
ZRF1
Feedrate
- Procedure for reference position establishment through automatic operation
If an automatic reference position return (G28) is specified before a
reference position is not established, steps (3) to (4) above are
performed automatically.
After the reference position is established, the automatic reference
position return is performed by setting of parameter RFS No.1818#0.
- Stopping the operation for establishing a reference position
The operation for establishing a reference position is stopped if any of
the following operations is performed in steps (3) to (4), described
above.
• Reset
• Setting the feed axis direction selection signal (+J1, -J1, +J2, -J2,
etc.) to 0
• Setting the Servo off signals (SVF1, SVF2, etc.) to 1
If any of the following operations is performed during the operation of
automatic reference position return (G28) before a reference position
is not established, the operation for establishing a reference position
stops:
• Reset
• Performing feed hold during movement from an intermediate
position
• Setting the Servo off signals (SVF1, SVF2, etc.) to 1
If the operation for establishing a reference position is stopped by an
operation other than a reset, the operation for establishing a reference
position must be reset and resumed.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1090 -
- Establishing a reference position and moving to the reference position
By following operation, establishing a reference position and moving
to the reference position is performed.
Moving through manual
operation in REF mode
Moving through automatic operation by
automatic reference position return (G28)
The reference
position is not
established.
Establishing the reference
position
Firstly, moving to the intermediate position, and
establishing the reference position.
Secondly, whether moving to the reference
position or not is performed by setting bit 0
(RFS) of parameter No.1818.
The reference
position is
established.
Moving to the reference
position
Whether moving to the intermediate position and
the reference position or not is performed by
setting bit 1 (RF2) of parameter No.1818.
- Feed axis synchronization control
In case of using the axis synchronization control, please confirm the
following items.
• When this function is used with axis synchronization control
axes, the linear scale with distance-coded reference marks (serial)
used for the master axis and that used for the slave axis must
have reference marks placed at identical intervals.
• The master axis scale and the slave axis scale should be installed
in parallel direction. (The zero positions should be faced the
same direction.)
• To the parameters, which relate to this function (except No.1883,
No.1884), the same value must be set for the master axis and for
the slave axis.
• The linear scale with distance-coded reference marks (serial)
should be applied for the master axis and the slave axis.
If either of the master axis or the slave axis is not the linear scale
with distance-coded reference marks (serial), alarm DS0018
occurs when reference position establishment is tried.
• During operating the establishment of reference position, the
state of signal for selecting synchronized axis(SYNCn<Gn138>
or SYNCJn<Gn140>) should be kept.
Procedure for reference position establishment by axis
synchronization control is as follows.
• Both of axes (master axis and slave axis) are fed on the reference
position return FL feedrate until distance coded scales of both
axes detect the absolute position.
• Then absolute position of both axes are calculated and Reference
Position Establishment Signals (ZRF1,ZRF2,...) turn to "1".
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1091 -
- Angular axis control
In case of using the angular axis control, please confirm the
following items.
• It is necessary to use the linear scale with distance-coded
reference marks (serial) for both the perpendicular axis and the
angular axis.
If not, the alarm DS0019 occurs when reference position
establishment is commanded.
• When the reference point establishment of angular and
perpendicular axes are tried, please set bit 2 (AZR) of parameter
No. 8200 to '0' and input signal NOZAGC <G063.5> to '0'.
If not, the alarm DS0019 occurs when reference position
establishment is commanded.
• When the reference point of the perpendicular axis is established,
it is necessary to establish the reference point of the angular axis
previously. When the reference point of the angular axis is not
previously established, the alarm DS0020 occurs.
• On angular axis control, if you use automatic setting of
parameter No.1883,1884 on reference point establishment (bit 2
(DATx) of parameter No.1819 = 1), please establish reference
point of perpendicular axis after reference point establishment
and return of angular axis.
In manual reference position return, the perpendicular axis cannot be
specified while the angular axis reference point is being established.
The perpendicular axis, if specified, is ignored.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1092 -
CAUTION
1 When the Linear scale with distance-coded
reference marks (serial) is used, please set bit 3
(SDCx) of parameter No.1818 to 1.
2 On the Linear scale with distance-coded reference
marks (serial), the axis does not stop until three
reference marks are detected. If this procedure is
started at the position near the scale end, CNC can
not detect three reference marks and the axis does
not stop until over travel alarm occurs. Please care
to start at the position that has enough distance
from scale end.
And if establishment of reference position is failed,
the establishment is retried. Then axis does not
stop until still more three reference marks are
detected. So please set the maximum move
amount (detection unit : parameter No.14010) not
to reach the scale end.
Scale end Reference marks
Start point (Bad) Start point (Good)
3 On flexible synchronization control mode,
reference position can't be established.
4 Straightness compensation function
When the reference point establishment of moving
axis is executed after the establishment of
compensation axis, the compensation axis is
moved by straightness compensation amount
when the reference point of moving axis is
established.
5 It is not available to use this function and the
temporary absolute coordinate setting together.
6 The reference point cannot be established during
twin table synchronous operation or single
operation.
7 Angular axis control cannot be performed together
with synchronous control, composite control, or
superposition control.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1093 -
3.12 MANUAL HANDLE RETRACE
Overview
In this function, the program can be executed both forward and
backward with a manual handle (manual pulse generator) under
automatic operation.
Therefore, errors of a program, interference, and so on can be checked
easily by working a machine actually.
- Checking mode
In this mode, the program can be executed forward and backward and
the program can be checked.
To change to the checking mode, it is necessary to change the mode to
the memory mode (MEM mode), and the checking mode signal
MMOD<Gn067.2> is set to "1". This function makes the data to
execute the program backward when the program is executed forward
in the checking mode.
To work a machine synchronizing with a pulse generated by a manual
handle in the checking mode, the manual handle check signal MCHK
<Gn067.3> is set to "1" in addition to the above-mentioned. As a
result, it becomes possible to check the program with a manual handle.
NOTE
During the checking mode, it is not possible to
change the parameter and offset.
- Forward movement with a manual handle
The "forward movement" is that the program is executed forward by
turning a manual handle in the positive direction (when the manual
handle check signal is set to "1".) or in no relation to rotation of a
manual handle (when the manual handle check signal is set to "0".).
When the manual handle check signal is set to "1", the execution
speed of the program is proportional to the number of rotations of a
manual handle. The program is executed forward rapidly when a
manual handle is turned to the positive direction rapidly. And, the
program is executed forward slowly when a manual handle is turned
to the positive direction slowly. The distance magnification traveled
per pulse from manual handle can be switched as same as a usual
manual handle feed function.
When the manual handle check signal is set to "0", the execution of
the program is controlled as same as an automatic operation.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1094 -
- Backward movement
The "backward movement " is that the program executed forward once
is executed backward by turning a manual handle in the negative
direction.
The program can be executed backward only for the block executed
forward. And, the number of blocks for it is about 190 blocks. This
block number changes by the content of the commanded program.
The program is executed backward rapidly when a manual handle is
turned to the negative direction rapidly. And the program is executed
backward slowly when a manual handle is turned to the negative
direction slowly. The distance traveled per pulse from manual handle
can switch magnification as well as a usual manual handle feed.
NOTE
In the system which exceeds 4 paths and 20
axes, the maximum number of blocks which can
move backward becomes about 97 blocks.
Explanation
- Control by the manual handle
Program execution start
The checking mode signal MMOD<Gn067.2> is set to "1" in the
memory mode (MEM mode) in order to change the checking mode.
Then, the program execution is begun by turning ST signal from "1"
to "0".
If the manual handle check signal MCHK <Gn067.3> is set to "1" at
this time, the execution of the program is controlled by a manual
handle. The program is executed synchronizing with rotation of a
manual handle.
When a manual handle check signal MCHK<Gn067.3> is set to "0", it
is controlled as usual execution.
When check mode signal MMOD<Gn067.2> is set to "1" during the
operation of the program, it is enabled a check mode from the block
that next buffering is done.
That is, even if check mode signal set to "1", check mode is not
always enabled at once.
When check mode is enabled, check mode confirmation signal
MMMOD<Fn091.3> is set to "1".
NOTE
After the signal MMOD is turned to "0" during the
execution of the program, the program cannot be
executed forward and backward.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1095 -
Control with the manual handle
The value of the parameter No.6410 and the scale factors decide the
moving speed of the machine by one pulse generated by a manual
handle.
When a manual handle is turned, the actual movement speed of the
machine is as follows.
[Feedrate command value] × [Number of the handle pulse per a
second]
× [Handle magnification] × ([Parameter setting value]/100) × (8/1000)
(mm/min or inch/min)
Example) When feedrate command value is 30mm/min, handle
magnification is 100, parameter No.6410 is set to 1 and manual pulse
generator is rotated at 100 pulse/rev, the feedrate of axis is decided as
follow.
[Feedrate]=30[mm/min] × 100[pulse/s] × 100 × (1/100) × (8/1000)[s]
=24[mm/min]
When the feedrate exceeds the override 100% feedrate by turning a
manual handle rapidly, the feedrate is clamped at the speed of override
100%. That is, if the pulse of the following formula exceeds "1", the
feedrate is clamped.
[Number of the handle pulse per a second]
× [Handle magnification] × ([Parameter setting value]/100) × (8/1000)
The rapid traverse feedrate is clamped at 10%. However, the feedrate
of the rapid traverse is clamped at 100% when bit 0 (HDRPD) of
parameter No.6400 is set to "1".
And if parameter No.6405 is set to an optional value, it can be
clamped to override by nearly optional value.
When the parameter No.6405 is set to larger value than "100", it is
clamped to nearly 100%.
When parameter No.6405 is set to "0", the setting of bit 0 (RPO) of
parameter No.6400 becomes valid.
The single block signal and the feed hold signal are effective in the
checking mode. When the execution of a program is stopped by the
single block stop or the feed hold stop, it is necessary to turn ST signal
from "1" to "0" in order to restart the program.
In the block with the movement and the block of dwell, the execution
speed of the program can be controlled by turning a manual handle.
As for the block of neither movement nor dwell such as the block of
only address M, S, T, and F, the program advances to the following
block even if a manual handle does not turn.
The rotation of the spindle does not synchronize with a pulse of a
manual handle. During the checking mode, the spindle rotates at the
specified rotation speed. As for the feed per revolution, a program is
executed at the feedrate which was converted from the rotation speed
of the spindle to the corresponding feed per minute inside CNC.
NOTE
The manual handle used by this function is always
the first. The 2nd and 3rd manual handle cannot be
used in this function.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1096 -
Forward movement and backward movement with a manual handle
The program is executed forward when a manual handle is turned to
the positive direction. And, the program is executed backward when a
manual handle is turned to the negative direction.
The program is executed backward as soon as a manual handle is
turned to the negative direction in executing the program forward.
When a manual handle keeps being turned in a negative direction, the
program is executed backward and the execution stops in the block of
O number. Then, if a manual handle is turned to the positive direction,
the program is executed forward again.
Even if a manual handle controls the program execution, the program
is executed forward in no relation to a pulse generated by a manual
handle on setting the manual handle check signal to "0".
Program end
When the block of M2 or M30 is executed, the manual handle retrace
ends. It is not possible to execute the program backward from the
block of M2 or M30.
When the execution of the program ends, RESET signal must be set to
"1", and the checking mode signal and the manual handle check signal
must be set to "0".
In 2 path control system, FIN signal must not be set to "1" when the
block of M2 or M30 is executed in only one of paths. After the block
of M2 or M30 has been executed in both paths, FIN signal is set to "1".
(Except for the block of waiting M code is commanded before M2 or
M30 in both paths.)
- Notice of the operation
Dry-run can not operate during the checking mode. Dry-run signal
must be set to "0".
Automatic operation starts immediately with the feedrate commanded
by the program, when the checking mode signal or the synchronous
operation with handle signal is turned off during executing the
program in the checking mode.
The edit of the program and the change of the parameter and the offset
must not be done.
- Backward movement of each code
All modal information of G, T, S-code is memorized in executing the
program forward. And, the memorized data of the modal G, T, S-code
are used in executing the program backward.
As for M-codes, they are grouped and the modal information is
managed by parameter No.6411 to 6490. Therefore, M-code can be
executed backward according to the information. As for the modal
information of the M-code, a change in each group is memorized in
the execution data.
As for the codes except for G, M, S, and T, the same code is output
between forward movement and backward movement.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1097 -
- G-code
If G-code that changes modal information is commanded in backward
movement, the modal information of previous block is executed.
Example)
N1G99;
N2G01X_F_;
N3X_Z_;
N4G98; ..................... backward movement starts from this block
N5X_Y_Z_;
If backward movement starts from N4 block, the modal information is
changed from G98 to G99 and G99 is executed from N3.
G-code with a movement is traced along the route opposite to forward
movement.
G-code that can be command in executing the program backward is as
follows.
The other G-codes cannot be command in executing the program
backward.
The G-codes in the G-code system B and C also can be used.
Lathe system
G00 G01 G02 G03 G04 G22 G23
G25 G26 G28 G30 G40 G41 G42
G50 G53 G65 G70 G71 G72 G73
G75 G80 G83 G85 G87 G89 G90
G94 G96 G97 G98 G99
(G-code system A)
Machining center system
G00 G01 G02 G03 G04 G22 G23
G25 G26 G28 G30 G40 G41 G42
G43 G44 G49 G53 G65 G73 G76
G80 G81 G82 G83 G85 G86 G87
G88 G89 G82 G94 G95 G96 G97
NOTE
1 In Small-Holl Pecking Drilling Cycle(G83),
backward movement is prohibited.
2 In forward movement of Boring Cycle(G88), the
sequence of actions at bottom of holl is shown as
follows (dwell -> stop of spindle motor -> hold
state). But in backward movement, that is (rotation
of spindle -> hold state -> dwell after restart).
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1098 -
- M-code
If there is M-code in the same group is commanded in previous blocks,
modal information of the M-code, commanded at the last in previous
blocks, is output.
If no M-code is commanded in previous blocks, the M-code set to the
first parameter in the same M-code group is output.
If M-code is not set to group M-code in parameter, the same M-code
is output in backward movement.
If the parameter RVN(6400#5) is set to "1", the backward movement
is prohibited when the M-code, which is not set to group M-code, is
commanded in backward movement.
NOTE
When setting the parameter RVN, backward
movement prohibition is enabled except the
M-code which was set in the grouping but
backward movement can be enabled for the
following M-code exceptionally.
1. Subprogram Call by M98/M99.
2. Subprogram Call using an M code
3. Macro Call using an M code
4. Waiting M code
5. M0
Example) Output of M-codes that are set to groups by parameters in
backward movement
Setting of parameters:
No.6400#2=1, #3=0 (5 M-codes/group and 16 groups)
No.6411=100
No.6412=101
No.6413=102
No.6414=103
No.6415=104
No.6416=200
No.6417=201
No.6418=202
No.6419=203
No.6420=204
Program O10 is executed in forward movement from N1 to N15 and
backward movement is executed from N15. In backward movement,
the output of M-codes is shown as next table.
Forward movement Backward movement
O10;
N1G4X1.;
N2M101; M101 M100 (*1)
N3G4X1.;
N4M204; M204 M200 (*1)
N5G4X1.;
N6M104; M104 M101 (*2)
N7G4X1.;
Group A
Group B
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1099 -
Forward movement Backward movement
N8M300; M300 M300
N9G4X1.;
N10M200; M200 M204 (*1)
N11G4X1.;
N12M0; M0 M0 (*3)
N13G4X1.;
N14M102; M102 M104 (*2)
N15G4X1.; Backward movement starts from this block
M2;
*1 No M-code in the same group is commanded before this block,
so the M-code, which is set in the 1st. parameter of the same
group, is output.
*2 M-code in the same group is commanded before this block, so
the M-code, which is commanded at the last before this block, is
output.
*3 M-code is not set to group M-code, so the same M-code is
output.
- S and T-code
A modal value of the previous block is output.
When movement command and S-code or T-code is commanded in
the same block, the timing of the output of the S-code and T-code is
different. Because, the timing where S-code and T-code are output at
the forward movement is different from that at the backward
movement. By setting bit 7 (STO) of parameter No.6401 to "1", the
timing of the output of S and T code at the forward movement is the
same as the one at the backward movement.
Example)
T-code output timing at the backward movement
T-code is output as follows when the program proceeds
backward after the forward movement to N8 block.
Backward movement Forward
movement Parameter
STO=0
Parameter
STO=1
O1000;
N1G98G00X0Z0; Default T output
N2G00X-10.T11; T11 output Default T output
N3G00X100.; T11 output
N4G00X10.Z20.T22; T22 output T11 output No T code output
N5G00X30.Z30.;
N6G00X-10.Z-20.; T22 output
N7G00X50.Z40.T33; T33 output T22 output T33 output
N8G04X5.; (Backward start) (Backward start)
M30;
The “Default T” means a T-code status at N1 block in forward
movement. If the status is T0, “T0” signal is output as “Default T”
in the backward movement.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1100 -
The timing of T-code output of N7 and N8 in O1000 shown in the
example above is as follows.
N6
N7 N8
T33 output
Forward movement :
with T22
N6
N7 N8
T22 output
Backward movement (When parameter STO is set to “0”) :
N6
N7 N8
T33 output
Backward movement (When parameter STO is set to “1”) :
T22 output
- Direction change prohibition
The direction change prohibition is a state not changing the direction
where the program is executed.
In the state, even if the rotating direction of a manual handle is
reversed, the reversed rotation is ignored. A manual handle must be
rotate in the same direction as present direction for removing this
state.
The direction change prohibition can be confirmed by output signal
MNCHG<Fn091.1>.
It becomes the change prohibition state under the following condition.
• While the block with the code waiting for FIN is executing
• After a block has done and until the next block begins to operate
• During thread cutting
• Modal G code of G68.1, G68 and G51.2
• The block with the axis that ends movement earlier in the block
with G02 or nonlinear type position (G00) etc.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1101 -
- Backward movement prohibition
The backward movement prohibition is a state that the program cannot
be executed from a certain block backward. In this state, the negative
rotation of a manual handle is ignored, and the only positive rotation
is effective. The program must be executed forward by rotating a
manual handle in the positive direction for removing this state.
The backward movement prohibition can be confirmed by output
signal MRVSP<Fn091.2>.
If the following blocks are executed in backward movement,
backward movement is prohibited.
• Program number block of main program (except subprogram and
macro program)
• Over the maximum number of the blocks for reverse movement
• The block including backward movement prohibition G-code
(which is not described in the paragraph "G-code")
• The block which is executed while in modal including backward
movement prohibition G-code (which is not described in the
paragraph "G-code")
- Status display
In manual handle retrace, the status of manual handle retrace is
displayed on clock display of CNC state display line. This status
display is displayed during the execution of manual handle retrace.
The clock is displayed usually.
When the all condition is filled, "M.H.RTR." is displayed on clock
display of CNC state display line. This status is displayed by the color
of color number 3 (INPUT KEY, O/N NO. and STATUS are the same
color). The screen display is as shown in Fig.3.12(a). When the
following conditions are not full, the clock is displayed.
• When bit 2 (CHS) of parameter No.6401 is set to "0":
1) Software option of handle manual retrace is enabled.
2) Status display disable/enable bit 6 (HST) of parameter
No.6401 is set to "1".
3) Check mode confirmation signal MMMOD<Fn091.3> is set
to "1".
• When bit 2 (CHS) of parameter No.6401 is set to "1":
1) Software option of handle manual retrace is enabled.
2) Status display disable/enable bit 6 (HST) of parameter
No.6401 is set to "1".
3) Cycle start signal STL<Fn000.5> is set to "1".
4) Check mode signal MMOD<Gn067.2> is set to "1".
5) Manual handle check signal MCHK<Gn067.3> is set to "1".
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1102 -
Fig. 3.12 (a) "M.H.RTR." status display
Besides, when reverse movement prohibition signal
MRVSP<Fn091.2> is set to "1",
the "NO RVRS." is displayed. This status is displayed by
blinking/reversing in the color of color number 1 (ALARM is the
same color). The screen display is as shown in Fig.3.12(b). When
reverse movement prohibition signal MRVSP<Fn091.2> is set to "0",
the " M.H.RTR." is displayed again.
Fig. 3.12 (b) " NO RVRS." status display
Besides, when direction change prohibition signal
MNCHG<F0091.1> is set to "1" and the direction of program’s
execution is changed by manual handle, this status display changes
from "M.H.RTR." to "NO.CHAG.".
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1103 -
This status is displayed by blinking/reversing in the color of color
number 3 (INPUT KEY, O/N NO. and STATUS are the same color) .
The screen display is shown as Fig.3.12(c). When the program is
executed in the direction as the same as before by manual handle or
direction change prohibition signal MNCHG<Fn091.1> is set to "0",
the " M.H.RTR." is displayed again.
Moreover, when parameter FWD(No.6400#1) is set to "1" and the
program is executed to change direction by manual handle, this status
display changes from "M.H.RTR." to "NO.CHAG.".
NOTE
When the improvement of direction change
movement in auxiliary function output block is
enabled, the state of direction change prohibition
signal MNCHG<Fn091.1> is set to "1" and direction
change is possible. Therefore please note that the
status display of the direction change prohibition is
displayed though it is possible to direction change.
Fig. 3.12 (c) "NO.CHAG." status display
Limitation
- Movement in automatic operation by DNC operation mode(RMT)
In the automatic operation by DNC operation mode(RMT), the
backward movement is prohibited though the forward movement is
enable.
- Movement in subprogram operation by external subprogram call
In M198 or M-code for subprogram operation by external subprogram
call (parameter No.6030), the backward movement is prohibited
though the forward movement is enable.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1104 -
- Movement command and M,S,T-code
When M,S,T-codes and movement commands are in the same block,
the timing outputting codes changes between in forward movement
and backward movement. Therefore, M, S, T-codes should be
commanded in backward movement after confirming that "DEN"
signal is set to "1".
Example of executing the following programs with lathe system
O0001 ;
M5 S0 F0 ;
G53 X0 Z0 ;................................ (1)
G1 W100 M3 S100 F1. ; ............ (2)
G0 U50. W50. ;........................... (3)
M2 ;
[Forward movement]
(1)G53 X0 Z0
(3) G0 U50 W50
(2) G1 W100.
M3 S100 F1.
The block of (2) moves with M3 S100 F1.
[Backward movement]
(1)G53 X0 Z0
(3) G0 U50. W50.
(2)G1 W100.
M5 S0 F1.
The block of (2) moves with M5 S0 F1.
- Non linear interpolation type positioning
In the non-linear interpolation type positioning, the route is different
between forward movement and backward movement.
X
Z
The route of forward movement
The route of backward movement
Please use the interpolation type positioning to ward off danger. (Set
the bit 1 (LRP) of parameter No.1401 to "1")
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1105 -
- Threading in forward movement
Threading (G32,G76,G84,G88,G92) is always executed at 100%
override speed. That is to say, a pulse generated by a manual handle is
ignored in executing a threading block. In thread cutting cycle, the
pulse is invalid at the time actually cutting thread, but the one are
valid in the other movements.
- Macro
In macro statement, the setting, operation, and so on of the macro
variable is executed in only first forward movement. That is to say, the
setting, operation, and so on of the macro variable is never executed in
the block executing them once.
- Axis control by PMC
The movement of axis control by PMC cannot be controlled by this
function.
- Multiple path simultaneous check in the multi-path system
When using the manual handle retrace function at the same time in
multiple paths, the timing of block operation may slightly differ
between these paths due to the repetition of forward and backward
motion or differences in the rotation speed of the manual handle. To
synchronize block operation between the paths, use the wait M code.
- Check of path unit by multi-path system
In the multi-path system, the program check of an arbitrary path is
possible. In the path not to check, please select the mode excluding the
MEM mode. Even if bit 4 (HMP) of parameter No.6400 is set to "1",
it is possible to execute the check of forward movement, direction
change and backward movement.
If waiting M code exist in the program, please set No-wait signal of
two path NOWT <Gn063.1>, or No-wait signal of three path
NMWT<Gn063.7> to "1".
- Modal display
In the backward movement with manual handle, the modal display is
updated according to the operation condition of the program.
- Modal information
In the backward movement with manual handle, the state of modal
information is updated according to the operation condition of the
program.
- Change in operation mode
When you change to EDIT mode during the checking mode, the
backward movement and the re-forward movement cannot be
executed in the blocks which have been already executed.
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1106 -
- ON/OFF of Manual Handle Retrace mode
When check mode signal MMOD<Gn067.2> is set to "0" and handle
available signal in checking mode MCHK<Gn067.3> is set to "0", the
check mode might not be turned off at once.
Basically, in the middle of block, the check mode doesn't switch from
ON to OFF or from OFF to ON. After the block is ended, the check
mode switches from ON to OFF or from OFF to ON.
- AI contour control
If the checking mode signal MMOD<Gn067.2> is "1", AI contour
control mode(G05.1Q1) is canceled. If AI contour control is canceled,
forward movement and backward movement can be executed.
Furthermore, if the signal MMOD<Gn067.2> is set to "1" in AI
contour control mode, the checking mode is not effective until AI
contour control mode is invalid(G05.1Q0).
- Multi Spindle
During the backward movement, both TYPE-A and TYPE-B multi
spindle control may not be operated exactly.
- Path Table Operation
In path table operation, the backward movement is prohibited.
Furthermore, in forward movement, regardless of manual handle, the
motion is performed as the command of path table operation.
- Execution of measurement G-code with the speed of override 100%
When bit 6 (MGO) of parameter No.6400 is set to "1", a handle pulse
is invalid and it is always executed at 100% override. When bit 6
(MGO) of parameter No.6400 is set to "0", this function is invalid and
a handle pulse is valid.
In the multi-path system, this function is not effective in the execution
of another path and handle pulse is valid in another path. The
measurement G code to which this function is effective is as follows.
1) G31 for skip
2) G31, G31P1, G31P2, G31P3, G31P4, G04, G04Q1, G04Q2,
G04Q3 and G04Q4 for multistage skip
3) G31P99 and G31P98 for torque limit skip
When the measurement by G36 and G37 (G37.1 and G37.2 when bit
3(G36) of parameter No.3405 is set to "1") of automatic tool
compensation is executed, a handle pulse is invalid and it is always
executed at 100% override regardless of setting bit 6 (MGO) of
parameter No.6400. At the rapid traverse before measurement, handle
pulse is valid.
When bit 7 (SKF) of parameter No.6200 is set to "0" and bit 2 (SFN)
of parameter No.6207 is set to "0", handle pulse at G31 is invalid and
it is always executed at 100% override regardless of setting bit 6
(MGO) of parameter No.6400.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1107 -
When bit 7 (MG4) of parameter No.6400 is set to "1" and the software
option of multistage skip is enabled and the setting of parameter from
No.6202 to No.6206 is enabled, the backward movement prohibition
is enabled in G04 block for multistage skip.
The G code to which this function is effective is as follows.
1) G04, G04Q1, G04Q2, G04Q03 and G04Q4 for multistage skip
- Relation to another function
This function cannot coexist with the following functions
• Retrace
• Learning control for parts cutting
• Preview repetitive control
• Learning control
3.MANUAL OPERATION OPERATION B-63944EN/03
- 1108 -
3.13 AUXILIARY FUNCTION OUTPUT BLOCK REVERSE
MOVEMENT FOR MANUAL HANDLE RETRACE
Overview
This function enables reverse movement during manual handle retrace
even if a move command and an auxiliary function (M/S/T/B code)
are specified in the same block.
This is an optional function.
Explanation
Reverse movement is enabled for an auxiliary function output block if
all the conditions and sequences described below are met.
<1> The function is effective when bit 0 (ADC) of parameter No.
6401 (auxiliary function output block reverse movement enable
parameter) is set to "1".
<2> The function is effective when a move command and an auxiliary
function (M/S/T/B code) are specified in the same block.
<3> If the rotation of the manual pulse generator is reversed when all
the conditions mentioned in <1> and <2> are met, the NC sets
auxiliary function output block reverse movement enable output
signal ADCO<Fn091.5> to "1".
<4> When auxiliary function output block reverse movement enable
output signal ADCO<Fn091.5> is set to "1", the PMC performs
the corresponding operation with a ladder language program.
After that, set finish signal FIN<Gn004.3> to "1". This enables
the NC to move the axis in reverse direction (move it backward
or move it forward again).
<5> When finish signal FIN<Gn004.3> is set to "1", the NC sets
ADCO<Fn091.5> to "0" and starts to move the axis in reverse
direction (move it backward or move it forward again).
As for parameter-grouped M codes or S or T codes, those of the
previous one block are output. As for M codes that are not
grouped by parameter or B codes, the same codes as for the
forward movement are also output for the reverse movement.
The figure below presents a timing chart depicting this process. The
chart shows an example of M codes.
This example describes how an auxiliary function is executed after
waiting for the move command to complete (distribution end signal
DEN) following the reverse movement.
It is also possible to execute an auxiliary function without waiting for
the move command to complete after the reverse movement.
B-63944EN/03 OPERATION 3.MANUAL OPERATION
- 1109 -
M command Mxxx
Move command
Code signals M00 to M31
Strobe signal MF
Operation on PMC side
Reverse movement enable output signal ADCO
Finish signal FIN
Distribution end signal DEN
<3> <4> <5>
Notes
NOTE
1 When a single auxiliary function is specified
individually, carry out the regular auxiliary function
completion sequence. Reverse movement
becomes possible after moving to the next (or
previous) block.
2 If a move command and an auxiliary function are
specified in the same block and if no travel
distance remains after movement, carry out the
regular auxiliary function completion sequence.
Reverse movement becomes possible after moving
to the next (or previous) block.
3 To enable reverse movement using this function
when an M code other than grouped M codes and
a move command are specified in the same block,
set bit 5 (RVN) of parameter No. 6400 to "0".
4 This function is not supported for M02 or M30.
5 If an auxiliary function is specified in a block having
no move command, such as G70, carry out the
regular auxiliary function completion sequence.
Reverse movement becomes possible after moving
to the next (or previous) block.
6 This function is optional.
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1110 -
4 AUTOMATIC OPERATION
Programmed operation of a CNC machine tool is referred to as
automatic operation.
This chapter explains the following types of automatic operation:
4.1 MEMORY OPERATION.......................................................1111
Operation by executing a program registered in CNC memory
4.2 MDI OPERATION.................................................................1114
Operation by executing a program entered from the MDI panel
4.3 DNC OPERATION ................................................................1118
Function for executing a program while reading the program
from an input device connected to the reader/puncher interface or
a memory card.
4.4 SCHEDULE OPERATION....................................................1121
Function for executing a program while reading the program
from an input device connected to the reader/puncher interface or
a memory card according to a schedule.
4.5 EXTERNAL SUBPROGRAM CALL (M198) ......................1124
Function for calling and executing subprograms (files) registered
in an external input/output device during memory operation
4.6 MANUAL HANDLE INTERRUPTION ...............................1127
Function for performing manual feed during movement executed
by automatic operation
4.7 MIRROR IMAGE ..................................................................1134
Function for enabling mirror-image movement along an axis
during automatic operation
4.8 PROGRAM RESTART..........................................................1136
Restarting a program for automatic operation from an
intermediate point
4.9 TOOL RETRACT AND RECOVER .....................................1149
Function for retracting the tool to a desired position
4.10 RETRACE ..............................................................................1161
Function for executing a program in the reverse direction.
4.11 ACTIVE BLOCK CANCEL ..................................................1172
Function for stopping operation and canceling the remaining
movement by inputting a signal during automatic operation.
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1111 -
4.1 MEMORY OPERATION
Programs are registered in memory in advance. When one of these
programs is selected and the cycle start switch on the machine
operator's panel is pressed, automatic operation starts, and the cycle
start LED goes on.
When the feed hold switch on the machine operator's panel is pressed
during automatic operation, automatic operation is stopped
temporarily. When the cycle start switch is pressed again, automatic
operation is restarted.
When the key on the MDI panel is pressed, automatic
operation terminates and the reset state is entered.
For the multi-path control, the programs for the multiple paths can be
executed simultaneously so the multiple paths can operate
independently at the same time.
The following procedure is given as an example. For actual operation,
refer to the manual supplied by the machine tool builder.
Memory operation
Procedure
1 Press the MEMORY mode selection switch.
2 Select a program from the registered programs. To do this,
follow the steps below.
2-1 Press key to display the program screen.
2-2 Press address
key.
2-3 Enter a program number using the numeric keys.
2-4 Press the [O SRH] soft key.
3 For the multi-path control, select the path to be operated with the
path selection switch on the machine operator's panel.
4 Press the cycle start switch on the machine operator's panel.
Automatic operation starts, and the cycle start LED goes on.
When automatic operation terminates, the cycle start LED goes
off.
5 To stop or cancel memory operation midway through, follow the
steps below.
a. Stopping memory operation
Press the feed hold switch on the machine operator's panel.
The feed hold LED goes on and the cycle start LED goes
off. The machine responds as follows:
(i) When the machine was moving, feed operation
decelerates and stops.
(ii) When dwell was being performed, dwell is stopped.
(iii) When M, S, or T was being executed, the operation is
stopped after M, S, or T is finished.
When the cycle start switch on the machine operator's panel
is pressed while the feed hold LED is on, machine operation
restarts.
b. Terminating memory operation
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1112 -
Press the key on the MDI panel.
Automatic operation is terminated and the reset state is
entered.
When a reset is applied during movement, movement
decelerates then stops.
Explanation
- Memory operation
After memory operation is started, the following are executed:
(1) A one-block command is read from the specified program.
(2) The block command is decoded.
(3) The command execution is started.
(4) The command in the next block is read.
(5) Buffering is executed. That is, the command is decoded to allow
immediate execution.
(6) Immediately after the preceding block is executed, execution of
the next block can be started. This is because buffering has been
executed.
(7) Hereafter, memory operation can be executed by repeating the
steps (4) to (6).
- Stopping and terminating memory operation
Memory operation can be stopped using one of two methods: Specify
a stop command, or press a key on the machine operator's panel.
• The stop commands include M00 (program stop), M01 (optional
stop), and M02 and M30 (program end).
• There are two keys to stop memory operation: The feed hold key
and reset key.
- Program stop (M00)
Memory operation is stopped after a block containing M00 is executed.
When the program is stopped, all existing modal information remains
unchanged as in single block operation. The memory operation can be
restarted by pressing the cycle start button. Operation may vary
depending on the machine tool builder. Refer to the manual supplied
by the machine tool builder.
- Optional stop (M01)
Similarly to M00, memory operation is stopped after a block
containing M01 is executed. This code is only effective when the
Optional Stop switch on the machine operator's panel is set to ON.
Operation may vary depending on the machine tool builder. Refer to
the manual supplied by the machine tool builder.
- Program end (M02, M30)
When M02 or M30 (specified at the end of the main program) is read,
memory operation is terminated and the reset state is entered.
In some machines, M30 returns control to the top of the program. For
details, refer to the manual supplied by the machine tool builder.
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1113 -
- Feed hold
When Feed Hold button on the operator's panel is pressed during
memory operation, the tool decelerates to a stop at a time.
- Reset
Automatic operation can be stopped and the system can be made to
the reset state by using key on the MDI panel or external reset
signal. When reset operation is applied to the system during a tool
moving status, the motion is slowed down then stops.
- Optional block skip
When the optional block skip switch on the machine operator's panel
is turned on, blocks containing a slash (/) are ignored.
- Cycle start for the multi-path control
For the multi-path control, a cycle start switch is provided for each
path. This allows the operator to activate a single paths to operate
them at the same time in memory operation or MDI operation. In
general, select the path to be operated with the path selection switch
on the machine operator's panel and then press the cycle start button to
activate the selected path. (The procedure may vary with the machine
tool builder. Refer to the appropriate manual issued by the machine
tool builder.)
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1114 -
4.2 MDI OPERATION
In the MDI mode, a program consisting of up to 511 characters can be
created in the same format as normal programs and executed from the
MDI panel.
MDI operation is used for simple test operations.
The following procedure is given as an example. For actual operation,
refer to the manual supplied by the machine tool builder.
MDI Operation
Procedure
1 Select the MDI mode.
For the multi-path control, select the path for which a program is
to be created with the path selection switch. Create a separate
program for each path.
2 Press the key to select the program screen. The following
screen appears:
MDI program screen
At this time, program number “O0000” is inserted automatically.
3 Prepare a program to be executed by an operation similar to
normal program editing. M99 specified in the last block can
return control to the beginning of the program after operation
ends. Word insertion, modification, deletion, word search,
address search, and program search are available for programs
created in the MDI mode.
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1115 -
4 To entirely erase a program created in MDI mode, use one of the
following methods:
a. Enter address
key, then press the key.
b. Alternatively, press the key. In this case, set
parameter MCL (No. 3203#7) to 1 in advance.
5 To execute a program, set the cursor on the head of the program.
Push Cycle Start button on the operator's panel. By this action,
the prepared program will start.
(For the multi-path control, select the path to be operated with
the path selection switch on the machine operator's panel
beforehand.) When the program end (M02, M30) or ER(%) is
executed, the prepared program will be automatically erased and
the operation will end.
By command of M99, control returns to the head of the prepared
program.
6 To stop or terminate MDI operation in midway through, follow
the steps below.
a. Stopping MDI operation
Press the feed hold switch on the machine operator's panel.
The feed hold LED goes on and the cycle start LED goes
off. The machine responds as follows:
(i) When the machine was moving, feed operation
decelerates and stops.
(ii) When dwell was being performed, dwell is stopped.
(iii) When M, S, or T was being executed, the operation is
stopped after M, S, or T is finished.
When the cycle start switch on the machine operator's panel
is pressed, machine operation restarts.
b. Terminating MDI operation
Press the key.
Automatic operation is terminated and the reset state is
entered.
When a reset is applied during movement, movement
decelerates then stops.
Explanation
The previous explanation of how to execute and stop memory
operation also applies to MDI operation, except that in MDI operation,
M30 does not return control to the beginning of the program (M99
performs this function).
- Erasing the program
Programs prepared in the MDI mode will be erased in the following
cases:
• In MDI operation, if M02, M30 or ER(%) is executed.
• When bit 6 (MER) of parameter No. 3203 is set to 1, and the last
block of the program is executed in single block operation
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1116 -
NOTE
In the two cases above, program erasure can be
prevented by setting bit 6 (MKP) of parameter No.
3204 to 1.
• In MEM mode, if memory operation is performed.
• In EDIT mode, if any editing is performed.
• When the
and keys are pressed.
• Upon reset when bit 7 (MCL) of parameter No.3203 is set to 1
NOTE
Upon reset when the parameter MCL = 0, the cursor
moves to the end of the program.
- Restart
If a program is not executed even once after the program is input, the
program is executed from the beginning, regardless of where the
cursor is placed. However, a program is executed starting at the
beginning of the block where the cursor is place, if the program is
stopped for a reason such as single block operation after restart of an
MDI operation then is restarted after an editing operation.
CAUTION
When an MDI program is restarted, the program is
executed starting at the beginning of the block
where the cursor is placed, regardless of the cursor
position in the block.
(Example)
When the cursor is placed on G90
:
G91 X100.0 G90Y200.0 Z300.0 ;
:
The program is executed starting at the
beginning (namely, G91) of this block. So, the
tool moves by 100.0 along the X-axis in the
incremental programming, and moves to 200.0
and 300.0 along the Y-axis and Z-axis,
respectively, in the absolute programming.
- Editing a program during MDI operation
A program can be edited during MDI operation. By setting bit 5
(MIE) of parameter No. 3203 to 1, editing can be disabled. However,
even when bit 5 (MIE) of parameter No. 3203 is set to 1, editing can
be enabled by resetting the operation.
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1117 -
- Absolute/incremental command
When bit 4 (MAB) of parameter No. 3401 is set to 1, the
absolute/incremental programming of MDI operation does not depend
on G90/G91. In this case, the incremental programming is set when
bit 5 (ABS) of parameter No. 3401 is set to 0, and the absolute
programming is set when bit 5 (ABS) of parameter No. 3401 is set to
1.
Parameter MAB
(No.3401#4)=0 Parameter MAB (No.3401#4)=1
Parameter ABS
(No.3401#5)=0
Parameter ABS
(No.3401#5)=1
Absolute mode
operation with G90
command, and
incremental
programming operation
with G91 command
Incremental mode
operation at all times,
independent of
G90/G91 command
Absolute mode
operation at all times,
independent of
G90/G91 command
NOTE
When G code system A is used on a lathe system,
the parameters MAB and ABS are invalid.
Limitation
- Program registration
Programs created in MDI mode cannot be registered.
- Number of characters in a program
A created program can consist of up to 511 characters including
"O0000" automatically inserted.
- Subprogram nesting
The subprogram call command (M98) can be described in a program
created in MDI mode. That is, programs that are registered in
memory through MDI operation can be called and executed. The
level of subprogram call nesting is the same as in MEM operation.
- Macro call
When the custom macro function is enabled, a macro program can be
created and executed even in the MDI mode. Moreover, a macro
program can be called for execution.
NOTE
The GOTO statement, WHILE statement, and DO
statement cannot be executed in a program
created in the MDI mode. An alarm PS0377 is
issued.
When a program including those statements is to
be executed, register the program in the program
memory then call the program for execution.
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1118 -
4.3 DNC OPERATION
By activating automatic operation during the DNC operation mode
(RMT), it is possible to perform machining (DNC operation) while a
program is being read in via reader/puncher interface.
To use the DNC operation function, it is necessary to set the
parameters related to the reader/punch interface in advance.
The procedure described below is just an example. For actual
operation, refer to the relevant manual of the machine tool builder.
DNC operation
Procedure
1 Press the REMOTE switch on the machine operator's panel to
enter the RMT mode.
2 Select the program to be executed.
• Selecting a DNC operation file
On the memory card (or floppy cassette) list screen, move
the cursor to the file to be subjected to DNC operation and
press "DNC SET" to select the file to be subjected to DNC
operation. (The selected file is marked with "D".)
• Releasing a DNC operation file
On the memory card (or floppy cassette) list screen, move
the cursor to the file for which DNC operation is released
and press "DNC CLEAR" to release the DNC operation file.
(The "D" mark for the file is removed.)
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1119 -
3 Press the cycle start switch to execute the selected file. For
details on the REMOTE switch, refer to the manual provided by
the machine tool builder.
4 During DNC operation, executed programs are listed on the
program check screen and program screen.
Fig. 4.3 (a) PROGRAM screen
Fig. 4.3 (b) PROGRAM CHECK screen
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1120 -
NOTE
1 Before selecting a DNC operation file, be sure to
release all schedule data. DNC operation and
schedule operation cannot be specified at the
same time.
2 A DNC operation file cannot be released during
DNC operation.
3 To switch between devices when DNC settings are
made, release the settings and then make the
settings again.
Explanation
During DNC operation, subprograms and macro programs stored in
memory can be called.
Limitation
- M198 (command for calling a program from within an external input/output unit)
In DNC operation, M198 cannot be executed. If M198 is executed,
alarm PS0210 is issued.
- Custom macro
In DNC operation, custom macros can be specified, but no repeat
instruction and branch instruction can be programmed. If a repeat
instruction or branch instruction is executed, alarm PS0123 is issued.
- M99
For returning from a subprogram or macro program to the calling
program during DNC operation, the specification of a return command
(M99P...) with a sequence number specified is not allowed.
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1121 -
4.4 SCHEDULE OPERATION
To perform schedule operation, select files (programs) registered in a
memory card and specify the sequence of execution and the repetition
count of each program.
Schedule operation
Procedure
1 Press the REMOTE switch on the machine operator's panel to
enter the RMT mode.
2 Select the program to be subjected to schedule operation.
• Setting a schedule
Move the cursor to the file to be subjected to schedule
operation and press the soft key [SCHEDUL ADD]. The
files registered as schedule data are marked with "S" on the
left sides of their file names. The files are subjected to
schedule operation in the order in which the files are
selected. When settings are made this way, the repetition
count of execution of each file is set to 1. To change the
repetition count or execution order or check the schedule,
press the soft key [SCHEDUL LIST] to display the
schedule list screen.
[SCHEDUL ADD]
Adds the file at the cursor position as schedule data.
[SCHEDUL DEL]
Deletes the file at the cursor position from schedule data when
the file is registered as schedule data.
[SCHEDUL LIST]
Lists the settings of schedule data to edit the repetition count or
the like (see the next page for details).
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1122 -
• Editing a schedule
To edit schedule data, press the soft key [SCHEDUL LIST] to
display the schedule list screen, on which schedule data can be
edited.
[FILE UP]
Moves the file at the cursor position up one line and moves the
replaced file down one line.
[FILE DOWN]
Moves the file at the cursor position down one line and moves
the replaced file up one line.
[DELETE]
Deletes the file at the cursor position and moves the files below
the cursor up one line.
[INSERT]
Moves the files below the cursor down one line.
[ALL DELETE]
Deletes all records.
3 Press the cycle start switch to execute the selected files. For
details on the REMOTE switch, refer to the manual provided by
the machine tool builder.
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1123 -
NOTE
1 Before setting schedule operation, release DNC
operation files in the MDI mode. DNC operation
and schedule operation cannot be specified at the
same time.
2 Before starting schedule operation, confirm that
schedule data is set correctly on the schedule list
screen.
3 Schedule data cannot be changed or edited during
schedule operation. Before changing schedule
data, make a reset to stop operation.
Restrictions
- Repetition count
The maximum repetition count during schedule operation is 9999.
When a negative value is specified, an endless loop (LOOP display) is
assumed. The file for which 0 is set is skipped and processing
proceeds to the next file.
- Number of registered files
The maximum number of programs that can be registered as schedule
setting data is 20.
- Selectable files
The files to be selected as schedule setting data must be registered in
the same directory. (Files in the different directories cannot be
selected.)
- M code
Even if a code other than M02 and M30 in the execution program is
executed, the current count on the schedule execution status screen is
not increased.
- Floppy disk directory display during execution of a file
During schedule operation, directories in a floppy disk cannot be
displayed in a background edit.
- Intervention during automatic operation
Intervention in schedule operation cannot be performed during
automatic operation.
- During multipath control
The scheduling function cannot be used by multiple paths at the same
time.
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1124 -
4.5 EXTERNAL SUBPROGRAM CALL (M198)
During memory operation, you can call and execute a subprogram
registered in an external device (such as a Memory Card, Handy File,
or Data Server) connected to the CNC.
Format
M198 Pxxxxxxxx Lyyyyyyyy ;
↑ ↑
Pxxxxxxxx : Program number (or file number)
Lyyyyyyyy : Number of repetitive calls
When address L is omitted, the number of repetitive calls is
assumed to be 1.
FS16 compatible command format
(The following command format is valid only when a 4-digit
program number is used.)
M198 Pxxxx yyyy ;
↑ ↑
xxxx : Number of repetitive calls
yyyy : Program number (or file number)
When the number of repetitive calls is omitted, it is assumed
to be 1.
Explanation
M code M198 specifies an external subprogram call. You can also
call an external subprogram using an M code set in parameter No.
6030. (When an M code other than M198 is set as an M code for
calling an external subprogram, M198 is executed as a normal M
code.)
Specify a program number (file number) registered in an external
device at address P. If the specified program number (file number) is
not registered in the connected external device, an alarm (PS1079) is
issued.
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1125 -
Example)
M198 P0123 L3;
This command specifies that the subprogram having
external subprogram number O0123 is to be called three
times repeatedly.
The subprogram is called from the main program and
executed as follows:
Main program Sub program
12 3
N0010 ... ;
N0020 ... ;
N0030 M198 P0123 L3 ;
N0040 ... ;
N0050 ;
N0060 ... ;
0123 ... ;
N1020 ... ;
N1030 ... ;
N1040 ... ;
N0050 ... ;
N1060 ... M99 ;
- Program number call
You can also specify a subprogram call with its program number
instead of the file number by the setting of bit 2 (SBP) of parameter
No. 3404.
NOTE
1 An external subprogram call can be specified only
during program operation in the MEM mode and
cannot be specified in the MDI mode.
2 An external subprogram call is available for the
following external devices:
External device name Program
number call File number call
Handy File Available Available
FLOPPY CASSTTE Available Available
Memory Card Available Unavailable
Data Server Available Unavailable
3 To perform a subprogram call using a Memory
Card as the external device, set bit 7 (MNC) of
parameter No. 138 to 1 and I/O channel (parameter
No. 0020) to 4.
A program number call is always enabled
regardless of the setting of bit 2 (SBP) of
parameter No. 3404.
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1126 -
NOTE
4 An external device subprogram call cannot be
performed from a subprogram called using another
external device subprogram call. (An alarm
(PS1080) is issued.)
Main program
(internal memory)
M198
Sub program
(External device)
M198
Sub program
(External device)
Cannot be
called.
(Alarm)
Can be called.
5 A subprogram registered in internal memory can be
called from a subprogram called using an external
device subprogram call. From the called
subprogram in internal memory, another external
device subprogram call cannot be performed. (An
alarm (PS1080) is issued.)
Main program
(internal memory)
M198
Sub program
(External
device)
M98
Can be called.
Sub program
(internal
memory)
M198
Sub program
(External
device)
Cannot be called.
(Alarm)
Can be called.
6 A call using the external device subprogram call
function is counted as one level of subprogram
nesting.
7 In a multipath system, an external device
subprogram call cannot be performed
simultaneously from multiple paths.
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1127 -
4.6 MANUAL HANDLE INTERRUPTION
By rotating the manual pulse generator in the automatic operation
mode (manual data input, DNC operation, or memory operation) or in
the memory editing mode, handle feed can be superimposed on
movement by automatic operation. A handle interruption axis is
selected using the manual handle interruption axis selection signal.
The minimum unit of travel distance per scale division is the least
input increment. One of four types of magnifiers selected with MP1
and MP2 <G019.4 and 5> can be applied. With bit 3 (HIT) of
parameter No. 7103, the minimum unit of travel distance can be
further 10 times greater. A handle feed magnifier is selected using
the manual handle feed amount selection signal. (See "MANUAL
HANDLE FEED".)
Programmed
depth of cut
Z
XTool position afte
r
handle interruption
Tool position
during automatic
o
p
eration
Depth of cut
by handle
interruption Workpiece
Fig. 4.6(a) Manual handle interruption
WARNING
The travel distance per scale division by manual
handle interruption is the least input increment as
with manual handle feed. With a machine of
metric input and inch output, for example, the travel
distance per 254 scale divisions is 0.01 inch. With
a machine of inch input and metric output, the
travel distance per 100 scale divisions is 0.254
mm.
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1128 -
Explanation
- Interruption operation
1 When the handle interruption axis selection signal for a handle
interruption axis is set to 1 in the automatic operation mode
(manual data input, DNC operation, or memory operation) or in the
memory editing mode, manual handle interruption can be
performed by rotating the handle of the manual pulse generator.
NOTE
Even when the feedrate override signal sets 0%,
manual handle interruption can be accepted.
2 For the method of selecting a manual handle interruption axis, refer
to the relevant manual of the machine tool builder.
3 The feedrate during manual handle interruption is the sum of
feedrate used for automatic operation and the feedrate used for
movement by manual handle interruption. However, the feedrate
during manual handle interruption is controlled so that it does not
exceed the maximum allowable cutting feedrate for the axis.
Example
Suppose that the maximum allowable cutting
feedrate for an axis is 5 m/min, and that a
movement is made in the + direction at 2 m/min
along the axis. In this case, manual handle
interruption can be accepted even when the manual
pulse generator is rotated up to a speed equivalent
to 3 m/min. Manual handle interruption by rotation
in one direction can be accepted even when the
manual pulse generator is rotated to a speed
equivalent to 7 m/min.
If the manual pulse generator is rotated to a speed
beyond the upper limits, those pulses from the
manual pulse generator that correspond to the
excess are lost, resulting in a mismatch between the
scale mark of the manual pulse generator and the
actually interrupted travel distance.
4 For a magnifier for manual handle interruption, refer to the
relevant manual of the machine tool builder.
5 If the travel direction is reversed as a result of manual handle
interruption, backlash compensation is performed. Pitch error
compensation is performed for the position after interruption.
6 In manual handle interruption, only acceleration/deceleration for
cutting feed is enabled. By setting bit 0 (MNJ) of parameter No.
1606 to 1, acceleration/deceleration for both of cutting feed and
jog feed can be applied to manual handle interruption.
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1129 -
- Manual handle interruption and coordinate system
1 The amount of manual handle interruption shifts the workpiece
coordinate systems and the local coordinate system. So, the
machine moves, but the coordinates in the workpiece coordinate
systems and the local coordinate system remain unchanged.
Regardless of which coordinate system is selected, all workpiece
coordinate systems and the local coordinate system shift by the
same amount.
• Absolute coordinates
→ Remain unchanged by handle interruption.
• Relative coordinates
→ Change by the amount of handle interruption.
• Machine coordinates
→ Change by the amount of handle interruption.
(Machine coordinate system)
(Workpiece coordinate system after
interruption)
(Workpiece coordinate system before
interruption)
Path after
interruption
Programmed path
Shift by manual handle
interruption
2 Even when manual handle interruption is performed, the machine
coordinate system remains unchanged. The absolute command
(G53) in the machine coordinate system is not affected by
manual handle interruption.
(G90G54****)
(G90G53****)
(Machine coordinate system)
(Workpiece coordinate system afte
r
interruption)
(Workpiece coordinate system before
interruption)
Path after
interruption
Programmed path
Shift by manual handle
interruption
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1130 -
3 In automatic reference position return (G28), the end point
(reference position) is not affected by manual handle interruption.
However, the midpoint is in the workpiece coordinate system, so
that the position shifted by the amount of interruption becomes
the midpoint.
- Cancellation of the amount of interruption
Operation by which the workpiece coordinate system shifted by
manual handle interruption from the machine coordinate system is
returned to the original workpiece coordinate system is referred to
cancellation of the amount of interruption.
When the amount of interruption is canceled, the workpiece
coordinate system is shifted by the amount of manual handle
interruption, and the amount of interruption is reflected in the absolute
coordinates.
Interruption shifts the workpiece coordinate system from the machine
coordinate system.
(Machine zero point)
Workpiece
coordinate system
before interruption
Workpiece
coordinate
system after
interruption
Position before interruption
Position after
interruption
Interruption
Workpiece
origin offset
By cancellation, the workpiece coordinate system returns to the state
present before handle interruption.
(Machine zero point)
Workpiece
coordinate system
after cancellation
Workpiece
coordinate
system before
cancellation
Position after
cancellation
Interruption amount
cancellation
Workpiece
origin
offset
In the following cases, the amount of interruption is canceled:
• When a reset is made (when bit 1 (RTH) of parameter No. 7103
is set to 1)
• When emergency stop state is canceled (when bit 1 (RTH) of
parameter No. 7103 is set to 1)
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1131 -
• When a manual reference position return operation is performed
(when G28 is specified before a reference position is established)
• When a reference position is set without dogs
• When the workpiece coordinate system is preset
NOTE
When the amount of interruption is cleared using
soft keys, only the indication of the amount of
interruption becomes 0, and the workpiece
coordinate system remains unchanged.
- Clearing the amount of interruption by soft keys
Clearing of the amount of interruption means that the indication of the
amount of interruption by manual handle interruption is set to 0. The
workpiece coordinate system does not change.
"Clearing all axes" or "Clearing any axis" is performed on the path for
which the amount of manual handle interruption is indicated.
When bit 3 (HLC) of parameter No. 7100 is enabled, soft key
[INTRPT CANCEL], which is used for this operation, appears.
When HLC is disabled, soft key [INTRPT CANCEL] does not appear.
To select "Clearing all axes" or "Clearing any axis", follow the
procedure below.
1 Press function key on the MDI panel.
2 Press function key [HANDLE].
3 Press function key [(OPRT)].
4 To prepare for "Clearing all axes" or "Clearing any axis", press
soft key [INTRPT CANCEL].
To prepare for "Clearing all axes" or "Clearing any axis", perform one
of the following.
• Clearing all axes
Press [INTRPT CANCEL] and then press [ALL AXIS].
• Clearing any axis
- Enter the axis name and then press [INTRPT CANCEL].
- Press [INTRPT CANCEL], enter the axis name, and press
[EXEC].
If an incorrect axis name is entered, a warning message stating
"FORMAT ERROR" appears.
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1132 -
- Relation with other functions
The following table indicates the relation between other functions and
the movement by handle interruption.
Table 4.6(a) Relation between other functions and the movement by
handle interruption
Signals Relation
Machine lock Machine lock is effective. When machine lock is on, no
movement is made due to handle interruption.
Interlock Interlock is effective. When interlock is on, no movement
is made due to handle interruption.
Mirror image
Mirror image is not effective. Interrupt functions on the plus
direction by plus direction command, even if this signal
turns on.
- Position display
The following table shows the relation between various position
display data and the movement by handle interruption.
Table4.6(b) relation between various position display data and the
movement by handle interruption
Signals Relation
Absolute coordinate
value
Handle interruption does not change absolute
coordinates.
Relative coordinate value Relative coordinates are changed by the travel
distance specified by handle interruption.
Machine coordinate
value
Machine coordinates are changed by the travel
distance specified by handle interruption.
- Travel distance display
Press the function key , then press the chapter selection soft key
[HNDL]. The move amount by the handle interruption is displayed.
The following 4 kinds of data are displayed concurrently.
Fig. 4.6 (b)
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1133 -
(a) INPUT UNIT:
Handle interruption move amount in input unit system
Indicates the travel distance specified by handle interruption
according to the least input increment.
(b) OUTPUT UNIT :
Handle interruption move amount in output unit system
Indicates the travel distance specified by handle interruption
according to the least command increment.
(c) RELATIVE:
Position in relative coordinate system
These values have no effect on the travel distance specified by
handle interruption.
(d) DISTANCE TO GO:
The remaining travel distance in the current block has no effect
on the travel distance specified by handle interruption.
The handle interruption move amount is cleared when the manual
reference position return ends every axis.
- Display for five-axis systems or better
Systems having five or more axes provide the same display as the
overall position display. See III-12.1.3.
Note
NOTE
1 In a manual operation mode such as the jog feed
mode, manual handle feed mode, or TEACH IN
HANDLE mode, handle interruption cannot be
performed.
2 During a machine lock or interlock, handle
interruption does not cause movement.
3 Manual handle interruption is disabled for the axis in
any of the following states.
- Follow-up state
- PMC axis control state
4 Manual handle interruption cannot be performed for
the axis specified in the G00 mode.
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1134 -
4.7 MIRROR IMAGE
During automatic operation, the mirror image function can be used for
movement along an axis. To use this function, set the mirror image
switch to ON on the machine operator's panel, or set the mirror image
setting to ON from the MDI panel.
Y
X
Tool
Y-axis mirror image goes on.
Programmed tool
path
Tool path after the
mirror image
function is used
Fig. 4.7 (a) Mirror image
Procedure for mirror image
Procedure
The following procedure is given as an example. For actual operation,
refer to the manual supplied by the machine tool builder.
1 Press the single block switch to stop automatic operation.
When the mirror image function is used from the beginning of
operation, this step is omitted.
2 Press the mirror image switch for the target axis on the machine
operator's panel.
Alternatively, turn on the mirror image setting by following the
steps below:
2-1 Set the MDI mode.
2-2 Press the function key .
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1135 -
2-3 Press the [SETING] soft key for chapter selection to display
the setting screen.
Fig. 4.7 (b) Setting screen
2-4 Move the cursor to the mirror image setting position, then
set the target axis to 1.
3 Enter an automatic operation mode (memory mode or MDI
mode), then press the cycle start button to start automatic
operation.
Explanation
• The mirror image function can also be turned on and off by
setting bit 0 (MIRx) of parameter No.0012 to 1 or 0.
• For the mirror image switches, refer to the manual supplied by
the machine tool builder.
Limitation
The direction of movement during manual operation, the direction of
movement from an intermediate point to the reference position during
automatic reference position return (G28), the direction of approach
during single direction positioning (G60), and the shift direction in a
boring cycle (G76, G87) cannot be reversed.
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1136 -
4.8 PROGRAM RESTART
This function specifies Sequence No. of a block to be restarted when a
tool is broken down or when it is desired to restart machining
operation after a day off, and restarts the machining operation from
that block. It can also be used as a high-speed program check
function.
There are two restart methods: the P-type method and Q-type
method.
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1137 -
Procedure for program restart by specifying a sequence number
Procedure 1
[P TYPE]
1 Retract the tool and replace it with a new one. When necessary,
change the offset. (Go to step 2.)
[Q TYPE]
1 When power is turned ON or emergency stop is released,
perform all necessary operations at that time, including the
reference position return.
2 Move the machine manually to the program starting point
(machining start point), and keep the modal data and coordinate
system in the same conditions as at the machining start.
3 If necessary, modify the offset amount. (Go to step 2.)
Procedure 2
[COMMON TO P TYPE / Q TYPE]
1 Turn the program restart switch on the machine operator's panel
ON.
2 Press key to display the desired program.
3 Find the program head. Press key.
4 Enter the sequence number of the block to be restarted, then
press the [P TYPE] or [Q TYPE] soft key.
If the same sequence number appears more than once, the
location of the target block must be specified. Specify a
frequency and a sequence number.
xxxxx
[Q TYPE]
or
[P TYPE]
Sequence
number
xxxyyyyy
[Q TYPE]
or
[P TYPE]
Sequence number (The rightmost five digits.)
Frequency
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1138 -
5 The sequence number is searched for, and the program restart
screen appears on the LCD display.
Fig. 4.8 (a) Program restart screen
DESTINATION shows the position at which machining is to
restart.
DISTANCE TO GO shows the distance from the current tool
position to the position where machining is to restart. A
number to the left of each axis name indicates the order of axes
(determined by parameter setting) along which the tool moves to
the restart position.
The coordinates and amount of travel for restarting the program
can be displayed for up to four axes. If your system supports
five or more axes, pressing the [RSTR] soft key again displays
the data for the fifth and subsequent axes.
M : Up to 35 most recently specified M codes. The maximum
number of displayed M codes differs depending on the size
of the display.
With 15-inch or 10.4-inch LCD/MDI panel :
Up to 30 M codes
With 7.2/8.4-inch LCD/MDI panel : Up to 6 M codes
T : Two most recently specified T codes
S : Most recently specified S code
B : Most recently specified B code
Codes are displayed in the order in which they are specified.
All codes are cleared by a program restart command or cycle
start in the reset state.
6 Turn the program re-start switch OFF. At this time, the figure
at the left side of axis name DISTANCE TO GO blinks.
7 Check the screen for the M, S, T, and B codes to be executed.
If they are found, enter the MDI mode, then execute the M, S, T,
and B functions. After execution, restore the previous mode.
These codes are not displayed on the program restart screen.
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1139 -
8 Check that the distance indicated under DISTANCE TO GO is
correct. Also check whether there is the possibility that the tool
might hit a workpiece or other objects when it moves to the
machining restart position. If such a possibility exists, move the
tool manually to a position from which the tool can move to the
machining restart position without encountering any obstacles.
9 Press the cycle start button. The tool moves to the machining
restart position at the dry run feedrate sequentially along axes in
the order specified by parameter No. 7310 settings. Machining
is then restarted.
Procedure for program restart by specifying a block Number
Procedure 1
[P TYPE]
1 Retract the tool and replace it with a new one. When necessary,
change the offset. (Go to step 2.)
[Q TYPE]
1 When power is turned ON or emergency stop is released,
perform all necessary operations at that time, including the
reference position return.
2 Move the machine manually to the program starting point
(machining start point), and keep the modal data and coordinate
system in the same conditions as at the machining start.
3 If necessary, modify the offset amount. (Go to step 2.)
Procedure 2
[COMMON TO P TYPE / Q TYPE]
1 Turn the program restart switch on the machine operator's panel
ON.
2 Press key to display the desired program.
3 Find the program head. Press key.
4 Enter the number of the block to be restarted then press the [P
TYPE] or [Q TYPE] soft key. The block number cannot exceed
eight digits.
Bxxxxxxxx
[Q TYPE]
or
[P TYPE]
Block number
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1140 -
5 The block number is searched for, and the program restart screen
appears on the LCD display.
Fig. 4.8 (b) Program restart screen
DESTINATION shows the position at which machining is to
restart.
DISTANCE TO GO shows the distance from the current tool
position to the position where machining is to restart. A
number to the left of each axis name indicates the order of axes
(determined by parameter setting) along which the tool moves to
the restart position.
The coordinates and amount of travel for restarting the program
can be displayed for up to four axes. If your system supports
five or more axes, pressing the [RSTR] soft key again displays
the data for the fifth and subsequent axes.
M : Up to 35 most recently specified M codes. The maximum
number of displayed M codes differs depending on the size
of the display.
With 15-inch or 10.4-inch LCD/MDI panel :
Up to 30 M codes
With 9.5-inch LCD/MDI panel : Up to 6 M codes
T : Two most recently specified T codes
S : Most recently specified S code
B : Most recently specified B code
Codes are displayed in the order in which they are specified.
All codes are cleared by a program restart command or
cycle start in the reset state.
6 Turn the program re-start switch OFF. At this time, the figure
at the left side of axis name DISTANCE TO GO blinks.
7 Check the screen for the M, S, T, and B codes to be executed.
If they are found, enter the MDI mode, then execute the M, S, T,
and B functions. After execution, restore the previous mode.
These codes are not displayed on the program restart screen.
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1141 -
8 Check that the distance indicated under DISTANCE TO GO is
correct. Also check whether there is the possibility that the tool
might hit a workpiece or other objects when it moves to the
machining restart position. If such a possibility exists, move the
tool manually to a position from which the tool can move to the
machining restart position without encountering any obstacles.
9 Press the cycle start button. The tool moves to the machining
restart position at the dry run feedrate sequentially along axes in
the order specified by parameter No. 7310 settings. Machining
is then restarted.
Outputting the M, S, T, and B codes for program restart
After the block to be restarted is searched for, you can perform the
following operations:
1 Before the tool is moved to the machining restart position
<1> The most recently specified M, S, T, and B codes can
automatically be output to the PMC.
The most recently specified S code is output as the
maximum spindle speed when the S code is specified in the
block containing G92 or as the specified spindle speed in
other cases. As the most recently specified S code, only
one S code is displayed on the program restart screen
regardless of whether the S code is specified in the block
containing G92.
<2> While the block to be restarted is being searched for, all
sampled M codes and most recently specified S, T, and B
codes can automatically be output to the PMC. Up to 35
M codes can be sampled. If the number of sampled M
codes exceeds 35, the 35 most recently specified M codes
are output to the PMC.
Switch between operations <1> and <2> using bit 6 (MOA) of
parameter No. 7300.
2 Before the tool reaches the machining restart position
On the program restart screen, you can specify M, S, T, and B
codes from the MDI panel in the MEM or RMT mode without
changing the mode.
Outputting the most recently specified M, S, T, and B codes
When bit 7 (MOP) of parameter No. 7300 is set to 1, pressing the
cycle start switch after searching for the block to be restarted
automatically outputs the most recently specified M, S, T, and B codes
to the PMC before the tool is moved to the machining restart position.
In the single block stop status, after the most recently specified M, S,
T, and B codes are output, pressing the cycle start switch again moves
the tool to the machining restart position.
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1142 -
Outputting all M codes and most recently specified S, T, and B codes
When bit 6 (MOA) of parameter No. 7300 is set to 1, pressing the
cycle start switch after searching for the block to be restarted
automatically outputs all M codes and most recently specified S, T,
and B codes to the PMC before the tool is moved to the machining
restart position.
(Example)
When M10, M11, M12, M13, M14, T0101, S1000, and B10 are
sampled, a program is executed in the format shown below
before the tool is moved to the machining restart position:
M10 T0101 S1000 B10 ;
M11 ;
M12 ;
M13 ;
M14 ;
Outputting M, S, T, and B codes on the program restart screen
When bit 7 (MOP) of parameter No. 7300 is set to 1, you can specify
M, S, T, and B codes from the MDI panel in the MEM or RMT mode
without changing the mode after searching for the block to be
restarted until the tool reaches the machining restart position.
Procedure
1 When the block to be restarted is searched for using the program
restart function, the program restart screen appears. When bit 7
(MOP) of parameter No. 7300 is set to 1, operation soft keys
[OVERSTORE], [ERASE], and [INPUT] are displayed.
Fig. 4.8 (c) Program restart screen (outputting M, S, T, and B codes)
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1143 -
2 Before the tool reaches the machining restart position, pressing
soft key [OVERSTORE] selects the over store mode. In the
over store mode, data can be entered in the M, S, T, and B fields
displayed in the (OVERSTORE) section.
To select the over store mode while the tool is moving to the
machining restart position, hold restart operation by feed hold
and press soft key [OVERSTORE].
Enter M, S, T, and B codes to be output in the (OVERSTORE)
section from the MDI panel.
(Example)
To enter M10, S1000, T101, and B20 in the
(OVERSTORE) section:
<1> Enter M10 from the MDI panel.
<2> Press the [INPUT] key.
You can also enter the S, T, and B codes by performing
steps <1> and <2>.
Fig. 4.8 (d) Program restart screen when M, S, T, and B codes are
output
3 When values have been entered in the (OVERSTORE) section,
pressing the cycle start switch outputs each code in the
(OVERSTORE) section. The values in the (OVERSTORE)
section are cleared.
4 To clear the values entered in the (OVERSTORE) section as M,
S, T, and B codes, press soft key [ERASE]. All entered values
are cleared.
5 Pressing soft key [OVERSTORE] again in the over store mode
cancels the mode. Pressing the reset key also cancels the over
store mode.
6 To continue with restart operation, cancel the over store mode
and press the cycle start switch.
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1144 -
CAUTION
1 The M, S, T, and B codes specified in the over store
mode are not displayed on the program restart
screen.
2 In the over store mode, changing the operation
mode to other than the MEM or RMT mode does not
cancel the over store mode. In this case, no
values can be entered in the (OVERSTORE)
section.
3 In lathe systems, do not specify a T code in the over
store mode. If a T code is specified, it is not
executed.
Explanation
- Block number
When the CNC is stopped, the number of executed blocks is displayed
on the program screen or program restart screen. The operator can
specify the number of the block from which the program is to be
restarted, by referencing the number displayed on the screen. The
displayed number indicates the number of the block that was executed
most recently. For example, to restart the program from the block at
which execution stopped, specify the displayed number, plus one.
The number of blocks is counted from the start of machining,
assuming one NC line of a CNC program to be one block.
(Example 1)
CNC Program Number of blocks
O 0001 ;
G90 G92 X0 Y0 Z0 ;
G01 X100. F100 ;
G03 X01 -50. F50 ;
M30 ;
1
2
3
4
5
(Example 2)
CNC Program Number of blocks
O 0001 ;
G90 G92 X0 Y0 Z0 ;
G90 G00 Z100. ;
G81 X100. Y0. Z120. R-80. F50. ;
#1=#1+1 ;
#2=#2+1 ;
#3=#3+1 ;
G00 X0 Z0 ;
M30 ;
1
2
3
4
4
4
4
5
6
Macro statements are not counted as blocks.
- Storing / clearing the block number
The block number is held in memory while no power is supplied.
The number can be cleared by cycle start in the reset state.
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1145 -
- Block number when a program is halted or stopped
The program screen usually displays the number of the block currently
being executed. When the execution of a block is completed, the
CNC is reset, or the program is executed in single-block stop mode,
the program screen displays the number of the program that was
executed most recently. When a CNC program is halted or stopped
by feed hold, reset, or single-block stop, the following block numbers
are displayed:
Feed hold : Block being executed
Reset : Block executed most recently
Single-block stop : Block executed most recently
For example, when the CNC is reset during the execution of block 10,
the displayed block number changes from 10 to 9.
- MDI intervention
When MDI intervention is performed while the program is stopped by
single-block stop, the CNC commands used for intervention are not
counted as a block.
- Block number exceeding eight digits
When the block number displayed on the program screen exceeds
eight digits, the block number is reset to 0 and counting continues.
Limitation
- P type Restart
In the following conditions, P type restart cannot be performed:
• Automatic operation has not been performed since power-on.
• Automatic operation has not been performed since emergency
stop was released.
• Automatic operation has not been performed since the coordinate
system was changed or shifted (change of the external workpiece
origin offset value).
The block that can be restored properly by P type program restart is a
block for which coordinate system setup or change was performed
most recently before machining was interrupted.
- Restart block
The block where the program is to restart is not necessarily be the
block at which the program was interrupted. You can restart the
program from any block. For P-type restart, however, the block
where the program is to restart must use the same coordinate system as
when program execution was interrupted.
- Single block
When the single-block operation is enabled at the time of a movement
to the restart point, a single-block stop occurs each time an axis
operation takes place. In this case, no MDI operation is allowed.
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1146 -
- Manual intervention
During movement to the restart point, manual intervention is allowed
for an axis for which a return operation has not yet been performed.
However, manual operations do not cause any movement along axes
for which a return operation has already been completed.
- MDI
When the search operation has ended, no move command can be
specified by MDI before axis movement.
- Reset
Do not perform a reset operation during the time from the start of the
search operation of the restart sequence until machining is restarted.
If a reset operation is performed, the restart steps must be performed
again from the beginning.
- Feed hold
If a feed hold operation is performed during the search, the restart
steps must be performed again from the beginning.
- Manual absolute
Every manual operation must be performed with the manual absolute
mode turned on regardless of whether the manual operation is
performed before or after machining.
- Reference position return
Unless an absolute position detector (absolute pulse coder) is provided,
be sure to perform reference position return after power-up, then
perform restart operation.
- Program restart switch
When the program restart switch is on, pressing the cycle start switch
does not start operation.
- Blocks specifying a macro statement, macro call, and subprogram call
Blocks specifying a macro statement, macro call, and subprogram call
are not searched for even when they have a sequence number. In
such a case, search for a block previously preceding such a block.
- Interruption type custom macro
During movement to the machining restart point at a dry run feedrate,
no interruption type custom macro can be started. If an interruption
type custom macro is started, alarm DS024 is issued.
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1147 -
- Commands that prevent program restart
Program restart cannot be performed for blocks placed in the
following modes:
• Cs contouring control
• Polygon turning (G50.2)
• Threading (G32,G33), Circular threading (G35,G36), Threading
cycle (G92), Multiple repetitive threading cycle (G76)
• Polar coordinate interpolation (G12.1)
• Balance cutting (G68)
• Rigid tapping
If any of the following commands is included between the beginning
of a program and the block where the program is to restart, program
restart cannot be performed:
• Workpiece coordinate system preset (G92.1,G50.3)
• Commands for enabling and disabling synchronous/composite
control and superimposed control
• Commands for enabling and disabling axis synchronous control
- M, S, and T commands not usable in over store mode
The M, S, and T functions listed below, unlike the other M, S, and T
functions, have special meanings within the CNC. These M, S, and
T commands cannot be specified from the over store screen. To
specify these commands, cancel the over store mode, and execute
them in MDI operation.
Example:
• Spindle positioning
• Rigid tapping
• Tool management
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1148 -
WARNING
As a rule, the tool cannot be returned to a correct position under
the following conditions.
Special care must be taken in the following cases since none of
them cause an alarm:
- Manual operation is performed when the manual absolute mode
is OFF.
- Manual operation is performed when the machine is locked.
- When the mirror image is used. However, P type return is
possible for a block that switched between ON and OFF most
recently or a subsequent block. In this case, the mirror image
signal status present when the program was interrupted must be
maintained.
- When no coordinate system is set up at the beginning of a
program in which main commands are executed in the
incremental mode.
- When manual operation is performed in the course of axis
movement for returning operation.
- When the program restart is commanded for a block between the
block for skip cutting and subsequent absolute command block.
- When program restart is specified in the machine lock state, then
the machine lock is canceled.
- When program restart specified for an intermediate block for a
multiple repetitive canned cycle
- In general, when a coordinate system is set up, changed, or
shifted after the search operation ends, the tool cannot be
returned to a correct position.
CAUTION
Keep the following in mind when restarting a program including
macro variables.
- Common variable
When the program is restarted, the previous values are inherited
as common variables without being preset automatically. Before
restarting the program, initialize the appropriate variables to the
original values used at start of the previous automatic operation.
- DI/DO
At restart of the program, DI can be read by a system variable, but
DO cannot be output.
- Clock
When the program is being restarted, the clock time can be
obtained by a system variable, but the time cannot be preset.
- Tool offset and workpiece origin offset
When the program is being restarted, the offset can be read by a
system variable, but change of the offset is allowed only for the Q
type.
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1149 -
4.9 TOOL RETRACT AND RECOVER
The tool can be retracted from a workpiece to replace the tool, if
damaged during machining, or to check the status of machining. Then,
the tool can be returned to restart machining efficiently.
Procedure for tool retract and recover
Procedure1 - Programming
Specify a retraction axis and distance in command G10.6IP_
beforehand. In the sample program below, the N20 block specifies
that the Z-axis is the retraction axis and the retraction distance is to be
50 mm.
N30
N10
(Sample program)
N10 G91 Z-50. ;
N20 G10.6 Z50. ;
N30 G01 X150. F500. ;
X
Z
Y
Procedure 2 - Retract
Suppose that the TOOL WITHDRAW switch on the machine
operator's panel is turned on when the tool is positioned at point A
during execution of the N30 block.
N30
A
Machine operator's panel
TOOL BEING
WITHDRAWN
RETRACTION
POSITION
TOOL
WITHDRAW
TOOL
RETURN
Next, the tool withdrawal mode is set and the TOOL BEING
WITHDRAWN LED goes on. At this time, automatic operation is
temporarily halted. The tool is then retracted by the programmed
distance. If point A is the end point of the block, retraction is
performed after automatic operation is stopped. Retraction is based
on linear interpolation. The dry run feedrate is used for retraction.
Upon completion of retraction, the RETRACT POSITION LED on
the operator's panel goes on.
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1150 -
N30
A
Point E
Machine operator's panel
TOOL BEING
WITHDRAWN
RETRACTION
POSITION
TOOL
WITHDRAW
TOOL
RETURN
During retraction, the screen displays PTRR and STRT.
• PTRR blinks in the field for indicating states such as the program
editing status.
• STRT is displayed in the automatic operation status field.
• MTN is displayed in the field for indicating status such as
movement along an axis.
Procedure 3 - Withdrawal
Set the manual operation mode, then withdraw the tool. For manual
operation, either jog feed incremental feed, handle feed, or manual
numerical command is possible.
3
X
Y
Z
1
2
4
56
7
8
910
11
12
Point E
Point A
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1151 -
Procedure 4 - Return
After withdrawing the tool and any additional operation such as
replacing the tool, move the tool back to the previous retraction
position. To return the tool to the retraction position, return the
mode to automatic operation mode, then turn the TOOL RETURN
switch on the operator's panel on then off again. The tool returns to
the retraction position at the dry run feedrate, regardless of whether
the dry run switch is on or off.
When the tool has returned to the retraction position, the
RETRACTION POSITION LED comes on.
X
Y
Z
9
Point A
Point E 1
2
5
3
6
4
7
10
8
11
12
During return operation, the screen displays PTRR and MSTR.
• PTRR blinks in the field for indicating states such as program
editing status.
• MSTR is displayed in the automatic operation status field.
• MTN is displayed in the field for indicating states such as
movement along an axis.
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1152 -
Procedure 5 - Repositioning
While the tool is at the retraction position (point E in the figure below)
and the RETRACTION POSITION LED is on, press the cycle start
switch. The tool is then repositioned at the point where retraction
was started (i.e. where the TOOL WITHDRAW switch was turned on).
Repositioning is based on linear interpolation. The dry run feedrate
is used for repositioning.
N30 A
Point E
Upon completion of repositioning, the tool withdraw mode is
cancelled, and the TOOL BEING WITHDRAWN LED goes off and
restart N30.
Limitation
1 If the origin, presetting, workpiece origin offset value (or
external workpiece origin offset value), or workpiece coordinate
shift amount (for a lathe system) is changed after the retraction
position is specified with G10.6 in the absolute mode, the change
is not reflected in the retraction position. After such changes
are made or the workpiece origin offset value (or external
workpiece origin offset value) or workpiece coordinate shift
amount (for a lathe system) is changed, respectively the
retraction position with G10.6.
2 When retracting the tool manually in the tool withdrawal mode,
do not use the machine lock, mirror-image, or scaling function.
WARNING
The retraction axis and retraction distance
specified in G10.6 must be changed in an
appropriate block according to the figure being
machined. Be very careful when specifying the
retraction distance; an incorrect retraction distance
may damage the workpiece, machine, or tool.
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1153 -
4.9.1 Retract
Explanation
- When no retraction distance is specified
If no retraction distance or direction required for retraction are
specified, retraction is not performed when the TOOL WITHDRAW
switch on the operator's panel is turned on. Instead, the block being
executed in automatic operation is interrupted (automatic operation is
held or stopped). In this state, the tool can be withdrawn and
returned.
N30 Point A
Point E
- Retraction from the automatic operation hold or stop state
When the single block switch is turned on during automatic operation,
or the TOOL WITHDRAW switch is turned on after the automatic
operation hold or stop state is set by feed hold: Retraction is
performed, then the automatic operation hold or stop state is set again.
- Stopping retraction
During retraction, feed hold operation is ignored. However, reset
operation is enabled (retraction is stopped at reset). When an alarm
is issued during retraction, the retraction is stopped immediately.
- Repositioning immediately after retraction
After retraction is completed, tool repositioning can be started without
performing the withdraw and return operations.
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1154 -
4.9.2 Withdrawal
Explanation
- Axis selection
To move the tool along an axis, select the corresponding axis selection
signal. Never specify axis selection signals for two or more axes at a
time.
- Path memorization
When the tool is moved in manual operation along an axis, the control
unit memorizes up to ten paths of movements. If the tool is stopped
after being moved along a selected axis and is then moved along
another selected axis, the position where this switch takes place is
memorized. After ten paths have been memorized, the control unit
does not memorize any additional switching points.
- Reset
Upon reset, memorized position data is lost and the tool withdraw
mode is cancelled.
NOTE
If an attempt is made to move the tool
simultaneously along two axes using the manual
numeric command in the tool withdrawal mode, an
alarm (PS0015) is issued.
4.9.3 Return
Explanation
- Return path
When there are more than ten return paths, the tool first moves to the
tenth position, then to the ninth position, then to the eighth position,
and so forth until the retraction position is reached.
- Single block
The single block switch is enabled during return operation. If the
single block switch is turned off, continuous return operation is
performed. If the single block switch is turned off, the tool stops at
each memorized position. In this case, return operation can be
resumed by turning the TOOL RETURN switch on then off again.
- Interruption of return operation
When an alarm is issued during return operation, return operation
stops.
- Feed hold
The feed hold function is enabled during return operation.
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1155 -
4.9.4 Repositioning
Explanation
- Feed hold
The feed hold function is disabled during repositioning.
- Operation after completion of repositioning
The operation after completion of repositioning depends on the
automatic operation state present when the TOOL WITHDRAW
switch is turned on.
1 When automatic operation is being started
After completion of repositioning, the interrupted execution of
the block is resumed.
2 When automatic operation is held or stopped
After completion of repositioning, the tool stops once at the
repositioned point, then the original automatic operation hold or
stop state is set. When the cycle start switch is pressed,
automatic operation is resumed.
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1156 -
4.9.5 Tool Retract and Recover for Threading
Explanation
- Differences between ordinary tool retract and recover and tool retract and recover
for threading
1 During retraction, chamfering is performed between the specified
retraction axis and threading axis.
2 After retraction, one block that does not specify threading is
executed and the tool stops.
3 When the major axis for threading is specified as the retraction
axis, retraction is not performed by turning the TOOL
WITHDRAW switch on. In this case, after a block that does
not specify threading is executed, an alarm PS0429 is issued and
the tool stops.
4 As repositioning, the tool is returned to the position specified in
the first block that does not specify threading.
- Operation procedure
1 Specify a retraction axis and retraction distance in command
“G10.6IP- -;”.
O1234
G90G0X0Z0 ;
S150 M03 ;
N10 G91 G00 X-50. ;
N20 G10.6 X40.0 ;
N30 G33 Z-100. F2.0 ;
N40 G00 X50. ;
N50 Z100. ;
M02;
Retraction axis: X
Retraction distance: 40.0
N10
N30
N50
N40
b
a
d
c
Threading
X
Z
2 Turn the TOOL WITHDRAW switch during the execution of a
threading command block.
3 The tool withdrawal mode is set and retraction is performed.
Chamfering at 45 degrees is performed between the retraction
axis and major axis for threading using the retraction distance as
the chamfering amount during retraction.
Details of retraction differ depending on whether the remaining
travel distance for the threading command is smaller than the
retraction distance when the TOOL WITHDRAW switch is
turned on as follows:
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1157 -
(1) When remaining travel distance for threading ≥ retraction
distance
d
c
45°
a
b
A
Retraction position
Retraction
distance
When the position where 45-degree chamfering by the
retraction distance ends does not exceed the threading end
position (c), the tool moves to the threading end position
after the termination of chamfering.
(2) When the remaining travel distance for threading <
retraction distance
d
c
a
b
A
Retraction position
Retraction distance
When the position where 45-degree chamfering by the
retraction distance ends exceeds the threading end position
(c), the tool moves to the retraction position along the
retraction axis after it reaches the threading end position.
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1158 -
4 After retraction is completed, the next block that does not specify
threading is executed and the tool stops.
d
c
a
b
Retraction position
Point E
In this example, “X50.0” is specified in the first block that does
not specify threading in the incremental mode, the tool moves to
point E and stops.
If the major axis for threading is specified as the retraction axis,
the block that does not specify threading is executed without
performing retraction, an alarm PS0429 is issued, and the tool
stops.
5 As repositioning, the tool returns to the position specified in the
first block that does not specify threading.
d
c
a
b
Retraction position
Point E
Repositioning
N50
In this example, the repositioning position is point d.
Automatic operation after repositioning starts at the N50 block.
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1159 -
4.9.6 Operation Procedure for a Canned Cycle for Drilling
Explanation
- Retract
When the TOOL WITHDRAW switch is turned on during a canned
cycle for drilling (abbreviated as a canned cycle below), retraction is
performed depending on the cycle operation being executed at that
time.
Operation 1: Positioning to a hole position
Operation 2: Rapid traverse to point R
Operation 3: Hole machining
Operation 4: Operation at the bottom of the hole
Operation 5: Retraction to point R
Operation 6: Rapid traverse to the initial point
Initial point
Point R
Operation 1
Operation 2 Operation 6
Operation 3 Operation 5
Operation 4
1 During operation 1, the tool moves by the retraction distance
specified in G10.6 in the same way as for ordinary retraction.
2 During operation 2, the tool stops operation 2, moves to the
initial point, and stops.
3 During operation 3, the tool stops operation 3, executes cycle
operations 4, 5, and 6 from that position, and stops at the initial
point.
4 During operation 4, 5, or 6, the tool continues the operation and
stops at the initial point.
When the TOOL WITHDRAW switch is turned on during
operation 2 to 6, the tool does not move according to the
retraction specified in G10.6. After the TOOL WITHDRAW
switch is turned on and the tool moves to the initial point,
however, the tool withdrawal mode is set.
When the second or subsequent canned cycle is being executed
and the TOOL WITHDRAW switch is turned on during
operation 2 to 6, the retraction position differs depending on G98
(return to initial level) or G99 (return to point R level).
• G98 (return to initial level): The tool moves to the initial
level.
• G99 (return to point R level):The tool moves to the point R
level.
5 During operation 2 to 6, the tool also moves to the initial point
and stops when the TOOL WITHDRAW switch is turned on
without the G10.6 command specified.
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1160 -
- Repositioning
When the tool is at the retraction position and the cycle start switch is
pressed, repositioning is performed for the canned cycle.
1 Repositioning performed when the TOOL WITHDRAW switch
is turned on during operation 1
After the completion of repositioning, automatic operation is
resumed in the same way as for ordinary repositioning.
2 Repositioning performed when the TOOL WITHDRAW switch
is turned on during operation 2
The canned cycle is reexecuted from operation 2.
3 Repositioning performed when the TOOL WITHDRAW switch
is turned on during operation 3
The canned cycle is reexecuted from operation 2.
4 Repositioning performed when the TOOL WITHDRAW switch
is turned on during operation 4, 5, or 6
The canned cycle is reexecuted for the same hole position from
operation 2.
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1161 -
4.10 RETRACE
M
Overview
The tool can retrace the path along which the tool has moved so far
(reverse execution). Furthermore, the tool can move along the
retraced path in the forward direction (forward reexecution). After
forward reexecution is performed until the tool reaches the position
at which reverse execution started, machining is continued as
programmed.
Procedure
- Forward execution → reverse execution
To perform forward execution of a program, set the “REVERSE”
switch on the machine operator’s panel to off, then perform a cycle
start operation. If the “REVERSE” switch on the machine operator’s
panel is set to on, reverse execution or the end of reverse execution
results.
To perform reverse execution of a program, use one of the following
three methods:
1) Set the “REVERSE” switch on the machine operator’s panel to
on during forward execution of a block.
2) Perform a single block stop operation during forward execution,
then set the “REVERSE” switch on the machine operator’s panel
to on.
3) Perform a feed hold stop operation during forward execution,
then set the “REVERSE” switch on the machine operator’s panel
to on.
When method 1) is used, reverse execution starts after the end of the
block being executed (after execution up to the single block stop
position). Reverse execution does not start as soon as the
“REVERSE” switch on the machine operator’s panel is set to on.
Fig. 4.10 (a)
If functions for gas cutting machine are enabled, however, only when
linear interpolation (G01), circular interpolation (G02, G03), or skip
function (G31) is specified, reverse execution starts at the position at
which the “REVERSE” switch is set to on.
Forward
Reverse
"REVERSE" switch = ON
Cycle start (start of forward execution)
Start of reverse execution
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1162 -
Fig. 4.10 (b)
When method 2) is used, performing a cycle start operation starts
reverse execution from the position at which a single block stop takes
place.
Single block stop
"REVERSE" switch = ON
Cycle start
Cycle start (start of forward execution)
Start of reverse execution
Forward
Reverse
Fig. 4.10 (c)
When method 3) is used, performing a cycle start operation starts
reverse execution from the position at which a feed hold stop takes
place.
Feed hold stop
"REVERSE" switch = ON
Cycle start
Cycle start (start of forward execution)
Start of reverse execution
Forward
Reverse
Fig. 4.10 (d)
- Reverse execution → forward reexecution
To perform forward reexecution of a program, use one of the
following three methods:
1) Set the “REVERSE” switch on the machine operator’s
panel to off during reverse execution of a block.
2) Set the “REVERSE” switch on the machine operator’s
panel to off after a single block stop takes place during
reverse execution.
3) Set the “REVERSE” switch on the machine operator’s
panel to off after a feed hold stop takes place during reverse
execution.
When method 1) is used, forward reexecution starts after the block
being executed ends (after execution up to the position at which a
single block stop takes place). Forward reexecution does not start as
soon as the “REVERSE” switch on the machine operator’s panel is set
to off.
"REVERSE" switch = ON
Cycle start (start of forward execution)
Start of reverse execution
Forward
Reverse
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1163 -
Cycle start (start of forward execution)
Start of forward "REVERSE" switch = OFF
reexecution
Forward
Reverse
Forward
reexecution
Start of reverse execution
Fig. 4.10 (e)
If functions for gas cutting machine are enabled, however, only when
linear interpolation (G01), circular interpolation (G02, G03), or skip
function (G31) is specified, forward reexecution starts at the position
at which the “REVERSE” switch is set to 0.
Fig. 4.10 (f)
When method 2) is used, performing a cycle start operation starts
forward reexecution from the position at which a single block stop
takes place.
Cycle start (start of forward execution)
Start of forward reexecution
Forward
Reverse
Forward
reexecution
Start of reverse execution
Restart of forward execution
Fig. 4.10 (g)
When method 3) is used, performing a cycle start operation starts
forward reexecution from the position at which a feed hold stop takes
place.
Feed hold stop
"REVERSE" switch = OFF
Cycle start
Cycle start (start of forward execution)
Start of forward reexecution
Forward
Reverse
Forward
reexecution
Start of reverse execution
Fig. 4.10 (h)
"REVERSE"
switch = OFF
Cycle start (start of forward execution)
Start of forward reexecution
Forward
Reverse
Forward
reexecution
Start of reverse
execution
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1164 -
- Reverse execution → end of reverse execution → forward reexecution
When a block to be executed is no longer present during reverse
execution (when reverse execution has been performed up to the block
where forward execution started, or when forward execution has not
yet been performed), the reverse execution end state is entered, and
operation stops.
Even when a cycle start operation is performed while the
“REVERSE” switch on the machine operator’s panel is held on,
operation is not performed, and the reverse execution end state is
maintained. Forward reexecution (or forward execution) is started
by setting the “REVERSE” switch on the machine operator’s panel to
off then performing a cycle start operation.
End of reverse execution
"REVERSE" switch =
OFF
Cycle start
Cycle start (start of forward execution)
Start of forward reexecution
Forward
Reverse
Forward
reexecution
Start of reverse execution
Fig. 4.10 (i)
- Forward reexecution → forward execution
After forward reexecution is performed up to the block at which
reverse execution started, forward execution starts automatically, and
commands are read from the program again and executed. No
particular operation is required.
Cycle start (start of forward execution)
Start of forward reexecution
Forward
Reverse
Forward
reexecution
Start of reverse execution
Restart of forward execution
Fig. 4.10 (j)
If reverse execution was performed after feed hold stop, forward
reexecution ends when the feed hold stop position is reached, then
forward execution is performed. Also if single block operation was
performed, forward reexecution ends at the single block stop position.
Cycle start (start of forward execution)
Start of forward reexecution
Forward
Reverse
Forward
reexecution
Feed hold stop
"REVERSE" switch = OFF, cycle start
Start of reverse execution
Restart of forward execution
Fig. 4.10 (k)
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1165 -
Explanation
- Reverse execution and forward execution
Usually in automatic operation, a program is executed in the
programmed order. This is called forward execution. This function
allows a program executed by forward execution to be executed in the
reverse direction. This is called reverse execution. Reverse
execution allows the tool to retrace the path along which the tool has
moved during forward execution.
Reverse execution of a program can be performed only for blocks that
have been executed by forward execution.
Furthermore, in single block operation, reverse execution can also be
performed on a block-by-block basis .
- Forward reexecution
Blocks that have been executed by reverse execution can be
reexecuted in the forward direction up to the block from which reverse
execution started. This is called forward reexecution. Forward
reexecution allows the tool to retrace the same tool path as in forward
execution until the position at which reverse execution started is
reached.
After the block from which reverse execution started is reached, the
program is executed again in the programmed order (forward
execution).
Furthermore, in single block operation, forward reexecution can also
be performed on a block-by-block basis.
- End of reverse execution
When a block to be executed is no longer present during reverse
execution (when stored blocks have all been executed during reverse
execution, or when forward execution has not yet been performed),
operation stops. This is called the end of reverse execution.
- Status indication
During reverse execution, characters "RVRS" blink on the screen.
During forward reexecution, characters "RTRY" blink to indicate that
forward reexecution is in progress. The "RTRY" indication is kept
blinking until the block at which reverse execution started is reached
and normal operation starts (until forward execution is restarted).
When a block to be executed is no longer present during reverse
execution, or if an attempt is made to perform reverse execution for a
block that cannot be executed by reverse execution, characters
"RVED" blink, notifying the user that reverse execution can no longer
be performed.
- Number of blocks that can be executed by reverse execution
Up to about 100 blocks can be executed by reverse execution.
Depending on the specified program, the maximum number of
executable blocks may decrease.
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1166 -
- Reset
A reset operation (the reset button on the MDI panel, the external reset
signal, or the reset & rewind signal) clears the blocks stored for
reverse execution.
- Feedrate
A feedrate to be applied during reverse execution can be specified in
parameter No. 1414. If this parameter is set to 0, the feedrate in
reverse execution is assumed to be the same as that in forward
execution. Rapid traverse, however, is performed always at the rapid
traverse rate, regardless of the setting of this parameter.
The feedrate in forward reexecution is always the same as that in
forward execution.
In reverse execution or forward reexecution, feedrate override, rapid
traverse override, and dry run are allowed.
- Start of reverse execution or forward reexecution after the end of a block
In a block for rapid traverse (G00), linear interpolation (G01), circular
interpolation (G02, G03), dwelling (G04), skip cutting (G31), or an
auxiliary function in an automatic operation mode (memory operation,
part program operation, or MDI operation), reverse execution or
forward reexecution can be started. However, reverse execution and
forward reexecution do not start as soon as the reverse execution
signal status is changed. When the block has ended, that is, after a
movement, dwelling, or an auxiliary function is completed, reverse
execution or forward reexecution starts.
- Start of reverse execution or forward reexecution after feed hold stop
When a feed hold stop operation is performed during execution of
rapid traverse (G00), linear interpolation (G01), circular interpolation
(G02, G03), or skip cutting (G31), then the reverse execution signal
status is changed and operation is restarted, reverse execution or
forward reexecution can be started immediately from the stop position.
This cannot be performed when dwelling (G04) or an auxiliary
function is being executed.
Start of
reverse
execution
Start of feed hold
"REVERSE" switch = ON
Cycle start
Start of feed hold
"REVERSE" switch = OFF
Cycle start
End of reverse execution, start of forward reexecution
Fig. 4.10 (l)
When reverse execution is started after feed hold stop operation, the
part from the start point of that block to the feed hold stop position is
stored as one block. Therefore, when forward reexecution is
performed with the single block switch set to 1, a single block stop
takes place as soon as the position at which reverse execution started
is reached.
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1167 -
- Start of reverse execution or forward reexecution after single block stop
After a single block stop takes place, reverse execution or forward
reexecution can be started immediately when the reverse execution
signal status is changed and restart operation is performed.
Limitation
- Blocks that cannot be executed by reverse execution
In the modes listed below, reverse execution cannot be performed.
When one of these commands appears during reverse execution,
reverse execution ends immediately and "RVED" is displayed.
• Involutes interpolation (G02.2, G03.2)
• Exponential interpolation (G02.3, G03.3)
• Three-dimensional circular interpolation (G02.4, G03.4)
• NURBS interpolation (G06.2)
• Cylindrical interpolation (G07.1,G107)
• Polar coordinate interpolation (G12.1, G13.1,G112,G113)
• Polar coordinate command (G16)
• Functions related thread cutting (G33,G34,G35,G36)
• 3-dimensional cutter compensation (G41.2, G41.3, G42.2,
G42.3)
• Tool length compensation in tool axis direction (G43.1)
• Tool center point control (G43.4, G43.5)
• Polygon turning (G50.2, G51.2)
• Tool axis direction control (G53.1)
• Single direction positioning (G60)
• Tapping mode (G63)
• Tapping cycle (G84,G74)
• Rigid tapping cycle (G84,G74,G84.2,G84.3)
• Fine boring ccyle (G76)
• Back boring ccyle (G87)
It is impossible to perform reverse execution for blocks specifying the
commands listed below. If one of these commands appears during
reverse execution, reverse execution ends immediately and "RVED" is
displayed.
Some of these commands turn a mode on and off. It is possible to
start reverse execution and perform forward reexecution in a mode set
by such a command. However, if a block that turns the mode on or
off is reached during reverse execution, the reverse execution ends at
that block, and "RVED" is displayed.
• Functions related AI contour control (G05,G05.1,G08)
• HRV3 on/off (G05.4)
• Hypothetical axis interpolation (G07)
• Inch/metric conversion (G20, G21)
• Stored stroke check on/off (G22, G23)
• Functions related referece position return (G27, G28, G29, G30)
• Floating referece position return (G30.1)
• 3-dimensional coordinate system conversion (G68, G69)
• Feature coordinate system (G68.2)
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1168 -
• Figure copying (G72.1,G72.2)
• Chopping (G81.1)
• Index table indexing
• Cs contouring control
• Spindle positioning
- Manual intervention
To execute a program in the reverse direction after a feed hold stop or
single block stop, when manual intervention is performed after the
stop, make a return to the original position and then turn on the
reverse signal. Movement by manual intervention is ignored during
reverse execution and forward reexecution.
- Single block stop position
A block that is internally generated by the control unit is also treated
as one block during reverse execution.
Path after compensation
Programmed path
②
2
34
5
Fig. 4.10 (m) Path when cutter compensation is applied
In the above example, the program specifies two blocks, but in actual
operation, move commands for five blocks are generated.
In such a case, positions at which a single block stop takes place may
differ between forward execution and reverse execution.
- Positioning (G00)
When non-linear type positioning is performed (bit 1 (LRP) of
parameter No. 1401 is set to 0), the tool path in reverse execution and
that in forward execution do not match. The tool path in forward
reexecution is the same as that in forward execution.
When linear type positioning is performed (bit 1 (LRP) of parameter
No. 1401 is set to 1), the tool path in reverse execution is the same as
that in forward execution.
Forward
Reverse
Forward reexecution
Non-linear type positioning
(LRP = 0)
Linear type positioning
(LRP = 1)
X
Y
Fig. 4.10 (n)
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1169 -
- Dwell command (G04)
During reverse execution or forward reexecution, the dwell command
(G04) is executed in the same way as in normal operation.
- Programmable data input (G10)
Tool compensation values, parameters, pitch error data, workpiece
origin offsets, and tool life management values set or modified by
programmable data input (G10) are ignored during reverse execution
and forward reexecution.
- Skip function (G31) and automatic tool length compensation (G37)
The skip signal and the automatic tool length measurement signal are
ignored during reverse execution and forward reexecution. During
reverse execution and forward reexecution, the tool moves along the
path that the tool has actually passed during forward execution.
Forward Reverse
reexecution execution
Forward execution
(Actual path)
Skip signal ON (G31)
or automatic tool length measurement signal ON (G37)
Signal not applied (G31)
(Programmed path)
Fig. 4.10 (o)
- Setup of a coordinate system (G92, G54 to G59, G54.1P_, G52, and G92.1)
When setup of a coordinate system (G92, G54 to G59, G54.1P_, and
G52) is specified during reverse execution, the indicated current
position may differ from the position indicated during forward
execution. However, the actual machine position does not differ.
- Mirror image
When a block to which a mirror image is applied by programmable
mirror image (G50.1, G51.1) is executed during reverse execution, the
tool moves along the actual path resulting from the application of a
mirror image in the reverse direction.
When a mirror image is applied to a block by setting or a machine
signal, the block with the mirror image not applied is stored. Mirror
image application by setting or a machine signal is enabled also
during reverse execution and forward reexecution. Therefore, during
reverse execution and forward reexecution, the mirror image by
setting data or machine signal must be turned on and off so that this
on/off status and the on/off status during forward execution match.
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1170 -
- Changing offsets
Even when cutter compensation data or tool length offsets are changed
during reverse execution or forward reexecution, the change in
compensation or offset data does not become valid until forward
reexecution ends and normal operation starts. Until then, the tool
moves with the offset data that was applied when the block was
executed for the first time during forward execution.
- Interrupt type custom macro
(1) Do not initiate any interrupt during reverse execution.
(2) Do not execute an interrupted block and the interrupt program in
reverse execution.
- Tool management function
The tool life is not counted during reverse execution and forward
reexecution.
- Inverse time feed (G93)
If a nonzero value is set as the feedrate to be applied during reverse
execution in parameter No. 1414, a block that moves the tool by
inverse time feed during forward execution is executed at the
parameter-set feedrate (feed per minute) during reverse execution.
If the feedrate during reverse execution (parameter No. 1414) is not
set (= 0), the same feedrate as applied during forward execution is
used.
- Maximum spindle speed clamp (G92Sxxxx)
Clamping at a maximum spindle speed specified during reverse
execution becomes valid. This means that if G92Sxxxx appears
during reverse execution, the spindle speed is clamped at Sxxxx in the
subsequent reverse execution. As a result, the clamp speed may
differ between reverse execution and forward execution even when the
same block is executed. The spindle speed is clamped when the G96
mode is set.
- Auxiliary functions
M, S, T, and the second auxiliary function (B function) are output
directly also during reverse execution and forward reexecution.
When specified together with a move command in the same block, M,
S, T, and the second auxiliary function (B function) are output with
the move command at the same time during forward execution,
reverse execution, and forward reexecution. Therefore, the output
positions of M, S, T, and the second auxiliary function (B function)
during reverse execution differ from those during forward execution
and forward reexecution.
- Custom macro operation
Custom macro operations are ignored during reverse execution and
forward reexecution.
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1171 -
- Tool retract and recover function
For retract operation and repositioning operation by the tool retract
and recover function, reverse execution cannot be performed.
Retract operation and repositioning operation are ignored during
reverse execution and forward reexecution.
- AI contour control
During reverse execution and forward reexecution, the feedrate clamp
function by acceleration under AI contour control is disabled.
- Display
During reverse execution and forward reexecution, the modal display
and the display of the currently executed program are not updated;
information obtained at the start of reverse execution is maintained.
Warning
WARNING
1 Auxiliary functions are output directly even during reverse
execution and forward reexecution. Accordingly, the
execution status of an auxiliary function during forward
execution may be reversed during reverse execution.
Example:
When forward rotation of the spindle (M03) and stop (M05)
are specified
When N3 is executed during reverse execution, M05 is
output. So, when N2 and N1 are executed during reverse
execution, operation is performed with the spindle stopped.
When N1 is executed during forward reexecution, M03 is
output. So, when N1 and N2 are executed during forward
reexecution, operation is performed with the spindle rotating
in the forward direction.
M03 (forward spindle
rotation)
Forward spindle rotation
Forward
Reverse
Forward
reexecution
Start of reverse execution
Restart of forward
execution
M05 (spindle stopped)
Spindle stopped
N1
N2
N3
2 To perform reverse execution after a feed hold stop or single
block stop operation, be sure to restore the original position if
manual intervention has been performed after the stop , then
set the "REVERSE" switch to on. Movements made by
manual intervention are ignored during reverse execution and
forward reexecution. (The same operation as in the manual
absolute off state takes place.)
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1172 -
4.11 ACTIVE BLOCK CANCEL FUNCTION
The automatic operation can be stopped by inputting block
cancellation signal BCAN<Gn297.0> while automatic operation.
After an automatic operation becomes stop, automatic operation signal
OP <Fn000.7> and cycle start lamp signal STL <Fn000.5> becomes
"0".
All modal information is preserved.
At this time,
(1) If the machine is moving, it stops while decelerating. And the
distance remaining is cleared.
(2) If the dwell is executing, it is canceled.
(3) If auxiliary function, spindle speed, tool function, the second
auxiliary function is executing, the each strobe signal MF, SF,
TF, BF becomes "0" and the block is ended.
If the high speed M/S/T/B interface (bit 7 (MHI) of parameter
No.3001 = 1) is used, the block is ended without the each strobe
signal MF, SF, TF and BF changing.
Therefore, after completion signal MFIN / SFIN / TFIN / BFIN
is matched in the same logical level as the strobe signal, it is
necessary to restart the operation.
An automatic operation is restarted from the next block of the
canceled block by cycle start.
Active block cancel function
Explanation
Operation when operation restarts
G90/G91
When the operation is restarted, the operation of the restart is decided
depending on the command in the next block of the canceled block.
When the next block is absolute command (G90), the operation is
restarted toward the terminal from the stopping position to the next
block. When the next block is incremental command (G91), the
incremental operation is restarted from the stopping position.
Position where tool halts by signal input
next block
When G91 is specified
in next block
Programmed tool path
When G90 is specified in next block
Fig. 4.11 (a) Absolute / Incremental
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1173 -
CAUTION
1 Because the tool becomes a start from the
canceled position when an automatic operation
restarts, the route of an actual movement is
different from original program route. Therefore,
there is a possibility that the tool route and the work
piece interfere at the restart. Please do the restart
operation after confirming neither the tool nor work
piece interfere.
2 If the part program is incremental command, the
terminal of the next block shifts cancellation
amount when automatic operation restarts. This
amount of the gap keeps remaining until the
absolute command is executed next. Therefore,
this function cannot be used to check the block
terminal by the program made by the incremental
command.
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1174 -
Tool radius / tool nose radius compensation
The offset mode is temporarily canceled at that time when canceling
in the tool radius / tool nose radius compensation mode. And, the
start-up operation is done at the restart.
For example, when canceling in N20 of the undermentioned program,
the movement of restarting is the start-up operation toward the
position commanded with N30 in the figure below.
Example
N10 G90 G01 G42 X_ D_ S_ F_ ;
N20 X_ ;
N30 X_ Y_;
N40 X_ ;
Position where tool halts by signal inpu
t
Tool path after cutter compensation
Specified program N30
Specified program N20
Specified program N40
Fig. 4.11 (b) Tool radius / tool nose radius compensation
B-63944EN/03 OPERATION 4.AUTOMATIC OPERATION
- 1175 -
Canned cycle for drilling
When a block is canceled during a canned cycle for drilling, that
canned cycle is canceled. Program execution is restarted from the next
block.
Example1 N10 G91 G84 X_ Y_ Z_ R_ K3 ;
N20 G90 G00 X_ Y_ Z_ ;
Position where tool halts by signal inpu
t
N10 N20
Fig. 4.11 (c)Canned cycle for drilling 1
Example 2 N10 G90 G84 X_ Y_ Z_ R_ ;
N20 X_ Y_ ;
N30 X_ Y_ ;
N40 X_ Y_ ;
N50 G00 X_ Y_ Z_ ;
Position where tool halts by signal
N10 N50 N20 N30 N40
Fig. 4.11 (d) Canned cycle for drilling 2
At the restart, the operation is executed from the next N30 block when
the operation is canceled while executing in N20 cycle.
At this time, because the G84 mode is maintained, the tool positions in
R point after moving to the X-Y position commanded with N30 and
starts the hole opening operation.
4.AUTOMATIC OPERATION OPERATION B-63944EN/03
- 1176 -
Notes
CAUTION
1 Please confirm neither the tool route nor work
piece interference when the operation is restarted.
2 When an automatic operation is restarted, the
route of an actual movement is different from an
original route because it is a start from the
canceled position. Therefore, there is a possibility
that the tool route and the work piece interference
at the restart.
3 When reset or the emergency stops is executed
during the stopping by this function, this function
becomes invalid. In a word, maintained various
data and modal data are changed to the clear or
reset states by the reset operation.
4 This function is effective only while automatic
operation. (OP=1 and STL=1)
5 If the part program is incremental command, the
terminal of the next block shifts cancellation
amount when automatic operation restarts. This
amount of the gap keeps remaining until the next
absolute command is executed. Therefore, this
function cannot be used to check the block
terminal by the program made by the incremental
command.
6 This function is not available during AI contour
control mode. Even if the cancel signal is input, it is
ignored.
B-63944EN/03 OPERATION 5.TEST OPERATION
- 1177 -
5 TEST OPERATION
The following functions are used to check before actual machining
whether the machine operates as specified by the created program.
5.1 MACHINE LOCK AND AUXILIARY FUNCTION LOCK 1178
5.2 FEEDRATE OVERRIDE.......................................................1180
5.3 RAPID TRAVERSE OVERRIDE..........................................1181
5.4 DWELL/AUXILIARY FUNCTION TIME OVERRIDE ......1182
5.5 DRY RUN ..............................................................................1184
5.6 SINGLE BLOCK ...................................................................1185
5.7 HIGH SPEED PROGRAM CHECK FUNCTION.................1187
5.TEST OPERATION OPERATION B-63944EN/03
- 1178 -
5.1 MACHINE LOCK AND AUXILIARY FUNCTION LOCK
To display the change in the position without moving the tool, use
machine lock.
There are two types of machine lock: all-axis machine lock, which
stops the movement along all axes, and specified-axis machine lock,
which stops the movement along specified axes only. In addition,
auxiliary function lock, which disables M, S, T, and B (2nd auxiliary
function) commands, is available for checking a program together
with machine lock.
Tool
Display unit
X
Y
Z
The tool does not move but the
position along each axis changes
on the dis
p
la
y
.
Workpiece
. . . . . . . . .
Fig. 5.1 (a) Machine lock
Machine lock and auxiliary function lock
Procedure
- Machine Lock
Press the machine lock switch on the operator's panel. The tool does
not move but the position along each axis changes on the display as if
the tool were moving.
Some machines have a machine lock switch for each axis. On such
machines, press the machine lock switches for the axes along which
the tool is to be stopped. Refer to the appropriate manual provided by
the machine tool builder for machine lock.
WARNING
The positional relationship between the workpiece
coordinates and machine coordinates may differ
before and after automatic operation using machine
lock. In such a case, specify the workpiece
coordinate system by using a coordinate setting
command or by performing manual reference
position return.
B-63944EN/03 OPERATION 5.TEST OPERATION
- 1179 -
- Auxiliary function lock
Press the auxiliary function lock switch on the operator's panel. M, S,
T, and B codes are disabled and not executed. Refer to the appropriate
manual provided by the machine tool builder for auxiliary function
lock.
Limitation
- M, S, T, B command by only machine lock
M, S, T and B commands are executed in the machine lock state.
- Reference position return under machine lock
When a G27, G28, or G30 command is issued in the machine lock
state, the command is accepted but the tool does not move to the
reference position and the reference position return LED does not go
on.
- M codes not locked by auxiliary function lock
M00, M01, M02, M30, M98, M99, and M198 (subprogram call
function) commands are executed even in the auxiliary function lock
state. M codes for calling a subprogram (parameters No. 6071 to
6079) and those for calling a custom macro (parameters No. 6080 to
6089) are also executed.
5.TEST OPERATION OPERATION B-63944EN/03
- 1180 -
5.2 FEEDRATE OVERRIDE
A programmed feedrate can be reduced or increased by a percentage
(%) selected by the override dial. This feature is used to check a
program.
For example, when a feedrate of 100 mm/min is specified in the
program, setting the override dial to 50% moves the tool at 50
mm/min.
Tool
Check the machining by
altering the feedrate from
the value specified in the
program.
Feedrate 100 mm/min
(Specified by programmed)
Feedrate 50 mm/min afte
r
feedrate override
Workpiece
Fig. 5.2 (a) Feedrate override
Feedrate override
Procedure
Set the feedrate override dial to the desired percentage (%) on the
machine operator's panel, before or during automatic operation.
On some machines, the same dial is used for the feedrate override dial
and jog feedrate dial. Refer to the appropriate manual provided by the
machine tool builder for feedrate override.
Limitation
- Override range
The override that can be specified ranges from 0 to 254%. For
individual machines, the range depends on the specifications of the
machine tool builder.
- Override during thread
During the threading process, the override setting is ignored; it is
always regarded as 100% during the process.
B-63944EN/03 OPERATION 5.TEST OPERATION
- 1181 -
5.3 RAPID TRAVERSE OVERRIDE
An override of four steps (F0, 25%, 50%, and 100%) can be applied to
the rapid traverse rate. F0 is set by a parameter No. 1421.
Rapid traverse rate
10m/min
Override
50% 5m/min
Fig. 5.3 (a) Rapid traverse override
Rapid traverse override
Procedure
Select one of the four feedrates with the rapid traverse override switch
during rapid traverse. Refer to the appropriate manual provided by the
machine tool builder for rapid traverse override.
Explanation
The following types of rapid traverse are available. Rapid traverse
override can be applied for each of them.
(1) Rapid traverse by G00
(2) Rapid traverse during a canned cycle
(3) Rapid traverse in G27, G28, G29, G30, G53
(4) Manual rapid traverse
(5) Rapid traverse of manual reference position return
5.TEST OPERATION OPERATION B-63944EN/03
- 1182 -
5.4 DWELL/AUXILIARY FUNCTION TIME OVERRIDE
An override can be applied to dwell and the auxiliary function
(M/S/T/B) in increments of 1% in the range from 0 to 100%.
For the auxiliary function, however, if the override is less than 100%,
the next block is started after a lapse of actual processing time plus
shortage time.
Dwell/auxiliary function time override
Procedure
Press the 1% rapid traverse override selection switch and turn the
1% rapid traverse override switch to select the desired percentage.
For details on 1% rapid traverse override, refer to the manual provided
by the machine tool builder.
Explanation
- Dwell
An override can be applied to dwell.
[Example]
Override and dwell time when G04 P10000; is executed
Override Dwell time
25% 40.0 sec.
50% 20.0 sec.
75% 13.3 sec.
100% 10.0 sec.
NOTE
An override is disabled for dwell per revolution.
- AUXILIARY functions (M/S/T/B)
An override can be applied in the time from when M/S/T/B is sent
until the FIN signal is turned off (or until MFIN, SFIN, TFIN, and
BFIN are changed in the case of the high speed M/S/T/B). The time
required to communicate with PMC is included.
When the FIN signal is turned off and then shortage time elapses, the
next block is started.
[Example]
When the following program is executed with the override set to
60%
N10 M03 ;
N20 ⋅ ⋅ ⋅ ⋅ ⋅ ;
When the processing time of the N10 block is 80 msec, the N20
block is started approx. 56 msec after completion of the
processing.
Shortage time = 80 msec × 100/60 - 80 msec = 53.333 ≅ 56 msec
B-63944EN/03 OPERATION 5.TEST OPERATION
- 1183 -
NOTE
The time count is incremented every 4 msec or 8
msec and the fraction is rounded up. The counting
cycle of time may depend on the system.
The 1% rapid traverse override signal reads the value upon completion
of the auxiliary function. Accordingly, the value is not ensured if the
override value changes between before and after the reading.
When the movement command and auxiliary function are specified in
the same block:
(1) When the movement command is completed first
• An override is enabled.
(2) When the auxiliary command is completed first
• An override is disabled.
When auxiliary functions are specified in the same block, the shortage
time is calculated using the auxiliary function with the longest
processing time.
NOTE
1 This function is disabled for dwell by PMC axis
control (04H) and the auxiliary functions (12H, 14H,
15H).
2 For the dwell, when the 1% rapid traverse override
signal is 0%, a transition to the next block is not
performed.
3 The time when a feed hold is caused in the auxiliary
function during shortage time is not included in the
shortage time.
4 For the auxiliary function, when the 1% rapid
traverse override signal is 0%, the setting of
parameter No. 3018 is used as the override value.
When the setting of the parameter is 0, it is
assumed to be 10%. While the 1% rapid traverse
override signal is 0%, a transition to the next block
is not performed.
5 For auxiliary functions M02 and M30, bit 7 (OVM) of
parameter No. 3002 can be used to enable or
disable an override.
5.TEST OPERATION OPERATION B-63944EN/03
- 1184 -
5.5 DRY RUN
The tool is moved at the feedrate specified by a parameter regardless
of the feedrate specified in the program. This function is used for
checking the movement of the tool under the state that the workpiece
is removed from the table.
Tool
Table
Fig. 5.5 (a) Dry run
Dry run
Procedure
Press the dry run switch on the machine operator's panel during
automatic operation.
The tool moves at the feedrate specified in a parameter. The rapid
traverse switch can also be used for changing the feedrate.
Refer to the appropriate manual provided by the machine tool builder
for dry run.
Explanation
- Dry run feedrate
The dry run feedrate changes as shown in the table below according to
the rapid traverse switch and parameters.
Table 5.5 (a)
Program command Rapid traverse
switch Rapid traverse Cutting feed
ON Rapid traverse rate Dry run feedrate × Jvmax(*2)
OFF Dry run feedrate × JV,
or rapid traverse rate (*1) Dry run feedrate × JV(*2)
Max. cutting feedrate ........... Setting by parameter No.1430
Rapid traverse rate ............... Setting by parameter No.1420
Dry run feedrate ................... Setting by parameter No.1410
(*1) Dry run feedrate × JV when parameter RDR (No. 1401#6) is 1.
Rapid traverse rate when parameter RDR is 0.
JV Jog feedrate override
(*2) Clamped to the maximum cutting feedrate
Jvmax Maximum value of jog feedrate override
B-63944EN/03 OPERATION 5.TEST OPERATION
- 1185 -
5.6 SINGLE BLOCK
Pressing the single block switch starts the single block mode. When
the cycle start button is pressed in the single block mode, the tool
stops after a single block in the program is executed. Check the
program in the single block mode by executing the program block by
block.
Tool
Cycle start Stop
Stop
Stop
Workpiece
Cycle start Cycle start
Fig. 5.6 (a) Single block
Single block
Procedure
1 Press the single block switch on the machine operator's panel.
The execution of the program is stopped after the current block is
executed.
2 Press the cycle start button to execute the next block. The tool
stops after the block is executed.
Refer to the appropriate manual provided by the machine tool
builder for single block execution.
5.TEST OPERATION OPERATION B-63944EN/03
- 1186 -
Explanation
- Reference position return and single block
If G28, G29, and G30 are issued, the single block function is effective
at the intermediate point.
- Single block during a canned cycle
In a canned cycle, the single block stop points are the end of <1>, <2>,
and <6> shown below. When the single block stop is made after the
point <1> or <2>, the feed hold LED lights.
<6>
<1>
<2>
<4>
<5>
Rapid
traverse
Cutting feed
<3>
Fig. 5.6 (b) Single block during canned cycle
- Subprogram call and single block
Single block stop is not performed in a block containing M98P_;.
M99; or G65.
However, single block stop is even performed in a block with M98P_
or M99 command, if the block contains an address other than O, N, P,
L.
B-63944EN/03 OPERATION 5.TEST OPERATION
- 1187 -
5.7 HIGH SPEED PROGRAM CHECK FUNCTION
When the cycle start button is pressed with the high speed program
check mode set to be enabled, the program syntax and stroke limit are
checked without axis movement.
A program check is performed at the maximum speed that can be
specified by the CNC, regardless of the specified speed.
NOTE
This function is optional.
High speed program check
Procedure
1 Perform position of the machine at the start position of the
machining program in advance.
Set the workpiece coordinate system or tool compensation to the
same state as in actual machining.
2 Reset the CNC and press the high speed program check switch
on the machine operator's panel to enter the high speed program
check mode. In the high speed program check mode,
"PRG-CHK" blinks at the lower-left of the CNC screen.
3 Press the cycle start button to execute the program without axis
movement. The feedrate is the maximum speed that can be
specified by the CNC, regardless of the specified speed.
The program syntax and stroke limit are checked during
execution of the program.
4 Upon completion of the check, reset the CNC and release the
high speed program check mode with the switch on the machine
operator's panel.
Explanation
- Stroke Limit Check
Following the stroke limit check is executed without axes movements
during the high speed program check mode.
• Stored stroke check 1
• Stored stroke check 2, 3
• Stroke limit check before move
• Rotation area interference check
If an alarm about the stroke limit occurs in the high speed program
check mode, clear the alarm as described below.
(1) Change the mode to other than MEM or DNC.
(2) Reset the CNC.
5.TEST OPERATION OPERATION B-63944EN/03
- 1188 -
WARNING
1 If the machine coordinate system is not
established, a stroke limit check is not performed
correctly. When a reference position return is
completed after power-on, perform a high speed
program check.
2 When the width of the prohibited area is small in a
stored stroke limit 2 and 3 check and rotation area
interference check, if a command to intersect the
prohibited area in one block is issued, the stroke
limit may not be detected. This means that a
program not causing a stroke check alarm in a high
speed program check may cause an alarm in
actual operation.
- Program Check Feedrate
During the high speed program check mode, the feedrate of program
execution becomes the maximum feedrate of CNC system regardless
of the specified feedrate.
The feedrate clamp, override and dry run are not effective.
The execution speed of circular interpolation, involute interpolation,
spiral/conical interpolation, and NURBS interpolation can be selected
by bit 7 (PGF) of parameter No. 1490 from the maximum speed and
dry run speed.
NOTE
1 The execution time of dwell is the same as a
normal operation.
2 The PS011 alarm occurs when there is no F
command in a normal operation. However, it is
executed at maximum speed without the alarm in
the high speed program check mode even if there
is no F command.
- Workpiece Coordinate System Preset
Upon completion of the high speed program check mode, the
workpiece coordinate system is automatically preset. This enables
program operation without making a reference position return upon
completion of a program check. For details, refer to the manual
provided by the machine tool builder.
B-63944EN/03 OPERATION 5.TEST OPERATION
- 1189 -
WARNING
When the coordinate system is set before the high
speed program check mode is turned on by the
work coordinate system setting G92 (machining
center system and G code system B or C of the
lathe system), G50 (G code system A of the lathe
system) and the local coordinate system setting
G52, their setting values are deleted by the
execution of the work coordinate system preset.
- Machine Coordinate Display For Program Check
During the high speed program check mode, it is possible to change
the display of machine coordinates from the actual machine
coordinates to the machine coordinates for the program check by
setting bit 7 (PGM) of parameter No.11320.
And it is possible to change the display of machine coordinate for
each axis from the actual machine coordinate to the machine
coordinate for the program check by setting bit 4 (PGA) of parameter
No.3115.
- Tool life
If tool life management command or tool management command is
specified during the high speed program check mode, tool life is not
counted.
- Unavailable command
Following functions can not be specified during the high speed
program check mode. If the following functions are specified, the
alarm PS5364 occurs.
• High speed cycle cutting
• Chopping
As for the chopping by the input signal:
The alarm PS5364 occurs when the program check is started
during the chopping by the input signal.
The alarm PS5364 occurs when the chopping by the input signal
is started at the program check execution.
• Simple electronic gear box
・Commands not covered by a high speed program check
Auxiliary functions and other commands are not covered by a high
speed program check. For details, refer to the manual provided by
the machine tool builder.
6.SAFETY FUNCTIONS OPERATION B-63944EN/03
- 1190 -
6 SAFETY FUNCTIONS
To immediately stop the machine for safety, press the Emergency stop
button. To prevent the tool from exceeding the stroke ends, Overtravel
check and Stored stroke check are available. This chapter describes
emergency stop, overtravel check, and stored stroke check.
Chapter 6, "SAFETY FUNCTIONS", consists of the following
sections:
6.1 EMERGENCY STOP .............................................................1191
6.2 OVERTRAVEL ......................................................................1192
6.3 STORED STROKE CHECK ..................................................1193
6.4 STROKE LIMIT CHECK BEFORE MOVE..........................1198
6.5 WRONG OPERATION PREVENTION FUNCTIONS.........1201
B-63944EN/03 OPERATION 6.SAFETY FUNCTIONS
- 1191 -
6.1 EMERGENCY STOP
If you press Emergency Stop button on the machine operator's panel,
the machine movement stops in a moment.
EMERGENCY STOP
Red
Fig. 6.1 (a) Emergency stop
This button is locked when it is pressed. Although it varies with the
machine tool builder, the button can usually be unlocked by twisting
it.
Explanation
EMERGENCY STOP interrupts the current to the motor.
Causes of trouble must be removed before the button is released.
6.SAFETY FUNCTIONS OPERATION B-63944EN/03
- 1192 -
6.2 OVERTRAVEL
When the tool tries to move beyond the stroke end set by the machine
tool limit switch, the tool decelerates and stops because of working the
limit switch and an OVER TRAVEL is displayed.
Deceleration
and stop
Stroke end Limit
switch
Y
X
Fig. 6.2 (a) Overtravel
Explanation
- Overtravel during automatic operation
When the tool touches a limit switch along an axis during automatic
operation, the tool is decelerated and stopped along all axes and an
overtravel alarm is displayed.
- Overtravel during manual operation
In manual operation, the tool is decelerated and stopped only along the
axis for which the tool has touched a limit switch. The tool still
moves along the other axes.
- Releasing overtravel
Press the reset button to reset the alarm after moving the tool to the
safety direction by manual operation. For details on operation, refer
to the operator's manual of the machine tool builder.
Alarm
Table6.2 (a)
Alarm No. Message Description
OT0506 + OVERTRAVEL ( HARD )
The stroke limit switch in the positive direction was triggered.
This alarm is generated when the machine reaches the stroke end.
When this alarm is not generated, feed of all axes is stopped during
automatic operation. During manual operation, only the feed of the axis
on which the alarm occurred is stopped.
OT0507 - OVERTRAVEL ( HARD )
The stroke limit switch in the negative direction was triggered.
This alarm is generated when the machine reaches the stroke end.
When this alarm is not generated, feed of all axes is stopped during
automatic operation. During manual operation, only the feed of the axis
on which the alarm occurred is stopped.
B-63944EN/03 OPERATION 6.SAFETY FUNCTIONS
- 1193 -
6.3 STORED STROKE CHECK
Three areas which the tool cannot enter can be specified with stored
stroke check 1, stored stroke check 2, and stored stroke check 3.
Stored stroke check 1
Stored
stroke
check 2
Stored stroke check 3
: Forbidden area for the tool
Fig. 6.3 (a) Stroke check
The following shows the areas which the tool cannot enter for each
stored stroke check.
• Stored stroke check 1: Outside
• Stored stroke check 2: Outside or inside (switchable)
• Stored stroke check 3: Inside
When the tool moves into the forbidden area, an alarm is displayed
and the tool is decelerated and stopped.
When the tool enters a forbidden area and an alarm is generated, the
tool can be moved in the reverse direction from which the tool came.
The stored stroke check 2 and 3 functions are optional.
6.SAFETY FUNCTIONS OPERATION B-63944EN/03
- 1194 -
Explanation
- Stored stroke check 1
Parameters (Nos. 1320, 1321 or Nos. 1326, 1327) set boundary.
Outside the area of the set limits is a forbidden area. The machine tool
builder usually sets this area as the maximum stroke.
When the tool enters a forbidden area and an alarm is generated, the
tool can be moved in the reverse direction from which the tool came.
At this time, a signal (overtravel alarm signal) can be output to the
PMC if bit 6 (OTS) of parameter No. 1301 is set to 1. In addition,
when the tool enters the forbidden area during manual operation, the
signal (overtravel alarm signal) can be output to the PMC without
generating the alarm by setting bit 1 (NAL) of parameter No. 1300 to
1. With this parameter setting, the alarm is generated when the tool
enters the forbidden area during automatic operation.
CAUTION
1 If the two points for specifying a forbidden area are
identical, all areas are handled as forbidden areas
for stored stroke check 1.
2 The size of a forbidden area must be set carefully.
If the size is set incorrectly, the stroke becomes
infinite.
- Stored stroke check 2
Parameters (Nos. 1322, 1323) or commands set these boundaries.
Inside or outside the area of the limit can be set as the forbidden area.
Parameter OUT (No. 1300#0) selects either inside or outside as the
forbidden area.
In case of program command a G22 command forbids the tool to enter
the forbidden area, and a G23 command permits the tool to enter the
forbidden area.
Each of G22; and G23; should be commanded independently of
another commands in a block.
The command below creates or changes the forbidden area:
(I, J, K)
(X, Y, Z)
X>I, Y>J, Z>K
G 22X_Y_Z_I_J_K_;
Fig. 6.3 (b) Creating or changing the forbidden area using a program
B-63944EN/03 OPERATION 6.SAFETY FUNCTIONS
- 1195 -
When setting the area by parameters, points A and B in the figure
below must be set.
X1>X2, Y1>Y2, Z1>Z2
A
(X1, Y1, Z1)
B(X2, Y2, Z2)
Fig. 6.3 (c) Creating or changing the forbidden area using a parameters
The values X1, Y1, Z1, X2, Y2, and Z2, which are set by parameters
No. 1322 and No. 1323, must be specified by the distance from the
machine coordinate system (machine unit). The values X, Y, Z, I, J,
and K, which are set by a G22 command, must be specified by the
distance in the least input increment (input unit).
Values set by a program are then converted in the machine increment
and the values are set as the parameters.
- Stored stroke check 3
Set the boundary with parameters No. 1324 and 1325. The area
inside the boundary becomes the forbidden area. The values X1, Y1,
Z1, X2, Y2, and Z2 must be set as coordinates (machine unit) in the
machine coordinate system.
CAUTION
1 If the two points for specifying a forbidden area are
identical, all areas are handled as movable areas
for stored stroke check 2/3.
2 Even if the two points for specifying a forbidden
area are erroneously set, the rectangular
parallelepiped having the points as vertices is
assumed as a boundary.
3 Since an axis without the reference position return
function has no forbidden areas, there are no
alarms about forbidden areas for the axis.
- Checkpoints in the forbidden area
The parameter setting or programmed value (XYZIJK) depends on
which part of the tool or tool holder is checked for entering the
forbidden area.
If point A (the top of the tool) is checked in Fig. 6.3(d), the distance
"a" should be set as the data for the stored stroke limit function. If
point B (the tool chuck) is checked, the distance "b" must be set.
When checking the tool tip (like point A), and if the tool length varies
for each tool, setting the forbidden area for the longest tool requires no
re-setting and results in safe operation.
6.SAFETY FUNCTIONS OPERATION B-63944EN/03
- 1196 -
• For machining center system
a
b
The position of the
tool after reference
position return
A
rea boundar
y
A
B
• For lathe system
The position of the
tool after reference
position return
Forbitten area boundary
b
a
B
A
Fig. 6.3 (d) Setting the forbidden area
- Forbidden area overlapping
Area can be set in piles.
Setting the forbidden area overlapping
Fig. 6.3 (e) Setting the forbidden area overlapping
Unnecessary limits should be set beyond the machine stroke.
- Condition under which each check is enabled
Each check becomes effective after the power is turned on and manual
reference position return or automatic reference position return by
G28 has been performed.
After the power is turned on, if the reference position is in the
forbidden area of each limit, an alarm is generated immediately.
(Only in G22 mode for stored stroke check 2).
B-63944EN/03 OPERATION 6.SAFETY FUNCTIONS
- 1197 -
- Releasing the alarms
If the enters a forbidden area and an alarm is generated, the tool can be
moved only in the backward direction. To cancel the alarm, move
the tool backward until it is outside the forbidden area and reset the
system. When the alarm is canceled, the tool can be moved both
backward and forward.
- Change from G23 to G22 in a forbidden area
When G23 is switched to G22 in the forbidden area, the following
results.
<1> When the forbidden area is inside, an alarm is informed in the
next move.
<2> When the forbidden area is outside, an alarm is informed
immediately.
- Timing for displaying an alarm
In stored stroke check 1/2/3, parameter BFA (bit 7 of No. 1300)
selects whether an alarm is displayed immediately before the tool
enters the forbidden area or immediately after the tool has entered the
forbidden area.
Alarm
Number Message Description
OT0500 + OVERTRAVEL (SOFT 1) A movement in the positive direction
exceeded stored stroke check 1.
OT0501 - OVERTRAVEL (SOFT 1) A movement in the negative direction
exceeded stored stroke check 1.
OT0502 + OVERTRAVEL (SOFT 2) A movement in the positive direction
exceeded stored stroke check 2.
OT0503 - OVERTRAVEL (SOFT 2) A movement in the negative direction
exceeded stored stroke check 2.
OT0504 + OVERTRAVEL (SOFT 3) A movement in the positive direction
exceeded stored stroke check 3.
OT0505 - OVERTRAVEL (SOFT 3) A movement in the negative direction
exceeded stored stroke check 3.
6.SAFETY FUNCTIONS OPERATION B-63944EN/03
- 1198 -
6.4 STROKE LIMIT CHECK BEFORE MOVE
During automatic operation, before the movement specified by a given
block is started, whether the tool enters the forbidden area defined by
stored stroke check 1, 2, or 3 is checked by determining the position
of the end point from the current position of the machine and a
specified amount of travel. If the tool is found to enter the forbidden
area defined by a stored stroke limit, the tool is stopped immediately
upon the start of movement for that block, and an alarm is displayed.
WARNING
Whether the coordinates of the end point, reached
as a result of traversing the distance specified in
each block, are in a forbidden area is checked. In
this case, the path followed by a move command is
not checked. However, if the tool enters the
forbidden area defined by stored stroke check 1, 2,
or 3, an alarm is issued. (See the examples below.)
Example 1)
The tool is stopped at point a according to stored stroke
check 1 or 2.
Immediately upon movement commencing from the start
point, the tool is stopped to enable a stroke limit check
before moving to be performed before movement.
Forbidden area defined by stored stroke
check 1 or 2
Start point
a
Forbidden area defined by stored stroke
check 1 or 2
End point
End point
B-63944EN/03 OPERATION 6.SAFETY FUNCTIONS
- 1199 -
Example 2)
End
point
End point
Start point
Immediately upon movement commencing from the start
point, the tool is stopped to enable a stroke limit check
before moving to be performed before movement.
The tool is stopped at point a according to stored
stroke check 2 or 3.
Forbidden area defined by stored stroke
check 2 or 3
Forbidden area defined by stored stroke
check 2 or 3
a
Explanation
When a stroke limit check before moving is performed, whether to
check the movement performed by a G31 (skip) block and G37
(automatic tool length measurement) block can be determined using
(parameter NPC (No. 1301#2)).
Limitation
- Machine lock
If machine lock is applied at the start of movement, no stroke limit
check made before movement is performed.
- G23
When stored stroke check 2 is disabled (G23 mode), no check is made
to determine whether the tool enters the forbidden area defined by
stored stroke check 2.
- Program restart
When a program is restarted, an alarm is issued if the restart position
is within a forbidden area.
- Manual intervention following a feed hold stop
When the execution of a block is restarted after manual intervention
following a feed hold stop, no alarm is issued even if the end point
following a manual intervention is within a forbidden area.
6.SAFETY FUNCTIONS OPERATION B-63944EN/03
- 1200 -
- A block consisting of multiple operations
If a block consisting of multiple operations (such as a canned cycle
and exponential interpolation) is executed, an alarm is issued at the
start point of any operation whose end point falls within a inhibited
area.
- Cylindrical interpolation mode
In cylindrical interpolation mode, no check is made.
- Polar coordinate interpolation mode
In polar coordinate interpolation mode, no check is made.
- Three-dimensional coordinate system conversion
In three-dimensional coordinate system conversion mode, no check is
made.
- PMC axis control
No check is made for a movement based on PMC axis control.
Alarm
Table 6.4 (a) Alarm
Number Message Description
OT0510 + OVERTRAVEL
( PRE-CHECK )
The block end point was found in the + side
stroke limit prohibition area during a stroke
check before movement.
Modify the program.
OT0511 - OVERTRAVEL
( PRE-CHECK )
The block end point was found in the - side
stroke limit prohibition area during a stroke
check before movement.
Modify the program.
B-63944EN/03 OPERATION 6.SAFETY FUNCTIONS
- 1201 -
6.5 WRONG OPERATION PREVENTION FUNCTIONS
An improper tool offset setting or an improper operation of the
machine can result in the workpiece being cut inadequately or the tool
being damaged. Also, if data is lost due to an operation mistake, it
takes extra time to recover from the mistake.
The operation confirmation functions described below are meant to
prevent the operator from performing any unintended operation
(hereinafter referred to as an improper operation).
1 Functions that are used when data is set
• Data check to verify that the offset data is within the valid
setting range
• Incremental input operation confirmation
• Prohibition of the absolute input by the soft key to prevent
any improper absolute or incremental input operation
• Confirmation of any operation of deleting the program or all
data
• Confirmation of a data update during the data setting
process
2 Functions that are used when the program is executed
• Highlighting of updated modal information
• Display of the executed block status prior to the program
execution
• Display of the axis status, such as the mirror image function
enabled or the interlock function enabled
• Check for starting from the middle of the program
• Data check to verify that the offset data is within the
effective setting range
• Maximum incremental value check
6.SAFETY FUNCTIONS OPERATION B-63944EN/03
- 1202 -
6.5.1 Functions that are Used When Data is Set
The following functions are provided to prevent improper operations
when data is set.
• Input data range check
• Confirmation of incremental input
• Prohibition of the absolute input by the soft key
• Confirmation of the deletion of the program
• Confirmation of the deletion of all data
• Confirmation of a data update during the data setting process
Set these functions on the operation confirmation function setting
screen. For the input data range check, set a valid input data range,
e.g. the upper and lower limits, for each input screen. For the other
functions, specify whether to enable or disable them.
For information about how to display the individual setting screens,
how to manipulate them, and other details, see the item “Operation
confirmation setting screen” that describes the operation procedures.
B-63944EN/03 OPERATION 6.SAFETY FUNCTIONS
- 1203 -
6.5.1.1 Input data range check
This function allows an effective data range to be set and checks
whether the input data is within the set range.
Input data range check
Explanation
- Outline of the input data range check
This function allows an effective data range to be set for the data of
each input screen listed later and checks whether the input data is
within the set range. If the input data is out of the effective data
range, the warning message "DATA IS OUT OF RANGE" is
displayed and the data is rejected.
For example, assume that the effective data range for a certain tool
offset number is set to -200. to 200, and that you are going to input
100.[INPUT]. Even if you inadvertently press the 0 key one more
time, resulting in 1000.[INPUT], the input of 1000. is not accepted.
The function detects a setting mistake and prevents the program from
running with invalid data.
- Input screens for which this function is effective
• Tool compensation
• Workpiece origin offset
T
• Y-axis tool offset
• Workpiece shift
- Settings
To enable this function, set an effective data range for each input
screen on the operation confirmation function setting screen. For
information about how to display the individual setting screens, how
to set data ranges, and other details, see the items that describe the
setting of the data ranges.
If the set data range is invalid, no data input is accepted. Correct the
data range setting, and then input data.
- Disabling the function
The input data range check is disabled if you make any of the
following settings on the operation confirmation function setting
screen.
• Both the upper and lower limit values for the tool offset number
or workpiece coordinate system are 0.
• The upper and lower limit values for each offset are identical.
6.SAFETY FUNCTIONS OPERATION B-63944EN/03
- 1204 -
- Messages displayed during the input data range check
When the cursor moves into an input field of an input screen, one of
the following messages and warning messages is displayed. No
message is displayed when the input data range check is disabled.
When the set effective data range is valid
Message list 1
Input data status Message Color
The data in the input field is
within the range.
Input range xxx - xxx Black
The data in the input field is out
of the range.
Input range xxx - xxx Red
xxx: Upper and lower limit values
When the set effective data range is invalid
Message list 2
Range check status Message Color
Tool offset number overlap NG SETTING (OFFSET NUM
OVERLAP)
Red
Workpiece coordinate system
overlap
NG SETTING (WORK COORD VAL
OVERLAP)
Red
Invalid upper and lower limit
values
NG SETTING (U-LMT AND L-LMT
ILLEGAL)
Red
The message "NG SETTING (U-LMT AND L-LMT ILLEGAL)" is
displayed in the following cases:
• The upper and lower limit values are reversed.
• The values are not effective (e.g., more pairs of offset numbers
than allowed are set).
• Either of the tool offset numbers is 0.
- Range check for data changed by G10 or system variable
If the data changed by G10 or system variable is out of the effective
data range, the alarm PS0334 "OFFSET DATA OUT OF RANGE" is
displayed.
B-63944EN/03 OPERATION 6.SAFETY FUNCTIONS
- 1205 -
6.5.1.2 Confirmation of incremental input
This function displays a confirmation message when you attempt to
input an incremental value by using the [+INPUT] soft key.
Confirmation of incremental input
Explanation
- Outline of the confirmation of incremental input
This function displays a confirmation message when you attempt to
input an incremental value by using the [+INPUT] soft key in any of
the input screens listed below. It lets you confirm whether you really
want to change data or not before making that change.
For example, when you set 5.[+INPUT] for 10., the message "15.
INPUT OK?" is displayed.
The function prevents improper absolute or incremental input
operations.
NOTE
This function cannot be used to input two or more
values consecutively by delimiting them by
semicolons (;).
- Input screens for which this function is effective
• Tool compensation
• Workpiece origin offset
• Settings
• Parameter
• Pitch error compensation
M
• Chopping
T
• Workpiece shift
• Y-axis tool offset
• Second tool geometry offset
• Chuck tail stock barrier
• Tool geometry data
- Settings
In the operation confirmation function setting screen, check or
uncheck the "INCREMENTAL INPUT" box to enable or disable this
function. For information about how to display the setting screen,
how to set the function, and other details, see the item “Operation
confirmation setting” that describes the setting of the operation
confirmation function.
6.SAFETY FUNCTIONS OPERATION B-63944EN/03
- 1206 -
6.5.1.3 Prohibition of the absolute input by the soft key
This function prohibits the absolute input using the [INPUT] soft key.
Prohibition of the absolute input by the soft key
Explanation
- Outline of the prohibition of the absolute input by the soft key
This function prohibits the absolute input by the [INPUT] soft key in
the input screens listed later.
It prevents improper absolute or incremental input operations by
requiring that the absolute input be made using the MDI key
and that the incremental input be made using the [+INPUT] soft key.
- Input screens for which this function is effective
• Tool compensation
• Workpiece origin offset
T
• Y-axis tool offset
• Workpiece shift
- Settings
In the operation confirmation function setting screen, check or
uncheck the "DISABLED SOFTKEY[INPUT] IN" box to enable or
disable this function. For information about how to display the
setting screen, how to set the function, and other details, see the item
“Operation confirmation setting” that describes the setting of the
operation confirmation function.
B-63944EN/03 OPERATION 6.SAFETY FUNCTIONS
- 1207 -
6.5.1.4 Confirmation of the deletion of the program
This function displays the confirmation message "DELETE
PROGRAM ?" when you attempt to delete the program.
Confirmation of the deletion of the program
Explanation
- Outline of the confirmation of the deletion of the program
When you attempt to delete the program, this function displays the
confirmation message "DELETE PROGRAM ?" It lets you confirm
whether you really want to delete the program or not before executing
the deletion.
The function prevents the program from being deleted due to an
improper operation.
- Settings
In the operation confirmation function setting screen, check or
uncheck the "PROGRAM DELETE" box to enable or disable this
function. For information about how to display the setting screen,
how to set the function, and other details, see the item “Operation
confirmation setting” that describes the setting of the operation
confirmation function.
6.SAFETY FUNCTIONS OPERATION B-63944EN/03
- 1208 -
6.5.1.5 Confirmation of the deletion of all data
This function displays the confirmation message "DELETE ALL
DATA?" when you attempt to delete all data.
Confirmation of the deletion of all data
Explanation
- Outline of the confirmation of the deletion of all data
When you attempt to delete all data on the input screen described later,
this function displays the confirmation message "DELETE ALL
DATA?". It lets you confirm whether you really want to delete all
data or not before executing the deletion.
The function prevents all data from being deleted due to an improper
operation.
- Input screens for which this function is effective
• Tool compensation
T
• Y-axis tool offset
- Settings
In the operation confirmation function setting screen, check or
uncheck the "ALL DATA DELETE" box to enable or disable this
function. For information about how to display the setting screen,
how to set the function, and other details, see the item “Operation
confirmation setting” that describes the setting of the operation
confirmation function.
B-63944EN/03 OPERATION 6.SAFETY FUNCTIONS
- 1209 -
6.5.1.6 Confirmation of a data update during the data setting process
This function displays the [CAN] and [EXEC] soft keys for
confirmation when you attempt to update the data of an input screen
during the data setting process.
Confirmation of a data update during the data setting process
Explanation
- Outline of the confirmation of a data update during the data setting process
When you input data in input screen during the data setting process,
this function displays the [CAN] and [EXEC] soft keys for
confirmation. It lets you confirm whether you really want to update
the data or not before executing the update.
The function prevents set values from being lost due to an improper
operation.
If you input data using the [+INPUT] soft key when the confirmation
of incremental input is enabled, a message is displayed to confirm the
incremental input.
- Settings
In the operation confirmation function setting screen, check or
uncheck the "INPUT IN SETTING" box to enable or disable this
function. For information about how to display the setting screen,
how to set the function, and other details, see the item “Operation
confirmation setting” that describes the setting of the operation
confirmation function.
6.SAFETY FUNCTIONS OPERATION B-63944EN/03
- 1210 -
6.5.2 Functions that are Used when the Program is Executed
Overview
The following functions are provided to prevent improper operations
when the program is executed.
• Display of updated modal information
• Start check signal
• Axis status display
• Confirmation of the start from a middle block
• Data range check
• Maximum incremental value check
In the operation confirmation function setting screen, specify whether
to enable or disable these functions individually.
For information about how to display the setting screen, how to
manipulate it, and other details, see the item “Operation confirmation
setting screen” that describes the operation procedures.
6.5.2.1 Display of updated modal information
This function allows modal information updated by the NC command
or RESET to be highlighted in the modal information display for the
current block.
Display of updated modal information
Explanation
- Outline of the display of updated modal information
This function allows modal information updated by the NC command
or RESET to be highlighted in the modal information display for the
current block.
For example, when a absolute command has been changed to an
incremental command or when the workpiece coordinate system has
been initialized by RESET, the function displays the changed part of
the data in an easy-to-recognize manner, in order to prevent improper
operations during the execution of the program.
- Settings
In the operation confirmation function setting screen, check or
uncheck the "UPDATE MODAL HIGHLIGHT DISPLAY" box to
enable or disable this function. For information about how to display
the setting screen, how to set the function, and other details, see the
item “Operation confirmation setting” that describes the setting of the
operation confirmation function.
B-63944EN/03 OPERATION 6.SAFETY FUNCTIONS
- 1211 -
6.5.2.2 Start check signal
This function displays the remaining amount of travel and modal
information of the block to be executed and puts the program to a
temporary halt before the program is executed.
Start check signal
Explanation
- Outline of the start check signal
When a cycle start is made with the start check signal STCHK
<G0408 #0> set to 1, the function displays the remaining amount of
travel and modal information of the block to be executed and puts the
program to a temporary halt. Making the cycle start again resumes
the execution of the program.
The function lets you check the status of the block before executing it,
thus helping to prevent improper operations at the time of execution.
Using this function in combination with the updated modal
information display function described in the preceding subsection
makes it easier to check the status of the block to be executed.
- Settings
This function does not require any setting on the operation
confirmation function setting screen.
6.SAFETY FUNCTIONS OPERATION B-63944EN/03
- 1212 -
6.5.2.3 Axis status display
This function displays the axis status to the left of the axis name in the
coordinate display screen.
Axis status display
Explanation
- Outline of the axis status display
This function displays the axis status to the left of the axis name in the
display of the machine coordinates, absolute coordinates, relative
coordinates, and remaining travel amounts.
For example, when the mirror image function is enabled for the X1
axis, the absolute coordinates are displayed as follows.
By displaying the axis status as shown above, the function prevents
improper operations at the time of execution.
- Axis status indication
The axis status is indicated as follows. These indications are listed in
order of priority.
AXIS DETACH : D
INTERLOCK : I
MACHINE LOCK : L
SERVO OFF : S
AXIS MOVING : *
MIRROR IMAGE : M
- Settings
In the operation confirmation function setting screen, check or
uncheck the "AXIS STATUS DISPLAY" box to enable or disable this
function. For information about how to display the setting screen,
how to set the function, and other details, see the item “Operation
confirmation setting” that describes the setting of the operation
confirmation function.
A
BSOLUTE
M X1 10.000
Y1 10.000
Z1 0.000
B-63944EN/03 OPERATION 6.SAFETY FUNCTIONS
- 1213 -
6.5.2.4 Confirmation of the start from a middle block
This function displays a confirmation message when you attempt to
execute a memory operation with the cursor placed on a block in the
middle of the program.
Confirmation of the start from a middle block
Explanation
- Outline of the confirmation of the start from a middle block
This function displays the confirmation message "START FROM
MIDDLE OF PROG (START/RESET)" when you attempt to execute
a memory operation with the cursor placed on a block in the middle of
the program. It lets you confirm whether you really want to start
execution from that block or not before executing the program.
The function prevents you from inadvertently making a cycle start
from a block in the middle of the program.
- Settings
In the operation confirmation function setting screen, check or
uncheck the "START FROM MIDDLE OF PROGRAM" box to
enable or disable this function. For information about how to display
the setting screen, how to set the function, and other details, see the
item “Operation confirmation setting” that describes the setting of the
operation confirmation function.
6.SAFETY FUNCTIONS OPERATION B-63944EN/03
- 1214 -
6.5.2.5 Data range check
This function lets you set an effective data range and check whether
the data to be used for execution is within the set range.
Data range check
Explanation
- Outline of the data range check
This function lets you set an effective data range for each data item
listed later and check whether the data to be used for execution is
within the set range. If the data is out of the effective range, the
alarm PS0334 "OFFSET DATA OUT OF EFFECTIVE RANGE" is
displayed.
The function detects data setting mistakes and prevents the program
from running with invalid data.
- Data for which this function is effective
• Tool compensation
• Workpiece origin offset
T
• Y-axis tool offset
• Workpiece shift
NOTE
To use this function, you need to set each effective
data range correctly. For information about how to
set the data ranges, see the item “Effective value
range for each data”.
B-63944EN/03 OPERATION 6.SAFETY FUNCTIONS
- 1215 -
6.5.2.6 Maximum incremental value check
This function checks the maximum incremental value specified for
each axis by the NC command.
Maximum incremental value check
Explanation
- Outline of the maximum incremental value check
When the maximum incremental value is specified by the NC
command described later, make sure that the absolute value of the
travel distance by the incremental command does not exceed the
specified value. If the specified value is exceeded, the alarm PS0337
"EXCESS MAXIMUM INCREMENTAL VALUE" is displayed.
A maximum incremental value can be specified on a per-axis basis
and remains effective until 0 is set or the value is reset.
For example, when AI contour control is used, the function checks
whether the amount of movement between blocks is kept to the
specified value or less. Through this process, it detects erroneous
program settings and prevents the program from running with invalid
data.
- Format
The format of the NC command used to specify the maximum
incremental value is as follows.
G91.1 IP_ ;
IP_ ; Maximum incremental value
To cancel the maximum incremental value check, set 0.
6.SAFETY FUNCTIONS OPERATION B-63944EN/03
- 1216 -
6.5.3 Setting Screen
This section describes how to display the operation confirmation
function setting screen and how to set the individual data items on this
screen.
The operation confirmation function setting screen allows you to set
the following items:
• Enabling or disabling each operation confirmation function
• Effective value range for the tool offset
• Effective value range for the workpiece origin offset
T
• Effective value range for the Y-axis tool offset
• Effective value range for the work shift
B-63944EN/03 OPERATION 6.SAFETY FUNCTIONS
- 1217 -
6.5.3.1 Operation confirmation function setting screen
This screen displays the enable/disable setting status of the following
operation confirmation functions and lets you change their settings.
(Hereinafter, the screen is referred to as the operation confirmation
function setting screen.)
• Confirmation of incremental input
• Prohibition of the absolute input by the soft key
• Confirmation of the deletion of the program
• Confirmation of the deletion of all data
• Confirmation of a data update during the data setting process
• Display of updated modal information
• Axis status display
• Confirmation of the start from a middle block
Displaying and setting the operation confirmation function setting screen
Procedure
1 Press the function key.
2 Press the continuous menu key at the right edge of the
screen several times until the [GUARD] soft key is displayed.
3 Click the [GUARD] soft key. The setting screen that was
displayed last with relation to any operation confirmation
function is displayed (the operation confirmation function setting
screen is the first such screen that appears after the system is
restarted).
4 If any screen other than the operation confirmation function
setting screen is displayed, click the [GUARD] soft key. The
operation confirmation function setting screen is displayed.
Fig. 6.5.3.1 (a) Operation confirmation function setting screen
6.SAFETY FUNCTIONS OPERATION B-63944EN/03
- 1218 -
5 In the operation confirmation function setting screen, the check
box of each enabled function is checked (✓). Move the cursor
to the check box of the item you want to set, by pressing the
, , , and keys.
6 Click the operation soft key [ON:1] or [OFF:0]. When you
click the [ON:1] soft key, a check mark (✓) appears in the
corresponding check box, indicating that the function is enabled.
When you click the [OFF:0] soft key, the check mark disappears
from the check box, indicating that the function is disabled.
Explanation
- Items to be set
The following table shows what is displayed for each item to be set
and the corresponding functions.
Displayed item Corresponding function
INCREMENTAL INPUT Confirmation of incremental input
DISABLED SOFTKEY[INPUT] IN
TOOL OFFSET, WORK SHIFT
Prohibition of the absolute input by the
soft key (tool offset, Y-axis tool offset
(lathe system), and work shift (lathe
system))
DISABLED SOFTKEY[INPUT] IN
WORK COORDINATES
Prohibition of the absolute input by the
soft key (workpiece origin offset)
PROGRAM DELETE Confirmation of the deletion of the
program
ALL DATA DELETE Confirmation of the deletion of all data
INPUT IN SETTING Confirmation of a data update during the
data setting process
UPDATE MODAL HIGHLIGHT
DISPLAY
Display of updated modal information
AXIS STATUS DISPLAY Axis status display
START FROM MIDDLE OF PROGRAM Confirmation of the start from a middle
block
B-63944EN/03 OPERATION 6.SAFETY FUNCTIONS
- 1219 -
6.5.3.2 Tool offset range setting screen
This screen displays the setting status of tool offset effective data
ranges and lets you change their settings. (Hereinafter, the screen is
referred to as the tool offset range setting screen.)
Up to 20 pairs of numbers can be specified to identify tool offset
number ranges, and an effective offset value range can be defined for
each of these 20 pairs.
Displaying and setting the tool offset range setting screen
Procedure
1 Press the function key.
2 Press the continuous menu key at the right edge of the
screen several times until the [GUARD] soft key is displayed.
3 Click the [GUARD] soft key. The setting screen that was
displayed last with relation to any operation confirmation
function is displayed (the operation confirmation function setting
screen is the first such screen that appears after the system is
restarted).
4 If any screen other than the tool offset range setting screen is
displayed, click the [OFFSET] soft key. The tool offset range
setting screen is displayed. What is displayed in this screen
differs depending on the system configuration described later.
Fig. 6.5.3.2 (a) Tool offset range setting screen
5 Move the cursor to the item you want to set, by using the
and keys, , , , and keys, or the
[SWITCH] soft key.
6 Press the MDI key, enter necessary data, and then click the
[INPUT] soft key.
6.SAFETY FUNCTIONS OPERATION B-63944EN/03
- 1220 -
If the set effective data range is invalid for any of the reasons listed
below, the input data range check is not performed normally and the
input data is rejected.
• There is a tool offset number overlap.
• The upper and lower limit values are reversed.
• The values are not effective (e.g., more pairs of offset numbers
than allowed are set).
• Either of the tool offset numbers is 0.
Also, the input data range check is invalidated in the following cases.
• Both the upper and lower limit values for the tool offset number
are 0.
• The upper and lower offset limit values are identical.
Explanation
- System configuration
What to set differs for each of the following system configurations:
M
• Tool offset memory A
• Tool offset memory B
• Tool offset memory C
T
• Without geometry and wear offset
• With geometry and wear offset
B-63944EN/03 OPERATION 6.SAFETY FUNCTIONS
- 1221 -
M
- What to set with tool offset memory A
With tool offset memory A, an effective data range is specified using
the following four items.
Displayed item What to set
FROM
RANGE TO Specify a tool offset number range.
LOW-LIMIT
- UP-LIMIT
Specify a valid tool offset value range in connection
with a specified tool offset number range.
- What to set with tool offset memory B
With tool offset memory A, an effective data range is specified using
the following six items.
Displayed item What to set
FROM
RANGE TO Specify a tool offset number range.
LOW-LIMIT
GEOM UP-LIMIT
Specify a valid tool offset value range for geometry in
connection with a specified tool offset number range.
LOW-LIMIT
WEAR UP-LIMIT
Specify a valid tool offset value range for wear in
connection with a specified tool offset number range.
- What to set with tool offset memory C
With tool offset memory C, an effective data range is specified using
the following ten items.
Displayed item What to set
FROM
RANGE TO Specify a tool offset number range.
LOW-LIMIT
LENGTH UP-LIMIT
Specify a valid tool offset value range for geometry
length in connection with a specified tool offset number
range.
LOW-LIMIT
GEOM
RADIUS UP-LIMIT
Specify a valid tool offset value range for geometry
radius in connection with a specified tool offset number
range.
LOW-LIMIT
LENGTH UP-LIMIT
Specify a valid tool offset value range for wear length in
connection with a specified tool offset number range.
LOW-LIMIT
WEAR
RADIUS UP-LIMIT
Specify a valid tool offset value range for wear radius in
connection with a specified tool offset number range.
In the case of this configuration, all the information needed to set an
input data range cannot be displayed in a single screen page. Set the
information while switching pages using the [SWITCH] soft key.
The screen provides an indication that lets you know which part of the
information is currently displayed.
6.SAFETY FUNCTIONS OPERATION B-63944EN/03
- 1222 -
T
- What to set without geometry/wear offset
Without geometry/wear offset, an effective data range is specified
using the following eight items.
Displayed item What to set
FROM
RANGE TO Specify a tool offset number range.
LOW-LIMIT
X UP-LIMIT
Specify a valid tool offset value range for the X-axis in
connection with a specified tool offset number range.
LOW-LIMIT
Z UP-LIMIT
Specify a valid tool offset value range for the Z-axis in
connection with a specified tool offset number range.
LOW-LIMIT
RADIUS UP-LIMIT
Specify a valid tool offset value range for tool-nose radius in
connection with a specified tool offset number range.
NOTE
The radius-related items are not displayed if the
cutter or tool nose radius compensation is not used.
- What to set with geometry/wear offset
With geometry/wear offset, an effective data range is specified using
the following 12 items.
Displayed item What to set
FROM
RANGE TO Specify a tool offset number range.
LOW-LIMIT
X UP-LIMIT
Specify a valid tool offset value range for the geometry
X-axis in connection with a specified tool offset number
range.
LOW-LIMIT
Z UP-LIMIT
Specify a valid tool offset value range for the geometry
Z-axis in connection with a specified tool offset number
range.
LOW-LIMIT
GEOM
RADIUS UP-LIMIT
Specify a valid tool offset value range for geometry
tool-nose radius in connection with a specified tool offset
number range.
LOW-LIMIT
X UP-LIMIT
Specify a valid tool offset value range for the wear X-axis
in connection with a specified tool offset number range.
LOW-LIMIT
Z UP-LIMIT
Specify a valid tool offset value range for the wear Z-axis
in connection with a specified tool offset number range.
LOW-LIMIT
WEAR
RADIUS UP-LIMIT
Specify a valid tool offset value range for wear tool-nose
radius in connection with a specified tool offset number
range.
In the case of this system, all the information needed to set an input
data range cannot be displayed in a single screen page. Set the
information while switching pages using the [SWITCH] soft key.
The screen provides an indication that lets you know which part of the
information is currently displayed.
NOTE
The radius-related items are not displayed if the
tool nose radius compensation option is not
displayed.
B-63944EN/03 OPERATION 6.SAFETY FUNCTIONS
- 1223 -
- Example of setting an input data range
For example, suppose that the following values are set with offset
memory A.
FROM : TO LOW-LIMIT : UP-LIMIT
1 : 20 0.000 : 100.000
In this case, the tool offset input screen accepts only offset values
from 0.000 to 100.000 for offset numbers 1 to 20.
If you attempt to input any other value, the warning message "DATA
IS OUT OF RANGE" is displayed.
6.SAFETY FUNCTIONS OPERATION B-63944EN/03
- 1224 -
6.5.3.3 Workpiece origin offset range setting screen
This screen displays the setting status of workpiece origin offset and
external workpiece origin offset effective data ranges and lets you
change their settings. (Hereinafter, the screen is referred to as the
workpiece origin offset range setting screen.)
Up to six pairs of values can be specified to identify workpiece
coordinate ranges for the workpiece origin offset, and an effective
offset value range can be defined for each of the axes of these six pairs.
As for the external workpiece origin offset, an effective offset value
range can be specified for each axis.
Displaying and setting the workpiece origin offset range setting screen
Procedure
1 Press the function key.
2 Press the continuous menu key at the right edge of the
screen several times until the [GUARD] soft key is displayed.
3 Click the [GUARD] soft key. The setting screen that was
displayed last with relation to any operation confirmation
function is displayed (the operation confirmation function setting
screen is the first such screen that appears after the system is
restarted).
4 If any screen other than the workpiece origin offset range setting
screen is displayed, click the [WORK] soft key. The workpiece
origin offset range setting screen is displayed.
Fig. 6.5.3.3 (a) Workpiece origin offset range setting screen
B-63944EN/03 OPERATION 6.SAFETY FUNCTIONS
- 1225 -
5 Move the cursor to the item you want to set, by using the
and keys, , , , and keys, or the
[SWITCH] soft key.
6 Press the MDI key, enter necessary data, and then click the
[INPUT] soft key.
If the set effective data range is invalid for any of the reasons listed
below, the input data range check is not performed normally and the
input data is rejected.
• There is a workpiece coordinate overlap.
• The upper and lower limit values are reversed.
• The values are not effective (e.g., an invalid workpiece
coordinate system is set).
• The upper limit value is set for the workpiece coordinate system
when 0 is set for the lower limit value.
Also, the input data range check is invalidated in the following cases.
• Both the upper and lower limit values for the workpiece
coordinate system are 0.
• The upper and lower limit values for each offset are identical.
Explanation
- What to set for the workpiece origin offset
For the workpiece origin offset, an effective data range is specified
using the following four items.
Displayed item What to set
FROM
RANGE TO Specify a workpiece coordinate system range.
LOW-LIMITAXIS
NAME UP-LIMIT
Specify a valid offset value range in connection with a
specified workpiece coordinate system range.
- What to set for the external workpiece origin offset
For the external workpiece origin offset, an effective data range is
specified using the following two items.
Displayed item What to set
LOW-LIMITAXIS
NAME UP-LIMIT
Specify a valid external workpiece origin offset value range
on each axis.
6.SAFETY FUNCTIONS OPERATION B-63944EN/03
- 1226 -
6.5.3.4 Y-axis tool offset range setting screen
T
In the case of a lathe system, this screen displays the setting status of
Y-axis tool offset effective data ranges and lets you change their
settings. (Hereinafter, the screen is referred to as the Y-axis tool
offset range setting screen.)
Up to four pairs of values can be specified to identify Y-axis tool
offset number ranges, and an effective offset value range can be
defined for each of these four pairs.
Displaying and setting the Y-axis tool offset range setting screen
Procedure
1 Press the function key.
2 Press the continuous menu key at the right edge of the
screen several times until the [GUARD] soft key is displayed.
3 Click the [GUARD] soft key. The setting screen that was
displayed last with relation to any operation confirmation
function is displayed (the operation confirmation function setting
screen is the first such screen that appears after the system is
restarted).
4 If any screen other than the Y-axis tool offset range setting
screen is displayed, click the [OFST.2] soft key. The Y-axis
tool offset range setting screen is displayed. What is displayed
in this screen differs depending on such factors as whether tool
geometry/wear offsets are present.
Fig. 6.5.3.4 (a) Y-axis tool offset range setting screen
B-63944EN/03 OPERATION 6.SAFETY FUNCTIONS
- 1227 -
5 Move the cursor to the item you want to set, by using the
and keys, , , , and keys, or the
[SWITCH] soft key.
6 Press the MDI key, enter necessary data, and then click the
[INPUT] soft key.
If the set effective data range is invalid for any of the reasons listed
below, the input data range check is not performed normally and the
input data is rejected.
• There is a tool offset number overlap.
• The upper and lower limit values are reversed.
• The values are not effective (e.g., more pairs of offset numbers
than allowed are set).
• Either of the tool offset numbers is 0.
Also, the input data range check is invalidated in the following cases.
• Both the upper and lower limit values for the tool offset number
are 0.
• The upper and lower offset limit values are identical.
Explanation
- What to set without geometry/wear offsets
Without geometry/wear offsets, an effective data range is specified
using the following four items.
Displayed item What to set
FROM
RANGE TO Specify a Y-axis tool offset number range.
LOW-LIMIT
- UP-LIMIT
Specify a valid tool offset value range in connection
with a specified Y-axis tool offset number range.
- What to set with geometry/wear offsets
With geometry/wear offsets, an effective data range is specified using
the following six items.
Displayed item What to set
FROM
RANGE TO Specify a Y-axis tool offset number range.
LOW-LIMIT
GEOM UP-LIMIT
Specify a valid tool offset value range for geometry in
connection with a specified Y-axis tool offset number
range.
LOW-LIMIT
WEAR UP-LIMIT
Specify a valid tool offset value range for wear in
connection with a specified Y-axis tool offset number
range.
6.SAFETY FUNCTIONS OPERATION B-63944EN/03
- 1228 -
6.5.3.5 Workpiece shift range setting screen
T
In the case of a lathe system, this screen displays the setting status of
shift effective data ranges of workpiece shift coordinate systems and
lets you change their settings. (Hereinafter, the screen is referred to
as the workpiece shift range setting screen.)
An offset value range can be specified for each axis.
Displaying and setting workpiece shift input ranges
Procedure
1 Press the function key.
2 Press the continuous menu key at the right edge of the
screen several times until the [GUARD] soft key is displayed.
3 Click the [GUARD] soft key. The setting screen that was
displayed last with relation to any operation confirmation
function is displayed (the operation confirmation function setting
screen is the first such screen that appears after the system is
restarted).
4 If any screen other than the workpiece shift range setting screen
is displayed, click the [WORK SHIFT] soft key. The
workpiece shift range setting screen is displayed.
Fig. 6.5.3.5 (a) Workpiece shift range setting screen
5 Move the cursor to the item you want to set, by using the
and keys, , , , and keys, or the
[SWITCH] soft key.
6 Press the MDI key, enter necessary data, and then click the
[INPUT] soft key.
B-63944EN/03 OPERATION 6.SAFETY FUNCTIONS
- 1229 -
If the set effective data range is invalid for any of the reasons listed
below, the input data range check is not performed normally and the
input data is rejected.
• The upper and lower limit values are reversed.
Also, the input data range check is invalidated in the following cases.
• The upper and lower offset limit values are identical.
Explanation
- What to set for the workpiece shift
For the workpiece shift, an effective data range is specified using the
following two items.
Displayed item What to set
LOW-LIMITAXIS
NAME UP-LIMIT
Specify a valid workpiece shift coordinate system shift
value range on each axis.
OPERATION B-63944EN/03
- 1230 -
7. ALARM AND SELF-DIAGNOSIS
FUNCTIONS
7 ALARM AND SELF-DIAGNOSIS
FUNCTIONS
When an alarm occurs, the corresponding alarm screen appears to
indicate the cause of the alarm. The causes of alarms are classified by
error codes and number. Up to 60 previous alarms can be stored and
displayed on the screen (alarm history display).
The system may sometimes seem to be at a halt, although no alarm is
displayed. In this case, the system may be performing some
processing. The state of the system can be checked using the
self-diagnosis function.
B-63944EN/03 OPERATION
- 1231 -
7.ALARM AND SELF-DIAGNOSIS
FUNCTIONS
7.1 ALARM DISPLAY
Explanation
- Alarm screen
When an alarm is issued, the display changes to the alarm screen.
Two alarm screens "DETAIL" and "ALL PATH" are provided. You
can choose one of the screens by pressing the corresponding soft key.
• Detail screen
Alarm information for the currently selected path is displayed.
Fig. 7.1 (a) Alarm detail screen
• All path screen
Alarm information for all paths is displayed sequentially from
path 1.
Fig. 7.1 (b) All path screen
OPERATION B-63944EN/03
- 1232 -
7. ALARM AND SELF-DIAGNOSIS
FUNCTIONS
- Displaying an alarm screen
ALM is sometimes indicated in the bottom part of the screen display
without displaying an alarm screen.
Fig. 7.1 (c) Parameter screen
In this case, display the alarm screen by following the steps below.
1 Press the function key .
2 Press the soft key [ALARM].
3 Pressing the [ALARM] soft key changes the screen display to the
"DETAIL" screen (or the alarm screen selected previously), and
the [DETAIL] and [ALL PATH] soft keys appears.
• Pressing the [DETAIL] soft key displays the "DETAIL"
screen.
• Pressing the [ALL PATH] soft key displays the "ALL
PATH" screen.
If the number of paths is 1, pressing the [ALARM] soft key
displays the "DETAIL" screen, but the [ALARM] soft key
indication remains unchanged.
4 You can change pages by using the page key.
- Releasing alarm
The cause of an alarm can be determined from the error code, number,
and associated message. To release the alarm, generally correct the
cause, then press the reset key.
- Error code and number
The type of an alarm is indicated by an error code and number.
Example: PS0010, SV0004, etc.
For details, see Appendix G, "ALARMS".
B-63944EN/03 OPERATION
- 1233 -
7.ALARM AND SELF-DIAGNOSIS
FUNCTIONS
7.2 ALARM HISTORY DISPLAY
Up to 60 alarms (in 10 screen pages) issued by the CNC including the
latest alarm are stored and displayed on the screen.
The display procedure is explained below.
Alarm history display
Procedure
1 Press the function key .
2 Press the soft key [HISTRY].
An alarm history is displayed.
The following information is displayed:
<1> Date and time of alarm issuance
<2> Alarm type
<3> Alarm number
<4> Alarm message (sometimes not displayed depending on the
alarm)
<5> Page No.
3 You can change pages by using the page key.
Fig. 7.2 (a) Alarm history screen
OPERATION B-63944EN/03
- 1234 -
7. ALARM AND SELF-DIAGNOSIS
FUNCTIONS
7.3 CHECKING BY DIAGNOSTIC DISPLAY
The system may sometimes seem to be at a halt, although no alarm has
occurred. In this case, the system may be performing some processing.
Diagnostic display can be used to check the system status.
Procedure for Diagnostic display
Procedure
1 Press the function key .
2 Press the soft key [DGNOS].
3 The diagnosis screen has more than 1 pages. Select the screen by
the following operation.
(1) Change the page by the page change key.
(2) Method by soft key
• Key input the number of the diagnosis data to be
displayed.
• Press the soft key [NO.SRH].
Fig. 7.3 (a) Diagnostic display
B-63944EN/03 OPERATION
- 1235 -
7.ALARM AND SELF-DIAGNOSIS
FUNCTIONS
7.4 RETURN FROM THE ALARM SCREEN
7.4.1 Return from the Alarm Screen
When alarms are cleared or function key is pressed on the
alarm screen, the screen displayed before the alarm screen appears.
To enable this function, set bit 4 (ADC) of parameter No. 11302 is set
to 1.
Switching between screens when alarms are cleared
When all alarms are cleared on the alarm screen, the screen displayed
before the alarm screen appears again.
When the alarm screen was displayed automatically due to occurrence
of an alarm, the screen displayed immediately before the alarm
appears again.
When the alarm screen was displayed by pressing function key
during occurrence of an alarm, the screen displayed immediately
before the alarm appears again.
(Example)
NOTE
Even if alarms are cleared when the alarm screen
is not displayed, the current screen is not changed.
ALARM screen
PROGRAM screen
Occurrence of
an alarm
Clearing of
alarm
OPERATION B-63944EN/03
- 1236 -
7. ALARM AND SELF-DIAGNOSIS
FUNCTIONS
Switching between screens by the function key
When function key is pressed on the alarm screen, the screen
displayed before the alarm screen appears. Press function key
to switch to the alarm screen for checking for alarms and then press
function key to return to the previous screen.
(Example)
If function key is pressed when
the alarm screen was displayed automatically due to occurrence of an
alarm, the screen displayed before the alarm screen appears again.
Restrictions
• Switching to the interactive macro screen is not performed.
• The screens to which the alarm screen can be switched are only
the screen selected by the chapter selection soft key.
PROGRAM screen
Function key
Function key
ALARM screen
B-63944EN/03 OPERATION
- 1237 -
7.ALARM AND SELF-DIAGNOSIS
FUNCTIONS
7.4.2 Relationship with Other Functions
Relationship between the screen switching function and a return from the
alarm screen during switching between paths
(1) When bit 5 (PSC) of parameter No. 3208 is set to 0, if paths are
switched by the path switching signal or switching to the loader,
the screen last selected in the path appears again.
At this time, even if a return from the alarm screen to the
previous screen is performed in one path, a return is not
performed in the other path and the alarm screen remains
displayed.
(Example)
<1> When the message key is pressed on the offset screen of
path 1, the alarm screen (path 1) appears.
<2> When switching to path 2 is performed on the alarm screen
of path 1, the position screen of path 2 appears (when the
screen last displayed in path 2 is the position screen).
<3> When the message key is pressed on the position screen of
path 2, the alarm screen (path 2) appears.
<4> When the alarm is cleared or the message key is pressed on
the alarm screen of path 2, a return to the position screen
(path 2) is performed.
<5> When switching to path 1 is performed, the alarm screen
(path 1) appears.
(2) When PSC of parameter No. 3208 is set to 1, if paths are
switched by the path switching signal or switching to the loader,
the screen displayed immediately before the path switching
appears again.
At this time, if a return from the alarm screen to the previous
screen is performed in one path, the screen of the path in which a
return was performed appears in the other path.
Path 1
Path 2
Alarm
Offset
Alarm
Position <3>
<4>
<5>
<1>
<2>
OPERATION B-63944EN/03
- 1238 -
7. ALARM AND SELF-DIAGNOSIS
FUNCTIONS
(Example)
<1> When the message key is pressed on the offset screen of
path 1, the alarm screen (path 1) appears.
<2> When switching to path 2 is performed on the alarm screen
of path 1, the alarm screen (path 2) appears.
<3> When the alarm is cleared on the alarm screen of path 2, the
offset screen (path 2) appears.
<5> When switching to path 1 is performed, the offset screen of
path 1 appears.
Path 1
Path 2
Alarm
Offset
Alarm
Position
<3>
<4>
<2>
<1>
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1239 -
8 DATA INPUT/OUTPUT
Information stored in external I/O devices can be read into the CNC,
and information can be written into external I/O devices.
External I/O devices include memory cards that can be mounted to the
memory card interface located on the left side of the display unit and
personal computers and data servers that can be connected via
embedded Ethernet.
The following types of data can be input and output.
Data type Default file name
Program ALL-PROG.TXT
Offset data TOOLOFST.TXT
Parameter CNC-PARA.TXT
Pitch error compensation data PITCH.TXT
Custom macro common variable MACRO.TXT
Workpiece coordinate system data EXT_WKZ.TXT
Operation history data OPRT_HIS.TXT
Maintenance information MAINTINF.TXT
Periodic maintenance data (periodic maintenance:status screen) MAINTENA.TXT
Tool management data (tool management function) TOOL_MNG.TXT
Magazine data (tool management function) MAGAZINE.TXT
Tool life status name (tool management function) STATUS.TXT
Customize data name (tool management function) CUSTOMIZ.TXT
Second geometry tool offset SEC_GEOM.TXT
Three-dimensional error compensation data COMP3D.TXT
Rotary table dynamic fixture offset FIXTURE.TXT
Customize data displayed as tool management data (tool
management expansion) DISPCSTM.TXT
Spindle waiting position name (tool management expansion) POSNAME.TXT
Decimal point position data of customize data (tool management
expansion) POINTPOS.TXT
Real time custom macro variable RTMMACRO.TXT
System configuration data SYS-CONF.TXT
PMC signal protect DIDOENBL.TXT
Tool geometry data (tool management function for oversize tools) TOOLGEOM.TXT
Cause data (tool management tool attachment/detachment
function) TLCAUSE.TXT
Attachment history data (tool management tool
attachment/detachment function) TLATAHIS.TXT
Detachment history data (tool management tool
attachment/detachment function) TLDTAHIS.TXT
Servo/spindle information SV_SP_ID.TXT
Machine system name data (periodic maintenance:machine
system screen) MAINTEMC.TXT
Servo waveform diagnosis WAVE-DGN.TXT
Tool geometry data (check for tool post interference) TOOL-FRM.TXT
P code variable PCODE.TXT
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1240 -
Data type Default file name
Learning control data (learning control for parts cutting) PRT_LN.TXT
Learning control data (learning control) LEARN.TXT
High precision pitch error compensation UPEC.TXT
The above types of data can be input and output on the screens for
displaying and setting those types of data.
If NC data such as programs and parameters is to be written to a
memory card, and if a file with the same name already exists, it is
possible to select whether to overwrite the existing file or cancel
writing with appropriate operation.
This function is enabled by setting bit 1 (COW) of parameter No.
11308.
The external I/O device set in NC parameter No. 0020 is selected. See
the table below for details.
Correspondence between settings and input/output units
Setting Description
0,1 RS-232-C serial port 1
2 RS-232-C serial port 2
4 Memory card interface
5 Data server interface
9 Embedded Ethernet interface
NOTE
External I/O devices can handle file names of up to
12 characters each. NC programs on the memory
of the CNC can each be assigned any file name of
up to 32 characters, but the name is restricted to
up to 12 characters in the input/output to and from
external I/O devices.
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1241 -
8.1 OVERWRITING FILES ON A MEMORY CARD
Screen display
When an attempt is made to output NC data to a memory card, and if
the specified file name or the default file name is the same as an
existing file name on the memory card, a confirmation message
"OVERWRITE?" appears. (Bit 1 (COW) of parameter No. 11308 = 1)
Fig. 8.1 (a) Screen display example
Procedure
On the output screen for the desired function, perform the following
operation.
1 Press the soft key [PUNCH].
2 Press the soft key [EXEC]. If a file with the same name does not
exist on the memory card, the file is output in this step.
3 If a file with the same name exists on the memory card, soft keys
[REWRITE] and [CAN] appear.
Pressing the soft key [REWRITE] causes the file to be
overwritten.
Pressing the soft key [CAN] causes output to be canceled.
Example) Output from the parameter screen (for 7.2/8.4/10.4-inch
display unit)
1 Press the function key .
2 Press the soft key [PARAMETER].
3 Enter the EDIT mode or state emergency stop.
4 Press the soft key [(OPRT)].
5 For 7.2/8.4-inch display unit, press the continuous menu key
.
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1242 -
6 Press the soft key [PUNCH]. The soft key display switches from
the one in Fig. 8.1 (b) to the one in Fig. 8.1 (c).
7 Press the soft key [EXEC]. Because no file name is specified, the
file is output with a file name of CNC-PARA.TXT, but if a file
with the same name exists on the memory card, the soft key
display switches from the one in Fig. 8.1 (c) to the one in Fig. 8.1
(d), with a confirmation message appearing.
If a file with the same name does not exist on the memory card,
the file is output directly.
8 Pressing the soft key [REWRITE] causes the file to be
overwritten.
Pressing the soft key [CAN] causes output to be canceled. If
wishing to output the file after changing the file name, specify a
file name after step 6, and perform step 7 again.
Fig. 8.1 (b) Soft key display before [PUNCH] is pressed
Fig. 8.1 (c) Soft key display after [PUNCH] is pressed
Fig. 8.1 (d) Soft key display after [EXEC] is pressed
Example) Output from the parameter screen (for 15-inch display
unit)
1 Press the function key .
2 Press the vertical soft key [PARAMETER].
3 Enter the EDIT mode or state emergency stop.
4 Press the horizontal soft key [PUNCH]. The horizontal soft key
display switches from the one shown in Fig. 8.1 (e) to the one in
Fig. 8.1 (f).
5 Press the horizontal soft key [EXEC]. Because no file name is
specified, the file is output with a file name of CNC-PARA.TXT,
but if a file with the same name exists on the memory card, the
horizontal soft key display switches from the one in Fig. 8.1 (f)
to the one in Fig. 8.1 (g), with a confirmation message appearing.
If a file with the same name does not exist on the memory card,
the file is output directly.
6 Pressing the horizontal soft key [REWRITE] causes the file to be
overwritten.
Pressing the horizontal soft key [CAN] causes output to be
canceled. If wishing to output the file after changing the file
name, specify a file name after step 4, and perform step 5 again.
Fig. 8.1 (e) Soft key display before [PUNCH] is pressed
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1243 -
Fig. 8.1 (f) Soft key display after [PUNCH] is pressed
Fig. 8.1 (g) Soft key display after [EXEC] is pressed
CAUTION
Even if soft key [REWRITE] is pressed, warning
message "OVER WRITE FAILED" is issued and
output is canceled in the following cases:
- The file to be overwritten is for read only.
- The memory card is pulled out while the
confirmation message appears.
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1244 -
8.2 INPUT/OUTPUT ON EACH SCREEN
This section explains how to input and output data of the following
types to and from each operation screen: program, parameter, offset,
pitch error compensation, three-dimensional error compensation,
macro variable, workpiece coordinate system data, operation history,
and tool management.
Section 8.2, "INPUT/OUTPUT ON EACH SCREEN", consists of the
following subsections:
8.2.1 Inputting and Outputting a Program ..................................1246
8.2.1.1 Inputting a program ............................................1246
8.2.1.2 Outputting a program..........................................1248
8.2.2 Inputting and Outputting Parameters .................................1250
8.2.2.1 Inputting parameters ...........................................1250
8.2.2.2 Outputting parameters ........................................1252
8.2.3 Inputting and Outputting Offset Data ................................1254
8.2.3.1 Inputting offset data............................................1254
8.2.3.2 Outputting offset data .........................................1256
8.2.4 Inputting and Outputting Pitch Error Compensation Data.1261
8.2.4.1 Inputting pitch error compensation data .............1261
8.2.4.2 Outputting pitch error compensation data ..........1263
8.2.4.3 Input/output format of pitch error compensation
data .....................................................................1264
8.2.5 Inputting and Outputting Three-dimensional Error
Compensation Data............................................................1265
8.2.5.1 Inputting three-dimensional error compensation
data .....................................................................1265
8.2.5.2 Outputting three-dimensional error compensation
data .....................................................................1267
8.2.5.3 Input/output format of three-dimensional error
compensation data ..............................................1268
8.2.6 Inputting and Outputting Custom Macro Common
Variables ............................................................................1270
8.2.6.1 Inputting custom macro common variables........1270
8.2.6.2 Outputting custom macro common variables .....1272
8.2.7 Inputting and Outputting Workpiece Coordinates System
Data ....................................................................................1274
8.2.7.1 Inputting workpiece coordinate system data ......1274
8.2.7.2 Outputting workpiece coordinate system data....1276
8.2.8 Inputting and Outputting Operation History Data .............1277
8.2.8.1 Outputting operation history data.......................1277
8.2.9 Inputting and Outputting Tool Management Data .............1279
8.2.9.1 Inputting tool management data .........................1279
8.2.9.2 Outputting tool management data.......................1281
8.2.9.3 Inputting magazine data......................................1282
8.2.9.4 Outputting magazine data...................................1284
8.2.9.5 Inputting tool life status name data.....................1285
8.2.9.6 Outputting tool life status name data ..................1287
8.2.9.7 Inputting name data of customize data ...............1288
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1245 -
8.2.9.8 Outputting name data of customize data ............1290
8.2.9.9 Inputting customize data displayed as tool
management data ................................................1291
8.2.9.10 Outputting customize data displayed as tool
management data ................................................1293
8.2.9.11 Inputting spindle waiting position name data.....1294
8.2.9.12 Outputting spindle waiting position name data ..1296
8.2.9.13 Inputting decimal point position data of
customize data ....................................................1297
8.2.9.14 Outputting decimal point position data of
customize data ....................................................1299
8.2.9.15 Inputting tool geometry data...............................1300
8.2.9.16 Outputting tool geometry data............................1302
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1246 -
8.2.1 Inputting and Outputting a Program
8.2.1.1 Inputting a program
The following explains how to input a program from an external
device to the memory of the CNC by using the program editing screen
or program folder screen.
Inputting a program (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key to display the program editing
screen or program folder screen.
3 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
4 Press the soft key [(OPRT)].
5 Press the continuous menu key until soft key [READ]
appears.
Press the soft key [READ].
6 Type the name of the file that you want to input.
Press the soft key [F SET]. To specify the program name to input,
type the program name and press the soft key [P SET].
If the input file name is omitted, default input file name
“ALL-PROG.TXT” is assumed.
For an explanation of the operations to be performed if an input
file name [F SET] and an input program name [P SET] are
omitted, see the table below.
7 Press the soft key [EXEC].
This starts reading the program, and “INPUT” blinks in the lower
right part of the screen. When the read operation ends, the
“INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
Once read, the program is registered in the currently selected
foreground folder.
NOTE
Foreground folders are displayed on the program
folder screen. For an explanation of foreground
folders, see II-12.1.3, and for how to change
foreground folders, see III-11.6
[F SET] [P SET] Input file name Input program Input program name
BLANK BLANK ALL-PROG.TXT All programs in ALL-PROG.TXT File name at the time the file is saved
BLANK INPUT ALL-PROG.TXT First program in ALL-PROG.TXT Program name set with [P SET]
INPUT BLANK
File name set
with [F SET]
All programs in the file specified
with [F SET] File name at the time the file is saved
INPUT INPUT
File name set
with [F SET]
First program in the file specified
with [F SET] Program name set with [P SET]
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1247 -
Inputting a program (for 15-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key .
3 Press the vertical soft key [PROGRAM] or [FOLDER] to display
programs or a program directory.
4 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
5 Press the continuous menu key until horizontal soft key
[READ] appears.
Press the horizontal soft key [READ].
6 Type the name of the file that you want to input.
Press the horizontal soft key [F SET]. To specify the program
name to input, type the program name and press the horizontal
soft key [P SET].
If the input file name is omitted, default input file name
“ALL-PROG.TXT” is assumed.
For an explanation of the operations to be performed if an input
file name [F SET] and an input program name [P SET] are
omitted, see the table below.
7 Press the horizontal soft key [EXEC].
This starts reading the program, and “INPUT” blinks in the lower
right part of the screen. When the read operation ends, the
“INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
Once read, the program is registered in the currently selected
foreground folder.
NOTE
Foreground folders are displayed on the program
folder screen. For an explanation of foreground
folders, see II-12.1.3, and for how to change
foreground folders, see III-11.6
[F SET] [P SET] Input file name Input program Input program name
BLANK BLANK ALL-PROG.TXT All programs in ALL-PROG.TXT File name at the time the file is saved
BLANK INPUT ALL-PROG.TXT First program in ALL-PROG.TXT Program name set with [P SET]
INPUT BLANK
File name set
with [F SET]
All programs in the file specified
with [F SET] File name at the time the file is saved
INPUT INPUT
File name set
with [F SET]
First program in the file specified
with [F SET] Program name set with [P SET]
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1248 -
8.2.1.2 Outputting a program
A program stored in the memory of the CNC unit is output to an
external device.
Outputting a program (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key to display the program editing
screen or program folder screen.
3 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
4 Press the soft key [(OPRT)].
5 Press the continuous menu key until soft key [PUNCH]
appears.
Press the soft key [PUNCH].
6 Type the program number to output and press the soft key [P
SET]. To specify an output file name, type the output file name
and press the soft key [F SET].
If, in this step, no output file name or no program name is
specified, all programs in the foreground folders are output to
"ALL-PROG.TXT".
For an explanation of the operations to be performed if an output
file name [F SET] and an output program name [P SET] are
omitted, see the table below.
7 Press the soft key [EXEC].
This starts outputting the program, and “OUTPUT” blinks in the
lower right part of the screen. When the read operation ends, the
“OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
NOTE
Foreground folders are displayed on the program
folder screen. For an explanation of foreground
folders, see II-12.1.3, and for how to change
foreground folders, see III-11.6
[F SET] [P SET] Output file name Output program
BLANK BLANK or (O-9999) ALL-PROG.TXT All programs in the foreground folders
displayed in the program folder
BLANK INPUT Program name set with [P SET] Program in the NC that is set with [P SET]
INPUT BLANK or (O-9999) File name set with [F SET] All programs in the foreground folders
displayed in the program folder
INPUT INPUT File name set with [F SET] Program in the NC that is set with [P SET]
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1249 -
Outputting a program (for 15-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the vertical soft key [PROGRAM] or [FOLDER] to display
programs or a program directory.
4 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
5 Press the continuous menu key until horizontal soft key
[PUNCH] appears.
Press the horizontal soft key [PUNCH].
6 Type the program number to output and press the horizontal soft
key [P SET]. To specify an output file name, type the output file
name and press the horizontal soft key [F SET].
If, in this step, no output file name or no program name is
specified, all programs in the foreground folders are output to
“ALL-PROG.TXT”.
For an explanation of the operations to be performed if an output
file name [F SET] and an output program name [P SET] are
omitted, see the table below.
7 Press the horizontal soft key [EXEC].
This starts outputting the program, and “OUTPUT” blinks in the
lower right part of the screen. When the read operation ends, the
“OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
NOTE
Foreground folders are displayed on the program
folder screen. For an explanation of foreground
folders, see II-12.1.3, and for how to change
foreground folders, see III-11.6
[F SET] [P SET] Output file name Output program
BLANK BLANK or (O-9999) ALL-PROG.TXT All programs in the foreground folders
displayed in the program folder
BLANK INPUT Program name set with [P SET] Program in the NC that is set with [P SET]
INPUT BLANK or (O-9999) File name set with [F SET] All programs in the foreground folders
displayed in the program folder
INPUT INPUT File name set with [F SET] Program in the NC that is set with [P SET]
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1250 -
8.2.2 Inputting and Outputting Parameters
8.2.2.1 Inputting parameters
Parameters are loaded into the memory of the CNC unit from an
external device. The input format is the same as the output format.
When a parameter is loaded which has the same data number as a
parameter already registered in the memory, the loaded parameter
replaces the existing parameter.
Inputting parameters (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key .
3 Press the continuous menu key until soft key [SETTING]
appears.
Press the soft key [SETTING].
4 Press the MDI switch on the machine operator’s panel or enter
state emergency stop.
5 Enter 1 in response to the prompt for “PARAMETER WRITE”
in setting data.
Alarm SW0100 appears.
6 Press the function key .
7 Press the soft key [PARAMETER], then the parameter screen
appears.
8 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
9 Press the soft key [(OPRT)].
10 Press the continuous menu key until soft key [READ]
appears.
Press the soft key [READ].
11 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“CNC-PARA.TXT” is assumed.
12 Press the soft key [EXEC].
This starts reading the parameter, and “INPUT” blinks in the
lower right part of the screen. When the read operation ends, the
“INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
13 Press the function key .
14 Press the soft key [SETTING].
15 Press the MDI switch on the machine operator’s panel or enter
state emergency stop.
16 Enter 0 in response to the prompt for “PARAMETER WRITE”
in setting data.
17 Turn the power of the CNC on again.
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1251 -
Inputting parameters (for 15-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[SETTING] appears.
Press the vertical soft key [SETTING].
4 Press the MDI switch on the machine operator’s panel or enter
state emergency stop.
5 Enter 1 in response to the prompt for “PARAMETER WRITE”
in setting data.
Alarm SW0100 appears.
6 Press the function key .
7 Press the vertical soft key [NEXT PAGE] until vertical soft key
[PARAMETER] appears.
Press the vertical soft key [PARAMETER], then the parameter
screen appears.
8 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
9 Press the horizontal soft key [READ].
10 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“CNC-PARA.TXT” is assumed.
11 Press the horizontal soft key [EXEC].
This starts reading the parameter, and “INPUT” blinks in the
lower right part of the screen. When the read operation ends, the
“INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
12 Press the function key .
13 Press the vertical soft key [SETTING].
14 Press the MDI switch on the machine operator’s panel or enter
state emergency stop.
15 Enter 0 in response to the prompt for “PARAMETER WRITE”
in setting data.
16 Turn the power of the CNC on again.
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1252 -
8.2.2.2 Outputting parameters
All parameters are output in a defined output format from the memory
of the CNC to an external device.
Outputting parameters (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the soft key [PARAMETER], then the parameter screen
appears.
4 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
5 Press the soft key [(OPRT)].
6 Press the continuous menu key until soft key [PUNCH]
appears.
Press the soft key [PUNCH].
7 Type the file name that you want to output.
If the file name is omitted, default file name “CNC-PARA.TXT”
is assumed.
8 Press the soft key [EXEC].
This starts outputting the parameter, and “OUTPUT” blinks in
the lower right part of the screen. When the read operation ends,
the “OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
Outputting parameters (for 15-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[PARAMETER] appears.
Press the vertical soft key [PARAMETER], then the parameter
screen appears.
4 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
5 Press the horizontal soft key [PUNCH].
6 Type the file name that you want to output.
If the file name is omitted, default file name “CNC-PARA.TXT”
is assumed.
7 Press the horizontal soft key [EXEC].
This starts outputting the parameter, and “OUTPUT” blinks in
the lower right part of the screen. When the read operation ends,
the “OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1253 -
Explanation
- Suppressing output of parameters set to 0
When bit 1 (PRM) of parameter No. 0010 is set to 1, and soft key
[EXEC] is pressed, the following parameters are not output:
Other than axis type Axis type
Bit type Parameter for which all bits are
set to 0.
Parameter for an axis for which
all bits are set to 0.
Value type Parameter whose value is 0. Parameter for an axis for which
the value is 0.
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1254 -
8.2.3 Inputting and Outputting Offset Data
8.2.3.1 Inputting offset data
Offset data is loaded into the memory of the CNC from an external
device. The input format is the same as for offset value output.
When an offset value is loaded which has the same offset number as
an offset number already registered in the memory, the loaded offset
data replaces existing data.
Inputting offset data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key .
3 Press the continuous menu key until soft key [OFFSET]
appears.
Press the soft key [OFFSET].
4 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
5 Press the soft key [(OPRT)].
6 Press the continuous menu key until soft key [READ]
appears.
Press the soft key [READ].
7 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“TOOLOFST.TXT” is assumed.
8 Press the soft key [EXEC].
This starts reading the offset data, and “INPUT” blinks in the
lower right part of the screen. When the read operation ends, the
“INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1255 -
Inputting offset data (for 15-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[OFFSET] appears.
Press the vertical soft key [OFFSET].
4 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
5 Press the horizontal soft key [READ].
6 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“TOOLOFST.TXT” is assumed.
7 Press the horizontal soft key [EXEC].
This starts reading the offset data, and “INPUT” blinks in the
lower right part of the screen. When the read operation ends, the
“INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1256 -
8.2.3.2 Outputting offset data
All offset data is output in a defined output format from the memory
of the CNC to an external device.
Outputting offset data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the continuous menu key until soft key [OFFSET]
appears.
Press the soft key [OFFSET].
4 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
5 Press the soft key [(OPRT)].
6 Press the continuous menu key until soft key [PUNCH]
appears.
Press the soft key [PUNCH].
7 Type the file name that you want to output.
If the file name is omitted, default file name “TOOLOFST.TXT”
is assumed.
8 Press the soft key [EXEC].
This starts outputting the offset data, and “OUTPUT” blinks in
the lower right part of the screen. When the read operation ends,
the “OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
Outputting offset data (for 15-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[OFFSET] appears.
Press the vertical soft key [OFFSET].
4 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
5 Press the horizontal soft key [PUNCH].
6 Type the file name that you want to output.
If the file name is omitted, default file name “TOOLOFST.TXT”
is assumed.
7 Press the horizontal soft key [EXEC].
This starts outputting the offset data, and “OUTPUT” blinks in
the lower right part of the screen. When the read operation ends,
the “OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1257 -
Explanation
- Output format
Output format is as follows:
M
• Tool compensation memory A
%
G10 G90 P01 R_ Q_
G10 G90 P02 R_ Q_
...
G10 G90 P_ R_
%
Q_ : Virtual tool nose number (TIP). Not output when the
virtual tool nose direction is not used.
P_ : Tool offset number (1 to the number of tool
compensation pairs)
R_ : Tool compensation data. Output with a decimal
point in the input unit used at output.
• Tool compensation memory B
%
G10 G90 L10 P01 R_ Q_
G10 G90 L11 P01 R_
G10 G90 L10 P02 R_ Q_
...
G10 G90 L11 P_ R_
%
L10 : Geometric compensation amount
L11 : Wear compensation amount
Q_, P_, and R_ have the same meanings as for tool
compensation memory A.
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1258 -
• Tool compensation memory C
%
G10 G90 L10 P01 R_ Q_
G10 G90 L11 P01 R_
G10 G90 L12 P01 R_
G10 G90 L13 P01 R_
G10 G90 L10 P02 R_ Q_
...
G10 G90 L12 P_ R_
G10 G90 L13 P_ R_
%
L10 : Geometry compensation amount corresponding to the
H code
L11 : Wear compensation amount corresponding to the H
code
L12 : Geometry compensation amount corresponding to the
D code
L13 : Wear compensation amount corresponding to the D
code
Q_, P_, and R_ have the same meanings as for tool
compensation memory A.
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1259 -
T
The tool compensation amount and tool nose radius compensation
amount are output in the following format.
%
G10 P01 X_ Z_ R_ Q_ Y_
G10 P02 X_ Z_ R_ Q_ Y_
...
G10 P__ X_ Z_ R_ Q_ Y_
G10 P10001 X_ Z_ R_ Y_
G10 P10002 X_ Z_ R_ Y_
...
G10 P100__ X_ Z_ R_ Y_
%
P_: Tool compensation number (1 to the number of tool
compensation pairs)
Tool offset number: Specification of the tool
compensation amount and tool wear compensation
amount
10000 + tool offset number: Specification of the tool
geometry compensation amount
X_: Tool compensation data (X). Output with a decimal
point in the input unit used at output.
Z_: Tool compensation data (Z). Same as X_.
R_: Tool nose radius offset amount (R). The data format
is the same as for X_.
When tool nose radius compensation is not provided,
this item is not output.
Q_: Virtual tool nose number (TIP). When tool nose
radius compensation is not provided, this item is not
output.
Y_ : Tool compensation data (Y). The data format is the
same as for X_.
When no Y-axis offset is provided, this item is not
output.
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1260 -
The second geometry tool offset data is output in the following
format.
