Eding CNC Manual Edingcnc V4.03

User Manual:

Open the PDF directly: View PDF .
Page Count: 214

Download
Open PDF In Browser	View PDF

EDING CNC

Manual

User Manual Eding CNC Software

Document Release 4.03

09 November 2018

Release 4.03

EDING CNC

Manual

Title:
Author:
Date:

Eding CNC user Manual Software
Bert Eding
Friday, 09 November 2018

Document History
Version
1
4.03.01

Date
2006-03-10
12-06-2017

Author
Bert Eding
Bert Eding

4.03.04

07-07-2017

Bert Eding

4.03.12

12-11-2017

Bert Eding

4.03.18

12-03-2018

Bert Eding

4.03.20

26-04-2018

Bert Eding

4.03.25

20-8-2018

Alfred Bos

4.03.26

24-08-2018

Bert Eding

4.03.26
4.03.31

08-09-2018
8-11-2018

Bert Eding
Bert Eding

09 November 2018

Comment
Initial version
Updated for V4.03
Start with new history for V4.03
Added description of new Trajectory
generator function, corner dependent
velocity control.
Updated the specification of G68.
Allow rotation in every plane.
Updated missing description of ctrlF9/F10 in auto menu and added
description of SafeFeed.
Added chapter 3.7.11 M Functions for
Laser mode (CNC7.. series CPU’s)
Updated description on Coordinates
page.
Added description for new addition
with GOTO, the Search TOOL function.
Show stock in graphics for turning.
Added usage of QR scanner for
loading a G-Code file.
Automatic vacuum bed with sections.
Enhanced Msg, logMsg, WarnMsg,
ErrMsg, so it can include the tool
description text from the tool table.
Added new interpreter command
called ZHCINITEX
with
separate grid sizes for X and Y
Added interpreter command
getToolInfo
Added new interpreter command
‘GetJobDistance’
Added new interpreter command:
‘GetHeightControlVact’ &
‘GetHeightControlVset’ &
‘Service ’
Added automatic oil pump function,
see service page.
Update description of Y->A mapping.
Added tanknive V-Groove example.
Added oil Pump function.
Added automatic vacuum sections
function.

Release 4.03

EDING CNC

Manual

© Copyright Eding CNC Holding B.V.
All rights reserved. Reproduction in whole or in part prohibited without the prior written
consent of the copyright owner.

09 November 2018

Release 4.03

EDING CNC

Manual

ACKNOWLEDGEMENTS
The G-Code part of this user manual has been derived from the full
report of the RS274/NGC language. Parts that are less relevant to Eding
CNC users or parts that are not supported are left out.

09 November 2018

Release 4.03

EDING CNC

Manual

Table of contents
Table of contents .................................................................................................................................. 5
1

Introduction ................................................................................................................................... 10

1.1

Context and scope ....................................................................................................... 11

1.2

Definitions, acronyms and abbreviations ...................................................................... 12

1.3

Minimum PC requirements ........................................................................................... 13

1.4

Installation of EDINGCNC ............................................................................................. 14

1.4.1
1.4.2
1.4.3
1.4.4
1.4.5
1.4.6
2

USB ............................................................................................................................................... 14
Ethernet ....................................................................................................................................... 16
Set admin mode and switch off UAC ........................................................................................... 20
Disable automatic update in Windows 10 ................................................................................... 22
Connected drives not visible Windows 10 ................................................................................... 24
Profiles, If you have different setups e.g. lathe and milling......................................................... 25

The user interface ....................................................................................................................... 27
2.1.1
Setup Pages .................................................................................................................................. 31
2.1.2
UI and Connection ....................................................................................................................... 31
2.1.3
Motor setup ................................................................................................................................. 32
2.1.4
Homing and ESTOP setup ............................................................................................................ 34
2.1.5
Backlash setup ............................................................................................................................. 35
2.1.6
LAF setup...................................................................................................................................... 36
2.1.7
Kinematic Setup ........................................................................................................................... 39
2.1.8
Tool change Area setup ............................................................................................................... 39
2.1.9
Tangential knife setup.................................................................................................................. 39
2.1.10 Safety/Door open Input setup ..................................................................................................... 43
2.1.11 Spindle and PWM setup ............................................................................................................... 43
2.1.12 UI setup items .............................................................................................................................. 46
2.1.13 IO setup ........................................................................................................................................ 47
2.1.14 Interpreter settings ...................................................................................................................... 48
2.1.15 Traffic light setup ......................................................................................................................... 48
2.1.16 JobTimeEstimation ....................................................................................................................... 49
2.1.17 Hand wheel Setup ........................................................................................................................ 49
2.1.18 Load/Run Automatically .............................................................................................................. 50
2.1.19 Probing Setup............................................................................................................................... 52
2.1.20 Camera Setup ............................................................................................................................... 53
2.1.21 CPUOPT ........................................................................................................................................ 54
2.1.22 Using a safety relay ...................................................................................................................... 55
2.1.22.1
Powering the safety relay .................................................................................................... 55
2.1.22.2
Input contacts of the safety relay ........................................................................................ 55
2.1.22.3
Output contacts of the safety relais..................................................................................... 56
2.1.22.4
Switching on the safety relay ............................................................................................... 56
2.1.23 Operate Page, this is where the machine is operated ................................................................. 58
2.1.24 Operate page introduction .......................................................................................................... 58
2.1.25 Reset Button F1............................................................................................................................ 60
2.1.26 Escape Button .............................................................................................................................. 60
2.1.27 The menus ................................................................................................................................... 60
2.1.27.1
Main Menu........................................................................................................................... 60
2.1.27.2
Home menu ......................................................................................................................... 60
2.1.27.3
Zero menu ............................................................................................................................ 61
09 November 2018

Release 4.03

EDING CNC

Manual

2.1.27.4
Auto menu ........................................................................................................................... 61
2.1.27.5
IO menu ............................................................................................................................... 67
2.1.27.6
Graphic menu....................................................................................................................... 67
2.1.27.7
Jog menu .............................................................................................................................. 68
2.1.27.8
Jog pad ................................................................................................................................. 68
2.1.27.9
User menu ............................................................................................................................ 69
2.1.28 Operate page tasks ...................................................................................................................... 70
2.1.28.1
Startup ................................................................................................................................. 70
2.1.28.2
Homing ................................................................................................................................. 70
2.1.28.3
Load and run a g-code file .................................................................................................... 70
2.1.29 Coordinate Page Tasks ................................................................................................................. 75
2.1.29.1
Calibrate/Activate coordinate systems ................................................................................ 75
2.1.29.2
Mapping X/Y G-code to cylinder on A-Axis .......................................................................... 76
2.1.29.3
Milling un-even surfaces ...................................................................................................... 78

2.2

Linear PITCH compensation .......................................................................................... 83

2.3

XY Non rectangular Cross compensation....................................................................... 84

2.4

Speed-PWM compensation .......................................................................................... 85

2.5

Automatic vacuum sections.......................................................................................... 87

2.6

Program Page, DXF and HPGL import ........................................................................... 88

2.7

Tools Page ................................................................................................................... 91

2.7.1
2.7.2
2.7.3
2.7.4
2.7.5
2.7.6

Milling .......................................................................................................................................... 91
Turning ......................................................................................................................................... 92
Tool change .................................................................................................................................. 92
Automatic user defined Tool change ATC .................................................................................... 92
Changing the tool number without actual tool change ............................................................... 93
The variable Page ......................................................................................................................... 93

2.8

IO Page ....................................................................................................................... 95

2.9

Service Page ................................................................................................................ 96

2.10

Util Page, Chipload and Feed/Speed ......................................................................... 98

2.11

homing and coordinate systems................................................................................ 99

2.11.1
2.11.2
2.11.3
2.11.4

Manual homing the machine ..................................................................................................... 100
Automatic homing the machine and HomeIsEstop ................................................................... 101
Tandem axes homing ................................................................................................................. 102
Work versus Machine coordinate system and zeroing .............................................................. 104

2.12

3D Printing ............................................................................................................. 105

2.13

Keyboard shortcuts................................................................................................. 108

2.14

Zero tool macro ...................................................................................................... 110

2.15

Tool measurement Macro ....................................................................................... 111

Input: the RS274/NGC Language ......................................................................................................... 115

3.1
3.2

System-Parameters/Variables .................................................................................... 116
Tool data ................................................................................................................... 120
3.2.1.1

Tool Orientation for lathes .................................................................................................... 120

3.3

Coordinate Systems ................................................................................................... 121

3.4

Format of a Line......................................................................................................... 122

3.4.1

Line Number .............................................................................................................................. 122

09 November 2018

Release 4.03

EDING CNC

Manual

3.4.2
Word .......................................................................................................................................... 122
3.4.2.1 Number .................................................................................................................................. 123
3.4.2.2 Parameter Value .................................................................................................................... 123
3.4.2.3 Expressions and Binary Operations........................................................................................ 124
3.4.2.4 Unary Operation Value .......................................................................................................... 124
3.4.3
Parameter Setting ...................................................................................................................... 125
3.4.4
Comments and Messages .......................................................................................................... 125
3.4.5
Item Repeats .............................................................................................................................. 125
3.4.6
Item order .................................................................................................................................. 126
3.4.7
Commands and Machine Modes ............................................................................................... 126

3.5

Modal Groups ............................................................................................................ 127

3.6

G Codes ..................................................................................................................... 129

3.6.1
Rapid Linear Motion - G0 ........................................................................................................... 129
3.6.2
Linear Motion at Feed Rate - G1 ................................................................................................ 131
3.6.3
Arc at Feed Rate - G2 and G3 ..................................................................................................... 132
3.6.3.1 Radius Format Arc .................................................................................................................. 132
3.6.3.2 Center Format Arc .................................................................................................................. 133
3.6.4
Dwell - G4 ................................................................................................................................... 134
3.6.5
Set Coordinate System Data -G10.............................................................................................. 134
3.6.6
Plane Selection - G17, G18, and G19 ......................................................................................... 134
3.6.7
Length Units - G20/G21 and G70/G71 ....................................................................................... 134
3.6.8
Return to Home - G28 and G30 ................................................................................................. 135
3.6.9
G33, G33.1 Spindle-Synchronized Motion ................................................................................. 136
3.6.10 Straight Probe - G38.2................................................................................................................ 137
3.6.10.1
The Straight Probe Command ............................................................................................ 137
3.6.10.2
Using the Straight Probe Command................................................................................... 137
3.6.10.3
Example Code .................................................................................................................... 138
3.6.11 Cutter Radius Compensation - G40, G41, G41.1, G42, G42.1 .................................................... 139
3.6.11.1
Example code for milling .................................................................................................... 140
3.6.11.2
Example code for turning ................................................................................................... 141
3.6.12 Tool Length Offsets - G43, G43 H, G43.1, and G49 ................................................................... 143
3.6.13 Scaling G50/G51......................................................................................................................... 143
3.6.14 Move in Absolute Coordinates - G53 ......................................................................................... 144
3.6.15 Select Coordinate System - G54 to G59.3 .................................................................................. 144
3.6.16 Path Control Mode and Look ahead feed- G61, and G64 .......................................................... 145
3.6.17 Coordinate system rotation G68................................................................................................ 151
3.6.18 Threading (Lathe) – G76 ............................................................................................................ 151
3.6.19 Cancel Modal Motion - G80 ....................................................................................................... 154
3.6.20 Canned Cycles - G81 to G89 ....................................................................................................... 154
3.6.20.1
Preliminary and In-Between Motion.................................................................................. 155
3.6.20.2
G81 Cycle ........................................................................................................................... 156
3.6.20.3
G82 Cycle ........................................................................................................................... 157
3.6.20.4
G83 Cycle ........................................................................................................................... 157
3.6.20.5
G73 Cycle ........................................................................................................................... 157
3.6.20.6
G84 Cycle ........................................................................................................................... 158
3.6.20.7
G74 Cycle ........................................................................................................................... 158
3.6.20.8
G85 Cycle ........................................................................................................................... 158
3.6.20.9
G86 Cycle ........................................................................................................................... 158
3.6.20.10 G87 Cycle ........................................................................................................................... 159
3.6.20.11 G88 Cycle ........................................................................................................................... 160
3.6.20.12 G89 Cycle ........................................................................................................................... 160
3.6.21 Set Distance Mode - G90 and G91 ............................................................................................. 160
3.6.22 Coordinate System Offsets - G92, G92.1, G92.2, G92.3............................................................. 161
3.6.23 Set Feed Rate Mode - G93, G94, G95 ........................................................................................ 162
3.6.24 Spindle Control Mode – G96, G97 ............................................................................................. 162

09 November 2018

Release 4.03

EDING CNC

Manual

3.6.25

3.7

Input M Codes ........................................................................................................... 163

3.7.1
3.7.2
3.7.3
3.7.4
3.7.5
3.7.6
3.7.7
3.7.8
3.7.9
3.7.10
3.7.11
3.7.12
3.7.13

3.8

Set Feed Rate - F ........................................................................................................................ 174
Set Spindle Speed - S .................................................................................................................. 174
Select Tool - T ............................................................................................................................. 174

Order of Execution ..................................................................................................... 175

Language extensions .............................................................................................................. 176

4.1

Flow control .............................................................................................................. 177

4.2

supported operations on expressions.......................................................................... 178

4.2.1
4.2.2
4.2.3

4.3

4.4

unary operations ........................................................................................................................ 178
binary operations: ...................................................................................................................... 178
An example: ............................................................................................................................... 179

Special interpreter commands, non G-Code ................................................................ 180

4.3.1
4.3.2
4.3.3
4.3.4
4.3.5
4.3.6
4.3.7
4.3.8
4.3.9
4.3.10
4.3.11
4.3.12
4.3.13
4.3.14
4.3.15
4.3.16
4.3.17
4.3.18
4.3.19
4.3.20

Msg ................................................................................................................. 180
ErrMsg ............................................................................................................. 180
WarnMsg ........................................................................................................ 180
LogFile, LogMsg ............................................................................................... 180
GetToolInfo ............................................................................. 180
DlgMsg ....................................................................................................................................... 182
Store position ............................................................................................................................. 184
TCAGuard [on | off] ................................................................................................................... 184
MCAGuard [on | off] .................................................................................................................. 184
HomeIsEstop [on | off] .............................................................................................................. 184
Exec <”parameter”> ..................................................... 184
SetAcc ............................................................................... 185
Vacuum [on | off] ...................................................................................................................... 185
GetJobDistance ............................................................................................................ 185
GetHeightControlVact .................................................................................................. 185
GetHeightControlVset .................................................................................................. 186
Service ............................................................................................................................ 186
Tool change example ................................................................................................................. 187
Changing the tool number without actual tool change ............................................................. 192
USER Reset ................................................................................................................................. 192

Run behavior during simulation and render ................................................................ 193

4.4.1
4.4.2
5

Program Stopping and Ending - M0, M1, M2, M30, M60 .......................................................... 164
Spindle/Head Control - M3, M4, M5, M90-M97........................................................................ 164
Tool Change - M6 ....................................................................................................................... 166
Coolant Control - M7, M8, M9 ................................................................................................... 167
Feed-Speed Override Control - M48-M53 ................................................................................. 168
Adaptive FeedOverride Control by spindle power..................................................................... 168
Standard CNC IO - M3..M9, M80..M87 ...................................................................................... 169
General purpose IO M54, M55, M56, M57 ................................................................................ 169
A axis clamping M26, M27 ......................................................................................................... 172
Torch height control M20, M21, M22........................................................................................ 172
M Functions for Lasermode (CNC7.. series CPU’s)..................................................................... 172
M Functions for 3D printing ....................................................................................................... 172
M Function override and user m-functions ............................................................................... 173

Other Input Codes ...................................................................................................... 174

3.8.1
3.8.2
3.8.3

3.9

Set Canned Cycle Return Level - G98 and G99........................................................................... 162

Example a check with error that we want to see always ........................................................... 193
Example a check with error showing only when running .......................................................... 193

Cutter Radius Compensation............................................................................................................... 194
09 November 2018

Release 4.03

EDING CNC

5.1

Manual

Introduction .............................................................................................................. 195

5.1.1

5.2

Data for Cutter Radius Compensation ....................................................................................... 196

Programming Instructions.......................................................................................... 197

5.2.1
Turning Cutter Radius Compensation On .................................................................................. 197
5.2.2
Turning Cutter Radius Compensation Off .................................................................................. 197
5.2.3
Sequencing ................................................................................................................................. 197
5.2.4
Use of D Number ....................................................................................................................... 197
5.2.5
Material Edge Contour ............................................................................................................... 197
5.2.6
Programming Entry Moves ........................................................................................................ 198
A.1.1.1 General Method ..................................................................................................................... 198
A.1.1.2 Simple Method....................................................................................................................... 200

5.3

Nominal Path Contour ............................................................................................... 202

5.4

Programming Errors and Limitations .......................................................................... 205

5.5

Extension IO board..................................................................................................... 208

5.6

Hardware installation tips.......................................................................................... 211

5.7

References ................................................................................................................. 214

09 November 2018

Release 4.03

EDING CNC

Manual

1 Introduction
This manual describes the usage of the CNC control system. Most hardware details can
be found in the hardware documentation on the Eding CNC download page.

09 November 2018

Release 4.03

EDING CNC

1.1

Manual

CONTEXT AND SCOPE

This section describes the context, hardware and software of a EDINGCNC controlled
Machine.

1. Operator
2. PC connected via USB or Ethernet to electronic cabinet which contains the EDINGCNC
CPU.
The PC runs the EDINGCNC Control Software.
3. Electronics cabinet, with power supplies, drives and Eding CNC CPU inside.
4. EDINGCNC CPU
5. CNC Machine
The connection from CPU to the PC is USB or Ethernet depending on the CPU model.
The CPU delivers STEP/Direction signals to the power stage of each motor (drive), the
motor connections of the drive go to the motors inside the machine.
Other connections like home-sensor/switches go directly from CPU to the machine.
For detailed info on all IO signals see the info in the technical flyers of the CPU, available
on the download page.
The Scope of the EDINGCNC product is the EDINGCNC software on the PC and the
EDINGCNC CPU.

09 November 2018

Release 4.03

EDING CNC

1.2

Manual

DEFINITIONS, ACRONYMS AND ABBREVIATIONS

CNC

Computerized Numerical Control

CPU

Central Processor Unit, a PCB board with a Processor on it.

DXF

Drawing Exchange Format) is a CAD data file format developed by
Autodesk

FIFO

First In First Out Buffer

HPGL

Hewlet Packard Graphical Language

GUI/UI

Graphical User Interface

INTERPRETER

A software function that is able to read a text file and execute the
commands contained therein.

JOBFILE

A job is the text file (G code) that will be executed by the interpreter.

GUI

Graphical User Interface.

PWM

Pulse Width Modulation

G-Code

CNC specific language to control the movements and IO of a milling
machine.
Look Ahead Feed, advanced motion algorithm that ensures minimal
machining time.

LAF

09 November 2018

Release 4.03

EDING CNC

1.3
•
•
•
•
•
•
•
•

Manual

MINIMUM PC REQUIREMENTS
1.4 GHz Atom.
Pentium, duo-core recommended for Ethernet.
1024 MB RAM for XP, 4G for Windows 7/8.
Windows 7/8/10, 32 or 64 bit.
Minimum Screen resolution 1024 x 768.
Graphic card with Open GL support is preferred.
USB-2 connection / Ethernet connection for Ethernet CPU's
Intel 100Mbit Ethernet card for Ethernet CPU's.

Windows XP my also work, but is no longer active supported.
Windows Vista is not supported at all

09 November 2018

Release 4.03

EDING CNC

1.4

Manual

INSTALLATION OF EDINGCNC

Download the installation executable from the website download page. Click on it to
install the software. Follow the screens. On Windows 7/8/10, click with the right mouse
button, choose start as administrator.
For setup of the hardware, check the hardware technical flyers for your CPU type. They
are on the download page of the website.

1.4.1

USB

During installation be sure to check "Install USB drivers":

After installation reboot the PC, when it is rebooted connect the CPU, after 10 – 60
seconds, you will see that windows has found an EDINGCNC COM port if you are using
and USB based CPU board. You can check that the USB driver is correctly installed in
windows device manager, press Windows start button==>my computer, click with right
mouse button and select "properties".
Select Device Manager:

09 November 2018

Release 4.03

EDING CNC

Manual

If you see this, the USB driver is correctly installed. The COM17 number may be
different on your system.

09 November 2018

Release 4.03

EDING CNC

1.4.2

Manual

Ethernet

If you have an USB only card, you can skip this chapter and continue to 1.4.3.
For Ethernet you need a free Ethernet connection on the PC, Add a 2nd network card if
needed. Connect the CPU using a 100 MBit UTP Cross cable. Then setup the Ethernet
adapter. Go to the windows network settings, the network adapter with No network
access is one for the CPU:

Click on the adapter with no network access, here: "LAN-verbinding 4" here, the text in
your PC may be different.

09 November 2018

Release 4.03

EDING CNC

Manual

.
Press Properties:

Switch on only TCP/IP V4 and uncheck the rest.

09 November 2018

Release 4.03

EDING CNC

Manual

Now press properties of the TCP/IP settings:

The PC LAN adapter gets IP Address 172.22.2.101.
The EDINGCNC CPU network is setup for 172.22.2.100.
Press OK, now you can test if the network is working, click the Windows Start button,
select all programs ==> accessories==>command prompt.
In the command prompt, enter ping 172.22.2.100, when connection OK, you should
see:

09 November 2018

Release 4.03

EDING CNC

Manual

When connection Failed, you will see:

If you have this, check you cable and your network settings again. Also check that the
yellow led on the CPU is flashing at approximately 1Hz.

09 November 2018

Release 4.03

EDING CNC

1.4.3

Manual

Set admin mode and switch off UAC

Eding CNC software needs real-time priority on Windows to control, your machine
correctly. This only allowed with Admin rights, so make sure, the user has Admin Rights,
these screens are from Windows 7, they are similar on Windows 8 and 10:
On Windows 10, Windows key + X allow to select the classic configuration settings,
from there go to user accounts.

And switch off UAC.

After the install you will have the program ICON on your desktop. Do not start it yet,
read further.
09 November 2018

Release 4.03

EDING CNC

Manual

The application must be started as Administrator and the user starting it must have
admin rights. Right click the mouse on the EdingCNC Icon and then select run as
Administrator on Windows 7/8/10.

You can now start the software.

09 November 2018

Release 4.03

EDING CNC

1.4.4

Manual

Disable automatic update in Windows 10

In Windows version prior to Windows 10 it was possible to disable automatic update or
set it to manual. This is recommended because an automatic update can stop the
running CNC operation which is probably not what you want.
The text below describes how to disable automatic updates on Windows 10.
Using Windows + X start the control panel.
Start Administrative tools.

Start services:

09 November 2018

Release 4.03

EDING CNC

Manual

Find Windows Update:

Change startup type from Automatics delayed start Disabled.
Press Stop. Automatic update is from now on disabled:

If after a while you want updates, undo this by setting Startup type back to Automatic
Delayed and Press start, let it update and then disable automatic update again.

09 November 2018

Release 4.03

EDING CNC

1.4.5

Manual

Connected drives not visible Windows 10

If you encounter that connected drives are not visible, her the explanation and how to
solve it. The drives are mapped using normal privileges when Windows is started up.
The EdingCNC software is started in Administrator mode because it needs Real-time
process priority. For Windows 10 this is a different user and the drives mapped for the
normal user are not visible due to this.
This can be solved by a setting called EnableLinkedConnections in the Windows
registry, this way:
Click Start, type regedit in the Start programs and files box, and then press ENTER.
Locate and then right-click the registry subkey
HKEY_LOCAL_MACHINE\SOFTWARE\Microsoft\Windows\CurrentVersion\Policies\System.
Point to New, and then click DWORD Value.
Type EnableLinkedConnections, and then press ENTER. Right-click
EnableLinkedConnections, and then click Modify. In the Value data box, type 1, and
then click OK. Exit Registry Editor, and then restart the computer.
Now everything works for you as expected.

09 November 2018

Release 4.03

EDING CNC

1.4.6

Manual

Profiles, If you have different setups e.g. lathe and milling

If you have e.g. a milling machine and a turning machine controlled from the same
computer, you can make a copy of the software ICON and then rename one to
“CNC4.03 TURN” and the other “CNC4.03 MILL”.
Now right click de ICON and select “properties”:

09 November 2018

Release 4.03

EDING CNC

Manual

Then you must tell the software which settings file to use. This can be done by editing
this line in the TAB “Shortcut”

Change this line "C:\CNC4.03\cnc.exe", add turning.ini at the end:
"C:\CNC4.03\cnc.exe" turning.ini
Now the software will use turning.ini to store your settings.
Without the turning.ini the software uses default file name cnc.ini to store the
parameters.

09 November 2018

Release 4.03

EDING CNC

Manual

2 The user interface
General info:
There are several views:
Operate , Program, Tools, Variables, Setup and Help.
Using control-tab, you can tab through them.
It is important that EDINGCNC is started started as administrator. On windows 7 this is
not automatically done like in XP.
Click on the right mouse button and select “Run As administrator”. You can also set this
in the ICON properties, compatibility.
When you start EDINGCNC for the first time you will get the Terms/Guarantee page click
the language you read the text. Then click agree if you agree. The operate page is
shown. This is the main screen to do all machine operation’s from.
Running a program and fast jogging is only possible after the machine is correctly
homed, so this must be setup first. The reason is that collision prevention is not
active when the machine isn’t homed, so damage to the machine may happen
when homing is not performed.
Program window "Operate" is shown All machine operation are performed from this
TAB.

If all settings for your machine you can press Reset (F1), this enables your drives.
Then you are asked to home the axes:

09 November 2018

Release 4.03

EDING CNC

Manual

When you see this, you can use the home menu or the button besides the Feed Speed
readout. Buttons you need often like this one is always nearby.
Homing is very important, after homing the position inside the software does match with
the physical machine. So only then the software will allow movements correctly and
stop just before the limits of the machine without collision against the machine limits.
So always make sure homing is working correctly!
Home can be done individually or in a sequence for all axes using these buttons:

09 November 2018

Release 4.03

EDING CNC

Manual

When homing is done you are free to move the axes by the JOG Keys, the position
display numbers have become white indicating that homing was performed.

These are the arrow keys on your keyboard:

With the keys you move the axes, we call this jogging.
Using the keys alone you have low speed, 10%.
Using the keys in combination with the CTRL key, you get 50% speed.
You get 100% speed in combination with the SHIFT key.

09 November 2018

Release 4.03

EDING CNC

Manual

You can set the axes position by clicking the axis position display:

And you can also move the axes by holding the CTRL key and clicking with the left
mouse button on the position display.

09 November 2018

Release 4.03

EDING CNC

2.1.1

Manual

Setup Pages

Before the system is actually used we have to setup the system to accommodate the
machine, we do that in the setup pages. There a two main setup pages:

2.1.2

UI and Connection

Connection to CPU: If you have 1 board connected to your PC, leave the setting at
AUTO, the software will find the board automatically. Otherwise
choose the here the CPU you want to work with. For CPU's with USB,
you see the COMx ports here, in case of a CPU5 with Ethernet, you
will see the IP-Address here.
Ethernet:

If you have a CPU with Ethernet, check the Ethernet checkbox.

Max Step Frequency:
The maximum step frequency that the CPU will generate. For motor
drives it is needed to lower the maximum frequency. In case the drive
is unable to handle the high step frequency or low step-pulse width.
Some of the digital drives from Leadshine cannot handle 125Khz steprate, they need a setting of 90Khz or lower.

09 November 2018

Release 4.03

EDING CNC

Manual

Language setup: Speaks for itself. After it is set, save the changes, then close
EDINGCNC and restart so that everything will be in the correct
language. The translations are in 2 files, cncgui-lang.txt and
cncserver-lang.txt, if you find translation mistakes you can correct
this here. Please send the corrected file to Eding CNC, the corrections
will then be incorporated into new versions.
Password:

You can protect the setup parameters from being modified by
unauthorized persons by using a password. Leave empty if no
password is desired.

INCH:
MM:

Machine setup is in inch mode.
Machine setup is in mm mode.

2.1.3

Motor setup

Visible:

Check if the axis should be visible in the GUI.

Port:

Map axis to a physical output port of the CPU.
If an axis is mapped and not visible, it can still be used in the
interpreter.

Mode :

Select mode for rotation axes, slave or special function:
•
•
•

•
•
•

ROT, default, axis behaves as a normal rotation axis.
SLAVE X, SLAVE Y or SLAVE Z axis is slave of X or Y or Z axes, for
Gantry machines with two independent (Tandem) motors on the
main axes. See also the Homing chapter for details on Slave axes.
FOAM CUT for A-Axis, if used as a Foam cutter with 4 linear axes.
X is the left horizontal axis, Y is the left vertical axis, A is the right
horizontal axis and Z is the right vertical axis. Feed calculation are
based on the X/Y or A/Z combination which ever makes the
biggest distance,
4th MILL, if used in 4 axes milling. Feed calculations are optimized
such that the tooltip gets the correct speed relative to the
material.
Tangential Knife, this option is available for the C-Axis only. The
Knife will rotate in the movement direction of X-Y. See also
trajectory setup.
2nd Z, for machines with 2 Z axes, where the A axis is used as
the 2nd Z.

Steps/AppUnit :
Fill in number of steps per millimeter for millimeter mode or number
of steps per inch for inch mode. For rotary axes, the unit is always
steps per degree. Fill in a negative number to reverse the motor
direction.
Example: Suppose your driver is set to 1600 steps/revolution (1/8
micro step) and you have coupled the motor directly to a spindle with
5mm pitch. The number to be filled in here = 1600 / 5 = 320.
If the movement direction is wrong, change it to -320.

09 November 2018

Release 4.03

EDING CNC

Manual

Positive limit: Maximum machine position.
Negative limit: Minimum machine position;
Vel :

Maximum axis velocity, all velocities, whether jogging, G0/G1/G2/G3
are limited to this value.

Acc:

Maximum acceleration.
When this value is set equal to the Vel parameter, it will take 1
second to reach the max velocity. When the value is 2x the Vel
parameter, the max velocity is reached in 0.5 second.

09 November 2018

Release 4.03

EDING CNC

2.1.4

Manual

Homing and ESTOP setup

Home Vel/Dir:

Homing velocity, a negative number reverses the homing direction.
When the velocity is set to 0, the axis is homed manually, see the
homing and coordinate systems chapter.

Home Position: Machine position at the moment the home switch activated. This
determines the machine coordinates. It is not really relevant where
the machine zero point lies, it should only match with the MIN/MAX
position.
Homing sensors should be setup such that they remain active until the mechanical end
of the machine. The space from home sensor activation to mechanical end is required to
ramp down the movement.

Machine Mechanical Range

Home Sensor behavior, good
Home Sensor behavior, WRONG!

Use only home X for all axes:
Check this option if you have all home sensors wired to one input.
HomeSensorIsEStop:
The home sensors can also be used as limit switch which generate an
E-Stop when activated. When this function is required, the sensors
should be mounted outside the normal machine area.
Check this option if the home sensors work as EStop when activated.
This option will work after homing is complete. The reason is that
otherwise homing itself will generate an E-Stop.
Note that if this option is used and a home sensor triggers, it will be
latched, so that it will remain visible in the UI also if it was triggered
by a short pulse. The Reset will clear the latch.
HomeInputSenseLevel:
Defines HomeSensor input behavior,
0 = low active (normally open switch),
1 = high active, (normally closed switch).
set the level of your end of stroke switches, these are used for
homing the machine. First check that the home sensors or switches
are working, activate them and look at the home-LED's at the lower
left side of the main Operate screen. If you see it working, take care
that the machine axes are at the working area, so that none of the
sensors are activated. Look at GUI "LEDs"

09 November 2018

Release 4.03

EDING CNC

Manual

EStopInputSenseLevel1:
Defines EStop input behavior,
0 = low active (NO switch CPU5 series, NC switch iCNC600),
1 = high active, (NC switch CPU5 series, NO switch iCNC600).
2 = OFF, not used
EStopInputSenseLevel2, CPU5B only:
Defines EStop input behavior for second EStop input,
0 = low active (normally open switch),
1 = high active, (normally closed switch).
2 = OFF, not used
ExtErrInputSenseLevel, CPU5B and iCNC600 ONLY:
Defines External Error input behavior (CPU5B only),
0 = low active, e-stop (NO switch CPU5B, NC switch iCNC600),
1 = high active, e-stop (NC switch CPU5B, NC switch iCNC600).
2 = OFF, not used
3 = low active, smooth stop
4 = high active, smooth stop
With smooth stop the axes speed is ramped down, this means that
there is no position loss.
The polarity settings for the home inputs, E-stop's and Extern error can be automatically
determined by pressing the "Auto detect polarity" button.
Note that if the estop or extern-error input triggers, it will be latched, so that it will
remain visible in the UI also if it was triggered by a short pulse. The Reset will clear the
latch.
ExtErrInputSenseLevel via Sync input, CPU5A ONLY:
CPU5A do not have an ExtErr input, but applications that do need this
function, can use the Sync input with limited functionality
Defines External Error input behavior (CPU5A only),
3 = low active, smooth stop
4 = high active, smooth stop
With smooth stop the axes speed is ramped down, this means that
there is no position loss.
SafeFeed:
Defines the max velocity [mm/second] used for jogging and running if
the safety input is active or if the machine is not yet homed.

2.1.5

Backlash setup

Backlash:

Set the amount of backlash for each axis that the software should
compensate. Experiment with velocities and acceleration, the backlash
compensation demands more from acceleration your motors than

09 November 2018

Release 4.03

EDING CNC

Manual
without backlash compensation. Do not try to compensate more than
0.1 millimeters. If there is more backlash, try to reduce it
mechanically first.

2.1.6

LAF setup

LAF minimum angle:
Look Ahead Feed calculations: Motion segments (g1,g2,g3) that are
connected with a smaller angle as specified in min.angle will
accelerate through which will give higher speeds especially with
programs consisting of small motion segments. This is a unique
feature which you don’t find easily on low cost CNC controllers.
Be carefully with the min.angle setting because this cause
acceleration spikes, it depends on your machine and the speed up till
what extend this is possible. I suggest performing tests with en check
whether you get step pulse loss.
A value of 0.1 .. 3 degrees is generally safe. Segments that are really
tangential connected will move fast that way.
An example of what I use:
When using CorelDraw, a circle is drawn of 100mm in diameter, and
exported as HPGL CorelDraw generates small line segments of
approximately 6 degrees. Now I have set the min.angle to 6, this
gives the possibility to mill the circle with a speed of F6000 while
without LAF the speed would be approx F1300 on my machine.
There are other run-time modifiable settings for LAF, see G64.
InterpolationTime and FifoTime:
Every motion command is chopped up in small motion segments with
a time of InterpolationTime in the setup.
The segments are send to the controller (CPU) which has a buffer
(FIFO) that holds the motion segments. The step-pulse generator
takes the motion segments one by one and generates stepper motor
pulses from that. The number of the segments in the FIFO is
depending on the FifoTime specified in the setup.

