Fanuc OT G Code Training Manual Cnc Program Gcodetraining 588

User Manual:

Open the PDF directly: View PDF .
Page Count: 104

Download
Open PDF In Browser	View PDF

CNC
PROGRAM MANUAL

PU
MA
450

TRAINING

Forward
Thank you very much for participating in our education.
DAEWOO constantly makes an effort to research and develop to satisfy the
requirements of customers positively.
DAEWOO does its utmost to accept and practice the Quality Confirmation of DAEWOO and Customers' requirements through the Dealer-net-work of about 350 as practicing the World Quality Management.
DAEWOO provides with the technical data and support the technical coaching, therefore, if you contact us when you need of them , we will immediately help you.
We will do our best during your education period.
Thank you.

TRAINING

O-T

DAEWOO
RESET

G
G
G
G
G
G
G

NC POWER
ON

NO.
01
02
03
04
05
06
07

X

Z

R

0.000
0.000
0.000
0.000
0.000
0.000
0.000

0.000
0.000
0.000
0.000
0.000
0.000
0.000

0.000
0.000
0.000
0.000
0.000
0.000
0.000

ACT. POSITION(RELATIVE)
U
0.000
NUM.
MZ
120.

O(

N)

GE

RC

7

8

9

ALTER

XU

YV

Z W 4TH

4

5

6

INSRT

I

JA

K@

F-NO

1

2

3

DELET

_

CURSOR

W
S MDI

,

M#

S=

T*

L+

P[

Q]

DH

BSP

POS

PRGRM

OFSET

DGNOS
PARAM

OPR
ALARM

AUX

CAN

INPUT

PAGE

0T

SHIFT

GEOM

EOB

0.000

OFF

WEAR

.

MENU

W.SHIFT MRCRO

?
80 100 120
140
150

20

120

?

LM

100 150

0

180

%

60
0

50

FEEDRATE OVERRIDE

EMERGENCY STOP

80
70

OUTPT
START

? N

90 100 110
50

60
40

MACRO

GRAPH

SPINDLE OVERRIDE

SPINDLE LOAD

SPINDLE SPEED

ALARM NO.

+X
X100
X

X10

Z

X1

–Z

MODE

INCREMENTAL FEED

+Z

START

RAPID

COOLANT

SINGLE
BLOCK

OPTIONAL OPTIONAL DRY RUN
BLOCK SKIP
STOP
β

N
100

–X

STOP

50

α

6 7 8
45
9
3
10
2
11
1
12

F0

CYCLE START

FEED HOLD

MACHINE READY EMG. RELEASE

RAPID OVERRIDE

TOOL NO.

1

MACHINE LOCK PROGRAM PROTECT

CHUCKING

TRAINING
G-FUNCTION
STANDARD G
CODE

SPECIAL
G CODE

#G00
G01
G02
G03

G00
G01
G02
G03

01

Positioning (Rapid feed)
Straight interpolation
Circular interpolation (CW)
Circular interpolation (CCW)

G04

G04

00

Dwell

G20
#G21

G20
G21

06

Data input (inch)
Data input (mm)

#G22
G23

G22

04

Stored distance limit is effective
(Spindle interference check ON)
Stored distance limit is ineffective
(Spindle interference check OFF)

GROUP

G23

FUNCTION

G27
G28
G29
G30

G27
G28
G29
G30

00

Machine reference return check
Automatic reference return
Return from reference
Tte 2nd rererence return

#G32

G33

01

Thread process

G40
G41
G42

G40
G41
G42

07

Cancel of compensation
Compensation of the left
Compensation of right

G50
G70
G71
G72
G73
G74
G75
G76

G92
G70
G71
G72
G73
G74
G75
G76

00

Creation of virtual coordinate/Setting the rotating time of principal spindle
Compound repeat cycle(Finishing cycle)
Compound repeat cycle(Stock removal in turning)
Compound repeat cycle(Stock removal in facing)
Compound repeat cycle(Pattern repeating cycle)
Compound repeat cycle(Peck drilling in Z direction)
Compound repeat cycle(Grooving in X direction)
Compound repeat cycle(Thread process cycle)

G90
G92
G94

G77
G78
G79

01

Fixed cycle(Process cycle in turning)
Fixed cycle(Thread process cycle)
Fixed cycle(Facing process cycle)

G96
#G97

G96
#G97

02

Control the circumference speed uniformly(mm/min)
Cancel the uniform control of circumference speed.
Designate r.p.m

G98
#G99

G94
#G95

05

Designate the feedrate per minute(mm/min)
Designate the feedrate per the rotation of principal spindle(mm/rev.)