%
G10 P20001 X_ Z_ Y_
G10 P20002 X_ Z_ Y_
G10 P200__ X_ Z_ Y_
%
P_ : Tool compensation number (1 to the number of tool
compensation pairs)
Tool offset number: Specification of the tool
compensation amount and tool wear compensation
amount
20000 + tool offset number: Specification of the
second tool geometry compensation amount
The other addresses are the same as for the tool
compensation amount.
NOTE
The input format and output format do not depend
on the G-code system A/B/C.
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1261 -
8.2.4 Inputting and Outputting Pitch Error Compensation Data
8.2.4.1 Inputting pitch error compensation data
Pitch error compensation data are loaded into the memory of the CNC
from an external device. The input format is the same as the output
format. When a pitch error compensation data is loaded which has
the corresponding data number as a pitch error compensation data
already registered in the memory, the loaded data replaces the existing
data.
Inputting pitch error compensation data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key .
3 Press the continuous menu key until soft key [SETTING]
appears.
Press the soft key [SETTING].
4 Press the MDI switch on the machine operator’s panel or enter
state emergency stop.
5 Enter 1 in response to the prompt for “PARAMETER WRITE”
in setting data.
Alarm SW0100 appears.
6 Press the function key .
7 Press the continuous menu key until soft key [PITCH
ERROR] appears.
Press the soft key [PITCH ERROR].
8 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
9 Press the soft key [(OPRT)].
10 Press the continuous menu key until soft key [READ]
appears.
Press the soft key [READ].
11 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“PITCH.TXT” is assumed.
12 Press the soft key [EXEC].
This starts reading the pitch error compensation data, and
“INPUT” blinks in the lower right part of the screen. When the
read operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
13 Press the function key .
14 Press the soft key [SETTING].
15 Press the MDI switch on the machine operator’s panel or enter
state emergency stop.
16 Enter 0 in response to the prompt for “PARAMETER WRITE”
in setting data.
17 Turn the power of the CNC on again.
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1262 -
Inputting pitch error compensation data (for 15-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[SETTING] appears.
Press the vertical soft key [SETTING].
4 Press the MDI switch on the machine operator’s panel or enter
state emergency stop.
5 Enter 1 in response to the prompt for “PARAMETER WRITE”
in setting data.
Alarm SW0100 appears.
6 Press the function key .
7 Press the vertical soft key [NEXT PAGE] until vertical soft key
[PITCH ERROR] appears.
Press the vertical soft key [PITCH ERROR].
8 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
9 Press the horizontal soft key [READ].
10 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“PITCH.TXT” is assumed.
11 Press the horizontal soft key [EXEC].
This starts reading the pitch error compensation data, and
“INPUT” blinks in the lower right part of the screen. When the
read operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
12 Press the function key .
13 Press the vertical soft key [SETTING].
14 Press the MDI switch on the machine operator’s panel or enter
state emergency stop.
15 Enter 0 in response to the prompt for “PARAMETER WRITE”
in setting data.
16 Turn the power of the CNC on again.
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1263 -
8.2.4.2 Outputting pitch error compensation data
All pitch error compensation data are output in a defined output
format from the memory of the CNC to an external device.
Outputting pitch error compensation data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the continuous menu key until soft key [PITCH
ERROR] appears.
Press the soft key [PITCH ERROR].
4 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
5 Press the soft key [(OPRT)].
6 Press the continuous menu key until soft key [PUNCH]
appears.
Press the soft key [PUNCH].
7 Type the file name that you want to output.
If the file name is omitted, default file name “PITCH.TXT” is
assumed.
8 Press the soft key [EXEC].
This starts outputting the pitch error compensation data, and
“OUTPUT” blinks in the lower right part of the screen. When the
read operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
Outputting pitch error compensation data (for 15-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[SETTING] appears.
Press the vertical soft key [PITCH ERROR].
4 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
5 Press the horizontal soft key [PUNCH].
6 Type the file name that you want to output.
If the file name is omitted, default file name “PITCH.TXT” is
assumed.
7 Press the horizontal soft key [EXEC].
This starts outputting the pitch error compensation data, and
“OUTPUT” blinks in the lower right part of the screen. When the
read operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1264 -
8.2.4.3 Input/output format of pitch error compensation data
Pitch error compensation data is input and output in the following
input and output formats.
- Keywords
The following alphabets are used as keywords.
The numeric value following each keyword has the meaning listed
below:
Keyword Meaning of the following numeric value
N Pitch error compensation data number + 10000
Q Data identification
(1 : Parameter data, 0 : Pitch error compensation data )
P Pitch error compensation data value
- Format
Pitch error compensation data is output in the following format:
N ***** Q0 P **** ;
The 5-digit numeric value following N indicates a pitch error
compensation data number to which a value of 10000 is added.
Q0 indicates pitch error compensation data
The numeric value following P indicates the value (integer value) of
pitch error compensation data between -128 to 127.
The semicolon (;) indicates the end of block (LF in the ISO code or
CR in the EIA code).
Example
N10001Q0P100;
Pitch error compensation data number 1
Pitch error compensation data value 100
- Beginning and end of a record
A pitch error compensation data record begins with % and ends
with %.
Example
% ; .....................................Beginning of record
N10000Q0P10;
N10001Q0P100;
:
N11279Q0P0;
% .............................................. End of record
When parameters and pitch error compensation data are integrated
into one file, % is added to the beginning and end of the file.
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1265 -
8.2.5 Inputting and Outputting Three-dimensional Error
Compensation Data
8.2.5.1 Inputting three-dimensional error compensation data
Three-dimensional error compensation data are loaded into the
memory of the CNC from an external device. The input format is the
same as the output format. When a three-dimensional error
compensation data is loaded which has the corresponding data number
as a three-dimensional error compensation data already registered in
the memory, the loaded data replaces the existing data.
Inputting three-dimensional error compensation data (for 7.2/8.4/10.4-inch display
unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key .
3 Press the continuous menu key until soft key [SETTING]
appears.
Press the soft key [SETTING].
4 Press the MDI switch on the machine operator’s panel or enter
state emergency stop.
5 Enter 1 in response to the prompt for “PARAMETER WRITE”
in setting data.
Alarm SW0100 appears.
6 Press the function key .
7 Press the continuous menu key until soft key [3D ERR
COMP] appears.
Press the soft key [3D ERR COMP].
8 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
9 Press the soft key [(OPRT)].
10 Press the continuous menu key until soft key [READ]
appears.
Press the soft key [READ].
11 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“COMP3D.TXT” is assumed.
12 Press the soft key [EXEC].
This starts reading the three-dimensional error compensation data,
and “INPUT” blinks in the lower right part of the screen. When
the read operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
13 Press the function key .
14 Press the soft key [SETTING].
15 Press the MDI switch on the machine operator’s panel or enter
state emergency stop.
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1266 -
16 Enter 0 in response to the prompt for “PARAMETER WRITE”
in setting data.
17 Turn the power of the CNC on again.
Inputting three-dimensional error compensation data (for 15-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[SETTING] appears.
Press the vertical soft key [SETTING].
4 Press the MDI switch on the machine operator’s panel or enter
state emergency stop.
5 Enter 1 in response to the prompt for “PARAMETER WRITE”
in setting data.
Alarm SW0100 appears.
6 Press the function key .
7 Press the vertical soft key [NEXT PAGE] until vertical soft key
[3D ERR COMP] appears.
Press the vertical soft key [3D ERR COMP].
8 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
9 Press the horizontal soft key [READ].
10 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“COMP3D.TXT” is assumed.
11 Press the horizontal soft key [EXEC].
This starts reading the three-dimensional error compensation data,
and “INPUT” blinks in the lower right part of the screen. When
the read operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
12 Press the function key .
13 Press the vertical soft key [SETTING].
14 Press the MDI switch on the machine operator’s panel or enter
state emergency stop.
15 Enter 0 in response to the prompt for “PARAMETER WRITE”
in setting data.
16 Turn the power of the CNC on again.
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1267 -
8.2.5.2 Outputting three-dimensional error compensation data
All three-dimensional error compensation data are output in a defined
output format from the memory of the CNC to an external device.
Outputting three-dimensional error compensation data (for 7.2/8.4/10.4-inch display
unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the continuous menu key until soft key [3D ERR
COMP] appears.
Press the soft key [3D ERR COMP].
4 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
5 Press the soft key [(OPRT)].
6 Press the continuous menu key until soft key [PUNCH]
appears.
Press the soft key [PUNCH].
7 Type the file name that you want to output.
If the file name is omitted, default file name “COMP3D.TXT” is
assumed.
8 Press the soft key [EXEC].
This starts outputting the three-dimensional error compensation
data, and “OUTPUT” blinks in the lower right part of the screen.
When the read operation ends, the “OUTPUT” indication
disappears.
To cancel the output, press the soft key [CAN].
Outputting three-dimensional error compensation data (for 15-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[3D ERR COMP] appears.
Press the vertical soft key [3D ERR COMP].
4 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
5 Press the horizontal soft key [PUNCH].
6 Type the file name that you want to output.
If the file name is omitted, default file name “COMP3D.TXT” is
assumed.
7 Press the horizontal soft key [EXEC].
This starts outputting the three-dimensional error compensation
data, and “OUTPUT” blinks in the lower right part of the screen.
When the read operation ends, the “OUTPUT” indication
disappears.
To cancel the output, press the horizontal soft key [CAN].
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1268 -
8.2.5.3 Input/output format of three-dimensional error compensation
data
Three-dimensional error compensation data is input and output in the
following input and output formats.
- Keywords
The following alphabets are used as keywords.
The numeric value following each keyword has the meaning listed
below:
Keyword Meaning of the following numeric value
N Data number (compensation point number + 100000) as
represented with six digits
A1 1st compensation axis
A2 2nd compensation axis
A3 3rd compensation axis
P Compensation data (-128 to 127)
- Format
Three-dimensional error compensation data is output in the following
format:
N ***** A1 P **** A2 P **** A3 P **** ;
The 6-digit numeric value following N indicates a three-dimensional
error compensation data number to which a value of 100000 is added.
The numeric value following P indicates the value (integer value) of
three-dimensional error compensation data between -128 to 127.
The semicolon (;) indicates the end of block (LF in the ISO code or
CR in the EIA code).
Example
N100001A1P100A2P110A3P120;
Three-dimensional error compensation data
number: 1
Error compensation data value for the 1st
compensation axis: 100
Error compensation data value for the 2nd
compensation axis: 110
Error compensation data value for the 3rd
compensation axis: 120
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1269 -
- Beginning and end of a record
A three-dimensional error compensation data record begins with %
and ends with %.
Example
% ; .....................................Beginning of record
N100001 A1 P1 A2 P2 A3 P3 ;
N100002 A1 P0 A2 P0 A3 P-3 ;
:
N115625 A1 P1 A2 P1 A3 P0 ;
% .............................................. End of record
- Input of compensation data using G10
Compensation data can be changed from a machining program, using
the programmable parameter input function.
The command format is as follows:
%
G10 L51 ;
N_ P_ R_ ;
N_ P_ R_ ;
:
G11 ;
%
G10 L51 : Three-dimensional error compensation data input
mode
G11 : Cancellation of three-dimensional error
compensation data input mode
N : Compensation point number (1-15625)
P : Compensation axis number (1-3)
R : Compensation data (-128-127)
NOTE
1 To input compensation data using G10, the option
of the programmable parameter input function is
required.
2 In three-dimensional error compensation data input
mode, no other NC statements can be issued.
3 The decimal point cannot be used in address N, P,
and R.
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1270 -
8.2.6 Inputting and Outputting Custom Macro Common Variables
8.2.6.1 Inputting custom macro common variables
The value of a custom macro common variable is loaded into the
memory of the CNC from an external device. The same format used
to output custom macro common variables is used for input.
Inputting custom macro common variables (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key .
3 Press the continuous menu key until soft key [MACRO]
appears.
Press the soft key [MACRO].
4 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
5 Press the soft key [(OPRT)].
6 Press the continuous menu key until soft key [READ]
appears.
Press the soft key [READ].
7 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“MACRO.TXT” is assumed.
8 Press the soft key [EXEC].
This starts reading the custom macro common variables, and
“INPUT” blinks in the lower right part of the screen. When the
read operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
Inputting custom macro common variables (for 15-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[MACRO] appears.
Press the vertical soft key [MACRO].
4 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
5 Press the horizontal soft key [READ].
6 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“MACRO.TXT” is assumed.
7 Press the horizontal soft key [EXEC].
This starts reading the custom macro common variables, and
“INPUT” blinks in the lower right part of the screen. When the
read operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1271 -
Explanation
- Common variables
The common variables (#500 to #549) can be input and output.
(When the option for addition of common variable is specified, values
from #500 to #999 can be input and output.) #100 to #149 can be
input when bit 3 (PV5) of parameter No. 6001 is set to 1. (When the
option for addition of common variable is specified, values from #100
to #199 can be input and output.)
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1272 -
8.2.6.2 Outputting custom macro common variables
Custom macro common variables stored in the memory of the CNC
can be output in a defined output format to an external device.
Outputting custom macro common variables (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the continuous menu key until soft key [MACRO]
appears.
Press the soft key [MACRO].
4 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
5 Press the soft key [(OPRT)].
6 Press the continuous menu key until soft key [PUNCH]
appears.
Press the soft key [PUNCH].
7 Type the file name that you want to output.
If the file name is omitted, default file name “MACRO.TXT” is
assumed.
8 Press the soft key [EXEC].
This starts outputting the custom macro common variables, and
“OUTPUT” blinks in the lower right part of the screen. When the
read operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
Outputting custom macro common variables (for 15-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[MACRO] appears.
Press the vertical soft key [MACRO].
4 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
5 Press the horizontal soft key [PUNCH].
6 Type the file name that you want to output.
If the file name is omitted, default file name “MACRO.TXT” is
assumed.
7 Press the horizontal soft key [EXEC].
This starts outputting the custom macro common variables, and
“OUTPUT” blinks in the lower right part of the screen. When the
read operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1273 -
Explanation
- Output format
The output format is as follows:
The values of custom macro variables are output in a bit-image
hexadecimal representation of double-precision floating-point type
data.
%
G10L85P200(0000000000000000)
G10L85P200(0000000000000000)
G10L85P200(FFFFFFFFFFFFFFFF)
:
G10L85P500(4024000000000000)
G10L85P501(4021000000000000)
G10L85P502(0000000000000000)
:
SETVN500[ABC,DEF]
SETVN501[GHI,JKL]
SETVN502[MNO,PQR]
:
M02
%
NOTE
The conventional custom macro statement
program format cannot be used for output.
By setting bit 0 (MCO) of parameter No. 6019, it is possible to output
macro variable numbers and variable data values as comments after
normally output data.
The output comments do not affect data input.
- Common variable
The common variables (#500 to #549) can be input and output.
(When the option for addition of common variable is specified, values
from #500 to #999 can be input and output.) #100 to #149 can be
output when bit 3 (PV5) of parameter No. 6001 is set to 1. (When the
option for addition of common variable is specified, values from #100
to #199 can be input and output.)
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1274 -
8.2.7 Inputting and Outputting Workpiece Coordinates System
Data
8.2.7.1 Inputting workpiece coordinate system data
Coordinate system variable data is loaded into the memory of the
CNC from an external device. The input format is the same as the
output format. When coordinate system variable data with a data
number corresponding to existing coordinate system variable data
registered in the memory is loaded, the loaded coordinate system
variable data replaces the existing coordinate system variable data.
Inputting workpiece coordinate system data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key .
3 Press the continuous menu key until soft key [WORK]
appears.
Press the soft key [WORK].
4 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
5 Press the soft key [(OPRT)].
6 Press the continuous menu key until soft key [READ]
appears.
Press the soft key [READ].
7 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“EXT_WKZ.TXT” is assumed.
8 Press the soft key [EXEC].
This starts reading the workpiece coordinate system data, and
“INPUT” blinks in the lower right part of the screen. When the
read operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1275 -
Inputting workpiece coordinate system data (for 15-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[WORK] appears.
Press veertical soft key [WORK].
4 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
5 Press the horizontal soft key [READ].
6 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“EXT_WKZ.TXT” is assumed.
7 Press the horizontal soft key [EXEC].
This starts reading the workpiece coordinate system data, and
“INPUT” blinks in the lower right part of the screen. When the
read operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1276 -
8.2.7.2 Outputting workpiece coordinate system data
All coordinate system variable data is output in the output format from
the memory of the CNC to an external device.
Outputting workpiece coordinate system data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the continuous menu key until soft key [WORK]
appears.
Press the soft key [WORK].
4 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
5 Press the soft key [(OPRT)].
6 Press the continuous menu key until soft key [PUNCH]
appears.
Press the soft key [PUNCH].
7 Type the file name that you want to output.
If the file name is omitted, default file name “EXT_WKZ.TXT”
is assumed.
8 Press the soft key [EXEC].
This starts outputting the workpiece coordinate system data, and
“OUTPUT” blinks in the lower right part of the screen. When the
read operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
Outputting workpiece coordinate system data (for 15-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[WORK] appears.
Press veertical soft key [WORK].
4 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
5 Press the horizontal soft key [PUNCH].
6 Type the file name that you want to output.
If the file name is omitted, default file name “EXT_WKZ.TXT”
is assumed.
7 Press the horizontal soft key [EXEC].
This starts outputting the workpiece coordinate system data, and
“OUTPUT” blinks in the lower right part of the screen. When the
read operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1277 -
8.2.8 Inputting and Outputting Operation History Data
Only output operation is permitted on operation history data.
The output data is in text format. So, to reference the output data
you must use an application that can handle text files on the personal
computer.
8.2.8.1 Outputting operation history data
All operation history data is output in the output format form the
memory of the CNC to an external device.
Outputting operation history data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the continuous menu key until soft key [OPERAT
HISTRY] appears.
Press the soft key [OPERAT HISTRY].
4 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
5 Press the soft key [(OPRT)].
6 Press the soft key [PUNCH].
7 Type the file name that you want to output.
If the file name is omitted, default file name “OPRT_HIS.TXT”
is assumed.
8 Press the soft key [EXEC].
This starts outputting the operation history data, and “OUTPUT”
blinks in the lower right part of the screen. When the read
operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1278 -
Outputting operation history data (for 15-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[OPERAT HISTRY] appears.
Press the vertical soft key [OPERAT HISTRY].
4 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
5 Press the horizontal soft key [PUNCH].
6 Type the file name that you want to output.
If the file name is omitted, default file name “OPRT_HIS.TXT”
is assumed.
7 Press the horizontal soft key [EXEC].
This starts outputting the operation history data, and “OUTPUT”
blinks in the lower right part of the screen. When the read
operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1279 -
8.2.9 Inputting and Outputting Tool Management Data
NOTE
1 For multi-path systems, place all paths in the EDIT
mode before performing input and output
operations.
2 The format used is the same as the registration
format of the G10 format.
8.2.9.1 Inputting tool management data
Tool management data is loaded into the memory of the CNC from an
external device. The input format is the same as the output format.
When tool management data with a data number corresponding to
existing tool management data registered in the memory is loaded, the
loaded tool management data replaces the existing tool management
data.
Inputting tool management data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key to display the tool management
screen or magazine screen.
3 Press the EDIT switch on the machine operator’s panel.
4 Press the soft key [(OPRT)].
5 Press the soft key [READ].
6 Press the soft key [TOOL].
7 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“TOOL_MNG.TXT” is assumed.
8 Press the soft key [EXEC].
This starts reading the tool management data, and “INPUT”
blinks in the lower right part of the screen. When the read
operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
NOTE
When using oversize tool support of the tool management
function, keep the following in mind.
- If a target tool is registered in a cartridge and interferes
with other tools in registration or modification of tool
geometry data of the tool management data, PS alarm
5360 is issued. (The data is not input.)
- When restoring backup data in the state where all data
related to the tool management function in the NC is
cleared, restore tool geometry data, tool management
data, and cartridge management table data in this order.
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1280 -
Inputting tool management data (for 15-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[TOOL MANAGER] appears.
Press the vertical soft key [TOOL MANAGER].
4 Press the vertical soft key [MAGAZINE] or [TOOL].
5 Press the EDIT switch on the machine operator’s panel.
6 Press the horizontal soft key [READ].
7 Press the horizontal soft key [TOOL].
8 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“TOOL_MNG.TXT” is assumed.
9 Press the horizontal soft key [EXEC].
This starts reading the tool management data, and “INPUT”
blinks in the lower right part of the screen. When the read
operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
NOTE
When using oversize tool support of the tool
management function, keep the following in mind.
- If a target tool is registered in a cartridge and
interferes with other tools in registration or
modification of tool geometry data of the tool
management data, PS alarm 5360 is issued.
(The data is not input.)
- When restoring backup data in the state where
all data related to the tool management function
in the NC is cleared, restore tool geometry data,
tool management data, and cartridge
management table data in this order.
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1281 -
8.2.9.2 Outputting tool management data
All tool management data is output in the output format from the
memory of the CNC to an external device.
Outputting tool management data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key to display the tool management
screen or magazine screen.
3 Press the EDIT switch on the machine operator’s panel.
4 Press the soft key [(OPRT)].
5 Press the soft key [PUNCH].
6 Press the soft key [TOOL].
7 Type the file name that you want to output.
If the output file name is omitted, default output file name
“TOOL_MNG.TXT” is assumed.
8 Press the soft key [EXEC].
This starts outputting the tool management data, and “OUTPUT”
blinks in the lower right part of the screen. When the read
operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
Outputting tool management data (for 15-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[TOOL MANAGER] appears.
Press the vertical soft key [TOOL MANAGER].
4 Press the vertical soft key [MAGAZINE] or [TOOL].
5 Press the EDIT switch on the machine operator’s panel.
6 Press the horizontal soft key [PUNCH].
7 Press the horizontal soft key [TOOL].
8 Type the file name that you want to output.
If the output file name is omitted, default output file name
“TOOL_MNG.TXT” is assumed.
9 Press the horizontal soft key [EXEC].
This starts outputting the tool management data, and “OUTPUT”
blinks in the lower right part of the screen. When the read
operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1282 -
8.2.9.3 Inputting magazine data
Magazine data is loaded into the memory of the CNC from an external
device. The input format is the same as the output format. When
magazine data with a data number corresponding to existing magazine
data registered in the memory is loaded, the loaded magazine data
replaces the existing magazine data.
Inputting magazine data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key to display the tool management
screen or magazine screen.
3 Press the EDIT switch on the machine operator’s panel.
4 Press the soft key [(OPRT)].
5 Press the soft key [READ].
6 Press the soft key [MAGAZINE].
7 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“MAGAZINE.TXT” is assumed.
8 Press the soft key [EXEC].
This starts reading the magazine data, and “INPUT” blinks in the
lower right part of the screen. When the read operation ends, the
“INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
NOTE
When using oversize tool support of the tool
management function, keep the following in mind.
- If a tool interferes with other tools in registration
in or modification to the cartridge management
table, PS alarm 5360 is issued. (The data is
not input.)
- When restoring backup data in the state where
all data related to the tool management function
in the NC is cleared, restore tool geometry data,
tool management data, and cartridge
management table data in this order.
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1283 -
Inputting magazine data (for 15-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[TOOL MANAGER] appears.
Press the vertical soft key [TOOL MANAGER].
4 Press the vertical soft key [MAGAZINE] or [TOOL].
5 Press the EDIT switch on the machine operator’s panel.
6 Press the horizontal soft key [READ].
7 Press the horizontal soft key [MAGAZINE].
8 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“MAGAZINE.TXT” is assumed.
9 Press the horizontal soft key [EXEC].
This starts reading the magazine data, and “INPUT” blinks in the
lower right part of the screen. When the read operation ends, the
“INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
NOTE
When using oversize tool support of the tool
management function, keep the following in mind.
- If a tool interferes with other tools in registration
in or modification to the cartridge management
table, PS alarm 5360 is issued. (The data is
not input.)
- When restoring backup data in the state where
all data related to the tool management function
in the NC is cleared, restore tool geometry data,
tool management data, and cartridge
management table data in this order.
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1284 -
8.2.9.4 Outputting magazine data
All magazine data is output in the output format from the memory of
the CNC to an external device.
Outputting magazine data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key to display the tool management
screen or magazine screen.
3 Press the EDIT switch on the machine operator’s panel.
4 Press the soft key [(OPRT)].
5 Press the soft key [PUNCH].
6 Press the soft key [MAGAZINE].
7 Type the file name that you want to output.
If the file name is omitted, default file name “MAGAZINE.TXT”
is assumed.
8 Press the soft key [EXEC].
This starts outputting the magazine data, and “OUTPUT” blinks
in the lower right part of the screen. When the read operation
ends, the “OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
Outputting magazine data (for 15-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[TOOL MANAGER] appears.
Press the vertical soft key [TOOL MANAGER].
4 Press the vertical soft key [MAGAZINE] or [TOOL].
5 Press the EDIT switch on the machine operator’s panel.
6 Press the horizontal soft key [PUNCH].
7 Press the horizontal soft key [MAGAZINE].
8 Type the file name that you want to output.
If the file name is omitted, default file name “MAGAZINE.TXT”
is assumed.
9 Press the horizontal soft key [EXEC].
This starts outputting the magazine data, and “OUTPUT” blinks
in the lower right part of the screen. When the read operation
ends, the “OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1285 -
8.2.9.5 Inputting tool life status name data
Tool life status name data is loaded into the memory of the CNC from
an external device. The input format is the same as the output format.
When tool life status name data with a data number corresponding to
existing tool life status name data registered in the memory is loaded,
the loaded tool life status name data replaces the existing tool life
status name data.
Inputting tool life status name data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key to display the tool management
screen or magazine screen.
3 Press the EDIT switch on the machine operator’s panel.
4 Press the soft key [(OPRT)].
5 Press the soft key [READ].
6 Press the soft key [STATUS].
7 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“STATUS.TXT” is assumed.
8 Press the soft key [EXEC].
This starts reading the tool life status name data, and “INPUT”
blinks in the lower right part of the screen. When the read
operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1286 -
Inputting tool life status name data (for 15-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[TOOL MANAGER] appears.
Press the vertical soft key [TOOL MANAGER].
4 Press the vertical soft key [MAGAZINE] or [TOOL].
5 Press the EDIT switch on the machine operator’s panel.
6 Press the horizontal soft key [READ].
7 Press the horizontal soft key [STATUS].
8 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“STATUS.TXT” is assumed.
9 Press the horizontal soft key [EXEC].
This starts reading the tool life status name data, and “INPUT”
blinks in the lower right part of the screen. When the read
operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1287 -
8.2.9.6 Outputting tool life status name data
All tool life status name data is output in the output format from the
memory of the CNC to an external device.
Outputting tool life status name data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key to display the tool management
screen or magazine screen.
3 Press the EDIT switch on the machine operator’s panel.
4 Press the soft key [(OPRT)].
5 Press the soft key [PUNCH].
6 Press the soft key [STATUS].
7 Type the file name that you want to output.
If the file name is omitted, default file name “STATUS.TXT” is
assumed.
8 Press the soft key [EXEC].
This starts outputting the tool life status name data, and
“OUTPUT” blinks in the lower right part of the screen. When the
read operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
Outputting tool life status name data (for 15-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[TOOL MANAGER] appears.
Press the vertical soft key [TOOL MANAGER].
4 Press the vertical soft key [MAGAZINE] or [TOOL].
5 Press the EDIT switch on the machine operator’s panel.
6 Press the horizontal soft key [PUNCH].
7 Press the horizontal soft key [STATUS].
8 Type the file name that you want to output.
If the file name is omitted, default file name “STATUS.TXT” is
assumed.
9 Press the horizontal soft key [EXEC].
This starts outputting the tool life status name data, and
“OUTPUT” blinks in the lower right part of the screen. When the
read operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1288 -
8.2.9.7 Inputting name data of customize data
Name data of customize data is loaded into the memory of the CNC
from an external device. The input format is the same as the output
format. When name data of customize data with a data number
corresponding to existing name data of customize data registered in
the memory is loaded, the loaded name data of customize data
replaces the existing data.
Inputting name data of customize data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key to display the tool management
screen or magazine screen.
3 Press the EDIT switch on the machine operator’s panel.
4 Press the soft key [(OPRT)].
5 Press the soft key [READ].
6 Press the soft key [CUSTOM].
7 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“CUSTOMIZ.TXT” is assumed.
8 Press the soft key [EXEC].
This starts reading the name data of customize data, and
“INPUT” blinks in the lower right part of the screen. When the
read operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1289 -
Inputting name data of customize data (for 15-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[TOOL MANAGER] appears.
Press the vertical soft key [TOOL MANAGER].
4 Press the vertical soft key [MAGAZINE] or [TOOL].
5 Press the EDIT switch on the machine operator’s panel.
6 Press the horizontal soft key [READ].
7 Press the horizontal soft key [CUSTOM].
8 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“CUSTOMIZ.TXT” is assumed.
9 Press the horizontal soft key [EXEC].
This starts reading the name data of customize data, and
“INPUT” blinks in the lower right part of the screen. When the
read operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1290 -
8.2.9.8 Outputting name data of customize data
All name data of customize data is output in the output format from
the memory of the CNC to an external device.
Outputting name data of customize data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key to display the tool management
screen or magazine screen.
3 Press the EDIT switch on the machine operator’s panel.
4 Press the soft key [(OPRT)].
5 Press the soft key [PUNCH].
6 Press the soft key [CUSTOM].
7 Type the file name that you want to output.
If the file name is omitted, default file name “CUSTOMIZ.TXT”
is assumed.
8 Press the soft key [EXEC].
This starts outputting the name data of customize data, and
“OUTPUT” blinks in the lower right part of the screen. When the
read operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
Outputting name data of customize data (for 15-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[TOOL MANAGER] appears.
Press the vertical soft key [TOOL MANAGER].
4 Press the vertical soft key [MAGAZINE] or [TOOL].
5 Press the EDIT switch on the machine operator’s panel.
6 Press the horizontal soft key [PUNCH].
7 Press the horizontal soft key [CUSTOM].
8 Type the file name that you want to output.
If the file name is omitted, default file name “CUSTOMIZ.TXT”
is assumed.
9 Press the horizontal soft key [EXEC].
This starts outputting the name data of customize data, and
“OUTPUT” blinks in the lower right part of the screen. When the
read operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1291 -
8.2.9.9 Inputting customize data displayed as tool management data
Customize data displayed as tool management data is loaded into the
memory of the CNC from an external device. The input format is the
same as the output format. When customize data displayed as tool
management data with a data number corresponding to existing
customize data displayed as tool management data registered in the
memory is loaded, the loaded customize data replaces the existing
data.
Inputting customize data displayed as tool management data (for 7.2/8.4/10.4-inch
display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key to display the tool management
screen, magazine screen, or each tool data screen.
3 Press the EDIT switch on the machine operator’s panel.
4 Press the soft key [(OPRT)].
5 Press the soft key [READ].
6 Press the soft key [DSP-LAYOUT].
7 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“DISPCSTM.TXT” is assumed.
8 Press the soft key [EXEC].
This starts reading the customize data displayed as tool
management data, and “INPUT” blinks in the lower right part of
the screen. When the read operation ends, the “INPUT”
indication disappears.
To cancel the input of the program, press the soft key [CAN].
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1292 -
Inputting customize data displayed as tool management data (for 15-inch display
unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[TOOL MANAGER] appears.
Press the vertical soft key [TOOL MANAGER].
4 Press the vertical soft key [MAGAZINE], [EACH TOOL], or
[TOOL].
5 Press the EDIT switch on the machine operator’s panel.
6 Press the horizontal soft key [READ].
7 Press the horizontal soft key [DSP-LAYOUT].
8 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“DISPCSTM.TXT” is assumed.
9 Press the horizontal soft key [EXEC].
This starts reading the customize data displayed as tool
management data, and “INPUT” blinks in the lower right part of
the screen. When the read operation ends, the “INPUT”
indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1293 -
8.2.9.10 Outputting customize data displayed as tool management
data
Customize data displayed as tool management data is output from the
memory of the CNC to an external device in the output format.
Outputting customize data displayed as tool management data (for 7.2/8.4/10.4-inch
display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key to display the tool management
screen, magazine screen, or each tool data screen.
3 Press the EDIT switch on the machine operator’s panel.
4 Press the soft key [(OPRT)].
5 Press the soft key [PUNCH].
6 Press the soft key [DSP-LAYOUT].
7 Type the file name that you want to output.
If the file name is omitted, default file name “DISPCSTM.TXT”
is assumed.
8 Press the soft key [EXEC].
This starts outputting the customize data displayed as tool
management data, and “OUTPUT” blinks in the lower right part
of the screen. When the read operation ends, the “OUTPUT”
indication disappears.
To cancel the output, press the soft key [CAN].
Outputting customize data displayed as tool management data (for 15-inch display
unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[TOOL MANAGER] appears.
Press the vertical soft key [TOOL MANAGER].
4 Press the vertical soft key [MAGAZINE], [EACH TOOL], or
[TOOL].
5 Press the EDIT switch on the machine operator’s panel.
6 Press the horizontal soft key [PUNCH].
7 Press the horizontal soft key [DSP-LAYOUT].
8 Type the file name that you want to output.
If the file name is omitted, default file name “DISPCSTM.TXT”
is assumed.
9 Press the horizontal soft key [EXEC].
This starts outputting the customize data displayed as tool
management data, and “OUTPUT” blinks in the lower right part
of the screen. When the read operation ends, the “OUTPUT”
indication disappears.
To cancel the output, press the horizontal soft key [CAN].
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1294 -
8.2.9.11 Inputting spindle waiting position name data
Spindle waiting position name data is loaded into the memory of the
CNC from an external device. The input format is the same as the
output format. When spindle waiting position name data with a data
number corresponding to existing spindle waiting position name data
registered in the memory is loaded, the loaded spindle waiting
position name data replaces the existing data.
Inputting spindle waiting position name data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key to display the tool management
screen, magazine screen, or each tool data screen.
3 Press the EDIT switch on the machine operator’s panel.
4 Press the soft key [(OPRT)].
5 Press the soft key [READ].
6 Press the soft key [SPWP-NAME].
7 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“POSNAME.TXT” is assumed.
8 Press the soft key [EXEC].
This starts reading the spindle waiting position name data, and
“INPUT” blinks in the lower right part of the screen. When the
read operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1295 -
Inputting spindle waiting position name data (for 15-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[TOOL MANAGER] appears.
Press the vertical soft key [TOOL MANAGER].
4 Press the vertical soft key [MAGAZINE], [EACH TOOL], or
[TOOL].
5 Press the EDIT switch on the machine operator’s panel.
6 Press the horizontal soft key [READ].
7 Press the horizontal soft key [SPWP-NAME].
8 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“POSNAME.TXT” is assumed.
9 Press the horizontal soft key [EXEC].
This starts reading the spindle waiting position name data, and
“INPUT” blinks in the lower right part of the screen. When the
read operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1296 -
8.2.9.12 Outputting spindle waiting position name data
Spindle waiting position name data is output from the memory of the
CNC to an external device in the output format.
Outputting spindle waiting position name data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key to display the tool management
screen, magazine screen, or each tool data screen.
3 Press the EDIT switch on the machine operator’s panel.
4 Press the soft key [(OPRT)].
5 Press the soft key [PUNCH].
6 Press the soft key [SPWP-NAME].
7 Type the file name that you want to output.
If the file name is omitted, default file name “POSNAME.TXT”
is assumed.
8 Press the soft key [EXEC].
This starts outputting the spindle waiting position name data
display, and “OUTPUT” blinks in the lower right part of the
screen. When the read operation ends, the “OUTPUT” indication
disappears.
To cancel the output, press the soft key [CAN].
Outputting spindle waiting position name data (for 15-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[TOOL MANAGER] appears.
Press the vertical soft key [TOOL MANAGER].
4 Press the vertical soft key [MAGAZINE], [EACH TOOL], or
[TOOL].
5 Press the EDIT switch on the machine operator’s panel.
6 Press the horizontal soft key [PUNCH].
7 Press the horizontal soft key [SPWP-NAME].
8 Type the file name that you want to output.
If the file name is omitted, default file name “POSNAME.TXT”
is assumed.
9 Press the horizontal soft key [EXEC].
This starts outputting the spindle waiting position name data
display, and “OUTPUT” blinks in the lower right part of the
screen. When the read operation ends, the “OUTPUT” indication
disappears.
To cancel the output, press the horizontal soft key [CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1297 -
8.2.9.13 Inputting decimal point position data of customize data
Decimal point position data of customize data is loaded into the
memory of the CNC from an external device. The input format is the
same as the output format. When decimal point position data of
customize data with a data number corresponding to existing decimal
point position data of customize data registered in the memory is
loaded, the loaded decimal point position data of customize data
replaces the existing data.
Inputting decimal point position data of customize data (for 7.2/8.4/10.4-inch display
unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key to display the tool management
screen, magazine screen, or each tool data screen.
3 Press the EDIT switch on the machine operator’s panel.
4 Press the soft key [(OPRT)].
5 Press the soft key [READ].
6 Press the soft key [CSTM-DPOINT].
7 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“POINTPOS.TXT” is assumed.
8 Press the soft key [EXEC].
This starts reading the decimal point position data of customize
data, and “INPUT” blinks in the lower right part of the screen.
When the read operation ends, the “INPUT” indication
disappears.
To cancel the input of the program, press the soft key [CAN].
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1298 -
Inputting decimal point position data of customize data (for 15-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[TOOL MANAGER] appears.
Press the vertical soft key [TOOL MANAGER].
4 Press the vertical soft key [MAGAZINE], [EACH TOOL], or
[TOOL].
5 Press the EDIT switch on the machine operator’s panel.
6 Press the horizontal soft key [READ].
7 Press the horizontal soft key [CSTM-DPOINT].
8 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“POINTPOS.TXT” is assumed.
9 Press the horizontal soft key [EXEC].
This starts reading the decimal point position data of customize
data, and “INPUT” blinks in the lower right part of the screen.
When the read operation ends, the “INPUT” indication
disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1299 -
8.2.9.14 Outputting decimal point position data of customize data
Decimal point position data of customize data is output from the
memory of the CNC to an external device in the output format.
Outputting decimal point position data of customize data (for 7.2/8.4/10.4-inch
display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key to display the tool management
screen, magazine screen, or each tool data screen.
3 Press the EDIT switch on the machine operator’s panel.
4 Press the soft key [(OPRT)].
5 Press the soft key [PUNCH].
6 Press the soft key [CSTM-DPOINT].
7 Type the file name that you want to output.
If the file name is omitted, default file name “POINTPOS.TXT”
is assumed.
8 Press the soft key [EXEC].
This starts outputting the decimal point position data of
customize data, and “OUTPUT” blinks in the lower right part of
the screen. When the read operation ends, the “OUTPUT”
indication disappears.
To cancel the output, press the soft key [CAN].
Outputting decimal point position data of customize data (for 15-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[TOOL MANAGER] appears.
Press the vertical soft key [TOOL MANAGER].
4 Press the vertical soft key [MAGAZINE], [EACH TOOL], or
[TOOL].
5 Press the EDIT switch on the machine operator’s panel.
6 Press the horizontal soft key [PUNCH].
7 Press the horizontal soft key [CSTM-DPOINT].
8 Type the file name that you want to output.
If the file name is omitted, default file name “POINTPOS.TXT”
is assumed.
9 Press the horizontal soft key [EXEC].
This starts outputting the decimal point position data of
customize data, and “OUTPUT” blinks in the lower right part of
the screen. When the read operation ends, the “OUTPUT”
indication disappears.
To cancel the output, press the horizontal soft key [CAN].
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1300 -
8.2.9.15 Inputting tool geometry data
Tool geometry data is loaded into the memory of the CNC from an
external device. The input format is the same as the output format.
When tool geometry data with a data number corresponding to
existing tool geometry data registered in the memory is loaded, the
loaded tool geometry data replaces the existing data.
Inputting tool geometry data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key to display the tool management
screen, magazine screen, each tool data screen, or tool geometry
data screen.
3 Press the EDIT switch on the machine operator’s panel.
4 Press the soft key [(OPRT)].
5 Press the soft key [READ].
6 Press the soft key [TOOL- GEOM].
7 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“TOOLGEOM.TXT” is assumed.
8 Press the soft key [EXEC].
This starts reading the tool geometry data, and “INPUT” blinks
in the lower right part of the screen. When the read operation
ends, the “INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
NOTE
1 If the tool with a number of tool geometry data to be
changed is registered to the magazine when an
attempt is made to change the tool geometry data,
an alarm PS5360 is issued. (The data is not
input.)
2 After data related to the tool management functions
in the NC has all been cleared, restore backup data
in the following order: Tool geometry data, tool
management data, and magazine management
table.
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1301 -
Inputting tool geometry data (for 15-inch display unit)
Procedure
1 Make sure the input device is ready for reading.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[TOOL MANAGER] appears.
Press the vertical soft key [TOOL MANAGER].
4 Press the vertical soft key [MAGAZINE], [EACH TOOL],
[TOOL], or [TOOL- GEOM].
5 Press the EDIT switch on the machine operator’s panel.
6 Press the horizontal soft key [READ].
7 Press the horizontal soft key [TOOL- GEOM].
8 Type the name of the file that you want to input.
If the input file name is omitted, default input file name
“TOOLGEOM.TXT” is assumed.
9 Press the horizontal soft key [EXEC].
This starts reading the tool geometry data, and “INPUT” blinks
in the lower right part of the screen. When the read operation
ends, the “INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
NOTE
1 If the tool with a number of tool geometry data to be
changed is registered to the magazine when an
attempt is made to change the tool geometry data,
an alarm PS5360 is issued. (The data is not
input.)
2 After data related to the tool management functions
in the NC has all been cleared, restore backup data
in the following order: Tool geometry data, tool
management data, and magazine management
table.
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1302 -
8.2.9.16 Outputting tool geometry data
Tool geometry data is output from the memory of the CNC to an
external device in the output format.
Outputting tool geometry data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key to display the tool management
screen, magazine screen, each tool data screen, or tool geometry
data screen.
3 Press the EDIT switch on the machine operator’s panel.
4 Press the soft key [(OPRT)].
5 Press the soft key [PUNCH].
6 Press the soft key [TOOL- GEOM].
7 Type the file name that you want to output.
If the output file name is omitted, default output file name
“TOOLGEOM.TXT” is assumed.
8 Press the soft key [EXEC].
This starts outputting the tool geometry data, and “OUTPUT”
blinks in the lower right part of the screen. When the read
operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
Outputting tool geometry data (for 15-inch display unit)
Procedure
1 Make sure the output device is ready for output.
2 Press the function key .
3 Press the vertical soft key [NEXT PAGE] until vertical soft key
[TOOL MANAGER] appears.
Press the vertical soft key [TOOL MANAGER].
4 Press the vertical soft key [MAGAZINE], [EACH TOOL],
[TOOL], or [TOOL- GEOM].
5 Press the EDIT switch on the machine operator’s panel.
6 Press the horizontal soft key [PUNCH].
7 Press the horizontal soft key [TOOL- GEOM].
8 Type the file name that you want to output.
If the output file name is omitted, default output file name
“TOOLGEOM.TXT” is assumed.
9 Press the horizontal soft key [EXEC].
This starts outputting the tool geometry data, and “OUTPUT”
blinks in the lower right part of the screen. When the read
operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1303 -
8.3 INPUT/OUTPUT ON THE ALL IO SCREEN
Just by using the ALL IO screen, you can input and output programs,
parameters, offset data, pitch error compensation data, macro variables,
workpiece coordinate system data, operation history data, and tool
management data.
NOTE
The ALL IO screen can be operated only if a memory
card interface is selected as an external I/O device.
The following explains how to display the ALL IO screen:
Displaying the ALL IO screen (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Press the function key .
2 Press the continuous menu key several times.
3 Press the soft key [ALL IO] to display the ALL IO screen.
The subsequent steps to select data from the ALL IO screen will be
explained for each type of data.
Displaying the ALL IO screen (for 15-inch display unit)
Procedure
1 Press the function key .
2 Press the vertical soft key [NEXT PAGE] until vertical soft key
[ALL I/O] appears.
3 Press the vertical soft key [ALL I/O] to display the ALL IO
screen.
The subsequent steps to select data from the ALL IO screen will be
explained for each type of data.
Configuration of this section
Section 8.3, "INPUT/OUTPUT ON THE ALL IO SCREEN", consists
of the following subsections:
8.3.1 Inputting/Outputting a Program............................................1304
8.3.2 Inputting and Outputting Parameters....................................1308
8.3.3 Inputting and Outputting Offset Data...................................1311
8.3.4 Inputting/Outputting Pitch Error Compensation Data..........1313
8.3.5 Inputting/Outputting Custom Macro Common Variables ....1316
8.3.6 Inputting and Outputting Workpiece Coordinates System
Data.......................................................................................1318
8.3.7 Inputting and Outputting Operation History Data................1320
8.3.8 Inputting and Outputting Tool Management Data................1321
8.3.9 File Format and Error Messages...........................................1329
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1304 -
8.3.1 Inputting/Outputting a Program
A program can be input and output using the ALL IO screen.
Inputting a program (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Press the soft key [PROGRAM] on the ALL IO screen.
2 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
3 Press the soft key [(OPRT)].
4 Press the soft key [N READ].
5 Set the name of the file that you want to input.
Type a file name, and press the soft key [F NAME].
If the input file name is omitted, default input file name
“ALL-PROG.TXT” is assumed.
See the table below for details.
6 Set the program number to be used after the input.
Type a program number, and press the soft key [P SET].
If no program number is specified here, the program number in
the file is adopted as is.
7 Press the soft key [EXEC].
This starts reading the program, and “INPUT” blinks in the lower
right part of the screen. When the read operation ends, the
“INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
[F SET] [P SET] Input file name Input program Input program name
BLANK BLANK ALL-PROG.TXT All programs in ALL-PROG.TXT File name at the time the file is saved
BLANK INPUT ALL-PROG.TXT First program in ALL-PROG.TXT Program name set with [P SET]
INPUT BLANK
File name set
with [F NAME]
All programs in the file specified
with [F NAME] File name at the time the file is saved
INPUT INPUT
File name set
with [F NAME]
First program in the file specified
with [F NAME] Program name set with [P SET]
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1305 -
Inputting a program (for 15-inch display unit)
Procedure
1 On the ALL IO screen, press the vertical soft key [NEXT PAGE]
until vertical soft key [PROGRAM] appears.
Press the vertical soft key [PROGRAM].
2 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
3 Press the horizontal soft key [N READ].
4 Set the name of the file that you want to input.
Type a file name, and press the horizontal soft key [F NAME].
If the input file name is omitted, default input file name
“ALL-PROG.TXT” is assumed.
See the table below for details.
5 Set the program number to be used after the input.
Type a program number, and press the horizontal soft key [P
SET].
If no program number is specified here, the program number in
the file is adopted as is.
6 Press the horizontal soft key [EXEC].
This starts reading the program, and “INPUT” blinks in the lower
right part of the screen. When the read operation ends, the
“INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
[F SET] [P SET] Input file name Input program Input program name
BLANK BLANK ALL-PROG.TXT All programs in ALL-PROG.TXT File name at the time the file is saved
BLANK INPUT ALL-PROG.TXT First program in ALL-PROG.TXT Program name set with [P SET]
INPUT BLANK
File name set
with [F NAME]
All programs in the file specified
with [F NAME] File name at the time the file is saved
INPUT INPUT
File name set
with [F NAME]
First program in the file specified
with [F NAME] Program name set with [P SET]
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1306 -
Outputting a program (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Press the soft key [PROGRAM] on the ALL IO screen.
2 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
3 Press the soft key [(OPRT)].
4 Press the soft key [PUNCH].
5 Set the program that you want to output.
Type a program number, and press the soft key [P SET].
If O-9999 is typed, all programs in the memory are output.
6 Set the file name to be output.
Type a file name, and press the soft key [F NAME].
When no file name is set, the output file name is assumed to be
“O-number” if a single program number is specified; if O-9999 is
specified, the output file name is assumed to be
“ALL-PROG.TXT”.
See the table below for details.
(For an explanation of foreground folders, see II-12.1.3, and for
how to change foreground folders, see III-11.6.)
7 Press the soft key [EXEC].
This starts outputting the program, and “OUTPUT” blinks in the
lower right part of the screen. When the read operation ends, the
“OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
[F SET] [P SET] Output file name Output program
BLANK BLANK or (O-9999) ALL-PROG.TXT All programs in the foreground folders
displayed in the program folder
BLANK INPUT Program name set with [P SET] Program in the NC that is set with [P SET]
INPUT BLANK or (O-9999) File name set with [F NAME] All programs in the foreground folders
displayed in the program folder
INPUT INPUT File name set with [F NAME] Program in the NC that is set with [P SET]
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1307 -
Outputting a program (for 15-inch display unit)
Procedure
1 On the ALL IO screen, press the vertical soft key [NEXT PAGE]
until vertical soft key [PROGRAM] appears.
Press the vertical soft key [PROGRAM].
2 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
3 Press the horizontal soft key [PUNCH].
4 Set the program that you want to output.
Type a program number, and press the horizontal soft key [P
SET].
If O-9999 is typed, all programs in the memory are output.
5 Set the file name to be output.
Type a file name, and press the horizontal soft key [F NAME].
When no file name is set, the output file name is assumed to be
“O-number” if a single program number is specified; if O-9999 is
specified, the output file name is assumed to be
“ALL-PROG.TXT”.
See the table below for details.
(For an explanation of foreground folders, see II-12.1.3, and for
how to change foreground folders, see III-11.6.)
6 Press the horizontal soft key [EXEC].
This starts outputting the program, and “OUTPUT” blinks in the
lower right part of the screen. When the read operation ends, the
“OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
[F SET] [P SET] Output file name Output program
BLANK BLANK or (O-9999) ALL-PROG.TXT All programs in the foreground folders
displayed in the program folder
BLANK INPUT Program name set with [P SET] Program in the NC that is set with [P SET]
INPUT BLANK or (O-9999) File name set with [F NAME] All programs in the foreground folders
displayed in the program folder
INPUT INPUT File name set with [F NAME] Program in the NC that is set with [P SET]
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1308 -
8.3.2 Inputting and Outputting Parameters
Parameters can be input and output using the ALL IO screen.
Inputting parameters (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Press the function key .
2 Press the continuous menu key until soft key [SETTING]
appears.
Press the soft key [SETTING].
3 Press the MDI switch on the machine operator’s panel or enter
state emergency stop.
4 Enter 1 in response to the prompt for “PARAMETER WRITE”
in setting data.Alarm SW0100 appears.
5 Press the soft key [PARAMETER] on the ALL IO screen.
6 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
7 Press the soft key [(OPRT)].
8 Press the soft key [N READ].
9 Set the name of the file that you want to input.
Type a file name, and press the soft key [F NAME].
If the input file name is omitted, default input file name
“CNC-PARA.TXT” is assumed.
10 Press the soft key [EXEC].
This starts reading the parameter, and “INPUT” blinks in the
lower right part of the screen. When the read operation ends, the
“INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
11 Press the function key .
12 Press the soft key [SETTING].
13 Press the MDI switch on the machine operator’s panel or enter
state emergency stop.
14 Enter 0 in response to the prompt for “PARAMETER WRITE”
in setting data.
15 Turn the power of the CNC on again.
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1309 -
Inputting parameters (for 15-inch display unit)
Procedure
1 Press the function key .
2 Press the vertical soft key [NEXT PAGE] until vertical soft key
[SETTING] appears.
Press the vertical soft key [SETTING].
3 Press the MDI switch on the machine operator’s panel or enter
state emergency stop.
4 Enter 1 in response to the prompt for “PARAMETER WRITE”
in setting data.Alarm SW0100 appears.
5 On the ALL IO screen, press the vertical soft key [NEXT PAGE]
until vertical soft key [PARAMETER] appears.
Press the vertical soft key [PARAMETER].
6 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
7 Press the horizontal soft key [N READ].
8 Set the name of the file that you want to input.
Type a file name, and press the horizontal soft key [F NAME].
If the input file name is omitted, default input file name
“CNC-PARA.TXT” is assumed.
9 Press the horizontal soft key [EXEC].
This starts reading the parameter, and “INPUT” blinks in the
lower right part of the screen. When the read operation ends, the
“INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
10 Press the function key .
11 Press the vertical soft key [SETTING].
12 Press the MDI switch on the machine operator’s panel or enter
state emergency stop.
13 Enter 0 in response to the prompt for “PARAMETER WRITE”
in setting data.
14 Turn the power of the CNC on again.
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1310 -
Outputting parameters (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Press the soft key [PARAMETER] on the ALL IO screen.
2 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
3 Press the soft key [(OPRT)].
4 Press the soft key [PUNCH].
5 Set the file name to be output.
Type a file name, and press the soft key [F NAME].
If the file name is omitted, default file name “CNC-PARA.TXT”
is assumed.
6 Press the soft key [EXEC].
This starts outputting the parameter, and “OUTPUT” blinks in
the lower right part of the screen. When the read operation ends,
the “OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
Outputting parameters (for 15-inch display unit)
Procedure
1 On the ALL IO screen, press the vertical soft key [NEXT PAGE]
until vertical soft key [PARAMETER] appears.
Press the vertical soft key [PARAMETER].
2 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
3 Press the horizontal soft key [PUNCH].
4 Set the file name to be output.
Type a file name, and press the horizontal soft key [F NAME].
If the file name is omitted, default file name “CNC-PARA.TXT”
is assumed.
5 Press the horizontal soft key [EXEC].
This starts outputting the parameter, and “OUTPUT” blinks in
the lower right part of the screen. When the read operation ends,
the “OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1311 -
8.3.3 Inputting and Outputting Offset Data
Offset data can be input and output using the ALL IO screen.
Inputting offset data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Press the soft key [OFFSET] on the ALL IO screen.
2 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
3 Press the soft key [(OPRT)].
4 Press the soft key [N READ].
5 Set the name of the file that you want to input.
Type a file name, and press the soft key [F NAME].
If the input file name is omitted, default input file name
“TOOLOFST.TXT” is assumed.
6 Press the soft key [EXEC].
This starts reading the offset data, and “INPUT” blinks in the
lower right part of the screen. When the read operation ends, the
“INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
Inputting offset data (for 15-inch display unit)
Procedure
1 On the ALL IO screen, press the vertical soft key [NEXT PAGE]
until vertical soft key [OFFSET] appears.
Press the vertical soft key [OFFSET].
2 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
3 Press the horizontal soft key [N READ].
4 Set the name of the file that you want to input.
Type a file name, and press the horizontal soft key [F NAME].
If the input file name is omitted, default input file name
“TOOLOFST.TXT” is assumed.
5 Press the horizontal soft key [EXEC].
This starts reading the offset data, and “INPUT” blinks in the
lower right part of the screen. When the read operation ends, the
“INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1312 -
Outputting offset data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Press the soft key [OFFSET] on the ALL IO screen.
2 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
3 Press the soft key [(OPRT)].
4 Press the soft key [PUNCH].
5 Set the file name to be output.
Type a file name, and press the soft key [F NAME].
If the file name is omitted, default file name “TOOLOFST.TXT”
is assumed.
6 Press the soft key [EXEC].
This starts outputting the offset data, and “OUTPUT” blinks in
the lower right part of the screen. When the read operation ends,
the “OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
Outputting offset data (for 15-inch display unit)
Procedure
1 On the ALL IO screen, press the vertical soft key [NEXT PAGE]
until vertical soft key [OFFSET] appears.
Press the vertical soft key [OFFSET].
2 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
3 Press the horizontal soft key [PUNCH].
4 Set the file name to be output.
Type a file name, and press the horizontal soft key [F NAME].
If the file name is omitted, default file name “TOOLOFST.TXT”
is assumed.
5 Press the horizontal soft key [EXEC].
This starts outputting the offset data, and “OUTPUT” blinks in
the lower right part of the screen. When the read operation ends,
the “OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1313 -
8.3.4 Inputting/Outputting Pitch Error Compensation Data
Pitch error compensation data can be input and output using the ALL
IO screen.
Inputting pitch error compensation data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Press the function key .
2 Press the continuous menu key until soft key [SETTING]
appears.
Press the soft key [SETTING].
3 Press the MDI switch on the machine operator’s panel or enter
state emergency stop.
4 Enter 1 in response to the prompt for “PARAMETER WRITE”
in setting data.Alarm SW0100 appears.
5 Press the soft key [PITCH] on the ALL IO screen.
6 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
7 Press the soft key [(OPRT)].
8 Press the soft key [N READ].
9 Set the name of the file that you want to input.
Type a file name, and press the soft key [F NAME].
If the input file name is omitted, default input file name
“PITCH.TXT” is assumed.
10 Press the soft key [EXEC].
This starts reading the pitch error compensation data, and
“INPUT” blinks in the lower right part of the screen. When the
read operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
11 Press the function key .
12 Press the soft key [SETTING].
13 Press the MDI switch on the machine operator’s panel or enter
state emergency stop.
14 Enter 0 in response to the prompt for “PARAMETER WRITE”
in setting data.
15 Turn the power of the CNC on again.
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1314 -
Inputting pitch error compensation data (for 15-inch display unit)
Procedure
1 Press the function key .
2 Press the vertical soft key [NEXT PAGE] until vertical soft key
[SETTING] appears.
Press the vertical soft key [SETTING].
3 Press the MDI switch on the machine operator’s panel or enter
state emergency stop.
4 Enter 1 in response to the prompt for “PARAMETER WRITE”
in setting data.Alarm SW0100 appears.
5 On the ALL IO screen, press the vertical soft key [NEXT PAGE]
until vertical soft key [PITCH ERROR] appears.
Press the vertical soft key [PITCH ERROR].
6 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
7 Press the horizontal soft key [N READ].
8 Set the name of the file that you want to input.
Type a file name, and press the horizontal soft key [F NAME].
If the input file name is omitted, default input file name
“PITCH.TXT” is assumed.
9 Press the horizontal soft key [EXEC].
This starts reading the pitch error compensation data, and
“INPUT” blinks in the lower right part of the screen. When the
read operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
10 Press the function key .
11 Press the vertical soft key [SETTING].
12 Press the MDI switch on the machine operator’s panel or enter
state emergency stop.
13 Enter 0 in response to the prompt for “PARAMETER WRITE”
in setting data.
14 Turn the power of the CNC on again.
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1315 -
Outputting pitch error compensation data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Press the soft key [PITCH] on the ALL IO screen.
2 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
3 Press the soft key [(OPRT)].
4 Press the soft key [PUNCH].
5 Set the file name to be output.
Type a file name, and press the soft key [F NAME].
If the file name is omitted, default file name “PITCH.TXT” is
assumed.
6 Press the soft key [EXEC].
This starts outputting the pitch error compensation data, and
“OUTPUT” blinks in the lower right part of the screen. When the
read operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
Outputting pitch error compensation data (for 15-inch display unit)
Procedure
1 On the ALL IO screen, press the vertical soft key [NEXT PAGE]
until vertical soft key [PITCH ERROR] appears.
Press the vertical soft key [PITCH ERROR].
2 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
3 Press the horizontal soft key [PUNCH].
4 Set the file name to be output.
Type a file name, and press the horizontal soft key [F NAME].
If the file name is omitted, default file name “PITCH.TXT” is
assumed.
5 Press the horizontal soft key [EXEC].
This starts outputting the pitch error compensation data, and
“OUTPUT” blinks in the lower right part of the screen. When the
read operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1316 -
8.3.5 Inputting/Outputting Custom Macro Common Variables
Custom macro common variables can be input and output using the
ALL IO screen.
Inputting custom macro common variables (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Press the soft key [MACRO] on the ALL IO screen.
2 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
3 Press the soft key [(OPRT)].
4 Press the soft key [N READ].
5 Set the name of the file that you want to input.
Type a file name, and press the soft key [F NAME].
If the input file name is omitted, default input file name
“MACRO.TXT” is assumed.
6 Press the soft key [EXEC].
This starts reading the custom macro common variables, and
“INPUT” blinks in the lower right part of the screen. When the
read operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
Inputting custom macro common variables (for 15-inch display unit)
Procedure
1 On the ALL IO screen, press the vertical soft key [NEXT PAGE]
until vertical soft key [MACRO] appears.
Press the vertical soft key [MACRO].
2 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
3 Press the horizontal soft key [N READ].
4 Set the name of the file that you want to input.
Type a file name, and press the horizontal soft key [F NAME].
If the input file name is omitted, default input file name
“MACRO.TXT” is assumed.
5 Press the horizontal soft key [EXEC].
This starts reading the custom macro common variables, and
“INPUT” blinks in the lower right part of the screen. When the
read operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1317 -
Outputting custom macro common variables (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Press the soft key [MACRO] on the ALL IO screen.
2 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
3 Press the soft key [(OPRT)].
4 Press the soft key [PUNCH].
5 Set the file name to be output.
Type a file name, and press the soft key [F NAME].
If the file name is omitted, default file name “MACRO.TXT” is
assumed.
6 Press the soft key [EXEC].
This starts outputting the custom macro common variables, and
“OUTPUT” blinks in the lower right part of the screen. When the
read operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
Outputting custom macro common variables (for 15-inch display unit)
Procedure
1 On the ALL IO screen, press the vertical soft key [NEXT PAGE]
until vertical soft key [MACRO] appears.
Press the vertical soft key [MACRO].
2 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
3 Press the horizontal soft key [PUNCH].
4 Set the file name to be output.
Type a file name, and press the horizontal soft key [F NAME].
If the file name is omitted, default file name “MACRO.TXT” is
assumed.
5 Press the horizontal soft key [EXEC].
This starts outputting the custom macro common variables, and
“OUTPUT” blinks in the lower right part of the screen. When the
read operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1318 -
8.3.6 Inputting and Outputting Workpiece Coordinates System
Data
Workpiece coordinates system data can be input and output using the
ALL IO screen.
Inputting workpiece coordinate system data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Press the soft key [WORK] on the ALL IO screen.
2 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
3 Press the soft key [(OPRT)].
4 Press the soft key [N READ].
5 Set the name of the file that you want to input.
Type a file name, and press the soft key [F NAME].
If the input file name is omitted, default input file name
“EXT_WKZ.TXT” is assumed.
6 Press the soft key [EXEC].
This starts reading the workpiece coordinate system data, and
“INPUT” blinks in the lower right part of the screen. When the
read operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
Inputting workpiece coordinate system data (for 15-inch display unit)
Procedure
1 On the ALL IO screen, press the vertical soft key [NEXT PAGE]
until vertical soft key [WORK] appears.
Press veertical soft key [WORK].
2 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
3 Press the horizontal soft key [N READ].
4 Set the name of the file that you want to input.
Type a file name, and press the horizontal soft key [F NAME].
If the input file name is omitted, default input file name
“EXT_WKZ.TXT” is assumed.
5 Press the horizontal soft key [EXEC].
This starts reading the workpiece coordinate system data, and
“INPUT” blinks in the lower right part of the screen. When the
read operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1319 -
Outputting workpiece coordinate system data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Press the soft key [WORK] on the ALL IO screen.
2 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
3 Press the soft key [(OPRT)].
4 Press the soft key [PUNCH].
5 Set the file name to be output.
Type a file name, and press the soft key [F NAME].
If the file name is omitted, default file name “EXT_WKZ.TXT”
is assumed.
6 Press the soft key [EXEC].
This starts outputting the workpiece coordinate system data, and
“OUTPUT” blinks in the lower right part of the screen. When the
read operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
Outputting workpiece coordinate system data (for 15-inch display unit)
Procedure
1 On the ALL IO screen, press the vertical soft key [NEXT PAGE]
until vertical soft key [WORK] appears.
Press veertical soft key [WORK].
2 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
3 Press the horizontal soft key [PUNCH].
4 Set the file name to be output.
Type a file name, and press the horizontal soft key [F NAME].
If the file name is omitted, default file name “EXT_WKZ.TXT”
is assumed.
5 Press the horizontal soft key [EXEC].
This starts outputting the workpiece coordinate system data, and
“OUTPUT” blinks in the lower right part of the screen. When the
read operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1320 -
8.3.7 Inputting and Outputting Operation History Data
Operation history data can be output on the ALL IO screen (with
function key for 15-inch display unit).
Only output operation is permitted for operation history data.
The output data is of text format. So, to reference the output data
you must use an application that can handle text files on the personal
computer.
Outputting operation history data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Press the soft key [OPERAT HISTRY] on the ALL IO screen.
2 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
3 Press the soft key [(OPRT)].
4 Press the soft key [PUNCH].
5 Set the file name to be output.
Type a file name, and press the soft key [F NAME].
If the file name is omitted, default file name “OPRT_HIS.TXT”
is assumed.
6 Press the soft key [EXEC].
This starts outputting the operation history data, and “OUTPUT”
blinks in the lower right part of the screen. When the read
operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
Outputting operation history data (for 15-inch display unit)
Procedure
1 Press the function key .
2 On the ALL IO screen, press the vertical soft key [NEXT PAGE]
until vertical soft key [OPERAT HISTRY] appears.
Press the vertical soft key [OPERAT HISTRY].
3 Press the EDIT switch on the machine operator’s panel or enter
state emergency stop.
4 Press the horizontal soft key [PUNCH].
5 Set the file name to be output.
If the file name is omitted, default file name “OPRT_HIS.TXT”
is assumed.
6 Press the horizontal soft key [EXEC].
This starts outputting the operation history data, and “OUTPUT”
blinks in the lower right part of the screen. When the read
operation ends, the “OUTPUT” indication disappears.To cancel
the output, press the horizontal soft key [CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1321 -
8.3.8 Inputting and Outputting Tool Management Data
Tool management data can be input and output using the ALL IO
screen.
NOTE
1 For multi-path systems, place all paths in the EDIT
mode before performing input and output
operations.
2 The format used is the same as the registration
format of the G10 format.
Inputting tool management data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Press the soft key [TOOL] on the ALL IO screen.
2 Press the EDIT switch on the machine operator’s panel.
3 Press the soft key [(OPRT)].
4 Press the soft key [N READ].
5 Set the name of the file that you want to input.
Type a file name, and press the soft key [F NAME].
If the input file name is omitted, default input file name
“TOOL_MNG.TXT” is assumed.
6 Press the soft key [EXEC].
This starts reading the tool management data, and “INPUT”
blinks in the lower right part of the screen. When the read
operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
Inputting tool management data (for 15-inch display unit)
Procedure
1 On the ALL IO screen, press the vertical soft key [NEXT PAGE]
until vertical soft key [TOOL] appears.
Press the vertical soft key [TOOL].
2 Press the EDIT switch on the machine operator’s panel.
3 Press the horizontal soft key [N READ].
4 Set the name of the file that you want to input.
Type a file name, and press the horizontal soft key [F NAME].
If the input file name is omitted, default input file name
“TOOL_MNG.TXT” is assumed.
5 Press the horizontal soft key [EXEC].
This starts reading the tool management data, and “INPUT”
blinks in the lower right part of the screen. When the read
operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1322 -
Outputting tool management data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Press the soft key [TOOL] on the ALL IO screen.
2 Press the EDIT switch on the machine operator’s panel.
3 Press the soft key [(OPRT)].
4 Press the soft key [PUNCH].
5 Set the file name to be output.
Type a file name, and press the soft key [F NAME].
If the output file name is omitted, default output file name
“TOOL_MNG.TXT” is assumed.
6 Press the soft key [EXEC].
This starts outputting the tool management data, and “OUTPUT”
blinks in the lower right part of the screen. When the read
operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
Outputting tool management data (for 15-inch display unit)
Procedure
1 On the ALL IO screen, press the vertical soft key [NEXT PAGE]
until vertical soft key [TOOL] appears.
Press the vertical soft key [TOOL].
2 Press the EDIT switch on the machine operator’s panel.
3 Press the horizontal soft key [PUNCH].
4 Set the file name to be output.
Type a file name, and press the horizontal soft key [F NAME].
If the output file name is omitted, default output file name
“TOOL_MNG.TXT” is assumed.
5 Press the horizontal soft key [EXEC].
This starts outputting the tool management data, and “OUTPUT”
blinks in the lower right part of the screen. When the read
operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1323 -
Inputting magazine data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Press the soft key [MAGAZINE] on the ALL IO screen.
2 Press the EDIT switch on the machine operator’s panel.
3 Press the soft key [(OPRT)].
4 Press the soft key [N READ].
5 Set the name of the file that you want to input.
Type a file name, and press the soft key [F NAME].
If the input file name is omitted, default input file name
“MAGAZINE.TXT” is assumed.
6 Press the soft key [EXEC].
This starts reading the magazine data, and “INPUT” blinks in the
lower right part of the screen. When the read operation ends, the
“INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
Inputting magazine data (for 15-inch display unit)
Procedure
1 On the ALL IO screen, press the vertical soft key [NEXT PAGE]
until vertical soft key [MAGAZINE] appears.
Press the vertical soft key [MAGAZINE].
2 Press the EDIT switch on the machine operator’s panel.
3 Press the horizontal soft key [N READ].
4 Set the name of the file that you want to input.
Type a file name, and press the horizontal soft key [F NAME].
If the input file name is omitted, default input file name
“MAGAZINE.TXT” is assumed.
5 Press the horizontal soft key [EXEC].
This starts reading the magazine data, and “INPUT” blinks in the
lower right part of the screen. When the read operation ends, the
“INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1324 -
Outputting magazine data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Press the soft key [MAGAZINE] on the ALL IO screen.
2 Press the EDIT switch on the machine operator’s panel.
3 Press the soft key [(OPRT)].
4 Press the soft key [PUNCH].
5 Set the file name to be output.
Type a file name, and press the soft key [F NAME].
If the file name is omitted, default file name “MAGAZINE.TXT”
is assumed.
6 Press the soft key [EXEC].
This starts outputting the magazine data, and “OUTPUT” blinks
in the lower right part of the screen. When the read operation
ends, the “OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
Outputting magazine data (for 15-inch display unit)
Procedure
1 On the ALL IO screen, press the vertical soft key [NEXT PAGE]
until vertical soft key [MAGAZINE] appears.
Press the vertical soft key [MAGAZINE].
2 Press the EDIT switch on the machine operator’s panel.
3 Press the horizontal soft key [PUNCH].
4 Set the file name to be output.
Type a file name, and press the horizontal soft key [F NAME].
If the file name is omitted, default file name “MAGAZINE.TXT”
is assumed.
5 Press the horizontal soft key [EXEC].
This starts outputting the magazine data, and “OUTPUT” blinks
in the lower right part of the screen. When the read operation
ends, the “OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1325 -
Inputting tool life status name data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Press the soft key [STATUS] on the ALL IO screen.
2 Press the EDIT switch on the machine operator’s panel.
3 Press the soft key [(OPRT)].
4 Press the soft key [N READ].
5 Set the name of the file that you want to input.
Type a file name, and press the soft key [F NAME].
If the input file name is omitted, default input file name
“STATUS.TXT” is assumed.
6 Press the soft key [EXEC].
This starts reading the tool life status name data, and “INPUT”
blinks in the lower right part of the screen. When the read
operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
Inputting tool life status name data (for 15-inch display unit)
Procedure
1 On the ALL IO screen, press the vertical soft key [NEXT PAGE]
until vertical soft key [STATUS] appears.
Press the vertical soft key [STATUS].
2 Press the EDIT switch on the machine operator’s panel.
3 Press the horizontal soft key [N READ].
4 Set the name of the file that you want to input.
Type a file name, and press the horizontal soft key [F NAME].
If the input file name is omitted, default input file name
“STATUS.TXT” is assumed.
5 Press the horizontal soft key [EXEC].
This starts reading the tool life status name data, and “INPUT”
blinks in the lower right part of the screen. When the read
operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1326 -
Outputting tool life status name data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Press the soft key [STATUS] on the ALL IO screen.
2 Press the EDIT switch on the machine operator’s panel.
3 Press the soft key [(OPRT)].
4 Press the soft key [PUNCH].
5 Set the file name to be output.
Type a file name, and press the soft key [F NAME].
If the file name is omitted, default file name “STATUS.TXT” is
assumed.
6 Press the soft key [EXEC].
This starts outputting the tool life status name data, and
“OUTPUT” blinks in the lower right part of the screen. When the
read operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
Outputting tool life status name data (for 15-inch display unit)
Procedure
1 On the ALL IO screen, press the vertical soft key [NEXT PAGE]
until vertical soft key [STATUS] appears.
Press the vertical soft key [STATUS].
2 Press the EDIT switch on the machine operator’s panel.
3 Press the horizontal soft key [PUNCH].
4 Set the file name to be output.
Type a file name, and press the horizontal soft key [F NAME].
If the file name is omitted, default file name “STATUS.TXT” is
assumed.
5 Press the horizontal soft key [EXEC].
This starts outputting the tool life status name data, and
“OUTPUT” blinks in the lower right part of the screen. When the
read operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1327 -
Inputting name data of customize data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Press the soft key [CUSTOM] on the ALL IO screen.
2 Press the EDIT switch on the machine operator’s panel.
3 Press the soft key [(OPRT)].
4 Press the soft key [N READ].
5 Set the name of the file that you want to input.
Type a file name, and press the soft key [F NAME].
If the input file name is omitted, default input file name
“CUSTOMIZ.TXT” is assumed.
6 Press the soft key [EXEC].
This starts reading the name data of customize data, and
“INPUT” blinks in the lower right part of the screen. When the
read operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
Inputting name data of customize data (for 15-inch display unit)
Procedure
1 On the ALL IO screen, press the vertical soft key [NEXT PAGE]
until vertical soft key [CUSTOM] appears.
Press the vertical soft key [CUSTOM].
2 Press the EDIT switch on the machine operator’s panel.
3 Press the horizontal soft key [N READ].
4 Set the name of the file that you want to input.
Type a file name, and press the horizontal soft key [F NAME].
If the input file name is omitted, default input file name
“CUSTOMIZ.TXT” is assumed.
5 Press the horizontal soft key [EXEC].
This starts reading the name data of customize data, and
“INPUT” blinks in the lower right part of the screen. When the
read operation ends, the “INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1328 -
Outputting name data of customize data (for 7.2/8.4/10.4-inch display unit)
Procedure
1 Press the soft key [CUSTOM] on the ALL IO screen.
2 Press the EDIT switch on the machine operator’s panel.
3 Press the soft key [(OPRT)].
4 Press the soft key [PUNCH].
5 Set the file name to be output.
Type a file name, and press the soft key [F NAME].
If the file name is omitted, default file name “CUSTOMIZ.TXT”
is assumed.
6 Press the soft key [EXEC].
This starts outputting the name data of customize data, and
“OUTPUT” blinks in the lower right part of the screen. When the
read operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the soft key [CAN].
Outputting name data of customize data (for 15-inch display unit)
Procedure
1 On the ALL IO screen, press the vertical soft key [NEXT PAGE]
until vertical soft key [CUSTOM] appears.
Press the vertical soft key [CUSTOM].
2 Press the EDIT switch on the machine operator’s panel.
3 Press the horizontal soft key [PUNCH].
4 Set the file name to be output.
Type a file name, and press the horizontal soft key [F NAME].
If the file name is omitted, default file name “CUSTOMIZ.TXT”
is assumed.
5 Press the horizontal soft key [EXEC].
This starts outputting the name data of customize data, and
“OUTPUT” blinks in the lower right part of the screen. When the
read operation ends, the “OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1329 -
8.3.9 File Format and Error Messages
Explanation
- File format
All files that are read from and written to an external device are of text
format. The format is described below.
A file starts with % or LF, followed by the actual data. A file always
ends with %. In a read operation, data between the first % and the
next LF is skipped. Each block ends with an LF, not a semicolon (;).
• LF: 0A (hexadecimal) of ASCII code
• When a file containing lowercase letters, kana characters, and
several special characters (such as $, \, and !) is read, those letters
and characters are ignored.
Example)
%
O0001(MEMORY CARD SAMPLE FILE)
G17 G49 G97
G92 X-11.3 Y2.33
:
:
M30
%
• ASCII code is used for input/output, regardless of the setting
parameter (ISO/EIA).
• Bit 3 (NCR) of parameter No. 0100 can be used to specify
whether the end of block code (EOB) is output as "LF" only, or
as "LF, CR, CR."
Limitation
- Memory card specification
Use memory cards that comply with PCMCIA Ver2.0 or JEIDA
Ver4.1.
- Attribute memory
Memory cards that have no attribute memory or contain no device
information in the attribute memory cannot be used.
- Flash ROM card
Flash ROM cards can be used for reading only.
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1330 -
8.4 EMBEDDED ETHERNET OPERATIONS
8.4.1 FTP File Transfer Function
The operation of the FTP file transfer function is described below.
Host file list display (for 7.2/8.4/10.4-inch display unit)
A list of the files held on the host computer is displayed.
Procedure
1 Press the function key .
2 Press the soft key [FOLDER]. The program list screen appears.
(If the soft key does not appear, press the continuous menu key
.)
3 Press the soft key [(OPRT)].
4 Press the soft key [DEVICE CHANGE].
5 Press the soft key [EMB ETHER], and the EMBEDDED
ETHERNET HOST FILE LIST screen appears.
Fig. 8.4.1 (a) Embedded Ethernet host file list screen
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1331 -
NOTE
1 When using the FTP file transfer function, check
that the valid device is the embedded Ethernet port.
The two conditions below determine a connection
destination on the host file list screen:
(1) Check that the valid device is the embedded
Ethernet port. Make a selection in "DEVICE
SELECTION" on the Ethernet setting screen.
(2) A host computer can be selected from
connection destinations 1, 2, and 3. Make a
selection according to soft key [HOST CHANGE]
described later.
2 File names including kanji, hiragana, and katakana
characters cannot be displayed correctly.
6 When a list of files is larger than one page, the screen display can
be switched using the page keys .
7 Press the soft key [REFRESH] to update the screen display.
8 Press the soft key [DETAIL OFF] to display the host file list (file
names only) screen. Press the soft key [DETAIL ON] to display
the host file list (detail) screen.
9 When selecting a folder with cursor and pressing the MDI key
, the selected folder is changed to the new current folder.
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1332 -
Host file list display (for 15-inch display unit)
A list of the files held on the host computer is displayed.
Procedure
1 Press the function key .
2 Press the vertical soft key [FOLDER]. The program list screen
appears.
3 Press the continuous menu key until horizontal soft key
[DEVICE CHANGE] appears.
Press the horizontal soft key [DEVICE CHANGE].
4 Press the horizontal soft key [EMB ETHER], and the
EMBEDDED ETHERNET HOST FILE LIST screen appears.
Fig. 8.4.1 (b) Embedded Ethernet host file list screen
NOTE
1 When using the FTP file transfer function, check
that the valid device is the embedded Ethernet port.
The two conditions below determine a connection
destination on the host file list screen:
(1) Check that the valid device is the embedded
Ethernet port. Make a selection in "DEVICE
SELECTION" on the Ethernet setting screen.
(2) A host computer can be selected from
connection destinations 1, 2, and 3. Make a
selection according to soft key [HOST
CHANGE] described later.
2 File names including kanji, hiragana, and katakana
characters cannot be displayed correctly.
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1333 -
5 When a list of files is larger than one page, the screen display can
be switched using the page keys .
6 Press the horizontal soft key [REFRESH] to update the screen
display.
7 Press the horizontal soft key [DETAIL OFF] to display the host
file list (file names only) screen. Press the horizontal soft key
[DETAIL ON] to display the host file list (detail) screen.
8 When selecting a folder with cursor and pressing the MDI key
, the selected folder is changed to the new current folder.
Display item (common to 7.2/8.4/10.4/15-inch display units)
AVAILABLE DEVICE
"EMBEDDED" or "PCMCIA" is displayed.
CONNECT HOST
The currently selected connection host number and host name are
displayed.
REGISTERED PROGRAM
The number of files registered in the work folder of the connected host
is displayed. Up to 8 digits can be displayed.
CURRENT FOLDER
The current folder name of the connected host is displayed.
If the folder-path is long compared with the display-item, characters:
“…” and only the first and last ten letters of the folder name are
displayed.
FILE LIST
There is no distinction between file names and folder names.
Although the maximum number of displayed characters is 127,
characters are displayed as far as they can be displayed in one line.
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1334 -
Operation list (common to 7.2/8.4/10.4/15-inch display units)
DETAIL ON, DETAIL OFF
The screen display can be switched between the display of file names
only and the display of details.
REFRESH
Display data can be updated.
READ
A file can be input from the host computer to the part program storage
memory of the CNC. This item is displayed only when 9 is set as the
I/O device number of the CNC.
PUNCH
A file can be output from the part program storage memory of the
CNC to the host computer. This item is displayed only when 9 is set
as the I/O device number of the CNC.
DELETE
A folder or file can be deleted from the host computer.
RENAME
A file or folder on the host computer can be renamed.
DELETE FOLDER
A folder can be deleted from the host computer.
CREATE FOLDER
A folder can be created on the host computer.
HOST CHANGE
The connected host can be changed.
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1335 -
NC program input (for 7.2/8.4/10.4-inch display unit)
A file (NC program) stored on the host computer can be input into the
part program storage memory of the CNC.
Procedure
1 Display the EMBEDDED ETHERNET HOST FILE LIST
screen.
2 Press the EDIT switch on the machine operator’s panel.
3 Press the soft key [(OPRT)].
4 Press the continuous menu key until soft key [READ]
appears.
Press the soft key [READ].
5 Position the cursor on the file to input, and press [F GET] or type
the file name to input.
Press the soft key [F SET].
If the input file name is omitted, default input file name
“ALL-PROG.TXT” is assumed.
6 Type the program name, and press the soft key [P SET].
For an explanation of the operations to be performed if an input
file name [F SET] and an input program name [P SET] are
omitted, see the table below.
7 Press the soft key [EXEC].
This starts reading the program, and “INPUT” blinks in the lower
right part of the screen. When the read operation ends, the
“INPUT” indication disappears.
To cancel the input of the program, press the soft key [CAN].
[F SET] [P SET] Input file name Input program Input program name
BLANK BLANK ALL-PROG.TXT All programs in ALL-PROG.TXT File name at the time the file is saved
BLANK INPUT ALL-PROG.TXT First program in ALL-PROG.TXT Program name set with [P SET]
INPUT BLANK
File name set
with [F SET]
All programs in the file specified
with [F SET] File name at the time the file is saved
INPUT INPUT
File name set
with [F SET]
First program in the file specified
with [F SET] Program name set with [P SET]
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1336 -
NC program input (for 15-inch display unit)
A file (NC program) stored on the host computer can be input into the
part program storage memory of the CNC.
Procedure
1 Display the EMBEDDED ETHERNET HOST FILE LIST
screen.
2 Press the EDIT switch on the machine operator’s panel.
3 Press the continuous menu key until horizontal soft key
[READ] appears.
Press the horizontal soft key [READ].
4 Position the cursor on the file to input, and press [F GET] or type
the file name to input.
Press the horizontal soft key [F SET].
If the input file name is omitted, default input file name
“ALL-PROG.TXT” is assumed.
5 Type the program name, and press the horizontal soft key [P
SET].
For an explanation of the operations to be performed if an input
file name [F SET] and an input program name [P SET] are
omitted, see the table below.
6 Press the horizontal soft key [EXEC].
This starts reading the program, and “INPUT” blinks in the lower
right part of the screen. When the read operation ends, the
“INPUT” indication disappears.
To cancel the input of the program, press the horizontal soft key
[CAN].
[F SET] [P SET] Input file name Input program Input program name
BLANK BLANK ALL-PROG.TXT All programs in ALL-PROG.TXT File name at the time the file is saved
BLANK INPUT ALL-PROG.TXT First program in ALL-PROG.TXT Program name set with [P SET]
INPUT BLANK
File name set
with [F SET]
All programs in the file specified
with [F SET] File name at the time the file is saved
INPUT INPUT
File name set
with [F SET]
First program in the file specified
with [F SET] Program name set with [P SET]
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1337 -
NC program output (for 7.2/8.4/10.4-inch display unit)
A file (NC program) stored in the part program storage memory of the
CNC can be output to the host computer.
Procedure
1 Display the EMBEDDED ETHERNET HOST FILE LIST
screen.
2 Press the EDIT switch on the machine operator’s panel.
3 Press the soft key [(OPRT)].
4 Press the continuous menu key until soft key [PUNCH]
appears.
Press the soft key [PUNCH].
5 Type the program name to output, and press the soft key [P SET].
To specify an output file name, type the output file name and
press the soft key [F SET].
If, in this step, no output file name or no program name is
specified, all programs in the foreground folders are output to
“ALL-PROG.TXT”.
For an explanation of the operations to be performed if an output
file name [F SET] and an output program name [P SET] are
omitted, see the table below.
(For an explanation of foreground folders, see II-12.1.3, and for
how to change foreground folders, see III-11.6)
6 Press the soft key [EXEC].
This starts outputting the program, and “OUTPUT” blinks in the
lower right part of the screen. When the read operation ends, the
“OUTPUT” indication disappears.
To cancel the output of the program, press the soft key [CAN].
[F SET] [P SET] Output file name Output program
BLANK BLANK or (O-9999) ALL-PROG.TXT All programs in the foreground folders
displayed in the program folder
BLANK INPUT Program name set with [P SET] Program in the NC that is set with [P SET]
INPUT BLANK or (O-9999) File name set with [F SET] All programs in the foreground folders
displayed in the program folder
INPUT INPUT File name set with [F SET] Program in the NC that is set with [P SET]
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1338 -
NC program output (for 15-inch display unit)
A file (NC program) stored in the part program storage memory of the
CNC can be output to the host computer.
Procedure
1 Display the EMBEDDED ETHERNET HOST FILE LIST
screen.
2 Press the EDIT switch on the machine operator’s panel.
3 Press the continuous menu key until horizontal soft key
[PUNCH] appears.
Press the horizontal soft key [PUNCH].
4 Type the program name to output, and press the horizontal soft
key [P SET]. To specify an output file name, type the output file
name and press the horizontal soft key [F SET].
If, in this step, no output file name or no program name is
specified, all programs in the foreground folders are output to
“ALL-PROG.TXT”.
For an explanation of the operations to be performed if an output
file name [F SET] and an output program name [P SET] are
omitted, see the table below.
(For an explanation of foreground folders, see II-12.1.3, and for
how to change foreground folders, see III-11.6)
5 Press the horizontal soft key [EXEC].
This starts outputting the program, and “OUTPUT” blinks in the
lower right part of the screen. When the read operation ends, the
“OUTPUT” indication disappears.
To cancel the output, press the horizontal soft key [CAN].
[F SET] [P SET] Output file name Output program
BLANK BLANK or (O-9999) ALL-PROG.TXT All programs in the foreground folders
displayed in the program folder
BLANK INPUT Program name set with [P SET] Program in the NC that is set with [P SET]
INPUT BLANK or (O-9999) File name set with [F SET] All programs in the foreground folders
displayed in the program folder
INPUT INPUT File name set with [F SET] Program in the NC that is set with [P SET]
B-63944EN/03 OPERATION 8.DATA INPUT/OUTPUT
- 1339 -
8.5 SCREEN HARD COPY FUNCTION
Overview
This function converts screen information displayed on the CNC into
bit map format data and output it to a memory card. Once output, bit
map format data can be displayed and edited on a personal computer.
Explanation
- Start/cancellation methods
The screen hard copy function is started by pressing and holding down
key for five seconds. The function can be canceled by pressing
key .
- Acquisition and output of screen data
When started, the screen hard copy function starts acquiring screen
data. As soon as it has acquired it, the function outputs bit map format
data to the memory card inserted into the LCD unit. While screen data
is being acquired, the screen remains stationary for a few seconds.
Acquired screen data can be output from the memory card screen.
Also, while screen data is being output, "OUTPUT" blinks in the
status display.
- Screen data file names
Bit map format screen data files created by this function are assigned
the names below, starting with the one created after the power is
turned on.
"HDCPY000.BMP" (name of the first file output to the memory card
after the power is turned on)
"HDCPY001.BMP" (name of the second file output to the memory card
after the power is turned on)
:
:
"HDCPY999.BMP" (name of the 1000th file output to the memory
card after the power is turned on)
If, after a file with "HDCPY999.BMP" is output, the screen hard copy
function is executed, the file name returns to "HDCPY000.BMP". If,
however, a file with the same file name as the one to be output when
the screen hard copy function is executed exists on the memory card,
alarm SR1973 is issued. If the capacity of the memory card is
exceeded, alarm SR1962 is issued.
In either case, screen data is not output, so that either the existing file
needs to be deleted or the memory card needs to be replaced with a
new one.
8.DATA INPUT/OUTPUT OPERATION B-63944EN/03
- 1340 -
Limitation
- Screens whose hard copies cannot be made
Hard copies of the BOOT screen, the IPL screen, and the system alarm
screen cannot be made.
- Foreground I/O devices
During DNC operation, for example, screen data cannot be output
while a foreground I/O device is in use.
- Canceling the hard copy function
If the hard copy function is canceled before a hard copy is completed,
an incomplete bit map file of data that has been output is created.
B-63944EN/03 OPERATION 9.CREATING PROGRAMS
- 1341 -
9 CREATING PROGRAMS
This chapter explains how to create programs by MDI of the CNC.
This chapter also explains automatic insertion of sequence numbers
and how to create programs in TEACH IN mode.
Creation/registration
Program creation
Editing
Management
Execution Output
Creating programs using MDI panel ..................... See III-9.1
A
utomatic insertion of sequence numbers ............ See III-9.2
Creating programs in TEACH IN mode................. See III-9.3
Program
registration
Registration from external input......................... See III-8.1.1
9.CREATING PROGRAMS OPERATION B-63944EN/03
- 1342 -
9.1 CREATING PROGRAMS USING THE MDI PANEL
Programs can be created in the EDIT mode using the program editing
functions described in III-10.
Procedure for Creating Programs Using the MDI Panel
1 Enter the EDIT mode.
2 Press the key.
3 Press address key and enter the program number.
4 Press the key.
5 Create a program using the program editing functions described
in III-10.
Explanation
- Comments in a program
Comments can be written in a program using the control in/out codes.
Example) O0001 (TEST PROGRAM) ;
M08 (COOLANT ON) ;
• When the key is pressed after the control-out code "(",
comments, and control-in code ")" have been typed, the typed
comments are registered.
• When the key is pressed midway through comments, to
enter the rest of comments later, the data typed before the
key is pressed may not be correctly registered (not entered,
modified, or lost) because the data is subject to an entry check
which is performed in normal editing.
• Control-out code "(" or Control-in code ")" cannot be registered
by itself.
B-63944EN/03 OPERATION 9.CREATING PROGRAMS
- 1343 -
9.2 AUTOMATIC INSERTION OF SEQUENCE NUMBERS
Sequence numbers can be automatically inserted in each block when a
program is created using the MDI keys in the EDIT mode.
Set the increment for sequence numbers in parameter No. 3216.
Procedure for automatic insertion of sequence numbers
Procedure
1 Enter 1 in response to the prompt for "SEQUENCE NO." in
setting data. (see III-12.3.1).
2 Enter the EDIT mode.
3 Press key to display the program screen.
4 Search for or register the number of a program to be edited and
move the cursor to the EOB (;) of the block after which
automatic insertion of sequence numbers is started.
When a program number is registered and an EOB (;) is entered
with the key, sequence numbers are automatically
inserted starting with 0. Change the initial value, if required,
according to step 10, then skip to step 7.
5 Press address key and enter the initial value of N.
6 Press key.
7 Enter each word of a block.
8 Press
key.
9.CREATING PROGRAMS OPERATION B-63944EN/03
- 1344 -
9 Press key. The EOB is registered in memory and
sequence numbers are automatically inserted. For example, if
the initial value of N is 10 and the parameter for the increment is
set to 2, N12 inserted and displayed below the line where a new
block is specified.
10 In the example above, if N12 is not necessary in the next block,
pressing the key after N12 is displayed deletes N12.
If wishing to insert N100, not N12, into the next block, type
N100 immediately after N12 is displayed, and press .
This causes N100 to be registered and the initial value to be
changed to 100.
B-63944EN/03 OPERATION 9.CREATING PROGRAMS
- 1345 -
9.3 CREATING PROGRAMS IN TEACH IN MODE
(PLAYBACK)
In the TEACH IN JOG or TEACH IN HANDLE mode, you can create
a program while inserting the coordinate of the current position along
each axis in the absolute coordinate system when the tool is moved by
manual operation into the program.
You can input the words other than axis names in the same way as in
the EDIT mode.
Program screen in the TEACH IN JOG mode
Displayed items
In the TEACH IN JOG or TEACH IN HANDLE MODE, the
following program screen is displayed.
On the left of the screen, the coordinates of the current position in the
absolute and relative coordinate systems are displayed; on the right of
the screen, the contents of a program are displayed. You can create a
program while checking the current position by manual operation.
Fig. 9.3 (a) Program screen in the TEACH IN JOG mode
9.CREATING PROGRAMS OPERATION B-63944EN/03
- 1346 -
Inputting the coordinates of the current position
You can use the following procedure to insert the coordinate of the
current position along each axis in the absolute coordinate system:
1 Select the TEACH IN JOG mode or TEACH IN HANDLE
mode.
2 Press key to display the program screen. Search for or
register the number of a program to be edited and move the
cursor to the position where the current position along each axis
is to be inserted.
3 Move the tool to the desired position with jog or handle.
4 Key in the axis name of an axis along which you want to insert
the coordinate of the current position.
5 Press the key. Then, the coordinate of the current
position along the specified axis is inserted in the program.
(Example) X10.521 Coordinate of the current position
X10521 Data inserted in the program
Example
O1234 ;
G92 X10000 Y0 Z10000 ;
G00 G90 X3025 Y23723 ;
G01 Z-325 F300 ;
M02 ;
X
Z
Y
P0
(
10.0
,
0
,
10.0
)
P1
P2
(3.025, 23.723, 10.0)
(3.025, 23.723, -0.325)
1 Select the TEACH IN HANDLE mode.
2 Make positioning at position P0 by the manual pulse generator.
3 Select the program screen.
4 Enter program number O1234 as follows:
This operation input program number O1234 in memory.
Next, press the following keys:
An EOB (;) is entered after program number O1234.
5 Enter the P0 machine position for data of the first block as
follows:
G 9 2 X Y
Z
This operation registers G92X10000Y0Z10000; in program.
6 Position the tool at P1 with the manual pulse generator.
O1234
B-63944EN/03 OPERATION 9.CREATING PROGRAMS
- 1347 -
7 Enter the P1 machine position for data of the second block as
follows:
G00G 9 0
XY
This operation input G00G90X3025Z23723; in program.
8 Position the tool at P2 with the manual pulse generator.
9 Enter the P2 machine position for data of the third block as
follows:
G01Z F 3 0 0
This operation input G01Z -325F300; in program.
10 Input M02; in program as follows:
M 0 2
This completes the registration of the sample program.
Explanation
- Registering a position with compensation
When an axis name and a numeric value are keyed in and the
key is pressed, the value keyed in is added to the absolute coordinate
of the current position and the coordinate is inserted. This operation
allows insertion of a corrected value for the absolute coordinate
position.
When an extended axis name is used and the name ends with a
numeric value, insert an equal sign (=) between the axis name and
numeric value.
- Registering commands other than position commands
Commands to be entered before and after a position command must be
entered before and after the machine position is registered, by using
the same operation as program editing in EDIT mode.
- Calculator-type input
When the calculator-type input format is disabled (bit 0 (DPI) of
parameter No. 3401 is set to 0), the coordinate of the current position
is inserted into the program in least input increments. When the
calculator-type input format is enabled (the bit is set to 1), the
coordinate is inserted with a decimal point.
(Example)
Coordinate of the current position X10.521
At this time, the X-axis coordinate is inserted into the program as
follows:
When the calculator-type input format is disabled X10521
When the calculator-type input format is enabled X10.521
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1348 -
10 EDITING PROGRAMS
This chapter describes how to edit programs registered in the CNC.
Editing includes the insertion, modification, and deletion of words.
Editing also includes deletion of the entire program and automatic
insertion of sequence numbers. In addition, PC-like program text copy
and move operations are possible. This chapter also describes program
search, sequence number search, word search, and address search,
which are performed before editing the program.
1) Program search .............................................................. See III-10.4.
2) Sequence number search ............................................... See III-10.5.
3) Word search................................................................. See III-10.2.1.
4) Address search ............................................................ See III-10.2.1.
1) Inserting, altering, and deleting a word...........See III-10.2.3 to 10.2.5.
2) Deleting blocks................................................................ See III-10.3.
3) Deleting programs.......................................................... See III-10.6.
4) Editing characters ........................................................... See III-10.9.
Search for part o
f
program to be
edited
Inserting, altering,
and deleting
programs
Management
ExecutionOutput
Creation and
registration
Editing
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1349 -
10.1 EDIT DISABLE ATTRIBUTE
Before a program can be edited, the edit disable attribute must be
removed.
The edit disable attribute can be set for each program and folder.
Programs with the edit disable attribute and programs in folders with
the edit disable attribute cannot be edited.
Procedure for removing the edit disable attribute
1 Select EDIT mode.
2 Press the function key .
3 Press the chapter selection soft key [FOLDER].
4 Press the soft key [DETAIL ON].
5 Move the cursor to the program or folder from which you want to
remove the edit disable attribute.
6 Press the soft key [CHANGE ATTR].
7 Press the soft key [EDIT ENABLE].
8 Press the soft key [END].
CAUTION
1 After completing editing, set the edit disable
attribute as necessary.
2 To set the edit disable attribute, follow the same
procedure as for removing the attribute.
In the step 7, press the soft key [EDIT DISABL].
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1350 -
10.2 INSERTING, ALTERING AND DELETING A WORD
This section outlines the procedure for inserting, altering, and deleting
a word in a program registered in memory.
Procedure for inserting, altering and deleting a word
1 Select EDIT mode.
2 Press the function key .
3 Select a program to be edited.
If a program to be edited is selected, perform the operation 4.
If a program to be edited is not selected, search for the program
number.
4 Move the cursor to the position to be edited, with one of the
methods below.
• Scan method
• Word search method
• Address search method
For each method, refer to III-10.2.1.
5 Perform an operation such as altering, inserting, or deleting a
word.
Explanation
- Concept of word and editing unit
A word is an address followed by a number. With a custom macro,
the concept of word is ambiguous.
So the editing unit is considered here.
The editing unit is a unit subject to alteration or deletion in one
operation. In one scan operation, the cursor indicates the start of an
editing unit.
An insertion is made after an editing unit.
Definition of editing unit
• Program portion from an address to immediately before the next
address
• An address is an alphabet, IF, WHILE, GOTO, END, DO=, or ;
(EOB).
According to this definition, a word is an editing unit.
The word "word," when used in the description of editing, means an
editing unit according to the precise definition.
WARNING
When a change, insertion, or deletion was performed on data of
a program by pausing machining with the single block stop, feed
hold, or other operations during execution of a program, be sure
to return the cursor to the original position before restarting the
program. To execute the program with the cursor positioned at
another position, be sure to make a reset.
Otherwise, the program may not be executed as expected from
the program shown on the screen after machining restarts.
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1351 -
10.2.1 Word Search
A word can be searched for by merely moving the cursor through the
text (scanning), by word search, or by address search.
Procedure for scanning a program
1 Press the cursor key .
The cursor moves forward word by word; the cursor is displayed
at a selected word.
2 Press the cursor key .
The cursor moves backward word by word; the cursor is
displayed at a selected word.
Example: Scanning Z1250.0
3 Holding down the cursor key or scans words
continuously.
4 The first word of the next block is searched for when the cursor
key is pressed.
5 The first word of the previous block is searched for when the
cursor key is pressed.
6 Holding down the cursor key or moves the cursor
to the head of a block continuously.
7 Pressing the page key displays the next page and searches
for the first word of the page.
8 Pressing the page key displays the previous page and
searches for the first word of the page.
9 Holding down the page key or displays one page
after another.
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1352 -
Procedure for searching a word
Example of searching for S12
1 Press soft key [SEARCH].
2 Key in address S.
3 Key in
1 2 .
• S12 cannot be searched for if only S1 is keyed in.
• S09 cannot be searched for by keying in only S9.
To search for S09, be sure to key in S09.
4 Pressing soft key [↓ SEARCH] starts searching forward from the
cursor position. Pressing [↑ SEARCH] starts searching
backward.
5 To search for the same word successively, press [↓ SEARCH] or
[↑ SEARCH].
Procedure for searching an address
Example of searching for M03
1 Pressing the [SEARCH] key
2 Key in address M.
3 Pressing soft key [↓ SEARCH] starts searching forward from the
cursor position. Pressing [↑ SEARCH] starts searching
backward.
4 To search for the same word successively, press [↓ SEARCH] or
[↑ SEARCH].
N01234 is being searched
for/scanned currentl
y
.
S12 is searched for.
N01234 is being searched
for/scanned currentl
y
.
M03 is searched for.
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1353 -
10.2.2 Heading a Program
The cursor can be jumped to the top of a program. This function is
called heading the program pointer. This section describes the four
methods for heading the program pointer.
Procedure for heading a program
Method 1 1 Press key when the program screen is selected in EDIT mode.
When the cursor has returned to the start of the program, the contents
of the program are displayed from its start on the screen.
Method 2 1 Search for the program number.
When the program screen is selected in MEMORY or EDIT mode,
enter a program number or program name.
When entering a program number, press address key O then type
the program number.
2 Press soft key [PROGRM SEARCH].
Method 3 1 Select the program screen or program check screen in MEMORY
mode.
2 Press soft key [(OPRT)].
3 Press soft key [REWIND].
Method 4 1 Select the program screen in EDIT mode.
2 Press soft key [(OPRT)].
3 Press soft key [LINE SEARCH].
4 Press soft key [TOP].
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1354 -
10.2.3 Inserting a Word
Procedure for inserting a word
1 Search for or scan the word immediately before a word to be
inserted.
2 Key in an address to be inserted.
3 Key in data.
4 Press the key.
Example of Inserting T15
1 Search for or scan Z1250.
2 Key in
T15.
3 Press the key.
Z1250.0 is searched
for/scanned.
T15 is inserted.
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1355 -
10.2.4 Altering a Word
Procedure for altering a word
1 Search for or scan a word to be altered.
2 Key in an address to be inserted.
3 Key in data.
4 Press the key.
Example of changing T15 to M15
1 Search for or scan T15.
2 Key in
M 15.
3 Press the key.
T15 is searched
for/scanned.
T15 is changed to M15.
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1356 -
10.2.5 Deleting a Word
Procedure for deleting a word
1 Search for or scan a word to be deleted.
2 Press the key.
Example of deleting X100.0
1 Search for or scan X100.0.
2 Press the key.
X100.0 is searched
for/scanned.
X100.0 is deleted.
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1357 -
10.3 DELETING BLOCKS
A block or blocks can be deleted in a program.
10.3.1 Deleting a Block
The portion from the current word position to the next EOB is deleted.
The cursor is then placed in the word next to the deleted EOB.
Procedure for deleting a block
1 Search for or scan address N for a block to be deleted.
2 Press the
key.
3 Press the editing key .
Example of deleting a block of N01234
1 Search for or scan N01234.
2 Press the
key.
3 Press the editing key .
N01234 is searched
for/scanned.
Block containing N01234
has been deleted.
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1358 -
10.3.2 Deleting Multiple Blocks
The several blocks in the forward direction from the current word
position up to the EOB of the farthest of those blocks are deleted.
The cursor is then placed in the word next to the deleted EOB.
Procedure for deleting blocks
1 Search for or scan a word in the first block of a portion to be
deleted.
2 Press the
key as many times as the number of blocks that
you want to delete.
3 Press the editing key .
Example of deleting blocks from N01234 to the EOB of a block which is two blocks
ahead
1 Search for or scan N01234.
2 Press
.
3 Press the editing key .
N01234 is searched
for/scanned.
Blocks from N01234
to the EOB of a block
which is two blocks
ahead are deleted.
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1359 -
10.4 PROGRAM SEARCH
When memory holds multiple programs, a program can be searched
for. There are four methods as follows.
Procedure for program search
Method 1 1 Select EDIT or MEMORY mode.
2 Press function key to display the program screen.
3 Enter a program number or program name. When entering a
program number, press address key then type the program
number.
4 Press soft key [PROGRM SEARCH]. Alternatively, press the cursor
key or .
5 Upon completion of search operation, the program number searched
for is displayed in the upper-right corner of the screen
If the program is not found , alarm PS0071 occurs.
Method 2 1 Select EDIT or MEMORY mode.
2 Press function key to display the program screen.
3 Press soft key [PROGRM SEARCH].
4 Then, press soft key [PREV PROGRM] or [NEXT PROGRM].
Pressing [PREV PROGRM] searches for the previous program on the
folder, and pressing [NEXT PROGRM] searches for the next program.
Method 3 This method searches for the program number (0001 to 0031)
corresponding to a signal on the machine tool side to start automatic
operation. Refer to the relevant manual prepared by the machine tool
builder for detailed information on operation.
1 Select MEMORY mode.
2 Set the reset state.
• The reset state is the state where the LED for indicating that
automatic operation is in progress is off. (Refer to the relevant
manual of the machine tool builder.)
3 Set the program number selection signal on the machine tool side to a
number from 01 to 31.
4 Press the cycle start button.
• When the signal on the machine tool side represents 00, program
number search operation is not performed.
• If the program corresponding to a signal on the machine tool side
is not registered, alarm DS0059 is raised.
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1360 -
Method 4 When bit 4 (PGS) of parameter No. 11308 is 1, search for an O number
program by specifying digits only.
1 Select EDIT or MEMORY mode.
2 Press function key to display the program screen.
3 Enter the digits of a program number. Address key
need not be
pressed before the digits.
4 Press soft key [PROGRM SEARCH]. Alternatively, press the cursor
key or .
Example
• When bit 4 (PGS) of parameter No. 11308 is 1
Specify "1000" → Search for program O1000.
Specify "ABC" → Search for program ABC.
• When bit 4 (PGS) of parameter No. 11308 is 0
Specify "1000" → Search for program 1000.
Specify "ABC" → Search for program ABC.
When bit 4 (PGS) of parameter No. 11308 is 1, it is not possible to
search for a program with any name consisting of digits only.
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1361 -
10.5 SEQUENCE NUMBER SEARCH
Sequence number search operation is usually used to search for a
sequence number in the middle of a program so that execution can be
started or restarted at the block of the sequence number.
Example)
Sequence number 02346 in a program (O0002) is searched for.
PROGRAM
O0001 ;
N01234 X100.0 Z100.0 ;
S12 ;
:
O0002 ;
N02345 X20.0 Z20.0 ;
N02346 X10.0 Z10.0 ;
:
O0003 ;
:
Selected pro
g
ram
Target sequence
number is found.
This section is searched
starting at the beginning.
(Search operation is
performed only within a
program.)
Procedure for sequence number search
Procedure
1 Select MEMORY mode.
2 Press function key .
3 If the program contains a sequence number to be searched for,
perform the operations 4 to 7 below.
If the program does not contain a sequence number to be
searched for, select the program number of the program that
contains the sequence number to be searched for.
4 Press address key .
5 Key in a sequence number to be searched for.
6 Press soft key [N SRH].
7 Upon completion of search operation, the sequence number
searched for is displayed in the upper-right corner of the screen.
If the specified sequence number is not found in the program
currently selected, alarm PS0060 occurs.
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1362 -
Explanation
- Operation during Search
Those blocks that are skipped do not affect the CNC. This means that
the data in the skipped blocks such as coordinates and M, S, and T
codes does not alter the CNC coordinates and modal values.
So, in the first block where execution is to be started or restarted by
using a sequence number search command, be sure to enter required
M, S, and T codes and coordinates. A block searched for by sequence
number search usually represents a point of shifting from one process
to another. When a block in the middle of a process must be searched
for to restart execution at the block, specify M, S, and T codes, G
codes, coordinates, and so forth as required from the MDI after closely
checking the machine tool and NC states at that point.
- Checking during search
During search operation, the following checks are made:
• Optional block skip
Limitation
- Searching in sub-program
During sequence number search operation, M98Pxxxx (subprogram
call) is not executed. So an alarm PS0060 is raised if an attempt is
made to search for a sequence number in a subprogram called by the
program currently selected.
O1234
:
:
M98 P5678 ;
:
:
Main program Subprogram
O5678
:
N88888
:
M99 ;
:
If an attempt is made to search for N8888 in the example above, an alarm occurs.
Fig. 10.5 (a)
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1363 -
10.6 DELETING PROGRAMS
Programs registered in memory can be deleted, either one program by
one program or all at once.
10.6.1 Deleting One Program
A single program in the folder containing the program currently being
edited can be deleted.
Procedure for deleting one program
1 Select the EDIT mode.
2 Press function key to display the program screen.
3 Press address key .
4 Key in a desired program number.
5 Press the editing key . The program with the entered
program number is deleted.
10.6.2 Deleting All Programs
All programs in the folder containing the program currently being
edited can be deleted.
Procedure for deleting all programs
1 Select the EDIT mode.
2 Press function key to display the program screen.
3 Press address key .
4 Key in -9999.
5 Press editing key to delete all programs.
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1364 -
10.7 EDITING OF CUSTOM MACROS
Unlike ordinary programs, custom macro programs are modified,
inserted, or deleted based on editing units.
Custom macro words can be entered in abbreviated form.
Comments can be entered in a program.
Refer to the III-9.1 for the comments of a program.
Explanation
- Editing unit
When editing a custom macro already entered, the user can move the
cursor to each editing unit that starts with any of the following
characters and symbols:
(a) Address
(b) # located at the start of the left side of a substitution statement
(c) /, (,=, and ;
(d) First character of IF, WHILE, GOTO, END, DO, POPEN,
BPRNT, DPRNT and PCLOS
On the screen, a blank is placed before each of the above characters
and symbols.
Example) Head positions where the cursor is placed
N001 X-#100 ;
#1 =123 ;
N002 /2 X[12/#3] ;
N003 X-SQRT[#3/3*[#4+1]] ;
N004 X-#2 Z#1 ;
N005 #5 =1+2-#10 ;
IF[#1NE0] GOTO10 ;
WHILE[#2LE5] DO1 ;
#[200+#2] =#2*10 ;
#2 =#2+1 ;
END1 ;
- Abbreviations of custom macro word
When a custom macro word is altered or inserted, the first two
characters or more can replace the entire word.
Namely,
WHILE → WH GOTO → GO XOR → XO AND → AN
SIN → SI ASIN → AS COS → CO ACOS → AC
TAN → TA ATAN → AT SQRT → SQ ABS → AB
BCD → BC BIN → BI FIX → FI FUP → FU
ROUND → RO END → EN POPEN → PO BPRNT → BP
DPRNT → DP PCLOS → PC EXP → EX THEN → TH
Example) Keying in
WH [AB [#2 ] LE RO [#3 ] ] has the same effect as
WHILE [ABS [#2 ] LE ROUND [#3 ] ]
The program is also displayed in this way.
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1365 -
10.8 CURSOR MOVEMENT LIMITATIONS ON PROGRAM
EDITING
If a program is to be edited while it is stopped or halted, limitations
are imposed so that already executed blocks and buffered blocks
cannot be edited. Modifiable blocks are those at and below the cursor
position at the time the system switches to the edit mode (EDIT). In
the remainder of this manual, the area of editable blocks is called the
edit-enabled area, while the area of executed blocks and buffered
blocks is called the edit-disabled area.
These limitations are applied when the automatic operation status
signal <F0000.7> is ON and when a single block execution of MDI
operation is edited, and are also applied to TEACH IN HNDL or
TEACH IN JOG mode when the playback option is enabled.
This function is enabled when bit 3 (FPD) of parameter No. 11308 is
1.
Explanation
- States where cursor movement limitations are imposed
• EDIT mode while automatic operation is stopped or halted
• MDI mode and when a single block is set
• TEACH IN HNDL or TEACH IN JOG mode (only when the
playback function is enabled)
- Cursor movement
Operations that cause the cursor to move to blocks above the edit
mode start position are ignored.
• ↑
• ←
• PAGE UP
• CAN (character editing)
- Search and replacement
Operations that cause the cursor to move to the edit-disabled area are
disabled.
• Top line search: Results in a search of the top line of the
edit-enabled block.
• Specified-line search (character editing): Made through the
edit-enabled area.
If, however, an attempt is made to search through the
edit-disabled area, warning "PROGRAM IN OPERATION" is
issued, and the operation is disabled.
• Upward search: Made through the edit-enabled area.
If attempted at the beginning of the edit-enabled block, this
operation is ignored.
• Upward search (replacement): Made through the edit-enabled
area.
If attempted at the beginning of the edit-enabled block, this
operation is ignored.
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1366 -
• Upward candidate search: Made through the edit-enabled area.
If attempted at the beginning of the edit-enabled block, this
operation is ignored.
• Character string + ↑ (search): Typing the character string to
search for and pressing the ↑ key searches for the character string.
This search is made through the edit-enabled area. If attempted at
the beginning of the edit-enabled block, this operation is ignored.
• Replace all: This operation is disabled.
- Reset
The program execution status is canceled, and the cursor movement
limitations are also canceled.
- Program search
If an attempt is made to search for the program currently used for
operation, warning "PROGRAM IN OPERATION" is issued, and the
operation is disabled.
- Time insertion
When the machining time stamp function is enabled, soft key
[INSERT TIME] does not appear in the state in which the cursor
movement limitations are imposed.
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1367 -
10.9 PASSWORD FUNCTION
The password function locks bit 4 (NE9) of parameter No. 3202,
which protects programs with program Nos. O9000 to O9999 and
programs and folders having the edit/display disable attribute,
according to the settings in two parameters, PASSWORD (parameter
No. 3210) and KEYWD (parameter No. 3211). In the locked state,
parameter NE9 cannot be set to 0. In this case, the protection of
programs with program Nos. O9000 to O9999 and programs and
folders having the edit/display disable attribute cannot be released
unless a correct keyword is set.
A locked state means that the value set in the parameter PASSWD
differs from the value set in the parameter KEYWD. The values set in
these parameters are not displayed. The locked state is released when
the value already set in the parameter PASSWD is also set in
parameter KEYWD. When 0 is displayed in parameter PASSWD,
parameter PASSWD is not set.
Procedure for locking and unlocking
Locking
1 Set the MDI mode.
2 Enable parameter writing (III-12.3.1). At this time, alarm PS0100
is issued on the CNC.
3 Set parameter No. 3210 (PASSWD). At this time, the locked
state is set.
4 Disable parameter writing.
5 Press the key to release the alarm state.
Unlocking
1 Set the MDI mode.
2 Enable parameter writing (III-12.3.1). At this time, alarm
SW0100 is issued on the CNC.
3 In parameter No. 3211 (KEYWD), set the same value as set in
parameter No. 3210 (PASSWD) for locking. At this time, the
locked state is released.
4 Set bit 4 (NE9) of parameter No.3202 to 0.
5 Disable parameter writing.
6 Press the key to release the alarm state.
7 Subprograms from program Nos. 9000 to 9999 can now be
edited.
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1368 -
Explanation
- Setting parameter PASSWD
The locked state is set when a value is set in the parameter PASSWD.
However, note that parameter PASSWD can be set only when the
locked state is not set (when PASSWD = 0, or PASSWD = KEYWD).
If an attempt is made to set parameter PASSWD in other cases, a
warning is given to indicate that writing is disabled. When the locked
state is set (when PASSWD ≠ 0 and PASSWD ≠ KEYWD), parameter
NE9 is automatically set to 1. If an attempt is made to set NE9 to 0, a
warning is given to indicate that writing is disabled.
- Changing parameter PASSWD
Parameter PASSWD can be changed when the locked state is released
(when PASSWD = 0, or PASSWD = KEYWD). After step 3 in the
procedure for unlocking, a new value can be set in the parameter
PASSWD. From that time on, this new value must be set in parameter
KEYWD to release the locked state.
- Setting 0 in parameter PASSWD
When 0 is set in the parameter PASSWD, the number 0 is displayed,
and the password function is disabled. In other words, the password
function can be disabled by either not setting parameter PASSWD at
all, or by setting 0 in parameter PASSWD after step 3 of the procedure
for unlocking. To ensure that the locked state is not entered, care
must be taken not to set a value other than 0 in parameter PASSWD.
- Re-locking
After the locked state has been released, it can be set again by setting a
different value in parameter PASSWD, or by turning the power to the
NC off then on again to reset parameter KEYWD.
CAUTION
1 Once the locked state is set, parameter NE9
cannot be set to 0 and parameter PASSWD cannot
be changed until the locked state is released or the
memory all-clear operation is performed. Special
care must be taken in setting parameter PASSWD.
2 The edit/display disable attribute cannot be set
unless parameter PASSWD is set.
3 In the locked state, programs with the edit/display
disable attribute are treated as follows:
• The presence of the programs is hidden. This
means that these programs are not displayed on
screens such as the program folder screen.
These programs cannot be edited either.
• These programs cannot be selected as a main
program. They can be called as subprograms.
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1369 -
CAUTION
4 In the unlocked state, programs with the
edit/display disable attribute are treated in the
same manner as ordinary programs.
5 The programs in a folder having the edit/display
disable attribute are also treated as described in
Caution 3 and 4 above.
6 In the locked state, the folders in a folder having
the edit/display disable attribute are treated as
follows:
• The presence of the folders is hidden. This
means that these folders are not displayed on
screens such as the program folder screen.
7 In the unlocked state, the folders in a folder having
the edit/display disable attribute are treated in the
same manner as ordinary folders.
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1370 -
10.10 EDITING PROGRAM CHARACTERS
This section describes how to edit programs registered in the CNC.
Editing operations include character insertion, modification, deletion,
and replacement.
While program word editing is performed by recognizing program
words, program character editing is performed on a
character-by-character basis.
Fig. 10.10 (a) Character editing
Explanation
- Edit unit
Character editing is performed on a character-by-character basis.
Select between character editing and word editing according to what
to edit.
- Line
A range delimited by an EOB is specified as a line.
In character editing, edited data is saved on a line-by-line basis.
When one program line contains many characters, it extends over
multiple lines on the screen, but these lines are counted as one
program line.
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1371 -
- Line splitting
When the cursor is on a line during line editing, pressing edit key
causes the line to be split into two, one before the cursor and
the other after the cursor.
Pressing edit key immediately after the line is split causes the
lines to return to a single one.
Alternatively, moving the cursor to the EOB of the first line resulting
from the split and pressing edit key causes the lines to return to
a single one.
- Line merging
If the EOB of a line is deleted, the line is combined with the next line
to form a single line.
- Maximum number of characters in one line
One line can consist of up to 140 characters.
- Line number
The number of lines are counted starting with the starting line of a
program, which is counted as the first line. Even when a line wraps
around to the next and subsequent lines, these lines are counted as a
single line.
- Clipboard
The clipboard is an area to store characters when a cut or copy
operation is performed. The area has a capacity for holding
approximately 4000 characters.
The characters that are cut or copied by one cut or copy operation are
stored. The most recently stored character string can be used by the
paste function.
The information stored by the paste operation is kept unchanged until
another cut or copy operation is performed.
The characters stored in the clipboard are maintained until the power
to the CNC is turned off unless the clipboard is updated again.
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1372 -
- Undo function
The function for undoing operations performed in program editing
undoes operations sequentially, starting with the one performed last. It
can undo only those operations that update character strings.
A single undo operation undoes a single input or deletion operation.
If data updated with replace operations is to be undone, a single undo
operation undoes the replacement of a single item.
Operations of the cursor keys and the page
keys cannot be undone with this function because they do
not update character strings.
- Example of the undo function
1 Suppose that the following character string is present before
modifications:
N110AX[#AXIS3]=100.0;
2 Edit key is pressed five times.
X[#AXIS3]=100.0;
3 Soft key [UNDO] is pressed five times. Then, the original
character string is restored as follows:
AX[#AXIS3]=100.0;
0AX[#AXIS3]=100.0;
10AX[#AXIS3]=100.0;
110AX[#AXIS3]=100.0;
N110AX[#AXIS3]=100.0;
- Input modes for editing
Input modes for program editing include insert mode and overwrite
mode.
To switch between the input modes, press soft key [INPUT MODE].
Initially, insert mode is set.
• Insert mode
In insert mode, an entered character is inserted between the
current cursor position and the preceding character position.
1234567890
When the cursor is placed at 6, and X is entered, the following
results:
12345X67890
• Overwrite mode
In overwrite mode, the character at the cursor position is replaced
by an entered character.
1234567890
When the cursor is placed at 6, and X is entered, the following
results:
12345X7890
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1373 -
- Restrictions on editing
O numbers and file names cannot be edited.
EOR (%) cannot be deleted.
- Line editing and automatic saving
When a line is edited, the line is displayed in the update color, blue
(which can be changed with color settings), to indicate that the line
has been edited. When the line is displayed in the update color, the
edit has not yet been saved.
When the cursor is moved to a line preceding or succeeding the edited
line, the edit is automatically saved, and the line display changes from
the update color to the normal color.
Alternatively, pressing soft key [SAVE] enables the edit to be saved.
- Function for automatically saving an edited line vs. function for undoing editing
operations (UNDO function)
When an edit operation is undone, the line is displayed in the update
color, and the edit is not saved any longer. If the cursor moves to
another line when the operation is undone, the edit is automatically
saved.
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1374 -
10.10.1 Available Keys
The available keys are as follows:
- Cursor keys
Cursor keys , , , and move the cursor.
- Editing key
Deletes the character at the cursor position.
- Editing key
Deletes the character immediately before the cursor position.
When the cursor is at the beginning of a line, the character at the end
of the previous line is deleted.
- Editing key
Causes a line change.
- Page change keys
Pages are changed using page key or
Page key moves to the next page.
When page key is pressed on the last page, the cursor moves to
the last character position of the last line (the % position).
Page key moves to the previous page.
When page key is pressed on the first page, the cursor moves
to the first character position of the first line.
- Character keys
Characters are entered using these keys.
10.10.2 Input Mode
Input modes include insert mode and overwrite mode.
Changing input mode
To switch between the input modes, use soft key [INPUT MODE].
Pressing soft key [INPUT MODE] causes insert mode and overwrite
mode to be selected alternately.
The current mode is indicated in the lower right part of the editing
screen.
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1375 -
10.10.3 Line Number Display
This function is used to display a program with line numbers.
Pressing soft key [LINE NUMBER] displays a program with line
numbers. Pressing soft key [LINE NUMBER] again causes the line
numbers to disappear.
10.10.4 Search
A program is searched for a character string.
Search
Procedure
1 Press soft key [SEARCH].
2 A search character string input area is displayed. Enter the
character string to search for. To cancel the search, press soft key
[CANCEL].
3 Upward search operation
Pressing soft key [UP] causes the program to be searched in the
upward direction (toward the top), starting at the current cursor
position.
When a search character string is found, the cursor moves to the
character string.
Pressing soft key [UP] again causes the program to be searched
for the next candidate.
4 Downward search operation
Pressing soft key [DOWN] causes the program to be searched in
the downward direction (toward the bottom), starting at the
current cursor position.
When a search character string is found, the cursor moves to the
character string.
Pressing soft key [DOWN] again causes the program to be
searched for the next candidate.
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1376 -
10.10.5 Replacement
A character string in a program is replaced with a specified character
string.
Replacement
Procedure
1 Press soft key [REPLCE].
2 Search and replacement character string input areas are displayed.
Enter a search character string (character string to be replaced)
and a replacement character string (character string to replace the
former character string).
To move between the search character string input area and the
replacement character string input area, use the cursor keys
and .
If a search character string is input, but no replacement character
string is input, the former character string will be deleted.
To cancel the replacement, press soft key [CANCEL].
3 Replacement operations
Replacement operations include an operation for searching for a
search character string and an operation for actually replacing it.
To perform an operation for searching for a search string, use
soft key [↑ SEARCH] or [↓ SEARCH].
To perform an operation for actually replacing it, use [REPLCE]
or [REPLCE ALL].
• Soft key [↑ SEARCH]
Searches the program in the upward direction (toward the
top), starting at the current cursor position.
When a search character string is found, the cursor moves to
the character string.
Pressing soft key [↑ SEARCH] again causes the program to
be searched for the next candidate.
• Soft key [↓ SEARCH]
Searches the program in the downward direction (toward the
bottom), starting at the current cursor position.
When a search character string is found, the cursor moves to
the character string.
Pressing soft key [↓ SEARCH] again causes the program to
be searched for the next candidate.
• Soft key [REPLCE]
Replaces the character string found with a search operation
with a replacement character string.
• Soft key [REPLCE ALL]
Replace all instances of the search character string in the
program text with the replacement character string.
Pressing this soft key causes message "ARE YOU SURE
YOU WANT TO EXECUTE?" to appear and also soft key
[YES] and soft key [NO] to appear. Pressing soft key [YES]
causes all replacements to be executed.
Pressing soft key [NO] cancels the replacement operation,
without executing the replacements.
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1377 -
10.10.6 Reversing Edit Operations (Undo Function)
Edit operations performed on a program can be undone sequentially
starting with the one performed last.
Reversing edit operations (undo function)
Procedure
1 Pressing soft key [UNDO] once undoes a single operation.
When there are no longer any operation to be undone, pressing
this soft key has no effect.
10.10.7 Copy
A selected character string can be copied to the clipboard.
Copying
Procedure
1 Move the cursor to the beginning of the character string to select.
2 Press soft key [SELECT].
3 Using the cursor keys and the page keys
, move the cursor to the end of the character string to
select.
At this time, the background of the selected character string is
displayed in the selection color (cursor color).
4 Press soft key [COPY] to copy the selected character string to the
clipboard.
To cancel the copying, press soft key [CANCEL].
10.10.8 Cut
A selected character string can be deleted.
When deleted, the character string is copied to the clipboard.
Cut
Procedure
1 Move the cursor to the beginning of the character string to select.
2 Press soft key [SELECT].
3 Using the cursor keys and the page keys
, move the cursor to the end of the character string to
select.
At this time, the background of the selected character string is
displayed in the selection color (cursor color).
4 Press soft key [CUT] to delete the selected character string.
To cancel the deletion, pres soft key [CANCEL].
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1378 -
10.10.9 Paste
The character string stored in the clipboard can be inserted at the
current cursor position.
After pasted, the character string remains stored in the clipboard, so
that the character string can be pasted as many times as necessary.
Paste
Procedure
1 Move the cursor to the position at which you want to paste a
character string.
2 Press the soft key [PASTE].
10.10.10 Saving
Moving the cursor to a line preceding or succeeding the edited line
causes the edit to be automatically saved, but it is possible to save the
edit by pressing soft key [SAVE], if necessary. For a program
consisting of only a single line, in particular, it is necessary to press
soft key [SAVE] to save the edit.
Saving
Procedure
1 Press the soft key [SAVE].
10.10.11 Creation
A new program can be created.
Creation
Procedure
1 Press soft key [NEW PROGRM].
2 A program name input area appears.
3 Enter the name of a program to be created.
4 Press the soft key [EXECUTE]. This creates a new program
and displays the editing screen.
To cancel the creation of a new program, press soft key
[CANCEL].
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1379 -
10.10.12 Line Search
The cursor can be moved to a specified line.
The cursor can be moved to a line with a specified line number, to the
first line of the program, and to the last line of the program.
Line search
Procedure
Movement to a line with a specified line number
1 Press soft key [LINE SEARCH].
2 A line number input area appears.
3 Enter a line number. The first line is regarded as having a line
number of 1.
4 Press soft key [LINE NUMBER], and the cursor moves to the
specified line.
Movement to the first line
1 Press soft key [LINE SEARCH].
2 Press soft key [TOP], and the cursor moves to the first line of the
program.
Movement to the last line
1 Press soft key [LINE SEARCH].
2 Press soft key [BOTTOM], and the cursor moves to the last line
of the program.
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1380 -
10.11 PROGRAM COPY FUNCTION
A program is copied or moved between folders.
Procedure for copying a program compact
Procedure
1 Press function key .
2 Press chapter selection soft key [FOLDER].
The following program folder screen appears:
3 Press the soft key [(OPRT)].
4 Move the cursor to a folder that contains the program that you
want to copy or move, and press soft key [CHANGE FOLDER].
5 Press the continuous menu key until soft key [SELECT
START] appears.
Press the soft key [SELECT START].
6 Move the cursor to the program that you want to select, and press
soft key [SELECT]. The background color of the selected
program becomes light blue, indicating the selected state.
7 Press the soft key [SELECT END]. The selected program is
determined.
8 Press soft key [CHANGE FOLDER], and move the cursor to the
folder to which you want to copy or move the program.
9 Press the soft key [COPY]. The selected program is copied. If
just one program is selected, pressing soft key [COPY] after
typing a program name performs a copy operation with the
entered name.
10 To move the program, press soft key [MOVE]. The selected
file is then moved. If just one program is selected, pressing soft
key [MOVE] after typing a program name performs a move
operation with the entered name.
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1381 -
Explanation
Operations are accepted only when the data protection key is set to
ON.
If the program storage capacity on the copy destination side is
insufficient, the copy operation is not accepted.
The currently selected program is highlighted. Multiple programs
can be selected in the same folder. Each time [SELECT] is pressed,
the program currently indicated by the cursor is selected.
A selected program can be deselected by pressing [SELECT] again or
by pressing [CANCEL].
If the same program name is already present in the copy or move
destination folder, "REWRITE: FILE NAME" is displayed, allowing
you to determine whether to overwrite the existing program by
pressing soft key [NO] or [REWRITE]. Pressing [REWRITE]
performs overwriting, and pressing [NO] does not perform the copy or
move operation of that program.
Pressing soft key [DELETE] deletes all the files currently selected.
A program can be neither copied nor moved to the same folder as the
selected folder.
When only one program is selected, and a program name is already
entered, however, the program can be copied or moved within the
same folder.
NOTE
Once a copy or move operation starts, it cannot be
canceled. So, start the operation very carefully.
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1382 -
10.11.1 Copying and Moving Files between Devices
Overview
Files can be copied and moved between different devices.
There are two procedures available on the program folder screen.
<1> File copying and moving (device change)
Select a source file first, and then select a destination folder by
first changing the device and then selecting a folder, decide on
the destination folder, and execute copy or move.
<2> File copying and moving with split display
On 10.4/15-inch LCDs, the program folder screen can be split.
By using this screen split function, it is possible to perform copy
or move operations while checking the file to be copied or
moved on the screen on which the folder containing the source
file and the destination folder are displayed at the same time.
File copying and moving (device change)
Procedure
1 Select EDIT mode.
2 Press function key to display the program folder screen.
3 Press soft key [(OPRT)].
4 Press the continuous menu key until [SELECT START]
appears. Press soft key [SELECT START].
5 Use the cursor keys as appropriate to position the cursor on the
desired file.
6 Press soft key [SELECT] to select the file.
7 After the desired file has been selected, press soft key [SELECT
END].
8 To select a destination device, press soft key [DEVICE
CNAHGE].
9 Select the desired device, using the soft key.
10 In the selected device, move to a destination folder.
11 To copy the selected file to the destination folder, press soft key
[COPY], and to move the file to the folder, press soft key
[MOVE].
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1383 -
File copying and moving with split display
Procedure１
- Procedure for selecting a file first and then a destination folder
1 Select EDIT mode.
2 Press function key to display the program folder screen.
3 Press soft key [(OPRT)].
4 Press the continuous menu key until [MULTI LIST]
appears. Press soft key [MULTI LIST].
5 In either of the folder displays, select the folder containing the
source file.
6 Press soft key [SELECT START].
7 Use the cursor keys as appropriate to position the cursor on the
desired file.
8 Press soft key [SELECT] to select the file.
9 Use the + cursor key combination, select the other folder
display.
10 To select a destination device, press soft key [DEVICE
CNAHGE].
11 Select the desired device, using the soft key.
12 In the selected device, move to a destination folder.
13 To copy the selected file to the destination folder, press soft key
[COPY], and to move the file to the folder, press soft key
[MOVE].
Procedure 2
- Procedure for selecting a destination folder first and then a file
1 Select EDIT mode.
2 Press function key to display the program folder screen.
3 Press soft key [(OPRT)].
4 Press the continuous menu key until [MULTI LIST]
appears. Press soft key [MULTI LIST].
5 In either of the folder displays, select the folder containing the
source file, use the + cursor key combination to switch to
the other folder display, and on this folder display, select a
destination folder.
6 Use the + cursor key combination to switch to the folder
display in which the source folder has been selected.
7 Press the continuous menu key until [SELECT START]
appears.
Press soft key [SELECT START].
8 Use the cursor keys as appropriate to position the cursor on the
desired file.
9 Press soft key [SELECT] to select the file.
10 After the file has been selected, press soft key [COPY] to copy
the selected file to the folder selected in the other folder display
and press soft key [MOVE] to move the file.
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1384 -
Explanation
- Multiple selectable files
Only multiple files that are in the same folder can be selected at the
same time with soft key [SELECT]. Files in other devices and folders
cannot be selected at the same time.
Up to ten files can be selected at the same time.
- Changing the file name during copying and movement
If only one file is selected for copying or moving, the file can be
copied or moved by changing its file name.
After selecting a file, enter a file name and press soft key [COPY] or
[MOVE]. This causes the file to be copied or moved with the entered
file name.
- Copying and moving a file to the same folder
It is not possible to copy and move a selected file to the folder that
contains the file.
If an attempt is made to do so, warning "SAMEFILE NOTCOPY" is
issued.
If, however, only one file is selected, and is to be copied or moved by
changing its file name, it can be copied or moved to the same folder.
- Overwriting files
When copying or moving is attempted, if a file with the same name
exists in the destination folder, message "REWRITE: File name"
flashes below the key-in buffer. If the file with the same name is to be
overwritten, press soft key [REWRITE] and otherwise, press soft key
[NO].
- File search when selecting a file
After soft key [SELECT START] is pressed, it is possible to search
for a file through a folder using soft key [SEARCH] when selecting
the file to copy or move.
Enter the file name to search for first and then press soft key
[SEARCH]. If a file with the entered file name exists, the cursor is
positioned on the file. If no file with the entered file name exists,
warning "SPECIFIED PROGRAM NOT FOUND" appears.
Soft key [SEARCH] simply moves the cursor to the program found on
the directory screen. It is not possible to switch operations, using bit 5
(PES) of parameter No. 11302.
- Display of a selected file name
When a file is selected with soft key [SELECT], the color of the
background of the file name display is changed. The color of the
background of the file name display remains unchanged until the file
is deselected.
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1385 -
- Deselecting a file
When a file is selected with soft key [SELECT], the selected file can
be deselected by positioning the cursor on the file and pressing soft
key [SELECT] again. All selected files are deselected when any of
the following operations is performed.
• Pressing of soft key [CANCEL] after performing a select
operation.
• Completion of a move operation.
• Change of the source folder during selection.
• Termination of a select operation with soft key [SELECT END]
and pressing of soft key [SELECT START] to enter the start of
selection state.
NOTE
When bit 6 (RTC) of parameter No. 11318 is 1, all
selected files are also deselected upon completion
of a copy operation.
Limitation
- Mode for performing copy and move operations
To copy and move files between different devices or data servers,
enter EDIT mode. In a multipath system, place all paths in EDIT
mode. If an attempt to perform an operation in a mode other than
EDIT mode, warning "CHANGE TO EDIT MODE" is issued.
- Restrictions on file operations in various devices
Those devices between which file copy and move operations can be
performed are as follows:
• CNC MEM
• MEM CARD (binary format)
(Note that a folder on a MEM CARD can be selected as a source
folder from which a file is to be read.)
• Data server
Between devices other than those above, copy or move operations
cannot be performed.
It is not possible to copy and move to devices other than those above
or to a MEM CARD or to move from a MEM CARD.
If an attempt is made to copy or move, warning "CAN NOT
COPY/MOVE" is issued.
- Folder copy and move operations
Folder copy or move operations cannot be performed.
If an attempt is made to select a folder as an object to copy or move,
warning "DISABLE TO SELECT" is issued.
Note
NOTE
Once a copy or move operation starts, it cannot be
canceled. Thus, check the files and folder subject to
the operation carefully before starting it.
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1386 -
10.12 KEYS AND PROGRAM ENCRYPTION
Overview
Program contents can be protected by setting parameters for
encryption and for the program security range.
Explanation
1 Security with a password and a security range
When the password and security range parameters are specified,
the display, editing, and input/output operations are disabled for
the programs within the security range.
This prevents the custom macro programs created by the machine
tool builder from being accidentally changed or deleted by the
end user. This also provides security because the contents of the
programs are not displayed.
2 Input/output of encrypted programs
The programs in the security range can be encrypted before being
output. Once encrypted, the programs cannot be decrypted. In
addition, encrypted programs can be input directly.
- Locking/unlocking
When the programs in the security range are secured, the program
memory is said to be locked.
If they are not secured, the program memory is said to be unlocked.
- Parameter
• Parameter PASSWORD (No.3220)
Set the password required to lock the program memory. A
password other than 0 can be set. The password is not displayed.
A password can be set when no password is set (PASSWORD =
0) or the program memory is unlocked.
• Parameter KEY (No.3221)
When KEY is set equal to PASSWORD, the program memory is
unlocked. The value set for the parameter is never displayed.
Each time the CNC is started, 0 is set for the parameter. This
means that whenever the CNC is started, a lock is provided if a
password is set (PASSWORD ≠ 0).
• Minimum value (in parameter No. 3222) and maximum value (in
parameter No. 3223) of the program security range
Set the desired security range. The value set for MINIMUM must
not be greater than that set for MAXIMUM. The programs in the
range of MINIMUM to MAXIMUM are secured. If MINIMUM
is set to 0, it is regarded as being 9000. If MAXIMUM is set to 0,
it is regarded as being 9999.
A range can be set when no password is set or the program
memory is unlocked.
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1387 -
NOTE
1 For security, the values set for PASSWORD and
KEY are not displayed. For the same reason,
PASSWORD, MINIMUM, and MAXIMUM can be
specified only when no password is set or the
program memory is unlocked. Set a password,
taking great care to avoid a situation where the
program memory cannot be unlocked because a
password is set incorrectly.
2 The [+INPUT] key used to specify PASSWORD and
KEY behave in the same way as the [INPUT] soft
key.
Example: When 99 is set for KEY, pressing 1
and [+INPUT] changes the value to.
3 These four parameters cannot be output externally.
Also, even when these parameters are input by the
parameter read operation, they are ignored.
- Inputting/outputting and collating programs
When a program is encrypted, a password is output. The password is
used to load the program.
The following output operations are enabled for programs outside the
security range if the locked state is present or for programs within the
security range if the unlocked state is present:
Outputting all programs
Locked/unlocked Results
Locked All the programs outside the security range are
output in the normal way.
Unlocked All the programs within the security range are
encrypted and output.
Password not set All the programs in the program memory are output
in the normal way.
Outputting a single program
Locked/unlocked Results
Locked If a program is outside the security range, it is output
in the normal way.
If it is within the security range, a warning
"PROTECTED" is issued.
Unlocked If a program is outside the security range, it is output
in the normal way.
If it is within the security range, it is encrypted and
output.
Password not set The program is output in a normal way.
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1388 -
Outputting specified multiple programs
Locked/unlocked Results
Locked When all of the specified programs fall outside the
protected range, they are output as usual.
When all of the specified programs are within the
security range, warning message "PROTECTED" is
issued.
When some of the specified program numbers are
outside the security range, and the others are within
the security range, only the programs outside the
security range are output normally.
When the programs to be output are not within the
specified range, warning message "THE WRONG
DATA IS USED" is issued.
Unlocked When all of the specified programs fall outside the
protected range, they are output as usual.
When all the specified programs fall within the
protected range, they are output as encoded
programs.
When some of the specified program numbers are
outside the security range, and the others are within
the security range, only the programs within the
security range are encoded and output.
When the programs to be output are not within the
specified range, warning message "THE WRONG
DATA IS USED" is issued.
Password not set The program is output in a normal way.
Inputting an un-encrypted program
Locked/unlocked Results
Locked When the program to be read is outside the security
range, it is input normally.
When the program to be read is within the security
range, warning message "PROTECTED" is issued.
Unlocked, or
password
not set
The program is input.
Inputting an encrypted program
Password set in the system
and password of the program Results
Password set in the system Warning “WRITE PROTECT” is issued.
Password for the program When the program is within the security
range, it is input normally.
When the program is outside the security
range, warning message "WRITE
PROTECTED" is issued.
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1389 -
Password set in the system
and password of the program Results
Password not set in the system The program is input.
The PSW in the file is set for parameter
No. 3220.
This applies if the program is in the
security range.
If the program is outside the security
range, warning message "PROTECTED"
is issued.
Collating a program with an encrypted program
In the unlocked state, the following takes place:
Password set in the system
and password of the program
Results
Password set in the system Alarm SR0075 “PROTECT” is issued.
Password set in the system =
Password of the program, or
password not set in the system
The program is collated.
In the locked state, program collation cannot be performed.
NOTE
To encrypt programs, set parameter ISO (bit 1 of
No.0000) to 1 (to specify that the punch code is
ISO).
- Program display
1 On the program folder screen, all program numbers are displayed
together with comments.
2 In the locked state, the programs within the security range are not
displayed on the program screen. In the unlocked state, the
programs within the security range are displayed in the same way
as normal programs.
NOTE
Immediately after switched from the unlocked state
to the locked state or from the locked state to the
unlocked state, programs are displayed in the
previous state. They are displayed in the new state
when a program search or other operation is
performed.
- Editing and deleting programs
When the program memory is locked, the programs within the security
range cannot be edited or deleted. When the program memory is
locked, an attempt to delete all programs results in only those
programs outside the security range being deleted.
In the locked state, the programs in the security range cannot be
selected as a main program. If an attempt is made to select such a
program on the program folder screen as a main program, warning
message "SETTING A MAIN PROGRAM FAILED" is issued.
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1390 -
- Searching for programs
In the locked state, a program search is performed within the protected
range as described below.
1 When no program number is specified, programs within the
protected range are skipped.
2 When an attempt is made to search for a program within the
security range by specifying a program number, the search
operation is ignored, resulting in warning message "Program is
protected".
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1391 -
10.13 SIMULTANEOUS EDITING OF MULTIPATH PROGRAMS
Simultaneous editing of multipath programs enables simultaneous
editing of programs for multiple paths on a single screen.
This function is enabled when bit 0 (DHD) of parameter No. 3106 is
1.
Explanation
- Procedure
1 Set the paths subject to simultaneous editing, with multipath
simultaneous display parameters Nos. 13131 and 13132.
(For details of the parameters, refer to the Parameter Manual
(B-63950EN).)
2 Place the paths subject to simultaneous editing in EDIT mode.
3 Press function key .
4 Press soft key [PROGRAM] to display the program editing
screen.
- Screen display
Figure 10.13 (a) to (c) show examples of performing simultaneous
editing of multipath programs.
Above each program is a status line on which three items of
information are displayed: the program name, "FG-EDIT", which
indicates that the program is being edited in the foreground, and the
path name.
For the program currently being edited, its status line is displayed in
reverse video.
Figure 10.13 (a) Simultaneous editing of multipath programs screen
(10.4-inch LCD)
Target of
editin
g
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1392 -
Figure 10.13 (b) Simultaneous editing of multipath programs screen
(15-inch LCD)
Figure 10.13 (c) Simultaneous editing of multipath programs screen
(7.2-inch LCD)
- Modes
When the paths to be displayed simultaneously are in either EDIT or
MEM mode, the multipath programs are displayed simultaneously on
the program screen. Selecting the path for which EDIT mode is
selected enables program editing to be performed.
Figure 10.13 (d) shows an example in which both EDIT and MEM
modes are selected.
For path 1, MEM mode (execution status screen) is selected, and for
path 2, EDIT mode (editing screen) is selected.
B-63944EN/03 OPERATION 10.EDITING PROGRAMS
- 1393 -
Soft keys are switched according to the mode for the currently
selected path.
Figure 10.13 (d) Screen on which both MEM and EDIT modes are
selected
- Switching the path subject to editing
The path selected with the path selection signal is subject to editing.
- Maximum number of paths that can be subject to editing simultaneously
The maximum number of paths that can be subject to editing
simultaneously on each LCD is as given in the table below.
LCD size
Maximum number of paths that can
be subject to editing
simultaneously
7.2, 8.4, or 10.4-inch 3
15-inch 4
- Conditions under which simultaneous editing is not usable
Simultaneous editing of multipath programs is disabled in the
following cases:
• The program screen is selected as a small screen.
• The paths to be displayed simultaneously include a path for
which a mode other than EDIT and MEM modes is selected.
• The virtual MDI key function is enabled.
If, in the state of simultaneous editing of multipath programs,
background editing is started, background editing is performed on all
screens. Simultaneous editing of multipath programs and background
editing cannot be used at the same time.
10.EDITING PROGRAMS OPERATION B-63944EN/03
- 1394 -
- Simultaneous editing on 7.2/8.4-inch LCDs
When simultaneous editing is performed on 7.2/8.4-inch LCDs, the
characters get smaller.
The number of characters per path in the editing area is as follows:
• Display of 38 columns and 10 rows for non-simultaneous display
• Display of 74 columns and 15 rows for 1-path simultaneous
display
• Display of 35 columns and 14 rows for 2-path simultaneous
display
• Display of 22 columns and 14 rows for 3-path simultaneous
display
B-63944EN/03 OPERATION 11.PROGRAM MANAGEMENT
- 1395 -
11 PROGRAM MANAGEMENT
Program management functions are classified into the following two
types:
• Functions for folders
• Functions for programs
Functions for folders include creation, deletion, change of names and
attributes, and so on.
Functions for programs include main program selection, deletion,
change of names and attributes, program compaction, and so on.
Management of
devices and
folders
Program
management
Creation and registration
Editing
Management
ExecutionOutput
Creating a folder.................................See III-11.2.
Renaming a folder..............................See III-11.3.
Changing folder attributes ..................See III-11.4.
Deleting a folder .................................See III-11.5.
Renaming a file.................................. See III-11.7.
Deleting a file..................................... See III-11.8.
Changing file attributes ...................... See III-11.9.
Selecting a main program .................. See III-11.10.
Making a program compact................ See III-11.11.
Selecting a default folder....................See III-11.6.
Selecting a device ..............................See III-11.1.
11.PROGRAM MANAGEMENT OPERATION B-63944EN/03
- 1396 -
11.1 SELECTING A DEVICE
When the fast data server function (option) is provided, a program
storage device can be selected. This section explains the selection
procedure.
Procedure for selecting a device
1 Press the function key .
2 Press the soft key [FOLDER].
3 Press the soft key [(OPRT)].
4 Press the soft key [DEVICECHANGE].
5 Press the soft key for the desired device.
B-63944EN/03 OPERATION 11.PROGRAM MANAGEMENT
- 1397 -
11.1.1 Selecting a Memory Card Program as a Device
Overview
By selecting a memory card including a program storage file (named
"FANUCPRG.BIN") as a device, memory operation can be performed
with the program in the program storage file selected as the main
program.
In addition, the content of a program storage file can be displayed on
the program list screen or a program in a program storage file can be
edited on the program edit screen.
A program storage file can be created using a memory card program
tool (A08B-9010-J700#ZZ11) on a commercially available personal
computer. To be used, the program storage file must be written to a
memory card formatted in FAT16 format.
(A program held in a program storage file is hereinafter referred to as
a memory card program. Moreover, a memory card storing a
program storage file is referred to as a program storage memory card.)
Procedure for selecting a device
1 Press the function key .
2 Press the soft key [FOLDER].
3 Press the soft key [(OPRT)].
4 Press the soft key [DEVICECHANGE].
5 Press the soft key [MEMCARD].
NOTE
1 A FAT16-formatted memory card containing the
program storage file FANUCPRG.BIN is recognized
as a program storage memory card.
2 For a program storage memory card containing
more than 63 folders and programs, the option for
extending the number of memory card program
registrations is required. The option for extending
the number of memory card program registrations is
applicable to a program storage memory card
containing a maximum of 1000 folders and
programs.
11.PROGRAM MANAGEMENT OPERATION B-63944EN/03
- 1398 -
Procedure for removing a device
When a program storage memory card is replaced or a memory card is
used for normal usage such as data input/output, clear the recognition
of the program storage memory card with removal operation.
1 Press the function key .
2 Press the soft key [FOLDER].
3 Press the soft key [(OPRT)].
4 Press the soft key [DEVICECHANGE].
5 Press the soft key [DETACH].
NOTE
1 This soft key appears when the CNC recognizes a
program storage memory card during device change
operation.
2 This operation is enabled only in EDIT mode or
MEM mode.
When a memory card program is selected in the
main programs of multiple paths in a multipath
control system, set the modes of all paths to EDIT
mode or MEM mode.
3 When the default folder is a folder in a program
storage file, it is changed to "//CNC_MEM/" by a
removal operation.
4 When the main program is a memory card program,
the main program enters the unselected state by a
removal operation.
Explanation
- About operation
A memory card program can be selected as a main program to perform
memory operation.
Memory operation has the following features:
• Subprogram call nesting is allowed.
• Macro program call nesting is allowed.
• In a custom macro, a control command using a GOTO
statement/WHILE statement can be specified.
• With the T series, a multiple repetitive canned cycle for turning
can be specified.
NOTE
To use the functions for calling macros, using
custom macros, and using a multiple repetitive
canned cycle for turning, the options corresponding
to the respective functions are required.
B-63944EN/03 OPERATION 11.PROGRAM MANAGEMENT
- 1399 -
- Selection as a main program
As a main program to be automatically executed in the memory mode,
a memory card program can be selected.
- Sub program (call using M98/G72.1/G72.2)
- Macro program (call using G65/G66/G66.1/M96)
The following subprogram/macro program held in the same folder as
containing the main program is called:
• Sub program call (M98)
• Macro call (Simple macro call G65 / Modal call G66,G66.1)
• Macro interrupt (M96)
• Figure copying (G72.1, G72.2)
If the program cannot be found in the same folder as the main program,
the following folder is searched:
• Common program folder on the CNC_MEM device (CNC
program storage memory)
NOTE
To use the functions for macro call, macro interrupt,
and figure copying, the options corresponding to
the respective functions are required.
- Sub program (call using M code/S code/T code/particular address/the second
auxiliary function)
- Macro program (call using G code/M code)
The following subprogram/macro program calls a program from the
CNC_MEM device (CNC program storage memory):
• Subprogram call using M code/S code/T code/particular
addresses/the second auxiliary function
• Macro call using G code/M code
The folders set as search targets are searched in the following order,
and the first found program is called:
1 Common program folder among the initial folders
2 MTB-dedicated folder 2 among the initial folders
3 MTB-dedicated folder 1 among the initial folders
4 System folder among the initial folders
Search target folders are set in parameter No. 3457.
NOTE
For a memory card program, subprogram call using
M code/S code/T code/particular addresses/the
second auxiliary function or macro call using G
code/M code can be specified. However, a
program on the CNC_MEM device (CNC program
storage memory) is called.
11.PROGRAM MANAGEMENT OPERATION B-63944EN/03
- 1400 -
- External program number search / External workpiece number search
A program on a program storage memory card can be searched for
with the external program number search function or external
workpiece number search function.
Limitation
For a memory card program, M198 cannot be specified. Moreover,
no memory card program can be called from a program on the
CNC_MEM device (CNC program storage memory) by specifying
M198.
When a setting is made to enable an external device subprogram call
from a memory card (M198) or DNC operation from a memory card
(bit 7 (MNC) of parameter No. 0138 = 1), the content of program
storage file cannot be displayed during automatic operation.
When a program storage memory card is selected, the memory card
cannot be used for the ordinary purposes listed below. To use a
memory card in such a case, perform a "removal" operation to cancel
the recognition of the program storage memory card.
• ALL I/O screen
Display of the contents of a memory card, and reading/punching
data to and from a memory card
• PMC data I/O screen
Display of the contents of a memory card, and reading/punching
to and from a memory card
• Program directory screen
Reading/punching program data to and from a memory card
• External device subprogram call (M198) operation
Subprogram call (M198) with a memory card set as an external
device
• DNC operation
DNC operation from a memory card
CAUTION
1 Do not remove the memory card when a program
that specifies a write to the memory card is being
edited. The data can be destructed.
2 If an editing operation is completed, the results of
editing are preserved even when the power to the
CNC is turned off.
B-63944EN/03 OPERATION 11.PROGRAM MANAGEMENT
- 1401 -
CAUTION
3 When removing the memory card, be sure to
perform a "removal" operation. If the memory card
is removed without performing a "removal" operation
and an attempt is made to access the memory card,
the alarm (SR1964) or alarm (IO1030) is issued.
If the card is removed inadvertently, insert the card
again and perform a "removal" operation.
When an alarm is issued, perform the following
operation:
- When the alarm (SR1964) is issued
Reset the alarm after performing a "removal"
operation.
- When the alarm (IO1030) is issued
The alarm can be reset only by turning off the
power to the CNC.
4 There are cases in which when a memory card is
replaced with another, the CNC cannot detect the
replacement. Thus, it is risky to replace a memory
card without performing a "removal" operation, and
this should never be attempted.
- Operation of creattion, edition, and management of a program
When “memory card program as a device” is selected, operation of
creattion, edition, and management of a program is below:
Item Usable
Creation of a program Unusable
Edition prohibition attribute Unusable
Inserting, alteration, and deletion a Word Usable
Deletion of a block Usable
Program search Usable
Sequence number search Usable
Deletion of a program Unusable
Editing a customa macro Usable
Password function Unusable
Editing a program character Usable
Program copy function Unusable
Key and program encryption Unusable
Selecting a device Usable
Creation of a folder Unusable
Renaming of a folder Unusable
Changing the attribute of a folder Unusable
Deletion of a folder Unusable
Selecting a default folder Usable
Renaming of a file Unusable
Deletion of a file Unusable
Changing the attribute of a file Unusable
Selecting a main program Usable
Making a program compact Unusable
Input/output of program Unusable
11.PROGRAM MANAGEMENT OPERATION B-63944EN/03
- 1402 -
11.2 CREATING A FOLDER
This section explains the procedure for creating a folder.
Procedure for creating a folder
1 Select EDIT mode.
2 Press the function key .
3 Move to the folder in which you want to create a folder.
Use the cursor keys and to move among folders.
After selecting the folder, press the key.
4 Press the soft key [(OPRT)].
5 Type folder name.
6 Press the soft key [CREATE FOLDER].
NOTE
1 Each folder name must be unique within the same
folder.
2 Each time a folder is created, the number of
programs that can be registered decreases by one.
3 Depending on the operation status and protection
status, a folder cannot sometimes be created.
B-63944EN/03 OPERATION 11.PROGRAM MANAGEMENT
- 1403 -
11.3 RENAMING A FOLDER
This section explains the procedure for renaming a folder.
Procedure for renaming a folder
1 Select EDIT mode.
2 Press the function key .
3 Press the soft key [FOLDER].
4 Select the folder that you want to rename.
To select a folder, use the cursor keys and .
5 Press the soft key [(OPRT)].
6 Type new folder name.
7 Press the soft key [RENAME].
NOTE
1 You cannot rename the initial folders.
2 Each folder name must be unique within the same
folder.
3 Depending on the operation status and protection
status, a folder cannot sometimes be renamed.
11.PROGRAM MANAGEMENT OPERATION B-63944EN/03
- 1404 -
11.4 CHANGING FOLDER ATTRIBUTES
This section explains the procedure for changing the attribute of a
folder (edit disable or edit/display disable).
Procedure for changing folder attributes
1 Select EDIT mode.
2 Press the function key .
3 Press the soft key [FOLDER].
4 Select the folder of which attribute is to be changed.
To select a folder, use the cursor keys and .
5 Press the soft key [(OPRT)].
6 Press the soft key [DETAILON].
7 Press the soft key [CHANGE ATTR].
• To disable editing, press the soft key [EDIT DISABL].
• To enable editing, press the soft key [EDIT ENABLE].
• To disable editing and display, press the soft key [DISP
DISABL].
• To enable editing and display, press the soft key [DISP
ENABLE].
NOTE
1 Depending on the operation status and protection
status, the attribute of a folder cannot sometimes
be changed.
2 When the edit disable attribute is set for a folder,
editing of folders and files in that folder is disabled.
3 When the edit/display disable attribute is set for a
folder, editing and display of folders and files in that
folder is disabled, and these folders and files are
not displayed.
4 The items that can be set vary depending on the
status of parameters and so on.
B-63944EN/03 OPERATION 11.PROGRAM MANAGEMENT
- 1405 -
11.5 DELETING A FOLDER
This section explains the procedure for deleting a folder.
Procedure for deleting a folder
1 Select EDIT mode.
2 Press the function key .
3 Press the soft key [FOLDER].
4 Select the folder that you want to delete.
To select a folder, use the cursor keys and .
5 Press the soft key [(OPRT)].
6 Press the soft key [DELETE].
• To perform the deletion, press the soft key [EXEC].
• To cancel the deletion, press the soft key [CANCEL].
NOTE
1 You cannot delete the initial folders.
2 A folder cannot be deleted unless the folder is
empty.
(An empty folder means that the folder contains
neither folders nor files.)
3 If a folder contains a folder or file having the
edit/display disable attribute, the folder may seem
to be empty when displayed, but the folder is not
actually empty, so it cannot be deleted.
4 Depending on the operation status and protection
status, a folder cannot sometimes be deleted.
11.PROGRAM MANAGEMENT OPERATION B-63944EN/03
- 1406 -
11.6 SELECTING A DEFAULT FOLDER
This section explains the procedure for selecting a foreground or
background default folder.
Procedure for selecting a default folder
1 Select EDIT mode.
2 Press the function key .
3 Press the soft key [FOLDER].
4 Move to the folder that you want to select as the default folder.
Use the cursor keys and to move among folders.
After selecting the folder, press the key.
5 Press the soft key [(OPRT)].
6 • To select the foreground, press the soft key [FORE
CHANGE].
• To select the background, press the soft key [BACK
CHANGE].
NOTE
1 When the foreground or background default folder
is not set, the path folder, which is an initial folder,
is assumed.
2 The settings for the foreground and background
default folders are stored in the default folder
setting file.
3 When a program file, program folder, or program
folder management file is cleared, the default folder
setting file is also cleared at the same time.
B-63944EN/03 OPERATION 11.PROGRAM MANAGEMENT
- 1407 -
11.7 RENAMING A FILE
This section explains the procedure for renaming a file.
Procedure for renaming a file
1 Select EDIT mode.
2 Press the function key .
3 Press the soft key [FOLDER].
4 Move to the folder containing the file that you want to rename.
Use the cursor keys and to move among folders.
After selecting the folder, press the key.
5 Select the file that you want to rename.
To select a file, use the cursor keys and .
6 Press the soft key [(OPRT)].
7 Type new file name.
8 Press the soft key [RENAME].
NOTE
1 Each file name must be unique within the same
file.
2 When the assigned file name cannot be treated as
a program number, the program in the file is
restricted as follows:
• Specification by program number is impossible.
(Such as a subprogram call)
• Information output by program number is
impossible.
3 Depending on the operation status and protection
status, a file cannot sometimes be renamed.
11.PROGRAM MANAGEMENT OPERATION B-63944EN/03
- 1408 -
11.8 DELETING A FILE
This section explains the procedure for deleting a file.
Procedure for deleting a file
1 Select EDIT mode.
2 Press the function key .
3 Press the soft key [FOLDER].
4 Move to the folder containing the file that you want to delete.
Use the cursor keys and to move among folders.
After selecting the folder, press the key.
5 Select the file that you want to delete.
To select a file, use the cursor keys and .
6 Press the soft key [(OPRT)].
7 Press the soft key [DELETE].
• To perform the deletion, press the soft key [EXEC].
• To cancel the deletion, press the soft key [CANCEL].
NOTE
Depending on the operation status and protection
status, a file cannot sometimes be deleted.
B-63944EN/03 OPERATION 11.PROGRAM MANAGEMENT
- 1409 -
11.9 CHANGING FILE ATTRIBUTES
This section explains the procedure for changing the attribute of a file
(edit disable, edit/display disable, encoding, or protection of data at
eight levels).
Procedure for selecting the attribute of a file
1 Select EDIT mode.
2 Press the function key .
3 Press the soft key [FOLDER].
4 Move to the folder containing the file of which attribute is to be
changed.
Use the cursor keys and to move among folders.
After selecting the folder, press the key.
5 Select the file of which attribute is to be changed.
To select a file, use the cursor keys and .
6 Press the soft key [(OPRT)].
7 Press the soft key [DETAILON].
8 Press the continuous menu key until the desired soft key
appears.
9 • To disable editing, press the soft key [EDIT DISABL].
• To enable editing, press the soft key [EDIT ENABLE].
• To disable editing and display, press the soft key [DISP
DISABL].
• To enable editing/display, press the soft key [DISP
ENABLE].
• To set encoding, press the soft key [ENCODESET].
• To cancel encoding, press the soft key [ENCODE RESET].
• To change the change protection level, type a change
protection level, then press the soft key [CHANGELEVEL].
• To change the output protection level, type an output
protection level, then press soft key [OUT LEVEL].
NOTE
1 Depending on the operation status and protection
status, a file cannot sometimes be deleted.
2 The items that can be set vary depending on the
status of options, parameters, and so on.
11.PROGRAM MANAGEMENT OPERATION B-63944EN/03
- 1410 -
11.10 SELECTING A MAIN PROGRAM
This section explains the procedure for selecting a main program.
Procedure for selecting a main program
1 Select EDIT mode.
2 Press the function key .
3 Press the soft key [FOLDER].
4 Move to the folder containing the file that you want to use as a
main program.
Use the cursor keys and to move among folders.
After selecting the folder, press the key.
5 Select the file that you want to use as the main program.
To select a file, use the cursor keys and .
6 Press the soft key [(OPRT)].
7 Press the soft key [MAIN PROGRM].
NOTE
Depending on the operation status and protection
status, the main program cannot sometimes be
selected.
B-63944EN/03 OPERATION 11.PROGRAM MANAGEMENT
- 1411 -
11.11 MAKING A PROGRAM COMPACT
This section explains the procedure for making a program compact.
Procedure for making a program compact
1 Select EDIT mode.
2 Press the function key .
3 Press the soft key [FOLDER].
4 Move to the folder containing the file of the program that you
want to make compact.
Use the cursor keys and to move among folders.
After selecting the folder, press the key.
5 Select the file of the program that you want to make compact.
To select a file, use the cursor keys and .
6 Press the soft key [(OPRT)].
7 Press the soft key [PROGRMCNDENS].
NOTE
1 Depending on the operation status and protection
status, a program cannot sometimes be made
compact.
2 nly programs on the CNC_MEM device can be
made compact.
11.PROGRAM MANAGEMENT OPERATION B-63944EN/03
- 1412 -
11.12 PROGRAM COPY FUNCTION
A program is copied or moved from folder to folder.
Procedure for copying a program compact
1 Press function key .
2 Press chapter selection soft key [FOLDER].
The following program folder screen appears:
3 Press the soft key [(OPRT)].
4 Display the folder from which the program to be copied or
moved. Move the cursor to the folder (indicated by
<FOLDER>) on the screen and press to move to the
folder.
5 Press the continuous menu key until soft key [SELECT
START] appears.
Press the soft key [SELECT START].
6 Move the cursor to the program that you want to select, and press
soft key [SELECT]. The background color of the selected
program changes to blue to indicate that the program is selected.
To select multiple programs, repeat this procedure.
7 Press the soft key [SELECT END]. The selected program is
determined.
8 Display the folder to which the program is to be copied or moved.
Move the cursor to the folder (indicated by <FOLDER>) on the
screen and press to move to the folder.
B-63944EN/03 OPERATION 11.PROGRAM MANAGEMENT
- 1413 -
9 Press soft key [COPY] in the folder to which the selected
program is copied to copy the program. If just one program is
selected, pressing soft key [COPY] after typing a program name
performs a copy operation with the entered name.
10 To move the program, press soft key [MOVE]. The selected
file is then moved. If just one program is selected, pressing soft
key [MOVE] after typing a program name performs a move
operation with the entered name.
Explanation
Operations are accepted only when the data protection key is set to
ON.
If the program storage capacity on the copy destination side is
insufficient, the copy operation is not accepted.
A selected program can be deselected by pressing [SELECT] again or
by pressing [CANCEL].
If a program with the same name is present in the copy or move
destination, soft keys [NO] and [REWRITE] are displayed together
with the "REWRITE: FILE NAME" message to ask whether to
overwrite the existing program. Pressing [REWRITE] performs
overwriting, and pressing [NO] does not perform the copy or move
operation of that program.
Pressing soft key [DELETE] deletes all the files currently selected.
A program can be neither copied nor moved to the same folder as the
selected folder.
However, when only one program is selected, if the name of the
program is entered, the program is copied or moved with the specified
name to the same folder.
NOTE
Once a copy or move operation starts, it cannot be
canceled. So, start the operation very carefully.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1414 -
12 SETTING AND DISPLAYING DATA
To operate a CNC machine tool, various data must be set on the MDI
panel for the CNC. The operator can monitor the state of operation
with data displayed during operation.
This chapter describes how to display and set data for each function.
Chapter 12, "SETTING AND DISPLAYING DATA", consists of the
following sections:
12.1 SCREENS DISPLAYED BY FUNCTION KEY ......1429
12.2 SCREENS DISPLAYED BY FUNCTION KEY ......1465
12.3 SCREENS DISPLAYED BY FUNCTION KEY ......1571
12.4 SCREENS DISPLAYED BY FUNCTION KEY ......1721
12.5 SCREENS DISPLAYED BY FUNCTION KEY ......1881
12.6 DISPLAYING THE PROGRAM NUMBER/NAME,
SEQUENCE NUMBER, AND STATUS, AND WARNING
MESSAGES FOR DATA SETTING OR INPUT/OUTPUT
OPERATION........................................................................1882
12.7 SCREEN ERASURE FUNCTION AND AUTOMATIC
SCREEN ERASURE FUNCTION.......................................1892
12.8 LOAD METER SCREEN ....................................................1894
Explanation
- Screen transition chart
The screen transition for when each function key on the MDI panel is
pressed is shown below. The subsections referenced for each screen
are also shown. See the appropriate subsection for details of each
screen and the setting procedure on the screen. See other chapters for
screens not described in this chapter.
See Chapter 7 for the screen that appears when function key is
pressed. In general, function key or is prepared by the
machine tool builder and used for macros. Refer to the manual issued
by the machine tool builder for the screen that appears when function
key or is pressed.
- Data protection key
The machine may have a data protection key to protect part programs,
tool compensation values, setting data, and custom macro variables.
Refer to the manual issued by the machine tool builder for where the
data protection key is located and how to use it.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1415 -
Screen displayed when the function key is pressed (for 7.2/8.4/10.4-inch
display unit)
ABS REL ALL HNDL (OPRT)
Page 1 +
(1) (2) (3) (4) (5)
Ø Ø Ø Ø
Position
display in
the
workpiece
coordinate
system
⇒ See III-12.1.1
Position
display in
the
workpiece
coordinate
system
⇒ See III-12.1.1
Position
display in
the
workpiece
coordinate
system
⇒ See III-12.1.1
Manual
handle
interruption
⇒ See III-4.4
Actual
feedrate
display
⇒ See III-12.1.5
Actual
feedrate
display
⇒ See III-12.1.5
Actual
feedrate
display
⇒ See III-12.1.5
Display of
run time
and parts
count
⇒ See III-12.1.6
Display of
run time
and parts
count
⇒ See III-12.1.6
Display of
run time
and parts
count
⇒ See III-12.1.6
MONI 3-D
MANUAL (OPRT)
Page 2 +
(6) (7) (8) (9) (10)
Ø Ø
Operating
monitor
display
⇒ See III-12.1.8
Display of
three-dime
nsional
manual
feed
⇒ See III-12.1.9
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1416 -
Screen displayed when the function key is pressed (for 15-inch display unit)
Page 1
(1) ALL ⇒
Overall position
display
⇒ See III-12.1.10
Actual feedrate
display
⇒ See
III-12.1.12
Display of run
time and parts
count
⇒ See III-12.1.13
(2) HANDLE ⇒
Manual handle
interruption
⇒ See III-4.5
(3) MONITO
R ⇒
Operating
monitor display
⇒ See III-12.1.15
(4) 3-D
MANUAL ⇒
Display of
3-dimensional
manual feed
⇒ See III-12.1.16
(5) VIRTUAL
AXIS
(6) ABSOLU
TE
(7) RELATI
VE
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1417 -
Screen displayed when the function key is pressed (for 7.2/8.4/10.4-inch
display unit)
PROGRA
M FOLDER NEXT CHECK (OPRT)
Page 1 +
(1) (2) (3) (4) (5)
Ø Ø Ø
Editing
programs
⇒ See III-10
Current
block
display
screen
⇒ See III-12.2.5
Program
check
screen
⇒ See III-12.2.6
Next block
display
screen
⇒ See III-12.2.5
RSTR JOG (OPRT)
Page 2 +
(6) (7) (8) (9) (10)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1418 -
Screen displayed when the function key is pressed (for 15-inch display unit)
Page 1
(1) PROGRM ⇒
Editing Programs
⇒ See III-10
(2) FOLDER
Program folder
screen
⇒ See III-12.2.13
(3) CHECK ⇒
Program check
screen
⇒ See III-12.2.15
(4) NEXT ⇒
Current block
display screen
⇒ See III-12.2.14
Next block display
screen
⇒ See III-12.2.14
(5) TIME
Stamping the
machining time
⇒ See III-12.2.17
(6) JOG
(7) RESTAR
T
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1419 -
Screen displayed when the function key is pressed (for 7.2/8.4/10.4-inch
display unit)
OFFSET SETTIN
G WORK (OPRT)
Page 1 +
(1) (2) (3) (4) (5)
Ø Ø Ø
Setting
and
displaying
the tool
offset
value
⇒ See III-2.1.1*1
Displaying
and
entering
setting
data
⇒ See III-12.3.1
Displaying
and setting
the
workpiece
origin
offset
value
⇒ See III-12.3.4
MACRO PATTER
N MENU OPR TOOL M
ANAGER (OPRT)
Page 2 +
(6) (7) (8) (9) (10)
Ø Ø Ø
Displaying
and setting
custom
macro
common
variables
⇒ See III-12.3.6
Displaying
and setting
pattern
data inputs
⇒ See III-12.3.15
Displaying
and setting
the
software
operator's
panel
⇒ See III-12.3.8
Setting and
displaying
tool
management
data
⇒ See III-12.3.9
OFST.2 W.SHFT GEOM.2 (OPRT)
Page 3 +
(11) (12) (13) (14) (15)
Ø Ø Ø
Y-axis
offset
⇒ See III-2.1.6*1
Setting the
workpiece
coordinate
system
shift value
⇒ See III-2.1.4*1
Setting tool
compensation
/ second
geometry
offset values
⇒ See III-2.1.5*1
PR-LV EXTEND
OFFSET (OPRT)
Page 4 +
(16) (17) (18) (19) (20)
Ø Ø
Precision
level
selection
⇒ See III-12.3.12
Setting the
4th/5th
axis offset
⇒ See III-2.1.8*1
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1420 -
CHUCK
TAIL LANG. PROTECT GUARD (OPRT)
Page 5 +
(21) (22) (23) (24) (25)
Ø Ø Ø Ø
Chuck and
tail stock
barriers
⇒ See III-2.1.9*1
Displaying
and
switching
the display
language
⇒ See III-12.3.10
Protection
of data at
eight levels
⇒ See III-12.3.11
Operation
confirmation
functions
⇒ See III-6.5
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1421 -
Screen displayed when the function key is pressed (for 15-inch display unit)
Page 1
Page 2
(1) OFFSET ⇒
Setting and
displaying the tool
offset value
⇒ See III-2.1.1 *1
(8) 2ND
GEOM ⇒
Setting tool
compensation/seco
nd geometry offset
values
⇒ See III-2.1.5 *1
(2) SETTIN
G ⇒
Displaying and
entering setting data
⇒ See III-12.3.16
(9) TOOL
FORM
(3) WORK ⇒
Displaying and
setting the
workpiece origin
offset value
⇒ See III-12.3.19
(10) CHOPPI
NG
(4) MACRO ⇒
Displaying and
setting custom
macro common
variables
⇒ See III-12.3.21
(11) CHUCK
TAIL ⇒
Chuck and tail
stock barriers
⇒ See III-2.1.7 *1
(5) OPERAT
PANEL ⇒
Displaying and
setting the software
operator’s pamel
⇒ See III-12.3.23
(12) LANGUA
GE ⇒
Displaying and
switching the
display language
⇒ See III-12.3.25
(6) Y OFFS
ET ⇒
Y-axis offset
⇒ See III-2.1.6 *1
(13) PROTEC
T ⇒
Protection of data
at eight levels
⇒ See III-12.3.26
(7) WORK
SHIFT ⇒
Setting the
workpiece
coordinate system
shift value
⇒ See III-2.1.4 *1
(14) GUARD ⇒
Operation
confirmation
functions
⇒ See III-6.5
NEXT
PAGE
NEXT
PAGE
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1422 -
Page 3
(15) PRECI
LEVEL ⇒
Precision level
selection
⇒ See III-12.3.27
(16) TOOL
LIFE ⇒
Setting and
displaying tool
management data
⇒ See III-12.3.24
(17) F-ACT
(18) F-OFFS
ET
(19)
(20) WORK
SET ER
(21)
NEXT
PAGE
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1423 -
Screen displayed when the function key is pressed (for 7.2/8.4/10.4-inch
display unit)
PARAME
TER
DIAGNO
SIS
SERVO
GUIDE SYSTEM (OPRT)
Page 1 +
(1) (2) (3) (4) (5)
Ø Ø Ø
Displaying
and setting
parameters
⇒ See III-12.4.1
Checking
by
self-diagno
sis screen
⇒ See III-7.3
SERVO
GUIDE
Mate
⇒ See
Maintenance
Manual
MEMORY PITCH
ERROR
SERVO
PARAM
SPINDL
SETING (OPRT)
Page 2 +
(6) (7) (8) (9) (10)
Ø Ø Ø Ø
Displaying
memory
⇒ See III-12.4.11
Displaying
and setting
pitch error
compensation
data
⇒ See III-12.4.2
Servo
parameters
⇒ See III-12.4.4
Spindle
setting
⇒ See III-12.4.6
PMC
MAINTE
PMC
LADDER
PMC
CONFIG (OPRT)
Page 3 +
(11) (12) (13) (14) (15)
MCNG
TUNING ALL IO ALL IO OPERAT
HISTRY (OPRT)
Page 4 +
(16) (17) (18) (19) (20)
Ø Ø Ø
Machining
parameter
tuning
⇒ See III-12.4.10
Input/
output on
the all IO
screen
⇒ See III-8.2
Input/
output on
the all IO
screen
⇒ See III-8.2
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1424 -
COLOR PERIOD
MAINTE
MAINTE
INFO
WAVE
DIAG (OPRT)
Page 5 +
(21) (22) (23) (24) (25)
Ø
Color
setting
screen
⇒ See III-12.4.9
FSSB PARAM
TUNING (OPRT)
Page 6 +
(26) (27) (28) (29) (30)
Ø Ø
FSSB data
display
and setting
screen
⇒ See
Maintenance
Manual
Machining
parameter
tuning
⇒ See III-12.4.10
EMBED
PORT
PCMCIA
LAN
ETHNET
BOARD
PROFI-
BUS MST (OPRT)
Page 7 +
(31) (32) (33) (34) (35)
M CODE 3D ERR
COMP (OPRT)
Page 8 +
(36) (37) (38) (39) (40)
Ø Ø
M code
grouping
function
⇒Ⅱ-11.3
3-dimensio
nal error
compensat
ion data
⇒Ⅱ-12.4.3
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1425 -
(OPRT)
Page 9 +
(41) (42) (43) (44) (45)
DUAL
CHECK
R.TIME
MACRO (OPRT)
Page 10 +
(46) (47) (48) (49) (50)
Ø Ø
Dual
Check
Safety
diagnosis
data
⇒ Dual Check
Safety
OPERATOR’S
MANUAL
(B-64004EN)
Real time
custom
macro
⇒Ⅱ-12.3.7
NOTE
For information about a dedicated screen for each
path control type in the lathe system/machining
center system, refer to the manuals:
*1: User's manual (T series) (B-63944EN-1)
*2: User's manual (M series) (B-63944EN-2)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1426 -
Screen displayed when the function key is pressed (for 15-inch display unit)
Page 1
Page 2
(1) PARAME
TER ⇒
Displaying and
setting parameters
⇒ See III-12.4.13 (8) PMC
MAINTE
(2) DIAGNO
SIS ⇒
Checking by
self-diagnosis
screen
⇒ See III-7.3
(9) LADDER
(3) SERVO
GUIDE ⇒
SERVO GUIDE
Mate
⇒ See Maintenance
Manual
(10) PMC
CONFIG
(4) MEMORY ⇒
Displaying memory
data
⇒ See III-12.4.23 (11)
(5) PITCH
ERROR ⇒
Displaying and
setting pitch error
compensation data
⇒ See III-12.4.14
(12) COLOR ⇒
Color setting
screen
⇒ See III-12.4.21
(6) SERVO
PARAM ⇒
Servo parameters
⇒ See III-12.4.16 (13) PERIOD
MAINTE
(7) SPINDL
SETING ⇒
Spindle setting
⇒ See III-12.4.18 (14) MAINTE
INFO
NEXT
PAGE
NEXT
PAGE
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1427 -
Page 3
Page 4
(15) FSSB ⇒
FSSB data display
and setting screen
⇒ See
Maintenance
Manual
(22) M CODE
GROUP ⇒
M code grouping
function
⇒ See II-11.3
(16) MCHN
TUNING ⇒
Machining
parameter tuning
⇒ See III-12.4.22 (23) EMBED
PORT
(17) WAVE
DIAG
(24) PCMCIA
LAN
(18) OPERAT
HISTRY
(25) ETHER
BOARD
(19) ALL IO ⇒
Input/ output on
the all IO screen
⇒ See III-8.2 (26) PROFI
MASTER
(20) ALL IO ⇒
Input/ output on
the all IO screen
⇒ See III-8.2 (27) PROFI
SLAVE
(21) PARAM
TUNING ⇒
Parameter tuning
⇒ See III-12.4.24 (28) 3D ERR
COMP ⇒
Displaying and setting
three-dimensional error
compensation data
⇒ See III-12.4.15
NEXT
PAGE
NEXT
PAGE
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1428 -
NOTE
For information about a dedicated screen for each
path control type in the lathe system/machining
center system, refer to the manuals:
*1: User's manual (T series) (B-63944EN-1)
*2: User's manual (M series) (B-63944EN-2)
Page 5
Page 6
(29) P.MATE
MGR.
(36)
(30) SYSTEM
(37) DEVNET
MASTER
(31) REMOTE
DIAG
(38) FL-net
(32) DUAL
CHECK ⇒
Dual Check Safety
diagnosis data
⇒ See Dual Check
Safety Operator’s
Manual (B-64004EN)
(39) DEVNET
SLAVE
(33) R.TIME
MACRO ⇒
Displaying and
setting real time
custom macro data
⇒ See III-12.3.22
(40) CUSTOM
BOARD
(34) HI-PIT
CH ERR
(41)
(35) PARTS
LEARN
(42)
NEXT
PAGE
NEXT
PAGE
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1429 -
12.1 SCREENS DISPLAYED BY FUNCTION KEY
Section 12.1, "SCREENS DISPLAYED BY FUNCTION KEY
", consists of the following subsections:
------ Screens of a 7.2/8.4/10.4-inch display unit ------
12.1.1 Position Display in the Workpiece Coordinate System .....1431
12.1.2 Position Display in the Relative Coordinate System .........1433
12.1.3 Overall Position Display ....................................................1436
12.1.4 Workpiece Coordinate System Preset................................1438
12.1.5 Actual Feedrate Display.....................................................1439
12.1.6 Display of Run Time and Parts Count ...............................1441
12.1.7 Setting the Floating Reference Position.............................1443
12.1.8 Operating Monitor Display ................................................1444
12.1.9 Display of Three-dimensional Manual Feed
(Tool Tip Coordinates, Number of Pulses, Machine
Axis Move Amount) ..........................................................1447
------ Screens of a 15-inch display unit ------
12.1.10 Overall Position Display (15-inch Display Unit)...............1451
12.1.11 Workpiece Coordinate System Preset (15-Inch Display
Unit) ...................................................................................1454
12.1.12 Actual Feedrate Display (15-inch Display Unit) ...............1455
12.1.13 Display of Run Time and Parts Count (15-Inch Display
Unit) ...................................................................................1457
12.1.14 Setting the Floating Reference Position (15-Inch
Display Unit)......................................................................1459
12.1.15 Operating Monitor Display (15-inch Display Unit)...........1460
12.1.16 Display of Three-dimensional Manual Feed
(Tool Tip Coordinates, Number of Pulses, Machine
Axis Move Amount) (15-inch Display Unit).....................1463
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1430 -
Screens of a 7.2/8.4/10.4-inch display unit
Press function key to display the current position of the tool.
The following three screens are used to display the current position of
the tool:
• Current position display screen for the workpiece coordinate
system.
• Current position display screen for the relative coordinate
system.
• Current overall position display screen.
The above screens can also display the feedrate, run time, and the
number of parts. In addition, a floating reference position can be set
on these screens.
Function key can also be used to display the load on the servo
motor and spindle motor and the rotation speed of the spindle motor
(operating monitor display).
Function key can also be used to display the screen for
displaying the distance moved by handle interruption. See III- 4.6 for
details on this screen.
On any of the position display screens, the status (such as D, I, L, S, *,
or M) of an axis is indicated on the left of the axis name to prevent
wrong operations. See "Axis status display" in III-6.5, "WRONG
OPERATION PREVENTION FUNCTIONS" for details.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1431 -
12.1.1 Position Display in the Workpiece Coordinate System
Displays the current position of the tool in the workpiece coordinate
system. The current position changes as the tool moves. The least
input increment is used as the unit for numeric values. The title at the
top of the screen indicates that absolute coordinates are used.
Display procedure for the current position screen in the workpiece coordinate
Procedure
1 Press function key .
2 Press soft key [ABSOLUTE].
Fig. 12.1.1 (a) Current position (absolute) screen (M series)(10.4-inch)
Fig. 12.1.1 (b) Current position (absolute) screen (T series)(10.4-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1432 -
Explanation
- Display including compensation values
M
Bits 6 (DAL) and 7 (DAC) of parameter No. 3104 can be used to
select whether the displayed values include tool length compensation
and cutter compensation.
T
Bit 1 (DAP) parameter No. 3129 and bit 7 (DAC) of parameter No.
3104 can be used to select whether the displayed values include tool
offset and tool nose radius compensation.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1433 -
12.1.2 Position Display in the Relative Coordinate System
Displays the current position of the tool in a relative coordinate
system based on the coordinates (see Explanation) set by the operator.
The current position changes as the tool moves. The increment system
is used as the unit for numeric values.
The title at the top of the screen indicates that relative coordinates are
used.
Display procedure for the current position screen with the relative coordinate
system
Procedure
1 Press function key .
2 Press soft key [RELATIVE].
Fig. 12.1.2 (a) Current position (relative) screen (M series)(10.4-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1434 -
Fig. 12.1.2 (b) Current position (relative) screen (T series) (10.4-inch)
See Explanation for the procedure for setting the coordinates.
Explanation
- Setting the relative coordinates
The current position of the tool in the relative coordinate system can
be reset to 0 or preset to a specified value as follows:
Procedure to set the axis coordinate to a specified value
Procedure
1 To reset the coordinate to 0, press soft key [ORGIN].
Key in an axis name to be reset (such as X or Y), then press soft
key [EXEC].
2 For presetting to a specified value, key in an axis name to be
preset and a preset value (such as X100.000), then press soft key
[PRESET].
- Display including compensation values
M
Bits 4 (DRL) and 5 (DRC) of parameter No. 3104 can be used to
select whether the displayed values include tool length compensation
and cutter compensation.
T
Bit 0 (DRP) parameter No. 3129 and bit 5 (DRC) of parameter No.
3104 can be used to select whether the displayed values include tool
offset and tool nose radius compensation.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1435 -
- Presetting by setting a coordinate system
M
Bit 3 (PPD) of parameter No. 3104 can be used to specify whether the
position indication values in the absolute coordinate system are preset
as those in the relative coordinate system during coordinate system
setting or manual reference position return by the G92 command.
T
Bit 3 (PPD) of parameter No. 3104 can be used to specify whether the
position indication values in the absolute coordinate system are preset
as those in the relative coordinate system during coordinate system
setting or manual reference position return by the G50 command (for
G code system A) or G92 command (for G code system B or C).
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1436 -
12.1.3 Overall Position Display
Displays the following positions on a screen : Current positions of the
tool in the workpiece coordinate system, relative coordinate system,
and machine coordinate system, and the remaining distance.
The relative coordinates can also be set on this screen. See III-12.1.2
for the procedure.
Procedure for displaying overall position display screen
Procedure
1 Press function key .
2 Press soft key [ALL].
Fig. 12.1.3 (a) Current position (overall) screen (M series) (10.4-inch)
Fig. 12.1.3 (b) Current position (overall) screen (T series) (10.4-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1437 -
Explanation
- Coordinate display
The current positions of the tool in the following coordinate systems
are displayed at the same time:
• Current position in the relative coordinate system
(relative coordinate)
• Current position in the workpiece coordinate system
(absolute coordinate)
• Current position in the machine coordinate system
(machine coordinate)
• Distance to go (distance to go)
- Distance to go
The distance remaining is displayed in the MEMORY or MDI mode.
The distance the tool is yet to be moved in the current block is
displayed.
- Machine coordinate system
The least command increment is used as the unit for values displayed
in the machine coordinate system. However, the least input increment
can be used by setting bit 0 (MCN) of parameter No. 3104.
- Resetting the relative coordinates
The total position display screen also supports the resetting of the
relative coordinates to 0 or presetting of them to specified values. See
the procedure for resetting the relative coordinates described in
Subsection III-12.1.2
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1438 -
12.1.4 Workpiece Coordinate System Preset
If a workpiece coordinate system has been shifted with manual
intervention or any other operation, an MDI operation can be
performed to preset the system to a workpiece coordinate system that
is offset by a workpiece origin offset, from the machine zero point that
has been set before the shifting.
A command (G92.1) can be programmed to preset a workpiece
coordinate system. (See II-7.2.4.)
Procedure for the workpiece coordinate system preset
Procedure
1 Press function key .
2 Press soft key [(OPRT)].
3 Enter the axis name ( , , ...) and .
4 Press soft key [PRESET].
Explanation
- Operation mode
This function can be executed when the reset state or automatic
operation stop state is entered, regardless of the operation mode.
- Presetting relative coordinates
As with absolute coordinates, bit 3 (PPD) of parameter No. 3104 is
used to specify whether to preset relative coordinates (RELATIVE).
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1439 -
12.1.5 Actual Feedrate Display
The actual feedrate on the machine (per minute) can be displayed on a
current position display screen or program check screen.
On the 12 soft keys display unit, the actual feedrate is always
displayed.
Display procedure for the actual feedrate on the current position display screen
Procedure
1 Press the function key to display a current position
display screen. At the location indicated by , an actual
feedrate is displayed.
Fig. 12.1.5 (a) Current position (absolute) screen (M series) (10.4-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1440 -
Fig. 12.1.5 (b) Current position (absolute) screen (T series) (10.4-inch)
The actual feedrate is displayed in units of millimeter/min or inch/min
(depending on the specified least input increment) under the display of
the current position.
Explanation
- Actual feedrate value
The actual rate is calculated by the following expression:
∑
=
n
1i
2
(fi)Fact＝
n : Number of axes
fi : Cutting feed rate in the tangential direction of
each axis or rapid traverse rate
Fact : Actual feedrate displayed
The display unit:
mm/min (metric input).
inch/min (Inch input, two digits below the decimal point are
displayed.)
- Actual feedrate display of feed per revolution
In the case of feed per revolution and thread cutting, the actual
feedrate displayed is the feed per minute rather than feed per
revolution.
- Actual feedrate display of rotary axis
In the case of movement of rotary axis, the speed is displayed in units
of deg/min but is displayed on the screen in units of input system at
that time. For example, when the rotary axis moves at 50 deg/min, the
following is displayed: 50 mm/min (in metric input) or 0.50 inch/min
(in inch input).
- Actual feedrate display on the other screen
The program check screen also displays the actual feedrate.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1441 -
12.1.6 Display of Run Time and Parts Count
The run time, cycle time, and the number of machined parts are
displayed on the current position display screens.
Procedure for displaying run time and parts count on the current position display
screen
Procedure
1 Press the function key to display a current position
display screen. At the location indicated by , a run time and
parts count are displayed.
Fig. 12.1.6 (a) Current position (relative) screen (M series) (10.4-inch)
Fig. 12.1.6 (b) Current position (relative) screen (T series) (10.4-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1442 -
The number of machined parts (PART COUNT), run time (RUN
TIME), and cycle time (CYCLE TIME) are displayed under the
current position.
Explanation
- PART COUNT
Indicates the number of machined parts. The number is incremented
each time M02, M30, or an M code specified by parameter No. 6710
is executed.
- RUN TIME
Indicates the total run time during automatic operation, excluding the
stop and feed hold time.
- CYCLE TIME
Indicates the run time of one automatic operation, excluding the stop
and feed hold time. This is automatically preset to 0 when a cycle start
is performed at reset state. It is preset to 0 even when power is
removed.
- Display on the other screen
Details of the run time and the number of machined parts are
displayed on the setting screen. See III-12.3.3.
- Parameter setting
The number of machined parts and run time cannot be set on current
position display screens.
The number of machined parts and run time cannot be set on current
position display screens. They can be set by parameters Nos. 6711,
6751, and 6752 or on the setting screen.
- Incrementing the number of machined parts
Bit 0 (PCM) of parameter No. 6700 is used to specify whether the
number of machined parts is incremented each time M02, M30, or an
M code specified by parameter No. 6710 is executed, or only each
time an M code specified by parameter No. 6710 is executed.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1443 -
12.1.7 Setting the Floating Reference Position
To perform floating reference position return with a G30.1 command,
the floating reference position must be set beforehand.
Procedure for setting the floating reference position
Procedure
1 Press function key to display a screen used for displaying
the current position.
2 Move the tool to the floating reference position by jogging.
3 Press soft key [(OPRT)].
4 Press soft key [SET FRP].
5 To register the floating reference positions for all axes, press soft
key [ALL AXIS].
To register the floating reference position of a specific axis, enter
the name of the axis ( , , etc.), then press soft key
[AXIS NAME]. Two or more names can be entered consecutively
(e.g., ) [AXIS NAME]).
The above operation stores the floating reference position. It can
be checked with parameter (No. 1244).
6 In step 4, the floating reference position along a specified axis
can also be stored by entering the axis name (such as or
) and pressing soft key [SET FRP].
Explanation
- Presetting the relative coordinate system
When bit 3 (FPC) of parameter No. 1201 is set to 1, the floating
reference position can be registered, while the relative position display
can be preset to 0.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1444 -
12.1.8 Operating Monitor Display
The load meter for a servo axis can be displayed. Also, the load meter
and speed meter for a serial spindle can be displayed.
To enable this function, bit 5 (OPM) of parameter No. 3111 must be
set to 1.
Procedure for displaying the operating monitor
Procedure
1 Press function key .
2 Press continuous menu key .
3 Press soft key [MONITOR].
Fig. 12.1.8 (a) Operating monitor (M series) (10.4-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1445 -
Fig. 12.1.8 (b) Operating monitor (T series) (10.4-inch)
Explanation
- Display of the servo axes
Servo axis load meters as many as the maximum number of controlled
axes of the path can be displayed. One screen displays load meters for
up to five axes at a time. By pressing the soft key [MONITOR], load
meters for the 6th axis and up are displayed.
- Display of the spindle axes
When serial spindles are used, the reading on the load meter and
speedometer can be displayed only for the main serial spindle.
- Unit of graph
The bar graph for the load meter shows load up to 200% (only a value
is displayed for load exceeding 200%).
The bar graph for the speedometer shows the ratio of the current
spindle speed to the maximum spindle speed (100%).
- Load meter
The reading on the load meter depends on servo parameter No. 2086
and spindle parameter No. 4127.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1446 -
- Speedometer
Although the speedometer normally indicates the speed of the spindle
motor, it can also be used to indicate the speed of the spindle by setting
bit 6 (OPS) of parameter No. 3111 to 1.
The spindle speed to be displayed during operation monitoring is
calculated from the speed of the spindle motor (see the formula below).
The spindle speed can therefore be displayed, during operation
monitoring, even when no position coder is used.
To display the correct spindle speed, however, the maximum spindle
speed for each gear (spindle speed at each gear ratio when the spindle
motor rotates at the maximum speed) must be set in parameters No.
3741 to No.3744.
The input of the clutch and gear signals for the first serial spindle is
used to determine the gear which is currently selected. Control the
input of the CTH1A and CTH2A signals according to the gear
selection, by referring to the table below.
(Formula for calculating the spindle speed to be displayed)
Maximum spindle speed
with the gear being used
Maximum speed of
spindle motor
Speed of spindle motor
Spindle speed displayed
during operation monitoring =×
The following table lists the correspondence between clutch and gear
selection signals CTH1A and CTH2A, used to determine the gear
being used, and parameters:
CTH1A CTH2A Parameter Serial spindle
spec
ification
0 0
=No.3741 (Maximum spindle speed
with gear 1) HIGH
0 1
=No.3742 (Maximum spindle speed
with gear 2) MEDIUM HIGH
1 0
=No.3743 (Maximum spindle speed
with gear 3) MEDIUM LOW
1 1
=No.3744 (Maximum spindle speed
with gear 4) LOW
The speed of the spindle motor and spindle can be displayed, during
operation monitoring, only for the first serial spindle and the spindle
switching axis for the first serial spindle. It cannot be displayed for the
second spindle.
- Color of graph
If the value of a load meter exceeds 100%, the bar graph turns purple.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1447 -
12.1.9 Display of Three-dimensional Manual Feed (Tool Tip
Coordinates, Number of Pulses, Machine Axis Move Amount)
The absolute coordinates of the tool tip, the number of pulses, and a
machine axis move amount based on three-dimensional manual feed
are displayed.
Displaying the screen for three-dimensional manual feed
Procedure
1 Press function key .
2 Press the continuous menu key several times to display the
soft key [3-D MANUAL].
3 Press the soft key [3-D MANUAL] to display the screen of
three-dimensional manual feed.
Fig. 12.1.9 (a) Three-dimensional manual feed screen(10.4-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1448 -
Explanation
- Tool tip position
The addresses of the three basic machine configuration axes for
performing three-dimensional manual feed and the current position of
the tool tip are displayed.
- Tool axis reference (number of pulses)
TD
The amount of travel in the tool axis direction in tool axis
direction handle feed, tool axis direction jog feed, or tool axis
direction incremental feed is displayed.
The unit is the least input increment of the axis in the direction
specified by parameter No. 19697.
R1
The amount of travel in the first axis direction in tool axis
right-angle direction handle feed, tool axis right-angle direction
jog feed, or tool axis right-angle direction incremental feed is
displayed.
The unit is the least input increment of the axis in the first axis
direction normal to the direction specified by parameter No.
19697.
R2
The amount of travel in the second axis direction in tool axis
right-angle direction handle feed, tool axis right-angle direction
jog feed, or tool axis normal direction incremental feed is
displayed.
The unit is the least input increment of the axis in the second axis
direction normal to the direction specified by parameter No.
19697.
- Tool tip center (number of pulses)
C1
The angular displacement in tool tip center rotation handle feed,
tool tip center rotation jog feed, or tool tip center rotation
incremental feed for rotation of the first rotary axis is displayed.
The unit is the least input increment of the first rotary axis.
C2
The angular displacement in tool tip center rotation handle feed,
tool tip center rotation jog feed, or tool tip center rotation
incremental feed for rotation of the second rotary axis is
displayed. The unit is the least input increment of the second
rotary axis.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1449 -
- Table reference (number of pulses)
VR
The amount of travel in the table reference vertical direction in
table reference vertical direction handle feed, table reference
vertical direction jog feed, or table reference vertical direction
incremental feed is displayed.
The unit is the least input increment of the axis in the direction
specified by parameter No. 19697.
H1
The amount of travel in the first axis direction in table reference
horizontal direction handle feed, table reference horizontal
direction jog feed, or table reference horizontal direction
incremental feed is displayed.
The unit is the least input increment of the axis in the first axis
direction normal to the direction specified by parameter No.
19697.
H2
The amount of travel in the second axis direction in table
reference horizontal direction handle feed, table reference
horizontal direction jog feed, or table reference horizontal
direction incremental feed is displayed.
The unit is the least input increment of the axis in the second axis
direction normal to the direction specified by parameter No.
19697.
- Amounts of machine axis travel
The addresses of machine configuration axes used for
three-dimensional manual feed and the sum of the amount of travel of
each axis used for three-dimensional manual feed are displayed.
The values of the basic three axes (X-axis, Y-axis, and Z-axis), the
first rotary axis, and the second rotary axis are displayed in this order.
For the definition of the first rotary axis and second rotary axis, see
the description of parameter No. 19680.
When bit 0 (CLR) of parameter No. 13113 is set to 1, the displayed
data is cleared by a reset.
- Absolute coordinates, machine coordinates
The absolute coordinates and machine coordinates of all axes are
displayed. If too many axes are involved for display on one screen, the
remaining axes can be displayed by pressing the soft key [3-D
MANUAL] for page feed.
- F (feedrate)
• When bit 3 (CFD) of parameter No. 13113 is set to 0
The composite feedrate at a control point on a linear axis or
rotary axis is displayed.
• When bit 3 (CFD) of parameter No. 13113 is set to 1
The feedrate of the tool tip is displayed.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1450 -
Operation
The display of the number of pulses can be cleared by soft key
operations.
1 Press soft key [(OPRT)].
2 Select the soft key corresponding to a function subject to clearing
of the amount of travel.
Pressing the rightmost soft key displays the second page.
3 Press soft key [ERASE] to clear the amount of travel of the
specified function. Press soft key [CAN] to cancel erase
operation.
Screens of a 15-inch display unit
Press function key to display the current overall position
display screen that shows the current position of the tool.
The above screen can also display the feedrate, run time, and the
number of parts. In addition, a floating reference position can be set
on this screen.
Function key can also be used to display the load on the servo
motor and spindle motor and the rotation speed of the spindle motor
(operating monitor display).
Function key can also be used to display the screen for
displaying the distance moved by handle interruption. See III-4.6 for
details on this screen.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1451 -
12.1.10 Overall Position Display (15-inch Display Unit)
Displays the following positions on a screen : Current positions of the
tool in the workpiece coordinate system, relative coordinate system,
and machine coordinate system, and the remaining distance.
The relative coordinates can also be set on this screen. (Refer to
Explanation.)
Procedure for displaying overall position display screen
Procedure
1 Press function key .
2 Press vertical soft key [ALL].
Fig. 12.1.10 (a) Current position screen (M series) (15-inch)
Fig. 12.1.10 (b) Current position screen (T series) (15-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1452 -
Explanation
- Coordinate display
The current positions of the tool in the following coordinate systems
are displayed at the same time:
• Current position in the relative coordinate system
(relative coordinate)
• Current position in the work coordinate system
(absolute coordinate)
• Current position in the machine coordinate system
(machine coordinate)
• Distance to go (distance to go)
- Distance to go
The distance remaining is displayed in the MEMORY or MDI mode.
The distance the tool is yet to be moved in the current block is
displayed.
- Machine coordinate system
The least command increment is used as the unit for values displayed
in the machine coordinate system. However, the least input increment
can be used by setting bit 0 (MCN) of parameter No. 3104.
- Setting the relative coordinates
The current position of the tool in the relative coordinate system can
be reset to 0 or preset to a specified value as follows:
Procedure to set the axis coordinate to a specified value
Procedure
1 To reset the coordinate to 0, press horizontal soft key [ORGIN].
Key in an axis name to be reset (such as X or Y), then press soft
key [EXEC].
2 For presetting to a specified value, key in an axis name to be
preset and a preset value (such as X100.000), then press
horizontal soft key [PRESET].
- Display including compensation values
M
The following parameters can be used to determine whether the
displayed values include tool length compensation and cutter
compensation.
• Workpiece coordinate system: Bits 6 (DAL) and 7 (DAC) of
parameter No. 3104
• Relative coordinate system: Bits 4 (DRL) and 5 (DRC) of
parameter No. 3104
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1453 -
T
The following parameters can be used to determine whether the
displayed values include tool offset and tool nose radius
compensation.
• Workpiece coordinate system: Bit 1 (DAP) of parameter No.