09 November 2018

Release 4.03

EDING CNC

Manual

This part runs on the PC side

GUI
CNC.EXE

CNCAPI.DLL

CNCServer.exe

Ethernet or USB

LAF

One motion segment, time = Interpolation time
#elements = FifoTime / InterpolationTime

FIFO

STEP-PULSE-GENERATOR
Controller CARD (CPU)

The FIFO makes it possible to perform smooth motion without
hiccups on a non-real-time operating system like Windows. Because
what happens is that sometimes Windows does things for itself
stopping the execution of CNCSERVER.EXE for short times. This is no
problem as long as the FIFO does not run empty (If the windows
hiccup is longer than the FifoTime).
The default value for InterpolationTime = 0.005 seconds. The
default FifoTime = 0.25 seconds. This means that the FIFO can hold
50 motion segments.
Why are these parameters adjustable?
1. For some applications it is desirable to have a lower interpolation
time, e.g. if you have a machine with very high acceleration. a
lower InterpolationTime may give smoother acceleration. The
minimum interpolation time is 0.0025 second.
2. For some applications it is desirable to have lower FifoTime, e.g.
Plasma THC, it will give more dynamic to the THC control if the
FifoTime is lower.
Setting the FifoTime or InterpolationTime lower also means
that the communication needs to be faster, so if these settings are
modified to lower values, a faster PC is required.
09 November 2018

Release 4.03

EDING CNC

Manual

FIFO UNDERRUN ERROR
If this happens then this indicates that the PC is too slow to keep
the FIFO full.
Possible causes are:
• PC too slow.
o The processor is too slow. (recommended minimum
is 1.3 GHz duo-core processor, 2G RAM for 32bit
Windows, 4G RAM for 64 bit Windows. If you
execute large 3D g-code files > 10 Million lines, 4G
RAM or more is recommended.
o Too little memory in the PC (can be checked in task
manager, there must always be Physical memory
available, if the system starts swapping to disk
because the memory is all used, changes on FIFO
UNDERRUN is high).
o PC has switched to energy saving mode and has
become slow. So always adjust the energy saving
settings such that there is maximum performance
always.
o Because you suddenly get an automatic Windows
Update, so always switch off automatic Update and
perform updates manually when you want.
o Because virus checkers become active making the
system slow. So always turn off anti-virus check
when running the CNC controller.
•

USB communication too slow or EMI disturbance that
corrupts the communication.
Take care that your cabinet is wired according EMC rules,
you can find some tips at the end of this manual.
If the USB chipset is slow, you could solve it by using a PCI
USB add-on card. If this is not possible, you need another
PC.

•

Ethernet communication too slow. This could happen if the
settings are not 100% equal to what is described in the
setup. E.g. for the used adapter card only the TCPIP
protocol must be on and all others must be OFF. There
must be a 1:1 connection from Controller Board to the PC
using a CROSS CAT5E cable. So you cannot connect the
CPU as part of your home network, it must be on a
separate network adapter.
Theoretically also Ethernet may suffer from EMI
disturbances due to bad unshielded cabling. In practice
Ethernet is very robust to this. Anyway always make the
wiring with the EMC rules in mind. See hardware tips at the
end of the manual.
There is also this experience, heavy browsing on internet
while doing CNC may cause FIFO UNDERRUN error,
especially on Windows XP. Windows 7 and Windows 8 are a
lot better than Windows XP with this.

09 November 2018

Release 4.03

EDING CNC

Manual

G0 Feed Factor:
With this you can apply a factor for the feed used at G0, this allows
different feeds for G0 positioning G1/G2/G3 milling.
G0 Acc Factor:
With this you can apply a factor for the acceleration used at G0, this
allows different acceleration for G0 positioning G1/G2/G3 milling.
FeedOverride input:
You can select “UI”, “UI & Hand wheel” (Default) or “analogue input 1
– 3” on the CPU, with analog input you can use a potentiometer to
control the feed override, recommended potentiometer value is 4K7.
When UI and hand wheel is selected you can control the Feed
Override using the F+ and F- buttons and the Hand wheel to control
the feed Override from 0-300%. Note that the machine will not go
faster than the maximum velocities of the motors allow.
FeedHold input: Here you can select a digital input from the CPU that sets the Feed
Override to zero immediately when activated. When released the Feed
Override will go back to the value before. This function may be used
by EDM machines to stop the feed when there is a short circuit
detection of the electrode.

2.1.7

Kinematic Setup

Trivial kinematics:
It is not needed for normal Cartesian machines, leave the Trivial 1:1
kinematics checked. Please contact Eding CNC if you have a special
machine or robot with non-Cartesian axes.

2.1.8

Tool change Area setup

XYZ Limits:

By setting the limits here to a value different from zero, the TCA (Tool
Change Area) guard will be activated. Using the values here you
define an area on the machine which is restricted to tool change. A
normal work piece program is not allowed to enter this area.
You can also not jog in this area or move to this area by MDI.
If you need to be in this are issue command "TCAGuard off" To reenable the protection "TCAGuard on".

Z DownToolLength:
For machine configurations where the tool chuck does not touch the
machine bed when the machine is at its lowest Z position. Here you
specify the tool length of the tool that fits when Z is at its lowest
position.
This information is important for collision guarding.

2.1.9

Tangential knife setup

TanKnife Angle:
Tangential Knife is a rotation motor (the C Axis) around Z. Tangential Knife works
09 November 2018

Release 4.03

EDING CNC

Manual

with normal G1, G2, G3 without tool-radius compensation G41, G42. The knife is
rotated automatically in the direction of the X-Y move. This parameter determines
the angle which 2 lines/Arcs can make without lifting the Z. If the angle is greater
as this value, the Z will move up (G0), rotate the knife (G0), then move down
again (G1). If the angle is lower, the rotation will take place without moving Z up.
TanKnife Z up distance:
Specifies the distance to lift up Z when detected angle is greater than Tan Knife
Angle.
TanKnife blend angle and blend distance:
When subsequent lines have an angle with current line which is less than the blend
angle and when the subsequent line or arc length is less than specified length the
knife is not rotated before the move but during the move. For small angles in
combination with small segment lengths this is in practice tolerable and will speed
up the cutting process a lot. Be aware however that the knife direction is not
exactly in the cutting direction and my break if the angle is too large.
The tangential knife is switched on and configured by interpreter commands.
These commands can be typed in MDI, part of the G-Code or hooked under the user
buttons in macro.cnc.
;Switch tan knife on or off. Tan knife must first be configured in the setup.
Tanknife off
Tanknife on
;map tan knife to B or C or both axis output.
Tanknife b
Tanknife c
Tanknife bc
Especially for BEND tangential knife
Tanknife lo
Define the low Z value in work coordinates, this is the deepest point in the groove (*).
Tanknife hi
Define the high Z position in work coordinates, usually is 1-5mm above the material (*).
Tanknife bend -1 | 1 define the direction to which the knife is bend for a 45 degree
knife (*).
Tanknife rw knife will be rotated back after nr of turns (anti-windup of
wires). (*).
Tanknife lu set new lift up distance for rotating. (*).
(*) These parameters are saved and used next time with Tanknife on command.
For usage of tangential knife that is bend 45 degree do calibration of the hi and lo
position first. Then switch the knife on by tanknife bend -1 or +1 depending on the side
to which it is bend. Set the C position to 0 when the sharp edge is pointing straight to
the +X direction.

09 November 2018

Release 4.03

EDING CNC

Manual

10.00

20.00

KNIFE (C=90)

Knife Height

KNIFE (C=-90)

Z Low position

mat

5.00

Z High position

10.00

5.00

10.00

It is clear that with the bend knife during a z-move, the XY axes should move as well
with same distance as Z, in the direction such that the sharp side of the knife moves
under 45 degrees into the material. The user will program Z moves, the interpreter will
rotate the knife (C axis) into the correct XY direction. Then kinematics will add the XY
correction depending on the Z position.
The correction direction is the C axis angle + or - 90 degrees depending to which side
the knife is bend. The correction amount in XY is the same as the height from the
deepest point in the groove to the height where the knife is bend. So, if we define the
tan knife low position as the deepest pointing the groove, then the compensation
distance can be calculated as: CD = Z current - Z low + knife height.
The low position is where the XY correction is zero. This is the Z position at the bottom
of the V-groove. The high position is where the compensation starts when coming from
above. This should be at the surface of the material or little above.

09 November 2018

Release 4.03

EDING CNC

Manual

Practical example:
;Test tangential knife
;Cut 2 lines
;Top of material Z is 0
;V cut 5mm deep
;
Tanknife hi 1.0
Tanknife lo -5.0
Tanknife bend 1
G0 Z10

;Start combined move 1mm above material surface
;Deepest Z value in V groove
;Note that bend can be -1 as well, depending on the
;knife construction.
;move above the material and above tanknife hi position

Tanknife on
G0 X0 Y0
G1 F200 Z-5
G1 F500 X100
G1 Y100
G1 Y0
G1 X0

;Do this before moving to the starting point.
;Starting point
;Knife into material deepest point in groove.
;Cut 100mm in X
;and 100mm in Y
;and backwards to make a V groove

G0 Z10
Tanknife off
M30

;done Z up
;Knife off

Note the we make the move twice, in either direction to make the V groove.
Blue is the programmed line, deepest point in the V groove at Z-5 in the example.

X100, Y100

X100, Y0

X0, Y0

If we would make a move at Z1 (tanknife hi position), then the move would be the
orange lines. With tanknife bend -1, the compensation is on the right side with respect
to the move direction. On the other side with tanknife bend 1.
The tanknife will automatically move up when the movement direction changes. The
move up distance is specified in the setup. Als the angle at which a lift-up is required is
specified in the setup.

09 November 2018

Release 4.03

EDING CNC

Manual

2.1.10 Safety/Door open Input setup
Safety Input Selection:

Select one of the AUX inputs to act as safety input, when
active, only low speeds are possible and the running g
code goes to pause (Feed hold, spindle off). This can only
be configured for CPU5B.
For professional users, there is more that can be
configured in the parameters file, cnc.ini:
Each AUX input can be setup to be guarded run time an
stop the running program or give a warning.
[SAFETY]
aux1InputCheckSenseLevel = 2
;Where 0,1,2=no action, 3=sstopOnLow, 4=stopOnHigh,
5=slowFeedOnLow, 6=slowFeedOnHigh, 7=warningOnLow,
8=warningOnHigh

Safety Feed:

Feed in [mm/s] to be applied when the safety input is
active and when the machine is not homed and homing is
mandatory is set.
Intended use is for a door switch.

Related to this functionality, there are these variables to be set (cnc.ini only)
noStartSpindleIfPauseActive:
when set to 1, the spindle cannot be switched on if the
pause input is active.
noStartJogIfPauseActive:
When set to 1, jogging the axis is not possible if the pause
input is active.

2.1.11 Spindle and PWM setup
MinS:

The lowest possible speed for you spindle. If a command
for a lower S values is used, then this minimum value is
applied.

MaxS:

The speed of your PWM controlled spindle when the PWM
signal is at 100%.

Ramp up Time:

The software waits this time between switching on the
spindle and starting the further machining.

StopOnPause:

Stop spindle when pause is activated.

zUpOnPause:

Z goes automatically up when pause is activated.

09 November 2018

Release 4.03

EDING CNC

Manual

autoStartAfterPause:

When start is pressed, the X,Y axes automatically
reposition to the pause position, the spindle is started,
then the Z goes down with approach feed and the program
continues.

zUpDistance:

Hom much the Z goes up when when pause is activated
and zUpOnPause is active. Software will protect against
going up beyond the Z limit.

approachFeed:

The feed used for Z down when autoStartAfterPause is on
and the start button is pressed.

RPMSensor:

Check if you have connected a spindle speed sensor to the
Sync input of the CPU. The sensor should give 1
pulse/revolution, minimum pulse width 0.5ms.

MistIsSpindleDirection:

Special for CPU5A, use mist output for spindle direction if
you need it (CPU5A has no separate spindle direction
output, that is why).

IsStepperMotor:

Step/Direction pulses will be generated if set instead of
PWM. A Stepper motor or Servo Spindle can be connected
to the PWM/TOOL-DIR output when selected.

SmoothStep:

Only in combination with IsStepperMotor, when checked
the ramp-up-profile is smoother than when not checked,
however when checked PWM2/PWM3 on the CPU5B cannot
be used as separate PWM output anymore..

CountsPerRev:

Provide the number of steps/revolution here if
IsStepperMotor is checked.

SpeedOverrideInput:

Specify UI or analogue input for controlling the speed
(CPU5B).

SpeedHoldInput:

Specify digital input for speed hold, when activated spindle
speed goes to zero. When release spindle restarts. Some
applications need this functionality.

SpindleReadyPortID:

User definable input which indicates that the spindle has
reached it speed. It is currently only available by editing
the cnc.ini file.

showInProgSpeed:

This setting is under [USERINTERFACE] in the cnc.ini file.
It can have these values:
0: Show programmed speed (Default)
1: Show PWM value
2: Show analog in 1
3: Show analog in 2
4: Show analog in 3
hese options are convenient if the spindle has an analog
output for power measurement.

showInProgSpeedAnaMulFactor :
09 November 2018

Release 4.03

EDING CNC

Manual
Multiplcation factor for the analog value for option 2-4 with
showInProgSpeed.

09 November 2018

Release 4.03

EDING CNC

Manual

Setup Page 2, press ">" button on first setup page to get here:

2.1.12 UI setup items
Invert JogKeys: Inverts the movement of the keyboard keys, for moving bed
machines, the bed moves in the direction you press the arrow.
IsTurningMachine: Check if your machine is a Lathe, this effects mainly the 3D display
which shows the X-Z plane for turning. Also the jog keys operate
differently. Futher the working plane is set to G18 (X-Z).
ShowStartupScreen:
When checked, the startup screen is shown when
EDINGCNC starts.
HomingMandatory: When checked, running a job and mdi is not allowed before the
machine is homed. Also the jog speed is limited to 5% speed. This
feature prevents damage to your machine because when the
machine isn’t homed, the limit guards are not working. So, I
advise to leave this item checked always.
SimpleZeroing:

09 November 2018

If checked, the zero buttons (beside the position display), will
simply set the work position to zero. If this item is not checked, a
dialog will be shown in which you can set the position. Default it
shows a value which is – tool-radius of the current tool. This is
handy when zeroing from the lower left corner with the endmill
against the material.

Release 4.03

EDING CNC

Manual

G10L20Zeroing:

If checked the active coordinate system (G54 – G59.3) is zeroed
instead of the global G92.
If not checked the global G92 global method is used.

AutoToolChange:
ShowMaximized:

If checked the running job will not stop when a tool change is
encountered. Use this when you have a ATC or if you simply always
have the tool already in.
GUI will start maximized taking the whole screen.

ShowM7:

Show or hide M7 button

ShowM8:

Show or hide M8 button

ShowAUX1:

Show or hide AUX1 button

KeyboardTimeout: Time out is used while jogging. This feature is introduced because
of the use of Bluetooth keyboards. It could happen that jog start is
pressed, but never released (jog stop) because to keyboard is no
longer in reach. The timeout will automatically jog stop of needed.
The default value of 1s is OK for most PC’s. I do not recommend to
set it lower because you may get unwanted time-outs.
REMARK: More ShowXXX options are available under
[USERINTERFACE] in the configuration file cnc.ini.
ShutDownOnFatal: If checked software will shut down automatically when a fatal error
such as disconnected CPU occurs. This may be used when the
electrical power is switched of and connection to the CPU gets lost.
Favorite Editor:

Specify your favorite editor here. I recommend notepad++, it is
freely downloadable at internet. E.g. for notepad++, specify
c:\program files\notepad++\notepad++.exe.
The advantage of notepad++ is that the editor jumps to the actual
G-Code line immediately, very handy when programming G-Code.

IconDirectory:

The name of the directory where the GUI icons are located.
nu means not used.
If you want to change the Icons on the buttons, you can make first
a copy of the entire icons and name that directory to myIcons.
Make your changes an place the directory name in this field.

OpenGL:

Check to use OpenGL graphics. This allows smooth panning,
zooming and rotation using the mouse.
Left mouse key; Pan
Right mouse key: Zoom
Control + Left mouse key: Rotate.

OpenGLPenSize:

Set PEN size shown in graphic, size is in millimeter.

2.1.13 IO setup
Invert IO:

Check if you want to invert the output.

09 November 2018

Release 4.03

EDING CNC

Manual

2.1.14 Interpreter settings
DiameterProgramming:
Check if you want diameter programming for turning, all X-axis
values are interpreted as diameter. The effect is that all
movements in the X-axis are divided by 2.
AbsoluteCenterCoords:
If Checked, the I,J,K value is interpreted as absolute value.
Incremental is used mostly.
LongFileModeCriterion:
Specify a number of Kbytes here. When the loaded job file is
larger, the UI switches to long file mode. The program listbox
changes and the graphics will show only outlines when a program
is loaded. This is all needed to preserve memory and speed for
large files.
In this mode the file itself is still executed from memory and allows
complex G-Code constructs (While, If then else, sub routines).
SuperLongFileModeCriterion:
Specify a number of KBytes here where super long file mode starts.
This number should be equal or bigger as LongFileModeCriterion.
For very long files from 20MByte and UP to 4G this mode is
required. It also puts the GUI in the same mode as with
LongFileMode, but as extra, the file itself is no longer executed
from memory. The means that complex G-Code constructs are no
longer possible. These type of files contain only straight forward gcode without "while-endwhile", "if-then-else" and "subroutines".
The tool changes are still executed from the macro.cnc file, so full
automatic tool change is still available.
Files with up to 100.000.000 lines of G-Code have been tested with
this.
Macro Filename:

Name of the macro file, it can be changed, the default is
macro.cnc.

User Macro Filename:

Name of the macro file, it can be changed, the default is
macro.cnc.

2.1.15 Traffic light setup
Red:

Specify output for RED color.

Yellow:

Specify output for YELLOW color.

Green:

Specify output for GREEN color.
CPU5B is required to view all colors because other CPU's do not have
enough amount of outputs.

09 November 2018

Release 4.03

EDING CNC

Manual

2.1.16 JobTimeEstimation
During the Render phase, after loading the job, the job time is estimated. But this is just
a quick estimation because a real calculation of time would take too much time,
therefore these parameters:
CorrectionFactor:

Correction factor for the time calculations, you can change this if
you see that your type of jobs require a correction.

RestimateRunTime: When checked, you will see the remaining estimated time of job
based on the average speed measured and the total distance to
go.

2.1.17 Hand wheel Setup
Cnt/Rev:

The number of counts of the hand wheel for one revolution, usually
400 for most CNC hand wheels.

Count:

Shows the actual Hand wheel count value, try to turn the hand
wheel and see it change.

V[%]:

Percentage of velocity from selected axis, this is the maximum
velocity the axis will move when using the hand wheel.

A[%]:

Percentage of acceleration from selected axis, this is the maximum
acceleration the axis will move when using the hand wheel..

X1..X100 Vel Mode:In velocity mode the most important is that the movement stops
immediately when the rotation of the hand wheel stops. The
position of the hand wheel will not be maintained if velocity mode
is on. The position of the handheld is maintained if velocity mode
is off. This also means that the axis may not immediately stop if
the hand wheel rotation stops. When turning beyond the limits of
the axis, you have to turn back the hand wheel the same amount
before the axis starts moving again.
My own experience is that it works best to use velocity mode at
X100 only. Jus play with it to experience the behavior and make
your own choice.
AxSelInput:

09 November 2018

Specify analogue input to be used for axis selection. A multi switch
with 5 1K resistors can be used to make this:
See hardware specification CPU_5B_FLYER_TECH.PDF, it is on the
download page of the website. This option is only applicable to
CPU5B. The max analog input value is 1023 and this corresponds
with 3.3 Volt.
INPUT VALUE
VOLTS
AXIS
SELECTED
< 100
<0.32V
(0.00)
120-220
0.38 – 0.71 (0.55)
1
290-390
0.94 – 1.26 (1.10)
2
460-560
1.48 – 1.81 (1.65)
3
630-730
2.03 – 2.35 (2.20)
4
800-900
2.58 – 2.90 (2.75)
5
> 970
>3.13
(3.30)
6

Release 4.03

EDING CNC

Manual
You can achieve this by putting 6 identical resistors in series and a
rotation switch. Example made for OFF-XYZ axis:
+3V3
Select C

CPU5B-IN3
PIN7 + PIN9

470R – 1K
Select B
470R – 1K
Select A
470R – 1K
Select Z

CPU5B-IN3
PIN 1 or
PIN 3 or
PIN 5
Variable Voltage

470R – 1K
Select Y

ROTARY
SELECTION
SWITCH

470R – 1K
Select X

Select Nothing

CPU5B-IN3
PIN8 + PIN10

470R – 1K

GND

MulSelInput:

Specify analogue input to be used for multiplication factor selection
X0.1 x1 x10 x100. This option is only Applicable to CPU5B.
INPUT
< 100
291-391
632-732
> 900

VOLTS
<0.32
0.94 – 1.26
2.04 – 2.36
>2.9

(0.00)
(1.10)
(2.20)
(3.30)

MUL. FACTOR
0.1
1
10
100

You can achieve this by putting 3 identical resistors in series and a
rotation switch:
+3V3
CPU5B-IN3
PIN7 + PIN9

X100

CPU5B-IN3
PIN 1 or
PIN 3 or
PIN 5

X10

Variable Voltage

470R – 1K

ROTARY
SELECTION
SWITCH

470R – 1K
X1

X0.1

CPU5B-IN3
PIN8 + PIN10

470R – 1K

GND

The axis selection can be done by pressing the CPU PAUSE input shortly. The
multiplication factor can be selected by pressing the CPU PAUSE input longer than 1
second.

2.1.18 Load/Run Automatically
watchFileChanged: If checked EDINGCNC will watch the loaded g-code file for changes
on disk if EDINGCNC is not running. When it is changed, e.g. by an
editor or because it is saved by a CAM software, then EDINGCNC
will ask you to reload the file:
09 November 2018

Release 4.03

EDING CNC

Manual

load automatically: If this is checked, the file is automatically loaded when it changes
on disk, no dialog will appear.
run automatically: If this is checked and also the load automatically check, then the
file will be loaded and immediately start running when changed on
disk.
fileName:

09 November 2018

This is the name of the file that EDINGCNC watches at startup. So
if EDINGCNC is started and this file time/date changes on disk, it
will be loaded.
If manually another g-code file is loaded, then USNCNC will watch
that one.

Release 4.03

EDING CNC

Manual

2.1.19 Probing Setup
StoreProbePoints: The touch points are stored in a file when this is checked. This is
used for digitizing.
Use Home input 4: If checked home input 4 is used instead of the standard probe
input.
File:

The file name for storing the touch points. The file is opened at the
first probe touch en closed when a M30 command is encountered,
usually at the end of the G-Code program.

M95:

Using a probe which is fixed on the machine. In this case the probetip will have an offset. For this you can use the M90-M97 function.
With this it is possible to select an offset for Spindle 1 (M90), Spindle
2 (M91), spindle 3 (M92), probe (M95) or camera (M97).
The offset can be calibrated as follows:
1. Take care that M90 is active (1st spindle), if not execute m90 in
MDI.
2. Mark a point on your machine bed and accurately move the tooltip to this point.
3. Zero the axes X,Y,Z at this position.
4. Now move the probe tip exactly to this position.
5. Execute in MDI “M95 Q1”.

09 November 2018

Release 4.03

EDING CNC

Manual

2.1.20 Camera Setup
CameraIndex:

Use 0 if you have only one camera, use 1 if you have 2 Cameras and
want to use the 2nd one.

CameraOn:

Select Camera if used.

CameraFlip:

Flip image vertically

Camera mirror: Mirror camera image horizontally
Rotation:

Rotate Camera image [Degrees]
Camera offset calibration, if you have mounted the camera on the
machine the camera will show a different position as the position of
the tool-tip. The difference is Camera offset.
The steps to calibrate this offset are:
1. Take care that M90 is active (1st spindle), if not execute m90 in
MDI.
2. Mark a point on your machine bed and accurately move the tooltip to this point. (Tip: drill hole at that point)
3. Zero the axes X,Y,Z at this position.
4. Now move the camera exactly to this position.
5. Execute in MDI “M97 Q1”.
Now when calibrated, you can use M97 to make camera offsets
active.
Tip: Use M97 P1 to position the camera at the tooltip position. Use
M90 P1 to activate and move the main spindle to the work
position.
In the GUI you can also select this by pressing control+F2 in the
graphic menu. Just try and you will see it.

09 November 2018

Release 4.03

EDING CNC

Manual

2.1.21 CPUOPT
CPU and Optional functions can be activated here:
• Enable the new AVX2 IO board
• Enable the new RLY8 IO Board
• Enable Plasma Torch Height Control
• Enable the 4th axis on a CPU3A
Note: This activation is not needed if you have after you bought a CPU.
It is needed only to enable optional functions.

These are the steps to follow:
In the dialog check e.g. the "enable axis 4" checkbox, enter tour name and press get
request code:

Send the request code to the supplier.
Copy and paste it into an email and send it to your EDINGCNC supplier.
To do this double click the code, press ctrl-c, in your e-mail press control-v.
Your supplier will send you a activation code.
Copy and paste this into the activation code area. then press activate.

09 November 2018

Release 4.03

EDING CNC

Manual

2.1.22 Using a safety relay

PNOZ S4
Safety of the machine should be independent of the CNC software.
The purpose of the safety relay is to check safety inputs like ESTOP buttons and possibly
door switches or fences and allow to switch ON only if everything is safe. If a ESTOP
button is pressed or some other way the safety chain is violated, the safety relay
switches off the dangerous power in the machine. For a milling machine this is the
spindle and the servo/stepper motors.
2.1.22.1 POWERING THE SAFETY RELAY

A1/A2 is connected to our 24V supply, the same supply as we use for the CPU card. This
power is switched on when the electronic cabinet is switched on.
2.1.22.2 INPUT CONTACTS OF THE SAFETY RELAY

The relay has input contacts S11/S12 and S21/S22 to which all ESTOP buttons and
door and fence switches are connected. We use ESTOP buttons with 2 contact like this:

In this chain of safety contacts, the contacts of an extra relay is added, this relay is
switched on when the CNC CPU is ready (system ready). Ideally this system Ready
should be derived from the CPU Watchdog signal. So that the system will switch off if
09 November 2018

Release 4.03

EDING CNC

Manual

the connection with the CPU is lost or the software hangs. The iCNC600 CPU’s have a
system ready output, for CPU5B this ouyput is defined in the cnc.ini file with:
systemReadyOutPortID = 0 ;Standard system ready port, 1 – 8 for output
AUX1-AUX8
2.1.22.3 OUTPUT CONTACTS OF THE SAFETY RELAIS

The relay has output contacts 13/14, 23/24, 33/34 to switch ON/OFF power of
safety related equipment. These output contacts are not intended to switch heavy loads,
so they are used to drive external power relays that switch on the power for the spindle
and drives. Addition: The machine guidelines require not 1 relay, but 2 in series to
switch this power. This is because a relay can mall function, 2 relays in series are safer.
OUTPUT contact 13/14 will switch ON the SPINDLE POWER using 2 external power
relays. Our frequency converter has a special enable input to which we connect the
13/14 output. OUTPUT contact 23/24 will switch ON the power supply for the motors
using 2 external power relays in series. We use a the same standard DIN rail relay 2x.
OUTPUT contact 33/34 will be connected to the ESTOP input of the CPU (ESTOP 1 for
CPU5B).
Example of a DIN rail power relay.

2.1.22.4 SWITCHING ON THE SAFETY RELAY

If everything is safe the relay can be switched on via a special RESET input.
This reset input can be a physical button or software operated. We want it to be
software operated, using the MACHINE ON button in the UI:

We set the relay mode to operate at a positive edge on the S34 input:

09 November 2018

Release 4.03

EDING CNC

Manual

We use the AUX1 output of the CPU to reset the safety relay and connect this output to
the AUX 1 output of the CPU. The iCNC600 has 24V outputs and can directly be
connected to S34. CPU5B has open collector outputs and cannot be directly connected,
here a small 24V relay is needed. The contacts of the relay are connected like this:

Configuration of the safety relay is done in the settings file, cnc.ini.
These are the parameters, which are located under section
[SAFETY]
safetyRelayPresent = 0 ;Set to 1 if safety relay present
systemReadyOutPortID = 0 ;Standard system ready port or use 1-9 for AUX port 1-9
safetyRelayResetOutPortID = 0 ;1-9: AUX1-AUX9
safetyRelayResetDelayMs = 500
safetyRelayPulseLengthMs = 250

Now, the sequence to switch on is as follows:
- Make sure the ESTOPs are not pressed.
- Press the MACHON button in the UI The software will first switch on the
systemReadyPortID, (note that this port switches a relay that is part of the
safety chain) then wait 500ms and then generates a 250ms pulse on the
safetyResetOutPortID. Finally the software waits again 500 ms and now
checks id the ESTOP input has switched. Of yes, all is OK and the machine is ON.
-

Next press the RESET button, this will switch on the amplifier enable.

09 November 2018

Release 4.03

EDING CNC

Manual

2.1.23 Operate Page, this is where the machine is operated
This is the operate page in menu Auto.

2.1.24 Operate page introduction
From this screen all machine operation like jogging, running a job, etc can be executed.
The Operate screen is designed such that it is mouse, mouse-less and touch-screen friendly.
In the middle we see the graphics showing the tool path. Blue/Red when loaded and
rendered. Yellow/Green when actually running. So it shows the tool path real-time.
Note that for Lathe/Turning the material Stock can be shown, this is done by adding these
directives to the g-code file:
;Define stock (turning/lathe only)
%stockdiameter=40
%stocklength=50
%stockZatWorkZero=1 (if zero, the Z machine limit is used instead of the work zero).
At the
•
•
•
•
•

left side there are buttons for common used IO:
Spindle on-off,
Flood
Mist Coolant on-off, and
AUX on-off (e.g. for the machine light).
MACHINE ON Button (Below Home C led)
This one has a few colors with different meaning:
o Grey means machine is off, drives switched off.

09 November 2018

Release 4.03

EDING CNC

Manual

o
o
o
o

Yellow Flash, amplifiers must be enabled, homing must be performed.
Yellow, waiting for operator action.
Green, machine running.
Red, error or estop. Flash when E-Stop still active.

The right part of the screen shows the axes positions, when homing you use the machine
coordinates and for all other operations the work coordinates.
The buttons beside the axes positions are for zeroing the work position, on the background
a G92 command is executed to perform this. The zero buttons can also be found in the zero
submenu, especially for people who do not like using the mouse at the machine.
below the machine positions we see the general status window:
You can select FS (Feed Speed), GMT (G-Code, M-Code, Tool) and T (time estimation for
running job).
There is a shortcut key: ctrl-v to change the selection here.
Feed/Speed
You see the actual value, set value and percentage.
If you do a G1 in this example, the feed will be 60.
If you switch on the spindle with M3, the spindle speed will be set to 100 rev/minute.

Pressing control-v will give:

This shows the actual G code and M code status as well as the actual tool number and the
machine state, READY, RUNNING etc.
control-v again gives
Here you see the actual running time of a job and also the estimated TOTAL time.

Job list box with g-code

The loaded g-code file is listed here. It is a special list box made to improve performance, a
g-code file can be millions of lines. Therefor we have no standard scrollbar, but buttons:
To begin / End of job
09 November 2018

Release 4.03

EDING CNC

Manual

Previous / Next line (+ctrl key 25, +shift key 100, both 1000)
Show nr of lines, click to set
line or search. Search runs
the interpreter up to given
line allowing to start from
there. This is shown in the
graphic.

2.1.25 Reset Button F1
This button has to be used after starting the software to enable the drives.
The amplifiers are switched on when pressing the reset button. Try this, you can feel at
the motor shaft if the amplifier is on. if you can still turn the motor by hand, you probably
need to reverse the amplifier enable polarity in the setup.
But the reset button does more:
• Enable the amplifier
• Recover from Error after you get one
• Stop a running program

2.1.26 Escape Button
This button pauses the current job execution if running.
This is just there for convenience, not for safety emergency stop.
For safety use a real E-STOP button!

2.1.27 The menus
2.1.27.1 MAIN MENU

The Main menu looks like this and has a user selectable logo at the right:

•
•
•
•
•
•
•
•
•
•

F1 reset, this key comes back un every sub menu
F2, to home menu.
F3, to zero menu.
F4, to auto menu.
F6, manual data input (ctrl-f6 works always too for MDI)
F7, machine I/O functions for spindle and coolants.
F8, graphic manipulation functions.
F9, jog with keyboard or hand wheel mode.
F10, jog pad for jogging by mouse or touch screen.
F11, user menu

2.1.27.2 HOME MENU

•
•
•
•
•

F1, reset
F2 - F7, Home X - Home C
F8, Home all axes
F10, go to g28 park position
F11, go to g30 park position

09 November 2018

Release 4.03

EDING CNC

Manual

• F12, return to main menu.
For homing setup see homing and coordinate systems chapter.
2.1.27.3 ZERO MENU

•
•
•
•
•

F1, Reset
F2 - F7, zero x - zero c
F8, zero all
F9, measure rotation and apply G68 R..
F12, back to main menu

F9 measure rotation is a feature that makes life easy. It automatically corrects your
work piece/clamp for rotation. This means that you no longer have to spend time to
setup your clamp / material very accurately, EDINGCNC will automatically correct for
you.

2.1.27.4 AUTO MENU

•
•
•
•
•
•
•
•
•
•
•

F1, Reset
F2, Load G-Code file
F3, redraw (re-render whole program through g-code interpreter)
F4, run/pause
F5 rewind job
F6 start editor
F7 start a job somewhere given a line number. (e.g. after a tool breakage).
F9, +Feed Override, with ctrl pressed +Speed override
F10, - Feed Override, with ctrl pressed –Speed override
F11, Show Nesting options.
F12, back to main menu

G28:
G30:

Perform G28 when the program finishes.
Perform G30 when the program finishes.