-

G90
G91

03

Absolute programming
Incremental programming

Note) 1. # mark instruction is he modal indication of initial condition which is immediately available
when power is supplied.
2. In general, the standard G code is used in lathe, and it is possible to select the special G code
according to setting of parameters.

2

TRAINING
NC LATHE M-CODE LIST
M-CODE

DESCRIPTION

REMARK M-CODE

DESCRIPTION

REMARK
OPTION

M00

PROGRAM STOP

M39

STEADY REST 1 UNCLAMP

M01

OPTIONAL STOP

M40

GEAR CHANGE NETURAL

M02

PROGRAM END

M41

GEAR CHANGE LOW

M03

MAIN-SPINDLE FORWARD

M42

GEAR CHANGE MIDDLE

M04

MAIN-SPINDLE REVERSE

M43

GEAR CHANGE HIGH

M05

MAIN-SPINDLE STOP

M46

PTS BODY UNCL & TRACT-BAR ADV.

OPTION

M07

HIGH PRESSURE COOLANT ON

M47

PTS BODY CL & TRACT-BAR RET.

OPTION

M08

COOLANT ON

M50

BAR FEEDER COMMAND 1

OPTION

M09

COOLANT OFF

M51

BAR FEEDER COMMAND 2

OPTION

M10

PARTS CATCHER ADVANCE

OPTION

M52

SPLASH GUARD DOOR OPEN

OPTION

M11

PARTS CATCHER RETRACT

OPTION

M53

SPLASH GUARD DOOR CLOSE

OPTION

M13

TURRET AIR BLOW

OPTION

M54

PARTS COUNT

OPTION

M14

MAIN-SPINDLE AIR BLOW

OPTION

M58

STEADY REST 2 CLAMP

OPTION

M15

AIR BLOW OFF

M59

STEADY REST 2 UNCLAMP

OPTION

M17

MACHINE LOCK ACT

M61

SWITCHING LOW SPEED (N.J)

α P60

M18

MACHINE LOCK CANCEL

OPTION
(ONLY)
MDI
(ONLY)
MDI

M62

SWITCHING HIGH SPEED (N.J)

α P60

M19

MAIN-SPINDLE ORIENTAION

OPTION

M63

MAIN-SPDL CW & COOLANT ON

M24

CHIP CONVEYOR RUN

OPTION

M64

MAIN-SPDL CCW & COOLANT OFF

M25

CHIP CONVEYOR STOP

OPTION

M65

MAIN-SPDL & COOLANT OFF

M30

PROGRAM END & REWIND

M66

DUAL CHUCKING LOW CLAMP

OPTION

M31

INTERLOCK BY-PASS(SPDL &T/S)

M67

DUAL CHUCK HIGH CLAMP

OPTION

M32

INTERLOCK BY-PASS(SPDL &S/R)

3 AXIS

M68

MAIN-CHUCK CLAMP

M33

REV.-TOOL-SPINDLE FORWARD

3 AXIS

M69

MAIN-CHUCK UNCLAMP

M34

REV.-TOOL-SPINDLE REVERSE

M70

DUAL TAILSTOCK LOW ADVANCE

M35

REV.-TOOL-SPINDLE STOP

M74

ERROR DETECT ON

M75

ERR0R DETECT OFF

M38

OPTION

OPTION

3

OPTION

TRAINING
NC LATHE M-CODE LIST
M-CODE

DESCRIPTION

REMARK M-CODE

DESCRIPTION

M76

CLAMFERING ON

M131

INTERLOCK BY-PASS (SUB-SPDL)