3129 and bit 7 (DAC) of parameter No. 3104
• Relative coordinate system: Bit 0 (DRP) of parameter No. 3129
and bit 5 (DRC) of parameter No. 3104
- Presetting by setting a coordinate system
M
Bit 3 (PPD) of parameter No. 3104 can be used to specify whether the
position indication values in the absolute coordinate system are preset
as those in the relative coordinate system during coordinate system
setting or manual reference position return by the G92 command.
T
Bit 3 (PPD) of parameter No. 3104 can be used to specify whether the
position indication values in the absolute coordinate system are preset
as those in the relative coordinate system during coordinate system
setting or manual reference position return by the G50 command (for
G code system A) or G92 command (for G code system B or C).
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1454 -
12.1.11 Workpiece Coordinate System Preset (15-inch Display Unit)
If a workpiece coordinate system has been shifted with manual
intervention or any other operation, an MDI operation can be
performed to preset the system to a workpiece coordinate system that
is offset by a workpiece origin offset, from the machine zero point that
has been set before the shifting.
A command (G92.1) can be programmed to preset a workpiece
coordinate system. (See II-7.2.4.)
Procedure for the workpiece coordinate system preset
Procedure
1 Press function key .
2 Press vertical soft key [ALL].
3 Enter the axis name ( , , ...) and .
4 Press soft key [PRESET].
Explanation
- Operation mode
This function can be executed when the reset state or automatic
operation stop state is entered, regardless of the operation mode.
- Presetting relative coordinates
As with absolute coordinates, bit 3 (PPD) of parameter No. 3104 is
used to specify whether to preset relative coordinates (RELATIVE).
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1455 -
12.1.12 Actual Feedrate Display (15-inch Display Unit)
The actual feedrate on the machine (per minute) can be displayed on a
current position display screen or program check screen.
Display procedure for the actual feedrate on the current position display screen
Procedure
1 Press the function key to display a current position
display screen. At the location indicated by , an actual
feedrate is displayed.
Fig. 12.1.12 (a) Current position screen (M series) (15-inch)
Fig. 12.1.12 (b) Current position screen (T series) (15-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1456 -
The actual feedrate is displayed in units of millimeter/min or
inch/min (depending on the specified least input increment)
under the display of the current position.
Explanation
- Actual feedrate value
The actual rate is calculated by the following expression:
∑
=
n
1i
2
(fi)Fact＝
n : Number of axes
fi : Cutting feed rate in the tangential direction of
each axis or rapid traverse rate
Fact : Actual feedrate displayed
The display unit:
mm/min (metric input).
inch/min (Inch input, two digits below the decimal point are
displayed.)
- Actual feedrate display of feed per revolution
In the case of feed per revolution and thread cutting, the actual
feedrate displayed is the feed per minute rather than feed per
revolution.
- Actual feedrate display of rotary axis
In the case of movement of rotary axis, the speed is displayed in units
of deg/min but is displayed on the screen in units of input system at
that time. For example, when the rotary axis moves at 50 deg/min, the
following is displayed: 50 mm/min (in metric input) or 0.50 inch/min
(in inch input).
- Actual feedrate display on the other screen
The program check screen also displays the actual feedrate.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1457 -
12.1.13 Display of Run Time and Parts Count (15-inch Display Unit)
The run time, cycle time, and the number of machined parts are
displayed on the current position display screens.
Procedure for displaying run time and parts count on the current position display
screen
Procedure
1 Press the function key to display a current position
display screen. At the location indicated by , a run time
and parts count are displayed.
Fig. 12.1.13 (a) Current position screen (M series) (15-inch)
Fig. 12.1.13 (b) Current position screen (T series) (15-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1458 -
The number of machined parts (PART COUNT), run time (RUN
TIME), and cycle time (CYCLE TIME) are displayed under the
current position.
Explanation
- PART COUNT
Indicates the number of machined parts. The number is incremented
each time M02, M30, or an M code specified by parameter No. 6710
is executed.
- RUN TIME
Indicates the total run time during automatic operation, excluding the
stop and feed hold time.
- CYCLE TIME
Indicates the run time of one automatic operation, excluding the stop
and feed hold time. This is automatically preset to 0 when a cycle start
is performed at reset state. It is preset to 0 even when power is
removed.
- Display on the other screen
Details of the run time and the number of machined parts are
displayed on the setting screen. See III-12.3.18.
- Parameter setting
The number of machined parts and run time cannot be set on current
position display screens.
The number of machined parts and run time cannot be set on current
position display screens. They can be set by parameters Nos. 6711,
6751, and 6752 or on the setting screen.
- Incrementing the number of machined parts
Bit 0 (PCM) of parameter No. 6700 is used to specify whether the
number of machined parts is incremented each time M02, M30, or an
M code specified by parameter No. 6710 is executed, or only each
time an M code specified by parameter No. 6710 is executed.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1459 -
12.1.14 Setting the Floating Reference Position (15-inch Display Unit)
To perform floating reference position return with a G30.1 command,
the floating reference position must be set beforehand.
Procedure for setting the floating reference position
Procedure
1 Press function key to display a screen used for displaying
the current position.
2 Move the tool to the floating reference position by jogging.
3 Press horizontal soft key [SET FRP].
4 To register the floating reference positions for all axes, press soft
key [ALL AXIS].
To register the floating reference position of a specific axis, enter
the name of the axis ( , , etc.), then press horizontal soft
key [AXIS NAME]. Two or more names can be entered
consecutively (e.g., ) [AXIS NAME]).
The above operation stores the floating reference position. It can
be checked with parameter (No. 1244).
5 In step 3, the floating reference position along a specified axis
can also be stored by entering the axis name (such as or
) and pressing horizontal soft key [SET FRP].
Explanation
- Presetting the relative coordinate system
When bit 3 (FPC) of parameter No. 1201 is set to 1, the floating
reference position can be registered, while the relative position display
can be preset to 0.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1460 -
12.1.15 Operating Monitor Display (15-inch Display Unit)
The load meter for each servo axis can be displayed. Also, the load
meter and speed meter for a serial spindle can be displayed.
To enable this function, bit 5 (OPM) of parameter No. 3111 must be
set to 1.
Procedure for displaying the operating monitor
Procedure
1 Press function key .
2 Press vertical soft key [MONITOR].
Fig. 12.1.15 (a) Operating monitor (M series) (15-inch)
Fig. 12.1.15 (b) Operating monitor (T series) (15-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1461 -
Explanation
- Display of the servo axes
Servo axis load meters as many as the maximum number of controlled
axes of the path can be displayed. One screen displays load meters for
up to five axes at a time. By pressing the vertical soft key
[MONITOR], load meters for the 6th axis and up are displayed.
- Display of the spindle axes
When serial spindles are used, the reading on the load meter and
speedometer can be displayed only for the main serial spindle.
- Unit of graph
The bar graph for the load meter shows load up to 200% (only a value
is displayed for load exceeding 200%).
The bar graph for the speedometer shows the ratio of the current
spindle speed to the maximum spindle speed (100%).
- Load meter
The reading on the load meter depends on servo parameter No. 2086
and spindle parameter No. 4127.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1462 -
- Speedometer
Although the speedometer normally indicates the speed of the spindle
motor, it can also be used to indicate the speed of the spindle by setting
bit 6 (OPS) of parameter No. 3111 to 1.
The spindle speed to be displayed during operation monitoring is
calculated from the speed of the spindle motor (see the formula below).
The spindle speed can therefore be displayed, during operation
monitoring, even when no position coder is used.
To display the correct spindle speed, however, the maximum spindle
speed for each gear (spindle speed at each gear ratio when the spindle
motor rotates at the maximum speed) must be set in parameters No.
3741 to No.3744.
The input of the clutch and gear signals for the first serial spindle is
used to determine the gear which is currently selected. Control the
input of the CTH1A and CTH2A signals according to the gear
selection, by referring to the table below.
(Formula for calculating the spindle speed to be displayed)
Maximum spindle speed
with the gear being used
Maximum speed of
spindle motor
Speed of spindle motor
Spindle speed displayed
during operation monitoring =×
The following table lists the correspondence between clutch and gear
selection signals CTH1A and CTH2A, used to determine the gear
being used, and parameters:
CTH1A CTH2A Parameter Serial spindle
spec
ification
0 0
=No.3741 (Maximum spindle speed
with gear 1) HIGH
0 1
=No.3742 (Maximum spindle speed
with gear 2) MEDIUM HIGH
1 0
=No.3743 (Maximum spindle speed
with gear 3) MEDIUM LOW
1 1
=No.3744 (Maximum spindle speed
with gear 4) LOW
The speed of the spindle motor and spindle can be displayed, during
operation monitoring, only for the first serial spindle and the spindle
switching axis for the first serial spindle. It cannot be displayed for the
second spindle.
- Color of graph
If the value of a load meter exceeds 100%, the bar graph turns red.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1463 -
12.1.16 Display of Three-dimensional Manual Feed (Tool Tip
Coordinates, Number of Pulses, Machine Axis Move Amount)
(15-inch Display Unit)
The absolute coordinates of the tool tip, the number of pulses, and a
machine axis move amount based on three-dimensional manual feed
are displayed.
Displaying the screen for three-dimensional manual feed
Procedure
1 Press function key .
2 Press the vertical soft key [3-D MANUAL] to display the screen
of three-dimensional manual feed.
Fig. 12.1.16 (a) Three-dimensional manual feed screen(15-inch)
Explanation
- Tool tip position
The addresses of the three basic machine configuration axes for
performing three-dimensional manual feed and the current position of
the tool tip are displayed.
- Tool axis reference (number of pulses)
TD
The amount of travel in the tool axis direction in tool axis
direction handle feed, tool axis direction jog feed, or tool axis
direction incremental feed is displayed.
The unit is the least input increment of the axis in the direction
specified by parameter No. 19697.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1464 -
R1
The amount of travel in the first axis direction in tool axis
right-angle direction handle feed, tool axis right-angle direction
jog feed, or tool axis right-angle direction incremental feed is
displayed.
The unit is the least input increment of the axis in the first axis
direction normal to the direction specified by parameter No.
19697.
R2
The amount of travel in the second axis direction in tool axis
right-angle direction handle feed, tool axis right-angle direction
jog feed, or tool axis normal direction incremental feed is
displayed.
The unit is the least input increment of the axis in the second axis
direction normal to the direction specified by parameter No.
19697.
- Tool tip center (number of pulses)
C1
The angular displacement in tool tip center rotation handle feed,
tool tip center rotation jog feed, or tool tip center rotation
incremental feed for rotation of the first rotary axis is displayed.
The unit is the least input increment of the first rotary axis. For
the definition of the first rotary axis, see the description of
parameter No. 19680.
C2
The angular displacement in tool tip center rotation handle feed,
tool tip center rotation jog feed, or tool tip center rotation
incremental feed for rotation of the second rotary axis is
displayed. The unit is the least input increment of the second
rotary axis. For the definition of the second rotary axis, see the
description of parameter No. 19680.
- Table reference (number of pulses)
VR
The amount of travel in the table reference vertical direction in
table reference vertical direction handle feed, table reference
vertical direction jog feed, or table reference vertical direction
incremental feed is displayed.
The unit is the least input increment of the axis in the direction
specified by parameter No. 19697.
H1
The amount of travel in the first axis direction in table reference
horizontal direction handle feed, table reference horizontal
direction jog feed, or table reference horizontal direction
incremental feed is displayed.
The unit is the least input increment of the axis in the first axis
direction normal to the direction specified by parameter No.
19697.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1465 -
H2
The amount of travel in the second axis direction in table
reference horizontal direction handle feed, table reference
horizontal direction jog feed, or table reference horizontal
direction incremental feed is displayed.
The unit is the least input increment of the axis in the second axis
direction normal to the direction specified by parameter No.
19697.
- Amounts of machine axis travel
The addresses of machine configuration axes used for
three-dimensional manual feed and the sum of the amount of travel of
each axis used for three-dimensional manual feed are displayed.
The values of the basic three axes (X-axis, Y-axis, and Z-axis), the
first rotary axis, and the second rotary axis are displayed in this order.
For the definition of the first rotary axis and second rotary axis, see
the description of parameter No. 19680.
When bit 0 (CLR) of parameter No. 13113 is set to 1, the displayed
data is cleared by a reset.
- Absolute coordinates, machine coordinates
The absolute coordinates and machine coordinates of all axes are
displayed. If too many axes are involved for display on one screen, the
remaining axes can be displayed by pressing the vertical soft key [3-D
MANUAL] for page feed.
- F (feedrate)
• When bit 3 (CFD) of parameter No. 13113 is set to 0
The composite feedrate at a control point on a linear axis or
rotary axis is displayed.
• When bit 3 (CFD) of parameter No. 13113 is set to 1
The feedrate of the tool tip is displayed.
Operation
The display of the number of pulses can be cleared to 0 with
horizontal soft keys.
1 Select the horizontal soft key corresponding to a function for
which the display of the amount of travel is to be cleared.
2 Press horizontal soft key [ERASE] to clear the display of the
amount of travel of the specified function, or press horizontal soft
key [CAN] to cancel the operation.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1466 -
12.2 SCREENS DISPLAYED BY FUNCTION KEY
Section 12.2, "SCREENS DISPLAYED BY FUNCTION KEY
", consists of the following subsections:
――――― Screens of a 7.2/8.4/10.4-inch display unit
12.2.1 Program Contents Display .................................................1467
12.2.2 Editing a Program ..............................................................1470
12.2.3 Program Screen for MDI Operation...................................1472
12.2.4 Program Folder Screen.......................................................1473
12.2.5 Next Block Display Screen ................................................1481
12.2.6 Program Check Screen.......................................................1482
12.2.7 Background Editing ...........................................................1483
12.2.8 Stamping the Machining Time...........................................1489
12.2.9 Screen for Assistance in Entering Tilted Working Plane
Command...........................................................................1499
――――― Screens of a 15-inch display unit
12.2.10 Program Contents Display (15-inch Display Unit)............1521
12.2.11 Editing a Program (15-inch Display Unit).........................1522
12.2.12 Program Screen for MDI Operation (15-Inch Display
Unit) ...................................................................................1524
12.2.13 Program Folder Screen (15-inch Display Unit) .................1525
12.2.14 Next Block Display Screen (15-inch Display Unit)...........1532
12.2.15 Program Check Screen (15-inch Display Unit) .................1533
12.2.16 Background Editing (15-inch Display Unit)......................1534
12.2.17 Stamping the Machining Time (15-inch Display Unit) .....1540
12.2.18 Screen for Assistance in Entering Tilted Working Plane
Command (15-inch Display Unit)......................................1550
Screens of a 7.2/8.4/10.4-inch display unit
This section describes the screens displayed by pressing function key
. The screens include a program editing screen, program folder
list display screen, and screens for displaying the command states of
the program currently being executed.
1. Program screen
2. Program folder screen
3. Next block display screen
4. Program check screen
On the program screen, you edit the program that is currently selected,
and display the block that is currently executed during program
operation. In MDI mode, you also edit an MDI operation program,
and display the block that is currently executed.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1467 -
12.2.1 Program Contents Display
Displays the program currently being executed in MEMORY mode.
Displaying the program being executed
Procedure
1 Press function key to display the program screen.
2 Press chapter selection soft key [PROGRAM].
The cursor is positioned at the block currently being executed.
Fig. 12.2.1 (a) Screen for displaying the program being executed
(10.4-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1468 -
12.2.1.1 Displaying the executed block
Overview
When the program being executed is displayed, one executed block
can be displayed. This function can be enabled by setting bit 3 (FPD)
of parameter No. 11308.
The program screen shows the following:
• Executed block
• Block being executed
• Look-ahead block(*)
• Non-look-ahead block
(*) For details on look-ahead, see the explanation "Program
look-ahead" below.
The executed block is displayed on the top of the screen, and ">" is
shown in front of the block being executed, across which the cursor is
placed. Below the block being executed, look-ahead blocks are
displayed. Below them, non-look-ahead blocks are displayed.
There is a dividing line between the look-ahead blocks and the
non-look-ahead blocks.
Fig. 12.2.1.1 (b) Screen for displaying the program being executed (MDI
mode)
Look-ahead block
Executed block
Block being executed
Non-look-ahead
block
Dividing line
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1469 -
Fig. 12.2.1.1 (c) Screen for displaying the program being executed (MEM
mode)
Explanation
- Program look-ahead
When an automatic operation cycle starts, a program is executed as
described below.
<1> The command of one block is read from the specified program.
<2> The read command is analyzed and converted to executable data.
<3> The command of the block is executed.
During execution of the command, steps <1> and <2> are performed
for the next block in advance. Upon completion of the current block,
execution of the next block can be started immediately. This
processing is referred to as look-ahead or buffering.
The number of look-ahead blocks depends on the processing status or
parameters.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1470 -
12.2.2 Editing a Program
A program can be edited in the EDIT mode.
Two modes of editing are available. One mode is word editing, which
performs word-by-word editing. The other is character editing, which
performs character-by-character editing.
For program creation and editing operation, see Chapter III-9,
“CREATING PROGRAMS” and Chapter III-10, “EDITING
PROGRAMS”.
Displaying the program editing screen
Procedure
1 Press function key to display the program screen.
2 Press chapter selection soft key [PROGRAM].
- Word editing
Editing operations such as text insertion, modification, and deletion,
and cursor movements are performed on a word-by-word basis.
Fig. 12.2.2 (a) Program word editing screen (10.4-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1471 -
- Character editing
Program editing operations and cursor movements are performed on a
character-by-character basis as with a general text editor.
Text is input directly to the cursor position instead of using the key
input buffer.
Fig. 12.2.2 (b) Program character editing screen (10.4-inch)
Switching between program editing modes
You can switch between word editing and character editing with soft
keys.
Procedure
1 Press function key to display the program screen.
2 Press chapter selection soft key [PROGRAM].
3 Press operation soft key [(OPRT)].
4 Pressing operation soft key [CHANGE EDITOR] switches the
editing mode between word editing and character editing.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1472 -
12.2.3 Program Screen for MDI Operation
During MDI operation or editing of an MDI operation program in the
MDI mode, the program currently being executed mode is displayed.
For MDI operation, see Section III-4.2, “MDI Operation”.
Procedure for displaying the program screen for MDI operation
Procedure
1 Press function key .
2 Press chapter selection soft key [PROGRAM].
The program input from the MDI is displayed.
Fig. 12.2.3 (a) MDI operation program screen (10.4-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1473 -
12.2.4 Program Folder Screen
A list of programs registered in the program memory is displayed.
For the program folder screen, see Chapter III-11, “PROGRAM
MANAGEMENT”.
Displaying the program folder screen
Procedure
1 Press function key .
2 Press chapter selection soft key [FOLDER].
Fig. 12.2.4 (a) Program folder screen (10.4-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1474 -
12.2.4.1 Split display on the program folder screen
Overview
On the program folder screen, the folder information display can be
split into two folder information views, upper and lower, as shown in
the figure below. This function is enabled by setting bit 1 (MLD) of
parameter No. 11318 to 1.
Fig. 12.2.4.1 (a) Program folder screen (split-display screen)(10.4-inch)
On the split folder display, file information about different sets of
devices or folders can be shown in different views at the same time, so
you can copy or move files easily.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1475 -
Example of copying a file from the CNC MEM to the Data Server
Procedure
<1> Change to a destination folder on the Data Server.
<2> Change to a folder on the CNC_MEM that contains a file you
want to copy.
<3> Select the file.
<4> Copy the file.
<2>
<1>
<3> <4>
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1476 -
Procedure for switching to split display
Procedure
1 Press function key to display the program folder screen.
2 Press soft key [(OPRT)].
3 Press continuous menu key twice.
Soft key [MULTI LIST] appears.
Fig. 12.2.4.1 (b) Program folder screen (normal screen)(10.4-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1477 -
4 Press soft key [MULTI LIST].
The folder information display is split into two folder views,
upper and lower, which show the same folder information.
Immediately after the splitting, the upper folder view becomes
active for operations. At the same time, soft key [SINGLE LIST]
appears.
Fig. 12.2.4.1 (c) Program folder screen (split-display screen)(10.4-inch)
5 Pressing soft key [SINGLE LIST] takes you back to the original
program folder display.
Then, the folders are shown which have been selected in the
active view for operations on the split display.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1478 -
Procedure for switching between active folder views for file operations on the split
display
On the split folder display, you can switch between active folder
views for file operations as described below.
In the active folder view for file operations, the cursor is displayed on
the file list.
Procedure
1 When the upper folder view is active for file operations and you
press MDI key and cursor key , the lower folder
view becomes active for file operations.
2 When the lower folder view is active for file operations and you
press MDI key and cursor key , the upper folder
view becomes active for file operations.
NOTE
1 In step 1, even if you press MDI key and
cursor key when the upper folder view is
active for file operations, the lower folder view
becomes active for file operations.
2 In step 2, even if you press MDI key and
cursor key when the lower folder view is
active for file operations, the upper folder view
becomes active for file operations.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1479 -
Explanation
- File operations on the split display
The following operations are allowed on the split display.
<1> You can select and display devices or folders individually in each
folder view.
<2> You can copy or move files between folders selected in different
folder views.
(For details, see the section on operations of copying/moving
between devices.)
In the selected folder view, you can perform the same operations as on
the normal screen.
- Path switching
When path switching is performed while the split display is provided
for a multi-path system, the folder view in which the CNC MEM is
selected as a device is changed to a view of the last selected folder for
each path on the CNC MEM.
- Device information display
The device information as shown in the normal program folder screen
(portion in a dotted box in the figure below) is not shown on the split
display (Fig. 12.2.4.1 (c)).
Fig. 12.2.4.1 (d) Program folder screen (normal screen)(10.4-inch)
You should see the device information on the normal screen.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1480 -
Limitation
- Device that can be selected in both views at the same time on the split display
The same device of any of the following types can be selected in both
views at the same time on the split display.
• CNC MEM
• MEM CARD(binary format)
• Data Server
For other types, the same device cannot be selected for display in the
folder views at the same time.
If any other type of device is selected when split display starts, the
upper and lower folder views cannot show the same sets of folders due
to the above limitation. Therefore, the lower folder view shows the
folder selected as a foreground folder.
- Display units that support the split display
The split display is supported on 10.4-inch and 15-inch display units.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1481 -
12.2.5 Next Block Display Screen
Displays the block currently being executed and the block to be
executed next.
Procedure for displaying the next block display screen
Procedure
1 Press function key .
2 Press chapter selection soft key [NEXT].
The G codes, addresses, command values specified in the block
currently being executed and the next block are displayed.
Fig. 12.2.5 (a) Next block display screen (10.4-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1482 -
12.2.6 Program Check Screen
Displays the program currently being executed, current position of the
tool, and modal data.
Procedure for displaying the program check screen
Procedure
1 Press function key .
2 Press chapter selection soft key [CHECK].
The program currently being executed, current position of the
tool, and modal data are displayed.
Fig. 12.2.6 (a) Program check screen (10.4-inch)
Explanation
- Program display
The program currently being executed is displayed.
The block being executed is displayed in reverse video.
- Current position display
The current position in the relative coordinate system, workpiece
coordinate system, and machine coordinate system, and the remaining
amount of travel are displayed.
- Modal G codes
Up to 24 modal G codes are displayed.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1483 -
12.2.7 Background Editing
Editing one program during execution of another program is referred
to as background editing. You can perform the same edit operations
in the background as those in normal editing (foreground editing).
On a 10.4-inch or 15-inch display, you can perform background
editing for the programs displayed in multiple tiled windows. You can
switch from a program displayed in one of the tiled windows to
another to perform copy, paste, and other edit operations, which
allows you to edit programs efficiently.
You can edit two programs simultaneously on a 10.4-inch display or
four programs on a 15-inch display.
Function
- Background editing
A program other than the currently selected program can be edited.
Background editing can be performed in any mode.
- Program selected in the foreground
If the program selected in the foreground is specified as a program to
be edited in the background, background editing is started in the
read-only mode. The text at an arbitrary position of the program
currently being executed can be checked.
- Switching from the program directory screen to the editing screen
By selecting a program from the program folder screen, background
editing can be started.
On the program folder screen, move the cursor to a program to be
edited in the background, then press the MDI key . The screen
display switches to the background editing screen.
Background editing can be started without entering a program name.
- Background editing on a multi-path system
Background editing does not depend on the path.
Even if the path to be operated is changed using the path selection
signal, the background editing currently being executed is just
continued.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1484 -
Display
When background editing starts, the ordinary program editing screen
switches to the background editing screen.
When two or more programs are edited in the background, the screen
is split to display these programs. For a 10.4-inch display, you can edit
two programs simultaneously; for a 15-inch display, you can edit four
programs simultaneously.
- Word editing
Fig. 12.2.7 (a) shows background word editing performed
simultaneously for two programs (right and left programs). On the
status line at the top of the window for each program, the program
name and “BG-EDIT” (indicating background editing in progress) are
displayed.
The status line of the program being edited is displayed in reverse
video.
Fig. 12.2.7 (a) Background editing screen (word editing) (10.4-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1485 -
- Character editing
Fig. 12.2.7 (b) shows background character editing performed
simultaneously for two programs (right and left programs). Similarly
to word editing, at the top of the window for each program, the status
line is displayed. In addition, the current input mode (INSERT
MODE or OVERWRITE MODE) is displayed at the upper right of
the screen for character editing.
The status line of the program being edited is displayed in reverse
video.
Fig. 12.2.7 (b) Background editing screen (character editing) (10.4-inch)
- Editing status
The following items are displayed on the status line and program
editing area according to the background editing status.
Editing status Displayed items
No program
selected
(BG-EDIT)
“NO PROGRAM” is displayed in the editing area.
Program opened program-name + (BG-EDIT)
Read-only program
opened
program-name + (BG:READ ONLY)
The contents of the program are displayed in green.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1486 -
Starting background editing from the editing screen
Procedure
Method 1
1 Press function key .
2 Press soft key [PROGRAM].
3 Press soft key [(OPRT)], then soft key [BG EDIT].
4 Press soft key [PROGRM SEARCH] to select a program to be
edited.
Method 2 (only for word editing)
1 Press function key .
2 Press soft key [PROGRAM].
3 Key in the name of a program to be edited in the background.
4 Press soft key [BG EDIT].
When background editing has already started and editing start
operation is performed again, the program being edited and newly
specified program are edited simultaneously.
Explanation
When a program name is input in the key-in buffer, background
editing for the program starts. When the specified program is not
found, a new program is created and background editing starts.
When background editing is started with no program name specified,
new background editing starts in the no program state. Perform a
program search or create a new program.
When character editing is selected, background editing starts in the no
program state first. Perform a program search or create a new
program.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1487 -
Starting background editing from the program folder screen
By selecting a program from the program folder screen, background
editing can be started. The cursor is used to select a program. You do
not need to enter a program name.
Procedure
1 Press function key .
2 Press soft key [FOLDER].
3 Move the cursor to a program to be edited.
4 Press the MDI key . The screen display is switched to the
background editing screen.
Background editing operation
- Editing operation
The same editing operations as performed in the foreground can be
performed.
- Switching from a program to another for editing
To switch from a program to another for editing when editing multiple
programs simultaneously in the background, press key, then
or .
- Editing operation in the read-only mode
Cursor movement and page switching are possible. However,
program editing is disabled.
- Copying and pasting text between programs
Text in a program selected and copied during program editing is kept
held after the program to be edited is changed. You can paste text in
a program onto another program.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1488 -
Background editing end operation
Background editing can be ended using the procedure described
below.
The procedure for ending background editing of one program and that
for ending all background editing of multiple programs are shown
below.
- Ending editing of one program
1 Press function key .
2 Press soft key [PROGRAM].
3 Select a program for which to end editing.
4 Press soft key [(OPRT)], then soft key [BG END].
- Ending editing of all programs
1 Press function key .
2 Press soft key [PROGRAM].
3 Press soft key [(OPRT)], then soft key [BG ALL END].
To return to ordinary foreground editing, end all background editing.
If at least one program is being edited in the background, you cannot
return to foreground editing.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1489 -
12.2.8 Stamping the Machining Time
The execution times of the most recently executed ten programs can
be displayed in hours, minutes, and seconds.
The calculated machining time can be inserted as a comment of the
program to check the machining time on the program folder screen.
Procedure for stamping the machining time
Procedure
- Displaying the machining time
1 Press function key .
2 Press the continuous menu key several times to display soft
key [TIME].
3 Press soft key [TIME]. The machining time display screen
appears.
Fig. 12.2.8 (a) Machining time display screen (10.4-inch)
- Calculating the machining time
1 Select the memory operation mode, then press the key.
2 Select the program screen, then select a program of which
machining time you want to calculate.
3 Execute the program to perform actual machining.
4 When the key is pressed or, M02 or M30 is executed, the
machining time count operation stops. When the machining
time display screen is selected, the program number of the
stopped main program and its machining time are displayed.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1490 -
5 The following figure shows the screen when the machining times
of the ten main programs O0020, O0040, …, and O0200 are
displayed and the screen when the machining time of O0220 is
newly calculated after that.
Fig. 12.2.8 (b) Stamping the machining time (10.4-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1491 -
Procedure for inserting the machining time on the program screen
Procedure
You can display the machining time of a program as a comment of the
program. The procedure is shown below:
1 To insert the calculated machining time of a program as a
comment, the machining time of the program must be displayed
on the machining time display screen. Before stamping the
machining time of the program, check that the program number
is displayed on the machining time display screen.
2 Set the edit mode or background editing state and select the
program screen. Then, select a program of which machining time
you want to insert.
3 Suppose that the machining time of O0100 is displayed on the
machining time display screen.
Press soft key [(OPRT)] to display the operation soft keys.
Then, press the continuous menu key several times to
display soft key [INSERT TIME]. Press soft key [INSERT
TIME]. The beginning of the program is displayed and the
machining time of the program is inserted after the program
name.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1492 -
Press soft key [INSERT TIME].
Fig. 12.2.8 (c) Program screen (10.4-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1493 -
4 If a comment is written in the block containing the program
number of a program of which machining time is to be inserted,
the machining time is inserted after the comment.
Press soft key [INSERT TIME].
Fig. 12.2.8 (d) Program screen (10.4-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1494 -
Display on the program folder screen
The machining time of a program inserted in the program as a
comment is displayed after the existing comment of the program on
the program folder screen.
Fig. 12.2.8 (e) Program folder screen (10.4-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1495 -
Explanation
- Machining time
The machining time is counted from the initial start after a reset in the
memory operation mode to the next reset. If a reset is not performed
during operation, the machining time is counted from the start to M02
or M30. The time during which operation is held is not counted, but
the time used to wait for the completion of the M, S, T, and/or B
functions is counted, however.
- Stamping the machining time
You can insert (stamp) the displayed machining time in a program
stored in memory as a comment. The machining time is inserted as a
comment after the program number.
- Program folder
You can display the machining time inserted after a program number
on the program folder screen. This operation lets you know the
machining time of each program to use the time as useful reference
data when planning processes on site.
Limitation
- Alarm
The execution of a program may be held by an alarm during the
machining time count operation. In this case, the machining time is
counted until the alarm is released by a reset.
- M02
It may be specified that M02 does not reset the CNC, but returns
completion signal FIN to the CNC to restart the program from the
beginning successively (bit 5 (M02) of parameter No. 3404 is set to 0).
In this case, when M02 returns completion signal FIN, the machining
time count operation stops.
- Stamping the machining time
When an attempt is made to stamp the machining time of a program in
the program, the machining time of the program may not be displayed
on the machining time display screen. In this case, the machining time
cannot be inserted in the program even if soft key [INSERT TIME] is
pressed.
- Correcting the machining time
If an incorrect machining time is calculated (such as when a reset is
made during the execution of a program), reexecute the program to
calculate the correct machining time. The same program number may
be displayed in two or more lines on the machining time display
screen. In this case, the latest calculated machining time is inserted in
the program.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1496 -
- States of the stamped machining time
In the following states, the stamped machining time is displayed on
the program folder screen as shown below.
1 When the comment of a program is longer than 16 characters
The 17th and subsequent characters of the comment are discarded
and the machining time display field is left blank.
Fig. 12.2.8 (f) 1. When the comment of a program is longer than 16
characters (10.4-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1497 -
2 When two or more machining times are stamped
The first machining time is displayed.
Fig. 12.2.8 (g) When two or more machining times are stamped
(10.4-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1498 -
3 When the format of an inserted machining time is not
“hhhHmmMssS” (H following a 3-digit number, M following a
2-digit number, and S following a 2-digit number, in this order)
The machining time display field is left blank.
Fig. 12.2.8 (h) When the format of an inserted machining time is not
“hhhHmmMssS” (H following a 3-digit number, M following a 2-digit
number, and S following a 2-digit number, in this order) (10.4-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1499 -
12.2.9 Screen for Assistance in Entering Tilted Working Plane
Command
The screens for assistance in entering tilted working plane commands
(hereinafter referred to as guidance screens) include a command type
selection screen and a tilted working plane data setting screen. The
command type selection screen is used to select a tilted working plane
command. The tilted working plane data setting screen is used to set
specified tilted working plane data required for the selected command.
By making settings and performing operations on these guidance
screens, a tilted working plane command block can be created.
The created block is reflected as a new insertion to a program being
edited or as a modification to an existing block.
This function can be enabled by setting bit 1 (GGD) of parameter No.
11304 to 1.
Creation of a new block
The following describes the procedure for creating a tilted working
plane command block on guidance screens and for inserting the block
to a program being edited on a program editing screen.
1 On a program editing screen, display a program to which you
want to insert a tilted working plane command block.
The foreground editing screen, background editing screen, or
MDI editing screen should be displayed.
• Displaying the foreground editing screen
<1> Select the EDIT mode.
<2> Press function key .
<3> Press soft key [PROGRAM].
• Displaying the background editing screen
<1> Press function key .
<2> Press soft key [FOLDER].
<3> Press any of the cursor keys to move the cursor to a
program to be edited in the background.
<4> Press key.
• Displaying the MDI editing screen
<1> Select the MDI mode.
<2> Press function key .
<3> Press soft key [PROGRAM].
The program editing screen is displayed.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1500 -
2 Press any of the cursor keys to move the cursor to a position
where you want to insert a block.
Note that a block created on the guidance screens is inserted after
the block at the cursor position. (If the block at the cursor
position includes a tilted working plane command, the existing
block is modified. See "Modification to an existing block"
below.)
3 Press soft key [(OPRT)].
4 Press continuous menu key several times, and then press
soft key [GUIDANCE].
The command type selection screen is displayed.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1501 -
5 Select a command type with any of the cursor keys, and then
press soft key [SELECT].
The tilted working plane data setting screen is displayed.
6 Enter command data for the setting items.
7 Press soft key [INSERT].
8 Press soft key [YES].
This takes you back to the program editing screen, where the new
block is inserted after the block at the cursor position.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1502 -
Modification to an existing block
The following describes the procedure for replacing a block in a
program being edited on a program editing screen, with a tilted
working plane command block created on a guidance screen.
1 On a program editing screen, display a program to be edited.
(For the procedure for displaying a program editing screen, see
step 1 in "Creation of a new block".)
The program editing screen is displayed.
2 Press any of the cursor keys to move the cursor to a block to be
modified.
For a command extending over more than one block, move the
cursor to the first block.
3 Press soft key [(OPRT)].
4 Press continuous menu key several times, and then press
soft key [GUIDANCE TWP]. The tilted working plane data
setting screen is displayed.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1503 -
5 Enter command data for setting items to be modified.
6 Press soft key [ALTER].
7 Press soft key [YES].
This takes you back to the program editing screen, where the
block at the cursor position is replaced.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1504 -
Guidance screen cancellation
Pressing soft key [CANCEL] on a guidance screen takes you back to
the program editing screen. At this time, the data that has been set on
the guidance screen is discarded.
NOTE
1 In addition to the above operation, the following
operations also cancel a guidance screen. The
data that has been set on the guidance screen is
discarded.
• When bit 7 (CPG) of parameter No. 11302 is 1
(setting for automatically switching between
program-related screens according to CNC
mode), the CNC mode is changed.
• When a guidance screen is displayed from the
foreground editing screen, the CNC mode is
changed to a mode other than EDIT, TJOG, or
THND.
• When a guidance screen is displayed from the
MDI editing screen, the CNC mode is changed
to a mode other than MDI.
• When a guidance screen is displayed on a
15-inch display unit, the screen is switched by
a vertical soft key.
• The screen is switched by an MDI key.
• The screen is switched by a path select signal.
• An event that causes screen switching has
occurred, including occurrence of an alarm,
display of an operator message, or
signal-based display of a screen (such as a
tool compensation screen, workpiece shift
screen, workpiece coordinate system setting
screen, or C language executor screen).
2 If MDI key is pressed after switching from a
guidance screen to another screen, a program
editing screen is displayed, instead of the guidance
screen.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1505 -
Notes
• Conditions under which soft key [GUIDANCE TWP] is
displayed
Soft key [GUIDANCE TWP] is displayed on a program editing
screen under the following conditions:
1 Foreground editing screen
- The CNC mode is EDIT, TJOG, or THND.
- The editing and display are not prohibited for a
program to be edited.
2 Background editing screen
- A program to be edited is not in reference mode.
- The editing and display are not prohibited for a
program to be edited.
3 MDI editing screen
- The CNC mode is MDI.
• Screen displayed when soft key [GUIDANCE TWP] is pressed
When soft key [GUIDANCE TWP] is pressed, which guidance
screen is displayed is automatically determined according to the
conditions described below.
1 When a tilted working plane command is not included in a
block at the cursor position on a program editing screen
The command type selection screen is displayed. A
block created on the guidance screens is inserted after
the block at the cursor position on the program editing
screen.
2 When a tilted working plane command is included in a
block at the cursor position on a program editing screen
The tilted working plane data setting screen is
displayed, which shows the data for the tilted working
plane command in the block at the cursor position on
the program editing screen. When a block of a tool
axis direction control command exists immediately
after the tilted working plane command, the command
data for the block is also shown. The tilted working
plane command in the block at the cursor position on
the program editing screen is replaced with a block
created on the guidance screen.
NOTE
If the CNC is in the reset state or emergency stop
state when soft key [GUIDANCE TWP] is pressed
on the foreground editing screen or MDI editing
screen, the warning "PROGRAM READ FAILED"
appears, and the operation cannot be continued.
(Soft keys other than [CANCEL] are not displayed.)
Press soft key [CANCEL] to return to the program
editing screen, and then press soft key
[GUIDANCE TWP] again.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1506 -
12.2.9.1 Command type selection screen
The command type selection screen is used to select the type of a
tilted working plane command you want to insert into a program to be
edited. One of the following command types can be selected:
• G68.2 / G68.4 (Euler’s angle)
• G68.2 / G68.4 P1 (Roll-Pitch-Yaw angle)
• G68.2 / G68.4 P2 (3 points specification)
• G68.2 / G68.4 P3 (2 vectors specification)
• G68.2 / G68.4 P4 (Projection angle)
• G68.3 (Tool Axis Direction)
G68.2 is an absolute command, and G68.4 is an incremental
command.
Fig. 12.2.9.1 (a) Command type selection screen (10.4-inch)
Selection of a command type
1 Press cursor key or to move the cursor to a
command type you want to select. As the cursor is moved, the
figure corresponding to the command type at the cursor position
is displayed.
2 When soft key [SELECT] is pressed, the command type at the
cursor position is accepted, and the tilted working plane data
setting screen is displayed.
NOTE
If the warning "PROGRAM READ FAILED"
appears when the command type selection screen
is displayed, the operation cannot be continued.
(Soft keys other than [CANCEL] are not displayed.)
Press soft key [CANCEL] to return to the program
editing screen, and then press soft key
[GUIDANCE TWP] again.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1507 -
12.2.9.2 Tilted working plane data setting screen
The tilted working plane data setting screen is used to set specified
tilted working plane data required for a tilted working plane command
of the type that has been selected on the command type selection
screen or has been selected when soft key [GUIDANCE TWP] is
pressed.
Different types of tilted working plane data setting screen are provided
for different command types. For details of each type of tilted working
plane data setting screen, see "Details of the tilted working plane data
setting screen".
Fig. 12.2.9.2 (a) Tilted working plane data setting screen－3 points
specification(10.4-inch)
Display of the tilted working plane data setting screen
When a new block is created, the initial values are set in the setting
and selection items.
When an existing block is modified, the command data for the block
at the cursor position on the program editing screen is reflected in the
setting and selection items.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1508 -
NOTE
1 For existing block modification, if the guidance
screen is displayed when the cursor is placed in
the middle of multiple blocks for a command, the
parameters for the block(s) before the cursor are
not reflected in the setting and selection items, but
only the parameters for the block(s) after the
cursor are reflected. If no data is to be reflected in
a setting or selection item, the initial value is set in
the item.
2 For existing block modification, only the commands
with parameter-specified axis names are reflected
in the setting items on the screen. (The values
specified in data for commands with incorrect axis
names are not reflected in the setting items.)
Command data input
• Item for which to enter a value
Press cursor key or to move the cursor to an item
you want to set.
Enter a value, and then press the key or soft key [INPUT].
Example)
When the origin of a feature coordinate system is set as
shown above, addresses X, Y, and Z are specified as
follows:
G68.2 X0.001 Y0.01 Z1000 ...
For two items "Tool Offset Number" and "From TCP to center",
the state with no command can be set by deleting the specified
values according to the following procedure.
1 Press cursor key or to move the cursor to the
item "Tool Offset Number" or "From TCP to Center".
2 Press or soft key [INPUT] without entering
anything.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1509 -
• Item to be selected from a list
1 Press cursor key or to move the cursor to an
item you want to set.
2 Press cursor key or to move the cursor to an
item you want to select.
Example)
Order of rotation for Roll-Pitch Yaw angle
Insertion of a block
If the guidance screen is displayed when the block at the cursor
position on the program editing screen does not include a tilted
working plane command, soft key [INSERT] is displayed on the tilted
working plane data setting screen. An operation for inserting a tilted
working plane command block is described below.
For warnings that may be issued at the time of block insertion, see
"Limitation".
1 Press soft key [INSERT].
The confirmation message "ARE YOU SURE YOU WANT TO
EXECUTE?" is displayed, and soft keys [YES] and [NO] are
displayed.
2 Press soft key [YES].
A block is created from the command type and command data
and then is inserted after the block at the cursor position in the
program to be edited. After block insertion, the guidance screen
is closed and the program editing screen is displayed.
Pressing soft key [NO] takes you back to the tilted working plane
data setting screen.
Example)
G00 X0.; When the guidance screen is displayed and
the 3-point specification is selected as a
command type for block insertion, a created
block is inserted after the block at the cursor
position.
G00 X0.;
G68.2 P2 Q0...
G68.2 P2 Q1...
G68.2 P2 Q2...
G68.2 P2 Q3...
↓
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1510 -
Replacement of a block
If the guidance screen is displayed when the block at the cursor
position on the program editing screen includes a tilted working plane
command, soft key [ALTER] is displayed on the tilted working plane
data setting screen. An operation for replacing a tilted working plane
command block is described below.
For warnings that may be issued at the time of block replacement, see
"Limitation".
1 Press soft key [ALTER].
The confirmation message "ARE YOU SURE YOU WANT TO
EXECUTE?" is displayed, and soft keys [YES] and [NO] are
displayed.
2 Press soft key [YES].
A block is created from the command type and command data
and then replaces the tilted working plane command in the block
at the cursor position on the program editing screen. After block
replacement, the guidance screen is closed and the program
editing screen is displayed.
Pressing soft key [NO] takes you back to the tilted working plane
data setting screen.
NOTE
1 If a block to be replaced includes a command other
than a tilted working plane command, the
command is deleted during block replacement.
However, only the sequence number at the
beginning is preserved.
2 If the guidance screen is displayed when the cursor
is placed in the middle of multiple blocks for a
command, the block(s) before the cursor are not
replaced. These blocks remain unchanged after
replacement.
3 If soft key [GUIDANCE TWP] is pressed when the
cursor is placed on a block of a tool axis direction
control command, the command type selection
screen is displayed in new insertion mode. A block
created on the guidance screens is inserted after
the block of the tool axis direction control
command.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1511 -
Limitation
The following lists the warnings that may be issued at the time of
block insertion or replacement.
If a warning is displayed, return to the program editing screen with
soft key [CANCEL] and press soft key [GUIDANCE TWP] again, or
eliminate the cause of the warning and retry the operation.
Warning Description
“PROGRAM WRITE
FAILED”
• The guidance screen was displayed from the foreground
editing screen or MDI editing screen, and a block insertion
or replacement operation was performed when the CNC
was in the reset state or emergency stop state.
”PROGRAM
CANNOT BE
WRITTEN”
• A block insertion or replacement operation was performed
after a program to be edited was updated due to program
downloading by an external application while the guidance
screen was displayed.
• A block insertion or replacement operation was performed
after the start of the main program was located by a reset
while the guidance screen was displayed.
“WRITE PROTECT” • A block insertion or replacement operation was performed
when the editing or display was prohibited for a program to
be edited.
• A block insertion or replacement operation was performed
when the memory protection signal (KEY signal) for
program registration or editing was off.
• A block insertion or replacement operation was performed
when the operation level of the 8-level data protection
function was lower than the protection level of a part
program editing operation.
Display of the command type selection screen
When soft key [COMMAND TYPE] is pressed, the command type
selection screen is displayed. When the command type is changed on
the command type selection screen, the values set on the tilted
working plane data setting screen are cleared.
When a tilted working plane command is included in the block at the
cursor position on the program editing screen, you can display the
guidance screen, change the command type on the command type
selection screen, and then perform block replacement. In this case, the
block at the cursor position on the program editing screen is replaced
with a block created from the command type and command data that
have been set.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1512 -
12.2.9.3 Details of the tilted working plane data setting screen
The following six tilted working plane commands are supported.
For details of the commands, see II-22.3, "TILTED WORKING
PLANE COMMANDS".
• G68.2 / G68.4 (Euler’s angle)
• G68.2 / G68.4 P1 (Roll-Pitch-Yaw angle)
• G68.2 / G68.4 P2 (3 points specification)
• G68.2 / G68.4 P3 (2 vectors specification)
• G68.2 / G68.4 P4 (Projection angle)
• G68.3 (Tool Axis Direction)
G68.2 is an absolute command, and G68.4 is an incremental
command.
G68.2 / G68.4(Euler’s angle)
Fig. 12.2.9.3 (a) Tilted working plane data setting screen-Euler’s
angle(10.4-inch)
• Multi Type
Absolute:
It is assumed that values of specified data are in a workpiece
coordinate system, regardless of whether tilted working
plane command mode is set.
Incremental:
It is assumed that values of specified data are in a feature
coordinate system if tilted working plane command mode is
already set.
• Origin of Feature Coordinate
Specify the origin (X, Y, and Z of point P) of a feature
coordinate system as coordinates in a workpiece coordinate
system (for the absolute type) or the current feature coordinate
system (for the incremental type).
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1513 -
• Euler’s angle
I : Specify an angle of rotation around the Z-axis of a
workpiece coordinate system (for the absolute type) or the
current feature coordinate system (for the incremental type).
This rotation determines coordinate system 1 (X1-Y1-Z1)
from the workpiece coordinate system (for the absolute
type) or the current feature coordinate system (for the
incremental type) (X-Y-Z).
J : Specify an angle of rotation around the X-axis of coordinate
system 1.
This rotation determines coordinate system 2 (X2-Y2-Z2)
from coordinate system 1 (X1-Y1-Z1).
K : Specify an angle of rotation around the Z-axis of coordinate
system 2.
After this rotation, a feature coordinate system is obtained
by shifting the origin of the workpiece coordinate system by
the coordinates specified in "Origin of Feature Coordinate".
G68.2 / G68.4(Roll-Pitch-Yaw angle)
Fig. 12.2.9.3 (b) Tilted working plane data setting screen- Roll-Pitch-Yaw
angle(10.4-inch)
• Multi Type
Absolute:
It is assumed that values of specified data are in a workpiece
coordinate system, regardless of whether tilted working
plane command mode is set.
Incremental:
It is assumed that values of specified data are in a feature
coordinate system if tilted working plane command mode is
already set.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1514 -
• Order of Rotation
Select an order in which the X-axis, Y-axis, and Z-axis are
rotated in a workpiece coordinate system (for the absolute type)
or the current feature coordinate system (for the incremental
type). The selectable rotation orders are as follows:
1st rotation
axis
2nd rotation
axis
3rd rotation
axis
X→Y→Z X-axis Y-axis Z-axis
X→Z→Y X-axis Z-axis Y-axis
Y→X→Z Y-axis X-axis Z-axis
Y→Z→X Y-axis Z-axis X-axis
Z→X→Y Z-axis X-axis Y-axis
Z→Y→X Z-axis Y-axis X-axis
• Origin of Feature Coordinate
Specify the origin (X, Y, and Z of point P) of a feature
coordinate system as coordinates in a workpiece coordinate
system (for the absolute type) or the current feature coordinate
system (for the incremental type).
• Rotation Angle about X-axis
Specify an angle of rotation around the X-axis of a workpiece
coordinate system (for the absolute type) or the current feature
coordinate system (for the incremental type).
• Rotation Angle about Y-axis
Specify an angle of rotation around the Y-axis of a workpiece
coordinate system (for the absolute type) or the current feature
coordinate system (for the incremental type).
• Rotation Angle about Z-axis
Specify an angle of rotation around the Z-axis of a workpiece
coordinate system (for the absolute type) or the current feature
coordinate system (for the incremental type).
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1515 -
G68.2 / G68.4(3 points specification)
Fig. 12.2.9.3 (c) Tilted working plane data setting screen- 3 points
specification(10.4-inch)
• Multi Type
Absolute:
It is assumed that values of specified data are in a workpiece
coordinate system, regardless of whether tilted working
plane command mode is set.
Incremental:
It is assumed that values of specified data are in a feature
coordinate system if tilted working plane command mode is
already set.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1516 -
• Shift of the Origin
Specify, in a feature coordinate system, an amount of shift from
the feature coordinate system origin specified for the 1st point
(point P1).
• Rotation Angle about the Z-axis in F-Coordinate
Specify an angle of rotation around the Z-axis of a feature
coordinate system. The direction of rotation angle R is positive
when a rotation is made clockwise as viewed in the Z-axis
direction of the feature coordinate system.
• 1st point (Origin of Feature Coordinate)
Specify the origin (X, Y, and Z of point P1) of a feature
coordinate system as coordinates in a workpiece coordinate
system (for the absolute type) or the current feature coordinate
system (for the incremental type).
• 2nd point
Specify the coordinates (X, Y, and Z of point P2) of the 2nd
point as coordinates in a workpiece coordinate system (for the
absolute type) or the current feature coordinate system (for the
incremental type). The 1st point and 2nd point determine the
X-axis of the feature coordinate system.
• 3rd point
Specify the coordinates (X, Y, and Z of point P3) of the 3rd point
as coordinates in a workpiece coordinate system (for the absolute
type) or the current feature coordinate system (for the
incremental type). Among the directions normal to the X-axis, a
direction with a smaller angle relative to the P1 → P3 vector is
the Y-axis of the feature coordinate system.
G68.2 / G68.4(2 vectors specification)
Fig. 12.2.9.3 (d) Tilted working plane data setting screen-2 vectors
specification(10.4-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1517 -
• Multi Type
Absolute:
It is assumed that values of specified data are in a workpiece
coordinate system, regardless of whether tilted working
plane command mode is set.
Incremental:
It is assumed that values of specified data are in a feature
coordinate system if tilted working plane command mode is
already set.
• Origin of Feature Coordinate
Specify the origin (X, Y, and Z of point P) of a feature
coordinate system as coordinates in a workpiece coordinate
system (for the absolute type) or the current feature coordinate
system (for the incremental type).
• V1 (X’) vector
Specify the X-axis direction vector of a feature coordinate
system as values in a workpiece coordinate system (for the
absolute type) or the current feature coordinate system (for the
incremental type).
• V2 (Z’) vector
Specify the Z-axis direction vector of a feature coordinate system
as values in a workpiece coordinate system (for the absolute
type) or the current feature coordinate system (for the
incremental type).
G68.2 / G68.4(Projection angle)
Fig. 12.2.9.3 (e) Tilted working plane data setting screen-Projection
angle(10.4-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1518 -
• Multi Type
Absolute:
It is assumed that values of specified data are in a workpiece
coordinate system, regardless of whether tilted working
plane command mode is set.
Incremental:
It is assumed that values of specified data are in a feature
coordinate system if tilted working plane command mode is
already set.
• Origin of Feature Coordinate
Specify the origin (X, Y, and Z of point P) of a feature
coordinate system as coordinates in a workpiece coordinate
system (for the absolute type) or the current feature coordinate
system (for the incremental type).
• Projection angle
I : Specify a projection angle relative to the X-axis of a
workpiece coordinate system (for the absolute type) or the
current feature coordinate system (for the incremental type).
J : Specify a projection angle relative to the Y-axis of a
workpiece coordinate system (for the absolute type) or the
current feature coordinate system (for the incremental type).
K : Specify an angle of rotation around the Z-axis of a feature
coordinate system.
G68.3(Tool Axis Direction)
Fig. 12.2.9.3 (f) Tilted working plane data setting screen-Tool Axis
Direction(10.4-inch)
(When "No" is selected in "Origin command of Feature Coordinate")
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1519 -
Fig. 12.2.9.3 (g) Tilted working plane data setting screen-Tool Axis
Direction(10.4-inch)
(When "Yes" is selected in "Origin command of Feature Coordinate")
• Origin command of Feature Coordinate
Select whether to specify a feature coordinate system origin.
Yes : A feature coordinate system origin is specified.
No : A feature coordinate system origin is not specified.
• Origin of Feature Coordinate
Specify the origin (X, Y, and Z of point P) of a feature
coordinate system as coordinates in a workpiece coordinate
system.
This setting cannot be made if "No" is selected in "Origin
command of Feature Coordinate".
• Rotation Angle about the Z-axis in F-Coordinate
Specify an angle of rotation around the Z-axis of a feature
coordinate system. The direction of rotation angle R is positive
when a rotation is made clockwise as viewed in the Z-axis
direction of the feature coordinate system.
12.2.9.4 Limitation
This function is supported on 10.4-inch and 15-inch display units.
This function is not displayed on 7.2-inch and 8.4-inch display units.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1520 -
Screens of a 15-inch display unit
This section describes the screens displayed by pressing function key
. The screens include a program editing screen, program folder
list display screen, and screens for displaying the command states of
the program currently being executed.
1. Program screen
2. Program folder screen
3. Next block display screen
4. Program check screen
On the program screen, you edit the program that is currently selected,
and display the block that is currently executed during program
operation. In MDI mode, you also edit an MDI operation program,
and display the block that is currently executed.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1521 -
12.2.10 Program Contents Display (15-inch Display Unit)
Displays the program currently being executed in MEMORY mode.
Displaying the program being executed
Procedure
1 Press function key to display the program screen.
2 Press vertical soft key [PROGRAM].
The cursor is positioned at the block currently being executed.
Fig. 12.2.10 (a) Screen for displaying the program being executed
(15-inch)
12.2.10.1 Displaying the executed block
For an explanation of how to display the executed block, see
Subsection 12.2.1.1, "Displaying the executed block".
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1522 -
12.2.11 Editing a Program (15-inch Display Unit)
A program can be edited in the EDIT mode.
Two modes of editing are available. One mode is word editing, which
performs word-by-word editing. The other is character editing, which
performs character-by-character editing.
For program creation and editing operation, see Chapter III-9,
“CREATING PROGRAMS “ and Chapter III-10, “EDITING
PROGRAMS”.
Displaying the program editing screen
Procedure
1 Press function key to display the program screen.
2 Press vertical soft key [PROGRAM].
- Word editing
Editing operations such as text insertion, modification, and deletion,
and cursor movements are performed on a word-by-word basis.
Fig. 12.2.11 (a) Program word editing screen (15-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1523 -
- Character editing
Program editing operations and cursor movements are performed on a
character-by-character basis as with a general text editor.
Text is input directly to the cursor position instead of using the key
input buffer.
Fig. 12.2.11 (b) Program character editing screen (15-inch)
Switching between program editing modes
You can switch between word editing and character editing with
horizontal soft keys.
Procedure
1 Press function key to display the program screen.
2 Press vertical soft key [PROGRAM].
3 Press continuous menu key to display horizontal soft key
[CHANGE EDITOR].
4 Pressing horizontal soft key [CHANGE EDITOR] switches the
editing mode between word editing and character editing.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1524 -
12.2.12 Program Screen for MDI Operation (15-inch Display Unit)
During MDI operation or editing of an MDI operation program in the
MDI mode, the program currently being executed mode is displayed.
For MDI operation, see Section III-4.2, “MDI Operation”.
Procedure for displaying the program screen for MDI operation
Procedure
1 Press function key .
2 Press vertical soft key [PROGRAM].
The program input from the MDI is displayed.
Fig. 12.2.12 (a) MDI operation program screen (15-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1525 -
12.2.13 Program Folder Screen (15-inch Display Unit)
A list of programs registered in the program memory is displayed.
For the program folder screen, see Chapter III-11, “PROGRAM
MANAGEMENT”.
Displaying the program folder screen
Procedure
1 Press function key .
2 Press vertical soft key [FOLDER].
Fig. 12.2.13 (a) Program folder screen (15-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1526 -
12.2.13.1 Split display on the program folder screen
Overview
On the program folder screen, the folder information display can be
split into two folder information views, upper and lower, as shown in
the figure below.
Fig. 12.2.13.1 (a) Program folder screen (split-display screen)(15-inch)
On the split folder display, file information about different sets of
devices or folders can be shown in different views at the same time, so
you can copy or move files easily.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1527 -
Example of copying a file from the CNC MEM to the Data Server
Procedure
<1> Change to a destination folder on the Data Server.
<2> Change to a folder on the CNC_MEM that contains a file you
want to copy.
<3> Select the file.
<4> Copy the file.
<3> <4>
<2>
<1>
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1528 -
Procedure for switching to split display
Procedure
1 Press function key to display the program folder screen.
2 Press horizontal soft key [(OPRT)].
3 Press continuous menu key twice.
Horizontal soft key [MULTI LIST] appears.
Fig. 12.2.13.1 (b) Program folder screen normal screen)(15-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1529 -
4 Press horizontal soft key [MULTI LIST].
The folder information display is split into two folder views,
upper and lower, which show the same folder information.
Immediately after the splitting, the upper folder view becomes
active for operations. At the same time, horizontal soft key
[SINGLE LIST] appears.
Fig. 12.2.13.1 (c) Program folder screen (split-display screen)(15-inch)
5 Pressing horizontal soft key [SINGLE LIST] takes you back to
the original program folder display.
Then, the folders are shown which have been selected in the
active view for operations on the split display.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1530 -
Procedure for switching between active folder views for file operations on the split
display
On the split folder display, you can switch between active folder
views for file operations as described below.
In the active folder view for file operations, the cursor is displayed on
the file list.
Procedure
1 When the upper folder view is active for file operations and you
press MDI key and cursor key , the lower folder
view becomes active for file operations.
2 When the lower folder view is active for file operations and you
press MDI key and cursor key , the upper folder
view becomes active for file operations.
NOTE
1 In step 1, even if you press MDI key and
cursor key when the upper folder view is
active for file operations, the lower folder view
becomes active for file operations.
2 In step 2, even if you press MDI key and
cursor key when the lower folder view is
active for file operations, the upper folder view
becomes active for file operations.
Explanation
- File operations on the split display
The following operations are allowed on the split display.
<1> You can select and display devices or folders individually in each
folder view.
<2> You can copy or move files between folders selected in different
folder views.
(For details, see the section on operations of copying/moving
between devices.)
In the selected folder view, you can perform the same operations as on
the normal screen.
- Path switching
When path switching is performed while the split display is provided
for a multi-path system, the folder view in which the CNC MEM is
selected as a device is changed to a view of the last selected folder for
each path on the CNC MEM.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1531 -
- Device information display
The device information as shown in the normal program folder screen
(portion in a dotted box in the figure below) is not shown on the split
display (Fig. 12.2.13.1 (c)).
Fig. 12.2.13.1 (d) Program folder screen (normal screen)(15-inch)
You should see the device information on the normal screen.
Limitation
- Device that can be selected in both views at the same time on the split display
The same device of any of the following types can be selected in both
views at the same time on the split display.
• CNC MEM
• MEM CARD(binary format)
• Data Server
For other types, the same device cannot be selected for display in the
folder views at the same time.
If any other type of device is selected when split display starts, the
upper and lower folder views cannot show the same sets of folders due
to the above limitation. Therefore, the lower folder view shows the
folder selected as a foreground folder.
- Display units that support the split display
The split display is supported on 10.4-inch and 15-inch display units.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1532 -
12.2.14 Next Block Display Screen (15-inch Display Unit)
Displays the block currently being executed and the block to be
executed next.
Procedure for displaying the next block display screen
Procedure
1 Press function key .
2 Press vertical soft key [NEXT].
The G codes, addresses, command values specified in the block
currently being executed and the next block are displayed.
Fig. 12.2.14 (a) Next block display screen (15-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1533 -
12.2.15 Program Check Screen (15-inch Display Unit)
Displays the program currently being executed, current position of the
tool, and modal data.
Procedure for displaying the program check screen
Procedure
1 Press function key .
2 Press vertical soft key [CHECK].
The program currently being executed, current position of the
tool, and modal data are displayed.
Fig. 12.2.15 (a) Program check screen (15-inch)
Explanation
- Program display
The program currently being executed is displayed.
The block being executed is displayed in reverse video.
- Current position display
The current position in the relative coordinate system, workpiece
coordinate system, and machine coordinate system, and the remaining
amount of travel are displayed.
- Modal G codes
Up to 24 modal G codes are displayed.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1534 -
12.2.16 Background Editing (15-inch Display Unit)
Editing one program during execution of another program is referred
to as background editing. You can perform the same edit operations
in the background as those in normal editing (foreground editing).
On a 10.4-inch or 15-inch display, you can perform background
editing for the programs displayed in multiple tiled windows. You can
switch from a program displayed in one of the tiled windows to
another to perform copy, paste, and other edit operations, which
allows you to edit programs efficiently.
You can edit two programs simultaneously on a 10.4-inch display or
four programs on a 15-inch display.
Function
- Background editing
A program other than the currently selected program can be edited.
Background editing can be performed in any mode.
- Program selected in the foreground
If the program selected in the foreground is specified as a program to
be edited in the background, background editing is started in the
read-only mode. The text at an arbitrary position of the program
currently being executed can be checked.
- Switching from the program directory screen to the editing screen
By selecting a program from the program folder screen, background
editing can be started.
On the program folder screen, move the cursor to a program to be
edited in the background, then press the MDI key . The screen
display switches to the background editing screen.
Background editing can be started without entering a program name.
- Background editing on a multi-path system
Background editing does not depend on the path.
Even if the path to be operated is changed using the path selection
signal, the background editing currently being executed is just
continued.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1535 -
Display
When background editing starts, the ordinary program editing screen
switches to the background editing screen.
When two or more programs are edited in the background, the screen
is split to display these programs. For a 10.4-inch display, you can edit
two programs simultaneously; for a 15-inch display, you can edit four
programs simultaneously.
- Word editing
Fig. 12.2.16 (a) shows background word editing performed
simultaneously for two programs (right and left programs). On the
status line at the top of the window for each program, the program
name and “BG-EDIT” (indicating background editing in progress) are
displayed.
The status line of the program being edited is displayed in reverse
video.
Fig. 12.2.16 (a) Background editing screen (word editing) (15-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1536 -
- Character editing
Fig. 12.2.16 (b) shows background character editing performed
simultaneously for two programs (right and left programs). Similarly
to word editing, at the top of the window for each program, the status
line is displayed. In addition, the current input mode (INSERT
MODE or OVERWRITE MODE) is displayed at the upper right of
the screen for character editing.
The status line of the program being edited is displayed in reverse
video.
Fig. 12.2.16 (b) Background editing screen (character editing) (15-inch)
- Editing status
The following items are displayed on the status line and program
editing area according to the background editing status.
Editing status Displayed items
No program
selected
(BG-EDIT)
“NO PROGRAM” is displayed in the editing area.
Program opened program-name + (BG-EDIT)
Read-only program
opened
program-name + (BG:READ ONLY)
The contents of the program are displayed in green.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1537 -
Starting background editing from the editing screen
Procedure
Method (only for word editing)
1 Press function key .
2 Press vertical soft key [PROGRAM].
3 Key in the name of a program to be edited in the background.
4 Press horizontal soft key [BG EDIT].
When background editing has already started and editing start
operation is performed again, the program being edited and newly
specified program are edited simultaneously.
Explanation
When a program name is input in the key-in buffer, background
editing for the program starts. When the specified program is not
found, a new program is created and background editing starts.
When background editing is started with no program name specified,
new background editing starts in the no program state. Perform a
program search or create a new program.
When character editing is selected, background editing starts in the no
program state first. Perform a program search or create a new
program.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1538 -
Starting background editing from the program folder screen
By selecting a program from the program folder screen, background
editing can be started. The cursor is used to select a program. You do
not need to enter a program name.
Procedure
1 Press function key .
2 Press vertical soft key [FOLDER].
3 Move the cursor to a program to be edited.
4 Press the MDI key . The screen display is switched to the
background editing screen.
Background editing operation
- Editing operation
The same editing operations as performed in the foreground can be
performed.
- Switching from a program to another for editing
To switch from a program to another for editing when editing multiple
programs simultaneously in the background, press key, then
or .
- Editing operation in the read-only mode
Cursor movement and page switching are possible. However,
program editing is disabled.
- Copying and pasting text between programs
Text in a program selected and copied during program editing is kept
held after the program to be edited is changed. You can paste text in
a program onto another program.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1539 -
Background editing end operation
Background editing can be ended using the procedure described
below.
The procedure for ending background editing of one program and that
for ending all background editing of multiple programs are shown
below.
- Ending editing of one program
1 Press function key .
2 Press vertical soft key [PROGRAM].
3 Select a program for which to end editing.
4 Press horizontal soft key [BG END].
- Ending editing of all programs
1 Press function key .
2 Press vertical soft key [PROGRAM].
3 Press horizontal soft key [BG ALL END].
To return to ordinary foreground editing, end all background editing.
If at least one program is being edited in the background, you cannot
return to foreground editing.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1540 -
12.2.17 Stamping the Machining Time (15-inch Display Unit)
The execution times of the most recently executed ten programs can
be displayed in hours, minutes, and seconds.
The calculated machining time can be inserted as a comment of the
program to check the machining time on the program folder screen.
Procedure for stamping the machining time
Procedure
- Displaying the machining time
1 Press function key .
2 Press vertical soft key [TIME]. The machining time display
screen appears.
Fig. 12.2.17 (a) Machining time display screen (15-inch)
- Calculating the machining time
1 Select the memory operation mode, then press the key.
2 Select the program screen, then select a program of which
machining time you want to calculate.
3 Execute the program to perform actual machining.
4 When the key is pressed or, M02 or M30 is executed, the
machining time count operation stops. When the machining
time display screen is selected, the program number of the
stopped main program and its machining time are displayed.
5 The following figure shows the screen when the machining times
of the ten main programs O0020, O0040, …, and O0200 are
displayed and the screen when the machining time of O0220 is
newly calculated after that.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1541 -
Fig. 12.2.17 (b) Stamping the machining time (15-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1542 -
Procedure for inserting the machining time on the program screen
Procedure
You can display the machining time of a program as a comment of the
program. The procedure is shown below:
1 To insert the calculated machining time of a program as a
comment, the machining time of the program must be displayed
on the machining time display screen. Before stamping the
machining time of the program, check that the program number
is displayed on the machining time display screen.
2 Set the edit mode or background editing state and select the
program screen. Then, select a program of which machining time
you want to insert.
3 For example, the machining time of O0100 is displayed on the
machining time display screen. Press continuous menu key
until horizontal soft key [INSERT TIME] appears. When
horizontal soft key [INSERT TIME] is pressed, the start of the
program is located, and the machining time of the program is
inserted after the program name.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1543 -
Press soft key [INSERT TIME].
Fig. 12.2.17 (c) Program screen (15-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1544 -
4 If a comment is written in the block containing the program
number of a program of which machining time is to be inserted,
the machining time is inserted after the comment.
Press soft key [INSERT TIME].
Fig. 12.2.17 (d) Program screen (15-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1545 -
Display on the program folder screen
The machining time of a program inserted in the program as a
comment is displayed after the existing comment of the program on
the program folder screen.
Fig. 12.2.17 (e) Program folder screen (15-inch)
Explanation
- Machining time
The machining time is counted from the initial start after a reset in the
memory operation mode to the next reset. If a reset is not performed
during operation, the machining time is counted from the start to M02
or M30. The time during which operation is held is not counted, but
the time used to wait for the completion of the M, S, T, and/or B
functions is counted, however.
- Stamping the machining time
You can insert (stamp) the displayed machining time in a program
stored in memory as a comment. The machining time is inserted as a
comment after the program number.
- Program folder
You can display the machining time inserted after a program number
on the program folder screen. This operation lets you know the
machining time of each program to use the time as useful reference
data when planning processes on site.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1546 -
Limitation
- Alarm
The execution of a program may be held by an alarm during the
machining time count operation. In this case, the machining time is
counted until the alarm is released by a reset.
- M02
It may be specified that M02 does not reset the CNC, but returns
completion signal FIN to the CNC to restart the program from the
beginning successively (bit 5 (M02) of parameter No. 3404 is set to 0).
In this case, when M02 returns completion signal FIN, the machining
time count operation stops.
- Stamping the machining time
When an attempt is made to stamp the machining time of a program in
the program, the machining time of the program may not be displayed
on the machining time display screen. In this case, the machining time
cannot be inserted in the program even if horizontal soft key [INSERT
TIME] is pressed.
- Correcting the machining time
If an incorrect machining time is calculated (such as when a reset is
made during the execution of a program), reexecute the program to
calculate the correct machining time. The same program number may
be displayed in two or more lines on the machining time display
screen. In this case, the latest calculated machining time is inserted in
the program.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1547 -
- States of the stamped machining time
In the following states, the stamped machining time is displayed on
the program folder screen as shown below.
1 When the comment of a program is longer than 16 characters
The 17th and subsequent characters of the comment are discarded
and the machining time display field is left blank.
Fig. 12.2.17 (f) When the comment of a program is longer than 16
characters (15-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1548 -
2 When two or more machining times are stamped
The first machining time is displayed.
Fig. 12.2.17 (g) When two or more machining times are stamped
(15-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1549 -
3 When the format of an inserted machining time is not
“hhhHmmMssS” (H following a 3-digit number, M following a
2-digit number, and S following a 2-digit number, in this order)
The machining time display field is left blank.
Fig. 12.2.17 (h) When the format of an inserted machining time is not
“hhhHmmMssS” (H following a 3-digit number, M following a 2-digit
number, and S following a 2-digit number, in this order) (15-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1550 -
12.2.18 Screen for Assistance in Entering Tilted Working Plane
Command (15-inch Display Unit)
The screens for assistance in entering tilted working plane commands
(hereinafter referred to as guidance screens) include a command type
selection screen and a tilted working plane data setting screen. The
command type selection screen is used to select a tilted working plane
command. The tilted working plane data setting screen is used to set
specified tilted working plane data required for the selected command.
By making settings and performing operations on these guidance
screens, a tilted working plane command block can be created.
The created block is reflected as a new insertion to a program being
edited or as a modification to an existing block.
This function can be enabled by setting bit 1 (GGD) of parameter No.
11304 to 1.
Creation of a new block
The following describes the procedure for creating a tilted working
plane command block on guidance screens and for inserting the block
to a program being edited on a program editing screen.
1 On a program editing screen, display a program to which you
want to insert a tilted working plane command block.
The foreground editing screen, background editing screen, or
MDI editing screen should be displayed.
• Displaying the foreground editing screen
<1> Select the EDIT mode.
<2> Press function key .
<3> Press vertical soft key [PROGRAM].
• Displaying the background editing screen
<1> Press function key .
<2> Press soft key [FOLDER].
<3> Press any of the cursor keys to move the cursor to a
program to be edited in the background.
<4> Press key.
• Displaying the MDI editing screen
<1> Select the MDI mode.
<2> Press function key .
<3> Press vertical soft key [PROGRAM].
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1551 -
The program editing screen is displayed.
2 Press any of the cursor keys to move the cursor to a position
where you want to insert a block.
Note that a block created on the guidance screens is inserted after
the block at the cursor position. (If the block at the cursor
position includes a tilted working plane command, the existing
block is modified. See "Modification to an existing block"
below.)
3 Press continuous menu key several times, and then press
horizontal soft key [GUIDANCE TWP].
The command type selection screen is displayed.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1552 -
4 Select a command type with any of the cursor keys, and then
press horizontal soft key [SELECT].
The tilted working plane data setting screen is displayed.
5 Enter command data for the setting items.
6 Press horizontal soft key [INSERT].
7 Press horizontal soft key [YES].
This takes you back to the program editing screen, where the new
block is inserted after the block at the cursor position.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1553 -
Modification to an existing block
The following describes the procedure for replacing a block in a
program being edited on a program editing screen, with a tilted
working plane command block created on a guidance screen.
1 On a program editing screen, display a program to be edited.
(For the procedure for displaying a program editing screen, see
step 1 in "Creation of a new block".)
The program editing screen is displayed.
2 Press any of the cursor keys to move the cursor to a block to be
modified.
For a command extending over more than one block, move the
cursor to the first block.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1554 -
3 Press continuous menu key several times, and then press
horizontal soft key [GUIDANCE TWP]. The tilted working
plane data setting screen is displayed.
4 Enter command data for setting items to be modified.
5 Press horizontal soft key [ALTER].
6 Press horizontal soft key [YES].
This takes you back to the program editing screen, where the
block at the cursor position is replaced.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1555 -
Guidance screen cancellation
Pressing horizontal soft key [CANCEL] on a guidance screen takes
you back to the program editing screen. At this time, the data that has
been set on the guidance screen is discarded.
NOTE
1 In addition to the above operation, the following
operations also cancel a guidance screen. The
data that has been set on the guidance screen is
discarded.
• When bit 7 (CPG) of parameter No. 11302 is 1
(setting for automatically switching between
program-related screens according to CNC
mode), the CNC mode is changed.
• When a guidance screen is displayed from the
foreground editing screen, the CNC mode is
changed to a mode other than EDIT, TJOG, or
THND.
• When a guidance screen is displayed from the
MDI editing screen, the CNC mode is changed
to a mode other than MDI.
• When a guidance screen is displayed on a
15-inch display unit, the screen is switched by
a vertical soft key.
• The screen is switched by an MDI key.
• The screen is switched by a path select signal.
• An event that causes screen switching has
occurred, including occurrence of an alarm,
display of an operator message, or
signal-based display of a screen (such as a
tool compensation screen, workpiece shift
screen, workpiece coordinate system setting
screen, or C language executor screen).
2 If MDI key is pressed after switching from a
guidance screen to another screen, a program
editing screen is displayed, instead of the guidance
screen.
Notes
• Conditions under which horizontal soft key [GUIDANCE TWP]
is displayed
Horizontal soft key [GUIDANCE TWP] is displayed on a
program editing screen under the following conditions:
1 Foreground editing screen
- The CNC mode is EDIT, TJOG, or THND.
- The editing and display are not prohibited for a
program to be edited.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1556 -
2 Background editing screen
- A program to be edited is not in reference mode.
- The editing and display are not prohibited for a
program to be edited.
3 MDI editing screen
- The CNC mode is MDI.
• Screen displayed when horizontal soft key [GUIDANCE TWP]
is pressed
When horizontal soft key [GUIDANCE TWP] is pressed, which
guidance screen is displayed is automatically determined
according to the conditions described below.
1 When a tilted working plane command is not included in a
block at the cursor position on a program editing screen
The command type selection screen is displayed. A
block created on the guidance screens is inserted after
the block at the cursor position on the program editing
screen.
2 When a tilted working plane command is included in a
block at the cursor position on a program editing screen
The tilted working plane data setting screen is
displayed, which shows the data for the tilted working
plane command in the block at the cursor position on
the program editing screen. When a block of a tool
axis direction control command exists immediately
after the tilted working plane command, the command
data for the block is also shown. The tilted working
plane command in the block at the cursor position on
the program editing screen is replaced with a block
created on the guidance screen.
NOTE
If the CNC is in the reset state or emergency stop
state when horizontal soft key [GUIDANCE TWP]
is pressed on the foreground editing screen or MDI
editing screen, the warning "PROGRAM READ
FAILED" appears, and the operation cannot be
continued. (Horizontal soft keys other than
[CANCEL] are not displayed.) Press horizontal soft
key [CANCEL] to return to the program editing
screen, and then press horizontal soft key
[GUIDANCE TWP] again.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1557 -
12.2.18.1 Command type selection screen
The command type selection screen is used to select the type of a
tilted working plane command you want to insert into a program to be
edited. One of the following command types can be selected:
• G68.2 / G68.4 (Euler’s angle)
• G68.2 / G68.4 P1 (Roll-Pitch-Yaw angle)
• G68.2 / G68.4 P2 (3 points specification)
• G68.2 / G68.4 P3 (2 vectors specification)
• G68.2 / G68.4 P4 (Projection angle)
• G68.3 (Tool Axis Direction)
G68.2 is an absolute command, and G68.4 is an incremental
command.
Fig. 12.2.18.1 (a) Command type selection screen (15-inch)
Selection of a command type
1 Press cursor key or to move the cursor to a
command type you want to select. As the cursor is moved, the
figure corresponding to the command type at the cursor position
is displayed.
2 When horizontal soft key [SELECT] is pressed, the command
type at the cursor position is accepted, and the tilted working
plane data setting screen is displayed.
NOTE
If the warning "PROGRAM READ FAILED"
appears when the command type selection screen
is displayed, the operation cannot be continued.
(Horizontal soft keys other than [CANCEL] are not
displayed.) Press horizontal soft key [CANCEL] to
return to the program editing screen, and then
press horizontal soft key [GUIDANCE TWP] again.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1558 -
12.2.18.2 Tilted working plane data setting screen
The tilted working plane data setting screen is used to set specified
tilted working plane data required for a tilted working plane command
of the type that has been selected on the command type selection
screen or has been selected when horizontal soft key [GUIDANCE
TWP] is pressed.
Different types of tilted working plane data setting screen are provided
for different command types. For details of each type of tilted working
plane data setting screen, see "Details of the tilted working plane data
setting screen".
Fig. 12.2.18.2 (a) Tilted working plane data setting screen－3 points
specification(15-inch)
Display of the tilted working plane data setting screen
When a new block is created, the initial values are set in the setting
and selection items.
When an existing block is modified, the command data for the block
at the cursor position on the program editing screen is reflected in the
setting and selection items.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1559 -
NOTE
1 For existing block modification, if the guidance
screen is displayed when the cursor is placed in
the middle of multiple blocks for a command, the
parameters for the block(s) before the cursor are
not reflected in the setting and selection items, but
only the parameters for the block(s) after the
cursor are reflected. If no data is to be reflected in
a setting or selection item, the initial value is set in
the item.
2 For existing block modification, only the commands
with parameter-specified axis names are reflected
in the setting items on the screen. (The values
specified in data for commands with incorrect axis
names are not reflected in the setting items.)
Command data input
• Item for which to enter a value
Press cursor key or to move the cursor to an item
you want to set.
Enter a value, and then press the key or horizontal soft
key [INPUT].
Example)
When the origin of a feature coordinate system is set as
shown above, addresses X, Y, and Z are specified as
follows:
G68.2 X0.001 Y0.01 Z1000 ...
For two items "Tool Offset Number" and "From TCP to center",
the state with no command can be set by deleting the specified
values according to the following procedure.
1 Press cursor key or to move the cursor to the
item "Tool Offset Number" or "From TCP to Center".
2 Press or horizontal soft key [INPUT] without
entering anything.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1560 -
↓
• Item to be selected from a list
1 Press cursor key or to move the cursor to an
item you want to set.
2 Press cursor key or to move the cursor to an
item you want to select.
Example)
Order of rotation for Roll-Pitch Yaw angle
Insertion of a block
If the guidance screen is displayed when the block at the cursor
position on the program editing screen does not include a tilted
working plane command, horizontal soft key [INSERT] is displayed
on the tilted working plane data setting screen. An operation for
inserting a tilted working plane command block is described below.
For warnings that may be issued at the time of block insertion, see
"Limitation".
1 Press horizontal soft key [INSERT].
The confirmation message "ARE YOU SURE YOU WANT TO
EXECUTE?" is displayed, and horizontal soft keys [YES] and
[NO] are displayed.
2 Press horizontal soft key [YES].
A block is created from the command type and command data
and then is inserted after the block at the cursor position in the
program to be edited. After block insertion, the guidance screen
is closed and the program editing screen is displayed.
Pressing horizontal soft key [NO] takes you back to the tilted
working plane data setting screen.
Example)
G00 X0.; When the guidance screen is displayed
and the 3-point specification is selected
as a command type for block insertion, a
created block is inserted after the block
at the cursor position.
G00 X0.;
G68.2 P2 Q0...
G68.2 P2 Q1...
G68.2 P2 Q2...
G68.2 P2 Q3...
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1561 -
Replacement of a block
If the guidance screen is displayed when the block at the cursor
position on the program editing screen includes a tilted working plane
command, horizontal soft key [ALTER] is displayed on the tilted
working plane data setting screen. An operation for replacing a tilted
working plane command block is described below.
For warnings that may be issued at the time of block replacement, see
"Limitation".
1 Press horizontal soft key [ALTER].
The confirmation message "ARE YOU SURE YOU WANT TO
EXECUTE?" is displayed, and horizontal soft keys [YES] and
[NO] are displayed.
2 Press horizontal soft key [YES].
A block is created from the command type and command data
and then replaces the tilted working plane command in the block
at the cursor position on the program editing screen. After block
replacement, the guidance screen is closed and the program
editing screen is displayed.
Pressing horizontal soft key [NO] takes you back to the tilted
working plane data setting screen.
NOTE
1 If a block to be replaced includes a command other
than a tilted working plane command, the
command is deleted during block replacement.
However, only the sequence number at the
beginning is preserved.
2 If the guidance screen is displayed when the cursor
is placed in the middle of multiple blocks for a
command, the block(s) before the cursor are not
replaced. These blocks remain unchanged after
replacement.
3 If horizontal soft key [GUIDANCE TWP] is pressed
when the cursor is placed on a block of a tool axis
direction control command, the command type
selection screen is displayed in new insertion
mode. A block created on the guidance screens is
inserted after the block of the tool axis direction
control command.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1562 -
Limitation
The following lists the warnings that may be issued at the time of
block insertion or replacement.
If a warning is displayed, return to the program editing screen with
horizontal soft key [CANCEL] and press horizontal soft key
[GUIDANCE TWP] again, or eliminate the cause of the warning and
retry the operation.
Warning Description
“PROGRAM WRITE
FAILED”
• The guidance screen was displayed from the foreground
editing screen or MDI editing screen, and a block insertion
or replacement operation was performed when the CNC
was in the reset state or emergency stop state.
”PROGRAM
CANNOT BE
WRITTEN”
• A block insertion or replacement operation was performed
after a program to be edited was updated due to program
downloading by an external application while the guidance
screen was displayed.
• A block insertion or replacement operation was performed
after the start of the main program was located by a reset
while the guidance screen was displayed.
“WRITE PROTECT” • A block insertion or replacement operation was performed
when the editing or display was prohibited for a program to
be edited.
• A block insertion or replacement operation was performed
when the memory protection signal (KEY signal) for
program registration or editing was off.
• A block insertion or replacement operation was performed
when the operation level of the 8-level data protection
function was lower than the protection level of a part
program editing operation.
Display of the command type selection screen
When horizontal soft key [COMMAND TYPE] is pressed, the
command type selection screen is displayed. When the command type
is changed on the command type selection screen, the values set on the
tilted working plane data setting screen are cleared.
When a tilted working plane command is included in the block at the
cursor position on the program editing screen, you can display the
guidance screen, change the command type on the command type
selection screen, and then perform block replacement. In this case, the
block at the cursor position on the program editing screen is replaced
with a block created from the command type and command data that
have been set.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1563 -
12.2.18.3 Details of the tilted working plane data setting screen
The following six tilted working plane commands are supported.
For details of the commands, see II-22.3, "TILTED WORKING
PLANE COMMANDS".
• G68.2 / G68.4 (Euler’s angle)
• G68.2 / G68.4 P1 (Roll-Pitch-Yaw angle)
• G68.2 / G68.4 P2 (3 points specification)
• G68.2 / G68.4 P3 (2 vectors specification)
• G68.2 / G68.4 P4 (Projection angle)
• G68.3 (Tool Axis Direction)
G68.2 is an absolute command, and G68.4 is an incremental
command.
G68.2 / G68.4(Euler’s angle)
Fig. 12.2.18.3 (a) Tilted working plane data setting screen-Euler’s
angle(15-inch)
• Multi Type
Absolute:
It is assumed that values of specified data are in a workpiece
coordinate system, regardless of whether tilted working
plane command mode is set.
Incremental:
It is assumed that values of specified data are in a feature
coordinate system if tilted working plane command mode is
already set.
• Origin of Feature Coordinate
Specify the origin (X, Y, and Z of point P) of a feature
coordinate system as coordinates in a workpiece coordinate
system (for the absolute type) or the current feature coordinate
system (for the incremental type).
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1564 -
• Euler’s angle
I : Specify an angle of rotation around the Z-axis of a
workpiece coordinate system (for the absolute type) or the
current feature coordinate system (for the incremental type).
This rotation determines coordinate system 1 (X1-Y1-Z1)
from the workpiece coordinate system (for the absolute
type) or the current feature coordinate system (for the
incremental type) (X-Y-Z).
J : Specify an angle of rotation around the X-axis of coordinate
system 1.
This rotation determines coordinate system 2 (X2-Y2-Z2)
from coordinate system 1 (X1-Y1-Z1).
K : Specify an angle of rotation around the Z-axis of coordinate
system 2.
After this rotation, a feature coordinate system is obtained
by shifting the origin of the workpiece coordinate system by
the coordinates specified in "Origin of Feature Coordinate".
G68.2 / G68.4(Roll-Pitch-Yaw angle)
Fig. 12.2.18.3 (b) Tilted working plane data setting screen-
Roll-Pitch-Yaw angle(15-inch)
• Multi Type
Absolute:
It is assumed that values of specified data are in a workpiece
coordinate system, regardless of whether tilted working
plane command mode is set.
Incremental:
It is assumed that values of specified data are in a feature
coordinate system if tilted working plane command mode is
already set.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1565 -
• Order of Rotation
Select an order in which the X-axis, Y-axis, and Z-axis are
rotated in a workpiece coordinate system (for the absolute type)
or the current feature coordinate system (for the incremental
type). The selectable rotation orders are as follows:
1st rotation
axis
2nd rotation
axis 3rd rotation axis
X→Y→Z X-axis Y-axis Z-axis
X→Z→Y X-axis Z-axis Y-axis
Y→X→Z Y-axis X-axis Z-axis
Y→Z→X Y-axis Z-axis X-axis
Z→X→Y Z-axis X-axis Y-axis
Z→Y→X Z-axis Y-axis X-axis
• Origin of Feature Coordinate
Specify the origin (X, Y, and Z of point P) of a feature
coordinate system as coordinates in a workpiece coordinate
system (for the absolute type) or the current feature coordinate
system (for the incremental type).
• Rotation Angle about X-axis
Specify an angle of rotation around the X-axis of a workpiece
coordinate system (for the absolute type) or the current feature
coordinate system (for the incremental type).
• Rotation Angle about Y-axis
Specify an angle of rotation around the Y-axis of a workpiece
coordinate system (for the absolute type) or the current feature
coordinate system (for the incremental type).
• Rotation Angle about Z-axis
Specify an angle of rotation around the Z-axis of a workpiece
coordinate system (for the absolute type) or the current feature
coordinate system (for the incremental type).
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1566 -
G68.2 / G68.4(3 points specification)
Fig. 12.2.18.3 (c) Tilted working plane data setting screen- 3 points
specification(15-inch)
• Multi Type
Absolute:
It is assumed that values of specified data are in a workpiece
coordinate system, regardless of whether tilted working
plane command mode is set.
Incremental:
It is assumed that values of specified data are in a feature
coordinate system if tilted working plane command mode is
already set.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1567 -
• Shift of the Origin
Specify, in a feature coordinate system, an amount of shift from
the feature coordinate system origin specified for the 1st point
(point P1).
• Rotation Angle about the Z-axis in F-Coordinate
Specify an angle of rotation around the Z-axis of a feature
coordinate system. The direction of rotation angle R is positive
when a rotation is made clockwise as viewed in the Z-axis
direction of the feature coordinate system.
• 1st point (Origin of Feature Coordinate)
Specify the origin (X, Y, and Z of point P1) of a feature
coordinate system as coordinates in a workpiece coordinate
system (for the absolute type) or the current feature coordinate
system (for the incremental type).
• 2nd point
Specify the coordinates (X, Y, and Z of point P2) of the 2nd
point as coordinates in a workpiece coordinate system (for the
absolute type) or the current feature coordinate system (for the
incremental type). The 1st point and 2nd point determine the
X-axis of the feature coordinate system.
• 3rd point
Specify the coordinates (X, Y, and Z of point P3) of the 3rd point
as coordinates in a workpiece coordinate system (for the absolute
type) or the current feature coordinate system (for the
incremental type). Among the directions normal to the X-axis, a
direction with a smaller angle relative to the P1 → P3 vector is
the Y-axis of the feature coordinate system.
G68.2 / G68.4(2 vectors specification)
Fig. 12.2.18.3 (d) Tilted working plane data setting screen-2 vectors
specification(15-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1568 -
• Multi Type
Absolute:
It is assumed that values of specified data are in a workpiece
coordinate system, regardless of whether tilted working
plane command mode is set.
Incremental:
It is assumed that values of specified data are in a feature
coordinate system if tilted working plane command mode is
already set.
• Origin of Feature Coordinate
Specify the origin (X, Y, and Z of point P) of a feature
coordinate system as coordinates in a workpiece coordinate
system (for the absolute type) or the current feature coordinate
system (for the incremental type).
• V1 (X’) vector
Specify the X-axis direction vector of a feature coordinate
system as values in a workpiece coordinate system (for the
absolute type) or the current feature coordinate system (for the
incremental type).
• V2 (Z’) vector
Specify the Z-axis direction vector of a feature coordinate system
as values in a workpiece coordinate system (for the absolute
type) or the current feature coordinate system (for the
incremental type).
G68.2 / G68.4(Projection angle)
Fig. 12.2.18.3 (e) Tilted working plane data setting screen-Projection
angle(15-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1569 -
• Multi Type
Absolute:
It is assumed that values of specified data are in a workpiece
coordinate system, regardless of whether tilted working
plane command mode is set.
Incremental:
It is assumed that values of specified data are in a feature
coordinate system if tilted working plane command mode is
already set.
• Origin of Feature Coordinate
Specify the origin (X, Y, and Z of point P) of a feature
coordinate system as coordinates in a workpiece coordinate
system (for the absolute type) or the current feature coordinate
system (for the incremental type).
• Projection angle
I : Specify a projection angle relative to the X-axis of a
workpiece coordinate system (for the absolute type) or the
current feature coordinate system (for the incremental type).
J : Specify a projection angle relative to the Y-axis of a
workpiece coordinate system (for the absolute type) or the
current feature coordinate system (for the incremental type).
K : Specify an angle of rotation around the Z-axis of a feature
coordinate system.
G68.3(Tool Axis Direction)
Fig. 12.2.18.3 (f) Tilted working plane data setting screen-Tool Axis
Direction(15-inch)
(When "No" is selected in "Origin command of Feature Coordinate")
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1570 -
Fig. 12.2.18.3 (g) Tilted working plane data setting screen-Tool Axis
Direction(15-inch)
(When "Yes" is selected in "Origin command of Feature Coordinate")
• Origin command of Feature Coordinate
Select whether to specify a feature coordinate system origin.
Yes : A feature coordinate system origin is specified.
No : A feature coordinate system origin is not specified.
• Origin of Feature Coordinate
Specify the origin (X, Y, and Z of point P) of a feature
coordinate system as coordinates in a workpiece coordinate
system.
This setting cannot be made if "No" is selected in "Origin
command of Feature Coordinate".
• Rotation Angle about the Z-axis in F-Coordinate
Specify an angle of rotation around the Z-axis of a feature
coordinate system. The direction of rotation angle R is positive
when a rotation is made clockwise as viewed in the Z-axis
direction of the feature coordinate system.
12.2.18.4 Limitation
This function is supported on 10.4-inch and 15-inch display units.
This function is not displayed on 7.2-inch and 8.4-inch display units.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1571 -
12.3 SCREENS DISPLAYED BY FUNCTION KEY
Section 12.3, “SCREENS DISPLAYED BY FUNCTION KEY
”, consists of the following subsections:
――――― Screens of a 7.2/8.4/10.4-inch display unit
12.3.1 Displaying and Entering Setting Data................................1573
12.3.2 Sequence Number Comparison and Stop...........................1576
12.3.3 Displaying and Setting Run Time, Parts Count, and Time 1578
12.3.4 Displaying and Setting the Workpiece Origin Offset
Value ..................................................................................1581
12.3.5 Direct Input of Workpiece Origin Offset Value Measured 1582
12.3.6 Displaying and Setting Custom Macro Common
Variables ............................................................................1584
12.3.7 Displaying and Setting Real Time Custom Macro Data....1586
12.3.8 Displaying and Setting the Software Operator’s Panel......1588
12.3.9 Setting and Displaying Tool Management Data ................1591
12.3.10 Displaying and Switching the Display Language ..............1612
12.3.11 Protection of Data at Eight Levels .....................................1614
12.3.12 Precision Level Selection...................................................1623
12.3.13 Displaying and Setting Tool Life Management Data ........1625
12.3.14 Displaying and Setting Workpiece Setting Error
Compensation Data............................................................1640
12.3.15 Displaying and Setting Pattern Data Inputs .......................1642
――――― Screens of a 15-inch display unit
12.3.16 Displaying and Entering Setting Data
(15-inch Display Unit) .......................................................1645
12.3.17 Sequence Number Comparison and Stop
(15-inch Display Unit) .......................................................1648
12.3.18 Displaying and Setting Run Time, Parts Count, and Time
(15-inch Display Unit) .......................................................1650
12.3.19 Displaying and Setting the Workpiece Origin Offset
Value (15-inch Display Unit).............................................1653
12.3.20 Direct Input of Workpiece Origin Offset Value Measured
(15-inch Display Unit) .......................................................1655
12.3.21 Displaying and Setting Custom Macro Common
Variables (15-inch Display Unit).......................................1657
12.3.22 Displaying and Setting Real Time Custom Macro Data
(15-inch Display Unit) .......................................................1659
12.3.23 Displaying and Setting the Software Operator’s Panel
(15-inch Display Unit) .......................................................1662
12.3.24 Setting and Displaying Tool Management Data
(15-inch Display Unit) .......................................................1665
12.3.25 Displaying and Switching the Display Language
(15-inch Display Unit) .......................................................1688
12.3.26 Protection of Data at Eight Levels (15-inch Display Unit) 1690
12.3.27 Precision Level Selection (15-inch Display Unit) .............1699
12.3.28 Displaying and Setting Tool Life Management Data
(15-inch Display Unit) .......................................................1701
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1572 -
12.3.29 Displaying and Setting Workpiece Setting Error
Compensation Data (15-inch Display Unit).......................1716
12.3.30 Displaying and Setting Pattern Data Inputs
(15-inch Display Unit) .......................................................1718
Screens of a 7.2/8.4/10.4-inch display unit
Press function key to display or set tool compensation values
and other data.
This section describes how to display or set the following data:
1. Tool compensation value
2. Settings
3. Sequence number comparison and stop
4. Run time and part count
5. Workpiece origin offset value
6. Custom macro common variables
7. Software operator’s panel
8. Tool management data
9. Display language switching
10. Protection of data at eight levels
11. Precision level selection
12. Tool life management data
13. Workpiece setting error compensation data
14. Pattern data input
The software operator’s panel, display language switching, precision
level selection, and pattern data input depend on the specifications of
the machine tool builder. See the manual issued by the machine tool
builder for details.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1573 -
12.3.1 Displaying and Entering Setting Data
Data such as the TV check flag and punch code is set on the setting
data screen. On this screen, the operator can also enable/disable
parameter writing, enable/disable the automatic insertion of sequence
numbers in program editing, and perform settings for the sequence
number comparison and stop function.
See III-9.2 for automatic insertion of sequence numbers.
See III-12.3.2 for the sequence number comparison and stop function.
This subsection describes how to set data.
Procedure for setting the setting data
Procedure
1 Select the MDI mode.
2 Press function key .
3 Press soft key [SETTING] to display the setting data screen.
This screen consists of several pages.
Press page key or until the desired screen is displayed.
An example of the setting data screen is shown below.
Fig. 12.3.1 (a) SETTING (HANDY) screen (10.4-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1574 -
Fig. 12.3.1 (b) SETTING (MIRROR IMAGE) screen (10.4-inch)
4 Move the cursor to the item to be changed by pressing cursor
keys .
5 Enter a new value and press soft key [INPUT].
Explanation
- PARAMETER WRITE
Setting whether parameter writing is enabled or disabled.
0 : Disabled
1 : Enabled
- TV CHECK
Setting to perform TV check.
0 : No TV check
1 : Perform TV check
- PUNCH CODE
Setting code when data is output through reader/puncher interface.
0 : EIA code output
1 : ISO code output
- INPUT UNIT
Setting a program input unit, inch or metric system
0 : Metric
1 : Inch
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1575 -
- I/O CHANNEL
Using channel of reader/puncher interface.
0 : Channel 0
1 : Channel 1
2 : Channel 2
- SEQUENCE NO.
Setting of whether to perform automatic insertion of the sequence
number or not at program edit in the EDIT mode.
0 : Does not perform automatic sequence number insertion.
1 : Perform automatic sequence number insertion.
- PROGRAM FORMAT
Setting of whether to use the Series 15 format.
0: Uses the standard format.
1: Uses the Series 15 format.
For the Series 15 format, refer to Chapter II-6 in the User’s Manual (T
series) or Chapter II-7 of Part II in the User’s Manual (M series).
- SEQUENCE STOP
Setting the sequence number with which the operation stops for the
sequence number comparison and stop function and the number of the
program to which the sequence number belongs
- MIRROR IMAGE
Setting of mirror image ON/OFF for each axes.
0 : Mirror image off
1 : Mirror image on
- Others
Page key or can also be pressed to display the
SETTING (TIMER) screen. See III-12.3.3 for this screen.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1576 -
12.3.2 Sequence Number Comparison and Stop
If a block containing a specified sequence number appears in the
program being executed, operation enters single block mode after the
block is executed.
Procedure for sequence number comparison and stop
Procedure
1 Select the MDI mode.
2 Press function key .
3 Press chapter selection soft key [SETTING].
4 Press page key or several times until the following
screen is displayed.
Fig. 12.3.2 (a) SETTING (HANDY) screen (10.4-inch)
5 Enter in (PROGRAM NO.) for SEQUENCE STOP the number
(1 to 99999999) of the program containing the sequence number
with which operation stops.
6 Enter in (SEQUENCE NO.) for SEQUENCE STOP (with eight
or less digits) the sequence number with which operation is
stopped.
7 When automatic operation is executed, operation enters single
block mode at the block containing the sequence number which
has been set.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1577 -
Explanation
- Sequence number after the program is executed
After the specified sequence number is found during the execution of
the program, the sequence number settting for sequence number
compensation and stop becomes “-1”.
- Exceptional blocks
If the predetermined sequence number is found in a block in which all
commands are those to be processed within the CNC control unit, the
execution does not stop at that block.
[Example] N1 #1=1 ;
N2 IF[#1 EQ 1]GOTO 08 ;
N3 GOTO 09 ;
N4 M98 P1000 ;
N5 M99 ;
In the example shown above, if the predetermined sequence number is
found, the execution of the program does not stop.
- Stop in the canned cycle
If the predetermined sequence number is found in a block which has a
canned cycle command, the execution of the program stops after the
return operation is completed.
- When the same sequence number is found several times in the program
If the predetermined sequence number appears twice or more in a
program, the execution of the program stops after the block in which
the predetermined sequence number is found for the first time is
executed.
- Block to be repeated a specified number of times
If the predetermined sequence number is found in a block which is to
be executed repeatedly, the execution of the program stops after the
block is executed specified times.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1578 -
12.3.3 Displaying and Setting Run Time, Parts Count, and Time
Various run times, the total number of machined parts, number of
parts required, and number of machined parts can be displayed.
This data can be set by parameters or on this screen (except for the
total number of machined parts and the time during which the power
is on, which can be set only by parameters).
This screen can also display the clock time. The time can be set on the
screen.
Procedure for Displaying and Setting Run Time, Parts Count and Time
Procedure
1 Select the MDI mode.
2 Press function key .
3 Press chapter selection soft key [SETTING].
4 Press page key or several times until the following
screen is displayed.
Fig. 12.3.3 (a) SETTING (TIMER) screen (10.4-inch)
5 To set the number of parts required, move the cursor to PARTS
REQUIRED and enter the number of parts to be machined.
6 To set the clock, move the cursor to DATE or TIME, enter a new
date or time, then press soft key [INPUT].
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1579 -
Explanation
- PARTS TOTAL
This value is incremented by one when M02, M30, or an M code
specified by parameter No. 6710 is executed. This value cannot be set
on this screen. Set the value in parameter No. 6712.
- PARTS REQUIRED
It is used for setting the number of machined parts required.
When the “0” is set to it, there is no limitation to the number of parts.
Also, its setting can be made by the parameter No 6713.
- PARTS COUNT
This value is incremented by one when M02, M30, or an M code
specified by parameter No. 6710 is executed. The value can also be set
by parameter No. 6711. In general, this value is reset when it reaches
the number of parts required. Refer to the manual issued by the
machine tool builder for details.
- POWER ON
Displays the total time which the power is on. This value cannot be set
on this screen but can be preset in parameter No. 6750.
- RUN TIME
Indicates the total run time during automatic operation, excluding the
stop and feed hold time.
This value can be preset in parameter No. 6751 or No. 6752.
- CUTTING TIME
Displays the total time taken by cutting that involves cutting feed such
as linear interpolation (G01) and circular interpolation (G02 or G03).
This value can be preset in parameter No. 6753 or No. 6754.
- FREE PURPOSE
This value can be used, for example, as the total time during which
coolant flows. Refer to the manual issued by the machine tool builder
for details.
- CYCLE TIME
Indicates the run time of one automatic operation, excluding the stop
and feed hold time. This is automatically preset to 0 when a cycle start
is performed at reset state. It is preset to 0 even when power is
removed.
- DATA and TIME
Displays the current date and time. The date and time can be set on
this screen.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1580 -
- Usage
When the command of M02 or M30 is executed, the total number of
machined parts and the number of machined parts are incremented by
one. Therefore, create the program so that M02 or M30 is executed
every time the processing of one part is completed. Furthermore, if an
M code set to the parameter No. 6710 is executed, counting is made in
the similar manner. Also, it is possible to disable counting even if
M02 or M30 is executed (bit 0 (PCM) of parameter No. 6700 is set to
1). For details, see the manual issued by machine tool builders.
Limitation
- Run time and part count settings
Negative value cannot be set. Also, the setting of “M” and “S” of run
time is valid from 0 to 59.
Negative value may not be set to the total number of machined parts.
- Time settings
Neither negative value nor the value exceeding the value in the
following table can be set.
Table 12.3.3 (a)
Item Maximum value Item Maximum value
Year 2096 Hour 23
Month 12 Minute 59
Day 31 Second 59
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1581 -
12.3.4 Displaying and Setting the Workpiece Origin Offset Value
Displays the workpiece origin offset for each workpiece coordinate
system (G54 to G59, G54.1 P1 to G54.1 P48 and G54.1 P1 to G54.1
P300) and external workpiece origin offset.
The workpiece origin offset value and external workpiece origin offset
value can be set on this screen.
Procedure for displaying and setting the workpiece origin offset value
Procedure
1 Press function key .
2 Press chapter selection soft key [WORK].
The workpiece coordinate system setting screen is displayed.
Fig. 12.3.4 (a) WORK COORDINATES screen (10.4-inch)
3 The screen for displaying the workpiece origin offset values
consists of two or more pages.
Display a desired page in either of the following two ways:
• Press the page key or .
• Enter the workpiece coordinate system number (0 : external
workpiece origin offset, 1 to 6: workpiece coordinate
systems G54 to G59, P1 to P48 : workpiece coordinate
systems G54.1 P1 to G54.1 P48, P1 to P300 : workpiece
coordinate systems G54.1 P1 to G54.1 P300) and press
operation selection soft key [NO.SRH].
4 Turn off the data protection key to enable writing.
5 Move the cursor to the workpiece origin offset to be changed.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1582 -
6 Enter a desired value by pressing numeric keys, then press soft
key [INPUT]. The entered value is specified in the workpiece
origin offset value. Or, by entering a desired value with numeric
keys and pressing soft key [+INPUT], the entered value can be
added to the previous offset value.
7 Repeat steps 5 and 6 to change other offset values.
8 Turn on the data protection key to disable writing.
12.3.5 Direct Input of Workpiece Origin Offset Value Measured
This function is used to compensate for the difference between the
programmed workpiece coordinate system and the actual workpiece
coordinate system. The measured offset for the origin of the
workpiece coordinate system can be input on the screen such that the
command values match the actual dimensions.
Selecting the new coordinate system matches the programmed
coordinate system with the actual coordinate system.
Procedure for direct input of workpiece origin offset value measured
Procedure
y
Programmed workpiece
origin
New offset
Previous offset
Origin
O'
Y
Surface A
Surface B
β
α
X
x
O
1 When the workpiece is shaped as shown above, position the
reference tool manually until it touches surface A of the
workpiece.
2 Retract the tool without changing the Y coordinate.
3 Measure distance α between surface A and the programmed origin
of the workpiece coordinate system as shown above.
4 Press function key .
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1583 -
5 To display the WORK COORDINATES screen, press the chapter
selection soft key [WORK].
Fig. 12.3.5 (a) WORK COORDINATES screen (10.4-inch)
6 Position the cursor to the workpiece origin offset value to be set.
7 Press the address key for the axis along which the offset is to be
set (Y-axis in this example).
8 Enter the measured value (α) then press soft key [MEASUR].
9 Move the reference tool manually until it touches surface B of
the workpiece.
10 Retract the tool without changing the X coordinate.
11 Enter the measured value of distance (β) to surface B as an X
value as with steps 7 and 8.
Limitation
- Consecutive input
Offsets for two or more axes cannot be input at the same time.
- During program execution
This function cannot be used while a program is being executed.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1584 -
12.3.6 Displaying and Setting Custom Macro Common Variables
Displays common variables (#100 to #149 or #100 to #199, and #500
to #531 or #500 to #999) on the screen.
The values for variables can be set on this screen.
Relative coordinates can also be set to variables.
Procedure for displaying and setting custom macro common variables
Procedure
1 Press function key .
2 Press the continuous menu key , chapter selection soft key
[MACRO], and soft key [(OPRT)] in the stated order.
The following screen is displayed.
Fig. 12.3.6 (a) CUSTOM MACRO screen (10.4-inch)
3 Move the cursor to the variable number to set using either of the
following methods:
• Enter the variable number and press soft key [NO.SRH].
• Move the cursor to the variable number to set by pressing
page keys and/or and cursor keys ,
, , and/or .
4 Enter data with numeric keys and press soft key [INPUT].
5 To set a relative coordinate in a variable, press address key ,
, or , then press soft key [INP.C.].
6 To set a blank in a variable, just press soft key [INPUT]. The
value field for the variable becomes blank.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1585 -
Explanation
If the value of a variable produced by an operation is not displayable,
an indication below is provided.
When the significant number of digits is 12 (with bit 0 (F16) of
parameter No. 6008 set to 0):
Variable value range Variable value indication
0 < Variable value < +0.00000000001 +Underflow
0 > Variable value > -0.00000000001 -Underflow
Variable value > 999999999999 +Overflow
Variable value < -999999999999 -Overflow
When the significant number of digits is 8 (with bit 0 (F16) of
parameter No. 6008 set to 1):
Variable value range Variable value indication
0 < Variable value < +0.0000001 +Underflow
0 > Variable value > -0.0000001 -Underflow
Variable value > 99999999 +Overflow
Variable value < -99999999 -Overflow
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1586 -
12.3.7 Displaying and Setting Real Time Custom Macro Data
Real time macro variables (RTM variables) are dedicated to real time
custom macros.
RTM variables are divided into temporary real time macro variables
(temporary RTM variables) and permanent real time macro variables
(permanent RTM variables).
The values of permanent RTM variables are kept stored after the
power is turned off.
Temporary RTM variables are cleared to 0 when the power is turned
off.
System variables (DI/DO variables) dedicated to real time custom
macros are used to read and write PMC interface signals. Data can be
read and written in bit and byte units. Before writing a signal, release
the protection of the corresponding variable on the PMC signal protect
screen.
Displaying and setting real time custom macro variables
Procedure
1 Press function key .
2 Press the continuous menu key several times, then press
chapter selection soft key [R.TIME MACRO]. The following
screen appears:
Fig. 12.3.7 (a) REAL TIME MACRO screen (10.4-inch)
3 To display or set real time custom macro variables of which
values are not stored at power-off, press soft key [TEMP. DATA].
4 To display or set real time custom macro variables of which
values are stored at power-off, press soft key [PERM. DATA].
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1587 -
5 Move the cursor to the number of a real time custom macro
variable you want to set using either of the following methods:
• Enter the number of a real time custom macro variable and
press soft key [NO. SRH].
• Move the cursor to the number of a real time custom macro
variable you want to set by pressing page keys
and/or and cursor keys , , , and/or
.
6 Enter data.
Displaying and setting DI/DO variables
Procedure
For setting in byte units:
1 Press function key .
2 Press the continuous menu key several times, then press
chapter selection soft key [R.TIME MACRO]. The following
screen appears:
3 Press soft key [BYTE SELECT]. The following screen appears:
Fig. 12.3.7 (b) BYTE SELECT screen (10.4-inch)
4 Move the cursor to the number of a DI/DO variable you want to
set using either of the following methods:
• Enter the number and press soft key [NO. SRH].
• Move the cursor to a desired number by pressing page keys
and/or and cursor keys , , ,
and/or .
5 Enter data.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1588 -
12.3.8 Displaying and Setting the Software Operator’s Panel
Operations on the MDI panel can substitute for the functions of
switches on the machine operator’s panel. This means that a mode
selection, jog feed override selection, and so forth can be made with
operations on the MDI panel, eliminating the need to use the
corresponding switches on the machine operator’s panel.
Jog feed can be performed using numeric keys.
Procedure for displaying and setting the software operator’s panel
Procedure
1 Press function key .
2 Press the continuous menu key , then press chapter selection
soft key [OPR].
3 The screen consists of several pages. Press page key or
until the desired screen is displayed.
Fig. 12.3.8 (a) Without the manual handle feed function (10.4-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1589 -
Fig. 12.3.8 (b) With the manual handle feed function (10.4-inch)
Fig. 12.3.8 (c) (10.4-inch)
4 Move the cursor to the desired switch by pressing cursor key
or .
5 Push the cursor key or to match the mark to an
arbitrary position and set the desired condition.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1590 -
6 Press one of the following arrow keys to perform jog feed. Press
the key together with an arrow key to perform jog rapid
traverse.
Fig. 12.3.8 (c) MDI arrow keys
Explanation
- Valid operations
The valid operations on the software operator’s panel are shown
below. Whether to use each group can be chosen using parameter
No. 7200. Those groups that are not used are not displayed on the
software operator’s panel.
Group1 : Mode selection
Group2 : Selection of jog feed axis, Manual rapid traverse
Group3 : Selection of manual pulse generator feed axis, selection of
manual pulse magnification
Group4 : Jog federate, federate override, rapid traverse override
Group5 : Optional block skip, single block, machine lock, dry run
Group6 : Protect key
Group7 : Feed hold
- Screens on which jog feed is valid
When the LCD indicates other than the software operator’s panel
screen and self-diagnosis screen, jog feed is not conducted even if the
arrow key is pushed.
- Jog feed and arrow keys
The feed axis and direction corresponding to the arrow keys can be set
with parameters (Nos. 7210 to 7217).
- General purpose switches
For the meanings of these switches, refer to the manual issued by
machine tool builder.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1591 -
12.3.9 Setting and Displaying Tool Management Data
The tool management function totally manages tool information
including tool offsets and tool life information.
This function provides a magazine screen and tool management screen.
This subsection explains how to set these screens.
12.3.9.1 Displaying and setting magazine screen
1 Press function key .
2 Press chapter selection soft key [TOOL MANAGER].
Alternatively, press function key several times until the
tool management screen appears.
Press soft key [MAGAZINE].
Fig. 12.3.9.1 (a) Tool management magazine screen (10.4-inch)
3 By using the page keys, cursor keys, and soft keys [←] and [→],
move the cursor to the pot No. position of the magazine for
which you want to set or modify data.
Alternatively, type the number of the tool management data you
wan to set or modify, and press soft key [NO. SRH].
4 Press soft key [EDIT].
5 To set the tool management data number of a pot, type the tool
management data number, then press soft key [INPUT].
To delete the tool management data number set for a pot, follow
the steps below.
<1> Press soft key [ERASE].
<2> Press soft key [CURDAT]. To delete the tool management
data numbers registered for all pots, press soft key [ALL].
<3> Press soft key [EXEC]. Alternatively, type 0.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1592 -
6 To end the edit operation, press soft key [EXIT].
This returns the screen display to the conventional tool
management screen.
Explanation
- Another method
Magazine data can be input/output also by using external I/O devices.
See III-8, “DATA I/O”.
- Displayed data
Pot : As many pots as specified in parameter No. 13222, 13227,
13232, or 13237 (settable for each magazine) are displayed.
The starting pot number can be set for each magazine in
parameter No. 13223, 13228, 13233, or 13238.
NO. : Tool management data numbers are displayed.
In the following cases, tools cannot be set in magazines:
1. A tool management data number beyond the range from 0 to
(the number of valid pairs in parameter No. 13220) is set.
2. Tool management data is invalid (bit 1 of tool information is
0).
3. The tool management data number to be set is already set for
another pot.
Type No. : Tool type numbers corresponding to tool management data
numbers are displayed.
Values cannot be set on this screen.
Spindle : The tool management data numbers and tool type numbers
of spindle positions are displayed.
Wait : The tool management data numbers and tool type numbers
of wait positions are displayed.
- Edit mode
To edit data, press soft key [EDIT] to enter tool management data edit
mode.
- Tool management data number
Tool management data numbers can optionally be extended to 64, 240,
or 1000 pairs. In addition, the number of tools used can be set in
parameter No. 13220.
- Display of the spindle positions and wait positions
The spindle position and wait position can be set for each path.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1593 -
12.3.9.2 Displaying and setting tool management screen
Procedure
1 Press function key .
2 Press chapter selection soft key [TOOL MANAGER].
Alternatively, press function key several times until the
tool management screen appears.
3 Press soft key [TOOL MANAGER].
Fig. 12.3.9.2 (a) Tool management data screen (10.4-inch)
4 By using the page keys, cursor keys, and soft keys [←] and [→],
move the cursor to the position of the tool information of the tool
number for which you want to set or modify data.
Alternatively, type the tool number of the data you want to set or
modify, and press soft key [NO. SRH].
5 Press soft key [EDIT].
6 To set tool data, type a desired value, then press soft key
[INPUT].
To delete tool information, follow the steps below.
<1> In step 4, move the cursor to the tool information you want
to erase.
<2> Press soft key [ERASE].
<3> Press soft key [CURDAT]. To delete entire tool information,
press soft key [ALL].
<4> Press soft key [EXEC].
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1594 -
7 To end the edit operation, press soft key [EXIT].
This returns the screen display to the conventional tool
management screen.
Fig. 12.3.9.2 (b) Tool management data screen (check function)
(10.4-inch)
8 When soft key [CHECK] is pressed, if there are tools with the
same number but with different count types (count and time), the
cursor moves to the tool type number of the smallest tool
management number in the tool type numbers and a warning
message appears.
The warning messages issued by the check function are shown
below.
<1> For the same type of tools with different count types
L-COUNT TYPE MISMATCH:XXXXXXXX
<2> For the same type of tools with the same count type
L-COUNT TYPE MATCH
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1595 -
Explanation
- Another method
Tool management data, customize data, and names set for tool states
can be input/output also by using external I/O devices.
See III-8, “DATA I/O”.
- Displayed information
• Life information
Fig. 12.3.9.2 (c) Tool management data life status screen(10.4-inch)
NO. : Tool management data numbers are displayed. These
numbers can be displayed but cannot be set. The tool
management data number of edited data is kept blinking
until tool management data edit mode ends. Tool
management data numbers set or deleted on the magazine
screen also blink on the tool management screen.
Type No. : Tool type numbers are displayed.
A value from 0 to 99,999,999 can be set.
MG : The magazine number assigned to each tool is indicated.
These numbers can be displayed but cannot be set.
Pot : The pot number assigned to each tool is indicated.
These numbers can be displayed but cannot be set.
T-INFO : The following five types of information are displayed
sequentially from the right:
• Tool management data: Valid (R)/invalid (-))
• Life count type: Time (T)/count (C)
• Tool type: Oversize tool (B)/normal tool (N)
• Data access: Locked (L)/unlocked (U)
• When a tool is not under life management:
Included in the tools to be searched (1)/not included in
the tools to be searched (0)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1596 -
NOTE
1 The tool types and data access information vary
depending on the specifications defined by the
machine tool builder.
2 The same type of tools must have the same life
count type.
L-COUNT : The number of use times/use period of time of each tool
is indicated.
Up to 99,999,999 times or 999 hours 59 minutes 59
seconds can be set.
MAX-LIFE : The maximum life value of each tool is indicated.
Up to 99,999,999 times or 999 hours 59 minutes 59
seconds can be set.
NOTICE-L : Noticed life value of a tool
Up to 99,999,999 times or 999 hours 59 minutes 59
seconds can be set.
L-STATE : Current tool state
One of the four states, including invalid (0), present (1,
2), not present (3), and broken (4), is indicated. The
numbers in parentheses are data values used when these
states are input in MDI.
• Spindle speed/feedrate
Fig. 12.3.9.2 (c) Tool management data spindle speed/feedrate screen
(10.4-inch)
S : Spindle speed.
A value from 0 to 99,999 can be set.
F : Feedrate.
A value from 0 to 99,999,999 can be set.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1597 -
• Tool offset information
Fig. 12.3.9.2 (d) Tool management data tool offset screen (10.4-inch)
H : Tool length compensation number (for machining center
systems only).
A value from 0 to 999 can be set.
D : Cutter compensation number (for machining center systems
only).
A value from 0 to 999 can be set.
TG : Tool geometry compensation number (for lathe systems only).
A value from 0 to 999 can be set.
TW : Tool wear compensation number (for lathe systems only).
A value from 0 to 999 can be set.
The displayed offset data is determined depending on the option
configuration and parameter settings (bits 1(DCR), 2(DOY), 3(DOB),
4(DO2), 6(DOT), and 7(DOM) of parameter No. 13202).
• Customize information
Fig. 12.3.9.2 (e) Tool management data customize data screen (10.4-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1598 -
Customize 0 : Bit-type customize information.
For each bit, 1 or 0 can be input.
Customize 1 to 4 : Customize information. Any value from
-99,999,999 to 99,999,999 can be set.
Customize 5 to 20 : Customize information. These items are
displayed only when customize data extension
option (5 to 20) of the tool management
function is enabled. Any value from
-99,999,999 to 99,999,999 can be set.
Customize 21 to 40 : Customize information. These items are
displayed only when customize data extension
option (5 to 40) of the tool management
function is enabled. Any value from
-99,999,999 to 99,999,999 can be set.
- Tool management data number
Tool management data numbers can optionally be extended to 64, 240,
or 1000 pairs. The number of tools used can be set in parameter No.
13220.
- Edit mode
To edit data, press soft key [EDIT] to enter tool management data edit
mode.
- Life count override
When the period of time is set as the tool life count type, the life count
can be overridden if bit 2 (LFV) of parameter No. 6801 is set to 1.
Specify an override value by using a switch on the machine operator’s
panel.
Example) When cutting is performed for 10 minutes with an override
of 0.1, one minute is counted in the tool life counter.
- Tool management extension function
When tool management extension functions are enabled, you can use
the following functions in addition to the tool management functions:
• A value with a decimal point can be set as customize data.
The maximum number of decimal places can be set to 7 by G10
data input and file read.
• Various types of tool management data can be protected using
KEY signals.
An attempt to enter a value to a protected data causes a warning
message “WRITE PROTECT.”
• Tool life count period selection
Bit 5 of tool information is used to make a life count period selection.
Item Description
Data length 1 byte (flag data)
#5 REV 0: A life count period of 1 sec is used.
1: A life count period of 8 msec is used.
Range of count is as follows.
1sec : 0 to 3,599,999 seconds (999 hours 59 minutes 59 seconds)
8msec : 0 to 3,599,992 ms (59 minutes 59 seconds 992 milliseconds)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1599 -
12.3.9.3 Each tool data screen
Each tool data screen
Procedure
1 Press function key .
2 Press chapter selection soft key [TOOL MANAGER].
Alternatively, press function key several times until the
tool management screen appears.
3 Press soft key [EACH TOOL]. The each tool data screen
appears.
Fig. 12.3.9.3 (a) Each tool data screen (10.4-inch)
Explanation
- Header
The following four data items are displayed: NO., TYPE NO., MG,
and POT.
When the data table of a tool extends over two or more pages, the
same header is displayed on these pages.
- Data table
The data table shows data items related to a tool at a time.
The data items are displayed from the upper left to the lower left, the
upper right, and the lower right in ascending order of screen display
position numbers specified using the customize function. The number
of digits displayed for one data item is fixed to 11.
Up to 24 data items are displayed on one page. (12 data items × 2
columns)
When more than 24 data items are set for a tool, the 25th and
subsequent data items are displayed on the next page. (Up to three
pages)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1600 -
When a data item is set as a screen element of the tool management
data screen twice or more using the tool management data display
customize function (one of the tool management extension functions),
only the data item with the smaller display position number is
displayed. When no value is set for a data item, the field for the data
item is not displayed and the next data item is displayed.
Key operations
- MDI key operations
• Numeral keys Inputs a numeric value.
• Displays the previous page for the same tool.
• Displays the next page for the same tool.
• Moves the cursor to the previous data item.
When the cursor is on the top row of the data
table, it moves to the bottom row of the left
column. When the cursor is on the first data item,
it moves to the last data item.
• Moves the cursor to the next data item.
When the cursor is on the bottom row of the data
table, it moves to the top row of the right column.
When the cursor is on the last data item, it moves
to the first data item.
• Moves the cursor left on the screen.
When the cursor is on the left column of the data
table, it moves to the right column on the row
immediately above. When the cursor is on the
first data item, it moves to the last data item.
• Moves the cursor right on the screen.
When the cursor is on the right column of the
data table, it moves to the left column on the row
immediately below. When the cursor is on the
last data item, it moves to the first data item.
- Soft key operations
• Soft key [EDIT]
Enters the management data edit mode.
• Soft key [NO.SRH]
Displays data with a tool management data number when pressed
after the tool management data number is entered.
• Soft key [PREV.TOOL]
Returns to the previous tool management data number.
• Soft key [NEXT.TOOL]
Proceeds to the next tool management number.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1601 -
Operation in the management data edit mode
To edit data, press soft key [EDIT] to enter the management data edit
mode.
Fig. 12.3.9.3 (b) Each tool data screen (10.4-inch)
In the management data edit mode, “EDITING” is displayed at the
lower right of the screen.
In addition to the above key operations, the following key operations
are available in the management data edit mode:
•
Actually writes a value entered using numeric keys.
• Soft key [END]
Ends the management data edit mode.
Operations for editing tool information are the same as those on
the tool management data screen.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1602 -
12.3.9.4 Displaying the total life of tools of the same type
Total life data screen
Procedure
1 Press function key .
2 Press chapter selection soft key [TOOL MANAGER].
Alternatively, press key several times until the tool
management screen appears.
3 Press soft key [TOTAL LIFE]. The total life data screen appears.
4 Press soft key [(OPRT)], then soft key [CHANGE] to switch the
display between total life data of the count counting type tools
and that of the time counting type tools.
Fig. 12.3.9.4 (a) Count display (10.4-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1603 -
Fig. 12.3.9.4 (b) Time display (10.4-inch)
Displayed information
S-NO. : Sequential number of each tool type
TYPE NO. : Tool type number
T-REM-LIFE : Total of remaining life values of tools with the same
tool type number
T-L-COUNT : Total of used counts/times of tools with the same
tool type number
T-MAX-LIFE : Total of maximum life values of tools with the same
tool type number
NUM : Number of tools with the same tool type number
T-NOTICE-L : Total of notice life values of tools with the same tool
type number when the tool life arrival signal is to be
output for each tool type
STATUS : Whether the tool life arrival signal has been output
when the signal is to be output for each tool type
Either of the two states (UNDONE and DONE) is
displayed.
When bit 3 (ETE) of parameter No. 13200 is set to 0 and bit 2 (TRT)
of parameter No. 13200 is set to 1, the tool life arrival signal is to be
output for each tool type number and T-NOTICE-L and STATUS are
displayed.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1604 -
Key operations
- MDI key operations
Displays the previous page. The cursor moves to the last data
item on that page.
Displays the next page. The cursor moves to the first data item
on that page.
Moves the cursor up on the screen.
Moves the cursor down on the screen.
Disabled.
Disabled.
- Soft key operations
Soft key [DETAIL]
Displays the detailed life data screen.
Soft key [UPDATE]
Updates data displayed on the total life data screen.
Soft key [CHANGE]
Switch the display between the count and time types.
Soft key [T-TYPENO. SRH]
Moves the cursor to a tool type number when pressed after the
number is entered.
Soft key [T-ASCE -SORT]
Sorts data in ascending order of tool type numbers.
Soft key [T-DESC -SORT]
Sorts data in descending order of tool type numbers.
Soft key [R-ASCE -SORT]
Sorts data in ascending order of remaining life values.
Soft key [R-DESC -SORT]
Sorts data in descending order of remaining life values.
NOTE
1 After soft key [T-ASCE -SORT], [T-DESC -SORT],
[R-ASCE -SORT], or [R-DESC -SORT] is pressed,
the cursor is positioned at the top of page 1 of the
total life data screen.
2 When the power is turned on, data of the count
counting type is displayed in ascending order of tool
type numbers. When the display type is changed or
data is sorted in a different order, the status is kept.
3 If soft key [DETAIL] is pressed when no data is
displayed on the total life data screen, the warning
message “NO DETAILED LIFE DATA SCREEN” is
output.
4 If an unregistered tool type is specified and soft key
[T-TYPENO. SRH] is pressed, the warning message
“UNREGISTERED NUMBER” is output.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1605 -
Detailed life data screen
Procedure
1 Press function key .
2 Press chapter selection soft key [TOOL MANAGER].
Alternatively, press several times until the tool
management screen appears.
3 Press soft key [TOTAL LIFE]. The total life data screen appears.
4 Press soft key [(OPRT)], then soft key [DETAIL]. The detailed
life data screen appears.
Fig. 12.3.9.4 (c) Detailed life data screen (10.4-inch)
- Displayed information
TYPE NO. : Tool type number
ORDER : Sequential number in ascending order of remaining life
times or the order in which the customize data is set.
NO. : Tool management data number
REM-LIFE : Remaining life value obtained by subtracting the life
count value from the maximum life value
L-COUNT : Total used count or time of the tool
MAX-LIFE : Maximum life value of the tool
NOTICE-L : Notice life value of the tool
STATUS : Life status of the tool
One of the four states (NO-MNG (0), ENABLE (1, 2),
NONE (3), and DAMAGED (4)) is displayed.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1606 -
Key operations
- MDI key operations
Displays the previous page.
Displays the next page.
Moves the cursor up on the screen. The cursor moves to the
last data item on that page.
Moves the cursor down on the screen. The cursor moves to the
first data item on that page.
Disabled.
Disabled.
- Soft key operations
Soft key [UPDATA]
Updates data displayed on the detailed life data screen.
The cursor is positioned at the beginning of page 1 after this soft
key is pressed.
Soft key [CLOSE]
Closes the detailed life data screen and returns to the total life
data screen.
NOTE
1 When soft key [CLOSE] is pressed and the total life
data screen is displayed again, the cursor on the
total life screen data is positioned as follows.
2 When the tools with the tool type number displayed
when the detailed data screen is closed are
registered as tool management data, the cursor on
the total life screen is positioned at that tool type
number.
3 When the tools with the tool type number displayed
when the detailed data screen is closed are not
registered as tool management data, the cursor on
the total life data screen is positioned at the first
total life data.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1607 -
12.3.9.5 Tool geometry data screen
Tool geometry data screen
Procedure
1 Press function key .
2 Press chapter selection soft key [TOOL MANAGER].
Alternatively, press several times until the tool
management screen appears.
3 Press continuous menu key , then soft key [TOOL-GEOM].
The tool geometry data screen appears.
Fig. 12.3.9.5 (a) Tool geometry data screen (10.4-inch)
- Displayed item
NO. : Tool geometry number
Up to 20 numbers can be displayed.
LEFT : Sets the number of pots on the left of the reference pot that
are to be occupied.
A value between 0 and 4 can be set.
RIGHT : Sets the number of pots on the right of the reference pot
that are to be occupied.
A value between 0 and 4 can be set.
UPPER : Sets the number of pots above the reference pot that are to
be occupied.
A value between 0 and 4 can be set. (Use this item when
the magazine is of the matrix type.)
LOWER : Sets the number of pots under the reference pot that are to
be occupied.
A value between 0 and 4 can be set. (Use this item when
the magazine is of the matrix type.)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1608 -
Key operations
- Operations in the standard mode
MDI key operations
Numeral keys Inputs a numeric value.
Moves the cursor up on the screen.
Moves the cursor down on the screen.
Moves the cursor left on the screen.
Moves the cursor right on the screen.
Soft key operations
Soft key [NO.SRH]
Moves the cursor on a tool geometry number when pressed after
the number is entered.
Soft key [EDIT]
Enters the data edit mode.
Soft key [READ]
Reads data related to the tool management functions.
This key is available only in the standard mode.
Put the NC in the EDIT mode.
Soft key [PUNCH]
Punches data related to the tool management functions.
This key is available only in the standard mode.
Put the NC in the EDIT mode.
In the management data edit mode, the following key operations
are available in addition to the above key operations.
- Operations in the edit mode
To edit data, press soft key [EDIT] to enter the edit mode. In the edit
mode, “EDITING” is displayed at the lower right of the screen.
MDI key operation
Actually writes a value entered using numeric keys.
Soft key operation
Soft key [END]
Ends the data edit mode.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1609 -
Example
Set the edit mode. When the tool geometry with tool geometry number
1 occupies 1 pot in the left direction, 0.5 pots in the right direction,
and 1.5 pots in the down direction, set data as shown in the figure
below:
Fig. 12.3.9.5 (b) Example of setting data on the tool geometry data
screen (10.4-inch)
- Display of occupied pots in the magazine management table
Each pot occupied by a tool stored in another pot is indicated with an
asterisk (*).
Fig. 12.3.9.5 © Magazine management table (10.4-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1610 -
If a tool to be registered for a magazine is determined to interfere with
another tool, the warning message “TOOL INTERFERENCE CHECK
ERROR:xxxx,xxxx” is displayed. xxxx indicates the tool number of
each of the two tools. If a tool is determined to interfere with
multiple tools, only the first tool detected by the NC interference
check is displayed.
If a tool is determined to interfere with the frame of a magazine, the
tool number of the tool to be stored and “FRAME” are displayed.
- Search for an empty pot for a oversize tool
In the management data edit mode, pressing soft key [(OPRT)], then
continuous menu key displays the soft keys for searching for an
empty pot for a oversize tool.
Fig. 12.3.9.5 (c) Searching for an empty pot for a oversize tool (10.4-inch)
Enter the tool geometry number in the key-in buffer and press a search
soft key. The cursor moves to an empty pot fit for the geometry.
EMPTY-SRCH.N : Searches for an empty pot forward.
EMPTY-SRCH.P : Searches for an empty pot backward.
EMPTY-SRCH : Searches for the pot nearest to the current
position.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1611 -
- Tool management screen
You can use bit 2 of tool information to switch between a oversize
tool and normal tool. For a oversize tool, set a tool geometry number
fit for the tool.
Fig. 12.3.9.5 (d) Bit for switching between a normal tool and oversize
tool (10.4-inch)
Fig. 12.3.9.5 (e) Tool geometry number (10.4-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1612 -
12.3.10 Displaying and Switching the Display Language
The language used for display can be switched to another language.
A display language can be set using a parameter. However, by
modifying the setting of the display language on this screen, the
display language can be switched without turning off then on the
power.
Displaying and setting the display language
Procedure
1 Press function key .
2 Press the continuous menu key several times.
3 Press soft key [LANGUAGE] to display the language screen.
Fig. 12.3.10 (a) LANGUAGE screen (10.4-inch)
4 Press page key or , then press cursor keys ,
to move the cursor to a desired display language.
5 Press operation soft key [APPLY]. The display language is
switched to the selected language. The language specified on this
screen continues to be used if the power is turned off then back
on.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1613 -
Explanation
- Language switching
The language screen can be displayed if bit 0 (NLC) of parameter No.
3280 is set to 0.
- Selectable languages
The display languages selectable on this screen are as follows:
1. English
2. Japanese
3. German
4. French
5. Chinese (Traditional)
6. Chinese (Simplified)
7. Italian
8. Korean
9. Spanish
10. Dutch
11. Danish
12. Portuguese
13. Polish
14. Hungarian
15. Swedish
16. Czech
17. Russian
18. Turkish
Among the languages listed above, English and other usable
languages are displayed on the screen as a list of switchable
languages.
Limitation
- Language parameter modification on the parameter screen
Which language to use for display is specified with parameter No.
3281. This parameter can be modified using the parameter screen as
well. However, if a modification is made on the parameter screen, the
new setting is not reflected until “APPLY” operation is performed on
the language screen or the power is turned on again. If an invalid
value is set in parameter No. 3281 on the parameter screen, the screen
is displayed in English after the power is turned on again.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1614 -
12.3.11 Protection of Data at Eight Levels
You can set eight CNC and PMC operation levels and one of eight
protection levels for each type of CNC and PMC data.
When an attempt is made to change CNC and PMC data or output it to
an external unit, the operation level is compared with the protection
level to determine whether to allow the change or external output.
12.3.11.1 Operation level setting
You can set eight CNC and PMC operation levels.
Displaying and setting the operation level setting screen
Procedure
1 Press function key .
2 Press the continuous menu key several times until soft key
[PROTECT] is displayed.
3 Press soft key [PROTECT].
The operation level setting screen shown below is displayed.
Fig. 12.3.11.1 (a) Operation level setting screen (10.4-inch)
4 Key in the password for an operation level to be set/modified,
then press soft key [INPUT PASSWD].
5 To return the operation level to 0, 1, 2, or 3, press soft key
[CANCEL PASSWD].
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1615 -
Explanation
- Operation level setting
To select operation level 0 to 3, use the corresponding memory
protection key signal.
To select operation level 4 to 7, use the corresponding password.
Table 12.3.11.1 (a) Operation level setting
Operation level Setting Sample grouping
7 (high) Password -
6 Password MTB
5 Password Dealer and integrator
4 Password End user
3 Memory protection key signal User level (level 1)
2 Memory protection key signal User level (level 2)
1 Memory protection key signal User level (level 3)
0 (low) Memory protection key signal User level (level 4)
When operation level 4 to 7 is set, the operation level remains
unchanged until the password is cleared.
(The operation level also remains unchanged if the power is turned
off.)
Operation level 7 is reserved for CNC and PMC maintenance.
NOTE
When a password is being entered, an asterisk (*)
is displayed instead of each entered character.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1616 -
12.3.11.2 Password modification
The current operation level is displayed.
The password for each of operation levels 4 to 7 can be modified.
Displaying and setting the password modification screen
Procedure
1 Press function key .
2 Press the continuous menu key several times until soft key
[PROTECT] is displayed.
3 Press soft key [PROTECT].
4 Press soft key [PASSWORD].
The PASSWORD CHANGE screen shown below is displayed.
Fig. 12.3.11.2 (a) PASSWORD CHANGE screen (10.4-inch)
5 Key in an operation level whose password is to be modified, then
press soft key [INPUT].
6 Key in the current password for the operation level whose
password is to be modified, then press soft key [INPUT].
7 Key in a new password, then press soft key [INPUT].
8 Key in the new password again for confirmation, then press soft
key [INPUT].
9 Press soft key [PASSWDCHANGE].
10 To clear the password, press soft key [PASSWDCLEAR].
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1617 -
Explanation
Up to eight characters (only uppercase alphabetic characters and
numeric characters) can be input.
NOTE
1 For a password, consisting of three to eight
characters, the following characters are available:
• Uppercase alphabetic characters
• Numeric characters
2 When a password is being entered, an asterisk (*)
is displayed instead of each entered character.
3 Whether a password can be changed at the current
operation level is determined as follows:
• Password of an operation level higher than the
current operation level
Cannot be changed.
• Password of the current operation level
Can be changed.
• Password of an operation level lower than the
current operation level
Can be changed (only to the initial password).
4 The set password is not displayed.
Be careful not to forget the password.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1618 -
12.3.11.3 Protection level setting
The current operation level is displayed.
The change protection level and output protection level of each data
item are displayed.
The change protection level and output protection level of each data
item can be changed.
Confirmation based on protection level setting
Procedure
1 Press function key .
2 Press the continuous menu key several times until soft key
[PROTECT] is displayed.
3 Press soft key [PROTECT].
4 Press soft key [DATA LEVEL] to change the protection level of
CNC data or press soft key [PMC LEVEL] to change the
protection level of PMC data.
The following protection level change screen is displayed.
Fig. 12.3.11.3 (a) Protection level change screen (10.4-inch)
5 Move the cursor to the change level or output level of a desired
data item.
6 Key in a new desired level, then press soft key [INPUT].
NOTE
When the protection level of PMC data is set, soft
key [SWITCH PMC] is used to switch between
PMC paths to be set, for multipath PMC.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1619 -
Explanation
When the protection level of a data item is higher than the current
operation level, the protection level of the data item cannot be
changed.
The protection level of a data item cannot be changed to a protection
level higher than the current operation level.
For each of the following types of data, you can set a data protection
level. There are the following two types of data protection levels:
• Change protection level
Sets the protection level used when data is changed.
• Output protection level
Sets the protection level used when data is output (punched out) to an
external unit.
As a protection level, you can set a value of 0 (low) to 7 (high).
Table 12.3.11.3 (a) Protection level of each type of data
Initial protection level
Type of data Change Output
Custom macro variable data <CUSTOM MACRO>
(including variable data dedicated to the macro executor) 0 0
Periodical maintenance data <PERIODICAL MAINTENANCE DATA> 0 0
Tool management data <TOOL LIFE TIME DATA> 0 0
Tool offset data <TOOL OFFSET DATA>
(For each type when tool geometry compensation and tool wear compensation
are treated differently)
0 0
Clock data <TIME> 0 0
Workpiece origin shift amount data <WORK ZERO SHIFT> 0 0
Workpiece origin offset data <WORK ZERO OFFSET> 0 0
Ethernet setting data <ETHER NET SETTING> 0 0
Fixture offset data <FIXTURE OFFSET DATA> 0 0
Parameter data <PARAMETER DATA> 4 0
Settings <SETTING DATA> 0 0
Pitch error compensation data <PITCH ERROR DATA>
(including three-dimensional error compensation data) 4 0
Parameter data for Power Mate CNC manager function
<PARAMETER DATA FOR POWER MATE CNC MANAGER> 0 0
Each part program <PROGRAMS FOR EACH PARTS> 0 0
Part program editing operation <CHANGE PROGRAMS FOR EACH PARTS> 0 0
Absolute coordinate preset operation <PRESET OF ABSOLUTE AXIS DATA> 0 0
Table 12.3.11.3 (b) Protection level of PMC data
Initial protection level
Type of data Change Output
Composition parameter 0 0
Setting (online) 0 0
Setting (each path) 0 0
Sequence program 0 0
PMC parameter 0 0
Timer 0 0
Counter 0 0
Keep relay 0 0
Keep relay (system) 0 0
Data table 0 0
Data table control 0 0
PMC momory 0 0
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1620 -
NOTE
1 For some types of data, the output function is not provided.
2 When the protection level of data is higher than the current operation level, the
protection level cannot be changed.
3 The protection level of data cannot be changed to a level higher than the current
operation level.
4 Settable types of data increase or decrease, depending on the option configuration.
5 For details on the protection level of PMC data, refer to “PMC Programming Manual
(B-63983EN)”.
6 Data related to tool information on the EACH TOOL DATA screen for the tool
management function is protected by protecting tool offset data.
7 The type of tool offset data put in effect varies depending on the tool compensation
value memory used.
8 To change the protection level for each part program, do so on the PROGRAM
FOLDERscreen rather than on the PROTECT LEVEL screen.
9 Part program editing includes program editing for the MDI mode.
10 Presetting absolute coordinates causes preset workpiece coordinate system values
to be protected.
11 During tool offset data input/output, if any tool offset data type is not allowed to be
changed or output to the outside, it is processed as follows:
- Input : Any data type other than those whose change is not allowed is changed.
- Output : Any data type other than those whose change is not allowed is output.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1621 -
12.3.11.4 Setting the change protection level and output protection
level of a program
The display/operations indicated below can be performed from the
directory screen.
The change protection level and output protection level of each part
program are displayed.
The change protection level and output protection level of each part
program can be changed.
Setting the change protection level and output protection level of a program
Procedure
1 Press function key .
2 Press soft key [FOLDER].
The program directory screen shown below is displayed.
Fig. 12.3.11.4 (a) Program directory screen (10.4-inch)
3 Press the continuous menu key several times until
[DETAIL ON] is displayed.
4 Press soft key [DETAIL ON]. The screen display switches to the
detail display screen.
5 Move the cursor to a desired program.
6 Press the continuous menu key several times until
[CHANGE LEVEL] is displayed.
7 Key in a new desired level, then press soft key [CHANGE
LEVEL].
8 To change the output protection level, key in a new desired level,
then press soft key [OUT LEVEL].
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1622 -
Explanation
The change protection level (0 to 7) and output protection level (0 to
7) are displayed as “CHANGE PROTECTION LEVEL
VALUE/OUTPUT PROTECTION LEVEL”.
NOTE
1 When the protection level of data is higher than the
current operation level, the protection level cannot
be changed.
2 The protection level of data cannot be changed to a
level higher than the current operation level.
3 A protection level can be set only for those part
programs that are held on the “CNC_MEM” device.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1623 -
12.3.12 Precision Level Selection
An intermediate precision level between the parameters for emphasis
on velocity (precision level 1) and the parameters for emphasis on
precision (precision level 10) set on the machining parameter tuning
screen can be selected. As shown in the figure below, the levels are
proportionally linear, and an intermediate level can be selected so that
optimal parameters can be automatically calculated to perform
machining.
Value
RMS value
1 10 Precision level
(RMS value: Root-Mean-Square value)
Fig. 12.3.12 (a) Image of “level”
Procedure for precision level selection
1 Select the MDI mode.
2 Press function key .
3 Press soft key [PR-LEV].
Fig. 12.3.12 (b) Precision level selection screen (10.4-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1624 -
4 To change the precision level, key in a desired precision level (1
to 10), then press the key on the MDI panel.
5 When the precision level is changed, a RMS value is obtained
from the velocity-emphasized parameter set and
precision-emphasized parameter set for parameter modification.
For the modified parameters, see the description of the
machining parameter tuning.
6 If there is an axis in addition to the currently displayed axes,
press page key or several times to display the
screen for the axis.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1625 -
12.3.13 Displaying and Setting Tool Life Management Data
Displaying tool life management data on a screen enables the current
status of tool life management to be grasped. Also on the screen,
tool life management data can be edited. The screen is either:
• Tool life management (list screen) or
• Tool life management (group editing screen)
Overview
EDIT
END
List screen
Tool life management (list screen)
Displayed items:
- NEXT GROUP
- SELECTED GROUP
- GROUP NO.
- LIFE
- TOOL MANAGEMENT STATUS
- GROUP TO BE CHANGE
Functions:
- Searching for groups
- Clearing execution data
- Setting the tool life counter
Tool life management (group editing screen)
Displayed items:
- NEXT GROUP - SELECTED GROUP
- MAX.TOOL PIECES - LIFE
- T-CODE - H-CODE and D-CODE
Functions:
- Setting tool data - Setting a tool status
- Selecting too skip
- Setting a life count type, life value, and tool life
counter
Pressing horizontal soft key [EDIT] or [END]
switches from the list screen to the group editing
screen or vice versa.
Group editing screen
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1626 -
M
If the tool life management B function is enabled (bit 4 (LFB) of
parameter No. 6805 = 1), the following parameters can be used to
display arbitrary groups and remaining set values.
• If bit 5 (TGN) of parameter No. 6802 = 1
An arbitrary group is displayed on the list and group editing
screens.
• If bit 3 (GRP) of parameter No. 6802 = 1
Remaining set values are displayed on the group editing screen.
The group editing screen always displays H and D codes.
T
The T series is provided with two tool change types, turret type and
ATC type. For the T series, displays vary depending on which tool
change type is in use.
If the turret type is in use (bit 3 (TCT) of parameter No. 5040 = 0)
• Neither the H code nor the D code is used; neither is displayed.
• No arbitrary group can be used; no arbitrary group is displayed.
If the ATC type is in use (bit 3 (TCT) of parameter No. 5040 = 1)
• The D code is displayed on the group editing screen.
• If the tool life management B function is enabled (bit 4 (LFB) of
parameter No. 6805 = 1) and bit 5 (TGN) of parameter No. 6802
= 1, arbitrary groups are displayed on the list and group editing
screens.
If the tool life management B function is enabled (bit 4 (LFB) of
parameter No.6805 = 1) and bit 3 (GRP) or parameter No. 6802 = 1,
remaining set values are displayed on the group editing screen.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1627 -
12.3.13.1 Tool life management (list screen)
This screen can display the life management status of all tools in tool
groups and whether the life of the tool groups has expired. It also
enables you to set tool life counters and clear execution data.
Displays on the list screen
Procedure
1 Press function key .
2 Press the continuous menu key several times to display soft
key [TOOL LIFE].
3 Press soft key [TOOL LIFE].
Fig. 12.3.13.1 (a) Displaying tool life management (list screen) (10.4-inch)
- Contents of (A)
(A) displays tool group numbers and an override value. If there is no
tool group to display, ****, instead of tool group numbers, is
displayed.
NEXT GROUP:
Tool group number for which life counting is started by the next
M06 command.
USING GROUP:
Tool group number for which life counting is currently under
way.
SELECTED GROUP:
Tool group number for which life counting is currently under
way or life counting has been performed most recently.
COUNT OVERRIDE:
“1.0TIMES” is displayed if the tool life counter override signal is
disabled (bit 2 (LFV) of parameter No. 6801 = 0).
(A)
(B)
(C)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1628 -
NOTE
If arbitrary group numbers are enabled, NEXT
GROUP, USING GROUP, and SELECTED GROUP
are each represented with an arbitrary group number
rather than the tool group number.
- Contents of (B)
(B) displays the set life value, the current content of the tool life
counter, and the registered tool numbers (in the order they are used)
for each tool group. If the life count type is specification by duration,
the measurement unit used in displaying and specifying set life values
and tool life counter values is selected according to the setting of bit 0
(FCO) of parameter No. 6805 as listed below.
Bit 0 (FCO) of parameter No. 6805 0 1
Measurement unit used in displaying and specifying
set life values and tool life counter values
1 minute 0.1 minutes
The following table lists the prefixes used with tool numbers.
Tool status Tool in use Tool not in use
Life remaining @ No indication
Skip # #
Life expired * *
NOTE
1 The tool life counter indicates the count value for the tool
indicated with @.
2 If bit 3 (EMD) of parameter No. 6801 = 0, a tool number
remains prefixed with @ even if the life of the tool has
expired until another tool is selected.
3 If bit 3 (EMD) of parameter No. 6801 =1, the following
differences can occur depending on the type of the life
counter in use.
• If the life counter type is specification by duration, the
prefix is changed to “*” (life expired) as soon as the tool
life expires.
• If the life counter type is specification by count, the
counter is incremented by one at the end of a program
(such as M02 or M30). So, the prefix is not changed to
“*” (life expired) even if the tool life counter matches the
life value. The symbol “*” (life expired) appears when
the tool life count is incremented after the CNC is reset.
4 If bit 2 (ETE) of parameter No. 6804 = 1, the symbol “*”
indicating the expiration of the life of the last tool appears
on the tool life management screen when the life counter
for the last tool of the tool group of interest matches the life
value. This way, the information about the last tool in the
FOCAS2 or PMC window indicates that the life of the tool
has expired if the tool change signal TLCH <Fn064.0> is 1.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1629 -
If arbitrary group numbers are enabled, an arbitrary group number is
displayed in the parentheses beside the tool group number. If no
arbitrary group number is specified, “********” is displayed instead.
Fig. 12.3.13.1 (b) Displaying arbitrary group numbers
Arbitrary group numbers are enabled by setting the following
parameters.
M
• The tool life management B function is enabled (bit 4 (LFB) of
parameter No. 6805 = 1).
• Arbitrary group numbers are enabled (bit 5 (TGN) of parameter
No. 6802 = 1).
T
• The current tool change type is ATC (bit 3 (TCT) of parameter No.
5040 = 1).
• The tool life management B function is enabled (bit 4 (LFB) of
parameter No. 6805 = 1).
• Arbitrary group numbers are enabled (bit 5 (TGN) of parameter
No. 6802 = 1).
- Contents of (C)
(C) displays tool group numbers for which a tool change signal has
been issued.
If there are so many tool group numbers that all the numbers cannot be
displayed, some are omitted, and “>>” is displayed instead.
If there is no tool group number in need of change, “****” is
displayed.
NOTE
If arbitrary group numbers are enabled, a tool group
number in need of change is represented with an
arbitrary group number rather than the tool group
number.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1630 -
Setting data on the list screen
Tool life management data can be specified in the reset state (both the
OP and RST signals are “0”). However, setting bit 1 (TCI) of
parameter No. 6804 to 1 enables tool life management data to be
specified even during automatic operation (the OP signal is “1”).
NOTE
As for USING GROUP or NEXT GROUP settings:
1) During automatic operation (OP signal = “1” and
bit 1 (TCI) of parameter No. 6804 = 1), only the
tool life counter can be changed.
2) In the reset state (OP signal = “0” and RST signal
“0”), the following editing operation stops life
management because it cannot be continued.
- Clearing execution data
Procedure
- Setting the tool life counter
The tool life counter can be set with a value, using the following
methods.
Method 1
1 Place the cursor on the tool life counter for a desired tool group.
2 Enter the value from the keypad.
3 Press soft key [INPUT].
Method 2
1 Place the cursor on the tool life counter for a desired tool group.
2 Enter the value from the keypad.
3 Press key.
- Clearing execution data
All existing execution data for a tool group selected by the cursor can
be cleared as follows:
1 Place the cursor on the tool group whose execution data you
want to clear.
2 Press soft key [ERASE].
3 Press soft key [EXEC].
NOTE
Setting bit 4 (GRS) of parameter No. 6800 to 1
enables execution data for all registered tool groups
to be cleared.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1631 -
- Selecting tool groups
Tool groups can be selected using the following methods.
Method 1
1 Enter a tool group number from the keypad.
2 Press soft key [NO.SRH].
NOTE
If arbitrary group numbers are enabled, a tool group
is selected by searching for an arbitrary group
number rather than the tool group number.
Method 2
1 Press page key or to display desired groups.
2 Press cursor key or to move the cursor to the
desired group at either the left or right.
- Switching to the group editing screen
Switch to tool life management (group editing screen).
1 Move the cursor to the tool group you want to edit:
2 Press soft key [EDIT].
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1632 -
12.3.13.2 Tool life management (group editing screen)
On this screen, it is possible to edit tool life management data (such as
tool life value, tool life counter, and tool data) for the tool group of
interest.
Displaying the group editing screen
Procedure
1 Place the cursor on the tool group you want to edit from the list
screen.
2 Press soft key [(OPRT)].
3 Press soft key [EDIT].
Fig. 12.3.13.2 (a) Displaying tool life management (group editing screen)
(10.4-inch)
NOTE
If no tool is registered with a tool group, none of a life
count type, a life value, and a tool life counter value
is displayed for the tool group.
- Contents of (A)
Like the counterpart of the list screen, (A) of the editing screen
displays the next tool group number and override value. If there is
no appropriate tool group, **** is displayed instead.
NEXT GROUP:
Tool group for which life counting is started by the next M06
command.
USING GROUP:
Tool group number for which life counting is currently under
way.
(A)
(B)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1633 -
SELECTED GROUP:
Tool group number for which life counting is currently under
way or life counting has been performed most recently.
COUNT OVERRIDE:
“1.0TIMES” is displayed if the tool life counter override signal is
disabled (bit 2 (LFV) of parameter No. 6801 = 0).
NOTE
If arbitrary group numbers are enabled, NEXT
GROUP, USING GROUP, and SELECTED GROUP
are each represented with an arbitrary group number
rather than the tool group number.
- Contents of (B)
(B) details tool life management data related to a selected tool group
as follows:
TYPE : 1 Specification by count
2 Specification by duration
LIFE : Tool life value
COUNT : Tool life counter
STATE : Tool status Tool in use Tool not in use
Life remaining @ No indication
Skip # #
Life expired * *
T-CODE : Tool number
M
H-CODE
:
Tool length compensation specification code
D-CODE
:
Cutter compensation specification code
T
H-CODE
:
No display.
D-CODE
:
Tool offset value specification code
if ATC type is in use (bit 3 (TCT) of parameter No.
5040 = 1)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1634 -
NOTE
1 The tool life counter indicates the count value for
the tool indicated with @.
2 If bit 3 (EMD) of parameter No. 6801 = 0, a tool
number remains prefixed with @ even if the life of
the tool has expired until another tool is selected.
3 If bit 3 (EMD) of parameter No. 6801 = 1, the
following differences can occur depending on the
type of the life counter in use.
• If the life counter type is specification by
duration, the prefix is changed to “*” (life
expired) as soon as the tool life expires.
• If the life counter type is specification by count,
the counter is incremented by one at the end of
a program (such as M02 or M30). So, the
prefix is not changed to “*” (life expired) even if
the tool life counter matches the life value. The
symbol “*” (life expired) appears when the tool
life count is incremented after the CNC is reset.
4 If bit 2 (ETE) of parameter No. 6804 = 1, the
symbol “*” indicating the expiration of the life of the
last tool appears on the tool life management
screen when the life counter for the last tool of the
tool group of interest matches the life value. This
way, the information about the last tool in the
FOCAS2 or PMC window indicates that the life of
the tool has expired if the tool change signal TLCH
<Fn064.0> is 1.
Displaying arbitrary groups and remaining set values
Fig. 12.3.13.2 (b) Displaying arbitrary group numbers and remaining set
values on the editing screen
M
If the tool life management B function is enabled (bit 4 (LFB) of
parameter No. 6805 = 1) and the following parameters are enabled,
arbitrary groups and remaining set values are displayed.
OPTION GROUP:
Arbitrary group number
(if bit 5 (TGN) of parameter No. 6802 = 1)
REST COUNT:
Remaining set value used until a new tool is selected
(if bit 3 (GRP) of parameter No. 6802 = 1)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1635 -
T
If the tool life management B function is enabled (bit 4 (LFB) of
parameter No. 6805 = 1)
Turret type (bit 3 (TCT) of parameter No. 5040 = 0)
• OPTION GROUP:
No display.
• REST COUNT:
Remaining set value used until a new tool is selected
(if bit 3 (GRP) of parameter No. 6802 = 1)
ATC type (bit 3 (TCT) of parameter No. 5040 = 1)
• OPTION GROUP:
Arbitrary group number
(if bit 5 (TGN) of parameter No. 6802 = 1)
• REST COUNT:
Remaining set value used until a new tool is selected
(if bit 3 (GRP) of parameter No. 6802 = 1)
Setting data on the group editing screen
Tool life management data can be specified in the reset state (both the
OP and RST signals are “0”). However, setting bit 1 (TCI) of
parameter No. 6804 to “1” enables tool life management data to be
specified even during automatic operation (the OP signal is “1”).
The available editing operations are listed below.
M
Items that can be edited Mode
Setting a life count type, life value, tool life counter, and tool
data (T code, H code, and D code)
All modes
Adding tool numbers (T code) MDI
Deleting all tool group data at a time MDI
Deleting tool data (status, T code, H code, and D code) MDI
Selecting tool skip MDI
Specifying to clear tool data (life re-set) MDI
T
Items that can be edited Mode
Setting a life count type, life value, tool life counter, and tool
data (T code and D code)
However, the D code can be edited only if the ATC type
is in use (bit 3 (TCT) of parameter No. 5040 = 1).
All modes
Adding tool numbers (T code) MDI
Deleting all tool group data at a time MDI
Deleting tool data (status, T code, and D code) MDI
Selecting tool skip MDI
Specifying to clear tool data (life re-set) MDI
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1636 -
M
T
If no tool is registered with a tool group, none of a life count type, a
tool life value, and a tool life counter value can be set for the tool
group. First of all, add a tool number (T code).
NOTE
1 As for USING GROUP or NEXT GROUP editing:
<1> During automatic operation (OP signal = “1”
and bit 1 (TCI) of parameter No. 6804 = 1),
only the tool life counter can be changed.
<2> In the reset state (OP signal = “0” and RST
signal “0”), the following editing operation
stops life management because it cannot be
continued.
- Adding tool numbers (T code)
- Deleting all tool group data at a time
- Deleting tool data (status, T code, H code,
and D code)
2 The following editing operations may set the tool
change signal to ”1”.
- Selecting tool skip for the last tool.
- Deleting tool numbers, resulting in any tool other
than those whose life has expired or who have
been skipped being not found in the tool group of
interest.
3 The following editing operations may reset the tool
change signal to ”0”.
- Adding tool numbers, leading to tools whose life
has not expired being set in the tool group of
interest.
- Selecting tool clear.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1637 -
Procedure
- Setting a life count type, tool life value, tool life counter, tool data, arbitrary group
number, and remaining set value
Setting a life count type, tool life value, tool life counter, tool data,
arbitrary group number, and remaining set value
Method 1
1 Place the cursor on the desired item.
2 Enter a value from the keypad.
3 Press soft key [INPUT].
Method 2
1 Place the cursor on the desired item.
2 Enter a value from the keypad.
3 Press .
NOTE
1 Changing a tool life value or tool life counter does
not affect the tool status or tool change signal.
2 Changing a life count type causes the tool life value
and too life counter to be reset to 0.
M
If the tool life management B function is enabled (bit 4 (LFB) of
parameter No. 6805 = 1) and the following parameters are enabled,
arbitrary groups and remaining set values can be specified
OPTION GROUP:
Arbitrary group number
(if bit 5 (TGN) of parameter No. 6802 = 1)
REST COUNT:
Remaining set value used until a new tool is selected
(if bit 3 (GRP) of parameter No. 6802 = 1)
T
If the tool life management B function is enabled (bit 4 (LFB) of
parameter No. 6805 = 1)
Turret type (bit 3 (TCT) of parameter No. 5040 = 0)
• OPTION GROUP:
Cannot be set.
• REST COUNT:
It is possible to set a remaining set value to be used until a new
tool is selected (if bit 3 (GRP) of parameter No. 6802 = 1).
ATC type (bit 3 (TCT) of parameter No. 5040 = 1)
• OPTION GROUP:
Arbitrary group numbers can be set (if bit 5 (TGN) of parameter
No. 6802 = 1).
• REST COUNT:
It is possible to set a remaining set value to be used until a new
tool is selected (if bit 3 (GRP) of parameter No. 6802 = 1).
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1638 -
- Adding tool numbers
Tool numbers can be added to a tool group as follows:
1 Select the MDI mode.
2 Place the cursor on the tool data (T code, H code, or D code) just
before a tool number to be added.
3 Enter the tool number from the key pad.
4 Press soft key [INSERT].
(Example)
Adding tool number 1550 between numbers 1 and 2 (for the M
series)
1 Move the cursor to the data for number 1, enter “1550”, and
press [INSERT].
2 The entered T code 1550 is inserted in the position of
number 2. The H and D codes are reset to 0.
- Deleting all tool group data at a time
All tool group data can be deleted at a time as follows:
1 Select the MDI mode.
2 Place the cursor on the tool data (T code, H code, or D code) just
Select the tool group from which all tool data you want to delete
at a time.
3 Press soft key [DELETE].
4 Press soft key [GROUP].
5 Press soft key [EXEC].
- Deleting tool data
Tool data can be deleted from a tool group as follows:
1 Select the MDI mode.
2 Place the cursor on the tool data (T code, H code, or D code) you
want to delete.
3 Press soft key [DELETE].
4 Press soft key [<CURS>].
NOTE
1 Deleting all tools from a tool group is equivalent to
deleting the tool group itself.
2 Deleting a tool indicated with @ (in use) results in @
being moved to the previous tool whose life has
expired or which has been skipped.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1639 -
- Selecting tool skip
Tool data can be placed in a skip state as follows:
1 Select the MDI mode.
2 Place the cursor on the tool data (T code, H code, or D code) for
a tool you want to skip.
3 Press soft key [STATE].
4 Press soft key [SKIP].
- Specifying to clear tool data (life re-set)
Tool data state can be cleared as follows:
1 Select the MDI mode.
2 Place the cursor on the tool data (T code, H code, or D code) for
a tool you want to clear.
3 Press soft key [STATE].
4 Press soft key [CLEAR].
- Selecting a tool group
A tool group can be selected as follows:
Method 1
1 Enter a tool group number from the keypad.
2 Press soft key [NO.SRH].
NOTE
If arbitrary group numbers are enabled, a tool group
is selected by searching for an arbitrary group
number rather than the tool group number.
Method 2
1 Press page key or to display the target tool group.
- Switching to the list screen
The tool life management (list screen) can be resumed as follows:
1 Press soft key [END].
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1640 -
12.3.14 Displaying and Setting Workpiece Setting Error
Compensation Data
An amount of error used in workpiece setting error compensation can
be set on the workpiece setting error screen.
The workpiece setting error screen is displayed as follows:
1 Press function key .
2 Press chapter selection soft key [WORD SET ER].
The workpiece setting error screen appears.
Fig. 12.3.14 (a) Workpiece setting error screen (10.4-inch)
Up to 7 sets (No. 01 to No. 07) of different amounts of workpiece
setting error can be specified. In addition, it is possible to specify an
amount of error (No. 00 (COMMON)) to be added to an error in the 7
sets in common.
The X-direction error ∆x, Y-direction error ∆y, and Z-direction error
∆z are specified, respectively, in the x, y, and z fields. The rotational
errors ∆a, ∆b, and ∆c are specified, respectively, in the a, b, and c
fields.
Table rotation axis positions 1 and 2 are specified in the fields under
the a, b, and c fields (C and B in the figure).
Rotation axis names specified in parameter Nos. 19681 and 19686 are
displayed in the axis name fields.
Table rotation axis positions 1 and 2 are specified for rotation axes.
No position must be specified for axes (including virtual axes) other
than table rotation axes. So, no such item is displayed for setting.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1641 -
Table rotation axis position setting items are displayed under the
following conditions.
• It must have been correctly specified which axis is a table
rotation axis.
If parameter No. 19680 = 12 (table rotation type), axis numbers
must have been specified correctly in parameter Nos. 19681 and
19686.
If parameter No. 19680 = 21 (mixed type), an axis number must
have been specified correctly in parameter No. 19686.
• Bit 0 of parameter No. 1006 must be 1 (rotation axis) for the axes
specified above.
The following soft key can be used in data setting.
• After a workpiece setting error number you want to display is
entered, pressing [NO.SRH] causes a setting screen for the target
workpiece setting error to appear.
• After a number is entered, pressing soft key [+INPUT] causes the
number to be added.
• After a number is entered, pressing soft key [INPUT] causes the
number to be set.
• Pressing soft key [ERASE] causes the next soft key to appear.
• After a workpiece setting error number you want to delete is
entered, pressing soft key [NO.] causes the data corresponding to
the error number to be deleted.
• Pressing soft key [ALL] causes the data corresponding to all
workpiece setting error numbers to be deleted.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1642 -
12.3.15 Displaying and Setting Pattern Data Inputs
Described below are a method for displaying machining menus
(pattern menus) created by machine tool builders and a method for
setting them. The descriptions are based on an example. For actual
pattern menus and pattern data, refer to manuals released by respective
machine tool builders.
Displaying pattern data and pattern menus
Given below is a procedure for displaying pattern menus.
1 Press function key .
2 Press the continuous menu key .
3 Press soft key [PATTERN MENU].
The pattern menu screen shown below appears.
Fig. 12.3.15 (a) Pattern menu screen (10.4-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1643 -
On this screen, a pattern to be used can be selected.
The following two methods can be used to select patterns.
• Using the cursor
Move the cursor to a pattern name you want to select, using
cursor key or , and then press soft key [SELECT] or
.
• Specifying a pattern number
Enter a number displayed at the left side of a pattern name, and
press soft key [SELECT] or .
The custom macro screen (pattern data screen) shown below appears.
Fig. 12.3.15 (b) Custom macro screen (pattern data) (10.4-inch)
Enter the necessary pattern data, and press .
After entering all necessary data, select the MEMORY mode and
press the cycle start button. Machining begins.
Explanation
- Explanations about the pattern menu screen
HOLE PATTERN
An arbitrary character string consisting of 12 or less characters can be
displayed as a menu title.
BOLT HOLE
An arbitrary character string consisting of 10 or less characters can be
displayed as a pattern name.
Machine tool builders should program menu title and pattern name
character strings, using custom macros, and save them in program
memory.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1644 -
- Explanations about the custom macro screen (pattern data screen)
BOLT HOLE
An arbitrary character string consisting of 12 or less characters can be
displayed as a pattern data title.
TOOL.
An arbitrary character string consisting of 10 or less characters can be
displayed as a variable name.
*BOLT HOLE*
The comment text consists of nine 12-character blocks, or the
comment can be up to 12 lines (10.4-inch display) or 8 lines (7.2 or
8.4-inch display) with one block counted as one line.
Machine tool builders should program variable name and comment
text character strings, using custom macros, and save them in program
memory.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1645 -
Screens of a 15-inch display unit
12.3.16 Displaying and Entering Setting Data (15-inch Display Unit)
Data such as the TV check flag and punch code is set on the setting
data screen. On this screen, the operator can also enable/disable
parameter writing, enable/disable the automatic insertion of sequence
numbers in program editing, and perform settings for the sequence
number comparison and stop function.
See III-9.2 for automatic insertion of sequence numbers.
See III-12.3.17 for the sequence number comparison and stop function.
This subsection describes how to set data.
Procedure for setting the setting data
Procedure
1 Select the MDI mode.
2 Press function key .
3 Press vertical soft key [SETTING] to display the setting data
screen.
This screen consists of several pages.
Press page key or until the desired screen is
displayed.
An example of the setting data screen is shown below.
Fig. 12.3.16 (a) SETTING (HANDY) screen (15-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1646 -
Fig. 12.3.16 (b) SETTING (MIRROR IMAGE) screen (15-inch)
4 Move the cursor to the item to be changed by pressing cursor
keys .
5 Enter a new value and press horizontal soft key [INPUT].
Explanation
- PARAMETER WRITE
Setting whether parameter writing is enabled or disabled.
0 : Disabled
1 : Enabled
- TV CHECK
Setting to perform TV check.
0 : No TV check
1 : Perform TV check
- PUNCH CODE
Setting code when data is output through reader/puncher interface.
0 : EIA code output
1 : ISO code output
- INPUT UNIT
Setting a program input unit, inch or metric system
0 : Metric
1 : Inch
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1647 -
- I/O CHANNEL
Using channel of reader/puncher interface.
0 : Channel 0
1 : Channel 1
2 : Channel 2
- SEQUENCE NO.
Setting of whether to perform automatic insertion of the sequence
number or not at program edit in the EDIT mode.
0 : Does not perform automatic sequence number insertion.
1 : Perform automatic sequence number insertion.
- PROGRAM FORMAT
Setting of whether to use the Series 15 format.
0: Uses the standard format.
1: Uses the Series 15 format.
For the Series 15 format, refer to Chapter II-6 in the User's Manual (T
series) or Chapter II-7 of Part II in the User's Manual (M series).
- SEQUENCE STOP
Setting the sequence number with which the operation stops for the
sequence number comparison and stop function and the number of the
program to which the sequence number belongs
- MIRROR IMAGE
Setting of mirror image ON/OFF for each axes.
0 : Mirror image off
1 : Mirror image on
- Others
Page key or can also be pressed to display the
SETTING (TIMER) screen. See III-12.3.18 for this screen.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1648 -
12.3.17 Sequence Number Comparison and Stop (15-inch Display
Unit)
If a block containing a specified sequence number appears in the
program being executed, operation enters single block mode after the
block is executed.
Procedure for sequence number comparison and stop
Procedure
1 Select the MDI mode.
2 Press function key .
3 Press vertical soft key [SETTING].
4 Press page key or several times until the following
screen is displayed.
Fig. 12.3.17 (a) SETTING (HANDY) screen (15-inch)
5 Enter in (PROGRAM NO.) for SEQUENCE STOP the number
(1 to 99999999) of the program containing the sequence number
with which operation stops.
6 Enter in (SEQUENCE NO.) for SEQUENCE STOP (with eight
or less digits) the sequence number with which operation is
stopped.
7 When automatic operation is executed, operation enters single
block mode at the block containing the sequence number which
has been set.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1649 -
Explanation
- Sequence number after the program is executed
After the specified sequence number is found during the execution of
the program, the sequence number set for sequence number
compensation and stop is decremented by one.
- Exceptional blocks
If the predetermined sequence number is found in a block in which all
commands are those to be processed within the CNC control unit, the
execution does not stop at that block.
[Example] N1 #1=1 ;
N2 IF[#1 EQ 1]GOTO 08 ;
N3 GOTO 09 ;
N4 M98 P1000 ;
N5 M99 ;
In the example shown above, if the predetermined sequence number is
found, the execution of the program does not stop.
- Stop in the canned cycle
If the predetermined sequence number is found in a block which has a
canned cycle command, the execution of the program stops after the
return operation is completed.
- When the same sequence number is found several times in the program
If the predetermined sequence number appears twice or more in a
program, the execution of the program stops after the block in which
the predetermined sequence number is found for the first time is
executed.
- Block to be repeated a specified number of times
If the predetermined sequence number is found in a block which is to
be executed repeatedly, the execution of the program stops after the
block is executed specified times.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1650 -
12.3.18 Displaying and Setting Run Time, Parts Count, and Time
(15-inch Display Unit)
Various run times, the total number of machined parts, number of
parts required, and number of machined parts can be displayed.
This data can be set by parameters or on this screen (except for the
total number of machined parts and the time during which the power
is on, which can be set only by parameters).
This screen can also display the clock time. The time can be set on the
screen.
Procedure for Displaying and Setting Run Time, Parts Count and Time
Procedure
1 Select the MDI mode.
2 Press function key .
3 Press vertical soft key [SETTING].
4 Press page key or several times until the following
screen is displayed.
Fig. 12.3.18 (a) SETTING (TIMER) screen (15-inch)
5 To set the number of parts required, move the cursor to PARTS
REQUIRED and enter the number of parts to be machined.
6 To set the clock, move the cursor to DATE or TIME, enter a new
date or time, then press horizontal soft key [INPUT].
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1651 -
Explanation
- PARTS TOTAL
This value is incremented by one when M02, M30, or an M code
specified by parameter No. 6710 is executed. This value cannot be set
on this screen. Set the value in parameter No. 6712.
- PARTS REQUIRED
It is used for setting the number of machined parts required.
When the "0" is set to it, there is no limitation to the number of parts.
Also, its setting can be made by the parameter No 6713.
- PARTS COUNT
This value is incremented by one when M02, M30, or an M code
specified by parameter No. 6710 is executed. The value can also be set
by parameter No. 6711. In general, this value is reset when it reaches
the number of parts required. Refer to the manual issued by the
machine tool builder for details.
- POWER ON
Displays the total time which the power is on. This value cannot be set
on this screen but can be preset in parameter No. 6750.
- RUN TIME
Indicates the total run time during automatic operation, excluding the
stop and feed hold time.
This value can be preset in parameter No. 6751 or No. 6752.
- CUTTING TIME
Displays the total time taken by cutting that involves cutting feed such
as linear interpolation (G01) and circular interpolation (G02 or G03).
This value can be preset in parameter No. 6753 or No. 6754.
- FREE PURPOSE
This value can be used, for example, as the total time during which
coolant flows. Refer to the manual issued by the machine tool builder
for details.
- CYCLE TIME
Indicates the run time of one automatic operation, excluding the stop
and feed hold time. This is automatically preset to 0 when a cycle start
is performed at reset state. It is preset to 0 even when power is
removed.
- DATA and TIME
Displays the current date and time. The date and time can be set on
this screen.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1652 -
- Usage
When the command of M02 or M30 is executed, the total number of
machined parts and the number of machined parts are incremented by
one. Therefore, create the program so that M02 or M30 is executed
every time the processing of one part is completed. Furthermore, if an
M code set to the parameter No. 6710 is executed, counting is made in
the similar manner. Also, it is possible to disable counting even if
M02 or M30 is executed (bit 0 (PCM) of parameter No. 6700 is set to
1). For details, see the manual issued by machine tool builders.
Limitation
- Run time and part count settings
Negative value cannot be set. Also, the setting of "M" and "S" of run
time is valid from 0 to 59.
Negative value may not be set to the total number of machined parts.
- Time settings
Neither negative value nor the value exceeding the value in the
following table can be set.
Table 12.3.18 (a)
Item Maximum value Item Maximum value
Year 2096 Hour 23
Month 12 Minute 59
Day 31 Second 59
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1653 -
12.3.19 Displaying and Setting the Workpiece Origin Offset Value
(15-inch Display Unit)
Displays the workpiece origin offset for each workpiece coordinate
system (G54 to G59, G54.1 P1 to G54.1 P48 and G54.1 P1 to G54.1
P300) and external workpiece origin offset.
The workpiece origin offset value and external workpiece origin offset
value can be set on this screen.
Procedure for displaying and setting the workpiece origin offset value
Procedure
1 Press function key .
2 Press vertical soft key [WORK].
The workpiece coordinate system setting screen is displayed.
Fig. 12.3.19 (a) WORK COORDINATES screen (15-inch)
3 The screen for displaying the workpiece origin offset values
consists of two or more pages.
Display a desired page in either of the following two ways:
• Press the page key or .
• Enter the workpiece coordinate system number (0 : external
workpiece origin offset, 1 to 6: workpiece coordinate
systems G54 to G59, P1 to P48 : workpiece coordinate
systems G54.1 P1 to G54.1 P48, P1 to P300 : workpiece
coordinate systems G54.1 P1 to G54.1 P300) and press
horizontal soft key [NO.SRH].
4 Turn off the data protection key to enable writing.
5 Move the cursor to the workpiece origin offset to be changed.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1654 -
6 Enter a desired value by pressing numeric keys, then press
horizontal soft key [INPUT]. The entered value is specified in the
workpiece origin offset value. Or, by entering a desired value
with numeric keys and pressing horizontal soft key [+INPUT],
the entered value can be added to the previous offset value.
7 Repeat steps 5 and 6 to change other offset values.
8 Turn on the data protection key to disable writing.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1655 -
12.3.20 Direct Input of Workpiece Origin Offset Value Measured
(15-inch Display Unit)
This function is used to compensate for the difference between the
programmed workpiece coordinate system and the actual workpiece
coordinate system. The measured offset for the origin of the
workpiece coordinate system can be input on the screen such that the
command values match the actual dimensions.
Selecting the new coordinate system matches the programmed
coordinate system with the actual coordinate system.
Procedure for direct input of workpiece origin offset value measured
Procedure
y
Programmed workpiece
origin
New offset
Previous offset
Origin
O'
Y
Surface A
Surface B
β
α
X
x
O
1 When the workpiece is shaped as shown above, position the
reference tool manually until it touches surface A of the
workpiece.
2 Retract the tool without changing the Y coordinate.
3 Measure distance α between surface A and the programmed
origin of the workpiece coordinate system as shown above.
4 Press function key .
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1656 -
5 To display the WORK COORDINATES screen, press vertical soft
key [WORK].
Fig. 12.3.20 (a) WORK COORDINATES screen (15-inch)
6 Position the cursor to the workpiece origin offset value to be set.
7 Press the address key for the axis along which the offset is to be
set (Y-axis in this example).
8 Enter the measured value (α) then press horizontal soft key
[MEASUR].
9 Move the reference tool manually until it touches surface B of
the workpiece.
10 Retract the tool without changing the X coordinate.
11 Enter the measured value of distance (β) to surface B as an X
value as with steps 7 and 8.
Limitation
- Consecutive input
Offsets for two or more axes cannot be input at the same time.
- During program execution
This function cannot be used while a program is being executed.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1657 -
12.3.21 Displaying and Setting Custom Macro Common Variables
(15-inch Display Unit)
Displays common variables (#100 to #149 or #100 to #199, and #500
to #531 or #500 to #999) on the screen.
The values for variables can be set on this screen.
Relative coordinates can also be set to variables.
Procedure for displaying and setting custom macro common variables
Procedure
1 Press function key .
2 Press vertical soft key [MACRO].
The following screen is displayed.
Fig. 12.3.21 (a) CUSTOM MACRO screen (15-inch)
3 Move the cursor to the variable number to set using either of the
following methods:
• Enter the variable number and press horizontal soft key
[NO.SRH].
• Move the cursor to the variable number to set by pressing
page keys and/or and cursor keys ,
, , and/or .
4 Enter data with numeric keys and press horizontal soft key
[INPUT].
5 To set a relative coordinate in a variable, press address key ,
, or , then press horizontal soft key [INP.C.].
6 To set a blank in a variable, just press horizontal soft key
[INPUT]. The value field for the variable becomes blank.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1658 -
Explanation
If the value of a variable produced by an operation is not displayable,
an indication below is provided.
When the significant number of digits is 12 (with bit 0 (F16) of
parameter No. 6008 set to 0):
Variable value range Variable value indication
0 < Variable value < +0.00000000001 +Underflow
0 > Variable value > -0.00000000001 -Underflow
Variable value > 999999999999 +Overflow
Variable value < -999999999999 -Overflow
When the significant number of digits is 8 (with bit 0 (F16) of
parameter No. 6008 set to 1):
Variable value range Variable value indication
0 < Variable value < +0.0000001 +Underflow
0 > Variable value > -0.0000001 -Underflow
Variable value > 99999999 +Overflow
Variable value < -99999999 -Overflow
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1659 -
12.3.22 Displaying and Setting Real Time Custom Macro Data
(15-inch Display Unit)
Real time macro variables (RTM variables) are dedicated to real time
custom macros.
RTM variables are divided into temporary real time macro variables
(temporary RTM variables) and permanent real time macro variables
(permanent RTM variables).
The values of permanent RTM variables are kept stored after the
power is turned off.
Temporary RTM variables are cleared to 0 when the power is turned
off.
System variables (DI/DO variables) dedicated to real time custom
macros are used to read and write PMC interface signals. Data can be
read and written in bit and byte units. Before writing a signal, release
the protection of the corresponding variable on the PMC signal protect
screen.
Displaying and setting real time custom macro variables
Procedure
1 Press function key .
2 Press vertical soft key [NEXT PAGE] several times and then
vertical soft key [R.TIME MACRO]. The screen shown below
appears.
Fig. 12.3.22 (a) REAL TIME MACRO screen (15-inch)
3 To display or set real time custom macro variables of which
values are not stored at power-off, press vertical soft key [TEMP.
DATA].
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1660 -
4 To display or set real time custom macro variables of which
values are stored at power-off, press vertical soft key [PERM.
DATA].
5 Move the cursor to the number of a real time custom macro
variable you want to set using either of the following methods:
• Enter the number of a real time custom macro variable and
press horizontal soft soft key [NO. SRH].
• Move the cursor to the number of a real time custom macro
variable you want to set by pressing page keys
and/or and cursor keys , , , and/or
.
6 Enter data.
Displaying and setting DI/DO variables
Procedure
For setting in byte units:
1 Press function key .
2 Press vertical soft key [NEXT PAGE] several times and then
vertical soft key [R.TIME MACRO]. The screen shown below
appears.
3 Press vertical soft key [BYTE SELECT]. The following screen
appears:
Fig. 12.3.22 (b) BYTE SELECT screen (15-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1661 -
4 Move the cursor to the number of a DI/DO variable you want to
set using either of the following methods:
• Enter the number and press horizontal soft key [NO. SRH].
• Move the cursor to a desired number by pressing page keys
and/or and cursor keys , , ,
and/or .
5 Enter data.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1662 -
12.3.23 Displaying and Setting the Software Operator’s Panel
(15-inch Display Unit)
Operations on the MDI panel can substitute for the functions of
switches on the machine operator’s panel. This means that a mode
selection, jog feed override selection, and so forth can be made with
operations on the MDI panel, eliminating the need to use the
corresponding switches on the machine operator’s panel.
Jog feed can be performed using numeric keys.
Procedure for displaying and setting the software operator’s panel
Procedure
1 Press function key .
2 Press vertical soft key [NEXT PAGE] and then vertical soft key
[OPERAT PANEL].
3 The screen consists of several pages. Press page key or
until the desired screen is displayed.
Fig. 12.3.23 (a) Without the manual handle feed function (15-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1663 -
Fig. 12.3.23 (b) With the manual handle feed function (15-inch)
Fig. 12.3.23 (c) (15-inch)
4 Move the cursor to the desired switch by pressing cursor key
or .
5 Push the cursor key or to match the mark to an
arbitrary position and set the desired condition.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1664 -
6 Press one of the following arrow keys to perform jog feed. Press
the key together with an arrow key to perform jog rapid
traverse.
Fig. 12.3.23 (d) MDI arrow keys
Explanation
- Valid operations
The valid operations on the software operator's panel are shown below.
Whether to use each group can be chosen using parameter No. 7200.
Those groups that are not used are not displayed on the software
operator's panel.
Group1 : Mode selection
Group2 : Selection of jog feed axis, Manual rapid traverse
Group3 : Selection of manual pulse generator feed axis, selection of
manual pulse magnification
Group4 : Jog federate, federate override, rapid traverse override
Group5 : Optional block skip, single block, machine lock, dry run
Group6 : Protect key
Group7 : Feed hold
- Screens on which jog feed is valid
When the LCD indicates other than the software operator's panel
screen and self-diagnosis screen, jog feed is not conducted even if the
arrow key is pushed.
- Jog feed and arrow keys
The feed axis and direction corresponding to the arrow keys can be set
with parameters (Nos. 7210 to 7217).
- General purpose switches
For the meanings of these switches, refer to the manual issued by
machine tool builder.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1665 -
12.3.24 Setting and Displaying Tool Management Data (15-inch
Display Unit)
The tool management function totally manages tool information
including tool offsets and tool life information.
This function provides a magazine screen and tool management screen.
This subsection explains how to set these screens.
12.3.24.1 Displaying and setting magazine screen (15-inch display unit)
Procedure
1 Press function key .
2 Press vertical soft key [NEXT PAGE] several times and then
vertical soft key [TOOL MANAGER]. The screen shown below
appears.
Fig. 12.3.24.1 (a) ) Tool management magazine screen (15-inch)
3 By using the page keys, cursor keys, and horizontal soft keys
[←] and [→], move the cursor to the pot No. position of the
magazine for which you want to set or modify data.
Alternatively, type the number of the tool management data you
wan to set or modify, and press horizontal soft key [NO. SRH].
4 Press horizontal soft key [EDIT].
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1666 -
5 To set the tool management data number of a pot, type the tool
management data number, then press MDI key .
To delete the tool management data number set for a pot, follow
the steps below.
<1> Press horizontal soft key [ERASE].
<2> Press horizontal soft key [CURDAT]. To delete the tool
management data numbers registered for all pots, press
horizontal soft key [ALL].
<3> Press horizontal soft key [EXEC]. Alternatively, type 0.
6 To end the edit operation, press horizontal soft key [EXIT].
This returns the screen display to the conventional tool
management screen.
Explanation
- Another method
Magazine data can be input/output also by using external I/O devices.
See III-8, "DATA I/O".
- Displayed data
Pot : As many pots as specified in parameter No. 13222, 13227,
13232, or 13237 (settable for each magazine) are displayed.
The starting pot number can be set for each magazine in
parameter No. 13223, 13228, 13233, or 13238.
NO. : Tool management data numbers are displayed.
In the following cases, tools cannot be set in magazines:
1. A tool management data number beyond the range from 0 to
(the number of valid pairs in parameter No. 13220) is set.
2. Tool management data is invalid (bit 1 of tool information is
0).
3. The tool management data number to be set is already set for
another pot.
Type No. : Tool type numbers corresponding to tool management data
numbers are displayed.
Values cannot be set on this screen.
Spindle : The tool management data numbers and tool type numbers
of spindle positions are displayed.
Wait : The tool management data numbers and tool type numbers
of wait positions are displayed.
- Edit mode
To edit data, press horizontal soft key [EDIT] to enter tool
management data edit mode.
- Tool management data number
Tool management data numbers can optionally be extended to 64, 240,
or 1000 pairs. In addition, the number of tools used can be set in
parameter No. 13220.
- Display of the spindle positions and wait positions
The spindle position and wait position can be set for each path.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1667 -
12.3.24.2 Displaying and setting tool management screen (15-inch
display unit)
Procedure
1 Press function key .
2 Press vertical soft key [NEXT PAGE] several times and then
vertical soft key [TOOL MANAGER].
3 Press vertical soft key [TOOL].
Fig. 12.3.24.2 (a) Tool management data screen (15-inch)
4 By using the page keys, cursor keys, and horizontal soft keys
[←] and [→], move the cursor to the position of the tool
information of the tool number for which you want to set or
modify data.
Alternatively, type the tool number of the data you want to set or
modify, and press horizontal soft key [NO. SRH].
5 Press horizontal soft key [EDIT].
6 To set tool data, type a desired value, then press MDI key .
To delete tool information, follow the steps below.
<1> In step 4, move the cursor to the tool information you want
to erase.
<2> Press horizontal soft key [ERASE].
<3> Press horizontal soft key [CURDAT]. To delete entire tool
information, press horizontal soft key [ALL].
<4> Press horizontal soft key [EXEC].
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1668 -
7 To end the edit operation, press horizontal soft key [EXIT].
This returns the screen display to the conventional tool
management screen.
Fig. 12.3.24.2 (b) Tool management data screen (check function)
(15-inch)
8 When horizontal soft key [CHECK] is pressed, if there are tools
with the same number but with different count types (count and
time), the cursor moves to the tool type number of the smallest
tool management number in the tool type numbers and a warning
message appears.
The warning messages issued by the check function are shown
below.
<1> For the same type of tools with different count types
L-COUNT TYPE MISMATCH:XXXXXXXX
<2> For the same type of tools with the same count type
L-COUNT TYPE MATCH
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1669 -
Explanation
- Another method
Tool management data, customize data, and names set for tool states
can be input/output also by using external I/O devices.
See III-8, "DATA I/O".
- Displayed information
• Life information
Fig. 12.3.24.2 (c) Tool management data life status screen(15-inch)
NO. : Tool management data numbers are displayed. These
numbers can be displayed but cannot be set. The tool
management data number of edited data is kept blinking
until tool management data edit mode ends. Tool
management data numbers set or deleted on the magazine
screen also blink on the tool management screen.
Type No. : Tool type numbers are displayed.
A value from 0 to 99,999,999 can be set.
MG : The magazine number assigned to each tool is indicated.
These numbers can be displayed but cannot be set.
Pot : The pot number assigned to each tool is indicated.
These numbers can be displayed but cannot be set.
Tool information: The following five types of information are
displayed sequentially from the right:
• Tool management data: Valid (R)/invalid (-))
• Life count type: Time (T)/count (C)
• Tool type: Oversize tool (B)/
normal tool (N)
• Data access: Locked (L)/unlocked (U)
• When a tool is not under life management:
Included in the tools to be searched
(1)/not included in the tools to be
searched (0)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1670 -
NOTE
1 The tool types and data access information vary
depending on the specifications defined by the
machine tool builder.
2 The same type of tools must have the same life
count type.
Life counter: The number of use times/use period of time of each
tool is indicated.
Up to 99,999,999 times or 999 hours 59 minutes 59
seconds can be set.
Maximum life: The maximum life value of each tool is indicated.
Up to 99,999,999 times or 999 hours 59 minutes 59
seconds can be set.
Noticed life: Noticed life value of a tool
Up to 99,999,999 times or 999 hours 59 minutes 59
seconds can be set.
Life state: Current tool state
One of the four states, including invalid (0), present (1,
2), not present (3), and broken (4), is indicated. The
numbers in parentheses are data values used when
these states are input in MDI.
• Spindle speed/feedrate
Fig. 12.3.24.2 (d) Tool management data spindle speed/feedrate screen
(15-inch)
S : Spindle speed.
A value from 0 to 99,999 can be set.
F : Feedrate.
A value from 0 to 99,999,999 can be set.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1671 -
• Tool offset information
Fig. 12.3.24.2 (e) Tool management data tool offset screen (15-inch)
H : Tool length compensation number (for machining center
systems only).
A value from 0 to 999 can be set.
D : Cutter compensation number (for machining center systems
only).
A value from 0 to 999 can be set.
TG : Tool geometry compensation number (for lathe systems only).
A value from 0 to 999 can be set.
TW : Tool wear compensation number (for lathe systems only).
A value from 0 to 999 can be set.
The displayed offset data is determined depending on the option
configuration and parameter settings (bits 1(DCR), 2(DOY), 3(DOB),
4(DO2), 6(DOT), and 7(DOM) of parameter No. 13202).
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1672 -
• Customize information
Fig. 12.3.24.2 (f) Tool management data customize data screen (15-inch)
Customize 0 : Bit-type customize information.
For each bit, 1 or 0 can be input.
Customize 1 to 4 : Customize information. Any value from
-99,999,999 to 99,999,999 can be set.
Customize 5 to 20 : Customize information. These items are
displayed only when customize data extension
option (5 to 20) of the tool management
function is enabled. Any value from
-99,999,999 to 99,999,999 can be set.
Customize 21 to 40 : Customize information. These items are
displayed only when customize data extension
option (5 to 40) of the tool management
function is enabled. Any value from
-99,999,999 to 99,999,999 can be set.
- Tool management data number
Tool management data numbers can optionally be extended to 64, 240,
or 1000 pairs. The number of tools used can be set in parameter No.
13220.
- Edit mode
To edit data, press horizontal soft key [EDIT] to enter tool
management data edit mode.
- Life count override
When the period of time is set as the tool life count type, the life count
can be overridden if bit 2 (LFV) of parameter No. 6801 is set to 1.
Specify an override value by using a switch on the machine operator's
panel.
Example) When cutting is performed for 10 minutes with an override
of 0.1, one minute is counted in the tool life counter.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1673 -
- Tool management extension function
When tool management extension functions are enabled, you can use
the following functions in addition to the tool management functions:
• A value with a decimal point can be set as customize data.
The maximum number of decimal places can be set to 7 by G10
data input and file read.
• Various types of tool management data can be protected using
KEY signals.
An attempt to enter a value to a protected data causes a warning
message “WRITE PROTECT.”
• Tool life count period selection
Bit 5 of tool information is used to make a life count period
selection.
Item Description
Data length 1 byte (flag data)
#5 REV 0: A life count period of 1 sec is used.
1: A life count period of 8 msec is used.
Range of count is as follows.
1sec : 0 to 3,599,999 seconds (999 hours 59 minutes 59 seconds)
8msec : 0 to 3,599,992 ms (59 minutes 59 seconds 992 milliseconds)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1674 -
12.3.24.3 Each tool data screen (15-inch display unit)
Each tool data screen
Procedure
1 Press function key .
2 Press vertical soft key [NEXT PAGE] several times and then
vertical soft key [TOOL MANAGER].
3 Press vertical soft key [EACH TOOL]. The each tool data screen
appears.
Fig. 12.3.24.3 (a) Each tool data screen (15-inch)
Explanation
- Header
The following four data items are displayed: NO., TYPE NO., MG,
and POT.
When the data table of a tool extends over two or more pages, the
same header is displayed on these pages.
- Data table
The data table shows data items related to a tool at a time.
The data items are displayed from the upper left to the lower left, the
upper right, and the lower right in ascending order of screen display
position numbers specified using the customize function. The number
of digits displayed for one data item is fixed to 11.
Up to 24 data items are displayed on one page. (12 data items × 2
columns)
When more than 24 data items are set for a tool, the 25th and
subsequent data items are displayed on the next page. (Up to three
pages)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1675 -
When a data item is set as a screen element of the tool management
data screen twice or more using the tool management data display
customize function (one of the tool management extension functions),
only the data item with the smaller display position number is
displayed. When no value is set for a data item, the field for the data
item is not displayed and the next data item is displayed.
Key operations
- MDI key operations
• Numeral keys Inputs a numeric value.
• Displays the previous page for the same tool.
• Displays the next page for the same tool.
• Moves the cursor to the previous data item.
When the cursor is on the top row of the data
table, it moves to the bottom row of the left
column. When the cursor is on the first data item,
it moves to the last data item.
• Moves the cursor to the next data item.
When the cursor is on the bottom row of the data
table, it moves to the top row of the right column.
When the cursor is on the last data item, it moves
to the first data item.
• Moves the cursor left on the screen.
When the cursor is on the left column of the data
table, it moves to the right column on the row
immediately above. When the cursor is on the
first data item, it moves to the last data item.
• Moves the cursor right on the screen.
When the cursor is on the right column of the
data table, it moves to the left column on the row
immediately below. When the cursor is on the
last data item, it moves to the first data item.
- Soft key operations
Horizontal soft key [EDIT]
Enters the management data edit mode.
Horizontal soft key [NO.SRH]
Displays data with a tool management data number when pressed
after the tool management data number is entered.
Horizontal soft key [PREV.TOOL]
Returns to the previous tool management data number.
Horizontal soft key [NEXT.TOOL]
Proceeds to the next tool management number.
Horizontal soft key [READ]
Reads data related to the tool management function.
Can be used only in the standard mode.
Requires placing the NC in the EDIT mode.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1676 -
Horizontal soft key [PUNCH]
Writes data related to the tool management function.
Can be used only in the standard mode.
Requires placing the NC in the EDIT mode.
Operation in the management data edit mode
To edit data, press horizontal soft key [EDIT] to enter the
management data edit mode.
Fig. 12.3.24.3 (b) Each tool data editing screen (15-inch)
In the management data edit mode, “EDITING” is displayed at the
lower right of the screen.
In the management data edit mode, the following key operations, in
addition to those mentioned above except [READ] and [PUNCH], can
be performed.
•
Actually writes a value entered using numeric keys.
• Horizontal soft key [END]
Ends the management data edit mode.
Operations for editing tool information are the same as those on the
tool management data screen.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1677 -
12.3.24.4 Displaying the total life of tools of the same type (15-inch
display unit)
Total life data screen
Procedure
1 Press function key .
2 Press vertical soft key [NEXT PAGE] several times and then
vertical soft key [TOOL MANAGER].
3 Press vertical soft key [TOTAL LIFE]. The total life data screen
appears.
4 Using horizontal soft key [CHANGE] can switch total tool life
data displays between specification by count and specification by
duration.
Fig. 12.3.24.4 (a) Count display (15-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1678 -
Fig. 12.3.24.4 (b) Time display (15-inch)
Displayed information
S-NO. : Sequential number of each tool type
TYPE NO. : Tool type number
T-REM-LIFE : Total of remaining life values of tools with the same
tool type number
T-L-COUNT : Total of used counts/times of tools with the same
tool type number
T-MAX-LIFE : Total of maximum life values of tools with the same
tool type number
T-NOTICE-L : Total of notice life values of tools with the same tool
type number when the tool life arrival signal is to be
output for each tool type
STATUS : Whether the tool life arrival signal has been output
when the signal is to be output for each tool type
Either of the two states (UNDONE and DONE) is
displayed.
NUM : Number of tools with the same tool type number
When bit 3 (ETE) of parameter No. 13200 is set to 0 and bit 2 (TRT)
of parameter No. 13200 is set to 1, the tool life arrival signal is to be
output for each tool type number and T-NOTICE-L and STATUS are
displayed.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1679 -
Key operations
- MDI key operations
Displays the previous page. The cursor moves to the last data
item on that page.
Displays the next page. The cursor moves to the first data item
on that page.
Moves the cursor up on the screen.
Moves the cursor down on the screen.
Disabled.
Disabled.
- Soft key operations
Horizontal soft key [DETAIL]
Displays the detailed life data screen.
Horizontal soft key [UPDATE]
Updates data displayed on the total life data screen.
Horizontal soft key [CHANGE]
Switch the display between the count and time types.
Horizontal soft key [T-TYPENO. SRH]
Moves the cursor to a tool type number when pressed after the
number is entered.
Horizontal soft key [T-ASCE -SORT]
Sorts data in ascending order of tool type numbers.
Horizontal soft key [T-DESC -SORT]
Sorts data in descending order of tool type numbers.
Horizontal soft key [R-ASCE -SORT]
Sorts data in ascending order of remaining life values.
Horizontal soft key [R-DESC -SORT]
Sorts data in descending order of remaining life values.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1680 -
NOTE
1 After horizontal soft key [T-ASCE -SORT],
[T-DESC -SORT], [R-ASCE -SORT], or [R-DESC
-SORT] is pressed, the cursor is positioned at the
top of page 1 of the total life data screen.
2 When the power is turned on, data of the count
counting type is displayed in ascending order of
tool type numbers. When the display type is
changed or data is sorted in a different order, the
status is kept.
3 If horizontal soft key [DETAIL] is pressed when no
data is displayed on the total life data screen, the
warning message “NO DETAILED LIFE DATA
SCREEN” is output.
4 If an unregistered tool type is specified and
horizontal soft key [T-TYPENO. SRH] is pressed,
the warning message “UNREGISTERED
NUMBER” is output.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1681 -
Detailed life data screen
Procedure
1 Press function key .
2 Press vertical soft key [NEXT PAGE] several times and then
vertical soft key [TOOL MANAGER].
3 Press vertical soft key [TOTAL LIFE]. The total life data screen
appears.
4 Selecting horizontal soft key [DETAIL] causes the detailed life
data screen to appear.
Fig. 12.3.24.4 (c) Detailed life data screen (15-inch)
- Displayed information
TYPE NO. : Tool type number
ORDER : Sequential number in ascending order of remaining life
times or the order in which the customize data is set.
NO. : Tool management data number
REM-LIFE : Remaining life value obtained by subtracting the life
count value from the maximum life value
L-COUNT : Total used count or time of the tool
MAX-LIFE : Maximum life value of the tool
NOTICE-L : Notice life value of the tool
STATUS : Life status of the tool
One of the four states (NO-MNG (0), ENABLE (1, 2),
NONE (3), and DAMAGED (4)) is displayed.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1682 -
Key operations
- MDI key operations
Displays the previous page.
Displays the next page.
Moves the cursor up on the screen. The cursor moves to the
last data item on that page.
Moves the cursor down on the screen. The cursor moves to the
first data item on that page.
Disabled.
Disabled.
- Soft key operations
Horizontal soft key [UPDATA]
Updates data displayed on the detailed life data screen.
The cursor is positioned at the beginning of page 1 after this soft
key is pressed.
Horizontal soft key [CLOSE]
Closes the detailed life data screen and returns to the total life
data screen.
NOTE
1 When horizontal soft key [CLOSE] is pressed and
the total life data screen is displayed again, the
cursor on the total life screen data is positioned as
follows.
2 When the tools with the tool type number displayed
when the detailed data screen is closed are
registered as tool management data, the cursor on
the total life screen is positioned at that tool type
number.
3 When the tools with the tool type number displayed
when the detailed data screen is closed are not
registered as tool management data, the cursor on
the total life data screen is positioned at the first
total life data.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1683 -
12.3.24.5 Tool geometry data screen (15-inch display unit)
Tool geometry data screen
Procedure
1 Press function key .
2 Press vertical soft key [NEXT PAGE] several times and then
vertical soft key [TOOL MANAGER].
3 Selecting vertical soft key [TOOL-GEOM] causes the tool
geometry data screen to appear.