ArcF %:

Reduce Feed for large Arc’s.

Single:

Activate single step mode, when F4 (Start) is pressed, only 1 line of the
job file is executed.

BlockDel:

When active all lines with '/' in front will not be executed.

M1Stop:

Optional stop M1, when an M1 is encountered in the g-code the program
will halt if this check is on.

Sim:

Simulation mode.

FastRtGraph:
The Real-time graph will not consume memory, use it when running long
programs (several hours or more). This function is also automatically
09 November 2018

Release 4.03

EDING CNC

Manual
activated when the file size of the job is bigger than LongFileModeCriterion
in the setup.

Fast Rendering: Also for very long programs, only the outlines (rectangle) of the part
are drawn. This is also automatically activated when the files size is longer
than SuperLongFileModeCriterion.

For loading a G-Code file in a production environment a QR Scanner can be used that
scans the file name.
We support this type:

Datalogic QBT2400

Some configuration is in the CNC.INI file, the device is connected with USB and can be
seen in device manager as COMx port, this port number is set in the CNC.INI file under
[USERINTERFACE]
..
QrScannerComportNumber = x
..
If x is set to zero, the Qr Scanner is not used.

09 November 2018

Release 4.03

EDING CNC

Manual

F7, GOTO line will give next popup dialog:
Use this functionality to start at given line number or tool change instead of starting
from the beginning.
If you have stopped while Paused, the line number will show the current
line of the job.
This happens also when you have pressed reset when paused.
Not that reset when pause is needed when you need to do e.g. a tool
change.
During Pause only jog movements are allowed.
You can store and retrieve the stored line number using the Store/Get
Stored buttons.
Press search-line to run the interpreter in Search mode up to the given line
number.
Press Search Tool to find a tool change to given Tool Number.
If 0 is used as Tool Number the interpreter will stop at every tool change
when Search Tool was pressed.
The graphic shows the search.

When you press the RUN button (F4) after a search or pause, the following
popup dialog may appear.
It appears only if any axis is not at the correct position or the spindle or
coolants are not correct, it allows you to synchronize the actual situation
with the required situation:
The Z >>> button will start move Z completely up.
The M6 T1 button shows the tool according to the interpreter,
This button is not visible at a start after Pause, only at start after search.
if the color is green the current tool matches the tool from the search
status.
If the color is red, the tool doesn't match and you can start a tool change
by pressing the button.
The Axis button show the position according to the interpreter on the
searched line, green is match, red is no match, press the button to move
the axis to the correct position, you can do this for all axes.
If any axis isn't synchronized, it will be done automatically when the start
button is pressed.
The M8/M7 On buttons allow to switch on the Coolants.
The S button switches the spindle On with correct S value from the Search status.
F= Plunge rate is the feed rate for the movement towards the work piece, you can
change this to a good value you want.

09 November 2018

Release 4.03

EDING CNC

Manual

As last, the Run button, this will start a G1 with F towards the search positions, then
restore the Feed to the search feed and start machining from there.
This way you are able to easily start half way in a g-code program.
For advance users of pause-start there are other options in the cnc.ini under [SAFETY]
;When 1 spindel stops on pause
stopSpindleOnPause = 1
;When 1 automatic start after pause occurs, movement and spindle is switched on.
autoStartAfterPause = 0
;Spindel goes up after pause
zUpOnPause = 0
;By this distance
zUpMoveDistanceOnPause = 10.0
;And this is the approach feed when auto starting in mm/sec.
approachFeed = 2.000000

09 November 2018

Release 4.03

EDING CNC

Manual

F11, Nesting:
Nesting is a feature that allows to produce a product multiple times in X/Y ROWS:
Nesting is reachable if the machine is in READY state, you can always press RESET to
get it in ready state if it isn't.

Material size:
Start offset:
Pitch:
Number:
Max:

set the material size in X and Y, it is shown in the graph.
set an offset for starting, play with it and you will see what it does.
the distances in X,Y of the products.
Specify the number of products.
EDINGCNC will determine the max number of products.

Apply:
Cancel:

Apply the current setting to the program.
Cancel nesting, back to only one product.

The Nest button F11, can be pressed to show/hide the nesting dialog.
Nesting internally uses coordinate system offset G59.3, the coordinate system offsets
may not be used in the program, otherwise nesting will not work, so no G54 .. G59.3
allowed in the program. The G54 offset should be 0.
G92 is allowed, but if changed must be set back to the original value at the end of the
program.
The program must end with M30 otherwise nesting will not work.
Use M60 instead of M30 when the spindle should not stop between the work pieces.
The values above can also be set in the G-Code file like so:
%mx=200
Material size X
%my=200
Material size Y
09 November 2018

Release 4.03

EDING CNC
%dx=200
%dy=200
%ox=200
%oy=200

Manual
the
the
the
the

delta X or pitch X
delta Y or pitch Y
offset X
offset Y

After pressing the Apply button, the nesting is applied to the program and shown:

Recommended is to create the g-code file for the product such that X0 Y0 is at the lower
left side.
If you like to start not at the beginning, use the goto-line function and apply the NX NY
values.
prerequisites
For nesting to work correctly, this must be taken into account:
• The lower left corner of the workpiece g-code should be at or near X0 and Y0.
• The program cannot use any coordinate system offsets G54 .. G59.3.
• G54 should be active and G54 offsets should be 0.
Happy production with Nesting!

09 November 2018

Release 4.03

EDING CNC

Manual

2.1.27.5 IO MENU

•
•
•
•
•
•
•
•
•
•

F1, Reset
F2, drivers on/off
F3, spindle on/off
F4, spindle direction left/right
F5, flood coolant on/off
F6, mist coolant on/off
F7, aux1 output on/off
F9, Speed F10, Speed +
F12, back to main menu

2.1.27.6 GRAPHIC MENU

•
•
•
•
•
•
•
•
•

F1, reset
F2, show camera view.
F5, switch between 2D X/Y plane and 3D iso-metric view.
F6, zoom fit
F7, zoom out
F8, zoom in
F9, zoom machine
F10, clear
F11, redraw (re-render whole program through interpreter)

The graph view shows a grid of 50mm in mm mode or 2 Inch in inch mode projected
on the machine bed (X-Y surface). For a representative view it is important that the
axes limits are correctly filled in and that the machine is homed manually or automatic.
The current work coordinate system origin is shown as a cyan colored cross in the x-y
plane. When you press the preview update button, a preview is shown of the loaded GCode program. The preview is created by running the entire g-code file through the
interpreter. So when interpreter errors occur, it shows in the log window and in the
operate view the program list box shows the wrong line in red color. Note that there
can be inaccuracy in what the display shows, this is there because of performance and
memory usage limitation reasons.
Zooming, rotate, pan, 2D/3D view and other possibilities are found in the graph submenu, see the example below.
With OpenGL activated in the setup, real-time pan, rotate and zoom is possible with the
mouse also:
pan
: left mouse button
rotate
: left mouse button + control
zoom
: right mouse button.

09 November 2018

Release 4.03

EDING CNC

Manual

2.1.27.7 JOG MENU

•
•
•
•
•
•
•
•
•
•
•
•

F1, Reset
F2, jog mode continuous
F3, jog mode step 0.0001 (Only visible in INCH mode G20)
F4, jog mode step 0.001
F5, jog mode step 0.01
F6, jog mode step 0.1
F7, jog mode step 1
F8, jog mode step user value
F9, jog mode hand wheel / mpg X1
F10, jog mode hand wheel / mpg X10
F11, jog mode hand wheel / mpg X100
F12, return to main menu

2.1.27.8 JOG PAD

Jog by mouse, F12 return to main menu.
The function is similar to the jog menu, but it has some extra functionality with jog step.

09 November 2018

Release 4.03

EDING CNC

Manual

When “Shift Coordinate System” is checked, jog-step functions as normal, the axes move
one step at a time. The work position however remains the same. This is accomplished by
modifying the active G92 offset. It is useful when e.g. during engraving you want to run the
G-Code program again, but a little deeper in Z. E.g. you want to run the program 0.1 mm
deeper, select jog step 0.1 and check “shift coordinate system” . Now press de arrow down
button to move Z 0.1 mm down. Notice that the axis moves down but that the position
remains the same. When you run your engraving program again the engraving will be 0.1
mm deeper into the material.
This option is also very handy during turning. Your program has run and you measure the
work piece and see its diameter is still a bit too big. So now use the –X button to compensate
the diameter. Run the program again and your work-piece diameter will be correct.
The amount of shift is shown at the right side. To reset the value to 0, which has no influence
on the active offset nor machine position, uncheck, and then check “shift coordinate system”.
2.1.27.9 USER MENU

•
•
•
•
•

F1, Reset
F2, Zero the Z coordinate using a flexible tool setter positioned on top of the material,
see ZERO TOOL MACRO chapter.
F3, measure the tool length and put the length in the tool-table using a fixed tool
setter, see TOOL MEASUREMENT MACRO chapter.
F4 - F11, user function user_3 .. user_10, user defined functions in macro.cnc
F12, return to main menu.

09 November 2018

Release 4.03

EDING CNC

Manual

2.1.28 Operate page tasks
2.1.28.1 STARTUP

When you just started the application you have to press reset F1.
This will enable the drives, the machine on button left will be green flashing, this means
the machine is ready but must be homed first.
2.1.28.2 HOMING

Homing is the next step to perform, this can be done via main->f2.
There you can do individual axis homing or home all axes art once.
For homing setup see homing and coordinate systems chapter.
All axes home at once can also be done using ctrl-h or the home all button beside the
status:

2.1.28.3 LOAD AND RUN A G-CODE FILE

After homing we a ready to run a program, we have to load a g-code file for doing that.
From the main menu press F4 (Auto), then F2 (load g-code file).
Go to the cnc-jobs directory and load demo.cnc.
The file is fully parsed through the g-code interpreter and the tool path is shown in the
graphic window:

09 November 2018

Release 4.03

EDING CNC

Manual

Using the mouse (ctrl+left mouse), you can rotate the tool-path and see it 3D.
Using the left mouse, you can PAN. Using the right mouse you can ZOOM:
It can be that while loading you get a collision error, this means that the tool-path does
not fit on the machine, because the work zero point is not at a correct position. he
Cian/Light blue colored line's indicate the Work-Zero point. Jog to the left and set zero X
further to the left using the button besides the X readout is the easiest way to do this.

The yellow rectangle shows the first place where the collision is discovered. We see here
clearly that a part of the tool-path is outside the machine area, a message is given
showing the line number L5 in this case where the collision occurred. The easiest way to
shift now is to jog to the place where you want to have the origin, the ctual place of the
work-coordinate system origin is shown as the cyan lines for X and Y.

09 November 2018

Release 4.03

EDING CNC

Manual

We see that the tool path fits without collision and we see the delta's in X, Y, Z, which is
the size of the tool path.

09 November 2018

Release 4.03

EDING CNC

Manual

F3 is also possible from here, this redraws and zooms to fit:

Now we can press run (F4) to run the program.

09 November 2018

Release 4.03

EDING CNC

Manual

We have no automatic tool changer, so the program stops when a tool change is
encountered asking us to put in the tool.:

The tool is already in, so we press F4 again, the program will continue and our machine
is working.
We see the tool path being drawn real-time on the screen:
If you check the G28 or G30 checkbox, then the machine will return to its G28 or G30
position when the job is done. You can specify those positions in the variables tab.

09 November 2018

Release 4.03

EDING CNC

Manual

2.1.29 Coordinate Page Tasks
2.1.29.1 CALIBRATE/ACTIVATE COORDINATE SYSTEMS

If you move to a position and press one of the calibrate buttons, the associated
coordinate system offset (G54 – G59.3) is set such that the position becomes zero on
this place when activated. See also G10 L20 P.. X.. Y.. Z.. because this is what is
actually executed. Activation of one of the coordinate offsets can be done using one if
the activate buttons, See G54 – G59.3.

09 November 2018

Release 4.03

EDING CNC

Manual

2.1.29.2 MAPPING X/Y G-CODE TO CYLINDER ON A-AXIS

This is useful if you have a 4th axis and want to mill on the outside of a cylinder as if it
was the X-Y plane. You must have setup the A axis as “4THMILL”. This is possible with
a normal XY G-Code file. EDINGCNC will perform the mapping for you. Some calibration
needs to be done to make this work. It is done on the new coordinates page. The
location of the A axis rotation point needs to be set and also the radius of the work piece
needs to be set first.

First we set the location of the A rotation point:
We move by jogging or MDI to the center point of rotation of the A axis, only Z and Y
are important here. Press button "1. Set to current position". Done, center is set.
Next we set the outside radius of the work piece:
There are 2 possibilities to do this: 1. Just type the radius if you know it and press "Set
Radius" Or we second possibility we move the Z up and touch the outside of the
material with the tool bit and press "2. Calibrate Radius".
Calibration is done. First we need to be sure that our Y axis is at the correct position
before we switch on the Y->A mapping. We need to do this now because when the
mapping is ON, Y can no longer be moved, as Y is now mapped to A. You can press
"Move Y to rotation point” to do the movement.
The mapping can be switched on now. Then we can load a standard G-Code file with
XYZ coordinates. Below we see how it looks in the graphic.

09 November 2018

Release 4.03

EDING CNC

Manual

Position the X and the Z where at the zero point of the drawing, so where the milling
should start.
Now Zero all axes in the operate screen
Important: Zero the Z at the top surface of the cylindric material, in this case my
material has a radius of 20 mm, so my Z zero is 20 mm higher as the CenterPoint.
Y to A mapping OFF

Y to A mapping ON

09 November 2018

Release 4.03

EDING CNC

Manual

2.1.29.3 MILLING UN-EVEN SURFACES

Intended use
The compensation is intended for relative small compensation with natural smooth behavior.
The compensation profile is directly added to the motion of the Z axis. The acceleration profile therefore is
determined by the shape of the compensation.
If the compensation is not continuous, then depending of the quantity of it and the speed in which the moves are
done this may lead to position loss with open-loop stepper motor systems or position following error with
closed loop systems.
Milling PCB’s is one example

09 November 2018

Release 4.03

EDING CNC

Manual

The Coordinates TAB will contain the new functionality:

“Start measurement”
will popup an interpreter dialog for the automatics measurement using a toch probe. It is explaned on next page
“Move to start position”
will move X and Y to the first measured position, there where the compensation is zero.
“Save measurement”
Will open a file-save dialog and allows to save the mesurement data.
“Load measurement”
Shows a file-open dialog to load existing measurement data.
“Check measurement”
Wil show some statics of the measured data, the max and minimum correction values and at which place they
are.
“ZheightComp ON”
Wil switch the compensation ON/OFF.
It will be shown in the position read out, the compensation value is shown above the normal work position of Z.

Now you can do normal XY engraving and while the Z is compensated using the measurement values.

09 November 2018

Release 4.03

EDING CNC

Manual

Starting the measurement

You specify the number of measurement in X and Y.
The height to which the probe should move to when going to the next point.
The minimum Z value to which the probe should move to during the measurement
(G38.2).
The size of the grid, distance between the measuring points.
And the feed for the down movement during G38.2. All other moves use G0 for highest
speed.
The measurement starts at WORK X0 Y0. maxZ and Min Z are also WORK coordinates.
The measurement data itself is in motor coordinates, so after the measurement you can
freely zero anywhere else on the work piece.
This is the subroutine to be added in the standard macro.cnc for this purpose.
If you have a self-modified macro.cnc, you can copy from default_macro.cnc to your
own macro.cnc
sub zhcmgrid
;;;;;;;;;;;;;
;probe scanning routine for eneven surface milling
;scanning starts at x=0, y=0
if [#4100 ==
#4100 = 10
#4101 = 5
#4102 = 40
#4103 = 10
#4104 = 1.0
#4105 = 100
endif
#110
#111
#112
#113
#114

=
=
=
=
=

0
0
0
0
1

0]
;nx
;ny
;max z
;min z
;step size
;probing feed

;Actual
;Actual
;Missed
;Number
;0: odd

nx
ny
measurements counter
of points added
x row, 1: even xrow

;Dialog
dlgmsg "gridMeas" "nx" 4100 "ny" 4101 "maxZ" 4102 "minZ" 4103 "gridSize" 4104 "Feed" 4105

09 November 2018

Release 4.03

EDING CNC

Manual

if [#5398 == 1] ; user pressed OK
;Move to startpoint
g0 z[#4102];to upper Z
g0 x0 y0 ;to start point
;ZHCINIT gridSize nx ny
ZHCINIT [#4104] [#4100] [#4101]
#111 = 0
;Actual ny value
while [#111 < #4101]
if [#114 == 1]
;even x row, go from 0 to nx
#110 = 0 ;start nx
while [#110 < #4100]
;Go up, goto xy, measure
g0 z[#4102];to upper Z
g0 x[#110 * #4104] y[#111 * #4104] ;to new scan point
g38.2 F[#4105] z[#4103];probe down until touch
;Add point to internal table if probe has touched
if [#5067 == 1]
ZHCADDPOINT
msg "nx="[#110 +1]" ny="[#111+1]" added"
#113 = [#113+1]
else
;ZHCADDPOINT
msg "nx="[#110 +1]" ny="[#111+1]" not added"
#112 = [#112+1]
endif
#110 = [#110 + 1] ;next nx
endwhile
#114=0
else
;odd x row, go from nx to 0
#110 = [#4100 - 1] ;start nx
while [#110 > -1]
;Go up, goto xy, measure
g0 z[#4102];to upper Z
g0 x[#110 * #4104] y[#111 * #4104] ;to new scan point
g38.2 F[#4105] z[#4103];probe down until touch
;Add point to internal table if probe has touched
if [#5067 == 1]
ZHCADDPOINT
msg "nx="[#110 +1]" ny="[#111+1]" added"
#113 = [#113+1]
else
;ZHCADDPOINT
msg "nx="[#110 +1]" ny="[#111+1]" not added"
#112 = [#112+1]
endif
#110 = [#110 - 1] ;next nx
endwhile
#114=1
endif
#111 = [#111 + 1] ;next ny
endwhile
g0 z[#4102];to upper Z
;Save measured table
ZHCS zHeightCompTable.txt
msg "Done, "#113" points added, "#112" not added"
else
;user pressed cancel in dialog
msg "Operation canceled"
endif
endsub

Milling un-even cylinders with y->a mapping on also works.
In that case the measurement must be done using with y->a mapping on.

09 November 2018

Release 4.03

EDING CNC

Manual

The compensation works only in the measured range. So of the mapping is measured
between 0-360 degrees for A, it will not compensate for e.g. 370 degrees.
The Z height compensation interpreter commands
For your own use if you want to customize the working:
ZHCINIT
This is the first command required before starting a measurement, it will reserve the
correct amount of memory to store the measured points.
ZHCINITEX
Instead of ZHCINIT you can use ZHCINITEX.
The difference with ZHCINIT is that this allows different grid sizes for X and Y.
Using G38.2 will do the actual measurement.
ZHCADDPOINT will add the last measured point to the data.
ZHCS will store the data to a file.
ZHCL will load the data from a file.
ZHC [ON | OFF] will switch the compensation on.
#5151 contains 1 if ZHC is ON and 0 if OFF. This can be used for run time checks if the
compensation is on. In case of tool change, you will probably want to switch it off and
switch it back ON after the tool change.

09 November 2018

Release 4.03

EDING CNC

2.2

Manual

LINEAR PITCH COMPENSATION

This is a way to improve the accuracy of the machine when the linear displacements are
not exactly correct. E.g. cheap rolled ball bearing spindles may have an inaccuracy of
several 0.1 mm at a meter length. Also the pitch may vary a bit depending on the
position. This compensation feature allows to correct this.
The compensation can be switched on by manually editing the cnc.ini file (contains all
settings).
Under each joint settings [JOINT_0] is the first, usually your X axis you find 2 settings:
• pitchCompensationOn = 1 (1 to switch compensation ON, 0 to switch OFF)
• pitchCompensationFileName = "Joint-X-pitchCompTable.txt" (name of the file
with the correction table)
when you switch on the compensation and the compensation table does not exist, one is
created as example for you, it is only an example to show the syntax. You need to adopt
it for your machine.
This is an example of a correction table:
;Pitch correction table for axis X
;This table contains 6 correction points
;machine-position calibrated-Position
0.0000 0.0000
50.0000 50.01000
200.0000 200.02000
300.0000 300.03000
400.0000 400.04000
500.0000 500.05000
The left value is the position of the machine.
The right value is the calibrated position that you have obtained by measuring it.
The table must be sorted, small to big values. Note that 0 is bigger than -100, so if you
have negative numbers the highest negative number comes first.
You can make the compensation value visible by checking Show in DRO on the
coordinates window. You will see this in the DRO:

The small number above the position shows the actual compensation value.

09 November 2018

Release 4.03

EDING CNC

2.3

Manual

XY NON RECTANGULAR CROSS COMPENSATION

This is a way to compensate the non-accuracy of the machine when the X and Y axis on
the machine are not exactly square/rectangular. By compensation the Y axis depending
on the position of the X axis and vice versa, this can be compensated.
The compensation can be switched on by manually editing the cnc.ini file (contains all
settings).
Under each joint settings [JOINT_0] is the first, usually your X axis you find 2 settings:
• crossCompensationBaseAxis = 1 (-1 = off, 0 = X base axis 1 = Y base axis)
• crossCompensationFileName = "X-pitchCompTable.txt" (name of the file with
the correction table)
when you switch on the compensation and the compensation table does not exist, one is
created as example for you, it is only an example to show the syntax. You need to adopt
it for your machine.
This is an example of a cross correction table for the X axis.
So this is compensating the X depending in the position of Y.
;XYCross correction table for axis X
;This table contains 10 correction points
;machine-position-Y-axis correction-value-X-axis
-600.0000
-0.0600
-500.0000
-0.0500
-400.0000
-0.0400
-300.0000
-0.0300
-200.0000
-0.0200
-100.0000
-0.0100
0.0000
0.0000
100.0000
0.0100
200.0000
0.0200
300.0000
0.0300
400.0000
0.0400
500.0000
0.0500
600.0000
0.0600
The
The
The
you

left value is the position of the machine, in this case the Y axis
right value is the compensation value for the X axis.
table must be sorted, small to big values. Note that -500 is bigger than -600, so if
have negative numbers the highest negative number comes first.

You can make the compensation value visible by checking Show in DRO on the
coordinates window. You will see this in the DRO, this matches the example table above,
as you see, the Y position equals -250 and the X compensation value here is -0.025

The small number above the position shows the actual compensation value.
Note: the interpreter command Crosscomp on switches the compensation on. You can
add it at the end of the home_all subroutine inside macro.cnc.
09 November 2018

Release 4.03

EDING CNC

2.4

Manual

SPEED-PWM COMPENSATION

The speed for a spindle is controlled by the PWM output.
The PWM is converted to an analogue signal which is fed to the VFD (Variable frequency
drive). There are often non linearity’s involved.
This cause that the programmed speed and the real speed does not match correctly.
This software feature allows to compensate this.
The compensation can be switched on by manually editing the cnc.ini file (contains all
settings).
Under each spindle settings [SPINDLE_0] is the first, usually your main spindle (M90)
axis you find 2 settings:
• pwmCompensationOn= 1 (1 to switch compensation ON, 0 to switch OFF)
• pwmCompensationFileName= " Spindle-0-pwmCompTable.txt" (name of the
file with the correction table)
when you switch on the compensation and the compensation table does not exist, one is
created as example for you, it is only an example to show the syntax. You need to adopt
it for your machine.
This is an example of a correction table:
;Speed PWM calibration table for spindle 0
;This table contains 15 correction points
;Speed PWM Percentage
0.00
0.00
720.00
8.00
1146.00
10.00
3468.00
20.00
5832.00
30.00
6000.00
31.00
8280.00
40.00
10740.00
50.00
13260.00
60.00
15780.00
70.00
18000.00
79.00
18120.00
80.00
21060.00
90.00
24000.00 100.00
The number on the left side is the Spindle Speed and on the right side the required PWM
value 0-100%.
You can see the PWM value in the IO screen and you can make it also visible at the
main screen instead of the programmed speed.
The setting is under [USERINTERFACE]
;0=programmed speed, 1=PWM value, 2=analogIn1, 3=analogIn2, 4=analogIn3
• showInProgSpeed = 1
• showInProgSpeedAnaMulFactor = 1.0000

09 November 2018

Release 4.03

EDING CNC

Manual

As you can see you can also choose to show an analogue input with a multiplication
factor, this can be used when the spindle has a power used signal.

09 November 2018

Release 4.03

EDING CNC

2.5

Manual

AUTOMATIC VACUUM SECTIONS

Large machines may have several vacuum sections which can be switched on
individually.
EdingCNC supports up to 64 vacuum sections.
During loading/rendering of the g-code file, the software automatically detects the
sections on which the operation stakes place.
These are special interpreter commands for the vacuum:
Vacuum ON:
Switches on all vacuum sections and related pumps.
Vacuum OFF:
Switches off the vacuum sections and pumps.
Vacuum ADD:
Add section under current position.
Vacuum CLEAR:
Clear all used sections.
The configuration of this is done by editing the CNC.INI file.
We will add this later in the GUI when our new GUI development is ready.
The first time, there will be only this in the CNC.INI:
[VACUUMBED]
automaticMode = 0
numberOfSections = 0
Note always close the software when making changes in the CNC.INI file.
Then set the number of sections required.
Start the software, then close the software, now the parameters for the sections
appear:
[VACUUMBED]
automaticMode = 1
numberOfSections = 2
section_1_OutputID = 0 ;0: NONE, 1-10: AUX1-AUX10, 101-108 GPIO CARD 1
OUPUT 1-8
sectionPump_1_OutputID = 0 ;0: NONE, 1-10: AUX1-AUX10, 101-108 GPIO CARD 1
OUPUT 1-8
section_1_XPosition = 0.000000
section_1_YPosition = 0.000000
section_1_XWidth = 0.000000
section_1_YWidth = 0.000000
section_2_OutputID = 0 ;0: NONE, 1-10: AUX1-AUX10, 101-108 GPIO CARD 1
OUPUT 1-8
sectionPump_2_OutputID = 0 ;0: NONE, 1-10: AUX1-AUX10, 101-108 GPIO CARD 1
OUPUT 1-8
section_2_XPosition = 0.000000
section_2_YPosition = 0.000000
section_2_XWidth = 0.000000
section_2_YWidth = 0.000000
You will need to specify the location and size of each section in machine coordinates.
Then each section has 2 associated outputs, the valve and the pump output. More sections can have the same
pump output.

09 November 2018

Release 4.03

EDING CNC

2.6

Manual

PROGRAM PAGE, DXF AND HPGL IMPORT

EDINGCNC uses a build in CAD/CAM library for these advanced import
functions. You can load a file and then perform one of these operations:
Loads a DXF or HPGL file
Select engraving, this is milling over the lines from the
drawing.
Drilling, draw points in the DXF file to use this.
Select profiling, this is for milling out objects and taking
the tool diameter into account. (*)
This is for pocketing, to mill out the complete object.
(*)
(*) these options may not be available.
After loading a DXF file, all layers will be visible. You can unselect layers
at the right side, such that you see only the part that you want to use.
You also can change the origin of the drawing by pressing the appropriate
09 November 2018

Release 4.03

EDING CNC

Manual

button under the layer selection list box. The positions of the buttons give
the positions of the origin. So e.g. when you press the upper right button,
then the most upper right position of the drawing will become x=0, y=0
when milling.
The DXF import supports:
- Lines
- Arcs
- Circles
- Poly lines with arcs
- Points for drilling
The workflow of using these features is:
1) Load drawing
2) Select the correct layers
3) Apply origin offset if wanted
4) Set correct parameters
5) Calculate tool path
6) Save tool path and optionally immediately load it for milling.

Parameters involved:
Save-Z
Start-Z
Final-Z
Z
Increment
Feed rate
Plunge rate
Spindle
speed
CW/CCW
Tool
number
Tool
Diameter
Method
Finish
allowance.
Step size

When moving from one region to another, the machine
goes to this height.
Z value where the tool touches the material to be
machined.
Z value specifying the milling depth lowest Z value.
Final Z must be lower than Start Z.
This specifies the step size when machining in passes.
Milling feed (F) in mm/min
Feed (F) that the Z moves down into the material also
mm/min
S value for spindle.
Spindle direction (M3/M4)
This is only used for the M6 tool change command
Diameter of the tool for the offset and pocketing
calculations.
Outside/inside/clockwise/counterclockwise operation
Material that is left for the finishing pass when
pocketing. This finishing pass is at full depth for
getting a clean edge.
Step oversize for pocketing, this value should be lower

09 November 2018

Release 4.03

EDING CNC

Manual

than the tool diameter.
For profiling, when switched on, the tool will be
switched off when moving from one region to another.
Make
Leave small pieces of material, that prevent you object
bridges
from falling out (and get damaged) when profiling.
Bridge
Approx distance, the exact distance is calculated such
distance
that all bridges have equal distance.
BridgeFinal Lowest Z value for bridge, this value should be
Z
between startZ and finalZ
BridgeWidth The width of a bridge.
Laser mode

When the parameters are set, press calculate tool path, it will be
visualized on the screen.
Here an example of profiling with bridges:

Note: The offset and pocket calculation might not always work, this is
usually because of small errors in the drawing like lines over each other
or not connecting lines. Experimenting with the Calculation Accuracy
might help. Also check/correction of your drawing may help.
The engraving function is robust and will always work.

09 November 2018

Release 4.03

EDING CNC

2.7
2.7.1

Manual

TOOLS PAGE
Milling

In this view you can define 99 tools with a Z-Offset(length) ZDelta (Delta
due to Wear in Z length), diameter and description. The tool information
is used when you use the tool radius and or tool length compensation
functions of the G-Code interpreter
commands (G40 – G43). See chapter 3.6. and further.
ZDelta is new and can be used e.g. if you see that you haven’t milled
deep enough, simple set a negative value to ZDelta and you run the
program again. G43 must be active to use this.

09 November 2018

Release 4.03

EDING CNC

2.7.2

Manual

Turning

As you can see, there are additional parameters for turning, X-Offset XDelta and Orientation.
2.7.3
Tool change
A tool change is performed in G-Code by M6 Tx where Tx is the new tool
number. Tool number 0 means no tool.
Normally the program is stopped on a tool change, with a user message
to change the tool, pressing run again will continue the program. If you
don’t want the program to stop, check AutoToolChange in the automatic
menu bar. This setting is saved when you press save INI file in the setup
screen.
2.7.4
Automatic user defined Tool change ATC
When you want to define you own tool change cycle, you can edit the file
“macro.cnc” in the EDINGCNC directory. When an M6 Tx is encountered,
this is translated to a GOSUB of subroutine change_tool in the
“macro.cnc” file. This subroutine then calls further subroutines
drop_tool_x and pick_tool_x, if you have a tool changer, you can add
extra movements to the right tool position and control I/O for actually
changing the tool.
09 November 2018

Release 4.03

EDING CNC

2.7.5

Manual

Changing the tool number without actual tool change

During installation and manipulation of tools it is possible to the change actual
tool number like this:
#5011 = 1 ;New actual tool number
M6 T#5011 ;Change the tool in the software without calling the change_tool
macro.

2.7.6

The variable Page

This page shows the standard variables used by the G-Code interpreter.
It also contains 4 watches to show your own variables if you are going to
use the extended programming features. You will understand the
meaning of this window after reading the G-Code interpreter functions
and extended programming with variables.

The G68 rotation can be reset with the reset button under G68 Rotation.
This is the same as entering G69 in MDI.
The G54 .. G59.3 offsets can be set by entering values and pressing enter.
The G54.. G59.3 X,Y values can be defined as zero at current machine position by
pressing the button. This works similar to G92 offset.
The MDI equivalent for setting G55 offsets is G10 L20 P2 X0 Y0.
09 November 2018

Release 4.03

EDING CNC

Manual

G92 is normally used for zeroing the machine at work piece coordinates. you can reset
all offsets here to zero. The G28 and G30 positions can be defined at current location by
pressing the associated button.

09 November 2018

Release 4.03

EDING CNC

2.8

Manual

IO PAGE

At this page you can monitor and set the I/O signals for CPU and IO extension board if
attached. You can see that the GPIO extension board signals can be given a more
meaningful name to your application. Note that this page shows the RAW IO values for
the digital IO and does not take inversion into account.
The internal GPIO (AUX) can be controlled by M54, M55, M56, e.g. M54 P1 switches
output AUX1 on and M55 P1 switches output AUX1 off.
The external GPIO can be controlled also by M54, M55, M56, e.g. M54 P101 switches
output 1 of card 1 on.
These M-Codes are further explained in the M Codes chapter of this document.

09 November 2018

Release 4.03

EDING CNC

2.9

Manual

SERVICE PAGE

At this page shows how much your machine is operated and if it needs service.
You can see:
Service status
Job time service :

It shows the number of hours the machine has
performed jobs.
Job distance:
The distance the machine has milled in meters.
Number of jobs done service: The number of jobs done.
These values can be reset to zero when the machine gets service with the reset button.
Machine working status
Job time total : It shows the number of hours the machine has performed jobs.
Job distance total:
The distance the machine has milled in meters.
Number of jobs done total:
The number of jobs done.
These values cannot be reset, it shows the total usage of the machine.
Service parameters
Service Time interval:
Service distance interval:

09 November 2018

The time interval for the service, the software will give
a message when this is passed at the end of a job.
The traveled distance for service. Also here the
software will give a message to indicate the machine
needs service.

Release 4.03

EDING CNC

Manual

Pump parameters (For Automatic machine oiling system)
Pump Interval Time :
Time in seconds between pump actions.
Pump pulse Time:
Duration of one pump action.
PumpTimeToNext:
Time to next pump action, read only.
Pump Output:
Output used for PUMP, set to NONE for no pump
action.
Save changes:

09 November 2018

Wil set the Pump Time To Next to 5 seconds once for
testing. After that every Pump Interval Time.

Release 4.03

EDING CNC

Manual

2.10 UTIL PAGE, CHIPLOAD AND FEED/SPEED

This page allows to calculate the right Feed/Speed for milling.
Chip load is the quantity of material that is removed by one teeth of the milling tool.
This is the most important parameter for calculating the feed given a Speed.