M77

CLAMFERING OFF

M163

SUB-SPDL CW & COOLANT ON

M78

TAILSTOCK QUILL ADVANCE

M164

SUB-SPDL CCW & COOLANT OFF

M79

TAILSTOCK QUILL RETRACT

M165

SUB-SPDL & COOLANT STOP

M80

Q-SETTER SWING ARM DOWN

OPTION

M168

SUB-CHUCK CLAMP

M81

Q-SETTER SWING ARM UP

OPTION

M169

SUB-CHUCK UNCLAMP

M84

TURRET CW ROTATION

M203

FORWARD SYNCHRONOUS COM.

M85

TURRET CCW ROTATION

M204

REVERSE SYNCHRONOUS COM.

M86

TORQUE SKIP ACT

B AXIS

M205

SYNCHRONOUS STOP

M87

TORQUE SKIP CANCEL

B AXIS

M206

SPINDLE ROTATION RELEASE

M88

SPINDLE LOW CLAMP

M89

SPINDLE HIGH CLAMP

M90

SPINDLE UNCLAMP

M91

EXTERNAL M91 COMMAND

3 AXIS

M92

EXTERNAL M92 COMMAND

3 AXIS

M93

EXTERNAL M93 COMMAND

M94

EXTERNAL M94 COMMAND

OPTION

M98

SUB-PROGRAM CALL

OPTION

M99

END OF SUB-PROGRAM

OPTION

M103

SUB-SPINDLE FORWARD

M104

SUB-SPINDLE REVERSE

M105

SUB-SPINDLE STOP

M110

PARTS CATCHER ADVANCE(SUB)

OPTION

M111

PARTS CATCHER RETRACT(SUB)

OPTION

M114

SUB-SPINDLE AIR BLOW

OPTION

M119

SUB-SPINDLE ORIENTATION

OPTION

4

REMARK

TRAINING
Note) 1. M00 : For this command, main spindle stop, cutting oil, motor stop, tape reading stop are
carriedout.
M01 : While this function is the same as M00, it is effective when the optional stop switch of
console is ON.
This command shall be overrided if the optional stop switch is OFF.
M02 : Indicates the end of main program.
M30 : This is the same as M02 and it returns to the starting position of the programme when
the memory and the tape are running.
2. M code should not be programmed in the command paragraph containing S code or T code.
It is favorable for M code to programe in a command paragraph independently.
3. The edges of processed material become round due to the effect of characteristics of AC
servo motor. To avoid it, M74 and M75 functions are used.

When command of M75

When command of M74

(Error detection is OFF)

(Error detection is ON)

4. M76, M77
These codes are effective when thread process is programmed by G92, and they are used for
ON and OFF of thread beveling. Thread chamferingis set as much as one pitch by setting of
parameters and it is possible to set double.

(Thread chamferingON)

(Thread chamferingOFF)

5

TRAINING

Function
Program number

Address

Meaning of address

O(EIA)/(ISO) Program number

Block sequence number

N

Sequence number

Preparatory function

G

Sercifies a motion mode (Linear, arc, etc)

Dimension word

X, Z

Command of moving position(absolute type) of each axis

U, W

Instruction of moving distance and direction(incremental type)

I, K
R
Feed function

F, E

Ingredient of each axis and chamfering volume of circulat center
Radius of circle, corner R, edge R
Designation of feedrate and thread lead

Auxiliary function

M

Command of ON/OFF for operating parts of machine

Spindle speed function

S

Designation of speed of main spindle or rotation time of main spindle

Function (Tool)

T

Designation of tool number and tool compensation number

Dwell

P, U, X

Dewignation of program number

P

Designation of sequence No

P, Q

Number of repetitions

L

Parameters

A, D, I, K

Designation of dwell time
Designation of calling number of auxiliary program
Callling of compound repeat cycle, end number
Repeat time of auxiliary program
Parameter at fixed cycle

One block is composed as follows

One block

N
G
Sequence Preparation
Auxiliary
function
No.