Fig. 12.3.24.5 (a) Tool geometry data screen (15-inch)
- Displayed item
NO. : Tool geometry number
Up to 20 numbers can be displayed.
LEFT : Sets the number of pots on the left of the reference pot that
are to be occupied.
A value between 0 and 4 can be set.
RIGHT : Sets the number of pots on the right of the reference pot
that are to be occupied.
A value between 0 and 4 can be set.
UPPER : Sets the number of pots above the reference pot that are to
be occupied.
A value between 0 and 4 can be set. (Use this item when
the magazine is of the matrix type.)
LOWER : Sets the number of pots under the reference pot that are to
be occupied.
A value between 0 and 4 can be set. (Use this item when
the magazine is of the matrix type.)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1684 -
Key operations
- Operations in the standard mode
MDI key operations
Numeral keys Inputs a numeric value.
Moves the cursor up on the screen.
Moves the cursor down on the screen.
Moves the cursor left on the screen.
Moves the cursor right on the screen.
Soft key operations
Horizontal soft key [NO.SRH]
Moves the cursor on a tool geometry number when pressed after
the number is entered.
Horizontal soft key [EDIT]
Enters the data edit mode.
Horizontal soft key [READ]
Reads data related to the tool management functions.
This key is available only in the standard mode.
Put the NC in the EDIT mode.
Horizontal soft key [PUNCH]
Punches data related to the tool management functions.
This key is available only in the standard mode.
Put the NC in the EDIT mode.
In the management data edit mode, the following key operations, in
addition to [NO.SRH] mentioned above, can be performed.
- Operations in the edit mode
To edit data, press horizontal soft key [EDIT] to enter the edit mode.
In the edit mode, “EDITING” is displayed at the lower right of the
screen.
MDI key operation
Actually writes a value entered using numeric keys.
Soft key operation
Horizontal soft key [END]
Ends the data edit mode.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1685 -
Example
Set the edit mode. When the tool geometry with tool geometry number
1 occupies 1 pot in the left direction, 0.5 pots in the right direction,
and 1.5 pots in the down direction, set data as shown in the figure
below:
Fig. 12.3.24.5 (b) Example of setting data on the tool geometry data
screen (15-inch)
- Display of occupied pots in the magazine management table
Each pot occupied by a tool stored in another pot is indicated with an
asterisk (*).
Fig. 12.3.24.5 (c) Magazine management table (15-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1686 -
If a tool to be registered for a magazine is determined to interfere with
another tool, the warning message “TOOL INTERFERENCE CHECK
ERROR:xxxx,xxxx” is displayed. xxxx indicates the tool number of
each of the two tools. If a tool is determined to interfere with
multiple tools, only the first tool detected by the NC interference
check is displayed.
If a tool is determined to interfere with the frame of a magazine, the
tool number of the tool to be stored and “FRAME” are displayed.
- Search for an empty pot for a oversize tool
During the management data editing, a horizontal soft key for
searching for empty oversize tool pots is displayed.
Fig. 12.3.24.5 (d) Searching for an empty pot for a oversize tool (15-inch)
Enter the tool geometry number in the key-in buffer and press a search
horizontal soft key. The cursor moves to an empty pot fit for the
geometry.
EMPTY-SRCH.N: Searches for an empty pot forward.
EMPTY-SRCH.P: Searches for an empty pot backward.
EMPTY-SRCH: Searches for the pot nearest to the current
position.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1687 -
- Tool management screen
You can use bit 2 of tool information to switch between a oversize
tool and normal tool. For a oversize tool, set a tool geometry number
fit for the tool.
Fig. 12.3.24.5 (e) Bit for switching between a normal tool and oversize
tool (15-inch)
Fig. 12.3.24.5 (f) Tool geometry number (15-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1688 -
12.3.25 Displaying and Switching the Display Language (15-inch
Display Unit)
The language used for display can be switched to another language.
A display language can be set using a parameter. However, by
modifying the setting of the display language on this screen, the
display language can be switched without turning off then on the
power.
Displaying and setting the display language
Procedure
1 Press function key .
2 Press vertical soft key [NEXT PAGE] several times to display
soft key [LANGUAGE].
3 Press vertical soft key [LANGUAGE] to display the language
screen.
Fig. 12.3.25 (a) LANGUAGE screen (15-inch)
4 Press page key or , then press cursor keys ,
to move the cursor to a desired display language.
5 Press horizontal soft key [APPLY]. The display language is
switched to the selected language. The language specified on this
screen continues to be used if the power is turned off then back
on.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1689 -
Explanation
- Language switching
The language screen can be displayed if bit 0 (NLC) of parameter No.
3280 is set to 0.
- Selectable languages
The display languages selectable on this screen are as follows:
1. English
2. Japanese
3. German
4. French
5. Chinese (Traditional)
6. Chinese (Simplified)
7. Italian
8. Korean
9. Spanish
10. Dutch
11. Danish
12. Portuguese
13. Polish
14. Hungarian
15. Swedish
16. Czech
17. Russian
18. Turkish
Among the languages listed above, English and other usable
languages are displayed on the screen as a list of switchable
languages.
Limitation
- Language parameter modification on the parameter screen
Which language to be used for display is specified with parameter No.
3281. This parameter can be modified using the parameter screen as
well. However, if a modification is made on the parameter screen, the
new setting is not reflected until "APPLY" operation is performed on
the language screen or the power is turned on again. If an invalid
value is set in parameter No. 3281 on the parameter screen, the screen
is displayed in English after the power is turned on again.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1690 -
12.3.26 Protection of Data at Eight Levels (15-inch Display Unit)
You can set eight CNC and PMC operation levels and one of eight
protection levels for each type of CNC and PMC data.
When an attempt is made to change CNC and PMC data or output it to
an external unit, the operation level is compared with the protection
level to determine whether to allow the change or external output.
12.3.26.1 Operation level setting (15-inch display unit)
You can set eight CNC and PMC operation levels.
Displaying and setting the operation level setting screen
Procedure
1 Press function key .
2 Press vertical soft key [NEXT PAGE] several times to display
soft key [PROTECT].
3 Press vertical soft key [PROTECT].
The operation level setting screen shown below is displayed.
Fig. 12.3.26.1 (a) Operation level setting screen (15-inch)
4 Key in the password for an operation level to be set/modified,
then press horizontal soft key [INPUT PASSWD].
5 To return the operation level to 0, 1, 2, or 3, press horizontal soft
key [CANCEL PASSWD].
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1691 -
Explanation
- Operation level setting
To select operation level 0 to 3, use the corresponding memory
protection key signal.
To select operation level 4 to 7, use the corresponding password.
Table 12.3.26.1 (a) Operation level setting
Operation level Setting Sample grouping
7 (high) Password -
6 Password MTB
5 Password Dealer and integrator
4 Password End user
3 Memory protection key signal User level (level 1)
2 Memory protection key signal User level (level 2)
1 Memory protection key signal User level (level 3)
0 (low) Memory protection key signal User level (level 4)
When operation level 4 to 7 is set, the operation level remains
unchanged until the password is cleared.
(The operation level also remains unchanged if the power is turned
off.)
Operation level 7 is reserved for CNC and PMC maintenance.
NOTE
When a password is being entered, an asterisk (*)
is displayed instead of each entered character.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1692 -
12.3.26.2 Password modification (15-inch display unit)
The current operation level is displayed.
The password for each of operation levels 4 to 7 can be modified.
Displaying and setting the password modification screen
Procedure
1 Press function key .
2 Press vertical soft key [NEXT PAGE] several times to display
soft key [PROTECT].
3 Press vertical soft key [PROTECT].
4 Press vertical soft key [PASSWORD].
The PASSWORD CHANGE screen shown below is displayed.
Fig. 12.3.26.2 (a) PASSWORD CHANGE screen (15-inch)
5 Key in an operation level whose password is to be modified, then
press horizontal soft key [INPUT].
6 Key in the current password for the operation level whose
password is to be modified, then press horizontal soft key
[INPUT].
7 Key in a new password, then press horizontal soft key [INPUT].
8 Key in the new password again for confirmation, then press
horizontal soft key [INPUT].
9 Press horizontal soft key [PASSWD CHANGE].
10 To clear the password, press horizontal soft key [PASSWD
CLEAR].
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1693 -
Explanation
Up to eight characters (only uppercase alphabetic characters and
numeric characters) can be input.
NOTE
1 For a password, consisting of three to eight
characters, the following characters are available:
• Uppercase alphabetic characters
• Numeric characters
2 When a password is being entered, an asterisk (*)
is displayed instead of each entered character.
3 Whether a password can be changed at the current
operation level is determined as follows:
• Password of an operation level higher than the
current operation level
Cannot be changed.
• Password of the current operation level
Can be changed.
• Password of an operation level lower than the
current operation level
Can be changed (only to the initial password).
4 The set password is not displayed.
Be careful not to forget the password.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1694 -
12.3.26.3 Protection level setting (15-inch display unit)
The current operation level is displayed.
The change protection level and output protection level of each data
item are displayed.
The change protection level and output protection level of each data
item can be changed.
Confirmation based on protection level setting
Procedure
1 Press function key .
2 Press vertical soft key [NEXT PAGE] several times to display
soft key [PROTECT].
3 Press vertical soft key [PROTECT].
4 Press vertical soft key [DATA LEVEL] to change the protection
level of CNC data or press vertical soft key [PMC LEVEL] to
change the protection level of PMC data.
The following protection level change screen is displayed.
Fig. 12.3.26.3 (a) Protection level change screen (15-inch)
5 Move the cursor to the change level or output level of a desired
data item.
6 Key in a new desired level, then press horizontal soft key
[INPUT].
NOTE
When the protection level of PMC data is set, soft
key [SWITCH PMC] is used to switch between
PMC paths to be set, for multipath PMC.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1695 -
Explanation
When the protection level of a data item is higher than the current
operation level, the protection level of the data item cannot be
changed.
The protection level of a data item cannot be changed to a protection
level higher than the current operation level.
For each of the following types of data, you can set a data protection
level. There are the following two types of data protection levels:
• Change protection level
Sets the protection level used when data is changed.
• Output protection level
Sets the protection level used when data is output (punched out)
to an external unit.
As a protection level, you can set a value of 0 (low) to 7 (high).
Table 12.3.26.3 (a) Protection level of each type of data
Initial protection level
Type of data Change Output
Custom macro variable data <CUSTOM MACRO>
(including variable data dedicated to the macro executor) 0 0
Periodical maintenance data <PERIODICAL MAINTENANCE DATA> 0 0
Tool management data <"TOOL LIFE TIME DATA> 0 0
Tool offset data <TOOL OFFSET DATA>
(For each type when tool geometry compensation and tool wear compensation
are treated differently)
0 0
Clock data <TIME> 0 0
Workpiece origin shift amount data <WORK ZERO SHIFT> 0 0
Workpiece origin offset data <WORK ZERO OFFSET> 0 0
Ethernet setting data <ETHER NET SETTING> 0 0
Fixture offset data <FIXTURE OFFSET DATA> 0 0
Parameter data <PARAMETER DATA> 4 0
Settings <SETTING DATA> 0 0
Pitch error compensation data <PITCH ERROR DATA>
(including three-dimensional error compensation data) 4 0
Parameter data for Power Mate CNC manager function
<PARAMETER DATA FOR POWER MATE CNC MANAGER> 0 0
Each part program <PROGRAMS FOR EACH PARTS> 0 0
Part program editing operation <CHANGE PROGRAMS FOR EACH PARTS> 0 0
Absolute coordinate preset operation <PRESET OF ABSOLUTE AXIS DATA> 0 0
Table 12.3.26.3 (b) Protection level of PMC data
Initial protection level
Type of data Change Output
Composition parameter 0 0
Setting (online) 0 0
Setting (each path) 0 0
Sequence program 0 0
PMC parameter 0 0
Timer 0 0
Counter 0 0
Keep relay 0 0
Keep relay (system) 0 0
Data table 0 0
Data table control 0 0
PMC momory 0 0
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1696 -
NOTE
1 For some types of data, the output function is not provided.
2 When the protection level of data is higher than the current operation level, the
protection level cannot be changed.
3 The protection level of data cannot be changed to a level higher than the current
operation level.
4 Settable types of data increase or decrease, depending on the option configuration.
5 For details on the protection level of PMC data, refer to “PMC Programming Manual
(B-63983EN)”.
6 Data related to tool information on the EACH TOOL DATA screen for the tool
management function is protected by protecting tool offset data.
7 The type of tool offset data put in effect varies depending on the tool compensation
value memory used.
8 To change the protection level for each part program, do so on the PROGRAM
FOLDERscreen rather than on the PROTECT LEVEL screen.
9 Part program editing includes program editing for the MDI mode.
10 Presetting absolute coordinates causes preset workpiece coordinate system values
to be protected.
11 During tool offset data input/output, if any tool offset data type is not allowed to be
changed or output to the outside, it is processed as follows:
- Input : Any data type other than those whose change is not allowed is changed.
- Output : Any data type other than those whose change is not allowed is output.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1697 -
12.3.26.4 Setting the change protection level and output protection
level of a program (15-inch display unit)
The display/operations indicated below can be performed from the
directory screen.
The change protection level and output protection level of each part
program are displayed.
The change protection level and output protection level of each part
program can be changed.
Setting the change protection level and output protection level of a program
Procedure
1 Press function key .
2 Press vertical soft key [FOLDER].
Fig. 12.3.26.4 (a) Program directory screen (15-inch)
3 Press horizontal soft key [DETAIL ON] to switch to detail
displays.
4 Move the cursor to a desired program.
5 Press the continuous menu key to display horizontal soft
key [CHANGE ATTR].
6 Press horizontal soft key [CHANGE ATTR].
7 Key in a new desired level, then press horizontal soft key
[CHANGE LEVEL].
8 To change the output protection level, key in a new desired level,
then press horizontal soft key [OUT LEVEL].
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1698 -
Explanation
The change protection level (0 to 7) and output protection level (0 to
7) are displayed as "CHANGE PROTECTION LEVEL
VALUE/OUTPUT PROTECTION LEVEL".
NOTE
1 When the protection level of data is higher than the
current operation level, the protection level cannot
be changed.
2 The protection level of data cannot be changed to a
level higher than the current operation level.
3 A protection level can be set only for those part
programs that are held on the "CNC_MEM" device.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1699 -
12.3.27 Precision Level Selection (15-inch Display Unit)
An intermediate precision level between the parameters for emphasis
on velocity (precision level 1) and the parameters for emphasis on
precision (precision level 10) set on the machining parameter tuning
screen can be selected. As shown in the figure below, the levels are
proportionally linear, and an intermediate level can be selected so that
optimal parameters can be automatically calculated to perform
machining.
Value
RMS value
1 10 Precision level
(RMS value: Root-Mean-Square value)
Fig. 12.3.27 (a) Image of "level"
Procedure for precision level selection
1 Select the MDI mode.
2 Press function key .
3 Press vertical soft key [NEXT PAGE] several times to display
vertical soft key [PRECI LEVEL].
4 Press vertical soft key [PRECI LEVEL].
Fig. 12.3.27 (b) Precision level selection screen
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1700 -
5 To change the precision level, key in a desired precision level (1
to 10), then press the key on the MDI panel.
6 When the precision level is changed, a RMS value is obtained
from the velocity-emphasized parameter set and
precision-emphasized parameter set for parameter modification.
For the modified parameters, see the description of the
machining parameter tuning.
7 If there is an axis in addition to the currently displayed axes,
press page key or several times to display the
screen for the axis.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1701 -
12.3.28 Displaying and Setting Tool Life Management Data (15-inch
Display Unit)
Displaying tool life management data on a screen enables the current
status of tool life management to be grasped. Also on the screen,
tool life management data can be edited. The screen is either:
• Tool life management (list screen) or
• Tool life management (group editing screen)
Overview
EDIT
END
List screen
Tool life management (list screen)
Displayed items:
- NEXT GROUP
- SELECTED GROUP
- GROUP NO.
- LIFE
- TOOL MANAGEMENT STATUS
- GROUP TO BE CHANGE
Functions:
- Searching for groups
- Clearing execution data
- Setting the tool life counter
Tool life management (group editing screen)
Displayed items:
- NEXT GROUP - SELECTED GROUP
- MAX.TOOL PIECES - LIFE
- T-CODE - H-CODE and D-CODE
Functions:
- Setting tool data - Setting a tool status
- Selecting too skip
- Setting a life count type, life value, and tool life
counter
Pressing horizontal soft key [EDIT] or [END]
switches from the list screen to the group editing
screen or vice versa.
Group editing screen
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1702 -
M
If the tool life management B function is enabled (bit 4 (LFB) of
parameter No. 6805 = 1), the following parameters can be used to
display arbitrary groups and remaining set values.
• If bit 5 (TGN) of parameter No. 6802 = 1
An arbitrary group is displayed on the list and group editing
screens.
• If bit 3 (GRP) of parameter No. 6802 = 1
Remaining set values are displayed on the group editing screen.
The group editing screen always displays H and D codes.
T
The T series is provided with two tool change types, turret type and
ATC type. For the T series, displays vary depending on which tool
change type is in use.
If the turret type is in use (bit 3 (TCT) of parameter No. 5040 = 0)
• Neither the H code nor the D code is used; neither is displayed.
• No arbitrary group can be used; no arbitrary group is displayed.
If the ATC type is in use (bit 3 (TCT) of parameter No. 5040 = 1)
• The D code is displayed on the group editing screen.
• If the tool life management B function is enabled (bit 4 (LFB) of
parameter No. 6805 = 1) and bit 5 (TGN) of parameter No. 6802
= 1, arbitrary groups are displayed on the list and group editing
screens.
If the tool life management B function is enabled (bit 4 (LFB) of
parameter No.6805 = 1) and bit 3 (GRP) or parameter No. 6802 = 1,
remaining set values are displayed on the group editing screen.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1703 -
12.3.28.1 Tool life management (list screen) (15-inch display unit)
This screen can display the life management status of all tools in tool
groups and whether the life of the tool groups has expired. It also
enables you to set tool life counters and clear execution data.
Displays on the list screen
Procedure
1 Press function key .
2 Press vertical soft key [NEXT PAGE] several times to display
soft key [TOOL LIFE].
3 Press vertical soft key [TOOL LIFE].
Fig. 12.3.28.1 (a) Displaying tool life management (list screen) (15-inch)
- Contents of (A)
(A) displays tool group numbers and an override value. If there is no
tool group to display, ****, instead of tool group numbers, is
displayed.
NEXT GROUP:
Tool group number for which life counting is started by the next
M06 command.
USING GROUP:
Tool group number for which life counting is currently under
way.
SELECTED GROUP:
Tool group number for which life counting is currently under
way or life counting has been performed most recently.
COUNT OVERRIDE:
“1.0TIMES” is displayed if the tool life counter override signal is
disabled (bit 2 (LFV) of parameter No. 6801 = 0).
(A)
(B)
(C)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1704 -
NOTE
If arbitrary group numbers are enabled, NEXT
GROUP, USING GROUP, and SELECTED GROUP
are each represented with an arbitrary group number
rather than the tool group number.
- Contents of (B)
(B) displays the set life value, the current content of the tool life
counter, and the registered tool numbers (in the order they are used)
for each tool group. If the life count type is specification by duration,
the measurement unit used in displaying and specifying set life values
and tool life counter values is selected according to the setting of bit 0
(FCO) of parameter No. 6805 as listed below.
Bit 0 (FCO) of parameter No. 6805 0 1
Measurement unit used in displaying and specifying
set life values and tool life counter values
1 minute 0.1 minutes
The following table lists the prefixes used with tool numbers.
Tool status Tool in use Tool not in use
Life remaining @ No indication
Skip # #
Life expired * *
NOTE
1 The tool life counter indicates the count value for the tool
indicated with @.
2 If bit 3 (EMD) of parameter No. 6801 = 0, a tool number
remains prefixed with @ even if the life of the tool has
expired until another tool is selected.
3 If bit 3 (EMD) of parameter No. 6801 =1, the following
differences can occur depending on the type of the life
counter in use.
• If the life counter type is specification by duration, the
prefix is changed to “*” (life expired) as soon as the tool
life expires.
• If the life counter type is specification by count, the
counter is incremented by one at the end of a program
(such as M02 or M30). So, the prefix is not changed to
“*” (life expired) even if the tool life counter matches the
life value. The symbol “*” (life expired) appears when
the tool life count is incremented after the CNC is reset.
4 If bit 2 (ETE) of parameter No. 6804 = 1, the symbol “*”
indicating the expiration of the life of the last tool appears
on the tool life management screen when the life counter
for the last tool of the tool group of interest matches the life
value. This way, the information about the last tool in the
FOCAS2 or PMC window indicates that the life of the tool
has expired if the tool change signal TLCH <Fn064.0> is 1.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1705 -
If arbitrary group numbers are enabled, an arbitrary group number is
displayed in the parentheses beside the tool group number. If no
arbitrary group number is specified, “********” is displayed instead.
Fig. 12.3.28.1 (b) Displaying arbitrary group numbers
Arbitrary group numbers are enabled by setting the following
parameters.
M
• The tool life management B function is enabled (bit 4 (LFB) of
parameter No. 6805 = 1).
• Arbitrary group numbers are enabled (bit 5 (TGN) of parameter
No. 6802 = 1).
T
• The current tool change type is ATC (bit 3 (TCT) of parameter No.
5040 = 1).
• The tool life management B function is enabled (bit 4 (LFB) of
parameter No. 6805 = 1).
• Arbitrary group numbers are enabled (bit 5 (TGN) of parameter
No. 6802 = 1).
- Contents of (C)
(C) displays tool group numbers for which a tool change signal has
been issued.
If there are so many tool group numbers that all the numbers cannot be
displayed, some are omitted, and “>>” is displayed instead.
If there is no tool group number in need of change, “****” is
displayed.
NOTE
If arbitrary group numbers are enabled, a tool group
number in need of change is represented with an
arbitrary group number rather than the tool group
number.
Setting data on the list screen
Tool life management data can be specified in the reset state (both the
OP and RST signals are “0”). However, setting bit 1 (TCI) of
parameter No. 6804 to 1 enables tool life management data to be
specified even during automatic operation (the OP signal is “1”).
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1706 -
NOTE
As for USING GROUP or NEXT GROUP settings:
1) During automatic operation (OP signal = “1” and
bit 1 (TCI) of parameter No. 6804 = 1), only the
tool life counter can be changed.
2) In the reset state (OP signal = “0” and RST signal
“0”), the following editing operation stops life
management because it cannot be continued.
- Clearing execution data
Procedure
- Setting the tool life counter
The tool life counter can be set with a value, using the following
methods.
Method 1
1 Place the cursor on the tool life counter for a desired tool group.
2 Enter the value from the keypad.
3 Press horizontal soft key [INPUT].
Method 2
1 Place the cursor on the tool life counter for a desired tool group.
2 Enter the value from the keypad.
3 Press key.
- Clearing execution data
All existing execution data for a tool group selected by the cursor can
be cleared as follows:
1 Place the cursor on the tool group whose execution data you
want to clear.
2 Press horizontal soft key [ERASE].
3 Press horizontal soft key [EXEC].
NOTE
Setting bit 4 (GRS) of parameter No. 6800 to 1
enables execution data for all registered tool groups
to be cleared.
- Selecting tool groups
Tool groups can be selected using the following methods.
Method 1
1 Enter a tool group number from the keypad.
2 Press soft key [NO.SRH].
NOTE
If arbitrary group numbers are enabled, a tool group
is selected by searching for an arbitrary group
number rather than the tool group number.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1707 -
Method 2
1 Press page key or to display desired groups.
2 Press cursor key or to move the cursor to the
desired group at either the left or right.
- Switching to the group editing screen
Switch to tool life management (group editing screen).
1 Move the cursor to the tool group you want to edit:
2 Press horizontal soft key [EDIT].
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1708 -
12.3.28.2 Tool life management (group editing screen) (15-inch display
unit)
On this screen, it is possible to edit tool life management data (such as
tool life value, tool life counter, and tool data) for the tool group of
interest.
Displaying the group editing screen
Procedure
1. Place the cursor on the tool group you want to edit from the list
screen.
2. Press horizontal soft key [EDIT].
Fig. 12.3.28.2 (a) Displaying tool life management (group editing screen)
(15-inch)
NOTE
If no tool is registered with a tool group, none of a
life count type, a life value, and a tool life counter
value is displayed for the tool group.
- Contents of (A)
Like the counterpart of the list screen, (A) of the editing screen
displays the next tool group number and override value. If there is
no appropriate tool group, **** is displayed instead.
NEXT GROUP:
Tool group for which life counting is started by the next M06
command.
USING GROUP:
Tool group number for which life counting is currently under
way.
(A)
(B)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1709 -
SELECTED GROUP:
Tool group number for which life counting is currently under
way or life counting has been performed most recently.
COUNT OVERRIDE:
“1.0TIMES” is displayed if the tool life counter override signal is
disabled (bit 2 (LFV) of parameter No. 6801 = 0).
NOTE
If arbitrary group numbers are enabled, NEXT
GROUP, USING GROUP, and SELECTED GROUP
are each represented with an arbitrary group number
rather than the tool group number.
- Contents of (B)
(B) details tool life management data related to a selected tool group
as follows:
TYPE :1 Specification by count
2 Specification by duration
LIFE : Tool life value
COUNT : Tool life counter
STATE
:
Tool status Tool in use Tool not in use
Life remaining @ No indication
Skip # #
Life expired * *
T-CODE : Tool number
M
H-CODE
:
Tool length compensation specification code
D-CODE
:
Cutter compensation specification code
T
H-CODE
:
No display.
D-CODE
:
Tool offset value specification code
if ATC type is in use (bit 3 (TCT) of parameter No.
5040 = 1)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1710 -
NOTE
1 The tool life counter indicates the count value for
the tool indicated with @.
2 If bit 3 (EMD) of parameter No. 6801 = 0, a tool
number remains prefixed with @ even if the life of
the tool has expired until another tool is selected.
3 If bit 3 (EMD) of parameter No. 6801 = 1, the
following differences can occur depending on the
type of the life counter in use.
• If the life counter type is specification by
duration, the prefix is changed to “*” (life
expired) as soon as the tool life expires.
• If the life counter type is specification by count,
the counter is incremented by one at the end of
a program (such as M02 or M30). So, the
prefix is not changed to “*” (life expired) even if
the tool life counter matches the life value. The
symbol “*” (life expired) appears when the tool
life count is incremented after the CNC is reset.
4 If bit 2 (ETE) of parameter No. 6804 = 1, the
symbol “*” indicating the expiration of the life of the
last tool appears on the tool life management
screen when the life counter for the last tool of the
tool group of interest matches the life value. This
way, the information about the last tool in the
FOCAS2 or PMC window indicates that the life of
the tool has expired if the tool change signal TLCH
<Fn064.0> is 1.
Displaying arbitrary groups and remaining set values
Fig. 12.3.28.2 (b) Displaying arbitrary group numbers and remaining set
values on the editing screen
M
If the tool life management B function is enabled (bit 4 (LFB) of
parameter No. 6805 = 1) and the following parameters are enabled,
arbitrary groups and remaining set values are displayed.
OPTION GROUP:
Arbitrary group number
(if bit 5 (TGN) of parameter No. 6802 = 1)
REST COUNT:
Remaining set value used until a new tool is selected
(if bit 3 (GRP) of parameter No. 6802 = 1)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1711 -
T
If the tool life management B function is enabled (bit 4 (LFB) of
parameter No. 6805 = 1)
Turret type (bit 3 (TCT) of parameter No. 5040 = 0)
• OPTION GROUP:
No display.
• REST COUNT:
Remaining set value used until a new tool is selected
(if bit 3 (GRP) of parameter No. 6802 = 1)
ATC type (bit 3 (TCT) of parameter No. 5040 = 1)
• OPTION GROUP:
Arbitrary group number
(if bit 5 (TGN) of parameter No. 6802 = 1)
• REST COUNT:
Remaining set value used until a new tool is selected
(if bit 3 (GRP) of parameter No. 6802 = 1)
Setting data on the group editing screen
Tool life management data can be specified in the reset state (both the
OP and RST signals are “0”). However, setting bit 1 (TCI) of
parameter No. 6804 to “1” enables tool life management data to be
specified even during automatic operation (the OP signal is “1”).
The available editing operations are listed below.
M
Items that can be edited Mode
Setting a life count type, life value, tool life counter, and tool
data (T code, H code, and D code)
All modes
Adding tool numbers (T code) MDI
Deleting all tool group data at a time MDI
Deleting tool data (status, T code, H code, and D code) MDI
Selecting tool skip MDI
Specifying to clear tool data (life re-set) MDI
T
Items that can be edited Mode
Setting a life count type, life value, tool life counter, and tool
data (T code and D code)
However, the D code can be edited only if the ATC type
is in use (bit 3 (TCT) of parameter No. 5040 = 1).
All modes
Adding tool numbers (T code) MDI
Deleting all tool group data at a time MDI
Deleting tool data (status, T code, and D code) MDI
Selecting tool skip MDI
Specifying to clear tool data (life re-set) MDI
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1712 -
M
T
If no tool is registered with a tool group, none of a life count type, a
tool life value, and a tool life counter value can be set for the tool
group. First of all, add a tool number (T code).
NOTE
1 As for USING GROUP or NEXT GROUP editing:
<1> During automatic operation (OP signal = “1”
and bit 1 (TCI) of parameter No. 6804 = 1),
only the tool life counter can be changed.
<2> In the reset state (OP signal = “0” and RST
signal “0”), the following editing operation
stops life management because it cannot be
continued.
- Adding tool numbers (T code)
- Deleting all tool group data at a time
- Deleting tool data (status, T code, H code,
and D code)
2 The following editing operations may set the tool
change signal to ”1”.
- Selecting tool skip for the last tool.
- Deleting tool numbers, resulting in any tool other
than those whose life has expired or who have
been skipped being not found in the tool group of
interest.
3 The following editing operations may reset the tool
change signal to ”0”.
- Adding tool numbers, leading to tools whose life
has not expired being set in the tool group of
interest.
- Selecting tool clear.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1713 -
Procedure
- Setting a life count type, tool life value, tool life counter, tool data, arbitrary group
number, and remaining set value
Setting a life count type, tool life value, tool life counter, tool data,
arbitrary group number, and remaining set value
Method 1
1 Place the cursor on the desired item.
2 Enter a value from the keypad.
3 Press horizontal soft key [INPUT].
Method 2
1 Place the cursor on the desired item.
2 Enter a value from the keypad.
3 Press .
NOTE
1 Changing a tool life value or tool life counter does
not affect the tool status or tool change signal.
2 Changing a life count type causes the tool life value
and too life counter to be reset to 0.
M
If the tool life management B function is enabled (bit 4 (LFB) of
parameter No. 6805 = 1) and the following parameters are enabled,
arbitrary groups and remaining set values can be specified
OPTION GROUP:
Arbitrary group number
(if bit 5 (TGN) of parameter No. 6802 = 1)
REST COUNT:
Remaining set value used until a new tool is selected
(if bit 3 (GRP) of parameter No. 6802 = 1)
T
If the tool life management B function is enabled (bit 4 (LFB) of
parameter No. 6805 = 1)
Turret type (bit 3 (TCT) of parameter No. 5040 = 0)
• OPTION GROUP:
Cannot be set.
• REST COUNT:
It is possible to set a remaining set value to be used until a new
tool is selected (if bit 3 (GRP) of parameter No. 6802 = 1).
ATC type (bit 3 (TCT) of parameter No. 5040 = 1)
• OPTION GROUP:
Arbitrary group numbers can be set (if bit 5 (TGN) of parameter
No. 6802 = 1).
• REST COUNT:
It is possible to set a remaining set value to be used until a new
tool is selected (if bit 3 (GRP) of parameter No. 6802 = 1).
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1714 -
- Adding tool numbers
Tool numbers can be added to a tool group as follows:
1 Select the MDI mode.
2 Place the cursor on the tool data (T code, H code, or D code) just
before a tool number to be added.
3 Enter the tool number from the key pad.
4 Press horizontal soft key [INSERT].
(Example)
Adding tool number 1550 between numbers 1 and 2 (for the M
series)
1 Move the cursor to the data for number 1, enter “1550”, and
press [INSERT].
2 The entered T code 1550 is inserted in the position of
number 2. The H and D codes are reset to 0.
- Deleting all tool group data at a time
All tool group data can be deleted at a time as follows:
1 Select the MDI mode.
2 Place the cursor on the tool data (T code, H code, or D code) just
Select the tool group from which all tool data you want to delete
at a time.
3 Press horizontal soft key [DELETE].
4 Press horizontal soft key [GROUP].
5 Press horizontal soft key [EXEC].
- Deleting tool data
Tool data can be deleted from a tool group as follows:
1 Select the MDI mode.
2 Place the cursor on the tool data (T code, H code, or D code) you
want to delete.
3 Press horizontal ssoft key [DELETE].
4 Press horizontal ssoft key [<CURS>].
NOTE
1 Deleting all tools from a tool group is equivalent to
deleting the tool group itself.
2 Deleting a tool indicated with @ (in use) results in @
being moved to the previous tool whose life has
expired or which has been skipped.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1715 -
- Selecting tool skip
Tool data can be placed in a skip state as follows:
1 Select the MDI mode.
2 Place the cursor on the tool data (T code, H code, or D code) for
a tool you want to skip.
3 Press horizontal soft key [STATE].
4 Press horizontal soft key [SKIP].
- Specifying to clear tool data (life re-set)
Tool data state can be cleared as follows:
1 Select the MDI mode.
2 Place the cursor on the tool data (T code, H code, or D code) for
a tool you want to clear.
3 Press horizontal soft key [STATE].
4 Press horizontal soft key [CLEAR].
- Selecting a tool group
A tool group can be selected as follows:
Method 1
1 Enter a tool group number from the keypad.
2 Press horizontal soft key [NO.SRH].
NOTE
If arbitrary group numbers are enabled, a tool group
is selected by searching for an arbitrary group
number rather than the tool group number.
Method 2
1 Press page key or to display the target tool group.
- Switching to the list screen
The tool life management (list screen) can be resumed as follows:
1 Press horizontal soft key [END].
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1716 -
12.3.29 Displaying and Setting Workpiece Setting Error
Compensation Data (15-inch Display Unit)
An amount of error used in workpiece setting error compensation can
be set on the workpiece setting error screen.
The workpiece setting error screen is displayed as follows:
1 Press function key .
2 Press vertical soft key [WORK SET ER].
The workpiece setting error screen appears.
Fig. 12.3.29 (a) Workpiece setting error screen (15-inch)
Up to 7 sets (No. 01 to No. 07) of different amounts of workpiece
setting error can be specified. In addition, it is possible to specify an
amount of error (No. 00 (COMMON)) to be added to an error in the 7
sets in common.
The X-direction error ∆x, Y-direction error ∆y, and Z-direction error
∆z are specified, respectively, in the x, y, and z fields. The rotational
errors ∆a, ∆b, and ∆c are specified, respectively, in the a, b, and c
fields.
Table rotation axis positions 1 and 2 are specified in the fields under
the a, b, and c fields (C and B in the figure).
Rotation axis names specified in parameter Nos. 19681 and 19686 are
displayed in the axis name fields.
Table rotation axis positions 1 and 2 are specified for rotation axes.
No position must be specified for axes (including virtual axes) other
than table rotation axes. So, no such item is displayed for setting.
Table rotation axis position setting items are displayed under the
following conditions.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1717 -
• It must have been correctly specified which axis is a table
rotation axis.
If parameter No. 19680 = 12 (table rotation type), axis numbers
must have been specified correctly in parameter Nos. 19681 and
19686.
If parameter No. 19680 = 21 (mixed type), an axis number must
have been specified correctly in parameter No. 19686.
• Bit 0 of parameter No. 1006 must be 1 (rotation axis) for the axes
specified above.
The following soft key can be used in data setting.
• After a workpiece setting error number you want to display is
entered, pressing horizontal soft key [NO.SRH] causes a setting
screen for the target workpiece setting error to appear.
• After a number is entered, pressing horizontal soft key [+INPUT]
causes the number to be added.
• After a number is entered, pressing horizontal soft key [INPUT]
causes the number to be set.
• Pressing horizontal soft key [CLEAR] causes the next soft key to
appear.
• After a workpiece setting error number to be deleted is entered,
pressing horizontal soft key [NO.] deletes the data corresponding
to the workpiece setting error number.
• Pressing horizontal soft key [ALL] deletes data for all workpiece
setting error numbers.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1718 -
12.3.30 Displaying and Setting Pattern Data Inputs
(15-inch Display Unit)
Described below are a method for displaying machining menus
(pattern menus) created by machine tool builders and a method for
setting them. The descriptions are based on an example. For actual
pattern menus and pattern data, refer to manuals released by respective
machine tool builders.
Displaying pattern data and pattern menus
Given below is a procedure for displaying pattern menus.
1 Press function key .
2 Press vertical soft key [NEXT PAGE] several times.
3 Press vertical soft key [PATTERN MENU].
The pattern menu screen shown below appears.
Fig. 12.3.30 (a) Pattern menu screen (15-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1719 -
On this screen, a pattern to be used can be selected.
The following two methods can be used to select patterns.
• Using the cursor
Move the cursor to a pattern name you want to select, using
cursor key or , and then press soft key [SELECT] or
.
• Specifying a pattern number
Enter a number displayed at the left side of a pattern name, and
press soft key [SELECT] or .
The custom macro screen (pattern data screen) shown below appears.
Fig. 12.3.30 (b) Custom macro screen (pattern data) (15-inch)
Enter the necessary pattern data, and press .
After entering all necessary data, select the MEMORY mode and
press the cycle start button. Machining begins.
Explanation
- Explanations about the pattern menu screen
HOLE PATTERN
An arbitrary character string consisting of 12 or less characters can be
displayed as a menu title.
BOLT HOLE
An arbitrary character string consisting of 10 or less characters can be
displayed as a pattern name.
Machine tool builders should program menu title and pattern name
character strings, using custom macros, and save them in program
memory.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1720 -
- Explanations about the custom macro screen (pattern data screen)
BOLT HOLE
An arbitrary character string consisting of 12 or less characters can be
displayed as a pattern data title.
TOOL.
An arbitrary character string consisting of 10 or less characters can be
displayed as a variable name.
*BOLT HOLE*
The comment text consists of nine 12-character blocks, or the
comment can be up to 12 lines (10.4-inch display) or 8 lines (7.2 or
8.4-inch display) with one block counted as one line.
Machine tool builders should program variable name and comment
text character strings, using custom macros, and save them in program
memory.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1721 -
12.4 SCREENS DISPLAYED BY FUNCTION KEY
When the CNC and machine are connected, parameters must be set to
determine the specifications and functions of the machine in order to
fully utilize the characteristics of the servo motor or other parts.
This chapter describes how to set parameters on the MDI panel.
Parameters can also be set with external input/output devices such as
the memory card (see III-8).
In addition, pitch error compensation data used for improving the
precision in positioning with the ball screw on the machine can be set
or displayed by the operations under function key .
See III-7 for the diagnosis screens displayed by pressing function key
.
Section 12.4, "SCREENS DISPLAYED BY FUNCTION KEY
", consists of the following subsections:
――――― Screens of a 7.2/8.4/10.4-inch display unit
12.4.1 Displaying and Setting Parameters ....................................1723
12.4.2 Displaying and Setting Pitch Error Compensation Data....1726
12.4.3 Displaying and Setting Three-Dimensional Error
Compensation Data............................................................1729
12.4.4 Servo Parameters................................................................1733
12.4.5 Servo Tuning......................................................................1734
12.4.6 Spindle Setting ...................................................................1735
12.4.7 Spindle Tuning...................................................................1736
12.4.8 Spindle Monitor .................................................................1737
12.4.9 Color Setting Screen ..........................................................1738
12.4.10 Machining Parameter Tuning.............................................1741
12.4.11 Displaying Memory Data...................................................1749
12.4.12 Parameter Tuning Screen ...................................................1751
12.4.13 Periodic Maintenance Screen.............................................1768
12.4.14 System Configuration Screen.............................................1776
12.4.15 Overview of the History Function .....................................1779
――――― Screens of a 15-inch display unit
12.4.16 Displaying and Setting Parameters (15-inch Display Unit)1802
12.4.17 Displaying and Setting Pitch Error Compensation Data
(15-inch Display Unit) .......................................................1805
12.4.18 Displaying and Setting Three-Dimensional Error
Compensation Data (15-inch Display Unit).......................1808
12.4.19 Servo Parameters (15-inch Display Unit) ..........................1812
12.4.20 Servo Tuning (15-inch Display Unit) ................................1813
12.4.21 Spindle Setting (15-inch Display Unit)..............................1814
12.4.22 Spindle Tuning (15-inch Display Unit) .............................1815
12.4.23 Spindle Monitor (15-inch Display Unit)............................1816
12.4.24 Color Setting Screen (15-inch Display Unit).....................1817
12.4.25 Machining Parameter Tuning (15-inch Display Unit) .......1820
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1722 -
12.4.25 Machining Parameter Tuning (15-inch Display Unit) .......1820
12.4.26 Displaying Memory Data (15-inch Display Unit) .............1828
12.4.27 Parameter Tuning Screen (15-inch Display Unit)..............1830
12.4.28 Periodic Maintenance Screen (15-inch Display Unit) .......1847
12.4.29 System Configuration Screen (15-inch Display Unit) .......1855
12.4.30 Overview of the History Function (15-inch Display Unit) 1858
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1723 -
Screens of a 7.2/8.4/10.4-inch display unit
12.4.1 Displaying and Setting Parameters
When the CNC and machine are connected, parameters are set to
determine the specifications and functions of the machine in order to
fully utilize the characteristics of the servo motor. The setting of
parameters depends on the machine. Refer to the parameter list
prepared by the machine tool builder.
Normally, the user need not change parameter setting.
Procedure for displaying and setting parameters
Procedure
1 Set 1 for PARAMETER WRITE to enable writing. See the
procedure for enabling/disabling parameter writing described
below.
2 Press function key .
3 Press chapter selection soft key [PARAM] to display the
parameter screen.
Fig. 12.4.1 (a) PARAMETER screen (10.4-inch)
4 Move the cursor to the parameter number to be set or displayed
in either of the following ways:
• Enter the parameter number and press soft key [NO.SRH] .
• Move the cursor to the parameter number using the page
keys, and , and cursor keys, , ,
, and .
5 To set the parameter, enter a new value with numeric keys and
press soft key [INPUT]. The parameter is set to the entered value
and the value is displayed.
6 Set 0 for PARAMETER WRITE to disable writing.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1724 -
Procedure for enabling/displaying parameter writing
Procedure
1 Select the MDI mode or enter state emergency stop.
2 Press function key .
3 Press soft key [SETTING] to display the setting screen.
Fig. 12.4.1 (b) SETTING screen (10.4-inch)
4 Move the cursor to PARAMETER WRITE using cursor keys.
5 Press soft key [(OPRT)], then press [ON:1] to enable parameter
writing.
At this time, the CNC enters the alarm state SW0100.
6 After setting parameters, return to the setting screen. Move the
cursor to PARAMETER WRITE and press soft key [(OPRT)] ,
then press [OFF:0].
7 Press the key to release the alarm condition.
When an alarm PW0000 occurred, however, it is not released
unless the power is turned off and back on.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1725 -
Explanation
- Setting parameters with external input/output devices
See III-8 for setting parameters with external input/output devices
such as the memory card.
- Parameters that require turning off the power
Some parameters are not effective until the power is turned off and on
again after they are set. Setting such parameters causes alarm PW0000.
In this case, turn off the power, then turn it on again.
- Parameter list
Refer to the Parameter Manual (B-63950EN) for the parameter list.
- Setting data
Some parameters can be set on the setting screen if the parameter list
indicates "Setting entry is acceptable". Setting 1 for PARAMETER
WRITE is not necessary when these parameters are set on the setting
screen.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1726 -
12.4.2 Displaying and Setting Pitch Error Compensation Data
If pitch error compensation data is specified, pitch errors of each axis
can be compensated in detection unit per axis.
Pitch error compensation data is set for each compensation point at the
intervals specified for each axis. The origin of compensation is the
reference position to which the tool is returned.
The pitch error compensation data is set according to the
characteristics of the machine connected to the NC. The content of
this data varies according to the machine model. If it is changed, the
machine accuracy is reduced. In principle, the end user must not alter
this data.
Pitch error compensation data can be set with external devices such as
the memory card (see Chapter III-8). Compensation data can also be
written directly with the MDI panel.
The following parameters must be set for pitch error compensation.
Set the pitch error compensation value for each pitch error
compensation point number set by these parameters.
In the following example, 33 is set for the pitch error compensation
point at the reference position.
1
2
3
3332
31 34 35 36 37
Compensation number
parameter for the reference
position (No. 3620)
Compensation number
parameter for the
compensation point having
the largest value (No.
3622)
-1
-2
Compensation number parameter fo
r
the compensation point having the
smallest value (No. 3621)
Compensation
position number
Compensation
value to be set
3
3
3
3
31
3
3
-3 +1 +1 +1 +2 -1 -3
Reference position
Compensation
interval paramete
r
(
No. 3624
)
Compensation magnification
parameter (No. 3623)
Pitch error compensation value (absolute value)
• Number of the pitch error compensation point at the reference
position (for each axis): Parameter No. 3620
• Number of the pitch error compensation point having the
smallest value (for each axis): Parameter No. 3621
• Number of the pitch error compensation point having the largest
value (for each axis): Parameter No. 3622
• Pitch error compensation magnification (for each axis):
Parameter No. 3623
• Interval of the pitch error compensation points (for each axis):
Parameter No. 3624
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1727 -
• Travel distance per revolution of pitch error compensation of the
rotary axis type (for each axis): Parameter No. 3625
- Bi-directional pitch error compensation
The bi-directional pitch error compensation function allows
independent pitch error compensation in different travel directions.
(When the movement is reversed, compensation is automatically
carried out as in a backlash.)
To use this function, specify pitch error compensation for each travel
direction, that is, separately for the positive and negative directions of
a movement.
When using bi-directional pitch error compensation (setting bit 0
(BDPx) of parameter No. 3605 to 1), specify the following parameters
in addition to the pitch error compensation parameter.
• Number of the pitch error compensation point at the negative end
(for travel in the positive direction, for each axis): Parameter No.
3621
• Number of the pitch error compensation point at the positive end
(for travel in the positive direction, for each axis): Parameter No.
3622
• Number of the pitch error compensation point at the negative end
(for travel in the negative direction, for each axis): Parameter No.
3626
• Pitch error compensation in the reference position when moving
to the reference position from opposite to the reference position
return direction (for each axis): Parameter No. 3627
Procedure for displaying and setting the pitch error compensation data
Procedure
1 Set the following parameters:
• Number of the pitch error compensation point at the
reference position (for each axis): Parameter No. 3620
• Number of the pitch error compensation point having the
smallest value (for each axis): Parameter No. 3621
• Number of the pitch error compensation point having the
largest value (for each axis): Parameter No. 3622
• Pitch error compensation magnification (for each axis):
Parameter No. 3623
• Interval of the pitch error compensation points (for each
axis): Parameter No. 3624
• Travel distance per revolution of pitch error compensation
of the rotary axis type (for each axis): Parameter No. 3625
When using bi-directional pitch error compensation (setting bit 0
(BDPx) of parameter No. 3605 to 1), specify the following
parameters in addition to the pitch error compensation parameter.
• Number of the pitch error compensation point at the
negative end (for travel in the positive direction, for each
axis): Parameter No. 3621
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1728 -
• Number of the pitch error compensation point at the
positive end (for travel in the positive direction, for each
axis): Parameter No. 3622
• Number of the pitch error compensation point at the
negative end (for travel in the negative direction, for each
axis): Parameter No. 3626
• Pitch error compensation in the reference position when
moving to the reference position from opposite to the
reference position return direction (for each axis):
Parameter No. 3627
2 Press function key .
3 Press the continuous menu key , then press chapter selection
soft key [PITCH ERROR]. The following screen is displayed:
Fig. 12.4.2 (a) PITCH ERROR COMPENSATION screen (10.4-inch)
4 Move the cursor to the compensation point number to be set in
either of the following ways:
• Enter the compensation point number and press the soft key
[NO.SRH].
• Move the cursor to the compensation point number using
the page keys, and , and cursor keys, ,
, , and .
5 Enter a value with numeric keys and press soft key [INPUT].
‚
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1729 -
12.4.3 Displaying and Setting Three-Dimensional Error
Compensation Data
In ordinary pitch error compensation, compensation is applied to a
specified compensation axis (single axis) by using its position
information. For example, pitch error compensation is applied to
X-axis by using the position information of X-axis.
Three-dimensional error compensation is a function that adjusts the
current position by calculating compensation data (for three axes)
from the compensation amounts at surrounding compensation points
(eight points) on the basis of the interior division ratio in the
compensation area (rectangular parallelepiped) containing the current
position on up to three compensation axes.
- Calculation of compensation
Three-dimensional error compensation is calculated as follows.
Suppose three compensation axes to be X, Y, and Z (three basic axes)
and the coordinates of the current position be P (Px, Py, Pz). consider
a compensation space (rectangular parallelepiped) containing P. Let its
vertexes be P1, P2, …, and P8 and the compensation values for the
individual axes at the individual vertexes be Cnx, Cny, and Cnz
(where n is a number between 1 and 8).
Let the interior division ratio on X-axis at P be x. Here, x is
standardized in the range of 0 to 1 as follows:
P1x and P2x are the X coordinates of P1 and P2. The interior division
ratios on Y and Z-axes are determined in the same way.
|12|
|1|
xPxP
xPPx
x−
−
=
P4 [C4x, C4y, C4z]
P (Px, Py, Pz)
P5 [C5x, C5y, C5z]P6 [C6x, C6y, C6z]
P1 [C1x, C1y, C1z]P2 [C2x, C2y, C2z]
P3 [C3x, C3y, C3z]
P8 [C8x, C8y, C8z]P7 [C7x, C7y, C7z]
x
y
z
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1730 -
The compensation amount Cx for X-axis at P is determined as
follows:
The compensation amount Cy and Cz on Y and Z-axes are determined
in the same way.
The actual compensation amounts are the calculated compensation
amounts multiplied by the compensation magnifications (Parameter
No.10809 to 10811).
- Number of compensation points
Up to 15625 compensation points (up to 25 points per axis) can be set.
The numbers of compensation points on the individual axes are set for
parameters No.10803 to 10805. The ordering of the compensation
point numbers in the compensation space is as follows.
Max1×Max2×Max3
Max1×Max2×(Max3-1）+1
…
…
Max1×Max2×3
Max1×Max2×2
Max1×Max2
…
…
Max1×Max2+1 Max1×3
Max1×2
1 2 3 ………………… Max1
Max1×Max2+Max1
zyxxCzyxxC
zyxxCzyxxC
zyxxCzyxxC
zyxxCzyxxCCx
××−×+×××+
×−××+×−×−×+
−××−×+−×××+
−
×−××
+
−
×
−
×
−
×
=
)1(87
)1(6)1()1(5
)1()1(4)1(3
)1()1(2)1()1()1(1
Max1 : Number of compensation points on the first axis (up to 25)
Max2 : Second axis (up to 25)
Max3 : Third axis (up to 25)
(
Third com
p
ensation axis
)
(
Second com
p
ensation axis
)
(
First com
p
ensation axis
)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1731 -
Displaying and setting three-dimensional error compensation data
Procedure
1 Set the following parameters:
• First compensation axis for three-dimensional error
compensation : Parameter No. 10800
• Second compensation axis for three-dimensional error
compensation : Parameter No. 10801
• Third compensation axis for three-dimensional error
compensation : Parameter No. 10802
• Number of compensation points for three-dimensional error
compensation (first compensation axis)
Parameter No. 10803
• Number of compensation points for three-dimensional error
compensation (second compensation axis)
Parameter No. 10804
• Number of compensation points for three-dimensional error
compensation (third compensation axis)
Parameter No. 10805
• Compensation point number of the reference position for
three-dimensional error compensation (first compensation
axis) : Parameter No. 10806
• Compensation point number of the reference position for
three-dimensional error compensation (second
compensation axis) : Parameter No. 10807
• Compensation point number of the reference position for
three-dimensional error compensation (third compensation
axis) : Parameter No. 10808
• Magnification for three-dimensional error compensation
(first compensation axis) : Parameter No. 10809
• Magnification for three-dimensional error compensation
(second compensation axis) : Parameter No. 10810
• Magnification for three-dimensional error compensation
(third compensation axis) : Parameter No. 10811
• Compensation interval for three-dimensional error
compensation (first compensation axis)
Parameter No. 10812
• Compensation interval for three-dimensional error
compensation (second compensation axis)
Parameter No. 10813
• Compensation interval for three-dimensional error
compensation (third compensation axis)
Parameter No. 10814
2 Press function key .
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1732 -
3 Press the continuous menu key several times, then press
chapter selection soft key [3D ERR COMP]. The following
screen appears:
Fig. 12.4.3 (a) 3-DIMENSIONAL ERROR COMPENSATION screen
(10.4-inch)
4 Move the cursor to the position of the compensation point
number you want to set using either of the following methods:
• Select the MDI mode.
• Set bit 0 (PWE) of parameter No. 8900 to 1.
• Enter a compensation point number and press soft key [NO.
SRH].
• Move the cursor to the compensation point number or
compensation axis you want to set by pressing page keys
and/or , and cursor keys , , ,
and .
5 Enter compensation data in detection units. The valid data
range is from -128 to 127.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1733 -
12.4.4 Servo Parameters
This subsection describes the initialization of digital servo parameters
performed, for example, at the time of field tuning of the machine
tool.
Procedure for servo parameter setting
Procedure
1 Turn on the power in the emergency stop state.
2 Set bit 0 (SVS) of parameter No. 3111 to 1 to display servo
setting and tuning screens.
3 Press function key , continuous menu key , then soft
key [SERVO PARAM].
4 Press soft key [SERVO PARAM] to select the servo parameter
screen.
The following screen appears:
Fig. 12.4.4 (a) Servo parameter setting screen (10.4-inch)
5 With the page keys and cursor keys, move the cursor to the
position of data to be set or modified.
6 Key in a desired value then press soft key [INPUT].
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1734 -
12.4.5 Servo Tuning
Data related to servo tuning is displayed and set.
Procedure for servo tuning
Procedure
1 Turn on the power in the emergency stop state.
2 Set bit 0 (SVS) of parameter No. 3111 to 1 to display servo
setting and tuning screens.
3 Press function key , continuous menu key , then soft
key [SERVO PARAM].
4 Press soft key [SERVO TUNE] to select the servo tuning screen.
5 Use the cursor and page keys to enter necessary data for initial
setting. The following screen appears:
Fig. 12.4.5 (a) Servo tuning screen (10.4-inch)
6 With the page keys and cursor keys, move the cursor to the
position of data to be set or modified.
7 Key in a desired value then press soft key [INPUT].
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1735 -
12.4.6 Spindle Setting
Parameters related to spindles are set and displayed. In addition to
the parameters, related data can be displayed. Screens for spindle
setting, spindle tuning, and spindle monitoring are provided.
Setting spindle parameters
Procedure
1 Set bit 1 (SPS) of parameter No. 3111 to 1 to display spindle
setting and tuning screens.
2 Press function key , continuous menu key , then soft
key [SPINDL SETING].
3 Press soft key [SPINDL SETING] to select the spindle setting
screen.
The following screen appears:
Fig. 12.4.6 (a) Spindle setting screen (10.4-inch)
4 With the page keys and cursor keys, move the cursor to the
position of data to be set or modified.
5 Key in a desired value then press soft key [INPUT].
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1736 -
12.4.7 Spindle Tuning
Spindle tuning data is displayed and set.
Setting for spindle tuning
Procedure
1 Set bit 1 (SPS) of parameter No. 3111 to 1 to display spindle
setting and tuning screens.
2 Press function key , continuous menu key , then soft
key [SPINDL SETING].
3 Press soft key [SPINDL TUNE] to select the spindle tune screen.
4 The following screen appears:
Fig. 12.4.7 (a) Spindle tuning screen (10.4-inch)
5 With the page keys and cursor keys, move the cursor to the
position of data to be set or modified.
6 Key in a desired value then press soft key [INPUT].
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1737 -
12.4.8 Spindle Monitor
Spindle-related data is displayed.
Displaying the spindle monitor
Procedure
1 Set bit 1 (SPS) of parameter No. 3111 to 1 to display spindle
setting and tuning screens.
2 Press function key , continuous menu key , then soft
key [SPINDL SETING].
3 Press soft key [SP.MON] to select the spindle monitor screen.
4 The following screen appears:
Fig. 12.4.8 (a) Spindle monitor screen (10.4-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1738 -
12.4.9 Color Setting Screen
Screen colors can be set on the color setting screen.
Displaying the color setting screen
Procedure
1 Press function key .
2 Press the continuous menu key several times to display soft
key [COLOR].
3 Press soft key [COLOR] to display the color setting screen.
Fig. 12.4.9 (a) Color setting screen (10.4-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1739 -
Procedure for operating the color setting screen
- Modifying the color (color palette values)
1 Press soft key [(OPRT)]. The soft key display changes to the
following operation soft keys:
2 Move the cursor to a color number whose color palette values are
to be modified.
The current color palette value set for each primary color is
displayed.
3 Select a primary color whose setting is to be modified, with the
corresponding operation soft key [RED], [GREEN], or [BLUE].
More than one primary color can be selected at the same time.
Each time operation soft key [RED], [GREEN], or [BLUE] is
pressed, the operation soft key toggles between selection and
deselection.
(When operation soft keys [RED], [GREEN], and [BLUE] are
not displayed, press the rightmost soft key to display the
operation soft keys.)
4 Select operation soft key [BRIGHT] or [DARK] to modify the
brightness of the selected prime color(s).
- Storing the color (color palette values)
The set color palette values can be stored.
1 Press operation soft key [COLOR1], [COLOR2], or [COLOR3]
to select a storage area.
(When operation soft keys [COLOR1], [COLOR2], and
[COLOR3] are not displayed, press the rightmost soft key to
display the operation soft keys.)
COLOR1 Standard color data parameters Nos. 6581 to 6595
COLOR2 Parameters Nos. 10421 to 10435
COLOR3 Parameters Nos. 10461 to 10475
2 Press operation soft key [MEMORY]. The operation soft key
display switches to the following:
3 Pressing operation soft key [EXEC] stores the current color
palette settings in the selected area.
Pressing operation soft key [CAN] or the leftmost key does not
store the current color palette settings in the selected area.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1740 -
- Calling the color (color palette values)
1 Press operation soft key [COLOR1], [COLOR2], or [COLOR3]
to select a storage area where color palette values are stored.
(When operation soft keys [COLOR1], [COLOR2], and
[COLOR3] are not displayed, press the rightmost soft key to
display the operation soft keys.)
2 Press operation soft key [RECALL]. The operation soft key
display switches to the following:
3 Pressing operation soft key [EXEC] calls the color palette values
from the selected area to enable the color to be modified. This
operation is invalid if no color palette values are stored.
Pressing operation soft key [CAN] or the leftmost key does not
call the color palette values from the selected area.
NOTE
1 Immediately after the power is turned on, the
settings of COLOR1 (parameters) are used for
display. If nothing is stored for COLOR1, the
default colors are used for display.
2 Do not modify the color setting data parameters
directly by MDI key input. When modifying the
standard color data, be sure to perform a storage
operation on the color setting screen.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1741 -
12.4.10 Machining Parameter Tuning
In AI contour control, by setting a velocity-emphasized parameter set
and precision-emphasized parameter set and setting the precision level
matching a machining condition such as rough machining or finish
machining on the precision level setting screen or by programming,
the parameters suitable for the condition can be automatically
calculated to perform machining.
On this screen, the parameter sets for emphasis on velocity (precision
level 1) and emphasis on precision (precision level 10) can be set.
Set the following parameters:
• Acceleration rate of acceleration/deceleration before
interpolation
• Acceleration change time (bell-shaped)
• Allowable acceleration change value for each axis in velocity
control based on acceleration change under jerk control
• Allowable acceleration change value for each axis in acceleration
change under jerk control in successive linear interpolation
operations
• Ratio of the change time of the rate of change of acceleration in
smooth bell-shaped acceleration/deceleration before interpolation
• Allowable acceleration rate
• Acceleration rate of acceleration/deceleration after interpolation
• Corner speed difference
• Maximum feedrate
• Items that can be set freely (2 items)
For details of each parameter, see the descriptions of AI contour
control and jerk control.
By setting bit 0 (MPR) of parameter No. 13601 to 1, this screen can be
hidden.
For the method of setting a precision level, see the description of the
precision level selection screen in Subsection 11.2.14.
Procedure for machining parameter tuning
Procedure
1 Set the MDI mode.
2 Press function key .
3 Press soft key [M-TUN] to display the machining parameter
tuning screen.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1742 -
Fig. 12.4.10 (a) Machining parameter tuning screen (10.4-inch)
Fig. 12.4.10 (b) Machining parameter tuning screen (10.4-inch)
4 Move the cursor to the position of a parameter to be set, as
follows:
Press page key or , and cursor keys , ,
and /or to move the cursor to the parameter.
5 Key in desired data then press the key on the MDI panel.
6 When data is input, a RMS value is found according to the
precision level parameters. (The precision level can be changed
on the precision level selection screen or parameter setting
screen.) If a RMS value calculation fails, a warning (indicating
that automatic setting failed) is displayed.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1743 -
7 Repeat steps 4 and 5 until all machining parameters are set.
8 In addition to the setting method described above, a parameter
setting method using soft keys is available. Pressing soft key
[INIT] displays the standard value (recommended by FANUC) of
the item selected by the cursor in the key input buffer. Pressing
soft key [EXEC] initializes the item to the standard value.
Pressing soft key [GROUP INIT] initializes all items of a group
(emphasis on velocity or emphasis on precision) selected by the
cursor to the standard values.
The table below indicates the initial settings.
Table 12.4.10 (a) Initial settings
AI contour control
Setting item Emphasis
on velocity
(LV1)
Emphasis
on precision
(LV10)
Unit
Acceleration rate of acceleration/deceleration before interpolation
<ACC FOR BIPL> 4902.000 1042.000 mm/sec2
Acceleration change time (bell-shaped) <ACC CHG TIME(BELL)> 32 64 msec
Allowable acceleration change value <JERK ACC DIFF> 0 0 mm/sec2
Allowable acceleration change value in successive linear
interpolation operations <JERK ACC DIFF(LIN)> 0 0 mm/sec2
Ratio of the change time of the jerk control <JERK ACC RATIO> 0 0 %
Allowable acceleration rate <MAX AACELERATION> 2977.000 596.000 mm/sec2
Time constant for acceleration/deceleration after interpolation
<T-CON AIPL ACC/DEC> 24 24 msec
Corner speed difference <CORNER FEED DIFFER> 1000 400 mm/min
Maximum cutting speed <MAX CUT FEEDRATE> 10000 10000 mm/min
Explanation
- Look-ahead acceleration/deceleration before interpolation
Set an acceleration rate for a linear portion in look-ahead
acceleration/deceleration before interpolation.
Unit of data: mm/sec2, inch/sec2, deg/sec2 (machine unit)
The parameter set on the machining parameter tuning screen is
reflected in the following parameters:
Parameter No. 13610 (velocity-emphasized parameter)
Parameter No. 13611 (precision-emphasized parameter)
Moreover, the following parameter is also set according to the
precision level:
Parameter No. 1660: Maximum allowable acceleration rate for each
axis in acceleration/deceleration before interpolation
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1744 -
- Acceleration change time (bell-shaped)
Set a time constant for a bell-shaped portion in acceleration/
deceleration before look-ahead interpolation.
Unit of data: ms
The parameter set on the machining parameter tuning screen is
reflected in the following parameters:
Parameter No. 13612 (velocity-emphasized parameter)
Parameter No. 13613 (precision-emphasized parameter)
Moreover, the following parameter is also set according to the
precision level:
Parameter No. 1772: Time constant for bell-shaped look-ahead
acceleration/deceleration before interpolation of
constant acceleration time type
CAUTION
A set time constant is applied to all axes. So, a
modification made to this item changes the settings
for all axes.
- Allowable acceleration change value in velocity control based on acceleration
change under jerk control
Unit of data: mm/sec2, inch/sec2, deg/sec2 (machine unit)
Set an allowable acceleration change value per ms for each axis in
velocity control based on acceleration change under jerk control.
The parameter set on the machining parameter tuning screen is
reflected in the following parameters:
Parameter No. 13614 (velocity-emphasized parameter)
Parameter No. 13615 (precision-emphasized parameter)
Moreover, the following parameter is also set according to the
precision level:
Parameter No. 1788: Allowable acceleration change value for each
axis in velocity control based on acceleration
change under jerk control
NOTE
This setting item is displayed only when the jerk
control function is enabled.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1745 -
- Allowable acceleration change value for each axis in velocity control based on
acceleration change under jerk control in successive linear interpolation
operations
Unit of data: mm/sec2, inch/sec2, deg/sec2 (machine unit)
Set an allowable acceleration change value per ms for each axis in
velocity control based on acceleration change under jerk control in
successive linear interpolation operations.
The parameter set on the machining parameter tuning screen is
reflected in the following parameters:
Parameter No. 13616 (velocity-emphasized parameter)
Parameter No. 13617 (precision-emphasized parameter)
Moreover, the following parameter is also set according to the
precision level:
Parameter No. 1789: Allowable acceleration change value for each
axis in velocity control based on acceleration
change under jerk control in successive linear
interpolation operations
CAUTION
1 For an axis with 0 set in this parameter, the
parameters (allowable acceleration change value
in velocity control based on acceleration change
under jerk control: No. 13614, No.13615) are valid.
2 For an axis with 0 set in the parameter (allowable
acceleration change value in velocity control based
on acceleration change under jerk control: No.
13614, No.13615), velocity control based on
acceleration change is disabled, so that this
parameter has no effect.
NOTE
This setting item is displayed only when the jerk
control function is enabled.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1746 -
- Ratio of the change time of the jerk control in smooth bell-shaped
acceleration/deceleration before interpolation
Unit of data: %
Set the ratio (in %) of the change time of jerk control to the change
time of acceleration in smooth bell-shaped acceleration/deceleration
before interpolation.
The parameter set on the machining parameter tuning screen is
reflected in the following parameters:
Parameter No. 13618 (velocity-emphasized parameter)
Parameter No. 13619 (precision-emphasized parameter)
Moreover, the following parameter is also set according to the
precision level:
Parameter No. 1790: Ratio of the change time of the jerk control in
smooth bell-shaped acceleration/deceleration
before interpolation
NOTE
This setting item is displayed only when the jerk
control function is enabled.
- Allowable acceleration rate
Set an allowable acceleration rate in acceleration-based speed
determination.
Unit of data: mm/sec2, inch/sec2, deg/sec2 (machine unit)
The parameter set on the machining parameter tuning screen is
reflected in the following parameters:
Parameter No. 13620 (velocity-emphasized parameter)
Parameter No. 13621 (precision-emphasized parameter)
Moreover, the following parameter is also set according to the
precision level:
Parameter No. 1735: Allowable acceleration rate for each axis
applicable to the deceleration function based
on acceleration in circular interpolation
Parameter No. 1737: Allowable acceleration rate for each axis
applicable to the deceleration function based
on acceleration in AI contour control
CAUTION
When bit 0 (MCR) of parameter No. 13600 is set to
1, the deceleration function based on acceleration
in circular interpolation is not set.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1747 -
- Time constant for acceleration/deceleration after interpolation
Set a time constant for acceleration/deceleration after interpolation.
Unit of data: ms
The parameter set on the machining parameter tuning screen is
reflected in the following parameters:
Parameter No. 13622 (velocity-emphasized parameter)
Parameter No. 13623 (precision-emphasized parameter)
Moreover, the following parameter is also set according to the
precision level:
Parameter No. 1769: Time constant for acceleration/deceleration
after cutting feed interpolation
- Corner speed difference
Set an allowable corner speed difference used for speed determination.
Unit of data: mm/sec, inch/sec, deg/sec (machine unit)
The parameter set on the machining parameter tuning screen is
reflected in the following parameters:
Parameter No. 13624 (velocity-emphasized parameter)
Parameter No. 13625 (precision-emphasized parameter)
Moreover, the following parameter is also set according to the
precision level:
Parameter No. 1783: Allowable speed difference for each axis in
automatic corner deceleration based on speed
difference
- Maximum cutting speed
Set a maximum cutting speed for each axis.
Unit of data: mm/sec, inch/sec, deg/sec (machine unit)
The parameter set on the machining parameter tuning screen is
reflected in the following parameters:
Parameter No. 13626 (velocity-emphasized parameter)
Parameter No. 13627 (precision-emphasized parameter)
Moreover, the following parameter is also set from the precision level:
Parameter No. 1432: Maximum cutting feedrate for each axis in the
AI contour control mode
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1748 -
- Arbitrary items
Two arbitrary parameters can be registered. Each item can correspond
to a CNC parameter or servo parameter. A parameter number
corresponding to each item is to be specified with parameters.
As indicated below, set the parameters for corresponding parameter
numbers, velocity-emphasized parameters (precision level 1), and
precision-emphasized parameters (precision level 10).
Table 12.4.10 (b) Parameters related to arbitrary items
Corresponding
parameter
number
Setting of
velocity-emphasized
(precision level 1)
value
Setting of
precision-emphasized
(precision level 10)
value
Arbitrary item 1 No.13628 No.13630 No.13632
Arbitrary item 2 No.13629 No.13631 No.13633
• Display
Tuning target parameter numbers are displayed.
CAUTION
As arbitrary items, the numbers of the following
parameters cannot be specified:
• Bit parameter
• Spindle parameters (Parameter Nos. 4000 to
4799)
• Real-type parameter
• Power-off parameter
• Nonexistent parameter
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1749 -
12.4.11 Displaying Memory Data
The contents of the CNC memory can be displayed starting at a
specified address.
Displaying memory data
Procedure
1 Set bit 0 (MEM) of parameter No. 8950 to 1 to display the
memory contents display screen.
2 Press function key .
3 Press the continuous menu key , then press chapter selection
soft key [MEMORY].
The following screen appears:
Fig. 12.4.11 (a) Memory contents display screen (10.4-inch)
4 Key in a desired address (hexadecimal) then press soft key
[ADDRES SEARCH]. Starting at the specified address, 256-byte
data is displayed.
(Example: When you input 100000 then press [ADDRES
SEARCH], data is displayed starting at 100000H.)
5 Display data can be switched by using page keys and
and cursor keys , , , and/or .
6 By pressing soft key [BYTE], [WORD], [LONG], or [DOUBLE],
select a data type to be displayed.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1750 -
Explanation
A memory data display format can be selected from the following four
options:
Byte display (1 byte in hexadecimal)
Word display (2 bytes in hexadecimal)
Long display (4 bytes in hexadecimal)
Double display (8 bytes in decimal: Double precision floating-point
display)
One screen displays 256-byte memory data.
NOTE
1 When an address is input, "H" for representing
"hexadecimal" need not be specified at the end of
the address. If H is added, a warning is displayed
to indicate that the format is invalid.
2 When word display is selected as the display
format, an input address is rounded to a multiple of
2 bytes. When long display or double display is
selected, an input address is rounded to a multiple
of 4 bytes.
WARNING
1 If a memory address that must not be accessed in
address search is input, a system alarm is issued.
When making an address search, check that the
address is accessible and that the address is input
correctly.
2 This function is designed for maintenance, and
must not be used by general users.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1751 -
12.4.12 Parameter Tuning Screen
The parameter tuning screen is a screen for parameter setting and
tuning designed to achieve the following:
1 The minimum required parameters that must be set when the
machine is started up are collectively displayed to facilitate
start-up of the machine.
2 The servo tuning screen, spindle tuning screen, and machining
parameter tuning screen are displayed for smooth tuning.
The parameter tuning screen consists of a menu screen and several
setting screens.
12.4.12.1 Displaying the menu screen and selecting a menu item
The parameter tuning menu screen displays the following items:
[START UP]
• SYSTEM SETTING
• AXIS SETTING
• FSSB (AMP)
• FSSB (AXIS)
• SERVO SETTING
• SPINDLE SETTING
• MISCELLANY
[TUNING]
• SERVO TUNING
• SPINDLE TUNING
• AICC TUNING
On the parameter tuning menu screen, one of the displayed items can
be selected to display the corresponding screen. From each setting
screen, you can return to the menu screen by performing a soft key
operation.
NOTE
1 Some items may not be displayed, depending on
the system configuration.
2 When bit 0 (SVS) of parameter No. 3111 is set to 0,
"SERVO SETTING" and "SERVO TUNING" are not
displayed. When bit 1 (SPS) of parameter No. 3111
is set to 0, "SPINDLE TUNING" is not displayed.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1752 -
Displaying the menu screen and selecting a setting screen
Procedure
1 Set the MDI mode.
2 Switch the setting of "PARAMETER WRITE" to "ENABLED".
For details, see the procedure for "PARAMETER WRITE" in
Subsection III-12.4.1.
3 Press function key .
4 Press the continuous menu key several times.
5 Press soft key [PARAM TUNING] to display the menu screen
for parameter tuning .
Fig. 12.4.12.1 (a) Menu screen for parameter tuning (10.4-inch)
6 Move the cursor to a desired item by pressing cursor key
or .
7 Press soft key [SELECT]. The screen display switches to the
selected screen.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1753 -
Returning to the menu screen
Procedure
1 Press soft key [SELECT] on the parameter tuning menu screen
described in Subsection III-12.4.12.1. The screen and soft keys
shown below are displayed. (The screen below is displayed when
"AXIS SETTING" is selected.)
Fig. 12.4.12.1 (b) Axis setting screen (10.4-inch)
2 Press the continuous menu key several times.
3 Press soft key [MENU].
The screen display returns to the parameter tuning menu screen.
4 Upon completion of parameter setting, switch the setting of
"PARAMETER WRITE" to "DISABLED".
NOTE
Some setting screens can also be displayed by a
chapter selection soft key. If a screen is selected
using a chapter selection soft key, however, you
cannot return to the parameter tuning menu screen.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1754 -
Explanation
- Items displayed with [START UP]
The items of [START UP] indicate the screens for setting the
minimum required parameters for starting up the machine.
Table 12.4.12.1 (a) Items displayed with [START UP]
Display item Description
SYSTEM SETTING Screen for setting CNC parameters related to the entire
system configuration
AXIS SETTING Screen for setting CNC parameters related to axes,
coordinates, feedrate, and acceleration/deceleration
FSSB (AMP) FSSB amplifier setting screen
FSSB (AXIS) FSSB axis setting screen
SERVO SETTING Servo setting screen
SPINDLE SETTING Screen for setting spindle-related parameters
MISCELLANY
Screen for setting parameters related to the allowable
number of M code digits and whether to display the
servo setting and spindle tuning screens
NOTE
Some items may not be displayed, depending on
the system configuration.
- Items displayed with [TUNING]
The items of [TUNING] indicate the screens for servo, spindle, and
high-speed high-precision machining tuning.
Fig. 12.4.12.1 (b) Items displayed with [TUNING]
Display item Description
SERVO TUNING Servo tuning screen
SPINDLE TUNING Spindle tuning screen
AICC TUNING Machining parameter tuning screen
NOTE
1 Some items may not be displayed, depending on
the system configuration.
2 When bit 0 (SVS) of parameter No. 3111 is set to
0, "SERVO SETTING" and "SERVO TUNING" are
not displayed. When bit 1 (SPS) of parameter No.
3111 is set to 0, "SPINDLE TUNING" is not
displayed.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1755 -
12.4.12.2 Parameter tuning screen (system setting)
This screen enables the parameters related to the entire system
configuration to be displayed and modified. The parameters can be
initialized to the standard values (recommended by FANUC).
Display and setting
Procedure
1 Move the cursor to [SYSTEM SETTING] by pressing cursor key
or on the parameter tuning menu screen described
in Subsection III-12.4.12.1.
2 Press soft key [SELECT]. The screen display switches to the
screen and soft keys shown below.
Fig. 12.4.12.2 (a) Parameter tuning screen (system setting) (10.4-inch)
3 Move the cursor to a parameter number to be set or displayed,
according to one of the methods below.
• Enter the parameter number and press soft key [NO.SRH] .
• Move the cursor to the desired parameter number by
pressing page key or , and cursor keys ,
, , and/or .
A brief description of the parameter where the cursor is
placed is provided at the bottom of the screen. However, no
description is provided when the cursor is placed on
multiple bits for bit parameters.
4 Input desired data then press the key on the MDI panel to
set the parameter.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1756 -
5 Press soft key [INIT]. The standard value (recommended by
FANUC) for the item selected by the cursor is displayed in the
key input buffer. Pressing soft key [EXEC] in this state initializes
the item to the standard value.
6 Press soft key [G_INIT]. A message asking whether to set the
group standard values is displayed on the screen. Pressing soft
key [EXEC] in this state inputs all of the standard values of the
group.
NOTE
1 If the cursor is placed on a parameter that has no
standard value assigned, no standard value is input
even when [INIT] is pressed.
2 When the cursor is placed on multiple bits for bit
parameters, the multiple bits can be input
simultaneously. When [INIT] is pressed in this
state, the key input buffer displays the standard
values for the bits where the cursor is placed. If a
bit has no standard value assigned, "*" is displayed
for the bit, and no value is input for the bit.
3 When [G_INIT] is pressed, those parameters that
have no standard values assigned are not
initialized.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1757 -
12.4.12.3 Parameter tuning screen (axis setting)
This screen enables the CNC parameters related to axes, coordinates,
feedrate, and acceleration/deceleration to be displayed and set. The
parameters displayed can be divided into four groups:
(Basic) group :
The parameters related to basic settings are displayed.
(Coordinate) group :
The parameters related to coordinates are displayed.
(Feedrate) group :
The parameters related to feedrate are displayed.
(Acceleration/deceleration) group:
The parameters related to acceleration/deceleration are displayed.
The parameters can be initialized to the standard values
(recommended by FANUC). For the display and setting procedure, see
the description of the parameter tuning screen (system setting) in
Subsection III-12.4.12.2.
Fig. 12.4.12.3 (a) Parameter tuning screen (axis setting) (10.4-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1758 -
12.4.12.4 Displaying and setting the FSSB amplifier setting screen
From the parameter tuning screen, the FSSB amplifier setting screen
can be displayed. For details of the FSSB amplifier setting screen, see
the description of the FSSB amplifier setting screen in Subsection
1.4.4 in the Connection Manual (Function) (B-63943EN-1).
Fig. 12.4.12.4 (a) FSSB amplifier setting screen (10.4-inch)
Fig. 12.4.12.4 (b) FSSB amplifier setting screen 2 (10.4-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1759 -
12.4.12.5 Displaying and setting the FSSB axis setting screen
From the parameter tuning screen, the FSSB axis setting screen can be
displayed. For details of the FSSB axis setting screen, see the
description of the FSSB axis setting screen Subsection 1.4.4 in the
Connection Manual (Function) (B-63943EN-1).
Fig. 12.4.12.5 (a) FSSB axis setting screen (10.4-inch)
12.4.12.6 Displaying and setting the servo setting screen
From the parameter tuning screen, the servo setting screen can be
displayed. For details of the servo setting screen, see the description of
the servo setting screen in Subsection III-12.4.4.
Fig. 12.4.12.6 (a) Servo setting screen (10.4-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1760 -
12.4.12.7 Parameter tuning screen (spindle setting)
The spindle-related parameters can be displayed and modified.
For the display and setting procedure, see the description of the
parameter tuning screen (system setting) in Subsection III-12.4.12.2.
Fig. 12.4.12.7 (a) Parameter tuning screen (spindle setting) (10.4-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1761 -
12.4.12.8 Parameter tuning screen (miscellaneous settings)
The parameters related to the allowable number of M code digits and
whether to display the servo setting and spindle tuning screens can be
displayed and modified. Moreover, the parameters can be initialized to
the standard values (recommended by FANUC).
For the display and setting procedure, see the description of the
parameter tuning screen (system setting) in Subsection III-12.4.12.2.
Fig. 12.4.12.8 (a) Parameter tuning screen (Miscellaneous setting)
(10.4-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1762 -
12.4.12.9 Displaying and setting the servo tuning screen
From the parameter tuning screen, the servo tuning screen can be
displayed. For details of the servo tuning screen, see the description of
the servo tuning screen in Subsection III-12.4.5.
Fig. 12.4.12.9 (a) Servo tuning screen (10.4-inch)
12.4.12.10 Displaying and setting the spindle tuning screen
From the parameter tuning screen, the spindle tuning screen can be
displayed. For details of the spindle tuning screen, see the description
of the spindle tuning screen in Subsection III-12.4.7.
Fig. 12.4.12.10 (a) Spindle tuning screen (10.4-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1763 -
12.4.12.11 Displaying and setting the machining parameter tuning
screen
From the parameter tuning screen, the machining parameter tuning
screen can be displayed. For details of the machining parameter
tuning screen, see the description of the machining parameter tuning
screen in Subsection III-12.4.10.
Fig. 12.4.12.11 (a) Machining parameter tuning screen (10.4-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1764 -
Explanation
- Parameters displayed for parameter tuning
Table 12.4.12 (a) Parameters displayed for parameter tuning (1)
Menu Group
Parameter
No. Name Brief description
Standard
setting
981 Sets the path of each axis.
982 Sets the path of each spindle.
983 Sets the T series/M series of each path. 0:T series/1:M series
984#0 LCP Sets the attribute of each path. 0:Normal/1:Loader control *1
3021 Sets the G/F signal address of each axis. *2
3022 Sets the G/F signal address of each spindle. *3
3006#0 GDC The deceleration signal for reference position return is:
0:X signal/1:G signal
1
3008#2 XSGx The signal address allocated to address X is:
0:Fixed/1:Set by the parameter
1
3013 Address allocated to the deceleration signal for reference position
return
*4
SYSTEM
SETTING
System
setting
3014 Bit position allocated to the deceleration signal for reference
position return
*5
*1 : The value 1 is set for the paths as many as the number of loader
paths starting from the greatest path number. For path 1, the value 0
is set at all times.
Example) When the number of loader paths is 3 in a 10-path system:
The value 1 is set for paths 8 to 10. The value 0 is set for
others.
*2 : When intra-path axis number ≤ 8, (path number - 1)*10+(intra-path
axis number - 1)
When intra-path axis number ≥ 9, no standard value is available.
Example) When path 1 has 9 axes, and path 2 has 3 axes:
0,1,...,7,(none) for axes of path 1, 10,11,12 for axes of path 2
*3 : When intra-path spindle number ≤ 4, (path number -
1)*10+(intra-path spindle number - 1)
When intra-path spindle number ≥ 5, no standard value is available.
Example) When path 1 has 5 spindles, and path 2 has 1 spindle:
0,1,...,4,(none) for spindles of path 1, 10 for spindle of path
2
*4 : When (path number ≤ 3) and (intra-path axis number ≤ 8)
Axes of path 1: 9
Axes of path 2: 7
Axes of path 3: 10
Other axes: No standard value is available.
Example) When path 1 has 9 axes, and path 2 has 3 axes:
9,9,9,9,9,9,9,9,(none) for axes of path 1, 7,7,7 for axes of
path 2
*5 : When (path number ≤ 3) and (intra-path axis number ≤ 8)
(Intra-path axis number - 1)
Other axes: No standard value is available.
Example) When path 1 has 9 axes, and path 2 has 3 axes:
0,1,...,7,(none) for axes of path 1, 0,1,2 for axes of path 2
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1765 -
Table 12.4.12 (b) Parameters displayed for parameter tuning (2)
Menu Group
Parameter
No. Name Brief description
Standard
setting
3716#0 A/Ss Sets the type of spindle motor: 0:Analaog/1:Serial.
3717 Sets a motor number to be assigned to each spindle.
SPINDLE
SETTING
Spindle
setting
3706#4 GTT Specifies a spindle gear selection method.
0:M type/1:T type
3718 Sets a suffix to be added to spindle speed display on a screen
such as the position display screen.
3735 Sets the minimum clamp speed of the spindle motor.
3736 Sets the maximum clamp speed of the spindle motor.
3741 Sets the maximum spindle speed for gear 1.
3742 Sets the maximum spindle speed for gear 2.
3743 Sets the maximum spindle speed for gear 3.
3744 Sets the maximum spindle speed for gear 4.
3772 Sets the maximum speed of the spindle.
When 0 is set, the speed is not clamped.
4133 Sets the motor model code of the serial spindle.
(This setting is not required for an analog spindle.)
4019#7 ***
The parameters for the serial spindle are:
0:Not automatically set/1:Automatically set
(This setting is not required for an analog spindle.)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1766 -
Table 12.4.12 (c) Parameters displayed for parameter tuning (3)
Menu Group
Parameter
No. Name Brief description Standard
setting
AXIS
SETTING
Basic 1001#0 INM Least command increment on linear axes:
0:Metric (millimeter machine) 1:Inch (inch machine)
1005#0 ZRNx When an automatic operation (other than G28) is executed before
reference position return:
0:Alarm is issued (PS224) 1:No alarm is issued.
0
1005#1 DLZx Reference position return without dogs: 0:Disabled 1:Enabled
1006#0 ROTx Setting of linear axes or rotary axis:
0:Linear axis 1:Rotation axis
1006#3 DIAx Setting of the amount of travel:
0:Radius specification 1: Diameter specification
1006#5 ZMIx Reference position return direction:
0:Plus direction 1:Minus direction
1008#0 ROAx Rotation axis roll-over function: 0:Disabled 1:Enabled 1
1008#2 RRLx With the amount of travel per revolution, relative coordinates are:
0:Not rounded 1:Rounded
1
1013#0 ISAx Sets the least input increment and least command increment:
0:IS-B 1:IS-A
1013#1 ISCx Sets the least input increment and least command increment:
0:IS-B 1:IS-C
1013#2 ISDx Sets the least input increment and least command increment:
0:IS-B 1:IS-D
1013#3 ISEx Sets the least input increment and least command increment:
0:IS-B 1:IS-E
1020 Program name *1
1022 Sets each axis in the basic coordinate system. *2
1023 Servo axis number
1815#1 OPTx A separate pulse coder is: 0:Not used 1:Used
1815#4 APZx The correspondence between machine positions and
absolute-position detector positions is: 0:Not established
1:Established
1815#5 APCx The position detector used is: 0:Other than an absolute-position
detector 1:Absolute-position detector
1825 Servo loop gain
1826 Effective area
1828 Positional deviation limit during travel
1829 Positional deviation limit during stop 500
*1 : For the M series: 88(X),89(Y),90(Z) sequentially starting with the
first axis (no standard value for the fourth axis and
up)
For the T series: 88(X),90(Z) (no standard value for the third axis
and up)
*2 : For the M series: 1,2,3 sequentially starting with the first axis (no
standard value for the fourth axis and up)
For the T series: 1,3 (no standard value for the third axis and up)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1767 -
Table 12.4.12 (d) Parameters displayed for parameter tuning (4)
Menu Group
Parameter
No. Name Brief description Standard
setting
AXIS SETTING Coordinate 1240 Machine coordinate of the first reference position
1241 Machine coordinate of the second reference position
1260 Amount of travel per revolution of a rotary axis 360.000
1320 Coordinate of the boundary of stored stroke check 1 in the
positive direction
1321 Coordinate of the boundary of stored stroke check 1 in the
negative direction
Feedrate 1401#6 RDR For a rapid traverse command, dry run is:
0:Disabled 1:Enabled
0
1410 Dry run feedrate
1420 Rapid traverse rate
1421 Rapid traverse override F0 rate
1423 Jog feedrate
1424 Manual rapid traverse rate
1425 FL feedrate for reference position return
1428 Reference position return feedrate
1430 Maximum cutting feedrate
Acceleration/
deceleration
1610#0 CTLx Acceleration/deceleration for cutting feed is:
0:Exponential acceleration/deceleration
1:Linear acceleration/deceleration after interpolation
1610#4 JGLx Acceleration/deceleration for jog feed is:
0:Exponential acceleration/deceleration
1:Same as acceleration/deceleration for cutting feed
(The settings of bit 1 (CTBx) and bit 0 (CTLx) of parameter
No. 1610 are followed.)
1620 Time constant for linear acceleration/deceleration for rapid
traverse
1622 Time constant for acceleration/deceleration for cutting feed
1623 FL feedrate for acceleration/deceleration after interpolation
for cutting feed
1624 Time constant for acceleration/deceleration for jog feed
1625 FL feedrate for exponential acceleration/deceleration for
jog feed
MISCELLANY MISC 3030 Allowable number of digits of an M code 3
3111#0 SVS The servo setting screen is: 0:Not displayed
1:Displayed
1
3111#1 SPS The spindle setting screen is: 0:Not displayed
1:Displayed
1
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1768 -
12.4.13 Periodic Maintenance Screen
Periodic maintenance screens are used for managing consumables
(such as the backlight of a LCD unit and backup batteries). By setting
the name of a consumable, its life time, and the method for counting
down the life time, the life of the consumable can be counted down in
the appropriate method set for the consumable, and the remaining life
time can be displayed.
With these screens, the user can easily manage consumables that
require periodic replacement.
Explanation
There are four periodic maintenance screens: the status screen, the
setting screen, the machine menu screen, and the NC menu screen.
• Status screen:
Item names, remaining times, and count statuses are displayed,
and item names are set.
• Setting screen:
Life times, remaining times, and count types (count-down
method) are set.
• Machine menu screen:
The names of consumables in the machine can be registered.
• NC menu screen:
The names of consumables in the NC are already registered.
Using periodic maintenance screens
<1> Referencing a periodic maintenance screen
Display the status screen. For the meanings of items on the status
screen, see Status screen.
<2> Adding the name of a new consumable item to a periodic
maintenance screen or editing an existing consumable item on
the screen
The name of a consumable item can be added or edited on the
machine menu screen. For details, see Machine menu screen.
<3> Adding or editing a life time, remaining time, and a method of
counting down the remaining time for a consumable on a
periodic maintenance screen
A life time and remaining time can be added or edited on the
setting screen. For details, see Setting screen.
<4> Newly displaying the item name and remaining time of a
consumable on a periodic maintenance screen.
1 Setting an item name
Select the item name of a consumable to be displayed from
the machine menu screen or NC menu screen, or enter the
name using the MDI keys. For the procedure, see Item
name in Status screen.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1769 -
2 Setting a life time, remaining time, and count type
Select the life time, remaining time, and count type of a
consumable to be displayed from the setting screen. For the
procedure, see Remaining time in Status screen.
Procedure for displaying a periodic maintenance screen
1 Press function key .
2 Press the continuous menu key several times to display
[PERIOD MAINTE].
3 Press soft key [PERIOD MAINTE] to display the periodic
maintenance screen.
Status screen
When soft key [STATUS] is pressed, the status screen is displayed.
The status screen shows the item names, count statuses, and remaining
times of managed consumables.
Fig. 12.4.13 (a) Status screen
- Item name
As the item name, set the name of a consumable to be managed by
periodic maintenance. To set an item name, select a name from the
machine menu screen or NC menu screen, or directly enter the name
using the MDI keys.
Setting an item name from a menu screen
1 On the status screen, move the cursor to a target item name, press
soft key [(OPRT)], then press soft key [ENTRY].
2 Press soft key [MACHINE] or [NC] to display the machine menu
screen or NC menu screen.
3 Move the cursor to an existing item name on the menu screen,
press soft key [(OPRT)], and press soft key [SELECT] then
[EXEC] successively.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1770 -
4 The screen display returns to the status screen, and the item name
selected on the menu screen is added to the status screen.
Initially, there is no item name set on the machine menu screen, so
item names must be registered in advance. For the registration method,
see the description of the procedure for registering item names on the
machine menu screen.
Setting an item name using the MDI keys
1 Press soft key [(OPRT)].
2 Type the alphanumeric characters to be input, then press soft key
[INPUT].
3 The entered item name is registered on the status screen.
When soft key [+INPUT] is pressed instead of soft key [INPUT], the
entered characters can be added to an existing item name.
When typing 2-byte characters, type "*" before and after the character
codes. The character codes must conform to FANUC codes. (See
Appendix G, "FANUC 2-BYTE CHARACTER CODE TABLE".)
An item name to be registered must be up to 24 characters long if it
consists of alphanumeric characters only; or it must be up to 12
characters long if it consists of 2-byte characters only.
Example: To register "LCD バックライト", enter the following:
>LCD＊110E10F410CC114010B610FE＊_
NOTE
1 An asterisk "*" is used as a control code, so it
cannot be used in item names. In addition,
characters "[", "]", "(", and ")" cannot be used in
item names.
2 When an item name consisting of both
alphanumeric characters and 2-byte characters is
registered, the warning "DATA OUT OF RANGE"
may be output.
Deleting an item name
To delete a registered item name, move the cursor to the item name,
press soft key [ERASE], then press soft key [EXEC].
When an item name is deleted, its life time, remaining time, and count
type are deleted at the same time.
- Remaining time
As the remaining time, the period of time left until the time for
replacement is reached by count down operation is displayed.
If the percentage of the remaining time to the life time has reached to
the value (%) specified by parameter No. 8911, or smaller, the
remaining time is displayed in red.
Even after the life time has expired, count down operation continues.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1771 -
Setting the remaining time
1 On the status screen, place the cursor on an item for which the
remaining time is to be set (the item name must have been set in
advance).
2 Press soft key [(OPRT)], then press soft key [CHANGE].
3 The screen display changes to the setting screen.
4 Set the life time, remaining time, and count type. For the setting
method and other information, see Setting screen.
NOTE
On the status screen, the remaining time and life
time cannot be set.
These items must be set on the setting screen.
- Count status
The count status is indicated on the left side of the item number as
follows:
Indication Count status
Blank Counting stopped
@ Counting in progress
＊ Life expired
Setting screen
On the setting screen, the life time, remaining time, and count type of
a managed consumable are set.
Fig. 12.4.13 (b) Setting screen
Display procedure
1 When the status screen is displayed, press soft key [(OPRT)].
2 Press soft key [CHANGE].
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1772 -
- Life time
Set the life time of a consumable.
Move the cursor to an existing item, type a life time, then press soft
key [INPUT] (or the key). The life time is then set, and the
same value is set also as the remaining time.
At this time, "------" is indicated in the count type field.
When soft key [+INPUT] is pressed, the entered value can be added to
the life time already set. The same value as the added value is added
also to the remaining time.
A value ranging from 0 to 65535 (in hours) can be set.
NOTE
1 If a setting operation is attempted when the item
name is not registered, the warning "EDIT
REJECTED" is issued.
2 If a value exceeding the valid range is entered, the
warning "DATA IS OUT OF RANGE" is issued.
3 If soft key [ERASE] or [TYPE] is pressed, the
warning "EDIT REJECTED" is issued.
- Remaining time
The period of time left until the time for replacement is reached by
count down operation is indicated.
If the percentage of the remaining time to the life time has reached the
value (%) specified by parameter No. 8911, or smaller, the remaining
time is displayed in red.
Even after the life time has expired, count down operation continues.
Move the cursor to the remaining time of a target registered number,
type a remaining time, then press soft key [INPUT] (or the
key). The remaining time is then set.
When soft key [+INPUT] is pressed, the entered value can be added to
the remaining time already set.
A value ranging from 0 to (life time) can be set.
When soft key [ERASE] then soft key [EXEC] are pressed, the same
value as the life time is set.
NOTE
1 If a setting operation is attempted when the item
name or life time is not registered, the warning
“EDIT REJECTED” is issued.
2 When a value exceeding the valid range is entered,
the warning “DATA IS OUT OF RANGE” is issued.
3 If soft key [TYPE] is pressed, the warning “EDIT
REJECTED” is issued.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1773 -
- Count type
As the count type, select the way of counting.
Place the cursor on the count type of a target registration number, then
press soft key [TYPE]. Count types are displayed as soft keys as
shown below. Select one of these soft keys, then press soft key
[EXEC].
Soft key Meaning Indication
[NO CNT] Counting is not performed (stopped) — — — — — —
[ALL] Counting is performed at all times All times
[POWER ON] Counting is performed when power
is on.
When power is on
[RUN] Counting is performed when
operation is in progress.
When operation is
in progress
[CUT] Counting is performed when cutting
is being performed.
When cutting is
being performed
NOTE
1 If a setting operation is attempted when the item
name or life time is not registered, the warning
“EDIT REJECTED” is issued.
2 Soft keys [INPUT] and [+INPUT] have no effect.
3 When counting is performed at all times, a 24-hour
error is generated in leap year.
4 If soft key [ERASE] is pressed, the warning “EDIT
REJECTED” is issued.
Machine menu screen
On the machine menu screen, the names of consumables of the
machine are registered. From this screen, item names can be added to
the status screen. For the method of addition to the status screen, see
the description of the status screen.
Fig. 12.4.13 (c) Machine menu screen
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1774 -
- Displaying the screen
1 When the status screen is displayed, press soft key [MACHINE].
On the machine menu screen, item names can be registered using one
of the following two methods:
• Registration from a program
• Registration using the MDI keys
- Registration from a program
By executing a program having the following format, an item name
can be registered in the menu of the machine:
Format
G10 L61 Px [n]
X Registration number
n Item name, format:
[alphanumeric-characters*2-byte-characters*alphanumeric-characters]
- Registration using the MDI keys
An item name can be registered on the menu screen of the machine by
typing the item name in the format shown below on the machine menu
screen, then pressing soft key [INPUT] (or the key).
When soft key [+INPUT] is pressed, the typed characters can be
added to an already registered item name.
Format
Alphanumeric-characters*2-byte-characters*alphanumeric-characters
Two-byte codes must conform to FANUC codes. (See Appendix G,
"FANUC 2-BYTE CHARACTER CODE TABLE".)
When typing 2-byte characters, type an asterisk "*" before and after
the character codes. An item name to be registered must be up to 24
characters long if it consists of alphanumeric characters only; or it
must be up to 12 characters long if it consists of 2-byte characters only.
Example:
To register "LCD バックライト", enter the following:
>LCD＊110E10F410CC114010B610FE＊_
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1775 -
NOTE
1 An asterisk "*" is used as a control code, so it
cannot be used in item names. In addition,
characters "[", "]", "(", and ")" cannot be used in
item names.
2 When an item name consisting of both
alphanumeric characters and 2-byte characters is
registered, the warning “DATA IS OUT OF
RANGE” may be output.
3 When a blank item name is selected on the
machine screen, the warning “EDIT REJECTED” is
issued.
To delete a registered item name, move the cursor to the item name,
press soft key [ERASE], then press soft key [EXEC].
From this screen, an item name can be registered on the status screen.
For the method of registration to the status screen, see the description
of the status screen.
Fig. 12.4.13 (d) NC menu screen
- Displaying the screen
1 When the status screen is displayed, press soft key [NC].
NOTE
On the NC screen, the registration, deletion, and
I/O of item names cannot be performed.
When a blank item name is selected, a blank is set.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1776 -
12.4.14 System Configuration Screen
The system configuration screen provides information about the types
of installed hardware and software.
Procedure for displaying the screen
Procedure
1 Press the key to display a screen that shows parameters
and other information.
2 Press soft key [SYSTEM]. The system configuration screen is
displayed.
There are two types of system configuration screens: the hardware
configuration screen and the software configuration screen. The screen
display can switch between these screens by using and .
When soft key [SERVO INFO] or [SPINDLE INFO] is pressed,
information about the connected servo system or spindles is displayed.
Fig. 12.4.14 (a) System configuration screen
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1777 -
Hardware configuration screen
This screen shows the names and IDs of the hardware used by the NC.
Fig. 12.4.14 (b) Hardware configuration screen
Software configuration screen
This screen shows the names and series/editions of the software used
by the NC.
Fig. 12.4.14 (c) Software configuration screen
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1778 -
Servo information screen
When a servo system is connected to the NC, ID information of the
connected servo devices (servo motors and servo amplifier modules)
can be displayed on the NC.
Displaying the screen
1 When the system configuration screen is displayed, press soft
key [SERVO INFO].
2 The servo information screen is displayed.
Fig. 12.4.14 (d) Servo information screen
Spindle information screen
When a spindle system is connected to the NC, the ID information of
the connected spindle devices (spindle motors and spindle amplifier
modules) can be displayed on the NC.
Displaying the screen
1 When the system configuration screen is displayed, press soft
key [SPINDLE INFO].
2 The spindle information screen is displayed.
Fig. 12.4.14 (e) Spindle information screen
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1779 -
12.4.15 Overview of the History Function
The history function makes it possible to record a history of
operations performed by the operator, alarms and external operator
messages issued, and other history data, check the history, and output
history data.
1 Conditions for recording history
a Display screen
A history of screens other than the operation history screen
is recorded.
b Signal selection
Up to 60 I/O signals can be selected so that they can be
recorded in history data.
c Parameter setting
With parameters, it is possible to separately set whether to
record an MDI key operation history and an external
operator message history, add external alarms and messages,
and record data modification histories such as operation
histories of parameters, tool offsets, workpiece offsets
(workpiece shift amounts), custom macro common variables,
and I/O signals.
d Storage capacity
When the storage capacity becomes full, data is deleted in
order from the oldest data.Up to about 8000 items of history
data can be recorded if the data consists of history data of
MDI key operations only.
2 Data output
All history data stored can be output to external input/output
devices. (See Subsection 12.4.15.5, "Outputting all history
data".)
3 Erasure of history data
If bit 7 (EKE) of parameter No. 3195 is set to 1, soft key
[CLEAR] is displayed, allowing the user to erase history data.
#7 #6 #5 #4 #3 #2 #1 #0
3195 EKE
[Data type] Bit
# 7 EKE Soft key [ALL CLEAR] for clearing all history data is:
0: Not displayed.
1: Displayed.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1780 -
NOTE
1 History data remains even after the power is turned
off.
Memory clear operation, however, erases history
data as well.
2 Set the time and date correctly on the setting
screen.
3 All history data including data of alarms, external
operator messages, operations, and I/O signals is
integrated and maintained in a single storage area.
When the storage capacity becomes full, history
data is erased in order from the oldest data
regardless of the history type.
When history data is erased, all history data is
erased, so care should be taken.
It is impossible to erase only a specific history.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1781 -
12.4.15.1 Alarm history
From all history data recorded, only alarm history is extracted and
displayed on the screen. Note that when the amount of history data
exceeds the storage capacity, history data is automatically erased in
order from the oldest history data.
Fig. 12.4.15.1 (a) Alarm history screen
Screen display
Issued alarms are displayed sequentially from the latest alarm.
The following information is displayed for each alarm:
• Path name (only when multipath operation is performed)
• Time and date of alarm occurrence
• Type and number of the alarm
• Alarm message
NOTE
To record also external alarm and macro alarm
messages as history data, set bit 3 (EAH) of
parameter No. 3112 to 1, and at the same time set
bit 7 (HAL) of parameter No. 3196 to 0.
When a name such as a path name, axis name, or spindle name has
been changed after the issuance of an alarm, a newly assigned name is
displayed on the alarm history screen.
When modal O data that is a program name is output, only the first
five characters are output.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1782 -
Procedure
1 Press function key to display a screen of parameters and
so on.
2 Press return menu key .
3 Press continuous menu key several times until soft key
[HISTRY] is displayed.
4 Press soft key [HISTRY]. The alarm history screen is then
displayed.
5 The screen display can be changed to the previous page and the
next page by using page keys and .
Erasing history data from the alarm history screen
Procedure
1 Display the alarm history screen.
2 Press soft key [(OPRT)].
3 Press soft key [CLEAR]. All history data is then erased.
NOTE
When history data is erased, not only alarm history
data but also other history data such as external
operator message history data and operation
history data is erased. It is impossible to erase
only a specific history.
Display of external alarms and macro alarms
When an external alarm or macro alarm is issued, it becomes possible
to record its message as well as the alarm number in the alarm history
if the parameter shown below is set. As the message of an external
alarm or macro alarm, the first 32 characters for the external alarm or
the first 26 characters for the macro alarm are recorded.
#7 #6 #5 #4 #3 #2 #1 #0
3112 EAH
[Data type] Bit
# 3 EAH Messages of the external alarm/macro alarm in alarm or operation
history:
0: Not recorded
1: Recorded
NOTE
This parameter is valid when bit 7 (HAL) of
parameter No. 3196 is set to 0.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1783 -
#7 #6 #5 #4 #3 #2 #1 #0
3196 HAL
[Data type] Bit
# 7 HAL When an alarm is issued, additional information (modal data, absolute
coordinates, and machine coordinates present at the issuance of the
alarm) is:
0: Recorded in the operation history and alarm history.
1: Not recorded in the operation history and alarm history.
NOTE
1 History data such as alarm history data, operation
history data, external operator message history
data, and data modification history data is stored in
the same storage area. Therefore, alarm history
data may be erased when the storage capacity is
exceeded by other history data.
2 The maximum number of history data items that
can be stored is as follows, where the history data
is assumed to include alarm data only:
When bit 7 (HAL) of parameter No. 3196 is set to 1,
up to about 4000 history data items can be stored.
When bit 7 (HAL) of parameter No. 3196 is set to 0,
modal information and coordinates observed when
an alarm is issued are also recorded, so the
maximum number of history data items that can be
stored varies from system to system. (Example:
For a 5-axis system, up to about 280 data items
can be stored; for a 10-axis system, up to about
200 data items can be stored.)
When bit 3 (EAH) of parameter No. 3112 is set to
1, however, macro and external alarm messages
are also stored, so the number of data items that
can be stored further decreases.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1784 -
12.4.15.2 External operator message history
From all history data recorded, only external operator message history
and macro message history are extracted and displayed on the screen.
When the amount of history data exceeds the storage capacity, history
data is automatically erased in order from the oldest history data.
Fig. 12.4.15.2 (a) External operator message history screen
Screen display
Procedure
1 Press function key .
2 Press continuous menu key several times until soft key
[MESSAGE HISTRY] is displayed.
3 Press soft key [MESSAGE HISTRY]. The external operator
message history screen is displayed.
4 The screen display can be changed to the previous page and the
next page by using page keys and .
NOTE
1 History data such as external operator message
history data, operation history data, alarm history
data, and data modification history data is stored in
the same storage area. Therefore, external operator
message history data may be erased when the
storage capacity is exceeded by other history data.
2 The maximum number of history data items that can
be stored is about 150 if the history data includes
external operator message data only.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1785 -
Erasing history data from the external operator message history screen
Procedure
1 Display the external operator message history screen.
2 Press soft key [(OPRT)].
3 Press soft key [CLEAR]. All history data is then erased.
NOTE
When history data is erased, not only external
operator message history data but also other
history data such as operation history data and
alarm history data is erased. It is impossible to
erase only a specific history.
Parameter setting
#7 #6 #5 #4 #3 #2 #1 #0
3112 OMH
[Data type] Bit
# 2 OMH The external operator message history screen is:
0: Not displayed.
1: Displayed.
#7 #6 #5 #4 #3 #2 #1 #0
3196 HOM
[Data type] Bit
# 6 HOM A history of external operator messages and macro messages is:
0: Recorded.
1: Not recorded.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1786 -
12.4.15.3 Operation history
This function displays a history of the operator's key operations and
signal operations made when a failure occurred or an alarm was issued,
and also information about alarms.
The following data is recorded:
a Operation history
ⅰ MDI key operations made by the operator
ⅱ I/O signal (X,Y,G,F) on/off switching
b Alarm history
ⅰ Alarms issued
ⅱ Modal information in a block executed and coordinates
observed when an alarm was issued
(Not displayed on the screen)
c Data modification history
ⅰ Modification of tool offset data
(When bit 0 (HTO) of parameter No. 3196 is set to 1)
ⅱ Modification of workpiece offset data/extended workpiece
offset data/workpiece shift (T series)
(When bit 1 (HWO) of parameter No. 3196 is set to 1)
ⅲ Modification of parameters
(When bit 2 (HPM) of parameter No. 3196 is set to 1)
ⅳ Modification of custom macro common variable data
(When bit 3 (HMV) of parameter No. 3196 is set to 1)
d External operator message history and macro message history
(When bit 6 (HOM) of parameter No. 3196 is set to 0)
e Time stamp (time and date)
With some exceptions, history data of the operation history and alarm
history can be viewed on the operation history screen. (The data
modification history, external operator message history, and alarm
messages are not displayed.)
All recorded history data can be output to external input/output
devices.
NOTE
Up to about 8000 items of history data can be
recorded if the data includes history data of MDI
key operations only. However, because history data
varies in size, the maximum number of history data
items that can be recorded is not fixed.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1787 -
Parameter setting
#7 #6 #5 #4 #3 #2 #1 #0
3106 OPH
[Data type] Bit
# 4 OPH The operation history screen is:
0: Not displayed.
1: Displayed.
3122 Time interval used to record time data in operation history
[Input type] Parameter input
[Data type] Word path
[Unit of data] min
[Valid data range] 0 to 1440
When history data is recorded within a set time period, the time for
each set time period is recorded in the history data.
When 0 is set, the specification of a time period of 10 minutes is
assumed.
If no data is recorded within a set time period, the time for that period
is not recorded.
NOTE
The same value must be set in this parameter for
all paths.
#7 #6 #5 #4 #3 #2 #1 #0
3195 EKE HDE HKE
[Input type] Parameter input
[Data type] Common to the bit system
# 5 HKE A key operation history is:
0: Recorded.
1: Not recorded.
# 6 HDE A DI/DO history is:
0: Recorded.
1: Not recorded.
# 7 EKE Soft key [ALL CLEAR] for clearing all history data is:
0: Not displayed.
1: Displayed.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1788 -
#7 #6 #5 #4 #3 #2 #1 #0
3196 HAL HOM HMV HPM HWO HTO
[Data type] Bit
# 0 HTO A modification history of tool offset data is:
0: Not recorded.
1: Recorded.
# 1 HWO A modification history of workpiece offset data/extended workpiece
offset data/workpiece shift (T series) is:
0: Not recorded.
1: Recorded.
# 2 HPM A modification history of parameters is:
0: Not recorded.
1: Recorded.
# 3 HMV A modification history of custom macro common variables is:
0: Not recorded.
1: Recorded.
# 6 HOM A history of external operator messages and macro messages is:
0: Recorded.
1: Not recorded.
# 7 HAL When an alarm is issued, additional information (modal data, absolute
coordinates, and machine coordinates present at the issuance of the
alarm) is:
0: Recorded in the operation history and alarm history.
1: Not recorded in the operation history and alarm history.
To record as many alarm history items as possible, rather than detailed
alarm information, set 1. The numbers of ten G code modal groups to
be recorded are set in parameter Nos. 12990 to 12999.
12990
(1st) G code modal group to be recorded in the history when an alarm is issued
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to the maximum number of G code groups
Set the number of a G code modal group to be recorded in the alarm
history and operation history when an alarm is issued.
* If a value beyond the valid data range is set, the status of group
01 is recorded.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1789 -
12991
(2nd) G code modal group to be recorded in the history when an alarm is issued
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to the maximum number of G code groups
Set the number of a G code modal group to be recorded in the alarm
history and operation history when an alarm is issued.
* If a value beyond the valid data range is set, the status of group
02 is recorded.
12992
(3rd) G code modal group to be recorded in the history when an alarm is issued
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to the maximum number of G code groups
Set the number of a G code modal group to be recorded in the alarm
history and operation history when an alarm is issued.
* If a value beyond the valid data range is set, the status of group
03 is recorded.
12993
(4th) G code modal group to be recorded in the history when an alarm is issued
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to the maximum number of G code groups
Set the number of a G code modal group to be recorded in the alarm
history and operation history when an alarm is issued.
* If a value beyond the valid data range is set, the status of group
04 is recorded.
12994
(5th) G code modal group to be recorded in the history when an alarm is issued
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to the maximum number of G code groups
Set the number of a G code modal group to be recorded in the alarm
history and operation history when an alarm is issued.
* If a value beyond the valid data range is set, the status of group
05 is recorded.
12995
(6th) G code modal group to be recorded in the history when an alarm is issued
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to the maximum number of G code groups
Set the number of a G code modal group to be recorded in the alarm
history and operation history when an alarm is issued.
* If a value beyond the valid data range is set, the status of group
06 is recorded.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1790 -
12996
(7th) G code modal group to be recorded in the history when an alarm is issued
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to the maximum number of G code groups
Set the number of a G code modal group to be recorded in the alarm
history and operation history when an alarm is issued.
* If a value beyond the valid data range is set, the status of group
07 is recorded.
12997
(8th) G code modal group to be recorded in the history when an alarm is issued
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to the maximum number of G code groups
Set the number of a G code modal group to be recorded in the alarm
history and operation history when an alarm is issued.
* If a value beyond the valid data range is set, the status of group
08 is recorded.
12998
(9th) G code modal group to be recorded in the history when an alarm is issued
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to the maximum number of G code groups
Set the number of a G code modal group to be recorded in the alarm
history and operation history when an alarm is issued.
* If a value beyond the valid data range is set, the status of group
09 is recorded.
12999
(10tht) G code modal group to be recorded in the history when an alarm is issued
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to the maximum number of G code groups
Set the number of a G code modal group to be recorded in the alarm
history and operation history when an alarm is issued.
* If a value beyond the valid data range is set, the status of group
10 is recorded.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1791 -
Screen display
Procedure
1 Press function key .
2 Press continuous menu key several times until soft key
[OPERAT HISTRY] is displayed.
3 Press soft key [OPERAT HISTRY], then press newly displayed
soft key [OPERAT HISTRY]. The operation history screen is then
displayed.
4 To display the previous page and next page of the operation
history, use page keys and .
To display a part across two pages, use the cursor keys and
. The screen display is shifted by half page.
(With the 7.2- and 8.4-inch display devices, the screen display is
shifted by one column.)
By pressing soft key [(OPRT)] on the operation history screen, it
becomes possible to perform the following soft key operations:
a [TOP] displays the starting page (the oldest data).
b [BOTTOM] displays the end page (the latest data).
c [NO.SRH] displays specified operation history data.
(Example) Specifying 50 then [NO.SRH] displays the 50th
data.
Fig. 12.4.15.3 (a) Operation history screen
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1792 -
Displayed information
1 Serial number and display start history number/total number of
history data items
A serial number is indicated on the left side of each recorded
history data item. A smaller serial number indicates an older data
item.
In the upper right part of the screen, the display start history
number and the total number of history data items are indicated.
The total number of history data items does not include history
data items not displayed on the screen.
2 Data
• MDI key
When bit 5 (HKE) of parameter No. 3195 is set to 0, key
operations are recorded.
A key operation is indicated following a path number (for
example, "1_[LEFT F]", and "2_[LEFT F]"). (When only
one path is used, the path number is not indicated.)
P_ used in "P_[LEFT F]", for example, indicates a key
operation made from the outside.
i Address keys and numeric keys
Characters such as A to Z, 0 to 9, ;, +, and - are
indicated directly.
These characters are displayed in black.
ii Function menu keys, operation menu keys, and soft
keys
These keys are enclosed in brackets [] (for example,
"[LEFT F]", "[SOFT 1]" to "[SOFT 10]", and
"[RIGHT F]"). These keys are displayed with green
characters.
iii Function keys, page keys, cursor keys, and so on
These keys are enclosed in angle brackets <> (for
example, "<POS>", "<SYSTEM>", "<PAGE ↑>",
"<CUR →>", "<RESET>", and "<INPUT>"). These
keys are displayed with green characters.
iv Power-on key
This key is displayed with white characters in the
green background.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1793 -
• I/O signals
When bit 6 (HDE) of parameter No. 3195 is set to 0, I/O
signals specified on the operation history signal selection
screen are recorded. Recorded signals are indicated on a
bit-by-bit basis with information about the signal address
and a change in bit. These signals are displayed with purple
characters.
G000.2 ↓
Change from 0 to 1 is indicated by ↑.
Change from 1 to 0 is indicated by ↓.
Indicates a bit.
Indicates the address of a signal.
NOTE
1 When more than one bit at the same address
changes at the same time, the changes of these
bits are treated as one history data item.
2 A signal fluctuation for less than 4 msec is not
recorded as history data.
• Alarms
Alarm numbers and the issuance times are displayed on the
operation history screen.
This alarm information is displayed with white characters in
the red background.
When a path name, axis name, or spindle name was
changed after the issuance of an alarm, the alarm is
indicated with a newly assigned name.
• Time and date
The time and date of the following are displayed in two
lines:
i The time and date of power-on. These are displayed
with white characters in the green background.
ii The time and date of power-off. These are displayed
with green characters.
iii Date on which the date changed. This is displayed with
black characters.
iv Date and time at regular intervals of the period set in
parameter No. 3122. These are displayed with black
characters.
Indicates the path number.
Indicates the alarm number.
For the servo axis type, indicates the servo axis name.
For the spindle type, indicates the spindle name or
spindle number.
1_OT0506
(
X
A1)
2004/01/11
Indicates the date and time of issuance in two lines.
11:22:33
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1794 -
v Date and time when history data was erased. These are
displayed with black characters.
NOTE
1 When times are recorded at regular intervals, if
there is no data to record within an interval, the
time is not recorded. (When the date is changed,
the time is recorded on the assumption that there is
data to record.)
2 When the date and time in the CNC system are
changed, the date and time at which the change is
made may be recorded as the date and time in iii or
iv above.
History data not displayed on the screen
In addition to history data of MDI keys, I/O signal status, alarms
issued, external operator messages (not displayed on the operation
history screen), and time stamps, data described below can be
recorded with time. Such history data cannot be displayed on the
screen but can be output to external input/output devices. (See
Subsection 12.4.15.5, "Outputting all history data".)
1 Detailed data at alarm issuance
If bit 7 (HAL) of parameter No. 3196 is set to 0, 10 modal G
codes, auxiliary function codes D, E, F, H, M, N, O, S, and T,
absolute coordinates, and machine coordinates in the block being
executed when an alarm was issued are recorded together with
the alarm number and the time of alarm issuance.
The group numbers of the 10 modal G codes to be recorded are
set in parameter Nos. 12990 to 12999. If these parameters are not
specified, modal G codes of groups 01 to 10 are recorded.
NOTE
1 For modal O data that is a program name, only the
first five characters are recorded.
2 To record as many items as possible instead of
recording detailed data at alarm issuance, set bit 7
(HAL) of parameter No. 3196 to 1.
2 External alarm messages and macro alarm messages
If bit 3 (EAH) of parameter No. 3112 is set to 1, external alarm
messages and macro alarm messages can also be recorded as
history data. However, only the first 64 characters of each
message are recorded.
NOTE
To record also external alarm and macro alarm
messages as history data, set bit 3 (EAH) of
parameter No. 3112 to 1, and at the same time set
bit 7 (HAL) of parameter No. 3196 to 0.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1795 -
3 Modification of tool offset data
If bit 0 (HTO) of parameter No. 3196 is set to 1, when tool offset
data is modified, the number and type of the tool offset are
recorded as well as the tool offset data before modification, the
tool offset data after modification, and the time of modification.
4 Modification of workpiece offset/extended workpiece
offset/workpiece shift (T series) data
If bit 1 (HWO) of parameter No. 3196 is set to 1, when
workpiece offset data is modified, the number of the modified
workpiece offset is recorded as well as the workpiece offset data
before modification, the workpiece offset data after modification,
and the time of modification. Similar data is recorded also when
extended workpiece offsets and workpiece shift amounts (T
series) are modified.
5 Modification of parameters
If bit 2 (HPM) of parameter No. 3196 is set to 1, when a
parameter is modified, the number and type (axis type, spindle
type, path type, or machine group type) of the parameter are
recorded as well as the parameter data before modification, the
parameter data after modification, and the time of modification.
NOTE
Modifications made at power-on and modifications of
passwords and keys are not recorded as history
data.
6 Modification of custom macro common variables (#100 to #999)
If bit 3 (HMV) of parameter No. 3196 is set to 1, when a custom
macro common variable is modified, the number of the common
variable is recorded as well as the common variable value before
modification, the common variable value after modification, and
the time of modification.
Erasing history data from the operation history screen
Procedure
1 Display the operation history screen.
2 Press soft key [(OPRT)].
3 Press soft key [ALL CLEAR].
4 Press soft key [EXEC]. All history data is erased.
NOTE
An erasure operation erases not only operation
history data but also other history data such as
external operator message history data and alarm
history data. It is impossible to erase only a specific
history.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1796 -
12.4.15.4 Selecting operation history signals
I/O signals to be recorded as history data can be selected. Up to 60
signals can be set.
Setting data
1 Press function key .
2 Press continuous menu key several times until soft key
[OPERAT HISTRY] is displayed.
3 Press soft key [OPERAT HISTRY].
4 Press soft key [SIGNAL SELECT] to display the operation
history signal selection screen.
5 Press soft key [(OPRT)].
6 Move the cursor to a desired position by using cursor keys
and .
7 Type a signal type (X, G, F, or Y) and an address, then press
.
Example:
When G0004 is entered then is pressed:
The entered signal address, G0004, is set in ADDRESS, and
initial value 00000000 is set in SIGNAL.
8 Select the bits to be recorded in the history.
To change the status of all bits of the specified signal address,
place the cursor in all bits so that the bits are highlighted (for
example, "00000000"), then press soft key [ON:1] or [OFF:0].
Then, the bits are set to 11111111 or 00000000.
To change the status of only a certain bit, move the cursor to the
bit by using cursor keys and , and press [ON:1] or
[OFF:0]. The selected bit is then set to 1 or 0.
9 Up to 60 addresses can be set to select signals. Addresses need
not necessarily be set sequentially starting from No. 1.
NOTE
1 While the operation history signal selection screen is
being displayed, recording of history data is not
performed.
2 Only X, Y, G, and F can be set for I/O signals.
For data not set, "********" is displayed.
3 Even when an address is set, history data is not
recorded if all bits are set to 0.
4 When the ON/OFF width of an input signal is less than 4
msec, recording of history data is not performed.
Also,there are some signals that are not recorded.
5 When many signals are selected, the processing speed
may lower.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1797 -
Clearing data individually
1 Display the operation history signal selection screen.
2 Move the cursor to the data to be cleared.
3 Press soft key [DELETE].
4 Press soft key [EXEC].
Clearing all data
1 Display the operation history signal selection screen.
2 Press soft key [ALLDEL].
3 Press soft key [EXEC].
Fig. 12.4.15.4 (a) Operation history signal selection screen
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1798 -
12.4.15.5 Outputting all history data
All history data can be output to external input/output devices.
It is impossible, however, to output history data individually.
Procedure
1 Make an output device ready for output.
2 Set the EDIT mode.
3 Press function key .
4 Press continuous menu key several times until soft key
[OPERAT HISTRY] is displayed.
5 Press soft key [OPERAT HISTRY], then press newly displayed
soft key [OPERAT HISTRY]. The operation history screen is
displayed.
6 Press soft key [(OPRT)].
7 Press soft key [PUNCH].
8 Enter a file name, and press soft key [EXEC].
When soft key [EXEC] is pressed without entering a file name,
the output file name is assumed to be OPRT_HIS.TXT.
Output format
History data is output as an ASCII file in the following format:
1 MDI keys
After "MDI", "path-number_", "key-data", and "input-time" are
output in this order.
(Key data input at power-on is indicated as "Power on MDI".)
<Example>
MDI 01_A 12:23:34
MDI 02_<CAN> 12:23:34
MDI 02_[SOFT HF1] 12:23:35
MDI P_<RESET> 12:34:56
Power on MDI 01_<RESET> 12:34:56
2 I/O signals
After "DI/DO", "PMC-number_", "signal-address_bit-status",
and "time-of-change" are output in this order.
<Example>
DI/DO 1_F0002.2_on 12:34:56
DI/DO 1_ G0043.0_off G0043.1_off 12:35:00
(For multiple bits at the same address)
3 Alarms
After "Alarm", "path-number_", "type", "alarm-number",
"G-code-modal-data", "modal-data-other-than-G-code",
"absolute-coordinate-value" and "machine-coordinate-value" for
each axis, and "date-and-time-of-alarm-issuance" are output in
this order.
An asterisk "*" is output before the modal data that was specified
in a block executed when the alarm was issued.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1799 -
<Example>
• Alarm 01_SR01973
*G0. G97. G69. G99. G21. G50.2 G25. G13.1 B0. D0. E0.
*F100. H0. M10. *N123. Test_ S1000. T1010.
X1 ABS 197.999 MCN 197.999 Y1 ABS -199806.00 MCN
-199806.00 Z1 ABS 297.009 MCN 0.123 C1 ABS
10395.999 MCN 0.000 at 2007/09/01 19:03:28
• Alarm 02_ OT00506(ZA2)
*G1. G17. G90. G22. G94. G20. *G42. G49. G80. G12.1
B0. *D12. E0. *F100. H34. M0. *N123. O123 S0. T0.
X2 ABS 123.999 MCN 234.000 Y2 ABS -123.00 MCN
-234.00 ZA2 ABS 1234.567 MCN –1234.567 at 2007/09/01
12:34:56
• When additional information is not to be recorded when an
alarm is issued (bit 7 (HAL) of parameter No. 3196 is set to
1), only "path-number_", "alarm-number", and
"date-and-time-of-alarm-issuance" are output.
Alarm 01_OT00506(XC1) at 2007/09/01 22:08:32
Alarm 02_SW00100 at 2007/09/01 19:07:52
• When external alarm/macro alarm messages are to be
recorded (bit 7 (HAL) of parameter No. 3196 is set to 0)
and bit 3 (EAH) of parameter No. 3112 is set to 1, the
messages are also output.
Alarm 01_MC00001 Message ATC ALARM
G0. G97. G69. G99. G21. G40. G25. G22. G80. D0. E0.
F0. H0. M0. N0. O9999 S0. T0.
X2 ABS 10.000 MCN 0.000Y2 ABS 123.000 MCN
0.000Z2 ABS 0.000 MCN 0.000 at 2007/09/01 10:06:43
4 External operator messages
After "EXT_Message", "message-number", "message", and
"date-and-time-of-issuance" are output in this order.
<Example>
EXT_Message 01234 OIL PRESSURE DECREASE at
2007/09/01 2:38:43
5 Modification of tool offset data
After "Tool Offset", "path-number_", "type", "offset-number",
"offset-data-before-modification",
"offset-data-after-modification", and "time-of-modification" are
output in this order. The following types are provided:
Common
to M/T
: G=Geometric
compensation
W=Wear
compensation
M series : H=Tool
length
compensation
D=Cutter
compensation
T series : R=Tool-nose
radius
compensation
T=Tool nose
direction
X2,Z2,Y2=Second geometric compensation
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1800 -
<Example>
Tool Offset 01_X0002 0.000 → 1 at 12:15:43
Tool Offset 02_XW0001 -9999.999 → 9999.999 at
12:15:46
Tool Offset 01_RG0032 0.000 → 0.003 at 12:15:52
Tool Offset 02_T0001 5. → 2. at 19:34:11
Tool Offset 02_W0123 -10.000 → 123.456 at 10:28:58
Tool Offset 01_HG0456 0.000 → 999.999 at 11:37:40
Tool Offset 01_ 0064 12.340 → 12.569 at 11:39:42
6 Modification of workpiece offset/extended workpiece
offset/workpiece shift (T series) data
After "Work Offset", "EXT Work Offset", or "Work Shift",
"path-number_(axis-name)", "type", "offset-number",
"offset-data-before-modification",
"offset-data-after-modification", and "time-of-modification" are
output in this order.
<Example>
Work Offset 01_G55(XA1) 15.000 → 0.007 at 09:23:03
Work Offset 02_EXT(Z2) 0.000 → 300.003 at 09:22:50
EXT Work Offset 02_G54.1P300 (Y2) 123.456 →
9999.999 at 12:15:46
Work Shift (X) 02_999999.999 → 999999.999 at 10:22:37
7 Modification of parameters
After "Parameter", "type", "parameter-number",
"parameter-before-modification", "parameter-after-modification",
and "time-of-modification" are output in this order.
The following types are provided:
Path type : L is added before the path number.
Axis type : A is added before the axis number.
Spindle type : S is added before the spindle number.
Machine group type : Indicated as the machine type. T is added
before the machine group number.
Others : No type is output.
<Example>
Paramater N03112 00000100 → 00001100 at
11:18:40
Paramater Path type N01410 L02 0.000 → 1000.000
at 18:58:48
Paramater Axis type N01423 A04(B2) 0.000 →
10000.000 at 18:58:48
Paramater Spindle type N04011 S1(S) 10011010 →
10011010 at 18:58:53
Paramater Machine type N06310 T01 0 → -32768 at
19:21:13
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1801 -
8 Modification of custom macro common variables (#100 to #999)
After "Macro variable", "path-number_", "#variable-number",
"common-variable-value-before-modification",
"common-variable-value-after-modification", and
"time-of-modification" are output in this order.
Variable values are output in the data format M × (10**(-E)).
<Example>
• When #149 on the first path was modified from <empty> to
12.345
Macro valiable 01_#149 Empty → 123450000*(10**-7) at
15:02:35
• When #549 on the second path was modified from -12.345
to 123456789012
Macro valiable 02_#549 -123450000*(10**-7)
→123456789*(10**3) at 15:03:27
9 Date and time
Power on at 2007/09/01 17:11:17 (Date and time of
power-on)
Power off at 2007/09/01 17:49:17 (Date and time of
power-off)
Date 2007/09/01 00:00:00 (Record indicating a
change in date)
Time stamp at 2007/09/01 15:51:00 (Record at regular
intervals)
Data delete at 2007/09/01 10:56:18 (Date and time when
history data was deleted)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1802 -
Screens of a 15-inch display unit
12.4.16 Displaying and Setting Parameters (15-inch Display Unit)
When the CNC and machine are connected, parameters are set to
determine the specifications and functions of the machine in order to
fully utilize the characteristics of the servo motor. The setting of
parameters depends on the machine. Refer to the parameter list
prepared by the machine tool builder.
Normally, the user need not change parameter setting.
Procedure for displaying and setting parameters
Procedure
1 Set 1 for PARAMETER WRITE to enable writing. See the
procedure for enabling/disabling parameter writing described
below.
2 Press function key .
3 Press vertical soft key [PARAM] to display the parameter screen.
Fig. 12.4.16 (a) PARAMETER screen (15-inch)
4 Move the cursor to the parameter number to be set or displayed
in either of the following ways:
• Enter the parameter number and press horizontal soft key
[NO.SRH] .
• Move the cursor to the parameter number using the page
keys, and , and cursor keys, , ,
, and .
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1803 -
5 To set the parameter, enter a new value with numeric keys and
press horizontal soft key [INPUT]. The parameter is set to the
entered value and the value is displayed.
6 Set 0 for PARAMETER WRITE to disable writing.
Procedure for enabling/displaying parameter writing
Procedure
1 Select the MDI mode or enter state emergency stop.
2 Press function key .
3 Press vertical soft key [SETTING] to display the setting screen.
Fig. 12.4.16 (b) SETTING screen (15-inch)
4 Move the cursor to PARAMETER WRITE using cursor keys.
5 Press horizontal soft key [ON:1] to enable parameter writing.
At this time, the CNC enters the alarm state SW0100.
6 After completing parameter setting, move the cursor to
PARAMETER WRITE on the setting screen again, and press
horizontal soft key [OFF:0].
7 Depress the key to release the alarm condition.
When an alarm PW0000 occurred, however, it is not released
unless the power is turned off and back on.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1804 -
Explanation
- Setting parameters with external input/output devices
See III-8 for setting parameters with external input/output devices
such as the memory card.
- Parameters that require turning off the power
Some parameters are not effective until the power is turned off and on
again after they are set. Setting such parameters causes alarm PW0000.
In this case, turn off the power, then turn it on again.
- Parameter list
Refer to the Parameter Manual (B-63950EN) for the parameter list.
- Setting data
Some parameters can be set on the setting screen if the parameter list
indicates "Setting entry is acceptable". Setting 1 for PARAMETER
WRITE is not necessary when three parameters are set on the setting
screen.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1805 -
12.4.17 Displaying and Setting Pitch Error Compensation Data
(15-inch Display Unit)
If pitch error compensation data is specified, pitch errors of each axis
can be compensated in detection unit per axis.
Pitch error compensation data is set for each compensation point at the
intervals specified for each axis. The origin of compensation is the
reference position to which the tool is returned.
The pitch error compensation data is set according to the
characteristics of the machine connected to the NC. The content of
this data varies according to the machine model. If it is changed, the
machine accuracy is reduced.
In principle, the end user must not alter this data.
Pitch error compensation data can be set with external devices such as
the memory card (see Chapter III-8). Compensation data can also be
written directly with the MDI panel.
The following parameters must be set for pitch error compensation.
Set the pitch error compensation value for each pitch error
compensation point number set by these parameters.
In the following example, 33 is set for the pitch error compensation
point at the reference position.
1
2
3
3332
31 34 35 36 37
Compensation number
parameter for the reference
position (No. 3620)
Compensation number
parameter for the
compensation point having
the largest value (No.
3622)
-1
-2
Compensation number parameter fo
r
the compensation point having the
smallest value (No. 3621)
Compensation
position number
Compensation
value to be set
3
3
3
3
31
3
3
-3 +1 +1 +1 +2 -1 -3
Reference position
Compensation
interval paramete
r
(
No. 3624
)
Compensation magnification
parameter (No. 3623)
Pitch error compensation value (absolute value)
• Number of the pitch error compensation point at the reference
position (for each axis): Parameter No. 3620
• Number of the pitch error compensation point having the
smallest value (for each axis): Parameter No. 3621
• Number of the pitch error compensation point having the largest
value (for each axis): Parameter No. 3622
• Pitch error compensation magnification (for each axis):
Parameter No. 3623
• Interval of the pitch error compensation points (for each axis):
Parameter No. 3624
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1806 -
• Travel distance per revolution of pitch error compensation of the
rotary axis type (for each axis): Parameter No. 3625
- Bi-directional pitch error compensation
The bi-directional pitch error compensation function allows
independent pitch error compensation in different travel directions.
(When the movement is reversed, compensation is automatically
carried out as in a backlash.)
To use this function, specify pitch error compensation for each travel
direction, that is, separately for the positive and negative directions of
a movement.
When using bi-directional pitch error compensation (setting bit 0
(BDPx) of parameter No. 3605 to 1), specify the following parameters
in addition to the pitch error compensation parameter.
• Number of the pitch error compensation point at the negative end
(for travel in the positive direction, for each axis): Parameter No.
3621
• Number of the pitch error compensation point at the positive end
(for travel in the positive direction, for each axis): Parameter No.
3622
• Number of the pitch error compensation point at the negative end
(for travel in the negative direction, for each axis): Parameter No.
3626
• Pitch error compensation in the reference position when moving
to the reference position from opposite to the reference position
return direction (for each axis): Parameter No. 3627
Procedure for displaying and setting the pitch error compensation data
Procedure
1 Set the following parameters:
• Number of the pitch error compensation point at the
reference position (for each axis): Parameter No. 3620
• Number of the pitch error compensation point having the
smallest value (for each axis): Parameter No. 3621
• Number of the pitch error compensation point having the
largest value (for each axis): Parameter No. 3622
• Pitch error compensation magnification (for each axis):
Parameter No. 3623
• Interval of the pitch error compensation points (for each
axis): Parameter No. 3624
• Travel distance per revolution of pitch error compensation
of the rotary axis type (for each axis): Parameter No. 3625
When using bi-directional pitch error compensation (setting bit 0
(BDPx) of parameter No. 3605 to 1), specify the following
parameters in addition to the pitch error compensation parameter.
• Number of the pitch error compensation point at the
negative end (for travel in the positive direction, for each
axis): Parameter No. 3621
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1807 -
• Number of the pitch error compensation point at the
positive end (for travel in the positive direction, for each
axis): Parameter No. 3622
• Number of the pitch error compensation point at the
negative end (for travel in the negative direction, for each
axis): Parameter No. 3626
• Pitch error compensation in the reference position when
moving to the reference position from opposite to the
reference position return direction (for each axis): Parameter
No. 3627
2 Press function key .
3 Press vertical soft key [PITCH ERROR]. The following screen is
displayed:
Fig. 12.4.17 (a) PITCH ERROR COMPENSATION screen (15-inch)
4 Move the cursor to the compensation point number to be set in
either of the following ways:
• Enter the compensation point number and press the
horizontal soft key [NO.SRH].
• Move the cursor to the compensation point number using
the page keys, and , and cursor keys, ,
, , and .
5 Enter a value with numeric keys and press horizontal soft key
[INPUT].
‚
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1808 -
12.4.18 Displaying and Setting Three-Dimensional Error
Compensation Data (15-inch Display Unit)
In ordinary pitch error compensation, compensation is applied to a
specified compensation axis (single axis) by using its position
information. For example, pitch error compensation is applied to
X-axis by using the position information of X-axis.
Three-dimensional error compensation is a function that adjusts the
current position by calculating compensation data (for three axes)
from the compensation amounts at surrounding compensation points
(eight points) on the basis of the interior division ratio in the
compensation area (rectangular parallelepiped) containing the current
position on up to three compensation axes.
- Calculation of compensation
Three-dimensional error compensation is calculated as follows.
Let three compensation axes be X, Y, and Z (three basic axes) and the
coordinates of the current position be P (Px, Py, Pz). consider a
compensation space (rectangular parallelepiped) containing P. Let its
vertexes be P1, P2, …, and P8 and the compensation values for the
individual axes at the individual vertexes be Cnx, Cny, and Cnz
(where n is a number between 1 and 8).
Let the interior division ratio on X-axis at P be x. Here, x is
standardized in the range of 0 to 1 as follows:
P1x and P2x are the X coordinates of P1 and P2. The interior division
ratios on Y and Z-axes are determined in the same way.
|12|
|1|
xPxP
xPPx
x−
−
=
P4 [C4x, C4y, C4z]
P (Px, Py, Pz)
P5 [C5x, C5y, C5z]P6 [C6x, C6y, C6z]
P1 [C1x, C1y, C1z]P2 [C2x, C2y, C2z]
P3 [C3x, C3y, C3z]
P8 [C8x, C8y, C8z]P7 [C7x, C7y, C7z]
x
y
z
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1809 -
The compensation amount Cx for X-axis at P is determined as
follows:
The compensation amount Cy and Cz on Y and Z-axes are determined
in the same way.
The actual compensation amounts are the calculated compensation
amounts multiplied by the compensation magnifications (Parameter
No.10809 to 10811).
- Number of compensation points
Up to 15625 compensation points (up to 25 points per axis) can be set.
The numbers of compensation points on the individual axes are set for
parameters No.10803 to 10805. The ordering of the compensation
point numbers in the compensation space is as follows.
Max1×Max2×Max3
Max1×Max2×(Max3-1）+1
…
…
Max1×Max2×3
Max1×Max2×2
Max1×Max2
…
…
Max1×Max2+1 Max1×3
Max1×2
1 2 3 ………………… Max1
Max1×Max2+Max1
zyxxCzyxxC
zyxxCzyxxC
zyxxCzyxxC
zyxxCzyxxCCx
××−×+×××+
×−××+×−×−×+
−××−×+−×××+
−
×−××
+
−
×
−
×
−
×
=
)1(87
)1(6)1()1(5
)1()1(4)1(3
)1()1(2)1()1()1(1
Max1 : Number of compensation points on the first axis (up to 25)
Max2 : Second axis (up to 25)
Max3 : Third axis (up to 25)
(
Third com
p
ensation axis
)
(
Second com
p
ensation axis
)
(
First com
p
ensation axis
)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1810 -
Displaying and setting three-dimensional error compensation data
Procedure
1 Set the following parameters:
• First compensation axis for three-dimensional error
compensation : Parameter No. 10800
• Second compensation axis for three-dimensional error
compensation : Parameter No. 10801
• Third compensation axis for three-dimensional error
compensation : Parameter No. 10802
• Number of compensation points for three-dimensional error
compensation (first compensation axis)
Parameter No. 10803
• Number of compensation points for three-dimensional error
compensation (second compensation axis)
Parameter No. 10804
• Number of compensation points for three-dimensional error
compensation (third compensation axis)
Parameter No. 10805
• Compensation point number of the reference position for
three-dimensional error compensation (first compensation
axis) : Parameter No. 10806
• Compensation point number of the reference position for
three-dimensional error compensation (second
compensation axis) : Parameter No. 10807
• Compensation point number of the reference position for
three-dimensional error compensation (third compensation
axis) : Parameter No. 10808
• Magnification for three-dimensional error compensation
(first compensation axis) : Parameter No. 10809
• Magnification for three-dimensional error compensation
(second compensation axis) : Parameter No. 10810
• Magnification for three-dimensional error compensation
(third compensation axis) : Parameter No. 10811
• Compensation interval for three-dimensional error
compensation (first compensation axis)
Parameter No. 10812
• Compensation interval for three-dimensional error
compensation (second compensation axis)
Parameter No. 10813
• Compensation interval for three-dimensional error
compensation (third compensation axis)
Parameter No. 10814
2 Press function key .
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1811 -
3 Press vertical soft key [NEXT PAGE] several times, then press
vertical soft key [3D ERR COMP]. The following screen
appears:
Fig. 12.4.18 (a) 3-DIMENSIONAL ERROR COMPENSATION screen
(15-inch)
4 Move the cursor to the position of the compensation point
number you want to set using either of the following methods:
• Select the MDI mode.
• Set bit 0 (PWE) of parameter No. 8900 to 1.
• Enter a compensation point number and press horizontal
soft key [NO. SRH].
• Move the cursor to the compensation point number or
compensation axis you want to set by pressing page keys
and/or , and cursor keys , , ,
and .
5 Enter compensation data in detection units. The valid data
range is from -128 to 127.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1812 -
12.4.19 Servo Parameters (15-inch Display Unit)
This subsection describes the initialization of digital servo parameters
performed, for example, at the time of field tuning of the machine
tool.
Procedure for servo parameter setting
Procedure
1 Turn on the power in the emergency stop state.
2 Set bit 0 (SVS) of parameter No. 3111 to 1 to display servo
setting and tuning screens.
3 Press function key then vertical soft key [SERVO
PARAM]. The following screen appears:
Fig. 12.4.19 (a) Servo parameter setting screen (15-inch)
4 With the page keys and cursor keys, move the cursor to the
position of data to be set or modified.
5 Key in a desired value then press horizontal soft key [INPUT].
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1813 -
12.4.20 Servo Tuning (15-inch Display Unit)
Data related to servo tuning is displayed and set.
Procedure for servo tuning
Procedure
1 Turn on the power in the emergency stop state.
2 Set bit 0 (SVS) of parameter No. 3111 to 1 to display servo
setting and tuning screens.
3 Press function key then vertical soft key [SERVO
PARAM].
4 Press vertical soft key [SERVO TUNE] to select the servo tuning
screen. The following screen appears:
Fig. 12.4.20 (a) Servo tuning screen (15-inch)
5 With the page keys and cursor keys, move the cursor to the
position of data to be set or modified.
6 Key in a desired value then press horizontal soft key [INPUT].
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1814 -
12.4.21 Spindle Setting (15-inch Display Unit)
Parameters related to spindles are set and displayed. In addition to
the parameters, related data can be displayed. Screens for spindle
setting, spindle tuning, and spindle monitoring are provided.
Setting spindle parameters
Procedure
1 Set bit 1 (SPS) of parameter No. 3111 to 1 to display spindle
setting and tuning screens.
2 Press function key then vertical soft key [SPINDL
SETING].
3 Press vertical soft key [SPINDL SETING] to select the spindle
setting screen.
The following screen appears:
Fig. 12.4.21 (a) Spindle setting screen (15-inch)
4 With the page keys and cursor keys, move the cursor to the
position of data to be set or modified.
5 Key in a desired value then press horizontal soft key [INPUT].
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1815 -
12.4.22 Spindle Tuning (15-inch Display Unit)
Spindle tuning data is displayed and set.
Setting for spindle tuning
Procedure
1 Set bit 1 (SPS) of parameter No. 3111 to 1 to display spindle
setting and tuning screens.
2 Press function key then vertical soft key [SPINDL
SETING].
3 Press vertical soft key [SPINDL TUNE] to select the spindle
tuning screen.
The following screen appears:
Fig. 12.4.22 (a) Spindle tuning screen (15-inch)
4 With the page keys and cursor keys, move the cursor to the
position of data to be set or modified.
5 Key in a desired value then press horizontal soft key [INPUT].
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1816 -
12.4.23 Spindle Monitor (15-inch Display Unit)
Spindle-related data is displayed.
Displaying the spindle monitor
Procedure
1 Set bit 1 (SPS) of parameter No. 3111 to 1 to display spindle
setting and tuning screens.
2 Press function key then vertical soft key [SPINDL
SETING].
3 Press vertical soft key [SPINDL MONIT.] to select the spindle
monitor screen.
The following screen appears:
Fig. 12.4.23 (a) Spindle monitor screen (15-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1817 -
12.4.24 Color Setting Screen (15-inch Display Unit)
Screen colors can be set on the color setting screen.
Displaying the color setting screen
Procedure
1 Press function key .
2 Press vertical soft key [NEXT PAGE] several times to display
vertical soft key [COLOR].
3 Press vertical soft key [COLOR] to display the color setting
screen.
Fig. 12.4.24 (a) Color setting screen (15-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1818 -
Procedure for operating the color setting screen
- Modifying the color (color palette values)
1 The following horizontal soft keys are displayed:
2 Move the cursor to a color number whose color palette values are
to be modified.
The current color palette value set for each primary color is
displayed.
3 Select a primary color whose setting is to be modified, with the
corresponding horizontal soft key [RED], [GREEN], or [BLUE].
More than one primary color can be selected at the same time.
Each time horizontal soft key [RED], [GREEN], or [BLUE] is
pressed, the operation soft key toggles between selection and
deselection.
4 Select horizontal soft key [BRIGHT] or [DARK] to modify the
brightness of the selected prime color(s).
- Storing the color (color palette values)
The set color palette values can be stored.
1 Press horizontal soft key [COLOR1], [COLOR2], or [COLOR3]
to select a storage area.
COLOR1 Standard color data parameters (Nos. 6581 to
6595)
COLOR2 Parameters (Nos. 10421 to 10435)
COLOR3 Parameters (Nos. 10461 to 10475)
2 Press horizontal soft key [MEMORY]. The horizontal soft key
display switches to the following:
3 Pressing horizontal soft key [EXEC] stores the current color
palette settings in the selected area.
Pressing horizontal soft key [CAN] or the leftmost key does not
store the current color palette settings in the selected area.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1819 -
- Calling the color (color palette values)
1 Press horizontal soft key [COLOR1], [COLOR2], or [COLOR3]
to select a storage area where color palette values are stored.
2 Press horizontal soft key [RECALL]. The horizontal soft key
display switches to the following:
3 Pressing horizontal soft key [EXEC] calls the color palette values
from the selected area to enable the color to be modified. This
operation is invalid if no color palette values are stored.
Pressing horizontal soft key [CAN] or the leftmost key does not
call the color palette values from the selected area.
NOTE
1 Immediately after the power is turned on, the
settings of COLOR1 (parameters) are used for
display. If nothing is stored for COLOR1, the
default colors are used for display.
2 Do not modify the color setting data parameters
directly by MDI key input. When modifying the
standard color data, be sure to perform a storage
operation on the color setting screen.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1820 -
12.4.25 Machining Parameter Tuning (15-inch Display Unit)
In AI contour control, by setting a velocity-emphasized parameter set
and precision-emphasized parameter set and setting the precision level
matching a machining condition such as rough machining or finish
machining on the precision level setting screen or by programming,
the parameters suitable for the condition can be automatically
calculated to perform machining.
On this screen, the parameter sets for emphasis on velocity (precision
level 1) and emphasis on precision (precision level 10) can be set.
Set the following parameters:
• Acceleration rate of acceleration/deceleration before
interpolation
• Acceleration change time (bell-shaped)
• Allowable acceleration change value for each axis in velocity
control based on acceleration change under jerk control
• Allowable acceleration change value for each axis in acceleration
change under jerk control in successive linear interpolation
operations
• Ratio of the change time of the rate of change of acceleration in
smooth bell-shaped acceleration/deceleration before interpolation
• Allowable acceleration rate
• Acceleration rate of acceleration/deceleration after interpolation
• Corner speed difference
• Maximum feedrate
• Items that can be set freely (2 items)
For details of each parameter, see the descriptions of AI contour
control and jerk control.
By setting bit 0 (MPR) of parameter No. 13601 to 1, this screen can be
hidden.
For the method of setting a precision level, see the description of the
precision level selection screen in Subsection 12.3.27.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1821 -
Procedure for machining parameter tuning
Procedure
1 Set the MDI mode.
2 Press function key .
3 Press vertical soft key [NEXT PAGE] several times to display
vertical soft key [MCHN TUNING]. The following screen
appears:
Fig. 12.4.25 (a) Machining parameter tuning screen (15-inch)
4 Move the cursor to the position of a parameter to be set, as
follows:
Press page key or , and cursor keys , ,
and /or to move the cursor to the parameter.
5 Key in desired data then press the key on the MDI panel.
6 When data is input, a RMS value is found according to the
precision level parameters. (The precision level can be changed
on the precision level selection screen or parameter setting
screen.) If a RMS value calculation fails, a warning (indicating
that automatic setting failed) is displayed.
7 Repeat steps 4 and 5 until all machining parameters are set.
8 In addition to the setting method described above, a parameter
setting method using horizontal soft keys is available. Pressing
horizontal soft key [INIT] displays the standard value
(recommended by FANUC) of the item selected by the cursor in
the key input buffer. Pressing horizontal soft key [EXEC]
initializes the item to the standard value. Pressing horizontal soft
key [GROUP INIT] initializes all items of a group (emphasis on
velocity or emphasis on precision) selected by the cursor to the
standard values.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1822 -
The table below indicates the initial settings.
Table 12.4.25 (a) Initial settings
AI contour control
Setting item Emphasis
on velocity
(LV1)
Emphasis
on precision
(LV10)
Unit
Acceleration rate of acceleration/deceleration before interpolation
<ACC FOR BIPL> 4902.000 1042.000 mm/sec2
Acceleration change time (bell-shaped) <ACC CHG TIME(BELL)> 32 64 msec
Allowable acceleration change value <JERK ACC DIFF> 0 0 mm/sec2
Allowable acceleration change value in successive linear
interpolation operations <JERK ACC DIFF(LIN)> 0 0 mm/sec2
Ratio of the change time of the jerk control <JERK ACC RATIO> 0 0 %
Allowable acceleration rate <MAX AACELERATION> 2977.000 596.000 mm/sec2
Time constant for acceleration/deceleration after interpolation
<T-CON AIPL ACC/DEC> 24 24 msec
Corner speed difference <CORNER FEED DIFFER> 1000 400 mm/min
Maximum cutting speed <MAX CUT FEEDRATE> 10000 10000 mm/min
Explanation
- Look-ahead acceleration/deceleration before interpolation
Set an acceleration rate for a linear portion in look-ahead
acceleration/deceleration before interpolation.
Unit of data: mm/sec2, inch/sec2, deg/sec2 (machine unit)
The parameter set on the machining parameter tuning screen is
reflected in the following parameters:
Parameter No. 13610 (velocity-emphasized parameter)
Parameter No. 13611 (precision-emphasized parameter)
Moreover, the following parameter is also set according to the
precision level:
Parameter No. 1660: Maximum allowable acceleration rate for each
axis in acceleration/deceleration before
interpolation
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1823 -
- Acceleration change time (bell-shaped)
Set a time constant for a bell-shaped portion in acceleration/
deceleration before look-ahead interpolation.
Unit of data: ms
The parameter set on the machining parameter tuning screen is
reflected in the following parameters:
Parameter No. 13612 (velocity-emphasized parameter)
Parameter No. 13613 (precision-emphasized parameter)
When bit 7 of parameter No. 13600 is set to 1, the parameter set on the
machining parameter tuning screen is reflected in the following
parameters for which the valid data range is extended to the range
from 0 to 200:
Parameter No. 13662 (velocity-emphasized parameter)
Parameter No. 13663 (precision-emphasized parameter)
Moreover, the following parameter is also set according to the
precision level:
Parameter No. 1772: Time constant for bell-shaped look-ahead
acceleration/deceleration before interpolation of
constant acceleration time type
CAUTION
A set time constant is applied to all axes. So, a
modification made to this item changes the settings
for all axes.
- Allowable acceleration change value in velocity control based on acceleration
change under jerk control
Unit of data: mm/sec2, inch/sec2, deg/sec2 (machine unit)
Set an allowable acceleration change value per ms for each axis in
velocity control based on acceleration change under jerk control.
The parameter set on the machining parameter tuning screen is
reflected in the following parameters:
Parameter No. 13614 (velocity-emphasized parameter)
Parameter No. 13615 (precision-emphasized parameter)
Moreover, the following parameter is also set according to the
precision level:
Parameter No. 1788: Allowable acceleration change value for each
axis in velocity control based on acceleration
change under jerk control
NOTE
This setting item is displayed only when the jerk
control function is enabled.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1824 -
- Allowable acceleration change value for each axis in velocity control based on
acceleration change under jerk control in successive linear interpolation
operations
Unit of data: mm/sec2, inch/sec2, deg/sec2 (machine unit)
Set an allowable acceleration change value per ms for each axis in
velocity control based on acceleration change under jerk control in
successive linear interpolation operations.
The parameter set on the machining parameter tuning screen is
reflected in the following parameters:
Parameter No. 13616 (velocity-emphasized parameter)
Parameter No. 13617 (precision-emphasized parameter)
Moreover, the following parameter is also set according to the
precision level:
Parameter No. 1789: Allowable acceleration change value for each
axis in velocity control based on acceleration
change under jerk control in successive linear
interpolation operations
CAUTION
1 For an axis with 0 set in this parameter, the
parameters (allowable acceleration change value
in velocity control based on acceleration change
under jerk control: No. 13614, No.13615) are valid.
2 For an axis with 0 set in the parameter (allowable
acceleration change value in velocity control based
on acceleration change under jerk control: No.
13614, No.13615), velocity control based on
acceleration change is disabled, so that this
parameter has no effect.
NOTE
This setting item is displayed only when the jerk
control function is enabled.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1825 -
- Ratio of the change time of the jerk control in smooth bell-shaped
acceleration/deceleration before interpolation
Unit of data: %
Set the ratio (in %) of the change time of jerk control to the change
time of acceleration in smooth bell-shaped acceleration/deceleration
before interpolation.
The parameter set on the machining parameter tuning screen is
reflected in the following parameters:
Parameter No. 13618 (velocity-emphasized parameter)
Parameter No. 13619 (precision-emphasized parameter)
Moreover, the following parameter is also set according to the
precision level:
Parameter No. 1790: Ratio of the change time of the jerk control in
smooth bell-shaped acceleration/deceleration
before interpolation
NOTE
This setting item is displayed only when the jerk
control function is enabled.
- Allowable acceleration rate
Set an allowable acceleration rate in acceleration-based speed
determination.
Unit of data: mm/sec2, inch/sec2, deg/sec2 (machine unit)
The parameter set on the machining parameter tuning screen is
reflected in the following parameters:
Parameter No. 13620 (velocity-emphasized parameter)
Parameter No. 13621 (precision-emphasized parameter)
Moreover, the following parameter is also set according to the
precision level:
Parameter No. 1735: Allowable acceleration rate for each axis
applicable to the deceleration function based
on acceleration in circular interpolation
Parameter No. 1737: Allowable acceleration rate for each axis
applicable to the deceleration function based
on acceleration in AI contour control
CAUTION
When bit 0 (MCR) of parameter No. 13600 is set to
1, the deceleration function based on acceleration
in circular interpolation is not set.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1826 -
- Time constant for acceleration/deceleration after interpolation
Set a time constant for acceleration/deceleration after interpolation.
Unit of data: ms
The parameter set on the machining parameter tuning screen is
reflected in the following parameters:
Parameter No. 13622 (velocity-emphasized parameter)
Parameter No. 13623 (precision-emphasized parameter)
Moreover, the following parameter is also set according to the
precision level:
Parameter No. 1769: Time constant for acceleration/deceleration
after cutting feed interpolation
- Corner speed difference
Set an allowable corner speed difference used for speed determination.
Unit of data: mm/sec, inch/sec, deg/sec (machine unit)
The parameter set on the machining parameter tuning screen is
reflected in the following parameters:
Parameter No. 13624 (velocity-emphasized parameter)
Parameter No. 13625 (precision-emphasized parameter)
Moreover, the following parameter is also set according to the
precision level:
Parameter No. 1783: Allowable speed difference for each axis in
automatic corner deceleration based on speed
difference
- Maximum cutting speed
Set a maximum cutting speed for each axis.
Unit of data: mm/sec, inch/sec, deg/sec (machine unit)
The parameter set on the machining parameter tuning screen is
reflected in the following parameters:
Parameter No. 13626 (velocity-emphasized parameter)
Parameter No. 13627 (precision-emphasized parameter)
Moreover, the following parameter is also set from the precision level:
Parameter No. 1432: Maximum cutting feedrate for each axis in the
AI contour control mode
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1827 -
- Arbitrary items
Two arbitrary parameters can be registered. Each item can correspond
to a CNC parameter or servo parameter. A parameter number
corresponding to each item is to be specified with parameters.
As indicated below, set the parameters for corresponding parameter
numbers, velocity-emphasized parameters (precision level 1), and
precision-emphasized parameters (precision level 10).
Table 12.4.25 (a) Parameters related to arbitrary items
Corresponding
parameter
number
Setting of
velocity-emphasized
(precision level 1)
value
Setting of
precision-emphasized
(precision level 10)
value
Arbitrary item 1 No.13628 No.13630 No.13632
Arbitrary item 2 No.13629 No.13631 No.13633
• Display
Tuning target parameter numbers are displayed.
CAUTION
As arbitrary items, the numbers of the following
parameters cannot be specified:
• Bit parameter
• Spindle parameters (Parameter Nos. 4000 to 4799)
• Real-type parameter
• Power-off parameter
• Nonexistent parameter
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1828 -
12.4.26 Displaying Memory Data (15-inch Display Unit)
The contents of the CNC memory can be displayed starting at a
specified address.
Displaying memory data
Procedure
1 Set bit 0 (MEM) of parameter No. 8950 to 1 to display the
memory contents display screen.
2 Press function key .
3 Press vertical soft key [MEMORY].
The following screen appears:
Fig. 12.4.26 (a) Memory contents display screen (15-inch)
4 Key in a desired address (hexadecimal) then press horizontal soft
key [ADDRES SEARCH]. Starting at the specified address,
256-byte data is displayed.
(Example: When you input 100000 then press [ADDRES
SEARCH], data is displayed starting at 100000H.)
5 Display data can be switched by using page keys and
and cursor keys , , , and/or .
6 By pressing horizontal soft key [BYTE], [WORD], [LONG], or
[DOUBLE], select a data type to be displayed.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1829 -
Explanation
A memory data display format can be selected from the following four
options:
Byte display (1 byte in hexadecimal)
Word display (2 bytes in hexadecimal)
Long display (4 bytes in hexadecimal)
Double display (8 bytes in decimal: Double precision floating-point
display)
One screen displays 256-byte memory data.
NOTE
1 When an address is input, "H" for representing
"hexadecimal" need not be specified at the end of
the address. If H is added, a warning is displayed to
indicate that the format is invalid.
2 When word display is selected as the display
format, an input address is rounded to a multiple of
2 bytes. When long display or double display is
selected, an input address is rounded to a multiple
of 4 bytes.
WARNING
1 If a memory address that must not be accessed in
address search is input, a system alarm is issued.
When making an address search, check that the
address is accessible and that the address is input
correctly.
2 This function is designed for maintenance, and must
not be used by general users.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1830 -
12.4.27 Parameter Tuning Screen (15-inch Display Unit)
The parameter tuning screen is a screen for parameter setting and
tuning designed to achieve the following:
1 The minimum required parameters that must be set when the
machine is started up are collectively displayed to facilitate
start-up of the machine.
2 The servo tuning screen, spindle tuning screen, and machining
parameter tuning screen are displayed for smooth tuning.
The parameter tuning screen consists of a menu screen and several
setting screens.
12.4.27.1 Displaying the menu screen and selecting a menu item
(15-inch display unit)
The parameter tuning menu screen displays the following items:
[START UP]
• SYSTEM SETTING
• AXIS SETTING
• FSSB (AMP)
• FSSB (AXIS)
• SERVO SETTING
• SPINDLE SETTING
• MISCELLANY
[TUNING]
• SERVO TUNING
• SPINDLE TUNING
• AICC TUNING
On the parameter tuning menu screen, one of the displayed items can
be selected to display the corresponding screen. From each setting
screen, you can return to the menu screen by performing a horizontal
soft key operation.
NOTE
1 Some items may not be displayed, depending on
the system configuration.
2 When bit 0 (SVS) of parameter No. 3111 is set to 0,
"SERVO SETTING" and "SERVO TUNING" are not
displayed. When bit 1 (SPS) of parameter No. 3111
is set to 0, "SPINDLE TUNING" is not displayed.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1831 -
Displaying the menu screen and selecting a setting screen
Procedure
1 Set the MDI mode.
2 Switch the setting of "PARAMETER WRITE" to "ENABLED".
For details, see the procedure for "PARAMETER WRITE" in
Subsection III-12.3.16.
3 Press function key .
4 Press vertical soft key [NEXT PAGE] several times then press
vertical soft key [PARAM TUNING]. The following screen
appears:
Fig. 12.4.27.1 (a) Parameter tuning menu screen (15-inch)
5 Move the cursor to a desired item by pressing cursor key
or .
6 Press horizontal soft key [SELECT]. The screen display switches
to the selected screen.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1832 -
Returning to the menu screen
Procedure
1 Press horizontal soft key [SELECT] on the parameter tuning
menu screen described in Subsection III-12.4.27.1. The screen
and soft keys shown below are displayed. (The screen below is
displayed when "AXIS SETTING" is selected.)
Fig. 12.4.27.1 (b) Axis setting screen (15-inch)
2 Press horizontal soft key [MENU].
The screen display returns to the parameter tuning menu screen.
3 Upon completion of parameter setting, switch the setting of
"PARAMETER WRITE" to "DISABLED".
NOTE
Part of the setting screens can be displayed also
by using a vertical soft key for chapter selection.
When these screens are displayed using the
vertical soft key for chapter selection, it becomes
impossible to return to the parameter tuning menu
screen.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1833 -
Explanation
- Items displayed with [START UP]
The items of [START UP] indicate the screens for setting the
minimum required parameters for starting up the machine.
Table 12.4.27.1 (a) Items displayed with [START UP]
Display item Description
SYSTEM SETTING Screen for setting CNC parameters related to the entire
system configuration
AXIS SETTING Screen for setting CNC parameters related to axes,
coordinates, feedrate, and acceleration/deceleration
FSSB (AMP) FSSB amplifier setting screen
FSSB (AXIS) FSSB axis setting screen
SERVO SETTING Servo setting screen
SPINDLE SETTING Screen for setting spindle-related parameters
MISCELLANY
Screen for setting parameters related to the allowable
number of M code digits and whether to display the
servo setting and spindle tuning screens
NOTE
Some items may not be displayed, depending on
the system configuration.
- Items displayed with [TUNING]
The items of [TUNING] indicate the screens for servo, spindle, and
high-speed high-precision machining tuning.
Fig. 12.4.27.1 (b) Items displayed with [TUNING]
Display item Description
SERVO TUNING Servo tuning screen
SPINDLE TUNING Spindle tuning screen
AICC TUNING Machining parameter tuning screen
NOTE
1 Some items may not be displayed, depending on
the system configuration.
2 When bit 0 (SVS) of parameter No. 3111 is set to
0, "SERVO SETTING" and "SERVO TUNING" are
not displayed. When bit 1 (SPS) of parameter No.
3111 is set to 0, "SPINDLE TUNING" is not
displayed.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1834 -
12.4.27.2 Parameter tuning screen (system setting) (15-inch display
unit)
This screen enables the parameters related to the entire system
configuration to be displayed and modified. The parameters can be
initialized to the standard values (recommended by FANUC).
Display and setting
Procedure
1 Move the cursor to [SYSTEM SETTING] by pressing cursor key
or on the parameter tuning menu screen described
in Subsection III-12.4.27.1.
2 Press horizontal soft key [SELECT]. The screen display switches
to the screen and horizontal soft keys shown below.
Fig. 12.4.27.2 (a) Parameter tuning screen (system setting) (15-inch)
3 Move the cursor to a parameter number to be set or displayed,
according to one of the methods below.
• Input the desired parameter number, then press horizontal
soft key [NO.SRH].
• Move the cursor to the desired parameter number by
pressing page key or , and cursor keys ,
, , and/or .
A brief description of the parameter where the cursor is
placed is provided at the bottom of the screen. However, no
description is provided when the cursor is placed on
multiple bits for bit parameters.
4 Input desired data then press the key on the MDI panel to
set the parameter.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1835 -
5 Press horizontal soft key [INIT]. The standard value
(recommended by FANUC) for the item selected by the cursor is
displayed in the key input buffer. Pressing horizontal soft key
[EXEC] in this state initializes the item to the standard value.
6 Press horizontal soft key [GROUP INIT]. A message asking
whether to set the group standard values is displayed on the
screen. Pressing horizontal soft key [EXEC] in this state inputs
all of the standard values of the group.
NOTE
1 If the cursor is placed on a parameter that has no
standard value assigned, no standard value is input
even when [INIT] is pressed.
2 When the cursor is placed on multiple bits for bit
parameters, the multiple bits can be input
simultaneously. When [INIT] is pressed in this state,
the key input buffer displays the standard values for
the bits where the cursor is placed. If a bit has no
standard value assigned, "*" is displayed for the bit,
and no value is input for the bit.
3 When [GROUP INIT] is pressed, those parameters
that have no standard values assigned are not
initialized.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1836 -
12.4.27.3 Parameter tuning screen (axis setting) (15-inch display unit)
This screen enables the CNC parameters related to axes, coordinates,
feedrate, and acceleration/deceleration to be displayed and set. The
parameters displayed can be divided into four groups:
(Basic) group :
The parameters related to basic settings are displayed.
(Coordinate) group :
The parameters related to coordinates are displayed.
(Feedrate) group :
The parameters related to feedrate are displayed.
(Acceleration/deceleration) group:
The parameters related to acceleration/deceleration are displayed.
The parameters can be initialized to the standard values
(recommended by FANUC). For the display and setting procedure, see
the description of the parameter tuning screen (axis setting) in
Subsection III-12.4.27.2.
Fig. 12.4.27.3 (a) Parameter tuning screen (axis setting) (15-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1837 -
12.4.27.4 Displaying and setting the FSSB amplifier setting screen
(15-inch display unit)
From the parameter tuning screen, the FSSB amplifier setting screen
can be displayed. For details of the FSSB amplifier setting screen, see
the description of the FSSB amplifier setting screen in Subsection
1.4.4 in the Connection Manual (Function) (B-63943EN-1).
Fig. 12.4.27.4 (a) FSSB amplifier setting screen (15-inch)
Fig. 12.4.27.4 (b) FSSB amplifier setting screen 2 (15-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1838 -
12.4.27.5 Displaying and setting the FSSB axis setting screen (15-inch
display unit)
From the parameter tuning screen, the FSSB axis setting screen can be
displayed. For details of the FSSB axis setting screen, see the
description of the FSSB axis setting screen Subsection 1.4.4 in the
Connection Manual (Function) (B-63943EN-1).
Fig. 12.4.27.5 (a) FSSB axis setting screen (15-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1839 -
12.4.27.6 Displaying and setting the servo setting screen (15-inch
display unit)
From the parameter tuning screen, the servo setting screen can be
displayed. For details of the servo setting screen, see the description of
the servo setting screen in Subsection III-12.4.19.
Fig. 12.4.27.6 (a) Servo setting screen (15-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1840 -
12.4.27.7 Parameter tuning screen (spindle setting) (15-inch display
unit)
The spindle-related parameters can be displayed and modified.
For the display and setting procedure, see the description of the
parameter tuning screen (system setting) in Subsection III-12.4.27.2.
Fig. 12.4.27.7 (a) Parameter tuning screen (spindle setting) (15-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1841 -
12.4.27.8 Parameter tuning screen (miscellaneous settings) (15-inch
display unit)
The parameters related to the allowable number of M code digits and
whether to display the servo setting and spindle tuning screens can be
displayed and modified. Moreover, the parameters can be initialized to
the standard values (recommended by FANUC).
For the display and setting procedure, see the description of the
parameter tuning screen (system setting) in Subsection III-12.4.27.2.
Fig. 12.4.27.8 (a) Parameter tuning screen (Miscellaneous setting)
(15-inch)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1842 -
12.4.27.9 Displaying and setting the servo tuning screen (15-inch
display unit)
From the parameter tuning screen, the servo tuning screen can be
displayed. For details of the servo tuning screen, see the description of
the servo tuning screen in Subsection III-12.4.20.
Fig. 12.4.27.9 (a) Servo tuning screen (15-inch)
12.4.27.10 Displaying and setting the spindle tuning screen (15-inch
display unit)
From the parameter tuning screen, the spindle tuning screen can be
displayed. For details of the spindle tuning screen, see the description
of the spindle tuning screen in Subsection III-12.4.22.
Fig. 12.4.27.10 (a) Spindle tuning screen (15-inch)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1843 -
12.4.27.11 Displaying and setting the machining parameter tuning
screen (15-inch display unit)
From the parameter tuning screen, the machining parameter tuning
screen can be displayed. For details of the machining parameter
tuning screen, see the description of the machining parameter tuning
screen in Subsection III-12.4.25.
Fig. 12.4.27.11 (a) Machining parameter tuning screen (15-inch)
Explanation
- Parameters displayed for parameter tuning
Table 12.4.27 (a) Parameters displayed for parameter tuning (1)
Menu Group
Parameter
No. Name Brief description
Standard
setting
981 Sets the path of each axis.
982 Sets the path of each spindle.
983 Sets the T series/M series of each path. 0:T series/1:M series
984#0 LCP Sets the attribute of each path. 0:Normal/1:Loader control *1
3021 Sets the G/F signal address of each axis. *2
3022 Sets the G/F signal address of each spindle. *3
3006#0 GDC The deceleration signal for reference position return is:
0:X signal/1:G signal
1
3008#2 XSGx The signal address allocated to address X is:
0:Fixed/1:Set by the parameter
1
3013 Address allocated to the deceleration signal for reference position
return
*4
SYSTEM
SETTING
System
setting
3014 Bit position allocated to the deceleration signal for reference
position return
*5
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1844 -
*1 : The value 1 is set for the paths as many as the number of loader
paths starting from the greatest path number. For path 1, the value 0
is set at all times.
Example) When the number of loader paths is 3 in a 10-path system:
The value 1 is set for paths 8 to 10. The value 0 is set for
others.
*2 : When intra-path axis number ≤ 8, (path number - 1)*10+(intra-path
axis number - 1)
When intra-path axis number ≥ 9, no standard value is available.
Example) When path 1 has 9 axes, and path 2 has 3 axes:
0,1,...,7,(none) for axes of path 1, 10,11,12 for axes of path 2
*3 : When intra-path spindle number ≤ 4, (path number -
1)*10+(intra-path spindle number - 1)
When intra-path spindle number ≥ 5, no standard value is available.
Example) When path 1 has 5 spindles, and path 2 has 1 spindle:
0,1,...,4,(none) for spindles of path 1, 10 for spindle of path
2
*4 : When (path number ≤ 3) and (intra-path axis number ≤ 8)
Axes of path 1: 9
Axes of path 2: 7
Axes of path 3: 10
Other axes: No standard value is available.
Example) When path 1 has 9 axes, and path 2 has 3 axes:
9,9,9,9,9,9,9,9,(none) for axes of path 1, 7,7,7 for axes of
path 2
*5 : When (path number ≤ 3) and (intra-path axis number ≤ 8)
(Intra-path axis number - 1)
Other axes: No standard value is available.
Example) When path 1 has 9 axes, and path 2 has 3 axes:
0,1,...,7,(none) for axes of path 1, 0,1,2 for axes of path 2
Table 12.4.27 (b) Parameters displayed for parameter tuning (2)
Menu Group
Parameter
No. Name Brief description
Standard
setting
3716#0 A/Ss Sets the type of spindle motor: 0:Analaog/1:Serial.
3717 Sets a motor number to be assigned to each spindle.
SPINDLE
SETTING
Spindle
setting
3706#4 GTT Specifies a spindle gear selection method.
0:M type/1:T type
3718 Sets a suffix to be added to spindle speed display on a screen
such as the position display screen.
3735 Sets the minimum clamp speed of the spindle motor.
3736 Sets the maximum clamp speed of the spindle motor.
3741 Sets the maximum spindle speed for gear 1.
3742 Sets the maximum spindle speed for gear 2.
3743 Sets the maximum spindle speed for gear 3.
3744 Sets the maximum spindle speed for gear 4.
3772 Sets the maximum speed of the spindle.
When 0 is set, the speed is not clamped.
4133 Sets the motor model code of the serial spindle.
(This setting is not required for an analog spindle.)
4019#7 ***
The parameters for the serial spindle are:
0:Not automatically set/1:Automatically set
(This setting is not required for an analog spindle.)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1845 -
Table 12.4.27 (c) Parameters displayed for parameter tuning (3)
Menu Group
Parameter
No. Name Brief description Standard
setting
AXIS
SETTING
Basic 1001#0 INM Least command increment on linear axes:
0:Metric (millimeter machine) 1:Inch (inch machine)
1005#0 ZRNx When an automatic operation (other than G28) is executed before
reference position return:
0:Alarm is issued (PS0224) 1:No alarm is issued.
0
1005#1 DLZx Reference position return without dogs: 0:Disabled 1:Enabled
1006#0 ROTx Setting of linear axes or rotary axis:
0:Linear axis 1:Rotation axis
1006#3 DIAx Setting of the amount of travel:
0:Radius specification 1: Diameter specification
1006#5 ZMIx Reference position return direction:
0:Plus direction 1:Minus direction
1008#0 ROAx Rotation axis roll-over function: 0:Disabled 1:Enabled 1
1008#2 RRLx With the amount of travel per revolution, relative coordinates are:
0:Not rounded 1:Rounded
1
1013#0 ISAx Sets the least input increment and least command increment:
0:IS-B 1:IS-A
1013#1 ISCx Sets the least input increment and least command increment:
0:IS-B 1:IS-C
1013#2 ISDx Sets the least input increment and least command increment:
0:IS-B 1:IS-D
1013#3 ISEx Sets the least input increment and least command increment:
0:IS-B 1:IS-E
1020 Program name *1
1022 Sets each axis in the basic coordinate system. *2
1023 Servo axis number
1815#1 OPTx A separate pulse coder is: 0:Not used 1:Used
1815#4 APZx The correspondence between machine positions and
absolute-position detector positions is: 0:Not established
1:Established
1815#5 APCx The position detector used is: 0:Other than an absolute-position
detector 1:Absolute-position detector
1825 Servo loop gain
1826 Effective area
1828 Positional deviation limit during travel
1829 Positional deviation limit during stop 500
*1 : For the M series: 88(X),89(Y),90(Z) sequentially starting with the
first axis (no standard value for the fourth axis and
up)
For the T series: 88(X),90(Z) (no standard value for the third axis
and up)
*2 : For the M series: 1,2,3 sequentially starting with the first axis (no
standard value for the fourth axis and up)
For the T series: 1,3 (no standard value for the third axis and up)
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1846 -
Table 12.4.27 (d) Parameters displayed for parameter tuning (4)
Menu Group
Parameter
No. Name Brief description Standard
setting
AXIS SETTING Coordinate 1240 Machine coordinate of the first reference position
1241 Machine coordinate of the second reference position
1260 Amount of travel per revolution of a rotary axis 360.000
1320 Coordinate of the boundary of stored stroke check 1 in the
positive direction
1321 Coordinate of the boundary of stored stroke check 1 in the
negative direction
Feedrate 1401#6 RDR For a rapid traverse command, dry run is:
0:Disabled 1:Enabled
0
1410 Dry run feedrate
1420 Rapid traverse rate
1421 Rapid traverse override F0 rate
1423 Jog feedrate
1424 Manual rapid traverse rate
1425 FL feedrate for reference position return
1428 Reference position return feedrate
1430 Maximum cutting feedrate
Acceleration/
deceleration
1610#0 CTLx Acceleration/deceleration for cutting feed is:
0:Exponential acceleration/deceleration
1:Linear acceleration/deceleration after interpolation
1610#4 JGLx Acceleration/deceleration for jog feed is:
0:Exponential acceleration/deceleration
1:Same as acceleration/deceleration for cutting feed
(The settings of bit 1 (CTBx) and bit 0 (CTLx) of parameter
No. 1610 are followed.)
1620 Time constant for linear acceleration/deceleration for rapid
traverse
1622 Time constant for acceleration/deceleration for cutting feed
1623 FL feedrate for acceleration/deceleration after interpolation
for cutting feed
1624 Time constant for acceleration/deceleration for jog feed
1625 FL feedrate for exponential acceleration/deceleration for
jog feed
MISCELLANY MISC 3030 Allowable number of digits of an M code 3
3111#0 SVS The servo setting screen is: 0:Not displayed
1:Displayed
1
3111#1 SPS The spindle setting screen is: 0:Not displayed
1:Displayed
1
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1847 -
12.4.28 Periodic Maintenance Screen (15-inch Display Unit)
Periodic maintenance screens are used for managing consumables
(such as the backlight of a LCD unit and backup batteries). By setting
the name of a consumable, its life time, and the method for counting
down the life time, the life of the consumable can be counted down in
the appropriate method set for the consumable, and the remaining life
time can be displayed.
With these screens, the user can easily manage consumables that
require periodic replacement.
Explanation
There are four periodic maintenance screens: the status screen, the
setting screen, the machine menu screen, and the NC menu screen.
• Status screen:
Item names, remaining times, and count statuses are displayed,
and item names are set.
• Setting screen:
Life times, remaining times, and count types (count-down
method) are set.
• Machine menu screen:
The names of consumables in the machine can be registered.
• NC menu screen:
The names of consumables in the NC are already registered.
Using periodic maintenance screens
<1> Referencing a periodic maintenance screen
Display the status screen. For the meanings of items on the status
screen, see Status screen.
<2> Adding the name of a new consumable item to a periodic
maintenance screen or editing an existing consumable item on
the screen
The name of a consumable item can be added or edited on the
machine menu screen. For details, see Machine menu screen.
<3> Adding or editing a life time, remaining time, and a method of
counting down the remaining time for a consumable on a
periodic maintenance screen
A life time and remaining time can be added or edited on the
setting screen. For details, see Setting screen.
<4> Newly displaying the item name and remaining time of a
consumable on a periodic maintenance screen.
1 Setting an item name
Select the item name of a consumable to be displayed from
the machine menu screen or NC menu screen, or enter the
name using the MDI keys. For the procedure, see Item
name in Status screen.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1848 -
2 Setting a life time, remaining time, and count type
Select the life time, remaining time, and count type of a
consumable to be displayed from the setting screen. For the
procedure, see Remaining time in Status screen.
Procedure for displaying a periodic maintenance screen
1 Press function key .
2 Press vertical soft key [NEXT PAGE] several times to display
[PERIOD MAINTE].
3 Press vertical soft key [PERIOD MAINTE] to display the
periodic maintenance screen.
Status screen
When vertical soft key [STATUS] is pressed, the status screen is
displayed. The status screen shows the item names, count statuses, and
remaining times of managed consumables.
Fig. 12.4.28 (a) Status screen
- Item name
As the item name, set the name of a consumable to be managed by
periodic maintenance. To set an item name, select a name from the
machine menu screen or NC menu screen, or directly enter the name
using the MDI keys.
Setting an item name from a menu screen
1 On the status screen, move the cursor to the name of the item to
be set, and press horizontal soft key [ENTRY].
2 Press vertical soft key [MACHINE] or [NC] to display the
machine menu screen or NC menu screen.
3 Move the cursor to an item name registered on the menu screen,
and press horizontal soft key [SELECT] then [EXEC]
successively.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1849 -
4 The screen display returns to the status screen, and the item name
selected on the menu screen is added to the status screen.
Initially, there is no item name set on the machine menu screen, so
item names must be registered in advance. For the registration method,
see the description of the procedure for registering item names on the
machine menu screen.
Setting an item name using the MDI keys
1 Type the alphanumeric characters to be input, then press
horizontal soft key [INPUT].
2 The entered item name is registered on the status screen.
When horizontal soft key [+INPUT] is pressed instead of horizontal
soft key [INPUT], the entered characters can be added to an existing
item name.
When typing 2-byte characters, type "*" before and after the character
codes. The character codes must conform to FANUC codes. (See
Appendix G, "FANUC 2-BYTE CHARACTER CODE TABLE".)
An item name to be registered must be up to 24 characters long if it
consists of alphanumeric characters only; or it must be up to 12
characters long if it consists of 2-byte characters only.
Example: To register "LCD バックライト", enter the following:
>LCD＊110E10F410CC114010B610FE＊_
NOTE
1 An asterisk "*" is used as a control code, so it
cannot be used in item names. In addition,
characters "[", "]", "(", and ")" cannot be used in
item names.
2 When an item name consisting of both
alphanumeric characters and 2-byte characters is
registered, the warning "DATA OUT OF RANGE"
may be output.
Deleting an item name
To delete a registered item name, move the cursor to the item name,
press horizontal soft key [ERASE], then press horizontal soft key
[EXEC].
When an item name is deleted, its life time, remaining time, and count
type are deleted at the same time.
- Remaining time
As the remaining time, the period of time left until the time for
replacement is reached by count down operation is displayed.
If the percentage of the remaining time to the life time has reached to
the value (%) specified by parameter No. 8911, or smaller, the
remaining time is displayed in red.
Even after the life time has expired, count down operation continues.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1850 -
Setting the remaining time
1 On the status screen, place the cursor on an item for which the
remaining time is to be set (the item name must have been set in
advance).
2 Press horizontal soft key [CHANGE].
3 The screen display changes to the setting screen.
4 Set the life time, remaining time, and count type. For the setting
method and other information, see Setting screen.
NOTE
On the status screen, the remaining time and life
time cannot be set.
These items must be set on the setting screen.
- Count status
The count status is indicated on the left side of the item number as
follows:
Indication Count status
Blank Counting stopped
@ Counting in progress
＊ Life expired
Setting screen
On the setting screen, the life time, remaining time, and count type of
a managed consumable are set.
Fig. 12.4.28 (b) Setting screen
Display procedure
1 Press horizontal soft key [CHANGE].
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1851 -
- Life time
Set the life time of a consumable.
Move the cursor to an existing item, type a life time, then press
horizontal soft key [INPUT] (or the key). The life time is then
set, and the same value is set also as the remaining time.
At this time, "------" is indicated in the count type field.
When horizontal soft key [+INPUT] is pressed, the entered value can
be added to the life time already set. The same value as the added
value is added also to the remaining time.
A value ranging from 0 to 65535 (in hours) can be set.
NOTE
1 If a setting operation is attempted when the item
name is not registered, the warning "EDIT
REJECTED" is issued.
2 If a value exceeding the valid range is entered, the
warning "DATA IS OUT OF RANGE" is issued.
3 If soft key [ERASE] or [TYPE] is pressed, the
warning "EDIT REJECTED" is issued.
- Remaining time
The period of time left until the time for replacement is reached by
count down operation is indicated.
If the percentage of the remaining time to the life time has reached the
value (%) specified by parameter No. 8911, or smaller, the remaining
time is displayed in red.
Even after the life time has expired, count down operation continues.
Move the cursor to the remaining time of a target registered number,
type a remaining time, then press horizontal soft key [INPUT] (or the
key). The remaining time is then set.
When horizontal soft key [+INPUT] is pressed, the entered value can
be added to the remaining time already set.
A value ranging from 0 to (life time) can be set.
When horizontal soft key [ERASE] then horizontal soft key [EXEC]
are pressed, the same value as the life time is set.
NOTE
1 If a setting operation is attempted when the item
name or life time is not registered, the warning
“EDIT REJECTED” is issued.
2 When a value exceeding the valid range is entered,
the warning “DATA IS OUT OF RANGE” is issued.
3 If horizontal soft key [TYPE] is pressed, the
warning “EDIT REJECTED” is issued.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1852 -
- Count type
As the count type, select the way of counting.
Place the cursor on the count type of a target registration number, then
press horizontal soft key [TYPE]. Count types are displayed as soft
keys as shown below. Select one of these soft keys, then press
horizontal soft key [EXEC].
Soft key Meaning Indication
[NO CNT] Counting is not performed (stopped) — — — — — —
[ALL] Counting is performed at all times All times
[POWER ON] Counting is performed when power
is on.
When power is on
[RUN] Counting is performed when
operation is in progress.
When operation is in
progress
[CUT] Counting is performed when cutting
is being performed.
When cutting is being
performed
NOTE
1 If a setting operation is attempted when the item
name or life time is not registered, the warning
“EDIT REJECTED” is issued.
2 Horizontal soft keys [INPUT] and [+INPUT] have no
effect.
3 When counting is performed at all times, a 24-hour
error is generated in leap year.
4 If horizontal soft key [ERASE] is pressed, the
warning “EDIT REJECTED” is issued.
Machine menu screen
On the machine menu screen, the names of consumables of the
machine are registered. From this screen, item names can be added to
the status screen. For the method of addition to the status screen, see
the description of the status screen.
Fig. 12.4.28 (c) Machine menu screen
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1853 -
- Displaying the screen
1 When the status screen is displayed, press vertical soft key
[MACHINE].
On the machine menu screen, item names can be registered using one
of the following two methods:
• Registration from a program
• Registration using the MDI keys
- Registration from a program
By executing a program having the following format, an item name
can be registered in the menu of the machine:
Format
G10 L61 Px [n]
X Registration number
n Item name, format:
[alphanumeric-characters*2-byte-characters*alphanumeric-characters]
- Registration using the MDI keys
An item name can be registered on the menu screen of the machine by
typing the item name in the format shown below on the machine menu
screen, then pressing horizontal soft key [INPUT] (or the key).
When horizontal soft key [+INPUT] is pressed, the typed characters
can be added to an already registered item name.
Format
Alphanumeric-characters*2-byte-characters*alphanumeric-characters
Two-byte codes must conform to FANUC codes. (See Appendix G,
"FANUC 2-BYTE CHARACTER CODE TABLE".)
When typing 2-byte characters, type an asterisk "*" before and after
the character codes. An item name to be registered must be up to 24
characters long if it consists of alphanumeric characters only; or it
must be up to 12 characters long if it consists of 2-byte characters only.
Example:
To register "LCD バックライト", enter the following:
>LCD＊110E10F410CC114010B610FE＊_
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1854 -
NOTE
1 An asterisk "*" is used as a control code, so it
cannot be used in item names. In addition,
characters "[", "]", "(", and ")" cannot be used in
item names.
2 When an item name consisting of both
alphanumeric characters and 2-byte characters is
registered, the warning “DATA IS OUT OF
RANGE” may be output.
3 When a blank item name is selected on the
machine screen, the warning “EDIT REJECTED” is
issued.
To delete a registered item name, move the cursor to the item name,
press horizontal soft key [ERASE], then press horizontal soft key
[EXEC].
From this screen, an item name can be registered on the status screen.
For the method of registration to the status screen, see the description
of the status screen.
Fig. 12.4.28 (a) NC menu screen
- Displaying the screen
1 When the status screen is displayed, press soft key [NC].
NOTE
On the NC screen, the registration, deletion, and
I/O of item names cannot be performed.
When a blank item name is selected, a blank is set.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1855 -
12.4.29 System Configuration Screen (15-inch Display Unit)
The system configuration screen provides information about the types
of installed hardware and software.
Procedure for displaying the screen
Procedure
1 Press the key, then press vertical soft key [NEXT PAGE]
several times until vertical soft key [SYSTEM] is displayed.
2 Press vertical soft key [SYSTEM]. The system configuration
screen is displayed.
There are two types of system configuration screens: the hardware
configuration screen and the software configuration screen. The screen
display can switch between these screens by using and .
When vertical soft key [SERVO INFO] or [SPINDLE INFO] is
pressed, information about the connected servo system or spindles is
displayed.
Fig. 12.4.29 (a) System configuration screen
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1856 -
Hardware configuration screen
This screen shows the names and IDs of the hardware used by the NC.
Fig. 12.4.29 (b) Hardware configuration screen
Software configuration screen
This screen shows the names and series/editions of the software used
by the NC.
Fig. 12.4.29 (c) Software configuration screen
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1857 -
Servo information screen
When a servo system is connected to the NC, ID information of the
connected servo devices (servo motors and servo amplifier modules)
can be displayed on the NC.
Displaying the screen
1 When the system configuration screen is displayed, press vertical
soft key [SERVO INFO].
2 The servo information screen is displayed.
Fig. 12.4.29 (d) Servo information screen
Spindle information screen
When a spindle system is connected to the NC, the ID information of
the connected spindle devices (spindle motors and spindle amplifier
modules) can be displayed on the NC.
Displaying the screen
1 When the system configuration screen is displayed, press vertical
soft key [SPINDLE INFO].
2 The spindle information screen is displayed.
Fig. 12.4.29 (e) Spindle information screen
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1858 -
12.4.30 Overview of the History Function (15-inch Display Unit)
The history function makes it possible to record a history of
operations performed by the operator, alarms and external operator
messages issued, and other history data, check the history, and output
history data.
1 Conditions for recording history
a Display screen
A history of screens other than the operation history screen
is recorded.
b Signal selection
Up to 60 I/O signals can be selected so that they can be
recorded in history data.
c Parameter setting
With parameters, it is possible to separately set whether to
record an MDI key operation history and an external
operator message history, add external alarms and messages,
and record data modification histories such as operation
histories of parameters, tool offsets, workpiece offsets
(workpiece shift amounts), custom macro common variables,
and I/O signals.
d Storage capacity
When the storage capacity becomes full, data is deleted in
order from the oldest data.Up to about 8000 items of history
data can be recorded if the data consists of history data of
MDI key operations only.
2 Data output
All history data stored can be output to external input/output
devices. (See Subsection 12.4.30.5, "Outputting all history
data".)
3 Erasure of history data
If bit 7 (EKE) of parameter No. 3195 is set to 1, soft key
[CLEAR] is displayed, allowing the user to erase history data.
#7 #6 #5 #4 #3 #2 #1 #0
3195 EKE
[Data type] Bit
# 7 EKE Soft key [ALL CLEAR] for clearing all history data is:
0: Not displayed.
1: Displayed.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1859 -
NOTE
1 History data remains even after the power is turned
off.
Memory clear operation, however, erases history
data as well.
2 Set the time and date correctly on the setting
screen.
3 All history data including data of alarms, external
operator messages, operations, and I/O signals is
integrated and maintained in a single storage area.
When the storage capacity becomes full, history
data is erased in order from the oldest data
regardless of the history type.
When history data is erased, all history data is
erased, so care should be taken.
It is impossible to erase only a specific history.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1860 -
12.4.30.1 Alarm history
From all history data recorded, only alarm history is extracted and
displayed on the screen. Note that when the amount of history data
exceeds the storage capacity, history data is automatically erased in
order from the oldest history data.
Fig. 12.4.30.1 (a) Alarm history screen
Screen display
Issued alarms are displayed sequentially from the latest alarm.
The following information is displayed for each alarm:
• Path name (only when multipath operation is performed)
• Time and date of alarm occurrence
• Type and number of the alarm
• Alarm message
NOTE
To record also external alarm and macro alarm
messages as history data, set bit 3 (EAH) of
parameter No. 3112 to 1, and at the same time set
bit 7 (HAL) of parameter No. 3196 to 0.
When a name such as a path name, axis name, or spindle name has
been changed after the issuance of an alarm, a newly assigned name is
displayed on the alarm history screen.
When modal O data that is a program name is output, only the first
five characters are output.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1861 -
Procedure
1 Press function key to display a screen of parameters and
so on.
2 Press vertical soft key [HISTRY] to display the alarm history
screen.
3 The screen display can be changed to the previous page and the
next page by using page keys and .
Erasing history data from the alarm history screen
Procedure
1 Display the alarm history screen.
2 Press horizontal soft key [CLEAR]. All history data is then
erased.
NOTE
When history data is erased, not only alarm history
data but also other history data such as external
operator message history data and operation
history data is erased. It is impossible to erase only
a specific history.
Display of external alarms and macro alarms
When an external alarm or macro alarm is issued, it becomes possible
to record its message as well as the alarm number in the alarm history
if the parameter shown below is set. As the message of an external
alarm or macro alarm, the first 32 characters for the external alarm or
the first 26 characters for the macro alarm are recorded.
#7 #6 #5 #4 #3 #2 #1 #0
3112 EAH
[Data type] Bit
# 3 EAH Messages of the external alarm/macro alarm in alarm or operation
history:
0: Not recorded
1: Recorded
NOTE
This parameter is valid when bit 7 (HAL) of
parameter No. 3196 is set to 0.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1862 -
#7 #6 #5 #4 #3 #2 #1 #0
3196 HAL
[Data type] Bit
# 7 HAL When an alarm is issued, additional information (modal data, absolute
coordinates, and machine coordinates present at the issuance of the
alarm) is:
0: Recorded in the operation history and alarm history.
1: Not recorded in the operation history and alarm history.
NOTE
1 History data such as alarm history data, operation
history data, external operator message history
data, and data modification history data is stored in
the same storage area. Therefore, alarm history
data may be erased when the storage capacity is
exceeded by other history data.
2 The maximum number of history data items that
can be stored is as follows, where the history data
is assumed to include alarm data only:
When bit 7 (HAL) of parameter No. 3196 is set to 1,
up to about 4000 history data items can be stored.
When bit 7 (HAL) of parameter No. 3196 is set to 0,
modal information and coordinates observed when
an alarm is issued are also recorded, so the
maximum number of history data items that can be
stored varies from system to system. (Example:
For a 5-axis system, up to about 280 data items
can be stored; for a 10-axis system, up to about
200 data items can be stored.)
When bit 3 (EAH) of parameter No. 3112 is set to
1, however, macro and external alarm messages
are also stored, so the number of data items that
can be stored further decreases.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1863 -
12.4.30.2 External operator message history
From all history data recorded, only external operator message history
and macro message history are extracted and displayed on the screen.
When the amount of history data exceeds the storage capacity, history
data is automatically erased in order from the oldest history data.
Fig. 12.4.30.2 (a) External operator message history screen
Screen display
Procedure
1 Press function key .
2 Press vertical soft key [MESAGE HISTRY] to display the
external operator message history screen.
3 The screen display can be changed to the previous page and the
next page by using page keys and .
NOTE
1 History data such as external operator message
history data, operation history data, alarm history
data, and data modification history data is stored in
the same storage area. Therefore, external
operator message history data may be erased
when the storage capacity is exceeded by other
history data.
2 The maximum number of history data items that
can be stored is about 150 if the history data
includes external operator message data only.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1864 -
Erasing history data from the external operator message history screen
Procedure
1 Display the external operator message history screen.
2 Press horizontal soft key [CLEAR]. All history data is then
erased.
NOTE
When history data is erased, not only external
operator message history data but also other
history data such as operation history data and
alarm history data is erased. It is impossible to
erase only a specific history.
Parameter setting
#7 #6 #5 #4 #3 #2 #1 #0
3112 OMH
[Data type] Bit
# 2 OMH The external operator message history screen is:
0: Not displayed.
1: Displayed.
#7 #6 #5 #4 #3 #2 #1 #0
3196 HOM
[Data type] Bit
# 6 HOM A history of external operator messages and macro messages is:
0: Recorded.
1: Not recorded.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1865 -
12.4.30.3 Operation history
This function displays a history of the operator's key operations and
signal operations made when a failure occurred or an alarm was issued,
and also information about alarms.
The following data is recorded:
a Operation history
ⅰ MDI key operations made by the operator
ⅱ I/O signal (X,Y,G,F) on/off switching
b Alarm history
ⅰ Alarms issued
ⅱ Modal information in a block executed and coordinates
observed when an alarm was issued
(Not displayed on the screen)
c Data modification history
ⅰ Modification of tool offset data
(When bit 0 (HTO) of parameter No. 3196 is set to 1)
ⅱ Modification of workpiece offset data/extended workpiece
offset data/workpiece shift (T series)
(When bit 1 (HWO) of parameter No. 3196 is set to 1)
ⅲ Modification of parameters
(When bit 2 (HPM) of parameter No. 3196 is set to 1)
ⅳ Modification of custom macro common variable data
(When bit 3 (HMV) of parameter No. 3196 is set to 1)
d External operator message history and macro message history
(When bit 6 (HOM) of parameter No. 3196 is set to 0)
e Time stamp (time and date)
With some exceptions, history data of the operation history and alarm
history can be viewed on the operation history screen. (The data
modification history, external operator message history, and alarm
messages are not displayed.)
All recorded history data can be output to external input/output
devices.
NOTE
Up to about 8000 items of history data can be
recorded if the data includes history data of MDI
key operations only. However, because history data
varies in size, the maximum number of history data
items that can be recorded is not fixed.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1866 -
Parameter setting
#7 #6 #5 #4 #3 #2 #1 #0
3106 OPH
[Data type] Bit
# 4 OPH The operation history screen is:
0: Not displayed.
1: Displayed.
3122 Time interval used to record time data in operation history
[Input type] Parameter input
[Data type] Word path
[Unit of data] min
[Valid data range] 0 to 1440
When history data is recorded within a set time period, the time for
each set time period is recorded in the history data.
When 0 is set, the specification of a time period of 10 minutes is
assumed.
If no data is recorded within a set time period, the time for that period
is not recorded.
NOTE
The same value must be set in this parameter for
all paths.
#7 #6 #5 #4 #3 #2 #1 #0
3195 EKE HDE HKE
[Input type] Parameter input
[Data type] Common to the bit system
# 5 HKE A key operation history is:
0: Recorded.
1: Not recorded.
# 6 HDE A DI/DO history is:
0: Recorded.
1: Not recorded.
# 7 EKE Soft key [ALL CLEAR] for clearing all history data is:
0: Not displayed.
1: Displayed.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1867 -
#7 #6 #5 #4 #3 #2 #1 #0
3196 HAL HOM HMV HPM HWO HTO
[Data type] Bit
# 0 HTO A modification history of tool offset data is:
0: Not recorded.
1: Recorded.
# 1 HWO A modification history of workpiece offset data/extended workpiece
offset data/workpiece shift (T series) is:
0: Not recorded.
1: Recorded.
# 2 HPM A modification history of parameters is:
0: Not recorded.
1: Recorded.
# 3 HMV A modification history of custom macro common variables is:
0: Not recorded.
1: Recorded.
# 6 HOM A history of external operator messages and macro messages is:
0: Recorded.
1: Not recorded.
# 7 HAL When an alarm is issued, additional information (modal data, absolute
coordinates, and machine coordinates present at the issuance of the
alarm) is:
0: Recorded in the operation history and alarm history.
1: Not recorded in the operation history and alarm history.
To record as many alarm history items as possible, rather than detailed
alarm information, set 1. The numbers of ten G code modal groups to
be recorded are set in parameter Nos. 12990 to 12999.
12990
(1st) G code modal group to be recorded in the history when an alarm is issued
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to the maximum number of G code groups
Set the number of a G code modal group to be recorded in the alarm
history and operation history when an alarm is issued.
* If a value beyond the valid data range is set, the status of group
01 is recorded.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1868 -
12991
(2nd) G code modal group to be recorded in the history when an alarm is issued
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to the maximum number of G code groups
Set the number of a G code modal group to be recorded in the alarm
history and operation history when an alarm is issued.
* If a value beyond the valid data range is set, the status of group
02 is recorded.
12992
(3rd) G code modal group to be recorded in the history when an alarm is issued
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to the maximum number of G code groups
Set the number of a G code modal group to be recorded in the alarm
history and operation history when an alarm is issued.
* If a value beyond the valid data range is set, the status of group
03 is recorded.
12993
(4th) G code modal group to be recorded in the history when an alarm is issued
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to the maximum number of G code groups
Set the number of a G code modal group to be recorded in the alarm
history and operation history when an alarm is issued.
* If a value beyond the valid data range is set, the status of group
04 is recorded.
12994
(5th) G code modal group to be recorded in the history when an alarm is issued
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to the maximum number of G code groups
Set the number of a G code modal group to be recorded in the alarm
history and operation history when an alarm is issued.
* If a value beyond the valid data range is set, the status of group
05 is recorded.
12995
(6th) G code modal group to be recorded in the history when an alarm is issued
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to the maximum number of G code groups
Set the number of a G code modal group to be recorded in the alarm
history and operation history when an alarm is issued.
* If a value beyond the valid data range is set, the status of group
06 is recorded.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1869 -
12996
(7th) G code modal group to be recorded in the history when an alarm is issued
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to the maximum number of G code groups
Set the number of a G code modal group to be recorded in the alarm
history and operation history when an alarm is issued.