09 November 2018

Release 4.03

EDING CNC

2.11

Manual

HOMING AND COORDINATE SYSTEMS

As I am like most people and don’t want to read a comprehensive manual, but
start right away. So I have written this little tutorial, it explains how to home
the machine and use the coordinate systems in a simple way. This part is very
important to read, you will have better experience with the machine if you use
the coordinate systems the right way!
When your machine is switched on, all axes can be at any position, these
positions are unknown by the software. The software however needs to know
the position to show a correct graphic in the graph screen and also for
preventing damage to your machine by running beyond the machine limits. The
process to match the machine position with the software is called homing.
Homing can be done either manually or automatic if end of stroke switches are
mounted. This tutorial describes homing.
Here are the homing buttons, F2 from the main menu.

With F2 .. F4 the X..Z axes can be homed individually.
With F8 and the button beside the Feed Speed window, the home sequence can
be started to home all axes in a sequence.
F11 is the same as the button besides the %100 feedOverride display.
What happens is that a few subroutines are called. The subroutines are in the
macro.cnc file in your EDINGCNC installation folder. They look like this:
;Homing per axis
Sub home_x
09 November 2018

Release 4.03

EDING CNC

Manual

home x
Endsub
Sub home_y
home y
Endsub
Sub home_z
home z
Endsub
;Home all axes, uncomment or comment the axes you want.
sub home_all
gosub home_z
gosub home_x
gosub home_y
endsub
A good reader has seen that the order of homing is defined by the home_all
subroutine and can be customized to your own needs.

2.11.1 Manual homing the machine
Homing is the first thing you always do after switching on the machine, I
recommend making a habit of it. Suppose your machine limits are:
X: +300 mm and -300 mm
Y: +200 mm and -200 mm
Z: +100 mm and 0 (0 is the bottom surface of the bed)
Set the Home velocity to 0 for all axes that have no EOS switch.
Mark a point somewhere on the machine that you want to use as home
reference point, let’s say X= -200.0mm, which is 100.0mm from the left edge
and Y= -150, which is 50.0 mm from the lower edge. For Z we take to bottom
of the bed at Z=0 mm. This position x=-250, Y=-150, Z=0 is entered in the
Home Position values in the set up screen, this need to be done once.
Using the arrow keys, jog the X,Y axes to the marked position on the bed and
move the Z completely up to the surface of the machine. When the machine is
at the position press the Home button in the Home submenu, F2-F7 for X-C.
Be sure that you have set the home velocities of the axes to zero, otherwise the
axes will start to move. Now click the buttons X, Y, Z, and A if you have an Aaxis. That is all, the axes are now homed and the software now knows the
machine position.
As a side effect, now also the software limit switches are enabled which protect
you from jogging further than the machine can go. Also the Software limit guard
is on that will stop a running program when going beyond the limits.

09 November 2018

Release 4.03

100

EDING CNC

Manual

You may also have noticed that the position mode is set to “machine”, this is
because homing directly affects the machine coordinate system. From this point
the machine coordinate system, is not changed any more, it stays as is.
HINT: Move your machine always back to the home position if you are done
with the machine. You don’t have to move manually to this point next time
when you switch back on the machine. You can do a fast move in machine
coordinates like this: g53 g0 x0 y0 z0, or first undo the preset (preset dialog,
undo preset) and then do a regular G0.
Another possibility to move quickly to the home positions is using g28,
In the variable window set G28 home positions to the same value as the home
positions in the set up window. Now you have to type only g28 to go to the
home position.

2.11.2 Automatic homing the machine and HomeIsEstop
The machine needs a homing sensor or switch for each axis connected the its
home input on the CPU board.
The homing switch is placed at a small distance of the mechanical end of the
machine. This distance is needed to ramp down the velocity after the switch is
activated.
The sensor should be mounted such that it remains active until the mechanical
limit of the machine.
For automatic homing the home velocity needs to be set to another value than
zero, use an equal or lower speed than the axis maximum speed. The axis
should start to move in the direction where your homing switch is mounted,
when it is needed to reverse the direction add a minus sign to the homing
velocity. Setup the HomeInputSenseLevel correctly. When the home input
led’s on the IO screen are grey when the input is not activated put a 1 here,
when the led’s are yellow when the switch is not activated, put a 0. This
depends whether you have used normally open or normally closed switch. I
recommend normally closed switches here.
Use the homing sub menu to home your axes.
1st Move: The machine first moves until the switch activates, then ramps down
and stops.
2nd Move: Then the direction reverses and ramps down when the switch
releases.
At the moment of the release of the switch, the position is captured and used to
set your machine position correctly.

09 November 2018

Release 4.03

101

EDING CNC

Manual

2.11.3 Tandem axes homing
Tandem axes, one main axis has 2 motors, the correct SlaveMode is set here.
For this mode, the slave and master must each have a homing sensor.

Also modify the macro.cnc because this contains the homing sequence, in this
example A is slave of X.
Sub home_x
homeTandem X
Endsub
And home_a contains nothing:
Sub home_a
Endsub
Note that sub routine home_all remains unchanged.
For tandem axes these special interpreter commands also exist, use them for
testing the sequence if you need, this is what homeTandem is doing in
separate steps. Use them in MDI for testing and understanding.
1. PrepareTandemHome X, Both slave and master are moved towards the
home sensor. The axes stop when both axes are on the sensor. When one
axis reaches the home sensor first, this one is stopped and the other
moves further. This movement is done when both axes have reached the
sensor.
2. Home X, home the X, the slave will just follow. The X home sensor is
used. Because the X is already are on the sensor, the move will be
towards the machining area off the sensor. The position is latched at the
moment the sensor de-activates. Then the movement stops and then the
correct position is calculated end set for the X.
3. Home A, exactly the same, but now the A Home sensor used and the A
position is set. When done, A is no longer a slave because the position is
different with X. Next command will make de master slave-coupling
again.
09 November 2018

Release 4.03

102

EDING CNC

Manual

4. At this point both master and slave have a correct known position but
probably different. It can be equalized by moving the slave axis to the
position of the A axis. This is done by command MoveSlaveToMaster A.
The slave will move to the same position as the master. The bridge is set
straight and we are done. (If the bridge is not straight, adjust the home
positions in the setup).

09 November 2018

Release 4.03

103

EDING CNC

Manual

2.11.4 Work versus Machine coordinate system and zeroing
The machine coordinate system does not change, however we want to be able
to do the milling of our part anywhere we want on the machine. We will
normally use the “work” coordinate system, we can shift it anywhere we want.
This can be done with several G-Codes, which are explained in chapter 3, it can
also be done using the “preset” button on the operator screen, we’ll see this in a
minute.
Suppose our g-code file containing the work piece is created with an origin of
X=0, Y=0, Z=0. This is because you have drawn your part in a CAD program
beginning from these coordinates and then converted to G-Code.
Now you have put your raw material somewhere on the machine, probably not
at coordinates X=0, Y=0, Z=0.
By the way, I prefer to define the upper surface of the material as Z=0, such
that a negative Z value goes into the material.
Just move to the zero point of the work piece and there press the zero buttons
in the operate screen besides the position display.
For the advanced users: The zeroing can also be done using a measuring probe
connected to the probe input. An example is provided in the standard macro.cnc
file. Under user_1 you find automatic zeroing. Under user_2 you find interactive
tool length measurement.
If you want to do it a more advanced way, look at G55 .. G59.3 and also at the
G92 variants.
When homing and zeroing is performed, the milling can start:
When the program is loaded, go to the graphics screen (Alt-g) and press update
preview, you will now see exactly where the part is going to be milled at the
surface of you machine bed.
Now press the F4 key or the run button to start milling, go to the graphic screen
and switch real time graph on to see what the machine is doing.
That’s all for this tutorial, happy milling!

09 November 2018

Release 4.03

104

EDING CNC

Manual

2.12 3D PRINTING
In the setup you can select is3DPrinter at interpreter settings.
This changes the A Axis into an E axis for Extruder.
The operate screen looks slightly different:

On the left side you see controls for the 3D printer:
WP Cooler fan: Controls the speed of the cooler fan that is cooling the work
piece. For Extruder and Bed temperature, you see the temperature setting and
the actual temperature. The temperature setting can be modified on the fly.

09 November 2018

Release 4.03

105

EDING CNC

Manual

An additional TAB 3D printer shows further controls of the temperature and FAN
of the 3D printer:

There are 2 equal parts for Extruder and Heat bed control and a slide to adjust
the cooler Fan for the work piece. The temperature is read from analog inputs of
the CPU and the Heat and Fan power is controlled by PWM outputs.
The temperature is controlled by a PID controller in software, KP, KD and KI are
the PID parameters.
KP: The output power is linear wit KP * temperature difference (set pointactual). By using the KP alone and leaver the KSD and KI zero, you can tune
the behavior of the system to keep the temperature stable within a small band.
The temperature should be reached in time.
If you get temperature overshoot or oscillation, your KP is too high.
KD (differential), the output power is linear with the derivative of the difference,
it looks at changes in temperature and compensates for that. It is not used
often but can obtain a more accurate control.
KI is to compensate last differences between set point and actual that cannot
be obtained with KP/KD.
Max Integrator power is the max power addition that the integrator function
can deliver.
Temp reached window , when the difference between the set point and actual
temperature is less than this value, the temperature is considered reached.

09 November 2018

Release 4.03

106

EDING CNC

Manual

Max power is the total maximum power that the system. will give to its PWM
output.
Max temp is a safety value when this temperature is reached the power is
switched off.
Standby temp, is activate when the system is put in standby mode.
Temp Reached turns green when reached.
PID on/off switch the PID control system OFF.
On/Off when checked you can directly control (to test) the actual power from
1-100%.
Standby activates the standby temperature.
M1
:All heating and Fans off
M104 S :Set extruder temperature, (M104 S50, sets temperature to 50
degree Celsius).
M106 S.. : Work piece cooling FAN ON optionally with S=0-255, for 0-100%
PWM
M107
:Work piece FAN off .
M109 S.. :Set extruder temperature and wait until reached.
M143 S.. :Maximum Hot-end temperature to prevent overheating.
M140 S.. :Bed temperature
M143 S.. :Set max extruder temperature
M190 S.. :Set Bed temperature and wait until reached.
All other un-useful or unimplemented special M functions are ignored.
A logging file for the temperature and power can be generated using interpreter
command: TempLog
The file can be graphically shown by gnuplot.
This script shows the extruder temperature and power, you can put it into a file
like “plot_temperature.plt” and open it with gnuplot:
set key autotitle columnhead
set ytics nomirror
set y2tics
set xlabel 'time'
set ylabel 'temp'
set y2label 'power'
#plot extruder act and set temperature and power
plot 'templog.dat' u 1:2 w l, "" u 1:3 w l, "" u 1:4 w l axes x1y2

09 November 2018

Release 4.03

107

EDING CNC

Manual

2.13 KEYBOARD SHORTCUTS
Besides the already explained keys for jogging etc, there are a few extra, these are
special for pendant builders.
Function
Control Q
Control TAB, Control shift TAB
Alt+O

Key
Quit program
Mode selection operate/coordinates/Program ..etc
mode operate

Control V, Control shift V
Control W
Control F6

Status tab next, previous
Toggle Work/Machine coordinates
toggle MDI

Alt
Alt
Alt
Alt
Alt
Alt
Alt
Alt
Alt
Alt
Alt

Main menu
Home menu
Zero menu
Auto menu
Machine IO menu
Graphics menu
Jog menu
Jog Pad
User 1 menu
User 2 menu
User macro 1 – User Macro 20

F1
F2
F3
F4
F7
F8
F9
F10
F11
F12
1,2,3 .. 0, Ctrl+Alt 1,2,3 .. 0

Control
Control
Control
Control
Control
Control
Control
Control

R
H,
1
2
3
4
5
6

Control
Control
Control
Control
Control
Control
Control
Control
Control
Control
Control
Control

+
+
+
+
+
+
+
+
+
+
+
J,

Alt
Alt
Alt
Alt
Alt
Alt

+
+
+
+
+
+

shift
shift
shift
shift
shift
shift

Reset
Home all
Zero x
Zero y
Zero z
Zero a
Zero b
Zero c
shift + A
shift + B
shift + C
shift + X
shift + Y
shift + Z
Alt + N
N
O
P
shift + N
+ shift J

Handwheel on A
Handwheel on B
Handwheel on C
Handwheel on X
Handwheel on Y
Handwheel on Z
Handwheel X0.1
Handwheel X1
Handwheel X10
Handwheel X100
Jog continue (Handwheel mode off)
Jog mode up, jog mode down

+
+
+
+
+
+

Select
Select
Select
Select
Select
Select

JOG
JOG
JOG
JOG
JOG
JOG

A
B
C
X
Y
Z

Select
Select
Select
Select
Select
Select

JOG
JOG
JOG
JOG
JOG
JOG

Speed Low
Speed Med
Speed High
Step 0.01
Step 0.1
Step 1

A
B
C
X
Y
Z

Control+Alt+Shift+O
Control+Alt+Shift+P
Control+Alt+Shift+Q
Control+Alt+Shift+R
Control+Alt+Shift+S
Control+Alt+Shift+T

09 November 2018

Release 4.03

108

EDING CNC

Manual

Alt+Shift+P
Alt+Shift+N
Alt+Shift+S

Start Jog+ selected axis
Start Jog- selected axis
Stop Jog

Control I
Control G, +shift
Control T
Control + B
Control F, +shift
Control S, Control + shift + S
Control+Alt+S
Control+Alt+F
Alt+Shift+O
Control+Alt+Shift+A
Control+Alt+Shift+E

Load g-code file
Run, Pause
Toggle Single line
Toggle Blockdelete
+Feed, -Feed
+Speed, -Speed
Speed override 100%
Feed override 100%
Open Teach
Add Point
Edit

Control D, Control + shift D
Control E, Control + shift D
Control K
Control L
Control M
Control+Alt+Shift+1
Control+Alt+Shift+2
Control+Alt+Shift+3
Control+Alt+Shift+4
Control+Alt+Shift+5
Control+Alt+Shift+6
Control+Alt+Shift+7
Control+Alt+Shift+8
Control+Alt+Shift+9

Spindle On right, Spindle Off
Spindle On left, Spindle Off
Toggle Flood
Toggle Mist
Toggle Aux1
Toggle Aux1 out
Toggle Aux2 out
Toggle Aux3 out
Toggle Aux4 out
Toggle Aux5 out
Toggle Aux6 out
Toggle Aux7 out
Toggle Aux8 out
Toggle Aux9 out

Control F1 - control F12

reserved

09 November 2018

Release 4.03

109

EDING CNC

Manual

2.14 ZERO TOOL MACRO
User button 1 contains gosub zero_z, explained here:
;* #4995 = ... ;(Variable tool setter height for zeroing Z, used in zero_z)
#4995 = 43

;set value for compatibility with previous macro.cnc, the tool setter height change if needed

Sub zero_z
if [[#5380==0] and [#5397==0]] ;do this only when not simulating and not rendering
msg "user_1, Zero Z (G92) using tool-setter"
(Start probe move, slow)
f30
g53 g38.2 z[#5103 + #4995] ;Probe move, not below variable tool setter height
(Move back to touch point)
g90 g0 z#5063
(Set position, the measuring device is 43mm in height, adapt for your measuring device)
G92 z#4995
(move 5 mm above measuring device)
g91 (incremental distance mode)
g0 z5
g90 (absolute distance mode)
endif
Endsub

The idea is to use a flexible position tool setter and put it on top of the workpiece.
Start this function and when done, the Z coordinate is set to 0 at the surface of the
workpiece.
The feed is set slow F30. A probe move G38.2 is started towards -Z, when the tool
setter is touched the position is stored and the movement is stopped. The machine
moves exactly to the touch point.
G92 is used with a Z value that specifies the height of you tool setter 43 mm in this
case. Change to match your tool setter. An incremental movement is started 5 mm
upwards, so you can remove the tool setter. The machine goes back to absolute mode
and is done.
The if statement around the code makes that the macro does nothing in simulation
mode and rendering. (Rendering is when the interpreter runs fir the graphics/limit check
after loading a job)
WARNING: Take care that you fully understand this macro before using it and that you
have adapted it for your own tool setter.

09 November 2018

Release 4.03

110

EDING CNC

Manual

2.15 TOOL MEASUREMENT MACRO
Under user menu button 2 you'll see this:
;Tool length measurement example
Sub user_2
goSub m_tool ;See sub m_tool
Endsub
The user 2 button calls subroutine m_tool.
This subroutine needs a few values that are stored:
#4996,
#4997,
#4998,
#4999,

Z coordinate at tool change safe height
X coordinate for tool change
Y coordinate for tool change
Z coordinate at tool length equals zero or calibration tool height.

Tool #99 is used as reference tool and should have filled in its tool length before
you start. This tool length can be 0 if you use the tool-chuck itself instead of a
calibration tool.
The values #4996 .. #4999 are to be determined once. This can be done using
the calibrate_tool_setter function below. Make sure the machine is homed
before you start this.

This routine calibrates the safe height, the XY position, the exact height of the
tool setter. The positions are stored into persistent variables #4996 - #4999.
The positions are used by subroutine m_tool that is under user button 2.
Your action
1.Open MDI and type :
gosub
calibrate_tool_setter

Machine message

Press enter to execute.
(Start the calibration
procedure)

09 November 2018

Release 4.03

111

EDING CNC

Manual

2.Close the MDI
window using F6,
Go to the tools tab and
check the tool length
of tool 99. For me it is
0 because I use the
tool chuck without
calibration tool.
Press save changes.
and go back to the
operate tab.
(tool 99 is used as
calibration tool, set
length correctly,
normally this would be
zero, or if the
calibration tool has a
defined length, set that
length)
3.The program is still
inside subroutine
calibrate_tool_sette
r.
Press RUN to continue.
(Calibration length is
set correctly in tool
table)
4.Do what the
message says:
Jog Z to safe height.
In my case this is
completely up.
Press RUN to continue
(This calibrates the
safe height)
5.Do what the
messages says:
Insert the calibration
tool if you have one, or
just leave the tool
chuck empty.
Jog using X, Y, Z just
above the tool setter.
When done jogging,
press RUN.

09 November 2018

The machine will move down to touch the tool setter,
The measured tool-chuck height is stored into
#4999.
Then the Z is moved up to safe height.

Release 4.03

112

EDING CNC

Manual

(This calibrates the XY
position of the tool
setter device)

Calibration DONE
We need to do this
only once.
You need to do this
again if you have
changed something
that influences the
calibrated data.
When all calibrated, the user button F2 can be used to measure the tool
length.
Make sure the correct tool is loaded before you start.
Press USER BUTTON 2.

The machine moves to safe height.
The dialog is shown:

Type correct values for tool number,
tool length and diameter.
Press OK.

The machine moves to the correct X,Y
The machine moves 10 mm above the
tool setter.
So make sure the approx tool length
above is OK.
The machine does the move towards
the tool setter,
Then calculates and stores the values.
Then machine moves Z to safe height.

Tool Length measurement Complete.

09 November 2018

Release 4.03

113

EDING CNC

Manual

Sub calibrate_tool_setter
warnmsg "close MDI, check correct calibration tool nr 99 data in tool table"
warnmsg "jog to toolchange safe height, when done press RUN"
#4996=#5073 ;Store toolchange safe height machine coordinates
warnmsg "insert calibrationtool 99 length=" #5499 ", jog just above tool setter, when done press RUN"
;store x y in non volatile parameters (4000 - 4999)
#4997=#5071 ;machine pos X
#4998=#5072 ;machine pos Y
;Determine minimum toochuck height and store into #4999
g38.2 g91 z-20 f30
#4999=[#5053 - #5499] ;probepos Z - calibration tool length = toolchuck height
g90
g0 g53 z#4996
msg "calibration done safe height="#4996 " X="#4997 " Y="#4998 " Chuck height="#4999
endSub
sub m_tool
;Check if toolsetter is calibrated
if [[#4996 == 0] and [#4997 == 0] and [#4998 == 0] and [#4999 == 0]]
errmsg "calibrate toolsetter first open mdi, enter gosub calibrate_tool_setter"
else
g0 g53 z#4996 ; move to safe z
dlgmsg "enter tool dimensions" "tool number" 5016 "approx tool length" 5017 "tool diameter" 5018
if [#5398 == 1];user pressed OK
if [[#5016 < 1] OR [#5016 > 15]]
ErrMsg "Tool must be in range of 0 .. 15"
endif
;move to toolsetter coordinates
g00 g53 x#4997 y#4998
;move to 10mm above chuck height + approx tool length + 10
g00 g53 z[#4999+10+#5017]
;measure tool length and pull 5mm back up
g38.2 g91 z-20 f30
g90
;back to safe height
g0 g53 z#4996
;Store tool length, diameter in tool table
#[5400 + #5016] = [#5053-#4999]
#[5500 + #5016] = #5018
#[5600 + #5016] = 0 ;Tool X offset is 0
msg "tool length measured="#[5400 + #5016]" stored at tool "#5016
endif
endif
endsub

09 November 2018

Release 4.03

114

EDING CNC

Manual

3 Input: the RS274/NGC Language
This chapter describes the input language, RS274/NGC. Overview
The RS274/NGC language is based on lines of code. Each line (also called a
"block") may include commands to a machining center to do several different
things. Lines of code may be collected in a file to make a program.
A typical line of code consists of an optional line number at the beginning
followed by one or more "words." A word consists of a letter followed by a
number (or something that evaluates to a number). A word may either give a
command or provide an argument to a command. For example, "G1 X3" is a
valid line of code with two words. "G1" is a command meaning "move in a
straight line at the programmed feed rate," and "X3" provides an argument
value (the value of X should be 3 at the end of the move). Most RS274/NGC
commands start with either G or M (for miscellaneous). The words for these
commands are called "G codes" and "M codes."
The RS274/NGC language has no indicator for the start of a program. The
RS274/NGC language has two commands (M2 or M30), either of which ends a
program.

09 November 2018

Release 4.03

115

EDING CNC

3.1

Manual

SYSTEM-PARAMETERS/VARIABLES

In the RS274/NGC language view, a machining center maintains an array of
5999 numerical parameters. They can be accessed by #1 .. #5999. The specific
parameters with dedicated function are listed in the table below. Other
parameters in range of 1..5999 are free to use in your G-Code program.
A simple example of usage:
#50=100 ; assign the value 100 to variable #50
G0[#50] ; use #50 to move to 100
Parameters with specific meaning are listed in this table below.

Meaning
Parameter number
Parameters wit this
background color are
read only.
1-26

Read only

Used for parameters when overriding mfunctions.
When in the g-code there is e.g.
M999 X100 S1000
And you have in your macro.cnc:
Sub m999
msg “this is my m999 X=”#24” S=”#19
Endsub
Inside the subroutine, the given X and S
parameters are at #24 and #19
#1-#26 = A – Z parameter value.
Values are negative -1e10 if not provided
with m999 in this example.

09 November 2018

Release 4.03

116

EDING CNC

Manual

Meaning
Parameter number
27-4999

Free to use, note that 4996 – 4999 are used by
the tool length measurement function under user
button 2.
Z#4996 safe height for tool measurement above
the fixed tool setter.
x#4997 y#4998 fixed tool setter position.
z#4999 chuck height, or zero length tool height,
chuck just touches the fixed tool setter at this
height.

5001-5006

Z#4995 is used for the tool setter height for
zeroing Z under user button 1.
Free to use, persistent, see above some of these
are used by tool length measurement and
zeroing.
POS X – C, interpreter position = work position

5008
5009
5010
5011
5012
5013
5014

Actual TOOL #
Actual TOOL Radius
Actual TOOL Z offset (Length + zDelta)
New tool during tool change
Actual tool X offset (X offset + xDelta)
Actual G43 Z offset (Z offset + zDelta)
Actual G43 X offset (X offset + xDelta)

5015 - 5050
5051 - 5056
5061 - 5066
5067
5068
5069
5070
5071-5076
5081-5086

Used in tool change sub routine
Probe position X – C in machine coordinates
Probe position X – C in work coordinates
1 if probe is triggered after G38.2, 0 otherwise.
Actual Probe value
Hand-wheel counter.
Spindle rate in rev/second
POS X – C, interpreter position without offsets
= Machine position.
Probe position X – C in joint coordinates

5101-5106
5111-5116
5121-5126
5131-5133
5141-5143

MCA NEG LIMIT X - C
MCA POS LIMIT X - C
HOME X-C
TCA NEG LIMIT X-Z
TCA POS LIMIT X-Z

4000-4999

09 November 2018

Release 4.03

117

EDING CNC

Manual

Meaning
Parameter number
5150

5151
5152

Active kin type:
1: Trivial
2: 4_AX_ACYLINDER (Y -> A mapping)
3: Virtual C
4-17 : System reserved
18-30: Custom 1 – Custom 12
ZHC is active
1: Spindle is ON, 0:Spindle = OFF

5161 - 5166
5181 - 5186

G28 home X - C
G30 home X - C

5190
5191
5192
5193
5194
5195
5196
G5200
G5204
G5205
G5206

G68 Rotation Method (0=OFF, 1=ON)
G68/G51 Rotation point X
G68/G51 Rotation point Y
G68/G51 Rotation point Z
G68 Rotation angle XY
G68 Rotation angle YZ
G68 Rotation angle XZ
G51 Scaling (0=OFF, 1 = ON)
G51 Scaling factor X
G51 Scaling factor Y
G51 Scaling factor Z (1.0 always)

5211 - 5216

G92 offset X - C

5220
5221
5241
5261
5281
5301
5321
5341
5361
5381
5390
5391
5394

Coord. System number
Coord. System 1 X – C
Coord. System 2 X – C
Coord. System 3 X – C
Coord. System 4 X – C
Coord. System 5 X – C
Coord. System 6 X – C
Coord. System 7 X – C
Coord. System 8 X – C
Coord. System 9 X – C
Spindle selection 0=M90 1=M91 2=M92
Alt spindle Offset X - Z
Spindle Speed MAX M90-M91

5226
5246
5266
5286
5306
5326
5346
5366
5386

- 5393
- 5396

5230
09 November 2018

Reserved for rotation coordinate system 1
Release 4.03

118

EDING CNC

Manual

Meaning
Parameter number
5250
5270
5290
5310
5330
5350
5370

5380
5397

for
for
for
for
for
for
for

rotation
rotation
rotation
rotation
rotation
rotation
rotation

coordinate
coordinate
coordinate
coordinate
coordinate
coordinate
coordinate

system
system
system
system
system
system
system

2
3
4
5
6
7
8

Simulation mode 0=normal 1=Simulation.
Running mode 0=normal 1=rendering
Use e.g. if you have G38.2 movements in your
macro file because during rendering G38.2
always runs until the given end point which may
give incorrect tool measurement results.
Always take care that the tool table contains
(approx.) correct tool data
Return value for dlgmsg (+1 OK, -1 Cancel)
Return value for M55, M56

5398
5399
5401
5501
5601
5701

Reserved
Reserved
Reserved
Reserved
Reserved
Reserved
Reserved

–
–
–
–

5499
5599
5699
5799

5801 - 5899
5901 - 5999

09 November 2018

Tool z offset (Length) Tool 1 – Tool 99
Tool diameter Tool 1 – Tool 99
Tool x offset (for Turning) Tool 1 – Tool 99
Tool orientation (for Turning) Tool 1 – Tool 99
(Currently supported only Tool 0 .. Tool 99)
Tool X Delta due to Wear
Tool Z Delta due to Wear

Release 4.03

119

EDING CNC

3.2

Manual

TOOL DATA

Tool ID

zOffset
(Length)

xOffset (For
turning)

1
2
..
99

Diameter

orientation
1-9
1-9
..
1-9

3.2.1.1 TOOL ORIENTATION FOR LATHES

When the G18 plane (X-Z) is selected, special LATHE tool radius compensation
can be used (G41, G42). Depending on the tool orientation and tool radius an
extra offset is applied.

The blue crosses show the radius center of the tool.
The green crosses show the controlled point depending on the tool orientation.
For orientation = 9 there is no offset compensation. For orientation = 2, the
compensation in X is –tool radius, in Z also –tool radius.

09 November 2018

Release 4.03

120

EDING CNC

3.3

Manual

COORDINATE SYSTEMS

In the RS274/NGC language view, a machining center has an absolute
coordinate system and nine program coordinate systems.
You can set the offsets of the nine program coordinate systems using G10 L2 Pn
(n is the number of the coordinate system) with values for the axes in terms of
the absolute coordinate system.
You can select one of the nine systems by using G54, G55, G56, G57, G58,
G59, G59.1, G59.2, or G59.3 . It is not possible to select the absolute
coordinate system directly.
You can offset the current coordinate system using G92 or G92.3. This offset
will then apply to all nine program coordinate systems. This offset may be
cancelled with G92.1 or G92.2.
You can make straight moves in the absolute machine coordinate system by
using G53 with either G0 or G1.
Data for coordinate systems is stored in parameters, see the previous section.

During initialization, the coordinate system is selected that is specified by
parameter 5220. A value of 1 means the first coordinate system (the one
G54 activates), a value of 2 means the second coordinate system (the
one G55 activates), and so on. It is an error for the value of parameter
5220 to be anything but a whole number between one and nine.
The g-code are described in detail in section 3.6

09 November 2018

Release 4.03

121

EDING CNC

3.4

Manual

FORMAT OF A LINE

A permissible line of input RS274/NGC code consists of the following, in order,
with the restriction that there is a maximum (currently 256) to the number of
characters allowed on a line.
• An optional line number.
• Any number of words, parameter settings, and comments.
Any input not explicitly allowed is illegal and will cause the Interpreter to signal
an error.
Spaces and tabs are allowed anywhere on a line of code and do not change the
meaning of the line, except inside comments. This makes some strange-looking
input legal. The line "g0x +0. 12 34y 7" is equivalent to "g0 x+0.1234 y7", for
example.
Blank lines are allowed in the input. They are to be ignored.
Input is case insensitive.

3.4.1

Line Number

A line number is the letter N followed by an integer (with no sign) between 0
and 99999 written with no more than five digits (000009 is not OK, for
example). Line numbers may be repeated or used out of order, although normal
practice is to avoid such usage.
Line numbers may also be skipped, and that is normal practice. A line number is
not required to be used, but must be in the proper place if used.

3.4.2

Word

A word is a letter other than N followed by a real value.
Words may begin with any of the letters shown in Table 3-2. The table includes
N for completeness, even though, as defined above, line numbers are not
words. Several letters (I, J, K, L, P, and R) may have different meanings in
different contexts.
Letter

Meaning

A-axis of machine

Tool radius compensation number

F
G

Feed rate

H
I
J
K

Tool length offset index
X-axis offset for arcs X offset in G87 canned cycle
Y-axis offset for arcs Y offset in G87 canned cycle
Z-axis offset for arcs Z offset in G87 canned cycle

L
M

number of repetitions in canned cycles key used with G10
miscellaneous function (see Table 3-6)

line number
dwell time in canned cycles dwell time with G4 key used with
G10

General function (see Table 3-4)

09 November 2018

Release 4.03

122

EDING CNC

Manual

Letter

Meaning

Q
R
S
T
X
Y
Z

feed increment in G83 canned cycle
arc radius, clear_z distance in canned cycle
spindle speed
tool selection
X-axis of machine
Y-axis of machine
Z-axis of machine

A-axis of machine

B-axis of machine

C-axis of machine

A real value is some collection of characters that can be processed to come up
with a number. A real value may be an explicit number (such as 341 or 0.8807), a parameter value, an expression, or a unary operation value.
Definitions of these follow immediately. Processing characters to come up with a
number is called "evaluating". An explicit number evaluates to itself.
3.4.2.1
NUMBER
The following rules are used for (explicit) numbers. In these rules a digit is a
single character between 0 and 9.
• A number consists of (1) an optional plus or minus sign, followed by (2)
zero to many digits, followed, possibly, by (3) one decimal point, followed
by (4) zero to many digits - provided that there is at least one digit
somewhere in the number.
• There are two kinds of numbers: integers and decimals. An integer does
not have a decimal point in it; a decimal does.
• Numbers may have any number of digits, subject to the limitation on line
length. Only about seventeen significant figures will be retained, however
(enough for all known applications).
• A non-zero number with no sign as the first character is assumed to be
positive.
Notice that initial (before the decimal point and the first non-zero digit) and
trailing (after the decimal point and the last non-zero digit) zeros are allowed
but not required.
A number written with initial or trailing zeros will have the same value when it is
read as if the extra zeros were not there.
Numbers used for specific purposes in RS274/NGC are often restricted to some
finite set of values or some to some range of values. In many uses, decimal
numbers must be close to integers; this includes the values of indexes (for
parameters and carousel slot numbers, for example), M codes, and G codes
multiplied by ten. A decimal number which is supposed be close to an integer is
considered close enough if it is within 0.0001 of an integer.
3.4.2.2

PARAMETER VALUE

09 November 2018

Release 4.03

123

EDING CNC

Manual

A parameter value is the pound character # followed by a real value. The real
value must evaluate to an integer between 1 and 5399. The integer is a
parameter number, and the value of the parameter value is whatever number is
stored in the numbered parameter.
The # character takes precedence over other operations, so that, for example,
"#1+2" means the number found by adding 2 to the value of parameter 1, not
the value found in parameter 3. Of course, #[1+2] does mean the value found
in parameter 3. The # character may be repeated; for example ##2 means the
value of the parameter whose index is the (integer) value of parameter 2.
3.4.2.3
EXPRESSIONS AND BINARY OPERATIONS
An expression is a set of characters starting with a left bracket [ and ending
with a balancing right bracket ]. In between the brackets are numbers,
parameter values, mathematical operations, and other expressions. An
expression may be evaluated to produce a number. The expressions on a line
are evaluated when the line is read, before
anything on the line is executed. An example of an expression is [ 1 + acos[0] [#3 ** [4.0/2]]].
Binary operations appear only inside expressions. Nine binary operations are
defined. There are four basic mathematical operations: addition (+), subtraction
(-), multiplication (*), and division (/). There are three logical operations: nonexclusive or (OR), exclusive or (XOR), and logical and (AND). The eighth
operation is the modulus operation (MOD). The ninth operation is the "power"
operation (**) of raising the number on the left of the operation to the power on
the right.
The binary operations are divided into three groups. The first group is: power.
The second group is: multiplication, division, and modulus. The third group is:
addition, subtraction, logical non-exclusive or, logical exclusive or, and logical
and. If operations are strung together (for example in the expression [2.0 / 3 *
1.5 - 5.5 / 11.0]), operations in the first group are to be performed before
operations in the second group and operations in the second group before
operations in the third group. If an expression contains more than one operation
from the same group (such as the first / and * in the example), the operation
on the left is performed first. Thus, the example is equivalent to: [((2.0 / 3) *
1.5) - (5.5 / 11.0)] , which simplifies to [1.0 - 0.5] , which is 0.5.
The logical operations and modulus are to be performed on any real numbers,
not just on integers. The number zero is equivalent to logical false, and any
non-zero number is equivalent to logical true.
3.4.2.4
UNARY OPERATION VALUE
A unary operation value is either "ATAN" followed by one expression divided by
another expression (for example "ATAN[2]/[1+3]") or any other unary
operation name followed by an expression (for example "SIN[90]"). The unary
operations are: ABS (absolute value), ACOS (arc cosine), ASIN (arc sine), ATAN
(arc tangent), COS (cosine), EXP (e raised to the given power), FIX (round
down), FUP (round up), LN (natural logarithm), ROUND (round to the nearest
whole number), SIN (sine), SQRT (square root), and TAN (tangent). Arguments
to unary operations which take angle measures (COS, SIN, and TAN) are in
09 November 2018

Release 4.03

124

EDING CNC

Manual

degrees. Values returned by unary operations which return angle measures
(ACOS, ASIN, and ATAN) are also in degrees.
The FIX operation rounds towards the left (less positive or more negative) on a
number line, so that FIX[2.8] =2 and FIX[-2.8] = -3, for example. The FUP
operation rounds towards the right (more positive or less negative) on a number
line; FUP[2.8] = 3 and FUP[-2.8] = -2, for example.