X
Y
Dimension
word

F
Feed
function

6

S
Spindle
speed
function

T
Tool
function

M
Function
auxiliary

:
EOB

TRAINING
Meaning of Address
T function is used for designation of tool numbers and tool compensation.
T function is a tool selection code made of 4 digits.
T

0

2

0

2
Designation of tool compensation number
Designation of tool number

Example) If it is designated as(T 0 2 0 2 )
0

2 calls the tool number and calls the tool compensation value of number , and

the tool is compensation as much as momoried volume in the storage.
The cancel of tool compensation is commanded as T

0

0

If you want to call the next tool and compensation, you should cancel the tool compensation. For convenient operation, it is recommended to used the same number of
tool and compensation.
It is not allowed to use the same tool compensation number for 2 different tools.
Minimum compensation value : + 0.001mm
Maximum compensation value : + 999.999mm
Tool compensation of X spindle is designated as diameter value.

7

TRAINING
G00(Positioning)

G00

Each axes moves as much as commanded data in rapid feedrate.

G00

X(U)

G00 X150.0 Z100.0

Z(W);

X200.0 Z200.0

X
X150
Z100

X200
Z200

G00 U150.0 W100.0

Z

U50.0 W100.0

(X0 Z0)

N1234 G00 X25. Z5.
+X

-Z

+Z

5

-X
8

Ø25

G00

TRAINING

G01
G01(Linear interpolation)
Each axes moves straigrtly as much as commanded data in commanded rate.

G01 X150.0 Z100.0 F0.2 :

G01

X(U)

Z(W)

F

X200.0 Z200.0 :

X
X150
Z100
(X0 Z0)

X200
Z200

G01 U150.0 W100.0 F0.2 :
U50.0 W100.0 :

Z

N1234 G01 X25. Z-30. F0.2
+X

-Z

+Z

30

-X
9

Ø25

G01

TRAINING
AUTO CHAMFERING “C” AND CORNER “R” (Option)
+X
C

+r

+i

A
B

Command path Z→X : A : Start point of instuction

-i
-r

C'

G01 Z(w) B C ( ¡ i) : B : End point of instruction

-X

G01 Z(w) B C ( ¡ r) :CC’ : Running point of command

A

-r

Command path X→Z :

+r

-Z

G01 X(u) B C ( ¡ k)

+Z
C'

-K

B

+K

C

G01 X(u) B R ( ¡ r)

Note) (1) After instructing from G01 to one axis, the next command paragraph should be fed in
vertical direction.
(2) If the next command paragraph is incremental type, designate the incremental volume
baed on B point.
(3) In following cases, errors occur. (G01 Mode)

– When instruction one of I, K, R and X and Z at the same time.
– When instructing two of I, K, R in the same block.
– When instructing Xand I or Z and K.
– When the moving distance is less than the next command
are not right angled.
(4) During the operation of single command paragraph, the operation at C point stops.

Example)
X

N1 G01 Z30.0 R6.0 F0.2 :

C3
N3
N2

N3 Z0 :
Z

Ø40

Ø100

R

6

N2 X100.0 K-3.0 :
N1

(N2 X100.0 C3.0 :)Normal

30
80

10

TRAINING
G01 PROGRAM

Ø80

Ø100

Example1)

50

30

15

O0001 :
N10 G50 S1500 T0100 M42 :

N20 G50 S2000 T0300 :

G96 S180 M03 :

G96 S200 M03 :

G00 X100.5 Z5.0 T0101 M08 :

G00 X85.0 Z5.0 T0303 M08 :

G01 Z-95.0 F0.25 :

Z0 :

G00 U2.0 Z0.5 :

G01 X-1.6 F0.2 :

G01 X-1.6 F0.2 :

G00 X80.0 Z3.0 :

G00 X95.0 W1.0 :

G42 Z1.0 :

G01 Z-37.3 F0.25 :

G01 Z-15.0 F0.18 :

X100.0 Z-45.5 :
G00 Z1.0 :
X90.0 :
G01 Z-29.8 :
X95.0 Z-37.3 :