* If a value beyond the valid data range is set, the status of group
07 is recorded.
12997
(8th) G code modal group to be recorded in the history when an alarm is issued
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to the maximum number of G code groups
Set the number of a G code modal group to be recorded in the alarm
history and operation history when an alarm is issued.
* If a value beyond the valid data range is set, the status of group
08 is recorded.
12998
(9th) G code modal group to be recorded in the history when an alarm is issued
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to the maximum number of G code groups
Set the number of a G code modal group to be recorded in the alarm
history and operation history when an alarm is issued.
* If a value beyond the valid data range is set, the status of group
09 is recorded.
12999
(10tht) G code modal group to be recorded in the history when an alarm is issued
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to the maximum number of G code groups
Set the number of a G code modal group to be recorded in the alarm
history and operation history when an alarm is issued.
* If a value beyond the valid data range is set, the status of group
10 is recorded.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1870 -
Screen display
Procedure
1 Press function key .
2 Press vertical soft key [NEXT PAGE] several times until soft key
[OPERAT HISTRY] is displayed.
3 Press vertical soft key [OPERAT HISTRY], then press newly
displayed vertical soft key [OPERAT HISTRY]. The operation
history screen is then displayed.
4 To display the previous page and next page of the operation
history, use page keys and .
To display a part across two pages, use the cursor keys
and . The screen display is shifted by half page.
(With the 7.2- and 8.4-inch display devices, the screen display is
shifted by one column.)
When the operation history screen is displayed, the following
horizontal soft key operations can be performed:
a [TOP] displays the starting page (the oldest data).
b [BOTTOM] displays the end page (the latest data).
c [NO.SRH] displays specified operation history data.
(Example) Specifying 50 then [NO.SRH] displays the 50th
data.
Fig. 12.4.30.3 (a) Operation history screen
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1871 -
Displayed information
1 Serial number and display start history number/total number of
history data items
A serial number is indicated on the left side of each recorded
history data item. A smaller serial number indicates an older data
item.
In the upper right part of the screen, the display start history
number and the total number of history data items are indicated.
The total number of history data items does not include history
data items not displayed on the screen.
2 Data
• MDI key
When bit 5 (HKE) of parameter No. 3195 is set to 0, key
operations are recorded.
A key operation is indicated following a path number (for
example, "1_[LEFT F]", and "2_[LEFT F]"). (When only
one path is used, the path number is not indicated.)
P_ used in "P_[LEFT F]", for example, indicates a key
operation made from the outside.
i Address keys and numeric keys
Characters such as A to Z, 0 to 9, ;, +, and - are
indicated directly.
These characters are displayed in black.
ii Function menu keys, operation menu keys, and soft
keys
These keys are enclosed in brackets [] (for example,
"[LEFT F]", "[SOFT 1]" to "[SOFT 10]", and
"[RIGHT F]"). These keys are displayed with green
characters.
iii Function keys, page keys, cursor keys, and so on
These keys are enclosed in angle brackets <> (for
example, "<POS>", "<SYSTEM>", "<PAGE ↑>",
"<CUR →>", "<RESET>", and "<INPUT>"). These
keys are displayed with green characters.
iv Power-on key
This key is displayed with white characters in the
green background.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1872 -
• I/O signals
When bit 6 (HDE) of parameter No. 3195 is set to 0, I/O
signals specified on the operation history signal selection
screen are recorded. Recorded signals are indicated on a
bit-by-bit basis with information about the signal address
and a change in bit. These signals are displayed with purple
characters.
G000.2 ↓
Change from 0 to 1 is indicated by ↑.
Change from 1 to 0 is indicated by ↓.
Indicates a bit.
Indicates the address of a signal.
NOTE
1 When more than one bit at the same address
changes at the same time, the changes of these
bits are treated as one history data item.
2 A signal fluctuation for less than 4 msec is not
recorded as history data.
• Alarms
Alarm numbers and the issuance times are displayed on the
operation history screen.
This alarm information is displayed with white characters in
the red background.
When a path name, axis name, or spindle name was
changed after the issuance of an alarm, the alarm is
indicated with a newly assigned name.
• Time and date
The time and date of the following are displayed in two
lines:
i The time and date of power-on. These are displayed
with white characters in the green background.
ii The time and date of power-off. These are displayed
with green characters.
iii Date on which the date changed. This is displayed with
black characters.
iv Date and time at regular intervals of the period set in
parameter No. 3122. These are displayed with black
characters.
Indicates the path number.
Indicates the alarm number.
For the servo axis type, indicates the servo axis name.
For the spindle type, indicates the spindle name or
spindle number.
1_OT0506
(XA1)
2004/01/11
Indicates the date and time of issuance in two lines.
11:22:33
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1873 -
v Date and time when history data was erased. These are
displayed with black characters.
NOTE
1 When times are recorded at regular intervals, if
there is no data to record within an interval, the
time is not recorded. (When the date is changed,
the time is recorded on the assumption that there
is data to record.)
2 When the date and time in the CNC system are
changed, the date and time at which the change
is made may be recorded as the date and time in
iii or iv above.
History data not displayed on the screen
In addition to history data of MDI keys, I/O signal status, alarms
issued, external operator messages (not displayed on the operation
history screen), and time stamps, data described below can be
recorded with time. Such history data cannot be displayed on the
screen but can be output to external input/output devices. (See
Subsection 12.4.30.5, "Outputting all history data".)
1 Detailed data at alarm issuance
If bit 7 (HAL) of parameter No. 3196 is set to 0, 10 modal G
codes, auxiliary function codes D, E, F, H, M, N, O, S, and T,
absolute coordinates, and machine coordinates in the block being
executed when an alarm was issued are recorded together with
the alarm number and the time of alarm issuance.
The group numbers of the 10 modal G codes to be recorded are
set in parameter Nos. 12990 to 12999. If these parameters are not
specified, modal G codes of groups 01 to 10 are recorded.
NOTE
1 For modal O data that is a program name, only the
first five characters are recorded.
2 To record as many items as possible instead of
recording detailed data at alarm issuance, set bit 7
(HAL) of parameter No. 3196 to 1.
2 External alarm messages and macro alarm messages
If bit 3 (EAH) of parameter No. 3112 is set to 1, external alarm
messages and macro alarm messages can also be recorded as
history data. However, only the first 64 characters of each
message are recorded.
NOTE
To record also external alarm and macro alarm
messages as history data, set bit 3 (EAH) of
parameter No. 3112 to 1, and at the same time set
bit 7 (HAL) of parameter No. 3196 to 0.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1874 -
3 Modification of tool offset data
If bit 0 (HTO) of parameter No. 3196 is set to 1, when tool offset
data is modified, the number and type of the tool offset are
recorded as well as the tool offset data before modification, the
tool offset data after modification, and the time of modification.
4 Modification of workpiece offset/extended workpiece
offset/workpiece shift (T series) data
If bit 1 (HWO) of parameter No. 3196 is set to 1, when
workpiece offset data is modified, the number of the modified
workpiece offset is recorded as well as the workpiece offset data
before modification, the workpiece offset data after modification,
and the time of modification. Similar data is recorded also when
extended workpiece offsets and workpiece shift amounts (T
series) are modified.
5 Modification of parameters
If bit 2 (HPM) of parameter No. 3196 is set to 1, when a
parameter is modified, the number and type (axis type, spindle
type, path type, or machine group type) of the parameter are
recorded as well as the parameter data before modification, the
parameter data after modification, and the time of modification.
NOTE
Modifications made at power-on and modifications of
passwords and keys are not recorded as history
data.
6 Modification of custom macro common variables (#100 to #999)
If bit 3 (HMV) of parameter No. 3196 is set to 1, when a custom
macro common variable is modified, the number of the common
variable is recorded as well as the common variable value before
modification, the common variable value after modification, and
the time of modification.
Erasing history data from the operation history screen
Procedure
1 Display the operation history screen.
2 Press horizontal soft key [ALL CLEAR].
3 Press horizontal soft key [EXEC]. All history data is erased.
NOTE
An erasure operation erases not only operation
history data but also other history data such as
external operator message history data and alarm
history data. It is impossible to erase only a specific
history.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1875 -
12.4.30.4 Selecting operation history signals
I/O signals to be recorded as history data can be selected. Up to 60
signals can be set.
Setting data
1 Press function key .
2 Press vertical soft key [NEXT PAGE] several times until vertical
soft key [OPERAT HISTRY] is displayed.
3 Press vertical soft key [OPERAT HISTRY].
4 Press vertical soft key [SIGNAL SELECT] to display the
operation history signal selection screen.
5 Move the cursor to a desired position by using cursor keys
and .
6 Type a signal type (X, G, F, or Y) and an address, then press
.
Example:
When G0004 is entered then is pressed:
The entered signal address, G0004, is set in ADDRESS, and
initial value 00000000 is set in SIGNAL.
7 Select the bits to be recorded in the history.
To change the status of all bits of the specified signal address,
place the cursor in all bits so that the bits are highlighted (for
example, "00000000"), then press horizontal soft key [ON:1] or
[OFF:0]. Then, the bits are set to 11111111 or 00000000.
To change the status of only a certain bit, move the cursor to the
bit by using cursor keys and , and press horizontal
soft key [ON:1] or [OFF:0]. The selected bit is then set to 1 or 0.
8 Up to 60 addresses can be set to select signals. Addresses need
not necessarily be set sequentially starting from No. 1.
NOTE
1 While the operation history signal selection screen is
being displayed, recording of history data is not
performed.
2 Only X, Y, G, and F can be set for I/O signals.
For data not set, "********" is displayed.
3 Even when an address is set, history data is not
recorded if all bits are set to 0.
4 When the ON/OFF width of an input signal is less than 4
msec, recording of history data is not performed.
Also,there are some signals that are not recorded.
5 When many signals are selected, the processing speed
may lower.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1876 -
Clearing data individually
1 Display the operation history signal selection screen.
2 Move the cursor to the data to be cleared.
3 Press horizontal soft key [DELETE].
4 Press horizontal soft key [EXEC].
Clearing all data
1 Display the operation history signal selection screen.
2 Press horizontal soft key [ALLDEL].
3 Press horizontal soft key [EXEC].
Fig. 12.4.30.4 (a) Operation history signal selection screen
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1877 -
12.4.30.5 Outputting all history data
All history data can be output to external input/output devices.
It is impossible, however, to output history data individually.
Procedure
1 Make an output device ready for output.
2 Set the EDIT mode.
3 Press function key .
4 Press vertical soft key [NEXT PAGE] several times until vertical
soft key [OPERAT HISTRY] is displayed.
5 Press vertical soft key [OPERAT HISTRY], then press newly
displayed vertical soft key [OPERAT HISTRY]. The operation
history screen is displayed.
7 Press horizontal soft key [PUNCH].
8 Enter a file name, and press horizontal soft key [EXEC].
When horizontal soft key [EXEC] is pressed without entering a
file name, the output file name is assumed to be OPRT_HIS.TXT.
Output format
History data is output as an ASCII file in the following format:
1 MDI keys
After "MDI", "path-number_", "key-data", and "input-time" are
output in this order.
(Key data input at power-on is indicated as "Power on MDI".)
<Example>
MDI 01_A 12:23:34
MDI 02_<CAN> 12:23:34
MDI 02_[SOFT HF1] 12:23:35
MDI P_<RESET> 12:34:56
Power on MDI 01_<RESET> 12:34:56
2 I/O signals
After "DI/DO", "PMC-number_", "signal-address_bit-status",
and "time-of-change" are output in this order.
<Example>
DI/DO 1_F0002.2_on 12:34:56
DI/DO 1_ G0043.0_off G0043.1_off 12:35:00
(For multiple bits at the same address)
3 Alarms
After "Alarm", "path-number_", "type", "alarm-number",
"G-code-modal-data", "modal-data-other-than-G-code",
"absolute-coordinate-value" and "machine-coordinate-value" for
each axis, and "date-and-time-of-alarm-issuance" are output in
this order.
An asterisk "*" is output before the modal data that was specified
in a block executed when the alarm was issued.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1878 -
<Example>
• Alarm 01_SR01973
*G0. G97. G69. G99. G21. G50.2 G25. G13.1 B0. D0. E0.
*F100. H0. M10. *N123. Test_ S1000. T1010.
X1 ABS 197.999 MCN 197.999 Y1 ABS -199806.00 MCN
-199806.00 Z1 ABS 297.009 MCN 0.123 C1 ABS
10395.999 MCN 0.000 at 2007/09/01 19:03:28
• Alarm 02_ OT00506(ZA2)
*G1. G17. G90. G22. G94. G20. *G42. G49. G80. G12.1
B0. *D12. E0. *F100. H34. M0. *N123. O123 S0. T0.
X2 ABS 123.999 MCN 234.000 Y2 ABS -123.00 MCN
-234.00 ZA2 ABS 1234.567 MCN –1234.567 at 2007/09/01
12:34:56
• When additional information is not to be recorded when an
alarm is issued (bit 7 (HAL) of parameter No. 3196 is set to
1), only "path-number_", "alarm-number", and
"date-and-time-of-alarm-issuance" are output.
Alarm 01_OT00506(XC1) at 2007/09/01 22:08:32
Alarm 02_SW00100 at 2007/09/01 19:07:52
• When external alarm/macro alarm messages are to be
recorded (bit 7 (HAL) of parameter No. 3196 is set to 0)
and bit 3 (EAH) of parameter No. 3112 is set to 1, the
messages are also output.
Alarm 01_MC00001 Message ATC ALARM
G0. G97. G69. G99. G21. G40. G25. G22. G80. D0. E0.
F0. H0. M0. N0. O9999 S0. T0.
X2 ABS 10.000 MCN 0.000Y2 ABS 123.000 MCN
0.000Z2 ABS 0.000 MCN 0.000 at 2007/09/01 10:06:43
4 External operator messages
After "EXT_Message", "message-number", "message", and
"date-and-time-of-issuance" are output in this order.
<Example>
EXT_Message 01234 OIL PRESSURE DECREASE at
2007/09/01 2:38:43
5 Modification of tool offset data
After "Tool Offset", "path-number_", "type", "offset-number",
"offset-data-before-modification",
"offset-data-after-modification", and "time-of-modification" are
output in this order. The following types are provided:
Common
to M/T
: G=Geometric
compensation
W=Wear
compensation
M series : H=Tool
length
compensation
D=Cutter
compensation
T series : R=Tool-nose
radius
compensation
T=Tool nose
direction
X2,Z2,Y2=Second geometric compensation
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1879 -
<Example>
Tool Offset 01_X0002 0.000 → 1 at 12:15:43
Tool Offset 02_XW0001 -9999.999 → 9999.999 at
12:15:46
Tool Offset 01_RG0032 0.000 → 0.003 at 12:15:52
Tool Offset 02_T0001 5. → 2. at 19:34:11
Tool Offset 02_W0123 -10.000 → 123.456 at 10:28:58
Tool Offset 01_HG0456 0.000 → 999.999 at 11:37:40
Tool Offset 01_ 0064 12.340 → 12.569 at 11:39:42
6 Modification of workpiece offset/extended workpiece
offset/workpiece shift (T series) data
After "Work Offset", "EXT Work Offset", or "Work Shift",
"path-number_(axis-name)", "type", "offset-number",
"offset-data-before-modification",
"offset-data-after-modification", and "time-of-modification" are
output in this order.
<Example>
Work Offset 01_G55(XA1) 15.000 → 0.007 at 09:23:03
Work Offset 02_EXT(Z2) 0.000 → 300.003 at 09:22:50
EXT Work Offset 02_G54.1P300 (Y2) 123.456 →
9999.999 at 12:15:46
Work Shift (X) 02_999999.999 → 999999.999 at 10:22:37
7 Modification of parameters
After "Parameter", "type", "parameter-number",
"parameter-before-modification", "parameter-after-modification",
and "time-of-modification" are output in this order.
The following types are provided:
Path type : L is added before the path number.
Axis type : A is added before the axis number.
Spindle type : S is added before the spindle number.
Machine group type : Indicated as the machine type. T is added
before the machine group number.
Others : No type is output.
<Example>
Paramater N03112 00000100 → 00001100 at
11:18:40
Paramater Path type N01410 L02 0.000 → 1000.000
at 18:58:48
Paramater Axis type N01423 A04(B2) 0.000 →
10000.000 at 18:58:48
Paramater Spindle type N04011 S1(S) 10011010 →
10011010 at 18:58:53
Paramater Machine type N06310 T01 0 → -32768 at
19:21:13
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1880 -
8 Modification of custom macro common variables (#100 to #999)
After "Macro variable", "path-number_", "#variable-number",
"common-variable-value-before-modification",
"common-variable-value-after-modification", and
"time-of-modification" are output in this order.
Variable values are output in the data format M × (10**(-E)).
<Example>
• When #149 on the first path was modified from <empty> to
12.345
Macro valiable 01_#149 Empty → 123450000*(10**-7) at
15:02:35
• When #549 on the second path was modified from -12.345
to 123456789012
Macro valiable 02_#549 -123450000*(10**-7)
→123456789*(10**3) at 15:03:27
9 Date and time
Power on at 2007/09/01 17:11:17 (Date and time of
power-on)
Power off at 2007/09/01 17:49:17 (Date and time of
power-off)
Date 2007/09/01 00:00:00 (Record indicating a
change in date)
Time stamp at 2007/09/01 15:51:00 (Record at regular
intervals)
Data delete at 2007/09/01 10:56:18 (Date and time when
history data was deleted)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1881 -
12.5 SCREENS DISPLAYED BY FUNCTION KEY
By pressing the function key , data such as alarms, and alarm
history data can be displayed.
For information relating to alarm display, see Section III-7.1. For
information relating to alarm history display, see Section III-7.2.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1882 -
12.6 DISPLAYING THE PROGRAM NUMBER/NAME,
SEQUENCE NUMBER, AND STATUS, AND WARNING
MESSAGES FOR DATA SETTING OR INPUT/OUTPUT
OPERATION
The program number, program name, sequence number, and current
CNC status are always displayed on the screen except when the power
is turned on, a system alarm occurs.
If data setting or the input/output operation is incorrect, the CNC does
not accept the operation and displays a warning message.
This section describes the display of the program number, sequence
number, and status, and warning messages displayed for incorrect data
setting or input/output operation.
Screens of a 10.4-inch display unit
12.6.1 Displaying the Program Number, Program Name, and
Sequence Number
The number and name of the program currently selected or currently
executed and the current sequence number are indicated in the upper
right part as shown below.
Fig. 12.6.1 (a) Program number and sequence number (10.4-inch)
In the EDIT mode, the number and name of the program currently
edited in the foreground are indicated.
Sequence number
Program numbe
r
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1883 -
12.6.2 Displaying the Status and Warning for Data Setting or
Input/Output Operation
The current mode, automatic operation state, alarm state, and program
editing state are displayed on the next to last line on the screen
allowing the operator to readily understand the operation condition of
the system. If data setting or the input/output operation is incorrect,
the CNC does not accept the operation and a warning message is
displayed on the next to last line of the screen. This prevents invalid
data setting and input/output errors.
Explanation
- Description of each display
Fig. 12.6.2 (a) Positions of status indications
(1) Current mode
MDI : Manual data input, MDI operation
MEM : Automatic operation (memory operation)
RMT : Automatic operation (DNC operation, or such like)
EDIT : Memory editing
HND : Manual handle feed
JOG : Jog feed
INC : Manual incremental feed
REF : Manual reference position return
**** : Mode other than the above
(2) Automatic operation status
**** : Reset (When the power is turned on or the state in
which program execution has terminated and automatic
operation has terminated.)
STOP : Automatic operation stop (The state in which one block
has been executed and automatic operation is stopped.)
HOLD : Feed hold (The state in which execution of one block
has been interrupted and automatic operation is
stopped.)
STRT : Automatic operation start-up (The state in which the
system operates automatically)
(1)
(2) (3) (4)
(5) :
(5) is displayed in the
area for (3) and (4).
(7) (8)
(10) :
(10) is displayed at the position
where (8) is now displayed.
(9)
(6)
DATA IS OUT OF RANGE
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1884 -
MSTR : Manual numerical command start state (The state in
which a manual numerical command is being executed)
Alternatively, tool retract and recover operation state
(The state in which a recover operation and
repositioning operation are being performed)
(3) Axis moving status/dwell status
MTN : Indicates that the axis is moving.
DWL : Indicates the dwell state.
*** : Indicates a state other than the above.
(4) State in which an auxiliary function is being executed
FIN : Indicates the state in which an auxiliary function is
being executed. (Waiting for the complete signal from
the PMC)
*** : Indicates a state other than the above.
(5) Emergency stop or reset status
-
-EMG-- : Indicates emergency stop.(Blinks in reversed display.)
-
RESET- : Indicates that the reset signal is being received.
(6) Alarm status
ALM : Indicates that an alarm is issued. (Blinks in reversed
display.)
BAT : Indicates that the voltage of the lithium battery (the
backup battery of the CNC) has decreased. (Blinks in
reversed display.)
APC : Indicates that the voltage of the backup battery of the
absolute pulse coder has decreased. (Blinks in reversed
display.)
FAN : Indicates that the rotation speed of the fan has
decreased. (Blinks in reversed display.)
Space : Indicates a state other than the above.
(7) Current time
hh : mm : ss - Hours, minutes, and seconds
(8) Program editing status
INPUT : Indicates that data is being input.
OUTPUT : Indicates that data is being output.
SEARCH : Indicates that a search is being performed.
EDIT : Indicates that another editing operation is being
performed (insertion, modification, etc.)
LSK : Indicates that labels are skipped when data is input.
RSTR : Indicates that the program is being restarted
COMPARE : Indicates that a data comparison is being made.
OFST : Indicates that the tool length compensation amount
measurement mode is set (for the machining center
system) or that the tool length compensation
amount write mode is set (for the lathe system).
WOFS : Indicates that the workpiece origin offset amount
measurement mode is set.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1885 -
AICC1 : Indicates that operation is being performed in the AI
contour control I mode.
AICC2 : Indicates that operation is being performed in the AI
contour control II mode.
MEM-CHK : Indicates that a program memory check is being
made.
WSFT : Indicates that the workpiece shift amount write
mode is set.
LEN : Indicates that the active offset value change mode
(tool length offset value of the M series) is set.
RAD : Indicates that the active offset value change mode
(tool radius compensation amount of the M series)
is set.
WZR : Indicates that the active offset value change mode
(workpiece origin offset value) is set.
TOFS : Indicates that the active offset value change mode
(tool offset value of the T series) is set.
OFSX : Indicates that the active offset value change mode
(X-axis tool offset value of the T series) is set.
OFSZ : Indicates that the active offset value change mode
(Z-axis tool offset value of the T series) is set.
OFSY : Indicates that the active offset value change mode
(Y-axis tool offset value of the T series).
TCP : Indicates that operation is being performed in the
tool center point control.
TWP : Indicates that operation is being performed in the
tilted working plane command mode.
Space : Indicates that no editing operation is being
performed.
(9) Warning for data setting or input/output operation
When invalid data is entered (wrong format, value out of range, etc.),
when input is disabled (wrong mode, write disabled, etc.), or when
input/output operation is incorrect (wrong mode, etc.), a warning
message is displayed. In this case, the CNC does not accept the setting
or input/output operation (retry the operation according to the
message).
Example 1)
When a parameter is entered
Example 2)
When a parameter is entered
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1886 -
Example 3)
When a parameter is output to an external input/output device
(10) Tool post name
The number of a path whose status is indicated is displayed.
PATH1 : Indicates that the status being indicated is for path 1.
Other names can be used depending on the settings of
parameters 3141 to 3147. The tool post name is displayed
at the position where (8) is now displayed. While the
program is edited, (8) is displayed.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1887 -
Screens of a 15-inch display unit
12.6.3 Displaying the Program Number, Program Name, and
Sequence Number (15-inch Display Unit)
The number and name of the program currently selected or currently
executed and the current sequence number are indicated in the upper
right part as shown below.
Fig. 12.6.3 (a) Program number and sequence number (15-inch)
In the EDIT mode, the number and name of the program currently
edited in the foreground are indicated.
Sequence number
Program numbe
r
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1888 -
12.6.4 Displaying the Status and Warning for Data Setting or
Input/Output Operation (15-inch Display Unit)
The current mode, automatic operation state, alarm state, and program
editing state are displayed on the next to last line on the screen
allowing the operator to readily understand the operation condition of
the system. If data setting or the input/output operation is incorrect,
the CNC does not accept the operation and a warning message is
displayed on the next to last line of the screen. This prevents invalid
data setting and input/output errors.
Explanation
- Description of each display
Fig. 12.6.4 (a) Positions of status indications
(1) Current mode
MDI : Manual data input, MDI operation
MEM : Automatic operation (memory operation)
RMT : Automatic operation (DNC operation, or such like)
EDIT : Memory editing
HND : Manual handle feed
JOG : Jog feed
INC : Manual incremental feed
REF : Manual reference position return
**** : Mode other than the above
(2) Automatic operation status
**** : Reset (When the power is turned on or the state in
which program execution has terminated and automatic
operation has terminated.)
STOP : Automatic operation stop (The state in which one block
has been executed and automatic operation is stopped.)
HOLD : Feed hold (The state in which execution of one block
has been interrupted and automatic operation is
stopped.)
STRT : Automatic operation start-up (The state in which the
system operates automatically)
(1)
(2) (3) (4)
(5) :
(5) is displayed in the
area for (3) and (4).
(7) (8)
(10) :
(10) is displayed at the position
where (8) is now displayed.
(6)
(9)
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1889 -
MSTR : Manual numerical command start state (The state in
which a manual numerical command is being executed)
Alternatively, tool retract and recover operation state
(The state in which a recover operation and
repositioning operation are being performed)
(3) Axis moving status/dwell status
MTN : Indicates that the axis is moving.
DWL : Indicates the dwell state.
*** : Indicates a state other than the above.
(4) State in which an auxiliary function is being executed
FIN : Indicates the state in which an auxiliary function is
being executed. (Waiting for the complete signal from
the PMC)
*** : Indicates a state other than the above.
(5) Emergency stop or reset status
-
-EMG-- : Indicates emergency stop.(Blinks in reversed display.)
-
RESET- : Indicates that the reset signal is being received.
(6) Alarm status
ALM : Indicates that an alarm is issued. (Blinks in reversed
display.)
BAT : Indicates that the voltage of the lithium battery (the
backup battery of the CNC) has decreased. (Blinks in
reversed display.)
APC : Indicates that the voltage of the backup battery of the
absolute pulse coder has decreased. (Blinks in reversed
display.)
FAN : Indicates that the rotation speed of the fan has
decreased. (Blinks in reversed display.)
Space : Indicates a state other than the above.
(7) Current time
hh : mm : ss - Hours, minutes, and seconds
(8) Program editing status
INPUT : Indicates that data is being input.
OUTPUT : Indicates that data is being output.
SEARCH : Indicates that a search is being performed.
EDIT : Indicates that another editing operation is being
performed (insertion, modification, etc.)
LSK : Indicates that labels are skipped when data is input.
RSTR : Indicates that the program is being restarted
COMPARE : Indicates that a data comparison is being made.
OFST : Indicates that the tool length compensation amount
measurement mode is set (for the machining center
system) or that the tool length compensation
amount write mode is set (for the lathe system).
WOFS : Indicates that the workpiece origin offset amount
measurement mode is set.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1890 -
AICC1 : Indicates that operation is being performed in the AI
contour control I mode.
AICC2 : Indicates that operation is being performed in the AI
contour control II mode.
MEM-CHK : Indicates that a program memory check is being
made.
WSFT : Indicates that the workpiece shift amount write
mode is set.
LEN : Indicates that the active offset value change mode
(tool length offset value of the M series) is set.
RAD : Indicates that the active offset value change mode
(tool radius compensation amount of the M series)
is set.
WZR : Indicates that the active offset value change mode
(workpiece origin offset value) is set.
TOFS : Indicates that the active offset value change mode
(tool offset value of the T series) is set.
OFSX : Indicates that the active offset value change mode
(X-axis tool offset value of the T series) is set.
OFSZ : Indicates that the active offset value change mode
(Z-axis tool offset value of the T series) is set.
OFSY : Indicates that the active offset value change mode
(Y-axis tool offset value of the T series).
TCP : Indicates that operation is being performed in the
tool center point control.
TWP : Indicates that operation is being performed in the
tilted working plane command mode.
Space : Indicates that no editing operation is being
performed.
(9) Warning for data setting or input/output operation
When invalid data is entered (wrong format, value out of range, etc.),
when input is disabled (wrong mode, write disabled, etc.), or when
input/output operation is incorrect (wrong mode, etc.), a warning
message is displayed. In this case, the CNC does not accept the setting
or input/output operation (retry the operation according to the
message).
Example 1)
When a parameter is entered
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1891 -
Example 2)
When a parameter is entered
Example 3)
When a parameter is output to an external input/output device
(10) Tool post name
The number of a path whose status is indicated is displayed.
PATH1 : Indicates that the status being indicated is for path 1.
Other names can be used depending on the settings of
parameters 3141 to 3147. The tool post name is displayed
at the position where (8) is now displayed. While the
program is edited, (8) is displayed.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1892 -
12.7 SCREEN ERASURE FUNCTION AND AUTOMATIC
SCREEN ERASURE FUNCTION
Overview
Keeping the same characters displayed in the same positions on the
screen for a long time will shorten the life of the LCD.
To prevent this, the CNC screen can be erased. The screen erasure
function allows the user to perform a key operation to erase the screen.
The automatic screen erasure function erases the screen automatically
when there has been no key operation for a parameter-set period of
time.
Screen erasure function
When 0 is set in parameter No. 3123, the CNC screen can be erased
by pressing the key and any function key (such as or
) at the same time. The CNC screen can be displayed again by
pressing any function key.
Automatic screen erasure function
When there has been no key operation for a time (in minutes) set in
parameter No. 3123, the CNC screen is erased automatically. The
CNC screen is displayed again by pressing a key.
- Screen erasure by the automatic screen erasure function
If the following conditions are all satisfied for the time (in minutes)
set in parameter No. 3123, the CNC screen is erased.
Conditions for automatically erasing the CNC screen
• Parameter No. 3123 ≠ 0
• None of the following key operations is performed.
MDI keys
Soft keys
External key input
• No alarm is issued.
- Redisplay of the screen by the automatic screen erasure function
If one of the following conditions is satisfied when the CNC screen is
off, the CNC screen is displayed again:
Conditions for redisplaying the CNC screen
• One of the following key operations is performed.
MDI keys
Soft keys
External key input
• An alarm is issued.
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1893 -
- Screen erasure by using the key + function key
When a non-zero value is set in parameter No. 3123, the screen is not
erased with the key and a function key.
- Set time
Only the time set in parameter No. 3123 for path 1 is valid.
- Alarm in another path
When an alarm is issued in any of the paths, the screen is not erased.
Parameter
3123 Time required before a screen saver is activated
[Input type] Setting input
[Data type] Byte path
[Unit of data] min
[Valid data range] 0 to 127
After a time (in minutes) set in parameter No. 3123 passes without key
operation, the NC screen is erased automatically. Pressing a key
causes the NC screen to reappear.
NOTE
1 Setting 0 disables automatic screen erasure.
2 This function cannot be used together with manual
screen erasure. If 1 or a larger value is set in this
parameter, manual screen erasure is disabled.
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1894 -
12.8 LOAD METER SCREEN
Overview
The servo and spindle load meters can be displayed in place of the
modal code display part and the remaining travel distance part of the
current position display on the program check screen.
This function is enabled only when the 10.4-inch display unit is used.
12.8.1 Single-Path Display
Screen layout
In the single-path display mode, the servo or spindle load meter is
displayed in place of the remaining travel distance display of the total
position display.
Fig. 12.8.1.(a) Servo load meter
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1895 -
Fig. 12.8.1 (b) Spindle load meter
Screen switching
The servo load meter and spindle load meter are displayed by pressing
soft key [MONITOR] on the left side of the screen. Initially the servo
load meter is displayed. Each time soft key [MONITOR] is pressed,
the servo load meter and spindle load meter alternate.
Servo load meter Spindle load meter
Switched by pressing soft key [MONITOR]
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1896 -
12.8.2 Two-Path Display and Three-Path Display
Screen layout
In the two- or three-path display mode, the modal information display
part on the program check screen can be replaced by the servo or
spindle load meter.
Fig. 12.4.30.5 (a) Servo load meter screen
Fig. 12.4.30.5 (a) Spindle load meter screen
B-63944EN/03 OPERATION 12.SETTING AND DISPLAYING DATA
- 1897 -
Screen switching
By pressing soft key [LOAD METER], the screen display can be
switched among the modal information display, servo load meter
display, and spindle load meter display.
Modal information
Press soft key [LOAD METER].
Spindle load meter
Press soft key [LOAD METER].
Servo load meter
Press soft key [LOAD METER].
12.SETTING AND DISPLAYING DATA OPERATION B-63944EN/03
- 1898 -
Parameter
#7 #6 #5 #4 #3 #2 #1 #0
3192 PLD
[Input type] Parameter input
[Data type] Bit
# 7 PLD When the current position is indicated for a path, and when the
program check screen is displayed in a two- or three-path system, the
function for displaying servo load meters and spindle load meters is :
0: Disabled.
1: Enabled.
13140 First character in spindle load meter display
13141 Second character in spindle load meter display
[Input type] Setting input
[Data type] Byte spindle
[Valid data range] These parameters set character codes to set the name of each spindle
that appears in spindle load meter display. Any character string
consisting of numeric characters, alphabetical characters, katakana
characters, and symbols with a maximum length of two characters can
be displayed as a spindle name.
If 0 is set, the following is displayed:
1st spindle S1
2nd spindle S2
3rd spindle S3
4th spindle S4
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1899 -
13 GRAPHIC FUNCTION
Chapter 13, "GRAPHIC FUNCTION", consists of the following
sections:
13.1 GRAPHIC DISPLAY...........................................................1900
13.2 DYNAMIC GRAPHIC DISPLAY.......................................1913
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1900 -
13.1 GRAPHIC DISPLAY
The graphic display functions enable drawing of the tool path of the
program currently used for machining.
These functions are intended to display the movement of the tool
during automatic operation or during manual operation.
This enables the operator to check the progress of machining and the
current tool position.
These functions include the following:
• The current tool position in the workpiece coordinate system is
displayed.
• Graphic coordinates can be set freely.
• Rapid traverse and cutting feed can be drawn using a different
color for each.
• The values of F, S, and T in the program during drawing are
displayed.
• Graphic enlargement or reduction is possible.
Graphic display procedure
Explanation
Press the function key then press the [GRAPH] soft key to
display the tool path graphic screen.
- Tool path graphic screen
The tool path graphic screen consists of three major areas:
• Graphic area for drawing a tool path
• Area for displaying machining information such as tool position
information
• Area for displaying a graphic coordinate system
Fig. 13.1 (a) Tool path graphic screen (M series)
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1901 -
Fig. 13.1 (b) Tool path graphic screen (T series)
- Tool path
In a graphic coordinate system set by the graphic parameters described
later, a tool path in the workpiece coordinate system is drawn.
Even when the tool position changes discontinuously for a cause such
as the setting of the origin and the switching of the workpiece
coordinate system, drawing is performed assuming that the tool has
moved.
A tool path is continuously drawn even when the screen display is
changed to another screen.
- Machining information
On the right side of the screen, the positions (along only three axes
used for drawing) in the workpiece coordinate system, feedrate (F),
spindle speed (S), and tool number (T) are displayed.
NOTE
Up to three graphic axes are used with the M
series, and up to two graphic axes are used with
the T series.
- Graphic coordinate system
On the lower-right portion of the screen, the coordinate axes and axis
names of the graphic coordinate system are displayed.
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1902 -
Graphic parameter screen
Explanation
Press the function key then press the [PARAM] soft key to
display the tool path graphic screen.
On the graphic parameter screen, make settings necessary for drawing
a tool path.
The graphic parameter screen consists of three pages.
M
- Graphic parameter screen page 1
Fig. 13.1 (c) Graphic parameter screen page 1
On graphic parameter screen page 1, a graphic coordinate system,
graphic range, and so forth are set.
In the setting of a graphic coordinate system, the coordinate axes and
axis names of the set coordinate system are graphically displayed.
When a three-dimensional coordinate system is displayed, a rotation
angle is also displayed.
A graphic range is set using one of two methods. One method sets a
graphic scale and graphic center coordinates. The other sets the
maximum values and minimum values of a graphic range.
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1903 -
- Graphic parameter screen page 2
Fig. 13.1 (d) Graphic parameter screen page 2
On graphic parameter screen page 2, graphic colors, rotation angles,
and whether to perform automatic erase operation are set.
- Graphic parameter screen page 3
Fig. 13.1 (e) Graphic parameter screen page 3
On graphic parameter screen page 3, coordinate axes to be used for
drawing are set.
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1904 -
T
- Graphic parameter screen page 1
Fig. 13.1 (f) Graphic parameter screen page 1
On graphic parameter screen page 1, a graphic coordinate system,
graphic range, and so forth are set.
In the setting of a graphic coordinate system, the coordinate axes and
axis names of the set coordinate system are graphically displayed.
When a three-dimensional coordinate system is displayed, a rotation
angle is also displayed.
A graphic range is set using one of two methods. One method sets a
graphic scale and graphic center coordinates. The other sets the
maximum values and minimum values of a graphic range.
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1905 -
- Graphic parameter screen page 2
Fig. 13.1 (g) Graphic parameter screen page 2 (T series)
On graphic parameter screen page 2, graphic colors and whether to
perform automatic erase operation are set.
- Graphic parameter screen page 3
Fig. 13.1 (h) Graphic parameter screen page 3
On graphic parameter screen page 3, coordinate axes to be used for
drawing are set.
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1906 -
Graphic parameter setting
Explanation
For tool path drawing, a graphic coordinate system, tool path graphic
colors, and graphic range need to be set on the graphic parameter
screen.
The graphic parameters to be set on the graphic parameter screen are
described below.
When a value is set for a parameter, the parameter value becomes
immediately effective. If a tool path is already drawn, the tool path
is cleared when new parameter values are set.
- Graphic coordinate system
Select a desired graphic coordinate system for tool path drawing then
set the corresponding number.
M
Y
X
0. XY Z
Y
1. YZ Y
Z
2. ZY
Z
X
3. XZ 4. XYZZ
XY
5. ZXYY
Z X
Fig. 13.1 (i) Graphic coordinate system (M series)
T
Setting = 0 Setting = 1 Setting = 2 Setting = 3
Setting = 4 Setting = 5 Setting = 6 Setting = 7
X
Z
Z
Z
Z
Z
Z
Z
Z
X
X
X
X
X
X
X
Fig. 13.1 (j) Graphic coordinate system (T series)
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1907 -
M
- Horizontal rotation angle
When a three-dimensional graphic coordinate system such as 4.XYZ
or 5.ZXY is selected, the coordinate system can be rotated with the
horizontal plane used as the rotation plane. Set a rotation angle from
-360° to +360°.
The initial rotation angle can be set with parameter No. 24831, and the
actual rotation angle is equal to the "initial rotation angle + specified
rotation angle".
In Fig. 13.1 (k) below, the graphic coordinate system XYZ is
converted to X”Y”Z” by the following settings:
Initial rotation angle: 180°
Horizontal rotation angle: 30°
Y X
Z
180°
X' Y'
X"
Y"
Horizontal
rotation plane
30°
Fig. 13.1 (k) Coordinate system rotation in horizontal direction
- Vertical rotation angle
When a three-dimensional coordinate system such as 4.XYZ or
5.ZXY is selected, the coordinate system can be rotated with an axis
on the horizontal plane specified as a vertical rotation axis. Set a
rotation angle from -360° to +360°.
A vertical rotation axis can be set with the angle with the horizontal
axis of the screen on the horizontal plane. This angle can be set with
parameter No. 24832.
In Fig. 13.1 (l) below, the graphic coordinate system XYZ is
converted to X'Y'Z' by the following settings:
Rotation angle of the vertical rotation axis: 65°
Vertical rotation angle: 20°
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1908 -
Y X
Z
X'
Z'
Vertical rotation axis
rotation plane
Initial vertical
rotation axis
Vertical rotation
plane 20°
65°
Y'
Vertical rotation
axis
Fig. 13.1 (l) Coordinate system rotation in vertical direction
- Graphic color
Set a graphic color number for a tool path for each of cutting feed and
rapid traverse.
1: Red 2: Green 3: Yellow 4: Blue
5: Purple 6: Sky blue 7: White
- Graphic range setting
Set a graphic range so that a tool path can be drawn in the tool path
graphic area. Two methods are available:
1. Method that sets graphic center coordinates and a scale
2. Method that sets the maximum values and minimum values of a
graphic range
Whether method 1 or method 2 is used is determined by which
parameters were set most recently. A set graphic range is preserved
even if the power is turned off.
1. Method that sets graphic center coordinates and a scale
Set the coordinates of the center of a tool path graphic area in the
workpiece coordinate system. Then, set a scale used to contain the
graphic range in the tool path graphic area.
Set a scale value from 0.01 to 100 (magnification).
As a smaller scale is set, a tool path can be drawn in a wider range.
As a larger scale is set, a tool path is drawn by enlarging the tool path
around the graphic center coordinates.
2. Method that sets the maximum values and minimum values of a graphic range
Set the maximum coordinates and minimum coordinates of a desired
graphic range in the workpiece coordinate system. Drawing is
performed so that the specified entire range is contained in the tool
path graphic area.
From set maximum values and minimum values, graphic center
coordinates and a sale are automatically calculated to update the
graphic center coordinates and scale on the graphic parameter screen.
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1909 -
When a scale is automatically determined, the scale is clamped to
within the range 0.01 to 100. Moreover, a maximum value must be
greater than the corresponding minimum value.
NOTE
When the maximum values and minimum values of
a graphic range are set, the graphic center
coordinates and scale are automatically updated.
However, when the graphic center coordinates and
scale are changed, the maximum values and
minimum values of the graphic range are not
automatically updated.
- Automatic erasure
Before drawing is started, the previous drawing can be erased
automatically.
1: Immediately before drawing is started, the previous drawing is
erased automatically.
0: The previous drawing is not erased automatically.
- Graphic axis number
Set which controlled axis to be assigned to which graphic axis.
For each controlled axis, set one of the following graphic axis
numbers:
First graphic axis: 1
Second graphic axis: 2
Third graphic axis: 3
Axis not used for drawing: 0
NOTE
1 When 0 is set for all controlled axes, it is assumed
that 1, 2, and 3 are set sequentially for the first to
the third controlled axes.
2 With the T series, a tool path is drawn along the
first and second graphic axes. No tool path is
drawn along the third graphic axis.
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1910 -
Operation for graphic parameter setting
Operation
- Moving the cursor
The cursor can be moved to a desired parameter by the page key
or and the cursor key , , , or .
With the cursor keys, however, you cannot move from page 1 or 2 to
page 3.
- Input of settings (absolute input)
Method 1
(1) Key in a value to be set.
(2) Press the [INPUT] soft key.
Method 2
(1) Key in a value to be set.
(2) Press the key.
- Input of settings (incremental input)
Method 1
(1) Key in a value to be incremented to or decremented from
the current setting.
(2) Press the [+INPUT] soft key.
Procedure for tool path drawing
Procedure
- Start of drawing
(1) Display the tool path graphic screen.
(2) Press the [START] soft key.
The state that enables the movement of the tool in automatic
operation or manual operation to be drawn is set.
Afterwards, tool path drawing continues even if another screen is
displayed.
(3) Start automatic operation or manual operation.
- End of drawing
(1) Display the tool path graphic screen.
(2) Press the [END] soft key.
Tool path drawing ends.
- Erasure of the drawing
(1) Press the [END] soft key to end drawing.
(2) Press the [CLEAR] soft key. The tool path drawn so far is
erased.
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1911 -
NOTE
1 Set the machine lock state to perform drawing only
without moving the tool.
2 When the feedrate is high, the tool path may not be
drawn correctly. In such a case, decrease the
feedrate by performing, for example, a dry run.
Enlarged/reduced display
On the tool path graphic screen, you can move the center position of
the tool path drawing or enlarge the tool path drawing while viewing
the drawn tool path.
If any of these operations is executed, the tool path already drawn is
cleared.
- Procedure for changing the graphic range by setting a graphic center and
magnification
The center position of drawing can be moved. At the same time, the
scale can also be changed. So, the tool path can be enlarged or
reduced at a desired new center position.
(1) Press the [SCALE] soft key then the [CENTER] soft key.
A yellow cursor appears at the center of the screen, and the soft
key display is changed.
(2) Move the yellow cursor to a new graphic center position by using
the cursor key , , , or .
(3) When changing the scale, key in a value from 0.01 to 100
(magnification) then press the [INPUT] soft key. An input
value is displayed at "SCALE" in the lower-right corner of the
screen.
When you press the [+INPUT] soft key, the current
magnification is incremented by an input value.
(4) Press the [EXEC] soft key to end the operation.
After this step, the setting for graphic movement is effective to
enable drawing with the new setting.
Before graphic movement After graphic movement
Fig. 13.1 (m) Graphic movement (magnification = 2.00）
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1912 -
- Procedure for changing the graphic range with a rectangle
A tool path can be drawn by enlarging a specified rectangular area.
(1) Press the [SCALE] soft key then the [RECTANGLE] soft key.
Two cursors, one in red and the other in yellow, appear at the
center of the screen, and the soft key display is changed.
(2) Move the yellow cursor by using the cursor key , ,
, or . The cursor to be moved can be switched by
pressing the [CURSOR UP/DOWN] soft key.
Move the two cursors to the diagonal points of a new rectangular
graphic range. A tool path is drawn next time so that the drawn
tool path is contained in this rectangular range.
(3) Press the [EXEC] soft key to end the operation.
After this step, the setting of graphic enlargement is effective to
enable drawing with the new setting.
Before graphic enlargement After graphic enlargement
Fig. 13.1 (n) Graphic enlargement
NOTE
1 To stop an enlargement/reduction operation, press
the [CANCEL] soft key.
2 Even if you perform an enlargement/reduction
operation, the tool path already drawn on the
screen is neither moved nor enlarged. The setting
for enlargement/reduction becomes effective
starting with tool path drawing after you press the
[EXEC] soft key.
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1913 -
13.2 DYNAMIC GRAPHIC DISPLAY
Overview
The dynamic graphic display function has two features:
• Path Drawing
The path of coordinates specified in a program is drawn on the
screen.
By displaying a travel path on the screen, the path can be
checked easily before performing machining actually.
• Animation
The figure of a workpiece to be machined by a programmed tool
movement is drawn.
By drawing the three-dimensional figure of a workpiece to be
machined in an animation-like way, the intermediate machining
process and final figure can be grasped easily.
When machining is performed according to a program, this function
can draw a tool path with another program.
This function performs drawing much faster than the graphic display
function based on automatic operation, so that a program check can be
made more swiftly.
This function is distinguished from automatic program operation as
indicated by the following terminology:
Automatic operation Operation performed for actual machining
Background operation Virtual operation performed for drawing
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1914 -
13.2.1 Path Drawing
Overview
The following tool path drawing screens are used to make various
settings and execute drawing:
• GRAPHIC PARAMETER (DYNAMIC GRAPHIC) screen
This screen is used to set data needed for tool path drawing.
• PATH GRAPHIC screen
This screen is used for tool path drawing.
• PATH GRAPHIC (TOOL POSITION) screen
This screen enables the position of the tool during operation to be
checked on the drawn tool path.
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1915 -
13.2.1.1 GRAPHIC PARAMETER (DYNAMIC GRAPHIC) screen
This screen is used to set graphic parameters needed for tool path
drawing.
Data set using this screen is made valid by displaying the PATH
GRAPHIC screen or executing drawing. If a tool path is already
drawn, the path is erased.
Graphic parameter data once set is preserved even if the power is
turned off.
Graphic Parameter (Dynamic Graphic) Screen Procedure
Procedure
1 Press the function key (or when a small MDI unit
is used) to display the GRAPHIC PARAMETER (DYNAMIC
GRAPHIC) screen.
Fig. 13.2.1.1 (a) GRAPHIC PARAMETER screen (first page)
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1916 -
Fig. 13.2.1.1 (b) GRAPHIC PARAMETER screen (second page)
2 Two screens are used for the GRAPHIC PARAMETER screen.
Use the MDI page keys to switch between the screens for display
of a desired setting item.
3 Move the cursor to a desired setting item with the MDI cursor
keys then key in a desired value with the numeric keys.
4 For direct input of the value set in step 3, press the key or
the [INPUT] soft key.
For incremental input of the value set in step 3, press the
[+INPUT] soft key.
For each setting item, see the explanation.
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1917 -
Explanation
The setting items on the GRAPHIC PARAMETER screen are
described below.
- Graphic coordinate system
Select a graphic coordinate system for drawing from the following and
set its number.
Y
X
Setting=0 (XY)
Z
Y
Setting=1 (ZY)
Z
Y
Setting=2 (YZ)
Z
X
Setting =3 (XZ)
Setting=5 (XYZ)
Z
XY
Setting=6 (YXZ)
Z
YX
X
Z
Setting=4 (ZX)
Setting=7 (YZX)
X
Y Z
Fig. 13.2.1.1 (c) Graphic coordinate system
- Scale
Set the scale factor for drawing in the range of 0.01 to 100.00 (times).
With a small scale factor, it is possible to draw within a wide range.
With a large scale factor, it is possible to draw in the vicinity of the
graphic center being enlarged.
- Graphic range center
To specify the center coordinates of a graphic range, set a coordinate
on each axis in the workpiece coordinate system of the program
executed for drawing.
NOTE
Set a coordinate on each axis in the machine
coordinate system in case of bit 3 (BGM) of
parameter No.11329=1.
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1918 -
- Blank figure
With a drawing program, set the figure, position, and dimensions of a
blank to be machined.
The graphic range where the blank figure is included in the drawing
area is automatically decided by the value set here.
NOTE
1 With a lathe system, no rectangular parallelepiped
can be set.
2 With a lathe system, the Y-axis, one of the basic
three axes, may not exist. In such a case, the
Y-axis for the reference position of a blank need
not be set.
3 When a figure or dimension is set, a scale value
and screen center coordinates are automatically
set as the initial graphic range values so that the
blank figure is located within the graphic range on
the screen. Until a modification is made to the
blank figure, dimension or the setting of the graphic
coordinate system, the graphic range is determined
by the set scale and screen center coordinates.
Figure
Select a type of blank figure from the following and set the
corresponding value:
Setting Figure
0 Column or cylinder
(parallel with the Z-axis)
1 Rectangular parallelepiped
Position
Set the reference position of a blank with coordinates (X,Y,Z) in the
workpiece coordinate system.
NOTE
Set the reference position of a blank with
coordinates (X,Y,Z) in the machine coordinate
system in case of bit 3 (BGM) of parameter
No.11329=1.
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1919 -
Dimensions
Set the dimensions of each type of blank figure as indicated below.
Type of
blank figure Dimension I Dimension J Dimension K
Rectangular
parallelepiped
Length in X-axis
direction
Length in Y-axis
direction
Length in Z-axis
direction
Column Diameter of
column 0 Length of
column
Cylinder Diameter of outer
circle of cylinder
Diameter of inner
circle of cylinder
Length of
cylinder
The relationship between the position and dimensions of a blank is
shown below.
ｖ
J
K
: Reference position (X,Y,Z)
I
X
Z
Y
X
Z
Y
I
J
K
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1920 -
- Rotation angle
Set a rotating angle of the graphic coordinate system that centers on
the graphic range center. The rotating angle is a range of -360°-+360°.
Set a rotating angle as a reference position (position of the rotating
angle 0°) on the indicated direction of each graphic coordinate system.
Vertical plane rotation angle
Set a rotating angle at the horizontal direction center in front of the
screen.
The rotation direction is as follows.
+ -
Rotation center
Horizontal plane rotation angle
Set a rotating angle at the vertical direction center in front of the
screen.
The rotation direction is as follows.
+
-
Rotation center
Screen center rotation angle
Set a rotating angle at the vertical direction center of the screen plane.
The rotation direction is as follows.
+ -
Rotation center
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1921 -
- Graphic color
Set colors to be used for tool path drawing.
The colors that can be set are indicated below together with their
setting values:
Graphic
color White Red Green Yellow Blue Purple Light
blue White
Setting
value 0 1 2 3 4 5 6 7
Path
Set colors to be used for a drawn tool path.
Tool position
Set a graphic cursor color to be used for PATH GRAPHIC (TOOL
POSITION) screen.
- Auto erase
When drawing is started with the [START] soft key from a state
where drawing is not being executed or is not stopped temporarily, the
previously drawn path can be erased.
Setting 0: The previously drawn path is not erased.
1: The previously drawn path is erased.
- Tool offset（Path）
For tool path drawing, whether to enable or disable the tool offset
function (tool length compensation, cutter/tool-noise radius
compensation) can be selected.
Setting 0: The tool offset function is enabled for drawing.
1: The tool offset function is disabled for drawing.
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1922 -
13.2.1.2 PATH GRAPHIC screen
The PATH GRAPHIC screen is used to draw a tool path. The
following operations can be performed:
• Starting/ending tool path drawing
• Rewind of a drawing target program
• Erasing a drawn tool path
The screen is composed of the following items:
(1) Drawing area
(2) Status display of Background operation
(3) Program name and sequence number for drawing execution
(4) Current coordinates (absolute coordinates)
(5) Feedrate and M/S/T/D code instruction information
(6) Graphic coordinate system
Fig. 13.2.1.2 (a) PATH GRAPHIC screen
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1923 -
Path Graphic Screen Procedure
Procedure
1 Press the function key (or when a small MDI unit
is used) to display the GRAPHIC PARAMETER (DYNAMIC
GRAPHIC) screen.
2 Press the [PATH EXEC] soft key. The PATH GRAPHIC
screen is displayed.
Fig. 13.2.1.2 (b) PATH GRAPHIC screen
3 Press the [(OPRT)] soft key. The soft keys for tool path
drawing are displayed.
Fig. 13.2.1.2 (c) PATH GRAPHIC screen (operation)
4 Press the continuous menu key to display the soft keys for
enlarging/reducing/moving the graphic range.
Fig. 13.2.1.2 (d) PATH GRAPHIC screen
(enlarging/reducing/moving the graphic range)
5 Press the [COORDINATES] soft key to display the soft keys for
changing the graphic coordinate system.
Fig. 13.2.1.2 (e) PATH GRAPHIC screen
(changing the graphic coordinate system)
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1924 -
6 Press the [ROTATION] soft key to display the soft keys for
rotating the graphic coordinate system.
Fig. 13.2.1.2 (f) PATH GRAPHIC screen
(rotating the graphic coordinate system)
For the operation of each soft key, see the explanation.
Explanation
- Graphic program selection
Press the [PRGRAM SELECT] soft key to select a drawing target
program.
Pressing the [PRGRAM SELECT] soft key displays the program list
screen.
On the program list screen, move the cursor to a desired program then
press the [DRAW SELECT] soft key.
Fig. 13.2.1.2 (g) Program list screen ([DRAW SELECT] soft key)
Pressing the [DRAW SELECT] soft key selects a drawing target
program and switches the screen display to the PATH GRAPHIC
screen.
The file whose name is prefixed by a "#" mark on the program list
screen is selected as the drawing target program. And the mark of "+"
is displayed in the file that has been selected as a program for drawing
in other path systems.
Fig. 13.2.1.2 (h) Program list screen (drawing target program selection
state)
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1925 -
NOTE
The file that can be selected as the drawing target
program is only a file that can be selected as the
main program.
- Rewind of a drawing target program
If the execution of drawing of a selected program has ended or is
stopped halfway, press the [REWIND] soft key to restart drawing
from the beginning of the program.
- Starting / Stopping drawing
To draw the tool path of a program selected for drawing, press one of
the following soft keys displayed by step 3 mentioned above:
• [START] soft key
This soft key starts drawing from the head of the program.
• [1BLOCK] soft key
This soft key executes the program for drawing and stops
temporarily on a block-by-block basis as with ordinary single
block stop operation.
If a program is executed with a soft key above, the soft key display is
changed to the following:
Fig. 13.2.1.2 (i) Soft keys displayed during drawing execution
The operations of these soft keys are as follows:
• [STOP] soft key
This soft key terminates the execution of the drawing target
program to stop drawing.
• [PAUSE] soft key
This soft key temporarily stops the execution of the drawing
target program to stop drawing temporarily.
• [1BLOCK] soft key
This soft key executes the program for drawing and stops
drawing temporarily on a block-by-block basis as with ordinary
single block stop operation.
• [RESTART] soft key
If the [RESTART] soft key is pressed in the stop state set by the
[PAUSE] soft key or the [1BLOCK] soft key, the execution of
drawing can be restarted from the block where drawing is
stopped.
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1926 -
NOTE
When the new path was drawn by the operation of
starting drawing without erasing of the old path
before the operation, it is impossible to redraw the
old path by each operation of
enlarging/reducing/moving the graphic range and
changing/rotating the graphic coordinate system.
The state of drawing is indicated as follows:
DRAWING: Indicates that drawing is being executed.
Fig. 13.2.1.2 (j) State indication during drawing
STOP: Indicates that drawing is temporarily stopped.
Fig. 13.2.1.2 (k) State indication during temporary stop
ALM: Indicates that occurring of alarm in the Background
operation.
Fig. 13.2.1.2 (l) State indication during occurring of alarm
- End of drawing
When M02 or M30 is executed, the program executed for drawing
terminates drawing.
Upon program termination, the soft key display returns to the soft
keys (Fig. 13.2.1.2 (c)) displayed before drawing is started.
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1927 -
- Erasing a drawn tool path
Press the [ERASE] soft key to erase a drawn tool path.
NOTE
1 If the screen display is switched or the path is
switched during tool path drawing, the background
operation is stopped to end drawing.
2 A tool path once drawn is erased when the screen
display is switched or the path is switched.
- Enlarging/reducing the graphic range
The following soft keys displayed by step 4 are used:
• [LARGE] soft key
This soft key increases the scale to enlarge the graphic range.
• [SMALL] soft key
This soft key decreases the scale to reduce the graphic range.
• [AUTO] soft key
When the blank figure specified in a graphic parameter is input,
this soft key automatically scales the graphic range so that the
blank figure is contained within the graphic range.
If no blank figure is input, this soft key has no effect.
NOTE
1 Set the unit of scale for one enlargement/reduction
operation in parameter No. 14713.
2 An enlargement/reduction scale used here is set in
the graphic parameter for scale.
- Moving the graphic range
The following soft keys displayed by step 4 are used:
• [←MOVE] soft key
This soft key moves the graphic range to left.
• [MOVE→] soft key
This soft key moves the graphic range to right.
• [↑MOVE] soft key
This soft key moves the graphic range upward.
• [↓MOVE] soft key
This soft key moves the graphic range downward.
• [CENTER] soft key
This soft key returns the graphic range to the original position.
NOTE
1 Set the travel increment made by one horizontal
move operation in parameter No. 14714.
2 Set the travel increment made by one vertical move
operation in parameter No. 14715.
3 The graphic range modified here is not set in the
graphic parameter for graphic range center.
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1928 -
- Changing the graphic coordinate system
The following soft keys displayed by step 5 are used.
A graphic coordinate system selected here is the same one as set in the
graphic parameter for the graphic coordinate system.
• [XY] soft key
This soft key selects the graphic coordinate system of XY (with a
setting of 0).
• [ZY] soft key
This soft key selects the graphic coordinate system of ZY (with a
setting of 1).
• [YZ] soft key
This soft key selects the graphic coordinate system of YZ (with a
setting of 2).
• [XZ] soft key
This soft key selects the graphic coordinate system of XZ (with a
setting of 3).
• [ZX] soft key
This soft key selects the graphic coordinate system of ZX (with a
setting of 4).
• [XYZ] soft key
This soft key selects the graphic coordinate system of XYZ (with
a setting of 5).
• [YXZ] soft key
This soft key selects the graphic coordinate system of YXZ (with
a setting of 6).
• [YZX] soft key
This soft key selects the graphic coordinate system of YZX (with
a setting of 7).
• [OK] soft key
This soft key changes the current graphic coordinate system to
the graphic coordinate system selected by one of the soft keys
above.
• [CANCEL] soft key
This soft key cancels the graphic coordinate system selected by
one of the soft keys above to return to the original graphic
coordinate system.
NOTE
The graphic coordinate system selected here is set
in the graphic parameter for the graphic coordinate
system.
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1929 -
- Rotating the graphic coordinate system
The following soft keys displayed by step 6 are used.
• [↑] soft key
This soft key rotates the graphic coordinate system upward.
• [↓] soft key
This soft key rotates the graphic coordinate system downward.
• [←] soft key
This soft key rotates the graphic coordinate system to left.
• [→] soft key
This soft key rotates the graphic coordinate system to right.
• [CW] soft key
This soft key rotates the graphic coordinate system clockwise.
• [CCW] soft key
This soft key rotates the graphic coordinate system
counterclockwise.
• [OK] soft key
This soft key changes the rotation angle of the current graphic
coordinate system to the one set by one of the soft keys above.
• [CANCEL] soft key
This soft key cancels the rotation of the graphic coordinate
system performed by one of the soft keys above to return to the
original graphic coordinate system.
NOTE
1 Set the travel increment made by one rotation
operation in parameter No. 14716.
2 The rotation angle of the graphic coordinate system
set here is not set in the graphic parameter for
rotation angle.
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1930 -
13.2.1.3 PATH GRAPHIC (TOOL POSITION) screen
The tool position during operation can be checked by displaying the
cursor for indicating the tool position during operation on the tool path
drawn on the PATH GRAPHIC (EXECUTION) screen.
The screen is composed of the following items:
(1) Drawing area
(2) Current coordinates (absolute coordinates)
(3) Feedrate and M/S/T/D code instruction information
(4) Graphic coordinate system
(5) Cursor to show tool position
Fig. 13.2.1.3 (a) PATH GRAPHIC (TOOL POSITION) screen
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1931 -
Path Graphic (Tool Position) Screen Procedure
Procedure
1 Press the function key (or when a small MDI unit
is used) to display the PATH GRAPHIC (PARAMETER) screen.
2 Press the [TOOL POS] soft key.
The screen display changes to the PATH GRAPHIC (TOOL
POSITION) screen and the cursor indicating the tool position is
displayed.
Fig. 13.2.1.3 (b) PATH GRAPHIC (TOOL POSITION) screen
For the method of checking the current tool position, see the
explanation.
Pressing a soft key other than the [TOOL POS] soft key displays
the corresponding screen.
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1932 -
Explanation
Use the following procedure to check the tool position during
operation on the PATH GRAPHIC (TOOL POSITION) screen:
(1) Select a drawing target program for operation.
(2) Draw the tool path of the selected program on the PATH
GRAPHIC screen.
(3) After the end of drawing, switch the screen display to the PATH
GRAPHIC (TOOL POSITION) screen.
(4) Start automatic operation with the program executed for tool path
drawing.
After automatic operation is started, the blinking cursor moves along
the drawn tool path as the tool moves. The cursor blinking rate is
fast when the tool is moving, and the cursor blinking rate is slow when
the tool is stopped.
The following items displayed on the screen are provided for the
program under automatic operation:
• Current coordinates
• Feedrate and M/S/T/D code specification information
NOTE
1 A tool path drawn by setting the tool offset
parameter to 1 (to disable the tool offset function) is
different from the actual tool path. In this case,
the cursor indicating the tool position may not move
along the drawn tool path.
2 The tool path cannot be drawn correctly if a
command not supporting drawing or a command
that specifies operation different from operation
performed during drawing is specified or if an
operation dependent on the operation state or
setting on the machine side is performed. So, the
tool path in actual operation may differ from a
drawn tool path. In this case, the cursor indicating
the tool position does not move along the drawn
tool path.
3 When the graphic parameter of the graphic
coordinate system, scale, graphic range center,
blank figure / position / dimensions and rotation
angle is changed, the drawn tool path drawn is
erased.
Therefore, please draw the tool path again on the
PATH GRAPHIC screen to display the tool position
by setting the changed graphic parameter.
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1933 -
13.2.2 Animation
Overview
For animation drawing, make necessary settings and perform
operations for drawing execution on the following screens:
• GRAPHIC PARAMETER (DYNAMIC GRAPHIC) screen
On this screen, data required to execute animation drawing can
be set.
• ANIMATION GRAPHIC screen
This screen is used for animation drawing.
On this screen, the graphic range can be reduced/enlarged, and
the graphic coordinate system can be rotated.
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1934 -
13.2.2.1 GRAPHIC PARAMETER (DYNAMIC GRAPHIC) SCREEN
This screen is used to set graphic parameters needed for animation
drawing.
Data set using this screen is made valid by displaying the
ANIMATION GRAPHIC screen or executing drawing.
Graphic parameter data once set is preserved even if the power is
turned off.
Graphic Parameter (Dynamic Graphic) Screen Procedure
Procedure
1 Press the function key (or when a small MDI unit
is used) to display the GRAPHIC PARAMETER (DYNAMIC
GRAPHIC) screen.
Fig. 13.2.2.1 (a) GRAPHIC PARAMETER screen (first page)
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1935 -
Fig. 13.2.2.1 (b) GRAPHIC PARAMETER screen (second page)
2 Two screens are used for the GRAPHIC PARAMETER screen.
Use the MDI page keys to switch between the screens for display
of a desired setting item.
3 Move the cursor to a desired setting item with the MDI cursor
keys then key in a desired value with the numeric keys.
4 For direct input of the value set in step 3, press the key or
the [INPUT] soft key.
For incremental input of the value set in step 3, press the
[+INPUT] soft key.
For each setting item, see the explanation.
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1936 -
Explanation
The setting items on the GRAPHIC PARAMETER screen are
described below.
However, the graphic parameters listed below are shared for tool path
drawing. So, refer to the explanation of the GRAPHIC
PARAMETER screen for tool path drawing.
• Graphic coordinate system
• Scale
• Graphic range center
• Rotation angles (vertical plane, horizontal plane, screen center)
- Blank figure
With a drawing program, set the figure, position, and dimensions of a
blank to be machined.
NOTE
1 With a lathe system, no rectangular parallelepiped
can be set.
2 With a lathe system, the Y-axis, one of the basic
three axes, may not exist. In such a case, the
Y-axis for the reference position of a blank need
not be set.
3 When a figure or dimension is set, a scale value
and screen center coordinates are automatically
set as the initial graphic range values so that the
blank figure is located within the graphic range on
the screen. Until a modification is made to the
blank figure, dimension or the setting of the graphic
coordinate system, the graphic range is determined
by the set scale and screen center coordinates.
Figure
Select a type of blank figure from the following and set the
corresponding value:
Setting Figure
0 Column or cylinder
(parallel with the Z-axis)
1 Rectangular parallelepiped
Position
Set the reference position of a blank with coordinates (X,Y,Z) in the
workpiece coordinate system.
NOTE
Set the reference position of a blank with
coordinates (X,Y,Z) in the machine coordinate
system in case of bit 3 (BGM) of parameter
No.11329=1.
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1937 -
Dimensions
Set the dimensions of each type of blank figure as indicated below.
Type of
blank figure Dimension I Dimension J Dimension K
Rectangular
parallelepiped
Length in X-axis
direction
Length in Y-axis
direction
Length in Z-axis
direction
Column Diameter of
column 0 Length of
column
Cylinder Diameter of outer
circle of cylinder
Diameter of inner
circle of cylinder
Length of
cylinder
The relationship between the position and dimensions of a blank is
shown below.
ｖ
J
K
: Reference position (X,Y,Z)
I
X
Z
Y
X
Z
Y
I
J
K
- Graphic color
Set colors to be used for animation drawing.
The colors that can be set are indicated below together with their
setting values:
Graphic
color White Red Green Yellow Blue Purple Light
blue White
Setting
value 0 1 2 3 4 5 6 7
Blank
Set the color of a blank to be drawn in animation drawing.
Tool
Set the color of a tool to be drawn in animation drawing.
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1938 -
- Tool length offset (Anime)
For animation drawing, whether to enable or disable the tool length
offset can be selected.
Setting 0: The tool length offset is disabled for drawing.
1: The tool length offset is enabled for drawing.
NOTE
In animation drawing, the cutter/tool-noise radius
compensation is always enabled for drawing.
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1939 -
13.2.2.2 ANIMATION GRAPHIC screen
The ANIMATION GRAPHIC screen is used to draw a animation.
The following operations can be performed:
• Starting/ending animation drawing
• Rewind of a drawing target program
• Initializing a blank
• Enlarging/reducing/moving the graphic range
• Rotating the graphic coordinate system
The screen configuration is as follows:
(1) Drawing area
(2) Status display of Background operation
(3) Program name and sequence number for drawing execution
(4) Current coordinates (absolute coordinates)
(5) Feedrate and M/S/T/D code instruction information
(6) Graphic coordinate system
(7) Material position, Material dimension, Scale, Graphic range
center of graphic Parameter
(8) Tool name
Fig. 13.2.2.2 (a) ANIMATION GRAPHIC screen
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1940 -
Animation Graphic Screen Procedure
Procedure
1 Press the function key (or when a small MDI unit
is used) to display the GRAPHIC PARAMETER (DYNAMIC
GRAPHIC) screen.
2 Press the [ANIME EXEC] soft key. The ANIMATION
GRAPHIC screen is displayed.
Fig. 13.2.2.2 (b) ANIMATION GRAPHIC screen
3 Press the [(OPRT)] soft key. The soft keys for tool path
drawing are displayed.
Fig. 13.2.2.2 (c) ANIMATION GRAPHIC screen (operation)
4 Press the continuous menu key to display the soft keys for
enlarging/reducing/moving the graphic range.
Fig. 13.2.2.2 (d) ANIMATION GRAPHIC screen
(enlarging/reducing/moving the graphic range)
5 Press the [COORDINATES] soft key to display the soft keys for
changing the graphic coordinate system.
Fig. 13.2.2.2 (e) ANIMATION GRAPHIC screen
(changing the graphic coordinate system)
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1941 -
6 Press the [ROTATION] soft key to display the soft keys for
rotating the graphic coordinate system.
Fig. 13.2.2.2 (f) ANIMATION GRAPHIC screen
(rotating the graphic coordinate system)
For the operation of each soft key, see the explanation.
Explanation
The operations listed below are the same operations as for the tool
path drawing screen. See the explanation of the tool path drawing
screen.
• Graphic program selection
• Rewind of a drawing target program
• Starting / Stopping of drawing
• End of drawing
- Initializing a blank
Press the [INIT.] soft key to initialize and return a drawn machining
profile to the original blank figure.
NOTE
1 Blank initialization can also be performed by any of
the following operations:
- Start of drawing
- Changing of the graphic coordinate system and
graphic range by performing
enlargement/reduction/movement/rotation
operations
- Change of screen
2 A machining profile once drawn for a blank is
erased when the screen or the path is switched.
- Enlarging/reducing the graphic range
The following soft keys displayed by step 4 are used:
• [LARGE] soft key
This soft key increases the scale to enlarge the graphic range.
• [SMALL] soft key
This soft key decreases the scale to reduce the graphic range.
• [AUTO] soft key
When the blank figure specified in a graphic parameter is input,
this soft key automatically scales the graphic range so that the
blank figure is contained within the graphic range.
If no blank figure is input, this soft key has no effect.
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1942 -
NOTE
1 Set the unit of scale for one enlargement/reduction
operation in parameter No. 14713.
2 An enlargement/reduction scale used here is set in
the graphic parameter for scale.
- Moving the graphic range
The following soft keys displayed by step 4 are used:
• [←MOVE] soft key
This soft key moves the graphic range to left.
• [MOVE→] soft key
This soft key moves the graphic range to right.
• [↑MOVE] soft key
This soft key moves the graphic range upward.
• [↓MOVE] soft key
This soft key moves the graphic range downward.
• [CENTER] soft key
This soft key returns the graphic range to the original position.
NOTE
1 Set the travel increment made by one horizontal
move operation in parameter No. 14714.
2 Set the travel increment made by one vertical move
operation in parameter No. 14715.
3 The graphic range modified here is not set in the
graphic parameter for graphic range center.
- Changing the graphic coordinate system
The following soft keys displayed by step 5 are used.
A graphic coordinate system selected here is the same one as set in the
graphic parameter for the graphic coordinate system.
• [XY] soft key
This soft key selects the graphic coordinate system of XY (with a
setting of 0).
• [ZY] soft key
This soft key selects the graphic coordinate system of ZY (with a
setting of 1).
• [YZ] soft key
This soft key selects the graphic coordinate system of YZ (with a
setting of 2).
• [XZ] soft key
This soft key selects the graphic coordinate system of XZ (with a
setting of 3).
• [ZX] soft key
This soft key selects the graphic coordinate system of ZX (with a
setting of 4).
• [XYZ] soft key
This soft key selects the graphic coordinate system of XYZ (with
a setting of 5).
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1943 -
• [YXZ] soft key
This soft key selects the graphic coordinate system of YXZ (with
a setting of 6).
• [YZX] soft key
This soft key selects the graphic coordinate system of YZX (with
a setting of 7).
• [OK] soft key
This soft key changes the current graphic coordinate system to
the graphic coordinate system selected by one of the soft keys
above.
• [CANCEL] soft key
This soft key cancels the graphic coordinate system selected by
one of the soft keys above to return to the original graphic
coordinate system.
NOTE
The graphic coordinate system selected here is set
in the graphic parameter for the graphic coordinate
system.
- Rotating the graphic coordinate system
The following soft keys displayed by step 6 are used.
• [↑] soft key
This soft key rotates the graphic coordinate system upward.
• [↓] soft key
This soft key rotates the graphic coordinate system downward.
• [←] soft key
This soft key rotates the graphic coordinate system to left.
• [→] soft key
This soft key rotates the graphic coordinate system to right.
• [CW] soft key
This soft key rotates the graphic coordinate system clockwise.
• [CCW] soft key
This soft key rotates the graphic coordinate system
counterclockwise.
• [OK] soft key
This soft key changes the rotation angle of the current graphic
coordinate system to the one set by one of the soft keys above.
• [CANCEL] soft key
This soft key cancels the rotation of the graphic coordinate
system performed by one of the soft keys above to return to the
original graphic coordinate system.
NOTE
1 Set the travel increment made by one rotation
operation in parameter No. 14716.
2 The rotation angle of the graphic coordinate system
set here is not set in the graphic parameter for
rotation angle.
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1944 -
- Drawing of a tool
In animation drawing, not only a blank figure but also a tool figure is
drawn in three dimensions.
NOTE
The following function is necessary to draw in the
tool figure.
- Tool geometry size data 100/300 pairs
Figure data
For tool figure drawing, the following data is used:
• Tool geometry size data 100/300 pairs
• Tool compensation data (tool-nose radius compensation value,
virtual tool tip direction, cutter compensation value)
• Parameters
The table below indicates the drawable types of tools and figure data
of each type of tool.
Table 13.2.2.2 (a) List of drawable tools (for turning)
Tool name Tool geometry size data Tool compensation Parameter No.
General-purpose tool Setting Tip position No.27350#0
Cutting edge angle Cutting edge
length
No.27351
Tool angle Holder length No.27352
Holder width No.27353
Holder length 2 No.27354
Holder width 2 No.27355
Threading tool Setting Tip position No.27356#0
Tool angle Cutting edge width No.27357
Holder length No.27358
Holder width No.27359
Grooving tool Setting Tip position No.27360#0
Tip width Holder length No.27361
Tip length Holder width No.27362
Round-nose tool Setting Tool-nose radius Tip position No.27363#0
Tip length Virtual tool tip Holder length No.27364
Holder width No.27365
Point nose straight Setting Tip position No.27366#0
tool Cutting edge angle Cutting edge
length
No.27367
Tool angle Holder length No.27368
Holder width No.27369
Holder length 2 No.27370
Holder width 2 No.27371
Versatile tool Setting Tip position No.27384#0
Tip width Holder length No.27385
Tip length Holder width No.27386
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1945 -
Table 13.2.2.2 (b) List of drawable tools (for milling)
Tool name Tool geometry size data Cutter compensation Parameter No.
Drill Setting Diameter Tip length No.27372
Tool angle
counter sink tool Setting Small diameter Tool angle No.27375
Cutter diameter Tip length No.27376
Cutter length No.27377
Shank length No.27378
Shank diameter No.27379
Flat end mill Setting Diameter Tip length No.27373
Ball end mill Setting Diameter Tip length No.27380
Tap Setting Diameter Tip length No.27374
Reamer Setting Diameter Tip length No.27381
Boring tool Setting Diameter Tip length No.27382
Face mill Setting Diameter Tip length No.27383
NOTE
In lathes system, the round-nose tool and milling
tools can be drawn only when the cutter
compensation/tool-nose radius compensation
function is provided.
Timing of drawing
If a code indicated below is specified during drawing execution, a tool
figure is drawn according to the tool geometry size data that has the
same number as the code.
• With a lathe system
T code command
If three numbers, namely, a tool number, tool geometry offset
number, and tool wear offset number, are specified in a T code,
the tool geometry size data that has the same number as the tool
geometry offset number is obtained.
NOTE
When the tool management function is
provided, a tool offset is specified with a D
code. So, the tool geometry size data that has
the offset number indicated by the D code is
obtained.
• With a machining center system
D code command
If the tool geometry size data corresponding to a specified number
does not exist or the tool geometry size data is not set correctly, tool
drawing is disabled with the warning "ILLEGAL SETTING OF
TOOL FIGURE DATA".
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1946 -
13.2.3 Programmable Data Input (G10) for Blank Figure Drawing
Parameters
Overview
Each of the drawing parameters for a blank figure, a position, and
dimensions that are for the automatic scaling of the drawing areas of
tool path drawing and animation drawing with the dynamic graphic
display function can be set with an NC program, using the
programmable data input command (G10 command).
Format
G10 L90 P_ IP_ I_ J_ K_ ;
P_ : Blank figure
IP_ : Addresses of the basic three axes and the
reference position of a blank
I_,J_,K_ : Dimensions of a blank
NOTE
1 This command is enabled only during the execution
of drawing. It is ignored during normal automatic
operation.
2 This command is a one-shot G code.
3 This command must be specified in a single block.
Explanation
- Blank figure (P_)
Specify the type of a blank figure with either of the following settings
for shapes.
Setting Figure
0 Column or cylinder
(parallel with the Z-axis)
1 Rectangular parallelepiped
The specified value is set in parameter No. 11343.
- Reference position of a blank (IP_)
Specify the reference position of a blank with coordinates (X,Y,Z) in
the workpiece coordinate system.
NOTE
Specify the reference position of a blank with
coordinates (X,Y,Z) in the machine coordinate
system in case of bit 3 (BGM) of parameter
No.11329=1.
The specified value is set in parameter No. 11344.
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1947 -
- Dimensions of a blank (I_,J_,K_)
For the shape of each blank, specify the dimensions of the blank as
follows:
Blank figure Address I Address J Address K
Rectangular
parallelepiped
Length in X-axis
direction
Length in Y-axis
direction
Length in Z-axis
direction
Column Diameter of
column 0 Length of
column
Cylinder Diameter of outer
circle of cylinder
Diameter of inner
circle of cylinder
Length of
cylinder
The specified value are set in parameter No.11345 (address I),
parameter No.11346 (address J), and parameter No.11347 (address K).
- Relationship between the position and dimensions of a blank
The relationship between the position and dimensions of a blank is
shown in the figure below.
J
K
: Reference position (X,Y,Z)
I
X
Z
Y
X
Z
Y
I
J
K
- Operation to be performed when this command is issued
When this command is executed in the background operation, the
specified values are set in the drawing parameters for the blank figure,
reference position, and dimensions that correspond to the specified
arguments, and the drawing area is automatically set again with the
values set.
This causes this command and subsequent commands to perform
drawing in the new drawing area.
NOTE
Before this command, drawing is performed as
described below.
- The tool path is erased.
- In animation drawing, the blank figure is
initialized.
- The drawing start position and the tool figure
become ineffective.
Thus, issue this command at the start of a drawing
program.
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1948 -
13.2.4 Warning Messages
Warning message Content
START REJECTED This program cannot be drawn.
NO PROGRAM SELECTED No drawing target program is selected.
UNAVAILABLE COMMAND IS IN DRAWING An NC statement/macro statement that can not execute drawing
is instructed.
ILLEGAL SETTING OF GRAPHIC PARAMETERS Graphic parameters are not set correctly.
ILLEGAL SETTING OF TOOL FIGURE DATA Tool figure data are not set correctly, or tool figure data are not
exist.
13.2.5 Note
NOTE
1 The coordinates used in drawing are absolute coordinates.
Therefore, even if the coordinate system is changed while it is drawing, it draws in
the coordinate system when having begun to draw.
2 The drawing target axes are the basic three axes.
The basic three axes are the X-axis, Y-axis, and Z-axis on the basic coordinate
system set with parameter No.1022.
3 In a drawing program having a sequence of contiguous small blocks, drawing
requires longer processing time, possibly causing machining time to become longer
than actual machining time.
4 When drawing is executed, data is treated as described below.
(1) Parameters
The same parameters as for automatic operation are used. However,
parameters cannot be rewritten with a command such as the G10 command.
If an attempt is made to rewrite a parameter with programmable parameter
input (G10L52), the command is ignored.
However, by setting bit 7 (GST) of parameter No.11329, drawing can be
temporarily stopped with the warning "UNAVAILABLE COMMAND IS IN
DRAWING".
(2) Tool compensation value/workpiece origin offset/extended workpiece origin
offset/macro variable/fixture offset data, etc.
For each of drawing execution and automatic operation, separate data is used.
At the start of drawing, data for drawing is produced by copying data for
automatic operation. In subsequent operations, the data for drawing and the
data for automatic operation are treated independently of each other. So,
even if data is rewritten with a command such as G10, drawing execution and
automatic operation do not affect each other. Note, however, that data
rewritten in drawing execution is not reflected in the data for automatic
operation but is deleted.
(3) Tool life management data, tool number offset data, three-dimensional error
correction data
These data items are not used for drawing execution. So, if an attempt is
made to rewrite data with G10, the command is ignored.
However, by setting bit 7 (GST) of parameter No.11329, drawing can be
temporarily stopped with the warning "UNAVAILABLE COMMAND IS IN
DRAWING".
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1949 -
13.2.6 Restrictions
- Simultaneous drawing with multiple paths
This function does not support simultaneous tool path drawing by
program execution with multiple paths.
For example, the tool paths of programs executed simultaneously with
multiple paths on a 2-path or 3-path lathe or a combined machine tool
cannot be drawn. This function supports only drawing executed
singly with a single path.
- Simultaneous multipath display
The screens of this function do not support simultaneous multipath
display based on the setting of parameter No. 13131 and No. 13132.
- Functions that operate differently in drawing execution and automatic operation
The operations of the following functions in drawing execution differ
from the operations in automatic operation:
1. Operations that differ, depending on the custom macro
1) Interface signal
#1000 to #1035 are assumed to be 0 at all times.
2) Message output
A message to be output with #3006 is not displayed but is
ignored.
3) clock
#3001 and #3002 are ignored. So, note that drawing is not
continued, for example, if the following is specified:
#3001=0 ;
WHILE [#3001 LE 100] DO1 ;
END1 ;
4) Mirror image
#3007 is assumed to be 0 at all times.
5) Program-restarted state
#3008 is assumed to be 0 at all times.
6) External output command
BPRNT, DPRNT, POPEN, and PCLOS are ignored.
2 Functions that perform partly different operations
1) When G28 (automatic reference position return) is specified,
up to the intermediate point is drawn.
2) When G29 (automatic return from the reference position) is
specified, drawing is performed from the intermediate point.
3) When G27 (reference position return check) is specified, no
reference position return check is made.
4) No stored stroke limit check is made.
5) When G31 (skip function), or G31.1, G31.2, or G31.3
(multistage skip function) is specified, drawing is performed
up to the specified position, regardless of the skip signal.
6) When G60 (single direction positioning) is specified,
drawing is performed directly up to the specified position at
all times even if the positioning direction is opposite.
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1950 -
3. Functions that perform different operations
If the following functions are specified, the operations described
below result:
1) G02.2/G03.2 (involute interpolation)
Circular interpolation is performed.
2) G02.3/G03.3 (exponential interpolation)
Linear interpolation is performed only with linear axes.
3) G07 (virtual axis interpolation)
Circular interpolation is performed.
4) G07.1 (cylindrical interpolation)
Linear interpolation is performed only with linear axes.
5) G12.1 (polar coordinate interpolation)
Linear interpolation is performed only with linear axes.
- Functions that do not support drawing
The following functions are ignored in drawing execution:
1) G04 (dwell)
2) G20, G21 (inch/metric switch)
3) Auxiliary function (M, S, T, B)
4) G22, G23 (stored stroke limit check on/off)
5) G10.6 (tool retract data setting)
6) G81.1 (chopping)
7) G25/G26 (spindle variation detection on/off)
8) G10 (programmable data input)
NOTE
If G10 (programmable data input) is specified,
drawing can be temporarily stopped with the
warning "UNAVAILABLE COMMAND IS IN
DRAWING" by setting bit 7 (GST) of parameter
No.11329.
The following functions are warning in drawing execution:
1) G02.4/G03.4 (three-dimensional circular interpolation)
2) M198 (external subprogram call)
- Functions that support drawing
The operations performed with the following program commands can
be drawn:
1) G00 (Positioning)
2) G01 (Linear interpolation)
3) G02/G03 (Circular interpolation)
However, helical interpolation with the instruction axis other
than basic three axes cannot be drawn.
4) G17/G18/G19 (Plane selection)
5) G33/G34 (Threading)
However, it is drawn as linear interpolation.
6) G35/G36 (Circular threading)
However, it is drawn as circular interpolation.
7) G40/G41/G42 (Cutter compensation/cancel)
8) G52 (Local coordinate system)
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1951 -
9) G53 (Machine coordinate system selection)
10) G54 to G59 (Workpiece coordinate system selection)
11) G54.1 (Extended workpiece coordinate system selection)
12) G65 (Macro call)
13) G68/G69 (Coordinate system rotation, three-dimensional
coordinate system conversion/cancel)
14) G90/G91 (Absolute/incremental command)
15) G92 (Workpiece coordinate system change)
16) G92.1 (Workpiece coordinate system preset)
17) G94/G95 (Feed per minute/Feed per rotation)
18) G96/G97 (Constant surface speed control/cancel)
19) M98 (Subprogram call)
20) G90/G92/G94 (Canned cycle, only Lathes system)
21) G71/G72/G73/G74/G75/G76/G70 (Multiple repetitive cycle,
only Lathes system)
22) G83/G84G85/G87/G87/G88/G80 (Canned cycle for drilling,
only Lathes system)
23) G73/G74/G76/G81/G82/G83/G84/G85/G86/G87/G88/G89/G80
(Canned cycle for drilling, only Machining center system)
NOTE
1 When a lathe system is used, refer to the G codes
above as codes of G code system B.
2 It is possible to draw with the G68 (Coordinate
system rotation, three-dimensional coordinate
system conversion) instruction only in the tool path
drawing.
And, the display of coordinates when instructing in
G68 is a coordinate value on the workpiece
coordinate system.
3 In threading cycle of canned cycle and multiple
repetitive cycle, movement of thread chamfering is
not drawn.
4 In animation drawing, shape by the movement of
back boring cycle command is different from actual
shape.
5 In animation drawing, movement to shift amount at
the bottom of a hole in the fine boring cycle and
back boring cycle command is not drawn by setting
bit 1 (ABC) of parameter No.11349=0.
- Operations that do not support drawing
The following operations cannot be drawn:
1) Backward movement based on the retrace function
2) Forward movement/backward movement/resumed forward
movement based on the manual handle retrace function
3) Movement made with skip signal input for a skip command or
multistage skip command
4) Movement on an axis based on PMC axis control
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1952 -
5) Movement on an axis based on real-time custom macro
specification
6) Operation based on manual interrupt, manual handle interrupt,
etc.
7) Operation based on synchronous control, mixture control, and
superimposed control
8) Operation based on mirror image of facing tool posts
9) Operation based on the 5-axis machining function
10) Operation based on the high-speed, high-precision function (AI
contour control I, AI contour control II and high-speed
processing)
11) Operation based on nano smoothing or NURBS interpolation
12) Operation based on the program coordinate system switching
function
13) Operation based on the offset memory switching function
14) Operation based on Cs contour control
15) Operation based on Spindle positioning.
- Dynamic switching of diameter/radius specification in the background operation
It is possible to perform drawing by switching the amount-of-travel
setting on each axis that is to be specified in the drawing program to a
diameter or radius value, using programmable switching of
diameter/radius specification (G10.9 command) of the function of
dynamic switching of diameter/radius specification.
When the G10.9 command of the function of dynamic switching of
diameter/radius specification is enabled (bit 5 (PGD) of parameter No.
3400 = 1), drawing is performed by internally switching the
diameter/radius specification for the move command for each axis in
the background operation, as follows:
• If the specified address value is 0 (radius specification) →
Drawing is performed with the radius specification.
• If the specified address value is 1 (diameter specification) →
Drawing is performed with the diameter specification.
NOTE
1 For the G10.9 command in the background
operation, the diameter/radius specification
switching status signal of the function of dynamic
switching of diameter/radius specification is not
output.
2 The diameter/radius specification switching signal
of the function of dynamic switching of
diameter/radius specification is ineffective to the
background operation.
3 The switching due to the G10.9 command in the
background operation is canceled if the
background operation is stopped.
4 Using this command requires the function of
dynamic switching of diameter/radius specification.
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1953 -
• Data items and commands that can be switched
For the following data item and command, switching of
diameter/radius specification is performed according to the
switched specification:
- Move command from a program
- Current position display
• Data items that cannot be switched
For the following data items, switching of diameter/radius
specification is not performed because they follow the setting of
bit 3 (DIAx) of parameter No. 1006.
- Parameter
- Offset
- Workpiece coordinate system
In custom macros, coordinates that can be read with the system
variables indicating position information, listed below.
#5001 to #5020 and #100001 to #100050: End point position in
the immediately preceding block (workpiece coordinate system)
#5021 to #5040 and #100051 to #100100: Specified current
position (machine coordinate system)
#5041 to #5060 and #100101 and #100150: Specified current
position (workpiece coordinate system)
#5061 to #5080 and #100151 to #100200: Skip position
(workpiece coordinate system)
NOTE
For offsets, the settings of bit 1 (ORC) and bit 2
(ODI) of parameter No. 5004 take precedence.
Screen center coordinates and values of blank (position) drawing
parameters are handled with radius specification regardless of the
setting of parameter bit DIAx.
- Operation of the P-CODE workpiece number search function in the background
operation
When drawing is started with the setting of bit 3 (WNS) of parameter
No. 11349, the execution macro specified in system variable #8610 is
executed before the drawing program.
• Calling conditions and operations
a) Bit 6 (PWSR) of compilation parameter No. 9002 is set to
1.
b) The program number of an execution macro is set in system
variable #8610 before the start of drawing.
If the conditions above are met, pressing soft key [START] or
[1BLOCK] to execute drawing causes the following operations
to be performed:
13.GRAPHIC FUNCTION OPERATION B-63944EN/03
- 1954 -
(1) The execution macro specified with system variable #8610
is called.
If bit 4 (P98) of compilation parameter No. 9163 is 0, the
execution macro is called with an operation equivalent to a
simple call (G65), and if P98 is 1, it is called with an
operation equivalent to a subprogram call (M98).
(2) When the execution macro terminates, the drawing program
is executed.
NOTE
1 This function calls an execution macro if the
conditions described in a) and b) are met,
regardless of the program selected. Thus, if using
this function to perform drawing with an execution
macro, modify the program of the execution macro
so that macro statements, auxiliary functions, and
other commands in the execution macro that are
not necessary for drawing are not executed, by
referring to the system variable below.
System
variable Value Execution state
1 Normal state (if drawing is not executed)
#3010 -1 Drawing execution
2 System variable #8610, referenced during the
execution of drawing, is the same as that used
during automatic operation. If, therefore, the value
of the variable is changed to execute drawing, it is
necessary to return the variable to the original
value before automatic operation is performed.
Also, automatic operation is performed with the
variable value at the time drawing is started and,
therefore, caution is required so that the value set
is not changed during automatic operation.
• Nesting and local variables
Nesting is accumulated in an execution macro. An execution
macro is called with an operation equivalent to a simple call
(G65) or a subprogram call (M98) and, therefore, other execution
macros can be called from the called execution macro with all
calling methods.
In the case of an operation equivalent to a simple call (G65), the
level of local variables is changed to that of the drawing program.
That is, the drawing program do not inherit the local variables
used in the execution macro.
In the case of an operation equivalent to a subprogram call (M98),
the local variables at the same level as the drawing program are
used. That is, the drawing program inherits the local variables
used in the execution macro.
B-63944EN/03 OPERATION 13.GRAPHIC FUNCTION
- 1955 -
- Drawing start position
In tool path drawing, if G92, G52, or G92.1 (machining center
system) or G50, G52, or G50.3 (lathe system) is specified at the start
of a drawing target program, the position specified with the G code is
the drawing start position. If none of these G codes is specified, the
end point of the first moving command is the drawing start position.
In animation drawing, the current position when the tool figure is
displayed is the drawing start position.
- Use of this function with other functions
When this function is specified, the following functions cannot be
used:
• Graphic display
• Manual Guide i
- VGA display based on the C language executor
If VGA display based on the C language executor is used, the VGA
window is erased when the screen display is switched to a screen of
this function.
So, when using the VGA window, determine the screen of this
function by screen number and close the VGA window before
switching the screen display.
- Use of the CNC screen display function
The following restriction exists when the screen of dynamic graphic
display function is displayed by the CNC screen display function.
1) The drawing screen is not displayed in the CNC screen display
function by way of via embedded Ethernet.
Please use the CNC screen display function by way of the FAST
Ethernet board.
2) The drawing screen is not displayed in the CNC screen dual
display function.
3) Please do not start / shut down the CNC screen display function
when you display the drawing screen. Please start / shut down the
CNC screen display function after it switches to other screens.
- Display unit
This function can be used with a 10.4-inch display unit.
On the screens of this function, the vertical soft keys displayed on a
10.4-inch display unit are not displayed.
To use the vertical soft keys, switch the screen display to another
screen.
- Use of the Screen hard copy function
If the screen is copied while executing drawing by screen hard copy
function, the drawing stops temporarily. The drawing can be restarted
by pushing [RESTART] soft key if necessary after the copy operation
is finished.
14.VIRTUAL MDI KEY FUNCTION OPERATION B-63944EN/03
- 1956 -
14 VIRTUAL MDI KEY FUNCTION
Chapter 14, "VIRTUAL MDI KEY FUNCTION", consists of the
following sections:
14.1 VIRTUAL MDI KEY .............................................................1957
B-63944EN/03 OPERATION 14.VIRTUAL MDI KEY FUNCTION
- 1957 -
14.1 VIRTUAL MDI KEY
Overview
This function is used to perform program editing and changing of
various data using the keyboard displayed on the LCD with a touch
panel.
Screen on which a CNC screen is displayed in the upper left 1/4 area
Explanation
A CNC screen equivalent to that displayed on 7.2/8.4-inch LCDs is
displayed in the upper left area of the screen, and the keyboard is
displayed in the remaining area.
Figure 14.1 (a) Screen on which a CNC screen is displayed in the upper
left area
Operation
- Input key
The display "INPUT" on the virtual MDI keyboard is equivalent to the
input key.
- Cancel key
The displays "BACK SPACE" and "CAN" on the virtual MDI
keyboard are equivalent to the cancel key.
- Shift key
The display "SHIFT" ↑ on the virtual MDI keyboard is equivalent to
the shift key.
Pressing the "SHIFT" key once places the system in the shift state, and
pressing the "SHIFT" key again or another key releases the system
from the state.
Pressing a key in the shift state causes the character indicated in the
upper left corner of the key to be entered.
14.VIRTUAL MDI KEY FUNCTION OPERATION B-63944EN/03
- 1958 -
- Simultaneous pressing of two keys
The operation to be performed for pressing two key simultaneously,
such as the "CAN" and "RESET" keys to erase alarm PS100, is as
follows:
(1) Press the "SPCL" key. The "SPCL" key is held down, and places
the system in SPCL mode.
(2) Press the keys to be pressed simultaneously, one at a time.
(3) Press the "INPUT" key. Of the keys pressed in SPCL mode, the
last two are assumed to have been pressed simultaneously. The
system is released from SPCL mode, and the SPCL key, which
has been held down, returns to the normal state.
Example: "SPCL" → "CAN" → "RESET" → "INPUT"
NOTE
1 In SPCL mode, other keys are disabled until the
"SPCL" or "INPUT" key is pressed.
2 Pressing the "SPCL" key in "SPCL" mode causes
all keys pressed in SPCL mode to be disabled. The
system is released from SPCL mode, and the
SPCL key, which has been held down, returns to
the normal state.
Screen on which a CNC screen is displayed in the entire area
Explanation
A CNC screen equivalent to that displayed on 7.2/8.4-inch LCDs is
displayed in the entire area. Function keys and the ON/OFF button for
virtual keys are displayed at the bottom of the screen.
Figure 14.1 (b) Screen on which a CNC screen is displayed in the entire
area
B-63944EN/03 OPERATION 14.VIRTUAL MDI KEY FUNCTION
- 1959 -
Operation
- Function key page switching
Pressing "MENU" located near the lower right corner of the screen
switches the screen to page 1, page 2, page 3, and back to page 1 in
this order.
Function keys on page 1
Function keys on page 2
Function keys on page 3
- Display of virtual keys
Pressing "KEY ON" located at the lower right corner of the screen
displays virtual MDI keys. The character string on the key top changes
to "KEYOFF".
Pressing "KEYOFF" hides virtual MDI keys.
Figure 14.1 (c) State in which virtual keys are ON
14.VIRTUAL MDI KEY FUNCTION OPERATION B-63944EN/03
- 1960 -
- Input key
The display "INPUT" on the virtual MDI keyboard is equivalent to the
input key.
- Cancel key
The displays "BS" and "CAN" on the virtual MDI keyboard are
equivalent to the cancel key.
- Shift key
The display "SHIFT" on the virtual MDI keyboard is equivalent to the
shift key.
The characters on the key tops change to those that can be entered in
the shift state.
Figure 14.1 (d) Key tops in the shift state
- Simultaneous pressing of two keys
The operation to be performed for pressing two key simultaneously,
such as the "CAN" and "RESET" keys to erase alarm PS100, is as
follows:
(1) Press the "SPCL" key. The "SPCL" key is held down, and places
the system in SPCL mode.
(2) Press the keys to be pressed simultaneously, one at a time.
(3) Press the "INPUT" key.
Example: "SPCL" → "CAN" → "RESET" → "INPUT"
NOTE
1 In SPCL mode, other keys are disabled until the
"SPCL" or "INPUT" key is pressed.
2 Pressing the "SPCL" key in "SPCL" mode causes
all keys pressed in SPCL mode to be disabled. The
system is released from SPCL mode, and the
SPCL key, which has been held down, returns to
the normal state.
14.1.1 Limitations
- Display of VGA windows on the C language executor
This function uses one VGA window, so that the number of VGA
windows that can be used on the C language executor is reduced by
one.
- LCDs
LCDs on which this function can be used are 10.4-inch LCDs with a
touch panel.
IV. MAINTENANCE
B-63944EN/03 MAINTENANCE 1.ROUTINE MAINTENANCE
- 1963 -
1 ROUTINE MAINTENANCE
This chapter describes routine maintenance work that the operator can
perform when using the CNC.
WARNING
Only those persons who have been educated for
maintenance and safety may perform maintenance
work not described in this chapter.
Chapter 1, "ROUTINE MAINTENANCE", consists of the following
sections:
1.1 ACTION TO BE TAKEN WHEN A PROBLEM
OCCURRED...........................................................................1964
1.2 BACKING UP VARIOUS DATA ITEMS.............................1965
1.3 METHOD OF REPLACING BATTERY...............................1967
1.ROUTINE MAINTENANCE MAINTENANCE B-63944EN/03
- 1964 -
1.1 ACTION TO BE TAKEN WHEN A PROBLEM OCCURRED
If an unexpected operation occurs or an alarm or warning is output
when the CNC and machine are used, the problem needs to be solved
quickly. For this purpose, the status of the problem must be
identified correctly, and a proper action must be taken.
The procedure for taking an action for a problem is shown below.
Problem!
Dangerous?
Dan
g
er to
y
ou and others
Not dangerous
Check and identify problem.
- Warning
-Alarm
- Abnormal operation
- Wrong operation, etc.
Dangerous
Take action to avoid danger.
- Stop machine immediately.
- Refuge to safe place immediately.
Check status and how problem
occurred.
- Time and place of problem
occurrence
- Operation procedure
Confirm and secure safety.
- Confirm current safety.
- Check machine and circumstances.
- Turn off power to machine.
Investigate cause and take action.
- Check and correct machining program and set data items.
- Review and modify operation procedure.
- Check and repair machine operation sections.
Recovery work
- Action by you or machine tool builder
- Check operation after recovery.
If recovery is impossible,
immediately notify sales agent or
supplier of problem details fo
r
action.
For details of investigation and action on problems arising from the
CNC, refer to "TROUBLESHOOTING PROCEDURE" in the
Maintenance Manual (B-63945EN) issued by FANUC.
B-63944EN/03 MAINTENANCE 1.ROUTINE MAINTENANCE
- 1965 -
1.2 BACKING UP VARIOUS DATA ITEMS
With the CNC, various data items such as offset data and system
parameters are stored in the SRAM of the control unit and are
protected by a backup battery. However, an accident can erase the
data. By storing the data at another location (outside the CNC), the
data, when lost, can be restored.
So, when the machine is started up or data is updated, for example, the
data should be backed up (stored outside the CNC).
- Data backup operation
The data items listed below should be backed up. For the method of
data output operation, see the chapter of "DATA INPUT/OUTPUT" in
this manual.
<1> System parameters
→ See III-8.1.2.
<2> Machining programs
→ See III-8.1.1.
<3> Tool offset data
→ See III-8.1.3.
<4> PMC data
→ See PMC PROGRAMMING MANUAL (B-63983EN).
<5> Pitch error compensation data (when the pitch error
compensation function is selected.)
→ See III-8.1.4.
<6> Three-dimensional error compensation (when the
three-dimensional error compensation function is selected.)
→ See III-8.1.5.
<7> Custom macro variables (when the custom macro function is
selected.)
→ See III-8.1.6.
<8> Workpiece coordinate system setting data (when the workpiece
coordinate system function is selected.)
→ See III-8.1.7.
<9> Tool management data (when the tool management function is
selected.)
→ See III-8.1.9.
It is recommended that recording media (such as floppy disks and
memory cards) daily used with the machine be used to store data.
Stored data should be managed properly so that the data can be
restored quickly if a problem occurs.
1.ROUTINE MAINTENANCE MAINTENANCE B-63944EN/03
- 1966 -
- Data restoration work
In order to restore lost data to the state of the stored data, input the
data backed up according to the previous item into the CNC. For the
method of data input operation, see the chapter of "DATA
INPUT/OUTPUT" in this manual.
WARNING
After inputting stored data, do not start an
operation immediately. Instead, check that the
data is input correctly and that settings are made to
meet a desired operation.
If an operation is executed without making this
check, the machine and workpiece can be
damaged and personal injury can occur due to an
unexpected machine movement. Use sufficient
care.
CAUTION
Before recovery of the following data items, consult
with the machine tool builder of the machine used:
• System parameters
• PMC data
• Macro programs and custom macro variables
• Pitch error compensation values
NOTE
The method of recovery described in this section is
intended just to restore the state of the backed up
data, and does not guarantee recovery of the state
that was present when the data was lost.
B-63944EN/03 MAINTENANCE 1.ROUTINE MAINTENANCE
- 1967 -
1.3 METHOD OF REPLACING BATTERY
This chapter describes how to replace the CNC backup battery and
absolute Pulsecoder battery. This section consists of the following
subsections::
1.3.1 Replacing Battery for LCD-mounted Type CNC Control
Unit .......................................................................................1968
1.3.2 Replacing the Battery for Stand-alone Type CNC Control
Unit .......................................................................................1971
1.3.3 Battery in the PANEL i (3 VDC) .........................................1973
1.3.4 Battery for Absolute Pulse coders ........................................1975
Battery for memory backup
Offset data, and system parameters are stored in SRAM in the control
unit. The power to the SRAM is backed up by a lithium battery
mounted on the front panel of the control unit. Therefore, the above
data is not lost even if the main battery fails. The backup battery is
installed in the control unit prior to being shipped from the factory.
This battery can provide backup for the memory contents for about a
year.
When the battery voltage falls, alarm message "BAT" blinks on the
LCD display and the battery alarm signal is output to the PMC.
When this alarm is displayed, replace the battery as soon as possible.
In general, the battery can be replaced within one or two weeks of the
alarm first being issued. This, however, depends on the system
configuration.
If the battery voltage subsequently drops further, backup of memory
can no longer be provided. Turning on the power to the control unit
in this state causes system alarm to be issued because the contents of
memory are lost. Replace the battery, clear the entire memory, then
reenter the data.
Replace the memory backup battery while the control unit is brought
off.
The following two kinds of batteries can be used.
• Lithium battery, incorporated into the CNC control unit.
• Two alkaline dry cells (size D) in an external battery case.
NOTE
A lithium battery is installed as standard at the
factory.
1.ROUTINE MAINTENANCE MAINTENANCE B-63944EN/03
- 1968 -
1.3.1 Replacing Battery for LCD-mounted Type CNC Control Unit
When using a lithium battery
- Replacement procedure
When a lithium battery is used
Prepare a new lithium battery (ordering code: A02B-0200-K102
(FANUC specification: A98L-0031-0012)).
<1> Turn on the power to the CNC. After about 30 seconds, turn off
the power.
<2> Remove the old battery from the back of the CNC control unit.
First, unplug the connector by yanking the battery cable, then
take the battery out of its case.
The battery case of a control unit without option slots is located
at the back of the unit as shown in the figure below. The battery
case of a control unit with option slots is located next to the fan
on the top of the unit.
<3> Insert a new battery and reconnect the connector.
<4> Clamp the battery cable as shown in Fig. 1.3.1 (c).
Lithium batter
y
A
02B-0236-K102
Connector
Battery case
Fig. 1.3.1 (a) Unit without option slots
B-63944EN/03 MAINTENANCE 1.ROUTINE MAINTENANCE
- 1969 -
Battery case
Connecto
r
Lithium batter
y
A02B-0236-K102
Fig. 1.3.1 (b) Unit with option slots
Battery cable
Fig. 1.3.1 (c) Clamping the battery cable
WARNING
Using other than the recommended battery may
result in the battery exploding. Replace the
battery only with the specified battery
(A02B-0200-K102).
CAUTION
Steps <1> to <3> should be completed within 30
minutes.
Do not leave the control unit without a battery for
any longer than the specified period. Otherwise,
the contents of memory may be lost.
If steps <1> to <3> may not be completed within 30
minutes, save all contents of the SRAM to the
memory card beforehand. Thus, if the contents of
the SRAM are lost, the contents can be restored
easily.
For the method of operation, refer to Maintenance
Manual.
When discarding a battery, observe the applicable ordinances or other
rules of your local government. Also, cover the terminals of the
battery with vinyl tape or the like to prevent a short-circuit.
1.ROUTINE MAINTENANCE MAINTENANCE B-63944EN/03
- 1970 -
When using commercial alkaline dry cells (size D)
- Replacement procedure
<1> Prepare two alkaline dry cells (size D) commercially available.
<2> Turn on the power to the control unit.
<3> Remove the battery case cover.
<4> Replace the cells, paying careful attention to their orientation.
<5> Reinstall the cover onto the battery case.
CAUTION
When replacing the alkaline dry cells while the
power is off, use the same procedure as that for
lithium battery replacement described above.
Cover
A
lkaline dry cell × 2
Connection terminal on the rear
Battery case
Mounting hole
×
4
B-63944EN/03 MAINTENANCE 1.ROUTINE MAINTENANCE
- 1971 -
1.3.2 Replacing the Battery for Stand-alone Type CNC Control Unit
When using a lithium battery
- Replacing the battery
If a lithium battery is used, have A02B-0200-K102 (FANUC internal
code: A98L-0031-0012) handy.
<1> Turn the CNC on. About 30 seconds later, turn the CNC off.
<2> Remove the battery from the top area of the CNC unit.
First, unplug the connector by yanking the battery cable, then
take the battery out of the case.
The battery case is provided in the top area of the face plate of
the main board.
<3> Replace the battery, then connect the connector.
Battery case
Lithium battery
A
02B-0200-K102
Connector
WARNING
The incorrect mounting of the battery may cause
an explosion. Avoid using any battery other than
the one specified here (A02B-0200-K102).
1.ROUTINE MAINTENANCE MAINTENANCE B-63944EN/03
- 1972 -
CAUTION
Complete steps <1> to <3> within 30 minutes.
If the battery is left removed for a long time, the
memory would lose the contents.
If there is a danger that the replacement cannot be
completed within 30 minutes, save the whole
contents of the SRAM to a memory card. The
contents of the memory can be easily restored with
the memory card in case the memory loses the
contents.
Discard the dead battery, observing appropriate municipal rules and
regulations. When discarding the battery, insulate the terminal with
a tape so that no short-circuit would occur.
When using commercial D-size alkaline dry cells
- Replacing the battery
<1> Have commercial D-size alkaline dry cells handy.
<2> Turn the CNC on.
<3> Remove the cover from the battery case.
<4> Replace the old dry cells with new ones. Mount the dry cells in
a correct orientation.
<5> Replace the cover on the battery case.
CAUTION
In the power-off state, the battery should be
replaced as in the case of the lithium battery, which
is descried above.
Connection terminal on the back
Case
4 mounting holes
2 dry cells
Cove
r
B-63944EN/03 MAINTENANCE 1.ROUTINE MAINTENANCE
- 1973 -
1.3.3 Battery in the PANEL i (3 VDC)
A lithium battery is used to back up BIOS data in the PANEL i. This
battery is factory-set in the PANEL i. This battery has sufficient
capacity to retain BIOS data for one year.
When the battery voltage becomes low, the following message
appears on the self test screen displayed at turn-on, and the self test
pauses.
CMOS Battery Failure
If this message appears, replace the battery as soon as possible (within
one week). FANUC recommends that the battery be replaced once
per year regardless of whether a battery alarm is issued.
- Replacing the battery
(1) To guard against the possible loss or destruction of BIOS
parameters, write down the BIOS parameter values.
(2) Obtain a new lithium battery (A02B-0200-K102).
(3) After power has been supplied for at least five seconds, turn off
the power to PANEL i. Remove the intelligent terminal from
the panel so that replacement work can be done from the rear of
the intelligent terminal.
(4) Detach the connector of the lithium battery, and remove the
battery from the battery holder.
(5) Attach the connector, and place the battery in the battery holder.
(6) Install PANEL i again.
(7) Turn on the power, and check that the BIOS parameters are
maintained (BIOS setup is not activated forcibly).
Between removing an old battery and inserting new battery, no more
than five minutes must be allowed to elapse.
1.ROUTINE MAINTENANCE MAINTENANCE B-63944EN/03
- 1974 -
Connector
(BAT1)
Lithium battery
A
02B-0200-K102
Fig. 1.3.3 (a) Lithium battery connection for PANEL i
B-63944EN/03 MAINTENANCE 1.ROUTINE MAINTENANCE
- 1975 -
1.3.4 Battery for Absolute Pulsecoders
(1) When the absolute pulsecoder battery voltage falls, "APC" blinks
in the status display on the screen. When the battery voltage
further falls, alarms DS0306 to 0308 are issued.
(2) When alarm DS0307 (alarm indicating the voltage of the battery
becomes low) occurs, replace the battery as soon as possible. In
general, the battery should be replaced within one or two weeks,
however, this depends on the number of Pulsecoders used.
(3) If the voltage of the battery becomes any lower, alarm DS0306
(battery zero alarm) occurs. In this case, the current positions
for the Pulsecoders can no longer be maintained.
In this state, alarm DS0300 (reference position return request
alarm) occurs. After replacing the batteries, be sure to perform
manual reference position return.
(4) The service life of the batteries is about two years if they are
used in a six-axis configuration with αi/βi series servo motors
and one year if they are used in a six-axis configuration with α/β
series servo motors. FANUC recommends that you replace the
batteries periodically according to the battery service life.
(5) To connect the battery, use the battery case or incorporate the
battery into the servo amplifier. Note that the attachment
method of the battery depends on the connection method and the
type of servo amplifier.
- Replacing batteries
To prevent absolute position information in absolute Pulsecoders from
being lost, turn on the machine power before replacing the battery.
The replacement procedure is described below. (Note: The
turning-on step is not required when the αi series servo motor or βi
series servo motor (βiS 0.4 to βiS 22) is used.)
(1) Turn the servo unit (machine) on.
(2) Place the machine in the emergency stop state.
(3) Confirm that servo motors are not active.
(4) Make sure the DC link charge LED is off.
(5) Remove the old battery and then attach a new one.
(6) Now, replacement has been completed. The system power can
be turned off.
1.ROUTINE MAINTENANCE MAINTENANCE B-63944EN/03
- 1976 -
NOTE
The absolute Pulsecoder of the servo motor αi/αis
series or βiS (βiS 0.4 to βiS 22) series is
incorporated with a backup capacitor as standard.
This backup capacitor enables an absolute position
detection to be continued for about 10 minutes.
Therefore, no manual reference position return
need be performed if the time during which servo
amplifier power is kept off for battery replacement
is within 10 minutes. If battery replacement takes
10 minutes or more, the power must remain turned
on.
WARNING
1 When replacing the battery, be careful not to touch
bare metal parts in the panel. In particular, be
careful not to touch any high-voltage circuits due to
the electric shock hazard.
2 Before replacing the battery, make sure the DC link
charge LED is off. Otherwise, an electric shock
may be received.
3 Be sure to use the specified battery. If another
type of battery is used, it may overheat, blow out,
or catch fire.
4 Install the battery with correct polarity. If the
battery is installed with incorrect polarity, it may
overheat, blow out, or catch fire. Or, absolute
position information in absolute Pulsecoders may
be lost.
5 During attachment of the battery, insert the
factory-attached protection socket into the CX5X or
CX5Y connector, whichever is not used. If the +6
V pin and 0 V pin are short-circuited, the battery
may overheat, blow out, or catch fire. Or,
absolute position information in absolute
Pulsecoders may be lost.
B-63944EN/03 MAINTENANCE 1.ROUTINE MAINTENANCE
- 1977 -
- Replacing D-size alkaline dry cells in the battery case
Replace four D-size alkaline batteries (A06B-6050-K061) in the
battery case installed in the machine.
(1) Have four D-size alkaline batteries on hand.
(2) Loosen the screws on the battery case. Remove the cover.
(3) Replace the alkaline batteries in the case. Pay careful attention to
the polarity of the alkaline batteries.
(4) Attach the cover.
Screws
Cover
WARNING
Install the battery with correct polarity. If the
battery is installed with incorrect polarity, it may
overheat, blow out, or catch fire. Or, absolute
position information in absolute Pulsecoders may
be lost.
1.ROUTINE MAINTENANCE MAINTENANCE B-63944EN/03
- 1978 -
- Attaching the built-in battery (αi series servo amplifier)
Attach the lithium battery (A06B-6073-K001) to the servo amplifier.
[Attachment procedure]
(1) Remove a battery cover from the servo amplifier.
(2) Attach the battery as shown below.
(3) Re-attach the cover.
(4) Connect the connector of battery with CX5X of the servo
amplifier.
SVM
CX5X, CX5Y
+6V
0V
Battery
Battery cover
Connector
Inserting way
Cable side
Red: +6V
Black: 0V
CAUTION
Attaching the battery from the cable outlet applies
tension to the cable. Therefore, attach the cable
from another place to prevent the cable from being
stretched. If this cable is connected on a stretch
condition, a bad conductivity may be occurred.
B-63944EN/03 MAINTENANCE 1.ROUTINE MAINTENANCE
- 1979 -
- Attaching the built-in battery (β series servo amplifier)
Attach the lithium battery (A06B-6093-K001) to the servo amplifier.
[Attachment procedure]
(1) In case of SVU-12 or SVU-20, remove the battery cover under
the servo amplifier grasping its left and right sides. In case of
SVU-40 or SVU-80, remove the cover attached on right side of
the servo amplifier grasping its upper and lower sides.
(2) Remove the connector of battery. (Connector CX5X or CX5Y)
(3) Replace the battery and connect the connector.
(4) Mount the battery cover.
Batter
y
Battery cover
SVU-12, SVU-20
Batter
y
Battery cover
Pass the battery cable to this slit.
SVU-40, SVU-80
1.ROUTINE MAINTENANCE MAINTENANCE B-63944EN/03
- 1980 -
CAUTION
1 The connector of the battery can be connected with
either of CX5X and CX5Y.
2 Attaching the battery from the cable outlet applies
tension to the cable. Therefore, attach the cable
from another place to prevent the cable from being
stretched. If this cable is connected on a stretch
condition, a bad conductivity may be occurred.
- Used batteries
Old batteries should be disposed as "INDUSTRIAL WASTES"
according to the regulations of the country or autonomy where your
machine has been installed.
APPENDIX
B-63944EN/03 APPENDIX A.PARAMETERS
- 1983 -
A PARAMETERS
This manual describes all parameters indicated in this manual.
For those parameters that are not indicated in this manual and other
parameters, refer to the parameter manual.
NOTE
A parameter that is valid with only one of the path
control types for the lathe system (T series) and
machining center system (M series) is indicated in
the upper or lower row as described below. A blank
represents an unusable parameter.
[Example 1]
The parameter HTG is common to the T series and
M series, and RTV and ROC are parameters used
with the T series only.
1403 RTV ROC
HTG
HTG
T series
M series
#7 #6 #5 #4 #3 #2 #1 #0
[Example 2]
The following parameter is used with the M series
only:
1411 Cutting feedrate
T series
M series
A.PARAMETERS APPENDIX B-63944EN/03
- 1984 -
A.1 DESCRIPTION OF PARAMETERS
#7 #6 #5 #4 #3 #2 #1 #0
0000 ISO TVC
[Input type] Setting input
[Data type] Bit path
# 0 TVC TV check
0: Not performed
1: Performed
# 1 ISO Code used for data output
0: EIA code
1: ISO code
NOTE
ASCII code is used at all times for output to the
memory card.
#7 #6 #5 #4 #3 #2 #1 #0
0001 FCV
[Input type] Setting input
[Data type] Bit path
# 1 FCV Program format
0: Series 16 standard format
1: Series 15 format
NOTE
1 Programs created in the Series 15 program format
can be used for operation on the following
functions:
1 Subprogram call M98
2 Thread cutting with equal leads G32 (T series)
3 Canned cycle G90, G92, G94 (T series)
4 Multiple repetitive canned cycle G71 to G76 (T
series)
5 Drilling canned cycle
G83.1, G80 to G89 (T series)
G73, G74, G76, G80 to G89(M series)
2 When the program format used in the Series 15 is
used for this CNC, some limits may add. Refer to
the User’s Manual.
B-63944EN/03 APPENDIX A.PARAMETERS
- 1985 -
#7 #6 #5 #4 #3 #2 #1 #0
0010 PRM
[Input type] Setting input
[Data type] Bit path
# 1 PRM When parameters are output, the parameters whose values are 0 are:
0: Output.
1: Not output.
#7 #6 #5 #4 #3 #2 #1 #0
0012 MIRx
[Input type] Setting input
[Data type] Bit axis
# 0 MIRx Mirror image for each axis
0: Mirror image is off. (Normal)
1: Mirror image is on. (Mirror)
0020 I/O CHANNEL : Input/output device selection, or interface number for a
foreground input device
[Input type] Setting input
[Data type] Byte
[Valid data range] 0 to 5
The CNC has the following interfaces for transferring data to and from
an external input/output device and the host computer:
Input/output device interface (RS-232-C serial ports 1 and 2)
Memory card interface
Data server interface
Embedded Ethernet interface
By setting bit 0 (IO4) of parameter No. 0110, data input/output can be
controlled separately. When IO4 is not set, data input/output is
performed using the channel set in parameter No. 0020. When IO4 is
set, a channel can be assigned to each of foreground input, foreground
output, background input, and background output.
In these parameters, specify the interface connected to each
input/output device to and from which data is to be transferred. See
the table below for these settings.
Correspondence between settings and input/output devices
Setting Description
0,1 RS-232-C serial port 1
2 RS-232-C serial port 2
4 Memory card interface
5 Data server interface
9 Embedded Ethernet interface
A.PARAMETERS APPENDIX B-63944EN/03
- 1986 -
#7 #6 #5 #4 #3 #2 #1 #0
0100 NCR CTV
[Input type] Setting input
[Data type] Bit
# 1 CTV Character counting for TV check in the comment section of a
program.
0: Performed
1: Not performed
# 3 NCR Output of the end of block (EOB) in ISO code
0: LF, CR, CR are output.
1: Only LF is output.
#7 #6 #5 #4 #3 #2 #1 #0
0138 MNC
[Input type] Parameter input
[Data type] Bit
# 7 MNC DNC operation from the memory card and external device
subprogram call from the memory card are:
0: Not performed.
1: Performed.
0983 Path control type of each path
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to 1
Set the path control type of each path.
The following two path control types are available:
T series (lathe system) : 0
M series (machining system) : 1
B-63944EN/03 APPENDIX A.PARAMETERS
- 1987 -
#7 #6 #5 #4 #3 #2 #1 #0
0984 LCP
[Input type] Parameter input
[Data type] Bit path
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
# 0 LCP Set whether the path is a loader control path.
0: The path is not a loader control path.
1: The path is a loader control path.
#7 #6 #5 #4 #3 #2 #1 #0
1001 INM
[Input type] Parameter input
[Data type] Bit path
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
# 0 INM Least command increment on the linear axis
0: In mm (metric system machine)
1: In inches (inch system machine)
#7 #6 #5 #4 #3 #2 #1 #0
1002 IDG XIK AZR JAX
[Input type] Parameter input
[Data type] Bit path
# 0 JAX Number of axes controlled simultaneously in jog feed, manual rapid
traverse and manual reference position return
0: 1 axis
1: 3 axes
A.PARAMETERS APPENDIX B-63944EN/03
- 1988 -
# 3 AZR When no reference position is set, the G28 command causes:
0: Reference position return using deceleration dogs (as during
manual reference position return) to be executed.
1: Alarm (PS0304) "G28 was specified when no reference position
is set" to be displayed.
NOTE
When reference position return without dogs is
specified, (when bit 1 (DLZ) of parameter No.1005 is
set to 1) the G28 command specified before a
reference position is set causes an alarm PS0304 to
be issued, regardless of the setting of AZR.
# 4 XIK When LRP, bit 1 of parameter No.1401, is set to 0, namely, when
positioning is performed using non-linear type positioning, if an
interlock is applied to the machine along one of axes in positioning,
0: The machine stops moving along the axis for which the interlock
is applied and continues to move along the other axes.
1: The machine stops moving along all the axes.
# 7 IDG When the reference position is set without dogs, automatic setting of
the IDGx parameter (bit 0 of parameter No.1012) to prevent the
reference position from being set again is:
0: Not performed.
1: Performed.
NOTE
When this parameter is set to 0, bit 0 (IDGx) of
parameter No. 1012 is invalid.
#7 #6 #5 #4 #3 #2 #1 #0
1004 IPR
[Input type] Parameter input
[Data type] Bit path
# 7 IPR When a number with no decimal point is specified, the least input
increment of each axis is:
0: Not 10 times greater than the least command increment
1: 10 times greater than the least command increment
When the increment system is IS-A, and bit 0 (DPI) of parameter No.
3401 is set to 1 (fixed-point format), the least input increment cannot
be 10 times greater than the least command increment.
B-63944EN/03 APPENDIX A.PARAMETERS
- 1989 -
#7 #6 #5 #4 #3 #2 #1 #0
1005 EDMx EDPx ZRNx
[Input type] Parameter input
[Data type] Bit axis
# 0 ZRNx If a move command other than G28 is specified by automatic
operation when no reference position return is performed yet after the
power is turned on:
0: The alarm (PS0224) "PERFORM REFERENCE POSITION
RETURN." is issued.
1: Operation is performed without issuing an alarm.
NOTE
1 The state in which a reference position has not
been established refers to the following state:
- When an absolute position detector is not used
and reference position return has not been
performed even once after power-up
- When an absolute position detector is used and
the association of the machine position with the
position detected with the absolute position
detector has not been completed (See the
description of bit 4 (APZx) of parameter No.
1815.)
2 When the Cs axis coordinates are to be set up, set
ZRN to 0.
# 4 EDPx In cutting feed, an external deceleration signal in the + direction for
each axis is:
0: Invalid
1: Valid
# 5 EDMx In cutting feed, an external deceleration signal in the - direction for
each axis is:
0: Invalid
1: Valid
A.PARAMETERS APPENDIX B-63944EN/03
- 1990 -
#7 #6 #5 #4 #3 #2 #1 #0
1006 ZMIx DIAx ROSx ROTx
[Input type] Parameter input
[Data type] Bit axis
NOTE
When at least one of these parameters is set, the
power must be turned off before operation is
continued.
ROTx, ROSx Setting linear or rotation axis.
ROSx ROTx Meaning
0 0 Linear axis
(1) Inch/metric conversion is done.
(2) All coordinate values are linear axis type. (Is not rounded in 0 to 360°)
(3) Stored pitch error compensation is linear axis type (Refer to parameter No.3624)
0 1 Rotation axis (A type)
(1) Inch/metric conversion is not done.
Machine coordinate values are rounded in 0 to 360°. Absolute coordinate values are rounded
or not rounded by parameter No.1008#0(ROAx) and #2(RRLx).
(2) Stored pitch error compensation is the rotation type. (Refer to parameter No.3624)
(3) Automatic reference position return (G28, G30) is done in the reference position return direction
and the move amount does not exceed one rotation.
1 1 Rotation axis (B type)
(1) Inch/metric conversion, absolute coordinate values and relative coordinate values are not done.
(2) Machine coordinate values, absolute coordinate values and relative coordinate values are
linear axis type. (Is not rounded in 0 to 360°).
(3) Stored pitch error compensation is linear axis type (Refer to parameter No.3624)
(4) Cannot be used with the rotation axis roll over function and the index table indexing function (M
series)
Except for the above. Setting is invalid (unused)
# 3 DIAx The move command for each axis is based on:
0: Radius specification
1: Diameter specification
# 5 ZMIx The direction of manual reference position return is:
0: + direction
1: - direction
B-63944EN/03 APPENDIX A.PARAMETERS
- 1991 -
#7 #6 #5 #4 #3 #2 #1 #0
1007 G90x RAAx
[Input type] Parameter input
[Data type] Bit axis
# 3 RAAx Rotary axis control is:
0: Not performed.
1: Performed.
When an absolute command is specified, the rotary axis control
function determines the direction of rotation from the sign of the
command value and determines an end coordinate from the absolute
value of the command value.
NOTE
RAA is valid when bit 0 (ROA) of parameter No. 1008
is set to 1 and bit 1 (RAB) of parameter No. 1008 is
set to 0.
To use this function, the option for rotary axis control
is required.
# 5 G90x A command for a rotary axis control (RAAx = 1) is:
0: Regarded as an absolute/incremental command according to the
G90/G91 mode setting.
1: Regarded as an absolute command at all times.
#7 #6 #5 #4 #3 #2 #1 #0
1008 RRLx RABx ROAx
[Input type] Parameter input
[Data type] Bit axis
NOTE
When at least one of these parameters is set, the
power must be turned off before operation is
continued.
# 0 ROAx The roll-over function of a rotation axis is
0: Invalid
1: Valid
NOTE
ROAx specifies the function only for a rotation axis
(for which bit 0 (ROTx) of parameter No.1006, is set
to 1)
A.PARAMETERS APPENDIX B-63944EN/03
- 1992 -
# 1 RABx In the absolute commands, the axis rotates in the direction
0: In which the distance to the target is shorter.
1: Specified by the sign of command value.
NOTE
RABx is valid only when ROAx is 1.
# 2 RRLx Relative coordinates are
0: Not rounded by the amount of the shift per one rotation
1: Rounded by the amount of the shift per one rotation
NOTE
1 RRLx is valid only when ROAx is 1.
2 Assign the amount of the shift per one rotation in
parameter No.1260.
#7 #6 #5 #4 #3 #2 #1 #0
1013 ISEx ISDx ISCx ISAx
[Input type] Parameter input
[Data type] Bit axis
NOTE
When at least one of these parameters is set, the
power must be turned off before operation is
continued.
# 0 ISA
# 1 ISC
# 2 ISD
# 3 ISE Increment system of each axis
Increment system #3 ISE #2 ISD #1 ISC #0 ISA
IS-A 0 0 0 1
IS-B 0 0 0 0
IS-C 0 0 1 0
IS-D 0 1 0 0
IS-E 1 0 0 0
#7 #6 #5 #4 #3 #2 #1 #0
1015 DWT
[Input type] Parameter input
[Data type] Bit path
# 7 DWT When time for dwell per second is specified by P, the increment
system:
0: Depends on the increment system
1: Does not depend on the increment system (1 ms)
B-63944EN/03 APPENDIX A.PARAMETERS
- 1993 -
1020 Program axis name for each axis
[Input type] Parameter input
[Data type] Byte axis
[Valid data range] 67,85 to 90
An axis name (axis name 1: parameter No. 1020) can be arbitrarily
selected from 'A', 'B', 'C', 'U', 'V', 'W', 'X', 'Y', and 'Z'. (When G code
system A is used with the lathe system, however, 'U', 'V', and 'W' are
not selectable.) When bit 0 (EEA) of parameter No. 1000 is set to 1,
the length of an axis name can be extended to three characters by
setting axis name 2 (parameter No. 1025) and axis name 3 (parameter
No. 1026) (extended axis name).
For axis names 2 and 3, a character from '0' to '9' and 'A' to 'Z' of
ASCII code can be arbitrarily selected. However, the setting of axis
name 3 for each axis is invalid if axis name 2 is not set. Moreover, if a
character from '0' to '9' is set as axis name 2, do not use a character
from 'A' to 'Z' as axis name 3.
(Tip) ASCII code
Axis name X Y Z A B C U V W
Setting 88 89 90 65 66 67 85 86 87
When G code system A is used with the lathe system, and the
character 'X','Y','Z', or 'C' is used as axis name 1 of an axis, a
command with 'U','V','W', or 'H' specified for axis name 1 represents
an incremental command for the axis.
NOTE
1 When a multiple repetitive canned cycle for turning is
used, no character other than 'X','Y', and 'Z' can be
used as the address of the axis.
2 An address other than addresses 'A', 'B', and 'C' cannot
be used as the address of a rotary axis used for the
function for tool length compensation in a specified
direction or the tool center point control function.
3 When the custom macro function is enabled, the same
extended axis name as a reserved word cannot be
used. Such an extended axis name is regarded as a
reserved word.
Because of reserved words of custom macros,
extended axis names that start with the following two
characters cannot be used:
AB,AC,AD,AN,AS,AT,AX,BC,BI,BP,CA,CL,CO,US,WH,
WR,XO
4 In a macro call, no extended axis name can be used as
an argument.
A.PARAMETERS APPENDIX B-63944EN/03
- 1994 -
1022 Setting of each axis in the basic coordinate system
[Input type] Parameter input
[Data type] Byte axis
[Valid data range] 0 to 7
To determine a plane for circular interpolation, cutter compensation,
and so forth (G17: Xp-Yp plane, G18: Zp-Xp plane, G19: Yp-Zp
plane) and a 3-dimensional tool compensation space (XpYpZp),
specify which of the basic three axes (X, Y, and Z) is used for each
control axis, or a parallel axis of which basic axis is used for each
control axis.
A basic axis (X, Y, or Z) can be specified only for one control axis.
Two or more control axes can be set as parallel axes for the same basic
axis.
Setting Meaning
0 Rotation axis (Neither the basic three axes nor a parallel axis )
1 X axis of the basic three axes
2 Y axis of the basic three axes
3 Z axis of the basic three axes
5 Axis parallel to the X axis
6 Axis parallel to the Y axis
7 Axis parallel to the Z axis
In general, the increment system and diameter/radius specification of
an axis set as a parallel axis are to be set in the same way as for the
basic three axes.
B-63944EN/03 APPENDIX A.PARAMETERS
- 1995 -
1023 Number of the servo axis for each axis
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Byte axis
[Valid data range] 0 to Number of controlled axes
Set the servo axis for each control axis.
Usually set to same number as the control axis number.
The control axis number is the order number that is used for setting
the axis-type parameters or axis-type machine signals
• With an axis for which Cs contour control/spindle positioning is
to be performed, set -(spindle number) as the servo axis number.
Example)
When exercising Cs contour control on the fourth controlled axis
by using the first spindle, set -1.
• For tandem controlled axes or electronic gear box (EGB)
controlled axes, two axes need to be specified as one pair. So,
make a setting as described below.
Tandem axis:
For a master axis, set an odd (1, 3, 5, 7, ...) servo axis number.
For a slave axis to be paired, set a value obtained by adding 1 to
the value set for the master axis.
EGB axis:
For a slave axis, set an odd (1, 3, 5, 7, ...) servo axis number. For
a dummy axis to be paired, set a value obtained by adding 1 to
the value set for the slave axis.
1025 Program axis name 2 for each axis
1026 Program axis name 3 for each axis
[Input type] Parameter input
[Data type] Byte axis
[Valid data range] 48 to 57, 65 to 90
When axis name extension is enabled (when bit 0 (EEA) of parameter
No. 1000 is set to 1), the length of an axis name can be extended to a
maximum of three characters by setting axis name 2 and axis name 3.
NOTE
If program axis name 2 is not set, program axis
name 3 is invalid.
A.PARAMETERS APPENDIX B-63944EN/03
- 1996 -
1031 Reference axis
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to Number of controlled axes
The unit of some parameters common to all axes such as those for dry
run feedrate and single-digit F1 feedrate may vary according to the
increment system. An increment system can be selected by a
parameter on an axis-by-axis basis. So, the unit of those parameters is
to match the increment system of a reference axis. Set which axis to
use as a reference axis.
Among the basic three axes, the axis with the finest increment system
is generally selected as a reference axis.
#7 #6 #5 #4 #3 #2 #1 #0
1201 FPC ZCL ZPR
[Input type] Parameter input
[Data type] Bit path
# 0 ZPR Automatic setting of a coordinate system when the manual reference
position return is performed
0: Not set automatically
1: Set automatically
NOTE
ZPR is valid while a workpiece coordinate system
function is not provided. If a workpiece coordinate
system function is provided, making a manual
reference position return always causes the
workpiece coordinate system to be established on
the basis of the workpiece zero point offset
(parameters No. 1220 to No. 1226), irrespective of
this parameter setting.
# 2 ZCL Local coordinate system when the manual reference position return is
performed
0: The local coordinate system is not canceled.
1: The local coordinate system is canceled.
NOTE
ZCL is valid when the workpiece coordinate system
option is specified. In order to use the local
coordinate system (G52), the workpiece coordinate
system option is required.
B-63944EN/03 APPENDIX A.PARAMETERS
- 1997 -
# 3 FPC When a floating reference position is set with a soft key, the relative
position indication is:
0: Not preset to 0 (The relative position indication remains
unchanged.)
1: Preset to 0.
#7 #6 #5 #4 #3 #2 #1 #0
1202 G92
[Input type] Parameter input
[Data type] Bit path
# 2 G92 When the CNC has commands G52 to G59 specifying workpiece
coordinate systems (optional function), if the G command for setting a
coordinate system (G92 for M series, G50 for T series (or the G92
command in G command system B or C)) is specified,
0: G command is executed and no alarm is issued.
1: G command is not executed and an alarm (PS0010) is issued.
1240 Coordinate value of the reference position in the machine coordinate system
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm, inch, degree (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
Set the coordinate values of the reference position in the machine
coordinate system.
A.PARAMETERS APPENDIX B-63944EN/03
- 1998 -
1241 Coordinate value of the second reference position in the machine coordinate
system
1242 Coordinate value of the third reference position in the machine coordinate
system
1243 Coordinate value of the fourth reference position in the machine coordinate
system
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm, inch, degree (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
Set the coordinate values of the second to fourth reference positions in
the machine coordinate system.
1244 Coordinate value of the floating reference position in the machine coordinate
system
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm, inch, degree (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
Set the coordinate values of the floating reference position in the
machine coordinate system.
1250 Coordinate system of the reference position used when automatic
coordinate system setting is performed
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm, inch, degree (input unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
Set the coordinate system of the reference position on each axis to be
used for setting a coordinate system automatically.
B-63944EN/03 APPENDIX A.PARAMETERS
- 1999 -
1260 The shift amount per one rotation of a rotation axis
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Real axis
[Unit of data] Degree
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 0 or positive 9 digit of minimum unit of data (refer to the standard
parameter setting table (B))
(When the increment system is IS-B, 0.0 to +999999.999)
Set the shift amount per one rotation of a rotation axis.
For the rotation axis used for cylindrical interpolation, set the standard
value.
#7 #6 #5 #4 #3 #2 #1 #0
1300 BFA NAL OUT
[Input type] Setting input
[Data type] Bit path
# 0 OUT The area inside or outside of the stored stroke check 2 is set as an
inhibition area
0: Inside
1: Outside
# 1 NAL When the tool enters the inhibition area of stored stroke limit 1:
0: The overtravel alarm signal is not output.
1: The overtravel alarm signal is output, and the tool is decelerated
to a stop.
If manual operation is in progress at this time, the alarm is not
output.
NOTE
When this parameter is set to 1, the alarm is issued
if the tool enters stored stroke limit 1 during
automatic operation.
# 7 BFA When the stored stroke check 1, 2, or 3 alarm is issued, an interference
alarm is issued with the inter-path interference check function (T
series), or a chuck/tail stock barrier (T series) alarm is issued:
0: The tool stops after entering the prohibited area.
1: The tool stops before the prohibited area.
A.PARAMETERS APPENDIX B-63944EN/03
- 2000 -
#7 #6 #5 #4 #3 #2 #1 #0
1301 OTS NPC
[Input type] Setting input
[Data type] Bit path
# 2 NPC As part of the stroke limit check performed before movement, the
movement specified in G31 (skip) and G37 (automatic tool length
measurement) blocks is:
0: Checked
1: Not checked
NOTE
This parameter is valid only when the option for
stroke limit check before movement is selected.
# 6 OTS When the overtravel alarm is issued:
0: The overtravel alarm signal is not output to the PMC.
1: The overtravel alarm signal is output to the PMC.
1320
Coordinate value I of stored stroke check 1 in the positive direction on each axis
1321
Coordinate value I of stored stroke check 1 in the negative direction on each axis
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm, inch, degree (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
Set the coordinate value of stored stroke check 1 on each axis in the +
or - direction in the machine coordinate system.
NOTE
1 Specify diameter values for any axes for which
diameter programming is specified.
2 The area outside the area set by parameter No.
1320 and No. 1321 is a prohibited area.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2001 -
1322
Coordinate value of stored stroke check 2 in the positive direction on each axis
1323
Coordinate value of stored stroke check 2 in the negative direction on each axis
[Input type] Setting input
[Data type] Real axis
[Unit of data] mm, inch, degree (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
Set the coordinate value of stored stroke check 2 on each axis in the +
or - direction in the machine coordinate system.
NOTE
1 Specify diameter values for any axes for which
diameter programming is specified.
2 Whether the inside area or outside area is a
prohibited area is set using bit 0 (OUT) of
parameter No. 1300.
1324
Coordinate value of stored stroke check 3 in the positive direction on each axis
1325
Coordinate value of stored stroke check 3 in the negative direction on each axis
[Input type] Setting input
[Data type] Real axis
[Unit of data] mm, inch, degree (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
Set the coordinate value of stored stroke check 3 on each axis in the +
or - direction in the machine coordinate system.
NOTE
1 Specify diameter values for any axes for which
diameter programming is specified.
2 The area inside the area set by parameter No.
1324 and No. 1325 is a prohibited area.
A.PARAMETERS APPENDIX B-63944EN/03
- 2002 -
1326
Coordinate value II of stored stroke check 1 in the negative direction on each axis
1327
Coordinate value II of stored stroke check 1 in the negative direction on each axis
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm, inch, degree (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
Set the coordinate value of stored stroke check 1 on each axis in the +
or - direction in the machine coordinate system.
When the stored stroke check switch signal EXLM is set to 1, or the
stored stroke check switch signal for each axis direction +EXLx is set
to 1, parameter No. 1326 and No. 1327 are used for stroke check
instead of parameter No.1320 and No. 1321.
NOTE
1 Specify diameter values for any axes for which
diameter programming is specified.
2 The area outside the area set by parameter No.
1326 and No. 1327 is a prohibited area.
3 The EXLM signal is valid only when bit 2 (LMS) of
parameter No. 1300 is set to 1.
4 The +EXLx signal is valid only when bit 0 (DLM) of
parameter No. 1301 is set to 1.
#7 #6 #5 #4 #3 #2 #1 #0
1401 RF0 LRP RPD
[Input type] Parameter input
[Data type] Bit path
# 0 RPD Manual rapid traverse during the period from power-on time to the
completion of the reference position return.
0: Disabled (Jog feed is performed.)
1: Enabled
# 1 LRP Positioning (G00)
0: Positioning is performed with non-linear type positioning so that
the tool moves along each axis independently at rapid traverse.
1: Positioning is performed with linear interpolation so that the tool
moves in a straight line.
When using three-dimensional coordinate conversion, set this
parameter to 1.
# 4 RF0 When cutting feedrate override is 0% during rapid traverse,
0: The machine tool does not stop moving.
1: The machine tool stops moving.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2003 -
#7 #6 #5 #4 #3 #2 #1 #0
1402 JRV NPC
[Input type] Parameter input
[Data type] Bit path
# 0 NPC Feed per revolution without the position coder (function for
converting feed per revolution F to feed per minute F in the feed per
revolution mode (G95)) is:
0: Not used
1: Used
# 4 JRV Jog feed or incremental feed is
0: Performed at feed per minute.
1: Performed at feed per rotation.
NOTE
1 Specify a feedrate in parameter No.1423.
2 For the machining center system, the option for
threading/synchronous feed is required.
#7 #6 #5 #4 #3 #2 #1 #0
1403 HTG
[Input type] Parameter input
[Data type] Bit path
# 5 HTG The feedrate for helical interpolation/helical involute interpolation/
three-dimensional circular interpolation is:
0: Specified using the feedrate along the tangent to an arc/involute
curve/three-dimensional arc
1: Specified using the feedrate along axes including a linear axis
(specified axes other than the circular interpolation axis in the
case of three-dimensional circular interpolation)
#7 #6 #5 #4 #3 #2 #1 #0
FM3
1404
[Input type] Parameter input
[Data type] Bit path
# 2 FM3 The increment system of an F command without a decimal point in
feed per minute is:
0: 1 mm/min (0.01 inch/min for inch input)
1: 0.001 mm/min (0.00001 inch/min for inch input)
A.PARAMETERS APPENDIX B-63944EN/03
- 2004 -
#7 #6 #5 #4 #3 #2 #1 #0
1405 FR3
[Input type] Parameter input
[Data type] Bit path
# 1 FR3 The increment system of an F command without a decimal point in
feed per revolution is:
0: 0.01 mm/rev (0.0001 inch/rev for inch input)
1: 0.001 mm/rev (0.00001 inch/rev for inch input)
#7 #6 #5 #4 #3 #2 #1 #0
1408 RFDx
[Input type] Parameter input
[Data type] Bit axis
# 0 RFDx Feedrate control on a rotation axis is exercised using:
0: Conventional method
1: Method that specifies a feedrate on the virtual circle of the
rotation axis
1410 Dry run rate
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
Set the dry run rate at the 100% position on the jog feedrate
specification dial. The unit of data depends on the increment system of
the reference axis.
1414
Feedrate for retrace
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
Set a cutting feedrate for retrace operation. When 0 is set, a retrace
operation is performed at a programmed feedrate.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2005 -
1420 Rapid traverse rate for each axis
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
Set the rapid traverse rate when the rapid traverse override is 100% for
each axis.
1421 F0 rate of rapid traverse override for each axis
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
Set the F0 rate of the rapid traverse override for each axis.
1423 Feedrate in manual continuous feed (jog feed) for each axis
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
(1) When JRV, bit 4 of parameter No.1402, is set to 0 (feed per
minute), specify a jog feedrate (feed per minute) under an
override of 100%.
(2) When JRV, bit 4 of parameter No.1402, is set to 1 (feed per
revolution), specify a jog feedrate (feed per revolution) under an
override of 100%.
NOTE
This parameter is clamped to the axis-by-axis
manual rapid traverse rate (parameter No. 1424).
A.PARAMETERS APPENDIX B-63944EN/03
- 2006 -
1424 Manual rapid traverse rate for each axis
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
Set the rate of manual rapid traverse when the rapid traverse override
is 100% for each axis.
NOTE
1 If 0 is set, the rate set in parameter 1420 (rapid
traverse rate for each axis) is assumed.
2 When manual rapid traverse is selected (bit 0 (RPD)
of parameter No. 1401 is set to 1), manual feed is
performed at the feedrate set in this parameter,
regardless of the setting of bit 4 (JRV) of parameter
No. 1402.
1425 FL rate of the reference position return for each axis
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
Set feedrate (FL rate) after deceleration when the reference position
return is performed for each axis.
1427 External deceleration rate of rapid traverse for each axis
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
Set the external deceleration rate of rapid traverse for each axis.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2007 -
1428 Reference position return feedrate for each axis
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
This parameter sets a rapid traverse rate for reference position return
operation using deceleration dogs, or for reference position return
operation before a reference position is set.
This parameter is also used to set a feedrate for the rapid traverse
command (G00) in automatic operation before a reference position is
set.
NOTE
1 To this feedrate setting (100%), a rapid traverse override (F0, 25, 50, or 100%) is
applicable.
2 For automatic return after completion of reference position return and machine
coordinate system establishment, the normal rapid traverse rate is used.
3 As a manual rapid traverse rate before machine coordinate system establishment
by reference position return, the jog feedrate or manual rapid traverse rate can be
selected with bit 0 (RPD) of parameter No. 1401.
Before coordinate system
establishment
After coordinate system
establishment
Automatic reference position return (G28) No.1428 No.1420
Automatic rapid traverse (G00) No.1428 No.1420
Manual reference position return *1 No.1428 No.1428 *3
Manual rapid traverse No.1423 *2 No.1424
4 When parameter No. 1428 is set to 0, the following parameter-set feedrates are
applied.
Before coordinate system
establishment
After coordinate system
establishment
Automatic reference position return (G28) No.1420 No.1420
Automatic rapid traverse (G00) No.1420 No.1420
Manual reference position return *1 No.1424 No.1424 *3
Manual rapid traverse No.1423 *2 No.1424
1420: rapid traverse rate
1423: Jog feedrate
1424: Manual rapid traverse rate
*1 : By using bit 2 (JZR) of parameter No. 1401, the jog feedrate can be used for
manual reference position return at all times.
*2 : When bit 0 (RPD) of parameter No. 1401 is set to 1, the setting of parameter
No. 1424 is used.
*3 : When rapid traverse is used for reference position return without dogs or
manual reference position return after reference position establishment,
regardless of the deceleration dog, the feedrate for manual reference position
return based on these functions is used (the setting of bit 1 (DLF) of parameter
No. 1404 is followed).
A.PARAMETERS APPENDIX B-63944EN/03
- 2008 -
1430 Maximum cutting feedrate for each axis
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
Specify the maximum cutting feedrate for each axis.
1432 Maximum cutting feedrate for all axes in the acceleration/deceleration before
interpolation
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
Set a maximum cutting feedrate for each axis in the
acceleration/deceleration before interpolation mode such as AI
contour control. When the acceleration/deceleration before
interpolation mode is not set, the maximum cutting feedrate set in
parameter No. 1430 is used.
1434 Maximum manual handle feedrate for each axis
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
Set a maximum manual handle feedrate for each axis in case of
maximum manual handle feedrate switch signal
HNDLF<Gn023.3>=1.
1441 External deceleration rate setting 2 for each axis in rapid traverse
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
Set external deceleration rate 2 for each axis in rapid traverse.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2009 -
1444 External deceleration rate setting 3 for each axis in rapid traverse
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
Set external deceleration rate 3 for each axis in rapid traverse.
1450 Change of feedrate for one graduation on the manual pulse generator during
one-digit F feed code
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to 127
Set the constant that determines the change in feedrate as the manual
pulse generator is rotated one graduation during one-digit F feed code.
n
iF
F100
max
=∆ (where, i=1 or 2)
In the above equation, set n. That is, the number of revolutions
of the manual pulse generator, required to reach feedrate Fmaxi is
obtained. Fmaxi refers to the upper limit of the feedrate for a one-digit
F code feed command, and set it in parameters No. 1460 or No. 1461.
Fmax1: Upper limit of the feedrate for F1 to F4 (parameter No. 1460)
Fmax2: Upper limit of the feedrate for F5 to F9 (parameter No. 1461)
1451
Feedrate for F1
to to
1459
Feedrate for F9
[Input type] Setting input
[Data type] Real path
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
These parameters set the feedrates for one-digit F code feed
commands F1 to F9. When a one-digit F code feed command is
specified, and the feedrate is changed by turning the manual pulse
generator, the parameter-set value also changes accordingly.
A.PARAMETERS APPENDIX B-63944EN/03
- 2010 -
1460
Upper limit of feedrate for F1 to F4
1461
Upper limit of feedrate for F5 to F9
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
Set the upper limit of feedrate for the one-digit F code feed command.
As the feedrate increases by turning the manual pulse generator, the
feedrate is clamped when it reaches the upper limit set. If a one-digit F
feed command F1 to F4 is executed, the upper limit is that set in
parameter No. 1460. If a one-digit F code feed command F5 to F9 is
executed, the upper limit is that set in parameter No. 1461.
1465 Radius of a virtual circle when a feedrate is specified on the virtual circle of a
rotation axis
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm, inch (input unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (B)
Set the radius of a virtual circle when a feedrate on the virtual circle of
a rotation axis is specified.
If 0 is set for a rotation axis, the axis is excluded from feedrate
calculation.
If the input unit is the inch, enter a value in inches.
The data is then converted to a millimeter value and displayed.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2011 -
#7 #6 #5 #4 #3 #2 #1 #0
1490 PGF
[Data type] Bit path
# 7 PGF The feedrate specified for circular interpolation, involute interpolation,
spiral/conical interpolation, and NURBS interpolation in the
high-speed program check mode is:
0: The dry run feedrate.
At this time, manual feedrate override signals *JV0 to *JV15
<Gn010 to Gn011> can be used.
1: The maximum feedrate specified by the CNC.
CAUTION
If this parameter is set to 1, feedrate clamp,
override, and dry run for circular interpolation,
involute interpolation, spiral/conical interpolation,
and NURBS interpolation are disabled. If a
movement around a stroke limit is specified,
therefore, a stroke limit check cannot sometimes
be made correctly.
#7 #6 #5 #4 #3 #2 #1 #0
1601 NCI
[Input type] Parameter input
[Data type] Bit path
# 5 NCI An in-position check:
0: Confirms that the specified feedrate becomes 0 (the
acceleration/deceleration delay becomes 0) at deceleration time
and that the machine position has reached a specified position
(the servo positional deviation is within the in-position width set
by parameter No. 1826).
1: Confirms only that the specified feedrate becomes 0 (the
acceleration/deceleration delay becomes 0) at deceleration time.
#7 #6 #5 #4 #3 #2 #1 #0
1604 SHP
[Input type] Parameter input
[Data type] Bit path
# 0 SHP When automatic operation is started, the state equivalent to the
specification of G5.1Q1 for AI contour control is:
0: Not set
1: Set
Upon reset, the state where G5.1Q1 is specified is set.
A.PARAMETERS APPENDIX B-63944EN/03
- 2012 -
#7 #6 #5 #4 #3 #2 #1 #0
1606 MNJx
[Input type] Parameter input
[Data type] Bit axis
# 0 MNJx In manual handle interrupt or automatic manual simultaneous
operation (interrupt type):
0: Only cutting feed acceleration/deceleration is enabled, and jog
feed acceleration/deceleration is disabled.
1: Both cutting feed acceleration/deceleration and jog feed
acceleration/deceleration are applied.
#7 #6 #5 #4 #3 #2 #1 #0
1610 CTBx CTLx
[Input type] Parameter input
[Data type] Bit axis
# 0 CTLx Acceleration/deceleration in cutting feed or dry run
0: Exponential acceleration/deceleration is applied.
1: Linear acceleration/deceleration after interpolation is applied.
# 1 CTBx Acceleration/deceleration in cutting feed or dry run
0: Exponential acceleration/deceleration or linear acceleration/
deceleration is applied.
(depending on the setting in CTLx, bit 0 of parameter No.1610)
1: Bell-shaped acceleration/deceleration is applied.
1620 Time constant T or T1 used for linear acceleration/deceleration or
bell-shaped acceleration/deceleration in rapid traverse for each axis
[Input type] Parameter input
[Data type] Word axis
[Unit of data] msec
[Valid data range] 0 to 4000
Specify a time constant used for acceleration/deceleration in rapid
traverse.
[Example]
For linear acceleration/deceleration
Speed Rapid traverse rate
(Parameter No. 1420)
Time
TT
T : Setting of parameter No. 1620
B-63944EN/03 APPENDIX A.PARAMETERS
- 2013 -
For bell-shaped acceleration/deceleration
Speed Rapid traverse rate
(Parameter No. 1420)
Time
T1
T2 T2T2T2
T1
T1 : Setting of parameter No. 1620
T2 : Setting of parameter No. 1621
(However, T1 ≥ T2 must be satisfied.)
Total acceleration (deceleration) time : T1 + T2
Time for linear portion : T1‐T2
Time for curve portion : T2 × 2
1622 Time constant of acceleration/deceleration in cutting feed for each axis
[Input type] Parameter input
[Data type] Word axis
[Unit of data] msec
[Valid data range] 0 to 4000
Set the time constant used for exponential acceleration/deceleration in
cutting feed, bell-shaped acceleration/deceleration after interpolation
or linear acceleration/deceleration after interpolation in cutting feed
for each axis. Which type to use is selected with bits 1(CTBx) and
0(CTLx) of parameter No.1610. Except for special applications, the
same time constant must be set for all axes in this parameter. If the
time constants set for the axes differ from each other, proper straight
lines and arcs cannot be obtained.
1624 Time constant of acceleration/deceleration in jog feed for each axis.
[Input type] Parameter input
[Data type] Word axis
[Unit of data] msec
[Valid data range] 0 to 4000
Set the time constant used for acceleration/deceleration in jog feed for
each axis.
A.PARAMETERS APPENDIX B-63944EN/03
- 2014 -
1660 Maximum allowable acceleration rate in acceleration/deceleration before
interpolation for each axis
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/sec2, inch/sec2, degree/sec2 (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (D)
(When the machine system is metric system, 0.0 to +100000.0. When
the machine system is inch system, machine, 0.0 to +10000.0.)
Set a maximum allowable acceleration rate in acceleration/
deceleration before interpolation for each axis.
If a value greater than 100000.0 is set, the value is clamped to
100000.0.
If 0 is set, the specification of 100000.0 is assumed. If 0 is set for all
axes, however, acceleration/deceleration before interpolation is not
performed.
If a maximum allowable acceleration rate set for one axis is greater
than a maximum allowable acceleration rate set for another axis by a
factor or 2 or more, the feedrate at a corner where the direction of
travel abruptly changes can decrease temporarily.
1671
Maximum allowable acceleration rate in acceleration/deceleration before
interpolation for linear rapid traverse for each axis, or maximum allowable
reference acceleration rate in optimum torque acceleration/deceleration
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/sec2, inch/sec2, degree/sec2 (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (D)
(When the machine system is metric system, 0.0 to +100000.0. When
the machine system is inch system, machine, 0.0 to +10000.0.)
(1) Set a maximum allowable acceleration rate in acceleration/
deceleration before interpolation for linear rapid traverse.
If a value greater than 100000.0, the value is clamped to
100000.0.
If 0 is set, the specification of the following is assumed:
1000.0 mm/sec2
100.0 inch/sec2
100.0 degrees/sec2
If 0 is specified for all axes, however, acceleration/deceleration
before interpolation is not performed.
(2) Maximum allowable reference acceleration rate in optimum
torque acceleration/deceleration
B-63944EN/03 APPENDIX A.PARAMETERS
- 2015 -
1672
Acceleration change time of bell-shaped acceleration/deceleration before
interpolation for linear rapid traverse, or acceleration change time of
bell-shaped acceleration/deceleration in optimum torque
acceleration/deceleration
[Input type] Parameter input
[Data type] 2-word path
[Unit of data] msec
[Valid data range] 0 to 200
(1) Set an acceleration change time of bell-shaped acceleration/
deceleration for linear rapid traverse (time for changing from the
state of constant feedrate (A) to the state of constant
acceleration/deceleration (C) at the acceleration rate calculated
from the acceleration rate set in parameter No. 1671: time of (B)
in the figure below).
(2) Set an acceleration change time of bell-shaped acceleration/
deceleration in optimum torque acceleration/deceleration (time
for changing from the state of constant feedrate (A) to the state of
acceleration/deceleration (C) at the acceleration rate calculated
from optimum torque acceleration/deceleration: time of (B) in
the figure below).
Feedrate in tangent direction Maximum acceleration rate not
exceeding maximum allowable
acceleration rate set by parameter
No. 1671 for each axis is
automatically calculated.
Time set by parameter No. 1672
(A) (B) (B) (B) (B) (A) (A) (C) (C)
A.PARAMETERS APPENDIX B-63944EN/03
- 2016 -
1710 Minimum deceleration ratio (MDR) for inner circular cutting feedrate change
by automatic corner override
[Input type] Parameter input
[Data type] Byte path
[Unit of data] %
[Valid data range] 0 to 100
Set a minimum deceleration ratio (MDR) for an inner circular cutting
feedrate change by automatic corner override.
In the case of circular cutting offset inward, the actual feedrate is
determined by a specified feedrate (F) as follows:
Thus, the feedrate along the programmed path satisfies the specified
value of F.
Programmed path
Tool center path
Rc
Rp
However, if Rc is too small when compared with Rp, Rc/Rp 0
results to stop the tool. So, a minimum deceleration ratio (MDR) is set,
and the feedrate of the tool is set to F×(MDR) when Rc/Rp ≤ MDR.
1711 Inner determination angle (θp) for inner corner override
[Input type] Parameter input
[Data type] Real path
[Unit of data] deg
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 2 to 178
Set an inner determination angle for inner corner override in automatic
corner overriding.
1712 Override value for inner corner override
[Input type] Parameter input
[Data type] Byte path
[Unit of data] %
[Valid data range] 1 to 100
Set an inner corner override value in automatic corner overriding.
Rp
Rc
F×Rc:Radius of tool center
path
Rp:Programmed radius
B-63944EN/03 APPENDIX A.PARAMETERS
- 2017 -
1713 Start distance (Le) for inner corner override
[Input type] Setting input
[Data type] Real path
[Unit of data] mm, inch (input unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
Set a start distance for inner corner override in automatic corner
overriding.
1714 End distance (Ls) for inner corner override
[Input type] Setting input
[Data type] Real path
[Unit of data] mm, inch (input unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
Set an end distance for inner corner override in automatic corner
overriding.
When θ ≤ θp, an inner corner is assumed. (Parameter No. 1711 is used
to set θp.)
When a corner is determined to be an inner corner, an override is
applied to the feedrate in the range of Le in the previous block from
the intersection of the corner and in the range of Ls in the next block
from the intersection of the corner.
Distances Le and Ls represent linear distances from the intersection of
a corner to points on the tool center path.
Le and Ls are set in parameter No. 1713 and No. 1714.
Programmed path
Tool center path
A
n override is applied to the range from point a to point b.
A.PARAMETERS APPENDIX B-63944EN/03
- 2018 -
1732 Minimum allowable feedrate for the deceleration function based on
acceleration in circular interpolation
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
With the deceleration function based on acceleration in circular
interpolation, an optimum feedrate is automatically calculated so that
acceleration produced by changing the move direction in circular
interpolation does not exceed the maximum allowable acceleration
rate specified in parameter No. 1735.
If the radius of an arc is very small, a calculated feedrate may become
too low.
In such a case, the feedrate is prevented from decreasing below the
value specified in this parameter.
NOTE
During involute interpolation, the minimum
allowable feedrate of "clamping of acceleration
near a basic circle" in involute interpolation
automatic feedrate control is used.
1735 Maximum allowable acceleration rate for the deceleration function based on
acceleration in circular interpolation for each axis
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/sec2, inch/sec2, degree/sec2 (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (D)
(When the machine system is metric system, 0.0 to +100000.0. When
the machine system is inch system, machine, 0.0 to +10000.0.)
Set a maximum allowable acceleration rate for the deceleration
function based on acceleration in circular interpolation.
Feedrate is controlled so that acceleration produced by changing the
move direction in circular interpolation does not exceed the value
specified in this parameter.
For an axis with 0 set in this parameter, the deceleration function
based on acceleration is disabled.
If a different value is set in this parameter for each axis, a feedrate is
determined from the smaller of the acceleration rates specified for the
two circular axes.
NOTE
During involute interpolation, the minimum
allowable feedrate of "clamping of acceleration
near a basic circle" in involute interpolation
automatic feedrate control is used.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2019 -
1737 Maximum allowable acceleration rate for the deceleration function based on
acceleration in AI contour control for each axis
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/sec2, inch/sec2, degree/sec2 (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (D)
(When the machine system is metric system, 0.0 to +100000.0. When
the machine system is inch system, machine, 0.0 to +10000.0.)
Set a maximum allowable acceleration rate produced by changing the
tool move direction.
For an axis with 0 set in this parameter, the deceleration function
based on acceleration is disabled. If 0 is set for all axes, the
deceleration function based on acceleration is not performed.
In circular interpolation, however, the deceleration function based on
feedrate control using acceleration in circular interpolation (parameter
No. 1735) is enabled.
1738 Minimum allowable feedrate for the deceleration function based on
acceleration in AI contour control
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
With the deceleration function based on acceleration in AI contour
control, a feedrate most suitable for a desired figure is automatically
calculated.
Depending on the figure, however, the calculated feedrate may
become too low.
In such a case, the feedrate is prevented from decreasing below the
value specified in this parameter.
If overriding using the deceleration function based on cutting load is
enabled, a feedrate lower than the minimum allowable feedrate may
be used.
1769 Time constant for acceleration/deceleration after cutting feed interpolation in
the acceleration/deceleration before interpolation mode
[Input type] Parameter input
[Data type] Word axis
[Unit of data] msec
[Valid data range] 0 to 4000
In the acceleration/deceleration before interpolation mode as in AI
contour control, not the ordinary time constant (parameter No. 1622)
but the value of this parameter is used.
Be sure to specify the same time constant value for all axes except for
a special application. If different values are set, correct linear and
circular figures cannot be obtained.
A.PARAMETERS APPENDIX B-63944EN/03
- 2020 -
1772 Acceleration change time of bell-shaped acceleration/deceleration before
interpolation
[Input type] Parameter input
[Data type] 2-word path
[Unit of data] msec
[Valid data range] 0 to 200
Set an acceleration change time of bell-shaped acceleration/
deceleration before interpolation (time for changing from the state of
constant feedrate (A) to the state of constant acceleration/deceleration
(C) at the acceleration rate calculated from the acceleration rate set in
parameter No. 1660: time of (B) in the figure below).
Feedrate in tangent direction
Optimum inclination is
automatically calculated from the
setting of parameter No. 1660.
Time set by parameter No. 1772
(A) (B) (B) (B) (B)(A) (A) (C) (C)
1783 Maximum allowable feedrate difference for feedrate determination based on
corner feedrate difference
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
If a feedrate component change for each axis exceeding the value set
in this parameter occurs at the joint of blocks, the feedrate
determination function based on corner feedrate difference finds a
feedrate not exceeding the set value and performs deceleration by
using acceleration/deceleration before interpolation. Thus, a shock to
the machine and machining error at a corner can be reduced.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2021 -
1788 Maximum allowable acceleration change rate in feedrate determination
based on acceleration change for each axis
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/sec2, inch/sec2, degree/sec2 (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (D)
(When the machine system is metric system, 0.0 to +100000.0. When
the machine system is inch system, machine, 0.0 to +10000.0.)
Set a maximum allowable acceleration change rate for each axis in
feedrate control based on acceleration change under control on the rate
of change of acceleration.
For an axis with 0 set in this parameter, feedrate control based on
acceleration change is disabled.
If 0 is set for all axes, feedrate control based on acceleration change is
not exercised.
1789 Maximum allowable acceleration change rate in feedrate determination
based on acceleration change for each axis (linear interpolation)
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/sec2, inch/sec2, degree/sec2 (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (D)
(When the machine system is metric system, 0.0 to +100000.0. When
the machine system is inch system, machine, 0.0 to +10000.0.)
Set a maximum allowable acceleration change rate for each axis in
feedrate control based on acceleration change under control on the rate
of change of acceleration in successive linear interpolation operations.
In feedrate control based on acceleration change at a corner between
linear interpolation operations, the maximum allowable acceleration
change rate not set in parameter No. 1788 but set in this parameter is
valid.
For an axis with 0 set in this parameter, the maximum allowable
acceleration change rate set in parameter No. 1788 is valid.
Feedrate control based on acceleration change is disabled for an axis
with 0 set in parameter No. 1788, so that the setting of this parameter
for such an axis is ignored.
A.PARAMETERS APPENDIX B-63944EN/03
- 2022 -
1790 Ratio of change time of the rate of change of acceleration in smooth
bell-shaped acceleration/deceleration before interpolation
[Input type] Parameter input
[Data type] Byte path
[Unit of data] %
[Valid data range] 0 to 50
Set the ratio of the change time of the rate of change of acceleration to
the change time of acceleration(*1) by percentage (%) in smooth
bell-shaped acceleration/deceleration before look-ahead interpolation.
If 0 is set in this parameter or a value not within the valid data range is
specified in this parameter, smooth bell-shaped acceleration/
deceleration before look-ahead interpolation is not performed.
(*1) Parameter No. 1772 for acceleration/deceleration before
look-ahead interpolation (cutting feed).
Parameter No. 1672 for acceleration/deceleration before
interpolation in linear rapid traverse, or for optimum torque
acceleration/ deceleration.
#7 #6 #5 #4 #3 #2 #1 #0
1802 DC2x DC4x
[Input type] Parameter input
[Data type] Bit axis
# 1 DC4x When the reference position is established on the linear scale with
reference marks:
0: An absolute position is established by detecting three reference
marks.
1: An absolute position is established by detecting four reference
marks.
# 2 DC2x Reference position establishment operation for a linear scale with
reference marks is performed as follows:
0: The setting of bit 1 (DC4) of parameter No. 1802 is followed.
1: An absolute position is established by detecting two
reference marks.
NOTE
1 When this parameter is set to 1, specify the
direction of the scale zero point by setting bit 4
(SCP) of parameter No. 1817.
2 When a rotary encoder with absolute address
reference marks is used, this parameter is invalid.
Even when this parameter is set to 1, the setting of
bit 1 (DC4) of parameter No. 1802 is followed.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2023 -
#7 #6 #5 #4 #3 #2 #1 #0
1815 APCx APZx DCRx OPTx
[Input type] Parameter input
[Data type] Bit axis
NOTE
When at least one of these parameters is set, the
power must be turned off before operation is
continued.
# 1 OPTx Position detector
0: A separate pulse coder is not used.
1: A separate pulse coder is used.
NOTE
Set this parameter to 1 when using a linear scale
with reference marks or a linear scale with an
absolute address zero point (full-closed system).
# 3 DCRx As a scale with absolute address reference marks:
0: A rotary encoder with absolute address reference marks is not
used.
1: A rotary encoder with absolute address reference marks is used.
NOTE
When using a rotary encoder with absolute address
reference marks, set also bit 2 (DCLx) of parameter
No. 1815 to 1.
# 4 APZx Machine position and position on absolute position detector when the
absolute position detector is used
0: Not corresponding
1: Corresponding
When an absolute position detector is used, after primary adjustment
is performed or after the absolute position detector is replaced, this
parameter must be set to 0, power must be turned off and on, then
manual reference position return must be performed. This completes
the positional correspondence between the machine position and the
position on the absolute position detector, and sets this parameter to 1
automatically.
# 5 APCx Position detector
0: Other than absolute position detector
1: Absolute position detector (absolute pulse coder)
A.PARAMETERS APPENDIX B-63944EN/03
- 2024 -
#7 #6 #5 #4 #3 #2 #1 #0
1817 TANx
[Input type] Parameter input
[Data type] Bit axis
NOTE
When this parameter is set, the power must be
turned off before operation is continued..
# 6 TANx Tandem control
0: Not used
1: Used
NOTE
Set this parameter to both master axis and slave
axis.
#7 #6 #5 #4 #3 #2 #1 #0
1818 SDC RF2x RFSx
[Input type] Parameter input
[Data type] Bit axis
# 0 RFSx If G28 is specified for an axis for which a reference position is not
established (ZRF = 0) when a linear scale with an absolute address
zero point or a linear scale with absolute address reference marks is
used:
0: A movement is made to the reference position after reference
position establishment operation.
1: No movement is made after reference position
establishment operation, but the operation is completed.
NOTE
This parameter disables movement based on the
G28 command to a reference position. So, use this
parameter only in special cases.
# 1 RF2x If G28 is specified for an axis for which a reference position is already
established (ZRF = 1) when a linear scale with an absolute address
zero point or a linear scale with absolute address reference marks is
used:
0: A movement is made to the reference position.
1: No movement is made to the intermediate position and
reference position, but the operation is completed.
NOTE
This parameter disables movement based on the
G28 command to a reference position. So, use this
parameter only in special cases.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2025 -
# 3 SDCx A linear scale with an absolute address zero point is:
0: Not used.
1: Used.
#7 #6 #5 #4 #3 #2 #1 #0
1819 DATx
[Input type] Parameter input
[Data type] Bit axis
# 2 DATx When a linear scale with an absolute address zero point or a linear
scale with absolute address reference marks is used, the automatic
setting of parameter No. 1883 and No. 1884 at manual reference
position return time is:
0: Not performed.
1: Performed.
The automatic setting procedure is as follows:
<1> Set an appropriate value in parameter No. 1815, No. 1821, and
No. 1882.
<2> Position the machine at the reference position by manual
operation.
<3> Set this parameter to 1.
<4> Perform a manual reference position return operation. Upon
completion of manual reference position return operation,
parameter No. 1883 and No. 1884 are set, and this parameter is
automatically set to 0.
A.PARAMETERS APPENDIX B-63944EN/03
- 2026 -
1820 Command multiplier for each axis (CMR)
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Byte axis
[Valid data range] See below :
Set a command multiplier indicating the ratio of the least command
increment to the detection unit for each axis.
Least command increment = detection unit × command multiplier
Relationship between the increment system and the least command
increment
(1) T series
Least input increment Least command
increment
0.001 mm (diameter specification) 0.0005 mm Millimeter
input 0.001 mm (radius specification) 0.001 mm
0.0001 inch (diameter specification) 0.0005 mm
Millimeter
machine Inch input 0.0001 inch (radius specification) 0.001 mm
0.001 mm (diameter specification) 0.00005 inch Millimeter
input 0.001 mm (radius specification) 0.0001 inch
0.0001 inch (diameter specification) 0.00005 inch
Inch
machine Inch input 0.0001 inch (radius specification) 0.0001 inch
IS-B
Rotation axis 0.001 deg 0.001 deg
Least input increment Least command
increment
0.0001 mm (diameter specification) 0.00005 mm Millimeter
input 0.0001 mm (radius specification) 0.0001 mm
0.00001 inch (diameter specification) 0.00005 mm
Millimeter
machine Inch input 0.00001 inch (radius specification) 0.0001 mm
0.0001 mm (diameter specification) 0.000005 inch Millimeter
input 0.0001 mm (radius specification) 0.00001 inch
0.00001 inch (diameter specification) 0.000005 inch
Inch
machine Inch input 0.00001 inch (radius specification) 0.00001 inch
IS-C
Rotation axis 0.0001 deg 0.0001 deg
Least input increment Least command
increment
0.00001 mm (diameter specification) 0.000005 mm Millimeter
input 0.00001 mm (radius specification) 0.00001 mm
0.000001 inch (diameter specification) 0.000005 mm
Millimeter
machine Inch input 0.000001 inch (radius specification) 0.00001 mm
0.00001 mm (diameter specification) 0.0000005 inch Millimeter
input 0.00001 mm (radius specification) 0.000001 inch
0.000001 inch (diameter specification) 0.0000005 inch
Inch
machine Inch input 0.000001 inch (radius specification) 0.000001 inch
IS-D
Rotation axis 0.00001 deg 0.00001 deg
B-63944EN/03 APPENDIX A.PARAMETERS
- 2027 -
Least input increment Least command
increment
0.000001 mm (diameter specification) 0.0000005 mm Millimeter
input 0.000001 mm (radius specification) 0.000001 mm
0.0000001 inch (diameter specification) 0.0000005 mm
Millimeter
machine Inch input 0.0000001 inch (radius specification) 0.000001 mm
0.000001 mm (diameter specification) 0.00000005 inchMillimeter
input 0.000001 mm (radius specification) 0.0000001 inch
0.0000001 inch (diameter specification) 0.00000005 inch
Inch
machine Inch input 0.0000001 inch (radius specification) 0.0000001 inch
IS-E
Rotation axis 0.000001 deg 0.000001 deg
(2) M series
Least input increment and least command increment Increment
system IS-A IS-B IS-C IS-D IS-E Unit
Millimeter
machine 0.01 0.001 0.0001 0.00001 0.000001 mm
Millimeter
input 0.001 0.0001 0.00001 0.000001 0.0000001 inch
Rotation
axis 0.01 0.001 0.0001 0.00001 0.000001 deg
Setting command multiply (CMR), detection multiply (DMR), and the
capacity of the reference counter
least
command
increment
×CMR Error counter DA
Converter
×DMR Position
detector
Reference counter
Command pulse
Feedback
pulse
Detection
unit
To
velocity
control
-
+
Set CMR and DMR so that the pulse weight of + input (command
from the CNC) into the error counter matches the pulse weight of
-input (feedback from the position detector).
[Least command increment]/CMR=[Detection unit]=
[Feedback pulse unit]/DMR
[Least command increment]:
Minimum unit of commands issued from the CNC to the
machine
[Detection unit]: Minimum unit for machine position detection
The unit of feedback pulses varies, depending on the type of detector.
[Feedback pulse unit]=[Amount of travel per rotation of the pulse
coder]/[Number of pulses per rotation of the pulse coder]
A.PARAMETERS APPENDIX B-63944EN/03
- 2028 -
As the size of the reference counter, specify the grid interval for the
reference position return in the grid method.
[Size of the reference counter]=[Grid interval]/[Detection unit]
[Grid interval]=[Amount of travel per rotation of the pulse coder]
The setting of a command multiplier is as follows:
(1) When command multiplier is 1 to 1/27
Set value = 1 / command multiplier + 100
Valid data range : 101 to 127
(2) When command multiply is 0.5 to 48
Set value = 2 × command multiplier
Valid data range : 1 to 96
NOTE
If a feedrate exceeding the feedrate found by the
expression below is used, an incorrect travel
amount may result or a servo alarm may be issued.
Be sure to use a feedrate not exceeding the
feedrate found by the following expression:
Fmax[mm/min] = 196602 × 104 × least command
increment / CMR
1821 Reference counter size for each axis
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] 2-word axis
[Unit of data] Detection unit
[Valid data range] 0 to 999999999
Set a reference counter size.
As a reference counter size, specify a grid interval for reference
position return based on the grid method.
When a value less than 0 is set, the specification of 10000 is assumed.
When a linear scale with absolute address reference marks is used, set
the interval of mark 1.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2029 -
1828 Positioning deviation limit for each axis in movement
[Input type] Parameter input
[Data type] 2-word axis
[Unit of data] Detection unit
[Valid data range] 0 to 99999999
Set the positioning deviation limit in movement for each axis.
If the positioning deviation exceeds the positioning deviation limit
during movement, a servo alarm (SV0411) is generated, and operation
is stopped immediately (as in emergency stop).
Generally, set the positioning deviation for rapid traverse plus some
margin in this parameter.
1829 Positioning deviation limit for each axis in the stopped state
[Input type] Parameter input
[Data type] 2-word axis
[Unit of data] Detection unit
[Valid data range] 0 to 99999999
Set the positioning deviation limit in the stopped state for each axis.
If, in the stopped state, the positioning deviation exceeds the
positioning deviation limit set for stopped state, a servo alarm
(SV0410) is generated, and operation is stopped immediately (as in
emergency stop).
1838 Position deviarion limit for each axis in moving during safety check
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Paramete input
[Data type] 2-word axis
[Unit of data] Detection unit
[Valid data range] 0 to 99999999
Position deviation limit for each axis during moving for safety check
of Dual Check Safety function is specified.
If position deviation of a moving axis exceeds position deviation limit
while Safety Check is carried out (Safety Monitoring Request
“*VLDVx” =0), a servo alarm SV0475 or SV1071 is generated and
axes are stopped immediately like emergency stop state..
In Dual Check Safety function, positin deviation is always checked by
CNC and Servo. In case that Safety Check is carried out (Safety
Monitoring Request “*VLDVx” =0), the servo alarm SV0475 or
SV1071 is generated when each CPU finds out that the deviation
exceeds position deviation limit in moving state.
A.PARAMETERS APPENDIX B-63944EN/03
- 2030 -
1841 Position deviation limit of each axis in moving state during other than Dual Check
Safety monitoring (for Dual Check Safety Function)
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] 2 word axis
[Unit of data] Detection unit
[Valid data range] 0 to 99999999
Set the positioning deviation limit in moving state for each axis for
Dual Check Safety function, in case that Safety Check is not carried
out (Safety Monitoring Request “*VLDVx”=1).
In case that Safety Check is not carried out (Safety Monitoring
Request “*VLDVx” =1), servo alarm (SV0475,SV1071) is generated
and operation is stopped immediately (as in emergency stop), when
each CPU finds out that the deviation exceeds position deviation limit
in moving state.
If the value of this parameter is “0”, the parameter No.1828 is used for
the value of deviation limit in moving state.
In case that Safety Check is carried out (Safety Monitoring Request
“*VLDVx” =0), the parameter No.1838 is used for the value of
deviation limit in moving state.
1851 Backlash compensating value for each axis
[Input type] Parameter input
[Data type] Word axis
[Unit of data] Detection unit
[Valid data range] -9999 to 9999
Set the backlash compensating value for each axis.
When the machine moves in a direction opposite to the reference
position return direction after the power is turned on, the first backlash
compensation is performed.
1882 Interval of mark 2 of a linear scale with absolute address reference marks
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] 2-word axis
[Unit of data] Detection unit
[Valid data range] 0 to 999999999
Set the interval of mark 2 of a linear scale with absolute address
reference marks.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2031 -
1883
Distance 1 from the scale zero point to reference position (linear scale with
absolute address reference marks) or
distance 1 from the base point to reference position (linear scale with an
absolute address zero point)
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] 2-word axis
[Unit of data] Detection unit
[Valid data range] -999999999 to 999999999
1884
Distance 2 from the scale zero point to reference position (linear scale with
absolute address reference marks) or distance 2 from the base point to
reference position (linear scale with an absolute address zero point)
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] 2-word axis
[Unit of data] Detection unit
[Valid data range] -999 to 999
When a linear scale with absolute address reference marks is used, set
the distance from the scale zero point to reference position in
parameter Nos. 1883 and 1884).
Distance from the zero point to the reference position of a linear
scale
= No. 1884 × 1,000,000,000 + No. 1883
The scale zero point represents a point where mark 1 and mark 2
match. Usually, this point is a virtual point that does not physically
exist on the scale. (See the figure below.)
If the reference position is placed in the + direction when viewed from
the scale zero point, set a positive value. If the reference position is
placed in the - direction when viewed from the scale zero point, set a
negative value.
A.PARAMETERS APPENDIX B-63944EN/03
- 2032 -
Mark 1 Mark 2 Mark 1 Mark 2
Zero point of encoder Encoder end Reference position
……..
Mark 1 = mark 2
41.8
8.242.0
8.0
Parameter No.1821
Parameter No.1882
Parameter No.1884
×
1,000,000,000 + Parameter No.1823
[Example of parameter settings] When an encoder as shown below is used with an IS-B, millimeter
machine:
20.000 19.980 9.940 10.060 9.960 10.040 9.980 10.020
5.000 20.000mm
20.020mm -
[
9960/
(
20020-20000
)
*20000+5000
]
= -9965000
Mark 1
Mark 2Mark 1 Mark 2 Mark 1
Mark 1Mark 2 Mark 1 Mark 1Mark 2
Mark 1 = mark 2
B
A
Scale zero point + direction - direction
Reference position
Parameters
No.1821 (interval of mark 1) = 20000
No.1882 (interval of mark 2) = 20020
No.1883 (reference position) = position of point A + 5.000
= distance between A and B/(mark 2 − mark 1) × mark 1 + 5000
= 9960/(20020-20000) × 20000 + 5000
= 9965000
= -9965000 (the reference position is on the negative side)
[Setting parameter No. 1883]
When it is difficult to measure the distance from the scale zero point
to the reference position (parameter No. 1883), the method described
below can be used to find the distance.
<1> Set parameter No. 1815 to enable this function.
Set an appropriate value in parameter No. 1821 and No. 1882.
Set 0 in parameter No. 1240.
Set 0 in parameter No. 1883 and No. 1884.
<2> At an appropriate position, establish a reference position.
(As a result, the machine coordinate represents the distance from
the scale zero point to the current position.)
B-63944EN/03 APPENDIX A.PARAMETERS
- 2033 -
<3> By jog feed or handle feed, place the machine at the accurate
reference position.
<4> In parameter No. 1883, set the machine coordinate of that time
converted to the detection unit (machine coordinate × CMR).
<5> If necessary, set parameter No. 1240.
When a linear scale with an absolute address zero point is used, set the
distance from the base point to the reference position in parameter
Nos. 1883 and 1884. The base point is a point at a scale end as shown
below.
If the reference position is located in the positive direction when
viewed from the base point, set a positive value; if the reference
position is located in the negative direction, set a negative value. Set
the value by following the steps explained below.
<1> Set bit 1 (OPT) of parameter No. 1815 , bit 2 (DCL) of parameter
No. 1815, and bit 3 (SDC) of parameter No. 1818 to enable this
function.
Set 0 in parameter No. 1240.
Set 0 in parameter No. 1883 and No. 1884.
<2> At an appropriate position, establish a reference position.
(Consequently, the machine coordinate value indicates the
distance from the base point to current position.)
<3> By jog feed or handle feed, place the machine at the accurate
reference position.
<4> In parameters Nos. 1883 and 1884, set the machine coordinate of
that time converted to the detection unit (machine coordinate ×
CMR).
If necessary, set parameter No. 1240.
NOTE
1 Set parameter Nos. 1883 and 1884 so that the distance from the scale zero point
(for a linear scale with absolute address reference marks) or the base point (for a
linear scale with an absolute address zero point) to the reference position is within
the range from -999,999,999,999 to +999,999,999,999. If a value beyond this range
is set, an alarm (PS 5325) is issued.
2 The scale area on the scale cannot be extended across the scale zero point or
base point. Make parameter settings not to cause the scale area to extend beyond
the scale zero point or base point.
Mark 1 Mark 2 Mark 1
Mark 2Mark 1Mark 1 Mark 2
Reference position
10.020 9.980 10.040 9.960 10.060 9.940
Base point
20.000
20.020
A.PARAMETERS APPENDIX B-63944EN/03
- 2034 -
#7 #6 #5 #4 #3 #2 #1 #0
1902 ASE FMD
[Input type] Parameter input
[Data type] Bit
NOTE
When at least one of these parameters is set, the
power must be turned off before operation is
continued.
# 0 FMD The FSSB setting mode is:
0: Automatic setting mode.
(When the relationship between an axis and amplifier is defined
on the FSSB setting screen, parameter Nos. 1023, 1905, 1936 to
1939, and 14340 to 14407 (plus parameter Nos. 14408 to 14425
and 14444 to 14459 if an additional axis board is attached) are
automatically set.
1: Manual setting 2 mode.
(Parameter Nos. 1023, 1905, 1936 to 1939 and 14340 to 14407
(plus parameter Nos. 14408 to 14425 and 14444 to 14459 if an
additional axis board is attached) are to be manually set.)
# 1 ASE When automatic setting mode is selected for FSSB setting (when the
FMD parameter (bit 0 of parameter No.1902) is set to 0), automatic
setting is:
0: Not completed.
1: Completed.
This bit is automatically set to 1 upon the completion of automatic
setting.
#7 #6 #5 #4 #3 #2 #1 #0
1905 PM2 PM1 PM4 PM3
[Input type] Parameter input
[Data type] Bit axis
NOTE
When at least one of these parameters is set, the
power must be turned off before operation is
continued.
# 1 PM3 The third separate detector interface unit is:
0: Not used.
1: Used.
# 2 PM4 The fourth separate detector interface unit is:
0: Not used.
1: Used.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2035 -
# 6 PM1 The first separate detector interface unit is:
0: Not used.
1: Used.
# 7 PM2 The second separate detector interface unit is:
0: Not used.
1: Used.
NOTE
When automatic setting mode is selected for FSSB
setting (when the parameter FMD (No.1902#0) is
set to 0), this parameter is automatically set when
input is performed with the FSSB setting screen.
When manual setting 2 mode is selected for FSSB
setting (when the parameter FMD (No.1902#0) is
set to 1), this parameter must be set directly. When
a separate detector interface unit is used, a
connector number must be set in the
corresponding parameter (No.1936, No.1937,
No.1938, or No.1939).
1936 Connector number of the first separate detector interface unit
1937 Connector number of the second separate detector interface unit
1938 Connector number of the third separate detector interface unit
1939 Connector number of the fourth separate detector interface unit
NOTE
When these parameters are set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Byte axis
[Valid data range] 0 to 7
Set the connector numbers corresponding to connectors to be
connected when the separate detector interface unit set by bit 1, 2, 6,
or 7 of parameter No. 1905 is used. The values to be set are indicated
below.
Within one separate detector interface unit, use connector numbers
sequentially. No intermediate number may be omitted.
Correspondence between connectors and connector numbers
Connector Connector number
JF101 0
JF102 1
JF103 2
JF104 3
JF105 4
JF106 5
A.PARAMETERS APPENDIX B-63944EN/03
- 2036 -
Correspondence between connectors and connector numbers
Connector Connector number
JF107 6
JF108 7
Example of setting)
Separate detector connection destination Parameter setting
Controlled
axis Connectors
for 1st unit
Connectors
for 2nd unit
Connectors
for 3rd unit
Connectors
for 4th unit
No.
1936
No.
1937
No.
1938
No.
1939
No.1905
(#7,#6,#2,#1)
X1 JF101 - - - 0 - - - 0,1,0,0
Y1 - JF102 - - - 1 - - 1,0,0,0
Z1 - - JF102 - - - 1 - 0,0,0,1
X2 - JF101 - - - 0 - - 1,0,0,0
Y2 - - - JF101 - - - 0 0,0,1,0
Z2 - - - - - - - - 0,0,0,0
A1 - - JF101 - - - 0 - 0,0,0,1
B1 - - - JF102 - - - 1 0,0,1,0
C1 - JF104 - - - 3 - - 1,0,0,0
A2 JF102 - - - 1 - - - 0,1,0,0
B2 - JF103 - - - 2 - - 1,0,0,0
C2 - - - JF103 - - - 2 0,0,1,0
NOTE
When automatic setting mode is selected for FSSB
setting (when the parameter FMD (No.1902#0) is set
to 0), these parameters are automatically set when
input is performed with the FSSB setting screen.
When manual setting 2 mode is selected for FSSB
setting (when the parameter FMD (No.1902#0) is set
to 1), these parameters must be set directly.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2037 -
Parameters No.2000 to 2999 are for digital servo, The following
parameters are not explained in this manual. Refer to FANUC AC
SERVO MOTOR αi series PARAMETER MANUAL (B-65270EN)
#7 #6 #5 #4 #3 #2 #1 #0
2011 XIAx
[Input type] Parameter input
[Data type] Bit axis
# 7 XIAx Temporary absolute coordinate setting is:
0: Not used.
1: Used.
NOTE
1 When temporary absolute coordinate setting is
used, bit 1 (OPTx) of parameter No. 1815, bit 5
(APCx) of parameter No. 1815, parameter No.
1874, and parameter No. 1875 must be set.
2 The setting of this parameter becomes effective
after the power is turned off then back on.
2031 Torque command difference threshold of torque difference alarm
[Input type] Parameter input
[Data type] Word axis
[Valid data range] 0 to 14564
If the absolute value of the torque command difference between two
axes exceeds the value set in this parameter, an alarm is issued.
Set the same value for two axes that are placed under axis
synchronous control.
The servo axis numbers of the synchronized master axis and slave axis
must be assigned so that an odd number is assigned to the master axis
and the next axis number is assigned to the slave axis. Examples are
(1,2) and (3,4).
#7 #6 #5 #4 #3 #2 #1 #0
3002 OVM POV
[Input type] Parameter input
[Data type] Bit path
# 6 POV Dwell/Auxiliary function time override function is:
0: Invalid.
1: Valid.
A.PARAMETERS APPENDIX B-63944EN/03
- 2038 -
# 7 OVM In Dwell/Auxiliary function time override function, override function
for M02,M30 is:
0: Invalid.
1: Valid.
#7 #6 #5 #4 #3 #2 #1 #0
3008 XSG
[Input type] Parameter input
[Data type] Bit path
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
# 2 XSG A signal assigned to an X address is:
0: Fixed at the address.
1: Able to be reassigned to an arbitrary X address.
NOTE
When this parameter is set to 1, set parameter No.
3013, No. 3014, No. 3012, and No. 3019. If
parameter No. 3013 and No. 3014 are not set, the
deceleration signal for reference position return is
assigned to bit 0 of X0000. If parameter No. 3012
and No. 3019 are not set, the skip signal, the PMC
axis control skip signal, the measurement position
arrival signal, the manual feed interlock signal for
each axis direction, and the tool compensation
value write signal are assigned to X0000.
3012 Skip signal assignment address
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Word path
[Valid data range] 0 to 727
Set an X address to which the skip signal (SKIPn) is to be assigned.
NOTE
This parameter is valid when bit 2 (XSG) of
parameter No. 3008 is set to 1.
Depending on the option configuration of the I/O
Link, the actually usable X addresses are:
X0 to X127, X200 to X327, X400 to X527, X600 to
X727
B-63944EN/03 APPENDIX A.PARAMETERS
- 2039 -
3013 X address to which the deceleration signal for reference position return is
assigned
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Word axis
[Valid data range] 0 to 727
Set an address to which the deceleration signal (*DECn) for reference
position return for each axis is to be assigned.
NOTE
This parameter is valid when bit 2 (XSG) of
parameter No. 3008 is set to 1.
Depending on the option configuration of the I/O
Link, the actually usable X addresses are:
X0 to X127, X200 to X327, X400 to X527, X600 to
X727
3018 Percentage assumed when the 1% rapid traverse override signal indicates
0% during execution of an auxiliary function
[Input type] Parameter input
[Data type] Byte path
[Unit of data] %
[Valid data range] 0 to 100
When the 1% rapid traverse override signal indicates 0% in the
dwell/auxiliary function time override function, this parameter sets the
percentage for calculating an insufficient time.
0% is assumed to be 10%.
3019 Address to which the PMC axis control skip signal and the measurement
position arrival signal are assigned
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Word path
[Valid data range] 0 to 727
Set an X address to which the PMC axis control skip signal ESKIP
and the measurement position arrival signals (XAE, YAE, and ZAE
(M series) or XAE and ZAE (T series)) are to be assigned.
A.PARAMETERS APPENDIX B-63944EN/03
- 2040 -
Example 1. When No.3012 is set to 5 and No.3019 is set to 6
When XSG (bit 2 of parameter No. 3008) is 1, the PMC axis control skip signal, and
measurement position arrival signal are allocated to X0006 and the skip signal is
allocated to X0005.
#7 #6 #5 #4 #3 #2 #1 #0
X005 SKIP SKIP6 SKIP5 SKIP4 SKIP3 SKIP2 SKIP8 SKIP7
(T series)
#7 #6 #5 #4 #3 #2 #1 #0
SKIP SKIP6 SKIP5 SKIP4 SKIP3 SKIP2 SKIP8 SKIP7
(M series)
#7 #6 #5 #4 #3 #2 #1 #0
X006 ESKIP -MIT2 +MIT2 -MIT1 +MIT1 ZAE XAE
(T series)
#7 #6 #5 #4 #3 #2 #1 #0
ESKIP ZAE YAE XAE
(M series)
Example 2. When No.3012 is set to 5 and No.3019 is set to 5
When XSG (bit 2 of parameter No. 3008) is 1, the PMC axis control skip signal,
measurement position arrival signal, and skip signal are allocated to X0005.
#7 #6 #5 #4 #3 #2 #1 #0
X005 ESKIP -MIT2 +MIT2 -MIT1 +MIT1 ZAE XAE
SKIP SKIP6 SKIP5 SKIP4 SKIP3 SKIP2 SKIP8 SKIP7
(T series)
#7 #6 #5 #4 #3 #2 #1 #0
ESKIP ZAE YAE XAE
SKIP SKIP6 SKIP5 SKIP4 SKIP3 SKIP2 SKIP8 SKIP7
(M series)
NOTE
This parameter is valid when bit 2 (XSG) of
parameter No. 3008 is set to 1.
Depending on the option configuration of the I/O
Link, the actually usable X addresses are:
X0 to X127, X200 to X327, X400 to X527, X600 to
X727
3021 Address to which an axis signal is assigned
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Byte axis
[Valid data range] 0 to 7, 10 to 17, 20 to 27, ... , 90 to 97
For each axis of the CNC, set a PMC interface address.
Set a value according to the tables below.
Value of parameter No. 3021 (the second digit)
Setting value Input signal address Output signal address
0 G0000 to G0767 F0000 to F0767
1 G1000 to G1767 F1000 to F1767
:
9 G9000 to G9767 F9000 to F9767
B-63944EN/03 APPENDIX A.PARAMETERS
- 2041 -
Value of parameter No. 3021 (the first digit)
Setting value Input signal address Output signal address
0 #0 #0
1 #1 #1
:
7 #7 #7
[Example of setting]
Axis number No.3021 Signal allocation
1 0
+J1<G0100#0>, -J1<G0102#0>,
ZP1<F0090#0>, ...
2 1
+J2<G0100#1>, -J2<G0102#1>,
ZP2<F0090#1>, ...
3 2
+J3<G0100#2>, -J3<G0102#2>,
ZP3<F0090#2>, ...
4 10
+J4<G1100#0>, -J4<G1102#0>,
ZP4<F1090#0>, ...
5 11
+J5<G1100#1>, -J5<G1102#1>,
ZP5<F1090#1>, ...
If eight or less axes are used per path, the following signal allocation
results when 0 is set for all axes:
Axis 1 of path 1 = Setting equivalent to 0
Axis 2 of path 1 = Setting equivalent to 1
:
Axis 1 of path 2 = Setting equivalent to 10
:
NOTE
Set this parameter when more than eight axes are
used per path.
The valid data range varies, depending on the NC
system type.
3022 Address to which a spindle signal is assigned
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Byte spindle
[Valid data range] 0to3,10to13,20to23, ... ,90to93
For each axis of the CNC, set a PMC interface address.
Set a value according to the tables below.
Value of parameter No. 3022 (the second digit)
Setting value Input signal address Output signal address
0 G0000toG0767 F0000toF0767
1 G1000toG1767 F1000toF1767
:
9 G9000toG9767 F9000toF9767
A.PARAMETERS APPENDIX B-63944EN/03
- 2042 -
Value of parameter No. 3022 (the first digit)
Setting value Input signal address Output signal address
0 Bit position A Bit position A
1 Bit position B Bit position B
2 Bit position C Bit position C
3 Bit position D Bit position D
(The bit positions A, B, C, and D vary, depending on the type of
signal.)
[Example of setting]
Spindle number No.3022 Signal allocation
1 0
TLMLA<G0070.0>, TLMHA<G0070.1>,
ALMA<F0045.0>, ...
2 1
TLMLB<G0074.0>, TLMHB<G0074.1>,
ALMB<F0049.0>, ...
3 10
TLMLA<G1070.0>, TLMHA<G1070.1>,
ALMA<F1045.0>, ...
4 11
TLMLB<G1074.0>, TLMHB<G1074.1>,
ALMB<F1049.0>, ...
If four or less axes are used per path, the following signal allocation
results when 0 is set for all axes:
Axis 1 of path 1 = Setting equivalent to 0
Axis 2 of path 1 = Setting equivalent to 1
:
Axis 1 of path 2 = Setting equivalent to 10
:
NOTE
The valid data range varies, depending on the
system software.
3030 Allowable number of digits for the M code
3031 Allowable number of digits for the S code
3032 Allowable number of digits for the T code
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to 8
Set the allowable numbers of digits for the M, S, and T codes.
When 0 is set, the allowable number of digits is assumed to be 8.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2043 -
3033 Allowable number of digits for the B code (second auxiliary function)
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to 8
Set the allowable number of digits for the second auxiliary function.
When 0 is set, the allowable number of digits is assumed to be 8.
To enable a decimal point to be specified, bit 0 (AUP) of parameter
No. 3450 must be set to 1. In this case, the allowable number of digits
set in this parameter includes the number of decimal places.
If a value exceeding the allowable number of digits is specified, the
alarm PS0003 is issued.
#7 #6 #5 #4 #3 #2 #1 #0
DAC DRC PPD MCN
3104 DAC DAL DRC DRL PPD MCN
[Input type] Parameter input
[Data type] Bit path
# 0 MCN Machine position
0: Regardless of whether input is made in mm or inches, the
machine position is displayed in mm for millimeter machines, or
in inches for inch machines.
1: When input is made in mm, the machine position is displayed in
mm, and when input is made in inches, the machine position is
displayed in inches accordingly.
# 3 PPD Relative position display when a coordinate system is set
0: Not preset
1: Preset
NOTE
If any of the following is executed when PPD is set
to 1, the relative position display is preset to the
same value as the absolute position display:
(1) Manual reference position return
(2) Coordinate system setting based on G92 (G50
for G code system A on the lathe system)
(3) Workpiece coordinate system presetting based
on G92.1 (G50.3 for G code system A on the
lath system)
(4) When a T code for the lathe system is
specified.
# 4 DRL Relative position
0: The actual position displayed takes into account tool length
offset.
1: The programmed position displayed does not take into account
tool length offset.
A.PARAMETERS APPENDIX B-63944EN/03
- 2044 -
# 5 DRC When relative positions are displayed:
0: Values not excluding the amount of travel based on tool radius ⋅
tool nose radius compensation are displayed.
1: Values excluding the amount of travel based on tool radius ⋅ tool
nose radius compensation (programmed positions) are displayed.
# 6 DAL Absolute position
0: The actual position displayed takes into account tool length
offset.
1: The programmed position displayed does not take into account
tool length offset.
NOTE
In lathe systems, whether to exclude a tool offset
when displaying the absolute position is
determined by the setting of bit 1 (DAP) of
parameter No. 3129.
# 7 DAC When an absolute position are displayed:
0: Values not excluding the amount of travel based on tool radius ⋅
tool nose radius compensation are displayed.
1: Values excluding the amount of travel based on tool radius ⋅ tool
nose radius compensation (programmed positions) are displayed.
#7 #6 #5 #4 #3 #2 #1 #0
3106 DAK
[Input type] Setting input
[Data type] Bit
# 6 DAK Specifies whether to display coordinates in the program coordinate
system or workpiece coordinate system as absolute coordinates when
the three-dimensional coordinate conversion mode, the tilted working
plane command mode or the workpiece setting error compensation
mode is set.
0: Display coordinates in the program coordinate system.
1: Display coordinates in the workpiece coordinate system.
#7 #6 #5 #4 #3 #2 #1 #0
3111 OPS OPM SPS SVS
[Input type] Setting input
[Data type] Bit path
# 0 SVS Servo setting screen and servo tuning screen
0: Not displayed
1: Displayed
# 1 SPS Spindle tuning screen
0: Not displayed
1: Displayed
B-63944EN/03 APPENDIX A.PARAMETERS
- 2045 -
# 5 OPM Operating monitor
0: Not displayed
1: Displayed
# 6 OPS The speedometer on the operating monitor screen indicates:
0: Spindle motor speed
1: Spindle speed
#7 #6 #5 #4 #3 #2 #1 #0
3115 NDAx NDPx
[Input type] Parameter input
[Data type] Bit axis
# 0 NDPx The current position is:
0: Displayed.