3.4.3

Parameter Setting

A parameter setting is the following four items one after the other: (1) a pound
character # , (2) a real value which evaluates to an integer between 1 and
5399, (3) an equal sign
= , and (4) a real value. For example "#3 = 15" is a parameter setting meaning
"set parameter 3 to 15."
A parameter setting does not take effect until after all parameter values on the
same line have been found. For example, if parameter 3 has been previously set
to 15 and the line "#3=6 G1 x#3" is interpreted, a straight move to a point
where x equals 15 will occur and the value of parameter 3 will be 6.

3.4.4

Comments and Messages

Printable characters and white space inside parentheses is a comment. A left
parenthesis always starts a comment. The comment ends at the first right
parenthesis found thereafter. Once a left parenthesis is placed on a line, a
matching right parenthesis must appear before the end of the line. Comments
may not be nested; it is an error if a left parenthesis is found after the start of a
comment and before the end of the comment.
Here’s an example of a line containing a comment: "G80 M5 (stop motion)".
Comments do not cause a machining center to do anything.
A comment contains a message if "MSG," appears after the left parenthesis and
before any other printing characters. Variants of "MSG," which include white
space and lower case characters are allowed. The rest of the characters before
the right parenthesis are considered to be a message. Messages should be
displayed on the message display device. Comments not containing messages
need not be displayed there.

3.4.5

Item Repeats

A line may have any number of G words, but two G words from the same modal
group may not appear on the same line.
A line may have zero to four M words. Two M words from the same modal group
may
not appear on the same line.
For all other legal letters, a line may have only one word beginning with that
letter.

09 November 2018

Release 4.03

125

EDING CNC

Manual

If a parameter setting of the same parameter is repeated on a line, "#3=15
#3=6", for example, only the last setting will take effect. It is silly, but not
illegal, to set the same parameter twice on the same line.
If more than one comment appears on a line, only the last one will be used;
each of the other comments will be read and its format will be checked, but it
will be ignored thereafter. It is expected that putting more than one comment
on a line will be very rare.

3.4.6

Item order

The three types of item whose order may vary on a line (as given at the
beginning of this section) are word, parameter setting, and comment. Imagine
that these three types of item are divided into three groups by type.
The first group (the words) may be reordered in any way without changing the
meaning of the line.
If the second group (the parameter settings) is reordered, there will be no
change in the meaning of the line unless the same parameter is set more than
once. In this case, only the last setting of the parameter will take effect. For
example, after the line "#3=15 #3=6" has been interpreted, the value of
parameter 3 will be 6. If the order is reversed to "#3=6 #3=15" and the line is
interpreted, the value of parameter 3 will be 15.
If the third group (the comments) contains more than one comment and is
reordered, only the last comment will be used.
If each group is kept in order or reordered without changing the meaning of the
line, then the three groups may be interleaved in any way without changing the
meaning of the line. For example, the line "g40 g1 #3=15 (foo) #4=-7.0" has
five items and means exactly the same thing in any of the 120 possible orders
(such as "#4=-7.0 g1 #3=15 g40 (foo)") for the five items.

3.4.7

Commands and Machine Modes

In RS274/NGC, many commands cause a machining center to change from one
mode to another, and the mode stays active until some other command changes
it implicitly or explicitly. Such commands are called "modal". For example, if
coolant is turned on, it stays on until it is explicitly turned off. The G codes for
motion are also modal. If a G1 (straight move) command is given on one line,
for example, it will be executed again on
the next line if one or more axis words are available on the line, unless an
explicit command is given on that next line using the axis words or cancelling
motion.
"Non-modal" codes have effect only on the lines on which they occur. For
example, G4 (dwell) is non-modal.

09 November 2018

Release 4.03

126

EDING CNC

3.5

Manual

MODAL GROUPS

Modal commands are arranged in sets called "modal groups", and only one
member of a modal group may be in force at any given time. In general, a
modal group contains commands for which it is logically impossible for two
members to be in effect at the same time - like measure in inches vs. measure
in millimeters. A machining center may be in many modes at the same time,
with one mode from each modal group being in effect. The modal groups are
shown in Table 3-3.
Table 3-3 Modal Groups
The modal groups for G codes are:
group 1 = {G0, G1, G2, G3, G38.2, G76, G80, G81,
G82, G83, G84, G85, G86, G87, G88, G89} motion
group 2 = {G17, G18, G19} plane selection
group 3 = {G90, G91} distance mode
group 5 = {G93, G94} feed rate mode
group 6 = {G20, G21} units
group 7 = {G40, G41, G42} cutter radius compensation
group 8 = {G43, G49} tool length offset
group 10 = {G98, G99} return mode in canned cycles
group 12 = {G54, G55, G56, G57, G58, G59, G59.1, G59.2, G59.3}
coordinate system selection
group 13 = {G61, G61.1, G64} path control mode
group 14 = {G68, G69} XY plane rotation.
The modal groups for M codes are:
group 4 = {M0, M1, M2, M30, M60} stopping
group 5 = {54, M55, M56, M64, M65, M66} AUX and general purpose
I/O
group 6 = {M6} tool change
group 7 = {M3, M4, M5} spindle turning
group 8 = {M7, M8, M9} coolant (special case: M7 and M8 may be active
at the same time)
group 9 = {M48, M49, M50, M51, M52} enable/disable feed and speed
override switches
group 10 = {M90, M91, M92, M95, M97} select standard or alternate
spindle or touch probe or camera offset, M90=standard.
Enable THC = {M20, M21} THC ON | THC OFF (Torch height control)
A axis clamp = {M26, M27} Clamp on | clamp off.
In addition to the above modal groups, there is a group for non-modal G
codes:
group 0 = {G4, G10, G28, G30, G53, G92, G92.1, G92.2, G92.3}
For several modal groups, when a machining center is ready to accept
commands, one member of the group must be in effect. There are default
settings for these modal groups. When the machining center is turned on or
otherwise re-initialized, the default values are automatically in effect.

09 November 2018

Release 4.03

127

EDING CNC

Manual

Group 1, the first group on the table, is a group of G codes for motion. One of
these is always in effect. That one is called the current motion mode.
It is an error to put a G-code from group 1 and a G-code from group 0 on the
same line if both of them use axis words. If an axis word-using G-code from
group 1 is implicitly in effect on a line (by having been activated on an earlier
line), and a group 0 G-code that uses axis words appears on the line, the
activity of the group 1 G-code is suspended for that line. The axis word-using Gcodes from group 0 are G10, G28, G30, and G92.

09 November 2018

Release 4.03

128

EDING CNC

3.6

Manual

G CODES

G codes of the RS274/NGC language are shown in Table 3-4 and described in
this Section.
The descriptions contain command prototypes, set in bold type.
In the command prototypes, three dots (…) stand for a real value. As described
earlier, a real value may be (1) an explicit number, 4, for example, (2) an
expression, [2+2], for example, (3) a parameter value, #88, for example, or
(4) a unary function value, acos[0], for example.
In most cases, if axis words (any or all of X…, Y…, Z…, A…, B…, C…) are
given, they specify a destination point. Axis numbers are in the currently active
coordinate system, unless explicitly described as being in the absolute
coordinate system. Where axis words are optional, any omitted axes will have
their current value. Any items in the command prototypes not explicitly
described as optional are required. It is an error if a required item is omitted.
In the prototypes, the values following letters are often given as explicit
numbers. Unless stated otherwise, the explicit numbers can be real values. For
example, G10 L2 could equally well be written G[2*5] L[1+1]. If the value of
parameter 100 were 2, G10 L#100 would also mean the same. Using real
values which are not explicit numbers as just shown in the examples is rarely
useful.
If L… is written in a prototype the "…" will often be referred to as the "L
number". Similarly the "…" in H… may be called the "H number", and so on for
any other letter.

3.6.1

Rapid Linear Motion - G0

For rapid linear motion, program G0 X… Y… Z… A…, where all the axis words
are optional, except that at least one must be used. The G0 is optional if the
current motion mode is G0. This will produce coordinated linear motion to the
destination point at the current traverse rate (or slower if the machine will not
go that fast). It is expected that cutting will not take place when a G0 command
is executing.
It is an error if:
• All axis words are omitted.
If cutter radius compensation is active, the motion will differ from the above;
see Appendix A. If G53 is programmed on the same line, the motion will also
differ.

09 November 2018

Release 4.03

129

EDING CNC

Table 3-4
G Code
G0
G1
G2
G3
G4
G10
G17
G18
G19
G20
G21
G28
G30
G33
G38.2
G40
G41
G42
G43
G49
G53
G54
G55
G56
G57
G58
G59
G59.1
G59.2
G59.3
G61
G61.1
G64
G68
G76
G80
G81
G82
G83
G84
G85
G86
G87
G88
G89
G90
G91
G92
G92.1

Manual

G Codes
Meaning
rapid positioning
linear interpolation
circular/helical interpolation (clockwise)
circular/helical interpolation (counterclockwise)
dwell
coordinate system origin setting
XY-plane selection
XZ-plane selection
YZ-plane selection
inch system selection
millimeter system selection
move to park position 1, setup on variable page
move to park position 2, setup on variable page
Lathe, motion synchronized to spindle
straight probe
cancel cutter radius compensation
start cutter radius compensation left
start cutter radius compensation right
tool length offset (plus) , tool X offset for lathe
cancel tool length offset
motion in machine coordinate system
use preset work coordinate system 1
use preset work coordinate system 2
use preset work coordinate system 3
use preset work coordinate system 4
use preset work coordinate system 5
use preset work coordinate system 6
use preset work coordinate system 7
use preset work coordinate system 8
use preset work coordinate system 9
set path control mode: exact path
set path control mode: exact stop
set path control mode: continuous
XY rotation
Lathe, threading
cancel motion mode (including any canned cycle)
canned cycle: drilling
canned cycle: drilling with dwell
canned cycle: peck drilling
canned cycle: right hand tapping
canned cycle: boring, no dwell, feed out
canned cycle: boring, spindle stop, rapid out
canned cycle: back boring
canned cycle: boring, spindle stop, manual out
canned cycle: boring, dwell, feed out
absolute distance mode
incremental distance mode
offset coordinate systems and set parameters
cancel offset coordinate systems and set parameters to zero

09 November 2018

Release 4.03

130

EDING CNC

G92.2
G92.3
G93
G94
G98
G99

3.6.2

Manual

cancel offset coordinate systems but do not reset parameters
apply parameters to offset coordinate systems
inverse time feed rate mode
units per minute feed rate mode
initial level return in canned cycles
R-point level return in canned cycles

Linear Motion at Feed Rate - G1

For linear motion at feed rate (for cutting or not), program G1 X… Y… Z… A…,
where all the axis words are optional, except that at least one must be used.
09 November 2018

Release 4.03

131

EDING CNC

Manual

The G1 is optional if the current motion mode is G1. This will produce
coordinated linear motion to the destination point at the current feed rate (or
slower if the machine will not go that fast).
It is an error if:
• All axis words are omitted.
If cutter radius compensation is active, the motion will differ from the above;
see Appendix A. If G53 is programmed on the same line, the motion will also
differ.

3.6.3

Arc at Feed Rate - G2 and G3

A circular or helical arc is specified using either G2 (clockwise arc) or G3
(counterclockwise arc). The axis of the circle or helix must be parallel to the X,
Y, or Z-axis of the machine coordinate system. The axis (or, equivalently, the
plane perpendicular to the axis) is selected with G17 (Z-axis, XY-plane), G18 (Yaxis, XZ-plane), or G19 (X-axis, YZ-plane). If the arc is circular, it lies in a plane
parallel to the selected plane.
If a line of RS274/NGC code makes an arc and includes rotational axis motion,
the rotational axes turn at a constant rate so that the rotational motion starts
and finishes when the XYZ motion starts and finishes. Lines of this sort are
hardly ever programmed.
If cutter radius compensation is active, the motion will differ from what is
described here. See Appendix A.
Two formats are allowed for specifying an arc. We will call these the center
format and the radius format. In both formats the G2 or G3 is optional if it is the
current motion mode.
3.6.3.1
RADIUS FORMAT ARC
In the radius format, the coordinates of the end point of the arc in the selected
plane are specified along with the radius of the arc. Program G2 X… Y… Z…
A… R… (or use G3 instead of G2). R is the radius. The axis words are all
optional except that at least one of the two words for the axes in the selected
plane must be used. The R number is the radius. A positive radius indicates that
the arc turns through 180 degrees or less, while a negative radius indicates a
turn of 180 degrees to 359.999 degrees. If the arc is helical, the value of the
end point of the arc on the coordinate axis parallel to the axis of the helix is also
specified.
It is not good practice to program radius format arcs that are nearly full circles
or are semicircles (or nearly semicircles) because a small change in the location
of the end point will produce a much larger change in the location of the center
of the circle (and, hence, the middle of the arc). The magnification effect is
large enough that rounding error in a number can produce out-of-tolerance
cuts. Nearly full circles are outrageously bad, semicircles (and nearly so) are
only very bad. Other size arcs (in the range tiny to 165 degrees or 195 to 345
degrees) are OK.

09 November 2018

Release 4.03

132

EDING CNC

Manual

Here is an example of a radius format command to mill an arc: G17 G2 x 10 y
15 r 20 z 5.
That means to make a clockwise (as viewed from the positive Z-axis) circular or
helical arc whose axis is parallel to the Z-axis, ending where X=10, Y=15, and
Z=5, with a radius of 20. If the starting value of Z is 5, this is an arc of a circle
parallel to the XY-plane; otherwise it is a helical arc.
3.6.3.2

CENTER FORMAT ARC

In the center format, the coordinates of the end point of the arc in the selected
plane are
specified along with the offsets of the center of the arc from the current
location. In this format, it is OK if the end point of the arc is the same as the
current point. It is an error if:
•

When the arc is projected on the selected plane, the distance from the
current point to the center differs from the distance from the end point to
the center by more than 0.0002 inch (if inches are being used) or 0.002
millimeter (if millimeters are being used).

When the XY-plane is selected, program G2 X… Y… Z… A… I… J… (or use G3
instead of G2). The axis words are all optional except that at least one of X and
Y must be used. I and J are the offsets from the current location (in the X and Y
directions, respectively) of the center of the circle. I and J are optional except
that at least one of the two must be used. It is an error if:
• I and J are both omitted.
When the XZ-plane is selected, program G2 X… Y… Z… A… I… K… (or use G3
instead of G2). The axis words are all optional except that at least one of X and
Z must be used. I and K are the offsets from the current location (in the X and Z
directions, respectively) of the center of the circle. I and K are optional except
that at least one of the two must be used. It is an error if:
• I and K are both omitted.
When the YZ-plane is selected, program G2 X… Y… Z… A… B… C… J… K…
(or use G3 instead of G2). The axis words are all optional except that at least
one of Y and Z must be used. J and K are the offsets from the current location
(in the Y and Z directions, respectively) of the center of the circle. J and K are
optional except that at least one of the two must be used. It is an error if:
• J and K are both omitted.
Here is an example of a center format command to mill an arc:
G17 G2 x10 y16 i3 j4 z9.
That means to make a clockwise (as viewed from the positive z-axis) circular or
helical arc whose axis is parallel to the Z-axis, ending where X=10, Y=16, and
Z=9, with its center offset in the X direction by 3 units from the current X
location and offset in the Y direction by 4 units from the current Y location. If
the current location has X=7, Y=7 at the outset, the center will be at X=10,
Y=11. If the starting value of Z is 9, this is a circular arc; otherwise it is a
helical arc. The radius of this arc would be 5.
09 November 2018

Release 4.03

133

EDING CNC

Manual

In the center format, the radius of the arc is not specified, but it may be found
easily as the distance from the center of the circle to either the current point or
the end point of the arc.

3.6.4

Dwell - G4

For a dwell, program G4 P… . This will keep the axes unmoving for the period of
time in seconds specified by the P number. It is an error if:
• the P number is negative.

3.6.5

Set Coordinate System Data -G10

To set the coordinate values for the origin of a coordinate system, program
G10 L2 P … X… Y… Z… A…, where the P number must evaluate to an integer
in the range 1 to 9 (corresponding to G54 to G59.3) and all axis words are
optional. The coordinates of the origin of the coordinate system specified by the
P number are reset to the coordinate values given (in terms of the absolute
coordinate system). Only those coordinates for which an axis word is included
on the line will be reset.
It is an error if:
• the P number does not evaluate to an integer in the range 1 to 9.
If origin offsets (made by G92 or G92.3) were in effect before G10 is used, they
will continue to be in effect afterwards.
The coordinate system whose origin is set by a G10 command may be active or
inactive at the time the G10 is executed.
Example:G10 L2 P1 x 3.5 y 17.2 sets the origin of the first coordinate system
(the one selected by G54) to a point where X is 3.5 and Y is 17.2 (in absolute
coordinates). The Z coordinate of the origin (and the coordinates for any
rotational axes) are whatever those coordinates of the origin were before the
line was executed.
G10 L20 P.. X.. Y.. Z.. A..
Set coordinate system given by P number relative to actual machine position.
Working is similar to G92. Jog to any position, then apply e.g. G10 L20 P1 X0 Y0
to set G54 coordinate system zero point at current machine position.

3.6.6

Plane Selection - G17, G18, and G19

Program G17 to select the XY-plane, G18 to select the XZ-plane, or G19 to
select the YZ-plane.

3.6.7

Length Units - G20/G21 and G70/G71

Program G20 to use inches for length units. Program G21 to use millimeters.

09 November 2018

Release 4.03

134

EDING CNC

Manual

It is usually a good idea to program either G20 or G21 near the beginning of a
program before any motion occurs, and not to use either one anywhere else in
the program. It is the responsibility of the user to be sure all numbers are
appropriate for use with the current length units. G70/G71 is added for CAM
software compatibility.

3.6.8

Return to Home - G28 and G30

Two home positions are defined (by parameters 5161-5166 for G28 and
parameters
5181-5186 for G30). The parameter values are in terms of the absolute
coordinate system, but are in unspecified length units.
To return to home position by way of the programmed position, program
G28 X… Y… Z… A… (or use G30). All axis words are optional. The path is
made by a traverse move from the current position to the programmed position,
followed by a traverse move to the home position. If no axis words are
programmed, the intermediate point is the current point, so only one move is
made. The order of Z depends on its position, if the end position is higher as the
current Z position Z will move first, otherwise Z will move last, this is to prevent
collision.
Addition for lathe: For lathe the X axis is moved first, assumption is that X
moves away from the turning center.

09 November 2018

Release 4.03

135

EDING CNC

3.6.9

Manual

G33, G33.1 Spindle-Synchronized Motion

For spindle-synchronized motion in one direction, program
G33 X… Y… Z… K… where K gives the distance moved in XYZ for each
revolution of the spindle.
For G33 the software performs this:
1. Start a synchronized move with spindle with K feed per revolution.
Assumed is that the spindle already runs (M3).
2. Done.
For G33.1 the software performs:
1. Start a synchronized move with spindle with K feed per revolution.
Assumed is that the spindle is running (M3).
2. Wait until this motion is done.
3. Reverse spindle direction.
4. Move back to original position where we were before the G33.1.
5. Done
All the axis words are optional, except that at least one must be used.
It is an error if:
• all axis words are omitted.
• the spindle is not turning when this command is executed.
• the requested linear motion exceeds machine velocity limits due to the
spindle speed.

09 November 2018

Release 4.03

136

EDING CNC

Manual

3.6.10 Straight Probe - G38.2
3.6.10.1
THE STRAIGHT PROBE COMMAND
Program G38.2 X… Y… Z… A… to perform a straight probe operation. The
rotational axis words are allowed, but it is better to omit them. If rotational axis
words are used, the numbers must be the same as the current position numbers
so that the rotational axes do not move. The linear axis words are optional,
except that at least one of them must be used. The tool in the spindle must be a
probe.
It is an error if:
• the current point is less than 0.254 millimeter or 0.01 inch from the programmed point.
• G38.2 is used in inverse time feed rate mode,
• any rotational axis is commanded to move,
• no X, Y, or Z-axis word is used.
In response to this command, the machine moves the controlled point (which
should be at the end of the probe tip) in a straight line at the current feed rate
toward the programmed point. If the probe trips, the probe is retracted slightly
from the trip point at the end of command execution. If the probe does not trip
even after overshooting the programmed point slightly, an error is signaled.
After successful probing, parameters 5061 to 5066 will be set to the program
coordinates of the location of the controlled point at the time the probe tripped.
The variables 5051 to 5056 will contain the machine coordinates. Useful for
measuring tools in absolute machine positions. G53 G38.2 will move in machine
coordinates.
3.6.10.2
USING THE STRAIGHT PROBE COMMAND
Using the straight probe command, if the probe shank is kept nominally parallel
to the Z-axis (i.e., any rotational axes are at zero) and the tool length offset for
the probe is used, so that the controlled point is at the end of the tip of the
probe:
• without additional knowledge about the probe, the parallelism of a face of
a part to the XY-plane may, for example, be found.
• if the probe tip radius is known approximately, the parallelism of a face of
a part to the YZ or XZ-plane may, for example, be found.
• if the shank of the probe is known to be well-aligned with the Z-axis and
the probe tip radius is known approximately, the center of a circular hole,
may, for example, be found.
• if the shank of the probe is known to be well-aligned with the Z-axis and
the probe tip radius is known precisely, more uses may be made of the
straight probe command, such as finding the diameter of a circular hole.
If the straightness of the probe shank cannot be adjusted to high accuracy, it is
desirable to know the effective radii of the probe tip in at least the +X, -X, +Y,
and -Y directions. These quantities can be stored in parameters either by being
included in the parameter file or by being set in an RS274/NGC program.
Using the probe with rotational axes not set to zero is also feasible. Doing so is
more complex than when rotational axes are at zero, and we do not deal with it
here.
09 November 2018

Release 4.03

137

EDING CNC

Manual

3.6.10.3
EXAMPLE CODE
As a usable example, the code for finding the center and diameter of a circular
hole is shown in Table 3-5. For this code to yield accurate results, the probe
shank must be well-aligned with the Z-axis, the cross section of the probe tip at
its widest point must be very circular, and the probe tip radius (i.e., the radius
of the circular cross section) must be known precisely. If the probe tip radius is
known only approximately (but the other conditions hold), the location of the
hole center will still be accurate, but the hole diameter will not.
In Table 3-5, an entry of the form is meant to be
replaced by an actual number that matches the description of number. After this
section of code has executed, the X-value of the center will be in parameter
1041, the Y-value of the center in parameter 1022, and the diameter in
parameter 1034. In addition, the diameter parallel to the X-axis will be in
parameter 1024, the diameter parallel to the Y-axis in parameter 1014, and the
difference (an indicator of circularity) in parameter 1035. The probe tip will be in
the hole at the XY center of the hole.
The example does not include a tool change to put a probe in the spindle. Add
the tool change code at the beginning, if needed.
Table 3-5 Code to Probe Hole
N010 (probe to find center and diameter of circular hole)
N020 (This program will not run as given here. You have to)
N030 (insert numbers in place of .)
N040 (Delete lines N020, N030, and N040 when you do that.)
N050 G0 Z F
N060 #1001=
N070 #1002=
N080 #1003=
N090 #1004=
N100 #1005=[/2.0 - #1004]
N110 G0 X#1001 Y#1002 (move above nominal hole center)
N120 G0 Z#1003 (move into hole - to be cautious, substitute G1 for G0
here)
N130 G38.2 X[#1001 + #1005] (probe +X side of hole)
N140 #1011=#5061 (save results)
N150 G0 X#1001 Y#1002 (back to center of hole)
N160 G38.2 X[#1001 - #1005] (probe -X side of hole)
N170 #1021=[[#1011 + #5061] / 2.0] (find pretty good X-value of hole
center)
N180 G0 X#1021 Y#1002 (back to center of hole)
N190 G38.2 Y[#1002 + #1005] (probe +Y side of hole)
N200 #1012=#5062 (save results) N210 G0 X#1021 Y#1002 (back to
center of hole)
N220 G38.2 Y[#1002 - #1005] (probe -Y side of hole)
N230 #1022=[[#1012 + #5062] / 2.0] (find very good Y-value of hole
center)

09 November 2018

Release 4.03

138

EDING CNC

Manual

N240 #1014=[#1012 - #5062 + [2 * #1004]] (find hole diameter in Ydirection)
N250 G0 X#1021 Y#1022 (back to center of hole)
N260 G38.2 X[#1021 + #1005] (probe +X side of hole)
N270 #1031=#5061 (save results)
N280 G0 X#1021 Y#1022 (back to center of hole)
N290 G38.2 X[#1021 - #1005] (probe -X side of hole)
N300 #1041=[[#1031 + #5061] / 2.0] (find very good X-value of hole
center)
N310 #1024=[#1031 - #5061 + [2 * #1004]] (find hole diameter in Xdirection)
N320 #1034=[[#1014 + #1024] / 2.0] (find average hole diameter)
N330 #1035=[#1024 - #1014] (find difference in hole diameters)
N340 G0 X#1041 Y#1022 (back to center of hole)
N350 M2 (that's all, folks)

3.6.11 Cutter Radius Compensation - G40, G41, G41.1, G42,
G42.1
To turn cutter radius compensation off, program G40. It is OK to turn
compensation
off when it is already off. Cutter radius compensation may be performed only if
the XY-plane is active.
To turn cutter radius compensation on left (i.e., the cutter stays to the left of
the programmed path when the tool radius is positive), program G41 D… . To
turn cutter radius compensation on right (i.e., the cutter stays to the right of
the programmed path when the tool radius is positive), program G42 D… . The
D word is optional; if there is no D word, the radius of the tool currently in the
spindle will be used. If used, the D number should normally be the slot number
of the tool in the spindle, although this is not required. It is OK for the D
number to be zero; a radius value of zero will be used.
It is an error if:
• the D number is not an integer, is negative or is larger than the number
of carousel slots,
• the XY-plane is not active or for turning the ZX plane is not active,
• cutter radius compensation is commanded to turn on when it is already
on.
The behavior of the machining center when cutter radius compensation is on is
described in Appendix A.
With G41.1 D… is the same as G41 D… except now the D number is not a tool
number but a tool diameter.
With G42.1 D… is the same as G42 D… except now the D number is not a tool
number but a tool diameter.

09 November 2018

Release 4.03

139

EDING CNC

3.6.11.1

Manual

EXAMPLE CODE FOR MILLING
This example mills out a rectangular
object from the outside and inside.
On the outside we use G42, tool
radius compensation right and for the
inside G41, tool radius compensation
left is used.
For both contours a tool-radiuscompensation
entry
move
is
programmed consisting of a line
which must be longer than the toolradius used and a circle, of which also
the radius is bigger than the tool.
By the way, all arc radii should be
bigger than the tool radius. If you
have inside corners, there should be
always an arc, so that the tool fits.

g0 z3
g0 x-15 y15
f500
/g42.1 D6
g1 x-5
(cutter comp entry move
1)
g2 x0 y10 r5 (cutter comp entry
move 2)
g1 z-3
(plunge down)
g3 x10 y0 r10
g1 x70
g3 x80 y10 r10
g1 y90
g3 x70 y100 r10
g1 x10
g3 x0 y90 r10
g1 x0 y10
/g40
g0 z3
g0 x30 y30
/g41.1 d6
g1 x20
g3 x10 y20 r10
g1 z-3
g3 x20 y10 r10
g1 x60
g3 x70 y20 r10
g1 y80
g3 x60 y90 r10
09 November 2018

The G42, G41 and G40 codes are
programmed with a / (block delete
sign) in front. This makes it easy to
debug tool comp programs. The
program is loaded with block delete
on, this is the blue curve.
Then the program is run with block
delete off resulting in the yellow
curve.
It is clear to see what the entry move
does.

Release 4.03

140

EDING CNC

Manual

g1 x20
g3 x10 y80 r10
g1 y20
/g40
g0 z3
m30
3.6.11.2
EXAMPLE CODE FOR TURNING

The movement starts at the
right upper corner.
The blue line is the
programmed contour. The
yellow is the contour with
tool-radius compensation
G41.
The first G1 line is the tool
comp entry move.
You can get this figure by
putting a / character in
front of the G41/G40 codes.
The load the program with
block delete on and execute
it with block delete off. With
block delete on the tool
comp is skipped.
(Radius programming)
(Use R word for arc’s)
g0 x-10 z20
/g41.1 d5
g1 x-10 z10
g3 x0 z0 r10
g1 x10
g2 x20 z-10 r10
g1 z-20
g3 x30 z-30 r10
/g40
m30
(Radius programming)
(Use I,K programming for
arc’s)
g0 x-10 z20
/g41.1 d5
g1 x-10 z10
g3 x0 z0 i10 k0
g1 x10
g2 x20 z-10 i0 k-10
g1 z-20
g3 x30 z-30 i10 k0
/g40

(Diameter programming)
(Use R word for Arcs)
g0 x-20 z20
/g41.1 d5
g1 x-20 z10
g3 x0 z0 r10
g1 x20
g2 x40 z-10 r10
g1 z-20
g3 x60 z-30 r10
/g40
m30
(Diameter programming)
(Use I,K programming for arc’s)
g0 x-20 z20
/g41.1 d5
g1 x-20 z10
g3 x0 z0 i10 k0
g1 x20
g2 x40 z-10 i0 k-10
g1 z-20
g3 x60 z-30 i10 k0
/g40
m30
09 November 2018

Release 4.03

141

EDING CNC

Manual

m30

09 November 2018

Release 4.03

142

EDING CNC

Manual

3.6.12 Tool Length Offsets - G43, G43 H, G43.1, and G49
A. To use the tool offset of the tool in the spindle use G43.
This assures that always the tool length of the tool in spindle is compensated.
B. To use a tool length offset from the tool table, program G43 H…, where the
H number is the desired index in the tool table. ( H = 1 - 99)
C. To use dynamic tool compensation (not from the tool-table), use G43.1 I.. K..
where I.. gives the tool X offset (turning) and K.. gives the tool Z offset (for
turning and milling)
Warning: If you use option B or C, the tool-length compensation will not adapt
to the new tool after M6T...
To have no tool length offset compensation, program G49
#5401 - #5499 is the tool-length of tool 1-99
#5501 - #5599 is the tool-diameter of tool 1-99
#5601 - #5699 is the tool-xoffset (width for turning) offset.
The variables can be modified runtime (in the G-Code file) if needed to
compensate for tool-wear.

3.6.13 Scaling G50/G51
G50 scaling off.
UNIFORM Scaling
G51 P.. I.. J..
P is scaling factor.
NON UNIFORM Scaling (X,Y different, only applicable when NO Arcs)
G51 X.. Y.. I.. J..
X is scaling factor for X coordinates.
Y is scaling factor for Y coordinates.
I is X coordinate scaling point
J is Y coordinate scaling point
When used in combination with G68, the rotation point and scaling point are the
same.

09 November 2018

Release 4.03

143

EDING CNC

Manual

3.6.14 Move in Absolute Coordinates - G53
For linear motion to a point expressed in absolute coordinates, program
G1 G53 X… Y… Z… A… (or use G0 instead of G1), where all the axis words are
optional, except that at least one must be used. The G0 or G1 is optional if it is
the current motion mode. G53 is not modal and must be programmed on each
line on which it is intended to be active. This will produce coordinated linear
motion to the programmed point. If G1 is active, the speed of motion is the
current feed rate (or slower if the machine will not go that fast). If G0 is active,
the speed of motion is the current traverse rate (or slower if the machine will
not go that fast).
It is an error if:
• G53 is used without G0 or G1 being active,
• G53 is used while cutter radius compensation is on.

3.6.15 Select Coordinate System - G54 to G59.3
To select coordinate system 1, program G54, and similarly for other coordinate
systems. The system-number-G-code pairs are: (1-G54), (2-G55), (3-G56), (4G57), (5-G58), (6-G59), (7-G59.1), (8-G59.2), and (9-G59.3).
It is an error if:
• one of these G-codes is used while cutter radius compensation is on.

09 November 2018

Release 4.03

144

EDING CNC

Manual

3.6.16 Path Control Mode and Look ahead feed- G61, and G64
Ideally one would like to have constant cutting speed during the work and
maximum accuracy. This ideal is physically not possible, similar as driving a
racecar on curvy roads is not possible with constant velocity. It is simply to
understand that it is needed to brake in the curves and accelerate on the
straight roads. If you would do the same speed in the curves as on the straight
road, the car will fly out of the curve and get an accident. With a CNC machine it
is the similar, constant speed and accuracy together are physically not possible.
It would require infinite acceleration to go through a corner from one direction
to another. In a CNC machine this would result in position/step loss of stepper
motors or high following error with servo’s. If the motion path to consist of
small lines (G1) it is even worse than driving a racecar, because there is a sharp
corner between every line. This is often the case with CAM generated motion
paths (g-code).
So a compromise has to be made. There are various options to choose the
optimum between accuracy and constant speed or fast speed versus jerkiness.
G61 puts the machining center into exact path mode, In G61, the motion
velocity between motion segments goes to zero, the end position in corners is
exactly reached, use this if you require maximum accuracy. When a work piece
consists of many small lines this gives a quite jerky/vibrating machine because
of the continuous acceleration-deceleration-stop behavior. More practical is to
use G64 and G64 P.. , see below.
G64
G64 is to be used for more smooth and fast motion.
There are 4 parameters that can be used, they are explained below individually
but the can be combined on one line.
G64 without further parameters switches on continuous/smooth velocity mode.
In G64, subsequent moves are blended, when previous move starts to
decelerate and reaches a velocity such that the specified accuracy isn’t violated,
the next move starts to accelerate, the two motions are added. The result is
smooth motion with highest constant speed. The corners however are rounded.
The amount of rounding is depending on the max acceleration of the machine.
The higher the acceleration, the less rounding.
G64 P..
The optional P value specifies the distance reached to the corner while blending.
The next move is blended with current such that the tool path remains no more
than P from the corner. This will cause a velocity ramp down in the corner but
not to zero. The figure below is a rectangle of 10x10 milled with F 2000. This is
done with P values from 0.1 to 1, you can see the impact. This gives the best
compromise between accuracy and smooth motion.
So you can say G64 P.. is like a compromise between G61 and G64 without P.