X100.0 Z-45.0 :
Z-95.0 :
G40 U2.0 W1.0
G00 X200.0 Z200.0 M09 T0300 :
M30 :

G00 Z1.0 :
X85.0 :

G50 : Setting the rotating time of max. speed of

G01 Z-22.3 :
X90.0 Z-29.8 :
G00 Z1.0 :
X80.5 :

main spindle
G96 : Constant surface speed control command
G40 : Compensation cancel
G42 : Right hand compensation

G01 Z-15.55 :
X85.0 Z-22.3 :
G00 X200.0 Z200.0 M09 T0100 :
M01 :

11

TRAINING
G01 PROGRAM
Example2)

C1

45

Ø50

Ø70

Ø60

C1

25

30

100
G01 Z-30.0 :

O0002 :

X60.3 Z-54.7 :

N10 G50 S2000 T0100 :

X72.0

G96 S180 M03 :
G00 X70.5 Z5.0 T0101 M08 :
G01 Z-100.0 F0.25 :
G00 U2.0 Z0.5 :
G01 X-1.6 F0.23 :

G00 X150.0 Z200.0 T0100 :
M01 :
N20 G50 S2300 T0300 :
G96 S200 M03 :
G00 X55.0 Z5.0 T0303 M08 :

G00 X65.0 W1.0 :

Z0 :

G01 Z-54.5 F0.25 :

G01 X-1.6 F0.2 :

G00 U2.0 Z1.0 :

G00 X46.0 Z3.0 :

X60.0 :
G01 Z-54.5 :

G42 Z1.0 :
G01 X50.0 Z-1.0 F0.15 :
Z-30.0 :

G00 U2.0 Z1.0 :

X60.0 Z-55.0 :

X55.0 :

X68.0 :

G01 Z-30.0 :

X70.0 W-1.0 :

X60.0 Z-54.5 :

Z-100.0 :

G00 U2.0 Z1.0 :

G40 U2.0 W1.0
X50.5 :

G00 X150.0 Z200.0 M09 T0300 :
M30 :

12

TRAINING

G02

G03
X

I (X)

Z

K(Z)
P0

P2

X

I

G02
P1
K

Z

N1234 G02 X.. Z.. (R..)
X
P2

G03

P1
-I

P0
-K

Z

N1234 G03 X.. Z.. (R..)

13

TRAINING
G02, G03(Circular interpolation)
Each axis interpolates circularly to the commanded coordinate in instructed speed.

Meaning
Instruction

Conditions
1

2

3

Rotation direction

Right hand coodinate

Left hand coodinate

G02

CW

CCW

G03

CCW

CW

Location of end point

X,Z

Location X,Z of commanded point from coordinate

Distance to the end point

U,W

Distance from start point to commanded point
Distance from start point to the center of and arc

Distance between start point
and the center point

I,K

with sign, radius value (I always designates the
radius)

Arc radius with no sign radius

R

Radius of circumference

of circumference
G02 X(u) Z(w) R_ F_ :

60
X

G01 X30.0 Z60.0 F0.3 :

30
5

Z35.0 :
G02 X40.0 Z30.0 I5.0 :
(G02 U10.0 W-5.0 I5.0)

G02

Ø30

Z

Ø50

R

G02

G01 X50.0 :
Z0 :

G03 X(u) Z(w) R_ F_ :

G01 X40.0 Z60.0 F0.3 :

60

X

G03

Z

Ø50

R

5

G03

14

G03 X50.0 Z55.0 K-5.0 :

TRAINING
Note) (1) If I or K is 0 it is omissible.
(2) G02 I_: Make a round of circle.
(3) It is recommended to use R as + value, and designates the circumferences less than
180.
G03 R_: No moving
(4) When designating R which is less than the half of moving distance, override R and make
half circle.
(5) When designating I, K and R at the same time, R is effective.
(6) When the moving end point is not on the circumference as a result of wrong designation
of and K :

P2

P2

r
P1

r
P1

15

TRAINING
G03

PROGRAM
)
G02

Ø20

Ø100

Example 1)

R4

5

40

N10

20.615

24.385

50

:

N20 G50 S2000 T0300 :
G96 S200 M03 :
G00 X0 Z3.0 T0303 M08 :
G42 G01 Z0 F0.2 :
G03 X20.0 Z-10.0 R10.0 :
G01 Z-50.0 :
G02 X100.0 Z-74.385 I40.0 K20.615 : (G02 X100.0 Z-74.385 R45.0)
G01 Z-125.0 :
G40 U2.0 W1.0
G00 X200.0 Z200.0 M09 T0300 :
M30 :

16

TRAINING
G02

PROGRAM
)
G03

16
R

46

N10

Ø35

Ø100
R

16

Example 2)

36

:

N20 G50 S2000 T0300 :
G96 S200 M03 :
G42 G00 X35.0 Z5.0 T0303 M08 :
G01 Z-20.0 F0.2 :
G02 X67.0 Z-36.0 R16.0 : (G02 X67.0 Z-36.0 I16.0 K0)
G01 X68.0 :
G03 X100.0 Z-52.0 R16.0 : (G02 X100.0 Z-52.0 I0 K-16.0)
G01 Z-82.0 :
G40 G00 X200.0 Z200.0 M09 T0300 :
M30 :

# When I and K instruction, if the data value is “0” it can be omitted.

17

TRAINING
G01
G02

PROGRAM

30
15

2.5

8

Ø102

15
24.33

Ø60
Ø80
Ø100

Ø40

Ø35

Ø30

R3

R1
.5

G03

)

42

O0000 :
G01 Z-14.8 F0.27 :

N10 (ø30 DRILL)

G00 U2.0 Z1.0 :

G50 T0200 :

X80.5 :

G97 S250 M03 :
G00 X0 Z5.0 T0202 M08 :

G01 Z-14.1 :

G01 Z-5.0 F0.07 :

G02 X81.9 Z-14.8 R0.7 :

W1.0 :

G00 X100.5 W1.0

Z-40.0 F0.25 :

G01 Z-29.8
G00 U2.0 Z-1.0 :

G00 Z5.0 :
Z-39.0 :

G01 X60.5 F0.23 :

G01 Z-60.0 :

G00 X82.0 W1.0 :
Z-2.4 :

G00 Z10.0 :

G01 X60.5 :

X200.0 Z200.0 T0200 :

X72.9 :

M01 :
N20 (Outside diameter stock removal)

G03 X80.5 Z-6.2 R3.8 :

G50 S1500 T0100 :

G00 U2.0 Z5.0 :
X200.0 Z200.0 T0100 :

G96 S180 M03 :

M01 :

G00 X94.0 Z5.0 T0101 M08 :
G01 Z-14.8 F0.27 :
G00 U2.0 Z0.5 :
G01 X28.0 F0.23 :
G00 X87.0 W1.0 :
18

TRAINING
N30 (Inside diameter stock removal)

N50 (Inside diameter finishing)

G50 S1500 T0400 :

G50 S1800 T0600 :

G96 S180 M03 :

G96 S200 M03 :

G00 X34.5 Z3.0 T0404 M08 :

G00 X40.0 Z5.0 T0606 M08 :

G01 Z-41.8 F0.27 :

G41 Z1.0 :

G00 U-0.5 Z1.0 :

G01 Z-15.0 F0.2 :

X39.5 :

X35.0 Z-24.33 :

G01 Z-15.0 :

Z-42.0 :

X34.5 Z-24.3 :
G00 Z10.0 :

X29.0 :
G40 G00 Z10.0 :

X200.0 Z200.0 T0400 :
M01 :

X200.0 Z200.0 T0600 M09 :
M30 :

N40 (Out diameter finishing)
G50 S1800 T0500 :
G96 S200 M03 :
G00 X63.0 Z5.0 T0505 M08 :
Z0 :
G01 X38.0 F0.2 :
G00 X60.0 Z3.0 :
G42 Z1.0 :
G01 Z-2.5 F0.2 :
X74.0 :
G03 X80.0 Z-5.5 R3.0 :
G01 Z-13.5 :
G02 X83.0 Z-15.0 R1.5 :
G01 X100.0 :
Z-30.0 :
X103.0 :
G40 G00 U2.0 W1.0 :
G00 Z10.0 :
X200.0 Z200.0 T0500 :
M01 :