1: Not displayed.
NOTE
When using the electric gear box (EGB) function,
set 1 for the EGB dummy axis to disable current
position display.
# 1 NDAx The current position and the amount of the movement to be made in
absolute and relative coordinates are:
0: Displayed.
1: Not displayed.
#7 #6 #5 #4 #3 #2 #1 #0
DAP DRP
3129
[Input type] Parameter input
[Data type] Bit path
# 0 DRP For relative coordinate display:
0: The actual position considering a tool offset (tool movement) is
displayed.
1: The programmed position excluding a tool offset (tool
movement) is displayed.
A.PARAMETERS APPENDIX B-63944EN/03
- 2046 -
# 1 DAP For absolute coordinate display:
0: The actual position considering a tool offset (tool movement) is
displayed.
1: The programmed position excluding a tool offset (tool
movement) is displayed.
NOTE
In machining center systems, whether to exclude
the tool length offset when displaying the absolute
position is determined according to the setting of bit
6 (DAL) of parameter No. 3104.
3131 Subscript of axis name
[Input type] Parameter input
[Data type] Byte axis
[Valid data range] 0 to 9, 65 to 90
In order to distinguish axes under parallel operation, synchronization
control, and tandem control, specify a subscript for each axis name.
Setting value Meaning
0 Each axis is set as an axis other than a parallel axis,
synchronization control axis, and tandem control axis.
1 to 9 A set value is used as a subscript.
65 to 90 A set letter (ASCII code) is used as a subscript.
Example) When the axis name is X, a subscript is added as
indicated below.
Setting value Axis name displayed on a screen such as the
position display screen
0 X
1 X1
77 XM
83 XS
If a multi-path system is used, no extended axis name is used within a
path, and no subscript is set for the axis names, then the path number
is automatically used as the subscript for the axis names. To disable
the display of axis name subscripts, set a blank (32) of ASCII code in
the parameter for specifying an axis name subscript.
NOTE
If even one axis in a path uses an extended axis
name when bit 2 (EAS) of parameter No. 11308 is
set to 0, subscripts cannot be used for axis names
in the path.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2047 -
3141 Path name (1st character)
3142 Path name (2nd character)
3143 Path name (3rd character)
3144 Path name (4th character)
3145 Path name (5th character)
3146 Path name (6th character)
3147 Path name (7th character)
[Input type] Parameter input
[Data type] Byte path
[Valid data range] See the character-code correspondence table.
Specify a path name with codes.
Any character string consisting of alphanumeric characters, katakana
characters, and special characters with a maximum length of seven
characters can be displayed as a series name.
NOTE
1 For characters and codes, see Appendix A,
“CHARACTER CODE LIST”.
2 When 0 is set in parameter No. 3141,
PATH1(,PATH2...) are displayed as path names.
#7 #6 #5 #4 #3 #2 #1 #0
3201 NPE
[Input type] Parameter input
[Data type] Bit path
# 6 NPE With an M02, M30, or M99 block, program registration is assumed to
be:
0: Completed
1: Not completed
A.PARAMETERS APPENDIX B-63944EN/03
- 2048 -
#7 #6 #5 #4 #3 #2 #1 #0
3202 NE9 NE8
[Input type] Parameter input
[Data type] Bit path
# 0 NE8 Editing of subprograms with program numbers 8000 to 8999
0: Not inhibited
1: Inhibited
When this parameter is set to 1, the following editing operations are
disabled:
(1) Program deletion (Even when deletion of all programs is
specified, programs with program numbers 8000 to 8999 are not
deleted.)
(2) Program output (Even when outputting all programs is specified,
programs with program numbers 8000 to 8999 are not output.)
(3) Program number search
(4) Program editing of registered programs
(5) Program registration
(6) Program collation
(7) Displaying programs
NOTE
This parameter setting does not affect the following
programs:
(1) Programs on the Data Server
(2) Programs for running and editing memory card
programs on a memory card
# 4 NE9 Editing of subprograms with program numbers 9000 to 9999
0: Not inhibited
1: Inhibited
When this parameter is set to 1, the following editing operations are
disabled:
(1) Program deletion (Even when deletion of all programs is
specified, programs with program numbers 9000 to 9999 are not
deleted.)
(2) Program output (Even when outputting all programs is specified,
programs with program numbers 9000 to 9999 are not output.)
(3) Program number search
(4) Program editing of registered programs
(5) Program registration
(6) Program collation
(7) Displaying programs
NOTE
This parameter setting does not affect the following
programs:
(1) Programs on the Data Server
(2) Programs for running and editing memory card
programs on a memory card
B-63944EN/03 APPENDIX A.PARAMETERS
- 2049 -
#7 #6 #5 #4 #3 #2 #1 #0
3203 MCL MER MZE
[Input type] Parameter input
[Data type] Bit path
# 5 MZE After MDI operation is started, program editing during operation is:
0: Enabled
1: Disabled
# 6 MER When the last block of a program has been executed at single block
operation in the MDI mode, the executed block is:
0: Not deleted
1: Deleted
NOTE
When MER is set to 0, the program is deleted if the
end-of-record mark (%) is read and executed. (The
mark % is automatically inserted at the end of a
program.)
# 7 MCL Whether a program prepared in the MDI mode is cleared by reset
0: Not deleted
1: Deleted
#7 #6 #5 #4 #3 #2 #1 #0
3204 MKP
[Input type] Parameter input
[Data type] Bit path
# 6 MKP When M02, M30, or EOR(%) is executed during MDI operation, the
created MDI program is:
0: Erased automatically.
1: Not erased automatically.
NOTE
If the bit 6 (MER) of parameter No. 3203 is 1,
executing the last block provides a choice of
whether to automatically erase a created program.
A.PARAMETERS APPENDIX B-63944EN/03
- 2050 -
#7 #6 #5 #4 #3 #2 #1 #0
3207 VRN
[Input type] Parameter input
[Data type] Bit
# 5 VRN On the custom macro variable screen, the variable names of common
variables #500 to #549 are:
0: Not displayed.
1: Displayed.
3210 Program protection (PSW)
[Input type] Parameter input
[Data type] 2-word
[Valid data range] 0 to 99999999
This parameter sets a password for protecting program Nos. 9000 to
9999. When a value other than zero is set in this parameter and this
value differs from the keyword set in parameter No.3211, bit 4 (NE9)
of parameter No.3202 for protecting program Nos. 9000 to 9999 is
automatically set to 1.
This disables the editing of program Nos. 9000 to 9999. Until the
value set as the password is set as a keyword, NE9 cannot be set to 0
and the password cannot be modified.
NOTE
1 The state where password ≠ 0 and password ≠
keyword is referred to as the locked state. When an
attempt is made to modify the password by MDI
input operation in this state, the warning message
"WRITE PROTECTED" is displayed to indicate that
the password cannot be modified. When an
attempt is made to modify the password with G10
(programmable parameter input), alarm (PS0231)
is issued.
2 When the value of the password is not 0, the
parameter screen does not display the password.
Care must be taken in setting a password.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2051 -
3211 Program protection key (KEY)
[Input type] Parameter input
[Data type] 2-word
[Valid data range] 0 to 99999999
When the value set as the password (set in parameter No.3210) is set
in this parameter, the locked state is released and the user can now
modify the password and the value set in bit 4 (NE9) of parameter
No.3202.
NOTE
The value set in this parameter is not displayed.
When the power is turned off, this parameter is set
to 0.
3220 Password (PSW)
[Input type] Locked parameter
[Data type] 2-word
[Valid data range] 0 to 99999999
This parameter sets a password (PSW). When a value other than 0 is
set, a password is set. When a password is set, a blank is displayed in
this parameter, and the state (locked state) where an operation such as
program editing is locked is set. When password (PSW) = 0, namely,
in the normal state, or when password (PSW) = keyword (KEY),
namely, in the unlock state, this parameter can be set.
3221 Keyword (KEY)
[Input type] Locked parameter
[Data type] 2-word
[Valid data range] 0 to 99999999
When the same value as the password (PSW) is set in this parameter,
the lock is released (unlock state). The value set in this parameter is
not displayed.
The value of this parameter is initialized to 0 automatically when the
power is turned on. So, if the power is turned off in the unlock state
then is turned on again, the lock state is automatically set.
A.PARAMETERS APPENDIX B-63944EN/03
- 2052 -
3222 Program protection range (minimum value) (PMIN)
3223 Program protection range (maximum value) (PMAX)
[Input type] Locked parameter
[Data type] 2-word
[Valid data range] 0 to 99999999
The programs in a range set here can be locked. Set the minimum
program number and maximum program number of a desired range.
Set these parameters to satisfy PMAX > PMIN.
These parameters can be set when password (PSW) = 0, namely, in
the normal state, or when password (PSW) = keyword (KEY), namely
in the unlock state.
Example)
Parameter No.3222 = 7000
Parameter No.3223 = 8499
When the values above are set, the programs from O7000 to O8499
can be locked.
When PMIN = 0, the specification of PMIN = 9000 is assumed. When
PMAX = 0, the specification of PMAX = 9999 is assumed. So, when
these parameters are set to the defaults, the programs from O9000 to
O9999 are locked.
NOTE
1 Parameter No. 3220 to No. 3223 are neither
punched nor read.
2 Parameter No. 3220 to No. 3223 are not cleared
even when a parameter file clear operation is
performed in the IPL state.
3 The values of a password (PSW) and keyword
(KEY) are not displayed. When password (PSW) =
0, 0 is displayed in parameter No. 3220 to indicate
that the normal state is set.
4 When a password (PSW) or keyword (KEY) is set,
[+INPUT] has the same effect as [INPUT]. For
example, if the input operation "1[+INPUT]" is
performed when 99 is set in the keyword (KEY)
parameter, "1" is set.
#7 #6 #5 #4 #3 #2 #1 #0
3233 PDM PCE
[Input type] Parameter input
[Data type] Bit
# 0 PCE Program editing is:
0: Performed in the word edit mode.
1: Performed in the character edit mode.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2053 -
# 1 PDM On the Data Server file list screen:
0: M198 operation folders and DNC operation files can be set.
1: Folders in the Data Server can be set as the foreground folder and
background folder.
NOTE
When an M198 external subprogram call or DNC
operation is performed on the Data Server, set this
bit to 0.
For the foreground and background folders, refer to
Chapter 12, "PROGRAM MANAGEMENT", in Part
III in the user's manual (B-63944EN).
#7 #6 #5 #4 #3 #2 #1 #0
3280 NLC
[Input type] Parameter input
[Data type] Bit
# 0 NLC Dynamic display language switching is:
0: Enabled.
1: Disabled.
When dynamic display language switching is disabled, the language
setting screen is not displayed. In this case, change the setting of
parameter No. 3281 on the parameter screen then turn on the power
again to switch the display language.
3281 Display language
[Input type] Parameter input
[Data type] Byte
[Valid data range] 0 to 17
Select a display language from the following:
0 : English
1 : Japanese
2 : German
3 : French
4 : Chinese(traditional characters)
5 : Italian
6 : Korean
7 : Spanish
8 : Dutch
9 : Danish
10 : Portuguese
11 : Polish
12 : Hungarian
13 : Swedish
14 : Czech
15 : Chinese(simplified characters)
16 : Russian
17 : Turkish
If a number not indicated above is set, English is selected.
A.PARAMETERS APPENDIX B-63944EN/03
- 2054 -
#7 #6 #5 #4 #3 #2 #1 #0
3400 PGD MGC
[Input type] Parameter input
[Data type] Bit path
# 1 MGC When a single block specifies multiple M commands, an M code
group check is:
0: Made.
1: Not made.
# 5 PGD The G10.9 command (programmable diameter/radius specification
switching) is:
0: Disabled.
1: Enabled.
NOTE
1 The option for the diameter and radius switching
function is required.
2 When the G10.9 command is enabled by this
parameter, signal-based diameter/radius switching
is disabled.
#7 #6 #5 #4 #3 #2 #1 #0
GSC GSB ABS MAB DPI
3401 ABS MAB DPI
[Input type] Parameter input
[Data type] Bit path
# 0 DPI When a decimal point is omitted in an address that can include a
decimal point
0: The least input increment is assumed. (Normal decimal point
input)
1: The unit of mm, inches, degree, or second is assumed. (Pocket
calculator type decimal point input)
# 4 MAB Switching between the absolute and incremental commands in MDI
operation
0: Performed by G90 or G91
1: Depending on the setting of bit 5 (ABS) of parameter No.3401
NOTE
When G code system A of the lathe system is
used, this parameter is invalid.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2055 -
# 5 ABS Program command in MDI operation
0: Assumed as an incremental command
1: Assumed as an absolute command
NOTE
ABS is valid when bit 4 (MAB) of parameter
No.3401 is set to 1. When G code system A of the
lathe system is used, this parameter is invalid.
# 6 GSB The G code system is set.
# 7 GSC
GSC GSB G code
0 0 G code system A
0 1 G code system B
1 0 G code system C
NOTE
G code system B and G code system C are
optional functions. When no option is selected, G
code system A is used, regardless of the setting of
these parameters.
#7 #6 #5 #4 #3 #2 #1 #0
G23 CLR FPM G91 G01
3402
G23 CLR G91 G19 G18 G01
[Input type] Parameter input
[Data type] Bit path
# 0 G01 G01 Mode entered when the power is turned on or when the control is
cleared
0: G00 mode (positioning)
1: G01 mode (linear interpolation)
# 1 G18 Plane selected when power is turned on or when the control is cleared
0: G17 mode (plane XY)
1: G18 mode (plane ZX)
# 2 G19 Plane selected when power is turned on or when the control is cleared
0: The setting of bit 1 (G18) of parameter No.3402 is followed.
1: G19 mode (plane YZ)
When this bit is set to 1, set bit 1 (G18) of parameter No.3402 to 0.
# 3 G91 When the power is turned on or when the control is cleared
0: G90 mode (absolute command)
1: G91 mode (incremental command)
A.PARAMETERS APPENDIX B-63944EN/03
- 2056 -
# 4 FPM At power-on time or in the cleared state:
0: G99 or G95 mode (feed per revolution) is set.
1: G98 or G94 mode (feed per minute) is set.
# 6 CLR Reset button on the MDI panel, external reset signal, reset and rewind
signal, and emergency stop signal
0: Cause reset state.
1: Cause clear state.
For the reset and clear states, refer to Appendix in the User's Manual.
# 7 G23 When the power is turned on
0: G22 mode (stored stroke check on)
1: G23 mode (stored stroke check off)
#7 #6 #5 #4 #3 #2 #1 #0
3404 M3B M02 M30 SBP
[Input type] Parameter input
[Data type] Bit path
# 2 SBP In an external device subprogram call, the address P format is based
on:
0: File number specification
1: Program number specification
NOTE
In memory card operation, the program number
specification format is used, regardless of the
setting of this parameter.
# 4 M30 When M30 is specified in a memory operation:
0: M30 is sent to the machine, and the head of the program is
automatically searched for. So, when the ready signal FIN is
returned and a reset or reset and rewind operation is not
performed, the program is executed, starting from the beginning.
1: M30 is sent to the machine, but the head of the program is not
searched for. (The head of the program is searched for by the
reset and rewind signal.)
# 5 M02 When M02 is specified in memory operation
0: M02 is sent to the machine, and the head of the program is
automatically searched for. So, when the end signal FIN is
returned and a reset or reset and rewind operation is not
performed, the program is executed, starting from the beginning.
1: M02 is sent to the machine, but the head of the program is not
searched for. (The head of the program is searched for by the
reset and rewind signal.)
B-63944EN/03 APPENDIX A.PARAMETERS
- 2057 -
# 7 M3B The number of M codes that can be specified in one block
0: One
1: Up to three
#7 #6 #5 #4 #3 #2 #1 #0
CCR G36 DWL AUX
3405 DWL AUX
[Input type] Parameter input
[Data type] Bit path
# 0 AUX When the second auxiliary function is specified in the calculator-type
decimal point input format or with a decimal point, the multiplication
factor for a value output (onto the code signal) relative to a specified
value is such that:
0: The same multiplication factor is used for both of metric input
and inch input.
1: A multiplication factor used for inch input is 10 times greater
than that used for metric input.
When the second auxiliary function is specified in the calculator-type
decimal point input format or with a decimal point, the value output
onto the code signal is a specified value multiplied by a value
indicated below.
Increment system Parameter
AUX=0
Parameter
AUX=1
IS-A for reference axis 100 times 100 times
IS-B for reference axis 1000 times 1000 times
IS-C for reference axis 10000 times 10000 times
IS-D for reference axis 100000 times 100000 times
Metric
input
system
IS-E for reference axis 1000000 times 1000000 times
IS-A for reference axis 100 times 1000 times
IS-B for reference axis 1000 times 10000 times
IS-C for reference axis 10000 times 100000 times
IS-D for reference axis 100000 times 1000000 times
Inch
input
system
IS-E for reference axis 1000000 times 10000000 times
# 1 DWL The dwell time (G04) is:
0: Always dwell per second.
1: Dwell per second in the feed per minute mode (G94), or dwell
per rotation in the feed per rotation mode (G95).
# 3 G36 As a G code to be used with the automatic tool length measurement
function (M series)/automatic tool offset function (T series) is:
0: G36 (T series only)/G37 is used.
1: G37.1/G37.2/G37.3 is used.
NOTE
If it is necessary to perform circular threading
(counterclockwise), set this parameter to 1.
A.PARAMETERS APPENDIX B-63944EN/03
- 2058 -
# 4 CCR Addresses used for chamfering
0: Address is “I”, “J”, or “K”.
In direct drawing dimension programming, addresses ",C", ",R",
and ",A" (with comma) are used in stead of "C", "R", and "A".
1: Address is “C”.
Addresses used for direct drawing dimension programming are
"C", "R", and "A" without comma.
NOTE
If this bit (CCR) is set to 0, the function for changing
the compensation direction by specifying I, J, or K in
a G01 block in the tool radius ⋅ tool nose radius
compensation mode cannot be used.
If this bit (CCR) is set to 1 when address C is used
as an axis name, the chamfer function cannot be
used.
#7 #6 #5 #4 #3 #2 #1 #0
3406 C07 C06 C05 C04 C03 C02 C01
#7 #6 #5 #4 #3 #2 #1 #0
3407 C15 C14 C13 C12 C11 C10 C09 C08
#7 #6 #5 #4 #3 #2 #1 #0
3408 C23 C22 C21 C20 C19 C18 C17 C16
#7 #6 #5 #4 #3 #2 #1 #0
3409 C30 C29 C28 C27 C26 C25 C24
[Input type] Parameter input
[Data type] Bit
C01 to C30 If bit 6 (CLR) of parameter No.3402 is set to 1, set a group of G codes
to be placed in the cleared state when the CNC is reset by the
key of the MDI panel, the external reset signal, the reset & rewind
signal, or the emergency stop signal.
The table below indicates the correspondence between bits and G code
groups
The setting of a bit has the following meaning:
0: Places the G code group in the cleared state.
1: Does not place G code group in the cleared state.
Parameter G code group
C01 01
C02 02
C03 03
: :
C30 30
B-63944EN/03 APPENDIX A.PARAMETERS
- 2059 -
3410 Tolerance of arc radius
[Input type] Setting input
[Data type] Real path
[Unit of data] mm, inch (input unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 0 or positive 9 digit of minimum unit of data (refer to the standard
parameter setting table (B))
(When the increment system is IS-B, 0.0 to +999999.999)
When a circular interpolation command is executed, the tolerance for
the radius between the start point and the end point is set.
3411 M code preventing buffering 1
3412 M code preventing buffering 2
:
3420 M code preventing buffering 10
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 0 to 999999999
Set M codes that prevent buffering the following blocks. If processing
directed by an M code must be performed by the machine without
buffering the following block, specify the M code.
M00, M01, M02, and M30 always prevent buffering even when they
are not specified in these parameters.
3421 Range specification 1 of M codes that do not perform buffering (lower limit)
3422 Range specification 1 of M codes that do not perform buffering (upper limit)
3423 Range specification 2 of M codes that do not perform buffering (lower limit)
3424 Range specification 2 of M codes that do not perform buffering (upper limit)
3425 Range specification 3 of M codes that do not perform buffering (lower limit)
3426 Range specification 3 of M codes that do not perform buffering (upper limit)
3427 Range specification 4 of M codes that do not perform buffering (lower limit)
3428 Range specification 4 of M codes that do not perform buffering (upper limit)
3429 Range specification 5 of M codes that do not perform buffering (lower limit)
3430 Range specification 5 of M codes that do not perform buffering (upper limit)
3431 Range specification 6 of M codes that do not perform buffering (lower limit)
A.PARAMETERS APPENDIX B-63944EN/03
- 2060 -
3432 Range specification 6 of M codes that do not perform buffering (upper limit)
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 3 to 99999999
When a specified M code is within the range specified with parameter
Nos.3421 and 3422, 3423 and 3424, 3425 and 3426, 3427 and 3428,
3429 and 3430, or 3431 and 3432, buffering for the next block is not
performed until the execution of the block is completed.
NOTE
M00, M01, M02, and M30 are M codes that do not
perform buffering, regardless of parameter setting.
M98, M99, M codes for calling subprograms, and M
codes for calling custom macros are M codes that
performs buffering, regardless of parameter setting.
3441 Start number of M codes for which an M code group can be set (1)
3442 Start number of M codes for which an M code group can be set (2)
3443 Start number of M codes for which an M code group can be set (3)
3444 Start number of M codes for which an M code group can be set (4)
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 0, 100to99999999
Code numbers 0 to 99 on the M code group setting screen correspond
to M00 to M99. When adding M codes after the first 100 M codes,
specify a start M code number in these parameters. Thus, up to 400 M
codes can be added to the M code group setting screen in groups of
100 M codes starting with the set value. When 0 is set, no M codes are
added to the M code group setting screen.
When setting these parameters, follow the setting condition described
below. If the condition is not satisfied, no M codes are added to the M
code group setting screen as in the case where 0 is set.
(Setting condition)
The settings of parameters (1) to (4) (excluding the setting of 0)
must satisfy:
99 < (1), (1)+99 < (2), (2)+99 < (39, (3) +99 < (4)
B-63944EN/03 APPENDIX A.PARAMETERS
- 2061 -
#7 #6 #5 #4 #3 #2 #1 #0
3450 BDX AUP
[Input type] Parameter input
[Data type] Bit path
# 0 AUP The second auxiliary function specified in the calculator-type decimal
point input format, with a decimal point, or with a negative value is:
0: Disabled.
1: Enabled.
If the second auxiliary function is specified after setting this bit to 0,
the following operation results:
1. When a value is specified without a decimal point
A specified value is output onto the code signal without
modification, regardless of the setting of the calculator-type
decimal point input format (with bit 0 (DPI) of parameter No.
3401).
2. When a value is specified with a decimal point
The alarm (PS0007) is issued.
3. When a negative value is specified
The alarm (PS0006) is issued.
# 7 BDX When ASCII code is called using the same address as the address for
the second auxiliary function (specified by parameter No.3460), this
parameter prevents the argument unit used when the option for the
second auxiliary function is selected from differing from the argument
unit used when the same option is not selected.
0: When bit 0 (AUP) of parameter No.3450 is set to 1, the argument
unit differs, depending on whether the option for the second
auxiliary function is selected or not.
1: The same argument unit is used. (The unit applied when the
option for the second auxiliary function is selected is used.)
[Example]
A setting is made so that address B is used to call O9004, and the
program O1 below is executed with parameter No.3460 = 66.
O1 O9004
B2 #500 = #146
M30 M99
When the increment system is IS-B, and metric input is used,
#500 assumes a value indicated in the table below.
BDX=0
Bit 0 (DPI) of
parameter No.
3401
Bit 0 (AUP) of
parameter No.
3450
Without the
second
auxiliary
function option
With the
second
auxiliary
function option
BDX=1
0 2.000 2.000 2.000
0 1 2.000 0.002 0.002
0 2.000 2.000 2.000
1 1 2.000 2.000 2.000
A.PARAMETERS APPENDIX B-63944EN/03
- 2062 -
#7 #6 #5 #4 #3 #2 #1 #0
3451 GQS
[Input type] Parameter input
[Data type] Bit path
# 0 GQS When threading is specified, the threading start angle shift function
(Q) is:
0: Disabled.
1: Enabled.
#7 #6 #5 #4 #3 #2 #1 #0
3452 EAP
[Input type] Parameter input
[Data type] Bit path
# 7 EAP When bit 0 (ADX) of parameter No.3455 is set to 1, calculator-type
decimal point input at a macro calling argument address is:
0: Enabled.
1: Disabled.
NOTE
This parameter is valid when bit 0 (DPI) of
parameter No.3401 is set to 0.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2063 -
#7 #6 #5 #4 #3 #2 #1 #0
3455 AXDx
[Input type] Parameter input
[Data type] Bit axis
# 0 AXDx If a decimal point is omitted for an axis address with which a decimal
point can be used, the value is determined:
0: In accordance with the least input increment. (Normal decimal
point input)
1: In millimeters, inches, or seconds. (calculator-type decimal point
input)
NOTE
This parameter specifies the calculator-type
decimal point input function for each axis.
For the same axis name, be sure to make the
same setting.
#7 #6 #5 #4 #3 #2 #1 #0
3457 SCF SCC SYS MC1 MC2 LIB
[Input type] Parameter input
[Data type] Bit path
NOTE
1 The parameters LIB, MC2, MC1, and SYS are used
to set a search folder for the following
subprogram/macro calls:
• Subprogram call based on an M code
• Subprogram call based on a particular address
• Subprogram call based on a second auxiliary
function code
• Macro call based on a G code
• Macro call based on an M code
• Macro call based on a T code
• One-touch macro call
2 The parameter SCF is used to set whether to add a
search folder for the following subprogram/macro
calls:
• Subprogram call based on M98
• Figure copy based on G72.1/G72.2
• Macro call based on G65/G66/G66.1
• Macro interrupt based on M96
# 0 LIB The common program directory "//CNC_MEM/USER/LIBRARY/" of
the initial directories is:
0: Set as a search directory.
1: Not set as a search directory.
A.PARAMETERS APPENDIX B-63944EN/03
- 2064 -
# 1 MC2 MTB dedicated directory 2 "//CNC_MEM/MTB2/" of the initial
directories is:
0: Set as a search directory.
1: Not set as a search directory.
# 2 MC1 MTB dedicated directory 1 "//CNC_MEM/MTB1/" of the initial
directories is:
0: Set as a search directory.
1: Not set as a search directory.
# 3 SYS The system directory "//CNC_MEM/SYSTEM/" of the initial
directories is:
0: Set as a search directory.
1: Not set as a search directory.
# 6 SCC The same folder as the main program is added to the top of the search
order as a search folder for the following each subprogram call and
macro call.
• Subprogram call by M code
• Subprogram call by ASCII code
• Subprogram call by the second auxiliary function code
• Macro call by Scode
• Macro call by T code
• Macro call by G code
• Macro call by M code
• One-touch macro call
The same folder as the main program is:
0: Not added in the search order.
1: Added in the search order.
When a search folder is added, a search is made in the following
order:
0) Folder only for embedded macro (With the embedded
macro-function.)
1) Folder where the main program is stored
2) Common program folder, which is an initial folder (LIBRARY)
3) MTB-dedicated folder 2, which is an initial folder (MTB2)
4) MTB-dedicated folder 1, which is an initial folder (MTB1)
5) System folder, which is an initial folder (SYSTEM)
The folders of 2) through 5) can be excluded from search target
folders by setting the bits 0 (LIB), 1 (MC2), 2 (MC1), and 3 (SYS) of
parameter No.3457.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2065 -
# 7 SCF A search folder is:
0: Not added.
1: Added.
When a search folder is added, a search is made in the following
order:
0) Folder only for embedded macro (With the embedded
macro-function.)
1) Folder where the main program is stored
2) Common program folder, which is an initial folder (LIBRARY)
3) MTB-dedicated folder 2, which is an initial folder (MTB2)
4) MTB-dedicated folder 1, which is an initial folder (MTB1)
5) System folder, which is an initial folder (SYSTEM)
The folders of 3) through 5) can be excluded from search target
folders by setting the bits 1 (MC2), 2 (MC1), and 3 (SYS) of
parameter No.3457.
3460 Second auxiliary function specification address
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 65to67, 85to87
Specify which of A, B, C, U, V, and W is to be used as the address for
specifying the second auxiliary function. If an address used as an axis
name is specified, the second auxiliary function is disabled.
Name A B C U V W
Setting value 65 66 67 85 86 87
Address B is assumed when a value other than the above is set.
However, the name U, V, or W can be used with the T series only
when G code system B or C is used. When a value from 85 to 87 is
specified with G code system A, the specification address for the
second auxiliary function is B.
3471
Allowable difference between the specified end position and the end
position obtained from the increase/decrease and frequency in spiral
interpolation or conic interpolation
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm, inch (input unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 0 or positive 9 digit of minimum unit of data (refer to the standard
parameter setting table (B))
(When the increment system is IS-B, 0.0 to +999999.999)
This parameter sets the maximum allowable difference (absolute
value) between the specified end position and the end position
obtained from the increase/decrease and frequency in spiral or conic
interpolation.
A.PARAMETERS APPENDIX B-63944EN/03
- 2066 -
3472 Minimum radius needed to maintain the actual speed in spiral or conic
interpolation
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm, inch (input unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] (For IS-B and millimeter machines, 1.0 to 999999.999; for inch
machines, 1.0 to 99999.9999)
If this parameter value is 0 or a value outside the valid data range, the
minimum value of the range is assumed.
In spiral interpolation and conic interpolation, the speed is generally
held constant. In an area near the center, the spiral radius decreases,
resulting in an extremely high angular velocity. To prevent this, once
the spiral radius has reached the parameter-set value, the angular
velocity subsequently remains constant. As a result, the actual speed
decreases.
#7 #6 #5 #4 #3 #2 #1 #0
3605 BDPx
[Input type] Parameter input
[Data type] Bit axis
NOTE
When this parameter is set, the power must be
turned off before operation is continued..
# 0 BDPx Both-direction pitch error compensation is:
0: Not used.
1: Used.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2067 -
3620 Number of the pitch error compensation position for the reference position
for each axis
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Word axis
[Valid data range] 0 to 1535
Set the number of the pitch error compensation position for the
reference position for each axis.
3621 Number of the pitch error compensation position at extremely negative
position for each axis
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Word axis
[Valid data range] 0 to 1535
Set the number of the pitch error compensation position at the
extremely negative position for each axis.
3622 Number of the pitch error compensation position at extremely positive
position for each axis
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Word axis
[Valid data range] 0 to 1535
Set the number of the pitch error compensation position at the
extremely positive position for each axis.
This value must be larger than set value of parameter (No.3620).
A.PARAMETERS APPENDIX B-63944EN/03
- 2068 -
3623 Magnification for pitch error compensation for each axis
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Byte axis
[Valid data range] 0 to 100
Set the magnification for pitch error compensation for each axis.
If the magnification is set to 1, the same unit as the detection unit is
used for the compensation data.
If 0 is set, compensation is not performed.
3624 Interval between pitch error compensation positions for each axis
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm, inch, degree (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] See the description below.
The pitch error compensation positions are arranged with equal
spacing. The space between two adjacent positions is set for each axis.
The minimum interval between pitch error compensation positions is
limited and obtained from the following equation:
Minimum interval between pitch error compensation positions =
maximum feedrate/7500
Unit : mm, inch, deg or mm/min, inch/min, deg/min
Example:
When the maximum feedrate is 15000 mm/min, the minimum
interval between pitch error compensation positions is 2 mm.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2069 -
3625 Travel distance per revolution in pitch error compensation of rotation axis type
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm, inch, degree (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] See the description below.
If the pitch error compensation of rotation axis type is performed (bit
1 (ROSx) of parameter No.1006 is set to 0 and bit 0 (ROTx) of
parameter No.1006 is set to 1), set the travel distance per revolution.
The travel distance per revolution does not have to be 360 degrees,
and a cycle of pitch error compensation of rotation axis type can be
set.
However, the travel distance per revolution, compensation interval,
and number of compensation points must satisfy the following
condition:
(Travel distance per revolution)
= (Compensation interval) × (Number of compensation points)
The compensation at each compensation point must be set so that the
total compensation per revolution equals 0.
NOTE
If 0 is set, the travel distance per revolution becomes
360 degrees.
3626 Number of the both-direction pitch error compensation position at extremely
negative position (for movement in the negative direction)
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Word axis
[Valid data range] 0 to 1023, 3000 to 4023
When using both-direction pitch error compensation, set the number
of compensation point at the farthest end in the negative direction for
a movement in the negative direction.
NOTE
1 For a movement in the positive direction, set the
compensation point number at the farthest end in the
negative direction in parameter No.3621.
2 A set of compensation data items for a single axis
should not be set to lie astride 1023 to 3000.
A.PARAMETERS APPENDIX B-63944EN/03
- 2070 -
3627
Pitch error compensation at reference position when a movement to the
reference position is made from the direction opposite to the direction of
reference position return
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Word axis
[Unit of data] Detection unit
[Valid data range] -32768 to 32767
Set the absolute value of pitch error compensation at reference
position when a movement to the reference position is made from the
negative direction if the direction of reference position return (bit 5
(ZMI) of parameter No.1006) is positive or from the positive direction
if the direction of reference position return is negative.
#7 #6 #5 #4 #3 #2 #1 #0
3700 NRF CRF
[Input type] Parameter input
[Data type] Bit path
# 0 CRF Reference position setting at an arbitrary position under Cs contour
control is:
0: Not used.
1: Used.
NOTE
When this function is used, an attempt to specify
G00 for a Cs contour control axis without
performing a reference position return operation
even once after switching the serial spindle to the
Cs contour control mode results in the alarm
(PS0303) even if bit 1 (NRF) of parameter No.
3700 is set to 0. Be sure to perform a reference
position return operation by specifying G28.
# 1 NRF With the first move command (G00) after switching the series spindle
to Cs contour control mode:
0: A reference position return operation is once performed then
positioning is performed.
1: A normal positioning operation is performed.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2071 -
#7 #6 #5 #4 #3 #2 #1 #0
3702 EMS
[Input type] Parameter input
[Data type] Bit path
# 1 EMS The multi-spindle control function is:
0: Used.
1: Not used.
#7 #6 #5 #4 #3 #2 #1 #0
3716 A/Ss
[Input type] Parameter input
[Data type] Bit spindle
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
# 0 A/Ss Spindle motor type is :
0: Analog spindle.
1: Serial spindle.
NOTE
1 When an analog spindle is used, the option for
spindle analog output is required.
2 When a serial spindle is used, the option for
spindle serial output is required.
3 The option for the number of controlled spindles
needs to be specified.
3717 Motor number to each spindle
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Byte spindle
[Valid data range] 0 to Maximum number of controlled axes
Set a spindle amplifier number to be assigned to each spindle.
0: No spindle amplifier is connected.
1: Spindle motor connected to amplifier number 1 is used.
2: Spindle motor connected to amplifier number 2 is used.
to
n: Spindle motor connected to amplifier number n is used.
A.PARAMETERS APPENDIX B-63944EN/03
- 2072 -
3741 Maximum spindle speed for gear 1
3742 Maximum spindle speed for gear 2
3743 Maximum spindle speed for gear 3
3744 Maximum spindle speed for gear 4
[Input type] Parameter input
[Data type] 2-word spindle
[Unit of data] min-1
[Valid data range] 0 to 99999999
Set the maximum spindle speed corresponding to each gear.
Spindle motor max. clamp speed
(Parameter No.3736)
Spindle speed command
(S command)
Max. speed (4095, 10V)
Spindle motor minimum clamp speed
(Parameter No.3735)
Spindle motor speed
Gear 1
Max. speed
(Parameter
No.3741)
Gear 2
Max. speed
(Parameter
No.3742)
Gear 3
Max. speed
(Parameter
No.3743)
3770 Axis as the calculation reference in constant surface speed control
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to Number of controlled axes
Set the axis as the calculation reference in constant surface speed
control.
NOTE
When 0 is set, constant surface speed control is
always applied to the X-axis. In this case,
specifying P in a G96 block has no effect on the
constant surface speed control.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2073 -
3781 P code for selecting the spindle in multi-spindle control
[Input type] Parameter input
[Data type] Word spindle
[Valid data range] 0 to 32767
If bit 3 (MPP) of parameter No. 3703 is set to 1, set the P code to
select each spindle under multi-spindle control. Specify the P code in
a block containing the S command.
Example)
If the P code value for selecting the second spindle is set to 3,
S1000 P3;
causes the second spindle to rotate at S1000.
NOTE
1 This parameter is valid if bit 3 (MPP) of parameter
No. 3703 is set to 1.
2 If this parameter is set to 0, the corresponding
spindle cannot be selected by a P code.
3 Under multipath control, the P code specified here
is valid for each path.
For instance, if the P code to select the first spindle
of path 2 is set to 21, specifying S1000 P21; in
path 1 causes the first spindle of path 2 to be
rotated at S1000.
4 Identical P code values cannot be used for
different spindles. (Identical P code values cannot
be used even if the paths are different.)
5 When this parameter is used (when bit 3 (MPP) of
parameter No. 3703 is set to 1), the spindle
command selection signal is invalid.
6 To use this parameter, the multi-spindle control
function is needed.
A.PARAMETERS APPENDIX B-63944EN/03
- 2074 -
Parameters Nos. 4000 to 4799 below are basically used with the serial
spindle amplifier. For details of these parameters, refer to either of the
following manuals and other related documents, depending on the
spindle that is actually connected.
• FANUC AC SPINDLE MOTOR αi series Parameter Manual
(B-65280EN)
#7 #6 #5 #4 #3 #2 #1 #0
4900 FLRs
[Input type] Parameter input
[Data type] Bit spindle
# 0 FLRs When the spindle speed fluctuation detection function is used, the unit
of an allowable ratio (q) and fluctuation ratio (r) set by parameter No.
4911 and No. 4912 is:
0: 1%
1: 0.1%
4911
Allowable speed ratio (q) used to assume that the spindle has reached a
specified speed
[Input type] Parameter input
[Data type] Word spindle
[Unit of data] 1%, 0.1%
[Valid data range] 1 to 100, 1 to 1000
When the spindle speed fluctuation detection function is used, set an
allowable speed ratio (q) used to assume that the spindle has reached a
specified speed.
NOTE
The unit of data is determined by bit 0 (FLR) of
parameter No. 4900.
4912 Spindle variation ratio (r) for not issuing a spindle speed fluctuation
detection alarm
[Input type] Parameter input
[Data type] Word spindle
[Unit of data] 1%, 0.1%
[Valid data range] 1 to 100, 1 to 1000
When the spindle speed fluctuation detection function is used, set a
spindle fluctuation ratio (r) for not issuing an alarm.
NOTE
The unit of data is determined by bit 0 (FLR) of
parameter No. 4900.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2075 -
4913 Spindle speed fluctuation width (i) for not issuing a spindle speed
fluctuation detection alarm
[Input type] Parameter input
[Data type] 2-word spindle
[Unit of data] min-1
[Valid data range] 0 to 99999
When the spindle speed fluctuation detection function is used, set an
allowable fluctuation width (i) for not issuing an alarm.
4914
Time (p) from the change of a specified speed until spindle speed fluctuation
detection is started
[Input type] Parameter input
[Data type] 2-word spindle
[Unit of data] msec
[Valid data range] 0 to 999999
When the spindle speed fluctuation detection function is used, set a
time (p) from the change of a specified speed until spindle speed
fluctuation detection is started. In other words, spindle speed
fluctuation detection is not performed until a set time has elapsed after
a specified speed is changed. However, when the actual spindle speed
is assumed to have reached a specified value within a set time (p),
spindle speed fluctuation detection is started.
#7 #6 #5 #4 #3 #2 #1 #0
4950 ISZs IDMs IORs
[Input type] Parameter input
[Data type] Bit spindle
# 0 IORs Resetting the system in the spindle positioning mode
0: Does not release the mode.
1: Releases the mode
# 1 IDMs The direction of spindle positioning (half-fixed angle positioning
based on M codes) is:
0: Plus direction.
1: Minus direction.
# 2 ISZs When an M code for switching to the spindle positioning mode is
specified for spindle positioning:
0: The spindle is switched to the spindle positioning mode, and
spindle orientation operation is performed.
1: Only the switching of the spindle to the spindle positioning mode
is performed. (Spindle orientation operation is not performed.)
A.PARAMETERS APPENDIX B-63944EN/03
- 2076 -
4960 M code specifying the spindle orientation
[Input type] Parameter input
[Data type] 2-word spindle
[Valid data range] 6 to 97
Set an M code for switching to the spindle positioning mode.
NOTE
1 Do not set an M code that duplicates other M
codes used for spindle positioning.
2 Do not set an M code used with other functions
(such as M00-05, 30, 98, and 99, and M codes for
calling subprograms).
4961 M code releasing the spindle positioning mode
[Input type] Parameter input
[Data type] 2-word spindle
[Valid data range] 6 to 97
Set an M code for canceling the spindle positioning mode on the
spindle positioning axis.
NOTE
1 Do not set an M code that duplicates other M
codes used for spindle positioning.
2 Do not set an M code used with other functions
(such as M00-05, 30, 98, and 99, and M codes for
calling subprograms).
B-63944EN/03 APPENDIX A.PARAMETERS
- 2077 -
4962 M code for specifying a spindle positioning angle
[Input type] Parameter input
[Data type] 2-word spindle
[Valid data range] 6 to 9999999
Two methods are available for specifying spindle positioning. One
method uses axis address for arbitrary-angle positioning. The other
use an M code for half-fixed angle positioning. This parameter sets an
M code for the latter method.
In this parameter, set an M code to be used for half-fixed angle
positioning based on M codes.
Six M code from Mα to M(α+5) are used for half-fixed angle
positioning, when α is the value of this parameter.
• When the number of M codes is set in parameter No. 4964, let α
be the value set in parameter No. 4962, and let β be the value set
in parameter No. 4964. Then, β M codes from Mα to M(α+β-1)
are used as M codes for half-fixed angle positioning based on M
codes.
The table below indicates the relationship between the M codes and
positioning angles.
M code Positioning angle
Example:
Positioning angle
when θ = 30°
Mα θ 30°
M(α+1) 2θ 60°
M(α+2) 3θ 90°
M(α+3) 4θ 120°
M(α+4) 5θ 150°
M(α+5) 6θ 180°
: : :
M(α+β-1) β×θ β×30°
β represents the number of M codes set in parameter No. 4964.
(When parameter No. 4964 is set to 0, β = 6.)
θ represents the basic angular displacement set in parameter No.4963.
NOTE
1 Do not set an M code that duplicates other M
codes used for spindle positioning.
2 Do not set an M code used with other functions
(such as M00-05, 30, 98, and 99, and M codes for
calling subprograms).
4963 Basic angle for half-fixed angle positioning
[Input type] Parameter input
[Data type] Real spindle
[Unit of data] Degree
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 0 to 60
This parameter sets a basic angular displacement used for half-fixed
angle positioning using M codes.
A.PARAMETERS APPENDIX B-63944EN/03
- 2078 -
4964 Number of M codes for specifying a spindle positioning angle
[Input type] Parameter input
[Data type] 2-word spindle
[Valid data range] 0 to 255
This parameter sets the number of M codes used for Half-fixed angle
positioning using M codes.
As many M codes as the number specified in this parameter, starting
with the M code specified in parameter No.4962, are used to specify
half-fixed angle positioning.
Let α be the value of parameter No.4962, and let β be the value of
parameter No.4964. That is, M codes from Mα to M(α+β-1) are used
for half-fixed angle positioning.
Setting this parameter to 0 has the same effect as setting 6. That is, M
code from Mα to M(α+5) are used for half-fixed angle positioning.
NOTE
1 Make sure that M codes from Mα to M (α+β-1) do
not duplicate other M codes.
2 Do not set an M code that duplicates other M
codes used for spindle positioning.
3 Do not set an M code used with other functions
(such as M00-05, 30, 98, and 99, and M codes for
calling subprograms).
#7 #6 #5 #4 #3 #2 #1 #0
EVO
5001 EVO TAL TLB TLC
[Input type] Parameter input
[Data type] Bit path
# 0 TLC
# 1 TLB These bits are used to select a tool length compensation type.
Type TLB TLC
Tool length compensation A 0 0
Tool length compensation B 1 0
Tool length compensation C - 1
The axis to which cutter compensation is applied varies from type to
type as described below.
Tool length compensation A :
Z-axis at all times
Tool length compensation B :
Axis perpendicular to a specified plane (G17/G18/G19)
Tool length compensation C :
Axis specified in a block that specifies G43/G44
# 3 TAL Tool length compensation C
0: Generates an alarm when two or more axes are offset
1: Not generate an alarm even if two or more axes are offset
B-63944EN/03 APPENDIX A.PARAMETERS
- 2079 -
# 6 EVO If a tool compensation value modification is made for tool length
compensation A or tool length compensation B in the offset mode
(G43 or G44):
0: The new value becomes valid in a block where G43, G44, or an
H code is specified next.
1: The new value becomes valid in a block where buffering is
performed next.
#7 #6 #5 #4 #3 #2 #1 #0
LWT LGN
5002
[Input type] Parameter input
[Data type] Bit path
# 1 LGN Geometry offset number of tool offset
0: Is the same as wear offset number
1: Specifies the geometry offset number by the tool selection
number
NOTE
This parameter is valid when the option for tool
geometry compensation or tool wear compensation
is specified.
# 2 LWT Tool wear compensation is performed by:
0: Moving the tool.
1: Shifting the coordinate system.
NOTE
This parameter is valid when the option for tool
geometry compensation or tool wear compensation
is specified.
A.PARAMETERS APPENDIX B-63944EN/03
- 2080 -
#7 #6 #5 #4 #3 #2 #1 #0
5003 SUV SUP
[Input type] Parameter input
[Data type] Bit path
# 0 SUP
# 1 SUV These bits are used to specify the type of startup/cancellation of tool
radius ⋅ tool nose radius compensation.
SUV SUP Type Operation
0 0 Type A A compensation vector perpendicular to the block next to the startup block or the block preceding
the cancellation block is output.
0 1 Type B A compensation vector perpendicular to the startup block or cancellation block and an
intersection vector are output.
1 0
1
Type C When the startup block or cancellation block specifies no movement operation, the tool is shifted
by the cutter compensation amount in a direction perpendicular to the block next to the startup or
the block before cancellation block.
When the block specifies movement operation, the type is set according to the SUP setting; if
SUP is 0, type A is set, and if SUP is 1, type B is set.
NOTE
When SUV,SUP = 0,1 (type B), an operation
equivalent to that of FS16i-T is performed.
Tool nose radius center path /
Tool center path
Programmed path
N1
N2
G41
N1
N2
N3
Intersection point
Shift
G41
Tool nose radius center path /
Tool center path
N1
N2
Intersection point
G41 Programmed path
Programmed path
Tool nose radius center path /
Tool center path
B-63944EN/03 APPENDIX A.PARAMETERS
- 2081 -
#7 #6 #5 #4 #3 #2 #1 #0
ORC
5004 ODI
[Input type] Parameter input
[Data type] Bit path
# 1 ORC The setting of a tool offset value is corrected as:
0: Diameter value
1: Radius value
NOTE
This parameter is valid only for an axis based on
diameter specification. For an axis based on radius
specification, specify a radius value, regardless of
the setting of this parameter.
# 2 ODI The setting of a tool radius ⋅ tool nose radius compensation value is
corrected as:
0: Radius value
1: Diameter value
#7 #6 #5 #4 #3 #2 #1 #0
5008 MCR
[Input type] Parameter input
[Data type] Bit path
# 4 MCR If G41/G42 (tool radius ⋅ tool nose radius compensation) is specified
in the MDI mode, an alarm is:
0: Not raised.
1: Raised. (alarm PS5257)
A.PARAMETERS APPENDIX B-63944EN/03
- 2082 -
Number of digits of an offset number used with a T code command
5028
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to 3
Specify the number of digits of a T code portion that is used for a tool
offset number (wear offset number when the tool geometry/wear
compensation function is used).
When 0 is set, the number of digits is determined by the number of
tool compensation values.
When the number of tool compensation values is 1 to 9: Lower 1 digit
When the number of tool compensation values is 10 to 99: Lower 2
digits
When the number of tool compensation values is 100 to 999: Lower 3
digits
Example :
When an offset number is specified using the lower 2 digits of a
T code, set 2 in parameter No. 5028.
Txxxxxx yy
xxxxxx : Tool selection
yy : Tool offset number
NOTE
A value longer than the setting of parameter No.
3032 (allowable number of digits of a T code) cannot
be set.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2083 -
5029 Number of tool compensation value memories common to paths
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Word
[Valid data range] 0 to 999
When using memories common to paths, set the number of common
tool compensation values in this parameter.
Ensure that the setting of this parameter does not exceed the number
of tool compensation values set for each path (parameter No. 5024).
[Example 1]
When parameter No. 5029 = 10, parameter No. 5024 (path 1) =
15, and parameter No. 5024 (path 2) = 30 in a 2-path system, tool
compensation numbers 1 to 10 of all paths are made common.
[Example 2]
When parameter No. 5029 = 20 and the other conditions are the
same as for Example 1, tool compensation numbers 1 to 15 are
made common.
NOTE
1 When a multi-path system involving the machining
center system and lathe system is used, memories
are made common in each system.
2 In each of the machining center system and lathe
system, the same unit of tool compensation values
needs to be used.
3 Ensure that the setting of parameter No. 5029 does
not exceed the number of tool compensation
values for each path (parameter No. 5024). If the
setting of parameter No. 5029 exceeds the number
of compensation values of a path, the least of the
numbers of compensation values in all paths is
made common.
4 When 0 or a negative value is set, memories
common to paths are not used.
A.PARAMETERS APPENDIX B-63944EN/03
- 2084 -
#7 #6 #5 #4 #3 #2 #1 #0
TCT OWD
5040
[Input type] Parameter input
[Data type] Bit path
# 0 OWD In radius programming (bit 1 (ORC) of parameter No. 5004 is set to
1),
0: Tool offset values of both geometry compensation and wear
compensation are specified by radius.
1: Tool offset value of geometry compensation is specified by
radius and tool offset value of wear compensation is specified by
diameter, for an axis of diameter programming.
NOTE
This parameter is valid when the option for tool
geometry compensation or tool wear compensation
is specified.
# 3 TCT The tool change method is based on:
0: Turret rotation. (Tool change operation is performed with a T
command only.)
With a T command, an auxiliary function and tool offset
operation are performed.
1: Automatic tool changer (ATC).
(Tool change operation is performed with an M command (such
as M06)).
With a T command, an auxiliary function only is performed.
This parameter is valid with a lathe system only.
WARNING
Before changing the setting of this parameter,
cancel the offset. If the setting is changed while the
offset is applied, the subsequent offset operation
may not be performed correctly.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2085 -
#7 #6 #5 #4 #3 #2 #1 #0
5042 OFE OFD OFC OFA
[Input type] Parameter input
[Data type] Bit path
NOTE
When at least one of these parameters is set, the powe
r
must be turned off before operation is continued.
# 0 OFA
# 1 OFC
# 2 OFD
# 3 OFE These bits are used to specify the increment system and valid data
range of a tool offset value.
For metric input
OFE OFD OFC OFA Unit Valid data range
0 0 0 1 0.01mm ±9999.99mm
0 0 0 0 0.001mm ±9999.999mm
0 0 1 0 0.0001mm ±9999.9999mm
0 1 0 0 0.00001mm ±9999.99999mm
1 0 0 0 0.000001mm ±999.999999mm
For inch input
OFE OFD OFC OFA Unit Valid data range
0 0 0 1 0.001inch ±999.999inch
0 0 0 0 0.0001inch ±999.9999inch
0 0 1 0 0.00001inch ±999.99999inch
0 1 0 0 0.000001inch ±999.999999inch
1 0 0 0 0.0000001inch ±99.9999999inch
Axis number for which Y-axis offset is used
5043
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to 24
Set the number of an axis for which the tool offset is corrected.
If 0 or a value beyond the valid data range is set, the Y-axis offset is
applied to the Y-axis of the basic three axes. If setting is made for the
X- or Z-axis of the basic three axes, the standard tool offset for the X-
or Z-axis is not used, and only the Y-axis offset is used.
A.PARAMETERS APPENDIX B-63944EN/03
- 2086 -
5071
Number of first axis for grinding –wheel wear compensation
5072
Number of second axis for grinding–wheel wear compensation
[Input Type] Parameter Input
[Data Type] Byte path
[Valid data Range] 1 to number of controlled axis
This parameter specifies the controlled axis numbers of the first and
second axis for which grinding-wheel wear compensation is applied.
5081 1st-axis coordinate value of compensation center 1 in grinding-wheel wear
compensation
5082 2nd-axis coordinate value of compensation center 1 in grinding-wheel wear
compensation
5083 1st-axis coordinate value of compensation center 2 in grinding-wheel wear
compensation
5084 2nd-axis coordinate value of compensation center 2 in grinding-wheel wear
compensation
5085 1st-axis coordinate value of compensation center 3 in grinding-wheel wear
compensation
5086 2nd-axis coordinate value of compensation center 3 in grinding-wheel wear
compensation
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm, inch (input unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
Set the coordinate value (in the workpiece coordinate system) of the
center of compensation in grinding-wheel wear compensation.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2087 -
#7 #6 #5 #4 #3 #2 #1 #0
5101 FXY
[Input type] Parameter input
[Data type] Bit path
# 0 FXY The drilling axis in the drilling canned cycle, or cutting axis in the
grinding canned cycle is:
0: In case of the Drilling canned cycle:
Z-axis at all times.
In case of the Grinding canned cycle:
• For the Lathe system
Z-axis at all times.
• For the Machining Center system
G75,G77 command :Y-axis
G78,G79 command :Z-axis
1: Axis selected by the program
NOTE
In the case of the T series, this parameter is valid
only for the drilling canned cycle in the Series 15
format.
#7 #6 #5 #4 #3 #2 #1 #0
5105 TFA
[Input type] Parameter input
[Data type] Bit path
# 5 TFA During tool center point control or tool length compensation in tool
axis direction, canned cycles:
0: Cannot be used.
1: Can be used. However, an alarm (PS5424) is issued if the
position of the rotation axis is not ±90° × n (n=0, 1, 2, ...) in the
workpiece coordinate system.
#7 #6 #5 #4 #3 #2 #1 #0
GFX
5106
[Input type] Parameter input
[Data type] Bit path
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
# 0 GFX When the options of multiple respective canned cycle and grinding
canned cycle are both specified, G71/G72/G73/G74 commands are:
0: Multiple respective canned cycle.
1: Grinding canned cycle.
A.PARAMETERS APPENDIX B-63944EN/03
- 2088 -
Grinding axis number in Traverse Grinding Cycle(G71)
5176
Grinding axis number in Plunge Grinding Cycle(G75)
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to Number of controlled axes
For the Lathe system:
Set the Grinding axis number of Traverse Grinding Cycle(G71).
For the Machining Center system:
Set the Grinding axis number of Plunge Grinding Cycle(G75).
NOTE
The axis number except for the cutting axis can be
specified. When the axis number which is same to
cutting axis is specified, PS0456 alarm is issued at
the time of execution. The Grinding Cycle is
executed when this parameter value is 0, PS0456
alarm is also issued.
Grinding axis number of Traverse direct constant-size Grinding cycle(G72)
5177 Grinding axis number of Direct Constant Dimension Plunge Grinding
Cycle(G77)
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to Number of controlled axes
For the Lathe system:
Set the Grinding axis number of Traverse direct constant-size
Grinding cycle(G72).
For the Machining Center system:
Set the Grinding axis number of Direct Constant Dimension
Plunge Grinding Cycle (G77).
NOTE
The axis number except for the cutting axis can be
specified. When the axis number which is same to
cutting axis is specified, PS0456 alarm is issued at
the time of execution. The Grinding Cycle is
executed when this parameter value is 0, PS0456
alarm is also issued.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2089 -
Grinding axis number of Oscillation Grinding Cycle(G73)
5178
Grinding axis number of Continuous feed surface grinding cycle(G78)
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to Number of controlled axes
For the Lathe system:
Set the Grinding axis number of Oscillation Grinding
Cycle(G73).
For the Machining Center system:
Set the Grinding axis number of Continuous feed surface
grinding cycle(G78).
NOTE
The axis number except for the cutting axis can be
specified. When the axis number which is same to
cutting axis is specified, PS0456 alarm is issued at
the time of execution. The Grinding Cycle is
executed when this parameter value is 0, PS0456
alarm is also issued.
Grinding axis number of Oscillation Direct Fixed Dimension Grinding
Cycle(G74)
5179
Grinding axis number of Intermittent feed surface grinding cycle(G79)
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to Number of controlled axes
For the Lathe system:
Set the Grinding axis number of Oscillation Direct Fixed
Dimension Grinding Cycle(G74).
For the Machining Center system:
Set the Grinding axis number of Intermittent feed surface
grinding cycle(G79).
NOTE
The axis number except for the cutting axis can be
specified. When the axis number which is same to
cutting axis is specified, PS0456 alarm is issued at
the time of execution. The Grinding Cycle is
executed when this parameter value is 0, PS0456
alarm is also issued.
A.PARAMETERS APPENDIX B-63944EN/03
- 2090 -
5180
Axis number of dressing axis in Plunge grinding cycle(G75)
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to Number of controlled axes
Set the axis number of dressing axis in Plunge grinding cycle(G75).
NOTE
The axis number except for the cutting axis or
grinding axis can be specified. When the axis
number which is same to cutting axis or grinding
axis is specified, PS0456 alarm is issued at the
time of execution. The Grinding Cycle is executed
when this parameter value is 0 and address "L" is
specified in NC program, the PS0456 alarm is also
issued.
5181 Axis number of dressing axis in Direct constant dimension plunge grinding
cycle(G75)
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to Number of controlled axes
Set the axis number of dressing axis in Direct constant dimension
plunge grinding cycle(G75).
NOTE
The axis number except for the cutting axis or
grinding axis can be specified. When the axis
number which is same to cutting axis or grinding
axis is specified, PS0456 alarm is issued at the
time of execution. The Grinding Cycle is executed
when this parameter value is 0 and address "L" is
specified in NC program, the PS0456 alarm is also
issued.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2091 -
5182 Axis number of dressing axis in Continuous feed surface grinding
cycle(G78)
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to Number of controlled axes
Set the axis number of dressing axis in Continuous feed surface
grinding cycle(G78).
NOTE
The axis number except for the cutting axis or
grinding axis can be specified. When the axis
number which is same to cutting axis or grinding
axis is specified, PS0456 alarm is issued at the
time of execution. The Grinding Cycle is executed
when this parameter value is 0 and address "L" is
specified in NC program, the PS0456 alarm is also
issued.
5183
Axis number of dressing axis in Intermittent feed surface grinding cycle(G79)
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to Number of controlled axes
Set the axis number of dressing axis in Intermittent feed surface
grinding cycle(G79).
NOTE
The axis number except for the cutting axis or
grinding axis can be specified. When the axis
number which is same to cutting axis or grinding
axis is specified, PS0456 alarm is issued at the
time of execution. The Grinding Cycle is executed
when this parameter value is 0 and address "L" is
specified in NC program, the PS0456 alarm is also
issued.
A.PARAMETERS APPENDIX B-63944EN/03
- 2092 -
#7 #6 #5 #4 #3 #2 #1 #0
5200 CRG G84
[Input type] Parameter input
[Data type] Bit path
# 0 G84 Method for specifying rigid tapping:
0: An M code specifying the rigid tapping mode is specified prior to
the issue of the G84 (or G74) command. (See parameter
No.5210).
1: An M code specifying the rigid tapping mode is not used. (G84
cannot be used as a G code for the tapping cycle; G74 cannot be
used for the reverse tapping cycle.)
# 2 CRG Rigid mode when a rigid mode cancel command is specified (G80,
G01 group G code, reset, etc.) :
0: Canceled after rigid tapping signal RGTAP is set to "0".
1: Canceled before rigid tapping signal RGTAP is set to "0".
#7 #6 #5 #4 #3 #2 #1 #0
5202 CHR
[Input type] Parameter input
[Data type] Bit path
NOTE
When this parameter is set, the power must be
turned off before operation is continued..
# 3 CHR Rigid tapping is:
0: Normal rigid tapping.
1: Interpolation type rigid tapping.
NOTE
1 The rigid tapping function and interpolation type
rigid tapping function cannot be used together
within a path.
2 Before the interpolation type rigid tapping function
can be used, the Cs contour control function is
required. If interpolation type rigid tapping is
specified when the Cs contour control function is
disabled, an alarm (PS1223) is issued.
3 The interpolation type rigid tapping function cannot
be used in a path that has a spindle positioning
axis. If interpolation type rigid tapping is specified
for a path that has a spindle positioning axis, an
alarm (PS1223) is issued.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2093 -
#7 #6 #5 #4 #3 #2 #1 #0
5203 HRM HRG
[Input type] Parameter input
[Data type] Bit path
# 0 HRG Rigid tapping by the manual handle is:
0: Disabled.
1: Enabled.
# 1 HRM When the tapping axis moves in the negative direction during rigid
tapping controlled by the manual handle, the direction in which the
spindle rotates is determined as follows:
0: In G84 mode, the spindle rotates in a normal direction. In G74
mode, the spindle rotates in reverse.
1: In G84 mode, the spindle rotates in reverse. In G74 mode, the
spindle rotates in a normal direction.
5241 Maximum spindle speed in rigid tapping (first gear)
5242 Maximum spindle speed in rigid tapping (second gear)
5243 Maximum spindle speed in rigid tapping (third gear)
Maximum spindle speed in rigid tapping (fourth gear)
5244
[Input type] Parameter input
[Data type] 2-word spindle
[Unit of data] min-1
[Valid data range] 0 to 9999
Spindle position coder gear ratio
1 : 1 0 to 7400
1 : 2 0 to 9999
1 : 4 0 to 9999
1 : 8 0 to 9999
Each of these parameters is used to set a maximum spindle speed for
each gear in rigid tapping.
Set the same value for both parameter No.5241 and parameter
No.5243 for a one-stage gear system. For a two-stage gear system, set
the same value as set in parameter No. 5242 in parameter No. 5243.
Otherwise, alarm PS0200 will be issued. This applies to the M series.
A.PARAMETERS APPENDIX B-63944EN/03
- 2094 -
#7 #6 #5 #4 #3 #2 #1 #0
5400 SCR XSC D3R
[Input type] Parameter input
[Data type] Bit path
# 2 D3R When Reset is done by reset operation or reset signal from PMC,
three-dimensional coordinate system conversion mode, tilted working
plane command mode and workpiece setting error compensation mode
is:
0: Canceled.
1: Not canceled.
# 6 XSC The setting of a scaling magnification (axis-by-axis scaling) is:
0: Disabled.
1: Enabled.
# 7 SCR Scaling (G51) magnification unit:
0: 0.00001 times (1/100,000)
1: 0.001 times
#7 #6 #5 #4 #3 #2 #1 #0
5401 SCLx
[Input type] Parameter input
[Data type] Bit axis
# 0 SCLx Scaling on this axis:
0: Invalidated
1: Validated
5411 Scaling (G51) magnification
[Input type] Setting input
[Data type] 2-word path
[Unit of data] 0.001 or 0.00001 times (Selected using SCR, #7 of parameter
No.5400)
[Valid data range] 1to999999999
This parameter sets a scaling magnification when axis-by-axis scaling
is disabled (with bit 6 (XSC) of parameter No. 5400 set to 0). If no
scaling magnification (P) is specified in the program, the setting of
this parameter is used as a scaling magnification.
NOTE
When bit 7 (SCR) of parameter No.5400 is set to 1,
the valid data range is 1 to 9999999.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2095 -
5412 Rapid traverse rate for canned cycle for drilling in three-dimensional
coordinate conversion mode
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
This parameter sets a rapid traverse rate for canned cycle for drilling
in the three-dimensional coordinate conversion mode, the tilted
working plane command mode, or the workpiece setting error
compensation mode.
5421 Scaling magnification for each axis
[Input type] Setting input
[Data type] 2-word axis
[Unit of data] 0.001 or 0.00001 times (Selected using SCR, #7 of parameter
No.5400)
[Valid data range] -999999999 to –1, 1 to 999999999
This parameter sets a scaling magnification for each axis when
axis-by-axis scaling is enabled (with bit 6 (XSC) of parameter No.
5400 set to 1). For the first spindle to the third spindle (X-axis to
Z-axis), the setting of this parameter is used as a scaling magnification
if scaling magnifications (I, J, K) are not specified in the program.
NOTE
When bit 7 (SCR) of parameter No.5400 is set to 1,
the valid data ranges are -9999999 to -1 and 1 to
9999999.
#7 #6 #5 #4 #3 #2 #1 #0
5431 MDL
[Input type] Parameter input
[Data type] Bit path
NOTE
When this parameter is set, the power must be
turned off before operation is continued..
# 0 MDL The G60 code (one-direction positioning) is:
0: One-shot G code (group 00).
1: Modal G code (group 01).
A.PARAMETERS APPENDIX B-63944EN/03
- 2096 -
5440 Positioning direction and overrun distance in single directional positioning
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm, inch, degree (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (A)
(When the increment system is IS-B, -999999.999 to +999999.999)
This parameter sets the positioning direction and overrun distance in
single directional positioning (G60) for each axis. The positioning
direction is specified using a setting data sign, and the overrun
distance using a value set here.
Overrun distance>0: The positioning direction is positive (+).
Overrun distance<0: The positioning direction is negative (*).
Overrun distance=0: Single directional positioning is not performed.
#7 #6 #5 #4 #3 #2 #1 #0
5450 PLS
[Input type] Parameter input
[Data type] Bit path
# 2 PLS The polar coordinate interpolation shift function is:
0: Not used.
1: Used.
This enables machining using the workpiece coordinate system with a
desired point which is not the center of the rotation axis set as the
origin of the coordinate system in polar coordinate interpolation.
5460 Axis (linear axis) specification for polar coordinate interpolation
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to number of controlled axes
This parameter sets control axis numbers of linear axis to execute
polar interpolation.
5461 Axis (rotation axis) specification for polar coordinate interpolation
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to number of controlled axes
This parameter sets control axis numbers of rotation axis to execute
polar interpolation.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2097 -
5463 Automatic override tolerance ratio for polar coordinate interpolation
[Input type] Parameter input
[Data type] Byte path
[Unit of data] %
[Valid data range] 0 to 100
Typical setting: 90% (treated as 90% when set to 0)
Set the tolerance ratio of the fastest cutting feedrate to the speed of the
rotation axis during automatic override of polar coordinate
interpolation.
5464 Compensation for error on hypothetical axis of polar coordinate
interpolation
[Input type] Parameter input
[Data type] Byte path
[Unit of data] mm, inch (input unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(For IS-B, -999999.999 to +999999.999)
This parameter is used to set the error if the center of the rotation axis
on which polar coordinate interpolation is performed is not on the
X-axis.
If the setting of the parameter is 0, regular polar coordinate
interpolation is performed.
5481
Feedrate of rotation of the normal direction controlled axis
[Input type] Parameter input
[Data type] Real axis
[Unit of data] deg/min
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (C)
This parameter sets the feedrate of the movement along the normal
direction controlled axis that is inserted at the start point of a block
during normal direction control.
A.PARAMETERS APPENDIX B-63944EN/03
- 2098 -
5483 Limit value of movement that is executed at the normal direction angle of a
preceding block
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm, inch (input unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 0 or positive 9 digit of minimum unit of data (refer to standard
parameter setting table (B)
N1
Tool center path N2
Travel distance
Programmed path
For straight line
When the travel distance of N2 in the figure on
the left does not exceed the setting, block N2 is
machined with the tool being normal to block N1.
N3
Diameter
Programmed path
Tool center path
N2
For arc
When the arc diameter of N2 in the figure on the left
does not exceed the setting, arc N2 is machined with
the tool being normal to block N1. A normal direction
axis is not controlled to move in the normal direction
according to the arc mov
N1
N3
#7 #6 #5 #4 #3 #2 #1 #0
5630 SPN
[Input type] Parameter input
[Data type] Bit path
# 0 SPN The amount of linear axis division (span value) in exponential
interpolation is:
0: Specified with parameter No.5643.
1: Specified using address K in a block containing G02.3/G03.3.
When address K is not specified, the value set with parameter
No.5643 is used.
5641 Linear axis number subject to exponential interpolation
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to number of controlled axes
This parameter sets the ordinal number, among the controlled axes, for
the linear axis to which exponential interpolation is applied.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2099 -
5642 Rotation axis number subject exponential interpolation
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to number of controlled axes
This parameter sets the ordinal number, among the controlled axes, for
the rotation axis to which exponential interpolation is applied.
5643 Amount of linear axis division (span value) in exponential interpolation
[Input type] Setting input
[Data type] Real path
[Unit of data] mm, inch (machine unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 0 to 999999999
This parameter sets an amount of linear axis division in exponential
interpolation when bit 0 (SPN) of parameter No.5630 is set to 0 or
when address K is not specified.
A.PARAMETERS APPENDIX B-63944EN/03
- 2100 -
#7 #6 #5 #4 #3 #2 #1 #0
SBM HGO MGO G67
6000 SBM HGO V15 MGO G67
[Input type] Parameter input
[Data type] Bit path
# 0 G67 If the macro modal call cancel command (G67) is specified when the
macro modal call mode (G66/G66.1) is not set:
0: Alarm PS0122 is issued.
1: The specification of G67 is ignored.
# 1 MGO When a GOTO statement for specifying custom macro control is
executed, a high-speed branch to 20 sequence numbers executed from
the start of the program is:
0: A high-speed branch is not caused to n sequence numbers from
the start of the executed program.
1: A high-speed branch is caused to n sequence numbers from the
start of the program.
# 3 V15 As system variable numbers for tool offset:
0 : The standard system variable numbers for the Series 16 are used.
1 : The same system variable numbers as those used for the Series
15 are used.
The tables below indicate the system variables for tool offset numbers
1 to 999. The values for tool offset numbers 1 to 200 can be read from
or assigned to the system variables in parentheses.
(1) Tool offset memory A
System variable number
V15 = 0 V15 = 1
Wear offset value #10001 to #10999
(#2001 to #2200)
#10001 to #10999
(#2001 to #2200)
(2) Tool offset memory B
System variable number
V15 = 0 V15 = 1
Geometry offset
value
#11001 to #11999
(#2201 to #2400)
#10001 to #10999
(#2001 to #2200)
Wear offset value #10001 to #10999
(#2001 to #2200)
#11001 to #11999
(#2201 to #2400)
(3) Tool offset memory C
System variable number
V15 = 0 V15 = 1
Geometry
offset value
#11001 to #11999
(#2201 to #2400)
#10001 to #10999
(#2001 to #2200)
Tool
length
offset Wear offset
value
#10001 to #10999
(#2001 to #2200)
#11001 to #11999
(#2201 to #2400)
Geometry
offset value #13001 to #13999 #12001 to #12999
Tool
radius
offset Wear offset
value #12001 to #12999 #13001 to #13999
B-63944EN/03 APPENDIX A.PARAMETERS
- 2101 -
# 4 HGO When a GOTO statement in a custom macro control command is
executed, a high-speed branch to the 30 sequence numbers
immediately before the executed statement is:
0: Not made.
1: Made.
# 5 SBM Custom macro statement
0: Not stop the single block
1: Stops the single block
If you want to disable the single blocks in custom macro statements
using system variable #3003, set this parameter to 0. If this parameter
is set to 1, the single blocks in custom macro statements cannot be
disabled using system variable #3003. To control single blocks in
custom macro statements using system variable #3003, use bit 7
(SBV) of parameter No. 6000.
#7 #6 #5 #4 #3 #2 #1 #0
6001 CCV TCS CRO PV5 PRT MIF
[Input type] Parameter input
[Data type] Bit path
# 0 MIF The custom macro interface signals are based on:
0: Standard specification.
(The signals UI000 to UI015, UO000 to UO015, and UO100 to
UO131 are used.)
1: Extended specification.
(The signals UI000 to UI031, UI100 to UI131, UI200 to UI231,
UI300 to UI331, UO000 to UO031, UO100 to UO131, UO200 to
UO231, and UO300 to UO331 are used.)
# 1 PRT Reading zero when data is output using a DPRINT command
0: Outputs a space
1: Outputs no data
A.PARAMETERS APPENDIX B-63944EN/03
- 2102 -
# 3 PV5 Custom macro common variables:
0: #500 to #549 are output. (Note)
1: #100 to #149 and #500 to 549 are output. (Note)
NOTE
Output variables are as follows according to the
combination of added options.
When the parameter PV5=0
Option “Addition of custom macro common
variables”
Non Yes
Non #500 to #549 #500 to #999
Option
“Embedded
macro” Yes #500 to #549 #500 to #999
When the parameter PV5=1
Option “Addition of custom macro common
variables”
Non Yes
Non #100 to #149 and
#500 to #549
#100 to #199 and
#500 to #999
Option
“Embedded
macro” Yes #100 to #149, #200 to
#499 and #500 to #549
#100 to #199, #200 to
#499 and #500 to #999
# 4 CRO ISO code in BPRWT or DPRNT command
0: Outputs only “LF” after data is output
1: Outputs “LF” and “CR” after data is output
# 5 TCS Custom macro (subprogram)
0: Not called using a T code
1: Called using a T code
# 6 CCV Common variables #100 to #149(NOTE) cleared by power-off are:
0: Cleared to <null> by reset
1: Not cleared by reset
NOTE
Cleared variables are as follows according to the
combination of added options.
Option “Addition of custom macro common
variables”
Non Yes
Non #100 to #149 #100 to #199
Option
“Embedded
macro” Yes #100 to #149 and
#200 to #499
#100 to #199 and
#200 to #499
B-63944EN/03 APPENDIX A.PARAMETERS
- 2103 -
#7 #6 #5 #4 #3 #2 #1 #0
6003 MSB MPR TSE MIN
[Input type] Parameter input
[Data type] Bit path
NOTE
When at least one of these parameters is set, the
power must be turned off before operation is
continued.
# 2 MIN Custom macro interrupt
0: Performed by interrupting an in-execution block (Custom macro
interrupt type I)
1: Performed after an in-execution block is completed (Custom
macro interrupt type II)
# 3 TSE Custom macro interrupt signal UINT
0: Edge trigger method (Rising edge)
1: Status trigger method
# 4 MPR Custom macro interrupt valid/invalid M code
0: M96/M97
1: M code set using parameters (Nos. 6033 and 6034)
# 5 MSB Interrupt program
0: Uses a dedicated local variable (Macro-type interrupt)
1: Uses the same local variable as in the main program
(Subprogram- type interrupt)
#7 #6 #5 #4 #3 #2 #1 #0
VHD NAT
6004 D15 NAT
[Input type] Parameter input
[Data type] Bit path
# 0 NAT The results of the custom macro functions ATAN (with 2 arguments)
and ASIN are specified as follows:
0: The result of ATAN is 0 to 360.0.
The result of ASIN is 270.0 to 0 to 90.0.
1: The result of ATAN is -180.0 to 0 to 180.0.
The result of ASIN is -90.0 to 0 to 90.0.
# 2 VHD With system variables #5121 to #5140:
0: The tool offset value (geometry offset value) in the block
currently being executed is read. (This parameter is valid only
when tool geometry/tool wear compensation memories are
available.)
1: An interrupt travel distance based on manual handle interrupt is
read.
A.PARAMETERS APPENDIX B-63944EN/03
- 2104 -
# 5 D15 When tool compensation memory C is used, for reading or writing
tool offset values (for up to offset number 200) for D code (tool
radius), the same system variables, #2401 through #2800, as Series 15
are:
0: Not used.
1: Used.
When bit 3 (V15) of parameter No. 6000 is set to 1
D code
Geometry Wear
Compensation
number Variable
number Variable name Variable
number Variable name
1 #2401 [#_OFSDG[1]] #2601 [#_OFSDW[1]]
2 #2402 [#_OFSDG[2]] #2602 [#_OFSDW[2]]
3 #2403 [#_OFSDG[3]] #2603 [#_OFSDW[3]]
: : : : :
199 #2599 [#_OFSDG[199]] #2799 [#_OFSDW[199]]
200 #2600 [#_OFSDG[200]] #2800 [#_OFSDW[200]]
#7 #6 #5 #4 #3 #2 #1 #0
6005 SQC
[Input type] Parameter input
[Data type] Bit path
# 0 SQC In the subprogram call function, a subprogram sequence number call
is:
0: Not used.
1: Used.
#7 #6 #5 #4 #3 #2 #1 #0
6007 CVA MGE BCS SCS DPG
[Input type] Parameter input
[Data type] Bit path
# 0 DPG Specifies whether to allow G codes with a decimal point to be called.
0: Do not allow.
1: Allow.
# 1 SCS Specifies whether to call subprograms with S codes.
0: Do not call with S codes.
1: Call with S codes.
# 2 BCS Specifies whether to call subprograms with the second auxiliary
function codes.
0: Do not call with the second auxiliary function codes.
1: Call with the second auxiliary function codes.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2105 -
# 3 MGE Specifies whether a G code modal call is made after movement or for
each block.
0: Make a call for each block (equivalent to G66.1).
1: Make a call after movement (equivalent to G66).
# 4 CVA The format for macro call arguments is specified as follows:
0: Arguments are passed in NC format without modifications.
1: Arguments are converted to macro format then passed.
Example)
When G65 P_ X10 ; is specified, the value in local variable #24
in the calling program is set as follows:
Command CVA=0 CVA=1
#24 0.01 0.01
ADP[#24] 10.0 0.01
NOTE
External operations are the same unless the ADP
function is used.
#7 #6 #5 #4 #3 #2 #1 #0
6008 IJK GMP ISO MCA F16
[Input type] Parameter input
[Data type] Bit path
# 0 F16 The precision of operation is based on:
0: New specification.
1: FS16i compatible specification.
# 1 MCA A macro alarm specification based on system variable #3000 is
selected as follows:
0: An alarm number obtained by adding 3000 to a value assigned to
variable #3000 and the corresponding message are displayed. (A
value from 0 to 200 can be assigned to variable #3000.)
1: A value assigned to variable #3000 and the corresponding
message are displayed. (A value from 0 to 4095 can be assigned
to variable #3000.)
(Example)
Execution of #3000=1 (ALARM MESSAGE);
When bit 1 (MCA) of parameter No. 6008 is set to 0:
The alarm screen displays "MC 3001 ALARM
MESSAGE".
When bit 1 (MCA) of parameter No. 6008 is set to 1:
The alarm screen displays "MC0001 ALARM MESSAGE".
# 4 ISO
0: When the EIA code is used, the bit patterns of codes specified
instead of [, ], #, *, =, ?, @, &, and _ are set in parameter No.
6010 to No. 6018.
1: When the ISO/ASCII code is used, the bit patters of codes
specified instead of [, ], #, *, =, ?, @, &, and _ are set in
parameter No. 6010 to No. 6018.
A.PARAMETERS APPENDIX B-63944EN/03
- 2106 -
# 6 GMP The calling of M, S, T, a second auxiliary function code, or a
particular code during the calling of a G code, and the calling of a G
code during the calling of M, S, T, a second auxiliary function code,
or particular code are:
0: Not allowed. (They are executed as an ordinary G, M, S, T,
second auxiliary function code, and NC address.)
1: Allowed.
#7 IJK For addresses I, J, and K specified as arguments:
0: Argument specification I or II is automatically determined.
1: Argument specification I is always used.
Example
When K_J_I_ is specified:
• When this parameter is set to 0:
Argument specification II is used and K=#6, J=#8,
and I=#10 are specified.
• When this parameter is set to1:
Argument specification I is used and I=#4, J=#5,
and K=#6 are specified regardless of the
specification order.
(Argument specification II cannot be used.)
B-63944EN/03 APPENDIX A.PARAMETERS
- 2107 -
#7 #6 #5 #4 #3 #2 #1 #0
6010 *7 *6 *5 *4 *3 *2 *1 *0
#7 #6 #5 #4 #3 #2 #1 #0
6011 =7 =6 =5 =4 =3 =2 =1 =0
#7 #6 #5 #4 #3 #2 #1 #0
6012 #7 #6 #5 #4 #3 #2 #1 #0
#7 #6 #5 #4 #3 #2 #1 #0
6013 [7 [6 [5 [4 [3 [2 [1 [0
#7 #6 #5 #4 #3 #2 #1 #0
6014 ]7 ]6 ]5 ]4 ]3 ]2 ]1 ]0
#7 #6 #5 #4 #3 #2 #1 #0
6015 ?7 ?6 ?5 ?4 ?3 ?2 ?1 ?0
#7 #6 #5 #4 #3 #2 #1 #0
6016 @7 @6 @5 @4 @3 @2 @1 @0
#7 #6 #5 #4 #3 #2 #1 #0
6017 &7 &6 &5 &4 &3 &2 &1 &0
#7 #6 #5 #4 #3 #2 #1 #0
6018 _7 _6 _5 _4 _3 _2 _1 _0
[Input type] Parameter input
[Data type] Bit path
*0 to *7 : The bit pattern of the EIA or ISO/ASCII code indicating * is set.
=0 to =7 : The bit pattern of the EIA or ISO/ASCII code indicating = is set.
#0 to #7 : The bit pattern of the EIA or ISO/ASCII code indicating # is set.
[0 to [7 : The bit pattern of the EIA or ISO/ASCII code indicating [ is set.
]0 to ]7 : The bit pattern of the EIA or ISO/ASCII code indicating ] is set.
?0 to ?7 : The bit pattern of the EIA or ISO/ASCII code indicating ? is set.
@0 to @7 : The bit pattern of the EIA or ISO/ASCII code indicating @ is set.
&0 to &7 : The bit pattern of the EIA or ISO/ASCII code indicating & is set.
_0 to _7 : The bit pattern of the EIA or ISO/ASCII code indicating _ is set.
0: A corresponding bit is 0.
1: A corresponding bit is 1.
A.PARAMETERS APPENDIX B-63944EN/03
- 2108 -
#7 #6 #5 #4 #3 #2 #1 #0
6019 MCO
[Input type] Parameter input
[Data type] Bit
#0 MCO When data is output, the decimal number value of the macro variable
data is
0: Not output as a comment.
1: Output at the same time as a comment.
After the number, data, and the variable name of the macro variable
are output when data output operation is performed the variable
number and the value of the macro variable data in decimal number
are output as a comment.
NOTE
1 Output data by this parameter is "Comment", and
this is ignored at the time of reading.
2 Accuracy of the output data of the comment is up
to 15 digits. The range of output data are nine
digits above decimalpoint and eight digits below
decimal point. "± OVER FLOW" is output instead of
a value when the total digits number is more than
16 and the digit number above the decimal point is
ten or more. When the number of digits below the
decimal point becomes nine digits or more, the
ninth place of the decimal point is rounded off and
output. Moreover, the seventh place or the eighth
place of the decimal point is rounded off and output
when the total digits number is more than 16 and
the digit number above decimal point is nine or
eight.
3 The output becomes "EMPTY" when displayed, the
macro variable data is "DATA EMPTY".
6030 M code to execute external device subprogram calls
[Input type] Setting input
[Data type] 2-word path
[Valid data range] 0 to 99999999
Set the M code to execute external device subprogram calls. When 0 is
set, M198 is used. M01, M02, M30, M98, and M99 cannot be used to
execute external device subprogram calls. When a negative number, 1,
2, 30, 98, or 99 is set for this parameter, M198 is used to execute
external device subprogram calls.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2109 -
6031 Start number of common variables to be protected among the common
variables (#500 to #999)
6032 End number of common variables to be protected among the common
variables (#500 to #999)
[Input type] Parameter input
[Data type] Word path
[Valid data range] 500 to 999
Among the common variables (#500 to #999), the range of common
variables specified by this parameter can be protected (by setting their
attributes to read-only). If a write attempt (on the left side) is made, an
alarm is issued.
NOTE
Set 0 in both parameter No. 6031 and No. 6032 not
to protect common variables.
6033 M code that validates a custom macro interrupt
6034 M code that invalidates a custom macro interrupt
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 03 to 99999999 (excluding 30, 98 and 99)
These parameters can be used when bit 4 (MPR) of parameter
No.6003, is 1. M96 is used as a valid M code and M97 is used as an
invalid M code when MPR is 0, irrespective of the state of this
parameter.
A.PARAMETERS APPENDIX B-63944EN/03
- 2110 -
6036 Number of custom macro variables common to tool path
(for #100 to #199 (#499))
[Input type] Parameter input
[Data type] Word
[Valid data range] 0 to 400
When the memory common to paths is used, this parameter sets the
number of custom macro common variables to be shared (custom
macro variables common to paths). Common variables #100 to #199
(up to #499 in a system with the embedded macro option) may be
shared. Ensure that the maximum number of usable macro common
variables is not exceeded.
Example
When 20 is set in parameter No. 6036
#100 to #119: Shared by all paths
#120 to #149: Used by each path independently
NOTE
1 To use up to #199, the option for adding custom
macro common variables is required.
2 To use up to #499, the embedded macro option is
required.
3 When 0 or a negative value is set, the memory
common to paths is not used.
4 When the option for embedded macro is effective
and the option for addition of custom macro
common variables is not effective, #150 to #199
can not be used but this parameter should be set
the number which includes #150 to #199.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2111 -
6037 Number of custom macro variables common to tool path (for #500 to #999)
[Input type] Parameter input
[Data type] Word
[Valid data range] 0 to 500
When the memory common to paths is used, this parameter sets the
number of custom macro common variables to be shared (custom
macro variables common to paths). Common variables #500 to #999
may be shared. Ensure that the maximum number of usable macro
common variables is not exceeded.
Example
When 50 is set in parameter No. 6037
#500 to #549: Shared by all paths
#550 to #599: Used by each path independently
NOTE
1 To use up to #999, the option for adding custom
macro common variables is required.
2 When 0 or a negative value is set, the memory
common to paths is not used.
6038 Start G code used to call a custom macro
[Input type] Parameter input
[Data type] Word path
[Valid data range] -9999 to 9999
6039 Start program number of a custom macro called by G code
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 1 to 9999
A.PARAMETERS APPENDIX B-63944EN/03
- 2112 -
6040 Number of G codes used to call custom macros
[Input type] Parameter input
[Data type] Word path
[Valid data range] 0 to 255
Set this parameter to define multiple custom macro calls using G
codes at a time. With G codes as many as the value set in parameter
No. 6040 starting with the G code set in parameter No. 6038, the
custom macros of program numbers as many as the value set in
parameter No. 6040 starting with the program number set in parameter
No. 6039 can be called. Set 0 in parameter No. 6040 to disable this
mode of calling.
If a negative value is set in parameter No. 6038, the modal call mode
is entered. Whether the modal call is equivalent to G66 or G66.1
depends on bit 3 (MGE) of parameter No. 6007.
Example)
When parameter No. 6038 = 900, parameter No. 6039 = 1000,
and parameter No. 6040 = 100 are set, a set of 100 custom macro
calls (simple calls) is defined as follows:
G900 → O1000
G901 → O1001
G902 → O1002
:
G999 → O1099
When the setting of parameter No. 6038 is changed to -900, the
same set of custom macro calls (modal calls) is defined.
NOTE
1 When the following conditions are satisfied, all calls
using these parameters are disabled:
1) When a value not within the specifiable range is
set in each parameter
2) (Value of parameter No.6039 + value of
parameter No.6040 - 1) > 9999
2 The specification of a mixture of simple calls and
modal calls is not allowed.
3 If a range of G codes set by these parameters
duplicate G codes specified in parameter No.6050
to No.6059, the calls specified by parameter
No.6050 to 6059 are made preferentially.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2113 -
6041 Start G code with a decimal point used to call a custom macro
[Input type] Parameter input
[Data type] Word path
[Valid data range] -999 to 999
6042 Start program number of a custom macro called by G code with a decimal point
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 1 to 9999
6043 Number of G codes with a decimal point used to call custom macros
[Input type] Parameter input
[Data type] Word path
[Valid data range] 0 to 255
Set this parameter to define multiple custom macro calls using G
codes with a decimal point at a time. With G codes with a decimal
point as many as the value set in parameter No. 6043 starting with the
G code with a decimal point set in parameter No. 6041, the custom
macros of program numbers as many as the value set in parameter No.
6043 starting with the program number set in parameter No. 6042 can
be called. Set 0 in parameter No. 6043 to disable this mode of calling.
If a negative value is set in parameter No. 6041, the modal call mode
is entered. Whether the modal call is equivalent to G66 or G66.1
depends on bit 3 (MGE) of parameter No. 6007.
Example)
When parameter No. 6041 = 900, parameter No. 6042 = 2000,
and parameter No. 6043 = 100 are set, a set of 100 custom macro
calls (simple calls) is defined as follows:
G90.0 → O2000
G90.1 → O2001
G90.2 → O2002
:
G99.9 → O2099
When the setting of parameter No. 6041 is changed to -900, the
same set of custom macro calls (modal calls) is defined.
NOTE
1 When the following conditions are satisfied, all calls using these parameters are
disabled:
1) When a value not within the specifiable range is set in each parameter
2) (Value of parameter No.6042 + value of parameter No.6043 - 1) > 9999
3) When bit 0 (DPG) of parameter No. 6007 = 0 (to disable calls using G codes
with a decimal point)
2 The specification of a mixture of simple calls and modal calls is not allowed.
3 If a range of G codes set by these parameters duplicate G codes specified in
parameter No.6060 to No.6069, the calls specified by parameter No.6060 to 6069
are made preferentially.
A.PARAMETERS APPENDIX B-63944EN/03
- 2114 -
6044 Start M code used to call a subprogram
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 3 to 99999999
6045 Start program number of a subprogram called by M code
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 1 to 9999
6046 Number of M codes used to call subprograms (number of subprograms
called by M codes)
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 0 to 32767
Set this parameter to define multiple subprogram calls using M codes
at a time. With M codes as many as the value set in parameter No.
6046 starting with the M code set in parameter No. 6044, the
subprograms of program numbers as many as the value set in
parameter No. 6046 starting with the program number set in 6045 can
be called. Set 0 in parameter No. 6046 to disable this mode of calling.
Example)
When parameter No. 6044 = 80000000, parameter No. 6045 =
3000, and parameter No. 6046 = 100 are set, a set of 100
subprogram calls is defined as follows:
M80000000 → O3000
M80000001 → O3001
M80000002 → O3002
:
M80000099 → O3099
NOTE
1 When the following conditions are satisfied, all calls
using these parameters are disabled:
1) When a value not within the specifiable range is
set in each parameter
2) (Value of parameter No. 6045 + value of
parameter No. 6046 - 1) > 9999
2 If a range of M codes set by these parameters
duplicate M codes specified in parameter No. 6071
to No. 6079, the calls specified by parameter No.
6071 to 6079 are made preferentially.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2115 -
6047 Start M code used to call a custom macro
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 3 to 99999999
6048 Start program number of a custom macro called by M code
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 1 to 9999
6049 Number of M codes used to call custom macros (number of custom macros
called by M codes)
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 0 to 32767
Set this parameter to define multiple custom macro calls using M
codes at a time. With M codes as many as the value set in parameter
No. 6049 starting with the M code set in parameter No. 6047, the
custom macros of program numbers as many as the value set in
parameter No. 6049 starting with the program number set in parameter
No. 6048 can be called. Set 0 in parameter No. 6049 to disable this
mode of calling.
Example)
When parameter No. 6047 = 90000000, parameter No. 6048 =
4000, and parameter No. 6049 = 100 are set, a set of 100 custom
macro calls (simple calls) is defined as follows:
M90000000 → O4000
M90000001 → O4001
M90000002 → O4002
:
M90000099 → O4099
NOTE
1 When the following conditions are satisfied, all calls
using these parameters are disabled:
1) When a value not within the specifiable range is
set in each parameter
2) (Value of parameter No. 6048 + value of
parameter No. 6049 - 1) > 9999
2 If a range of M codes set by these parameters
duplicate M codes specified in parameter No. 6080
through No. 6089, the calls specified by parameter
No. 6080 through 6089 are made preferentially.
A.PARAMETERS APPENDIX B-63944EN/03
- 2116 -
6050 G code that calls the custom macro of program number 9010
6051 G code that calls the custom macro of program number 9011
6052 G code that calls the custom macro of program number 9012
6053 G code that calls the custom macro of program number 9013
6054 G code that calls the custom macro of program number 9014
6055 G code that calls the custom macro of program number 9015
6056 G code that calls the custom macro of program number 9016
6057 G code that calls the custom macro of program number 9017
6058 G code that calls the custom macro of program number 9018
6059 G code that calls the custom macro of program number 9019
[Input type] Parameter input
[Data type] Word path
[Valid data range] (-9999 to 9999 : excluding 0, 5, 65, 66 and 67)
Set the G codes used to call the custom macros of program numbers
9010 to 9019. However, note that when a negative value is set in this
parameter, it becomes a modal call. For example, if this parameter is
set to -11, the modal call mode is entered by G11.
Whether the modal call is equivalent to G66 or G66.1 depends on bit 3
(MGE) of parameter No. 6007.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2117 -
6060 G code with a decimal point used to call the custom macro of program
number 9040
6061 G code with a decimal point used to call the custom macro of program
number 9041
6062 G code with a decimal point used to call the custom macro of program
number 9042
6063 G code with a decimal point used to call the custom macro of program
number 9043
6064 G code with a decimal point used to call the custom macro of program
number 9044
6065 G code with a decimal point used to call the custom macro of program
number 9045
6066 G code with a decimal point used to call the custom macro of program
number 9046
6067 G code with a decimal point used to call the custom macro of program
number 9047
6068 G code with a decimal point used to call the custom macro of program
number 9048
6069 G code with a decimal point used to call the custom macro of program
number 9049
[Input type] Parameter input
[Data type] Word path
[Valid data range] -999 to 999
Set the G codes used to call the custom macros of program numbers
9040 to 9049. However, note that when a negative value is set in this
parameter, it becomes a modal call. For example, if this parameter is
set to -11, the modal call mode is entered by G1.1.
Whether the modal call is equivalent to G66 or G66.1 depends on bit 3
(MGE) of parameter No. 6007. Set G codes in the format Gm.n. The
value expressed by (m×10+n) is set in the parameter. The values m
and n must satisfy the following relationships: 0 ≤m ≤99, 0 ≤n ≤9.
NOTE
Parameter Nos. 6060 to 6069 are valid when bit 0
(DPG) of parameter No. 6007 is set to 1.
A.PARAMETERS APPENDIX B-63944EN/03
- 2118 -
6071 M code used to call the subprogram of program number 9001
6072 M code used to call the subprogram of program number 9002
6073 M code used to call the subprogram of program number 9003
6074 M code used to call the subprogram of program number 9004
6075 M code used to call the subprogram of program number 9005
6076 M code used to call the subprogram of program number 9006
6077 M code used to call the subprogram of program number 9007
6078 M code used to call the subprogram of program number 9008
6079 M code used to call the subprogram of program number 9009
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 3 to 99999999 (excluding 30, 98 and 99)
These parameters set the M codes that call the subprograms of
program numbers 9001 to 9009.
NOTE
If the same M code is set in these parameters, the
younger number is called preferentially. For
example, if 100 is set in parameter No. 6071 and
6072, and programs O9001 and O9002 both exist,
O9001 is called when M100 is specified.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2119 -
6080 M code used to call the custom macro of program number 9020
6081 M code used to call the custom macro of program number 9021
6082 M code used to call the custom macro of program number 9022
6083 M code used to call the custom macro of program number 9023
6084 M code used to call the custom macro of program number 9024
6085 M code used to call the custom macro of program number 9025
6086 M code used to call the custom macro of program number 9026
6087 M code used to call the custom macro of program number 9027
6088 M code used to call the custom macro of program number 9028
6089 M code used to call the custom macro of program number 9029
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 3 to 99999999 (excluding 30, 98 and 99)
Set the M codes used to call the custom macros of program numbers
9020 to 9029. The simple call mode is set.
NOTE
1 If the same M code is set in these parameters, the
younger number is called preferentially. For
example, if 200 is set in parameter No. 6081 and
No. 6082, and programs O9021 and O9022 both
exist, O9021 is called when M200 is specified.
2 If the same M code is set in a parameter (No. 6071
to No. 6079) used to call subprograms and in a
parameter (No. 6080 to No. 6089) used to call
custom macros, a custom macro is called
preferentially. For example, if 300 is set in
parameter No. 6071 and No. 6081, and programs
O9001 and O9021 both exist, O9021 is called
when M300 is specified.
A.PARAMETERS APPENDIX B-63944EN/03
- 2120 -
6090 ASCII code that calls the subprogram of program number 9004
6091 ASCII code that calls the subprogram of program number 9005
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 65(A:41H) to 90(Z:5AH)
These parameters set the ASCII codes that call subprograms in
decimal.
The settable addresses are indicated below.
Address Parameter setting value T series M series
A 65 O O
B 66 O O
D 68 X O
F 70 O O
H 72 O O
I 73 O O
J 74 O O
K 75 O O
L 76 O O
M 77 O O
P 80 O O
Q 81 O O
R 82 O O
S 83 O O
T 84 O O
V 86 X O
X 88 X O
Y 89 X O
Z 90 X O
NOTE
1 When address L is set, the number of repeats
cannot be specified.
2 Set 0 when no subprogram is called.
#7 #6 #5 #4 #3 #2 #1 #0
6200 SKF SRE SLS HSS SK0 GSK
[Input type] Parameter input
[Data type] Bit path
# 0 GSK As a skip signal, the skip signal SKIPP is:
0: Invalid.
1: Valid.
# 1 SK0 This parameter specifies whether the skip signal is made valid under
the state of the skip signal SKIP and the multistage skip signals SKIP2
to SKIP8.
0: Skip signal is valid when these signals are 1.
1: Skip signal is valid when these signals are 0.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2121 -
# 4 HSS
0: The skip function does not use high-speed skip signals while skip
signals are input. (The conventional skip signal is used.)
1: The step skip function uses high-speed skip signals while skip
signals are input.
# 5 SLS
0: The multi-step skip function does not use high-speed skip signals
while skip signals are input. (The conventional skip signal is
used.)
1: The multi-step skip function uses high-speed skip signals while
skip signals are input.
NOTE
The skip signals (SKIP and SKIP2 to SKIP8) are
valid regardless of the setting of this parameter.
They can also be disabled using bit 4 (IGX) of
parameter No. 6201.
# 6 SRE When a high-speed skip signal or high-speed measurement position
arrival signal is used:
0: The signal is assumed to be input on the rising edge (contact
open → close).
1: The signal is assumed to be input on the falling edge (contact
close → open).
# 7 SKF Dry run, override, and automatic acceleration/deceleration for G31
skip command
0: Disabled
1: Enabled
#7 #6 #5 #4 #3 #2 #1 #0
6201 SKPXE CSE IGX TSE SEB
[Input type] Parameter input
[Data type] Bit path
# 1 SEB When a skip signal or measurement position arrival signal goes on
while the skip function, or the automatic tool length measurement (M
series) or automatic tool compensation (T series) is used, the
accumulated pulses and positional deviation due to
acceleration/deceleration are:
0: Ignored.
1: Considered and compensated.
The accumulated pulses and positional deviation due to actual
acceleration/deceleration when the skip signal or measurement
position arrival signal goes on are considered to obtain the position at
which the signal is input.
A.PARAMETERS APPENDIX B-63944EN/03
- 2122 -
# 2 TSE When the torque limit skip function (G31 P98/99) is used, the skip
position held in a system variable (#5061 to #5080) is:
0: Position that is offset considering the delay (positional deviation)
incurred by the servo system.
1: Position that does not reflect the delay incurred by the servo
system.
Position during skip operation
Current position of CNC
Machine position Error amount
Position in consideration of delay
Position without consideration of delay
Origin of the coordinate system Stop point
# 4 IGX When the high-speed skip function is used, SKIP, SKIPP, and SKIP2
to SKIP8 are:
0: Enabled as skip signals.
1: Disabled as skip signals.
# 5 CSE For the continuous high-speed skip command, high-speed skip signals
are:
0: Effective at either a rising or falling edge (depending on the
setting of bit 6 (SRE) of parameter No. 6200).
1: Effective at both the rising and falling edges.
# 7 SKPXE For the skip function (G31), the skip signal SKIP is:
0: Enabled.
1: Disabled.
Whether the skip signals are enabled or disabled
Parameter IGX
(No.6201#4)
GSK
(No.6200#0)
SKPXE
(No.6201#7)
Skip signal
SKIPP
Skip signal
SKIP
Multistage skip signals
SKIP2-SKIP8
0 0 0 Disabled Enabled Enabled
0 1 0 Enabled Enabled Enabled
0 0 1 Disabled Disabled Enabled
0 1 1 Enabled Disabled Enabled
1 0 0 Disabled Disabled Disabled
1 1 0 Disabled Disabled Disabled
1 0 1 Disabled Disabled Disabled
Setting
1 1 1 Disabled Disabled Disabled
Bit 4 (IGX) of parameter No. 6201 is valid for the skip function using
high-speed skip signals (when bit 4 (HSS) of parameter No. 6200 is
set to 1) or for the multistage skip function using high-speed skip
signals (when bit 5 (SLS) of parameter No. 6200 is set to 1).
To use multistage skip signals, the multistage skip function option is
required.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2123 -
#7 #6 #5 #4 #3 #2 #1 #0
6202 1S8 1S7 1S6 1S5 1S4 1S3 1S2 1S1
[Input type] Parameter input
[Data type] Bit path
1S1 to 1S8 These parameters specify whether to enable or disable each
high-speed skip signal when the G31 skip command is issued.
The following table shows the correspondence between the bits, input
signals, and commands.
The settings of the bits have the following meaning :
0: The high-speed skip signal corresponding to a bit is disabled.
1: The high-speed skip signal corresponding to a bit is enabled.
Parameter High-speed skip
signals Parameter High-speed skip
signals
1S1 HDI0 1S5 HDI4
1S2 HDI1 1S6 HDI5
1S3 HDI2 1S7 HDI6
1S4 HDI3 1S8 HDI7
NOTE
Do not specify the same signal simultaneously for
different paths.
A.PARAMETERS APPENDIX B-63944EN/03
- 2124 -
#7 #6 #5 #4 #3 #2 #1 #0
6203 2S8 2S7 2S6 2S5 2S4 2S3 2S2 2S1
#7 #6 #5 #4 #3 #2 #1 #0
6204 3S8 3S7 3S6 3S5 3S4 3S3 3S2 3S1
#7 #6 #5 #4 #3 #2 #1 #0
6205 4S8 4S7 4S6 4S5 4S4 4S3 4S2 4S1
#7 #6 #5 #4 #3 #2 #1 #0
6206 DS8 DS7 DS6 DS5 DS4 DS3 DS2 DS1
[Input type] Parameter input
[Data type] Bit path
1S1to1S8, 2S1to2S8, 3S1to3S8, 4S1to4S8, DS1toDS8
Specify which skip signal is enabled when the skip command (G31, or
G31P1 to G31P4) and the dwell command (G04, G04Q1 to G04Q4)
are issued with the multi-step skip function.
The following table shows the correspondence between the bits, input
signals, and commands.
The setting of the bits have the following meaning :
0: The skip signal corresponding to a bit is invalid.
1: The skip signal corresponding to a bit is enabled.
Multi-step skip function
Command
Input
signal
G31
G31P1
G04Q1
G31P2
G04Q2
G31P3
G04Q3
G31P4
G04Q4
G04
SKIP/HDI0 1S1 2S1 3S1 4S1 DS1
SKIP2/HDI1 1S2 2S2 3S2 4S2 DS2
SKIP3/HDI2 1S3 2S3 3S3 4S3 DS3
SKIP4/HDI3 1S4 2S4 3S4 4S4 DS4
SKIP5/HDI4 1S5 2S5 3S5 4S5 DS5
SKIP6/HDI5 1S6 2S6 3S6 4S6 DS6
SKIP7/HDI6 1S7 2S7 3S7 4S7 DS7
SKIP8/HDI7 1S8 2S8 3S8 4S8 DS8
NOTE
HDI0 to HDI7 are high-speed skip signals. Do not
specify the same signal simultaneously for different
paths.
When bit 0 (GSK) of parameter No. 6200 is set to 1, commands to be
skipped can be selected by setting the following parameter:
Commands skipped by SKIPP signal <G006#6>
Parameter Command skipped
When bit 0 (1S1) of parameter No. 6202 is set to 1 G31P1,G04Q1
When bit 0 (2S1) of parameter No. 6203 is set to 1 G31P2,G04Q2
When bit 0 (3S1) of parameter No. 6204 is set to 1 G31P3,G04Q3
When bit 0 (4S1) of parameter No. 6205 is set to 1 G31P4,G04Q4
When bit 6 (DS1) of parameter No. 6206 is set to 1 G04,G04Q1,G04Q2,G04Q3,G04Q4
B-63944EN/03 APPENDIX A.PARAMETERS
- 2125 -
#7 #6 #5 #4 #3 #2 #1 #0
6207 SFN SFP
[Input type] Parameter input
[Data type] Bit path
# 1 SFP The feedrate used when the skip function (G31) is being executed is:
0: Feedrate of a programmed F code.
1: Feedrate set in parameter No. 6281.
NOTE
For the multi-stage skip function and high-speed
skip, see the description of bit 2 (SFN ) of
parameter No. 6207.
# 2 SFN The feedrate used when the skip function based on high-speed skip
signals (with bit 1 (HSS) of parameter No. 6200 set to 1) or the
multi-skip function is being executed is:
0: Feedrate of a programmed F code.
1: Feedrate set in a parameter from parameter No. 6282 to No.
6285.
NOTE
For not the multistage skip function, but the skip
function using no high-speed skip signals (when bit
4 (HSS) of parameter No. 6200 is set to 0), see the
description of bit 1 (SFP) of parameter No. 6207.
#7 #6 #5 #4 #3 #2 #1 #0
6208 9S8 9S7 9S6 9S5 9S4 9S3 9S2 9S1
[Input type] Parameter input
[Data type] Bit path
9S1 to 9S8 Specify which high-speed skip signal is enabled for the continuous
high-speed skip command G31P90 or the EGB skip command G31.8.
The settings of each bit have the following meaning:
0: The high-speed skip signal corresponding to the bit is disabled.
1: The high-speed skip signal corresponding to the bit is enabled.
The bits correspond to signals as follows:
Parameter High-speed skip
signal Parameter High-speed skip
signal
9S1 HDI0 9S5 HDI4
9S2 HDI1 9S6 HDI5
9S3 HDI2 9S7 HDI6
9S4 HDI3 9S8 HDI7
A.PARAMETERS APPENDIX B-63944EN/03
- 2126 -
6220 Period during which skip signal input is ignored for the continuous
high-speed skip function and EGB axis skip function
[Input type] Parameter input
[Data type] Byte path
[Unit of data] 8msec
[Valid data range] 3 to 127(× 8msec)
This parameter specifies the period from when a skip signal is input to
when the next skip signal can be input for the continuous high-speed
skip function and EGB axis skip function. This parameter is used to
ignore chattering in skip signals.
If a value that falls outside the valid range is specified, the setting is
assumed to be 24 msec.
Signal ignoring period (parameter No. 6220)
Skip signal
This signal is ignored.
When high-speed skip signals are used and bit 5 (CSE) of parameter
No. 6201 is set to 1, signals are handled as follows:
Signal ignoring period (parameter No. 6220)
High-speed skip
signals These signals
are ignored.
6221 Torque limit dead zone time for a torque limit skip command
[Input type] Parameter input
[Data type] 2-word axis
[Unit of data] msec
[Valid data range] 0 to 65535
The torque limit skip arrival signal is ignored for a set period of time.
If G31P98 is specified, skip operation is not performed for a set period
of time after the torque limit skip arrival signal is set to 1.
If G31P99 is specified, skip operation is not performed for a set period
of time after the torque limit skip arrival signal is set to 1.
However, if a skip signal is input, skip operation is performed,
regardless of the period of time set in this parameter.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2127 -
6254 ε value on the X axis during automatic tool compensation (T series)
ε value during automatic tool length measurement (M series) (for the XAE1
and GAE1 signals)
6255 ε value on the Z axis during automatic tool compensation (T series)
ε value during automatic tool length measurement (M series) (for the XAE2
and GAE2 signals)
[Input type] Parameter input
[Data type] 2-word path
[Unit of data] mm, inch, deg (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
These parameters set the relevant ε value during automatic tool
compensation (T series) or automatic tool length measurement (M
series).
NOTE
1 For the M series, when the setting of
parameter No. 6252 or 6253 is 0, the setting
of parameter No. 6251 is used.
2 Set a radius value regardless of whether
diameter or radius programming is specified.
6281 Feedrate for the skip function (G31)
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
This parameter sets a feedrate for the skip function (G31). This
parameter is valid when bit 1 (SFP) of parameter No. 6207 is set to 1.
NOTE
For the multi-stage skip function and high-speed
skip, see the description of parameter No. 6282 to
No. 6285.
A.PARAMETERS APPENDIX B-63944EN/03
- 2128 -
6282 Feedrate for the skip function (G31, G31 P1)
6283 Feedrate for the skip function (G31 P2)
6284 Feedrate for the skip function (G31 P3)
6285 Feedrate for the skip function (G31 P4)
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
Each of these parameters sets a feedrate for each skip function G code.
These parameters are valid when bit 2 (SFN) of parameter No. 6207 is
set to 1.
6287 Positional deviation limit in torque limit skip
[Input type] Parameter input
[Data type] 2-word axis
[Unit of data] Detection unit
[Valid data range] 0 to 327670
This parameter sets a positional deviation limit for each axis imposed
when torque limit skip is specified. When the actual positional
deviation exceeds the positional deviation limit, the alarm (SV0004) is
issued and an immediate stop takes place.
#7 #6 #5 #4 #3 #2 #1 #0
6400 MG4 MGO RVN HMP MC8 MC5 FWD RPO
[Input type] Parameter input
[Data type] Bit path
# 0 RPO With the manual handle retrace function, the rapid traverse rate is
clamped, assuming that:
0: An override of 10% is used.
1: An override of 100% is used.
# 1 FWD With the manual handle retrace function, program execution can be
performed:
0: In both forward and backward directions.
1: In the forward direction only. Execution in the backward
direction is not permitted.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2129 -
# 2 MC5
# 3 MC8
These parameters set the number of M code groups and the number of
M codes per group.
(See explanations of parameters Nos. 6411 to 6490.)
MC5 MC8 M code group setting
0 0 Standard (20 groups of four)
1 0 16 groups of five
0 1 10 groups of eight
When 16 groups of five are used, the meanings of parameters are
changed as follows:
Group A No.6411(1) to No.6415(5)
Group B No.6416(1) to No.6420(5)
:
Group P No.6486(1) to No.6490(5)
When 10 groups of eight are used, they are changed as follows:
Group A No.6411(1) to No.6418(8)
Group B No.6419(1) to No.6426(8)
:
Group J No.6483(1) to No.6490(8)
# 4 HMP When inversion or backward movement is inhibited in other paths:
0: Inversion or backward movement is not inhibited for the
currently executed path.
1: Inversion or backward movement is inhibited also for the
currently executed path.
# 5 RVN When the manual handle retrace function is used, M codes other than
grouped M codes:
0: Do not disable backward movement.
1: Disable backward movement.
When this parameter is set to 1, M codes other than grouped M codes
disable backward movement in general. Exceptionally, however, the
following M codes allow backward movement:
1. Subprogram call based on M98/M99
2. Subprogram call based on an M code
3. Macro call based on an M code
4. Waiting M code
5. M0
# 6 MGO When the manual handle retrace function is used, handle pulses during
execution of a G code related to measurement are:
0: Valid.
1: Invalid. A speed with an override of 100% is used for execution
at all times.
A.PARAMETERS APPENDIX B-63944EN/03
- 2130 -
# 7 MG4 In the manual handle retrace function, for blocks for which multi-step
skip G04 is enabled (when the multi-step skip software option is used,
and the settings of parameter Nos. 6202 to 6206 are valid):
0: Backward movement is not prohibited.
1: Backward movement is prohibited.
#7 #6 #5 #4 #3 #2 #1 #0
6401 STO HST CHS
[Input type] Parameter input
[Data type] Bit path
# 2 CHS In manual handle retrace:
0: The status is displayed if the following conditions are all
satisfied:
(1) The manual handle retrace software option is used.
(2) Bit 6 (HST) of parameter No. 6401, which specifies
whether to enable or disable status display, is set to 1.
(3) Check mode output signal MMMOD<Fn091.3> is set to 1.
1: The status is displayed if the following conditions are all
satisfied:
(1) The manual handle retrace software option is used.
(2) Bit 6 (HST) of parameter No. 6401, which specifies
whether to enable or disable status display, is set to 1.
(3) Cycle start lamp signal STL<Fn000.5> is set to 1.
(4) Check mode input signal MMOD<Gn067.2> is set to 1.
(5) Handle input signal MCHK<Gn067.3> is set to 1 in the
check mode.
# 6 HST When the manual handle retrace function is used, the time display
field on the status display line of the CNC screen:
0: Does not display status.
1: Displays status.
# 7 STO In the manual handle retrace function, the timing for outputting an S
code and T code during backward movement is:
0: Different from the timing during forward movement:
1: The same as during forward movement.
6405 Override value (equivalence) for clamping the rapid traverse rate used with
the manual handle retrace function
[Input type] Parameter input
[Data type] Word path
[Unit of data] %
[Valid data range] 0 to 100
This parameter sets an override value (equivalence) for clamping the
rapid traverse rate used with the manual handle retrace function. If a
value greater than 100 is set in parameter (No.6405), the rapid traverse
rate is clamped to an override of 100%. This function is invalid if 0 is
set in parameter (No.6405). In this case, the setting of bit 0 (RPO) of
parameter No. 6400 is used.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2131 -
6410 Travel distance per pulse generated from the manual pulse generator
[Input type] Parameter input
[Data type] Word path
[Unit of data] %
[Valid data range] 0 to 100
Set the travel distance per pulse generated from the manual pulse
generator in terms of the override value.
The distance traveled by the machine when the manual handle is
actually turned can be found by the following expression:
[Specified speed] × [Handle magnification] × ([Setting of this
parameter]/100) × (8/60000) (mm or inch)
[Example]
When a specified feedrate is 30mm/min, the manual handle
magnification is 100, and parameter No. 6410 is set to 1, the
travel distance per pulse generated from the manual pulse
generator is calculated as follows:
[Travel distance per pulse]
=30[mm/min] × 100 × (1/100) × (8/60000)[min]= 0.004mm
6411 M code of group A in manual handle retrace (1)
to
6414 M code of group A in manual handle retrace (4)
6415 M code of group B in manual handle retrace (1)
to
6418 M code of group B in manual handle retrace (4)
6419 M code of group C in manual handle retrace (1)
to
6422 M code of group C in manual handle retrace (4)
6423 M code of group D in manual handle retrace (1)
to
6426 M code of group D in manual handle retrace (4)
6427 M code of group E in manual handle retrace (1)
to
6430 M code of group E in manual handle retrace (4)
6431 M code of group F in manual handle retrace (1)
to
6434 M code of group F in manual handle retrace (4)
6435 M code of group G in manual handle retrace (1)
to
6438 M code of group G in manual handle retrace (4)
A.PARAMETERS APPENDIX B-63944EN/03
- 2132 -
6439 M code of group H in manual handle retrace (1)
to
6442 M code of group H in manual handle retrace (4)
6443 M code of group I in manual handle retrace (1)
to
6446 M code of group I in manual handle retrace (4)
6447 M code of group J in manual handle retrace (1)
to
6450 M code of group J in manual handle retrace (4)
6451 M code of group K in manual handle retrace (1)
to
6454 M code of group K in manual handle retrace (4)
6455 M code of group L in manual handle retrace (1)
to
6458 M code of group L in manual handle retrace (4)
6459 M code of group M in manual handle retrace (1)
to
6462 M code of group M in manual handle retrace (4)
6463 M code of group N in manual handle retrace (1)
to
6466 M code of group N in manual handle retrace (4)
6467 M code of group O in manual handle retrace (1)
to
6470 M code of group O in manual handle retrace (4)
6471 M code of group P in manual handle retrace (1)
to
6474 M code of group P in manual handle retrace (4)
6475 M code of group O in manual handle retrace (1)
to
6478 M code of group Q in manual handle retrace (4)
6479 M code of group R in manual handle retrace (1)
to
6482 M code of group R in manual handle retrace (4)
6483 M code of group S in manual handle retrace (1)
to
6486 M code of group S in manual handle retrace (4)
B-63944EN/03 APPENDIX A.PARAMETERS
- 2133 -
6487 M code of group T in manual handle retrace (1)
to
6490 M code of group T in manual handle retrace (4)
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 0 to 9999
Set a group of M codes output during backward movement.
For backward movement for an M code, the modal M code in the
same group set by the parameter is output.
The first M code in each group is set as the default.
When the number of M codes in a group is 3 or less, set the parameter
corresponding to an unused M code to 0.
For backward movement for "M0", "M0" is output regardless of
which M code is set for the parameter. "0" set in the parameter is
ignored.
For an M code which is not set in any group by any of the above
parameters, the M code for forward movement is output.
With these parameters, an M code in the same group can be output in
backward movement only when the M code is the first M code in each
block. When a block contains two or more M codes, the same M codes
as output in forward movement are output as a second M code and up.
NOTE
The above explanation of M code groups applies to
the standard settings. The number of M codes in
each group and the number of M code groups vary
depending on the settings of bit 2 (MC5) and bit 3
(MC8) of parameter No. 6400.
6581 RGB value of color palette 1
to
6595 RGB value of color palette 15
[Input type] Parameter input
[Data type] 2-word
[Valid data range] 0 to 151515
Each of these parameters sets the RGB value of each color palette by
specifying a 6-digit number as described below.
rrggbb: 6-digit number (rr: red data, gg: green data, bb: blue data)
The valid data range of each color is 0 to 15 (same as the tone levels
on the color setting screen). When a number equal to or greater than
16 is specified, the specification of 15 is assumed.
Example)
When the tone level of a color is: red:1 green:2, blue:3, set 10203
in the parameter.
A.PARAMETERS APPENDIX B-63944EN/03
- 2134 -
#7 #6 #5 #4 #3 #2 #1 #0
6700 PCM
[Input type] Parameter input
[Data type] Bit path
# 0 PCM M code that counts the total number of machined parts and the number
of machined parts
0: M02, or M30, or an M code specified by parameter No.6710
1: Only M code specified by parameter No.6710
6710 M code that counts the number of machined parts
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 0 to 999999999
The total number of machined parts and the number of machined parts
are counted (+1) when the M code set is executed.
NOTE
The setting of 0 is invalid (no count operation is
performed with M00.) Moreover, M98, M99, M198
(external device subprogram calling), and M codes
used for subprogram calling and macro calling
cannot be set as M codes for count-up operation.
(Even when such an M code is set, count-up
operation is not performed, ignoring the M code.)
6711 Number of machined parts
[Input type] Setting input
[Data type] 2-word path
[Valid data range] 0 to 999999999
The number of machined parts is counted (+1) together with the total
number of machined parts when the M02, M30, or a M code specified
by parameter No.6710 is executed.
NOTE
The number of parts is not counted for M02, M03,
when bit 0 (PCM) of parameter No. 6700 is set to
1.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2135 -
6712 Total number of machined parts
[Input type] Setting input
[Data type] 2-word path
[Valid data range] 0 to 999999999
This parameter sets the total number of machined parts.
The total number of machined parts is counted (+1) when M02, M30,
or an M code specified by parameter No.6710 is executed.
NOTE
The number of parts is not counted for M02, M30,
when bit 0 (PCM) of parameter No. 6700 is set to
1.
6713 Number of required parts
[Input type] Setting input
[Data type] 2-word path
[Valid data range] 0 to 999999999
This parameter sets the number of required machined parts.
Required parts finish signal PRTSF <F0062.7> is output to PMC
when the number of machined parts reaches the number of required
parts. The number of parts is regarded as infinity when the number of
required parts is zero. The PRTSF signal is then not output.
6750 Integrated value of power-on period
[Input type] Parameter input
[Data type] 2-word path
[Unit of data] min
[Valid data range] 0 to 999999999
This parameter displays the integrated value of power-on period.
6751 Operation time (integrated value of time during automatic operation) 1
[Input type] Setting input
[Data type] 2-word path
[Unit of data] msec
[Valid data range] 0 to 59999
For details, see the description of parameter No. 6752.
6752 Operation time (integrated value of time during automatic operation) 2
[Input type] Setting input
[Data type] 2-word path
[Unit of data] min
[Valid data range] 0 to 999999999
This parameter displays the integrated value of time during automatic
operation (neither stop nor hold time included).
The actual time accumulated during operation is the sum of this
parameter No. 6751 and parameter No. 6752.
A.PARAMETERS APPENDIX B-63944EN/03
- 2136 -
6753 Integrated value of cutting time 1
[Input type] Setting input
[Data type] 2-word path
[Unit of data] msec
[Valid data range] 0 to 59999
For details, see the description of parameter No. 6754.
6754 Integrated value of cutting time 2
[Input type] Setting input
[Data type] 2-word path
[Unit of data] min
[Valid data range] 0 to 999999999
This parameter displays the integrated value of a cutting time that is
performed in cutting feed such as linear interpolation (G01) and
circular interpolation (G02 or G03).
The actual time accumulated during cutting is the sum of this
parameter No. 6753 and parameter No. 6754.
#7 #6 #5 #4 #3 #2 #1 #0
6800 M6T IGI SNG GRS SIG LTM GS2 GS1
[Input type] Parameter input
[Data type] Bit path
# 0 GS1
# 1 GS2 For the maximum number of groups set in parameter No. 6813, up to
four tools can be registered per group. The combination of the number
of registrable groups and the number of tools per group can be
changed by setting GS1 and GS2.
GS2 GS1 Number of groups Number of tools
0 0 1/8 of maximum number of groups (No.6813) 32
0 1 1/4 of maximum number of groups (No.6813) 16
1 0 1/2 of maximum number of groups (No.6813) 8
1 1 Maximum number of groups (No.6813) 4
NOTE
After changing these parameters, set data again by
using G10 L3 ;(registration after deletion of data of all
groups).
B-63944EN/03 APPENDIX A.PARAMETERS
- 2137 -
# 2 LTM The tool life count is specified by:
0: Count.
1: Duration.
NOTE
After changing this parameter,set data again by
using G10 L3 ;(registration after deletion of data of all
groups).
# 3 SIG When a tool is skipped by a signal, the group number is:
0: Not input by the tool group number selection signals.
1: Input by the tool group number selection signals.
NOTE
When this parameter is set to 0, a tool of the
currently used group is skipped.
# 4 GRS When the tool change reset signal (TLRST) is input:
0: If the life of the group specified by the tool group number
selection signals has expired, the execution data of the group is
cleared.
1: The execution data of all registered groups is cleared.
If this parameter is set to 1, the execution data of all registered groups
is cleared also when the clear operation to clear execution data is
performed on the tool life management list screen.
# 5 SNG When the tool skip signal (TLSKP) is input while a tool not controlled
by the tool life management function is being used:
0: A tool of the most recently used group or a specified group (bit 3
(SIG) of parameter No. 6800) is skipped.
1: The tool skip signal is ignored.
# 6 IGI Tool back numbers are:
0: Not ignored.
1: Ignored.
# 7 M6T A T code specified in the same block as M06 is:
0: Assumed to be a back number.
1: Assumed to be a command specifying the next tool group.
A.PARAMETERS APPENDIX B-63944EN/03
- 2138 -
#7 #6 #5 #4 #3 #2 #1 #0
M6E EMD LVF TSM
6801 M6E EMD LVF
NOTE
The use of this parameter varies depending on
whether the tool management function or tool life
management function is used.
[Input type] Parameter input
[Data type] Bit path
# 1 TSM In the tool life management function, life counting is performed as
follows when more than one offset is specified:
0: Counting is performed for each tool number.
1: Counting is performed for each tool.
# 2 LVF When the life value is counted by duration in the tool management
function or tool life management function, tool life count override
signals *TLV0 to *TLV9 <G049.0 to G050.1> are:
0: Not used.
1: Used.
# 3 EMD In the tool life management function, the mark "*" indicating that the
life has expired is displayed when:
0: The next tool is used.
1: The life has just expired.
NOTE
If this parameter is set to 0, the "@" mark
(indicating that the tool is in use) is kept displayed
unless the next tool whose life has not expired is
used. If this parameter is set to 1, marks are
displayed in different ways depending on the life
count type.
If the life count type is the duration specification type,
the "*" mark (indicating that the life has expired)
appears when the life has expired. If the life count
type is the count specification type, one count is not
assumed until the end of the program (M02, M30,
and so on). Therefore, even when the life value and
the tool life counter value match, the "*" mark (life
has expired) does not appear. The "*" mark (life has
expired) appears when the tool is used again by a
tool group command (T code) or tool change
command (M06) issued after the CNC is reset.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2139 -
# 7 M6E When a T code is specified in the same block as M06:
0: The T code is treated as a back number or the group number to
be selected next.
Which number is assumed depends on the setting of bit 7 (M6T)
of parameter No. 6800.
1: Life counting for the tool group starts immediately.
#7 #6 #5 #4 #3 #2 #1 #0
6802 RMT TSK TGN ARL GRP E17 TCO T99
[Input type] Parameter input
[Data type] Bit path
# 0 T99 When M99 of the main program is executed, and there is a the life was
expired tool group:
0: The tool change signal is not output.
1: The tool change signal is output, and the automatic operation
becomes a stopped state..
If the life count is specified by use count and this parameter 1, the tool
change signal TLCH <Fn064.0> is output and the automatic operation
becomes a stopped state if the life of at least one tool group has
expired when the M99 command is specified.
If the life count type is the duration specification type, the automatic
operation becomes a stopped state if the life of at least one tool group
has expired when the M99 command is specified.
M
If the life count is specified by use count, after the M99 command is
specified, a tool group command (T code) selects, from a specified
group, a tool whose life has not expired, and the next tool change
command (M06) increments the tool life counter by one.
T
If the life count is specified by use count, ｗhen a tool group
command (T code) is specified after the M99 command is specified, a
tool whose life has not expired is selected from a specified group, and
the tool life counter is incremented by one.
When the tool change type is the ATC type (bit 3 (TCT) of parameter
No. 5040 = 1), the same specifications as for the M series apply.
A.PARAMETERS APPENDIX B-63944EN/03
- 2140 -
#1 TCO
#2 E17
Specifies whether to allow the FOCAS2 or PMC window function to
write tool information of a group being used or a group to be used
next during automatic operation (the OP signal is set to "1").
6802#1(TCO)
1
6802#2(E17)
Condition 0
1 0
Tool being used × ○ Group being used or
to be used next Tool not being used × ○ ○
During
automatic
operation Group neither being used nor to be used next ○ ○ ○
Not during automatic operation ○ ○ ○
○: Tool information can be written from FOCAS2 and PMC
window.
×: Tool information cannot be written from FOCAS2 and PMC
window.
When an attempt is made to write tool information from PMC
window, completion code 13 (REJECT ALARM) is returned.
: Tool information cannot be cleared.
NOTE
When tool information of a tool being used (marked
with "@") in the group being used or to be used next or
tool information of the most recently used tool (marked
with "@") in a group that is neither the group being
used nor the group to be used next is cleared, the life
counter is reset to 0.
It is possible to modify tool information of a tool in the
group to be used next. However, because tool
selection is already completed, the selected tool does
not change even when the tool information is modified.
This parameter has no influence on modifications to tool
information by edit operations from the tool life
management screen.
# 3 GRP Management data of tool life arrival notice signal TLCHB is:
0: Managed using the remaining life value set in parameter No.
6844 and 6845.
1: Managed using the remaining life value set in tool life
management data.
NOTE
When the tool life arrival notice signal function is
used, bit 4 (LFB) of parameter No. 6805 must be set
to 1 to enable the tool life management B function.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2141 -
# 4 ARL Tool life arrival notice signal TLCHB of tool life management is:
0: Output for each tool.
1: Output for the last tool of a group.
This parameter is valid only when bit 3 (GRP) of parameter No. 6802
is set to 1.
# 5 TGN In the tool life management function, the optional group number
function is:
0: Not used.
1: Used.
NOTE
When the optional group number function is used,
bit 4 (LFB) of parameter No. 6805 must be set to 1
to enable the tool life management B function.
In lathe systems, the optional group number function
can be used if the tool change type is the ATC type
(bit 3 (TCT) of parameter No. 5040 = 1).
# 6 TSK If the count type in tool life management is the duration type, then
when the last tool of a group is skipped by a signal:
0: The count value for the last tool equals the life value.
1: The count value for the last tool remains unchanged.
# 7 RMT Tool life arrival notice signal TLCHB is turned on and off as follows:
0: The signal is turned on if the remaining life value (the life value
minus the life counter value) is smaller than or equal to the
remaining life setting. The signal is turned off if the remaining
life value (the life value minus the life counter value) is greater
than the remaining life setting.
1: The signal is turned on if the remaining life value (the life value
minus the life counter value) is equal to the remaining life setting.
The signal is turned off if the remaining life value (the life value
minus the life counter value) is not equal to the remaining life
setting.
NOTE
When using the life count override feature, set bit 7
(RMT) of parameter No. 6802 to 0. When the life
count is specified by duration, the unit used for
determining the result of comparison between the
remaining life and the remaining life setting varies
depending on the life count interval (bit 0 (FCO) of
parameter No. 6805). If the life is counted every
second, the comparison is made in units of 1 minute;
if the life is counted every 0.1 second, the
comparison is made in units of 0.1 minute.
A.PARAMETERS APPENDIX B-63944EN/03
- 2142 -
#7 #6 #5 #4 #3 #2 #1 #0
6804 LFI ETE TCI
[Input type] Parameter input
[Data type] Bit path
# 1 TCI During automatic operation (the OP signal is "1"), editing of tool life
data is:
0: Disabled.
1: Enabled.
NOTE
When this parameter is set to 1, tool life data can be
edited even during automatic operation (the OP
signal is "1"). If the target group for editing is the
group being used or the group to be used next,
however, only presetting of the life counter is
permitted, and other data cannot be modified.
# 2 ETE In the tool life management screen, the mark of the tool at the life was
expired of the final tool in the group :
0: depends on setting parameter EMD (No.6801#3).
1: is "*" mark.
If bit 2 (ETE) of parameter No. 6804 is set to 1, when the life counter
of the final tool in the group becomes equal to the life value, display
mark "*" in the final tool of the tool life management screen.
When tool change signal TLCH<Fn064.0> is "1", the state of the life
was expired of the tool can be read by reading tool information on the
final tool in FOCAS2 or the PMC window.
# 6 LFI In tool life management, counting of the life of a selected tool is:
0: Enabled.
1: Enabled or disabled according to the status of tool life counting
disable signal LFCIV<G048.2>.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2143 -
#7 #6 #5 #4 #3 #2 #1 #0
6805 TAD TRU TRS LFB FGL FCO
[Input type] Parameter input
[Data type] Bit path
# 0 FCO If the life count type is the duration specification type, the life is
counted as follows:
0: Every second.
1: Every 0.1 second.
According to the setting of this parameter, the increment system of life
values and tool life counter values displayed on the tool life
management screen is set as follows:
Parameter FCO 0 1
Increment system for display and setting of life
values and life counter values
1-minute
increments
0.1-minute
increments
NOTE
After changing the setting of this parameter, set data
again by using G10L3;(registration after deletion of
data of all groups).
# 1 FGL If the life count type is the duration specification type, life data
registered by G10 is:
0: In one-minute increments.
1: In 0.1-second increments.
# 4 LFB The tool life management B function is:
0: Disabled.
1: Enabled.
When the tool life management B function is enabled, the following
functions can be used:
<1> Tool life value extension (count specification: 99999999 times,
duration specification: 100000 minutes)
<2> Optional group number function
<3> Tool life arrival notice function
In lathe systems, if the tool change type is the ATC type (bit 3 (TCT)
of parameter No. 5040 = 1), the optional group number function can
be used.
A.PARAMETERS APPENDIX B-63944EN/03
- 2144 -
# 5 TRS Tool change reset signal TLRST is valid when reset signal RST is not
"1" and:
0: The reset state (automatic operation signal OP is "0") is
observed.
1: The reset state (automatic operation signal OP is "0"), automatic
operation stop state (The STL and SPL signals are "0" and the
OP signal is "1"), or the automatic operation pause state (the STL
signal is "0" and the SPL signal is "1") is observed. The TLRST
signal, however, is invalid when the automatic operation stop
state, automatic operation pause state, and automatic operation
start state (the STL signal is "1") is observed during execution of
a data setting command (G10L3).
# 6 TRU When the life count type is the duration specification type, and the life
is counted every second (bit 0 (FCO) of parameter No. 6805 is set to
0):
0: Cutting time less than one second is discarded and is not counted.
1: Cutting time less than one second is rounded up and is counted as
one second.
NOTE
If the life is counted every 0.1 second (bit 0 (FCO) of
parameter No. 6805 is set to 1), cutting time less
than 0.1 second is always rounded up and is counted
as 0.1 second.
# 7 TAD With tool change type D (bit 7 (M6E) of parameter No. 6801 is set to
1), when a block specifying M06 contains no T command:
0: An alarm PS0153 is issued.
1: No alarm is issued.
6810 Tool life management ignore number
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 0 to 99999999
This parameter sets the tool life management ignore number.
When the value specified in a T code exceeds the value set in this
parameter, the value obtained by subtracting the parameter-set value
from the T code value is assumed to be the tool group number for tool
life management.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2145 -
6811 Tool life count restart M code
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to 127 (except 01, 02, 30, 98, and 99)
When 0 is specified, it is ignored.
When the life is specified by count, the tool change signal (TLCH) is
output if the life of at least one tool group has expired when the tool
life count restart M code is issued.
The T code (tool life management group command) specified after the
tool life count restart M code selects a tool whose life has not expired
from a specified group, and the next M06 command increments the
tool life counter by one.
When the life is specified by duration, specifying the tool life count
restart M code causes nothing. When 0 is set in this parameter, the tool
life count restart M code is invalid. When the data of M code exceeds
127 values, set 0 in parameter No.6811, and set the value of M code in
parameter No.13221. The data range of parameter No.13221 is from 0
to 255.
NOTE
The use of this parameter varies depending on
whether the tool management function or tool life
management function is used.
6813 Maximum number of groups in tool life management
NOTE
A
fter this parameter has been set, the power must be
turned off then back on for the setting to become
effective.
[Input type] Parameter input
[Data type] Word path
[Unit of data] Group
[Valid data range] 0, 8, 16 to 256
This parameter sets the maximum number of groups to be used for
each path. As the maximum number of groups, set a multiple of eight.
When the tool life management function is not used, 0 must be set. Set
this parameter so that the total number of groups in all paths does not
exceed the total number of groups in the entire system (256 groups).
NOTE
When the power is turned on, all tool life
management file data is initialized. So, tool life
management data must be set for all paths that use
tool life management.
A.PARAMETERS APPENDIX B-63944EN/03
- 2146 -
6844 Remaining tool life (use count)
[Input type] Parameter input
[Data type] Word path
[Valid data range] 0 to 9999
This parameter sets a remaining tool life (use count) used to output the
tool life arrival notice signal when the tool life is specified by use
count. If a value greater than the tool life value or 0 is set in this
parameter, the tool life arrival notice signal is not output.
6845 Remaining tool life (use duration)
[Input type] Parameter input
[Data type] 2-word path
[Unit of data] min
[Valid data range] Not greater than the tool life value
This parameter sets the remaining tool life (use duration) used to
output the tool life arrival notice signal when the tool life is specified
by use duration. If a value greater than the tool life value or 0 is
specified in this parameter, the tool life arrival notice signal is not
output.
NOTE
When the life is counted every 0.1 second (bit 0
(FCO) of parameter No. 6805 = 1), the parameter
value is in 0.1-minute increments.
6930 Maximum value of the operating range of the 1-st position switch (PSW101)
6931 Maximum value of the operating range of the 2-nd position switch (PSW102)
to to
6945 Maximum value of the operating range of the 16-th position switch (PSW116)
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm, inch, degree (machine unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
Set the maximum value of the operating range of the first to sixteenth
position switches.
NOTE
1 For a diameter-specified axis, use radius values to
specify the parameters used to set the maximum
and minimum values of an operating range.
2 The position switch function is enabled upon
completion of reference position return.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2147 -
6950 Minimum value of the operating range of the 1-st position switch (PSW201)
6951 Minimum value of the operating range of the 2-nd position switch (PSW202)
to to
6965 Minimum value of the operating range of the 16-th position switch (PSW216)
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm, inch, degree (machine unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
Set the minimum value of the operating range of the first to sixteenth
position switches.
NOTE
1 For a diameter-specified axis, use radius values to
specify the parameters used to set the maximum
and minimum values of an operating range.
2 The position switch function is enabled upon
completion of reference position return.
#7 #6 #5 #4 #3 #2 #1 #0
7001 JST
[Input type] Parameter input
[Data type] Bit path
# 2 JST In manual numerical specification, the STL signal indicating that
automatic operation is being started is:
0: Not output.
1: Output.
#7 #6 #5 #4 #3 #2 #1 #0
7002 JBF JTF JSF JMF
[Input type] Parameter input
[Data type] Bit path
# 0 JMF In manual numerical specification, M function specification is:
0: Allowed.
1: Not allowed.
# 1 JSF In manual numerical specification, S function specification is:
0: Allowed.
1: Not allowed.
A.PARAMETERS APPENDIX B-63944EN/03
- 2148 -
# 2 JTF In manual numerical specification, T function specification is:
0: Allowed.
1: Not allowed.
# 3 JBF In manual numerical specification, B function specification is:
0: Allowed.
1: Not allowed.
#7 #6 #5 #4 #3 #2 #1 #0
7040 RPS
[Input type] Parameter input
[Data type] Bit path
# 2 RPS When the tool retract signal TRESC is set to 1 after G10.6 is specified
alone:
0: The tool is not retracted.
1: The tool is retracted with the value set for parameter No. 7041 or
1261 used as the incremental retraction distance.
7041 Retraction distance in tool retract and return
[Input type] Setting input
[Data type] Real axis
[Unit of data] mm, inch, deg (input unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
This parameter sets the retraction distance used when G10.6 is
specified alone for the tool retract and return. The tool is retracted by
the distance set for this parameter in the incremental mode. This data
is valid only when bit 2 (RPS) of parameter No. 7040 is set to 1.
During tool center point control and workpiece setting error
compensation, however, this parameter is valid if parameter No.
11261 is set to 0.
#7 #6 #5 #4 #3 #2 #1 #0
7055 BCG
[Input type] Parameter input
[Data type] Bit path
# 3 BCG The pre-interpolation bell-shaped acceleration/deceleration time
constant change function is:
0: Disabled.
1: Enabled.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2149 -
7066 Acceleration/deceleration reference speed for the time constant change
function of bell-shaped acceleration/deceleration before interpolation
[Input type] Setting input
[Data type] Real path
[Unit of data] mm/min, inch/min, degree/min (input unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
This parameter is used when the time constant change function of
bell-shaped acceleration/deceleration before interpolation is used.
#7 #6 #5 #4 #3 #2 #1 #0
7100 HCL THD JHD
[Input type] Parameter input
[Data type] Bit path
# 0 JHD Manual handle feed in JOG feed mode or incremental feed in the
manual handle feed
0: Invalid
1: Valid
# 1 THD In the TEACH IN JOG mode, the manual pulse generator is:
0: Disabled.
1: Enabled.
# 3 HCL The clearing of handle interruption amount display by soft key [CAN]
operation is:
0: Disabled.
1: Enabled.
#7 #6 #5 #4 #3 #2 #1 #0
7102 HNGx
[Input type] Parameter input
[Data type] Bit axis
# 0 HNGx Axis movement direction for rotation direction of manual pulse
generator
0: Same in direction
1: Reverse in direction
A.PARAMETERS APPENDIX B-63944EN/03
- 2150 -
#7 #6 #5 #4 #3 #2 #1 #0
7103 HIT HNT RTH
[Input type] Parameter input
[Data type] Bit path
# 1 RTH By a reset or emergency stop, the amount of manual handle
interruption is:
0: Not canceled.
1: Canceled.
# 2 HNT When compared with the travel distance magnification selected by the
manual handle feed travel distance selection signals (incremental feed
signals) (MP1, MP2), the travel distance magnification for
incremental feed/manual handle feed is:
0: Same.
1: 10 times greater.
# 3 HIT When compared with the travel distance magnification selected by the
manual handle feed travel distance selection signals (incremental feed
signals (MP1, MP2), the travel distance magnification for manual
handle interrupt is:
0: Same.
1: 10 times greater.
7117 Allowable number of pulses that can be accumulated during manual handle
feed
[Input type] Parameter input
[Data type] 2-word path
[Unit of data] Pulse
[Valid data range] 0 to 999999999
This parameter sets the number of pulses from the manual pulse
generator that exceed the rapid traverse rate and can be accumulated
without being discarded if manual handle feed faster than the rapid
traverse rate is specified.
The amount of pulses exceeding the rapid traverse rate can be saved
by CNC as B. And amount of pulses B will be exported as pulses C.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2151 -
t
Rapid Traverse Rate
A
：amount of pulses corresponds to value of Rapid Traverse Rate.
B：amount of pulses accumulated in CNC.
C：amount of pulses the same as B.
A
B
C
Amount of pulses exported by CNC in Manual Handle Feed
Amount of pulses B is calculated in 2 cases as following:
In case of
1) Parameter No.7117 = 0
The feedrate is clamped at the Rapid Traverse Rate and
generated pulses exceeding the Rapid Traverse Rate are ignored
(B=0)
In case of
2) Parameter No.7117 > 0
The feedrate is clamped as the Rapid Traverse Rate, but the
pulses exceeding the Rapid Traverse Rate is not ignored. Amount
of pulses accumulated in CNC is calculated as following.
(Although stopping the rotation of manual pulse generator, if
there is pulses accumulated in CNC, it will be exported and the
tool will move as long as amount of it.)
Magnification set by MP1，MP2<Gn019.4,.5> is m, value of
parameter No.7117 is n.
n < m: Clamping is set performed at value of parameter No.7117.
n ≥ m: Amount A+B, showed in figure, which’s value is multiple
of m and small than n. As a result, clamping is performed as an
integral multiple of the selected magnification.
n
m
A
B
pulses over (k⋅m) will be ignored
A
: amount of pulses the same as Rapid Traverse Rate.
B: amount of pulses saved in CNC.
k : integer number
A+B=k⋅m
Amount of pulses exceeding the Rapid Traverse Rate (n ≥ m)
A.PARAMETERS APPENDIX B-63944EN/03
- 2152 -
NOTE
Due to change of mode, clamping can be
performed not as an integral multiple of the
selected magnification.
The distance the tool moves may not match the
graduations on the manual pulse generator.
7160 Approach handle clamp feedrate
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] Refer to standard parameter setting table (C)
Approach handle clamp feedrate is set.
When the setting is 0, the feedrate is not clamped.
7161 Guidance handle clamp feedrate
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] Refer to standard parameter setting table (C)
Guidance handle clamp feedrate is set.
When the setting is 0, the feedrate is not clamped.
#7 #6 #5 #4 #3 #2 #1 #0
7200 OP7 OP6 OP5 OP4 OP3 OP2 OP1
[Input type] Parameter input
[Data type] Bit path
NOTE
When at least one of these parameters is set, the
power must be turned off before operation is
continued.
# 0 OP1 Mode selection on software operator's panel
0: Not performed
1: Performed
# 1 OP2 JOG feed axis select and manual rapid traverse select on software
operator's panel
0: Not performed
1: Performed
B-63944EN/03 APPENDIX A.PARAMETERS
- 2153 -
# 2 OP3 Manual pulse generator's axis select and manual pulse generator's
magnification select on software operator's panel
0: Not performed
1: Performed
# 3 OP4 JOG feedrate override select, feedrate override select, and rapid
traverse override select on software operator's panel
0: Not performed
1: Performed
# 4 OP5 Optional block skip select, single block select, machine lock select,
and dry run select on software operator's panel
0: Not performed
1: Performed
# 5 OP6 Protect key on software operator's panel
0: Not performed
1: Performed
# 6 OP7 Feed hold on software operator's panel
0: Not performed
1: Performed
A.PARAMETERS APPENDIX B-63944EN/03
- 2154 -
7210 Jog-movement axis and its direction on software operator's panel “↑”
7211 Jog-movement axis and its direction on software operator's panel “↓”
7212 Jog-movement axis and its direction on software operator's panel “→”
7213 Jog-movement axis and its direction on software operator's panel “←”
7214 Jog-movement axis and its direction on software operator's panel “ ”
7215 Jog-movement axis and its direction on software operator's panel “ ”
7216 Jog-movement axis and its direction on software operator's panel “ ”
7217 Jog-movement axis and its direction on software operator's panel “ ”
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to 8
On software operator's panel, set a feed axis corresponding to an
arrow key on the MDI panel when jog feed is performed.
Setting value Feed axis and direction
0 Not moved
1 First axis, positive direction
2 First axis, negative direction
3 Second axis, positive direction
4 Second axis, negative direction
5 Third axis, positive direction
6 Third axis, negative direction
7 Fourth axis, positive direction
8 Fourth axis, negative direction
Example)
Under X, Y, and Z axis configuration, to set arrow keys to feed
the axes in the direction specified as follows, set the parameters
to the values given below. [8↑] to the positive direction of the Z
axis, [2↓] to the negative direction of the Z axis, [6→] to the
positive direction of the X axis [4←] to the negative direction of
the X axis, [1 ] to the positive direction of the Y axis, [9 ] to
the negative direction of the Y axis
Parameter No.7210 = 5 (Z axis, positive direction)
Parameter No.7211 = 6 (Z axis, negative direction)
Parameter No.7212 = 1 (X axis, positive direction)
Parameter No.7213 = 2 (X axis, negative direction)
Parameter No.7214 = 3 (Y axis, positive direction)
Parameter No.7215 = 4 (Y axis, negative direction)
Parameter No.7216 = 0 (Not used)
Parameter No.7217 = 0 (Not used)
Arrow keys on MDI panel
B-63944EN/03 APPENDIX A.PARAMETERS
- 2155 -
#7 #6 #5 #4 #3 #2 #1 #0
7300 MOU MOA
[Input type] Parameter input
[Data type] Bit path
# 6 MOA In program restart operation, before movement to a machining restart
point:
0: The last M, S, T, and B codes are output.
1: All M codes and the last S, T, and B codes are output.
This parameter is enabled when the MOU parameter is set to 1.
# 7 MOU In program restart operation, before movement to a machining restart
point after restart block search:
0: The M, S, T, and B codes are not output.
1: The last M, S, T, and B codes are output.
7310 Ordinal number of an axis along which a movement is made in dry run after
program restart
[Input type] Setting input
[Data type] Byte axis
[Valid data range] 1 to (Number of controlled axes)
This parameter sets the ordinal number of an axis along which a
movement is made in dry run after the program is restarted.
#7 #6 #5 #4 #3 #2 #1 #0
7501 IPC IT2 IT1 IT0
[Input type] Parameter input
[Data type] Bit path
# 4 IT0
# 5 IT1
# 6 IT2
IT2 IT1 IT0 Interpolation of high-speed cutting G05 data (ms)
0 0 0 8
0 0 1 2
0 1 0 4
0 1 1 1
1 0 0 16
1 1 1 0.5
# 7 IPC While high-speed cutting (G05) is being executed using cycle
machining data, monitoring to see whether distribution processing is
stopped or not is:
0: Not performed.
1: Performed. (If distribution processing is stopped in the middle,
an alarm (PS0179) is issued after distribution is completed.)
A.PARAMETERS APPENDIX B-63944EN/03
- 2156 -
#7 #6 #5 #4 #3 #2 #1 #0
7502 LC2 LC1
[Input type] Parameter input
[Data type] Bit path
# 4 LC1
# 5 LC2
LC2 LC1 End timing of servo learning function during
high-speed cycle cutting retract function
0 0
Disables the servo learning function, after which
retract operation starts.
0 1
Disables the servo learning function upon the
completion of retract operation.
1 0
Disables the servo learning function upon the
completion of a retract cycle.
#7 #6 #5 #4 #3 #2 #1 #0
7503 HCT
[Input type] Parameter input
[Data type] Bit path
# 4 HCT The variable number for starting storage of high-speed cycle
machining distribution data is:
0: Specified by 1/10.
1: Specified by 1/100.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2157 -
#7 #6 #5 #4 #3 #2 #1 #0
7505 HUN
[Input type] Parameter input
[Data type] Bit axis
NOTE
When this parameter bit is set, the power must be
turned off before operation is continued.
# 1 HUN During high-speed cutting, the increment system of distribution data
is:
0: 1 pulse.
1: 10 pulses.
NOTE
If data distributed at one time is longer than one
word because of the least input increment and the
maximum movement feedrate, this parameter is
used. If bit parameter HUN is set to 1 for an axis,
high-speed cycle machining data distributed to that
axis is internally multiplied by 10 by the CNC and
then input. Therefore, when using HUN for an axis,
set a tenth of high-speed cycle machining data to
be distributed to that axis.
7510 Number of controlled axes for high-speed cycle machining
[Input type] Parameter input
[Data type] Word path
[Valid data range] 1 to number of controlled axes
Set the number of axes to be controlled when G05 is specified to
perform high-speed cycle machining.
7514 Retract direction and retract feedrate in high-speed cycle machining retract
operation
[Input type] Parameter input
[Data type] Real axis
[Valid data range] Refer to standard parameter setting table (C)
This parameter sets a retract direction and retract feedrate along each
axis in a high-speed cycle machining retract operation. The
superimposed feedrate for each axis is specified, and the retract
direction is specified with a sign.
A.PARAMETERS APPENDIX B-63944EN/03
- 2158 -
7515 Number of retract operation distributions in a high-speed cycle machining
retract operation
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 0 to 99999999
This parameter sets the number of retract operation distributions in a
high-speed cycle machining retract operation.
When the cycle currently being executed ends before the number of
distributions specified in this parameter are performed, retract
operation is terminated. When 0 is specified in this parameter, the
number of retract operation distributions is assumed to be infinite. In
this case, retract operation is performed until the cycle currently being
executed ends.
#7 #6 #5 #4 #3 #2 #1 #0
7600 PLZ
[Input type] Parameter input
[Data type] Bit path
# 7 PLZ Reference position return based on a G28 command on the tool
rotation axis for polygon turning is:
0: Performed in the same sequence as manual reference position
return.
1: Performed by positioning using the rapid traverse rate.
The synchronous axis returns to the reference position in the same
sequence as the manual reference position return when no
return-to-reference position is performed after the power is turned on.
7610 Control axis number of tool rotation axis for polygon turning
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to number of controlled axes
This parameter sets the control axis number of a rotation tool axis
used for polygon turning.
However, when a G51.2 command is executed by setting 0 in this
parameter, operation stops with the alarm (PS0314).
B-63944EN/03 APPENDIX A.PARAMETERS
- 2159 -
7640 Master axis in spindle-spindle polygon turning
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to Maximum number of controlled axes (Within a path)
This parameter sets the master axis in spindle-spindle polygon turning.
NOTE
1 Spindle-spindle polygon turning is enabled only for serial spindles.
2 When any one of parameter No. 7640 and No. 7641 is set to 0, polygon turning is
performed using the first spindle (master axis) and the second spindle (polygon
synchronous axis) in the path to which the parameter belongs.
3 When a spindle other than the first serial spindle is used as a master axis, the
multi-spindle control option is required to specify an S command for the master
axis.
4 When the PMC window function or G10 command is used to rewrite this parameter,
rewrite this parameter before the block specifying the spindle-spindle polygon
command G51.2. When the PMC window function is used to rewrite this parameter
in the block immediately before G51.2, specify the rewriting of this parameter by
using an M code (parameter No. 3411 and up) without buffering.
7641 Polygon synchronous axis in spindle-spindle polygon turning
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to Maximum number of controlled axes (Within a path)
This parameter sets the polygon synchronous (slave) axis in
spindle-spindle polygon turning.
NOTE
1 Spindle-spindle polygon turning is enabled only for serial spindles.
2 When any one of parameter No. 7640 and No. 7641 is set to 0, polygon turning is
performed using the first spindle (master axis) and the second spindle (polygon
synchronous axis) in the path to which the parameter belongs.
3 When a spindle other than the first serial spindle is used as a master axis, the
multi-spindle control option is required to specify an S command for the master
axis.
4 When the PMC window function or G10 command is used to rewrite this parameter,
rewrite this parameter before the block specifying the spindle-spindle polygon
command G51.2. When the PMC window function is used to rewrite this parameter
in the block immediately before G51.2, specify the rewriting of this parameter by
using an M code (parameter No. 3411 and up) without buffering.
A.PARAMETERS APPENDIX B-63944EN/03
- 2160 -
7642 Master axis in spindle-spindle polygon turning (spindle number common to
the system)
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to Maximum number of controlled axes (Common to the system)
This parameter sets the master axis in spindle-spindle polygon turning.
NOTE
1 Spindle-spindle polygon turning is enabled only for serial spindles.
2 This parameter is invalid if either parameter No. 7642 or No.7643 is set to 0. In this
case, the settings of parameter No. 7640 and No.7641 are valid.
3 When a spindle other than the first serial spindle is used as a master axis, the
multi-spindle control option is required to specify an S command for the master
axis.
4 When the PMC window function or G10 command is used to rewrite this parameter,
rewrite this parameter before the block specifying the spindle-spindle polygon
command G51.2. When the PMC window function is used to rewrite this parameter
in the block immediately before G51.2, specify the rewriting of this parameter by
using an M code (parameter No. 3411 and up) without buffering.
5 A spindle number common to the system is to be set in this parameter. When using
this parameter, set 0 in parameter No. 7640 and No. 7641.
7643 Polygon synchronous axis in spindle-spindle polygon turning (spindle
number common to the system)
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to Maximum number of controlled axes (Common to the system)
This parameter sets the polygon synchronous (slave) axis in
spindle-spindle polygon turning.
NOTE
1 Spindle-spindle polygon turning is enabled only for serial spindles.
2 This parameter is invalid if either parameter No. 7642 or No.7643 is set to 0. In this
case, the settings of parameter No. 7640 and No.7641 are valid.
3 When a spindle other than the first serial spindle is used as a master axis, the
multi-spindle control option is required to specify an S command for the master
axis.
4 When the PMC window function or G10 command is used to rewrite this parameter,
rewrite this parameter before the block specifying the spindle-spindle polygon
command G51.2. When the PMC window function is used to rewrite this parameter
in the block immediately before G51.2, specify the rewriting of this parameter by
using an M code (parameter No. 3411 and up) without buffering.
5 A spindle number common to the system is to be set in this parameter. When using
this parameter, set 0 in parameter No. 7640 and No. 7641.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2161 -
#7 #6 #5 #4 #3 #2 #1 #0
7700 HDR HBR
[Input type] Parameter input
[Data type] Bit path
# 0 HBR When the electronic gear box (EGB) function is used, performing a
reset:
0: Cancels the synchronous mode (G81 or G81.5).
1: Does not cancel the synchronous mode. The mode is canceled
only by the G80 or G80.5 command.
# 2 HDR Direction of helical gear compensation (usually, set 1.)
(Example) To cut a left-twisted herical gear when the direction of
rotation about the C-axis is the negative (-) direction:
0: Set a negative (-) value in P.
1: Set a positive (+) value in P.
When HDR = 1
+C
C : +, Z : +, P : +
Compensation direction:+
(a)
-Z
+Z +C
C : +, Z : +, P : -
Compensation direction:-
(b)
+C
C : +, Z : -, P : +
Compensation direction:-
(c)
+C
C : +, Z : -, P : -
Compensation direction:+
(d)
-Z
+Z
C : -, Z : +, P : +
C : Compensation direction:-
(e)
-C
C : -, Z : +, P : -
Compensation direction:+
(f)
-C
C : -, Z : -, P : +
Compensation direction:+
(g)
-C
C : -, Z : -, P : -
Compensation direction:-
(h)
-C
When HDR = 0 ((a), (b), (c), and (d) are the same as when HDR = 1)
-Z
+Z
C : -, Z : +, P : +
Compensation direction:+
(e)
-C
C : -, Z : +, P : -
Compensation direction:-
(f)
-C
C : -, Z : -, P : +
Compensation direction:-
(g)
-C
C : -, Z : -, P : -
Compensation direction:+
(h)
-C
A.PARAMETERS APPENDIX B-63944EN/03
- 2162 -
#7 #6 #5 #4 #3 #2 #1 #0
7701 LZR
[Input type] Parameter input
[Data type] Bit path
# 3 LZR When L (number of hob threads) = 0 is specified at the start of EGB
synchronization (G81):
0: Synchronization is started, assuming that L = 1 is specified.
1: Synchronization is not started, assuming that L = 0 is specified.
However, helical gear compensation is performed.
#7 #6 #5 #4 #3 #2 #1 #0
7702 PHD PHS ART TDP
[Input type] Parameter input
[Data type] Bit path
# 0 TDP The specifiable number of teeth, T, of the electronic gear box (G81)
is:
0: 1 to 1000
1: 0.1 to 100 (1/10 of a specified value)
NOTE
In either case, a value from 1 to 1000 can be
specified.
# 3 ART The retract function executed when an alarm is issued is:
0: Disabled.
1: Enabled.
When an alarm is issued, a retract operation is performed with a set
feedrate and travel distance (parameter Nos. 7740 and 7741).
NOTE
If a servo alarm is issued for other than the axis
along which a retract operation is performed, the
servo activating current is maintained until the
retract operation is completed.
# 6 PHS When the G81/G80 block contains no R command:
0: Acceleration/deceleration is not performed at the start or
cancellation of EGB synchronization.
1: Acceleration/deceleration is performed at the start or cancellation
of EGB synchronization. After acceleration at the start of
synchronization, phase synchronization is automatically
performed.
# 7 PHD The direction of movement for automatic phase synchronization is:
0: Positive (+).
1: Negative (-).
B-63944EN/03 APPENDIX A.PARAMETERS
- 2163 -
#7 #6 #5 #4 #3 #2 #1 #0
7703 ARO ARE ERV
[Input type] Parameter input
[Data type] Bit path
# 0 ERV During EGB synchronization (G81), feed per revolution is performed
for:
0: Feedback pulses.
1: Pulses converted to the speed for the workpiece axis.
# 1 ARE The retract function executed when an alarm is issued retracts the tool
during:
0: EGB synchronization or automatic operation (automatic
operation signal OP = 1).
1: EGB synchronization.
# 2 ARO The retract function executed when an alarm is issued retracts the tool
during:
0: EGB synchronization.
1: EGB synchronization and automatic operation (automatic
operation signal OP = 1).
NOTE
This parameter is valid when bit 1 (ARE) of
parameter No. 7703 is set to 1.
The following table lists the parameter settings and corresponding
operation.
ARE ARO Operation
1 0 During EGB synchronization
1 1 During EGB synchronization and automatic operation
0 0
0 1
During EGB synchronization or automatic operation
NOTE
1 Parameters ARE and ARO are valid when bit 3
(ART) of parameter No. 7702 is set to 1 (when the
retract function executed when an alarm is
issued ).
2 This parameter is valid when bit 1 (ARE) of
parameter No. 7703 is set to 1.
A.PARAMETERS APPENDIX B-63944EN/03
- 2164 -
7710 Axis number of an axis to be synchronized using the method of command
specification for a hobbing machine
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 1 to Number of controlled axes
When there are several groups of axes to be synchronized (the axes for
which bit 0 (SYNMOD) of parameter No. 2011 is set to 1), an axis for
which to start synchronization is specified using the following
command (for a hobbing machine):
G81 T t L ± l ;
t: Spindle speed (1 ≤ t ≤ 1000)
l: Number of synchronized axis rotations (1 ≤ l ≤ 21)
Synchronization between the spindle and a specified axis is
established with the ratio of ±l rotations about the synchronized axis
to t spindle rotations.
t and l correspond to the number of teeth and the number of threads on
the hobbing machine, respectively.
Above command is issued without setting this parameter when there
are several groups of axes to be synchronized, the alarm (PS1593) is
issued.
When only one group of axes is to be synchronized, this parameter is
ignored.
#7 #6 #5 #4 #3 #2 #1 #0
7731 ECN EFX
[Input type] Parameter input
[Data type] Bit path
# 0 EFX As the EGB command:
0: G80 and G81 are used.
1: G80.4 and G81.4 are used.
NOTE
When this parameter is set to 0, no drilling canned
cycle can be used.
# 3 ECN When the automatic phase synchronization function for the electronic
gear box is disabled, during EGB synchronization, the G81 or G81.5
command:
0: Cannot be issued again. (The alarm (PS1595) is issued.)
1: Can be issued again.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2165 -
7740 Feedrate during retraction
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
This parameter sets the feedrate during retraction for each axis.
7772 Number of position detector pulses per rotation about the tool axis
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 1 to 999999999
This parameter sets the number of pulses per rotation about the tool
axis (on the spindle side), for the position detector.
For an A/B phase detector, set this parameter with four pulses
equaling one A/B phase cycle.
7773 Number of position detector pulses per rotation about the workpiece axis
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 1 to 999999999
This parameter sets the number of pulses per rotation about the
workpiece axis (on the slave side), for the position detector.
Set the number of pulses output by the detection unit.
Set parameters Nos. 7772 and 7773 when using the G81 EGB
synchronization command.
[Example 1] When the EGB master axis is the spindle and the EGB slave axis is
the C-axis
Synchronization
switch
CNC
Detection unit
β
p/rev
α p/rev
C-axis
Least command increment
0.001deg
Command
pulses
×
FFG
Gear ratio
A
Detector
×CMR
Slave axis
Gear
ratio B
Error counter
Follow-up
×CMR
Dummy axis
n/m
×
FFG
N/M
Motor
Detector
Spindle
Error counter Speed/current control
Synchronization
facto
r
Gear ratio of the spindle to the detector B:
1/1 (The spindle and detector are directly connected to each
other.)
Number of detector pulses per spindle rotation β: 80,000 pulses/rev
(Calculated for four pulses for one A/B phase cycle)
A.PARAMETERS APPENDIX B-63944EN/03
- 2166 -
FFG N/M of the EGB dummy axis: 1/1
Gear ratio of the C-axis A: 1/36 (One rotation about the C-axis to 36
motor rotations)
Number of detector pulses per C-axis rotation α: 1,000,000 pulses/rev
C-axis CMR: 1
C-axis FFG n/m: 1/100
In this case, the number of pulses per spindle rotation is:
80000 × 1/1 = 80000
Therefore, set 80000 for parameter No. 7772.
The number of pulses per C-axis rotation in the detection unit is:
1000000 ÷ 1/36 × 1/100 = 360000
Therefore, set 360000 for parameter No. 7773.
[Example 2] When the gear ratio of the spindle to the detector B is 2/3 for the
above example (When the detector rotates twice for three spindle
rotations)
In this case, the number of pulses per spindle rotation is:
3
160000
=
3
2
80000 ×
160000 cannot be divided by 3 without a remainder. In this case,
change the setting of parameter No. 7773 so that the ratio of the
settings of parameters Nos. 7772 and 7773 indicates the value you
want to set.
1080000
160000
=
3360000
160000
=
360000
3
160000
=
No.7773
No.7772
×
Therefore, set 160000 for parameter No. 7772 and 1080000 for
parameter No. 7773.
As described above, all the settings of parameters Nos. 7772 and 7773
have to do is to indicate the ratio correctly. So, you can reduce the
fraction indicated by the settings. For example, you may set 16 for
parameter No. 7772 and 108 for parameter No. 7773 for this case.
7776 Feedrate during automatic phase synchronization for the workpiece axis
[Input type] Parameter input
[Data type] Real path
[Unit of data] deg/min
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
This parameter sets the feedrate during automatic phase
synchronization for the workpiece axis.
When this parameter is set to 0, the rapid traverse rate (parameter No.
1420) is used as the feedrate during automatic phase synchronization.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2167 -
7777 Angle shifted from the spindle position (one-rotation signal position) which
the workpiece axis uses as the reference of phase synchronization
[Input type] Parameter input
[Data type] Real path
[Unit of data] deg
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
This parameter sets the angle shifted from the spindle position
(one-rotation signal position) which the workpiece axis uses as the
reference of phase synchronization.
7778 Acceleration for acceleration/deceleration for the workpiece axis
[Input type] Parameter input
[Data type] Real axis
[Unit of data] deg/sec2
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (D)
(For a millimeter machine, 0.0 to +100000.0, for an inch machine, 0.0
to +10000.0)
This parameter sets an acceleration for acceleration/deceleration for
the workpiece axis.
NOTE
1 In the FS16i series, acceleration/deceleration for
automatic phase matching is set by specifying a
feedrate and a time constant in parameter Nos.
2135 and 2136 separately; in the FS30i series,
acceleration/deceleration is directly set in
parameter No. 7778.
2 If this parameter is set to 0, specifying G81 results
in an alarm (PS1598).
7782 Number of pulses from the position detector per EGB master axis rotation
[Input type] Parameter input
[Data type] 2-word axis
[Valid data range] 1 to 999999999
For a slave axis, set the number of pulses generated from the position
detector per EGB master axis rotation.
For an A/B phase detector, set this parameter with four pulses
equaling one A/B phase cycle.
A.PARAMETERS APPENDIX B-63944EN/03
- 2168 -
7783 Number of pulses from the position detector per EGB slave axis rotation
[Input type] Parameter input
[Data type] 2-word axis
[Unit of data] Detection unit
[Valid data range] 1 to 999999999
For a slave axis, set the number of pulses generated from the position
detector per EGB slave axis rotation.
Set the number of pulses output by the detection unit.
Set this parameter when using the G81.5 EGB synchronization
command.
The method for setting parameters Nos. 7782 and 7783 is the same as
for parameters Nos. 7772 and 7773. For the method, see the
description of parameters Nos. 7772 and 7773.
The ratio of the number of pulses for the master slave to that of pulses
for the slave axis may be valid, but the settings of the parameters may
not indicate the actual number of pulses. For example, the number of
pulses may not be able to be divided without a remainder for the
reason of the master and slave axis gear ratios as described in example
2. In this case, the following methods cannot be used for the G81.5
command:
G81.5 T_ C_ ; When the speed is specified for the master axis and
the travel distance is specified for the slave axis
G81.5 P_ C0 L_ ; When the number of pulses is specified for the
master axis and the speed is specified for the slave
axis
#7 #6 #5 #4 #3 #2 #1 #0
8001 RDE OVE MLE
[Input type] Parameter input
[Data type] Bit path
# 0 MLE Whether all axis machine lock signal MLK is valid for
PMC-controlled axes
0: Valid
1: Invalid
The axis-by-axis machine lock signal MLKx depends on the setting of
bit 1 of parameter No. 8006.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2169 -
# 2 OVE Signals related to dry run and override used in PMC axis control
0: Same signals as those used for the CNC
1: Signals specific to the PMC
The signals used depend on the settings of these parameter bits as
indicated below.
Signals No.8001#2=0
(same signals as those used for the CNC)
No.8001#2=1
(signals specific to the PMC)
Feedrate override signals *FV0 to *FV7 G012 *EFV0 to *EFV7 G151
Override cancellation signal OVC G006. EOVC G150.5
Rapid traverse override signals ROV1,2 G014.0, .1 EROV1,2 G150.0, .1
Dry run signal DRN G46.7 EDRN G150.7
Rapid traverse selection signal RT G19.7 ERT G150.6
(The signal addresses at PMC selection time are for the first group.)
# 3 RDE Whether dry run is valid for rapid traverse in PMC axis control
0: Invalid
1: Valid
#7 #6 #5 #4 #3 #2 #1 #0
8002 FR2 FR1 PF2 PF1 F10 RPD
[Input type] Parameter input
[Data type] Bit path
# 0 RPD Rapid traverse rate for PMC-controlled axes
0: Feedrate specified with parameter No.1420
1: Feedrate specified with the feedrate data in an axis control
command by PMC
# 3 F10 Least increment for the feedrate for cutting feed (per minute) in PMC
axis control
The following settings are applied when bit 4 (PF1) of parameter No.
8002 is set to 0 and bit 5 (PF2) of parameter No. 8002 is set to 0.
F10 IS-A IS-B IS-C IS-D IS-E
0 10 1 0.1 0.01 0.001
Millimeter input
(mm/min) 1 100 10 1 0.1 0.01
0 0.1 0.01 0.001 0.0001 0.00001Inch input
(inch/min) 1 1 0.1 0.01 0.001 0.0001
# 4 PF1
# 5 PF2 Set the feedrate unit of cutting feedrate (feed per minute) for an axis
controlled by the PMC.
Bit 5 (PF2) of parameter
No. 8002
Bit 4 (PF1) of parameter
No. 8002 Feedrate unit
0 0 1 / 1
0 1 1 / 10
1 0 1 / 100
1 1 1 / 1000
A.PARAMETERS APPENDIX B-63944EN/03
- 2170 -
# 6 FR1
# 7 FR2 Set the feedrate unit for cutting feedrate (feed per rotation) for an axis
controlled by the PMC.
Bit 7 (FR2) of
parameter No. 8002
Bit 6 (FR1) of
parameter No. 8002
Millimeter
input
(mm/rev)
Inch input
(inch/rev)
0 0
1 1
0.0001 0.000001
0 1 0.001 0.00001
1 0 0.01 0.0001
#7 #6 #5 #4 #3 #2 #1 #0
8004 NCI
[Input type] Parameter input
[Data type] Bit path
# 6 NCI In axis control by the PMC, a position check at the time of
deceleration is:
0: Performed.
1: Not performed.
#7 #6 #5 #4 #3 #2 #1 #0
8005 EDC
[Input type] Setting input
[Data type] Bit path
# 0 EDC In axis control by the PMC, an external deceleration function is:
0: Disabled.
1: Enabled.
#7 #6 #5 #4 #3 #2 #1 #0
8006 EZR EFD
[Input type] Parameter input
[Data type] Bit path
# 4 EFD When cutting feed (feed per minute) is used in PMC axis control, the
specification unit of feedrate data is:
0: Unchanged (1 times).
1: 100 times greater.
NOTE
When this parameter is set to 1, bit 3 (F10) of
parameter No. 8002 is invalid.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2171 -
# 6 EZR In PMC axis control, bit 0 (ZRNx) of parameter No. 1005 is:
0: Invalid.
With a PMC controlled axis, the alarm (PS0224) is not issued.
1: Valid.
A reference position return state check is made on a PMC
controlled axis as with an NC axis according to the setting of bit
0 (ZRNx) of parameter No. 1005.
#7 #6 #5 #4 #3 #2 #1 #0
8008 EMRx
[Input type] Parameter input
[Data type] Bit axis
# 0 EMRx When a PMC axis control command is issued in mirror image state,
the mirror image is:
0: Not considered.
1: Considered.
This parameter is valid in the mirror image mode set with the mirror
image signals MI1 to MI8 <G106.0 to .7> set to 1 or bit 0 (MIRx) of
parameter No. 12 set to 1.
If a movement is made along the same axis by doubly specifying a
command with the CNC and PMC axis control when this parameter is
set to 0, and the mirror image mode is set, a coordinate shift can occur
afterwards. So, do not attempt to make such a movement.
8010 Selection of the DI/DO group for each axis controlled by the PMC
[Input type] Parameter input
[Data type] Byte axis
[Valid data range] 1 to 40
Specify the DI/DO group to be used to specify a command for each
PMC-controlled axis.
For addresses of the fifth group and up, 1000 is added in steps of 4
groups.
For example:
The start address of the 10th group is G2154.
The start address of the 25th axis is G6142.
P8010 Description
1 DI/DO 1st group (G142 to G153) is used.
2 DI/DO 2nd group (G154 to G165) is used.
3 DI/DO 3rd group (G166 to G177) is used.
4 DI/DO 4th group (G178 to G189) is used.
5 DI/DO 5th group (G1142 to G1153) is used.
6 DI/DO 6th group (G1154 to G1165) is used.
: :
13 DI/DO 13th group (G3142 to G3153) is used.
: :
20 DI/DO 20th group (G4178 to G4189) is used.
21 DI/DO 21st group (G5142toG5153) is used.
: :
A.PARAMETERS APPENDIX B-63944EN/03
- 2172 -
P8010 Description
29 DI/DO 29th group (G7142toG7153) is used.
: :
35 DI/DO 35th group (G8166toG8177) is used.
36 DI/DO 36th group (G8178toG8189) is used.
37 DI/DO 37th group (G9142toG9153) is used.
38 DI/DO 38th group (G9154toG9165) is used.
39 DI/DO 39th group (G9166toG9177) is used.
40 DI/DO 40th group (G9178toG9189) is used.
NOTE
When a value other than the above is set, the axis
is not controlled by the PMC.
#7 #6 #5 #4 #3 #2 #1 #0
8011 XRT
[Input type] Parameter input
[Data type] Bit axis
# 0 XRT The axis that uses the group specified by parameter No. 8010 is:
0: Not controlled by the real time custom macro.
1: Controlled by the real time custom macro.
NOTE
1 This parameter is invalid for the axis for which 0 or a
value outside the range is set by parameter No.
8010
2 When multiple axes are assigned to the same group
by parameter No. 8010, these axes cannot be
controlled by the real time custom macro. When
multiple axes are assigned to the same group, be
sure to set this bit to 0.
3 When this parameter (No. 8011) is all 0s, the axis is
used for PMC axis control.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2173 -
8030 Time constant for exponential acceleration/deceleration in cutting feed or
continuous feed under PMC axis control
[Input type] Parameter input
[Data type] 2-word axis
[Unit of data] msec
[Valid data range] 0 to 4000
For each axis, this parameter sets a time constant for exponential
acceleration/deceleration in cutting feed or continuous feed under
PMC axis control.
NOTE
When 0 is set in this parameter, the value set in
parameter No. 1622 is used.
The value set in parameter No. 1622 is used also
for linear acceleration/deceleration after cutting
interpolation.
#7 #6 #5 #4 #3 #2 #1 #0
8103 MWP MWT
[Input type] Parameter input
[Data type] Bit
NOTE
When at least one of these parameters is set, the
power must be turned off before operation is
continued.
# 0 MWT As the signal interface for the waiting M code:
0: The path individual signal interface is used.
1: The path common signal interface is used.
This parameter can be selected only when 2-path control is used.
# 1 MWP To specify a P command for the waiting M code/balance cut:
0: A binary value is used as conventionally done.
1: A path number combination is used.
8110 Waiting M code range (minimum value)
8111 Waiting M code range (maximum value)
[Input type] Parameter input
[Data type] 2-word
[Valid data range] 0 ,100to99999999
A range of M code values can be set by specifying a minimum waiting
M coder value (parameter No. 8110) and a maximum waiting M code
value (parameter No. 8111).
(parameter No. 8110) ≤ (waiting M code) ≤ (parameter No. 8111)
Set 0 in these parameters when the waiting M code is not used.
A.PARAMETERS APPENDIX B-63944EN/03
- 2174 -
#7 #6 #5 #4 #3 #2 #1 #0
8162 PKUx
[Input type] Parameter input
[Data type] Bit axis
# 2 PKUx In the parking state,
0: The absolute, relative, and machine coordinates are not updated.
1: The absolute and relative coordinates are updated. The machine
coordinates are not updated.
NOTE
1 With an axis for which polar coordinate
interpolation is specified, set this parameter to 1. If
this parameter is set to 0, a coordinate shift can
occur when a single block stop or feed hold is
performed in the polar coordinate interpolation
mode.
2 With an axis that is set to function as a
synchronous master axis and synchronous slave
axis at the same time (with bit 1 (SYWx) of
parameter No. 8167), set this parameter to 1.
3 With an axis specified in the three-dimensional
coordinate conversion mode, set this parameter to
1. If this parameter is set to 0, the alarm (PS0367)
is issued.
#7 #6 #5 #4 #3 #2 #1 #0
8163 NUMx
[Input type] Parameter input
[Data type] Bit axis
# 7 NUMx When neither synchronous control nor composite control is applied, a
move command for the axis is:
0: Not disabled.
1: Disabled.
NOTE
If a move command is specified for an axis with
NUMx set to 1 when neither synchronous control
nor composite control is applied, alarm PS0353 is
issued.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2175 -
8180 Master axis with which an axis is synchronized under synchronous control
[Input type] Parameter input
[Data type] Word axis
[Valid data range] 101, 102, 103, . . . , (path number)*100+(intra-path relative axis
number) (101, 102, 103, . . . , 201, 202, 203, . . . , 1001, 1002,
1003, . . .)
This parameter sets the path number and intra-path relative axis
number of the master axis with which each axis is synchronized.
When zero is specified, the axis does not become a slave axis and is
not synchronized with another axis. When an identical number is
specified in two or more parameters, one master axis has two or more
slave axes.
8183 Composite control axis of the other path in composite control for each axis
[Input type] Parameter input
[Data type] Word axis
[Valid data range] 101, 102, 103, . . . , (path number)*100+(intra-path relative axis
number) (101, 102, 103, . . . , 201, 202, 203, . . . , 1001, 1002,
1003, . . .)
This parameter sets with which axis each axis is to be placed under
composite control. When zero is specified, control of the axis is not
replaced under composite control. An identical number can be
specified in two or more parameters, but composite control cannot be
exercised for all of them at a time.
NOTE
When the two-path interface is used (bit 1 (MIX) of
parameter No. 8166 is set to 1), set this parameter
for path 2.
A.PARAMETERS APPENDIX B-63944EN/03
- 2176 -
8186 Master axis under superimposed control
[Input type] Parameter input
[Data type] Word axis
[Valid data range] 101, 102, 103, . . . , (path number)*100+(intra-path relative axis
number) (101, 102, 103, . . . , 201, 202, 203, . . . , 1001, 1002,
1003, . . .)
This parameter sets the path number and intra-path relative axis
number of a superimposed master axis for each axis when
superimposed control is exercised. When zero is specified, the axis
does not become a slave axis under superimposed control and the
move pulse of another axis is not superimposed.
An identical number can be specified in two or more parameters to
exercise superimposed control simultaneously. This means that
superimposed control with one master axis and multiple slave axes is
possible.
A slave axis may function as the master axis of another axis to allow
three-generation superimposed control: parent (master axis) - child
(slave axis/master axis) - grandchild (slave axis).
In this case, a movement along the child is made by its travel distance
plus the travel distance of the parent, and a movement along the
grandchild is made by its travel distance plus the travel distance of the
child plus the travel distance of the parent.
Example of the relationship of parent (X1 of path 1) - child (X2 of
path 2) - grandchild (X3 of path 3):
The travel distance of X1 is superimposed on X2, and the travel
distances of X1 and X2 are further superimposed on X3.
Parameter No. 8186x of path 2 = 101
Parameter No. 8186x of path 3 = 201
#7 #6 #5 #4 #3 #2 #1 #0
8200 AZR AAC
[Input type] Parameter input
[Data type] Bit path
NOTE
When at least one of these parameters is set, the
power must be turned off before operation is
continued.
# 0 AAC
0: Does not perform angular axis control.
1: Performs inclined axis control.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2177 -
# 2 AZR
0: The machine tool is moved along the Cartesian axis during
manual reference position return along the slanted axis under
angular axis control.
1: The machine tool is not moved along the Cartesian axis during
manual reference position return along the slanted axis under
angular axis control.
#7 #6 #5 #4 #3 #2 #1 #0
8201 A53 AO3 AO2 AOT
[Input type] Parameter input
[Data type] Bit path
NOTE
When at least one of these parameters is set, the
power must be turned off before operation is
continued.
# 0 AOT Stored stroke limit 1 under angular axis control is handled as:
0: Value in the slanted coordinate system.
1: Value in the Cartesian coordinate system.
# 1 AO2 Stored stroke limit 2 under angular axis control is handled as:
0: Value in the slanted coordinate system.
1: Value in the Cartesian coordinate system.
# 2 AO3 Stored stroke limit 3 under angular axis control is handled as:
0: Value in the slanted coordinate system.
1: Value in the Cartesian coordinate system.
# 6 A53 So far, if a slanted axis is singly specified by a machine coordinate
command (G53) in angular axis control, this parameter set to 0
specifies that "compensation is applied to the Cartesian axis", and this
parameter set to 1 specifies that "a movement is made along the
slanted axis only". However, the specification has been changed so
that "a movement is made along the slanted axis only", regardless of
whether this parameter is set to 0 or 1.
8210 Slant angle of a slanted axis in angular axis control
[Input type] Parameter input
[Data type] Real path
[Unit of data] Degree
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] -180.000 to 180.000. However, angular axis control is disabled in the
ranges -95.000 to -85.000 and 85.000 to 95.000 (in the case of IS-B).
A.PARAMETERS APPENDIX B-63944EN/03
- 2178 -
8211 Axis number of a slanted axis subject to angular axis control
8212 Axis number of a Cartesian axis subject to slanted axis control
NOTE
When these parameters are set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Word path
[Valid data range] 1 to number of controlled axes
When angular axis control is to be applied to an arbitrary axis, these
parameters set the axis numbers of a slanted axis and Cartesian axis. If
0 is set in either of the two parameters, the same number is set in the
two parameters, or a number other than the controlled axis numbers is
set in either of the two parameters, a slanted axis and Cartesian axis
are selected as indicated in the following table:
Slanted axis Cartesian axis
M
series
Y-axis (axis with 2 set in
parameter No. 1022) of the
basic three axes
Z-axis (axis with 3 set in
parameter No. 1022) of the basic
three axes
T
series
X-axis (axis with 1 set in
parameter No. 1022) of the
basic three axes
Z-axis (axis with 3 set in
parameter No. 1022) of the basic
three axes
#7 #6 #5 #4 #3 #2 #1 #0
8301 SYA
[Input type] Parameter input
[Data type] Bit path
# 4 SYA In the servo-off state in axis synchronous control, the limit of the
difference between the positioning deviation of the master axis and
that of the slave axis is:
0: Checked.
1: Not checked.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2179 -
#7 #6 #5 #4 #3 #2 #1 #0
8302 SMA
[Input type] Parameter input
[Data type] Bit path
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
# 7 SMA When an absolute position detector is attached, and bit 4 (APZ) of
parameter No. 1815 for an axis in synchronous operation is set to OFF,
APZ of the pairing axis in synchronous operation is:
0: Not set to OFF.
1: Set to OFF.
#7 #6 #5 #4 #3 #2 #1 #0
8303 SOF SAF ATS ATE
[Input type] Parameter input
[Data type] Bit axis
NOTE
When at least one of these parameters is set, the
power must be turned off before operation is
continued.
# 0 ATE In axis synchronous control, automatic setting for grid positioning is:
0: Disabled
1: Enabled
Set this parameter with a slave axis.
# 1 ATS In axis synchronous control, automatic setting for grid positioning is:
0: Not started
1: Started
Set this parameter with a slave axis.
NOTE
When starting automatic setting for grid positioning,
set ATS to 1. Upon the completion of setting, ATS
is automatically set to 0.
# 2 SAF In axis synchronous control, a movement along a slave axis is:
0: Not added to actual feedrate display.
1: Added to actual feedrate display.
Set this parameter with a slave axis.
A.PARAMETERS APPENDIX B-63944EN/03
- 2180 -
# 7 SOF In axis synchronous control, the synchronization establishment
function based on machine coordinates is:
0: Disabled.
1: Enabled.
Set this parameter with a slave axis.
When using synchronization error compensation, set this parameter to
0.
#7 #6 #5 #4 #3 #2 #1 #0
8304 SYE SMS SCA MVB CLP ADJ SSA
[Input type] Parameter input
[Data type] Bit axis
# 0 SSA When the one-direction synchronization establishment function under
axis synchronous control is used:
0: The axis with a larger machine coordinate is used as the
reference.
1: The axis with a smaller machine coordinate is used as the
reference.
NOTE
1 When at least one of these parameters is set, the
power must be turned off before operation is
continued.
2 Set this parameter (SSA) to the same value for
both the master and slave axes.
# 2 ADJ In axis synchronous control, this parameter specifies an axis along
which a movement is made in the modification mode.
0: A movement is not made in the modification mode along the
axis.
1: A movement is made in the modification mode along the axis.
When this parameter is set to 1, the modification mode is set.
Along an axis with this parameter set to 1, a movement is made by a
move command for the master axis.
Set this parameter for one of the master and slave axes.
When there are multiple slave axes for one master axis, set this
parameter to 1 for an axis with which a synchronization error
excessive alarm is issued for recovery. If an alarm is issued with
multiple axes, modify this parameter after recovery of one axis to
recover another axis.
# 3 CLP In axis feed synchronous control, synchronization error compensation
is:
0: Disabled.
1: Enabled.
Set this parameter with a slave axis.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2181 -
# 4 MVB In the modification mode, a move command in a direction that
increases a synchronization error is:
0: Ignored.
1: Valid.
When there are multiple slave axes for one master axis, an attempt to
reduce the synchronous error of a slave axis by a movement along the
master axis can increase the synchronization error of another slave
axis. If this parameter is set to 0 in such a case, a movement can be
made in neither direction along the master axis. In this case, set bit 2
(ADJ) of parameter No. 8304 to make a movement along a slave axis
to perform a corrective operation.
# 5 SCA In axis synchronous control:
0: Synchronous operation is performed when the axis synchronous
control manual feed selection signal SYNCJ or the axis
synchronous control selection signal SYNC for slave axes is set
to 1.
1: Synchronous operation is performed at all times.
Set this parameter with a slave axis.
# 6 SMS The synchronization error smooth suppress function is:
0: Disabled.
1: Enabled.
Set this parameter with a slave axis.
# 7 SYE When external machine coordinate system shift is specified by
external data input/output for the master axis in synchronous control,
the slave axis is:
0: Not shifted.
1: Shifted by the same amount as specified for the master axis.
Set this parameter for the slave axis.
This function is disabled during normal operation.
#7 #6 #5 #4 #3 #2 #1 #0
8305 SSE SSO
[Input type] Parameter input
[Data type] Bit path
# 0 SSO The uni-directional synchronization function in axis synchronous
control is:
0: Disabled.
1: Enabled.
# 1 SSE After emergency stop, the uni-directional synchronization function in
axis synchronous control is:
0: Disabled.
1: Enabled.
A.PARAMETERS APPENDIX B-63944EN/03
- 2182 -
8311 Axis number of master axis in axis synchronous control
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Byte axis
[Valid data range] 0 to Number of controlled axes
Select a master axis in axis synchronous control. In the parameter for
the slave axis, set the axis number of the master axis.
Example 1)
When one set of axis synchronous control is used:
When the master axis is the first axis (X-axis), and the slave axis
is the third axis (Z-axis), set parameter No. 8311 as follows:
Parameter No.8311 X (first axis) = 0
Parameter No.8311 Y (second axis) = 0
Parameter No.8311 Z (third axis) = 1
Parameter No.8311 A (fourth axis) = 0
Example 2)
When three sets of axis synchronous control is used:
When the master axes are the first axis, second axis, and third
axis, and the slave axes are the sixth axis, fifth axis, and fourth
axis, set parameter No. 8311 as follows:
Parameter No.8311 X (first axis) = 0
Parameter No.8311 Y (second axis) = 0
Parameter No.8311 Z (third axis) = 0
Parameter No.8311 A (fourth axis) = 3
Parameter No.8311 B (fifth axis) = 2
Parameter No.8311 C (sixth axis) = 1
B-63944EN/03 APPENDIX A.PARAMETERS
- 2183 -
8312 Enabling/disabling mirror image in axis synchronous control
[Input type] Parameter input
[Data type] Word axis
[Valid data range] -127 to 128
This parameter sets mirror image for the slave axis. When 100 or a
more value is set with this parameter, the mirror image function is
applied to synchronous control. Set this parameter to the slave axis.
Example)
For reverse synchronization with the master axis being the third
axis and the slave axis being the fourth axis, set parameter No.
8312 as follows:
Parameter No.8312 X (first axis) = 0
Parameter No.8312 Y (second axis) = 0
Parameter No.8312 Z (third axis) = 0
Parameter No.8312 A (fourth axis) = 100
NOTE
In synchronous operation with mirror image
applied, synchronization error compensation,
synchronization establishment, synchronization
error checking, and modification mode cannot be
used.
8314 Maximum allowable error in synchronization error check based on machine
coordinates
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm, inch, degree (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 0 or positive 9 digit of minimum unit of data (refer to the standard
parameter setting table (B))
(When the increment system is IS-B, 0.0 to +999999.999)
This parameter sets a maximum allowable error in a synchronization
error check based on machine coordinates. When the error between
the master and slave axes in machine coordinates exceeds the value set
in this parameter, the machine stops with the servo alarm (SV0005).
Set this parameter with a slave axis.
NOTE
Set 0 in this parameter when a synchronization
error check is not made.
A.PARAMETERS APPENDIX B-63944EN/03
- 2184 -
8323 Limit in positional deviation check in axis synchronous control
[Input type] Parameter input
[Data type] 2-word axis
[Unit of data] Detection unit
[Valid data range] 0 to 999999999
This parameter sets the maximum allowable difference between the
master axis and slave axis position deviations. When the absolute
value of a positional deviation difference exceeds the value set in this
parameter in axis synchronous control, the alarm (DS0001) is issued.
Set this parameter with a slave axis. If 0 is specified in this parameter,
no position deviation difference check is made.
8325 Maximum compensation value in synchronization establishment based on
machine coordinates
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm, inch, degree (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 0 or positive 9 digit of minimum unit of data (refer to the standard
parameter setting table (B))
(When the increment system is IS-B, 0.0 to +999999.999)
This parameter sets the maximum compensation value for
synchronization. When a compensation value exceeding the value set
in this parameter is detected, the servo alarm (SV0001) is issued, and
the synchronization establishment is not performed.
Specify a slave axis for this parameter. To enable this parameter, set
the parameter SOF (bit 7 of parameter No.8303) to 1. When 0 is set in
this parameter, synchronization establishment is not performed.
8326 Difference between master axis and slave axis reference counters
[Input type] Parameter input
[Data type] 2-word axis
[Unit of data] Detection unit
[Valid data range] 0 to 999999999
The difference between the master axis reference counter and slave
axis reference counter (master axis and slave axis grid shift) is
automatically set when automatic setting for grid positioning is
performed. Then, the difference is transferred together with an
ordinary grid shift value to the servo system when the power is turned
on. This parameter is set with a slave axis.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2185 -
8327 Torque difference alarm detection timer
[Input type] Parameter input
[Data type] 2-word axis
[Unit of data] msec
[Valid data range] 0 to 4000
This parameter sets a time from the servo preparation completion
signal, SA <F000.6>, being set to 1 until torque difference alarm
detection is started in axis synchronous control.
When 0 is set in this parameter, the specification of 512 msec is
assumed.
Set this parameter with a slave axis.
8330 Multiplier for a maximum allowable synchronization error immediately after
power-up
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Word path
[Valid data range] 1 to 100
Until synchronization establishment is completed immediately after
power-up, synchronization error excessive alarm 2 is checked using
the maximum allowable error (parameter No. 8332) multiplied by the
value set in this parameter.
If the result produced by multiplying the value of parameter No. 8332
by the value of this parameter exceeds 32767, the value is clamped to
32767.
8331 Maximum allowable synchronization error for synchronization error
excessive alarm 1
[Input type] Parameter input
[Data type] 2-word axis
[Unit of data] Detection unit
[Valid data range] 1 to 32767
This parameter sets a maximum allowable synchronization error for
synchronization error excessive alarm 1.
Set this parameter with a slave axis.
A.PARAMETERS APPENDIX B-63944EN/03
- 2186 -
8332 Maximum allowable synchronization error for synchronization error
excessive alarm 2
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] 2-word axis
[Unit of data] Detection unit
[Valid data range] 1 to 32767
This parameter sets a maximum allowable synchronization error for
synchronization error excessive alarm 2.
Set this parameter with a slave axis.
8333 Synchronization error zero width for each axis
[Input type] Parameter input
[Data type] 2-word axis
[Unit of data] Detection unit
[Valid data range] 1 to 32767
When a synchronization error below the value set in this parameter is
detected, synchronization error compensation is not performed.
Set this parameter with a slave axis.
8334 Synchronization error compensation gain for each axis
[Input type] Parameter input
[Data type] Word axis
[Valid data range] 1 to 1024
This parameter sets a synchronization error compensation gain.
Compensation pulses found by the following expression are output for
the slave axis:
Compensation pulses = Synchronization error × (Ci/1024)
Ci: Compensation gain
Set this parameter with a slave axis.
8335 Synchronization error zero width 2 for each axis
[Input type] Parameter input
[Data type] 2-word axis
[Unit of data] Detection unit
[Valid data range] 0 to 32767
This parameter sets synchronization error zero width 2 for
synchronization error smooth suppression.
Set this parameter with a slave axis.
NOTE
Set a value less than the value set in parameter
No. 8333.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2187 -
8336 Synchronization error compensation gain 2 for each axis
[Input type] Parameter input
[Data type] Word axis
[Valid data range] 0 to 1024
This parameter sets synchronization error compensation gain 2 for
synchronization error smooth suppression.
Set this parameter with a slave axis.
NOTE
Set a value less than the value set in parameter
No. 8334.
8337 M code for turning off synchronization in axis synchronous control
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 1 to 999999999
This parameter specifies an M code for switching from synchronous
operation to normal operation.
The M code set in this parameter is not buffered.
8338 M code for turning on synchronization in axis synchronous control
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 1 to 999999999
This parameter specifies an M code for switching from normal
operation to synchronous operation.
The M code set in this parameter is not buffered.
#7 #6 #5 #4 #3 #2 #1 #0
8451 NOF ZAG
[Input type] Setting input
[Data type] Bit path
# 4 ZAG The deceleration function based on cutting load in AI contour control
(deceleration based on Z-axis fall angle) is:
0: Not performed.
1: Performed.
When this parameter is set to 1, be sure to set parameter Nos. 8456,
8457, and 8458.
# 7 NOF In AI contour control, an F command is:
0: Not ignored.
1: Ignored.
When this parameter is set to 1, the specification of the maximum
allowable feedrate set in parameter No. 8465 is assumed.
A.PARAMETERS APPENDIX B-63944EN/03
- 2188 -
8456 Override for range 2 that is applied during deceleration according to the
cutting load in AI contour control
8457 Override for range 3 that is applied during deceleration according to the
cutting load in AI contour control
8458 Override for range 4 that is applied during deceleration according to the
cutting load in AI contour control
[Input type] Setting input
[Data type] Word path
[Unit of data] %
[Valid data range] 1 to 100
For the function of decelerating according to the cutting load in AI
contour control, the override set in a parameter can be applied
according to the angle at which the tool moves downward along the
Z-axis. The feedrate obtained according to other conditions is
multiplied by the override for the range containing angle θ at which
the tool moves downward.
However, when bit 1 (ZG2) of parameter No. 19515 is set to 0, no
parameter is available to range 1, and 100% is applied at all times.
When bit 1 (ZG2) of parameter No. 19515 is set to 1, set an override
value for range 1 in parameter No. 19516.
Range 1 0°≤θ<30°
Range 2 30°≤θ<45°
Range 3 45°≤θ<60°
Range 4 60°≤θ≤90°
8465 Maximum allowable feedrate for AI contour control
[Input type] Setting input
[Data type] Real path
[Unit of data] mm/min, inch/min, degree/min (input unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
This parameter sets the maximum allowable feedrate for contour
control.
If a feedrate higher than the setting of this parameter is specified in the
AI contour control mode, the feedrate is clamped to that set in this
parameter.
If this parameter is set to 0, no clamping is performed.
When bit 7 (NOF) of parameter No. 8451 is set to 1, the tool moves,
assuming that the feedrate set in this parameter is specified. If 0 is set
in this parameter at this time, a movement is made at the specified
feedrate.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2189 -
8486 Maximum travel distance of a block where smooth interpolation or Nano
smoothing is applied
[Input type] Setting input
[Data type] Real path
[Unit of data] mm, inch (input unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
This parameter specifies a block length used as a reference to decide
whether to apply smooth interpolation or Nano smoothing. If the line
specified in a block is longer than the value set in the parameter,
smooth interpolation or Nano smoothing is not applied to that block.
8487 Angle at which smooth interpolation or Nano smoothing is turned off
[Input type] Setting input
[Data type] Real path
[Unit of data] Degree
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 0 to 90
This parameter sets the angle used to determine whether to apply
smooth interpolation or Nano smoothing.
At a point having a difference in angle greater than this setting,
smooth interpolation or Nano smoothing is turned off.
8490 Minimum travel distance of a block where smooth interpolation or Nano
smoothing is applied
[Input type] Setting input
[Data type] Real path
[Unit of data] mm, inch (input unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
This parameter sets a block length used to determine whether to apply
smooth interpolation or Nano smoothing.
If the line specified in a block is shorter than the value set in this
parameter, smooth interpolation or Nano smoothing is not applied to
that block.
A.PARAMETERS APPENDIX B-63944EN/03
- 2190 -
#7 #6 #5 #4 #3 #2 #1 #0
8900 PWE
[Input type] Setting input
[Data type] Bit
# 0 PWE The setting, from an external device and MDI panel, of those
parameters that cannot be set by setting input is:
0: Disabled.
1: Enabled.
10461 RGB value of color palette 1 for text for color set 3
10462 RGB value of color palette 2 for text for color set 3
:
10475 RGB value of color palette 15 for text for color set 3
[Input type] Parameter input
[Data type] 2-word
[Valid data range] 0 to 151515
Each of these parameters sets the RGB value of each color palette for
text by specifying a 6-digit number as described below.
rrggbb: 6-digit number (rr: red data, gg: green data, bb: blue data)
The valid data range of each color is 0 to 15 (same as the tone levels
on the color setting screen). When a number equal to or greater than
16 is specified, the specification of 15 is assumed.
Example)
When the tone level of a color is: red:1 green:2, blue:3, set 10203
in the parameter.
10800 First compensation axis for three-dimensional error compensation
10801 Second compensation axis for three-dimensional error compensation
10802 Third compensation axis for three-dimensional error compensation
NOTE
When these parameters are set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to Number of controlled axes
These parameters set three compensation axes for applying
three-dimensional error compensation.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2191 -
10803 Number of compensation points for three-dimensional error compensation
(first compensation axis)
10804 Number of compensation points for three-dimensional error compensation
(second compensation axis)
10805 Number of compensation points for three-dimensional error compensation
(third compensation axis)
NOTE
When these parameters are set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 2 to 25
These parameters set the number of compensation points for each axis
for three-dimensional error compensation.
10806 Compensation point number of the reference position for three-dimensional
error compensation (first compensation axis)
10807 Compensation point number of the reference position for three-dimensional
error compensation (second compensation axis)
10808 Compensation point number of the reference position for three-dimensional
error compensation (third compensation axis)
NOTE
When these parameters are set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to number of compensation points
These parameters set the compensation point number of the reference
position for each axis for three-dimensional error compensation.
A.PARAMETERS APPENDIX B-63944EN/03
- 2192 -
10809 Magnification for three-dimensional error compensation (first compensation
axis)
10810 Magnification for three-dimensional error compensation (second
compensation axis)
10811 Magnification for three-dimensional error compensation (third compensation
axis)
NOTE
When these parameters are set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to 100
These parameters set the magnification for each axis for
three-dimensional error compensation.
10812 Compensation interval for three-dimensional error compensation (first
compensation axis)
10813 Compensation interval for three-dimensional error compensation (second
compensation axis)
10814 Compensation interval for three-dimensional error compensation (third
compensation axis)
NOTE
When these parameters are set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm, inch (machine unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
These parameters set the compensation interval for each axis for
three-dimensional error compensation.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2193 -
#7 #6 #5 #4 #3 #2 #1 #0
11005 SIC
[Input type] Parameter input
[Data type] Bit
# 0 SIC Spindle indexing is:
0: Performed based on absolute coordinates.
1: Performed based on machine coordinates.
11090 Path number with which the rotation of each spindle is specified
[Input type] Parameter input
[Data type] Byte spindle
[Valid data range] 0 to 10
When a path is specified for spindle commands, this parameter sets a
path number with which the rotation of a spindle can be specified.
0: Spindle commands can be issued from all paths.
1 to 10: Spindle commands can be issued from a set path.
NOTE
1 This parameter is valid when SPSP<Gn536.7> is
set to 1.
2 If the setting is illegal, an alarm (PS5305) is issued
when a spindle command is issued from any one of
the paths.