09 November 2018

Release 4.03

145

EDING CNC

Manual

This figure shows the impact of the P parameter on the amount of rounding.

You may also conclude here that it is very important to have high acceleration
on the machine because we can ramp down faster in the corner and have more
accurate corners at higher speed.
G64 Q..
The optional Q parameter activates an embedded line simplification algorithm,
which tries to combine short lines and make one longer line. The optional Q
parameter gives the tolerance used in the algorithm. Again to reduce the
amount of small corners.
The behavior of a long g-code program with short line segments is further
optimized by look ahead feed, see next page.

09 November 2018

Release 4.03

146

EDING CNC

Manual

Look Ahead feed
To explain this, I will compare a running CNC machine again with driving a race
car.

The road maximum velocity signs have to be obeyed and you have to drive your
car exactly over the white line in the middle of the road. You will try to reach
the maximum allowed velocity where possible. When you see a curve coming up
ahead, you will brake so that you will not drift off the road. You will try to look
ahead as far as you can see and you take care that you can stop in time if the
road suddenly stops.
When you would maintain your speed in sharp curves, you will drift off the road
resulting possibly into a car accident. When the road has many short curves,
then you will not be able to reach the desired speed. The more PS you have in
the car, the higher speed you will reach because you can accelerate faster.
I think this is a good comparison with a CNC machine, the same issues apply. A
machine cannot suddenly change velocity, to reach a velocity the motors must
accelerate first for a certain time to reach the velocity.
LAF behaves like the ideal racecar driver, it will reach the highest possible
velocity without violating the maximum motor accelerations.
There is one additional problem while running CNC programs, some programs
consists of short line pieces. When the line pieces connect tangentially (are in
line), then LAF will accelerate through over the lines, reaching the maximum
allowed speed. Without LAF the speed would not be reached.
The angle to which LAF considers the segments in line is a setup parameter. The
theoretical ideal value would be very small, so that no acceleration value occurs.
More practical values are in the range of 1 to 4 degrees, the experience learns
that most machines can handle acceleration spikes up to a certain limit.
The value can be set up to 180 degrees in this case you must know what you
are doing, it can be useful during e.g. foam cutting wing profiles. Be aware
however that if the curve contains real sharp angles that step pulse loss may be
the result when using large minimum LAF angles.
09 November 2018

Release 4.03

147

EDING CNC

Manual

In practice we have seen that milling times of complex 3D work pieces can be
done in 50% of the time compared to competitors who do not have LAF.
With G64 R.. the LAF angle can be changed in the g-code file, see explanation of
G64 and G61. The standard LAF angle is in the software set-up.
To give some realistic values: A value of 3 is good for most machines. A value of
6 may already give too much Jerky ness on some machines. Still there are
customers using values of 20 here, but they have quite specific machine
constructions and application e.g. dental milling.
G64 F..
The F parameter defines the value of the Accel/Decel filter placed behind LAF.
LAF with high R values (Angle) can cause acceleration spikes because LAF will
travel through corners without stopping. The F parameter filters the trajectory
generated by LAF and takes care the acceleration is never violated.
F1 will give a RAMP time that matches with the max velocity / max acceleration
from the setup and so F1 and maximum speed will lead to the max max
acceleration that is allowed. Smaller F values filter less. This can be used if the
milling velocity is less than the max velocity of the machine. Example:
Max velocity in the setup is 200 and used milling velocity is F6000 (100 mm/s),
Then F0.5 is safe to use. So now you can do this G64 R100 F1 and you will not
get acceleration spikes but very smooth an fast movement. The price to pay is
corner rounding which is depending on the max acceleration of the machine, the
higher the max acceleration, the less corner rounding.
A good application example is with milling rubber or similar flexible material, the
milling speed must be constant otherwise more material is removed in the
corners due to the lower speed and the flexibility of the rubber. The F1 in
combination with R100 will give constant and high speed for good milling
surface quality of the rubber.
Application F: For milling e.g. rubber when constant speed is more important
than rounding. To have an acceptable amount of rounding the machine needs to
have very high acceleration. This function was tested and used on a machine
with relative low speed (100 mm/sec) and very high acceleration (4000 mm/sec
* sec).

G64 R..
The R parameter is the look-ahead feed angle, when subsequent lines/arcs have
an angle together less than this value, the trajectory-generator will accelerate
through over these segments and this way optimizes the production time. With
R0, LAF is switched off, with LAF off a (much) lower but more constant speed is
achieved. The higher the angle, the higher the speed, but the jerkier for the
machine because high accel peaks. This needs to be tuned depending on the
quality of the machine and the power of the used motors.
A compromise is to be found between speed and machine behavior.

09 November 2018

Release 4.03

148

EDING CNC

Manual

G64 R.. S.. D.. (NEW for V4.03.xx)
New algorithm:
With the standard LAF setting G64 R.. (no S.. andno D..), the velocity in corners
will be zero when the angle between the segments is bigger than LAF angle in
the set-up. But there are angles that are big and also smaller angles, so we
were seeking for and found a solution where depending on the angle size, the
speed in the corner the velocity is limited but not to zero and further limited if
the angle gets bigger. This allows faster production especially for 3D work.
Putting a circle to the original path would be a solution. But this cannot be done
in real-time and is also not always wanted because we want the contour to be
milled as specified in the g-code.
Still we could calculate a circle between 2 segments when knowing its start and
end vector. The circle radius could then be used to calculate an allowable
velocity in the corner taking the max acceleration into account like this:
Vcorner = SQRT ( Amax * R)
Where A max is the maximum possible acceleration which is known by the setup
and R is the calculated Radius depending on the angle between the segments
and the D value supplied in the G64 command.
This is basically the idea. If we draw it, it gets more clear:
Segment 2, V2

Alfa

Beta
D

Segment 1, V1

Segment 1 and segment 2 are 2 subsequent motion segments.
Alfa is the change of direction angle between the segments.
Beta is the angle between the lines to fit the circle.
D is the user supplied max deviation between junction and the circle, this
determines how far the junction speed is limited.
R is the calculated radius from D and Beta.
So D is the parameter that determines the amount of speed reduction in the
corner. Practical values are in the order of 0.01 .. 0.0001 for D. The smaller the
value the smaller the circle radius, the smaller the velocity in the corner.
09 November 2018

Release 4.03

149

EDING CNC

Manual

This value needs to be tuned by experimenting on the target machine, if the
value is too high the machine will move jerky. Note that the corner is not
actually traveled, the original path is traveled, but the corner velocity is limited
as if there was an arc between the segments.
Both new and old algorithm co-exist in the proto software. So the user can
specify 2 angles and the D parameters now with G64 together with existing P
parameter.
G64 P.. R.. S.. D..
P: Parameter for max rounding when blending
R: LAF angle for standard algorithm where LAF will travel full speed of angle is
lower.
S: 2nd angle, the new algorithm will work between the R.. angle and S.. angle.
D: deviation of virtual circle in the corner used in the algorithm.
Example: G64 P0.1 R3 S90 D0.001
Full speed when angle is less than R angle.
Reduced speed depending on D when angle is between the R and S angle. For
angles bigger than S.. angle blending kicks in and uses the P.. as tolerance.

G64 P.. Q.. R.. S.. D.. F..
There are 6 parameters which can be combined with G64.
For normal milling, mostly G64 P.. is used.

09 November 2018

Release 4.03

150

EDING CNC

Manual

3.6.17 Coordinate system rotation G68
G68 X.. Y.. Z.. I.. J.. K.. R..
X.. Y.. Z.. :

Optional Specifies to rotation point, if not given, the current Work
Zero point is used.

I.. J.. K.. :

Optional, without I J K the rotation takes place in the actual
PLANE G17/G18/G19. Either I1 or J1 or K1 can be used, not a
combination.
I1 rotation about X in YZ plane, J1 rotation about Y in XZ plane,
K1 rotation about Z in XY plane.

R Rotation angle in degrees, positive is counter-clockwise, negative is clockwise.
X Y Rotation point in current coordinate system.
Use G69 to switch off G68.

3.6.18 Threading (Lathe) – G76

G76 P- Z- I- J- R- K- Q- H- E- LP Pitch
Z driveline endpoint
I Outside thread diameter, always positive.
J First cut is J beyond I, always positive.
R Depth regression, use 1.0 for constant cutting depths or leave parameter
away.
K Full thread depth beyond thread peak, always positive.
Q Compound slide angle, typical 30.
H Additional spring passes at full depth, use 0 for none.
E Taper distance along drive line.
L Taper place, none, enter, exit, both.
;Create a thread from z=20 to z=10, outside diameter=15, inside diameter=14,
10 passes.
G0 X20 Z20
G76 P1.0 Z10 I15 J0.1 K1.0
It is an error if:
•
•
•
•
•
•

The active plane is not the ZX plane
Other axis words, such as X- or Y-, are specified
The R- degression value is less than 1.0.
All the required words are not specified
P-, J-, K- or H- is negative
E- is greater than half the drive line length

09 November 2018

Release 4.03

151

EDING CNC

Manual

The “drive line” is a safe line outside the thread material. The “drive line” goes
from the initial location to the Z- value specified with G76. The Z extent of the
thread is the same as the drive line.
The “thread pitch”, or distance per revolution, is given by the P- value.
The “thread peak” is given by the I- value, which is an offset from the drive line.
Negative I values indicate external threads, and positive I values indicate
internal threads. Generally the material has been turned to this size before the
G76 cycle.
The “initial cut depth” is given by the J- value. The first threading cut will be J
beyond the “thread peak” position. J- is positive, even when I- is negative.
The “full thread depth” is given by the K- value. The final threading cut will be K
beyond the “thread peak” position. K- is positive, even when I- is negative.
The “depth degression” is given by the R- value. R1.0 selects constant depth on
successive threading passes. R2.0 selects constant area. Values between 1.0
and 2.0 select decreasing depth and increasing area. Values above 2.0 select
decreasing area. Beware that unnecessarily high degression values will cause a
large number of passes to be used.
The “compound slide angle” Q- is the angle (in degrees) describing to what
extent successive passes should be offset along the drive line. This is used to
cause one side of the tool to remove more material than the other. A positive Q
value causes the leading edge of the tool to cut more heavily. Typical values are
29, 29.5 or 30.
The number of “spring passes” is given by the H- value. Spring passes are
additional passes at full thread depth. If no additional passes are desired,
program H0.
Tapered entry and exit moves can be programmed using E- and L-. E- gives a
distance along the drive line used for the taper. E0.2 will give a taper for the
first/last 0.2 length units along the thread. L- is used to specify which ends of
the thread get the taper. Program L0 for no taper (the default), L1 for entry
taper, L2 for exit taper, or L3 for both entry and exit tapers.
The tool will pause briefly for synchronization before each threading pass, so a
relief groove will be required at the entry unless the beginning of the thread is
past the end of the material or an entry taper is used.
Unless using an exit taper, the exit move (traverse to original X) is not
synchronized to the spindle speed. With a slow spindle, the exit move might
take only a small fraction of a revolution. If the spindle speed is increased after
several passes are complete, subsequent exit moves will require a larger portion
of a revolution, resulting in a very heavy cut during the exit move. This can be
avoided by providing a relief groove at the exit, or by not changing the spindle
speed while threading.

09 November 2018

Release 4.03

152

EDING CNC

Manual

The sample program g76.ngc shows the use of the G76 canned cycle, and can
be previewed and executed on any machine using the sim/lathe.ini
configuration.

Figure: G76 canned cycle

09 November 2018

Release 4.03

153

EDING CNC

Manual

This is how it works:
1) Before the start, the spindle rate is measured.
2) The feed for de z-axis is calculated: F = pitch * spindleRate
3) The CPU programmed such that a movement is started on the spindle
pulse.
4) The movement is calculated and send to the CPU.
5) The movement is started when the spindle pulse passes.
6) Before the treading starts, the spindle-rate is measured, averaged and
the feed is calculated from this.
Not that the inside and outside thread diameter are determined by the start
position, the position before G76 and the I, K parameters.

3.6.19 Cancel Modal Motion - G80
Program G80 to ensure no axis motion will occur.
It is an error if:
• Axis words are programmed when G80 is active, unless a modal group 0
G code is programmed which uses axis words.

3.6.20 Canned Cycles - G81 to G89
The canned cycles G81 through G89 have been implemented as described in
this section. Two examples are given with the description of G81 below.
All canned cycles are performed with respect to the currently selected plane.
Any of the three planes (XY, YZ, and ZX) may be selected. Throughout this
section, most of the descriptions assume the XY-plane has been selected. The
behavior is always analogous if the YZ or XZ-plane is selected.
Rotational axis words are allowed in canned cycles, but it is better to omit them.
If rotational axis words are used, the numbers must be the same as the current
position numbers so that the rotational axes do not move.
All canned cycles use X, Y, R, and Z numbers in the NC code. These numbers
are used to determine X, Y, R, and Z positions. The R (usually meaning retract)
position is along the axis perpendicular to the currently selected plane (Z-axis
for XY-plane, X-axis for YZ-plane, Y-axis for XZ-plane). Some canned cycles use
additional arguments.
For canned cycles, we will call a number "sticky" if, when the same cycle is used
on several lines of code in a row, the number must be used the first time, but is
optional on the rest of the lines. Sticky numbers keep their value on the rest of
the lines if they are not explicitly programmed to be different. The R number is
always sticky.

09 November 2018

Release 4.03

154

EDING CNC

Manual

In incremental distance mode: when the XY-plane is selected, X, Y, and R
numbers are treated as increments to the current position and Z as an
increment from the Z-axis position before the move involving Z takes place;
when the YZ or XZ-plane is selected, treatment of the axis words is analogous.
In absolute distance mode, the X, Y, R, and Z numbers are absolute positions in
the current coordinate system.
The L number is optional and represents the number of repeats. L=0 is not
allowed. If the repeat feature is used, it is normally used in incremental distance
mode, so that the same sequence of motions is repeated in several equally
spaced places along a straight line. In absolute distance mode, L > 1 means "do
the same cycle in the same place several times," Omitting the L word is
equivalent to specifying L=1. The L number is not sticky.
When L>1 in incremental mode with the XY-plane selected, the X and Y
positions are determined by adding the given X and Y numbers either to the
current X and Y positions (on the first go-around) or to the X and Y positions at
the end of the previous go-around (on the repetitions). The R and Z positions do
not change during the repeats.
The height of the retract move at the end of each repeat (called "clear Z" in the
descriptions below) is determined by the setting of the retract mode: either to
the original Z position (if that is above the R position and the retract mode is
G98, OLD_Z), or otherwise to the R position. See Section 3.6.20
It is an error if:
• X, Y, and Z words are all missing during a canned cycle,
• a P number is required and a negative P number is used,
• an L number is used that does not evaluate to a positive integer,
• rotational axis motion is used during a canned cycle,
• inverse time feed rate is active during a canned cycle,
• cutter radius compensation is active during a canned cycle.
When the XY plane is active, the Z number is sticky, and it is an error if:
• the Z number is missing and the same canned cycle was not already
active,
• the R number is less than the Z number.
When the XZ plane is active, the Y number is sticky, and it is an error if:
• the Y number is missing and the same canned cycle was not already
active,
• the R number is less than the Y number.
When the YZ plane is active, the X number is sticky, and it is an error if:
• the X number is missing and the same canned cycle was not already
active,
• the R number is less than the X number.
3.6.20.1
PRELIMINARY AND IN-BETWEEN MOTION
At the very beginning of the execution of any of the canned cycles, with the XYplane

09 November 2018

Release 4.03

155

EDING CNC

Manual

selected, if the current Z position is below the R position, the Z-axis is traversed
to the R position. This happens only once, regardless of the value of L.
In addition, at the beginning of the first cycle and each repeat, the following one
or two moves are made:
1. a straight traverse parallel to the XY-plane to the given XY-position,
2. a straight traverse of the Z-axis only to the R position, if it is not already
at the R position.
If the XZ or YZ plane is active, the preliminary and in-between motions are
analogous.
3.6.20.2
G81 CYCLE
The G81 cycle is intended for drilling. Program G81 X… Y… Z… A… B… C…
R… L…
1. Preliminary motion, as described above.
2. Move the Z-axis only at the current feed rate to the Z position.
3. Retract the Z-axis at traverse rate to clear Z.
Example: Suppose the current position is (1, 2, and 3) and the XY-plane has
been selected, and the following line of NC code is interpreted.
G90 G81 G98 X4 Y5 Z1.5 R2.8
This calls for absolute distance mode (G90) and OLD_Z retract mode (G98) and
calls for the G81 drilling cycle to be performed once. The X number and X
position are 4. The Y number and Y position are 5. The Z number and Z position
are 1.5. The R number and clear Z are 2.8. Old Z is 3. The following moves take
place.
1. a traverse parallel to the XY-plane to (4,5,3)
2. a traverse parallel to the Z-axis to (4,5,2.8)
3. a feed parallel to the Z-axis to (4,5,1.5)
4. a traverse parallel to the Z-axis to (4,5,3)
Example: Suppose the current position is (1, 2, and 3) and the XY-plane has
been selected, and the following line of NC code is interpreted.
G91 G81 G98 X4 Y5 Z-0.6 R1.8 L3
This calls for incremental distance mode (G91) and OLD_Z retract mode (G98)
and calls for the G81 drilling cycle to be repeated three times. The X number is
4, the Y number is 5, the Z number is -0.6 and the R number is 1.8. The initial X
position is 5 (=1+4), the initial Y position is 7 (=2+5), the clear Z position is 4.8
(=1.8+3), and the Z position is 4.2 (=4.8-0.6). Old Z is 3.
The first move is a traverse along the Z-axis to (1,2,4.8), since old Z < clear Z.
The first repeat consists of 3 moves.
1. a traverse parallel to the XY-plane to (5,7,4.8)
2. a feed parallel to the Z-axis to (5,7, 4.2)
3. a traverse parallel to the Z-axis to (5,7,4.8)

09 November 2018

Release 4.03

156

EDING CNC

Manual

The second repeat consists of 3 moves. The X position is reset to 9 (=5+4) and
the Y position to 12 (=7+5).
1. a traverse parallel to the XY-plane to (9,12,4.8)
2. a feed parallel to the Z-axis to (9,12, 4.2)
3. a traverse parallel to the Z-axis to (9,12,4.8)
The third repeat consists of 3 moves. The X position is reset to 13 (=9+4) and
the Y position to 17 (=12+5).
1. a traverse parallel to the XY-plane to (13,17,4.8)
2. a feed parallel to the Z-axis to (13,17, 4.2)
3. a traverse parallel to the Z-axis to (13,17,4.8)
3.6.20.3
G82 CYCLE
The G82 cycle is intended for drilling. Program G82 X… Y… Z… A… R… L…
P…
1. Preliminary motion, as described above.
2. Move the Z-axis only at the current feed rate to the Z position.
3. Dwell for the P number of seconds.
4. Retract the Z-axis at traverse rate to clear Z.
3.6.20.4
G83 CYCLE
The G83 cycle (often called peck drilling) is intended for deep drilling or milling
with chip breaking. The retracts in this cycle clear the hole of chips and cut off
any long stringers (which are common when drilling in aluminum). This cycle
takes a Q number which represents a "delta" increment along the Z-axis.
Program G83 X… Y… Z… A… R… L… Q…
1. Preliminary motion, as described above.
2. Move the Z-axis only at the current feed rate downward by delta or to the
Z position, whichever is less deep.
3. Rapid back out to the clear_z.
4. Rapid back down to the current hole bottom, backed off a bit.
5. Repeat steps 1, 2, and 3 until the Z position is reached at step 1.
6. Retract the Z-axis at traverse rate to clear Z.
It is an error if:
• the Q number is negative or zero.
3.6.20.5 G73 CYCLE
The G73 cycle (often called peck drilling) is intended for deep drilling or milling
with chip breaking. The retracts in this cycle clear the hole of chips and cut off
any long stringers (which are common when drilling in aluminum). This cycle
takes a Q number which represents a "delta" increment along the Z-axis.
Program G73 X… Y… Z… A… R… L… Q…
1. Preliminary motion, as described above.
2. Move the Z-axis only at the current feed rate downward by delta or to the
Z position, whichever is less deep.
3. Rapid back out but only with increment Q, this is the difference with G83
above.
4. Rapid back down to the current hole bottom, backed off a bit.
5. Repeat steps 1, 2, and 3 until the Z position is reached at step 1.
6. Retract the Z-axis at traverse rate to clear Z.
09 November 2018

Release 4.03

157

EDING CNC

Manual

It is an error if:
• the Q number is negative or zero.
3.6.20.6
G84 CYCLE
The G84 cycle is intended for right hand tapping.
Program G84 X… Y… Z… A… B… C… R… L…
1. Preliminary motion, as described above.
2. Move the Z-axis only at the current feed rate/per revolution to the Z
position.
So assume the spindle is running M3 S600. Then and F value of F1 will
give A feed of 600 /minute. Feed starts synchronized with spindle pulse
allowing to tap the same hole again.
3. When Z position reached, reverse spindle M4. (Waits until spindle rampup and new measurement of spindle speed)
4. Retract the Z-axis at the current feed rate to clear Z.
3.6.20.7
G74 CYCLE
The G74 cycle is intended for left hand tapping.
Program G74 X… Y… Z… A… B… C… R… L…
5. Preliminary motion, as described above.
6. Move the Z-axis only at the current feed rate/per revolution to the Z
position.
So assume the spindle is running M3 S600. Then and F value of F1 will
give A feed of 600 /minute. Feed starts synchronized with spindle pulse
allowing to tap the same hole again.
7. When Z position reached, reverse spindle M4. (Waits until spindle rampup and new measurement of spindle speed)
8. Retract the Z-axis at the current feed rate to clear Z.

3.6.20.8
G85 CYCLE
The G85 cycle is intended for boring or reaming, but could be used for drilling or
milling. Program G85 X… Y… Z… A… B… C… R… L…
Preliminary motion, as described above.
Move the Z-axis only at the current feed rate to the Z position.
Retract the Z-axis at the current feed rate to clear Z.
3.6.20.9
G86 CYCLE
The G86 cycle is intended for boring. This cycle uses a P number for the number
of seconds to dwell. Program G86 X… Y… Z… A… B… C… R… L… P…
Preliminary motion, as described above.
Move the Z-axis only at the current feed rate to the Z position.
Dwell for the P number of seconds.
Stop the spindle turning.
Retract the Z-axis at traverse rate to clear Z.
Restart the spindle in the direction it was going.
The spindle must be turning before this cycle is used. It is an error if:
the spindle is not turning before this cycle is executed.
09 November 2018

Release 4.03

158

EDING CNC

Manual

3.6.20.10
G87 CYCLE
The G87 cycle is intended for back boring.
Program G87 X… Y… Z… A… R… L… I… J… K…
The situation, as shown in Figure 3-1, is that you have a through hole and you
want to counter bore the bottom of hole. To do this you put an L-shaped tool in
the spindle with a cutting surface on the UPPER side of its base. You stick it
carefully through the hole when it is not spinning and is oriented so it fits
through the hole, then you move it so the stem of the L is on the axis of the
hole, start the spindle, and feed the tool upward to make the counter bore.
Then you stop the tool, get it out of the hole, and restart it.
This cycle uses I and J numbers to indicate the position for inserting and
removing the tool. I and J will always be increments from the X position and the
Y position, regardless of the distance mode setting. This cycle also uses a K
number to specify the position along the Z-axis of the controlled point top of the
counter bore. The K number is a Z-value in the current coordinate system in
absolute distance mode, and an increment (from the Z position) in incremental
distance mode.
1. Preliminary motion, as described above.
2. Move at traverse rate parallel to the XY-plane to the point indicated by I
and J.
3. Stop the spindle in a specific orientation.
4. Move the Z-axis only at traverse rate downward to the Z position.
5. Move at traverse rate parallel to the XY-plane to the X,Y location.
6. Start the spindle in the direction it was going before.
7. Move the Z-axis only at the given feed rate upward to the position
indicated by K.
8. Move the Z-axis only at the given feed rate back down to the Z position.
9. Stop the spindle in the same orientation as before.
10.Move at traverse rate parallel to the XY-plane to the point indicated by I
and J.
11.Move the Z-axis only at traverse rate to the clear Z.
12.Move at traverse rate parallel to the XY-plane to the specified X,Y
location.
13.Restart the spindle in the direction it was going before.
When programming this cycle, the I and J numbers must be chosen so that
when the tool is stopped in an oriented position, it will fit through the hole.
Because different cutters are made differently, it may take some analysis and/or
experimentation to determine appropriate values for I and J.

09 November 2018

Release 4.03

159

EDING CNC

Manual

3.6.20.11
G88 CYCLE
The G88 cycle is intended for boring. This cycle uses a P word, where P specifies
the
number of seconds to dwell. Program G88 X… Y… Z… A… R… L… P…
Preliminary motion, as described above.
1. Move the Z-axis only at the current feed rate to the Z position.
2. Dwell for the P number of seconds.
3. Stop the spindle turning.
4. Stop the program so the operator can retract the spindle manually.
5. Restart the spindle in the direction it was going.
3.6.20.12
G89 CYCLE
The G89 cycle is intended for boring. This cycle uses a P number, where P
specifies the
number of seconds to dwell. program G89 X… Y… Z… A… R… L… P…
1. Preliminary motion, as described above.
2. Move the Z-axis only at the current feed rate to the Z position.
3. Dwell for the P number of seconds.
4. Retract the Z-axis at the current feed rate to clear Z.

3.6.21 Set Distance Mode - G90 and G91
To make the current point have the coordinates you want (without motion),
program G92 X… Interpretation of RS274/NGC code can be in one of two
distance modes: absolute or incremental.
To go into absolute distance mode, program G90. In absolute distance mode,
axis numbers (X, Y, Z, A, B, C) usually represent positions in terms of the
currently active coordinate system.
To go into incremental distance mode, program G91. In incremental distance
mode, axis numbers (X, Y, Z, A, B, C) usually represent a distance from the
current values of the numbers.

09 November 2018

Release 4.03

160

EDING CNC

Manual

I and J numbers always represent increments, regardless of the distance mode

3.6.22 Coordinate System Offsets - G92, G92.1, G92.2, G92.3
To make the current point have the coordinates you want (without motion),
program
G92 X… Y… Z… A… , where the axis words contain the axis numbers you
want. All axis words are optional, except that at least one must be used. If an
axis word is not used for a given axis, the coordinate on that axis of the current
point is not changed.
It is an error if:
• all axis words are omitted.
When G92 is executed, the origin of the currently active coordinate system
moves. To do this, origin offsets are calculated so that the coordinates of the
current point with respect to the moved origin are as specified on the line
containing the G92. In addition, parameters 5211 to 5216 are set to the X, Y, Z,
A, B, and C-axis offsets. The offset for an axis is the amount the origin must be
moved so that the coordinate of the controlled point on the axis has the
specified value.
Here is an example. Suppose the current point is at X=4 in the currently
specified coordinate system and the current X-axis offset is zero, then G92 x7
sets the X-axis offset to -3, sets parameter 5211 to -3, and causes the Xcoordinate of the current point to be 7.
The axis offsets are always used when motion is specified in absolute distance
mode using any of the nine coordinate systems (those designated by G54 G59.3). Thus all nine coordinate systems are affected by G92.
Being in incremental distance mode has no effect on the action of G92.
Non-zero offsets may already be in effect when the G92 is called. If this is the
case, the new value of each offset is A+B, where A is what the offset would be if
the old offset were zero, and B is the old offset. For example, after the previous
example, the X-value of the current point is 7. If G92 x9 is then programmed,
the new X-axis offset is -5, which is calculated by [[7-9] + -3].
To reset axis offsets to zero, program G92.1 or G92.2. G92.1 sets parameters
5211 to 5216 to zero, whereas G92.2 leaves their current values alone.
To set the axis offset values to the values given in parameters 5211 to 5216,
program G92.3.
You can set axis offsets in one program and use the same offsets in another
program. Program G92 in the first program. This will set parameters 5211 to
5216. Do not use G92.1 in the remainder of the first program. The parameter
values will be saved when the first program exits and restored when the second
one starts up. Use G92.3 near the beginning of the second program. That will
restore the offsets saved in the first program. If other programs are to run
between the program that sets the offsets and the one that restores them,

09 November 2018

Release 4.03

161

EDING CNC

Manual

make a copy of the parameter file written by the first program and use it as the
parameter file for the second program.

3.6.23 Set Feed Rate Mode - G93, G94, G95
Three feed rate modes are recognized, depending on selected mode the Feed of
the axes is calculated differently:
• G93 inverse time, a move is completed in 1/F minutes. For example if F=6
the move is completed in 10 seconds. When G93 is active, the F must be
specified on every line containing G1,G3 or G3.
• G94 units per minute, this is the normal mode for milling, F means units
per minute, in millimeter mode mm/minute, in INCH mode inch/minute.
• G95 Units per revolution, here the F word is the number of units that
should be cut per spindle revolution. So the feed of the axes is depending on
the rotation speed of the spindle. G95 F2 means cut 2mm every spindle
revolution, so when S=500, the feed for XZ would be FEED = F * S = 2 *
500 = 1000.

3.6.24 Spindle Control Mode – G96, G97
Two spindle control modes are possible, depending on the mode the spindle
speed is calculated differently:
• G96 (Only for Lathe), select constant surface speed, S is now specified as
meters per minute in mm mode (G21) or Feet per minute in inch mode
(G20). This means that the spindle speed is adapted automatically when the
Radius changes. Suppose you program G96 S150 in millimeter mode, the
spindle speed is calculated by: RPM = S / (2 * PI * X), X is the radius. So
your X zero must be where the diameter is zero.
Example: Your actual X position is 100 (100 millimeter = 0.1 meter), you
program G96 S150 D1000, this would result in a spindle RPM of 150 / (2 * PI
* 0.1) = 238.7 rev/min. D1000 limits the maximum speed to 1000 RPM.
•
G97 is normal RPM mode, S specifies the RPM.

3.6.25 Set Canned Cycle Return Level - G98 and G99
When the spindle retracts during canned cycles, there is a choice of how far it
retracts:
(1) retract perpendicular to the selected plane to the position indicated by the R
word, or
(2) retract perpendicular to the selected plane to the position that axis was in
just before the canned cycle started (unless that position is lower than the
position indicated by the R word, in which case use the R word position).
To use option (1), program G99. To use option (2), program G98. Remember
that the R word has different meanings in absolute distance mode and
incremental distance mode.

09 November 2018

Release 4.03

162

EDING CNC

3.7

Manual

INPUT M CODES

M codes of the RS274/NGC language are shown in Table 3-6
Table 3-6 M Codes
M
Code
M0
M1
M2
M3
M4
M5
M6
M7
M8
M9
M20
M21
M22
M30
M48
M49
M60

Meaning
program stop
optional program stop
program end
turn spindle clockwise
turn spindle counterclockwise
stop spindle turning
tool change
mist coolant on
flood coolant on
mist and flood coolant off
Plasma Torch Height Control ON
Plasma Torch Height Control OFF
M23 Q.. Set Plasma THC set point value;
program end, spindle and coolants off and rewind.
enable speed and feed overrides
disable speed and feed overrides
program stop, use this with nesting instead of M60, so that the
spindle/coolants remain on during transition from one to the next
run.

M54
M55
M56
M80
M81

set general purpose output for CPU5B
clear general purpose output for CPU5B
read general purpose input for CPU5B
Drive enable ON
Drive enable OFF

M90
M91
M93
M95
M97

Standard
Alternate
Alternate
Alternate
Alternate

Head/spindle
Head/2nd spindle
Head/3rd spindle
Head/Probe
Head/Camera

Note that a head may as well be e.g. a tangential knife
configuration
M104
M106
M107
M109
M143
M140

Specials for 3D printing
M104 S.. Set extruder temperature, (M104 S50, sets
temperature to 50 degree Celsius).
M106 S.. Work piece cooling FAN ON optionally with S=0-255,
for 0-100% PWM.
M107 Work piece FAN off.
M109 S.. Set extruder temperature and wait until reached.
M143 S.. Maximum Hot-end temperature to prevent overheating.
M140 S.. Bed temperature.

09 November 2018

Release 4.03

163

EDING CNC

M190

3.7.1

Manual

M190 Wait for bed temperature reached target.

Program Stopping and Ending - M0, M1, M2, M30, M60

To halt a running program temporarily, program M0. If a program is stopped
by an M0, pressing the cycle start button will restart the program at the
following line, so the program will continue.
To optionally halt a program when the stopM1 check in the user interface is
checked program M1
program M30 for next effects:
•
•
•
•
•
•
•
•
•
•
•

Selected plane is set to CANON_PLANE_XY (like G17).
Distance mode is set to MODE_ABSOLUTE (like G90).
Feed rate mode is set to UNITS_PER_MINUTE (like G94).
Feed and speed overrides are set to ON (like M48).
Cutter compensation is turned off (like G40).
The spindle is stopped (like M5).
The current motion mode is set to G_1 (like G1).
Coolants are turned off (like M9).
Note that the coordinate system are no longer reset, I modified this
behavior because I have broken a lot of bits due to this so I modified it.
Program is re-winded to the first line, ready for next start.
All 3D printer heating OFF.

Program M60 instead of M30 if the spindle and coolants should remain ON, this
is usefully with nesting.