19

TRAINING
1G04 (Dwell)
After passing as much time as commanded by X(u) or P code in the same block, carry out the next
block.
In case of 10 seconds' dwell
G04 X10.0 : (G04 X10000 : )
G04 U10.0 : (G04 U10000 : )
G04 P10000.0 : (G04 P1000 : )
Automatic reference return
Reference means certain point fixed in the machine, and coordinate value of reference is set in NC
parameter.
Parameter NO

OT-C/F

FS16/18T

N708(X)

N1240(X, Z)

N709(Z)
1) G27(Reference return check)
Position is decided through rapid feed to the position of value set in NC PARAMETER by command.
Example) When PARAMETER N708(X) is 330000
N709(Z) is 529000
G00 X100.0 Z100.0 :

End point(Machine reference)

G27 X330.0 Z529.0 :
X100.0
(
)
Z100.0

(

X330.0
)
Z529.0

Start point(0.0)
If arrived position is the reference, reference Lamp is ON.
Note) When instructing G27, you should cancel the OFFSET volume
2) G28(Reference automatic return)
By command, commanded axis automatically returns to the reference.
G28 X(u) Z(w) :
Example) When PARAMETER N708(X) is 330000
N709(Z) is 529000

20

TRAINING
G28 U0 W0 :

G27 X100.0 Z100.0

(

X330.0
)
Z529.0

(

X100.0
(
)
Z100.0

X330.0
)
Z529.0

Action of G28 block presents that the commanded axis goes via the center in rapid feedrate and
returns to the reference.
Note) When instructing G28 block, tool, tool compensation, tool location offset should be canceled principlly.
3) G29(Automatic return in reference)
Commanded spindle goes via the remoried center point and decides the position as commanded point.
G29 X(u) Z(w) :
∴Generally, it is used right after G28 or G30 command.
G28 X100.0 Z100.0 :
Machine referebce
Center point
G29 X50.0 Z200.0 :

Return point

X100.0
Z100.0

Start point

X50.0
Z200.0

4) G30(The 2nd reference return)
Commanded spindle automatically returns to the 2nd reference
(coordinate point set in parameter)
G30 X(u) Z(w)) :
∴You should input appropriate distance between works and tool exchangeposition in the relative
parameter.
PARAMETER NO N735(X) = 200000

FS16/18T

N736(Z) = 300000

N1241(X,Z)
The 2nd reference

X

X200.0

G30 U0 W0 :

Z300.0
Z

Reference) Generally, the 2nd reference is used for the start point of program.

21

TRAINING
G32(THREAD CYCLE)
According to G32 command, straight thread and taper thread of certain lead are cut.
G32 Z(w) F : (G32 is applied to only single block)
X(u) F :
Example 1) STRAIGHT lead

Lead of screw : 3mm

X
20

δ1 : 5mm

Z

Depth of cut : 1mm(2cut two times)

Ø50

δ1

δ2

δ2 : 1.5mm

70

(ABSOLUTE)
G50 T0100 :
G97 S800 M03 :
G00 X90.0 Z5.0 T0101 M8 :
X48.0 :
G32 Z-71.5 F3.0 :
G00 X90.0 :
Z5.0 :
X46.0 :
G32 Z-71.5 :
G00 X90.0 :
Z5.0
X150.0 Z150.0 T0100 :
M30 :

∗ When processing G32 thread, feed(pitch) is modal.

22

TRAINING
Example 1) STRAIGHT lead
G32 X(u) Z(w) F : Because it is taper, it is applied to both axis at the same time.