3 This setting does not apply to spindle commands
using the spindle select signals (SWS1 to
SWS4<Gn027.0 to .2, Gn026.3>).
#7 #6 #5 #4 #3 #2 #1 #0
11200 RCM
[Input type] Setting input
[Data type] Bit path
# 0 RCM When workpiece setting error compensation is performed with a
5-axis machine, tool direction compensation (compensation for a
rotation axis) is:
0: Not performed.
1: Performed.
NOTE
When this parameter is set to 0, machining cannot
be performed precisely. For 5-axis machines,
usually set this parameter to 1.
A.PARAMETERS APPENDIX B-63944EN/03
- 2194 -
11201 The number of decimal places of rotation direction errors in workpiece
setting error compensation
[Input type] Setting input
[Data type] Byte path
[Valid data range] 0 to 8
This parameter sets the number of decimal places of rotation direction
errors in workpiece setting error compensation.
Parameter No. 11201 1 2 3 4
Least input increment (deg) 0.1 0.01 0.001 0.0001
Maximum settable value (deg) ±99,999,999.9 ±9999,999.99 ±999,999.999 ±99,999.9999
Parameter No. 11201 5 6 7 8
Least input increment (deg) 0.00001 0.000001 0.0000001 0.00000001
Maximum settable value (deg) ±9,999.99999 ±999.999999 ±99.9999999 ±9.99999999
Note, however, that a value from 1 to 8 can be specified in this
parameter.
If a value not within the specifiable range is specified in this
parameter, the least input increment of the reference axis is followed.
Unit system of
reference axis IS-A IS-B IS-C IS-D IS-E
Least input
increment (deg) 0.01 0.001 0.0001 0.00001 0.000001
Maximum settable
value (deg)
±999,999.99 ±999,999.999 ±99,999.9999 ±9,999.99999 ±999.999999
11202 Override for maximum cutting feedrate during workpiece setting error
compensation mode
[Input type] Parameter input
[Data type] Byte path
[Unit of data] %
[Valid data range] 0 to 100
When the parameter RCM(No.11200#0)=1 in order to enable tool
direction compensation, during workpiece setting error compensation
or during tool center point control with three-dimensional coordinate
conversion or with tilted working plane command, the override for
maximum cutting feedrate (Parameter No.1432) is set.
This override is done only to rotary axes.
In the case of 0 of this parameter, the override is regarded as 100%.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2195 -
11203 Override for rapid traverse during workpiece setting error compensation
mode
[Input type] Parameter input
[Data type] Byte path
[Unit of data] %
[Valid data range] 0 to 100
When the parameter RCM (No.11200#0)=1 in order to enable tool
direction compensation, during workpiece setting error compensation
or during tool center point control with three-dimensional coordinate
conversion or with tilted working plane command, the override for
rapid traverse (Parameter No.1420) is set.
This override is done only to rotary axes.
In the case of 0 of this parameter, the override is regarded as 100%.
11204 Angle to decide singular posture (for Workpiece setting error compensation)
[Input type] Parameter input
[Data type] Real path
[Unit of data] Degree
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A)
(When the increment system is IS-B, -999999.999 to +999999.999)
When Tool direction is compensated(Parameter
RCM(No.11200#0)=1), in the case that Tool center point control is
active during Workpiece setting error compensation, 3-dimension
coordinates system conversion or Tilted working plane command,
rotary axes are compensated. Then, compensation may be different
when the tool is in singular posture.
When the angle between the tool posture and the singular posture is
less than this parameter, the compensation is done regarding tool
posture as singular posture.
11220 Minimum distance used for determining a plane when a tilted working plane
command with three points is specified
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm, inch (input unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 0 or positive 9 digit of minimum unit of data (refer to the standard
parameter setting table (B))
(When the increment system is IS-B, 0.0 to +999999.999）
When a tilted working plane command with three points is specified,
if the distance (used for determining a place) between a straight line
passing two points and the remaining one point is short, the plane is
unstable. In this parameter, set the minimum distance used for
determining a plane. If the distance is shorter than the value set in this
parameter, an alarm (PS5457) is issued.
A.PARAMETERS APPENDIX B-63944EN/03
- 2196 -
#7 #6 #5 #4 #3 #2 #1 #0
11221 MTW
[Input type] Parameter input
[Data type] Bit path
# 0 MTW Multiple tilted working plane commands are:
0: Not used.
1: Used.
#7 #6 #5 #4 #3 #2 #1 #0
11222 PDM CIM NIM
[Input type] Parameter input
[Data type] Bit path
# 0 NIM Automatic conversion of a coordinate system by an inch/metric
conversion command (G20 or G21) is:
0: Not performed.
1: Performed.
# 1 CIM When an inch/metric conversion command (G20 or G21) is specified,
if the workpiece coordinate system is shifted by the shift amount as
described below:
0: An alarm (PS1298) is issued.
1: Clearing is performed.
If bit 0 (NIM) of parameter No. 11222 is set to 1, or if bit 2 (IRF) of
parameter No. 14000 is set to 1, this parameter clears the following:
• Manual intervention made when the manual absolute signal is off
• Issuance of a move command with the machine locked
• Movement by handle interrupt
• Operation with a mirror image
• Shifting of a workpiece coordinate system when a local
coordinate system or workpiece coordinate system is set up
# 7 PDM When switching between diameter and radius specification is made
with the function for dynamic switching of diameter/radius
specification, coordinates in the machine coordinate system select
command (G53) are:
0: Switched between diameter and radius specification.
1: Set according to the setting of bit 3 (DIAx) of parameter No.
1006.
#7 #6 #5 #4 #3 #2 #1 #0
11240 FAE
[Input type] Parameter input
[Data type] Bit path
# 0 FAE During positioning when the AI contour control mode is canceled, the
optimum torque acceleration/deceleration is:
0: Disabled.
1: Enabled.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2197 -
11261 The amount of a retract operation in the tool axis direction during tool retract
and return
[Input type] Setting input
[Data type] Real axis
[Unit of data] mm, inch, degree (input unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999）
This parameter sets the amount of a retract operation in the tool axis
direction when G10.6 is specified alone during tool retraction and
return (during tool center point control and workpiece setting error
compensation). The retract operation is performed by using the value
set in this parameter in an incremental manner. This data is valid only
when bit 2 (RPS) of parameter No. 7040 is set to 1. If 0 is set in this
parameter, a retract operation in the tool axis direction is not
performed, but a retract operation is performed according to the
setting of parameter No. 7041.
#7 #6 #5 #4 #3 #2 #1 #0
11304 GGD
[Input type] Parameter input
[Data type] Bit
NOTE
When this parameter is set, the power must be
turned off before operation is continued..
# 1 GGD The G code guidance screen is:
0: Not displayed.
1: Displayed.
11305 Maximum number of simultaneously displayed axes
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to 2
By setting this parameter, the maximum number of simultaneously
displayed axes at the current position can be changed. A value set in
this parameter corresponds to the maximum number of simultaneously
displayed axis as follows:
Max. number of simultaneously displayed axes 5 10 20
Setting 0 1 2
A value other than 1 and 2 is assumed to be 0.
A.PARAMETERS APPENDIX B-63944EN/03
- 2198 -
11307 Display sequence of the coordinates in current position display
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to 5
This parameter sets the display sequence of the coordinates of a
position displayed on the following screens:
10.4- and 15-inch display units
• Total position display screen
• Total position display on each screen
7.2- and 8.4-inch display units
• Total position display screen
When the maximum number of simultaneously displayed axes is set
to 20 (when 2 is set in parameter No. 11305), two sets of coordinates
are displayed simultaneously as the current position display on each
screen.
When the first set is displayed, switching to the second set can be
made by pressing then pressing the chapter selection soft key
being selected.
When the above operation is performed again, the displayed set
changes to the first set.
The display sequence of coordinates corresponds to the parameter
setting as follows:
Display sequence of
coordinates
Setting
1 2 3 4
0 Relative
coordinates
Absolute
coordinates
Machine
coordinates
Remaining travel
distance
1 Relative
coordinates
Machine
coordinates
Absolute
coordinates
Remaining travel
distance
2 Relative
coordinates
Remaining travel
distance
Absolute
coordinates
Machine
coordinates
3 Absolute
coordinates
Machine
coordinates
Relative
coordinates
Remaining travel
distance
4 Absolute
coordinates
Remaining travel
distance
Relative
coordinates
Machine
coordinates
5 Machine
coordinates
Remaining travel
distance
Relative
coordinates
Absolute
coordinates
If the setting is beyond the valid data range, 0 is assumed.
When the multipath simultaneous display function is enabled
(parameter No. 13131 is set to a nonzero value, and parameter No.
13132 is set to 1 or a greater value), this parameter becomes invalid.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2199 -
#7 #6 #5 #4 #3 #2 #1 #0
11308 COW
[Input type] parameter input
[Data type] Bit
#1 COW When the file of specified name already exists on memory card,
0: It is not overwritten
Alarm (SR1973 FILE ALREADY EXIST) is generated.
1: It is overwritten.
Because the confirmation message is displayed before
overwriting even if COW is 1, overwriting can be canceled.
NOTE
When the overwritten file is read only attribute, it is
not possible to overwrite even if parameter COW
(No.11308#1)=1.
#7 #6 #5 #4 #3 #2 #1 #0
11329 GST BGM
[Input type] Parameter input
[Data type] Bit path
#3 BGM Coordinates used by the dynamic graphic display function are:
0: Absolute coordinates.
1: Machine coordinates.
#7 GST When drawing cannot be performed for a command with the dynamic
graphic display function:
0: The command is ignored, and drawing continues without
stopping drawing.
1: Drawing stops.
11343 Blank figure in dynamic graphic display
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to 1
This parameter sets the type of a blank figure in dynamic graphic
display.
Setting Figure
0 Cylinder or hollow cylinder (parallel to the Z-axis)
1 Rectangular parallelepiped
A.PARAMETERS APPENDIX B-63944EN/03
- 2200 -
11344 Blank reference position in dynamic graphic display
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm,inch (input unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999）
This parameter sets the reference position of a blank in the dynamic
graphic display function by using coordinate values in the workpiece
coordinate system.
NOTE
If bit 3 (BGM) of parameter No. 11329 is set to 1,
set coordinate values in the machine coordinate
system.
11345 Blank dimension I in dynamic graphic display
11346 Blank dimension J in dynamic graphic display
11347 Blank dimension K in dynamic graphic display
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm,inch (input unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 0 or positive 9 digit of minimum unit of data (refer to the standard
parameter setting table (B))
(When the increment system is IS-B, 0.000 to +999999.999）
These parameters set the dimensions of a blank in the dynamic graphic
display function according to the blank figure as follows:
Blank type Dimension I Dimension Ｊ Dimension Ｋ
Cylinder Column diameter 0 Column length
Hollow
cylinder
Diameter of outer
circle of cylinder
Diameter of inner
circle of cylinder
Cylinder length
Rectangular
prism
Length in X-axis
direction
Length in Y-axis
direction
Length in Z-axis
direction
B-63944EN/03 APPENDIX A.PARAMETERS
- 2201 -
#7 #6 #5 #4 #3 #2 #1 #0
11349 WNS ABC
[Input type] Parameter input
[Data type] Bit
# 1 ABC In animated simulation in the dynamic graphic display function, when
a fine boring cycle or back boring cycle, which is a hole machining
canned cycle, is performed, the movement for a shift at the hole
bottom is:
0: Not drawn.
1: Drawn.
# 3 WNS In the dynamic graphic display function, P-CODE workpiece number
search is:
0: Disabled.
1: Enabled.
NOTE
A macro executor option, or a macro executor and C
executor options are required.
#7 #6 #5 #4 #3 #2 #1 #0
11353 SEK
[Input type] Parameter input
[Data type] Bit
#0 SEK When the power is turned on, or when the clear state is present,
sequence numbers are:
0: Not maintained.
1: Maintained.
NOTE
During a subprogram call, the sequence number of
the subprogram is maintained.
#7 #6 #5 #4 #3 #2 #1 #0
11630 FRD
[Data type] Bit path
# 0 FRD The minimum command unit of the rotation angles of coordinate
rotation and three-dimensional coordinate system conversion is:
0: 0.001 degree.
1: 0.00001 degree. (1/100,000)
A.PARAMETERS APPENDIX B-63944EN/03
- 2202 -
12310
States of the manual handle feed axis selection signals when tool axis
direction handle feed/interrupt and table-based vertical direction handle
feed/interrupt are performed
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to 24
This parameter sets the states of the manual handle feed axis selection
signal (HS1A to HS1E for the first manual handle) or the manual
handle interrupt axis selection signal (HS1IA to HS1IE for the first
manual handle) to perform tool axis direction handle feed/interrupt
and table-based vertical direction handle feed/interrupt.
The handle for which the signal states are set is determined by
parameter No. 12323.
<Table of correspondence with the manual handle feed axis
selection signals>
If parameter No. 12323 is set to 1, the states of the manual handle feed
axis selection signals or manual handle interrupt axis selection signals
for the first manual handle in the three-dimensional manual feed
(handle feed) mode and corresponding parameter settings are listed in
the table below. When the first manual handle pulse generator is
turned after setting the signals corresponding to the value set in the
parameter, operation is performed in the specified mode.
HS1E
(HS1IE)
HS1D
(HS1ID)
HS1C
(HS1IC)
HS1B
(HS1IB)
HS1A
(HS1IA)
Parameter
(No.12310)
0 0 0 0 1 1
0 0 0 1 0 2
0 0 0 1 1 3
0 0 1 0 0 4
0 0 1 0 1 5
0 0 1 1 0 6
0 0 1 1 1 7
0 1 0 0 0 8
0 1 0 0 1 9
0 1 0 1 0 10
0 1 0 1 1 11
0 1 1 0 0 12
0 1 1 0 1 13
0 1 1 1 0 14
0 1 1 1 1 15
1 0 0 0 0 16
1 0 0 0 1 17
1 0 0 1 0 18
1 0 0 1 1 19
1 0 1 0 0 20
1 0 1 0 1 21
1 0 1 1 0 22
1 0 1 1 1 23
1 1 0 0 0 24
If parameter No. 12323 is set to 2 to 5, replace "1" in HS1A to HS1E
and HS1IA to HS1IE above with 2 to 5.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2203 -
12311
States of the manual handle feed axis selection signals when a movement is
made in the first axis direction in tool axis normal direction handle
feed/interrupt and table-based horizontal direction handle feed/interrupt
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to 24
This parameter sets the states of the manual handle feed axis selection
signals (HS1A to HS1E for the first manual handle) or the manual
handle interrupt axis selection signal (HS1IA to HS1IE for the first
manual handle) when a movement is made in the first axis direction.
(For settings, see "Table of correspondence with the manual handle
feed axis selection signals" in the description of parameter No.
12310.)
The handle for which the signal states are set is determined by
parameter No. 12323.
The table below indicates the relationships of tool axis directions, first
axis directions, and second axis directions.
Parameter
No.19697
Tool axis
directions
First axis
directions
Second axis
directions
1 X Y Z
2 Y Z X
3 Z X Y
Note, however, that the table above indicates the directions applicable
when the angles of all rotation axes are set to 0.
In tool axis direction/tool axis normal direction feed (not table-based),
the directions indicated above assume that 0 is set in parameter No.
19698 and No. 19699. When a rotation axis has made a turn or a
nonzero value is set in these parameters in tool axis direction/tool axis
normal direction feed, the relevant directions are inclined accordingly.
12312
States of the manual handle feed axis selection signals when a movement is
made in the second axis direction in tool axis normal direction handle
feed/interrupt and table-based horizontal direction handle feed/interrupt
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to 24
This parameter sets the states of the manual handle feed axis selection
signals (HS1A to HS1E for the first manual handle) or the manual
handle interrupt axis selection signals (HS1IA to HS1IE for the first
manual handle) when a movement is made in the second axis direction.
(For settings, see "Table of correspondence with the manual handle
feed axis selection signals" in the description of parameter No.
12310.)
The handle for which the signal states are set is determined by
parameter No. 12323.
A.PARAMETERS APPENDIX B-63944EN/03
- 2204 -
12313 States of the manual handle feed axis selection signals when the first
rotation axis is turned in tool tip center rotation handle feed/interrupt
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to 24
This parameter sets the states of the manual handle feed axis selection
signals (HS1A to HS1E for the first manual handle) or the manual
handle interrupt axis selection signals (HS1IA to HS1IE for the first
manual handle) when the first rotation axis is turned in tool tip center
rotation handle feed or interrupt. (For settings, see "Table of
correspondence with the manual handle feed axis selection signals" in
the description of parameter No. 12310.)
The handle for which the signal states are set is determined by
parameter No. 12323.
12314 States of the manual handle feed axis selection signals when the second
rotation axis is turned in tool tip center rotation handle feed/interrupt
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 1 to 24
This parameter sets the states of the manual handle feed axis selection
signals (HS1A to HS1E for the first manual handle) or the manual
handle interrupt axis selection signals (HS1IA to HS1IE for the first
manual handle) when the second rotation axis is turned in tool tip
center rotation handle feed or interrupt. (For settings, see "Table of
correspondence with the manual handle feed axis selection signals" in
the description of parameter No. 12310.)
The handle for which the signal states are set is determined by
parameter No. 12323.
12318 Tool length in three-dimensional machining manual feed
[Input type] Setting input
[Data type] Real path
[Unit of data] mm, inch (machine unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
This parameter sets a tool length when tool tip center rotation feed is
performed with the three-dimensional machining manual feed function
and when the three-dimensional machining manual feed screen is
displayed.
NOTE
Specify a radius value to set this parameter.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2205 -
#7 #6 #5 #4 #3 #2 #1 #0
12320 JFR FLL TWD
[Input type] Parameter input
[Data type] Bit path
# 0 TWD The directions of three-dimensional machining manual feed (other
than tool tip center rotation feed) when the tilted working plane
command is issued are:
0: Same as those not in the tilted working plane command. That is,
the directions are:
Tool axis normal direction 1 (table-based horizontal direction 1)
Tool axis normal direction 2 (table-based horizontal direction 2)
Tool axis direction (table-based vertical direction)
1: X, Y, and Z directions in the feature coordinate system.
# 1 FLL The directions of tool axis normal direction feed or table-based
horizontal direction feed in the three-dimensional machining manual
feed mode are:
0: Tool axis normal direction 1 (table-based horizontal direction 1) and
tool axis normal direction 2 (table-based horizontal direction 2).
1: Longitude direction and latitude direction.
Parameter FLL
(No.12320#1)
Parameter TWD
(No.12320#0) Directions of three-dimensional machining manual feed
0 0 Conventional directions
0 1
When the tilted working plane command is issued: X, Y, and Z
directions in the feature coordinate system
When the command is not issued: Conventional directions
1 0 Longitude direction and latitude direction
1 1
When the tilted working plane command is issued: X, Y, and Z
directions in the feature coordinate system
When the command is not issued: Longitude direction and
latitude direction
# 2 JFR As the feeedrate of three-dimensional machining manual feed (jog
feed or incremental feed) :
0: The dry run rate (parameter No. 1410) is used.
1: The jog feedrate (parameter No. 1423) is used.
12321 Normal axis direction
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to 3
When a tilted working plane command (G68.3) is issued to perform
three-dimensional machining manual feed in the latitude direction,
longitude direction, and tool axis direction, this parameter sets an axis
parallel to the normal direction.
1 : Positive (+) X-axis direction
2 : Positive (+) Y-axis direction
3 : Positive (+) Z-axis direction
0 : Reference tool axis direction (parameter No. 19697)
A.PARAMETERS APPENDIX B-63944EN/03
- 2206 -
12322 Angle used to determine whether to assume the tool axis direction to be
parallel to the normal direction (parameter No. 12321)
[Input type] Parameter input
[Data type] Real path
[Unit of data] deg
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 0 to 90
When a tilted working plane command (G68.3) is issued to perform
three-dimensional machining manual feed in the latitude direction,
longitude direction, and tool axis direction, if the angle between the
tool axis direction and normal direction (parameter No. 12321) is too
small, the tool axis direction is assumed to be parallel to the normal
direction (parameter No. 12321). This parameter sets the maximum
angle at which the tool axis direction is assumed to be parallel to the
normal direction.
When this parameter is set to 0 or a value outside the valid range, it is
set to 1 degree.
12323 Number of a manual handle used for three-dimensional machining manual
feed
[Input type] Setting input
[Data type] Byte path
[Valid data range] 0 to 5
When three-dimensional machining manual feed (handle feed) is
performed, set the number of the manual handle to be used.
When the second or third manual handle is used for three-dimensional
machining manual feed, the option for manual handle feed with 2/3
handles is required.
When the fourth or fifth manual handle is used for three-dimensional
machining manual feed, the option for manual handle feed with 4/5
handles is required.
If 0 or the number of an unavailable handle is set, the first handle is
assumed.
12600 Identification Number for synchronous, composite and superimposed
control with program command
[Input type] Parameter input
[Data type] Word axis
[Valid data range] 0,1 to 32767
Set identification numbers that can be specified with P,Q addresses.
The axis whose identification number is "0" cannot become under
synchronous /composite /superimposed control by CNC program.
The same identification number cannot be set to two or more axes
through all paths.
When the same identification number is set, PS alarm (PS5339) occurs
at G50.4/G50.5/G50.6/G51.4/G51.5/G51.6 block.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2207 -
#7 #6 #5 #4 #3 #2 #1 #0
13113 CFD CLR
[Input type] Parameter input
[Data type] Bit path
# 0 CLR Upon reset, the display of a travel distance by three-dimensional
machining manual feed is:
0: Not cleared.
1: Cleared.
# 3 CFD As feedrate F, the three-dimensional machining manual feed screen
displays:
0: Composite feedrate at the linear axis/rotation axis control point.
1: Feedrate at the tool tip.
#7 #6 #5 #4 #3 #2 #1 #0
13200 ETE TRT
[Input type] Parameter input
[Data type] Bit path
# 2 TRT As the remaining lifetime value for outputting the tool life arrival
notice signal:
0: The remaining lifetime of the last tool is used.
1: The sum of the remaining lifetimes of the tools with the same
type number is used.
NOTE
This parameter is valid when bit 3 (ETE) of
parameter No. 13200 is set to 0 (arrival notice for
each type number).
# 3 ETE The tool life arrival notice signal is output:
0: For each tool type.
1: For each tool.
A.PARAMETERS APPENDIX B-63944EN/03
- 2208 -
#7 #6 #5 #4 #3 #2 #1 #0
13201 TDN TDC
[Input type] Parameter input
[Data type] Bit
NOTE
When at least one of these parameters is set, the
power must be turned off before operation is
continued.
# 0 TDC The function of customizing the tool management data screen of the
tool management function is:
0: Disabled.
1: Enabled.
# 1 TDN On the tool management function screen, the character string for
indicating the tool life status can contain:
0: Up to 6 characters.
1: Up to 12 characters.
#7 #6 #5 #4 #3 #2 #1 #0
13202 DOM DOT DO2 DOB DOY DCR
[Input type] Parameter input
[Data type] Bit
# 1 DCR On the tool management function screen, tool nose radius
compensation data is:
0: Displayed.
1: Not displayed.
NOTE
This parameter is valid when the machine control
type is the lathe system or compound system.
# 2 DOY On the tool management function screen, Y-axis offset data is:
0: Displayed.
1: Not displayed.
NOTE
This parameter is valid when the machine control
type is the lathe system or compound system.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2209 -
# 3 DOB On the tool management function screen, B-axis offset data is:
0: Displayed.
1: Not displayed.
NOTE
This parameter is valid when the machine control
type is the lathe system or compound system.
# 4 DO2 On the tool management function screen, the second geometry tool
offset data is:
0: Displayed.
1: Not displayed.
NOTE
This parameter is valid when the machine control
type is the lathe system or compound system.
# 6 DOT On the tool management function screen, the tool offset data (X, Z) of
the T series is:
0: Displayed.
1: Not displayed.
NOTE
This parameter is valid when the machine control
type is the lathe system or compound system.
# 7 DOM On the tool management function screen, the tool offset data of the M
series is:
0: Displayed.
1: Not displayed.
NOTE
This parameter is valid when the machine control
type is the machining center system or compound
system.
#7 #6 #5 #4 #3 #2 #1 #0
13204 TDL
[Input type] Parameter input
[Data type] Bit
# 0 TDL The protection function for tool management data using a key is:
0: Disabled.
1: Enabled.
A.PARAMETERS APPENDIX B-63944EN/03
- 2210 -
13220 Number of valid tools in tool management data
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Word
[Valid data range] 0 to 64 (Extended to 240 or 1000 by the addition of an option)
This parameter sets the number of valid tools in tool management
data.
13221 M code for tool life count restart
[Input type] Parameter input
[Data type] Word path
[Valid data range] 0 to 65535
When 0 is set in this parameter, this parameter is ignored.
When an M code for tool life count restart is specified, the counting of
the life of the tool attached at the spindle position is started. When the
type for counting the number of use times is selected, the target of life
counting is switched to the tool attached at the spindle position, and
the life count is incremented by 1.
When the type for counting time is selected, the target of life counting
is switched to the tool attached at the spindle position but no other
operations are performed. If the tool attached at the spindle position is
not a tool under tool life management, no operation is performed.
The M code set in parameter No. 6811 waits for FIN. However, the M
code set in this parameter does not wait for FIN.
The M code set in parameter No. 13221 must not be specified in a
block where another auxiliary function is specified.
The M code set in parameter No. 13221 does not wait for FIN. So, do
not use the M code for other purposes.
NOTE
The use of this parameter varies depending on
whether it is used by the tool management function
or tool life management function.
13222 Number of data items in the first cartridge
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Word
[Valid data range] 1 to 64 (Extended to 240 or 1000 by the addition of an option)
This parameter sets the number of data items used with the first
cartridge.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2211 -
13223 Start pot number of the first cartridge
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Word
[Valid data range] 1 to 9999
This parameter sets the start pot number to be used with the first
cartridge. Pot numbers starting with the value set in this parameter and
sequentially incremented by 1 are assigned to all data items.
13227 Number of data items in the second cartridge
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Word
[Valid data range] 1 to 64(Extended to 240 or 1000 by the addition of an option)
This parameter sets the number of data items used with the second
cartridge.
13228 Start pot number of the second cartridge
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Word
[Valid data range] 1 to 9999
This parameter sets the start pot number to be used with the second
cartridge. Pot numbers starting with the value set in this parameter and
sequentially incremented by 1 are assigned to all data items.
13232 Number of data items in the third cartridge
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Word
[Valid data range] 1 to 64(Extended to 240 or 1000 by the addition of an option)
This parameter sets the number of data items used with the third
cartridge.
A.PARAMETERS APPENDIX B-63944EN/03
- 2212 -
13233 Start pot number of the third cartridge
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Word
[Valid data range] 1 to 9999
This parameter sets the start pot number to be used with the third
cartridge. Pot numbers starting with the value set in this parameter and
sequentially incremented by 1 are assigned to all data items.
13237 Number of data items in the fourth cartridge
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Word
[Valid data range] 1 to 64(Extended to 240 or 1000 by the addition of an option)
This parameter sets the number of data items used with the fourth
cartridge.
13238 Start pot number of the fourth cartridge
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Word
[Valid data range] 1 to 9999
This parameter sets the start pot number to be used with the fourth
cartridge. Pot numbers starting with the value set in this parameter and
sequentially incremented by 1 are assigned to all data items.
13252 M code for specifying a particular tool
[Input type] Parameter input
[Data type] Word path
[Valid data range] 0 to 65535
This parameter sets not a tool type number but an M code for directly
specifying the T code of a particular tool.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2213 -
13265
Number for selecting a spindle position offset number with tool life or
H code for using the tool length offset in tool life management with tool life
management
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 0 to 999
• With tool management functions
This parameters sets an H/D code for selecting an offset number
registered in the data of the tool attached at the spindle position.
When 0 is set, an ordinary used code such as H99/D99 is used.
When a value other than 0 is set, H99/D99 no longer has a
particular meaning. So, when H99/D99 is specified in this case,
the specification of offset number 99 is assumed.
With the T series, address D only is used to specify a tool
number and offset number, so that a restriction is imposed on the
number of digits. So, the valid data range of this parameter varies
according the number of digits of an offset number.
When the number of digits of an offset number is 1: to 9
When the number of digits of an offset number is 2: to 99
When the number of digits of an offset number is 3: to 999
• With tool life management functions
Usually, when H99 is specified, tool length offset is enabled by
the H code of the tool being used. By setting any H code in this
parameter, the H code instead of H99 can be used. If 0 is
specified, H99 is assumed.
A value ranging from 0 to 9999 can be set.
13266 D code for enabling cutter compensation in tool life management
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 0 to 9999
Usually in tool life management, specifying D99 allows the D code of
the tool being used to enable cutter compensation. By setting any D
code in this parameter, the D code instead of D99 can be used. If 0 is
set, D99 is assumed.
A value ranging from 0 to 9999 can be set.
#7 #6 #5 #4 #3 #2 #1 #0
13451 ATW
[Input type] Parameter input
[Data type] Bit path
# 1 ATW When I, J, and K are all set to 0 in a block that specifies a feature
coordinate system setup command (G68.2), which is a tilted working
plane command:
0: An alarm (PS5457) is issued.
1: A feature coordinate system with a tilted plane angle of 0 degrees
is assumed for operation.
A.PARAMETERS APPENDIX B-63944EN/03
- 2214 -
#7 #6 #5 #4 #3 #2 #1 #0
13600 MSA MCR
[Input type] Parameter input
[Data type] Bit path
# 0 MCR When an allowable acceleration rate adjustment is made with the
machining condition selection function (machining parameter
adjustment screen, precision level selection screen), parameter No.
1735 for the deceleration function based on acceleration in circular
interpolation is:
0: Modified.
1: Not modified.
# 7 MSA When the machining condition selection function is used, the
acceleration rate change time (bell-shaped) (LV1, LV10) is:
0: Set using parameter Nos. 13612 and 13613.
1: Set using parameter Nos. 13662 and 13663.
#7 #6 #5 #4 #3 #2 #1 #0
13601 MPR
[Input type] Parameter input
[Data type] Bit
NOTE
When this parameter is set, the power must be
turned off before operation is continued.
# 0 MPR The machining parameter adjustment screen is:
0: Displayed.
1: Not displayed.
Even when this parameter is set to 1, the precision level selection
screen is displayed.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2215 -
13610 Acceleration rate for acceleration/deceleration before look-ahead
interpolation in AI contour control (precision level 1)
13611 Acceleration rate for acceleration/deceleration before look-ahead
interpolation in AI contour control (precision level 10)
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/sec/sec, inch/sec/sec, degree/sec/sec (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (D)
(When the machine system is metric system, 0.0 to +100000.0. When
the machine system is inch system, machine, 0.0 to +10000.0)
Each of these parameters sets an acceleration rate for acceleration/
deceleration before interpolation in AI contour control. Set a value
(precision level 1) with emphasis placed on speed, and a value
(precision level 10) with emphasis on precision.
13612 Acceleration rate change time (bell-shaped) when AI contour control is used
(precision level 1)
13613 Acceleration rate change time (bell-shaped) when AI contour control is used
(precision level 10)
[Input type] Parameter input
[Data type] Byte path
[Unit of data] msec
[Valid data range] 0 to 127
Each of these parameters sets an acceleration rate change time
(bell-shaped) in AI contour control. Set a value (precision level 1)
with emphasis placed on speed, and a value (precision level 10) with
emphasis on precision.
A.PARAMETERS APPENDIX B-63944EN/03
- 2216 -
13614
Allowable acceleration rate change amount for each axis in speed control
based on acceleration rate change under control on the rate of change of
acceleration (precision level 1)
13615
Allowable acceleration rate change amount for each axis in speed control
based on acceleration rate change under control on the rate of change of
acceleration (precision level 10)
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/sec/sec, inch/sec/sec, degree/sec/sec (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (D)
(When the machine system is metric system, 0.0 to +100000.0. When
the machine system is inch system, machine, 0.0 to +10000.0)
Each of these parameters sets an allowable acceleration rate change
amount per 1 ms for each axis in speed control based on acceleration
rate change under control on the rate of change of acceleration during
AI contour control.
Set a value (precision level 1) with emphasis placed on speed, and a
value (precision level 10) with emphasis on precision.
13616
Allowable acceleration rate change amount for each axis in speed control
based on acceleration rate change under control on the rate of change of
acceleration in successive linear interpolation operations (precision level 1)
13617
Allowable acceleration rate change amount for each axis in speed control
based on acceleration rate change under control on the rate of change of
acceleration in successive linear interpolation operations (precision level 10)
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/sec/sec, inch/sec/sec, degree/sec/sec (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (D)
(When the machine system is metric system, 0.0 to +100000.0. When
the machine system is inch system, machine, 0.0 to +10000.0)
Each of these parameters sets an allowable acceleration rate change
amount per 1 ms for each axis in speed control based on acceleration
rate change under control on the rate of change of acceleration in
successive linear interpolation operations during AI contour control.
Set a value (precision level 1) with emphasis placed on speed, and a
value (precision level 10) with emphasis on precision.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2217 -
NOTE
1 For an axis with 0 set in this parameter, parameter
No. 13614 and No. 13615 (allowable acceleration
rate change amount in speed control based on
acceleration rate change under control on the rate
of change of acceleration) are valid.
2 For an axis with 0 set in parameter No. 13614 and
No. 13615 (allowable acceleration rate change
amount in speed control based on acceleration rate
change under control on the rate of change of
acceleration), speed control based on acceleration
rate change is disabled, so that the specification of
this parameter has no effect.
13618
Rate of change time of the rate of change of acceleration in smooth
bell-shaped acceleration/deceleration before interpolation when AI contour
control is used (precision level 1)
13619
Rate of change time of the rate of change of acceleration in smooth
bell-shaped acceleration/deceleration before interpolation when AI contour
control is used (precision level 10)
[Input type] Parameter input
[Data type] Byte path
[Unit of data] %
[Valid data range] 0 to 50
Each of these parameters sets the rate (percentage) of the change time
of the rate of change of acceleration to the change time of acceleration
rate change in smooth bell-shaped acceleration/deceleration before
look-ahead interpolation during AI contour control.
Set a value (precision level 1) with emphasis placed on speed, and a
value (precision level 10) with emphasis on precision.
NOTE
When 0 or a value not within the valid data range is
set in this parameter, smooth bell-shaped
acceleration/deceleration before look-ahead
interpolation is not performed.
A.PARAMETERS APPENDIX B-63944EN/03
- 2218 -
13620 Allowable acceleration rate when AI contour control is used (precision level 1)
13621 Allowable acceleration rate when AI contour control is used (precision level 10)
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/sec/sec, inch/sec/sec, degree/sec/sec (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (D)
(When the machine system is metric system, 0.0 to +100000.0. When
the machine system is inch system, machine, 0.0 to +10000.0)
Each of these parameters sets an allowable acceleration rate in AI
contour control. Set a value (precision level 1) with emphasis placed
on speed, and a value (precision level 10) with emphasis on precision.
13622 Time constant for acceleration/deceleration after interpolation when AI
contour control is used (precision level 1)
13623 Time constant for acceleration/deceleration after interpolation when AI
contour control is used (precision level 10)
[Input type] Parameter input
[Data type] Word axis
[Unit of data] msec
[Valid data range] 1 to 512
Each of these parameters sets a time constant for acceleration/
deceleration after interpolation when AI contour control is used. Set a
value (precision level 1) with emphasis placed on speed, and a value
(precision level 10) with emphasis on precision.
13624 Corner speed difference when AI contour control is used (precision level 1)
13625 Corner speed difference when AI contour control is used (precision level 10)
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
Each of these parameters sets an allowable speed difference for speed
determination based on corner speed difference in AI contour control.
Set a value (precision level 1) with emphasis placed on speed, and a
value (precision level 10) with emphasis on precision.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2219 -
13626 Maximum cutting speed when AI contour control is used (precision level 1)
13627 Maximum cutting speed when AI contour control is used (precision level 10)
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm/min, inch/min, degree/min (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (C)
(When the increment system is IS-B, 0.0 to +999000.0)
Each of these parameters sets a maximum cutting speed in AI contour
control. Set a value (precision level 1) with emphasis placed on speed,
and a value (precision level 10) with emphasis on precision.
13628 Parameter number corresponding to arbitrary item 1 when AI contour control
is used
13629 Parameter number corresponding to arbitrary item 2 when AI contour control
is used
NOTE
When these parameters are set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] 2-word path
[Valid data range] 1 to 65535
These parameters set the parameter numbers corresponding to
arbitrary items 1 and 2.
NOTE
The parameter numbers corresponding to the
following cannot be specified:
• Bit parameters
• Spindle parameters (No. 4000 to No. 4799)
• Parameters of real number type
• Parameters that require power-off (for which the
alarm (PW0000) is issued)
• Nonexistent parameters
A.PARAMETERS APPENDIX B-63944EN/03
- 2220 -
13630 Value with emphasis on speed (precision level 1) of the parameter
corresponding to arbitrary item 1 when AI contour control is used
13631 Value with emphasis on speed (precision level 1) of the parameter
corresponding to arbitrary item 2 when AI contour control is used
13632 Value with emphasis on speed (precision level 10) of the parameter
corresponding to arbitrary item 1 when AI contour control is used
13633 Value with emphasis on speed (precision level 10) of the parameter
corresponding to arbitrary item 2 when AI contour control is used
[Input type] Parameter input
[Data type] 2-word axis
[Unit of data] Depend on the type of parameter for an arbitrary item
[Valid data range] Depend on the type of parameter for an arbitrary item
Each of these parameters sets a value with emphasis placed on speed
or precision for a parameter.
13662 Acceleration rate change time (bell-shaped) when AI contour control is used
(precision level 1), range extended
13663 Acceleration rate change time (bell-shaped) when AI contour control is used
(precision level 10), range extended
[Input type] Parameter input
[Data type] 2-word path
[Unit of data] msec
[Valid data range] 0 to 200
Each of these parameters sets an acceleration rate change time
(bell-shaped) in AI contour control. Set a value (precision 1) with
emphasis placed on speed, and a value (precision level 10) with
emphasis on precision.
#7 #6 #5 #4 #3 #2 #1 #0
14000 IRF
[Input type] Parameter input
[Data type] Bit axis
# 2 IRF An inch-metric switch command (G20, G21) at the reference position
is:
0: Disabled.
1: Enabled.
When this function is enabled for an axis, if an attempt to switch
between the inch and metric unit is made although the tool is not at the
reference position on that axis, an alarm (PS5362) is issued, and
switching between the inch and metric unit is canceled.
Be sure to move the tool to the reference position by, for example,
specifying G28 before switching between the inch and metric unit.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2221 -
14010 Maximum allowable travel distance when the reference position is
established for a linear scale with an absolute address reference position
[Input type] Parameter input
[Data type] 2-word axis
[Unit of data] Detection unit
[Valid data range] 0 to 99999999
This parameter sets the maximum allowable travel distance at the FL
feedrate when the reference position is established for a linear scale
with an absolute address reference position. When the travel distance
exceeds the setting of this parameter, the alarm (PS5326) (SCALE
WITH REFERENCE POSITION: REFERENCE POSITION
ESTABLISHMENT FAILED) is issued. When this parameter is set to
0, the maximum allowable travel distance is not checked.
14340 ATR value corresponding to slave 01 on FSSB line 1
14341 ATR value corresponding to slave 02 on FSSB line 1
:
14357 ATR value corresponding to slave 18 on FSSB line 1
NOTE
When these parameters are set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Byte
[Valid data range] 0 to 23, 64, -56, -96
Each of these parameters sets the value (ATR value) of the address
translation table corresponding to each of slave 1 to slave 18 on FSSB
line 1 (first optical connector).
The slave is a generic term for servo amplifiers and separate detector
interface units connected via an FSSB optical cable to the CNC.
Numbers 1 to 18 are assigned to slaves, with younger numbers
sequentially assigned to slaves closer to the CNC.
A 2-axis amplifier consists of two slaves, and a 3-axis amplifier
consists of three slaves. In each of these parameters, set a value as
described below, depending on whether the slave is an amplifier,
separate detector, or nonexistent.
• When the slave is an amplifier:
Set a value obtained by subtracting 1 from the setting of
parameter No. 1023 for the axis to which the amplifier is
assigned.
• When the slave is a separate detector interface unit:
Set 64 for the first separate detector interface unit (connected
near the CNC), and set -56 for the second separate detector
interface unit (connected far from the CNC).
• When the slave is nonexistent:
Set -96.
A.PARAMETERS APPENDIX B-63944EN/03
- 2222 -
NOTE
1 When the electric gear box (EGB) function is used
Although an amplifier is not actually required for an EGB dummy axis, set this
parameter with assuming that a dummy amplifier is connected. That is, as the
address conversion table value for a nonexistent slave, set the value obtained by
subtracting 1 from the setting of parameter No. 1023 for the EGB dummy axis,
instead of -96.
2 When the FSSB is set to the automatic setting mode (when the parameter FMD
(No.1902#0) is set to 0), parameter Nos. 14340 to 14357 are automatically set as
data is input on the FSSB setting screen. When the manual setting 2 mode is set
(when the parameter FMD (No.1902#0) is set to 1), be sure to directly set values in
parameter Nos. 14340 to 14357.
Example of axis configuration and parameter settings
- Example 1
10
21
32
43
54
664
75
8-56
9 to 18 -96
Slave
number
ATR
No.14340
to 14357
X
A
Y
Z
B
(M1)
C
(M2)
(None)
Axis
1 X 1
2 Y 3
3 Z 4
4 A 2
5 B 5
6 C 6
Controlled
axis
number
Program axis
name
No.1020
Servo axis
No.1023
CNC
Two-axis
amplifier
Single-axis
amplifier
M1
Two-axis
amplifier
Single-axis
amplifier
M2
M1/M2: First/second separate detector interface units
10
22
33
41
54
664
75
8-56
9 to 18 -96
Slave
number
X
Y
Z
A
B
(M1)
C
(M2)
(None)
Axis
1 X 1
2 Y 3
3 Z 4
4 A 2
5 B 5
6 C 6
Controlled
axis
number
Program axis
name
No.1020
Servo
axis
No.1023
CNC
Two-axis
amplifier
Single-axis
amplifier
M1
Two-axis
amplifier
Single-axis
amplifier
M2
ATR
No.14340
to 14357
B-63944EN/03 APPENDIX A.PARAMETERS
- 2223 -
- Example 2
Example of axis configuration and parameter settings when the
electronic gear box (EGB) function is used
(EGB slave axis: A-axis, EGB dummy axis: B-axis)
10
21
32
44
55
6 64
7 -56
83
Slave
number
ATR
No.14340
to 14357
X
Y
A
Z
C
(M1)
(M2)
B(Dummy)
Axis
1
X
1
2 Y 2
3 Z 5
4 A 3
5 B 4
6 C 6
Controlled
axis
number
Program axis
name
No.1020
Servo axis
No.1023
CNC
Two-axis
amplifier
Single-axis
amplifier
M1
Two-axis
amplifier
M2
9 -96
10 -96
(None)
(None)
M1/M2: First/second separate detector interface units
A.PARAMETERS APPENDIX B-63944EN/03
- 2224 -
14358 ATR value corresponding to slave 01 on FSSB line 2
14359 ATR value corresponding to slave 02 on FSSB line 2
:
14375 ATR value corresponding to slave 18 on FSSB line 2
NOTE
When these parameters are set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Byte
[Valid data range] 0 to 23, 80, -40, -96
Each of these parameters sets the value (ATR value) of the address
translation table corresponding to each of slave 1 to slave 18 on FSSB
line 2 (second optical connector).
• When the slave is an amplifier:
Set a value obtained by subtracting 1 from the setting of
parameter No. 1023 for the axis to which the amplifier is
assigned.
• When the slave is a separate detector interface unit:
Set 80 for the third separate detector interface unit (connected
near the CNC), and set -40 for the fourth separate detector
interface unit (connected far from the CNC).
• When the slave is nonexistent:
Set -96.
NOTE
1 Set these parameters only when a servo axis
control card with two optical connectors (FSSB
lines) is used.
2 When the FSSB is set to the automatic setting
mode (when the parameter FMD (No.1902#0) is
set to 0), parameter Nos. 14358 to 14375 are
automatically set as data is input on the FSSB
setting screen. When the manual setting 2 mode is
set (when the parameter FMD (No.1902#0) is set
to 1), be sure to directly set values in parameter
Nos. 14358 to 14375.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2225 -
14376 ATR value corresponding to connector 1 on the first separate detector
interface unit
14377 ATR value corresponding to connector 2 on the first separate detector
interface unit
:
14383 ATR value corresponding to connector 8 on the first separate detector
interface unit
14384 ATR value corresponding to connector 1 on the second separate detector
interface unit
:
14391 ATR value corresponding to connector 8 on the second separate detector
interface unit
14392 ATR value corresponding to connector 1 on the third separate detector
interface unit
:
14399 ATR value corresponding to connector 8 on the third separate detector
interface unit
14400 ATR value corresponding to connector 1 on the fourth separate detector
interface unit
:
14407 ATR value corresponding to connector 8 on the fourth separate detector
interface unit
NOTE
When these parameters are set, the power must be
turned off before operation is continued.
[Input type] Parameter input
[Data type] Byte
[Valid data range] 0 to 32
Each of these parameters sets the value (ATR value) of the address
translation table corresponding to each connector on a separate
detector interface unit.
The first and second separate detector interface units are connected to
FSSB line 1, and the third and fourth separate detector interface units
are connected to FSSB line 2.
In each of these parameters, set a value obtained by subtracting 1 from
the setting of parameter No. 1023 for the axis connected to a
connector on a separate detector interface unit.
When there are axes for which settings are made to use a separate
detector interface unit (bit 6 (PM1x) of parameter No. 1905 is set to 1,
bit 7 (PM2x) of parameter No. 1905 is set to 1, bit 1 (PM3x) of
parameter No. 1905 is set to 1, or bit 2 (PM4x) of parameter No. 1905
is set to 1), set 32 for connectors not used.
NOTE
When the FSSB is set to the automatic setting mode
(when the parameter FMD (No.1902#0) is set to 0),
parameter Nos. 14376 to 14407 are automatically set
as data is input on the FSSB setting screen. When
the manual setting 2 mode is set (when the parameter
FMD (No.1902#0) is set to 1), be sure to directly set
values in parameter Nos. 14376 to 14407.
A.PARAMETERS APPENDIX B-63944EN/03
- 2226 -
14713 Unit of magnification by which enlargement and reduction is performed with
the dynamic graphic display function
[Input type] Parameter input
[Data type] Word
[Valid data range] 0 to 255
This parameter sets the unit of magnification by which enlargement
and reduction is performed with the dynamic graphic display function.
Unit of magnification = 64 / setting
If 0 is set, 64 is assumed.
14714 Unit of horizontal movement when a movement is made with the dynamic
graphic display function
[Input type] Parameter input
[Data type] Word
[Valid data range] 0 to 255
This parameter sets the unit of horizontal movement (in dots) applied
when a movement is made with the dynamic graphic display function.
If 0 is set, 64 is assumed.
14715 Unit of vertical movement when a movement is made with the dynamic
graphic display function
[Input type] Parameter input
[Data type] Word
[Valid data range] 0 to 255
This parameter sets the unit of vertical movement (in dots) applied
when a movement is made with the dynamic graphic display function.
If 0 is set, 35 is assumed.
14716 Unit of rotation angle when rotation is performed with the dynamic graphic
display function
[Input type] Parameter input
[Data type] Word
[Valid data range] 0 to 255
This parameter sets the unit (in degrees) of a rotation angle by which
the drawing coordinate system is rotated with the dynamic graphic
display function.
If 0 is set, 10 is assumed.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2227 -
18060 M code that prohibits backward movement
[Input type] Parameter input
[Data type] Word path
[Valid data range] 1 to 999
When an M code that prohibits backward movement is specified
during backward movement, backward movement of blocks before the
M code is prohibited. In this case, backward movement prohibition
signal MRVSP<Fn091.2> is output.
The M code that prohibits backward movement is not output as an M
code. As the M code that prohibits backward movement, set an M
code that is not used by auxiliary functions and macros.
18065 M code that prohibits backward movement 1
[Input type] Parameter input
[Data type] Word path
[Valid data range] 1 to 999
When an M code that prohibits backward movement is specified
during backward movement, backward movement of blocks before the
M code is prohibited. In this case, backward movement prohibition
signal MRVSP<Fn091.2> is output.
18066 M code that prohibits backward movement 2
[Input type] Parameter input
[Data type] Word path
[Valid data range] 1 to 999
When an M code that prohibits backward movement is specified
during backward movement, backward movement of blocks before the
M code is prohibited. In this case, backward movement prohibition
signal MRVSP<Fn091.2> is output.
A.PARAMETERS APPENDIX B-63944EN/03
- 2228 -
#7 #6 #5 #4 #3 #2 #1 #0
19500 FNW
[Input type] Parameter input
[Data type] Bit path
# 6 FNW When the feedrate is determined according to the feedrate difference
and acceleration in AI contour control:
0: The maximum feedrate at which the allowable feedrate
difference and acceleration for each axis are not exceeded is
used.
1: The maximum feedrate at which the allowable feedrate
difference and acceleration for each axis are not exceeded is used.
The feedrate is determined so that the decreased feedrate is
constant regardless of the move direction when the profile is the
same.
A feedrate is determined to satisfy the condition that the allowable
feedrate difference and allowable acceleration rate of each axis are not
exceeded, and also to ensure that a constant deceleration rate is
applied to the same figure regardless of the direction of movement.
#7 #6 #5 #4 #3 #2 #1 #0
19501 FRP
[Input type] Parameter input
[Data type] Bit path
# 5 FRP Linear rapid traverse is:
0: Acceleration/deceleration after interpolation
1: Acceleration/deceleration before interpolation
Set a maximum allowable acceleration rate for each axis in parameter
No. 1671.
When using bell-shaped acceleration/deceleration before interpolation,
set an acceleration rate change time in parameter No. 1672.
When this parameter is set to 1, acceleration/deceleration before
interpolation is also applied to rapid traverse if all conditions below
are satisfied. At this time, acceleration/deceleration after interpolation
is not applied.
• Bit 1 (LRP) of parameter No. 1401 is set to 1: Linear
interpolation type positioning
• A value other than 0 is set in parameter No. 1671 for an axis.
• The AI contour control mode is set.
If all of these conditions are not satisfied, acceleration/deceleration
after interpolation is applied.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2229 -
#7 #6 #5 #4 #3 #2 #1 #0
19503 ZOL HPF
[Input type] Parameter input
[Data type] Bit path
# 0 HPF When a feedrate is determined based on acceleration in AI contour
control, smooth feedrate control is:
0: Not used.
1: Used.
# 4 ZOL The deceleration function based on cutting load in AI contour control
(deceleration based on Z-axis fall angle) is:
0: Enabled for all commands.
1: Enabled for linear interpolation commands only.
#7 #6 #5 #4 #3 #2 #1 #0
19515 ZG2
[Input type] Parameter input
[Data type] Bit path
# 1 ZG2 When the deceleration function based on cutting load in AI contour
control (deceleration based on Z-axis fall angle) is used:
0: Stepwise override values are applied.
1: Inclined override values are applied.
This parameter is valid only when bit 4 (ZAG) of parameter No. 8451
is set to 1.
When this parameter is set to 1, be sure to set parameter Nos. 19516,
8456, 8457, and 8458.
19516 Override for area 1 in deceleration based on cutting load in AI contour
control
[Input type] Parameter input
[Data type] Word path
[Unit of data] %
[Valid data range] 1 to 100
This parameter sets an override value for area 1 when the deceleration
function based on cutting load in AI contour control is used.
This parameter is valid only when bit 1 (ZG2) of parameter No. 19515
is set to 1.
A.PARAMETERS APPENDIX B-63944EN/03
- 2230 -
#7 #6 #5 #4 #3 #2 #1 #0
19530 CYS
[Input type] Parameter input
[Data type] Bit path
# 6 CYS Specifies whether when the cylindrical interpolation cutting point
compensation function is used, cutting point compensation is
performed between blocks or together with a block movement if the
cutting point compensation value is less than the setting of parameter
No. 19534.
0: Performed between blocks.
1: Performed together with a block movement if the cutting point
compensation value is less than the setting of parameter No.
19534.
19534 Limit for changing cylindrical interpolation cutting point compensation in a
single block
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm, inch (input unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 1 to 999999999
The following operation is performed, depending on the setting of
parameter No.19530:
(1) Bit 6 (CYS) of parameter No. 19530) is set to 0
If the amount of cylindrical interpolation cutting point
compensation is smaller than the value set in this parameter,
cylindrical interpolation cutting point compensation is not
performed. Instead, this ignored amount of cylindrical
interpolation cutting point compensation is added to the next
amount of cylindrical interpolation cutting point compensation to
determine whether to perform cylindrical interpolation cutting
point compensation.
(2) Bit 6 (CYS) of parameter No. 19530) is set to 1
If the amount of cylindrical interpolation cutting point
compensation is smaller than the value set in this parameter,
cylindrical interpolation cutting point compensation is performed
together with the movement of the specified block.
NOTE
Set this parameter as follows:
Setting > (setting for a rotation axis in parameter
No. 1422) × 4/3 where 4/3 is a constant for internal
processing.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2231 -
19535 Limit of travel distance moved with the cylindrical interpolation cutting point
compensation in the previous block unchanged.
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm, inch (input unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 1 to 999999999
The following operation is performed, depending on the type of
interpolation:
(1) For linear interpolation
If the travel distance in a specified block is smaller than the value
set in this parameter, machining is performed without changing
the cylindrical interpolation cutting point compensation in the
previous block.
(2) For circular interpolation
If the diameter of a specified arc is smaller than the value set in
this parameter, machining is performed without changing the
cylindrical interpolation cutting point compensation in the
previous block. Cylindrical interpolation cutting point
compensation is not performed according to a circular
movement.
#7 #6 #5 #4 #3 #2 #1 #0
19540 FAP
[Input type] Parameter input
[Data type] Bit path
# 0 FAP Optimal torque acceleration/deceleration is:
0: Disabled.
1: Enabled.
When the linear positioning parameters, namely bit 1 (LRP) of
parameter No. 1401 and bit 0 (FAP) of parameter No. 19540, are set
to 1, and a value other than 0 is set in reference acceleration parameter
(No. 1671) for an axis, the acceleration/deceleration for rapid traverse
becomes optimal torque acceleration/deceleration in the mode for
acceleration/deceleration before look-ahead interpolation (or the AI
contour control mode). Optimal torque acceleration/ deceleration is
controlled according to parameter-set restricted acceleration curve
data.
Setting an acceleration pattern
A.PARAMETERS APPENDIX B-63944EN/03
- 2232 -
A
cceleration
S
p
eed
FbFa
A
a
P1 P2
P3
P4 P5
A
b
A
cceleration pattern
P0
Set the speed at each of the acceleration setting points (P0 to P5) in a
corresponding parameter, then in parameters for each axis, set
acceleration rates applicable in the following four cases at these
speeds: when a movement in the positive direction is accelerated,
when a movement in the positive direction is decelerated, when a
movement in the negative direction is accelerated, and when a
movement in the negative direction is decelerated.
The line connecting the acceleration setting points is the acceleration
pattern.
The acceleration rate for each axis is calculated. For example, between
speeds Fa to Fb in the above figure, the acceleration rates
corresponding to these speeds, Aa to Ab, are used for calculation.
The tangent acceleration is controlled so that it does not exceed the
calculated acceleration rate for each axis.
CAUTION
When an acceleration pattern is set, setting a high
acceleration rate immediately after a speed of 0
can cause an impact on the machine, so it is not
desirable. Therefore, be sure to apply a
relatively low acceleration rate at a speed of 0
as shown in the above figure.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2233 -
19541 Optimal torque acceleration/deceleration (speed at P1)
19542 Optimal torque acceleration/deceleration (speed at P2)
19543 Optimal torque acceleration/deceleration (speed at P3)
19544 Optimal torque acceleration/deceleration (speed at P4)
[Input type] Parameter input
[Data type] Word axis
[Unit of data] 0.01%
[Valid data range] 0 to 10000
The speeds at acceleration setting points P1 to P4 are to be set with
speed parameters Nos. 19541 to 19544 as ratios to the rapid traverse
speed (parameter No. 1420). The speed at P0 is 0, and the speed at P5
is the rapid traverse rate specified with parameter (No. 1420). Any
acceleration setting point for which the speed parameter (one of Nos.
19541 to 19544) is set to 0 will be skipped.
19545 Optimal torque acceleration/deceleration (acceleration at P0 during
movement in + direction and acceleration)
19546 Optimal torque acceleration/deceleration (acceleration at P1 during
movement in + direction and acceleration)
19547 Optimal torque acceleration/deceleration (acceleration at P2 during
movement in + direction and acceleration)
19548 Optimal torque acceleration/deceleration (acceleration at P3 during
movement in + direction and acceleration)
19549 Optimal torque acceleration/deceleration (acceleration at P4 during
movement in + direction and acceleration)
19550 Optimal torque acceleration/deceleration (acceleration at P5 during
movement in + direction and acceleration)
19551 Optimal torque acceleration/deceleration (acceleration at P0 during
movement in - direction and acceleration)
19552 Optimal torque acceleration/deceleration (acceleration at P1 during
movement in - direction and acceleration)
19553 Optimal torque acceleration/deceleration (acceleration at P2 during
movement in - direction and acceleration)
19554 Optimal torque acceleration/deceleration (acceleration at P3 during
movement in - direction and acceleration)
19555 Optimal torque acceleration/deceleration (acceleration at P4 during
movement in - direction and acceleration)
A.PARAMETERS APPENDIX B-63944EN/03
- 2234 -
19556 Optimal torque acceleration/deceleration (acceleration at P5 during
movement in - direction and acceleration)
19557 Optimal torque acceleration/deceleration (acceleration at P0 during
movement in + direction and deceleration)
19558 Optimal torque acceleration/deceleration (acceleration at P1 during
movement in + direction and deceleration)
19559 Optimal torque acceleration/deceleration (acceleration at P2 during
movement in + direction and deceleration)
19560 Optimal torque acceleration/deceleration (acceleration at P3 during
movement in + direction and deceleration)
19561 Optimal torque acceleration/deceleration (acceleration at P4 during
movement in + direction and deceleration)
19562 Optimal torque acceleration/deceleration (acceleration at P5 during
movement in + direction and deceleration)
19563 Optimal torque acceleration/deceleration (acceleration at P0 during
movement in - direction and deceleration)
19564 Optimal torque acceleration/deceleration (acceleration at P1 during
movement in - direction and deceleration)
19565 Optimal torque acceleration/deceleration (acceleration at P2 during
movement in - direction and deceleration)
19566 Optimal torque acceleration/deceleration (acceleration at P3 during
movement in - direction and deceleration)
19567 Optimal torque acceleration/deceleration (acceleration at P3 during
movement in - direction and deceleration)
19568 Optimal torque acceleration/deceleration (acceleration at P5 during
movement in - direction and deceleration)
[Input type] Parameter input
[Data type] Word axis
[Unit of data] 0.01%
[Valid data range] 0 to 32767
For each travel direction and each acceleration/deceleration operation,
set the allowable acceleration rate at each of the acceleration setting
points (P0 to P5). As an allowable acceleration rate, set a ratio to the
value set in the reference acceleration parameter (No. 1671). When 0
is set, the specification of 100% is assumed.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2235 -
19581 Tolerance smoothing for nano smoothing
[Input type] Setting input
[Data type] Real path
[Unit of data] mm, inch, degree (input unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 0 or positive 9 digit of minimum unit of data (refer to the standard
parameter setting table (B))
(When the increment system is IS-B, 0.0 to +999999.999)
This parameter sets a tolerance value for a program created using
miniature line segments in nano smoothing.
When 0 is set in this parameter, a minimum amount of travel in the
increment system is regarded as a tolerance value.
19582 Minimum amount of travel of a block that makes a decision based on an
angular difference between blocks for nano smoothing
[Input type] Setting input
[Data type] Real path
[Unit of data] mm, inch, degree (input unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 0 or positive 9 digit of minimum unit of data (refer to the standard
parameter setting table (B))
(When the increment system is IS-B, 0.0 to +999999.999)
This parameter sets the minimum amount of travel of a block that
makes a decision based on an angular difference between blocks for
nano smoothing. A block that specifies an amount of travel less than
the value set in this parameter makes no decision based on an angular
difference.
When 0 is set in this parameter, a decision based on an angular
difference is made with all blocks.
A value greater than the value set in parameter No. 8490 for making a
decision based on the minimum travel distance of a block must be set.
19587 Tolerance of rotary axes for nano smoothing 2
[Input type] Setting input
[Data type] Real axis
[Unit of data] degree (input unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 0 or positive 9 digit of minimum unit of data (refer to the standard
parameter setting table (B))
(When the increment system is IS-B, 0.0 - +999999.999)
This parameter sets the tolerance of rotation axes in a program created
using small line segments in nano smoothing 2. This parameter is
valid only for the rotation axes specified in nano smoothing 2.
When 0 is set in this parameter, a minimum amount of travel in the
increment system is regarded as a tolerance value.
A.PARAMETERS APPENDIX B-63944EN/03
- 2236 -
#7 #6 #5 #4 #3 #2 #1 #0
19604 TPC
[Input type] Setting input
[Data type] Bit path
# 5 TPC In the case that there is no address P at the start of tool center point
control (G43.4/G43.5), tool posture control
0: Does not work.
1: Works.
#7 #6 #5 #4 #3 #2 #1 #0
19605 NSC
[Input type] Parameter input
[Data type] Bit path
# 0 NSC For the machine type that has no rotation axis for rotating the tool
(when parameter No. 19680 is set to 12 to specify the table rotation
type), control point shifting in the tilted working plane command is:
0: Enabled.
Set bit 4 (SPR) and bit 5 (SVC) of parameter No. 19665.
1: Disabled.
#7 #6 #5 #4 #3 #2 #1 #0
CAV SPG
19607 CAV WCD SPG
[Input type] Parameter input
[Data type] Bit path
# 1 SPG To apply 3-dimensional tool compensation to a machine having a
table rotation axis, as the G code to be specified:
0: G41.2/G42.2 is used regardless of the machine type.
1: G41.4/G42.4 is used for a table rotation type machine;
G41.5/G42.5 for a mixed type machine.
# 3 WCD This parameter specify a direction of compensation vector by a sign of
offset value in geinding-wheel wear compensation
Offset vale by D code
Minus Plus
0Direction from
compensation center to
command end position.
Direction from command
end position to
compensation center
19607#3
1Direction from command
end position to
compensation center
Direction from
compensation center to
command end position.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2237 -
Compensation vector
Programmed path
Tool center path
Compensation
Center
Z
Y
Direction from compensation center to command end position
Compensation Vector
Programmed path
Tool center path
Compensation
center
Z
Y
Direction from command end position to compensation center
# 5 CAV When an interference check finds that interference (overcutting)
occurred:
0: Machining stops with the alarm (PS0041).
(Interference check alarm function)
1: Machining is continued by changing the tool path to prevent
interference (overcutting) from occurring. (Interference check
avoidance function)
For the interference check method, see the descriptions of bit 1 (CNC)
of parameter No. 5008 and bit 3 (CNV) of parameter No. 5008.
A.PARAMETERS APPENDIX B-63944EN/03
- 2238 -
#7 #6 #5 #4 #3 #2 #1 #0
19608 MIR PRI DET NI5
[Input type] Parameter input
[Data type] Bit path
#1 NI5 The interference check in 3-dimensional cutter compensation is
performed by:
0: Projecting a look-ahead command position onto a plane
perpendicular to the tool axis direction of a block for which
compensation is planned.
The interference check avoidance function cannot be used.
1: Projecting a look-ahead command position onto a plane that is
always perpendicular to the tool axis direction. When a table
rotation axis is present, checking is made in the table coordinate
system.
The interference check avoidance function can be used.
# 2 DET When the programming coordinate system is fastened to the table in
tool center point control or 3-dimensional tool compensation, the
relative position and absolute position of a specified path are:
0: Displayed in the programming coordinate system (fastened to the
table).
1: Displayed in the workpiece coordinate system (not fastened to
the table).
# 5 PRI Among multiple end point candidates that exist when a movement is
made on a rotation axis by a command such as I, J, and K when a
slanted surface machining command is specified under tool center
point control (type 2) or 3-dimensional tool compensation (type 2):
0: A combination in which the master (first rotation axis) makes a
smaller angular movement is selected for a machine of tool
rotation type or table rotation type. A combination in which the
table (second rotation axis) makes a smaller angular movement is
selected for a machine of composite type.
1: A combination in which the slave (second rotation axis) makes a
smaller angular movement is selected for a machine of tool
rotation type or table rotation type. A combination in which the
tool (first rotation axis) makes a smaller angular movement is
selected for a machine of composite type.
# 6 MIR When programmable mirror image is applied to a linear axis in tool
center point control (type 2) or 3-dimensional tool compensation (type
2), mirror image is:
0: Not applied to a specified I, J, or K command
1: Applied to a specified I, J, or K command.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2239 -
19631 Variation for determining an angle when the leading-edge offset function is
performed
[Input type] Parameter input
[Data type] Real axis
[Unit of data] degree
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999）
In the leading-edge offset function is performed, this parameter sets
the range of variations applicable when the included angle of the tool
direction vector (VT) and the advancing direction vector (VM) is
determined to be 0°, 180°, or 90°.
For example, let the included angle between VT and VM be θ (0 ≤ θ ≤
180) and the angle set in this parameter be ∆θ. θ is then determined as
follows:
If 0 ≤ θ ≤ ∆θ θ = 0°
(180-∆θ)≤θ≤180 θ = 180°
(90-∆θ)≤θ≤(90+∆θ) θ = 90°
Normally, set a value around 1.0.
19632 Distance from a programmed point (pivot point) to tool center point position
(cutting point)
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm, inch (input unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999）
This parameter sets the distance from a programmed point to the
actual cutting point to perform vector calculation for 3-dimensional
cutter compensation at the tool center point.
When this parameter is set to 0, the tool center point is not supported
by the 3-dimensional cutter compensation function.
NOTE
This parameter can be rewritten only before the
3-dimensional cutter compensation mode is
entered.
A.PARAMETERS APPENDIX B-63944EN/03
- 2240 -
19635 Angle used as a criterion for the interference check in 3-dimensional cutter
compensation
[Input type] Setting input
[Data type] Real axis
[Unit of data] degree
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999）
In 3-dimensional cutter compensation, if the difference in angle
between two tool direction vectors is equal to or greater than the
setting of this parameter, the tool direction is determined to have been
changed.
When 0 is set, 45 degrees is assumed.
Let two tool direction vectors be Va and Vb. Then, if the difference in
angle is α degrees or greater as shown in the figure below, the tool
direction vector is determined to have changed.
α degrees
Va
Vb
19636 Angle used to determine whether to execute the interference
check/avoidance function of 3-dimensional tool compensation machining
[Input type] Setting input
[Data type] Real path
[Unit of data] deg
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
The interference check/avoidance function of 3-dimensional tool
compensation machining is executed when the angle difference
between the tool direction vectors for the target two points is less than
the setting.
This parameter is valid when bit 1 (NI5) of parameter No. 19608 is set
to 1. When the setting is 0, the angle is assumed to be 10.0 degrees.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2241 -
19658 Angular displacement of a rotation axis
[Input type] Parameter input
[Data type] Real axis
[Unit of data] deg
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (B))
(When the increment system is IS-B, -999999.999 to +999999.999)
This parameter sets the coordinate of a rotation axis, among the
rotation axes determining the tool axis direction, which is not
controlled by the CNC for the tool axis direction tool length
compensation function. Whether this parameter is valid or invalid is
determined by the setting of bit 1 (RAP) of parameter No. 19650.
19659 Offset value for the angular displacement of a rotation axis
[Input type] Parameter input
[Data type] Real axis
[Unit of data] deg
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
An offset can be applied to the angular displacement for the tool axis
direction tool length compensation function to compensate for the
move direction.
19660 Origin offset value of a rotation axis
[Input type] Parameter input
[Data type] Real axis
[Unit of data] deg
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
This parameter sets an angular displacement shifted from the origin
for a rotation axis for the tool axis direction tool length compensation
function.
A.PARAMETERS APPENDIX B-63944EN/03
- 2242 -
19661 Rotation center compensation vector in tool axis direction tool length
compensation
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm, inch (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
This parameter sets the vector from the first rotation axis center to the
second rotation axis center for the tool axis direction tool length
compensation function.
19662 Spindle center compensation vector in tool axis direction tool length
compensation
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm, inch (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
This parameter sets the compensation vector for the spindle center for
the tool axis direction tool length compensation function.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2243 -
#7 #6 #5 #4 #3 #2 #1 #0
19665 SVC SPR
[Input type] Parameter input
[Data type] Bit path
# 4 SPR The controlled point is shifted by:
0: Automatic calculation.
1: Using parameter No. 19667.
Bit 5 (SVC) of
parameter No.
19665
Bit 4 (SPR) of
parameter No.
19665
Shift of controlled point
0 - Shift is not performed as not done conventionally.
1 0
The controlled point is shifted according to the result of the following
automatic calculation:
- (Intersection offset vector between the tool axis and the first rotation axis of
the tool + intersection offset vector between the second and first rotation axes
of the tool + tool holder offset (parameter No. 19666))
(See the figure below.)
1 1
The controlled point is shifted.
As the shift vector, the vector set in parameter No. 19667 is used.
Shift of controlled point
Tool length offset
Tool holder offset
Controlled-point shift vector
D
E
Tool center point
Controlled point
Second rotary axis of tool
F
First rotary axis of tool
[Controlled-point shift vector when automatically calculated]
# 5 SVC The controlled point is:
0: Not shifted.
1: Shifted.
The method of shifting is specified by bit 4 (SPR) of parameter No.
19665.
NOTE
When the machine has no rotation axis for rotating
the tool (when parameter No. 19680 is set to 12 to
specify the table rotation type), the controlled point
is not shifted regardless of the setting of this
parameter.
A.PARAMETERS APPENDIX B-63944EN/03
- 2244 -
19666 Tool holder offset value
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm, inch (machine unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
When the tool axis direction tool length compensation function, tool
tip center rotation handle feed/interrupt, and the display of the tool
center point position are performed, specify the offset for the
machine-specific section from the rotation center of the rotation axis
to the tool mounting position (the tool holder offset value) in tool
length compensation during tool center point control and tilted
working plane command mode (after G53.1). For the tool axis
direction tool length compensation function, the tool holder offset
function can be enabled or disabled by setting bit 7 (ETH) of
parameter No. 19665.
NOTE
Set a radius value.
19667 Controlled-point shift vector
[Input type] Parameter input
[Data type] Real axis
[Unit of data] mm, inch (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
Set the shift vector for the controlled point. This value becomes valid
when bit 5 (SVC) of parameter No. 19665 is set to 1, and bit 4 (SPR)
of parameter No. 19665 is set to 1.
NOTE
Set a radius value.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2245 -
19680 Mechanical unit type
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to 21
Specify the type of the mechanical unit.
Parameter
No. 19680 Mechanical unit type Controlled rotation axis Master and slave
0 Mechanism having no rotation axis
2 Tool rotation type Two rotation axes of the tool The first rotation axis is the master, and
the second rotation axis is the slave.
12 Table rotation type Two rotation axes of the table The first rotation axis is the master, and
the second rotation axis is the slave.
21 Mixed type One rotation axis of the tool + one
rotation axis of the table
The first rotation axis is the tool rotation
axis, and the second rotation axis is the
table rotation axis.
First rotar
y
axis
(
master
)
Second rotar
y
axis
(
slave
)
First rotary axis (master)
Second rotary axis (slave) Tool rotary
axes
Table rotary
axes
NOTE
A hypothetical axis is also counted as a
controlled rotary axis.
<Hypothetical axis>
In some cases, it is convenient to use an
imaginary rotary axis whose angle is fixed to a
certain value. For example, suppose that a tool is
mounted in a tilted manner through an attachment.
In such a case, the rotary axis considered
hypothetically is a hypothetical axis. Bits 0 (IA1)
and 1 (IA2) of parameter No. 19696 determine
whether each rotary axis is an ordinary rotary axis
or a hypothetical axis.
A.PARAMETERS APPENDIX B-63944EN/03
- 2246 -
19681 Controlled-axis number for the first rotation axis
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to Number of controlled axes
Set the controlled-axis number for the first rotation axis.
For a hypothetical axis (when bit 0 (IA1) of parameter No. 19696 is 1),
set 0.
Example)
Assuming that the axis configuration in path 1 is X,Y,Z,B,C and
the axis configuration in path 2 is X,Z,C,Y,B, set the parameter
to 5 in path 1 and to 3 in path 2 if C is the first rotation axis in
each path.
19682 Axis direction of the first rotation axis
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to 6
Specify the axis direction of the first rotation axis.
1: On X-axis
2: On Y-axis
3: On Z-axis
4: On an axis tilted a certain angle from the X-axis from the
positive X-axis to positive Y-axis
5: On an axis tilted a certain angle from the Y-axis from the
positive Y-axis to positive Z-axis
6: On an axis tilted a certain angle from the Z-axis from the positive
Z-axis to positive X-axis
(A value 4 to 6 is to be set when the inclined rotation axis control
function is used.)
Y
Z
X
2
3
1
Parameter No.19682
B-63944EN/03 APPENDIX A.PARAMETERS
- 2247 -
19683 Inclination angle when the first rotation axis is an inclined axis
[Input type] Parameter input
[Data type] Real path
[Unit of data] Degree
[Minimum unit of data] The increment system of the reference axis is to be followed.
[Valid data range] Nine digits of the least input increment (see standard parameter setting
table (A).)
(-999999.999 to +999999.999 for IS-B)
When a value 1 to 3 is set in parameter No. 19682, set 0 degrees.
When a value 4 to 6 is set in parameter No.19682, specify the
inclination angle.
Parameter No.19682
Y
Z
X
5
4
6
Parameter No.19683
19684 Rotation direction of the first rotation axis
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to 1
Set the direction in which the first rotation axis rotates as a mechanical
motion when a positive move command is issued.
0: Clockwise direction as viewed from the negative to positive
direction of the axis specified in parameter No. 19682
(right-hand thread rotation)
1: Counterclockwise direction as viewed from the negative to
positive direction of the axis specified in parameter No. 19682
(left-hand thread rotation)
Normally, 0 is set for a tool rotation axis, and 1 is set for a table
rotation axis.
A.PARAMETERS APPENDIX B-63944EN/03
- 2248 -
19685 Rotation angle when the first rotation axis is a hypothetical axis
[Input type] Parameter input
[Data type] Real path
[Unit of data] Degree
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
When the first rotation axis is a hypothetical axis (bit 0 (IA1) of
parameter No. 19696 is 1), set the rotation angle.
19686 Controlled-axis number for the second rotation axis
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to Number of controlled axes
Set the controlled-axis number for the second rotation axis.
For a hypothetical axis (bit 1 (IA2) of parameter No. 19696 is 1), set
0.
Example)
Assuming that the axis configuration in path 1 is X,Y,Z,B,C and
the axis configuration in path 2 is X,Z,C,Y,B, set the parameter
to 4 in path 1 and to 5 in path 2 if B is the second rotation axis in
each path.
19687 Axis direction of the second rotation axis
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to 6
Specify the axis direction of the second rotation axis.
1: On X-axis
2: On Y-axis
3: On Z-axis
4: On an axis tilted a certain angle from the X-axis from the
positive X-axis to positive Y-axis
5: On an axis tilted a certain angle from the Y-axis from the
positive Y-axis to positive Z-axis
6: On an axis tilted a certain angle from the Z-axis from the positive
Z-axis to positive X-axis
(A value 4 to 6 is to be set when the inclined rotation axis control
function is used.)
When the second rotation axis is the slave axis, the direction when the
master axis is at 0 degrees must be set.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2249 -
19688 Inclination angle when the second rotation axis is inclined
[Input type] Parameter input
[Data type] Real path
[Unit of data] Degree
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
(When the increment system is IS-B, -999999.999 to +999999.999)
If parameter No. 19687 is set to a value 1 to 3, set 0 degrees.
If parameter No. 19687 is set to a value 4 to 6, set the inclination
angle.
19689 Rotation direction of the second rotation axis
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to 1
Set the direction in which the second rotation axis rotates as a
mechanical motion when a positive move command is issued.
0: Clockwise direction as viewed from the negative to positive
direction of the axis specified in parameter No. 19687
(right-hand thread rotation)
1: Counterclockwise direction as viewed from the negative to
positive direction of the axis specified in parameter No. 19687
(left-hand thread rotation)
Normally, 0 is set for a tool rotation axis, and 1 is set for a table
rotation axis.
19690 Rotation angle when the second rotation axis is a hypothetical axis
[Input type] Parameter input
[Data type] Real path
[Unit of data] Degree
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
When the second rotation axis is a hypothetical axis (bit 1 (IA2) of
parameter No. 19696 is 1), set the rotation angle.
A.PARAMETERS APPENDIX B-63944EN/03
- 2250 -
#7 #6 #5 #4 #3 #2 #1 #0
19696 RFC WKP NPC IA2 IA1
[Input type] Parameter input
[Data type] Bit path
# 0 IA1
0: The first rotation axis is an ordinary rotation axis.
1: The first rotation axis is a hypothetical axis.
If IA1 is 1, set 0 as the controlled-axis number for the first rotation
axis (parameter No. 19681).
Also, set parameter Nos. 19682 to 19685 on the assumption that there
is a rotation axis.
# 1 IA2
0: The second rotation axis is an ordinary rotation axis.
1: The second rotation axis is a hypothetical axis.
If IA2 is 1, set 0 as the controlled-axis number for the second rotation
axis (parameter No. 19686).
Also, set parameter Nos. 19687 to 19690 on the assumption that there
is a rotation axis.
# 3 NPC In tool posture control for tool center point control type II, when the
change of tool posture at the block end is not done with the parameters
(No.19738, 19739), even if the tool posture passes the singular
posture,
0: Program is executed without the change of tool posture.
1: The alarm PS5421 occurs.
# 5 WKP For a 5-axis machine having a table rotation axis, as the programming
coordinate system for tool center point control or 3-dimensional tool
compensation machining:
0: The table coordinate system (coordinate system fixed on the
rotary table) is used.
1: The workpiece coordinate system is used.
NOTE
For 3-dimensional tool compensation machining,
the setting of this parameter is used only when bit
4 (TBP) of parameter No. 19746 is set to 1.
# 6 RFC In tool center point control, when a command that does not move the
tool center point with respect to the workpiece is issued, the feedrate
of the rotation axis is:
0: The maximum cutting feedrate (parameter No. 1422).
1: A specified feedrate.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2251 -
19697 Reference tool axis direction
[Input type] Parameter input
[Data type] Byte path
[Valid data range] 0 to 3
Set the tool axis direction in the machine coordinate system when the
rotation axes for controlling the tool are all at 0 degrees. Also, set the
tool axis direction in the machine coordinate system in a mechanism
in which only the rotation axes for controlling the table are present
(there is no rotation axis for controlling the tool).
1: Positive X-axis direction
2: Positive Y-axis direction
3: Positive Z-axis direction
When the reference tool axis direction is neither the X-, Y-, nor Z-axis
direction, set the reference direction in this parameter, then set
appropriate angles as the reference angle RA and reference angle RB
(parameter Nos. 19698 and 19699).
Reference tool axis direction
X
Y
Z
Tool axis direction is positive X-axis direction.
Tool axis direction is positive Y-axis direction.
Tool axis direction is positive Z-axis direction.
A.PARAMETERS APPENDIX B-63944EN/03
- 2252 -
19698 Angle when the reference tool axis direction is tilted (reference angle RA)
19699 Angle when the reference tool axis direction is tilted (reference angle RB)
[Input type] Parameter input
[Data type] Real path
[Unit of data] Degree
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
(When the increment system is IS-B, -999999.999 to +999999.999)
When the reference tool axis direction (parameter No. 19697) is set to
1, the tool axis is tilted the RA degrees on the Z-axis from the positive
X-axis direction to positive Y-axis direction, then the tool axis is tilted
the RB degrees on the X-axis from the positive Y-axis direction to
positive Z-axis direction.
When the reference tool axis direction (parameter No. 19697) is set to
2, the tool axis is tilted the RA degrees on the X-axis from the positive
Y-axis direction to positive Z-axis direction, then the tool axis is tilted
the RB degrees on the Y-axis from the positive Z-axis direction to
positive X-axis direction.
When the reference tool axis direction (parameter No. 19697) is set to
3, the tool axis is tilted the RA degrees on the Y-axis from the positive
Z-axis direction to positive X-axis direction, then the tool axis is tilted
the RB degrees on the Z-axis from the positive X-axis direction to
positive Y-axis direction.
Tool axis direction when the reference tool axis direction is Z-axis
RA
X
Y
Z
X
Y
Z
RB
X
Z
Tool holder offset
Tool length offset
Y
B-63944EN/03 APPENDIX A.PARAMETERS
- 2253 -
19700 Rotary table position (X-axis of the basic three axes)
19701 Rotary table position (Y-axis of the basic three axes)
19702 Rotary table position (Z-axis of the basic three axes)
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm, inch (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
Set these parameters when parameter No. 19680 is set to 12 or 21. The
vector from the origin of the machine coordinate system to point A on
the first rotation axis of the table is set as the rotary table position in
the machine coordinate system.
Rotary table position
Zm
Ym
Xm
First rotary axis o
f
table
Rotary table position
A
NOTE
As point A, set a position that is easy to measure
on the first rotary axis of the table.
Set a radius value.
If the rotary table is moved along the X-, Y-, or
Z-axis or all of these axes, set the position of the
rotary table when the machine coordinates of the
X-, Y-, and Z-axes are all set to 0.
A.PARAMETERS APPENDIX B-63944EN/03
- 2254 -
19703 Intersection offset vector between the first and second rotation axes of the
table (X-axis of the basic three axes)
19704 Intersection offset vector between the first and second rotation axes of the
table (Y-axis of the basic three axes)
19705 Intersection offset vector between the first and second rotation axes of the
table (Z-axis of the basic three axes)
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm, inch (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
Set these parameters when the first rotation axis and second rotation
axis of the table do not intersect. These parameters are valid when
parameter No. 19680 is set to 12. When the rotation axes for
controlling the table are all at 0 degrees, the vector from point A to
point B on the second rotation axis of the table is set as the
intersection offset vector in the machine coordinate system.
When table rotary axes do not intersect
Zm
Ym
Xm
Second rotary axis of table
First rotary axis of
table
Rotary table position
Intersection offset vector between first and second rotary
axes of table
B
A
NOTE
As point B, set a position that is easy to measure
on the second rotary axis of the table.
Set a radius value.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2255 -
19709 Intersection offset vector between the tool axis and tool rotation axis (X-axis
of the basic three axes)
19710 Intersection offset vector between the tool axis and tool rotation axis (Y-axis
of the basic three axes)
19711 Intersection offset vector between the tool axis and tool rotation axis (Z-axis
of the basic three axes)
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm, inch (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
Set these parameters when the tool axis and tool rotation axis do not
intersect.
These parameters are valid when parameter No. 19680 is set to 2 or
21.
If parameter No. 19680 is 21, set the vector from point D on the tool
axis to point E determined on the tool rotation axis as the intersection
offset vector in the machine coordinate system when the rotation axes
for controlling the tool are all at 0 degrees.
If parameter No. 19680 is 2, set the vector from point D on the tool
axis to point E determined on the second rotation axis of the tool as
the intersection offset vector in the machine coordinate system when
the rotation axes for controlling the tool are all at 0 degrees.
When tool axis and tool rotary axis do not intersect
Tool length offset
Tool holder offset
Intersection offset vector between tool axis and
tool rotary axis
D
E
Tool center point
Controlled point
Tool rotary
axis
NOTE
Point D is determined by adding the tool length
offset and tool holder offset (parameter No. 19666)
to the tool tip. As point E, set a position that is easy
to measure.
Set a radius value.
A.PARAMETERS APPENDIX B-63944EN/03
- 2256 -
19712 Intersection offset vector between the second and first rotation axes of the
tool (X-axis of the basic three axes)
19713 Intersection offset vector between the second and first rotation axes of the
tool (Y-axis of the basic three axes)
19714 Intersection offset vector between the second and first rotation axes of the
tool (Z-axis of the basic three axes)
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm, inch (machine unit)
[Minimum unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
Set these parameters when the rotation axes of the tool do not
intersect.
These parameters are valid when parameter No. 19680 is set to 2.
Set the vector from point E on the second rotation axis of the tool to
point F on the first rotation axis of the tool as the intersection offset
vector in the machine coordinate system when the rotation axes for
controlling the tool are all at 0 degrees.
When tool axis and tool rotary axis do not intersect
Tool length offset
Tool holder offset
Intersection offset vector between tool axis and second
rotary axis of tool
D
E
Tool center point
Controlled point
Second rotary
axis of tool
F
First rotary axis of tool
Intersection offset vector between second and first
rotary axes of tool
NOTE
As point F, set a position that is easy to measure.
Set a radius value.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2257 -
19738 Angle to check if Tool posture is near Singular posture or not
[Input type] Parameter input
[Data type] Real path
[Unit of data] degree
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table(A))
(When the increment system is IS-B, -999999.999 to +999999.999)
In the case of tool posture control for tool center point control (type II),
when the difference(angle) between a tool posture and the singular
posture is less than this parameter, the tool posture is regarded as ‘near
the singular posture’. Then, the tool posture at the block end is
changed so that the tool posture passes the singular posture during the
block.
If this parameter is 0.0, the tool posture at the block end is not
changed.
19739 Angle to decide that the tool posture at block end is not changed
[Input type] Parameter input
[Data type] Real path
[Unit of data] degree
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table(A))
(When the increment system is IS-B, -999999.999 to +999999.999)
When an appropriate value is set in parameter No. 19738 in tool
posture control for tool center point control (type II), a tool posture
near the singular point may occur during the execution of a block. If
this happens, change the tool posture at the end point so that the
singular posture is passed within the block. With respect to the angle
of the rotation axis nearer to the workpiece before and after the tool
posture is changed (the rotation axis is the master axis when tehe tool
turns, the slave axis when the table turns, or the table roration axis
when the rotation is of the mixed type), however, the tool posture
must not be changed if both the difference between the angle after the
change and (angle before the change + 180 degrees) and the difference
between the angle after the change and (angle before the change − 180
degrees) are equal to or greater than the value set in the parameter,
A.PARAMETERS APPENDIX B-63944EN/03
- 2258 -
19741 Upper limit of the movement range of the first rotation axis
[Input type] Parameter input
[Data type] Real path
[Unit of data] Degree
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
(When the increment system is IS-B, -999999.999 to +999999.999)
This parameter sets the upper limit of the movement range of the first
rotation axis in tool center point control (type 2), 3-dimensional cutter
compensation (type 2), or tool axis direction control of the tilted
working plane command (G53.1). When the movement range of the
first rotation axis is not specified, this parameter and parameter No.
19742 must both be set to 0.
19742 Lower limit of the movement range of the first rotation axis
[Input type] Parameter input
[Data type] Real path
[Unit of data] Degree
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
(When the increment system is IS-B, -999999.999 to +999999.999)
This parameter sets the lower limit of the movement range of the first
rotation axis in tool center point control (type 2), 3-dimensional cutter
compensation (type 2), or tool axis direction control of the tilted
working plane command (G53.1). When the movement range of the
first rotation axis is not specified, this parameter and parameter No.
19741 must both be set to 0.
19743 Upper limit of the movement range of the second rotation axis
[Input type] Parameter input
[Data type] Real path
[Unit of data] Degree
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
(When the increment system is IS-B, -999999.999 to +999999.999)
This parameter sets the upper limit of the movement range of the
second rotation axis in tool center point control (type 2),
3-dimensional cutter compensation (type 2), or tool axis direction
control of the tilted working plane command (G53.1). When the
movement range of the second rotation axis is not specified, this
parameter and parameter No. 19744 must both be set to 0.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2259 -
19744 Lower limit of the movement range of the second rotation axis
[Input type] Parameter input
[Data type] Real path
[Unit of data] Degree
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
(When the increment system is IS-B, -999999.999 to +999999.999)
This parameter sets the lower limit of the movement range of the
second rotation axis in tool center point control (type 2),
3-dimensional cutter compensation (type 2), or tool axis direction
control of the tilted working plane command (G53.1). When the
movement range of the second rotation axis is not specified, this
parameter and parameter No. 19743 must both be set to 0.
#7 #6 #5 #4 #3 #2 #1 #0
19746 CRS TBP LOZ LOD PTD
[Input type] Parameter input
[Data type] Bit path
# 1 PTD When 3-dimensional cutter compensation is performed for a table
rotation type machine, the direction of the tool is:
0: Specified by parameter Nos. 19697, 19698, and 19699.
1: Specified as a direction perpendicular to the plane specified by
G17, G18, or G19.
# 2 LOD As the tool length for three-dimensional machining manual feed:
0: The value of parameter No. 12318 is used.
1: The tool length currently used for tool length compensation is
used.
# 3 LOZ When bit 2 (LOD) of parameter No. 19746 is set to 1 and tool length
compensation is not applied, as the tool length for three-dimensional
machining manual feed:
0: The value of parameter No. 12318 is used.
1: 0 is used.
# 4 TBP For a 5-axis machine having a table rotation axis, as the programming
coordinate system for 3-dimensional tool compensation machining:
0: The workpiece coordinate system is used.
1: The setting of bit 5 (WKP) of parameter No. 19696 is used.
A.PARAMETERS APPENDIX B-63944EN/03
- 2260 -
# 6 CRS In tool center point control, when the deviation from the path during
movement at the specified cutting feedrate or rapid traverse rate is
determined to exceed the limit:
0: The feedrate or rapid traverse rate is not decreased.
1: The feedrate or rapid traverse rate is controlled so that the limit
of the deviation from the path set in the parameter for the cutting
feed or rapid traverse is not exceeded.
When this parameter is set to 1:
In the rapid traverse mode, the rapid traverse rate is decreased so that
the deviation from the path does not exceed the limit specified in
parameter No. 19751.
In the cutting feed mode, the cutting feedrate is decreased so that the
deviation from the path does not exceed the limit specified in
parameter No. 19752.
19751 Limit of the deviation from the path (for rapid traverse)
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm, inch (machine unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
This parameter sets the limit of the deviation from the path in the rapid
traverse mode in tool center point control.
If the tool moves at the specified rate, the deviation from the path may
exceed the value specified in this parameter. In this case, the rate is
decreased so that the tool moves along the path.
This parameter is valid when bit 6 (CRS) of parameter No. 19746 is
set to 1.
When 0 is set, the least input increment is assumed to be the limit of
the deviation from the path.
If a negative value is set, the rapid traverse rate is not decreased.
NOTE
The error generated after the rate is decreased
may be smaller than the value set in this parameter
depending on the calculation error.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2261 -
19752 Limit of the deviation from the path (for cutting feed)
[Input type] Parameter input
[Data type] Real path
[Unit of data] mm, inch (machine unit)
[Minimum unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting
table (A))
(When the increment system is IS-B, -999999.999 to +999999.999)
This parameter sets the limit of the deviation from the path in the
cutting feed mode in tool center point control.
If the tool moves at the specified rate, the deviation from the path may
exceed the value specified in this parameter. In this case, the rate is
decreased so that the tool moves along the path.
This parameter is valid when bit 6 (CRS) of parameter No. 19746 is
set to 1.
When 0 is set, the least input increment is assumed to be the limit of
the deviation from the path.
If a negative value is set, the cutting feedrate is not decreased.
NOTE
The error generated after the rate is decreased
may be smaller than the value set in this parameter
depending on the calculation error.
#7 #6 #5 #4 #3 #2 #1 #0
27350 GTP
[Input type] Parameter input
[Data type] Bit
# 0 GTP When a general-purpose tool is drawn in animated simulation, the tip
is:
0: Positioned on the front.
1: Positioned on the rear.
Front Rear
Tip
Holder Holder
A.PARAMETERS APPENDIX B-63944EN/03
- 2262 -
27351 Cutting edge length applied when a general-purpose tool is drawn in
animated simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the cutting edge length applied when a
general-purpose tool is drawn in animated simulation.
Cutting edge length
Tip
Holder
When 0 is set, 12 mm for metric input or 0.4724 inch for inch input is
assumed.
27352 Holder length applied when a general-purpose tool is drawn in animated
simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the holder length applied when a general-purpose
tool is drawn in animated simulation.
Holder length
Tip
Holder
When 0 is set, 50 mm for metric input or 1.9685 inch for inch input is
assumed.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2263 -
27353 Holder width applied when a general-purpose tool is drawn in animated
simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the holder width applied when a general-purpose
tool is drawn in animated simulation.
Holder width
Tip
Holder
When 0 is set, 14 mm for metric input or 0.5512 inch for inch input is
assumed.
27354 Holder length 2 applied when a general-purpose tool is drawn in animated
simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the holder length 2 applied when a
general-purpose tool is drawn in animated simulation.
Holder length 2
Tip
Holder
A.PARAMETERS APPENDIX B-63944EN/03
- 2264 -
27355 Holder width 2 applied when a general-purpose tool is drawn in animated
simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the holder width 2 applied when a general-purpose
tool is drawn in animated simulation.
Holder width 2
Tip
Holder
Holder width
#7 #6 #5 #4 #3 #2 #1 #0
27356 TTP
[Input type] Parameter input
[Data type] Bit
# 0 TTP When a threading tool is drawn in animated simulation, the tip is:
0: Positioned on the front.
1: Positioned on the rear.
Front Rear
Tip
Holder Holder
B-63944EN/03 APPENDIX A.PARAMETERS
- 2265 -
27357 Cutting edge width applied when a threading tool is drawn in animated
simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the cutting edge width applied when a threading
tool is drawn in animated simulation.
Cutting edge width
Tip
Holder
When 0 is set, 3 mm for metric input or 0.11811 inch for inch input is
assumed.
27358 Holder length applied when a threading tool is drawn in animated simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the holder length applied when a threading tool is
drawn in animated simulation.
Holder length
Tip
Holder
When 0 is set, 50 mm for metric input or 1.9685 inch for inch input is
assumed.
A.PARAMETERS APPENDIX B-63944EN/03
- 2266 -
27359 Holder width applied when a threading tool is drawn in animated simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the holder width applied when a threading tool is
drawn in animated simulation.
Holder width
Tip
Holder
When 0 is set, 14 mm for metric input or 0.5512 inch for inch input is
assumed.
#7 #6 #5 #4 #3 #2 #1 #0
27360 GVP
[Input type] Parameter input
[Data type] Bit
# 0 GVP When a groove cutting tool is drawn in animated simulation, the tip is:
0: Positioned on the front.
1: Positioned on the rear.
Front Rear
Tip
Holder Holder
B-63944EN/03 APPENDIX A.PARAMETERS
- 2267 -
27361 Holder length applied when a groove cutting tool is drawn in animated
simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the holder length applied when a groove cutting
tool is drawn in animated simulation.
Holder length
Tip
Holder
When 0 is set, 50 mm for metric input or 1.9685 inch for inch input is
assumed.
27362 Holder width applied when a groove cutting tool is drawn in animated
simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the holder width applied when a groove cutting
tool is drawn in animated simulation.
Holder width
Tip
Holder
When 0 is set, 14 mm for metric input or 0.5512 inch for inch input is
assumed.
A.PARAMETERS APPENDIX B-63944EN/03
- 2268 -
#7 #6 #5 #4 #3 #2 #1 #0
27363 BTP
[Input type] Parameter input
[Data type] Bit
# 0 BTP When a round-nose tool is drawn in animated simulation, the tip is:
0: Positioned on the front.
1: Positioned on the rear.
Front Rear
Tip
Holder Holder
27364 Holder length applied when a round-nose tool is drawn in animated
simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the holder length applied when a round-nose tool
is drawn in animated simulation.
Holder length
Tip
Holder
When 0 is set, 50 mm for metric input or 1.9685 inch for inch input is
assumed.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2269 -
27365 Holder width applied when a round-nose tool is drawn in animated
simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the holder width applied when a round-nose tool
is drawn in animated simulation.
Holder width
Tip
Holder
When 0 is set, 14 mm for metric input or 0.5512 inch for inch input is
assumed.
#7 #6 #5 #4 #3 #2 #1 #0
27366 STP
[Input type] Parameter input
[Data type] Bit
# 0 STP When a point nose straight tool is drawn in animated simulation, the
tip is:
0: Positioned on the front.
1: Positioned on the rear.
Front Rear
Tip
Holder Holder
A.PARAMETERS APPENDIX B-63944EN/03
- 2270 -
27367 Cutting edge length applied when a point nose straight tool is drawn in
animated simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the cutting edge length applied when a point nose
straight tool is drawn in animated simulation.
Cutting edge length
Tip
Holder
When 0 is set, 12 mm for metric input or 0.4724 inch for inch input is
assumed.
27368 Holder length applied when a point nose straight tool is drawn in animated
simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the holder length applied when a point nose
straight tool is drawn in animated simulation.
Holder length
Tip
Holder
When 0 is set, 50 mm for metric input or 1.9685 inch for inch input is
assumed.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2271 -
27369 Holder width applied when a point nose straight tool is drawn in animated
simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the holder width applied when a point nose
straight tool is drawn in animated simulation.
Holder width
Tip
Holder
When 0 is set, 14 mm for metric input or 0.5512 inch for inch input is
assumed.
27370 Holder length 2 applied when a point nose straight tool is drawn in animated
simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the holder length 2 applied when a point nose
straight tool is drawn in animated simulation.
Holder length 2
Tip
Holder
A.PARAMETERS APPENDIX B-63944EN/03
- 2272 -
27371 Holder width 2 applied when a point nose straight tool is drawn in animated
simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the holder width 2 applied when a point nose
straight tool is drawn in animated simulation.
Holder width 2
Tip
Holder
Holder width
27372 Length of cut applied when a drill tool is drawn in animated simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the length of cut applied when a drill tool is drawn
in animated simulation.
Length of cut
When 0 is set, 50 mm for metric input or 1.9685 inch for inch input is
assumed.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2273 -
27373 Length of cut applied when a flat end milling cutter is drawn in animated
simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the length of cut applied when a flat end milling
cutter is drawn in animated simulation.
Length of cut
When 0 is set, 50 mm for metric input or 1.9685 inch for inch input is
assumed.
27374 Length of cut applied when a tapping tool is drawn in animated simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the length of cut applied when a tapping tool is
drawn in animated simulation.
Length of cut
When 0 is set, 50 mm for metric input or 1.9685 inch for inch input is
assumed.
A.PARAMETERS APPENDIX B-63944EN/03
- 2274 -
27375 Included angle applied when a chamfering tool is drawn in animated
simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] degree
[Valid data range] 0 to 90
This parameter sets the included angle applied when a a chamfering
tool is drawn in animated simulation.
Included angle
27376 Length of cut applied when a chamfering tool is drawn in animated
simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the length of cut applied when a chamfering tool
is drawn in animated simulation.
Length of cut
When 0 is set, 26 mm for metric input or 1.0236 inch for inch input is
assumed.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2275 -
27377 Cutter length applied when a chamfering tool is drawn in animated
simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the cutter length applied when a chamfering tool is
drawn in animated simulation.
Cutter length
When 0 is set, 50 mm for metric input or 1.9685 inch for inch input is
assumed.
27378 Shank length applied when a chamfering tool is drawn in animated
simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the shank length applied when a chamfering tool
is drawn in animated simulation.
Shank length
When 0 is set, 130 mm for metric input or 5.1181 inch for inch input
is assumed.
A.PARAMETERS APPENDIX B-63944EN/03
- 2276 -
27379 Shank diameter applied when a chamfering tool is drawn in animated
simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the shank diameter applied when a chamfering
tool is drawn in animated simulation.
Shank diameter
When 0 is set, 32 mm for metric input or 1.2598 inch for inch input is
assumed.
27380 Length of cut applied when a ball end mill is drawn in animated simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the length of cut applied when a ball end mill is
drawn in animated simulation.
Length of cut
When 0 is set, 50 mm for metric input or 1.9685 inch for inch input is
assumed.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2277 -
27381 Length of cut applied when a reamer is drawn in animated simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the length of cut applied when a reamer is drawn
in animated simulation.
Length of cut
When 0 is set, 50 mm for metric input or 1.9685 inch for inch input is
assumed.
27382 Length of cut applied when a boring tool is drawn in animated simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the length of cut applied when a boring tool is
drawn in animated simulation.
Length of cut
When 0 is set, 50 mm for metric input or 1.9685 inch for inch input is
assumed.
A.PARAMETERS APPENDIX B-63944EN/03
- 2278 -
27383 Length of cut applied when a face milling cutter is drawn in animated
simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the length of cut applied when a face milling
cutter is drawn in animated simulation.
Length of cut
When 0 is set, 63 mm for metric input or 2.4803 inch for inch input is
assumed.
#7 #6 #5 #4 #3 #2 #1 #0
27384 VRP
[Input type] Parameter input
[Data type] Bit
# 0 VRP When a multifunction tool is drawn in animated simulation, the tip is:
0: Positioned on the front.
1: Positioned on the rear.
Front Rear
Tip
Holder Holder
B-63944EN/03 APPENDIX A.PARAMETERS
- 2279 -
27385 Holder length applied when a multifunction tool is drawn in animated
simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the holder length applied when a multifunction
tool is drawn in animated simulation.
Holder length
Tip
Holder
When 0 is set, 50 mm for metric input or 1.9685 inch for inch input is
assumed.
27386 Holder width applied when a multifunction tool is drawn in animated
simulation
[Input type] Parameter input
[Data type] 2-word
[Unit of data] 0.001mm (metric input), 0.0001inch (inch input)
[Valid data range] 0 or larger
This parameter sets the holder width applied when a multifunction
tool is drawn in animated simulation.
Holder width
Tip
Holder
When 0 is set, 14 mm for metric input or 0.5512 inch for inch input is
assumed.
A.PARAMETERS APPENDIX B-63944EN/03
- 2280 -
A.2 DATA TYPE
Parameters are classified by data type as follows:
Data type Valid data range Remarks
Bit
Bit machine group
Bit path
Bit axis
Bit spindle
0 or 1
Byte
Byte machine group
Byte path
Byte axis
Byte spindle
-128 to 127
0 to 255
Some parameters handle
these types of data as
unsigned data.
Word
Word machine group
Word path
Word axis
Word spindle
-32768 to 32767
0 to 65535
Some parameters handle
these types of data as
unsigned data.
2-word
2-word machine group
2-word path
2-word axis
2-word spindle
0 to ±999999999
Some parameters handle
these types of data as
unsigned data.
Real
Real machine group
Real path
Real axis
Real spindle
See the standard
parameter setting
tables.
NOTE
1 Each of the parameters of the bit, bit machine group, bit path, bit axis, and bit
spindle types consists of 8 bits for one data number (parameters with eight different
meanings).
2 For machine group types, parameters corresponding to the maximum number of
machine groups are present, so that independent data can be set for each machine
group.
3 For path types, parameters corresponding to the maximum number of paths are
present, so that independent data can be set for each path.
4 For axis types, parameters corresponding to the maximum number of control axes
are present, so that independent data can be set for each control axis.
5 For spindle types, parameters corresponding to the maximum number of spindles
are present, so that independent data can be set for each spindle axis.
6 The valid data range for each data type indicates a general range. The range varies
according to the parameters. For the valid data range of a specific parameter, see
the explanation of the parameter.
B-63944EN/03 APPENDIX A.PARAMETERS
- 2281 -
A.3 STANDARD PARAMETER SETTING TABLES
This section defines the standard minimum data units and valid data
ranges of the CNC parameters of the real type, real machine group
type, real path type, real axis type, and real spindle type. The data type
and unit of data of each parameter conform to the specifications of
each function.
NOTE
1 Values are rounded up or down to the nearest
multiples of the minimum data unit.
2 A valid data range means data input limits, and
may differ from values representing actual
performance.
3 For information on the ranges of commands to the
CNC, refer to Appendix D, "Range of Command
Value."
(A) Length and angle parameters (type 1)
Unit of data Increment Minimum Valid data range
IS-A 0.01 -999999.99 to +999999.99
IS-B 0.001 -999999.999 to +999999.999
IS-C 0.0001 -99999.9999 to +99999.9999
IS-D 0.00001 -9999.99999 to +9999.99999
mm
deg.
IS-E 0.000001 -999.999999 to +999.999999
IS-A 0.001 -99999.999 to +99999.999
IS-B 0.0001 -99999.9999 to +99999.9999
IS-C 0.00001 -9999.99999 to +9999.99999
IS-D 0.000001 -999.999999 to +999.999999
inch
IS-E 0.0000001 -99.9999999 to +99.9999999
(B) Length and angle parameters (type 2)
Unit of data Increment
system
Minimum
data unit Valid data range
IS-A 0.01 0.00 to +999999.99
IS-B 0.001 0.000 to +999999.999
IS-C 0.0001 0.0000 to +99999.9999
IS-D 0.00001 0.00000 to +9999.99999
mm
deg.
IS-E 0.000001 0.000000 to +999.999999
IS-A 0.001 0.000 to +99999.999
IS-B 0.0001 0.0000 to +99999.9999
IS-C 0.00001 0.00000 to +9999.99999
IS-D 0.000001 0.000000 to +999.999999
inch
IS-E 0.0000001 0.0000000 to +99.9999999
A.PARAMETERS APPENDIX B-63944EN/03
- 2282 -
(C) Velocity and angular velocity parameters
Unit of data Increment
system
Minimum
data unit Valid data range
IS-A 0.01 0.00 to +999000.00
IS-B 0.001 0.000 to +999000.000
IS-C 0.0001 0.0000 to +99999.9999
IS-D 0.00001 0.00000 to +9999.99999
mm/min
degree/min
IS-E 0.000001 0.000000 to +999.999999
IS-A 0.001 0.000 to +96000.000
IS-B 0.0001 0.0000 to +9600.0000
IS-C 0.00001 0.00000 to +4000.00000
IS-D 0.000001 0.000000 to +400.000000
inch/min
IS-E 0.0000001 0.0000000 to +40.0000000
(D)Acceleration and angular acceleration parameters
Unit of data Increment
system
Minimum
data unit Valid data range
IS-A 0.01 0.00 to +999999.99
IS-B 0.001 0.000 to +999999.999
IS-C 0.0001 0.0000 to +99999.9999
IS-D 0.00001 0.00000 to +9999.99999
mm/sec2
deg./sec2
IS-E 0.000001 0.000000 to +999.999999
IS-A 0.001 0.000 to +99999.999
IS-B 0.0001 0.0000 to +99999.9999
IS-C 0.00001 0.00000 to +9999.99999
IS-D 0.000001 0.000000 to +999.999999
inch/sec2
IS-E 0.0000001 0.0000000 to +99.9999999
B-63944EN/03 APPENDIX B.PROGRAM CODE LIST
- 2283 -
B PROGRAM CODE LIST
ISO code EIA code Custom macro
Character name Character Code
(hexadecimal) Character Code
(hexadecimal)
without
custom
macro
with
custom
macro
Usable as file
name
Number 0 0 30 0 20 *
Number 1 1 B1 1 01 *
Number 2 2 B2 2 02 *
Number 3 3 33 3 13 *
Number 4 4 B4 4 04 *
Number 5 5 35 5 15 *
Number 6 6 36 6 16 *
Number 7 7 B7 7 07 *
Number 8 8 B8 8 08 *
Number 9 9 39 9 19 *
Address A A 41 a 61 *
Address B B 42 b 62 *
Address C C C3 c 73 *
Address D D 44 d 64 *
Address E E C5 e 75 *
Address F F C6 f 76 *
Address G G 47 g 67 *
Address H H 48 h 68 *
Address I I C9 i 79 *
Address J J CA j 51 *
Address K K 4B k 52 *
Address L L CC l 43 *
Address M M 4D m 54 *
Address N N 4E n 45 *
Address O O CF o 46 *
Address P P 50 p 57 *
Address Q Q D1 q 58 *
Address R R D2 r 49 *
Address S S 53 s 32 *
Address T T D4 t 23 *
Address U U 55 u 34 *
Address V V 56 v 25 *
Address W W D7 w 26 *
Address X X D8 x 37 *
Address Y Y 59 y 38 *
Address Z Z 5A z 29 *
Delete DEL FF Del 7F
Back space BS 88 BS 2A
Tabulator HT 09 Tab 2E
End of block LF or NL 0A
CR or EOB 80
Carriage return CR 8D
B.PROGRAM CODE LIST APPENDIX B-63944EN/03
- 2284 -
ISO code EIA code Custom macro
Character name Character Code
(hexadecimal) Character Code
(hexadecimal)
without
custom
macro
with
custom
macro
Usable as file
name
Space SP A0 SP 10
Absolute rewind stop
% A5 ER 0B
Control out (start of
comment) ( 28 (2-4-5) 1A
Control in (end of
comment) ) A9 (2-4-7) 4A
Plus sign + 2B + 70 *
Minus sign - 2D - 40 *
Colon (address O) : 3A
Optional block skip / AF / 31
Period (decimal point) . 2E . 6B *
Sharp # A3
Parameter
(No.6012)
Dollar sign $ 24
Ampersand & A6 & 0E
Apostrophe ’ 27
Asterisk * AA
Parameter
(No.6010)
Comma , AC , 3B
Semicolon ; FB
Left angle bracket < 2C
Equal sign = BD Parameter
(No.6011)
Right angle bracket > BE
Question mark ? 3F
Commercial at mark @ C0
Quotation mark “ 22
Left square bracket [ DB Parameter
(No.6013)
Right square bracket ] DD Parameter
(No.6014)
Underscore _ 6F
Parameter
(No.6018) *
Lowercase letter a a E1 *
Lowercase letter b b E2 *
Lowercase letter c c 63 *
Lowercase letter d d E4 *
Lowercase letter e e 65 *
Lowercase letter f f 66 *
Lowercase letter g g E7 *
Lowercase letter h h E8 *
Lowercase letter i i 69 *
Lowercase letter j j 6A *
Lowercase letter k k EB *
Lowercase letter l l 6C *
Lowercase letter m m ED *
Lowercase letter n n EE *
Lowercase letter o o 6F *
Lowercase letter p p F0 *
B-63944EN/03 APPENDIX B.PROGRAM CODE LIST
- 2285 -
ISO code EIA code Custom macro
Character name Character Code
(hexadecimal) Character Code
(hexadecimal)
without
custom
macro
with
custom
macro
Usable as file
name
Lowercase letter q q 71 *
Lowercase letter r r 72 *
Lowercase letter s s F3 *
Lowercase letter t t 74 *
Lowercase letter u u F5 *
Lowercase letter v v F6 *
Lowercase letter w w 77 *
Lowercase letter x x 78 *
Lowercase letter y y F9 *
Lowercase letter z z FA *
NOTE
1 The symbols used in the "Custom macro" column
have the following meanings.
(Space) : The character will be registered in
memory and has a specific meaning. It is
used incorrectly in a statement other than
a comment, an alarm occurs.
: The character will not be registered in
memory and will be ignored.
: The character will be registered in
memory, but will be ignored during
program execution. The character that
has "*" in its "Usable as file name" field
and is used as a file name is not ignored.
: The character will be registered in
memory. If it is used in a statement other
than a comment, an alarm occurs.
: If it is used in a statement other than a
comment, the character will not be
registered in memory. If it is used in a
comment, it will be registered in memory.
2 The symbol used in the column "Usable as file
name" has the following meaning:
* : Capable of being coded between "<" and
">" as a file name.
3 Codes not in this table are ignored if their parity is
correct.
4 Codes with incorrect parity cause the TH alarm.
But they are ignored without generating the TH
alarm when they are in the comment section.
APPENDIX B-63944EN/03
- 2286 -
C. LIST OF FUNCTIONS AND
PROGRAM FORMAT
C LIST OF FUNCTIONS AND PROGRAM
FORMAT
With some functions, the format used for specification on the
machining center system differs from the format used for specification
on the lathe system. Moreover, some functions are used for only one
of the control types for the machining center system and lathe system.
Some functions cannot be added as options depending on the model.
For details of command formats, see the relevant sections or
subsections.
In the list, the following symbols are used:
• For machining center
x : 1st basic axis (X),
y : 2nd basic axis (Y),
z : 3rd basic axis (Z)
• For lathe
x : 1st basic axis (X),
z : 2nd basic axis (Z),
coded using G code system A
• IP_ : presents a combination of arbitrary axis addresses using
X,Y,Z,A,B and C (such as X_ Y_ Z_).
B-63944EN/03 APPENDIX
- 2287 -
C.LIST OF FUNCTIONS AND
PROGRAM FORMAT
(1/11)
Functions Illustration Program format
Positioning
(G00) Start point
IP
G00 IP_ ;
Linear interpolation
(G01)
Start
p
oint
IP
G01 IP_ F_;
Circular interpolation
(G02, G03)
(x, y)
G03
(x, y)
J
R
I
G02
R
I
J
Start point
Start point
• For machining center
G02
G03 X_ Y_
R_
I_ J_ F_ ;
G17
G02
G03 X_ Z_
R_
I_ K_ F_ ;
G18
G02
G03 Y_ Z_
R_
J_ K_ F_ ;
G19
• For lathe
G02
G03
X_ Z_ R
_
I
_
K
_
F_ ;
Helical interpolation
(G02, G03)
(x, y)
(xyz)
z
Start
point
In case of G03 on X-Y plane
G02
G03
X_ Y_
R_
I_ J_ α_ F_ ;
G17
G02
G03
X_ Z_
R_
I_ K_ α_ F_ ;
G18
G02
G03
Y_ Z_
R_
J_ K_ α_ F_ ;
G19
α
: Arbitrary address except the circular
interpolation axis
Involute interpolation
(G02.2, G03.2)
Yp
Pe
0
R
Xp
Ps
Base circle
Po
Start
point
End point
I
J
(In case of X-Y plane)
G02.2
G03.2
Xp_ Yp_ I_ J_ R_ F_ ;
G17
G02.2
G03.2
Zp_Xp_ K_ I_ R_ F_ ;
G18
G02.2
G03.2
Yp_ Zp_ J_ K_ R_ F_ ;
G19
Exponential interpolation
(G02.3, G03.3)
A
(Rotary axis)
X (Linear axis)
∆
X
∆
A
Relationship between X-axis and A-axis
Positive rotation
G02.3 X_ Y_ Z_ I_ J_ K_ R_ F_ Q_;
Negative rotation
G03.3 X_ Y_ Z_ I_ J_ K_ R_ F_ Q_;
APPENDIX B-63944EN/03
- 2288 -
C. LIST OF FUNCTIONS AND
PROGRAM FORMAT
(2/11)
Functions Illustration Program format
Three-dimensional circular
interpolation
(G02.4, G03.4)
X
Y
Z
Start
point
Intermediate point
(X1,Y1,Z1)
End point (X2,Y2,Z2)
G02.4 XX1 YY1 ZZ1 αα1 ββ1 ;
First block (mid-point of the arc)
X
X2 YY2 ZZ2 αα2 ββ2 ;
Second block (end point of the
arc)
α, β : Arbitrary axes other than the
3-dimensional circular interpolation axis
(up to two axes)
G03.4 can also be specified instead of G02.4.
Dwell
(G04) G04 X_ ;
P_
AI contour control
(G05)
G05 P10000 ; AI contour control start
G05 P0 ; AI contour control end
AI contour control
(G05.1)
G05.1 Q1 ; AI contour control mode on
G05.1 Q0 ; AI contour control mode off
Nano smoothing
(G05.1)
G05.1 Q3 IP0 ; Nano smoothing mode on
G05.1 Q0 ; Nano smoothing mode off
Smooth interpolation
(G05.1)
G05.1 Q2 ; Smooth interpolation mode on
G05.1 Q0 ; Smooth interpolation mode off
NURBS interpolation
(G06.2)
G06.2[P_] K_ IP_ [R_] [F_];
NURBS interpolation mode on
P : Rank of NURBS curve
IP : Control point
R : Weight
K : Knot
F : Feedrate
Hypothetical axis interpolation
(G07)
G07 IP0 ; Hypothetical axis setting
G07 IP1 ; Hypothetical axis cancel
Cylindrical interpolation
(G07.1) G07 IP_ r_; Cylindrical interpolation mode
r : Cylinder radius
G07 IP 0; Cylindrical interpolation mode cancel
AI contour control (Advanced
preview control)
(G08)
G08 P1 ; AI contour control mode on
G08 P0 ; AI contour control mode off
Exact stop
(G09)
Speed
Time
In-position check
G09 IP_ ;
G01
G02
G03
B-63944EN/03 APPENDIX
- 2289 -
C.LIST OF FUNCTIONS AND
PROGRAM FORMAT
(3/11)
Functions Illustration Program format
Programmable data input
(G10) • For machining center
Tool compensation memory A
G10 L01 P_ R_ ;
Tool compensation memory B
G10 L10 P_ R_ ; (Geometry offset amount)
G10 L11 P_ R_ ; (Wear offset amount)
Tool compensation memory C
G10 L10 P_ R_ ; (Geometry offset amount/H)
G10 L11 P_ R_ ; (Wear offset amount/H)
G10 L12 P_ R_ ; (Geometry offset amount/D)
G10 L13 P_ R_ ; (Wear offset amount/D)
• For lathe
Geometry offset amount
G10 P_ X_ Z_ R_ Q_ ;
P = 10000 + Geometry offset number
Wear offset amount
G10 P_ X_ Z_ C_ Q_ ;
P = Wear offset number
Tool retract and recover
(G10.6)
IP
Retract Re
p
ositionin
g
Withdrawal
Return
G10.6 IP_ ; Specify the amount of retraction
G10.6 (as a single block containing no other
commands) ;
Cancel the amount of retraction
Polar coordinate interpolation
(G12.1, G13.1)
G12.1 ; Polar coordinate interpolation mode on
G13.1 ; Polar coordinate interpolation cancel
Polar coordinate command
(G15, G16)
Y
p
Xp
Yp
Xp
Local coordinate system
Workpiece coordinate system
G17 G16 Xp_ Yp_ . . . ;
G18 G16 Zp_ Xp_ . . . ;
G19 G16 Yp_ Zp_ . . . ;
G15 ; Cancel
Plane selection
(G17, G18, G19) G17 ; Xp Yp-plane selection
G18 ; Zp Xp-plane selection
G19 ; Yp Zp-plane selection
Inch/metric conversion
(G20, G21) Inch input G20 ;
Metric input G21 ;
Stored stroke check
(G22, 23)
(XYZ)
(IJK)
G22 X_ Y_ Z_ I_ J_ K_ ;
G23 ; Cancel
Reference position return check
(G27) Start point
IP
G27 IP_ ;
APPENDIX B-63944EN/03
- 2290 -
C. LIST OF FUNCTIONS AND
PROGRAM FORMAT
(4/11)
Functions Illustration Program format
Reference position return
(G28)
2nd Reference position return
(G30) Start point
Reference position (G28)
Intermediate point
2nd reference
p
osition
(
G30
)
IP
G28 IP_ ;
G30 IP_ ;
Movement from reference
position
(G29)
Reference position
IP
Intermediate point
G29 IP_ ;
Floating reference position
return
(G30.1)
Start
point
Floating reference position
Intermediate point
IP
G30.1 IP_ ;
Skip function
(G31)
Start
p
oint Ski
p
si
g
nal
IP G31 IP_ F_ ;
Threading
(G33)
• For machining center
G33 IP_ F_ ;
F : Lead
Threading
(G32)
F
• For lathe
Equal lead threading
G32 P_ F_ ;
Tool radius/tool nose radius
compensation, 3-dimensional
cutter compensation
(G38, G39, G40 to G42)
G41
G42
G40
• For machining center
G17
G18
G19
G41
G42 D_ ;
D : Tool compensation number
G40 : Cancel
Tool radius/tool nose radius
compensation
(G40 to G42)
(G38, G39)
• For lathe only
G41
G42
G40 : Cancel
IP ;
3-dimensional cutter
compensation
(G41.2, G42.2)
(G41.3)
Compensatio
n plane
YZ
X
Too l ve c to r
Cutter compensation
amount
Tool center path
(path after
compensation)
Programmed path
(path before compensation)
Cutter compensation vector
Tool side offset
Tool used
Reference
tool
Cutter
compensatio
n vector
Χυττερ χοµπενσατιο
ν α
µ
ουντ
Tool center path
(path after
compensation)
Programmed
path
Tool vector
Leading edge offset
G41.2
G42.2 IP
_
D_ ; Tool side offset
G40 IP_ ; Cancellation of cutter compensation
G41.3 D_ ; Leading edge offset
G40 ; Canceling the leading edge offset
B-63944EN/03 APPENDIX
- 2291 -
C.LIST OF FUNCTIONS AND
PROGRAM FORMAT
(5/11)
Functions Illustration Program format
Normal direction control
(G40.1, G41.1, G42.1)
Too l
Too l
C-axis C-axis
Programmed
path
Normal direction (in
which the tool moves
)
G41.1 ; Normal direction control on : right
G42.1 ; Normal direction control on : left
G40.1 ; Normal direction control cancel
Tool length compensation
(G43, G44, G49)
Z
Compensation
G43
Z_ H_ ;
G44
G43
H_ ;
G44
H : Tool compensation number
G49 : Cancel
Tool length compensation in
tool axis direction
(G43.1)
CB
Z
Y
X
C
B
Tool axis direction
Workpiece
G43.1 H_ ; Tool length compensation in tool
axis direction
H : Compensation number
G49 ; Compensation cancel
Tool center point control
(TYPE1)
(G43.4)
G43.4 IP α β H ;
Tool center point control (TYPE1) start
IP α β ;
IP : In the case of an absolute command, the
coordinate value of the end point of the tool
tip movement
In the case of an incremental command,
the amount of the tool tip movement
α, β :In the case of an absolute command, the
coordinate value of the end point of the
rotation axes
In the case of an incremental command,
the amount of the rotation axis movement
H : Tool compensation number
Tool center point control
(TYPE2)
(G43.5)
G43.5 IP H Q ;
Tool center point control (TYPE2) start
IP I J K ;
IP : In the case of an absolute command, the
coordinate value of the end point of the tool
tip movement
In the case of an incremental command,
the amount of the tool tip movement
I,J,K : Tool axis direction at the block end point
as seen from the programming
coordinate system
H : Tool compensation number
Q : Inclination angle of the tool (in degrees)
Tool offset
(G43.7)
• For lathe only
APPENDIX B-63944EN/03
- 2292 -
C. LIST OF FUNCTIONS AND
PROGRAM FORMAT
(6/11)
Functions Illustration Program format
Tool offset
(G45 to G48)
G 45
G 46
G 47
G 48
Increase
Decrease
Double decrease
Double increase
Offset amount
IP
IP
• For machining center
IP
_
D
_
;
G45
G46
G47
G48
D : Tool offset number
Scaling
(G50, G51)
P1'
P1 P2
P4P3
P2'
P4' P3'
IP
• For machining center
G51 X_ Y_ Z_ P_
I_ J_ K_ ;
P, I, J, K : Scaling magnification
X, Y, Z : Control position of scaling
G50 : Cancel
• For lathe only
Enabled when G code system B/C is used
Programmable mirror image
(G50.1, G51.1)
Mirror
IP
G51.1 IP_ ;
G50.1 ; . . . Cancel
Synchronous, composite, and
superimposed control by
program command
(G50.4, G51.4, G50.5, G51.5,
G50.6, G51.6)
G51.4 P_Q_(L_) ; Start synchronous control (L_
can be omitted.)
G50.4 Q_ ; Cancel synchronous control.
P : Number to identify synchronous master axis
Q : Number to identify synchronous slave axis
L : Parking start command
G51.5 P_Q_ ; Start composite control
G50.5 P_Q_ ; Cancel composite control
P : Number to identify composite axis 1
Q : Number to identify composite axis 2
G51.6 P_Q_ ; Start superimposed control
G50.6 Q_ ; Cancel superimposed control
P : Number to identify superimposed master
axis
Q : Number to identify superimposed slave axis
Coordinate system setting
Maximum spindle speed clamp
(G50)
X
Z
• For lathe only
G50 IP_ ; (Coordinate system setting)
G50 S_ ; (Maximum spindle speed clamp)
Local coordinate system setting
(G52) x
y
Local coordinate
system
Workpiece
coordinate system
IP
G52 IP_ ;
Command in machine
coordinate system
(G53)
G53 IP_ ;
Tool axis direction control
(G53.1)
G53.1 ; Tool axis direction control
B-63944EN/03 APPENDIX
- 2293 -
C.LIST OF FUNCTIONS AND
PROGRAM FORMAT
(7/11)
Functions Illustration Program format
Selection of workpiece
coordinate system
(G54 to G59)
Workpiece coordinate system
Workpiece
origin
offset
IP
Machine coordinate system
G54
:
:IP
_
;
G59
Rotary table dynamic fixture
offset
(G54.2)
X
Y
X
Y
X
Y
F0
F
θ
0
θ
Z
W
Machine coordinate
system origin
W : Workpiece origin offset value
θ
0 : Reference angle
F0 : Reference fixture offset value
θ
: Rotation axis angle
F : Fixture offset value
C
Rotation axis
center
• For machining center
G54.2 P_ ; Fixture offset
P : Reference fixture offset value number
G54.2 P0 ; Offset cancel
Workpiece setting error
compensation
(G54.4)
Z
X
x, y, z
Y
a
bc
x : X-axis direction error
y : Y-axis direction error
z : Z-axis direction error
a : Rotation direction error (about
the X-axis)
b : Rotation direction error (about
the Y-axis)
c : Rotation direction error (about
the Z-axis)
G54.4 P_ ; Workpiece setting error
compensation
P : Workpiece setting error number
G54.4 P0 ; Workpiece setting error
compensation cancel
Single direction positioning
(G60)
IP
G60 IP_ ;
Cutting mode (G64)
Exact stop mode (G61)
Tapping mode (G63)
v
t
G64
G64_ ; Cutting mode
G61_ ; Exact stop mode
G63_ ; Tapping mode
Automatic corner override
(G62) v
G61
t
G62_ ; Automatic corner override
Custom macro
(G65, G66, G66.1, G67)
G65 P_L_ ; O_ ;
M99 ;
Macro
One-shot call
G65 P_ L_ <Argument assignment> ;
P : Program number
L : Number of repetition
Modal call
G66 P_ L_ <Argument assignment> ;
Call after the move command
G66.1 P_ L_ <Argument assignment> ;
Each block call
G67 ; Cancel
APPENDIX B-63944EN/03
- 2294 -
C. LIST OF FUNCTIONS AND
PROGRAM FORMAT
(8/11)
Functions Illustration Program format
Mirror image for double turret
(G68, G69)
• For lathe only
G68 : Mirror image for double turret
G69 : Mirror image cancel
Coordinate system rotation,
Three-dimensional coordinate
conversion
(G68, G69)
(G68.1, G69.1)
Y
X
(x y)
α
In case of X-Y plane
• For machining center
G68
G17 X_ Y_
G18 Z_ X_
G19 Y_ Z_
R α ;
G69 ; Cancel
• For lathe
G68.1
G17 X_ Y_
G18 Z_ X_
G19 Y_ Z_
R α ;
G69.1 ; Cancel
Tilted working plane command
(G68.2)
G68.2 X_ Y_ Z_ I_ J_ K_ ;
Tilted working plane command
G69 ; Tilted working plane command cancel
X, Y, Z : Feature coordinate system origin
I, J, K : Euler angles for determining the
orientation of the feature coordinate system
Tilted working plane command
with guidance
(G68.2, G68.4)
G68.2/G68.4 P_ X_ Y_ Z_ I_ J_ K_ ;
G68.2 : Tilted working plane command
G68.4 : Tilted working plane command
(incremental multiplexed command)
G69 ; Tilted working plane command cancel
Without P : Euler's angle
P1 : Roll, pitch, yaw
P2 : Three points
P3 : Two vectors
P4 : Projection angle
Angular surface command by
tool axis direction (G68.3)
Xc
Yc
Zc
Feature coordinate system Xc-Yc-Zc
R
G68.3 X_ Y_ Z_ R_ ;
G69 ; Cancel
X,Y, Z : Feature coordinate system origin
R : Feature coordinate system rotation
angle about the Z-axis
B-63944EN/03 APPENDIX
- 2295 -
C.LIST OF FUNCTIONS AND
PROGRAM FORMAT
(9//11)
Functions Illustration Program format
Figure copy
(G72.1, G72.2)
Y
P1
P0
Start point
60°
X
Start point P0
P1
X
Y
Rotational copy
G72.1
X_ Y_
Z_ X_
Y_ Z_
R_ ;
P_ L_
(G17)
(G18)
(G19)
Linear copy
G72.2
I_ J_
K_ I_
J_ K_
;
P_ L_
(G17)
(G18)
(G19)
Canned cycle for drilling
(G73, G74, G80 to G89)
• For machining center
G80 ; Cancel
G73
G74
G76
G81
:
G89
Canned cycle
(G71 to G76)
(G90, G92, G94)
• For lathe only
N G70P Q ;
G71U R ;
G71P Q U W F S T ;
G72W R ;
G72P Q U W F S T ;
G73U W R ;
G73P Q U W F S T ;
G74R ;
G74X(u) Z(w) P Q R F ;
G75R ;
G75X(u) Z(w ) P Q R F ;
G76P Q R ;
G76X(u) Z(w) P Q R F ;
G90
G92 X_ Z_ I_ F_ ;
G94X Z K F ;
Canned grinding cycle (for
grinding machine)
(G71 to G75, G77 to G79)
• For machining center
G75 I_ J_ K_ α_ R_ F_ P_ L_ ;
G77 I_ J_ K_ α_ R_ F_ P_ L_ ;
G78 I_ (J_) K_ α_ F_ P_ L_ ;
G79 I_ J_ K_ α_ R_ F_ P_ L_ ;
α : Arbitrary axis address of the grinding axis
• For lathe
G71 A_ B_ W_ U_ I_ K_ H_ ;
G72 P_ A_ B_ W_ U_ I_ K_ H_ ;
G73 A_ (B_) W_ U_ K_ H_ ;
G74 P_ A_ (B_) W_ U_ K_ H_ ;
X_Y_Z_P_Q_R_F_K_ ;
APPENDIX B-63944EN/03
- 2296 -
C. LIST OF FUNCTIONS AND
PROGRAM FORMAT
(10/11)
Functions Illustration Program format
Absolute/incremental
programming
(G90/G91)
• For machining center
G90_ ; Absolute programming
G91_ ; Incremental programming
:
G90_ G91_ ; Programming in both modes
• For lathe
X Z C : Absolute programming
U W H : Incremental programming
Distinguished by an address specified in
combined use with a G function such as G00
and G01.
Maximum incremental command
value check (G91.1)
G91.1 IP_ ;
IP_ ; Maximum incremental value
Set 0 to cancel maximum incremental value
check.
Change of workpiece
coordinate system (G92)
Maximum spindle speed clamp
(G92)
IP
• For machining center
G92 IP_ ; Change of workpiece coordinate
system
G92 S_ ; Constant surface speed control :
Maximum spindle speed clamp
Workpiece coordinate system
preset
(G92.1)
• For machining center
G92.1 IP 0 ;
Inverse time feed
(G93)
G93 ; Inverse time setting mode
Feed per minute,
Feed per revolution
(G94, G95)
(G98, G99)
mm/min inch/min
mm/rev inch/rev
• For machining center
G94 F_ ; Feed per minute
G95 F_ ; Feed per revolution
• For lathe
G98 F_ ; Feed per minute
G99 F_ ; Feed per revolution
Constant surface speed control
(G96, G97)
Surface speed (m/min or feet/min)
Spindle
speed
N(min-1)
G96 S_ ; Constant surface speed control on
(surface speed specification)
G97 S_ ; Constant surface speed control off
(spindle speed specification)
B-63944EN/03 APPENDIX
- 2297 -
C.LIST OF FUNCTIONS AND
PROGRAM FORMAT
(11/11)
Functions Illustration Program format
Speed display function of a
milling tool with servo motor
(G96.1,G96.2,G96.3,G96.4)
G96.1 P_R_; The next block starts operating
upon completion of spindle
indexing (the SV speed control
mode is off).
G96.2 P_R_; The next block starts operating
without waiting for spindle
indexing to complete.
G96.3 P_; The next block starts operating
after confirming the completion of
spindle indexing (the SV speed
control mode is off).
G96.4 P_; The SV speed control mode is on.
Initial point return / R point
return
(G98, G99) G99
G98 Initial level
R level
Z
p
oint
• For machining center
G98_ ;
G99_ ;
Optional chamfering/corner R K
I
R
• For machining center
,C_ : Chamfering
,R_ : Corner R
Chamfering/corner R
• For lathe only
C±K
X_ P_;
R_
C±K
Z_ P_;
R_
In-feed control (for grinding
machine)
(G160, G161)
• For machining center
G161 R_ ;
G160 ;
Figure program (G01, G02, G03)
D.RANGE OF COMMAND VALUE APPENDIX B-63944EN/03
- 2298 -
D RANGE OF COMMAND VALUE
Linear axis
- In case of millimeter input, feed screw is millimeter
Increment system
IS-A IS-B IS-C IS-D IS-E
Least input increment (mm) 0.01 0.001 0.0001 0.00001 0.000001
Least command increment
(mm) 0.01 0.001 0.0001 0.00001 0.000001
Max. programmable
dimension (mm)
±999,999.99 ±999,999.999 ±99,999.9999 ±9,999.99999 ±999.999999
Max. rapid traverse
(mm/min)*1 999,000 999,000 100,000 10,000 1,000
Feedrate range (mm/min)*1 0.01 to 999,000 0.01 to 999,000 0.0001 to 100,000 0.00001 to 10,000 0.000001 to 1,000
Incremental feed (mm/step)
0.01
0.1
1.0
10.0
0.001
0.01
0.1
1.0
0.0001
0.001
0.01
0.1
0.00001
0.0001
0.001
0.01
0.000001
0.00001
0.0001
0.001
Tool compensation amount
(mm)*2 0 to ±9,999.99 0 to ±9,999.999 0 to ±9,999.9999 0 to ±9,999.99999 0 to ±999.999999
Backlash compensation
amount (pulses)*3 0 to ±9,999 0 to ±9,999 0 to ±9,999 0 to ±9,999 0 to ±9,999
Dwell (sec)*4 0 to 999,999.99 0 to 999,999.999 0 to 99,999.9999 0 to 9,999.99999 0 to 999.999999
- In case of inch input, feed screw is millimeter
Increment system
IS-A IS-B IS-C IS-D IS-E
Least input increment (inch) 0.001 0.0001 0.00001 0.000001 0.0000001
Least command increment
(inch) 0.001 0.0001 0.00001 0.000001 0.0000001
Max. programmable
dimension (inch)
±39,370.078 ±39,370.0787 ±3,937.00787 ±393.700787 ±39.3700787
Max. rapid traverse
(mm/min)*1 999,000 999,000 100,000 10,000 1,000
Feedrate range (inch/min)*1 0.001 to 96,000 0.0001 to 9,600 0.00001 to 4,000 0.000001 to 400 0.0000001 to 40
Incremental feed (inch/step)
0.001
0.01
0.1
1.0
0.0001
0.001
0.01
0.1
0.00001
0.0001
0.001
0.01
0.000001
0.00001
0.0001
0.001
0.0000001
0.000001
0.00001
0.0001
Tool compensation amount
(inch)*2 0 to ±999.999 0 to ±999.9999 0 to ±999.99999 0 to ±999.999999 0 to ±99.9999999
Backlash compensation
amount (pulses)*3 0 to ±9,999 0 to ±9,999 0 to ±9,999 0 to ±9,999 0 to ±9,999
Dwell (sec)*4 0 to 999,999.99 0 to 999,999.999 0 to 99,999.9999 0 to 9,999.99999 0 to 999.999999
B-63944EN/03 APPENDIX D.RANGE OF COMMAND VALUE
- 2299 -
- In case of inch input, feed screw is inch
Increment system
IS-A IS-B IS-C IS-D IS-E
Least input increment (inch) 0.001 0.0001 0.00001 0.000001 0.0000001
Least command increment
(inch) 0.001 0.0001 0.00001 0.000001 0.0000001
Max. programmable
dimension (inch)
±99,999.999 ±99,999.9999 ±9,999.99999 ±999.999999 ±99.9999999
Max. rapid traverse
(inch/min)*1 96,000 9,600 4,000 400 40
Feedrate range (inch/min)*1 0.001 to 96,000 0.0001 to 9,600 0.00001 to 4,000 0.000001 to 400 0.0000001 to 40
Incremental feed (inch/step)
0.001
0.01
0.1
1.0
0.0001
0.001
0.01
0.1
0.00001
0.0001
0.001
0.01
0.000001
0.00001
0.0001
0.001
0.0000001
0.000001
0.00001
0.0001
Tool compensation amount
(inch)*4 0 to ±999.999 0 to ±999.9999 0 to ±999.99999 0 to ±999.999999 0 to ±99.9999999
Backlash compensation
amount (pulses)*3 0 to ±9,999 0 to ±9,999 0 to ±9,999 0 to ±9,999 0 to ±9,999
Dwell (sec)*4 0 to 999,999.99 0 to 999,999.999 0 to 99,999.9999 0 to 9,999.99999 0 to 999.999999
- In case of millimeter input, feed screw is inch
Increment system
IS-A IS-B IS-C IS-D IS-E
Least input increment (mm) 0.01 0.001 0.0001 0.00001 0.000001
Least command increment
(mm) 0.01 0.001 0.0001 0.00001 0.000001
Max. programmable
dimension (mm)
±999,999.99 ±999,999.999 ±99,999.9999 ±9,999.99999 ±999.999999
Max. rapid traverse
(inch/min)*1 96,000 9,600 4,000 400 40
Feedrate range (mm/min)*1 0.01 to 999,000 0.001 to 999,000 0.0001 to 100,000 0.00001 to 10,000 0.000001 to 1,000
Incremental feed (mm/step)
0.01
0.1
1.0
10.0
0.001
0.01
0.1
1.0
0.0001
0.001
0.01
0.1
0.00001
0.0001
0.001
0.01
0.000001
0.00001
0.0001
0.001
Tool compensation amount
(mm)*2 0 to ±9,999.99 0 to ±9,999.999 0 to ±9,999.9999 0 to ±9,999.99999 0 to ±999.999999
Backlash compensation
amount (pulses)*3 0 to ±9,999 0 to ±9,999 0 to ±9,999 0 to ±9,999 0 to ±9,999
Dwell (sec)*4 0 to 999,999.99 0 to 999,999.999 0 to 99,999.9999 0 to 9,999.99999 0 to 999.999999
D.RANGE OF COMMAND VALUE APPENDIX B-63944EN/03
- 2300 -
- Rotary axis
Increment system
IS-A IS-B IS-C IS-D IS-E
Least input increment (deg) 0.01 0.001 0.0001 0.00001 0.000001
Least command increment (deg) 0.01 0.001 0.0001 0.00001 0.000001
Max. programmable dimension
(deg)
±999,999.99 ±999,999.999 ±99,999.9999 ±9,999.99999 ±999.999999
Max. rapid traverse (deg/min)*1 999,000 999,000 100,000 10,000 1,000
Feedrate range (deg/min)*1 0.01 to 999,000 0.001 to 999,000 0.0001 to 100,000 0.00001 to 10,000 0.000001 to 1,000
Incremental feed (deg/step)
0.01
0.1
1.0
10.0
0.001
0.01
0.1
1.0
0.0001
0.001
0.01
0.1
0.00001
0.0001
0.001
0.01
0.000001
0.00001
0.0001
0.001
Tool compensation amount
(deg)*2 0 to ±9,999.99 0 to ±9,999.999 0 to ±9,999.9999 0 to ±9,999.99999 0 to ±999.999999
Backlash compensation amount
(pulses)*3 0 to ±9,999 0 to ±9,999 0 to ±9,999 0 to ±9,999 0 to ±9,999
Dwell (sec)*4 0 to 999,999.99 0 to 999,999.999 0 to 99,999.9999 0 to 9,999.99999 0 to 999.999999
NOTE
*1 The feedrate range shown above are limitations
depending on CNC interpolation capacity. As a
whole system, limitations depending on servo
system must also be considered.
*2 If the mode of input is switched between inch input
and metric input, the maximum compensation value
that can be set at inch input time is (maximum
compensation value) × 1/25.4. If a value
exceeding this value is specified at inch input time,
the compensation value is not converted to a metric
value correctly when the mode of input is switched
to metric input.
*3 The unit is the detection unit.
*4 Depends on the increment system of the axis at in
address X.
B-63944EN/03 APPENDIX E.NOMOGRAPHS
- 2301 -
E NOMOGRAPHS
Appendix E, "NOMOGRAPHS", consists of the following sections:
E.1 INCORRECT THREADED LENGTH...................................2302
E.2 SIMPLE CALCULATION OF INCORRECT THREAD
LENGTH.................................................................................2304
E.3 TOOL PATH AT CORNER ...................................................2306
E.4 RADIUS DIRECTION ERROR AT CIRCLE CUTTING .....2309
E.NOMOGRAPHS APPENDIX B-63944EN/03
- 2302 -
E.1 INCORRECT THREADED LENGTH
The leads of a thread are generally incorrect in δ1 and δ2, as shown in
Fig. E.1 (a), due to automatic acceleration and deceleration.
Thus distance allowances must be made to the extent of δ1 and δ2 in
the program.
δ
2δ1
Fig. E.1 (a) Incorrect thread position
Explanation
- How to determine δ2
δ2=T1V (mm ). . . . (1)
V = 1
60RL
T1 : Time constant of servo system (sec)
V : Threading speed (mm/sec)
R : Spindle speed (min-1)
L : Thread feed (mm)
Time constant T1 (sec) of the servo system: Usually 0.033 s.
- How to determine δ1
δ1 = {t - T1 + T1exp( - t
T1
)} V . . . . . (2)
a = exp( - t
T1
) . . . . . (3)
T1 : Time constant of servo system (sec)
V : Threading speed (mm/sec)
Time constant T1 (sec) of the servo system: Usually 0.033 s.
The lead at the beginning of thread cutting is shorter than the specified
lead L, and the allowable lead error is ∆L. Then as follows.
a=
∆
L
L
When the value of “a” is determined, the time lapse until the thread
accuracy is attained. The time “t” is substituted in (2) to determine δ1:
Constants V and T1 are determined in the same way as for δ2. Since
the calculation of δ1 is rather complex, a nomography is provided on
the following pages.
B-63944EN/03 APPENDIX E.NOMOGRAPHS
- 2303 -
- How to use nomograph
First specify the class and the lead of a thread. The thread accuracy, a,
will be obtained at (1), and depending on the time constant of cutting
feed acceleration/ deceleration, the δ1 value when V = 10mm/s will be
obtained at (2). Then, depending on the speed of thread cutting, δ1 for
speed other than 10mm/s can be obtained at (3).
(Note) See the graph in reference later in the manual for an actual example.
V=40mm/sec V=20mm/sec
(3)
0
δ1a
L
L
(1)
(2)
δ1(V=10mm/sec)
T1
T2
Time constant of servo system
Fig. E.1 (b) Nomograph
NOTE
The equations for δ1, and δ2 are for when the
acceleration/ deceleration time constant for cutting
feed is 0.
E.NOMOGRAPHS APPENDIX B-63944EN/03
- 2304 -
E.2 SIMPLE CALCULATION OF INCORRECT THREAD
LENGTH
δ2δ1
Fig. E.2 (a) Incorrect threaded portion
Explanation
- How to determine δ2
a=
∆
L
L(mm)
R : Spindle speed (min-1)
L : Thread lead (mm)
* When time constant T1 of the servo system is 0.033 s.
- How to determine δ1
δ1= LR
1800*( - 1 - lna) (mm)
=δ2( - 1 - lna)(mm)
R : Spindle speed (min-1)
L : Thread lead (mm)
* When time constant T1 of the servo system is 0.033 s.
Following a is a permited value of thread.
a-1-lna
0.005 4.298
0.01
0.015
0.02
3.605
3.200
2.912
Example
R=350rpm
L=1mm
a=0.01
then
δ2 = 350×1
1800 = 0.194(mm)
δ1 = δ2×3.605 = 0.701(mm)
B-63944EN/03 APPENDIX E.NOMOGRAPHS
- 2305 -
Reference
V : Speed in threading
Servo time constant
50msec
V=10mm/sec
( 0.39in/sec)
V=20mm/sec
(
0.79in/sec
)
V=30mm/sec
( 1.18in/sec)
V=40mm/sec
( 1.57in/sec)
V=2in/sec V=1in/sec
δ1 (V=10mm/sec)
33msec
δ18 (mm)
0.3 (in)
δ1
6420
0.2 0.1
0.007 0.010 0.015 0.020 0.025
Metric thread
JIS class 1
JIS class 2
Unified thread
3.3 3.0 2.5 2.0 1.5 1.2 1.0 0.9 0.7 0. 0.4 0.3 (mm) P Lead
P Lead
a= (
∆
L
L
5.0 4.0 3.5 3.0 2.5 2.0 1.75 1.5 1.25 1.0 0.9 0.8 0.75 (mm)
45678910 121314 161820
6
あ
7 8 9 1012 14161820
Ridge/inch
Ridge/inch
)
JIS 2A
JIS 3A
(Theoretical accuracy)
Fig. E.2 (b) Nomograph for obtaining approach distance δ1
E.NOMOGRAPHS APPENDIX B-63944EN/03
- 2306 -
E.3 TOOL PATH AT CORNER
When servo system delay (by exponential acceleration/deceleration at
cutting or caused by the positioning system when a servo motor is
used) is accompanied by cornering, a slight deviation is produced
between the tool path (tool center path) and the programmed path as
shown in Fig. E.3 (a).
Time constant T1 of the exponential acceleration/deceleration is fixed
to 0.
θ
V1
V2
Tool path
Programmed path
Fig. E.3 (a) Slight deviation between the tool path and the programmed
path
This tool path is determined by the following parameters:
• Feedrate (V1, V2)
• Corner angle (θ)
• Exponential acceleration / deceleration time constant (T1) at
cutting (T1 = 0)
• Presence or absence of buffer register.
The above parameters are used to theoretically analyze the tool path
and above tool path is drawn with the parameter which is set as an
example.
When actually programming, the above items must be considered and
programming must be performed carefully so that the shape of the
workpiece is within the desired precision.
In other words, when the shape of the workpiece is not within the
theoretical precision, the commands of the next block must not be read
until the specified feedrate becomes zero. The dwell function is then
used to stop the machine for the appropriate period.
B-63944EN/03 APPENDIX E.NOMOGRAPHS
- 2307 -
Explanation
- Analysis
The tool path shown in Fig. E.3 (b) is analyzed based on the following
conditions:
• Feedrate is constant at both blocks before and after cornering.
• The controller has a buffer register. (The error differs with the
reading speed of the tape reader, number of characters of the next
block, etc.)
θ
V
VX1
VY1
φ
2
VY2
VX2
φ
2
V
Z
X
0
Fig. E.3 (b) Example of tool path
- Description of conditions and symbols
V
X1 = Vcos φ1
V
Y1 = Vsin φ1
V
X2 = Vcos φ2
V
Y2 = Vsin φ2
V : Feedrate at both blocks before and after cornering
VX1 : X-axis component of feedrate of preceding block
VY1 : Y-axis component of feedrate of preceding block
VX2 : X-axis component of feedrate of following block
VY2 : Y-axis component of feedrate of following block
θ : Corner angle
φ1 : Angle formed by specified path direction of preceding block and
X-axis
φ2 : Angle formed by specified path direction of following block and X-axis
E.NOMOGRAPHS APPENDIX B-63944EN/03
- 2308 -
- Initial value calculation
Y0
X0
V
0
Fig. E.3 (c) Initial value
The initial value when cornering begins, that is, the X and Y
coordinates at the end of command distribution by the controller, is
determined by the feedrate and the positioning system time constant of
the servo motor.
T1 : Exponential acceleration/deceleration time constant. (T=0)
T2 : Time constant of positioning system (Inverse of position loop gain)
- Analysis of corner tool path
The equations below represent the feedrate for the corner section in
X-axis direction and Y-axis direction.
Therefore, the coordinates of the tool path at time t are calculated from
the following equations:
)TT(VX X2110 +=
)TT(VY Y2110 +=
]V)}
T
t
exp(T)
T
t
exp(T{
TT
V
)[VV(V X
X
XX
)t(
X1
2
2
1
1
21
1
12 1+−−−
−
−−=
)}]
T
t
exp(T)
T
t
exp(T{
TT
V
[V X
X
2
2
1
1
21
1
21−−−
−
−=
2
2
2
1
1
21
21
Y
YY
)t(
YV)}
T
t
exp(T)
T
t
exp(T{
TT
VV
V+−−−
−
−
=
0
1
0Xdt)t(V)t(X X−= ∫
)tTT(V)}
T
t
exp(T)
T
t
exp(T{
TT
VV
X
XX −+−−−−
−
−
=212
2
2
2
1
2
1
21
12
0
1
0Ydt)t(V)t(Y Y−= ∫
)tTT(V)}
T
t
exp(T)
T
t
exp(T{
TT
VV
Y
YY −+−−−−
−
−
=212
2
2
2
1
2
1
21
12
B-63944EN/03 APPENDIX E.NOMOGRAPHS
- 2309 -
E.4 RADIUS DIRECTION ERROR AT CIRCLE CUTTING
When a servo motor is used, the positioning system causes an error
between input commands and output results. Since the tool advances
along the specified segment, an error is not produced in linear
interpolation. In circular interpolation, however, radial errors may be
produced, sepecially for circular cutting at high speeds.
This error can be obtained as follows:
Command path
A
ctual path
r
Y
Z
∆
r
. . . . . (1)
∆r : Maximum radius error (mm)
v : Feedrate (mm/sec)
r : Circle radius (mm)
T1 : Exponential acceleration/deceleration time constantat cutting (sec)
(T=0)
T2 : Time constant of positoning system (sec)
(Inverse of positon loop gain)
α : Feed forward coefficient (%)
In the case of bell-shaped acceleration/deceleration and linear
acceleration/deceleration after cutting feed interpolation, an approximation
of this radius error can be obtained with the following expression:
Linear acceleration/deceleration after cutting feed interpolation
Bell-shaped acceleration/deceleration after cutting feed interpolation
Thus, the radius error in the case of bell-shaped acceleration/deceleration
and linear acceleration/deceleration after interpolation is smaller than in
case of exponential acceleration/deceleration by a factor of 12, excluding
any error caused by a servo loop time constant.
Since the machining radius r (mm) and allowable error ∆r (mm) of
the workpiece is given in actual machining, the allowable limit
feedrate v (mm /sec) is determined by equation (1).
Since the acceleration/deceleration time constant at cutting which is
set by this equipment varies with the machine tool, refer to the manual
issued by the machine tool builder.
r
V
))-(1T(T
2
1
r
2
2
2
2
2
1α∆ +=
r
V
))-(1T
2
1
T
24
1
(r
2
2
2
2
2
1α∆ +=
r
V
))-(1T
2
1
T
48
1
(r
2
2
2
2
2
1α∆ +=
APPENDIX B-63944EN/03
- 2310 -
F. SETTINGS AT POWER-ON,
IN THE CLEAR STATE, OR
IN THE RESET STATE
F SETTINGS AT POWER-ON, IN THE
CLEAR STATE, OR IN THE RESET
STATE
B-63944EN/03 APPENDIX
- 2311 -
F.SETTINGS AT POWER-ON, IN
THE CLEAR STATE, OR IN THE
RESET STATE
Either the clear state or reset state is entered during a reset is set by bit
6 (CLR) of parameter No. 3402 (0: reset state/1: clear state).
The symbols in the figure below have the following meanings.
○ : The setting remains unchanged or the operation continues.
× : The setting is deleted or the operation stops.
Item Power-on Clear state Reset state
Offset ○ ○ ○
Set data ○ ○ ○
Settings
Parameter ○ ○ ○
Program in memory ○ ○ ○
Information of the block
read in advance during
automatic operation
× × ×
N (sequence number) × (Note 7) × (Notes 1, 2, 7) ○ (Note 1, 2)
One-shot G code × × ×
Modal G code
Initial value (Note 3)
G20 and G21 are set to the
state at the previous
power-off.
Initial value (Note 3)
G20 and G21 are not
changed (Note 2).
○ (Note 2 and 6)
F 0 0 ○ (Note 2)
S, T, M × ○ (Note 2) ○ (Note 2)
Various
data
items
K (count specification) × × ×
Coordin
ate Workpiece coordinates 0 (Note 4) ○ ○
Movement × × ×
Dwell × × ×
M, S, T code output × × ×
Tool position
compensation
× See "Tool Position
Compensation at a Reset".
See "Tool Position
Compensation at a Reset".
Tool length compensation
× Depending on the setting of
bit 6 (LVK) of parameter
No. 5003
Depending on the setting of
bit 6 (LVK) of parameter
No. 5003
Tool radius/tool nose
radius compensation
× × ×
Operati
on
during
executi
on
Storing a called
subprogram
× × (Note 5) ×
CNC alarm signal AL "0”(when no alarm cause is
present)
“0” (when no alarm cause
is present)
“0” (when no alarm cause
is present)
Reference position return
completion signal ZPx × ○ (or × for emergency stop) ○(or × for emergency stop)
S, T, B codes × ○ ○
M code × × ×
M, S, T, B strobe signals × × ×
Spindle rotation signal
(S analog signal)
× ○ ○
CNC ready signal MA “1” ○ ○
Servo ready signal SA
“1”
(when a servo alarm does
not occur)
“1”
(when a servo alarm does
not occur)
“1”
(when a servo alarm does
not occur)
Cycle start signal STL × × ×
Output
signals
Feed hold signal SPL × × ×
APPENDIX B-63944EN/03
- 2312 -
F. SETTINGS AT POWER-ON,
IN THE CLEAR STATE, OR
IN THE RESET STATE
Tool position compensation at a reset
○ : Cancelled.
× : Not canceled.
Bit 3 (LVC) of parameter No. 5006 and bit 7 (TGC) of parameter
No. 5003
Compensation method
LVC=0
TGC=0
LVC=1
TGC=0
LVC=0
TGC=1
LVC=1
TGC=1
Wear compensation Tool movement
Geometry compensation
× ○
(Axis movement)
× ○
(Axis movement)
Wear compensation × ○ × ○ Coordinate shift
Geometry compensation × × ○ ○
NOTES
1 When the beginning position is found, the main program number is displayed.
2 If a reset is made during execution of a block, the states of the modal G code and
modal address (such as N, F, S, T, or M) specified in the block are not reflected.
The modal information specified in the previous and preceding blocks is kept.
3 The initial value of the modal G code depends on the following parameters. For
details, refer to the parameter manual (B-63950).
- Parameter G01 (No.3402#0)
- Parameter G18 (No.3402#1)
- Parameter G19 (No.3402#2)
- Parameter G91 (No.3402#3)
- Parameter G23 (No.3402#7)
- Parameters No. 3406 to No. 3409
4 For detection of an absolute position, the value is generated from machine
coordinates and a workpiece origin offset.
5 When a reset is made during execution of a subprogram, a return to the main
program is performed. Execution at a midpoint in the subprogram is impossible.
6 When one of the following two settings, which hold the modal G code in group 1 by
a reset is set:
- Reset state (bit 6 of parameter No. 3402 is 0)
- Clear state (bit 1 of parameter No. 3402 is 1) and
the modal G code in group 1 is held at a time of a reset (bit 1 of parameter No.
3406 is 1),
if a reset is made during execution of one of the following canned cycles, which
cause cycle operation, the mode of the modal G code in group 1 is changed to the
G01 mode.
- G90 : Outer surface/inner surface turning cycle
- G92 : Threading cycle
- G94 : Edge turning cycle
7 When bit 0 (SEK) of parameter No. 11353 is set to 1, sequence number N can be
held even at power-on or in the clear state.
B-63944EN/03 APPENDIX
- 2313 -
G.CHARACTER-TO-CODES
CORRESPONDENCE TABLE
G CHARACTER-TO-CODES
CORRESPONDENCE TABLE
Appendix G, "CHARACTER-TO-CODES CORRESPONDENCE
TABLE", consists of the following sections:
G.1 CHARACTER-TO-CODES CORRESPONDENCE TABLE 2314
G.2 FANUC DOUBLE-BYTE CHARACTER CODE TABLE....2315
APPENDIX B-63944EN/03
- 2314 -
G. CHARACTER-TO-CODES
CORRESPONDENCE
G.1 CHARACTER-TO-CODES CORRESPONDENCE TABLE
Character Code Comment Character Code Comment
A 065 6 054
B 066 7 055
C 067 8 056
D 068 9 057
E 069 032 Space
F 070 ! 033 Exclamation mark
G 071 ” 034 Quotation mark
H 072 # 035 Sharp
I 073 $ 036 Dollar sign
J 074 % 037 Percent
K 075 & 038 Ampersand
L 076 ’ 039 Apostrophe
M 077 ( 040 Left parenthesis
N 078 ) 041 Right parenthesis
O 079 * 042 Asterisk
P 080 + 043 Plus sign
Q 081 , 044 Comma
R 082 - 045 Minus sign
S 083 . 046 Period
T 084 / 047 Slash
U 085 : 058 Colon
V 086 ; 059 Semicolon
W 087 < 060 Left angle bracket
X 088 = 061 Equal sign
Y 089 > 062 Right angle bracket
Z 090 ? 063 Question mark
0 048 @ 064 At mark
1 049 [ 091 Left square bracket
2 050 ] 093 Right square bracket
3 051 ^ 094
4 052 _ 095 Underscore
5 053
B-63944EN/03 APPENDIX
- 2315 -
G.CHARACTER-TO-CODES
CORRESPONDENCE TABLE
G.2 FANUC DOUBLE-BYTE CHARACTER CODE TABLE
APPENDIX B-63944EN/03
- 2316 -
G. CHARACTER-TO-CODES
CORRESPONDENCE
B-63944EN/03 APPENDIX
- 2317 -
G.CHARACTER-TO-CODES
CORRESPONDENCE TABLE
APPENDIX B-63944EN/03
- 2318 -
G. CHARACTER-TO-CODES
CORRESPONDENCE
B-63944EN/03 APPENDIX
- 2319 -
G.CHARACTER-TO-CODES
CORRESPONDENCE TABLE
APPENDIX B-63944EN/03
- 2320 -
G. CHARACTER-TO-CODES
CORRESPONDENCE
B-63944EN/03 APPENDIX H.ALARM LIST
- 2321 -
H ALARM LIST
Appendix H, "ALARM LIST", consists of the following itemss:
(1) Alarms on program and operation (PS alarm)...........................2322
(2) Background edit alarms (BG alarm) .........................................2322
(3) Communication alarms (SR alarm)...........................................2322
(4) Parameter writing alarm (SW alarm) ........................................2361
(5) Servo alarms (SV alarm) ...........................................................2361
(6) Overtravel alarms (OT alarm) ...................................................2368
(7) Memory file alarms (IO alarm) .................................................2369
(8) Alarms requiring power to be turned off (PW alarm) ...............2369
(9) Spindle alarms (SP alarm).........................................................2371
(10) Alarm list (serial spindle)........................................................2374
(11) Overheat alarms (OH alarm) ...................................................2383
(12) Other alarms (DS alarm) .........................................................2384
(13) Malfunction prevention function alarms (IE alarm)................2388
H.ALARM LIST APPENDIX B-63944EN/03
- 2322 -
(1) Alarms on program and operation (PS alarm)
(2) Background edit alarms (BG alarm)
(3) Communication alarms (SR alarm)
Alarm numbers are common to all these alarm types.
Depending on the state, an alarm is displayed as in the following
examples:
PS"alarm number" Example: PS0003
BG"alarm number" Example: BG0085
SR"alarm number" Example: SR0001
Number Message Description
0001 TH ERROR A TH error was detected during reading from an input device.
The read code that caused the TH error and how many
statements it is from the block can be verified in the diagnostics
screen.
0002 TV ERROR An error was detected during the single–block TV error.
The TV check can be suppressed by setting TVC parameter No.
0000#0 to “0”.
0003 TOO MANY DIGIT Data entered with more digits than permitted in the NC
instruction word.
The number of permissible digits varies according to the
function and the word.
0004 INVALID BREAK POINT OF WORDS NC word(s) address + numerical value not in word format. This
alarm is also generated when a custom macro does not contain
a reserved word, or does not conform to the syntax.
0005 NO DATA AFTER ADDRESS NC word(s) address + numerical value not in word format. This
alarm is also generated when a custom macro does not contain
a reserved word, or does not conform to the syntax.
0006 ILLEGAL USE OF MINUS SIGN A minus sign (–) was specified at an NC instruction word or
system variable where no minus signal may be specified.
0007 ILLEGAL USE OF DECIMAL POINT A decimal point (.) was specified at an address where no
decimal point may be specified, or two decimal points were
specified.
0009 IMPROPER NC-ADDRESS An illegal address was specified, or parameter 1020 is not set.
0010 IMPROPER G-CODE An unusable G code is specified.
0011 FEED ZERO ( COMMAND ) The cutting feedrate instructed by an F code has been set to 0.
This alarm is also generated if the F code instructed for the S
code is set extremely small in a rigid tapping instruction as the
tool cannot cut at the programmed lead.
0014 CAN NOT COMMAND G95 A synchronous feed is specified without the option for threading
/ synchronous feed. Modify the program.
0015 TOO MANY SIMULTANEOUS AXES A move command was specified for more axes than can be
controlled by simultaneous axis control.
Either add on the simultaneous axis control extension option, or
divide the number of programmed move axes into two blocks.
0020 OVER TOLERANCE OF RADIUS An arc was specified for which the difference in the radius at the
start and end points exceeds the value set in parameter No.
3410. Check arc center codes I, J and K in the program.
The tool path when parameter No. 3410 is set to a large value is
spiral.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2323 -
Number Message Description
0021 ILLEGAL PLANE SELECT The plane selection instructions G17 to G19 are in error.
Reprogram so that same 3 basic parallel axes are not specified
simultaneously.
This alarm is also generated when an axis that should not be
specified for plane machining is specified, for example, for
circular interpolation or involute interpolation.
To enable programming of 3 or more axes, the helical
interpolation option must be added to each of the relevant axes.
0022 R OR I,J,K COMMAND NOT FOUND The command for circular interpolation lacks arc radius R or
coordinate I, J, or K of the distance between the start point to
the center of the arc.
0025 CIRCLE CUT IN RAPID (F0) F0 (rapid traverse in inverse feed or feed specified by an F code
with 1–digit number) was specified during circular interpolation
(G02, G03) or involute interpolation (G02.2, G03.2).
0027 NO AXES COMMANDED IN G43/G44 No axis is specified in G43 and G44 blocks for the tool length
offset type C.
Offset is not canceled but another axis is offset for the tool
length offset type C.
Multiple axes were specified for the same block when the tool
length compensation type is C.
0028 ILLEGAL PLANE SELECT The plane selection instructions G17 to G19 are in error.
Reprogram so that same 3 basic parallel axes are not specified
simultaneously.
This alarm is also generated when an axis that should not be
specified for plane machining is specified, for example, for
circular interpolation or involute interpolation.
To enable programming of 3 or more axes, the helical
interpolation option must be added to each of the relevant axes.
0029 ILLEGAL OFFSET VALUE Illegal offset No.
0030 ILLEGAL OFFSET NUMBER An illegal offset No. was specified.
This alarm is also generated when the tool shape offset No.
exceeds the maximum number of tool offset sets in the case of
tool offset memory B.
0031 ILLEGAL P COMMAND IN G10 The relevant data input or option could not be found for the L
No. of G10.
No data setting address such as P or R was specified.
An address command not concerned with data setting was
specified. An address varies with the L No.
The sign or decimal point of the specified address is in error, or
the specified address is out of range.
0032 ILLEGAL OFFSET VALUE IN G10 In setting an offset amount by G10 or in writing an offset amount
by system variables, the offset amount was excessive.
0033 NO INTERSECTION AT CUTTER
COMPENSATION
The intersection cannot be obtained by the intersection
calculation in tool radius/tool nose radius compensation. Modify
the program.
0034 NO CIRC ALLOWED IN STUP/EXT
BLK
In tool radius/tool nose radius compensation, a startup or
cancellation is performed in the G02 or G03 mode. Modify the
program.
H.ALARM LIST APPENDIX B-63944EN/03
- 2324 -
Number Message Description
0035 CAN NOT COMMANDED G31 - G31 cannot be specified. This alarm is generated when a G
code (such as for tool radius/tool nose radius compensation)
of group 07 is not canceled.
- A torque limit skip was not specified in a torque limit skip
command (G31P98 or P99). Specify the torque limit skip in the
PMC window or the like. Or, specify the torque limit override
by address Q.
0037 CAN NOT CHANGE PLANE IN
G41/G42
The compensation plane G17/G18/G19 was changed during
cutter or tool-nose radius compensation. Modify the program.
0038 INTERFERENCE IN CIRCULAR
BLOCK
Overcutting will occur in tool radius/tool nose radius
compensation because the arc start point or end point coincides
with the arc center. Modify the program.
0039 CHF/CNR NOT ALLOWED IN
G41,G42
Chamfering or corner R was specified with a start-up, a cancel,
or switching between G41 and G42 in G41 and G42 commands
(tool radius/tool nose radius compensation). The program may
cause overcutting to occur in chamfering or corner R. Modify the
program.
0041 INTERFERENCE IN CUTTER
COMPENSATION
In tool radius/tool nose radius compensation, excessive cutting
may occur. Modify the program.
0042 G45/G48 NOT ALLOWED IN CRC Tool offset (G45 to G48) is commanded in tool radius
compensation or 3-dimensional cutter compensation. Modify the
program.
0043 ILLEGAL T-CODE COMMAND On a system with a DRILL-MATE ATC installed, M06 is not
specified in a block that specifies a T code. Alternatively, a T
code beyond the allowable range is specified.
0044 G27-G30 NOT ALLOWED IN FIXED
CYC
One of G27 to G30 is commanded in canned cycle mode.
Modify the program.
0045 ADDRESS Q NOT FOUND (G73/G83) In a high-speed peck drilling cycle (G73) or peck drilling cycle
(G83), the amount of each-time cutting is not specified by
address Q, or Q0 is specified. Modify the program.
0046 ILLEGAL REFERENCE RETURN
COMMAND
A command for a return to the second, third or fourth reference
position is error. (The address P command is in error.)
Although an option for a return to the third or fourth reference
position was not set, 3 or 4 was specified in address P.
0047 ILLEGAL AXIS SELECT Two or more parallel axes (in parallel with a basic axis) have
been specified upon start-up of 3-dimensional tool
compensation or three-dimensional coordinate conversion.
0048 BASIC 3 AXIS NOT FOUND Start-up of 3-dimensional tool compensation or
three-dimensional coordinate conversion has been attempted,
but the three basic axes used when Xp, Yp, or Zp is omitted are
not set in parameter No. 1022.
0049 ILLEGAL COMMAND(G68,G69) When three-dimensional coordinate conversion (G68 or G69)
was specified, the tool compensation was not canceled. Or,
programs of three-dimensional coordinate conversion (G68,
G69) and tool compensation (G43, G44 or G49) were not
nested. Or, the three-dimensional coordinate conversion was
specified during the tool length compensation and another tool
length compensation was specified.
0050 CHF/CNR NOT ALLOWED IN THRD
BLK
Chamfering or corner R is commanded in the thread cutting
block. Modify the program.
0051 MISSING MOVE AFTER CNR/CHF Improper movement or the move distance was specified in the
block next to the chamfering or corner R block. Modify the
program.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2325 -
Number Message Description
0052 CODE IS NOT G01 AFTER CHF/CNR The block next to the chamfering or corner R block is not G01
(or vertical line). Modify the program.
0053 TOO MANY ADDRESS COMMANDS In the chamfering and corner R commands, two or more of I, J,
K and R are specified.
0054 NO TAPER ALLOWED AFTER
CHF/CNR
A block in which chamfering in the specified angle or the corner
R was specified includes a taper command. Modify the program.
0055 MISSING MOVE VALUE IN CHF/CNR In chamfering or corner R block, the move distance is less than
chamfer or corner R amount. Modify the program.
0056 NO END POINT & ANGLE IN
CHF/CNR
In direct dimension drawing programming, both an end point
and an angle were specified in the block next to the block in
which only an angle was specified (Aa). Modify the program.
0057 NO SOLUTION OF BLOCK END Block end point is not calculated correctly in direct dimension
drawing programming. Modify the program.
0058 END POINT NOT FOUND Block end point is not found in direct dimension drawing
programming. Modify the program.
0060 SEQUENCE NUMBER NOT FOUND [External data input/output]
The specified number could not be found for program number
and sequence number searches.
Although input/output of a pot number of tool data or offset
input was requested, no tool number was input after power on.
The tool data corresponding to the entered tool number could
not be found.
[External workpiece number search]
The program corresponding to the specified workpiece
number could not be found.
[Program restart]
In the program restart sequence number specification, the
specified sequence number could not be found.
0061 P OR Q COMMAND IS NOT IN THE
MULTIPLE REPETIVE CYCLES
BLOCK
Address P or Q is not specified in multiple repetitive cycle (G70,
G71, G72, or G73) command.
0062 THE CUTTING AMOUNT IS ILLEGAL
IN THE ROUGH CUTTING CYCLE
A zero or a negative value was specified in a multiple repetitive
canned rough-cutting cycle (G71 or G72) as the depth of cut.
0063 THE BLOCK OF A SPECIFIED
SEQUENCE NUMBER IS NOT
FOUND
The sequence number specified by addresses P and Q in
multiple repetitive cycle (G70, G71, G72, or G73) command
cannot be searched.
0064 THE FINISHING SHAPE IS NOT A
MONOTONOUS CHANGE(FIRST
AXES)
In a shape program for the multiple repetitive canned
rough-cutting cycle (G71 or G72), the command for the first
plane axis was not a monotonous increase or decrease.
0065 G00/G01 IS NOT IN THE FIRST
BLOCK OF SHAPE PROGRAM
In the first block of the shape program specified by P of the
multiple repetitive canned cycle (G70, G71, G72, or G73), G00
or G01 was not specified.
0066 UNAVAILABLE COMMAND IS IN THE
MULTIPLE REPETIVE CYCLES
BLOCK
An unavailable command was found in a multiple repetitive
canned cycle (G70, G71, G72, or G73) command block.
0067 THE MULTIPLE REPETIVE CYCLES
IS NOT IN THE PART PROGRAM
STORAGE
A multiple repetitive canned cycle (G70, G71, G72, or G73)
command is not registered in a tape memory area.
0069 LAST BLOCK OF SHAPE PROGRAM
IS AN ILLEGAL COMMAND
In a shape program in the multiple repetitive canned cycle (G70,
G71, G72, or G73), a command for the chamfering or corner R
in the last block is terminated in the middle.
0070 NO PROGRAM SPACE IN MEMORY The memory area is insufficient.
Delete any unnecessary programs, then retry.
H.ALARM LIST APPENDIX B-63944EN/03
- 2326 -
Number Message Description
0071 DATA NOT FOUND - The address to be searched was not found.
- The program with specified program number was not found
in program number search.
- In the program restart block number specification, the
specified block number could not be found.
Check the data.
0072 DATA NOT FOUND The number of programs to be stored exceeded 63 (basic), 125
(option), 200 (option), 400 (option) or 1000 (option). Delete
unnecessary programs and execute program registration again.
0073 PROGRAM NUMBER ALREADY IN
USE
The commanded program number has already been used.
Change the program number or delete unnecessary programs
and execute program registration again.
0074 PROGRAM NUMBER ALREADY IN
USE
The program number is other than 1 to 9999. Modify the
program number.
0075 PROTECT An attempt was made to register a program whose number was
protected.
In program matching, the password for the encoded program
was not correct.
An attempt was made to select a program being edited in the
background as the main program.
An attempt was made to call a program being edited in the
background as a subprogram.
0076 PROGRAM NOT FOUND The specified program is not found in the subprogram call,
macro call or graphic copy.
The M, G, T or S codes are called by a P instruction other than
that in an M98, G65, G66, G66.1 or interrupt type custom
macro, and a program is called by a No. 2 auxiliary function
code.
This alarm is also generated when a program is not found by
these calls.
0077 TOO MANY SUB,MACRO NESTING The total number of subprogram and macro calls exceeds the
permissible range.
Another subprogram call was executed during an external
memory subprogram call.
0078 SEQUENCE NUMBER NOT FOUND The specified sequence No. was not found during sequence
number search.
The sequence No. specified as the jump destination in GOTO––
and M99P–– was not found.
0079 PROGRAM NOT MATCH The program in memory does not match the program stored on
tape.
Multiple programs cannot be matched continuously when
parameter No. 2200#3 is set to “1”.
Set parameter No. 2200#3 to “0” before executing a match.
0080 G37 MEASURING POSITION
REACHED SIGNAL IS NOT
PROPERLY INPUT
- For machining center series
When the tool length measurement function (G37) is
performed, a measuring position reached signal goes 1 in front
of the area determined by the ε value specified in parameter
No.6254. Alternatively, the signal does not go 1.
- For lathe
When the automatic tool compensation function (G36, G37) is
used, a measuring position reached signals (XAE1, XAE2)
does not go 1 within the range determined by the ε value
specified in parameters No.6254 and No.6255.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2327 -
Number Message Description
0081 G37 OFFSET NO. UNASSIGNED - For machining center series
The tool length measurement function (G37) is specified
without specifying an H code.
Correct the program.
- For lathe
The automatic tool compensation function (G36, G37) is
specified without specifying an T code.
Correct the program.
0082 G37 SPECIFIED WITH H CODE - For machining center series
The tool length measurement function (G37) is specified
together with an H code in the same block.
Correct the program.
- For lathe
The automatic tool compensation function (G36, G37) is
specified together with an T code in the same block.
Correct the program.
0083 G37 IMPROPER AXIS COMMAND - For machining center series
An error has been found in axis specification of the tool length
measurement function (G37). Alternatively, a move command
is specified as an incremental command.
Correct the program.
- For lathe
An error has been found in axis specification of the automatic
tool compensation function (G36, G37).
Alternatively, a command is specified as an incremental
command.
Correct the program.
0085 OVERRUN ERROR The next character was received from the I/O device connected
to reader/punch interface 1 before it could read a previously
received character.
0086 DR OFF During I/O process by reader/punch interface 1, the data set
ready input signal of the I/O device (DR) was OFF. Possible
causes are an I/O device not turn on, a broken cable, and a
defective printed circuit board.
0087 BUFFER OVERFLOW During a read by reader/punch interface 1, although a read stop
command was issued, more than 10 characters were input. The
I/O device or printed circuit board was defective.
0090 REFERENCE RETURN
INCOMPLETE
1. The reference position return cannot be performed normally
because the reference position return start point is too close
to the reference position or the speed is too slow. Separate
the start point far enough from the reference position, or
specify a sufficiently fast speed for reference position return.
2. An attempt was made to set the zero position for the
absolute position detector by return to the reference position
when it was impossible to set the zero point.
Rotate the motor manually at least one turn, and set the
zero position of the absolute position detector after turning
the CNC and servo amplifier off and then on again.
0091 MANUAL REFERENCE POSITION
RETURN IS NOT PERFORMED IN
FEED HOLD
Manual return to the reference position cannot be performed
when automatic operation is halted. Perform the manual return
to the reference position when automatic operation is stopped or
reset.
0092 ZERO RETURN CHECK (G27)
ERROR
The axis specified in G27 has not returned to zero.
Reprogram so that the axis returns to zero.
H.ALARM LIST APPENDIX B-63944EN/03
- 2328 -
Number Message Description
0094 P TYPE NOT ALLOWED (COORD
CHG)
P type cannot be specified when the program is restarted. (After
the automatic operation was interrupted, the coordinate system
setting operation was performed.) Perform the correct operation
according to the User's manual.
0095 P TYPE NOT ALLOWED (EXT OFS
CHG)
P type cannot be specified when the program is restarted. (After
the automatic operation was interrupted, the external workpiece
offset amount changed.) Perform the correct operation
according to the User's manual.
0096 P TYPE NOT ALLOWED (WRK OFS
CHG)
P type cannot be specified when the program is restarted. (After
the automatic operation was interrupted, the workpiece offset
amount changed.) Perform the correct operation according to
the User's manual.
0097 P TYPE NOT ALLOWED (AUTO
EXEC)
P type cannot be directed when the program is restarted. (After
power ON, after emergency stop or alarms 0094 to 0097 reset,
no automatic operation is performed.) Perform automatic
operation.
0098 G28 FOUND IN SEQUENCE RETURN A command of the program restart was specified without the
reference position return operation after power ON or
emergency stop, and G28 was found during search. Perform the
reference position return.
0099 MDI EXEC NOT ALLOWED AFT.
SEARCH
After completion of search in program restart, a move command
is given with MDI.
0109 FORMAT ERROR IN G08 A value other than 0 or 1 was specified after P in the G08 code,
or no value was specified.
0110 OVERFLOW :INTEGER An integer went out of range during arithmetic calculations.
0111 OVERFLOW :FLOATING A decimal point (floating point number format data) went out of
range during arithmetic calculations.
0112 ZERO DIVIDE An attempt was made to divide by zero in a custom macro.
0113 IMPROPER COMMAND A function which cannot be used in custom macro is
commanded. Modify the program.
0114 ILLEGAL EXPRESSION FORMAT The format used in an expression in a custom macro statement
is in error. The parameter tape format is in error.
0115 VARIABLE NO. OUT OF RANGE A number that cannot be used for a local variable, common
variable, or system variable in a custom macro is specified.
In the EGB axis skip function (G31.8), a non-existent custom
macro variable number is specified. Or, the number of custom
macro variables used to store skip positions is not sufficient.
Alternatively, the header data in high-speed cycle machining is
improper. This alarm is issued in the following cases.
1) The header corresponding to the specified call machining
cycle number is absent.
2) The value of cycle connection information falls outside the
allowable range (0 to 999).
3) The number of data items in the header falls outside the
allowable range (1 to 65535).
4) The storage start data variable number of executable data
falls outside the allowable ranges (#20000 to
#85535/#200000 to #986431/#2000000 to #3999999).
5) The storage end data variable number of executable data
falls outside the allowable ranges
(#85535/#986431/#3999999).
6) The storage start data variable number of executable data
is the same as the variable number used by the header.
0116 WRITE PROTECTED VARIABLE An attempt was made in a custom macro to use on the left side
of an expression a variable that can only be used on the right
side of an expression.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2329 -
Number Message Description
0118 TOO MANY BRACKET NESTING Too many brackets “[ ]” were nested in a custom macro.
The nesting level including function brackets is 5.
0119 ARGUMENT VALUE OUT OF RANGE The value of an argument in a custom macro function is out of
range.
0122 TOO MANY MACRO NESTING Too many macro calls were nested in a custom macro.
0123 ILLEGAL MODE FOR
GOTO/WHILE/DO
A GOTO statement or WHILE–DO statement was found in the
main program in the MDI or DNC mode.
0124 MISSING END STATEMENT The END instruction corresponding to the DO instruction was
missing in a custom macro.
0125 MACRO STATEMENT FORMAT
ERROR
The format used in a macro statement in a custom macro is in
error.
0126 ILLEGAL LOOP NUMBER DO and END Nos. in a custom macro are in error, or exceed the
permissible range (valid range: 1 to 3).
0127 DUPLICATE NC,MACRO
STATEMENT
An NC statement and macro statement were specified in the
same block.
0128 ILLEGAL MACRO SEQUENCE
NUMBER
The specified sequence No. could not be found for sequence
number search.
The sequence No. specified as the jump destination in GOTO--
and M99P-- could not be found.
0129 USE 'G' AS ARGUMENT G is used as an argument in a custom macro call. G can be
specified as an argument only in an every-block call (G66.1).
0130 NC AND PMC AXIS ARE
CONFLICTED
The NC command and the PMC axis control command were
conflicted. Modify the program or ladder.
0136 SPOS AXIS - OTHER AXIS SAME
TIME
The spindle positioning axis and another axis are specified in
the same block.
0137 M-CODE & MOVE CMD IN SAME
BLK.
The spindle positioning axis and another axis are specified in
the same block.
0138 SUPERIMPOSED DATA OVERFLOW The total distribution amount of the CNC and PMC is too large
during superimposed control for PMC axis control.
0139 CANNOT CHANGE PMC CONTROL
AXIS
The PMC axis was selected for the axis for which the PMC axis
is being controlled.
0140 PROGRAM NUMBER ALREADY IN
USE
In the background, an attempt was made to select or delete the
program being selected in the foreground. Perform the correct
operation for the background edition.
0141 CAN NOT COMMAND G51 IN 3-D
OFFSET
G51 (Scaling ON) is commanded in the 3-dimensional tool
compensation mode. Modify the program.
0142 ILLEGAL SCALE RATE The scaling rate is 0 times or 10000 times or more.
Modify the setting of the scaling rate. (G51P_ … or G51I_J_K_
… or parameter (No. 5411 or 5421))
0143 COMMAND DATA OVERFLOW An overflow occurred in the storage length of the CNC internal
data. This alarm is also generated when the result of internal
calculation of scaling, coordinate rotation and cylindrical
interpolation overflows the data storage. It also is generated
during input of the manual intervention amount.
0144 ILLEGAL PLANE SELECTED The coordinate rotation plane and arc or tool radius⋅tool nose
radius compensation plane must be the same. Modify the
program.
0145 ILLEGAL USE OF G12.1/G13.1 The axis No. of plane selection parameter No. 5460 (linear axis)
and No. 5461(axis of rotation) in the polar coordinate
interpolation mode is out of range (1 to number of controlled
axes).
H.ALARM LIST APPENDIX B-63944EN/03
- 2330 -
Number Message Description
0146 ILLEGAL USE OF G-CODE The modal G code group contains an illegal G code in the polar
coordinate interpolation mode or when a mode was canceled.
Only the following G codes are allowed: G40, G50, G69.1
An illegal G code was specified while in the polar coordinate
interpolation mode.
The following C codes are not allowed: G27, G28, G30, G30.1,
G31 to G31.4, G37 to G387.3, G52, G92, G53, G17 to G19,
G81 to G89, G68
In the 01 group, G codes other than G01, G02, G03, G02.2 and
G03.2 cannot be specified.
0148 SETTING ERROR Automatic corner override deceleration rate is out of the settable
range of judgement angle. Modify the parameters (No.1710 to
No.1714).
0149 FORMAT ERROR IN G10L3 In registration (G10L3 to G11) of tool life management data, an
address other than Q1, Q2, P1, and P2 or an unusable address
was specified.
0150 ILLEGAL LIFE GROUP NUMBER The tool group number exceeded the maximum allowable value.
The tool group number (P after specification of G10 L3;) or the
group number given by the tool life management T code in a
machining program.
0151 GROUP NOT FOUND AT LIFE DATA The tool group specified in a machining program is not set in
tool life management data.
0152 OVER MAXIMUM TOOL NUMBER The number of tools registered in one group exceeded the
maximum allowable registration tool number.
0153 T-CODE NOT FOUND In registration of tool life data, a block in which the T code needs
to be specified does not include the T code. Alternatively, in
tool exchange method D, M06 is specified solely. Modify the
program.
0154 NOT USING TOOL IN LIFE GROUP - For the tool management command
H99 or D99 was specified when no tool management data
number is assigned to the spindle position. Modify the
program.
- For the tool life management command
The H99 command, D99 command, or the H/D code set by
parameters No. 13265 and No. 13266 was specified when no
tool belonging to a group is used.
0155 ILLEGAL T-CODE COMMAND In the machining program, the T code that is present in the
block containing M06 does not correspond to the group currently
being used. Modify the program.
0156 P/L COMMAND NOT FOUND The P and L commands are not specified in the beginning of a
program for setting a tool group. Modify the program.
0157 TOO MANY TOOL GROUPS In registration of tool life management data, the group setting
command block counts of P (group number) and L (tool life)
exceeded the maximum group count.
0158 TOOL LIFE VALUE OUT OF RANGE The life value that is being set is too large. Change the setting.
0159 ILLEGAL TOOL LIFE DATA Tool life management data is corrupted for some reason.
Register the tool data in the tool group or the tool data in the
group again by G10L3; or MDI input.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2331 -
Number Message Description
0160 MISMATCH WAITING M-CODE A waiting M-code is in error.
<1> When different M codes are specified for path 1 and path 2
as waiting M codes without a P command.
<2> When the waiting M codes are not identical even though
the P commands are identical
<3> When the waiting M codes are identical and the P
commands are not identical (This occurs when a P
command is specified with binary value.)
<4> When the number lists in the P commands contain a
different number even though the waiting M codes are
identical (This occurs when a P command is specified by
combining path numbers.)
<5> When a waiting M code without a P command (2-path
waiting) and a waiting M code with a P command
(3-or-more-path waiting) were specified at the same time
<6> When a waiting M code without a P command was
specified for 3 or more paths.
0161 ILLEGAL P OF WAITING M-CODE P in a waiting M-code is incorrect.
<1> When address P is negative
<2> When a P value inappropriate for the system configuration
was specified
<3> When a waiting M code without a P command (2-path
waiting) was specified in the system having 3 or more
paths.
0163 ILLEGAL COMMAND IN G68/G69 G68 and G69 are not independently commanded in balance cut.
An illegal value is commanded in a balance cut combination
(address P).
0169 ILLEGAL TOOL GEOMETRY DATA Incorrect tool figure data in interference check. Set correct data,
or select correct tool figure data.
0175 ILLEGAL G07.1 AXIS An axis which cannot perform cylindrical interpolation was
specified. More than one axis was specified in a G07.1 block.
An attempt was made to cancel cylindrical interpolation for an
axis that was not in the cylindrical interpolation mode.
For the cylindrical interpolation axis, set not “0” but one of 5, 6 or
7 (parallel axis specification) to parameter No. 1022 to instruct
the arc with axis of rotation (ROT parameter No. 1006#1 is set
to “1” and parameter No. 1260 is set) ON.
0176 ILLEGAL G-CODE USE(G07.1 MODE) A G code was specified that cannot be specified in the
cylindrical interpolation mode. This alarm also is generated
when an 01 group G code was in the G00 mode or code G00
was instructed.
Cancel the cylindrical interpolation mode before instructing code
G00.
H.ALARM LIST APPENDIX B-63944EN/03
- 2332 -
Number Message Description
0178 ILLEGAL COMMAND G05 The settings of bits 4 to 6 of parameter No.7501 are invalid or
G05 was specified in any of the following mode.
- Hypothetical axis interpolation (G07)
- Cylindrical interpolation (G07.1)
- Polar coordinate interpolation (G12.1)
- Polar coordinates command (G16)
- Spindle speed fluctuation detection (G26)
- Tool radius ⋅ tool nose radius compensation (G41/G42)
- Normal direction control (G41.1/G42.1)
- Scaling (G51)
- Programmable mirror image (G51.1)
- Coordinate system rotation (G68)
- Canned cycle (G81 to G89)
- Constant surface speed control (G96)
- Macro interruption(M96)
0179 PARAM. (NO.7510) SETTING ERROR The number of controlled axes set by the parameter No. 7510
exceeds the maximum number. Modify the parameter setting
value.
The distribution of high-speed cycle machining stopped.
0190 ILLEGAL AXIS SELECTED (G96) An illegal value was specified in P in a G96 block or parameter
No. 5844.
0194 SPINDLE COMMAND IN
SYNCHRO-MODE
A Cs contour control mode, spindle positioning command, or
rigid tapping mode was specified during the spindle
synchronous control mode or simple spindle synchronous
control mode.
0197 C-AXIS COMMANDED IN SPINDLE
MODE
The program specified a movement along the Cs-axis when the
Cs contour control switching signal was off.
0199 MACRO WORD UNDEFINED Undefined macro word was used. Modify the custom macro.
0200 ILLEGAL S CODE COMMAND In the rigid tap, an S value was out of range or was not
specified. The parameter (Nos. 5241 to 5243) setting is an S
value which can be specified for the rigid tap.
Correct the parameters or modify the program.
0201 FEEDRATE NOT FOUND IN RIGID
TAP
The command F code for a cutting feedrate is a zero.
If the value of F command is much smaller than that of the S
command, when a rigid tap command is specified, this alarm is
generated. This is because cutting is not possible by the lead
specified by the program.
0202 POSITION LSI OVERFLOW In the rigid tap, spindle distribution value is too large. (System
error)
0203 PROGRAM MISS AT RIGID TAPPING In the rigid tap, position for a rigid M code (M29) or an S
command is incorrect. Modify the program.
0204 ILLEGAL AXIS OPERATION In the rigid tap, an axis movement is specified between the rigid
M code (M29) block and G84 (or G74) block. Modify the
program.
0205 RIGID MODE DI SIGNAL OFF Although a rigid M code (M29) is specified in rigid tapping, the
rigid mode DI signal (DGN G061.0) is not ON during execution
of the G84 (or G74) block. Check the PMC ladder diagram to
find the reason why the DI signal is not turned on.
0206 CAN NOT CHANGE PLANE (RIGID
TAP)
Plane changeover was instructed in the rigid mode. Modify the
program.
0207 RIGID DATA MISMATCH The specified distance was too short or too long in rigid tapping.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2333 -
Number Message Description
0210 CAN NOT COMMAND M198/M99 1 The execution of an M198 or M99 command was attempted
during scheduled operation. Alternatively, the execution of an
M198 command was attempted during DNC operation. Modify
the program.
2 The execution of an M99 command was attempted by an
interrupt macro during pocket machining in a multiple
repetitive canned cycle.
0212 ILLEGAL PLANE SELECT The direct drawing dimensions programming is commanded for
the plane other than the Z-X plane. Correct the program.
0213 ILLEGAL COMMAND IN
SYNCHRO-MODE
In feed axis synchronization control, the following errors
occurred during the synchronous operation.
1) The program issued the move command to the slave axis.
2) The program issued the manual operation to the slave axis.
3) The program issued the automatic reference position return
command without specifying the manual reference position
return after the power was turned on.
0214 ILLEGAL COMMAND IN
SYNCHRO-MODE
Coordinate system is set or tool compensation of the shift type
is executed in the synchronous control. Correct the program.
0217 DUPLICATE G51.2(COMMANDS) G51.2 is further commanded in the G51.2 mode. Modify the
program.
0218 NOT FOUND P/Q COMMAND P or Q is not commanded in the G51.2 block, or the command
value is out of the range. Modify the program. For a polygon
turning between spindles, more information as to why this alarm
occurred is indicated in DGN No. 471.
0219 COMMAND G51.2/G50.2
INDEPENDENTLY
G51.2 and 50.2 were specified in the same block for other
commands. Modify the program in another block.
0220 ILLEGAL COMMAND IN
SYNCHR-MODE
In the synchronous operation, movement is commanded by the
NC program or PMC axis control interface for the synchronous
axis. Modify the program or check the PMC ladder.
0221 ILLEGAL COMMAND IN
SYNCHR-MODE
Polygon machining synchronous operation and axis control or
balance cutting are executed at a time. Modify the program.
0222 DNC OP. NOT ALLOWED IN BG-EDIT Input and output are executed at a time in the background
edition. Execute a correct operation.
0224 ZERO RETURN NOT FINISHED A reference return has not been performed before the start of
automatic operation.
(Only when bit 0 (ZRNx) of parameter No. 1005 is 0)
Perform a reference position return.
0230 R CODE NOT FOUND Cut depth R is not specified in the block including G161.
Alternatively, the value specified for R is negative.
Modify the program.
0231 ILLEGAL FORMAT IN G10 L52 Errors occurred in the specified format at the
programmable-parameter input.
0232 TOO MANY HELICAL AXIS
COMMAND
Three or more axes were specified as helical axes in the helical
interpolation mode. Five or more axes were specified as helical
axes in the helical interpolation B mode.
0233 DEVICE BUSY When an attempt was made to use a unit such as that
connected via the RS-232-C interface, other users were using it.
0241 ILLEGAL FORMAT IN G02.2/G03.2 The end point of an involute curve on the currently selected
plane, or the center coordinate instruction I, J or K of the
corresponding basic circle, or basic circle radius R was not
specified.
H.ALARM LIST APPENDIX B-63944EN/03
- 2334 -
Number Message Description
0242 ILLEGAL COMMAND IN G02.2/G03.2 An illegal value was specified in the involute curve.
The coordinate instruction I, J or K of the basic circle on the
currently selected plane or the basic circle radius R is “0”, or the
start and end points are not inside the basic circle.
0243 OVER TOLERANCE OF END POINT The end point is not positioned on the involute curve that
passes through the start point, and this error exceeds the
permissible error limit (parameter No. 2510).
0245 T-CODE NOT ALLOWED IN THIS
BLOCK
One of the G codes, G50, G10, and G04, which cannot be
specified in the same block as a T code, was specified with a T
code.
0247 THE MISTAKE IS FOUND IN THE
OUTPUT CODE OF DATA.
When an encrypted program is output, EIA is set for the output
code. Specify ISO.
0250 TOOL CHANGE ILLEGAL Z AXIS
COMMAND
A Z-axis move command was performed in the same block for
M06 command.
0251 TOOL CHANGE ILLEGAL T
COMMAND
An unusable T code was specified in M06Txx.
0253 G05 CAN NOT BE COMMANDED A binary operation was specified during advanced preview
control mode.
0300 ILLEGAL COMMAND IN SCALING An illegal G code was specified during scaling. Modify the
program. For the T system, one of the following functions is
specified during scaling, this alarm is generated.
- finishing cycle (G70 or G72)
- outer surface rough-cutting cycle (G71 or G73)
- end side rough-cutting cycle (G72 or G74)
- closed loop cutting cycle (G73 or G75)
- end side cutting-off cycle (G74 or G76)
- outer surface or inner surface cutting-off cycle (G75 or G77)
- multiple repetitive threading cycle (G76 or G78)
- face drill cycle (G83 or G83)
- face tap cycle (G84 or G84)
- face boring cycle (G85 or G85)
- side drill cycle (G87 or G87)
- side tap cycle (G88 or G88)
- side boring cycle (G89 or G89)
- outer surface turning cycle or inner surface boring cycle (G77
or G20)
- threading cycle (G78 or G21)
- end side turning cycle (G79 or G24)
(Specify G codes for systems B and C in that order.)
0301 RESETTING OF REFERENCE
RETURN IS INHIBITED
Although parameter No. 1012#0 (IDGx) was set to 1 to inhibit
the reference position from being set again for a return to the
reference position without a dog, an attempt was made to
perform a manual return to the reference position.
0302 SETTING THE REFERENCE
POSITION WITHOUT DOG IS NOT
PERFORMED
The reference position could not be set for a return to the
reference position without a dog. Possible causes are:
- The axis was not moved in the direction of a return to the
reference position for jog feeding.
- The axis was moved in the direction opposite to the direction
of a manual return to the reference position.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2335 -
Number Message Description
0303 REFERENCE POSITION RETURN IS
NOT PERFORMED
When the setting of a reference position at any position was
possible in Cs contour control (parameter CRF (No. 3700#0) =
1), a G00 command was issued for the Cs contour axis without
a return to the reference position after the serial spindle was
switched to Cs contour control mode.
Perform a reference position return with a G28 command before
issuing a G00 command.
0304 G28 IS COMMANDED WITHOUT
ZERO RETURN
Although a reference position was not set, an automatic return
to the reference position (G28) was commanded.
0305 INTERMEDIATE POSITION IS NOT
ASSIGNED
Although a G28 (automatic return to the reference position),
G30 (return to the second, third, or fourth reference position), or
G30/1 (return to the floating reference position) command was
not issued after power-up, G29 (return from the reference
position) was commanded.
0306 MISMATCH AXIS WITH CNR/CHF The correspondence between the moving axis and the I, J, or K
command is incorrect in a block in which chamfering is
specified.
0307 CAN NOT START REFERENCE
RETURN WITH MECHANICAL
STOPPER SETTING
An attempt was made to set a butt-type reference position for an
axis for which to use the function to set a reference position
without a dog.
0308 G72.1 NESTING ERROR G72.1 was specified again during G72.1 rotation copying.
0309 G72.2 NESTING ERROR G72.2 was specified again during G72.2 parallel copying.
0310 FILE NOT FOUND The specified file could not be found during a subprogram or
macro call.
0311 CALLED BY FILE NAME FORMAT
ERROR
An invalid format was specified to call a subprogram or macro
using a file name.
0312 ILLEGAL COMMAND IN DIRECT
DRAWING DIMENSIONS
PROGRAMMING
Direct input of drawing dimensions was commanded in an
invalid format.
An attempt was made to specify an invalid G code during direct
input of drawing dimensions.
Two or more blocks not to be moved exist in consecutive
commands that specify direct input of drawing dimensions.
Although non-use of commas (,) (parameter No. 3405#4 = 1)
was specified for direct input of drawing dimensions, a comma
was specified.
0313 ILLEGAL LEAD COMMAND The variable-lead threading increment specified in address K
exceeds the specified maximum value in variable-lead
threading. Or, a negative lead value was specified.
0314 ILLEGAL SETTING OF POLYGONAL
AXIS
An axis was specified invalidly in polygon turning.
For polygon turning:
A tool rotation axis is not specified.
(Parameter No. 7610)
For polygon turning between spindles:
Valid spindles are not specified.
(Parameter Nos. 7640 to 7643)
- A spindle other than the serial spindle.
- A spindle is not connected.
0315 ILLEGAL NOSE ANGLE COMMAND
IS IN THE THREAD CUTTING CYCLE
An invalid tool tip angle is specified in a multiple repetitive
canned threading cycle (G76).
0316 ILLEGAL CUTTING AMOUNT IS IN
THE THREAD CUTTING CYCLE
An minimum depth of cut higher than the thread height is
specified in a multiple repetitive canned threading cycle (G76).
0317 ILLEGAL THREAD COMMAND IS IN
THE THREAD CUTTING CYCLE
A zero or a negative value is specified in a multiple repetitive
canned threading cycle (G76) as the thread height or the depth
of cut.
H.ALARM LIST APPENDIX B-63944EN/03
- 2336 -
Number Message Description
0318 ILLEGAL RELIEF AMOUNT IS IN THE
DRILLING CYCLE
Although an escape directions is set in a multiple repetitive
canned cutting-off cycle (G74 or G75), a negative value is
specified for ∆d.
0319 THE END POINT COMMAND IS
ILLEGAL IN THE DRILLING CYCLE
Although the ∆i or ∆k travel distance is set to 0 in a multiple
repetitive canned cutting-off cycle (G74 or G75), a value other
than 0 us specified for a U or W.
0320 ILLEGAL MOVEMENT
AMOUNT/CUTTING AMOUNT IS IN
THE DRILLING CYCLE
A negative value is specified in a multiple repetitive canned
cutting-off cycle (G74 or G75) as ∆i or ∆k (travel distance/the
depth of cut).
0321 ILLEGAL REPEATED TIME IS IN THE
PATTERN REPEATING CYCLE
A zero or a negative value is specified in a multiple repetitive
canned closed loop cycle (G73) as a repeated time.
0322 FINISHING SHAPE WHICH OVER OF
STARTING POINT
An invalid shape which is over the cycle starting point is
specified in a shape program for a multiple repetitive canned
rough-cutting cycle (G71 or G72).
0323 THE FIRST BLOCK OF SHAPE
PROGRAM IS A COMMAND OF
TYPE II
Type II is specified in the first block of the shape program
specified by P in a multiple repetitive canned rough-cutting cycle
(G71 or G72). Z (W) command is for G71.
X (U) command is for G72.
0324 THE INTERRUPTION TYPE MACRO
WAS DONE IN THE MULTIPLE
REPETIVE CYCLES
An interruption type macro was issued during the multiple
repetitive canned cycle (G70, G71, G72, or G73).
0325 UNAVAILABLE COMMAND IS IN
SHAPE PROGRAM
An usable command was issued in a shape program for a
multiple repetitive canned cycle (G70, G71, G72, or G73).
0326 LAST BLOCK OF SHAPE PROGRAM
IS A DIRECT DRAWING
DIMENSIONS
In a shape program in the multiple repetitive canned cycle (G70,
G71, G72, or G73), a command for direct input of drawing
dimensions in the last block is terminated in the middle.
0327 MODAL THAT MULTIPLE REPETIVE
CYCLES CANNOT BE DONE
A multiple repetitive canned cycle (G70, G71, G72, or G73) was
commanded in a modal state in which a multiple repetitive
canned cycle could not be commanded.
0328 ILLEGAL WORK POSITION IS IN THE
TOOL NOSE RADIUS
COMPENSATION
The specification for the blank side for a tool nose radius
compensation (G41 or G42) is incorrect in a multiple repetitive
canned cycle (G71 or G72).