3.7.2

Spindle/Head Control - M3, M4, M5, M90-M97

To start the spindle turning clockwise at the currently programmed speed,
program M3.
To start the spindle turning counterclockwise at the currently programmed
speed, program M4.
To stop the spindle from turning, program M5.
It is OK to use M3 or M4 if the spindle speed is set to zero. If this is done (or if
the speed override switch is enabled and set to zero), the spindle will not start
turning. If, later, the spindle speed is set above zero (or the override switch is
09 November 2018

Release 4.03

164

EDING CNC

Manual

turned up), the spindle will start turning. It is OK to use M3 or M4 when the
spindle is already turning or to use M5 when the spindle is already stopped.
If there are more than one spindles in your machine, or of you have a mounted
touch probe on th Z slide or a camera you can select the offset/IO you want
• M90 standard spindle
• M91 alternate 2nd spindle
• M92 alternate 3rd spindle
• M93 alternate 4th spindle
• M95 touch probe
• M97 Camera
Each spindle is connected to different set of outputs and has different
parameters.
Alternate spindle 1 and 2 may have defined offsets for x,y,z.
Because this option is rarely used by customers, you have to perform the
settings yourself by editing the cnc.ini file.
There are 5 sets of parameters for each spindle configuration. For the 2nd 3rd 4th
and 5th spindle configuration you can set the axis offsets with respect to the 1nd
spindle. Note that the 4th and 4th spindle configuration is used for a touch probe
and camera.
Example system:
1. Spindle, 2. tan knife, and possible 3. oscillating tan knife, 4. Touch probe, 5
Camera.
Because this function is used only by a few customers, it is left out of the setup
in the GUI. The settings have to be added manually in the cnc.ini settings file:
[SPINDLE_0]
spindleRampUpTime = 1.00
spindleNmax = 24000.00
spindleNmin = 1000.00
spindleUseRPMSensor = 0
onOffOutputPortID = 0 ;0: Standard tool output, 1-9: AUX1-AUX9
directionOutputPortID = 0 ;0: Standard tool output, 1-9: AUX1-AUX9, -2: MIST COOLANT Output
pwmOutputPortID = 1 ;0: Standard PWM output, 1-3: PWM1-PWM3 Output
[SPINDLE_1]
spindleRampUpTime = 1.00
spindleNmax = 24000.00
spindleNmin = 1000.00
spindleUseRPMSensor = 0
onOffOutputPortID = 0 ;0: Standard tool output, 1-9: AUX1-AUX9
directionOutputPortID = 0 ;0: Standard tool output, 1-9: AUX1-AUX9, -2: MIST COOLANT Output
pwmOutputPortID = 1 ;0: Standard PWM output, 1-3: PWM1-PWM3 Output
xOffset = 0.0000
yOffset = 0.0000
zOffset = 0.0000
[SPINDLE_2]
spindleRampUpTime = 1.00
spindleNmax = 24000.00
spindleNmin = 1000.00
spindleUseRPMSensor = 0
onOffOutputPortID = 0 ;0: Standard tool output, 1-9: AUX1-AUX9
directionOutputPortID = 0 ;0: Standard tool output, 1-9: AUX1-AUX9, -2: MIST COOLANT Output

09 November 2018

Release 4.03

165

EDING CNC

Manual

pwmOutputPortID = 1 ;0: Standard PWM output, 1-3: PWM1-PWM3 Output
xOffset = 0.0000
yOffset = 0.0000
zOffset = 0.0000
[SPINDLE_3]
;Mounted Probe M95
xOffset = 0.0000
yOffset = 0.0000
zOffset = 0.0000
onOffOutputPortID = 0 ;0: Standard tool output, 1-9: AUX1-AUX9
[SPINDLE_4]
;Mounted camera M97
xOffset = 0.0000
yOffset = 0.0000
zOffset = 0.0000
onOffOutputPortID = 0 ;0: Standard tool output, 1-9: AUX1-AUX9

The x,y,z Offset parameter for the [SPINDLE_1] and [SPINDLE_2] [SPINDLE_3]
and [SPINDLE_4] configuration are offsets with respect to [SPINDLE_0]. Every
spindle has its own parameters including IO ports for switching on/off and
controlling the speed.

3.7.3

Tool Change - M6

To change a tool in the spindle from the tool currently in the spindle to the tool
most
recently selected (using a T word - see Section 3.7.3), program M6. When the
tool change is complete:
• The spindle will be stopped.
• The tool that was selected (by a T word on the same line or on any line
after the previous tool change) will be in the spindle. The T number is an
integer giving the changer slot of the tool (not its id).
• If the selected tool was not in the spindle before the tool change, the tool
that was in the spindle (if there was one) will be in its changer slot.
• The coordinate axes will be stopped in the same absolute position they
were in before the tool change (but the spindle may be re-oriented).
• No other changes will be made. For example, coolant will continue to flow
during the tool change unless it has been turned off by an M9.
The tool change may include axis motion while it is in progress. It is OK (but not
useful) to program a change to the tool already in the spindle. It is OK if there is
no tool in the selected slot; in that case, the spindle will be empty after the tool
change. If slot zero was last selected, there will definitely be no tool in the
spindle after a tool change.
The tool change command will call the change_tool subroutine inside
macro.cnc.
You can adapt the behavior for your own needs in this function e.g:
• Perform automatic tool-length measurement
• Perform tool change with an automatic tool changer.
For a (nonfunctional) example of how to implement automatic tool change for a
16-tool changer. see the contents of the default_macro.cnc file at the end of
09 November 2018

Release 4.03

166

EDING CNC

Manual

this document. It checks whether current tool is already in the spindle. It check
that the tool number is in range of 1-4. Then it first drops current tool and picks
the new tool:

3.7.4

Coolant Control - M7, M8, M9

To turn mist coolant on, program M7. To turn flood coolant on, program M8. To
turn all coolant off, program M9. It is always OK to use any of these commands,
regardless of what coolant is on or off.

09 November 2018

Release 4.03

167

EDING CNC

3.7.5

Manual

Feed-Speed Override Control - M48-M53

M48 Enable feed and speed override, set back to last user feed override value.
M49 Disable feed and speed override and set to 100%
M50 P.. Set feed Override to given P value, if P value is less than zero feed
override is disabled and the value remains as is.
M51 P.. Set speed Override to given P value, if P value is less than zero speed
override is switched off.
M52 Enable feed Override by analog input. M52 P0 disable feed Override
by analog input. P1 is optional.
M53 Enable feed Hold input. M53 P0 disable feed Hold input. P1 is
optional.
To enable the speed and feed override switches, program M48. To disable both
switches, program M49.

3.7.6

Adaptive FeedOverride Control by spindle power

This function allows to change the feedOverride when the consumed power of
the spindle changes, higher Feed if the power goes lower, lower feed if the
power goes higher and complete stop id the power goes to high. The consumed
power is in this case an analogue output of the Spindle VFD that is connected to
one of the analogue inputs of the EdingCNC CPU.
These parameters are not part of the set-up UI, but are available in the set-up
file cnc.ini.
[FEEDSPEEDOVERRIDE]
feedOverideSource = 3
adaptiveSpindlePowerFeedOv = 1
analogFeedOvAtMaxVoltage = 20.000
analogFeedOvAtMinVoltage = 120.000
analogStopOnHigherTreshold = 0
feedOverideSource:
Select the analog output number to be used with feed override.
0: off
1: hand wheel
2: analog input 1
3: analog input 2
4: analog input 3
5: analog input 4
6: analog input 5
adaptiveSpindlePowerFeedOv:
0: Off
1: Adaptive control with spindle power.
analogFeedOvAtMaxVoltage:
0..300: FeedOverride percentage analog input is at Max value.
(depending on CPU 3.3 or 10V).

09 November 2018

Release 4.03

168

EDING CNC

Manual

analogFeedOvAtMinVoltage:
0..300: FeedOverride percentage analog input is at zero Volt value.
analogStopOnHigherTreshold:
0: Off
1..1023: Analog value threshold for stop when consumed power is too high.
The Pause command is executed if this happends.
(For CPU 5 and 6 series, For CPU7 series `1..4096)
To control this function at runtime, the M52 command is extended:
M52 P.. Q.. R.. S..
P: 0 -> Function is OFF, 1 -> function is ON.
Q: 0..300 Set analogFeedOvAtMinVoltage
R: 0..300 Set analogFeedOvAtMaxVoltage
S: 0..1023 Set threshold value.

3.7.7

Standard CNC IO - M3..M9, M80..M87

To control the outputs, these functions have been added besides the standard
M-Functions.
Standard, according to [NIST]
M3 PWM according S value, TOOLDIR = on
M4 PWM according S value, TOOLDIR = off
M5 PWM off, TOOLDIR off.
M7 Mist on
M8 Flood on
M9 Mist/Flood off

3.7.8

General purpose IO M54, M55, M56, M57

M54 Px
Set output x.
M54 P1 (set AUX1 out to 1)
M54 Ex Qy
Set PWM output x to promille value y (0 <= y <= 1000)
M54 E2 Q500 (Set PWM2 to 50% PWM)
M55 Px
Clear output x.
M55 P1 (set AUX1 out to 0)
M56 Px
Read input x. result stored on #5399
09 November 2018

Release 4.03

169

EDING CNC

Manual

M56 P3 (Read AUX in 3)
If [#5399 == 1]
Msg “AUX3=ON”
Else
Msg “AUX3=OFF”
endif
M56 Px Ly Qy
Read digital input and specify wait mode, result stored in #5399
Px: x is input number
L0: do not wait
L1: Wait for High
L2: Wait for Low
Qy: y is timeout
M56 P3 L2 Q30 (Read AUX in 3)
If [#5399 == -1]
Errmsg “Timeout while waiting for AUX3 becoming low”
Else
Msg “AUX3 is off”
Endif
Note that we use wait (L2) here, in case if time-out, the value of #5399 is -1.
To make this code simulation and rendering proof we need to extend it like this,
this is explained further in chapter:
4.4 RUN BEHAVIOR DURING SIMULATION AND RENDER
If [[#5380 == 0] and [#5397 == 0]] ;;Check only if running job
M56 P3 L2 Q30 (Read AUX in 3)
If [#5399 == -1]
Errmsg “Timeout while waiting for AUX3 becoming low”
Else
Msg “AUX3 is off”
Endif
Endif
M56 Ex
Read analogue input, result stored in #5399
Ex: x is input number
M56 E3
Msg “analog value is ”#5399
Read other inputs using M56
M56 Px
Home Inputs

x = 51 – 56 (X .. C)

09 November 2018

Release 4.03

170

EDING CNC

Probe Input
Sync Input
HWA Input
HWB Input
ESTOP1
ESTOP2
EXTERR
PAUSE

Manual

:
:
:
:
:
:
:
:

x = 61
x = 62
x = 63
x = 64
x = 65
x = 66
x = 67
x = 68

Example, read home-input of X axis:
M56 P51
If [#5399 == 1]
Msg “HOMEX=ON”
Else
Msg “HOMEX=OFF”
endif
Read outputs using M57
Read output X, store result in #5399
M57 Px
AUX1-AUXn
Machine On
Drive Enable
Coolant1 (Flood)
Coolant2 (Mist)
Tool
Tool direction

:
:
:
:
:
:
:

x= 1..n
x = 51
x = 52
x = 61
x = 62
x = 63
x = 64

M57 Ex
Read PWM output, result stored in #5399
Ex: x is PWM number
PWM1-PWMn
:
x=1..n
Example, read PWM 3:
M57 E3
If [#5399 == 0]
Msg “PWM IS OFF”
Else
Msg “PWM IS ON, VALUE=”#5399
endif

Optional IOCARD
If the new I2C or RS485 GPIO CARD is used, the IO number P or E is specified
as follows:
103 means card 1 port 3.
208 means card 2 port 8
09 November 2018

Release 4.03

171

EDING CNC

3.7.9

Manual

A axis clamping M26, M27

The A axis is often used to rotate the work piece on the machine and then do
milling on that side of the work piece. To be sure the work piece is fixed at its
place an axis clamp (Brake) can be used for A.
M26 P1 enables the clamp and the optional P1 specifies the output that controls
the brake, P1 means AUX 1. (See also M54)
M27 P1 disables the clamp and the optional P1 here specifies the output
controlling the brake.
When M26 is active, the software does not accept movements g-code and
jogging, an error message will appear that the A axis is clamped.

3.7.10 Torch height control M20, M21, M22
M20 - THC off
M21 - THC on
M22 Q.. – THC setpoint voltage

3.7.11 M Functions for Lasermode (CNC7.. series CPU’s)
M10 - laser off
M11 - laser on
If the command “LaserEngrave” On was given this kind of code is possible:
LaserEngrave ON
M10
G1 F.. X..
M11
G1 X..
M10 X..
G1 X..
LaserEngrave OFF
M30
The laser on/off m11 and m10 are executed while moving exactly on the right position.

3.7.12 M Functions for 3D printing
M1
:All heating and Fans off
M104 S :Set extruder temperature, (M104 S50, sets temperature to 50
degree Celsius).
M106 S.. : Work piece cooling FAN ON optionally with S=0-100, for 0-100%
PWM
M107
:Work piece FAN off .
M109 S.. :Set extruder temperature and wait until reached.
M143 S.. :Maximum Hot-end temperature to prevent overheating.
M140 S.. :Bed temperature
M143 S.. :Set max extruder temperature
M190 S.. :Set Bed temperature and wait until reached.
09 November 2018

Release 4.03

172

EDING CNC

Manual

M100 P.. :Change a axis resolution on the fly by a factor (factor 1 is standard,
1.01 is 1% more, 0.99 is 1% less.

3.7.13 M Function override and user m-functions
The system allows M functions in the range of M1..M999.
This means there are many un-used m-functions.
The user can create his own M-Function by creating a subroutine for it in the
macro.cnc. or usermacro.cnc file
e.g:
sub m100
;Do your stuff here
Msg “my M100”
M54 p1; switch on AUX output 1
endsub

So if the g-code file performs M100, the subroutine will be called.
Also parameters in the form M100 S100 is possible.
In the subroutine the parameter can be accessed using #19 (#1 .. #26
accesses parameter A..Z), S is number 19 in the alphabet.
This creates further possibilities:
It is possible to override existing M functions as well.
Suppose you want additional function for M3 which is spindle on standard.
If you spindle has an output speed-reached, you can wait for it like this:
sub m3
msg "my customized m3"
m3 s#19;The real m3, inside sub routine this m3 will execute the real m3
m56 P1 L2 Q60 ; Wait max. 1 minute for input 1 to become low
endsub

When you are inside your m3 subroutine and perform an m3, then the
subroutine is not called, but the default m3 is called in stead.
There are some limitations on using the M Function override:
• There must be nothing else on the G-code line as the M-Function, e.g.
N2000 M3 S1000 is OK.
N2000 M3 M8 G1X100 is NOT OK!
•

The user parameters 1-26 will be used as parameter and will be
overwritten when M-Function subroutines are used. Take this into account
and do not use #1..#26 in your program if you use this functionality.
Variable 1-26 match with the letter of the alphabet, #1 will get the value
of parameter A, #26 will get the value of parameter Z.

09 November 2018

Release 4.03

173

EDING CNC

3.8
3.8.1

Manual

OTHER INPUT CODES
Set Feed Rate - F

To set the feed rate, program F… . The application of the feed rate is as
described in
Section 2.1.2.5, unless inverse time feed rate mode is in effect, in which case
the feed rate is as described in Section 3.6.23.

3.8.2

Set Spindle Speed - S

To set the speed in revolutions per minute (rpm) of the spindle, program S… .
The spindle will turn at that speed when it has been programmed to start
turning. It is OK to program an S word whether the spindle is turning or not. If
the speed override switch is
enabled and not set at 100%, the speed will be different from what is
programmed. It is OK to program S0; the spindle will not turn if that is done.
The CPU’s that support PWM output will have its PWM value set conform the
requested spindle speed if the spindle is turned on.
It is an error if:
• the S number is negative.

3.8.3

Select Tool - T

To select a tool, program T…, where the T number is the carousel slot for the
tool. The tool is not changed until an M6 is programmed (see Section 3.7.3).
The T word may appear on the same line as the M6 or on a previous line. It is
OK, but not normally useful, if T words appear on two or more lines with no tool
change. The carousel may move a lot, but only the most recent T word will take
effect at the next tool change. It is OK to
program T0; no tool will be selected. This is useful if you want the spindle to be
empty after a tool change.
It is an error if:
• a negative T number is used,
• a T number larger than the number of slots in the carousel is used.
On some machines, the carousel will move when a T word is programmed, at
the same time machining is occurring. On such machines, programming the T
word several lines before a tool change will save time. A common programming
practice for such machines is to put the T word for the next tool to be used on
the line after a tool change. This maximizes the time available for the carousel
to move.

09 November 2018

Release 4.03

174

EDING CNC

3.9

Manual

ORDER OF EXECUTION

The order of execution of items on a line is critical to safe and effective machine
operation. Items are executed in the order shown in Table 3-7 if they occur on
the same line.
Table 3-7 Order of execution
1. comment (includes message).
2. set feed rate mode (G93, G94 -inverse time or per minute).
3. set feed rate (F).
4. set spindle speed (S).
5. select tool (T).
6. change tool (M6).
7. spindle on or off (M3, M4, M5).
8. coolant on or off (M7, M8, M9).
9. enable or disable overrides (M48, M49).
10.dwell (G4).
11.set active plane (G17, G18, G19).
12.set length units (G20, G21).
13.cutter radius compensation on or off (G40, G41, G42)
14.cutter length compensation on or off (G43, G49)
15.coordinate system selection (G54, G55, G56, G57, G58, G59,
G59.1, G59.2, G59.3).
16.set path control mode (G61, G61.1, G64)
17.set distance mode (G90, G91).
18.set retract mode (G98, G99).
19.home (G28, G30) or change coordinate system data (G10) or set
axis offsets (G92, G92.1, G92.2, G94).
20.perform motion (G0 to G3, G80 to G89), as modified (possibly) by
G53.
21.stop(M0,M1, M2,M30,M60).

09 November 2018

Release 4.03

175

EDING CNC

Manual

Language extensions

To provide additional flexibility, EdingCNC created some extensions in the
language that allow for flexible programming.

09 November 2018

Release 4.03

176

EDING CNC

4.1

Manual

FLOW CONTROL

You can use the following flow control commands in a job:
IF[x]-ELSE-ENDIF constructs to define x dependent execution
WHILE[x]-ENDWHILE constructs to define x dependent repeated execution
SUB -ENDSUB constructs to define a subroutine
GOSUB construct to call a subroutine

09 November 2018

Release 4.03

177

EDING CNC

4.2
4.2.1

Manual

SUPPORTED OPERATIONS ON EXPRESSIONS

unary operations

abs
acos
asin
atan[y]/[x]
cos
exp
fix
fup
int
ln
round
sin
sqrt
tan
not
ResetModulo

4.2.2
/
mod
**
*
and
xor
or
+
>
>=
<
<=
==
<>
band
bxor
bor
<<
>>

absolute value
arc cosine
arc sine
arc tangent
cosine
e raised to
round down
round
integer part
natural log of
round
sine
square root
tangent
logical not
[A|B|C] reset a rotation axis to its modulo position.

binary operations:
divided by
modulo
power
times
logic and
logic exclusive or
minus
logic nonexclusive or
plus
greater then
greater than or equal
less then
less than or equal
is equal
not equal
bitwise and
bitwise exclusive or
bitwise nonexclusive or
shift left
shift right

Some examples below.

09 November 2018

Release 4.03

178

EDING CNC

4.2.3

Manual

An example:

sub do_circle_holes
#100=0
g0 z1 x0 y0
while [#100 <> 360]
#102 = [10 * sin[#100]]
#103 = [10 * cos[#100]]
g0 x[#103] y[#102]
g1 z-1
g1 z1
#100 = [#100 + 30]
if [#100 == 360]
msg "Done"
else
msg "processing at angle "#100
endif
endwhile
endsub
gosub do_circle_holes
m30
This example drills holes at a circle with a radius of 10, each 30 degrees. The
code that performs this is put in a subroutine, which can be called as many
times as needed in the main program.

09 November 2018

Release 4.03

179

EDING CNC

4.3
4.3.1

Manual

SPECIAL INTERPRETER COMMANDS, NON G-CODE
Msg

Msg "Hello there, the value of #1 = "#1" and the value of #2 = "#2
Note: If you make a fast while loop generating a lot of messages in a short
time, messages may be lost because the message queuing is limited.

4.3.2

ErrMsg

Same as Msg, but this one generates an warning

4.3.3

WarnMsg

Same as Msg, but this one generates an error and stops the interpreter

4.3.4

LogFile, LogMsg

Log anything to a file, first create a new file or open the file using LogFile, then
write to the file using LogMsg.
LogFile <1=append, 0=open new>
LogMsg
Example:
LogFile “text.txt” 1
LogMsg “Hi, the current position of X is “#5001
Now check the contents of file text.txt.
Msg, LogMsg, WarnMsg, ErrMsg can now use %txx (xx = 0-99) and this will
show the tool description text.
Example: msg %t#5011 " is changed to "Tool number 5" this is text from the
tool table.

4.3.5

GetToolInfo

Get info from used tools inside job and store in given variable number.
Example:
GetToolInfo num 200 ➔ will store the number of used tools in job at #200
GetToolInfo first 201 ➔ will store first tool number at #201
GetToolInfo next 201 ➔ will store next tool number at #201
Practical example:
;Example to enumerate tools used in a job.
;Can e.g. be used to measure the length of all tools at once before runing the
job.
sub measure_used_tools
GetToolInfo num 5025 ;
Msg "number of tools used = " #5025

09 November 2018

Release 4.03

180

EDING CNC

Manual

;Note that 5025 is used as tool number in m_tool_no_dlg above.
GetToolInfo first 5025
while [#5025 <> -1]
gosub m_tool_no_dlg ;
msg "Tool "#5025" is measured"
GetToolInfo next 5025
endwhile
endsub

09 November 2018

Release 4.03

181

EDING CNC

4.3.6

Manual

DlgMsg

Gives a dialog message for an interactive g-code program.
DlgMsg ...

Example:
DlgMsg "Give parameters" par1 100 par2 101
The dialog woll have an OK and a Cancel button.
When the user selects OK, variable #5398 is set to 1 and the program
automatically continues. When the user selects CANCEL, variable #5398 is set
to -1, program continues. Just try and you will see what this is about.
if .png picture exist it will be show.
During render mode, when the program is loaded and parsed to show in the
graphics the dialogs will not appear logically, in that case #5398 is set to 1
indicating OK.
So you must give your variables a good predefined value that works.
You can also use “if [#5397 == 0]” this indicates normal running mode.
#5397 = 1 during the render mode.
EXAMPLE of dlg msg:
For this example we created a subroutine associated with user_3 button in the
UI.
Sub user_3 ;Example of dlgmsg
#1 = 0
#2 = 0
#3 = 0
#4 = 0
#5 = 0
#6 = 0
#7 = 0
#8 = 0
#9 = 0
#10 = 0
#11 = 0
#12 = 0
;dlgmsg will pop up a dialog with picture EdingCNC.png from c:\program files
(x86)\cnc4.01\dialogPictures directory
dlgmsg "edingcnc" "A" 1 "B" 2 "C" 3 "D" 4 "E" 5 "F" 6 "G" 7 "H" 8 "I" 9 "J" 10 "K" 11 "L"
12
if [#5398 == 1]
msg "OK #1="#1 "#2="#2 "#3="#3 "#4="#4 "#5="#5 "#6="#6 "#7="#7 "#8="#8 "#9="#9
"#10="#10 "#11="#11 "#12="#12
else
msg "CANCEL #1="#1 "#2="#2 "#3="#3 "#4="#4 "#5="#5 "#6="#6 "#7="#7 "#8="#8 "#9="#9
"#10="#10 "#11="#11 "#12="#12
endif
Endsub

09 November 2018

Release 4.03

182

EDING CNC

Manual

The dialog looks like this:

09 November 2018

Release 4.03

183

EDING CNC

4.3.7

Manual

Store position

SP [0 or 1]
This command stores the actual position in given file name.
The extra parameter 0 means create the file, 1 means add to existing file.
If only file name is given, the position is added to existing file.

4.3.8

TCAGuard [on | off]

Switches on or off the tool change area guard.
This is used during the rendering process, where the job file is checked for
collisions with the machine area and tool change area.

4.3.9

MCAGuard [on | off]

Switches on or off the machine area guard, no collisions will be given.
This is used during the rendering process, where the job file is checked for
collisions with the machine area and tool change area.

4.3.10 HomeIsEstop [on | off]
This allows to control the homeIsEstop feature.
When on, a EStop is generated when one of the home sensors activate.

4.3.11 Exec <”parameter”>
This allows to execute an external program within the interpreter and wait until
finished. The return code of the program is returned in #5399
Example:
Exec “notepad.exe” “hallo.txt” 60000
This executes notepad.exe and waits 1 minute for it to finish.
An error is generated if it does not finish within given time.
The maximum time is 10 minutes.
Whenever a G-Code file is loaded, also the file “macro.cnc” is loaded. In this file
you may put your frequently used subroutines, these can be invoked by the GCode file through GOSUB subroutineName.
The file contains default one special subroutine called “change_tool”, this
function is called automatically when a M6 Tx command (Tool change) is
encountered in the G-Code file. With this it is possible to define your own tool
change, especially useful when you have an automatic tool changer. You can put
moves and I/O actions there as well as automatic tool length measurement
using the probe with G38.2.
The tool change area can be guarded for collision, if it is defined the rendering
process will detect eventual collisions and report it. So a normal workpiece
program is not allowed to go through the Tool change Area.
The tool change itself is allowed to go to this area. Therefor the change_tool
09 November 2018

Release 4.03

184

EDING CNC

Manual

subroutine contains the statement TCAGuard off at the beginning and
TCAGuard on at the end.

4.3.12 SetAcc
This command allows to change the max acceleration of an axis.
Example: SetAcc Y 400 -> Set the max acceleration value for the Y-Axis to
400.

4.3.13 Vacuum [on | off]
Switches on or off vacuum sections that are used this is especially useful for
large machines with different vacuum sections.
The software will determine in which section will be machined, then this
command will switch only the used sections.
Configuration of the vacuum sections is not available in the GUI settings, and is
must be entered in the cnc.ini file, which contains all settings.
Definition of the vacuum sections is manually in the cnc.ini under [VACUUMBED]
automaticMode = 1
numberOfSectionsX = 14
numberOfSectionsY = 1
Automatic mode tells that we use the vacuum functions, and we give the
number of sections. In this case there are 14 sections in X that use the whole Y
range.
Then for each section the position and size,
section_1_OutputID = 101 ;0: none, 1-10: AUX1-AUX10, GPIO101 GPIO408
section_1_XPosition = 0.000000
section_1_YPosition = 0.000000
section_1_XWidth = 999.000000
section_1_YWidth = 3000.000000

4.3.14 GetJobDistance
Retrieves the traveled distance of the current job. The returned value is stored
in #
Example:
GetJobDistance 5399

4.3.15 GetHeightControlVact

09 November 2018

Release 4.03

185

EDING CNC

Manual

Retrieves the actual value of the Vact of the height control. The returned value
is stored in #
Example:
GetHeighControlVact 5399
Remark: this command will only be executed when the application is in ‘plasma’
or ‘laser’ mode.

4.3.16 GetHeightControlVset
Retrieves the actual value of the Vset of the height control. The returned value
is stored in #
Example:
GetHeighControlVset 5399
Remark: this command will only be executed when the application is in ‘plasma’
or ‘laser’ mode.

4.3.17 Service
For obtaining and resetting service items.
CMD options:
- JOBP, Get Job Progress in meters #5399
- MT_SLS, Get machine running time since last service #5399
- MT_TOT, Get machine running time total in #5399
- TD_SLS, Get traveled distance since last service #5399
- TD_TOT, Get Traveled distance total #5399
- NJ_SLS, Get number of jobs done since last service #5399
- NJ_TOT, Get number of jobs done total #5399
- TTG_PUMP, Get pump action Time to go.
- R_TTG_PUMP, Set pump action time to go to 5 seconds, so pump action will
be done after 5 seconds.
- R_SERVICE, Reset service counters when service is done.

09 November 2018

Release 4.03

186

EDING CNC

Manual

4.3.18 Tool change example

;* http://www.youtube.com/watch?v=_kp0SAeR-Kg
The grey marked code below is already prepared for you in the standard
macro.cnc file.
This change_tool subroutine is automatically called when the interpreter
encounters e.g.
m6 t1
(If automatic tool change in the setup is switched on).
;This example shows how to make your own tool_changer work.
;It is made for 6 tools and a simple KRESS Tool changer.
;First current tool is dropped, then the new tool is picked
;There is a check whether selected tool is already in the spindle
;Also a check that the tool is within 1-16
;There is a picktool subroutine for each tool and a droptool subroutine for each tool.
;These routines need to be modified to fit your machine and tool changer

sub change_tool
;Switch off guard for tool change area collision
TCAGuard off
;Switch off spindle
m5
;Use #5015 to indicate succesfull toolchange
#5015 = 0 ; Tool change not performed
if [ [#5011] == [#5008] ]
msg "Tool already in spindle"
endif
; check tool in spindle and exit sub
If [ [#5011] <> [#5008] ]
if [[#5011] > 6 ]
; our tool changer supports 6 tools 1-6
errmsg "Please select a tool from 1 to 6."
else
;Drop current tool
If [[#5008] == 0]
GoSub DropTool0
endif
If [[#5008] == 1]
GoSub DropTool1
endif
If [[#5008] == 2]
GoSub DropTool2
endif
If [[#5008] == 3]
GoSub DropTool3
endif
If [[#5008] == 4]
GoSub DropTool4
endif

09 November 2018

Release 4.03

187

EDING CNC

Manual
If [[#5008] == 5]
GoSub DropTool5
endif
If [[#5008] == 6]
GoSub DropTool6
endif
;Pick new tool
if [[#5011] == 0]
GoSub PickTool0
endif
if [[#5011] == 1]
GoSub PickTool1
endif
if [[#5011] == 2]
GoSub PickTool2
endif
if [[#5011] == 3]
GoSub PickTool3
endif
if [[#5011] == 4]
GoSub PickTool4
endif
if [[#5011] == 5]
GoSub PickTool5
endif
if [[#5011] == 6]
GoSub PickTool6
endif

endif
endif
If [[#5015] == 1]
msg "Tool "#5008" Replaced by tool "#5011" Tool length compensation G43 switched on"
m6t[#5011]
if [#5011 <> 0]
G43 ;Use tool-length compensation
endif
else
errmsg "tool change failed"
endif
;Switch on guard for tool change area collision
TCAGuard on
EndSub

09 November 2018

Release 4.03

188

EDING CNC

Manual

The code below is also inside file macro.cnc, for each tool there is a DropTool
sub-routine and a Pick-tool sun-routine. DropTool makes the movements and IO
for putting the tool from spindle in the tool holder. PickTool makes the
movements and I/O to pick the tool from the tool holder and put it in the
spindle.
These subroutines below are machine dependent and need to be filled in by
yourself.
This example works only for the Kress Tool changer.
;Drop tool subroutines, these put the tool in spindle in the tool-holder
Sub DropTool0
msg "Dropping tool 0"
;Tool 0 is no tool, so we just open yhe tool station here for PickTool which comes next
M54P3
;Open toolstation OUTPUT AUX3
G4P1
;Wait 1 seconds
endsub
Sub DropTool1
msg "Dropping tool 1"
M5
G53G0Z100
G53G0X825.00Y173.00
M54P3
G4P1
G53G1X867.206Y173.156F220
g53G0Z60
g53G01Z32.000F120
M54P1
G4P1
G53G01Z45F100
M55P1
G53G0Z100
endsub
Sub DropTool2
msg "Dropping tool 2"
M5
G53G0Z100
G53G0X825.00Y208.00
M54P3
G4P01
G53G1X867.200Y208.156F220
g53G0Z60
g53G01Z32.000F120
M54P1
G4P1
G53G01Z45F100
M55P1
G53G0Z100
endsub
Sub DropTool3
msg "Dropping tool 3"
M5
G53G0Z100
G53G0X825.00Y243.00
M54P3
G4P01
G53G1X867.116Y243.156F220
G53G0Z60
G53G01Z32.000F120
M54P1
G4P1
G53G01Z45F100
M55P1
G53G0Z100
endsub

;Z up 110 is and machinebed is zero
;Move just before drop place
;Open toolstation
;Wait 1 seconds
;Move into drop place
;Move down fast but not fully to the endposition
;Move down the last mm slower
;AUX1 ON air pressure toolchange
;Wait 1 second
;Move up slowly to move free from toolstation
;AUX1 off, tool dropped
;Further up and done with dropping tool

Sub DropTool4
msg "Dropping tool 4"
M5

09 November 2018

Release 4.03

189

EDING CNC
G53G0Z100
G53G0X825.00Y278.00
M54P3
G4P01
G53G1X867.026Y278.156F220
g53G0Z60
g53G01Z32.000F120
M54P1
G4P1
G53G01Z45F100
M55P1
G53G0Z100
endsub
Sub DropTool5
msg "Dropping tool 5"
M5
G53G0Z100
G53G0X825.00Y313.00
M54P3
G4P01
G53G1X866.936Y313.156F220
g53G0Z60
g53G01Z32.000F120
M54P1
G4P1
G53G01Z45f100
M55P1
G53G0Z100
endsub
Sub DropTool6
msg "Dropping tool 6"
M5
G53G0Z100
G53G0X825.00Y348.00
M54P3
G4P01
G53G1X866.850Y348.156F220
g53G0Z60
g53G01Z32.000F120
M54P1
G4P1
G53G01Z45f100
M55P1
G53G0Z100
endsub
;Pick tool subroutines
Sub PickTool0
msg "Picking tool 0"
M55P3
#5015 = 1
endsub
Sub PickTool1
msg "Picking tool 1"
M5
G53G0Z100
G53G0X825.00Y173.00
M54P3
G4P01
G53G1X867.206Y173.156F220
G53G0Z50
M54P1
G4P01
G53G01Z23.000F120
G4P0.5
M55P1
G53G01Z60F120
G53G0X825Z100
M55P3
#5015 = 1
endsub

Manual
;Z up 110 is and machinebed is zero
;Move just before drop place
;Open toolstation
;Wait 1 seconds
;Move into drop place
;Move down fast but not fully to the endposition
;Move down the last mm slower
;AUX1 ON air pressure toolchange
;Wait 1 second
;Move up slowly to move free from toolstation
;AUX1 off, tool dropped
;Further up and done with dropping tool

;Tool 0 is nothing, just close the tool station
;OUT3 off, closes toolstation
;toolchange succes

;Be sure that spindle is off
;Z up where zero is machinebed and 110 is top
;Move before pick place
;Open toolstation
;Wait 1 second
;Move into pick place
;Move down fast but not fully to the end
;AUX1 ON for opening collet clamp
;wait 1 second
;Move down last mm down slower to pick up toolholder
;Wait 1 second
;AUX1 off, tool picked
;Move slowly up to pick up tool and move free
;Further up and done with dropping
;OUT3 off, closes toolstation
;toolchange succes

Sub PickTool2

09 November 2018

Release 4.03

190

EDING CNC
msg "Picking tool 2"
M5
G53G0z100
G53G0X825.00Y208.00
M54P3
G4P01
G53G1X867.200Y208.156F220
g53G0Z50
M54P1
G4P1
G53G01Z23.000F120
G4P0.5
M55P1
G53G01Z60F120
G53G0X825Z100
M55P3
#5015 = 1
endsub
Sub PickTool3
msg "Picking tool 3"
M5
G53G0z100
G53G0X825.00Y243.00
M54P3
G4P01
G53G1X867.116Y243.156F220
G53G0Z50
M54P1
G4P1
G53G01Z23.000F120
G4P01
M55P1
G53G01Z60F120
G53G0X825Z100
M55P3
#5015 = 1
endsub
Sub PickTool4
msg "Picking tool 4"
M5
G53G0z100
G53G0X825.00Y278.00
M54P3
G4P01
G53G1X867.026Y278.156F220
g53G0Z50
M54P1
G4P1
G53G01Z23.000F120
G4P0.5
M55P1
G53G01Z60F120
G53G0X825Z100
M55P3
#5015 = 1
endsub
Sub PickTool5
msg "Picking tool 5"
M5
G53G0z100
G53G0X825.00Y313.00
M54P3
G4P01
G53G1X866.936Y313.156F220
G53G0Z60
M54P1
G4P1
G53G01Z23.000F120
G4P0.5
M55P1
G53G01Z60F120
G53G0X825Z100
M55P3
#5015 = 1

09 November 2018

Manual

;Be sure that spindle is off
;Z up where zero is machinebed and 110 is top
;Move before pick place
;Open toolstation
;Wait 1 second
;Move into drop place
;Move down fast but not fully to the end
;AUX1 ON for opening collet clamp
;wait 1 second
;Move down last mm down slower to pick up toolholder
;Wait 1 second
;AUX1 off, tool picked
;Move slowly up to pick up tool and move free
;Further up and done with dropping
;OUT3 off, closes toolstation
; toolchange succes

;Be sure that spindle is off
;Z up where zero is machinebed and 110 is top
;Move before pick place
;Open toolstation
;Wait 1 second
;Move into drop place
;Move down fast but not fully to the end
;AUX1 ON for opening collet clamp
; wait 1 second
;Move down last mm down slower to pick up toolholder
;Wait 1 second
;AUX1 off, tool picked
;Move slowly up to pick up tool and move free
;Further up and done witg dropping
;OUT3 off, closes toolstation
; toolchange succes

;Be sure that spindle is off
;Z up where zero is machinebed and 110 is top
;Move before pick place
;Open toolstation
;Wait 1 second
;Move into drop place
;Move down fast but not fully to the end
;AUX1 ON for opening collet clamp
;wait 1 second
;Move down last mm down slower to pick up toolholder
;Wait 1 second
;AUX1 off, tool picked
;Move slowly up to pick up tool and move free
;Further up and done witg dropping
;OUT3 off, closes toolstation
; toolchange succes

Release 4.03

191

EDING CNC

Manual

endsub
Sub PickTool6
msg "Picking tool 6"
M5
M5
G53G0z100
G53G0X825.00Y348.00
M54P3
G4P01
G53G1X866.850Y348.156F220
g53G0Z60
M54P1
G4P1
g53G01Z23.000F120
G4P0.5
M55P1
G53G01Z60F120
G53G0X825Z100
M55P3
#5015 = 1
endsub

;Be sure that spindle is off
;Z up where zero is machinebed and 110 is top
;Move before pick place
;Open toolstation
;Wait 1 second
;Move into drop place
;Move down fast but not fully to the end
;AUX1 ON for opening collet clamp
;wait 1 second
;Move down last mm down slower to pick up toolholder
;Wait 1 second
;AUX1 off, tool picked
;Move slowly up to pick up tool and move free
;Further up and done witg dropping
;OUT3 off, closes toolstation
;toolchange succes

4.3.19 Changing the tool number without actual tool change
During installation and manipulation of tools it is possible to the change actual
tool number like this:
#5011 = 1 ;New actual tool number
M6 T#5011 ;Change the tool in the software without calling the change_tool
macro.

4.3.20 USER Reset
A subroutine called user_reset can be added to macro.cnc.
This allows to perform extra reset actions, e.g. set/reset IO using M54/M55.
Example of user reset, this one toggles AUX1 for resetting servo drives.
;Remove comments if you want additional reset actions
;when reset button was pressed in UI
sub user_reset
m54 p1
g4 p0.1
m55 p1
msg "Ready for operation"
endsub

09 November 2018

Release 4.03

192

EDING CNC

4.4

Manual

RUN BEHAVIOR DURING SIMULATION AND RENDER

Simulation is the software mode when there is no hardware connected.
Render is performed during loading of a g-code file, the file is run by the
interpreter while generating output for the graphic. During this no actions to the
machine are applied, no motion and no IO, only checks if the g-code is valid and
stay’s within the machine limits.
If there is advanced macro programming, e.g. because the machine has
automatic tool change, there it is important to take into account that in
simulation and render mode no machine actions take place.

4.4.1

Example a check with error that we want to see always

Suppose we have a machine with a 6 tool automatic tool changer. A check is
programmed hat generates an error if a g-code file is loaded that tries to
change tool to a number that we do not have:
if [#5011 > 6]
ErrMsg “Please select a tool in range 1-6”
Else
..
;Code to perform the tool change
Endif
It is logic that we want this “ErrMsg …” line to be executed always, when
running but also in simulation mode and when loading the file.

4.4.2

Example a check with error showing only when running

sub check_airpresure
m56 p5
if [#5399 == 0]
errmsg "Error, No Air pressure"
else
msg "Air Presure OK"
endif
endsub
This check on air pressure will not work correctly while loading a g-code file or
while the system is in simulation mode, because no actual inputs are read.
sub check_airpresure
;;Check only if not rendering and not simulation
if [[#5380 == 0] and [#5397 == 0]]
m56 p5
if [#5399 == 0]
errmsg "Error, No Air pressure"
else
msg "Air Presure OK"
endif
endif
endsub
Here we see the modification to make the on the air pressure sensor input 5
simulation and render proof, the check is only performed when we are not in
render or simulation mode, only an extra if statement that checks #5380 (1
when simulation mode) and #5397 (1 when rendering) is added.

09 November 2018

Release 4.03

193

EDING CNC

Manual

5 Cutter Radius Compensation
This appendix discusses cutter radius compensation. It is intended for NC
programmers and machine operators.
See chapter 5 for additional information on cutter radius compensation.

09 November 2018

Release 4.03

194

EDING CNC

5.1

Manual

INTRODUCTION

The cutter radius compensation capabilities of the Interpreter enable the
programmer to specify that a cutter should travel to the right or left of an
open or closed contour in the XY-plane composed of arcs of circles and
straight line segments.
Cutter radius compensation is performed only with the XY-plane active. All
the figures in this appendix, therefore, show projections on the XY-plane.
Where the adjacent sides of remaining material meet at a corner, there
are two common ways to handle the tool path. The tool may pass in an
arc around the corner, or the tool path may continue straight in the
direction it was going along the first side until it reaches a point where it
changes direction to go straight along the second side. Figure A-1 shows
these two types of path. On Figure A-1:
• Uncut material is shaded in the figures. Note that the inner
triangles have the same shape with both tool paths.
• The white areas are the areas cleared by the tool.
• The lines in the center of the white areas represent the path of the
tip of a cutting tool.
• The tool is the cross-hatched circles.
Both paths will clear away material near the shaded triangle and leave the
shaded triangle uncut. When the Interpreter performs cutter radius
compensation, the tool path is rounded at the corners, as shown on the
left in Figure A-1. In the method on the right (the one not used), the tool
does not stay in contact with the shaded triangle at sharp corners, and
more material than necessary is removed.
There are also two alternatives for the path that is programmed in NC
code during cutter radius compensation. The programmed path may be
either (1) the edge of the material to remain uncut (for example, the edge
of the inner triangle on the left of Figure A-1), or (2) the nominal tool path
(for example, the tool path on the left side of Figure A-1). The nominal
tool path is the path that would be used if the tool were exactly the
intended size. The Interpreter will handle both cases without being told
which one it is. The two cases are very similar, but different enough that
they are described in separate sections see below.

09 November 2018

Release 4.03

195

EDING CNC

Manual

Figure A-1

Z-axis motion may take place while the contour is being followed in the
XY-plane. Portions of the contour may be skipped by retracting the Z-axis
above the part, following the contour to the next point at which machining
should be done, and re-extending the Z-axis. These skip motions may be
performed at feed rate (G1) or at traverse rate (G0). The Z motion will
not interfere with the XY path following. The sample NC code in this
appendix does not include moving the Z-axis. In actual programs, include
Z-axis motion wherever you want it.
Rotational axis motions (A, B, and C axes) are allowed with cutter radius
compensation, but using them would be very unusual.
Inverse time feed rate (G93) or units per minute feed rate (G94) may be
used with cutter radius compensation. Under G94, the feed rate will apply
to the actual path of the cutter tip, not to the programmed contour.

5.1.1

Data for Cutter Radius Compensation

The Interpreter world model keeps three data items for cutter radius
compensation: the setting itself (right, left, or off), program_x, and
program_y. The last two represent the X and Y positions which are given
in the NC code while compensation is on. When compensation is off, these
both are set to a very small number (10-20) whose symbolic value is
"unknown". The Interpreter world model uses the data items current_x
and
current_y to represent the position of the center of the tool tip (in the
currently active coordinate system) at all times.

09 November 2018

Release 4.03

196

EDING CNC

5.2
5.2.1

Manual

PROGRAMMING INSTRUCTIONS
Turning Cutter Radius Compensation On

To start cutter radius compensation keeping the tool to the left of the
contour, program G41 D…. The D word is optional (see "Use of D
Number", just below).
To start cutter radius compensation keeping the tool to the right of the
contour, program G42 D… .
In Figure A-1, for example, if G41 were programmed, the tool would move
clockwise around the triangle, so that the tool is always to the left of the
triangle when facing in the direction of travel. If G42 were programmed,
the tool would stay right of the triangle and move counter clockwise
around the triangle.

5.2.2

Turning Cutter Radius Compensation Off

To stop cutter radius compensation, program G40. It is OK to turn
compensation off when it is already off.

5.2.3

Sequencing

If G40, G41, or G42 is programmed on the same line as tool motion,
cutter
compensation will be turned on or off before the motion is made. To make
the motion come first, the motion must be programmed on a separate,
previous line of code.

5.2.4

Use of D Number

Programming a D word with G41 or G42, is optional.
If a D number is programmed, it must be a non-negative integer. It
represents the slot number of the tool whose radius (half the diameter
given in the tool table) will be used, or it may be zero (which is not a slot
number). If it is zero, the value of the radius will also be zero. Any slot in
the tool table may be selected. The D number does not have to be the
same as the slot number of the tool in the spindle, although it is rarely
useful for it not to be.
If a D number is not programmed, the slot number of the tool in the
spindle will be used as the D number.

5.2.5

Material Edge Contour

When the contour is the edge of the material, the outline of the edge is described
in the NC program.
09 November 2018

Release 4.03

197

EDING CNC

Manual

For a material edge contour, the value for the diameter in the tool table is
the actual value of the diameter of the tool. The value in the table must
be positive. The NC code for a material edge contour is the same
regardless of the (actual or intended) diameter of the tool.

5.2.6

Programming Entry Moves

In general, two pre-entry moves and one entry move are needed to begin
compensation correctly. However, if there is a convex corner on the
contour, a simpler method is available using zero or one pre-entry move
and one entry move. The general method,
which will work in all situations, is described first. We assume here that
the programmer knows what the contour is already and has the job of
adding entry moves.
A.1.1.1
GENERAL METHOD
The general method includes programming two pre-entry moves and one
entry move. See Figure A-2. The shaded area is the remaining material. It
has no corners, so the simple method cannot be used. The dotted line is
the programmed path. The solid line is the actual path of the tool tip. Both
paths go clockwise around the remaining material. A cutter one unit in
diameter is shown part way around the path. The black dots mark points
at the beginning or end of programmed or actual moves. The figure shows
the second pre-entry move but not the first, since the beginning point of
the first pre-entry move could be anywhere.

09 November 2018

Release 4.03

198

EDINGCNC

Manual

Figure A-2, Cutting radius compensation entry moves (for material edge
contour)

First, pick a point A on the contour where it is convenient to attach an
entry arc. Specify an arc outside the contour which begins at a point B
and ends at A tangent to the contour (and going in the same direction as
it is planned to go around the contour). The radius of the arc should be
larger than half the diameter given in the tool table. Then extend a line
tangent to the arc from B to some point C, located so that the line BC is
more than one tool radius long. After the construction is finished, the code
is written in the reverse order from the construction. The NC code is
shown in Table A-1; the first three lines are the entry moves just
described.
Table A-1 NC program for figure A-2
N0010 G1 X1 Y5 (make first pre-entry move to C)
N0020 G41 G1 Y4 (turn compensation on and make second pre-entry
move to point B)
N0030 G3 X2 Y3 I1 (make entry move to point A)
N0040 G2 X3 Y2 J-1 (cut along arc at top)
N0050 G1 Y-1 (cut along right side)
N0060 G2 X2 Y-2 I-1 (cut along arc at bottom right)
N0070 G1 X-2 (cut along bottom side)
N0080 G2 X-2.6 Y-0.2 J1 (cut along arc at bottom left)
N0090 G1 X1.4 Y2.8 (cut along third side)
N0100 G2 X2 Y3 I0.6 J-0.8 (cut along arc at top of tool path)
N0110 G40 (turn compensation off)
Cutter radius compensation is turned on after the first pre-entry move and
before the second pre-entry move (including G41 on the same line as the
second pre-entry move turns compensation on before the move is made).
In the code above, line N0010 is the first pre-entry move, line N0020
09 November 2018

Release 4.03

199

EDINGCNC

Manual

turns compensation on and makes the second pre-entry move, and line
N0030 makes the entry move.
A.1.1.2
SIMPLE METHOD
If there is a convex (sticking out, not in) corner somewhere on the
contour, a simpler method of making an entry is available. See Figure A3.
First, pick a convex corner. There is only one corner in Figure A-3. It is at
A, and it is convex. Decide which way you want to go along the contour
from A. In our example we are keeping the tool to the left of the
remaining material and going clockwise. Extend the side to be cut (DA in
the figure) to divide the area outside the material near A into two regions;
DA extended is the dotted line AC on the figure. Make a pre-entry move to
anywhere in the region on the same side of DC as the remaining material
(point B on the figure) and not so close to the remaining material that the
tool is cutting into it. Anywhere in the diagonally shaded area of the figure
(or above or to the left of that area) is OK. If the tool is already in region,
no pre-entry move is needed. Write a line of NC code to move to B, if
necessary. Then write a line of NC code for a straight entry move that
turns compensation on and goes to point A.
If B is at (1.5, 4), the two lines of code for the pre-entry and entry moves
would be:
N0010 G1 X1.5 Y4 (move to B)
N0020 G41 G1 X3 Y3 (turn compensation on and make entry move to A)

These two lines would be followed by four lines identical to lines N0050 to
N0080 from Table A-1, but the end of the program would be different
since the shape of remaining material is different.
It would be OK for B to be on line AC. In fact, B could be placed on the
extension outside the part of any straight side of the part. B could be
placed on EF extended to the right (but not to the left, for going
clockwise), for example.
If DA were an arc, not a straight line, the two lines of code above would
still be suitable. In this case, the dotted line extending DA should be
tangent to DA at A.
Figure A-3 Simpler cutter radius compensation entry move (for material
edge contour)

09 November 2018

Release 4.03

200

EDINGCNC

Manual

Figure A-3 Simpler compensation entry move

09 November 2018

Release 4.03

201

EDINGCNC

5.3

Manual

NOMINAL PATH CONTOUR

When the contour is a nominal path contour (the path a tool with exactly
the intended diameter would take), the tool path is described in the NC
program. It is expected that (except for during the entry moves) the path
is intended to create some part geometry. The path may be generated
manually or by a post-processor, considering the part geometry which is
intended to be made. For the Interpreter to work, the tool path must be
such that the tool stays in contact with the edge of the part geometry, as
shown on the left side of Figure A-1. If a path of the sort shown on the
right of Figure A-1 is used, in which the tool does not stay in contact with
the part geometry all the time, the Interpreter will not be able to
compensate properly when undersized tools are used. A nominal path
contour has no corners, so the simple method just described will not work.
For a nominal path contour, the value for the cutter diameter in the tool
table will be a small positive number if the selected tool is slightly
oversized and will be a small negative number if the tool is slightly
undersized. If a cutter diameter value is negative, the Interpreter
compensates on the other side of the contour from the one programmed
and uses the absolute value of the given diameter. If the actual tool is the
correct size, the value in the table should be zero. Suppose, for example,
the diameter of the cutter currently in the spindle is 0.97, and the
diameter assumed in generating the tool path was 1.0. Then the value in
the tool table for the diameter for this tool should be -0.03.
The nominal tool path needs to be programmed so that it will work with
the largest and smallest tools expected to be actually used. We will call
the difference between the radius of the largest expected tool and the
intended radius of the tool the "maximum
radius difference." This is usually a small number.
The method includes programming two pre-entry moves and one entry
moves. See Figure A-4. The shaded area is the remaining material. The
dashed line is the programmed tool path. The solid line is the actual path
of the tool tip. Both paths go clockwise around the remaining material.
The actual path is to the right of the programmed path even though G41
was programmed, because the diameter value is negative. On the figure,
the distance between the two paths is larger than would normally be
expected. The 1-inch diameter tool is shown part way around the path.
The black dots mark points at the beginning or end of programmed
moves. The corresponding points on the actual path have not been
marked. The actual path will have a very small additional arc near point B
unless the tool diameter is exactly the size intended. The figure shows the
second pre-entry move but not the first, since the beginning point of the
first pre-entry move could be anywhere.
First, pick a point A on the contour where it is convenient to attach an
entry arc. Specify an arc outside the contour which begins at a point B
and ends at A tangent to the contour (and going in the same direction as
it is planned to go around the contour). The radius of the arc should be
larger than the maximum radius difference. Then extend a line tangent to
09 November 2018

Release 4.03

202

EDINGCNC

Manual

the arc from B to some point C, located so that the length of line BC is
more than the maximum radius difference. After the construction is
finished, the code is written in the reverse order from the construction.
The NC code is shown in Table A-2; the first three lines are the entry
moves just described.
Table A-2 NC program for Figure A-4
N0010 G1 X1.5 Y5 (make first pre-entry move to C)
N0020 G41 G1 Y4 (turn compensation on and make second pre-entry
move to point B)
N0030 G3 X2 Y3.5 I0.5 (make entry move to point A)
N0040 G2 X3.5 Y2 J-1.5 (cut along arc at top)
N0050 G1 Y-1 (cut along right side)
N0060 G2 X2 Y-2.5 I-1.5 (cut along arc at bottom right)
N0070 G1 X-2 (cut along bottom side)
N0080 G2 X-2.9 Y0.2 J1.5 (cut along arc at bottom left)
N0090 G1 X1.1 Y3.2 (cut along third side)
N0100 G2 X2 Y3.5 I0.9 J-1.2 (cut along arc at top of tool path)
N0110 G40 (turn compensation off)

09 November 2018

Release 4.03

203

EDINGCNC

Manual

Figure A-4 Cutter radius compensation entry moves

Cutter radius compensation is turned on after the first pre-entry move and
before the second pre-entry move (including G41 on the same line as the
second pre-entry move turns compensation on before the move is made).
In the code above, line N0010 is the first pre-entry move, line N0020
turns compensation on and makes the second pre-entry move, and line
N0030 makes the entry move.

09 November 2018

Release 4.03

204

EDINGCNC

5.4

Manual

PROGRAMMING ERRORS AND LIMITATIONS

The Interpreter will issue the following error messages involving cutter
radius compensation. In addition to these, there are several bug
messages related to cutter compensation, but they should never occur.
1. Cannot change axis offsets with cutter radius comp
2. Cannot change units with cutter radius comp
3. Cannot probe with cutter radius comp on
4. Cannot turn cutter radius comp on out of xy-plane
5. Cannot turn cutter radius comp on when on
6. Cannot use g28 or g30 with cutter radius comp
7. Cannot use g53 with cutter radius comp
8. Cannot use xz-plane with cutter radius comp
9. Cannot use yz-plane with cutter radius comp
10.Concave corner with cutter radius comp
11.Cutter gouging with cutter radius comp
12.D word with no g41 or g42
13.Multiple d words on one line
14.Negative d word tool radius index used
15.Tool radius index too big
16.Tool radius not less than arc radius with comp
17.Two g codes used from same modal group.
Most of these are self-explanatory. For those that require explanation, an
explanation is given below.
Changing a tool while cutter radius compensation is on is not treated as
an error, although it is unlikely this would be done intentionally. The
radius used when cutter radius compensation was first turned on will
continue to be used until compensation is turned off, even though a new
tool is actually being used.
A.1.2 Concave Corner and Tool Radius Too Big (10 and 16)
When cutter radius compensation is on, it must be physically possible for
a circle whose radius is the half the diameter given in the tool table to be
tangent to the contour at all points of the contour. In particular, the
Interpreter treats concave corners and concave arcs into which the circle
will not fit as errors, since the circle cannot be kept tangent to the contour
in these situations. See Figure A-5. This error detection does not limit the
shapes which can be cut, but it does require that the programmer specify
the actual shape to be cut (or path to be followed), not an approximation.
In this respect, the NIST
RS274/NGC Interpreter differs from interpreters used with many other
controllers, which often allow these errors silently and either gouge the
part or round the corner.
concave corner
-tool does not fit

09 November 2018

concave arc too small
-tool does not fit

Release 4.03

205

EDINGCNC

Manual

Figure A-5, Two cutter radius compensation errors
In both examples, the line represents a contour, and the circle represents
the cross section of a tool following the contour using cutter radius
compensation (tangent to one side of the path.)
A.1.3 Cannot Turn Cutter Radius Comp on When On (5)
If cutter radius compensation has already been turned on, it cannot be
turned on again. It must be turned off first; then it can be turned on
again. It is not necessary to move the
cutter between turning compensation off and back on, but the move after
turning it back on will be treated as a first move, as described below.
It is not possible to change from one cutter radius index to another while
compensation is on because of the combined effect of rules 5 and 12. It is
also not possible to switch compensation from one side to another while
compensation is on.
A.1.4 Cutter Gouging (11)
If the tool is already covering up the next XY destination point when cutter
radius compensation is turned on, the gouging message is given when the
line of NC code
which gives the point is reached. In this situation, the tool is already
cutting into material it should not cut. More details are given in Section
A.6.
A.1.5 Tool Radius Index Too Big (15)
If a D word is programmed that is larger than the number of tool carousel
slots, this error message is given. In the SAI, the number of slots is 68.
A.1.6 Two G Codes Used from Same Modal Group (17)
This is a generic message used for many sets of G codes. As applied to
cutter radius
compensation, it means that more than one of G40, G41, and G42
appears on a line of NC code. This is not allowed.
A.2 First Move into Cutter Compensation
The algorithm used for the first move after cutter radius compensation is
turned on, when the first move is a straight line, is to draw a straight line
from the programmed destination point which is tangent to a circle whose
center is at the current point and whose radius is the radius of the tool.
The destination point of the tool tip is then found as the center of a circle
of the same radius tangent to the tangent line at the destination point. If
the programmed point is inside the initial cross section of the tool (the
circle on the left), an error is signaled. The concept of the algorithm is
shown in Figure A-6.
The function that locates the destination point actually takes a
computational shortcut based on the fact that the line (not drawn on the
09 November 2018

Release 4.03

206

EDINGCNC

Manual

figure) from the current point to the programmed point is the hypotenuse
of a right triangle having the destination point at the corner with the right
angle.
Figure A-6, First cutter radius compensation move - Straight

If the first move after cutter radius compensation has been turned on is
an arc, the arc which is generated is derived from an auxiliary arc which
has its center at the programmed center point, passes through the
programmed end point, and is tangent to the cutter at its current location.
If the auxiliary arc cannot be constructed, an error is signaled. The
generated arc moves the tool so that it stays tangent to the auxiliary arc
throughout the move. This is shown in Figure A-7.
Figure A-7, First cutter radius compensation move - Arc

Figure A-7 shows the conceptual approach for finding the arc. The actual
computations differ between the center format arc and the radius format
arc (see Section 3.6.3).
After the entry moves of cutter radius compensation, the Interpreter
keeps the tool tangent to the programmed path on the appropriate side. If
a convex corner is on the path, an arc is inserted to go around the corner.
The radius of the arc is half the diameter given in the tool table.
When cutter radius compensation is turned off, no special exit move takes
place. The next move is what it would have been if cutter radius
compensation had never been turned on and the previous move had
placed the tool at its current position.

09 November 2018

Release 4.03

207

EDINGCNC

5.5

Manual

EXTENSION IO BOARD

The extension I/O board is not so often used, so all related settings are to be set directly in
the cnc.ini file.
Special for GPIO card settings:
If you have an additional General purpose IO board, such as the RLY8 board with 8 output
relays and 8 opto-isolated inputs, there are extra options currently only available by editing
the cnc.ini file. This is the file soring all the parameters of the machine.
The CPIO card can guard the inputs and an action can be coupled when a guard triggers.
There is a text that is displayed by the GUI when a guard triggers. You specify which inputs
must be guards, this is given by a bit mask.
1 means only input 1.
3 means input 1 and input 2.
This table apply’ s for input 0-3, the total table would be 255 lines long:
Participant bits
Value Participant bits
Value
Input 8 .. Input 1
Input 8 .. Input 1
0000 0000 (-)
0
0100 0000 (I7)
64
0000 0001 (I1)
1
1000 0000 (I8)
128
0000 0010 (I2)
2
0000 0100 (I3)
4
Example (I4 & I5)
0000 1000 (I4)
8
0000 1000
0001 0000 (I5)
16
0001 0000
Add =
0010 0000 (I6)
32
0001 1000
24

Next you specify the compare value if the guard should trigger when an input becomes ON
(1), specify a 1 for that input, for OFF specify a zero.
Next, the action can be specified:
09 November 2018

Release 4.03

208

EDINGCNC
0
1
2
3

=
=
=
=

Manual

nothing.
warning.
smooth stop (with ramp down).
quick stop (immediately, no ramp down, this may give position loss.

This is how it looks in the cnc.ini for 1 rule,
there are max 8 rules for the RLY8 card.
[GPIO_RULES]
;Give warning message when Oil pressure 1 or 2 is low
;Input 4 = 0000 1000, input 5 = 0001 0000 together 0001 1000
;So the value for participant bits is 8 + 16 = 24
;When one of the inputs becomes 1, we want a warning message
;So compare bits are also 24
;Action is 1, warning
card_1_rule_1_text = "---Warning Oil is pressure low---"
card_1_rule_1_inputParticipantBits = 24
card_1_rule_1_inputCompareBits = 24
card_1_rule_1_action = 1
;Give smooth stop when Vacuum is to low
;Input 1 = 0000 0001
;So the value for participant bits is 1
;When one of the inputs becomes 1, we want a smooth stop
;So compare bits are 1
;Action is 2, smooth stop
card_1_rule_2_text = "---Warning Vacuum is pressure low---"
card_1_rule_2_inputParticipantBits = 1
card_1_rule_2_inputCompareBits = 1
card_1_rule_2_action = 2
;Give ESTOP when the water pressure is low
;Input 2 = 0000 0010
;So the value for participant bits is 2
;When one of the inputs becomes 1, we want a smooth stop
;So compare bits are 1
;Action is 3, ESTOP
card_1_rule_3_text = "---Water pressure low---"
card_1_rule_3_inputParticipantBits = 2
card_1_rule_3_inputCompareBits = 2
card_1_rule_3_action = 3
What also can be specified is the name of the IO in or output for the GUI. It is also done
directly in the cnc.ini.
[GPIO_NAMES]
gp_output_101_name = "Oil pump on"
gp_output_102_name = "Water pump on"
gp_output_103_name = "Touch Probe down"
gp_output_104_name = "Touch Probe up"
gp_output_105_name = "Vacuum 1"
gp_output_106_name = "Vacuum 2"
gp_output_107_name = "Vacuum 3"
gp_output_108_name = "Vacuum 4"
gp_input_101_name = "Vacuum pressure low"
gp_input_102_name = "No water pressure"
gp_input_103_name = ""
gp_input_104_name = "Oil pressure 1 low"
09 November 2018

Release 4.03

209

EDINGCNC
gp_input_105_name
gp_input_106_name
gp_input_107_name
gp_input_108_name

Manual
=
=
=
=

"Oil pressure 2 low"
""
""
""

These are the IO’s for card 1, the IO’s for card 2 have numbers 201 etc. instead of 101,
card 3 has numbers 301.. etc.
If a name is not filled in, the GUI will show the number.

09 November 2018

Release 4.03

210

EDINGCNC

5.6

Manual

HARDWARE INSTALLATION TIPS

Building a reliable CNC system is not just making the right connections. EMC plays an
important role here. We have several components that generate a lot of EMC noise, the
drivers, the power supplies if they are switched mode supplies, the VFD if we have a HF
spindle. The CPU and the communication to the PC, especially USB is very sensitive for
EMC and may stop functioning when we make "spaghetti" wiring and no good functional
Earth. So the routing of the cabling must be done in a right way. Very important is making
a good EMC functional Earth using a star point GND.
To prevent this miss function due to EMC, the EDINGCNC CPU should be build in correctly
according these general EMC rules:
•
•
•

Mount all electronics in a metal cabinet or on a metal plate in a plastic cabinet.
Use a mains filter.
Create a central GND point near the filter and connect the PE (Protective Earth) as well
as the GND from all power supplies to this point.

•

Route motor cables nicely along the cabinet edge, as far as possible away from the
CPU. This way the cables noise radiation can flow away to the cabinet.
Use shielded cables for the motor connections, both inside the cabinet and outside the
cabinet. Connect the shield at one side to the central ground point, leave the other side
un-connected.
Use a professional USB2 cable, double shielded with ferrites like this:

•
•

Keep all GND cables especially short and use thick flexible cable
If not possible to keep it short, then connect it to the metal GND plate.

•

09 November 2018

Release 4.03

211

EDINGCNC

Manual
Schematic drawing of a possible good layout in the cabinet.

Here a picture of my own system, it contains various EMC problem makers, like 2 Switched
mode power supplies and a frequency inverter for a HF spindle. Check the routing of the
Motor and drive supply wires.
Also there a 4 stepper-motor drives working at 75 Volt, motor currents 4,2 Amp.

09 November 2018

Release 4.03

212

EDINGCNC

09 November 2018

Manual

Release 4.03

213

EDINGCNC

5.7

Manual

REFERENCES

[Albus]

[Allen-Bradley]

[EIA]

[Fanuc]

[Kramer1]

[Kramer2]

[Kramer3]

[Kramer4]

[K&T]

[NCMS]

[Proctor]

Albus, James S; et al; NIST Support to the Next Generation Controller Program:
1991 Final Technical Report; NISTIR 4888; National Institute of Standards and
Technology, Gaithersburg, MD; July 1992
Allen-Bradley; RS274/NGC for the Low End Controller; First Draft; Allen-Bradley;
August 1992
Electronic Industries Association; EIA Standard EIA-274-D Interchangeable
Variable Block Data Format for Positioning, Contouring, and
Contouring/Positioning Numerically Controlled Machines; Electronic Industries
Association; Washington, DC; February 1979
Fanuc Ltd.; Fanuc System 9-Model A Operators Manual; Pub B-52364E/03;
Fanuc Ltd; 1981
Kramer, Thomas R.; Proctor, Frederick M.; Michaloski, John L.; The NIST
RS274/NGC Interpreter, Version 1; NISTIR 5416; National Institute of Standards
and Technology, Gaithersburg, MD; April 1994
Kramer, Thomas R.; Proctor, Frederick M.; The NIST RS274KT Interpreter;
NISTIR 5738; National Institute of Standards and Technology, Gaithersburg, MD;
October 1995
Kramer, Thomas R.; Proctor, Frederick M.; The NIST RS274/NGC Interpreter Version 2; NISTIR 5739; National Institute of Standards and Technology,
Gaithersburg, MD; October 1995
Kramer, Thomas R.; Proctor, Frederick M.; The NIST RS274/VGER Interpreter;
NISTIR 5754; National Institute of Standards and Technology, Gaithersburg, MD;
November 1995
Kearney and Trecker Co.; Part Programming and Operating Manual, KT/CNC
Control, Type C; Pub 687D; Kearney and Trecker Corp.; 1980
National Center for Manufacturing Sciences; The Next Generation Controller Part
Programming Functional Specification (RS-274/NGC); Draft; NCMS; August 1994
Proctor, Frederick M.; Kramer, Thomas R.; Michaloski, John L.; Canonical
Machining Commands; NISTIR 5970; National Institute of Standards and
Technology, Gaithersburg, MD; January 1997

09 November 2018

Release 4.03

214

Source Exif Data:

File Type                       : PDF
File Type Extension             : pdf
MIME Type                       : application/pdf
PDF Version                     : 1.7
Linearized                      : No
Page Count                      : 214
Language                        : nl-NL
Tagged PDF                      : Yes
XMP Toolkit                     : 3.1-701
Producer                        : Microsoft® Word voor Office 365
Title                           : Eding CNC manual
Creator                         : Bert Eding
Creator Tool                    : Microsoft® Word voor Office 365
Create Date                     : 2018:11:09 08:26:43+01:00
Modify Date                     : 2018:11:09 08:26:43+01:00
Document ID                     : uuid:6BCF5357-70FE-442C-BB76-47D5620FF6B2
Instance ID                     : uuid:6BCF5357-70FE-442C-BB76-47D5620FF6B2
Part                            : 3
Conformance                     : A
Author                          : Bert Eding

EXIF Metadata provided by EXIF.tools

Eding CNC Manual Edingcnc V4.03

Navigation menu

Versions of this User Manual:

Views

Navigation