0329 THE FINISHING SHAPE IS NOT A
MONOTONOUS CHANGE(SECOND
AXES)
In a shape program for the multiple repetitive canned
rough-cutting cycle (G71 or G72), the command of the second
plane axis was not a monotonous increase or decrease.
0330 ILLEGAL AXIS COMMAND IS IN THE
TURNING CANNED CYCLE
An axis other than the plane is specified n a canned cycle(G90,
G92, or G94).
0331 ILLEGAL AXIS NUMBER IN AX[] An illegal value is specified for an AX[] axis number.
0332 ILLEGAL AXIS ADDRESS IN
AXNUM[]
An illegal value is specified for an AXNUM[] axis address.
0333 TOO MANY SPINDLE COMMANDS Multiple spindle commands could be found in the same block in
using an expansion spindle name.
Only one spindle could be commanded in the same block.
0334 OFFSET IS OUT OF EFFECTIVE
RANGE
An offset data which was out of the effective range was
specified. (malfunction prevention function)
0335 PLURAL M CODE Multiple M codes are commanded simultaneously in a block for
a wait function with peripheral devices by an M code.
0336 TOOL COMPENSATION
COMMANDED MORE TWO AXES
For a tool length compensation C, an attempt was made to
command the offset to other axes without canceling the offset.
Or, for a tool length compensation C, multiple axes are specified
in G43 or G44 block.
0337 EXCESS MAXIMUM INCREMENTAL
VALUE
The command value exceeded the maximum amount of
incremental. (malfunction prevention function)
B-63944EN/03 APPENDIX H.ALARM LIST
- 2337 -
Number Message Description
0338 CHECK SUM ERROR An incorrect value was detected in a check sum.
(malfunction prevention function)
0340 ILLEGAL RESTART(NANO
SMOOTHING)
With manual absolute turned on, an attempt was made to restart
the operation in nano smoothing mode after performing the
manual interaction.
0341 TOO MANY COMMAND BLOCK
(NANO SMOOTHING)
There are more blocks than can be commanded consecutively
in nano smoothing mode.
0342 CUSTOM MACRO INTERRUPT
ENABLE IN NANO SMOOTHING
A custom macro interrupt was enabled in nano smoothing
mode. Or, nano smoothing mode was commanded with a
custom macro interrupt enabled.
0343 ILLEGAL COMMAND IN NANO
SMOOTHING
G43, G44, or G49 was commanded during a nano smoothing.
0344 CANNOT CONTINUE NANO
SMOOTHING
An illegal command or operation by which a nano smoothing
could not be continued was performed.
0345 TOOL CHANGE ILLEGAL Z AXIS
POS
A tool change position on the Z-axis is incorrect.
0346 TOOL CHANGE ILLEGAL TOOL NUM A tool change position is not set.
0347 TOOL CHANGE ILLEGAL COMMAND
IN SAME BLK.
Tool changing is commanded twice or more in the same block.
0348 TOOL CHANGE Z AXIS POS NOT
ESTABLISHED
A tool change spindle on the Z-axis is not set.
0349 TOOL CHANGE SPINDLE NOT STOP A tool change spindle stop is not stopped.
0350 PARAMETER OF THE INDEX OF
THE SYNCHRONOUS CONTROL
AXIS SET ERROR.
An illegal synchronization control axis number (parameter No.
8180) is set.
0351 BECAUSE THE AXIS IS MOVING,
THE SYNC CONTROL IS CAN'T BE
USED.
While the axis being subject to synchronization control was
moving, an attempt was made to start or cancel the
synchronization control by a synchronization control axis
selection signal.
0352 SYNCHRONOUS CONTROL AXIS
COMPOSITION ERROR.
This error occurred when:
1) An attempt was made to perform synchronization control for
the axis during a synchronization, composition, or
superposition.
2) An attempt was made to synchronize a further
great-grandchild for a parent-child-grandchild relation.
3) An attempt was made to operate synchronization control
although a parent-child-grandchild relation was not set.
0353 THE INSTRUCTION WAS DONE FOR
THE AXIS WHICH WAS NOT ABLE
TO MOVE.
This error occurred when:
- For synchronization
1) A move command was issued to the axis for which
parameter No. 8163#7NUMx is set to 1.
2) A move command was issued to the slave axis.
- For composition
1) A move command was issued to the axis for which
parameter No. 8163#7NUMx is set to 1.
2) A move command was issued to the axis for which
parameter No. 8162#7MUMx is set to 1.
0354 THE G28 WAS INSTRUCTED IN
WITH THE REF POS NOT FIXED IN
SYNC MODE
This error occurred when G28 was specified to the master axis
being parking during synchronization control, but an axis
reference position is not set for the slave axis.
0355 PARAMETER OF THE INDEX OF
THE COMPOSITE CONTROL AXIS
SET ERROR.
An illegal composite control axis number (parameter No. 8183)
is specified.
H.ALARM LIST APPENDIX B-63944EN/03
- 2338 -
Number Message Description
0356 BECAUSE THE AXIS IS MOVING,
THE COMP CONTROL IS CAN'T BE
USED.
While the axis being subject to composite control was moving,
an attempt was made to start or cancel the composite control by
a composite control axis selection signal.
0357 COMPOSITE CONTROL AXIS
COMPOSITION ERROR.
This error occurred when an attempt was made to perform
composite control for the axis during a synchronization,
composition, or superposition.
0359 THE G28 WAS INSTRUCTED IN
WITH THE REF POS NOT FIXED IN
COMP MODE
This error occurred when G28 was specified to the composite
axis during composite control, but a reference position is not set
to the other part of the composition.
0360 PARAMETER OF THE INDEX OF
THE SUPERPOS CONTROL AXIS
SET ERROR.
An illegal superposition control axis number (parameter No.
8186) is specified.
0361
BECAUSE THE AXIS IS MOVING,
THE SUPERPOS CONTROL IS
CAN'T BE USED.
While the axis being subject to superposition control was
moving, an attempt was made to start or cancel the
superposition control by a superposition control axis selection
signal.
0362 SUPERPOSITION CONTROL AXIS
COMPOSITION ERROR.
This error occurred when:
1) An attempt was made to perform superposition control for
the axis during a synchronization, composition, or
superposition.
2) An attempt was made to synchronize a further
great-grandchild for a parent-child-grandchild relation.
0363 THE G28 WAS INSTRUCTED IN TO
THE SUPERPOS CONTROL SLAVE
AXIS.
This error occurred when G28 was specified to the
superposition control slave axis during superposition control.
0364 THE G53 WAS INSTRUCTED IN TO
THE SUPERPOS CONTROL SLAVE
AXIS.
This error occurred when G53 was specified to the slave axis
being moved during superposition control.
0365 TOO MANY MAXIMUM SV/SP AXIS
NUMBER
PER PATH
The maximum control axis number or maximum control spindle
number which could be used within a path was exceeded.
(For a loader path, this alarm is generated if the number of axis
per path is set to 5 or greater.)
0366 IMPROPER G-CODE IN TURRET
METHOD
When the turret change tools method was selected (parameter
No. 5040#3 (TCT) = 0), G43, G43.1, G43.4, G43.5, or G43.7
was commanded.
0367 3-D CONV. WAS COMMANDED IN
SYNC MODE AS THE PARAMETER
PKUx(NO.8162#2) IS 0.
A three-dimensional coordinate conversion was commanded
during synchronization control when the parameter PKUx
(No.8162#2) was 0.
0368 OFFSET REMAIN AT OFFSET
COMMAND
When the ATC change tools method was selected (parameter
No. 5040#3 (TCT) = 1) during G43, G43.1, G43.4, or G43.5
mode, G43.7 was commanded. Or, G43, G43.1, G43.4, or
G43.5 was commanded during G43.7 mode.
0369 G31 FORMAT ERROR - No axis is specified or tow or more axes are specified in the
torque limit switch instruction (G31P98/P99).
- The specified torque Q value in the torque limit switch
instruction is out of range. The torque Q range is 1 to 254.
- The high-speed continuous skip option is not present.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2339 -
Number Message Description
0370 G31P/G04Q ERROR 1) The specified address P value for G31 is out of range. The
address P range is 1 to 4 in a multistage skip function.
2) The specified address Q value for G04 is out of range. The
address Q range is 1 to 4 in a multistage skip function.
3) P1-4 for G31, or Q1-4 for G04 was commanded without a
multistage skip function option.
4) <T series > The specified value of address P of G72 or G74
falls outside the range. Address P ranges from 1 to 4 in the
multistage skip function. P1-4 was specified in G72 or G74
even though the multistage skip function option is not
present.
0371 ILLEGAL FORMAT IN G10 OR L50 In a command format for a programmable parameter input, an
attempt was made to change the parameter for an encryption
(No. 3220), key (No. 3221), or protection range (No.3222 or
No.3223) as a "the encryption function for the key and program."
Modify the program.
0372 REFERENCE RETURN
INCOMPLETE
An attempt was made to perform an automatic return to the
reference position on the orthogonal axis before the completion
of a return to the reference position on the angular axis.
However, this attempt failed because a manual return to the
reference position during angular axis control or an automatic
return to the reference position after power-up was not
commanded. First, return to the reference position on the
angular axis, then return to the reference position on the
orthogonal axis.
0373 ILLEGAL HIGH-SPEED SKIP SIGNAL In the skip commands (G31, G31P1 to G31P4) and dwell
commands (G04, G04Q1 to G04Q4), the same high-speed
signal is selected in different paths.
0374 ILLEGAL REGISTRATION OF TOOL
MANAGER(G10)
G10L75 or G10L76 data was registered during the following
data registration:
- From the PMC window.
- From the FOCAS2.
- By G10L75 or G10L76 in another system.
Command G10L75 or G10L76 again after the above operation
is completed.
0375 CAN NOT ANGULAR
CONTROL(SYNC:MIX:OVL)
Angular axis control is disabled for this axis configuration.
1) When some related axes under angular axis control are not
in synchronous control mode or when one angular axis is not
paired with the other angular axis or one Cartesian axis is
not paired with the other Cartesian axis in synchronous
control
2) When some related axes under composite control are not in
composite control mode or when one angular axis is not
paired with the other angular axis or one Cartesian axis is
not paired with the other Cartesian axis in composite control
3) When related axes under angular axis control is switched to
superposition control mode1)
0376 SERIAL DCL: ILLEGAL PARAMETER 1. When Parameter No.1815#1 is set to “1”, parameter
No.2002#3 is set to “0”
2. The absolute-position detection function is enabled.
(Parameter No.1815#5 is set to “1”. )
0387 ILLEGAL RTM DI/DO VAR There is no DI/DO variable that has a specified signal address
(alphabet, number).
H.ALARM LIST APPENDIX B-63944EN/03
- 2340 -
Number Message Description
0389 ILLEGAL RTM SIGNAL BIT Bits other than bits 0 to 7 cannot be specified with a DI/DO
signal.
0391 RTM BRANCH OVER The number of branches supported with real time custom
macros was exceeded.
0392 TOO MANY SENTENCE CONTROL Many reserved words (ZONCE, ZEDGE, ZWHILE, ZDO, ZEND,
G65, M99) for RTM control were used in a real time macro
command.
0393 NO SENTENCE CONTROL In a real time macro command, there is no data to be assigned.
0394 ILLEGAL SENTENCE CONTROL
The matching of reserved words (ZONCE, ZEDGE, ZWHILE,
ZDO, ZEND, G65, M99) for RTM control is incorrect.
0395 ILLEGAL NC WORD CONTROL Control code G65 or M99 for calling a subprogram or returning
from a subprogram is not coded correctly.
0396 ILLEGAL RTM SENTENCE
CONTROL
In other than a real time macro command, a reserved word
(ZONCE, ZEDGE, ZWHILE, ZDO, or ZEND) for RTM control is
used.
0397 RTM BUFFER OVER There is no buffer available for real time macro commands.
Too many blocks read in advance are buffered as triggers used
by real time macro commands.
0398 'ID OVER IN BUFFER In blocks read in advance, there are too many real time macro
commands with the same ID.
0399 'ID EXECUTION IN SAME TIME An attempt was made to execute real time macro commands
with the same ID by using the same NC statement as a trigger.
0400 ONESHOT CMDOVER Too many one-shot real time macro commands are specified.
0401 EXEC CMD NUM OVER IN SAME
TIME
The number of real time macro commands that can be executed
simultaneously was exceeded
0402 ILLEGAL TOKEN FOR RTM A token, variable, or function that is not supported by the real
time custom macro function was detected.
0403 ACCESS TO RTM PROTECT VAR An attempt was made to access a protected variable.
0404 RTM ERROR An error related to a real time macro command occurred.
0406 CODE AREA SHORTAGE The storage size of the real time macro area is insufficient.
0407 DOULE SLASH IN RTM MODE In the compile mode, an attempt was made to set the compile
mode again.
0408 G90 IS NOT PERMITTED The absolute command cannot be specified.
0409 ILLEGAL AXIS NO An invalid axis number is specified.
0410 MIDDLE POINT IS NOT ZERO An intermediate point other than 0 is specified with G28.
0411 SIMULTANEOUSLY AXES OVER The maximum number of axes that can be controlled
simultaneously was exceeded.
0412 ILLEGAL G CODE An unusable G code was used.
0413 ILLEGAL ADDRESS An unusable address was used.
0414 ILLEGAL PMC AXIS NO. An invalid PMC axis number is specified.
0415 GROUP IS IN USE The group to which the specified axis belongs is already in
used.
0416 UNABLE TO USE THE AXIS The specified axis cannot be used.
0417 AXIS IS UNABLE TO MOVE The specified axis is placed in the inoperative state.
0418 ILLEGAL FEED SETTING An incorrect feedrate is set.
0419 ILLEGAL DISTANCE SETTING A travel distance beyond the specifiable range is specified.
0420 CONSTANT NUMBER P A subprogram is specified not by using a constant.
0421 ILLEGAL ARGUMENT G54 With G65, an invalid argument, L, is used.
0422 ILLEGAL ARGUMENT G54 With G65, an invalid argument is used.
0423 NO PMC AXIS CONTROL OPTION The option for PMC axis control is missing.
0424 MULTIPLE AXES IN ONE GROUP Multiple axes are using one group.
0425 ONE AXIS USE MULTIPLE GROU One axis is using multiple groups.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2341 -
Number Message Description
0429 ILLEGAL COMMAND IN G10.6 When retract was started in a threading block, a retract
command had been issued for the long axis direction of
threading.
0430 TOOL LIFE PAIRS ZERO Tool life management group number parameter No.6813 is 0.
0431 ILLEGAL T/R DATA OF TOOL LIFE The arbitrary group number (T) or remaining amount setting (R)
is invalid.
0432 UNAVAILABLE POSTURE IN TPC A command specifying an impossible tool posture was issued in
tool posture control. Review the machine configuration and
command.
0436 ILLEGAL PARAMETER IN WSC An incorrect parameter was specified in compensation of
workpiece placement error.
- The basic three axes are not specified in parameter No.1022.
0437 ILLEGAL COMMAND IN WSC An invalid command related to compensation of workpiece
placement error was specified.
- An illegal G code was specified in the workpiece placement
error compensation mode.
- There is an error in the modal setting used when the
compensation of workpiece placement error is started.
- G54.4 was not specified solely.
- There is not the P command in the block including the G54.4
command. Alternatively, the value following P is out of the
range.
- Compensation of workpiece placement error was specified
redundantly.
0438 ILLEGAL PARAMETER IN TOOL
DIRC CMP
When compensation of workpiece placement error is performed
in a 5-axis cutting machine (compensation in the tool direction
(bit 0 (RCM) of parameter No. 11200 is 0)), an illegal parameter
is set.
- Acc./Dec. before interpolation is disabled. Set parameter No.
1660.
- Acc./Dec. before rapid traverse interpolation is disabled. Set
bit 1 of parameter No. 1401, bit 5 of parameter No. 1950, and
parameter No. 1671.
- The parameters (No.19680 to No.19714) for configuring the
machine are incorrect.
- The axis set by parameters No. 19681 and No. 19686 is not a
rotation axis.
- The basic three axes are not set in parameter No. 1022.
- Bit 6 (TOS) of parameter No. 5006 is set to 0 when tool length
compensation is performed during compensation of workpiece
placement error. Set this parameter to 1.
0439 ILLEGAL COMMAND IN TOOL DIRC
CMP
When compensation of workpiece placement error was
performed in a 5-axis cutting machine (compensation in the tool
direction (bit 0 (RCM) of parameter No. 11200 is 0)), an illegal
command was issued.
- An unspecifiable G code was specified.
- There is an error in the modal setting used during startup.
- An axis not related to 5-axis machining was specified.
- The absolute coordinates of a rotation axis could not be
obtained in the startup block of compensation of workpiece
placement error or tool center point control.
0445 ILLEGAL AXIS OPERATION The positioning command was issued in the speed control
mode. Check the SV speed control mode signal.
H.ALARM LIST APPENDIX B-63944EN/03
- 2342 -
Number Message Description
0446 ILLEGAL COMMAND IN
G96.1/G96.2/G96.3/G96.4
G96.1, G96.2, G96.3, and G96.4 are specified in the block that
includes other commands. Modify the program.
0447 ILLEGAL SETTING DATA The live tool axis is incorrectly set. Check the parameter for
the live tool control function by a servo motor.
0455 ILLEGAL COMMAND IN GRINDING In grinding canned cycles:
1) <M series> The signs of the I, J, and K commands do not
match.
2) <M series/T series > The amount of travel of the grinding
axis is not specified.
0456 ILLEGAL PARAMETER IN GRINDING Parameters related to grinding canned cycles are incorrectly set.
Probable causes are given below.
1) <M series/T series> The axis number of the grinding axis is
incorrectly set (parameters No. 5176 to No. 5179).
2) <M series> The axis number of the dressing axis is
incorrectly set (parameters No. 5180 to No. 5183).
3) <M series/T series> The axis numbers of the cut axis,
grinding axis, and dressing axis (only for the M series)
overlap.
0460 ILLEGAL TORCH AXIS NUMBER The axis number set in parameter No. 5490 (torch control axis)
exceeds the number of control axes.
0461 ILLEGAL SETTING OF ROTATE AXIS
FOR TORCH
The parameter setting (bit 0 of parameter No. 1006 = 1) of the
rotation axis is not applied to the torch turning axis.
1014 ILLEGAL FORMAT OF PROGRAM
NO.
Address O or N is not followed by a number.
1016 EOB NOT FOUND EOB (End of Block) code is missing at the end of a program
input in the MDI mode.
1018 M99 IN MAIN PROGRAM A M99 was commanded during main program when the
parameter AMM (No. 7712#4) = 1 was set.
1059 COMMAND IN BUFFERING MODE The manual intervention compensation request signal MIGET
became “1” when a advanced block was found during automatic
operation.
To input the manual intervention compensation during automatic
operation, a sequence for manipulating the manual intervention
compensation request signal MIGET is required in an M code
instruction without buffering.
1077 PROGRAM IN USE An attempt was made in the foreground to execute a program
being edited in the background.
The currently edited program cannot be executed, so end
editing and restart program execution.
1079 PROGRAM FILE NOT FOUND The program of the specified file No. is not registered in an
external device. (external device subprogram call)
1080 DUPLICATE DEVICE SUB
PROGRAM CALL
Another external device subprogram call was made from a
subprogram after the subprogram called by the external device
subprogram call.
1081 EXT DEVICE SUB PROGRAM CALL
MODE ERROR
The external device subprogram call is not possible in this
mode.
1091 DUPLICATE SUB-CALL WORD More than one subprogram call instruction was specified in the
same block.
1092 DUPLICATE MACRO-CALL WORD More than one macro call instruction was specified in the same
block.
1093 DUPLICATE NC-WORD & M99 An address other than O, N, P or L was specified in the same
block as M99 during the macro modal call state.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2343 -
Number Message Description
1095 TOO MANY TYPE-2 ARGUMENT More than ten sets of I, J and K arguments were specified in the
type–II arguments (A, B, C, I, J, K, I, J, K, ...) for custom
macros.
1096 ILLEGAL VARIABLE NAME An illegal variable name was specified. A code that cannot be
specified as a variable name was specified. [#_OFSxx] does not
match the tool offset memory option configuration.
1097 TOO LONG VARIABLE NAME The specified variable name is too long.
1098 NO VARIABLE NAME The specified variable name cannot be used as it is not
registered.
1099 ILLLEGAL SUFFIX [ ] A suffix was not specified to a variable name that required a
suffix enclosed by [ ].
A suffix was specified to a variable name that did not require a
suffix enclosed by [ ].
The value enclosed by the specified [ ] was out of range.
1100 CANCEL WITHOUT MODAL CALL Call mode cancel (G67) was specified even though macro
continuous–state call mode (G66) was not in effect.
1101 ILLEGAL CNC STATEMENT IRT. An interrupt was made in a state where a custom macro
interrupt containing a move instruction could not be executed.
1115 READ PROTECTED VARIABLE An attempt was made in a custom macro to use on the right
side of an expression a variable that can only be used on the left
side of an expression.
1120 ILLEGAL ARGUMENT FORMAT The specified argument in the argument function (ATAN, POW)
is in error.
1124 MISSING DO STATEMENT The DO instruction corresponding to the END instruction was
missing in a custom macro.
1125 ILLEGAL EXPRESSION FORMAT The description of the expression in a custom macro statement
contains an error.
A parameter program format error.
The screen displayed to enter periodic maintenance data or item
selection menu (machine) data does not match the data type.
1128 SEQUENCE NUMBER OUT OF
RANGE
The jump destination sequence No. in a custom macro
statement GOTO instruction was out of range (valid range: 1 to
99999999).
1131 MISSING OPEN BRACKET The number of left brackets ([) is less than the number of right
brackets (]) in a custom macro statement.
1132 MISSING CLOSE BRACKET The number of right brackets (]) is less than the number of left
brackets ([) in a custom macro statement.
1133 MISSING '=' An equal sign (=) is missing in the arithmetic calculation
instruction in a custom macro statement.
1134 MISSING ',' A delimiter (,) is missing in a custom macro statement.
1137 IF STATEMENT FORMAT ERROR The format used in the IF statement in a custom macro is in
error.
1138 WHILE STATEMENT FORMAT
ERROR
The format used in the WHILE statement in a custom macro is
in error.
1139 SETVN STATEMENT FORMAT
ERROR
The format used in the SETVN statement in a custom macro is
in error.
1141 ILLEGAL CHARACTER IN VAR.
NAME
The SETVN statement in a custom macro contacts a character
that cannot be used in a variable name.
1142 TOO LONG V-NAME (SETVN) The variable name used in a SETVN statement in a custom
macro exceeds 8 characters.
1143 BPRNT/DPRNT STATEMENT
FORMAT ERROR
The format used in the BPRINT statement or DPRINT
statement is in error.
H.ALARM LIST APPENDIX B-63944EN/03
- 2344 -
Number Message Description
1144 G10 FORMAT ERROR The G10 L No. contains no relevant data input or corresponding
option.
Data setting address P or R is not specified.
An address not relating to the data setting is specified. Which
address to specify varies according to the L No.
The sign, decimal point or range of the specified address are in
error.
1145 G10.1 TIME OUT The response to a G10.1 instruction was not received from the
PMC within the specified time limit.
1146 G10.1 FORMAT ERROR The G10.1 instruction format is in error.
1152 G31.9/G31.8 FORMAT ERROR The format of the G31.9 or G31.8 block is erroneous in the
following cases:
- The axis was not specified in the G31.9 or G31.8 block.
- Multiple axes were specified in the G31.9 or G31.8 block.
- The P code was specified in the G31.9 or G31.8 block.
1153 CANNOT USE G31.9 G31.9 cannot be specified in this modal state. This alarm is also
generated when G31.9 is specified when a group 07 G code
(e.g. tool radius compensation) is not canceled.
1160 COMMAND DATA OVERFLOW An overflow occurred in the position data within the CNC.
This alarm is also generated if the target position of a command
exceeds the maximum stroke as a result of calculation such as
coordinate conversion, offset, or introduction of a manual
intervention amount.
1180 ALL PARALLEL AXES IN PARKING All of the axis specified for automatic operation are parked.
1196 ILLEGAL DRILLING AXIS SELECTED An illegal axis was specified for drilling in a canned cycle for
drilling.
If the zero point of the drilling axis is not specified or parallel
axes are specified in a block containing a G code in a canned
cycle, simultaneously specify the parallel axes for the drilling
axis.
1200 PULSCODER INVALID ZERO
RETURN
The grid position could not be calculated during grid reference
position return using the grid system as the one–revolution
signal was not received before leaving the deceleration dog.
This alarm is also generated when the tool does not reach a
feedrate that exceeds the servo error amount preset to
parameter No. 1841 before the deceleration limit switch is left
(deceleration signal *DEC returns to “1”).
1202 NO F COMMAND AT G93 F codes in the inverse time specification mode (G93) are not
handled as modal, and must be specified in individual blocks.
1223 ILLEGAL SPINDLE SELECT 1) An attempt was made to execute an instruction that uses the
spindle although the spindle to be controlled has not been
set correctly.
2) Interpolation type rigid tapping was specified in a path in
which the Cs contour control function is not enabled.
1282 ILLEGAL COMMAND IN 3-D OFFSET An illegal G code was specified in the 3-dimensional tool
compensation mode.
1283 ILLEGAL IJK IN 3-D OFFSET When bit 0 (ONI) of parameter No. 6029 is set to 1, I, J, and K
commands are specified without the decimal point in
three–dimensional tool compensation mode.
1298 ILLEGAL INCH/METRIC
CONVERSION
An error occurred during inch/metric switching.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2345 -
Number Message Description
1300 ILLEGAL ADDRESS The axis No. address was specified even though the parameter
is not an axis–type while loading parameters or pitch error
compensation data from a tape or by entry of the G10
parameter.
Axis No. cannot be specified in pitch error compensation data.
1301 MISSING ADDRESS The axis No. was not specified even though the parameter is an
axis–type while loading parameters or pitch error compensation
data from a tape or by entry of the G10 parameter.
Or, data No. address N, or setting data address P or R are not
specified.
1302 ILLEGAL DATA NUMBER A non–existent data No. was found while loading parameters or
pitch error compensation data from a tape or by entry of the G10
parameter.
An invalid address R value is specified in a pattern program for
each machining purpose on the high–speed high–precision
setting screen.
This alarm is also generated when illegal word values are found.
1303 ILLEGAL AXIS NUMBER An axis No. address exceeding the maximum number of
controlled axes was found while loading parameters from a tape
or by entry of the G10 parameter.
1304 TOO MANY DIGIT Data with too many digits was found while loading parameters or
pitch error compensation data from a tape.
1305 DATA OUT OF RANGE Out–of–range data was found while loading parameters or pitch
error compensation data from a tape.
The values of the data setting addresses corresponding to L
Nos. during data input by G10 was out of range.
This alarm is also generated when NC programming words
contain out–of–range values.
1306 MISSING AXIS NUMBER A parameter which requires an axis to be specified was found
without an axis No. (address A) while loading parameters from a
tape.
1307 ILLEGAL USE OF MINUS SIGN Data with an illegal sign was found while loading parameters or
pitch error compensation data from a tape, or by entry of the
G10 parameter. A sign was specified to an address that does
not support the use of signs.
1308 MISSING DATA An address not followed by a numeric value was found while
loading parameters or pitch error compensation data from a
tape.
1329 ILLEGAL MACHINE GROUP
NUMBER
An machine group No. address exceeding the maximum
number of controlled machine groups was found while loading
parameters from a tape or by entry of the G10 parameter.
1330 ILLEGAL SPINDLE NUMBER An spindle No. address exceeding the maximum number of
controlled spindles was found while loading parameters from a
tape or by entry of the G10 parameter.
1331 ILLEGAL PATH NUMBER An path No. address exceeding the maximum number of
controlled path was found while loading parameters from a tape
or by entry of the G10 parameter.
1332 DATA WRITE LOCK ERROR Could not load data while loading parameters, pitch error
compensation data and work coordinate data from tape.
1333 DATA WRITE ERROR Could not write data while loading data from tape.
1360 PARAMETER OUT OF RANGE
(TLAC)
Illegal parameter setting. (Set value is out of range.)
1361 PARAMTER SETTING ERROR 1
(TLAC)
Illegal parameter setting. (axis of rotation setting)
H.ALARM LIST APPENDIX B-63944EN/03
- 2346 -
Number Message Description
1362 PARAMETER SETTING ERROR 2
(TLAC)
Illegal parameter setting (tool axis setting)
1370 PARAMETER SETTING ERROR
(DM3H-1)
Out–of–range data was set during setting of the
three–dimensional handle feed parameter.
1371 PARAMETER SETTING ERROR
(DM3H-2)
An illegal axis of rotation was set during setting of the
three–dimensional handle feed parameter.
1372 PARAMETAR SETTING ERROR
(DM3H-3)
An illegal master axis was set during setting of the
three–dimensional handle feed parameter.
1373 PARAMETER SETTING ERROR
(DM3H-4)
An illegal parallel axis or twin table was set during setting of the
three–dimensional handle feed parameter.
1470 G40.1 –G42.1 PARAMETER MISS A parameter setting related to normal direction control is illegal.
The axis number of a normal direction controlled axis is set in
parameter No. 5480, but that axis number is in the range of the
number of controlled axes.
The axis set as a normal direction controlled axis is not set as a
rotation axis (ROTx, bit 0 of parameter No. 1006) = 1 and
No.1022=0).
Set the feedrate at which to insert rotation about a normal
direction controlled axis in parameter No. 5481, in the range of 1
to 15000 mm/min.
1508 DUPLICATE M-CODE (INDEX TABLE
REVERSING)
A function to which the same code as this M code is set exists.
(index table indexing)
1509 DUPLICATE M-CODE
(SPOS AXIS ORIENTATION)
A function to which the same code as this M code is set exists.
(spindle positioning, orientation)
1510 DUPLICATE M-CODE (SPOS AXIS
POSITIONING)
A function to which the same code as this M code is set exists.
(spindle positioning, positioning)
1511 DUPLICATE M-CODE (SPOS AXIS
RELEASE)
A function to which the same code as this M code is set exists.
(spindle positioning, mode cancel)
1531 ILLEGAL USE OF DECIMAL POINT
(F-CODE)
When the feedrate instruction contains valid data below the
decimal point, the alarm is set and the F code contains valid
data below the decimal point.
1532 ILLEGAL USE OF DECIMAL POINT
(E-CODE)
When the feedrate instruction contains valid data below the
decimal point, the alarm is set and the E code contains valid
data below the decimal point.
1533 ADDRESS F UNDERFLOW (G95) The feedrate for the hole drilling axis calculated from the F and
S codes is too slow in the feed per single rotation mode (G95).
1534 ADDRESS F OVERFLOW (G95) The feedrate for the hole drilling axis calculated from the F and
S codes is too fast in the feed per single rotation mode (G95).
1535 ADDRESS E UNDERFLOW (G95) The feedrate for the hole drilling axis calculated from the E and
S codes is too slow in the feed per single rotation mode (G95).
1536 ADDRESS E OVERFLOW (G95) The feedrate for the hole drilling axis calculated from the E and
S codes is too fast in the feed per single rotation mode (G95).
1537 ADDRESS F UNDERFLOW
(OVERRIDE)
The speed obtained by applying override to the F instruction is
too slow.
1538 ADDRESS F OVERFLOW
(OVERRIDE)
The speed obtained by applying override to the F instruction is
too fast.
1539 ADDRESS E UNDERFLOW
(OVERRIDE)
The speed obtained by applying override to the E instruction is
too slow.
1540 ADDRESS E OVERFLOW
(OVERRIDE)
The speed obtained by applying override to the E instruction is
too fast.
1541 S-CODE ZERO “0” has been instructed as the S code.
1542 FEED ZERO (E-CODE) “0” has been instructed as the feedrate (E code).
1543 ILLEGAL GEAR SETTING The gear ratio between the spindle and position coder, or the
set position coder number of pulses is illegal in the spindle
positioning function.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2347 -
Number Message Description
1544 S-CODE OVER MAX The S command exceeds the maximum spindle rotation
number.
1548 ILLGAL AXIS MODE The spindle positioning axis/Cs contour control axis was
specified during switching of the controlled axis mode.
1561 ILLEGAL INDEXING ANGLE The specified angle of rotation is not an integer multiple of the
minimum indexing angle.
1564 INDEX TABLE AXIS – OTHER AXIS
SAME TIME
The index table indexing axis and another axis have been
specified in the same block.
1567 INDEX TABLE AXIS DUPLICATE
AXIS COMMAND
Index table indexing was specified during axis movement or on
an axis for which the index table indexing sequence was not
completed.
1580 ENCODE ALARM (PSWD&KEY) When an attempt was made to read a program, the specified
password did not match the password on the tape and the
password on tape was not equal to 0.
When an attempt was made to punch an encrypted tape, the
password was not in the range 0 to 99999999.
The password parameter is No. 2210.
1581 ENCODE ALARM (PARAMETER) When an attempt was made to punch an encrypted tape, the
punch code parameter was set to EIA. Set parameter ISO (No.
0000#1) to “0”. An incorrect instruction was specified for
program encryption or protection.
This alarm is generated if an attempt is made to perform
program editing, deletion, or range-specified punch-out in the
protected range in the lock state. Or, a program outside the
protected range is specified in rage specification punch-out in
the unlock state.
The protected range is defined from the program No. preset by
parameter No. 3222 up to the program No. preset to parameter
No. 3223. When both parameters are set to “0”, the protected
range becomes O9000 to O9999.
1590 TH ERROR A TH error was detected during reading from an input device.
The read code that caused the TH error and how many
statements it is from the block can be verified in the diagnostics
screen.
1591 TV ERROR An error was detected during the single–block TV error.
The TV check can be suppressed by setting TVC parameter No.
0000#0 to “0”.
1592 END OF RECORD The EOR (End of Record) code is specified in the middle of a
block.
This alarm is also generated when the percentage at the end of
the NC program is read.
For the program restart function, this alarm is generated if a
specified block is not found.
1593 EGB PARAMETER SETTING ERROR Error in setting a parameter related to the EGB
(1) The setting of SYN, bit 0 of parameter No. 2011, is not
correct.
(2) The slave axis specified with G81 is not set as a rotation
axis. (ROT, bit 0 of parameter No. 1006)
(3) Number of pulses per rotation (Parameter (No. 7772 or No.
7773) or (No. 7782 or 7783) is not set.)
(4) For a hobbing-machine-compatible command, parameter No.
7710 is not specified.
H.ALARM LIST APPENDIX B-63944EN/03
- 2348 -
Number Message Description
1594 EGB FORMAT ERROR Error in the format of the block of an EGB command
(1) T (number of teeth) is not specified in the G81 block.
(2) In the G81 block, the data specified for one of T, L, P, and Q
is out of its valid range.
(3) n the G81 block, only one of P and Q is specified.
(4) In the G81.5 block, there is no command for the master or
slave axis.
(5) In the G81.5 block, data out of the specified range is
specified for the master or slave axis.
1595 ILL-COMMAND IN EGB MODE During synchronization with the EGB, a command that must not
be issued is issued.
(1) Slave axis command using G27, G28, G29, G30,G30.1,
G33, G53, etc.
(2) Inch/metric conversion command using G20, G21, etc.
1596 EGB OVERFLOW An overflow occurred in the calculation of the synchronization
coefficient.
1597 EGB AUTO PHASE FORMAT ERROR Format error in the G80 or G81 block in EGB automatic phase
synchronization
(1) R is outside the permissible range.
1598 EGB AUTO PHASE PARAMETER
SETTING ERROR
Error in the setting of a parameter related to EGB automatic
phase synchronization
(1) The acceleration/deceleration parameter is not correct.
(2) The automatic phase synchronization parameter is not
correct.
1618 ILLEGAL P-DATA(WHEEL WEAR
COMPENSATION)
There is an error in P-data in compensation selection of grinding
wheel wear compensation. Alternatively, the P command is not
present.
1619 ILLEGAL AXIS(WHEEL WEAR
COMPENSATION)
The compensation axis was switched in the grinding wheel wear
compensation mode or compensation vector hold mode.
Alternatively, parameters No. 5071 and No. 5072, which
determine the axis to be subjected to grinding wheel wear
compensation, are incorrectly set.
1805 ILLEGAL COMMAND [I/O Device]
An attempt was made to specify an illegal command during I/O
processing on an I/O device.
[G30 Zero Return]
The P address Nos. for instructing No. 2 to No. 4 zero return
are each out of the range 2 to 4.
[Single Rotation Dwell]
The specified spindle rotation is “0” when single rotation dwell
is specified.
[3-dimensional tool compensation]
A G code that cannot be specified was specified in the
3-dimensional tool compensation mode.
Scaling instruction G51, skip cutting G31 and automatic tool
length measurement G37 were specified.
1806 DEVICE TYPE MISS MATCH An operation not possible on the I/O device that is currently
selected in the setting was specified.
This alarm is also generated when file rewind is instructed even
though the I/O device is not a FANUC Cassette.
1807 PARAMETER SETTING ERROR An I/O interface option that has not yet been added on was
specified.
The external I/O device and baud rate, stop bit and protocol
selection settings are erroneous.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2349 -
Number Message Description
1808 DEVICE DOUBLE OPENED An attempt was made to open a device that is being accessed.
1809 ILLEGAL COMMAND IN G41/G42 Specified direction tool length compensation parameters are
incorrect.
A move instruction for a axis of rotation was specified in the
specified direction tool length compensation mode.
1820 ILLEGAL DI SIGNAL STATE 1. An each axis workpiece coordinate system preset signal
was turned “1” in the state in which all axes on the path
including the axis on which to perform preset with the each
axis workpiece coordinate system were not stopped or in
which a command was in execution.
2. When an M code for performing preset with an each axis
workpiece coordinate system preset signal was specified,
the each axis workpiece coordinate system preset signal
was not turned “1”.
3. The auxiliary function lock is enabled.
4. When bit 6 (PGS) of parameter No. 3001 was set to 0 (M, S,
T, and B codes are not output in the high speed program
check mode), an M code for turning “1” an each axis
workpiece coordinate system preset signal in the high speed
program check mode was specified.
1823 FRAMING ERROR(1) The stop bit of the character received from the I/O device
connected to reader/punch interface 1 was not detected.
1830 DR OFF(2) The data set ready input signal DR of the I/O device connected
to reader/punch interface 2 turned OFF.
1832 OVERRUN ERROR(2) The next character was received from the I/O device connected
to reader/punch interface 2 before it could read a previously
received character.
1833 FRAMING ERROR(2) The stop bit of the character received from the I/O device
connected to reader/punch interface 2 was not detected.
1834 BUFFER OVERFLOW(2) The NC received more than 10 characters of data from the I/O
device connected to reader/punch interface 2 even though the
NC sent a stop code (DC3) during data reception.
1889 ILLEGAL COMMAND IN G54.3 An illegal command was issued in G54.3 block.
(1) An attempt was made to command G54.3 in a mode in which
it cannot be accepted.
(2) The command was not issued in a single block.
1898 ILLEGAL PARAMETER IN G54.2 An illegal parameter (Nos. 6068 to 6076) was specified for
fixture offset.
1912 V-DEVICE DRIVER ERROR (OPEN) An error occurred during device driver control.
1960 ACCESS ERROR (MEMORY CARD) Illegal memory card accessing
This alarm is also generated during reading when reading is
executed up to the end of the file without detection of the EOR
code.
1961 NOT READY (MEMORY CARD) The memory card is not ready.
1962 CARD FULL (MEMORY CARD) The memory card has run out of space.
1963 CARD PROTECTED (MEMORY
CARD)
The memory card is write–protected.
1964 NOT MOUNTED (MEMORY CARD) The memory card could not be mounted.
1965 DIRECTORY FULL (MEMORY CARD) The file could not be generated in the root directory for the
memory card.
1966 FILE NOT FOUND (MEMORY CARD) The specified file could not be found on the memory card.
1967 FILE PROTECTED (MEMORY CARD) The memory card is write–protected.
H.ALARM LIST APPENDIX B-63944EN/03
- 2350 -
Number Message Description
1968 ILLEGAL FILE NAME (MEMORY
CARD)
Illegal memory card file name
1969 ILLEGAL FORMAT (MEMORY CARD) Check the file name.
1970 ILLEGAL CARD (MEMORY CARD) This memory card cannot be handled.
1971 ERASE ERROR (MEMORY CARD) An error occurred during memory card erase.
1972 BATTERY LOW (MEMORY CARD) The memory card battery is low.
1973 FILE ALREADY EXIST A file having the same name already exists on the memory card.
1990 SPL:ILLEGAL AXIS COMMAND The axis specified by the smooth interpolation (G5.1Q2) is
illegal.
1993 SPL:CAN'T MAKE VECTOR The end point and the 2 previous point are the same in
generation of the 3–dimensional tool compensation vector by
the end point for smooth interpolation.
1995 ILLEGAL PARAMETER IN
G41.2/G42.2
The parameter settings (parameter Nos. 6080 to 6089) for
determining the relationship between the axis of rotation and the
rotation plane are incorrect.
1999 ILLEGAL PARAMETER IN G41.3 The parameter settings (parameter Nos. 6080 to 6089) for
determining the relationship between the axis of rotation and the
rotation plane are incorrect.
2002 NO KNOT COMMAND (NURBS) Knot has not been specified, or a block not related to NURBS
interpolation was specified in the NURBS interpolation mode.
2003 ILLEGAL AXIS COMMAND (NURBS) An axis not specified as a control point was specified in the No.
1 block.
2004 ILLEGAL KNOT There is an insufficient number of knot individual blocks.
2005 ILLEGAL CANCEL (NURBS) The NURBS interpolation mode was turned OFF even though
NURBS interpolation was not completed.
2006 ILLEGAL MODE (NURBS) A mode that cannot be paired with the NURBS interpolation
mode was specified.
2007 ILLEGAL MULTI-KNOT Nested knots for each level can be specified for the start and
end points.
2032 EMBEDDED ETHERNET/DATA
SERVER ERROR
An error was returned in the built-in Ethernet/data server
function.
For details, see the error message screen of the built-in
Ethernet or data server.
2051 #200-#499ILLEGAL P-CODE MACRO
COMMON INPUT(NO OPTION)
An attempt was made to enter a custom macro common
variable not existing in the system.
2052 #500-#549P-CODE MACRO
COMMON SELECT(CANNOT USE
SETVN)
The variable name cannot be entered.
The SETVN command cannot be used with the P-CODE macro
common variables #500 to #549.
2053 THE NUMBER OF #30000 IS
UNMATCH
An attempt was made to enter a P-CODE-only variable not
existing in the system.
2054 THE NUMBER OF #40000 IS
UNMATCH
An attempt was made to enter an extended P-CODE-only
variable not existing in the system.
2060 ILLEGAL PARAMETER IN
G43.4/G43.5
The parameter for the pivot tool length compensation is
incorrect.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2351 -
Number Message Description
2061 ILLEGAL COMMAND IN G43.4/G43.5 An illegal command was specified in tool center point control.
- A rotation axis command was specified in tool center point
control (type 2) mode.
- With a table rotary type or mixed-type machine, a I, J, or K
command was specified in the tool center point control (type
2) command (G43.5) block.
- A command that does not move the tool center point (only a
rotation axis is moved) was specified for the workpiece in the
G02 mode.
- G43.4 or G43.5 was specified in the tool center point control
mode.
- When the workpiece coordinate system is set as the
programming coordinate system (bit 5 (WKP) of parameter
No. 19696 is 1), G02 or G03 was specified while the rotation
axis was not perpendicular to the plane.
4010 ILLEGAL REAL VALUE OF OBUF : The real value for a output buffer is in error.
5006 TOO MANY WORD IN ONE BLOCK The number of words in a block exceeds the maximum. The
maximum is 26 words. However, this figure varies according to
NC options. Divide the instruction word into two blocks.
5007 TOO LARGE DISTANCE Due to compensation, point of intersection calculation,
interpolation or similar reasons, a movement distance that
exceeds the maximum permissible distance was specified.
Check the programmed coordinates or compensation amounts.
5009 PARAMETER ZERO (DRY RUN) The dry run feedrate parameter No. 1410 or maximum cutting
feedrate parameter No. 1422 for each axis has been set to 0.
5010 END OF RECORD The EOR (End of Record) code is specified in the middle of a
block. This alarm is also generated when the percentage at the
end of the NC program is read.
5011 PARAMETER ZERO (CUT MAX) The maximum cutting feedrate parameter No. 1430 has been
set to 0.
5014 TRACE DATA NOT FOUND A transfer could not be made because of no trace data.
5015 NO ROTATION AXIS No rotation axis was found in a handle feed in the tool axis
direction or in the tool axis right angle direction.
5016 ILLEGAL COMBINATION OF M
CODES
M codes which belonged to the same group were specified in a
block. Alternatively, an M code which must be specified without
other M codes in the block was specified in a block with other M
codes.
5018 POLYGON SPINDLE SPEED ERROR In G51.2 mode, the speed of the spindle or polygon
synchronous axis either exceeds the clamp value or is too small.
The specified rotation speed ratio thus cannot be maintained.
For polygon turning between spindles:
More information as to why this alarm occurred is indicated in
DGN No. 471.
5020 PARAMETER OF RESTART ERROR An invalid value is set in parameter No. 7310, which specifies
the axis order in which the tool is moved along axes to the
machining restart position in dry run. A value ranging from 1 to
the number of controlled axes may be set in this parameter.
5043 TOO MANY G68 NESTING Three-dimensional coordinate conversion has been specified
three or more times.
To perform another coordinate conversion, perform cancellation,
then specify the coordinate conversion.
H.ALARM LIST APPENDIX B-63944EN/03
- 2352 -
Number Message Description
5044 G68 FORMAT ERROR Errors for three-dimensional coordinate conversion command
are:
(1) No I, J, or K command was issued in three-dimensional
coordinate conversion command block. (without coordinate
rotation option)
(2) All of I, J, or K command were 0 in three-dimensional
coordinate conversion command block.
(3) No rotation angle R was not commanded in
three-dimensional coordinate conversion command block.
5046 ILLEGAL PARAMETER (S-COMP) The setting of a parameter related to straightness compensation
contains an error.
Possible causes include:
- A non-existent axis number is set in a moving or
compensation axis parameter.
- More than 128 pitch error compensation points are set
between the furthest points in the negative and position
regions.
- The straightness compensation point numbers do not have
correct magnitude relationships.
- No straightness compensation point is found between the
furthest pitch error compensation point in the negative region
and that in the positive region.
- The compensation per compensation point is either too large
or too small.
5050 ILL-COMMAND IN G81.1 MODE During chopping, a move command has been issued for the
chopping axis.
5058 G35/G36 FORMAT ERROR A command for switching the major axis has been specified for
circular threading. Alternatively, a command for setting the
length of the major axis to 0 has been specified for circular
threading.
5060 ILLEGAL PARAMETER IN
G02.3/G03.3
The axis parameter setting to perform an exponential
interpolation is in error.
Parameter No. 5641:
A liner axis number for performing an exponential interpolation
Parameter No. 5642:
A rotation axis number for performing an exponential
interpolation
The settable value is 1 to the number of control axes, but it must
not be duplicated.
5061 ILLEGAL FORMAT IN G02.3/G03.3 The exponential interpolation command (G02.3/G03.3) has a
format error.
The command range for address I or J is -89.0 to -1.0 or +1.0 to
+89.0. No I or J is specified or out-of -range value is specified.
No address R, or 0 is specified.
5062 ILLEGAL COMMAND IN G02.3/G03.3 The value specified in an exponential interpolation command
(G02.3/03.3) is illegal. A value that does not allow exponential
interpolation is specified. (For example, the value for In is 0 or
negative.)
5064 DIFFERRENT AXIS UNIT Circular interpolation has been specified on a plane consisting
of axes having different increment systems.
5065 DIFFERRENT AXIS UNIT(PMC AXIS) Axes having different increment systems have been specified in
the same DI/DO group for PMC axis control. Modify the setting
of parameter No. 8010.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2353 -
Number Message Description
5066 RESTART ILLEGAL SEQUENCE
NUMBER
A sequence number from 7000 to 7999 was read during the
search for the next number in a restart program for the back or
restart function.
5068 FORMAT ERROR IN G31P90 No travel axis was specified. Two or more travel axes were
specified.
5073 NO DECIMAL POINT No decimal point has been specified for an address requiring a
decimal point.
5074 ADDRESS DUPLICATION ERROR The same address has been specified two or more times in a
single block. Alternatively, two or more G codes in the same
group have been specified in a single block.
5085 SMOOTH IPL ERROR 1 A block for specifying smooth interpolation contains a syntax
error.
5110 IMPROPER G-CODE (AICC MODE) An unspecifiable G code was specified in the AI contour control
mode.
5115 ILLEGAL ORDER (NURBS) There is an error in the specification of the rank.
5116 ILLEGAL KNOT VALUE (NURBS) Monotone increasing of knots is not observed.
5117 ILLEGAL 1ST CONTROL POINT
(NURBS)
The first control point is incorrect.
Or, it does not provide a continuity from the previous block.
5118 ILLEGAL RESTART (NURBS) After manual intervention with manual absolute mode set to on,
NURBS interpolation was restarted.
5122 ILLEGAL COMMAND IN SPIRAL A spiral interpolation or conical interpolation command has an
error. Specifically, this error is caused by one of the following:
1) L = 0 is specified.
2) Q = 0 is specified.
3) R/, R/, C is specified.
4) Zero is specified as height increment.
5) Zero is specified as height difference.
6) Three or more axes are specified as the height axes.
7) A height increment is specified when there are two height
axes.
8) Q is specified when radius difference = 0.
9) Q < 0 is specified when radius difference > 0.
10) Q > 0 is specified when radius difference < 0.
11) A height increment is specified when no height axis is
specified.
5123 OVER TOLERANCE OF END POINT
IN SPIRAL
The difference between a specified end point and the calculated
end point exceeds the allowable range (parameter 3471).
5124 CAN NOT COMMAND SPIRAL A spiral interpolation or conical interpolation was specified in
any of the following modes:
1) Scaling
2) Polar coordinate interpolation
3) In tool radius⋅tool nose radius compensation mode, the
center is set as the end point.
5130 NC AND SUPERIMPOSE AXIS
CONFLICT
In the PMC superposition axis control, the NC command and
The PMC axis control command were conflicted. Modify the
program and the ladder.
5131 NC COMMAND IS NOT COMPATIBLE The PMC axis control and three-dimensional coordinate
conversion or a polar coordinate interpolation were specified
simultaneously.
5132 CANNOT CHANGE SUPERIMPOSED
AXIS
The superposition axis was selected for the axis for which the
PMC superposition axis is being controlled.
H.ALARM LIST APPENDIX B-63944EN/03
- 2354 -
Number Message Description
5195 DIRECTION CAN NOT BE JUDGED Measurement is invalid in the tool compensation measurement
value direct input B function.
[For 1-contact input]
1. The recorded pulse direction is not constant.
- The machine is at a stop in the offset write mode.
- The servo power is off.
- Pulse directions are diverse.
2. The tool is moving along the two axes (X-axis and Y-axis).
[For the movement direction discrimination specification]
1. The recorded pulse direction is not constant.
- The machine is at a stop in the offset write mode.
- The servo power is off.
- Pulse directions are diverse.
2. The tool is moving along the two axes (X-axis and Z-axis).
3. The direction indicated by the tool compensation write
signal does not match the movement direction of the axis.
5196 ILLEGAL AXIS OPERATION During HPCC or during the execution of a 5-axis-related
function, an unavailable function was used.
5220 REFERENCE POINT ADJUSTMENT
MODE
In case of distance coded linear scale I/F, the reference point
auto setting parameter (No.1819#2) is set to "1". Move the
machine to reference position by manual operation and execute
manual reference return.
5242 ILLEGAL AXIS NUMBER A master axis number or a slave axis number was not set
correctly when the flexible synchronization control mode was
turned from off to on during automatic operation.
5243 DATA OUTRANGE A gear ratio was not set correctly when the flexible
synchronization control mode was turned from off to on during
automatic operation.
5244 TOO MANY DI ON - During automatic operation, the mode signal was not turned on
or off if the flexible synchronization control mode was turned
from off to on or or from on to off, after an M code was
executed.
- An attempt was made to turn on or off the flexible
synchronization control mode when the axis was not stopped.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2355 -
Number Message Description
5245 OTHERAXIS ARE COMMANDED - For a flexible synchronization control group for which a PMC
axis was a master axis, an attempt was made to turn on the
synchronous mode during time other than automatic operation.
- An attempt was made to turn on a synchronization group for
which an PMC axis was a master axis when there existed a
flexible synchronization control group for which a non-PMC,
normal axis was a master axis.
- The master and slave axes as synchronous axes overlap the
EGB axis.
- The master and slave axes as synchronous axes overlap the
chopping axis.
- The master and slave axes as synchronous axes overlap the
axis related to angular axis control.
- The master and slave axes as synchronous axes overlap the
axis related to composite control.
- The master and slave axes as synchronous axes overlap the
axis related to superposition control.
- The slave axis as a synchronous axis overlaps the axis related
to synchronization control.
- The reference position return mode is turned on (was turned
on).
5255 G12.4/G13.4 FORMAT ERROR The specified P, I, and K are incorrect or I is less than K.
5257 G41/G42 NOT ALLOWED IN MDI
MODE
Tool radius/tool nose radius compensation was specified in MDI
mode. (Depending on the setting of the parameter MCR (No.
5008#4))
5303 TOUCH PANEL ERROR The touch panel is not connected correctly, or the touch panel
cannot be initialized when the power is turned on. Correct the
cause then turn on the power again.
5305 ILLEGAL SPINDLE NUMBER In a spindle select function by address P for a multiple spindle
control,
1) Address P is not specified.
2) Parameter No.3781 is not specified to the spindle to be
selected.
3) An illegal G code which cannot be commanded with an
S_P_; command is specified.
4) A multi spindle cannot be used because the parameter EMS
(No. 3702#1) is 1.
5) The spindle amplifier number of each spindle is not set in
parameter No. 3717.
6) A prohibited command for a spindle was issued (parameter
No. 11090).
7) An invalid value is set in parameter No. 11090.
5312 ILLEGAL COMMAND IN G10
L75/76/77
One of formats in G10L75, G10L76, or G10L77 to G11
commands is in error, or the command value is out of data
range. Modify the program.
5316 TOOL TYPE NUMBER NOT FOUND A tool with the specified tool-type number could not be found.
Modify the program or register the tool.
5317 ALL TOOL LIFE IS OVER The lives of all tools with the specified tool-type number have
expired.
Replace the tool.
5320 DIA./RAD. MODE CAN’T BE
SWITCHED .
In any of the following states, diameter/radius specification was
switched:
1) When a buffered program is being executed
2) When a movement is being made on the axis
H.ALARM LIST APPENDIX B-63944EN/03
- 2356 -
Number Message Description
5329 M98 AND NC COMMAND IN SAME
BLOCK
A subprogram call which is not a single block was commanded
during canned cycle mode.
5339 ILLEGAL FORMAT COMMAND IS
EXECUTED IN SYNC/MIX/OVL
CONTROL.
1. The value of P, Q, or L specified by
G51.4/G50.4/G51.5/G50.5/G51.6/G50.6 is invalid.
2. A duplicate value is specified by parameter No. 12600.
5346 RETURN TO REFERENCE POINT The coordinate establishment of the Cs contour control axis is
not made.
Perform a manual reference position return.
1. When Cs coordinate establishment is made for the Cs-axis
for which the Cs-axis reference position status signal
CSPENx is 0
2. When positional information is not sent from the spindle
amplifier
3. When the servo off state is entered during the start of
Cs-axis coordinate establishment
4. When the Cs-axis is subjected to synchronous control or
superposition control
5. When the emergency stop state is entered during
coordinate establishment
6. When an attempt is made to release composite control for
the Cs axis being subjected to coordinate establishment
7. When an attempt is made to start synchronous, composite,
or superposition control for the Cs axis being subjected to
coordinate establishment.
5360 TOOL INTERFERENCE CHECK
ERROR
This alarm is issued when interference with another tool is
caused by a data modification based on G10 data input or file
reading or when an attempt is made to modify the tool figure
data of a tool registered in the cartridge.
5361 ILLEGAL MAGAZINE DATA Tools stored in the cartridge are interfering with each other.
Reregister the tools in the cartridge, or modify the tool
management data or tool figure data. If this alarm is issued, no
tool interference check is made when tools are registered in the
cartridge management table. Moreover, empty pot search
operation does not operate normally. If this alarm is issued, the
power must be turned off before operation is continued.
5362 CONVERT INCH/MM AT REF-POS An inch/metric conversion was performed at a position other
than the reference position. Perform an inch/metric conversion
after returning to the reference position.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2357 -
Number Message Description
5364 ILLEGAL COMMAND IN PROGRAM
CHECK
(1) An unspecifiable G code was specified in the high-speed
program check mode.
(2) The angular axis control option or customer's board option is
enabled.
(3) One of the following operations was performed.
- Chopping in the high-speed program check mode
- Starting the high-speed program check mode during
chopping
- High-speed cycle machining in the high-speed program
check mode
- Reference position return of an axis for which the reference
position is not established, in the high-speed program
check mode
(4) Switching of PMC axis selection signal EAX*<G0136> was
performed.
(5) G10 was specified for bit 3 (PGR) of parameter No. 3454 in
the high-speed program check mode.
(6) G10 was specified for bit 6 (PGS) of parameter No. 3001 in
the high-speed program check mode.
5365 NOT CHANGE OF PROGRAM
CHECK MODE
(1) Switching of high-speed program check input signal
PGCK<Gn290.5> was performed during execution of the
program.
5381 INVALID COMMAND IN FSC MODE An attempt was made to issue the following commands:
- When the reference position for the master axis under flexible
synchronization control has not been established, G28
command for the master axis.
- G27/G28/G29/G30/G30.1/G53 command for a slave axis.
5391 CAN NOT USE G92 Workpiece coordinate system setting G92 (or G50 for the lathe
system G-code system A) cannot be specified.
(1) After tool length compensation was changed by tool length
compensation shift type, G92 was specified when no
absolute command is present.
(2) G92 was specified in the block in which G49 is present.
5406 G41.3/G40 FORMAT ERROR (1) The G41.3 or G40 block contains a move command.
(2) The G41.3 block contains a G or M code that suppresses
buffering.
5407 ILLEGAL COMMAND IN G41.3 (1) In the G41.3 mode, a G code of group 01 other than G00
and G01 is specified.
(2) In the G41.3 mode, an offset command (a G code of group
07) is specified.
(3) The block next to G41.3 (startup) specifies no movement.
5408 G41.3 ILLEGAL START_UP (1) In a mode of group 01 other than G00 and G01, G41.3
(startup) is specified.
(2) The included angle between the tool vector and move vector
is 0 or 180 degrees at the time of startup.
5420 ILLEGAL PARAMETER IN
G43.4/G43.5
A parameter related to tool center point control is illegal.
- Acceleration/deceleration before interpolation is disabled. Set
parameter No. 1660.
- Rapid traverse acceleration/deceleration before interpolation is
disabled. Set bit 1 of parameter No. 1401, bit 5 of parameter
No. 19501, parameter No. 1671, and parameter No. 1672.
H.ALARM LIST APPENDIX B-63944EN/03
- 2358 -
Number Message Description
5421 ILLEGAL COMMAND IN G43.4/G43.5 An illegal command was specified in tool center point control.
- A rotation axis command was specified in tool center point
control (type 2) mode.
- With a table rotary type or mixed-type machine, a I,J,K
command was specified in the tool center point control (type 2)
command (G43.5) block.
- A command that does not move the tool center point (only a
rotation axis is moved) was specified for the workpiece in the
G02 mode.
- When the workpiece coordinate system is set as the
programming coordinate system (bit 5 (WKP) of parameter No.
19696 is 1), G02 or G03 was specified while the rotation axis
was not perpendicular to the plane.
- A G code not specifiable during the tool center point control
mode was specified.
- The modal code used to specify tool center point control is
incorrect.
- During the tool center point control mode, an axis not related
to tool center point control was specified.
- When bit 0 (RCM) of parameter No. 11200 is set to 0 to
disable tool direction compensation, tool center point control is
specified during the workpiece setting error
compensation/tilted working plane command mode.
- When tool posture control is enabled under tool center point
control (type 2), a command is specified to set a tool posture
near a singular point. (This alarm may be suppressed with bit
3 (NPC) of parameter No. 19696.) Check the machine
configuration and specification.
- When tool posture control is enabled under tool center point
control (type 1), a rotary axis angular displacement that
disables tool posture control is specified. Check the machine
configuration and specification.
- During tool center point control (type 2) or tool posture control,
NURBS interpolation is specified. Check the specification.
5422 EXCESS VELOCITY IN G43.4/G43.5 An attempt was made to make a movement at an axis feedrate
exceeding the maximum cutting feedrate by tool center point
control.
5424 ILLEGAL TOOL DIRECTION The rotation axis position for specifying the tool axis direction is
not ±90° × n (n = 0, 1, 2,･･･).
5425 ILLEGAL OFFSET VALUE The offset number is incorrect.
5430 ILLEGAL COMMAND IN 3-D CIR In a modal state in which three-dimensional circular interpolation
cannot be specified, a three-dimensional circular interpolation
(G02.4/G03.4) is specified. Alternatively, in three-dimensional
circular interpolation mode, a code that cannot be specified is
specified.
5432 G02.4/G03.4 FORMAT ERROR A three-dimensional circular interpolation command
(G02.4/G03.4) is incorrect.
5433 MANUAL INTERVENTION IN
G02.4/G03.4 (ABS ON)
In three-dimensional circular interpolation mode (G02.4/G03.4),
manual intervention was made when the manual absolute switch
was on.
5435 PARAMETER OUT OF RANGE (TLAC) Illegal parameter setting.
(Set value is out of range.)
Check parameters No. 19655, No. 19656, No. 19657, and No.
1022.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2359 -
Number Message Description
5436 ILLEGAL PARAMETER SETTING OF
ROTARY AXIS(TLAC)
Illegal parameter setting.
(axis of rotation setting)
5437 ILLEGAL PARAMETER SETTING OF
MASTER ROTARY AXIS(TLAC)
Illegal parameter setting.
(master axis of rotation setting)
5445 CAN NOT COMMAND MOTION IN
G39
Corner circular interpolation (G39) of tool radius/tool nose radius
compensation is not specified alone but is specified with a move
command.
5446 NO AVOIDANCE AT G41/G42 Because there is no interference avoidance vector, the
interference check avoidance function of tool radius/tool nose
radius compensation does not work.
5447 DANGEROUS AVOIDANCE AT
G41/G42
The interference check avoidance function of tool radius/tool
nose radius compensation operation will lead to danger.
5448 INTERFERENCE TO AVD. AT
G41/G42
In the interference check avoidance function of tool radius/tool
nose radius compensation, a further interference occurs for an
already created interference avoidance vector.
5456 TOO MANY G68.2 NESTING Tilted working plane command G68.2 was specified more than
once.
To perform another coordinate conversion, perform cancellation,
then specify the coordinate conversion.
5457 G68.2 FORMAT ERROR A G68.2 format error occurred.
5458 ILLEGAL USE OF G53.1 - G53.1 was specified preceding G68.2.
- G53.1 needs to be specified solely.
- There is no angle solution for the rotation axis that controls the
tool direction in the +Z-axis direction of the feature coordinate
system.
- In the setting by which compensation in the tool direction is not
performed (when bit 0 (RCM) of parameter No. 11200 is 0),
G53.1 was specified in the workpiece placement error
compensation mode.
5459 MACHINE PARAMETER INCORRECT - The parameter No. 19665 to No. 19667, No. 19680 to No.
19744 for configuring the machine are incorrect.
- The axis specified with parameter No. 19681 or No. 19686 is
not a rotary axis.
- In parameter No. 1022, the basic three axes are not set.
- A rotary axis end point found by the NC with tool center point
control type 2, 3-dimensional cutter compensation type 2, or
the tilted working plane command is not within the range set by
parameter No. 19741 to No. 19744.
- No rotary axis end point was found with tool center point
control type 2 or 3-dimensional cutter compensation type 2.
Check the machine configuration and specification.
- On a machine whose rotary axis is a virtual axis, tool center
point control type 2 or 3-dimensional cutter compensation type
2 was specified.
- When programming is performed in the workpiece coordinate
system, tool center point control type 2 or 3-dimensional cutter
compensation type 2 is specified.
H.ALARM LIST APPENDIX B-63944EN/03
- 2360 -
Number Message Description
5460 ILLEGAL USE OF 3-DIMENSIONAL
CUTTER COMPENSATION
- In the 3-dimensional cutter compensation mode (except the
tool side offset function for a tool rotation type machine), a
move command other than G00/G01 is specified.
- With a table rotation type machine, when bit 1 (PTD) of
parameter No. 19746 is set to 1, a plane selection is made
with an axis other than the basic three axes at the start of
3-dimensional cutter compensation.
- When bit 1 (SPG) of parameter No. 19607 is set to 1, there is
a discrepancy between the machine type set in parameter No.
19680 and a G code specifying 3-dimensional cutter
compensation (G41.2, G42.2, G41.4, G42.4, G41.5, or G42.5).
- With a machine that is not of the tool rotation type, G41.3 is
specified.
- When bit 5 (WKP) of parameter No. 19696 is set to 0, and bit 4
(TBP) of parameter No. 19746 is set to 0, 3-dimensional cutter
compensation and tool center point control are used at the
same time.
- A rotation axis command is specified in the 3-dimensional
cutter compensation mode (type 2).
- With a table rotation type or mixed type machine, IJK is
specified in a block that specifies 3-dimensional cutter
compensation (type 2) (G41.6/G42.6).
- An illegal G code is specified in the 3-dimensional cutter
compensation mode.
- When 3-dimensional cutter compensation is specified, the
modal state is illegal.
- When the table coordinate system is set as the programming
coordinate system, table rotate and 3-dimensional cutter
compensation are specified after the start of tool center point
control.
- There is a difference in type1/type 2 specification between
3-dimensional cutter compensation and tool center point
control.
- When 3-dimensional cutter compensation and tool center point
control are used at the same time, one of these functions that
is specified earlier than the other is canceled earlier.
5461 ILLEGAL USE OF
G41.2/G42.2/G41.5/G42.5
A move command other than G00 or G01 was performed during
3-dimensional cutter compensation in a mixed-type machine.
5462 ILLEGAL COMMAND (G68.2/G69) (1) The modal setting used when G68.2 or G69 is specified is
incorrect.
(2) An unspecifiable G code was specified in the G68.2 mode.
(3) The offset vector of tool radius/tool nose radius
compensation is not canceled when G68.2 or G69 is
specified.
5463 ILLEGAL PARAMETER IN
3-DIMENSIONAL CUTTER
COMPENSATION
A parameter related to 3-dimensional cutter compensation is
illegal.
- Acceleration/deceleration before interpolation is disabled. Set
parameter No. 1660.
- Rapid traverse acceleration/deceleration before interpolation is
disabled. Set bit 1 (LRP) of parameter No. 1401, bit 5 (FRP) of
parameter No. 19501, and parameter Nos. No.1671 and 1672.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2361 -
(4) Parameter writing alarm (SW alarm)
Number Message Description
SW0100 PARAMETER ENABLE SWITCH ON The parameter setting is enabled (PWE, one bit of parameter
No. 8000 is set to “1”).
To set the parameter, turn this parameter ON. Otherwise, set
to OFF.
(5) Servo alarms (SV alarm)
Number Message Description
SV0001 SYNC ALIGNMENT ERROR In feed axis synchronization control, the amount of
compensation for synchronization exceeded the parameter
(No. 8325) setting value.
This alarm occurs only for a slave axis.
SV0002 SYNC EXCESS ERROR ALARM 2 In feed axis synchronization control, the amount of
synchronization error exceeded the parameter (No. 8332)
setting value. When the synchronization is not completed
after power-up, the determination is made by the parameter
value (No. 8332) multiplied by the parameter (No. 8330)
multiplier.
This alarm occurs only for a slave axis only.
SV0003 SYNCHRONOUS/COMPOSITE/SUPERI
MPOSED CONTROL MODE CAN'T BE
CONTINUED
Since as axis in synchronization, composition, or
superposition mode caused a servo alarm, the mode could
not be continued, If one of the axes in a mode causes a
servo alarm, all axes relating to the axis enter the servo-off
state. This alarm is generated to enable the cause of the
servo-off state to be checked.
SV0004 EXCESS ERROR (G31) The amount of positional deviation during torque limit skip
command operation exceeded the limit value of the
parameter No.6287.
SV0005 SYNC EXCESS ERROR (MCN) In feed axis synchronization control, for synchronization, the
difference value of the machine coordinate between a master
and slave axes exceeded the parameter (No. 8314) setting
value.
This alarm occurs for a master or slave axis.
SV0006 ILLEGAL TANDEM AXIS For the slave axis under tandem control, absolute position
detection is set (parameter bit 5 (APC) of parameter No.
1815 = 1).
SV0007 SV ALM ANOTHER PATH(MULTI AMP.) When a multiaxis amplifier was used in a multipath system
across paths, a servo alarm occurred on an axis belonging to
another path.
When a system with two or more paths and multiple servo
axes between paths are controlled by a multiaxis amplifier, if
a servo alarm occurs on an axis belonging to another path of
the same amplifier, the MCC of the amplifier goes down and
SV0401 V-READY OFF occurs on an axis belonging to the
local path in the same amplifier. Since SV0401 is caused
by a servo alarm occurred on an axis in another path,
SV0007 is caused together to clearly indicate the fact.
The axis belonging to another path in the same amplifier
resolves the cause of the servo alarm.
H.ALARM LIST APPENDIX B-63944EN/03
- 2362 -
Number Message Description
SV0301 APC ALARM: COMMUNICATION
ERROR
Since the absolute-position detector caused a
communication error, the correct machine position could not
be obtained. (data transfer error)
The absolute-position detector, cable, or servo interface
module is thought to be defective.
SV0302 APC ALARM: OVER TIME ERROR Since the absolute-position detector caused an overtime
error, the correct machine position could not be obtained.
(data transfer error)
The absolute-position detector, cable, or servo interface
module is thought to be defective.
SV0303 APC ALARM: FRAMING ERROR Since the absolute-position detector caused a framing error,
the correct machine position could not be obtained. (data
transfer error)
The absolute-position detector, cable, or servo interface
module is thought to be defective.
SV0304 APC ALARM: PARITY ERROR Since the absolute-position detector caused a parity error,
the correct machine position could not be obtained. (data
transfer error)
The absolute-position detector, cable, or servo interface
module is thought to be defective.
SV0305 APC ALARM: PULSE ERROR Since the absolute-position detector caused a pulse error,
the correct machine position could not be obtained.
The absolute-position detector, or cable is thought to be
defective.
SV0306 APC ALARM: OVER FLOW ERROR Since the amount of positional deviation overflowed, the
correct machine position could not be obtained.
Check to see the parameter No. 2084 or No. 2085.
SV0307 APC ALARM: MOVEMENT EXCESS
ERROR
Since the machine moved excessively, the correct machine
position could not be obtained.
SV0360 ABNORMAL CHECKSUM(INT) The checksum alarm occurred on the built–in Pulsecoder.
SV0361 ABNORMAL PHASE DATA(INT) The phase data abnormal alarm occurred on the built–in
Pulsecoder.
SV0362 ABNORMAL REV. DATA(INT) The speed count abnormal alarm occurred on the built-in
Pulsecoder.
SV0363 ABNORMAL CLOCK(INT) The clock alarm occurred on the built–in Pulsecoder.
SV0364 SOFT PHASE ALARM(INT) A digital servo soft detected an abnormality on the built in
Pulsecoder.
SV0365 BROKEN LED(INT) The digital servo software detected abnormal data on the
built–in Pulsecoder.
SV0366 PULSE MISS(INT) A pulse error occurred on the built–in Pulsecoder.
SV0367 COUNT MISS(INT) A count error occurred on the built–in Pulsecoder.
SV0368 SERIAL DATA ERROR(INT) The communications data could not be received from the
built–in Pulsecoder.
SV0369 DATA TRANS. ERROR(INT) A CRC error or stop bit error occurred in the communications
data from the built–in Pulsecoder.
SV0380 BROKEN LED(EXT) Separate detector error
SV0381 ABNORMAL PHASE (EXT) An abnormal alarm in the position data occurred on the
separate detector.
SV0382 COUNT MISS(EXT) A count error occurred on the separate detector.
SV0383 PULSE MISS(EXT) A pulse error occurred on the separate detector.
SV0384 SOFT PHASE ALARM(EXT) The digital servo software detected abnormal data on the
separate detector.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2363 -
Number Message Description
SV0385 SERIAL DATA ERROR(EXT) The communications data could not be received from the
separate detector.
SV0386 DATA TRANS. ERROR(EXT) A CRC error or stop bit error occurred in the communications
data from the standalone detector.
SV0387 ABNORMAL ENCODER(EXT) An abnormality occurred on a separate detector. For more
information, contact the scale manufacturer.
SV0401 IMPROPER V_READY OFF Although the ready signal (PRDY) of the position control was
ON, the ready signal (VRDY) of the velocity control was OFF.
SV0403 CARD/SOFT MISMATCH The combination of the axis control card and the servo
software is incorrect.
Probable causes are given below.
- The correct axis control card is not attached.
- The correct servo software is not installed in flash memory.
SV0404 IMPROPER V_READY ON Although the ready signal (PRDY) of the position control was
OFF, the ready signal (VRDY) of the velocity control was ON.
SV0407 EXCESS ERROR The difference value of the amount of positional deviation for
the synchronization axis exceeded the setting value. (during
synchronization control only)
SV0409 DETECT ABNORMAL TORQUE An abnormal load was detected on the servo motor, or during
Cs axis or spindle positioning.
The alarm can be canceled by RESET.
SV0410 EXCESS ERROR (STOP) The amount of positional deviation during stopping exceeded
the parameter (No. 1829) setting value.
SV0411 EXCESS ERROR (MOVING) The amount of positional deviation during traveling became
excessive than the parameter setting value.
SV0413 LSI OVERFLOW The counter for the amount of positional deviation overflowed
SV0415 MOTION VALUE OVERFLOW The velocity exceeding the travel velocity limit was
commanded.
SV0417 ILL DGTL SERVO PARAMETER A digital serve parameter setting is incorrect.
When bit 4 of diagnosis information No. 203 is 1, an illegal
parameter was detected by the servo software. Identify the
cause with reference to diagnosis information No. 352.
When bit 4 of diagnosis information No. 203 is 0, the CNC
software detected an illegal parameter. Probable causes
are given below (see diagnosis information No. 280).
1) The value specified in parameter No. 2020 as the motor
model falls outside the specified range.
2) The motor rotation direction in parameter No. 2022 is not
set to a correct value (111 or -111).
3) The speed feedback pulse count per motor rotation in
parameter No. 2023 is set to a negative or other incorrect
value.
4) The position feedback pulse count per motor rotation in
parameter No. 2024 is set to a negative or other incorrect
value.
SV0420 SYNC TORQUE EXCESS In feed axis synchronization control, for synchronization, the
difference value of torque between a master and slave axes
exceeded the parameter (No. 2031) setting value.
This alarm occurs for a master axis.
SV0421 EXCESS ERROR(SEMI-FULL) The difference between the feedback from the semi and full
sides exceeded the setting of parameter No.1729.
H.ALARM LIST APPENDIX B-63944EN/03
- 2364 -
Number Message Description
SV0422 EXCESS VELOCITY IN TORQUE In torque control, the commanded permissible velocity was
exceeded.
SV0423 EXCESS ERROR IN TORQUE In torque control, the total permissible move value specified
as a parameter was exceeded.
SV0430 SV MOTOR OVERHEAT The servo motor has overheated.
SV0431 CNV. OVERLOAD PSM : Overheat
β series SVU : Overheat
SV0432 CNV. LOW VOLT CONTROL PSM : The control power supply voltage has dropped.
PSMR : The control power supply voltage has dropped.
β series SVU : The control power supply voltage has
dropped.
SV0433 CNV. LOW VOLT DC LINK PSM : Low DC link voltage
PSMR : Low DC link voltage
α series SVU : Low DC link voltage
β series SVU : Low DC link voltage
SV0434 INV. LOW VOLT CONTROL SVM : Low control power voltage
SV0435 INV. LOW VOLT DC LINK SVM : Low DC link voltage
SV0436 SOFTTHERMAL(OVC) The digital servo software detected a software thermal
(OVC).
SV0437 CNV. OVERCURRENT POWER PSM : Overcurrent on input circuit section.
SV0438 INV. ABNORMAL CURRENT SVM : Motor overcurrent
α series SVU : Motor overcurrent
β series SVU : Motor overcurrent
SV0439 CNV. OVER VOLT DC LINK PSM : The DC link voltage is too high.
PSMR : The DC link voltage is too high.
β series SVU : The DC link voltage is too high.
SV0440 CNV. EX DECELERATION POW. PSMR : Excessive generative discharge
α series SVU : Excessive generative discharge, or abnormal
error in generative power circuit
SV0441 ABNORMAL CURRENT OFFSET The digital servo software detected an abnormality in the
motor current detection circuit.
SV0442 CNV. CHARGE FAILURE PSM : The spare charge circuit for the DC link is abnormal.
PSMR : The spare charge circuit for the DC link is abnormal.
SV0443 CNV. COOLING FAN FAILURE PSM : Internal cooling fan failure.
PSMR : Internal cooling fan failure.
β series SVU : Internal cooling fan failure.
SV0444 INV. COOLING FAN FAILURE SVM : Internal cooling fan failure.
SV0445 SOFT DISCONNECT ALARM The digital servo software detected a disconnected
Pulsecoder.
SV0446 HARD DISCONNECT ALARM The hardware detected a disconnected built–in Pulsecoder.
SV0447 HARD DISCONNECT(EXT) The hardware detected a disconnected separate detector.
SV0448 UNMATCHED FEEDBACK ALARM The sign of the feedback signal from the standalone detector
is opposite to that from the feedback signal from the built–on
Pulsecoder.
SV0449 INV. IPM ALARM SVM : The IPM (Intelligent Power Module) detected an alarm.
α series SVU : The IPM (Intelligent Power Module) detected
an alarm.
SV0453 SPC SOFT DISCONNECT ALARM Software disconnection alarm of the α Pulsecoder.
Turn off the power to the CNC, then remove and insert the
Pulsecoder cable. If this alarm is issued again, replace the
Pulsecoder.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2365 -
Number Message Description
SV0454 ILLEGAL ROTOR POS DETECT The magnetic pole detection function terminated abnormally.
The magnetic pole could not be detected because the motor
did not run.
SV0456 ILLEGAL CURRENT LOOP An attempt was made to set the current loop that could not
be set.
The amplifier pulse module in use does not comply with
HIGH SPEED HRV. Or, requirements to control are not
satisfied in the system.
SV0458 CURRENT LOOP ERROR The specified current loop differs from the actual current
loop.
SV0459 HI HRV SETTING ERROR For two axes whose servo axis numbers (parameter No.
1023) are consecutively even and odd numbers, HIGH
SPEED HRV control is possible for one axis and impossible
for the other.
SV0460 FSSB DISCONNECT The FSSB connection was discontinued.
Probable causes are:
1. The FSSB connection cable was disconnected or broken.
2. The amplifier was turned off .
3. In the amplifier, the low-voltage alarm occurred.
SV0462 SEND CNC DATA FAILED The correct data could not be received on a slave side
because of the FSSB communication error.
SV0463 SEND SLAVE DATA FAILED The correct data could not be received in the servo software
because of the FSSB communication error.
SV0465 READ ID DATA FAILED A read of the ID information for the amplifier has failed at
power-on.
SV0466 MOTOR/AMP. COMBINATION The maximum current of an amplifier is different to that of a
motor.
Probable causes are:
1. The connection command for an amplifier is incorrect.
2. The parameter (No.2165) setting is incorrect
SV0468 HI HRV SETTING ERROR(AMP) An attempt was made to set up HIGH SPEED HRV control
for use when the controlled axis of an amplifier for which
HIGH SPEED HRV control could not be used.
SV0474 EXCESS ERROR(STOP:SV ) The servo detected that the positional deviation during a stop
exceeded the setting (parameters No. 1839 and No. 1842) in
the n-axis.
SV0475 EXCESS ERROR(MOVE:SV) The servo detected that the positional deviation during a
travel exceeded the setting (parameters No. 1838 and No.
1841) in the n-axis.
SV0476 ILLEGAL SPEED CMD.(SV ) The servo detected that the speed command exceeded the
safety speed (parameters No. 13821 to No. 13824 (during
position control) or parameters No. 13826 to No. 13829
(during speed control)) during safety monitoring (when safety
monitoring request signal *VLDVx is 0) in the n-axis. Keep
the safety speed.
SV0477 ILLEGAL MACHINE POS.(SV) The servo detected that the machine position fell outside the
safety area (setting by parameters No. 13831 to No. 13838)
during safety monitoring (when safety monitoring request
signal *VLDVx is 0) in the n-axis. Keep the safety area.
A machine position check is performed only on the axis for
which the reference position has been established. The
axis for which the reference position is not established is not
subjected to a machine position check.
H.ALARM LIST APPENDIX B-63944EN/03
- 2366 -
Number Message Description
SV0478 ILLEGAL AXIS DATA(SV) The servo detected that an error occurred during transfer of
axis data in the n-axis.
When an alarm occurred because the configuration of the
servo amplifier was changed, set the axis number for the
servo amplifier (set bit 4 of parameter No. 2212 of the
corresponding axis to 1 and then 0 and turn off the power of
the entire system). When using a multiaxis amplifier, this
operation may not clear the alarm. In this case, repeat this
operation for the axes on which the alarm persists.
If an alarm occurs due to a cause other than the above,
replace the servo amplifier.
SV0481 SAFETY PARAM ERROR(SV) The servo detected that a safety parameter error occurred in
the n-axis.
SV0484 SAFETY FUNCTION ERROR(SV) A safety function error related to the servo was detected in
the n-axis.
- The servo or CNC detected that the safety function was not
executed in the servo.
- The result of a servo safety function check did not match
the result of a CNC safety function check.
- An error occurred during a test of the CPU of the servo.
- An error occurred during a check of RAM of the servo.
SV0488 SELF TEST OVER TIME An MCC interruption test was not complete within the set
period of time (parameter No. 1946). Check the MCC
contact.
SV0489 SAFETY PARAM ERROR(CNC) The CNC detected that a safety parameter error occurred in
the n-axis.
SV0490 SAFETY FUNCTION ERROR(CNC) A CNC safety function error occurred in the n-axis.
- The servo detected that the safety function was not
executed in the CNC.
- The result of a servo safety function check did not match
the result of a CNC safety function check.
SV0494 ILLEGAL SPEED CMD.(CNC) The CNC detected that the speed command exceeded the
safety speed (parameters No. 13821 to No. 13824 (during
position control) or parameters No. 13826 to No. 13829
(during speed control)) during safety monitoring (when safety
monitoring request signal *VLDVx is 0) in the n-axis. Keep
the safety speed.
SV0495 ILLEGAL MACHINE POS.(CNC) The CNC detected that the machine position fell outside the
safety area (set range by parameters No. 13831 to No.
13838) during safety monitoring (when safety monitoring
request signal *VLDVx is 0) in the n-axis. Keep the safety
area.
A machine position check is performed only on the axis for
which the reference position has been established.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2367 -
Number Message Description
SV0496 ILLEGAL AXIS DATA(CNC) The CNC detected that an error occurred during transfer to
axis data.
When an alarm occurred because the configuration of the
servo amplifier was changed, set the axis number for the
servo amplifier (set bit 4 of parameter No. 2212 of the
corresponding axis to 1 and 0 again and turn off the power of
the entire system). When using a multiaxis amplifier, this
operation may not clear the alarm. In this case, repeat this
operation for the axes on which the alarm persists.
If an alarm occurs due to a cause other than the above,
replace the servo amplifier.
SV0498 AXIS NUMBER NOT SET(CNC) The CNC detected that the axis number of the n-axis was not
set for the servo amplifier. The axis number is set
automatically, so turn off the power of the entire system.
SV0600 INV. DC LINK OVER CURRENT SVM : DC link overcurrent.
β SVU : DC link overcurrent.
SV0601 INV. RADIATOR FAN FAILURE SVM : Radiator cooling fan failure.
β SVU : Radiator cooling fan failure.
SV0602 INV. OVERHEAT SVM : The servo motor has overheated.
SV0603 INV. IPM ALARM(OH) SVM : The IPM (Intelligent Power Module) detected an
overheat alarm.
β SVU : The IPM (Intelligent Power Module) detected an
overheat alarm.
SV0604 AMP. COMMUNICATION ERROR The communication between SVM and PSM is in error.
SV0605 CNV. EX. DISCHARGE POW. PSMR : The motor regenerative power is too much.
SV0606 CNV. RADIATOR FAN FAILURE PSM : External radiator cooling fan failure.
PSMR : External radiator cooling fan failure.
SV0607 CNV. SINGLE PHASE FAILURE PSM : The input power supply has a missing phase.
PSMR : The input power supply has a missing phase.
SV0646 ABNORMAL ANALOG SIGNAL(EXT) An error occurred in the analog 1Vp-p output of the separate
detector. The separate detector, cable, or separate detector
interface unit may be failed.
SV1025 V_READY ON (INITIALIZING ) The ready signal (VRDY) of the velocity control which should
be OFF is ON while the servo control is ON.
SV1026 ILLEGAL AXIS ARRANGE The parameter for servo axis arrange is not set correctly.
A negative value, duplicate value, or greater value than the
number of control axes was set to the parameter No. 1023
"The servo axis number of each axis."
SV1055 ILLEGAL TANDEM AXIS In tandem control, the setting of the parameter No. 1023 is
incorrect.
SV1056 ILLEGAL TANDEM PAIR In tandem control, the setting of the parameter TDM
(No.1817#6) is incorrect.
SV1067 FSSB:CONFIGURATION ERROR(SOFT) An FSSB configuration error occurred (detected by software).
The connected amplifier type is incompatible with the FSSB
setting value.
SV1068 DUAL CHECK SAFETY ALARM An alarm that turns off the MCC of the entire system
occurred in the Dual Check Safety function.
SV1069 EXCESS ERROR(SERVO OFF:CNC) The CNC detected that the positional deviation during
servo-off exceeded the set value (parameter No. 1840) in the
n-axis.
SV1070 EXCESS ERROR(SERVO OFF:SV) The servo detected that the positional deviation during
servo-off exceeded the set value (parameter No. 1840) in the
n-axis.
H.ALARM LIST APPENDIX B-63944EN/03
- 2368 -
Number Message Description
SV1071 EXCESS ERROR(MOVE:CNC) The CNC detected that the positional deviation during a
travel exceeded the set value (parameters No. 1838 and No.
1841) in the n-axis.
SV1072 EXCESS ERROR(STOP:CNC) The CNC detected that the positional deviation during a stop
exceeded the set value (parameters No. 1839 and No. 1842)
in the n-axis.
SV1100 S-COMP. VALUE OVERFLOW The amount of compensation for the straightness exceeded
a maximum value of 32767.
SV5134 FSSB:OPEN READY TIME OUT In the initialization, the FSSB could not be in an open ready
sate. The axis card is thought to be defective.
SV5136 FSSB:NUMBER OF AMP. IS
INSUFFICIENT
The number of amplifier identified by the FSSB is insufficient
than the number of control axes. Or, the setting of the
number of axes or the amplifier connection is in error.
SV5137 FSSB:CONFIGURATION ERROR An FSSB configuration error occurred.
The connecting amplifier type is incompatible with the FSSB
setting value.
SV5139 FSSB:ERROR Servo initialization has not completed successfully. It is
probable that an optical cable failed or a connection between
the amplifier and another module failed.
SV5197 FSSB:OPEN TIME OUT The initialization of the FSSB was completed, but it could not
be opened. Or, the connection between the CNC and the
amplifier in is incorrect.
SV5197 FSSB:OPEN TIME OUT The FSSB could not be opened although the CNC permitted
the opening of the FSSB.
Check the connection between the CNC and the amplifier.
SV5311 FSSB:ILLEGAL CONNECTION 1. This alarm is issued if axes, whose servo axis numbers
(parameter No. 1023) are even and odd numbers, are
allocated to the amplifiers connected to the FSSBs of
different paths.
2. This alarm is issued if an attempt is made to set up for
use of the pulse modules connected to the FSSBs of
different paths. And the system did not satisfy the
requirements for performing HIGH SPEED HRV control.
(6) Overtravel alarms (OT alarm)
Number Message Description
OT0500 + OVERTRAVEL ( SOFT 1 ) Exceeded the positive side stored stroke check 1.
OT0501 - OVERTRAVEL ( SOFT 1 ) Exceeded the negative side stored stroke check 1.
OT0502 + OVERTRAVEL ( SOFT 2 ) Exceeded the positive side stored stroke check 2. Or, in the
chuck tail stock barrier, an entry to the inhibited area was
made during movement in the positive direction.
OT0503 - OVERTRAVEL ( SOFT 2 ) Exceeded the negative side stored stroke check 2. Or, in the
chuck tail stock barrier, an entry to the inhibited area was
made during movement in the negative direction.
OT0504 + OVERTRAVEL ( SOFT 3 ) Exceeded the positive side stored stroke check 3.
OT0505 - OVERTRAVEL ( SOFT 3 ) Exceeded the - side stored stroke check 3.
OT0506 + OVERTRAVEL ( HARD ) The stroke limit switch in the positive direction was triggered.
This alarm is generated when the machine reaches the
stroke end.
When this alarm is not generated, feed of all axes is stopped
during automatic operation.
During manual operation, only the feed of the axis on which
the alarm occurred is stopped.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2369 -
Number Message Description
OT0507 - OVERTRAVEL ( HARD ) The stroke limit switch in the negative direction was
triggered.
This alarm is generated when the machine reaches the
stroke end.
When this alarm is not generated, feed of all axes is stopped
during automatic operation.
During manual operation, only the feed of the axis on which
the alarm occurred is stopped.
OT0508 INTERFERENCE:+ A tool moving in the positive direction along the n axis has
fouled another tool post.
OT0509 INTERFERENCE:- A tool moving in the negative direction along the n axis has
fouled another tool post.
OT0510 + OVERTRAVEL ( PRE-CHECK ) The tool exceeded the limit in the negative direction during
the stroke check before movement.
OT0511 - OVERTRAVEL ( PRE-CHECK ) The tool exceeded the limit in the positive direction during the
stroke check before movement.
OT0514 (n) INTERFERENCE:+ An interference occurred on the plus side of the n-axis in a
rotation area interference check.
OT0515 (n) INTERFERENCE:- An interference occurred on the minus side of the n-axis in a
rotation area interference check.
OT1710 ILLEGAL ACC. PARAMETER
(OPTIMUM TORQUE ACC/DEC)
The permissible acceleration parameter for the optimum
torque acceleration/deceleration is in error. A possible cause
is either of the following:
(1) The ratio of a negative acceleration to a positive
acceleration is not more than the limit value.
(2) The time to reduce to a velocity of 0 exceeded the
maximum time.
(7) Memory file alarms (IO alarm)
Number Message Description
IO1001 FILE ACCESS ERROR The resident–type file system could not be accessed as an
error occurred in the resident–type file system.
IO1002 FILE SYSTEM ERROR The file could not be accessed as an error occurred in the
CNC file system.
IO1030 CHECK SUM ERROR The checksum of the CNC part program storage memory is
incorrect.
IO1032 MEMORY ACCESS OVER RANGE Accessing of data occurred outside the CNC part program
storage memory range.
IO1104 OVER MAXIMUM TOOL LIFE PAIRS The maximum number of tool life management pairs is
exceeded. Modify the setting of the maximum number of tool
life management pairs in parameter No. 6813.
(8) Alarms requiring power to be turned off (PW alarm)
Number Message Description
PW0000 POWER MUST BE OFF A parameter was set for which the power must be turned
OFF then ON again.
PW0001 X-ADDRESS(*DEC) IS NOT ASSIGNED. The X address of the PMC could not be assigned correctly.
This alarm may occur in the following case:
- During the setting of parameter No. 3013, the X address
could not be assigned correctly for the deceleration dog
(*DEC) for a return to the reference position.
H.ALARM LIST APPENDIX B-63944EN/03
- 2370 -
Number Message Description
PW0002 PMC address is not correct(AXIS). The address to assign the axis signal is incorrect.
This alarm may occur in the following case:
- The parameter No.3021 setting is incorrect.
PW0003 PMC address is not correct(SPINDLE). The address to assign the spindle signal is incorrect.
This alarm may occur in the following case:
- The parameter No.3022 setting is incorrect.
PW0004 SETTING THE LOADER SYSTEM PATH
IS NOT CORRECT.
The loader system could not be assigned correctly.
The parameter No. 984 setting is incorrect.
- The number of loader systems and the number of systems
specified to the loader system in the parameter No.
984#0(LCP) does not match.
- The parameter No. 984#0 of the system 1 is set to 1.
PW0006 POWER MUST BE OFF (ILL-EXEC-CHK) The malfunction prevention function detected an alarm to
require the power off.
PW0007 X-ADDRESS(SKIP) IS NOT ASSIGNED The X address of PMC could not be assigned correctly.
Possible causes are:
- During the set of parameter No. 3012, the skip signal of the
X address was not assigned correctly.
- During the set of parameter No. 3019, the address other
than the skip signal of the X address was not assigned
correctly.
PW0008 CPU SELF TEST ERROR(DCS PMC) On the DCS PMC side:
- An error was detected by the CPU self diagnosis function.
- An error was detected by the RAM check function.
PW0009 CPU SELF TEST ERROR(PMC) On the PMC side:
- An error was detected by the CPU self diagnosis function.
- An error was detected by the RAM check function.
PW0010 SAFE I/O CROSS CHECK ERROR(DCS
PMC)
On the DCS PMC side, an error was detected by the I/O
cross check function in system-defined safety-related DI/DO.
PW0011 SAFE I/O CROSS CHECK ERROR(PMC) On the PMC side, an error was detected by the I/O cross
check function in system-defined safety-related DI/DO.
PW0012 USER I/O CROSS CHECK ERROR(DCS
PMC)
On the DCS PMC side, an error was detected by the I/O
cross check function in user-defined safety-related DI/DO.
PW0013 USER I/O CROSS CHECK
ERROR(PMC)
On the PMC side, an error was detected by the I/O cross
check function in user-defined safety-related DI/DO.
PW0014 CPU TEST ALARM (CNC) An error occurred in a test of the CPU of the CNC.
PW0015 SAFETY PARAM ERROR The CNC detected that an error occurred in a safety
parameter for other than servo axes or spindle axes.
PW0016 RAM CHECK ERROR An error was detected in a RAM check of the CNC.
PW0017 INEXECUTION OF SAFETY
FUNCTIONS
The safety function was not executed normally in the CNC.
PW0018 CRC CHECK ERROR An error was detected in a CRC check of the CNC.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2371 -
Number Message Description
PW1102 ILLEGAL PARAMETER (I-COMP.) The parameter for setting slope compensation is incorrect.
This alarm occurs in the following cases:
- When the number of pitch error compensation points on the
axis on which slope compensation is executed exceeds
128 between the most negative side and most positive side
- When the size relationship between the slope
compensation point Nos. is incorrect
- When the slope compensation point is not located between
the most negative side and most positive side of pitch error
compensation
- When the compensation per compensation point is too
small or too great.
PW1103 ILLEGAL PARAMETER (S-COMP.128) The parameter for setting 128 straightness compensation
points or the parameter compensation data is incorrect,
PW5046 ILLEGAL PARAMETER (S-COMP.) The parameter for setting straightness compensation is
incorrect.
PW5390 R-ADDRESS SETTING IS ILLEGAL The start address or the set range of the PMC R addresses
set by parameters No.13541 and No.13542 is invalid.
(9) Spindle alarms (SP alarm)
Number Message Description
SP0740 RIGID TAP ALARM : EXCESS ERROR The positional deviation of the stopped spindle has exceeded
the set value during rigid tapping.
SP0741 RIGID TAP ALARM : EXCESS ERROR The positional deviation of the moving spindle has exceeded
the set value during rigid tapping.
SP0742 RIGID TAP ALARM : LSI OVERFLOW An LSI overflow has occurred for the spindle during rigid
tapping.
SP0752 SPINDLE MODE CHANGE ERROR This alarm is generated if the system does not properly
terminate a mode change. The modes include the Cs contour
control, spindle positioning, rigid tapping, and spindle control
modes. The alarm is activated if the spindle control unit does
not respond correctly to the mode change command issued
by the NC.
SP0754 ABNORMAL TORQUE An abnormal load was detected in a spindle motor.
The alarm can be canceled by RESET.
SP0755 SAFETY FUNCTION ERROR The CNC CPU detected that the safely function of the n-th
spindle was not executed. Alternatively, the result of a CNC
safety function check did not match the result of a spindle
safety function check.
SP0756 ILLEGAL AXIS DATA The CNC CPU detected that the connection state and the
hardware setting of the spindle amplifier were incompatible
on the n-th spindle. If an alarm occurs because of the
configuration change of the spindle amplifier , set the spindle
amplifier correctly.
SP0757 SAFETY SPEED OVER The CNC CPU detected that during safety monitoring (when
safety monitoring request signal *VLDPs is 0), the spindle
motor speed was greater than the safety speed (parameter
No. 4372, 4438, 4440, or 4442) on the n-th spindle. Operate
within the safety speed.
SP1202 SPINDLE SELECT ERROR In a multi spindle control, the spindle number other than the
valid spindle number was selected by a position coder select
signal. An attempt was made to select the spindle number of
the system having no valid spindle.
H.ALARM LIST APPENDIX B-63944EN/03
- 2372 -
Number Message Description
SP1210 TOOL CHANGE SP MOTION
OVERFLOW
The amount of distribution to a spindle is too much.
(specific to the FANUC ROBODRILL)
SP1211 TOOL CHANGE SP ORTN EXCESS
ERROR
During a tool change, a too much orientation error was
detected for the spindle.
(specific to the FANUC ROBODRILL)
SP1212 TOOL CHANGE SP MOVE EXCESS
ERROR
During a tool change, a too much moving error was detected
for the spindle.
(specific to the FANUC ROBODRILL)
SP1213 TOOL CHANGE SP STOP EXCESS
ERROR
During a tool change, a too much stop error was detected for
the spindle.
(specific to the FANUC ROBODRILL)
SP1214 TOOL CHANGE SP ILLEGAL
SEQUENCE
During changing tools, an abnormal spindle sequence was
detected.
(specific to the FANUC ROBODRILL)
SP1220 NO SPINDLE AMP. Either the cable connected to a serial spindle amplifier is
broken, or the serial spindle amplifier is not connected.
SP1221 ILLEGAL MOTOR NUMBER The spindle No. and the motor No. are incorrectly matched.
SP1224 ILLEGAL SPINDLE-POSITION CODER
GEAR RATIO
The spindle–position coder gear ratio was incorrect.
SP1225 CRC ERROR (SERIAL SPINDLE) A CRC error (communications error) occurred in
communications between the CNC and the serial spindle
amplifier.
SP1226 FRAMING ERROR (SERIAL SPINDLE) A framing error occurred in communications between the
CNC and the serial spindle amplifier.
SP1227 RECEIVING ERROR (SERIAL SPINDLE) A receive error occurred in communications between the
CNC and the serial spindle amplifier.
SP1228 COMMUNICATION ERROR (SERIAL
SPINDLE)
A communications error occurred between the CNC and the
serial spindle amplifier.
SP1229 COMMUNICATION ERROR SERIAL
SPINDLE AMP.
A communications error occurred between serial spindle
amplifiers (motor Nos. 1 and 2, or motor Nos. 3–4).
SP1231 SPINDLE EXCESS ERROR (MOVING) The position deviation during spindle rotation was greater
than the value set in parameters.
SP1232 SPINDLE EXCESS ERROR (STOP) The position deviation during spindle stop was greater than
the value set in parameters.
SP1233 POSITION CODER OVERFLOW The error counter/speed instruction value of the position
coder overflowed.
SP1234 GRID SHIFT OVERFLOW Grid shift overflowed.
SP1240 DISCONNECT POSITION CODER The analog spindle position coder is broken.
SP1241 D/A CONVERTER ERROR The D/A converter for controlling analog spindles is
erroneous.
SP1243 ILLEGAL SPINDLE PARAMETER
SETTING(GAIN)
The setting for the spindle position gain is incorrect.
SP1244 MOTION VALUE OVERFLOW The amount of distribution to a spindle is too much
SP1245 COMMUNICATION DATA ERROR A communication data error was detected on the CNC.
SP1246 COMMUNICATION DATA ERROR A communication data error was detected on the CNC.
SP1247 COMMUNICATION DATA ERROR A communication data error was detected on the CNC.
SP1700 SAFETY PARAM ERROR The CNC detected that a safety parameter error occurred in
the n-th spindle.
SP1969 SPINDLE CONTROL ERROR An error occurred in the spindle control software.
SP1970 SPINDLE CONTROL ERROR Initialization of spindle control ended in error.
SP1971 SPINDLE CONTROL ERROR An error occurred in the spindle control software.
SP1972 SPINDLE CONTROL ERROR An error occurred in the spindle control software.
SP1974 ANALOG SPINDLE CONTROL ERROR An error occurred in the spindle control software.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2373 -
Number Message Description
SP1975 ANALOG SPINDLE CONTROL ERROR An position coder error was detected on the analog spindle.
SP1976 SERIAL SPINDLE COMMUNICATION
ERROR
The amplifier No. could not be set to the serial spindle
amplifier.
SP1977 SERIAL SPINDLE COMMUNICATION
ERROR
An error occurred in the spindle control software.
SP1978 SERIAL SPINDLE COMMUNICATION
ERROR
A time–out was detected during communications with the
serial spindle amplifier.
SP1979 SERIAL SPINDLE COMMUNICATION
ERROR
The communications sequence was no longer correct during
communications with the serial spindle amplifier.
SP1980 SERIAL SPINDLE AMP. ERROR Defective SIC–LSI on serial spindle amplifier
SP1981 SERIAL SPINDLE AMP. ERROR An error occurred during reading of the data from SIC–LSI on
the analog spindle amplifier side.
SP1982 SERIAL SPINDLE AMP. ERROR An error occurred during reading of the data from SIC–LSI on
the serial spindle amplifier side.
SP1983 SERIAL SPINDLE AMP. ERROR Could not clear on the spindle amplifier side.
SP1984 SERIAL SPINDLE AMP. ERROR An error occurred during re–initialization of the spindle
amplifier.
SP1985 SERIAL SPINDLE CONTROL ERROR Failed to automatically set parameters
SP1986 SERIAL SPINDLE CONTROL ERROR An error occurred in the spindle control software.
SP1987 SERIAL SPINDLE CONTROL ERROR Defective SIC–LSI on the CNC
SP1988 SPINDLE CONTROL ERROR An error occurred in the spindle control software.
SP1989 SPINDLE CONTROL ERROR An error occurred in the spindle control software.
SP1996 ILLEGAL SPINDLE PARAMETER
SETTING
The spindle was assigned incorrectly. Check to see the
following parameter. (No.3716 or 3717)
SP1998 SPINDLE CONTROL ERROR An error occurred in the spindle control software.
SP1999 SPINDLE CONTROL ERROR An error occurred in the spindle control software.
H.ALARM LIST APPENDIX B-63944EN/03
- 2374 -
(10) Alarm list (serial spindle)
When a serial spindle alarm occurs, the following number is displayed
on the CNC.
NOTE
*1 Note that the meanings of the SPM indications
differ depending on which LED, the red or yellow
LED, is on. When the red LED is on, the SPM
indicates a 2-digit alarm number. When the yellow
LED is on, the SPM indicates an error number that
designates a sequence problem (for example,
when a rotation command is entered with the
emergency stop state not released).
See "Error Codes (Serial Spindle)."
*2 For serial spindle alarms with a number not listed,
refer to the following documents depending on the
spindle motor to which a connection is actually
made.
- FANUC AC SPINDLE MOTOR αi series
Maintenance Manual (B-65285JA)
- Technical Report etc.
Number Message
SPM
indication
(*1)
Faulty location and remedy Description
SP9001 SSPA:01 MOTOR
OVERHEAT
01 1 Check and correct the
peripheral temperature and
load status.
2 If the cooling fan stops,
replace it.
The thermostat embedded in the motor
winding operated.
The internal temperature of the motor
exceeds the specified level.
The motor is used in excess of the
continuous rating, or the cooling
component is abnormal.
SP9002 SSPA:02 EX
DEVIATION SPEED
02 1 Check and correct the
cutting conditions to
decrease the load.
2 Correct parameter No. 4082.
The motor speed cannot follow a
specified speed.
An excessive motor load torque is
detected.
The acceleration/deceleration time in
parameter No. 4082 is insufficient.
SP9003 SSPA:03 DC-LINK
FUSE IS BROKEN
03 1 Replace the SPM unit.
2 Check the motor insulation
status.
3 Replace the interface cable.
The PSM becomes ready (00 is
indicated), but the DC link voltage is
too low in the SPM.
The fuse in the DC link section in the
SPM is blown. (The power device is
damaged or the motor is
ground-fault.)
The JX1A/JX1B connection cable is
abnormal.
SP9004 SSPA:04 POWER
SUPPLY ERROR
04 Check the state of the input
power supply to the PSM.
The PSM found a missing power
supply phase. (PSM alarm 5)
SP9006 THERMAL SENSOR
DISCONNECT
06 1 Check and correct the
parameter.
2 Replace the feedback cable.
The temperature sensor of the motor
is disconnected.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2375 -
Number Message
SPM
indication
(*1)
Faulty location and remedy Description
SP9007 SSPA:07 OVER
SPEED
07 Check for a sequence error.
(For example, check whether
spindle synchronization was
specified when the spindle
could not be turned.)
The motor speed has exceeded
115% of its rated speed. When the
spindle axis was in position control
mode, positional deviations were
accumulated excessively (SFR and
SRV were turned off during spindle
synchronization.)
SP9009 SSPA:09
OVERHEAT MAIN
CIRCUIT
09 1 Improve the heat sink
cooling status.
2 If the heat sink cooling fan
stops, replace the SPM unit.
Abnormal temperature rise of the
power transistor radiator
SP9010 SSPA:10 LOW VOLT
INPUT POWER
09 1 Replace the cables.
2 Replace the spindle
amplifier control printed
circuit board.
The control power voltage of the
spindle amplifier is reduced.
SP9011 SSPA:11
OVERVOLT POWER
CIRCUIT
11 1 Check the selected PSM.
2 Check the input power
voltage and change in power
during motor deceleration.
If the voltage exceeds 253
VAC (for the 200-V system)
or 530 VAC (for the 400-V
system), improve the power
supply impedance.
Overvoltage of the DC link section of
the PSM was detected. (PSM alarm
indication: 7)
PSM selection error. (The maximum
output specification of the PSM is
exceeded.)
SP9012 SSPA:12
OVERCURRENT
POWER CIRCUIT
12 1 Check the motor insulation
status.
2 Check the spindle
parameters.
3 Replace the SPM unit.
The motor output current is
abnormally high.
A motor-specific parameter does not
match the motor model.
Poor motor insulation
SP9013 SSPA:13 CPU DATA
MEMORY FAULT
13 Replace the SPM control
printed circuit board.
Abnormality in an SPM control circuit
component is detected. (RAM within
the SPM is abnormal.)
SP9015 SSPA:15 SPINDLE
SWITCHING FAULT
15 1 Check and correct the
ladder sequence.
2 Replace the switching MC.
The switch sequence in spindle
switch/output switch operation is
abnormal.
The switching MC contact status
check signal and command do not
match.
SP9016 SSPA:16 RAM
ERROR
16 Replace the SPM control
printed circuit board.
Abnormality in an SPM control circuit
component is detected. (RAM for
external data is abnormal.)
SP9018 SSPA:18
SUMCHECK
ERROR PROGRAM
ROM
18 Replace the SPM control
printed circuit board.
Abnormality in an SPM control circuit
component is detected. (Program
ROM data is abnormal.)
SP9019 SSPA:19 EXCESS
OFFSET CURRENT
U
19 Replace the SPM unit. Abnormality in an SPM component is
detected. (The initial value for the U
phase current detection circuit is
abnormal.)
H.ALARM LIST APPENDIX B-63944EN/03
- 2376 -
Number Message
SPM
indication
(*1)
Faulty location and remedy Description
SP9020 SSPA:20 EXCESS
OFFSET CURRENT
V
20 Replace the SPM unit. Abnormality in an SPM component is
detected. (The initial value of the V
phase current detection circuit is
abnormal.)
SP9021 POS SENSOR
POLARITY ERROR
21 Check and correct the
parameters.
(No. 4000#0, 4001#4)
The polarity parameter setting of the
position sensor is wrong.
SP9024 SSPA:24 SERIAL
TRANSFER ERROR
24 1 Place the CNC-to-spindle
cable away from the power
cable.
2 Replace the cable.
The CNC power is turned off (normal
power-off or broken cable).
An error is detected in
communication data transferred to
the CNC.
SP9027 SSPA:27
DISCONNECT
POSITION CODER
27 1 Replace the cable.
2 Re-adjust the BZ sensor
signal.
1 The spindle position coder
(connector JY4) signal is abnormal.
2 The signal amplitude (connector
JY2) of the MZ or BZ sensor is
abnormal.
(Unconnected cable, adjustment
error, etc.)
SP9029 SSPA:29
OVERLOAD
29 Check and correct the load
status.
Excessive load has been applied
continuously for a certain period of
time. (This alarm is issued also when
the motor shaft has been locked in
the excitation state.)
SP9030 SSPA:30
OVERCURRENT
INPUT CIRCUIT
30 Check and correct the power
supply voltage.
Overcurrent is detected in PSM main
circuit input. (PSM alarm indication:
1)
Unbalanced power supply.
PSM selection error (The maximum
PSM output specification is
exceeded.)
SP9031 SSPA:31 MOTOR
LOCK OR
DISCONNECT
DETECTOR
31 1 Check and correct the load
status.
2 Replace the motor sensor
cable (JY2 or JY5).
The motor cannot rotate at a
specified speed. (A level not
exceeding the SST level for the
rotation command has existed
continuously.)
Abnormality in the speed detection
signal.
SP9032 SSPA:32 SIC-LSI
RAM FAULT
32 Replace the SPM control
printed circuit board.
Abnormality in an SPM control circuit
component is detected. (The LSI
device for serial transfer is
abnormal.)
SP9033 SSPA:33
SHORTAGE
POWER CHARGE
33 1 Check and correct the power
supply voltage.
2 Replace the PSM unit.
Charging of direct current power
supply voltage in the power circuit
section is insufficient when the
magnetic contractor in the amplifier
is turned on (such as open phase
and defective charging resistor).
B-63944EN/03 APPENDIX H.ALARM LIST
- 2377 -
Number Message
SPM
indication
(*1)
Faulty location and remedy Description
SP9034 SSPA:34 ILLEGAL
PARAMETER
34 Correct a parameter value
according to the manual.
If the parameter number is
unknown, connect the spindle
check board, and check the
indicated parameter.
Parameter data exceeding the
allowable limit is set.
SP9036 SSPA:36
OVERFLOW
ERROR COUNTER
36 Check whether the position
gain value is too large, and
correct the value.
An error counter overflow occurred.
SP9037 SSPA:37 ILLEGAL
SETTING
VELOCITY
DETECTOR
37 Correct the value according to
the parameter manual.
The setting of the parameter for the
number of pulses in the speed
detector is incorrect.
SP9041 SSPA:41 ILLEGAL
1REV SIGN OF
POSITION CODER
41 1 Check and correct the
parameter.
2 Replace the cable.
3 Re-adjust the BZ sensor
signal. Re-adjust the BZ
sensor signal.
1 The 1-rotation signal of the spindle
position coder (connector JY4) is
abnormal.
2 The 1-rotation signal (connector
JY2) of the MZ or BZ sensor is
abnormal.
3 Parameter setting error
SP9042 SSPA:42 NO 1REV
SIGN OF POSITION
CODER
42 1 Replace the cable.
2 Re-adjust the BZ sensor
signal.
1 The 1-rotation signal of the spindle
position coder (connector JY4) is
disconnected.
2 The 1-rotation signal (connector
JY2) of the MZ or BZ sensor is
disconnected.
SP9043 SSPA:43
DISCONNECT
POSITION CODER
DEF. SPEED
43 Replace the cable. The differential speed position coder
signal (connector JY8) in SPM type 3
is abnormal.
SP9047 SSPA:47 ILLEGAL
SIGNAL OF
POSITION CODER
47 1 Replace the cable.
2 Re-adjust the BZ sensor
signal.
3 Correct the cable layout
(vicinity of the power line).
1 The A/B phase signal of the
spindle position coder (connector
JY4) is abnormal.
2 The A/B phase signal (connector
JY2) of the MZ or BZ sensor is
abnormal.
The relationship between the A/B
phase and 1-rotation signal is
incorrect (Pulse interval mismatch).
SP9049 SSPA:49 DEF.
SPEED IS OVER
VALUE
49 Check whether the calculated
differential speed value
exceeds the maximum motor
speed.
In differential speed mode, the speed
of the other spindle converted to the
speed of the local spindle has
exceeded the allowable limit (the
differential speed is calculated by
multiplying the speed of the other
spindle by the gear ratio).
SP9050 SSPA:50
SYNCRONOUS
VALUE IS OVER
SPEED
50 Check whether the calculated
value exceeds the maximum
motor speed.
In spindle synchronization, the speed
command calculation value
exceeded the allowable limit (the
motor speed is calculated by
multiplying the specified spindle
speed by the gear ratio).
H.ALARM LIST APPENDIX B-63944EN/03
- 2378 -
Number Message
SPM
indication
(*1)
Faulty location and remedy Description
SP9051 SSPA:51 LOW VOLT
POWER CIRCUIT
51 1 Check and correct the power
supply voltage.
2 Replace the MC.
Input voltage drop was detected. (PSM
alarm indication: 4) (Momentary power
failure or poor MC contact)
SP9052 SSPA:52 ITP FAULT
1
52 1 Replace the SPM control
printed circuit board.
2 Replace the spindle
interface printed circuit
board in the CNC.
NC interface abnormality was
detected (the ITP signal stopped).
SP9053 SSPA:53 ITP FAULT
2
53 1 Replace the SPM control
printed circuit board.
2 Replace the spindle
interface printed circuit
board in the CNC.
NC interface abnormality was
detected (the ITP signal stopped).
SP9054 SSPA:54
OVERCURRENT
54 Review the load state. An overload current was detected.
SP9055 SSPA:55 ILLEGAL
POWER LINE
55 1 Replace the magnetic
contactor.
2 Check and correct the
sequence.
The power line state signal of the
magnetic contactor for selecting a
spindle or output is abnormal.
SP9056 COOLING FAN
FAILURE
56 Replace the SPM unit. The cooling fan in the SPM control
circuit stopped.
SP9057 CONV. EX.
DECELERATION
POW.
57 1 Decrease the
acceleration/deceleration
duty.
2 Check the cooling condition
(peripheral temperature).
3 If the cooling fan stops,
replace the resistor.
4 If the resistance is abnormal,
replace the resistor.
An overload was detected in the
regenerative resistance. (PSMR alarm
indication: 8)
Thermostat operation or short-time
overload was detected.
The regenerative resistor was
disconnected, or an abnormal
resistance was detected.
SP9058 CNV. OVERLOAD 58 1 Check the PSM cooling
status.
2 Replace the PSM unit.
The temperature of the radiator of
the PSM has increased abnormally.
(PSM alarm indication: 3)
SP9059 CNV. COOLING FAN
FAILURE
59 Replace the PSM unit. The cooling fan in the PSM stopped.
(PSM alarm indication: 2)
SP9061 SERIAL SPINDLE
ALARM
61 Check parameter settings. The error between the semi-closed
and full-closed sides when the dual
position feedback function is used is
too large.
SP9065 SERIAL SPINDLE
ALARM
65 1 Check parameter settings.
2 Check sensor connections
and signals.
3 Check power line
connections.
The move distance is too long when
the magnetic pole is confirmed
(synchronization spindle)
SP9066 COM. ERROR
BETWEEN SP
AMPS
66 1 Replace the cable.
2 Check and correct the
connection.
An error was found in communication
between amplifiers.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2379 -
Number Message
SPM
indication
(*1)
Faulty location and remedy Description
SP9069 SAFETY SPEED
OVER
69 1 Check the specified speed.
2 Check parameter settings.
3 Check the sequence.
In the state in which safety speed
monitoring was enabled, the system
detected that the motor speed
exceeded the safety speed or
detected an error during a free-run
stop.
SP9070 ILLEGAL AXIS DATA 70 1 Check connections (JA7A of
the second spindle requires
a dedicated connector).
2 Replace the SPM control
printed-circuit board.
An error was detected in an axis
number check.
SP9071 SAFETY
PARAMETER
ERROR
71 Replace the SPM control
printed-circuit board.
An error was detected in an axis
parameter check.
SP9072 MISMATCH RESULT
OF MOTOR SPEED
CHECK
72 1 Replace the SPM control
printed-circuit board.
2 Replace the spindle
interface printed circuit
board in the CNC.
A mismatch was detected between
the safety speed check results of the
SPM and those of the CNC.
SP9073 MOTOR SENSOR
DISCONNECTED
73 1 Replace the feedback cable.
2 Check the shield processing.
3 Check and correct the
connection.
4 Adjust the sensor.
The motor sensor feedback signal is
not present.
SP9074 CPU TEST ERROR 74 Replace the SPM control
printed-circuit board.
An error was detected in a CPU test.
SP9075 CRC ERROR 75 Replace the spindle amplifier
control printed circuit board.
An error occurred in a spindle
amplifier CRC test.
SP9076 INEXECUTION OF
SAFETY
FUNCTIONS
76 Replace the SPM control
printed-circuit board.
The SPM detected that safety
functions were not executed.
SP9077 MISMATCH RESULT
OF AXIS NUMBER
CHECK
77 1 Replace the SPM control
printed-circuit board.
2 Replace the spindle
interface printed circuit
board in the CNC.
A mismatch was detected between
the axis number check results of the
SPM and those of the CNC.
SP9078 MISMATCH RESULT
OF SAFETY
PARAMETER
CHECK
78 1 Replace the SPM control
printed-circuit board.
2 Replace the spindle
interface printed circuit
board in the CNC.
A mismatch was detected between
the safety parameter check results of
the SPM and those of CNC.
SP9079 INITIAL TEST
ERROR
79 Replace the spindle amplifier
control printed circuit board.
An error was detected in a spindle
amplifier initial test.
SP9080 ALARM AT THE
OTHER SP AMP.
80 Remove the cause of the
alarm of the remote SPM.
During inter-SPM communication, an
alarm was generated on the remote
SPM.
SP9081 1-ROT MOTOR
SENSOR ERROR
81 1 Check and correct the
parameter.
2 Replace the feedback cable.
3 Adjust the sensor.
The one-rotation signal of the motor
sensor cannot be correctly detected.
SP9082 NO 1-ROT MOTOR
SENSOR
82 1 Replace the feedback cable.
2 Adjust the sensor.
The one-rotation signal of the motor
sensor is not generated.
H.ALARM LIST APPENDIX B-63944EN/03
- 2380 -
Number Message
SPM
indication
(*1)
Faulty location and remedy Description
SP9083 MOTOR SENSOR
SIGNAL ERROR
83 1 Replace the feedback cable.
2 Adjust the sensor.
An irregularity was detected in a
motor sensor feedback signal.
SP9084 SPNDL SENSOR
DISCONNECTED
84 1 Replace the feedback cable.
2 Check the shield processing.
3 Check and correct the
connection.
4 Check and correct the
parameter.
5 Adjust the sensor.
The spindle sensor feedback signal
is not present.
SP9085 1-ROT SPNDL
SENSOR ERROR
85 1 Check and correct the
parameter.
2 Replace the feedback cable.
3 Adjust the sensor.
The one-rotation signal of the spindle
sensor cannot be correctly detected.
SP9086 NO 1-ROT SPNDL
SENSOR
86 1 Replace the feedback cable.
2 Adjust the sensor.
The one-rotation signal of the spindle
sensor is not generated.
SP9087 SPNDL SENSOR
SIGNAL ERROR
87 1 Replace the feedback cable.
2 Adjust the sensor.
An irregularity was detected in a
spindle sensor feedback signal.
SP9088 COOLING RADI FAN
FAILURE
88 Replace the SPM external
cooling fan.
The external cooling fan stopped.
SP9089 COOLING RADI FAN
FAILURE
89 1 Check the connection
between the SPM and the
submodule SM (SSM).
2 Replace the submodule
SM(SSM).
3 Replace the SPM control
printed-circuit board.
Submodule SM (SSM) error
(synchronous spindle)
SP9110 AMP
COMMUNICATION
ERROR
b0 1 Replace the communication
cable between amplifier and
module.
2 Replace the SPM or PSM
control printed circuit board.
Communication error between
amplifier and module
SP9111 CONV. LOW VOLT
CONTROL
b1 Replace the PSM control
printed circuit board.
Low converter control power supply
voltage (PSM indication = 6)
SP9112 CONV. EX.
DISCHARGE POW.
b2 1 Check the regenerative
resistance.
2 Check the motor selection.
3 Replace the PSM
Excessive converter regenerative
power (PSM indication = 8)
SP9113 CONV. COOLING
FAN FAILURE
b3 Replace the cooling fan. Stopped cooling fan of the converter
radiator (PSM indication = A)
SP9120 COMMUNICATION
DATA ERROR
C0 1 Replace the communication
cable between CNC and
SPM.
2 Replace the SPM control
printed circuit board.
3 Replace the CNC side
spindle interface printed
circuit board.
Communication data alarm
B-63944EN/03 APPENDIX H.ALARM LIST
- 2381 -
Number Message
SPM
indication
(*1)
Faulty location and remedy Description
SP9121 COMMUNICATION
DATA ERROR
C1 1 Replace the communication
cable between CNC and
SPM.
2 Replace the SPM control
printed circuit board.
3 Replace the CNC side
spindle interface printed
circuit board.
Communication data alarm
SP9122 COMMUNICATION
DATA ERROR
C2 1 Replace the communication
cable between CNC and
SPM.
2 Replace the SPM control
printed circuit board.
3 Replace the CNC side
spindle interface printed
circuit board.
Communication data alarm
SP9123 SERIAL SPINDLE
ALARM
C3 Replace the submodule
SW(SSW).
Submodule SW (SSW) error (spindle
switching)
SP9135 SAFETY SPEED
ZERO ERROR(SP)
D5 Perform operation within the
safety speed zero range.
The motor position exceeded the
safety speed zero monitoring width.
SP9136 MISMATCH RESULT
OF SAFETY SPEED
ZERO CHECK(SP)
D6 Replace the spindle amplifier
control printed circuit board.
The spindle amplifier speed zero
determination result did not match
the CNC speed zero determination
result.
H.ALARM LIST APPENDIX B-63944EN/03
- 2382 -
Error codes (serial spindle)
NOTE
*1 Note that the meanings of the SPM indications
differ depending on which LED, the red or yellow
LED, is on. When the yellow LED is on, an error
code is indicated with a 2-digit number. An error
code is indicated in the CNC diagnosis, No.712.
When the red LED is on, the SPM indicates the
number of an alarm generated in the serial spindle.
→ See “(10) Serial spindle alarms (SP alarm).”
SPM
indication
(*1)
Faulty location and remedy Description
01 Although neither *ESP (emergency stop signal; there
are two types of signals including the input signal and
PSM contact signal) nor MRDY (machine ready
signal) is input, SFR (forward rotation signal)/SRF
(reverse rotation signal)/ORCM (orientation
command) is input.
Check the *ESP and MRDY sequence. For MRDY,
pay attention to the parameter setting regarding the
use of the MRDY signal (parameter No. 4001#0).
03 The parameter settings are such that a position
sensor is not used (position control not performed)
(bits 3, 2, 1, 0 of parameter No. 4002 = 0, 0, 0, 0), but
a Cs contour control command is input.
In this case, the motor is not excited.
Check the parameter settings.
04 The parameter settings are such that a position
sensor is not used (position control not performed)
(bits 3, 2, 1, 0 of parameter No.4002 = 0, 0, 0, ), but
a servo mode (rigid tapping, spindle positioning, etc.)
or spindle synchronization command is input.
In this case, the motor is not excited.
Check the parameter settings.
05 The orientation function option parameter is not
specified, but ORCM (orientation command) is
input.
Check the orientation function parameter settings.
06 The output switching control function option
parameter is not specified, but low-speed
characteristic winding is selected (RCH = 1).
Check the output switching control function
parameter settings and the power line state check
signal (RCH).
07 A Cs contour control command is input, but SFR
(clockwise rotation command)/SRV
(counterclockwise rotation command) is not input.
Check the sequence.
08 A servo mode (rigid tapping, spindle positioning,
etc.) control command is input, but SFR (clockwise
rotation command)/SRV (counterclockwise rotation
command) is not input.
Check the sequence.
09 A spindle synchronization command is input, but
SFR (clockwise rotation command)/SRV
(counterclockwise rotation command) is not input.
Check the sequence.
10 A Cs contour control command is input, but another
mode (servo mode, spindle synchronization, or
orientation) is specified.
Do not switch to another mode during a Cs
contour control command.
Before moving to another mode, cancel the Cs
contour control command.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2383 -
SPM
indication
(*1)
Faulty location and remedy Description
11 A servo mode (rigid tapping, spindle positioning,
etc.) command is input, but another mode (Cs
contour control, spindle synchronization, or
orientation) is specified.
Do not switch to another mode during a servo
mode command.
Before moving to another mode, cancel the servo
mode command.
12 A spindle synchronization command is input, but
another mode (Cs contour control, servo mode, or
orientation) is specified.
Do not switch to another mode during a spindle
synchronization command.
Before moving to another mode, cancel the
spindle synchronization command.
14 Both SFR (clockwise rotation command) and SRV
(counterclockwise rotation command) are input at
the same time.
Issue either of them.
17 The speed detector parameter settings (bits 2, 1,
and 0 of parameter No. 4011) are not valid.
There is no corresponding speed detector.
Check the parameter settings.
18 The parameter settings are such that a position
sensor is not used (position control not performed
(bits 3, 2, 1, and 0 of parameter No. 4002), but
position coder system orientation is issued.
Check the parameter settings and the input signal.
24 If index is performed continuously in position coder
system orientation, an incremental operation is
performed first (INCMD = 1), then an absolute
position command (INCMD = 0) is input.
Check INCMD (incremental command).
If an absolute position command is to follow, be
sure to perform absolute position command
orientation first.
29 The parameter settings are such that the
shortest-time orientation function is used (bit 6 of
parameter No. 4018 = 0, Nos. 4320 to 4323 ≠0).
In the αi series spindle amplifier, the shortest-time
orientation function cannot be used. Use
normal-system orientation.
31 The hardware configuration is such that the spindle
FAD function cannot be used.
In this case, the motor is not activated.
Check the CNC model.
33 The hardware configuration is such that the spindle
EGB function cannot be used.
In this case, the motor is not activated.
Check the CNC model.
34 Both the spindle FAD function and the spindle EGB
function are enabled.
In this case, the motor is not activated.
The two functions cannot be used at the same
time. Enable either function only.
34 The submodule SM (SSM) is faulty or the
connection between SPM and SSM is in error.
Submodule SM (SSM) error (synchronous
spindle)
NOTE
*2 PSM contact signal
Between ESP1 and ESP2 on the PSM
Contact open: Emergency stop
Contact closed: Normal operation
(11) Overheat alarms (OH alarm)
Number Message Description
OH0700 LOCKER OVERHEAT CNC cabinet overheat
OH0701 FAN MOTOR STOP PCB cooling fan motor abnormality
H.ALARM LIST APPENDIX B-63944EN/03
- 2384 -
Number Message Description
OH0704 OVERHEAT Spindle overheat due to detection of changes in the spindle
speed
- When the cutting load is large, offload the cutting
conditions.
- Check if the cutting tool became dull.
- Check if the spindle amplifier malfunctions.
(12) Other alarms (DS alarm)
Number Message Description
DS0001 SYNC EXCESS ERROR (POS DEV) In feed axis synchronization control, the difference in the
amount of positional deviation between the master and slave
axes exceeded the parameter (No. 8323) setting value.
This alarm occurs only for the slave axis.
DS0002 SYNC EXCESS ERROR ALARM 1 In feed axis synchronization control, the difference in the
amount of synchronization between the master and slave
axes exceeded the parameter (No. 8331) setting value.
This alarm occurs only for the slave axis.
DS0003 SYNCHRONIZE ADJUST MODE The system is in the synchronize adjust mode.
DS0004 EXCESS MAXIMUM FEEDRATE The malfunction prevention function detected the command
in which a value exceeding the maximum speed was
specified.
DS0005 EXCESS MAXIMUM ACCELERATION The malfunction prevention function detected the command
in which a value exceeding the maximum acceleration was
specified.
DS0006 ILLEGAL EXECUTION SEQUENCE The malfunction prevention function detected an illegal
execution sequence.
DS0007 ILLEGAL EXECUTION SEQUENCE The malfunction prevention function detected an illegal
execution sequence.
DS0008 ILLEGAL EXECUTION SEQUENCE The malfunction prevention function detected an illegal
execution sequence.
DS0009 ILLEGAL EXECUTION SEQUENCE The malfunction prevention function detected an illegal
execution sequence.
DS0010 ILLEGAL REFERENCE AREA The malfunction prevention function detected an invalid
reference area.
DS0011 ILLEGAL REFERENCE AREA The malfunction prevention function detected an invalid
reference area.
DS0012 ILLEGAL REFERENCE AREA The malfunction prevention function detected an invalid
reference area.
DS0013 ILLEGAL REFERENCE AREA The malfunction prevention function detected an invalid
reference area.
DS0014 TOOL CHANGE DETECT MACHINE
LOCK
A machine lock is turned on for the Z axis for which the tool is
being changed.
DS0015 TOOL CHANGE DETECT MIRROR
IMAGE
A mirror image is turned on for the Z axis for which the tool is
being changed.
DS0016 SERIAL DCL:FOLLOW-UP ERROR (1) The settings of parameters No.1883 and No.1884 fall
outside the range.
(2) The current position at establishment of the origin
subtracted by the distance between the reference
positions (detection unit) exceeded ±2147483647.
Change the current position or reference position to
prevent this situation.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2385 -
Number Message Description
DS0017 SERIAL DCL:REF-POS ESTABLISH
ERR
The travel amount at the FL speed at establishment of the
origin exceeded the setting of parameter No. 14010.
DS0018 SERIAL DCL:MISMATCH(SSYNC CTRL) Of the master and slave axes for feed axis synchronous
control, one axis is a linear scale with the origin and the other
is not a linear scale with the origin. In such a configuration,
the feed axis synchronous control selection signal
(SYNC<Gn138> or SYNCJ <Gn140>) needs to be set to 0 to
establish the origin.
DS0020 REFERENCE RETURN INCOMPLETE An attempt was made to perform an automatic return to the
reference position on the perpendicular axis before the
completion of a return to the reference position on the
angular axis.
However, this attempt failed because a manual return to the
reference position during angular axis control or an automatic
return to the reference position after power-up was not
commanded. First, return to the reference position on the
angular axis, then return to the reference position on the
perpendicular axis.
DS0022 DUAL CHECK SAFETY IS NOT
WORKED
Bit 6 (DCE) of parameter No. 1902 has set the Dual Check
Safety function to be disabled.
DS0023 ILLEGAL PARAMETER (I-COMP VAL) The setting of the inclination compensation parameter is
incorrect.
The compensation per compensation point is too large or too
small.
DS0024 UINT SIGNAL WAS ILLEGALLY INPUT An interruption custom macro was started during movement
to the machining restart position at the dry run speed.
DS0025 G60 CANNOT BE EXECUTED The state of a mirror image is different between the time
when look-ahead of a block for unidirectional positioning was
performed and the time when execution of the block was
started, so unidirectional positioning cannot be performed.
Modify the program.
DS0026 MISMATCH OF ANGULAR AXIS(D.C.S) On angular axis control, one of the angular/perpendicular
axes is the scale with ref-pos, and the other of them is not
the scale with ref-pos. Such system is not admired.
DS0027 MISMATCH OF SYNCHRONOUS
AXIS(D.C.S)
Master/slave axes of axis synchronous control, one of them
is the linear scale with distance-coded reference marks, and
the other of them is not the linear scale with distance-coded
reference marks.
Please establish reference position with the input signal
SYNCn<G138>, SYNCJn<G140> or parameter setting to 0.
DS0029 UNAVAILABLE ROT AXIS MOVE IN TPC In tool posture control, the rotation axis fell outside the set
operation range (parameters No. 19741 to No. 19744).
Review the machine configuration and command.
DS0030 TOOL DIRC CMP IMPOSSIBLE When tool center point control is performed in the angular
surface machining command mode or workpiece placement
error compensation is performed in a 5-axis cutting machine,
if settings are made to make compensation in the tool
direction (bit 0 (RCM) of parameter No. 11200 is 1), the
position of the rotation axis could not be obtained.
H.ALARM LIST APPENDIX B-63944EN/03
- 2386 -
Number Message Description
DS0059 SPECIFIED NUMBER NOT FOUND [External data I/O]
The No. specified for a program No. or sequence No.
search could not be found.
There was an I/O request issued for a pot No. or offset (tool
data), but either no tool numbers have been input since
power ON or there is no data for the entered tool No.
[External workpiece No. search]
The program corresponding to the specified workpiece No.
could not be found.
DS0131 TOO MANY MESSAGE An attempt was made to display an external operator
message or external alarm message, but five or more
displays were required simultaneously.
DS0132 MESSAGE NUMBER NOT FOUND An attempt to cancel an external operator message or
external alarm message failed because the specified
message number was not found.
DS0133 TOO LARGE NUMBER A value other than 0 to 4095 was specified as the external
operator message or the external alarm message number.
DS0300 APC ALARM: NEED REF RETURN A setting to zero position for the absolute position detector
(association with reference position and the counter value of
the absolute position detector) is required. Perform the return
to the reference position.
This alarm may occur with other alarms simultaneously.
In this case, other alarms must be handled first.
DS0306 APC ALARM: BATTERY VOLTAGE 0 The battery voltage of the absolute position detector has
dropped to a level at which data can no longer be held. Or,
the power was supplied to the Pulsecoder for the first time.
The battery or cable is thought to be defective. Replace the
battery with the machine turned on.
DS0307 APC ALARM: BATTERY LOW 1 The battery voltage of the absolute position detector has
dropped to a level at which a replacement is required.
Replace the battery with the machine turned on.
DS0308 APC ALARM: BATTERY LOW 2 The battery voltage of the absolute position detector dropped
to a level at which a replacement was required in the past.
(including during power off)
Replace the battery with the machine turned on.
DS0309 APC ALARM: REF RETURN
IMPOSSIBLE
An attempt was made to set the zero point for the absolute
position detector by MDI operation when it was impossible to
set the zero point.
Rotate the motor manually at least one turn, and set the zero
position of the absolute position detector after turning the
CNC and servo amplifier off and then on again.
DS0310 NOT ON RETURN POINT The return position recorded during retraction is not reached
during recovery. The position may be displaced during
recovery due to a machine lock or mirror image.
Perform the operation again after making a reset.
DS0405 ZERO RETURN END NOT ON REF The axis specified in automatic zero return was not at the
correct zero point when positioning was completed.
Perform zero return from a point whose distance from the
zero return start position to the zero point is 2 or more
revolutions of the motor.
Other probable causes are:
- The positional deviation after triggering the deceleration
dog is less than 128.
- Insufficient voltage or malfunctioning Pulsecoder.
B-63944EN/03 APPENDIX H.ALARM LIST
- 2387 -
Number Message Description
DS1120 UNASSIGNED ADDRESS (HIGH) The upper 4 bits (EIA4 to EIA7) of an external data I/O
interface address signal are set to an undefined address
(high bits).
DS1121 UNASSIGNED ADDRESS (LOW) The lower 4 bits (EIA0 to EIA3) of an external data I/O
interface address signal are set to an undefined address (low
bits).
DS1124 OUTPUT REQUEST ERROR OUTPUT REQUEST ERROR An output request was issued
during external data output, or an output request was issued
for an address that has no output data.
DS1128 DI.EIDLL OUT OF RANGE The numerical value input by external data input signals ED0
to ED31 has exceeded the permissible range.
DS1130 SEARCH REQUEST NOT ACCEPTED No requests can be accepted for a program No. or a
sequence No. search as the system is not in the memory
mode or the reset state.
DS1131 EXT-DATA ERROR (OTHER) [External Data I/O]
An attempt was made to input tool data for tool offset by a
tool No. during loading by the G10 code.
DS1150 A/D CONVERT ALARM A/D converter malfunction
DS1184 PARAMETER ERROR IN TORQUE An invalid parameter was set for torque control.
The torque constant parameter is set to “0”.
DS1185 OVER MAXIMUM FEED The maximum cutting feedrate or rapid traverse feedrate was
exceeded in G54.3.
DS1448 ILLEGAL PARAMETER (D.C.S.) The setting value of parameter for reference marks is
satisfied the following any conditions.
- The absolute-position detection function is enabled.
- Either parameter 1821 (mark-1 interval) or parameter 1882
(mark-2 interval) is set to 0.
- Parameters 1821 and 1882 have identical settings.
- The difference between the settings made for parameters
1821 and 1882 is greater than or equal to twice either
setting.
- The setting value of parameters 1883 and 1884 are over
the valid data range.
DS1449 REFERENCE MARK ARE DIFFERENT
FROM PARAMETER
In case of distance coded linear scale I/F, the actual interval
of reference marks is different from parameter
(No.1821,1882) setting value.
DS1450 ZERO RETURN NOT FINISHED 1st reference position return (CDxX7 to CDxX0: 17h (Hex))
was specified when the manual reference position return was
not executed with the reference position return function
enabled (parameter ZRN (No. 1005#0) set to “0”).
DS1451 IMPROPER PMC AXIS COMMAND The PMC axes cannot be controlled in this state.
DS1512 EXCESS VELOCITY The feedrate of the linear axis during polar coordinate
interpolation exceeded the maximum cutting feedrate.
DS1514 ILLEGAL MOTION IN G12.1 MODE In a hypothetical axis direction compensation during the polar
coordinate interpolation mode, an attempt is made to travel
to the area in which the travel cannot be made.
DS1553 EXCESS VELOCITY IN G43.4/G43.5 The axis rate was attempt to exceed the maximum cutting
feedrate and travel by the pivot tool length compensation.
H.ALARM LIST APPENDIX B-63944EN/03
- 2388 -
Number Message Description
DS1710 ILLEGAL ACC. PARAMETER
(OPTIMUM TORQUE ACC/DEC)
There are errors in the parameters of permissible
acceleration for Optimum Torque Acceleration/Deceleration.
One of the following is the cause.
1) The ratio of the acceleration for deceleration to the
acceleration for the acceleration is lower than the limited
value.
2) The time to decelerate to 0 is larger than the maximum.
DS1931 MACHINE PARAMETER INCORRECT One of parameters Nos. 19665 to 19667 and Nos.19680 to
19744 used to configure the machine contains an error.
DS1932 DI.THML SIGNAL ON One of the parameters used to configure the machine is
rewritten while the tool direction thermal displacement
compensation function is enabled.
DS1933 NEED REF RETURN(SYNC:MIX:OVL) The relation between a machine coordinate of an axis in
synchronization, composition, or superposition control, and
the absolute, or relative coordinate was displaced.
Perform the manual return to the reference position.
(13) Malfunction prevention function alarms (IE alarm)
Number Message Description
IE0001 + OVERTRAVEL ( SOFT 1 ) The malfunction prevention function detected that stored stroke
check 1 on the positive side was exceeded.
IE0002 - OVERTRAVEL ( SOFT 1 ) The malfunction prevention function detected that stored stroke
check 1 on the negative side was exceeded.
IE0003 + OVERTRAVEL ( SOFT 2 ) The malfunction prevention function detected that stored stroke
check 2 on the positive side was exceeded.
IE0004 - OVERTRAVEL ( SOFT 2 ) The malfunction prevention function detected that stored stroke
check 2 on the negative side was exceeded.
IE0005 + OVERTRAVEL ( SOFT 3 ) The malfunction prevention function detected that stored stroke
check 3 on the positive side was exceeded.
IE0006 - OVERTRAVEL ( SOFT 3 ) The malfunction prevention function detected that stored stroke
check 3 on the negative side was exceeded.
IE0007 EXCESS MAXIMUM REV. DATA The malfunction prevention function detected the command in
which a value exceeding the maximum speed was specified.
IE0008 ILLEGAL ACC/DEC The malfunction prevention function detected the
acceleration/deceleration error.
IE0009 ILLEGAL MCN COODINATE The malfunction prevention function detected the displacement of
a machine coordinate in the check point.
B-63944EN/03 APPENDIX
- 2389 -
I.PC TOOL FOR MEMORY CARD
PROGRAM OPERATION/EDITING
I PC TOOL FOR MEMORY CARD
PROGRAM OPERATION/EDITING
Appendix I, "PC TOOL FOR MEMORY CARD PROGRAM
OPERATION/EDITING", consists of the following sections:
I.1 PC TOOL FOR MEMORY CARD PROGRAM
OPERATION/EDITING.........................................................2390
I.2 NAMING RULES...................................................................2401
I.3 RULES OF CHARACTERS IN PROGRAM FILE ...............2403
I.4 ERROR MESSAGE AND NOTE...........................................2406
APPENDIX B-63944EN/03
- 2390 -
I. PC TOOL FOR MEMORY CARD
PROGRAM OPERATION/EDITING
I.1 PC TOOL FOR MEMORY CARD PROGRAM
OPERATION/EDITING
Overview
By using this PC tool, you can make the memory card program file
("FANUCPRG.BIN") which is needed for the function "Memory Card
Program Operation/Editing".
The maximum size of the memory card program file is 2048 Mbytes
(2 Gbytes). The "Memory Card Program Operation/Editing" function
needs the memory card which has the memory card program file on
the FAT formatted memory card.
This PC tool can be operated on a PC in the marketplace and with
following OS :
• Windows(R)NT4.0 Workstation (SP5 or later)
• Windows(R)2000 Professional
And acceptable specification is as followings :
• Memory : 32Mbytes or more
• Hard disk : 10Mbytes or more free space and additional
space for the memory card program file
I.1.1 Usage Notes
Before using this PC tool, please make sure there is no [temp] folder
on the same place of this PC tool.
[temp] folder is created and used by this PC tool as work folder.
If [temp] folder is created, please do not access this folder.
[temp] folder and the files located in this folder will be deleted by this
PC tool.
I.1.2 List of Functions of PC Tool
• Browsing the folders of the memory card program file
• Adding a program to the memory card program file by dropping
the program into this PC tool from Explorer etc. (hereinafter
referred to as "drop in")
• Extracting a program in the memory card program file as a text
file on Windows file system by dropping out from this PC tool
into Explorer etc. (hereinafter referred to as "drop out")
• Renaming a program in the memory card program file
• Deleting a program in the memory card program file
• Creating a new folder into the memory card program file
• Renaming a folder in the memory card program file
• Deleting a folder in the memory card program file
• Display of free space on the memory card program file
• Sorting list view of the memory card program file
B-63944EN/03 APPENDIX
- 2391 -
I.PC TOOL FOR MEMORY CARD
PROGRAM OPERATION/EDITING
I.1.3 Explanation Of Operations
- Outline of screen
1) Menu bar : The menu of this PC tool is displayed.
2) Tree view : Browsing the folders of the memory card program
file.
3) Column : Attributes of each file or folder in the memory card
program file.
4) List view : Contents of selected folder are displayed.
5) Status bar : Used and Unused space in the memory card program
file are displayed.
- Initial Option dialogue window
When this PC tool starts up, the Option dialogue window is displayed.
Please select "Open an existing file" or "Create a new file".
(1)
(2)
(3)
(4)
(5)
APPENDIX B-63944EN/03
- 2392 -
I. PC TOOL FOR MEMORY CARD
PROGRAM OPERATION/EDITING
• When "Open an existing file" is selected
After OK button pushed, "Open" dialogue window is displayed.
Please select the existing memory card program file.
• When "Create a new file" is selected
After OK button pushed, "Save As" dialogue window is
displayed.
Please create a new memory card program file on the selected
folder.
B-63944EN/03 APPENDIX
- 2393 -
I.PC TOOL FOR MEMORY CARD
PROGRAM OPERATION/EDITING
When the new the memory card program file is created, the following
items need to be selected:
• Folder/Program Numbers
• Program Size
"Folder/Program Numbers" can be selected among 63 / 500 / 1000.
The default value is 63.
"Program Size" can be selected among 2Mbyte, 4Mbyte, 8Mbyte, and
Customize. The default value is 2Mbyte.
NOTE
1 When "Customize" size is selected, it is available to
cover the range from 2Mbyte to 2048Mbyte.
2 Though the maximum size is 2048Mbyte, a slight
loss exists by system use.
3 The number of "Folders" in the status bar includes
number of program file and folder.
During creating of the memory card program file, the progress bar is
being displayed. This progress bar is also displayed during executing
of Drop-in and Drop-out.
If you push [Cancel] button, the execution is stopped.
APPENDIX B-63944EN/03
- 2394 -
I. PC TOOL FOR MEMORY CARD
PROGRAM OPERATION/EDITING
- Menu
File menu
[New]
Create a new memory card program file.
[Open...]
Open the existing memory card program file.
[Exit]
Terminate this PC tool.
Edit menu
[New Folder]
Create new folder. It is available during Tree view selected.
Up to seven hierarchical levels starting from the user root folder
(/USER) are permitted.
/USER/PATH1/Aaa/Bbb/Ccc/Ddd/O123
1 2 3 4 5 6 7(not folder)
[Delete]
Delete program files or folders.
If you delete a folder, all folders and program files in the folder
will be deleted.
[Rename]
Rename a folder or file.
B-63944EN/03 APPENDIX
- 2395 -
I.PC TOOL FOR MEMORY CARD
PROGRAM OPERATION/EDITING
NOTE
For naming folder and program file, characters
which can be used are limited. Please refer to
"Naming rules".
Option menu
[Hide Confirm Message]
When the following operations are executed, the following
Confirm Message is popped up before the memory card program
file is modified.
1. Delete folder or program file
2. Rename folder or program file
3. Drop-in program file
4. Add folder
If the [OK] button is pushed, the operation advances.
If the [Cancel] button is pushed, the operation is abandoned.
When the [Hide Confirm Message] in menu bar is checked, the
Confirm Message is not displayed and the operation advances at
once. The default setting is the Confirm Message displayed.
[Ignore Error Code]
When the [Ignore Error Code] in menu bar is checked, program
file which includes unusable characters can be dropped in. The
unusable characters in the program file will be ignored and will
not be written into the memory card program file.
APPENDIX B-63944EN/03
- 2396 -
I. PC TOOL FOR MEMORY CARD
PROGRAM OPERATION/EDITING
[Change Work Folder]
Work folder is used for temporarily keeping the dropped out files.
If work folder has no enough free space, Drop-out will not be
executed. To avoid this, you can check this option and change
the work folder to an area where there is enough free space. With
default setting, work folder [temp] will be created on the same
place of this PC tool "FPRG_30i.exe".
If you changed the default work folder, the following warning
message is popped up.
If the [OK] button is pushed, the operation advances.
If the [Cancel] button is pushed, the operation is abandoned.
If the work folder has been changed before, the following
warning message is popped up.
If the [OK] button is pushed, the operation advances.
If the [Cancel] button is pushed, the operation is abandoned.
WARNING
1 At this PC tool terminated, all files in the work
folder are deleted.
2 During this PC tool executing, do not access the
files in the work folder. If the access is done, there
is no assurance of normal operation.
B-63944EN/03 APPENDIX
- 2397 -
I.PC TOOL FOR MEMORY CARD
PROGRAM OPERATION/EDITING
Help menu
[About...]
Version number of this PC tool is displayed.
- Mouse Operation
[Drop-in and Drop-out]
• Drop-in from Explorer
NC program can be added by dropping files including the NC
files into the List view window of this PC tool from Explorer
NC program name and update time is the same as the Dropped-in
files.
If "Oxxxxxxxx" or "<xxxx>" exists at the top of files, These
"Oxxxxxxxx" and "<xxxx>" become NC program name. If not
exist, each file name becomes NC program name.
Examples
Name of external file Top of external file Name of internal file Program number
O1234 N10G00 O1234 1234
O123N10G00 N10G00 O123N10G00 Not an O number program
test.txt O1234N10G00 O1234 1234
test.txt <O1234> O1234 1234
test.txt <O1234N10> O1234N10 Not an O number program
O1234 <O1234N10> O1234N10 Not an O number program
O001234 N10G00 O1234 1234
O001234N10G00 N10G00 O001234N10G00 Not an O number program
test.txt O001234 O1234 1234
test.txt <O001234> O1234 1234
test.txt <O001234N10G00> O001234N10G00 Not an O number program
APPENDIX B-63944EN/03
- 2398 -
I. PC TOOL FOR MEMORY CARD
PROGRAM OPERATION/EDITING
NOTE
1 For naming program file, please refer to the
following chapter "Naming rules of Program file".
2 For usable characters in Program file, please refer
to the following chapter "Rules of characters in
Program file".
3 The updating time of program file is available from
1997 to 2037.
This PC tool can check contents of dropped-in program file
according to "Rules of characters in Program file". However, this
PC tool does not check grammar of NC program.
The program file can only have one NC program. Therefore, the
NC program output from CNC cannot be dropped in directly.
O1
G91 X10. Y10.
M30
O10
G91 X10. Y10.
M30
%
O1
G91 X10. Y10.
M30
%
O1
G91 X10. Y10.
M30
Available for Drop-in
Example of Program
<O1>
G91 X10. Y10.
M30
Unavailable for Drop-in
NOTE
1 If the same named program file exists, another
same named program file cannot be dropped in.
2 If free space on the memory card program file is
lacking, new program file cannot be dropped in.
3 If the NC program name is not compliant with
"Naming rules of Program file", the program file can
not be dropped in.
If the File name acts as Program number, "O" is displayed on the
first row of list view.
B-63944EN/03 APPENDIX
- 2399 -
I.PC TOOL FOR MEMORY CARD
PROGRAM OPERATION/EDITING
• Drop-out from List view window
Drop-out from list view of this PC tool to Explorer is available.
NOTE
Do not drop out to Work folder. If dropped out to
Work folder, this PC tool cannot continue to
function normally.
- Pop-up menu
Pop-up menu is displayed by clicking the right mouse button.
• Focus on Tree view
Clicking "New Folder", a new folder is created on selected
folder.
Clicking "Delete", the selected folder is deleted.
Clicking "Rename", the selected folder is renamed.
If clicking on root folder, "Delete" and "Rename" are not activated.
• Focus on List view
• Clicking "Delete", the selected folder or program file is deleted.
• Clicking "Rename", the selected folder or program file is
renamed.
APPENDIX B-63944EN/03
- 2400 -
I. PC TOOL FOR MEMORY CARD
PROGRAM OPERATION/EDITING
- Display of free space on the memory card program file ("FANUCPRG.BIN")
Number of used folder, size of used space, number of unused folder,
and size of free space are displayed on status bar in the lower portion
of the screen.
When a new memory card program file is created, two reserved folder
are also created. Therefore, the number of used folder is two. However
it does not show that number of unused folder is reduced.
The display of status bar is renewed at creating or deleting a folder,
dropping-in from Explorer, and deleting a program file.
- Sorting list view of the memory card program file
When a column is being clicked, the list view of the memory card
program file is being sorted by the column key in ascending or
descending order.
The initial display is sorted by NAME key in ascending order.
Clicking
B-63944EN/03 APPENDIX
- 2401 -
I.PC TOOL FOR MEMORY CARD
PROGRAM OPERATION/EDITING
I.2 NAMING RULES
Overview
Naming rules of folder and program file are described as follows.
I.2.1 Naming Rules of Program File
Here are Naming rules of Program file:
• Program file name can have a maximum of 32 characters.
• Program file name can have following characters.
Alphabet(Upper and lower case letter), numeric character,
"-"(minus), "+"(plus), "_"(under bar), "."(dot)
"." and ".." can not be used since these are reserved for system
use.
- The File name acts as Program number
When the File name is "O"+ 1-99999999, the file name acts as
Program number.
Example)
"O123" Program number 123
"O1" Program number 1
"O3000" Program number 3000
"O99999999" Program number 99999999
"O0123" Program number 123
The file name does not act as Program number, and can be dropped in:
"ABC" Top of character is not upper case letter of "O".
"o123" Top of character is not upper case letter of "O".
"O0123XY" Characters following the "O" contains alphabet.
The file name does not act as Program number, and cannot be dropped
in:
"O123456789" Numeric characters exceed 8 digits.
NOTE
1 Program file name cannot be repeated in a Folder.
2 If program file name starts with "O" and the next
eight characters are all numeric characters, the "0"
(zero) after the "O" will be deleted.
APPENDIX B-63944EN/03
- 2402 -
I. PC TOOL FOR MEMORY CARD
PROGRAM OPERATION/EDITING
I.2.2 Naming Rules Of Folder
Here are Naming rules of Folder:
• Folder name can have a maximum of 32 characters.
• Folder name can have following characters.
Alphabet(Upper and lower case letter), numeric character,
"-"(minus), "+"(plus), "_"(under bar), "." (dot)
"." and ".." can not be used since these are reserved for system
use.
NOTE
Folder name cannot be repeated in a Folder.
B-63944EN/03 APPENDIX
- 2403 -
I.PC TOOL FOR MEMORY CARD
PROGRAM OPERATION/EDITING
I.3 RULES OF CHARACTERS IN PROGRAM FILE
Overview
Words in parentheses "( )" in Program file are treated as comments.
The mark of comment start "(" is named "Control-out".
The mark of comment end ")" is named "Control-in".
"Control-out" and "Control-in" must make a pair. The order is 1st -
"Control-out" and 2nd -"Control-in". And nested parentheses is not
available.
NOTE
1 When a program file is dropped in, space code
(0x20 SPC) , tab code (0x09 HT) , carriage return
code(0x0d CR) and percent code(0x25 %) is
deleted. If "%" is found in Control-in, characters
between "%" and next "LF" (0x0a) is deleted.
2 The front of program number ":" is changed to
"O"(O as in Oscar) while the program file dropped
in.
3 The program file can only have one NC program.
APPENDIX B-63944EN/03
- 2404 -
I. PC TOOL FOR MEMORY CARD
PROGRAM OPERATION/EDITING
I.3.1 Usable Characters in Program File
- Usable characters in Control-in
List of ANSI(ASCII) codes of usable characters(hexadecimal form)
Code Character Code Character Code Character Code Character
0a LF 3f ? 58 X 74 t
23 # 40 @ 59 Y 75 u
26 & 41 A 5a Z 76 v
28 ( 42 B 5b [ 77 w
29 ) 43 C 5d ] 78 x
2a * 44 D 5f _ 79 y
2b + 45 E 61 a 7a z
2c , 46 F 62 b
2d - 47 G 63 c
2e . 48 H 64 d
2f / 49 I 65 e
30 0 4a J 66 f
31 1 4b K 67 g
32 2 4c L 68 h
33 3 4d M 69 i
34 4 4e N 6a j
35 5 4f O 6b k
36 6 50 P 6c l
37 7 51 Q 6d m
38 8 52 R 6e n
39 9 53 S 6f o
3a : 54 T 70 p
3c < 55 U 71 q
3d = 56 V 72 r
3e > 57 W 73 s
NOTE
In the Control-in, "O", ":", and "<" can not be used
at top of the line except for the 1st line.
B-63944EN/03 APPENDIX
- 2405 -
I.PC TOOL FOR MEMORY CARD
PROGRAM OPERATION/EDITING
- Usable characters in Control-out(characters in parentheses)
List of ANSI(ASCII) codes of usable characters(hexadecimal form)
Code Character Code Character Code Character Code Character
0a LF 3c < 55 U 71 q
20 SPC 3d = 56 V 72 r
22 “ 3e > 57 W 73 s
23 # 3f ? 58 X 74 t
24 $ 40 @ 59 Y 75 u
26 & 41 A 5a Z 76 v
27 ‘ 42 B 5b [ 77 w
2a * 43 C 5d ] 78 x
2b + 44 D 5f _ 79 y
2c , 45 E 61 a 7a z
2d - 46 F 62 b
2e . 47 G 63 c
2f / 48 H 64 d
30 0 49 I 65 e
31 1 4a J 66 f
32 2 4b K 67 g
33 3 4c L 68 h
34 4 4d M 69 i
35 5 4e N 6a j
36 6 4f O 6b k
37 7 50 P 6c l
38 8 51 Q 6d m
39 9 52 R 6e n
3a : 53 S 6f o
3b ; 54 T 70 p
APPENDIX B-63944EN/03
- 2406 -
I. PC TOOL FOR MEMORY CARD
PROGRAM OPERATION/EDITING
I.4 ERROR MESSAGE AND NOTE
Error may occur when using this application, hereafter explains the
error messages and gives relative instructions.
I.4.1 List of Error Message
When an error occurred, the error message box is displayed as
follows.
Message Remarks
Failed to open the file you specified. If failed to open once again, the file may be broken.
Failed to read or write to the specified file.
There is insufficient disk space. There is no enough free space to create a new memory card
program file or to put drop out files to work folder. In the latter
case, please refer to chapter "Menu" [Change Work Folder]
File name is not correct. Please refer to the chapter "Naming rules of Program file".
Input name is already exists. Please input another name.
File name is already exists. Please input another name.
Input name is not correct. Please refer to the chapter "Naming rules".
Please input an integer between 2 and
2048
The size of the memory card program file is available from
2Mbyte to 2048Mbyte.
An illegal character is included in the
specified file.
Please refer to the chapter "Rules of characters in Program file".
Last update time of the specified file is
unsupported.
The updating time of program file is available from 1997 to 2037.
The memory card program file you
specified cannot be identified.
The specified file format is not the memory card program file
There is insufficient free folder. Please delete unnecessary program files or folders.
There is insufficient free program space. Please delete unnecessary program files.
Folder deeper than 7 cannot be created.
Root folder cannot be deleted.
Root folder cannot be renamed.
Failed to create work folder. Please check whether the [temp] work folder is able to create or
not.
In default, the [temp] work folder is created on the same place of
this PC tool "FPRG_30i.exe".
Process has been cancelled.
The specified work folder is not found. The Drop-out cannot be executed.
Terminate this PC tool. And check the setting of Work Folder on
the Option dialogue window.
Only one instance of this application can
be executed.
Double activation of this PC tool cannot be executed.
I.4.2 Note
- Folder and Program Numbers
Folder and Program Numbers can be selected among 63 / 500 / 1000.
For selecting the Numbers of 500 or 1000, the option "Registered
programs expan. On the memory card" is needed in CNC side.
B-63944EN/03 INDEX
i-1
INDEX
<Number>
10.4" LCD CNC Display Panel................................... 1001
12.1" LCD CNC Display Panel................................... 1001
15" LCD CNC Display Panel...................................... 1002
3-DIMENSIONAL CUTTER COMPENSATION........897
5-AXIS MACHINING FUNCTION ............................. 772
7.2" LCD CNC Display Panel..................................... 1000
8.4" LCD CNC Display Panel..................................... 1000
<A>
ABSOLUTE AND INCREMENTAL
PROGRAMMING ........................................................ 210
Absolute multiple command .........................................885
ACTION TO BE TAKEN WHEN A PROBLEM
OCCURRED............................................................... 1964
ACTIVE BLOCK CANCEL FUNCTION.................. 1172
Actual Feedrate Display.............................................. 1439
Actual Feedrate Display (15-inch Display Unit)......... 1455
Addition of Workpiece Coordinate System Pair (G54.1
or G54) .......................................................................... 201
ADJUSTMENT OF THE BRIGHTNESS OF
THE MONOCHROME LCD........................................997
AI CONTOUR CONTROL FUNCTION I AND AI
CONTOUR CONTROL FUNCTION II (G05.1).......... 653
ALARM AND SELF-DIAGNOSIS FUNCTIONS..... 1230
Alarm Display ..................................................... 996, 1231
Alarm history ..................................................... 1781,1860
ALARM HISTORY DISPLAY .................................. 1233
ALARM LIST............................................................. 2321
Altering a Word ..........................................................1355
Angular Axis Control.................................................. 1085
Animation.................................................................... 1933
ANIMATION GRAPHIC screen ................................ 1939
ARBITRARY ANGULAR AXIS CONTROL.............. 721
ARITHMETIC AND LOGIC OPERATION ................502
ARITHMETIC AND LOGICAL OPERATION........... 596
Automatic Coordinate System Setting .......................... 203
Automatic Corner Override...........................................166
AUTOMATIC INSERTION OF SEQUENCE
NUMBERS ................................................................. 1343
AUTOMATIC OPERATION .............................. 986,1110
Automatic override for inner corners (G62).................. 166
Automatic Setting for Grid Position Matching..............701
AUXILIARY FUNCTION............................................306
AUXILIARY FUNCTION (M FUNCTION)................307
AUXILIARY FUNCTION OUTPUT BLOCK
REVERSE MOVEMENT FOR MANUAL
HANDLE RETRACE .................................................1108
Available Keys............................................................1374
Axis Configuration for Axis Synchronous Control ....... 693
Axis Control by PMC..................................................1084
AXIS CONTROL COMMAND....................................608
AXIS CONTROL FUNCTIONS...................................691
Axis status display.......................................................1212
Axis Synchronization Control .....................................1083
AXIS SYNCHRONOUS CONTROL ...........................692
Axis Synchronous Control Torque Difference Alarm...706
<B>
Background Editing.....................................................1483
Background Editing (15-inch Display Unit) ...............1534
BACKING UP VARIOUS DATA ITEMS .................1965
Battery for Absolute Pulsecoders ................................1975
Battery in the PANEL i (3 VDC) ................................1973
BRANCH AND REPETITION.....................................512
<C>
Canceling Spindle Positioning ......................................234
CHANGING FILE ATTRIBUTES ............................. 1409
CHANGING FOLDER ATTRIBUTES ...................... 1404
Changing Workpiece Coordinate System......................194
CHARACTER-TO-CODES CORRESPONDENCE
TABLE............................................................... 2313,2314
Check by Running the Machine ....................................988
CHECKING BY DIAGNOSTIC DISPLAY...............1234
CIRCULAR INTERPOLATION (G02, G03).................59
CIRCULAR THREADING (G35, G36) .......................134
CODES AND RESERVED WORDS USED IN
CUSTOM MACROS ....................................................558
Color Setting Screen....................................................1738
Color Setting Screen (15-inch Display Unit) ..............1817
COMMAND FOR MACHINE OPERATIONS -
AUXILIARY FUNCTION..............................................29
Command type selection screen ......................... 1506,1557
COMMON MEMORY BETWEEN EACH PATH.......972
INDEX B-63944EN/03
i-2
COMPENSATION FUNCTION................................... 370
Condition Transition (ZEDGE Statement)....................600
Conditional Branch (IF Statement) ...............................515
Conditional Branch (ZONCE Statement)......................599
Confirmation of a data update during the data setting
process......................................................................... 1209
Confirmation of incremental input ..............................1205
Confirmation of the deletion of all data ...................... 1208
Confirmation of the deletion of the program............... 1207
Confirmation of the start from a middle block............ 1213
CONSTANT SURFACE SPEED CONTROL
(G96, G97) ....................................................................225
CONTINUOUS HIGH-SPEED SKIP FUNCTION ...... 143
CONTROL ON REAL TIME MACRO
COMMANDS ...............................................................598
CONTROLLED AXES...................................................34
Controlled axis configuration example ......................... 761
COORDINATE SYSTEM ............................................186
Coordinate System on Part Drawing and Coordinate
System Specified by CNC - Coordinate System ............. 18
COORDINATE VALUE AND DIMENSION.............. 209
Copy............................................................................ 1377
Copying and Moving Files between Devices .............. 1382
CREATING A FOLDER ............................................ 1402
CREATING PROGRAMS.......................................... 1341
CREATING PROGRAMS IN TEACH IN MODE
(PLAYBACK)............................................................. 1345
CREATING PROGRAMS USING THE MDI
PANEL........................................................................ 1342
Creation.......................................................................1378
Current Position Display ............................................... 995
CURSOR MOVEMENT LIMITATIONS ON
PROGRAM EDITING................................................ 1365
CUSTOM MACRO.......................................................437
Custom Macro Variables............................................... 594
Customization of Tool Management Data Display .......265
Cut............................................................................... 1377
Cutter Compensation in Composite Type Machine ......939
Cutter Compensation in Table Rotation Type Machine 931
Cutter Compensation in Tool Rotation Type Machine . 900
CUTTING FEED .......................................................... 158
CUTTING FEEDRATE CONTROL ............................ 164
CUTTING POINT INTERPOLATION FOR
CYLINDRICAL INTERPOLATION (G07.1)................90
CUTTING SPEED - SPINDLE FUNCTION..................27
CYLINDRICAL INTERPOLATION (G07.1) ................85
<D>
DATA INPUT/OUTPUT ............................................1239
Data range check ......................................................... 1214
DATA TYPE...............................................................2280
DECIMAL POINT PROGRAMMING.........................216
Default Folders..............................................................322
Definition of the Custom Macro Screen........................641
Definition of the Pattern Menu Screen..........................639
DEFINITION OF THE SCREEN ................................. 638
DEFINITION OF WARNING, CAUTION, AND
NOTE............................................................................. s-2
Deleting a Block..........................................................1357
DELETING A FILE....................................................1408
DELETING A FOLDER.............................................1405
Deleting a Word ..........................................................1356
Deleting All Programs.................................................1363
DELETING BLOCKS ................................................1357
Deleting Multiple Blocks ............................................1358
Deleting One Program.................................................1363
DELETING PROGRAMS ..........................................1363
Description of commands compatible with those for
a hobbing machine (G80, G81) .....................................756
DESCRIPTION OF PARAMETERS..........................1984
Details of Functions ......................................................567
Details of the tilted working plane data setting
screen ................................................................. 1512,1563
DIAMETER AND RADIUS PROGRAMMING..........218
DIAMETER AND RADIUS SETTING SWITCHING
FUNCTION...................................................................219
Direct Input of Workpiece Origin Offset Value
Measured.....................................................................1582
Direct Input of Workpiece Origin Offset Value
Measured (15-inch Display Unit)................................1655
Disabling Life Count.....................................................305
DISPLAY......................................................................994
Display of Run Time and Parts Count.........................1441
Display of Run Time and Parts Count
(15-inch Display Unit) ................................................1457
Display of Three-dimensional Manual Feed (Tool Tip
Coordinates, Number of Pulses, Machine Axis Move
Amount) ......................................................................1447
B-63944EN/03 INDEX
i-3
Display of Three-dimensional Manual Feed (Tool Tip
Coordinates, Number of Pulses, Machine Axis Move
Amount) (15-inch Display Unit) ................................. 1463
Display of updated modal information........................ 1210
Displaying and Entering Setting Data ......................... 1573
Displaying and Entering Setting Data (15-inch Display
Unit) ............................................................................ 1645
Displaying and Setting Custom Macro Common
Variables ..................................................................... 1584
Displaying and Setting Custom Macro Common
Variables (15-inch Display Unit) ................................ 1657
DISPLAYING AND SETTING DATA........................ 991
Displaying and setting magazine screen .....................1591
Displaying and setting magazine screen
(15-inch display unit) .................................................. 1665
Displaying and Setting Parameters.............................. 1723
Displaying and Setting Parameters
(15-inch Display Unit) ................................................ 1802
Displaying and Setting Pattern Data Inputs................. 1642
Displaying and Setting Pattern Data Inputs
(15-inch Display Unit) ................................................ 1718
Displaying and Setting Pitch Error Compensation
Data............................................................................. 1726
Displaying and Setting Pitch Error Compensation
Data (15-inch Display Unit)........................................ 1805
Displaying and Setting Real Time Custom Macro
Data............................................................................. 1586
Displaying and Setting Real Time Custom Macro
Data (15-inch Display Unit)........................................ 1659
Displaying and Setting Run Time, Parts Count, and
Time ............................................................................ 1578
Displaying and Setting Run Time, Parts Count, and
Time (15-inch Display Unit) ....................................... 1650
Displaying and setting the FSSB amplifier setting
screen .......................................................................... 1758
Displaying and setting the FSSB amplifier setting
screen (15-inch Display Unit) ..................................... 1837
Displaying and setting the FSSB axis setting screen... 1759
Displaying and setting the FSSB axis setting screen
(15-inch Display Unit) ................................................ 1838
Displaying and setting the machining parameter
tuning screen ............................................................... 1763
Displaying and setting the machining parameter
tuning screen (15-inch Display Unit) ..........................1843
Displaying and setting the servo setting screen...........1759
Displaying and setting the servo setting screen
(15-inch Display Unit) ................................................1839
Displaying and setting the servo tuning screen ........... 1762
Displaying and setting the servo tuning screen
(15-inch Display Unit) ................................................1842
Displaying and Setting the Software Operator’s
Panel............................................................................1588
Displaying and Setting the Software Operator’s
Panel (15-inch Display Unit).......................................1662
Displaying and setting the spindle tuning screen ........ 1762
Displaying and setting the spindle tuning screen
(15-inch Display Unit) ................................................1842
Displaying and Setting the Workpiece Origin Offset
Value ...........................................................................1581
Displaying and Setting the Workpiece Origin Offset
Value (15-inch Display Unit) ...................................... 1653
Displaying and Setting Three-Dimensional Error
Compensation Data .....................................................1729
Displaying and Setting Three-Dimensional Error
Compensation Data (15-inch Display Unit) ................ 1808
Displaying and Setting Tool Life Management Data ..1625
Displaying and Setting Tool Life Management Data
(15-inch Display Unit) ................................................1701
Displaying and setting tool management screen .........1593
Displaying and setting tool management screen
(15-inch display unit) ..................................................1667
Displaying and Setting Workpiece Setting Error
Compensation Data .....................................................1640
Displaying and Setting Workpiece Setting Error
Compensation Data (15-inch Display Unit) ................ 1716
Displaying and Switching the Display Language........1612
Displaying and Switching the Display Language
(15-inch Display Unit) ................................................1688
Displaying Memory Data ............................................1749
Displaying Memory Data (15-inch Display Unit).......1828
Displaying the executed block ........................... 1468,1521
Displaying the menu screen and selecting a menu item1751
Displaying the menu screen and selecting a menu item
(15-inch Display Unit) ................................................1830
Displaying the Program Number, Program Name, and
Sequence Number .......................................................1882
Displaying the Program Number, Program Name, and
Sequence Number (15-inch Display Unit) ..................1887
INDEX B-63944EN/03
i-4
DISPLAYING THE PROGRAM NUMBER/NAME,
SEQUENCE NUMBER, AND STATUS, AND
WARNING MESSAGES FOR DATA SETTING OR
INPUT/OUTPUT OPERATION.................................1882
Displaying the Status and Warning for Data Setting or
Input/Output Operation ...............................................1883
Displaying the Status and Warning for Data Setting or
Input/Output Operation (15-inch Display Unit) .......... 1888
Displaying the total life of tools of the same type....... 1602
Displaying the total life of tools of the same type
(15-inch display unit) .................................................. 1677
DISTANCE CODED LINEAR SCALE
INTERFACE............................................................... 1080
Distance Coded Rotary Encoder .................................1082
DNC OPERATION.....................................................1118
DRY RUN...................................................................1184
DWELL......................................................................... 174
DWELL/AUXILIARY FUNCTION TIME
OVERRIDE ................................................................ 1182
DYNAMIC GRAPHIC DISPLAY.............................. 1913
<E>
Each tool data screen................................................... 1599
Each tool Data Screen ................................................... 276
Each tool data screen (15-inch display unit) ...............1674
EDIT DISABLE ATTRIBUTE................................... 1349
Editing a Program ............................................... 990, 1470
Editing a Program (15-inch Display Unit) ..................1522
EDITING OF CUSTOM MACROS ...........................1364
EDITING PROGRAM CHARACTERS..................... 1370
EDITING PROGRAMS..............................................1348
Electronic Gear Box...................................................... 736
Electronic Gear Box 2 Pair............................................753
Electronic Gear Box Automatic Phase Synchronization746
EMBEDDED ETHERNET OPERATIONS................ 1330
EMERGENCY STOP ................................................. 1191
ERROR MESSAGE AND NOTE............................... 2406
Exact Stop (G09, G61), Cutting Mode (G64),
Tapping Mode (G63)..................................................... 165
Examples.......................................................................958
EXPLANATION........................................................... 631
EXPLANATION OF OPERATION ............................. 634
Explanation Of Operations.......................................... 2391
EXPONENTIAL INTERPOLATION (G02.3, G03.3)..102
EXTERNAL I/O DEVICES........................................1025
External operator message history ..................... 1784,1863
EXTERNAL OUTPUT COMMANDS......................... 559
EXTERNAL SUBPROGRAM CALL (M198) ........... 1124
<F>
FANUC DOUBLE-BYTE CHARACTER CODE
TABLE........................................................................2315
FEED FUNCTIONS......................................................154
FEED-FEED FUNCTION...............................................16
FEEDRATE INSTRUCTION ON IMAGINARY
CIRCLE FOR A ROTARY AXIS.................................169
FEEDRATE OVERRIDE ...........................................1180
FIGURE COPYING (G72.1, G72.2).............................351
File Attributes................................................................325
File Format and Error Messages..................................1329
File Name...................................................................... 323
FILES............................................................................323
FLOATING REFERENCE POSITION RETURN
(G30.1) ..........................................................................184
Folder Attributes ...........................................................321
Folder Configuration.....................................................318
FOLDERS.....................................................................318
FTP File Transfer Function .........................................1330
Function Keys .............................................................1012
FUNCTION KEYS AND SOFT KEYS......................1009
Functions that are Used When Data is Set ..................1202
Functions that are Used when the Program is
Executed...................................................................... 1210
FUNCTIONS TO SIMPLIFY PROGRAMMING ........350
<G>
G CODE LIST IN THE LATHE SYSTEM ...................45
G CODE LIST IN THE MACHINING CENTER
SYSTEM.........................................................................41
G53, G28, G30, and G30.1 Commands in Tool Length
Compensation Mode .....................................................377
GENERAL ............................................................3,13,981
General Screen Operations..........................................1010
GENERAL WARNINGS AND CAUTIONS ................ s-3
GOTO Statement Using Stored Sequence Numbers .....513
GRAPHIC DISPLAY..................................................1900
GRAPHIC FUNCTION ..............................................1899
GRAPHIC PARAMETER (DYNAMIC GRAPHIC)
screen ................................................................ 1915, 1934
B-63944EN/03 INDEX
i-5
<H>
Heading a Program......................................................1353
HELICAL INTERPOLATION (G02, G03)....................65
HELICAL INTERPOLATION B (G02, G03) ................67
HIGH SPEED PROGRAM CHECK FUNCTION...... 1187
HIGH-SPEED CUTTING FUNCTIONS...................... 652
HIGH-SPEED CYCLE MACHINING ......................... 689
HIGH-SPEED SKIP SIGNAL (G31)............................ 142
How to Indicate Command Dimensions for Moving
the Tool (Absolute, Incremental Commands) .................24
How to View the Position Display Change without
Running the Machine ....................................................989
HYPOTHETICAL AXIS INTERPOLATION (G07) ...131
<I>
INCH/METRIC CONVERSION (G20, G21) ............... 212
INCLINED ROTARY AXIS CONTROL.....................894
INCORRECT THREADED LENGTH ....................... 2302
INCREMENT SYSTEM.................................................37
INCREMENTAL FEED ............................................. 1034
Incremental multiple command..................................... 888
INDIRECT AXIS ADDRESS SPECIFICATION......... 509
Input data range check ................................................ 1203
Input Mode.................................................................. 1374
Input of Customize Data with the Decimal Point..........272
Input/output format of pitch error compensation data. 1264
Input/output format of three-dimensional error
compensation data....................................................... 1268
INPUT/OUTPUT ON EACH SCREEN...................... 1244
INPUT/OUTPUT ON THE ALL IO SCREEN........... 1303
Inputting a program..................................................... 1246
Inputting and Outputting a Program............................ 1246
Inputting and Outputting Custom Macro Common
Variables ..................................................................... 1270
Inputting and Outputting Offset Data................. 1254,1311
Inputting and Outputting Operation History
Data.................................................................... 1277,1320
Inputting and Outputting Parameters.................. 1250,1308
Inputting and Outputting Pitch Error Compensation
Data............................................................................. 1261
Inputting and Outputting Three-dimensional Error
Compensation Data ..................................................... 1265
Inputting and Outputting Tool Management
Data.................................................................... 1279,1321
Inputting and Outputting Workpiece Coordinates
System Data ....................................................... 1274,1318
Inputting custom macro common variables.................1270
Inputting customize data displayed as tool management
data.............................................................................. 1291
Inputting decimal point position data of customize
data.............................................................................. 1297
Inputting magazine data ..............................................1282
Inputting name data of customize data........................1288
Inputting offset data ....................................................1254
Inputting parameters....................................................1250
Inputting pitch error compensation data......................1261
Inputting spindle waiting position name data..............1294
Inputting three-dimensional error compensation data .1265
Inputting tool geometry data .......................................1300
Inputting tool life status name data .............................1285
Inputting tool management data ..................................1279
Inputting workpiece coordinate system data ...............1274
Inputting/Outputting a Program ..................................1304
Inputting/Outputting Custom Macro Common
Variables .....................................................................1316
Inputting/Outputting Pitch Error Compensation Data . 1313
Inserting a Word..........................................................1354
INSERTING, ALTERING AND DELETING
A WORD..................................................................... 1350
Interference Check and Interference Avoidance ...........946
Internal circular cutting feedrate change .......................168
INTERPOLATION FUNCTIONS..................................50
INTERRUPTION TYPE CUSTOM MACRO ..............565
<J>
JERK CONTROL .........................................................671
JOG FEED (JOG)........................................................1032
<K>
Key Input and Input Buffer .........................................1023
KEYS AND PROGRAM ENCRYPTION ..................1386
<L>
Leading edge offset .......................................................921
Line Number Display..................................................1375
Line Search .................................................................1379
LINEAR INTERPOLATION (G01) ...............................56
LINEAR SCALE WITH DISTANCE-CODED
REFERENCE MARKS (SERIAL) .............................1087
List of Error Message.................................................. 2406
INDEX B-63944EN/03
i-6
LIST OF FUNCTIONS AND PROGRAM
FORMAT .................................................................... 2286
List of Functions of PC Tool.......................................2390
LOAD METER SCREEN........................................... 1894
LOCAL COORDINATE SYSTEM ..............................206
Local variables .............................................................. 595
Look-Ahead Smooth Bell-Shaped
Acceleration/Deceleration before Interpolation ............674
<M>
M Code Group Check Function ....................................313
M CODE GROUPING FUNCTION ............................. 309
MACHINE COORDINATE SYSTEM......................... 187
MACHINE LOCK AND AUXILIARY FUNCTION
LOCK.......................................................................... 1178
MACHINING CONDITION SELECTING
FUNCTION ..................................................................670
Machining Parameter Tuning...................................... 1741
Machining Parameter Tuning (15-inch Display Unit). 1820
MACRO CALL...................................................... 520,605
Macro Call Using a G Code ..........................................540
Macro Call Using a G Code (Specification of Multiple
Definitions) ...................................................................542
Macro Call Using a G Code with a Decimal Point
(Specification of Multiple Definitions) .........................543
Macro Call Using an M Code .......................................544
Macro Call Using an M Code (Specification of Multiple
Definitions) ...................................................................545
MACRO STATEMENTS AND NC STATEMENTS... 511
MAKING A PROGRAM COMPACT........................ 1411
MANUAL ABSOLUTE ON AND OFF ..................... 1040
MANUAL HANDLE FEED .......................................1036
MANUAL HANDLE INTERRUPTION ....................1127
MANUAL HANDLE RETRACE............................... 1093
MANUAL LINEAR/CIRCULAR
INTERPOLATION .....................................................1046
MANUAL NUMERICAL COMMAND..................... 1055
MANUAL OPERATION..................................... 982,1029
MANUAL REFERENCE POSITION RETURN........ 1030
Maximum incremental value check ............................ 1215
MAXIMUM STROKE....................................................38
MDI OPERATION ..................................................... 1114
MEMORY OPERATION ...........................................1111
METHOD OF REPLACING BATTERY ...................1967
Methods of Alarm Recovery by Synchronous Error
Check ............................................................................704
MIRROR IMAGE ....................................................... 1134
Modal Call: Each Block Call (G66.1) ..........................537
Modal Call: Call After the Move Command (G66).......532
Modal Real Time Macro Command / One-shot Real
Time Macro Command .................................................581
MUITI-PATH CONTROL FUNCTION.......................963
MULTIPLE M COMMANDS IN A SINGLE
BLOCK .........................................................................308
Multi-statement (ZDO...ZEND Statement) ...................602
MULTI-STEP SKIP (G31)............................................141
<N>
NAMES OF AXES .........................................................36
NAMING RULES.......................................................2401
Naming Rules Of Folder .............................................2402
Naming Rules of Program File....................................2401
NANO SMOOTHING ..................................................113
Next Block Display Screen .........................................1481
Next Block Display Screen (15-inch Display Unit) .... 1532
NOMOGRAPHS.........................................................2301
NORMAL DIRECTION CONTROL
(G40.1,G41.1,G42.1).....................................................391
Note........................................................... 1085,1948,2406
NOTES..........................................................................622
NOTES ON READING THIS MANUAL ........................8
NOTES ON VARIOUS KINDS OF DATA......................9
NUMBER OF CONTROLLED AXES...........................35
NURBS INTERPOLATION (G06.2)............................121
NURBS Interpolation Additional Functions .................127
<O>
Operating Monitor Display .........................................1444
Operating Monitor Display (15-inch Display Unit) ....1460
Operation confirmation function setting screen ..........1217
Operation history................................................ 1786,1865
Operation level setting ................................................1614
Operation level setting (15-inch display unit) ............. 1690
Operation Procedure for a Canned Cycle for Drilling.1159
OPERATIONAL DEVICES ................................ 998,1006
OPTIMUM TORQUE
ACCELERATION/DECELERATION .........................676
OTHERS .......................................................................607
Outputting a program ..................................................1248
B-63944EN/03 INDEX
i-7
Outputting all history data.................................. 1798,1877
Outputting custom macro common variables.............. 1272
Outputting customize data displayed as tool
management data......................................................... 1293
Outputting decimal point position data of customize
data.............................................................................. 1299
Outputting magazine data............................................1284
Outputting name data of customize data .....................1290
Outputting offset data.................................................. 1256
Outputting operation history data................................1277
Outputting parameters................................................. 1252
Outputting pitch error compensation data ................... 1263
Outputting spindle waiting position name data ........... 1296
Outputting three-dimensional error compensation
data.............................................................................. 1267
Outputting tool geometry data..................................... 1302
Outputting tool life status name data...........................1287
Outputting tool management data ...............................1281
Outputting workpiece coordinate system data ............ 1276
Overall Position Display .............................................1436
Overall Position Display (15-inch Display Unit) ........ 1451
OVERTRAVEL .......................................................... 1192
Overview of the History Function............................... 1779
Overview of the History Function
(15-inch Display Unit) ................................................ 1858
OVERWRITING FILES ON A MEMORY CARD.... 1241
<P>
Parameter Tuning Screen ............................................ 1751
Parameter Tuning Screen (15-inch Display Unit) .......1830
Parameter tuning screen (axis setting)......................... 1757
Parameter tuning screen (axis setting)
(15-inch Display Unit) ................................................ 1836
Parameter tuning screen (miscellaneous settings) ....... 1761
Parameter tuning screen (miscellaneous settings)
(15-inch Display Unit) ................................................ 1841
Parameter tuning screen (spindle setting).................... 1760
Parameter tuning screen (spindle setting)
(15-inch Display Unit) ................................................ 1840
Parameter tuning screen (system setting) ....................1755
Parameter tuning screen (system setting)
(15-inch Display Unit) ................................................ 1834
PARAMETERS ..........................................................1983
PART DRAWING AND TOOL MOVEMENT .............17
Part Program Storage Size / Number of Registerable
Programs .......................................................................330
Parts Count Display, Run Time Display .......................996
PASSWORD FUNCTION ..........................................1367
Password modification ................................................1616
Password modification (15-inch display unit)............. 1692
Paste ............................................................................1378
Path Drawing............................................................... 1914
PATH GRAPHIC (TOOL POSITION) screen............1930
PATH GRAPHIC screen.............................................1922
PATTERN DATA INPUT ............................................629
PC TOOL FOR MEMORY CARD PROGRAM
OPERATION/EDITING .................................... 2389,2390
Periodic Maintenance Screen ......................................1768
Periodic Maintenance Screen (15-inch Display Unit) .1847
PLANE SELECTION ...................................................208
POLAR COORDINATE INTERPOLATION (G12.1,
G13.1) .............................................................................76
POLYGON TURNING (G50.2, G51.2)........................709
Position Display in the Relative Coordinate System...1433
Position Display in the Workpiece Coordinate
System......................................................................... 1431
POSITIONING (G00) .....................................................51
Power Disconnection...................................................1028
POWER ON/OFF........................................................1027
Precision Level Selection ............................................ 1623
Precision Level Selection (15-inch Display Unit) ....... 1699
PREPARATORY FUNCTION (G FUNCTION)...........39
Procedure for Reference Position Establishment ........1080
PROCESSING MACRO STATEMENTS ....................555
Program Check Screen ................................................ 1482
Program Check Screen (15-inch Display Unit)...........1533
PROGRAM CODE LIST............................................2283
PROGRAM COMPONENTS OTHER THAN
PROGRAM SECTIONS ...............................................333
PROGRAM CONFIGURATION............................. 30,331
Program Contents Display...........................................1467
Program Contents Display (15-inch Display Unit) .....1521
PROGRAM COPY FUNCTION........................ 1380,1412
Program Display............................................................994
Program Folder Screen................................................1473
Program Folder Screen (15-inch Display Unit)........... 1525
PROGRAM MANAGEMENT............................. 317,1395
PROGRAM RESTART ..............................................1136
INDEX B-63944EN/03
i-8
Program Screen for MDI Operation............................ 1472
Program Screen for MDI Operation
(15-inch Display Unit) ................................................ 1524
PROGRAM SEARCH ................................................ 1359
PROGRAM SECTION CONFIGURATION................ 336
Programmable Data Input (G10) for Blank Figure
Drawing Parameters ....................................................1946
PROGRAMMABLE MIRROR IMAGE
(G50.1, G51.1) ..............................................................389
PROGRAMMABLE PARAMETER INPUT (G10) ..... 626
Prohibition of the absolute input by the soft key......... 1206
Protection level setting................................................ 1618
Protection level setting (15-inch display unit)............. 1694
Protection of Data at Eight Levels .............................. 1614
Protection of Data at Eight Levels
(15-inch Display Unit) ................................................ 1690
Protection of Various Tool Information Items with
the KEY Signal ............................................................. 275
<R>
RADIUS DIRECTION ERROR AT CIRCLE
CUTTING ................................................................... 2309
RANGE OF COMMAND VALUE ............................ 2298
RAPID TRAVERSE .....................................................157
RAPID TRAVERSE OVERRIDE .............................. 1181
Real time macro variables (RTM variables) ................592
REAL-TIME CUSTOM MACRO ................................ 577
REFERENCE POSITION............................................. 176
Reference Position (Machine-specific Position) .............17
Reference Position Return................................... 177, 1082
REGISTERING CUSTOM MACRO PROGRAMS .....557
Registering, Changing, and Deleting Tool Life
Management Data .........................................................284
Related Parameters........................................................ 329
RELATION WITH CONVENTIONAL FUNCTIONS 326
Relation with File Names..............................................328
Relation with Folders .................................................... 326
Relationship with Other Functions.............................. 1237
RENAMING A FILE .................................................. 1407
RENAMING A FOLDER ........................................... 1403
Repetition (WHILE Statement)..................................... 517
Repetition (ZWHILE Statement) .................................. 601
Replacement................................................................ 1376
Replacing Battery for LCD-mounted Type CNC
Control Unit ................................................................ 1968
Replacing the Battery for Stand-alone Type CNC
Control Unit ................................................................1971
Repositioning ..............................................................1155
Restriction on machine configurations having table
rotation axes (table rotation type and composite type)..954
Restriction on tool rotation type....................................953
Restrictions........................................................... 950,1949
RESTRICTIONS...........................................................563
Restrictions common to machine configurations ..........950
RETRACE ..................................................................1161
Retract .........................................................................1153
Retract function.............................................................770
Return.......................................................................... 1154
Return from the Alarm Screen ....................................1235
Reversing Edit Operations (Undo Function) ...............1377
RIGID TAPPING BY MANUAL HANDLE..............1052
Rotary Axis Control ......................................................720
Rotary Axis Roll-over ...................................................719
ROUTINE MAINTENANCE .....................................1963
RULES OF CHARACTERS IN PROGRAM FILE....2403
<S>
SAFETY FUNCTIONS ..............................................1190
SAFETY PRECAUTIONS ............................................s-1
Sample programs...........................................................762
Saving..........................................................................1378
SCALING (G50, G51) ..................................................379
SCHEDULE OPERATION.........................................1121
SCREEN ERASURE FUNCTION AND
AUTOMATIC SCREEN ERASURE FUNCTION.....1892
Screen for Assistance in Entering Tilted Working
Plane Command ..........................................................1499
Screen for Assistance in Entering Tilted Working
Plane Command (15-inch Display Unit) .....................1550
SCREEN HARD COPY FUNCTION......................... 1339
Screens Displayed By Function Key ...............1429
Screens Displayed By Function Key ...............1466
Screens Displayed By Function Key ...............1571
Screens Displayed By Function Key ...............1721
Screens Displayed By Function Key ...............1881
Search..........................................................................1375
SECOND AUXILIARY FUNCTIONS (B CODES).....314
B-63944EN/03 INDEX
i-9
SELECTING A DEFAULT FOLDER........................ 1406
SELECTING A DEVICE............................................ 1396
SELECTING A MAIN PROGRAM ........................... 1410
Selecting a Memory Card Program as a Device.......... 1397
Selecting a Workpiece Coordinate System ...................193
Selecting operation history signals..................... 1796,1875
Selection of a Tool Life Count Period...........................275
SELECTION OF TOOL USED FOR VARIOUS
MACHINING - TOOL FUNCTION............................... 28
Sequence Number Comparison and Stop .................... 1576
Sequence Number Comparison and Stop
(15-inch Display Unit) ................................................ 1648
SEQUENCE NUMBER SEARCH ............................. 1361
Servo Parameters.........................................................1733
Servo Parameters (15-inch Display Unit).................... 1812
Servo Tuning............................................................... 1734
Servo Tuning (15-inch Display Unit).......................... 1813
Setting a Workpiece Coordinate System....................... 190
Setting an M Code Group Number Using a Program.... 312
Setting an M Code Group Number Using the Setting
Screen............................................................................309
SETTING AND DISPLAY UNITS .............................. 999
SETTING AND DISPLAYING DATA...................... 1414
Setting and Displaying Tool Management Data.......... 1591
Setting and Displaying Tool Management Data
(15-inch Display Unit) ................................................ 1665
Setting of Spindle Position / Standby Position Display 270
Setting Screen .............................................................1216
Setting the change protection level and output
protection level of a program ......................................1621
Setting the change protection level and output
protection level of a program (15-inch display unit)... 1697
Setting the Character-codes........................................... 645
Setting the Floating Reference Position ...................... 1443
Setting the Floating Reference Position
(15-inch Display Unit) ................................................ 1459
SETTINGS AT POWER-ON, IN THE CLEAR
STATE, OR IN THE RESET STATE ........................ 2310
SIMPLE CALCULATION OF INCORRECT THREAD
LENGTH..................................................................... 2304
Simple Call (G65) .........................................................521
SIMULTANEOUS EDITING OF MULTIPATH
PROGRAMS............................................................... 1391
SINGLE BLOCK ........................................................ 1185
SINGLE DIRECTION POSITIONING (G60)................53
Single-Path Display..................................................... 1894
SKIP FUNCTION (G31)...............................................139
Skip Function for EGB Axis .........................................751
Small MDI Unit (ONG Key).......................................1005
SMOOTH INTERPOLATION (G05.1) ........................109
Soft Keys.....................................................................1013
Specification Method ....................................................566
Specification method (G80.5, G81.5)............................753
SPECIFYING THE SPINDLE SPEED VALUE
DIRECTLY (S5-DIGIT COMMAND) .........................224
SPECIFYING THE SPINDLE SPEED WITH
A CODE........................................................................224
Speed Control with Change of Acceleration on Each
Axis ...............................................................................671
SPINDLE CONTROL BETWEEN EACH PATH........974
Spindle Control with Servo Motor ................................241
Spindle Indexing Function ............................................242
Spindle Monitor ..........................................................1737
Spindle Monitor (15-inch Display Unit) .....................1816
Spindle Orientation .......................................................231
Spindle Positioning .......................................................232
SPINDLE POSITIONING FUNCTION .......................230
Spindle Setting ............................................................1735
Spindle Setting (15-inch Display Unit) .......................1814
SPINDLE SPEED FLUCTUATION DETECTION .....236
SPINDLE SPEED FUNCTION (S FUNCTION)..........223
Spindle Tuning ............................................................1736
Spindle Tuning (15-inch Display Unit).......................1815
SPIRAL INTERPOLATION, CONICAL
INTERPOLATION (G02, G03)......................................68
Split display on the program folder screen......... 1474,1526
Stamping the Machining Time....................................1489
Stamping the Machining Time
(15-inch Display Unit) ................................................1540
Standard MDI Unit (ONG Key) ..................................1003
Standard MDI Unit (QWERTY Key)..........................1004
STANDARD PARAMETER SETTING TABLES.....2281
Start check signal ........................................................1211
STORED STROKE CHECK ......................................1193
STROKE LIMIT CHECK BEFORE MOVE ..............1198
SUBPROGRAM (M98, M99).......................................344
Subprogram Call Using a Specific Address ..................551
Subprogram Call Using an M Code ..............................546
INDEX B-63944EN/03
i-10
Subprogram Call Using an M Code (Specification of
Multiple Definitions).....................................................547
Subprogram Calls Using a Secondary Auxiliary
Function ........................................................................550
Subprogram Calls Using a T Code................................548
Subprogram Calls Using an S Code ..............................549
Synchronization ratio specification range ..................... 766
Synchronous Error Check .............................................702
Synchronous Error Compensation.................................696
Synchronous Establishment .......................................... 698
SYNCHRONOUS, COMPOSITE AND
SUPERIMPOSED CONTROL BY PROGRAM
COMMAND (G50.4, G51.4, G50.5, G51.5, G50.6,
AND G51.6).................................................................. 715
SYNCHRONOUS/COMPOSITE/SUPERIMPOSED
CONTROL....................................................................975
System Configuration Screen...................................... 1776
System Configuration Screen (15-inch Display Unit). 1855
System variables .................................................... 589,594
SYSTEM VARIABLES................................................ 445
<T>
Table Horizontal Direction Handle Feed / Table
Horizontal Direction JOG Feed / Table Horizontal
Direction Incremental Feed......................................... 1076
Table Vertical Direction Handle Feed / Table Vertical
Direction JOG Feed / Table Vertical Direction
Incremental Feed......................................................... 1074
TANDEM CONTROL.................................................. 771
TEST OPERATION....................................................1177
TESTING A PROGRAM..............................................988
THREE-DIMENSIONAL CIRCULAR
INTERPOLATION .......................................................149
THREE-DIMENSIONAL COORDINATE SYSTEM
CONVERSION ............................................................. 359
THREE-DIMENSIONAL MANUAL FEED.............. 1064
Tilted Working Plane Command...................................838
Tilted working plane command based on projection
angles ............................................................................882
Tilted working plane command based on
roll-pitch-yaw................................................................ 871
Tilted working plane command based on three points .. 875
Tilted working plane command based on two vectors ..879
Tilted Working Plane Command by Tool Axis
Direction .......................................................................862
Tilted Working Plane command with Guidance ...........870
Tilted working plane data setting screen ............ 1507,1558
Tool Axis Direction Handle Feed / Tool Axis Direction
JOG Feed / Tool Axis Direction Incremental Feed ..... 1065
Tool Axis Right-Angle Direction Handle Feed / Tool
Axis Right-Angle Direction JOG Feed / Tool Axis
Right-Angle Direction Incremental Feed ....................1067
TOOL CENTER POINT CONTROL ...........................773
TOOL FUNCTION (T FUNCTION) ............................244
Tool geometry data screen ..........................................1607
Tool geometry data screen (15-inch display unit) .......1683
TOOL LENGTH COMPENSATION
(G43, G44, G49) ...........................................................371
Tool Life Count Restart M Code...................................303
Tool Life Counting and Tool Selection.........................299
TOOL LIFE MANAGEMENT .....................................279
Tool life management (group editing screen)..............1632
Tool life management (group editing screen)
(15-inch display unit) ..................................................1708
Tool life management (list screen)..............................1627
Tool life management (list screen)
(15-inch display unit) ..................................................1703
Tool Life Management Commands in Machining
Program.........................................................................290
Tool Life Management Data .........................................281
TOOL MANAGEMENT EXTENSION FUNCTION ..265
TOOL MANAGEMENT FUNCTION..........................247
TOOL MANAGEMENT FUNCTION FOR OVERSIZE
TOOLS..........................................................................277
TOOL MOVEMENT ALONG WORKPIECE PARTS
FIGURE-INTERPOLATION..........................................14
TOOL MOVEMENT BY PROGRAMING -
AUTOMATIC OPERATION .......................................984
TOOL MOVEMENT RANGE - STROKE.....................33
Tool offset range setting screen...................................1219
TOOL PATH AT CORNER .......................................2306
TOOL POSTURE CONTROL......................................828
TOOL RETRACT AND RECOVER ...................732,1149
Tool Retract and Recover for Threading.....................1156
TOOL SELECTION FUNCTION.................................245
Tool side offset..............................................................901
Tool Tip Center Rotation Handle Feed / Tool Tip
Center Rotation JOG Feed / Tool Tip Center Rotation
Incremental Feed......................................................... 1071
B-63944EN/03 INDEX
i-11
Tool tip position (cutting point) command.................... 927
TORQUE LIMIT SKIP.................................................145
Total Life Time Display for Tools of The Same Type.. 276
Turning on the Power.................................................. 1027
Two-Path Display and Three-Path Display................. 1896
TYPES OF REAL TIME MACRO COMMANDS....... 581
<U>
Unconditional Branch (GOTO Statement).................... 512
Usable Characters in Program File.............................. 2404
Usage Notes ................................................................2390
<V>
VARIABLE LEAD THREADING (G34).....................133
VARIABLES ......................................................... 438,588
Variables Dedicated To Real Time Custom Macros .....589
VIRTUAL MDI KEY .................................................1957
VIRTUAL MDI KEY FUNCTION ............................ 1956
<W>
WAITING FUNCTION FOR PATHS ..........................966
Warning Messages ............................................. 1024,1948
WARNINGS AND CAUTIONS RELATED TO
HANDLING................................................................... s-9
WARNINGS AND CAUTIONS RELATED TO
PROGRAMMING ......................................................... s-6
WARNINGS RELATED TO DAILY
MAINTENANCE ........................................................ s-12
Withdrawal.................................................................. 1154
Word Search................................................................1351
WORKPIECE COORDINATE SYSTEM ....................190
Workpiece Coordinate System Preset .........................1438
Workpiece Coordinate System Preset
(15-inch Display Unit) ................................................ 1454
Workpiece Coordinate System Preset (G92.1)..............198
Workpiece Coordinate System Shift .............................204
Workpiece origin offset range setting screen .............. 1224
WORKPIECE SETTING ERROR
COMPENSATION........................................................397
Workpiece shift range setting screen........................... 1228
WRONG OPERATION PREVENTION
FUNCTIONS .............................................................. 1201
<
Ｙ
>
Y-axis tool offset range setting screen ........................ 1226
Revision Record
FANUC Series 30i/300i/300is-MODEL A, Series 31i/310i/310is-MODEL A, Series 32i/320i/320is-MODEL A
USER’S MANUAL (Common to Lathe System/Machining Center System )(B-63944EN)
03
Dec., 2007 Total revision
02
Jun, 2004
Addition of functions
Addition of following models
- Series 31i /310i /310is-MODEL A5
- Series 31i /310i /310is-MODEL A
- Series 32i /320i /320is-MODEL A
01
Jul., 2003
Edition Date Contents Edition Date Contents