Lead of screw : 3mm
X

δ1 : 5mm
δ2 : 1.5mm

δ2
Z

Depth of cut : 1mm(2cut two times)

Ø25

Ø50

δ1

70

(ABSOLUTE)

(INCREMENTAL)

G50 S800 T0100 :

G50 S800 T0100 :

G97 S800 M03 :

G97 S800 M03 :

G00 X90.0 Z5.0 T0101 :

G00 X90.0 Z5.0 T0101 :

X22.026 :

U-67.974 :

G32 X49.562 Z-71.5 F3.0 :

G32 U27.321 W-76.5 F3.0 :

G00 X90.0 :

G00 U40.438 :

Z5.0 :

W76.5 :

X21.052 :

U-68.948 :

G32 X48.588 Z-71.5 :

G32 U27.321 W-76.5 :

G00 X90.0 :

G00 X90.0 :

Z5.0 :

W76.5 :

X150.0 Z150.0 T0100 :

X150.0 Z150.0 T0100 :

M30 :

M30 :

Reference)
Values of incomplete thread δ1 and δ2.
δ1= 3.6 x L x n
1800

L = Lead of thread
n = Rotating time of main spindle

δ2= L x n
1800

23

TRAINING

G42

R

-X

-Z

+Z

+X

+X

-Z

+Z

-X
24

TRAINING

G41 G42
6

2

1

9
5

7

R
4

8

3

G41

G42

25

TRAINING

G40
G42

N100
N105
N110
N115

G42 G00 X.. Z..
G01 Z-.. F..
G02 X.. Z-.. R..
G40 G00 X.. Z..

+X

G40
N115
N100

G42
N110

N105

-Z

+Z

-X

G41
G40

N100
N105
N110
N115

G41 G00 X.. Z..
G01 Z-.. F..
G02 X.. Z-.. R..
G40 G00 X.. Z..

+X

-Z

+Z

-X
26

TRAINING
Tool diameter compensation

G40 : R compensation cancel
G41 : When located on the left side of material based on the progressing direction,
G42 : When located on the right side of material based on the progressing direction,

X

X
G41

G42

Z

Z

What is Tool diameter compensation?
If R is on the end of the tool edge, parts which are not impensated only by tool position OFFSET
are occured during the taper cutting or circlar cutting. Therefor, impensating this error automatically
is namelyR compensation.(During the tool diameter compensation, add theR and T-direction in the
R compensation column of OFFSET PAGE.

Example 1) When not using tool diameter compensation(R compensation a and b should be calculated)
compensation ¡ 0.5

C

2

PROGRAM
G01 X25.0 Z0 F0.2 :

0.
8

X30.0 Z-2.5 :

R

45°

compensation

Ø30

b

( ¡ 0.5)

a

G00 U1.0 Z1.0 :
G28 UO WO :
M30 :
∗

27

TRAINING
Example 2) When using tool diameter compensation
∗ You do not have to calculate R compensation a and b
∗ If a position and b position are given on the program, the tool performs automatically R compensation and moves to the next progressing direction.

2

compensation ¡ 0.5
C

G42 X26.0 Z0 F0.2 :
compensation

b

( ¡ 0.5)

Ø30

X = 30.0
Z = –2.0

PROGRAM

G01 X30.0 Z-2.0 :
Z-30.0 :
G00 U1.0 Z1.0 :

X = 26.0 a
Z=0

G28 UO WO :
M30 :
∗

Presentation 1) In case of no compensation

Presentation 2) In case of compensation

28

TRAINING
1) Direction of imaginary (In case of right hand coordinate)

Direction of imaginary seen from the center of radius is decided by the cutting direction of tool
during the cutting. Therefor, it should be set as much as compensation volume.
Direction and number of imaginary are decided among the following eight
types.
X

4

X

8

3
Z

1

X

5

7

Z

9

6

2



1

2

4

3

5
6

29

Z

TRAINING

8
7

9

2) Compensation setting of

X

T
OFFSET No.

Z

OFFSETNO.

X

Z

TOOL DIRECTION

01

0.75

-0.93

0.4

3

0.2

-1.234

10.987

0.8

2

.

.

.

.

.

.

.

.

.

.

16

.

.

.

.

Command scope of OFFSET volume0– + 999.999mm

30

TRAINING

G70
FINISHING CYCLE
G70 P Q :

+X
N70

N55
N60

N60

-Z

+Z

-X

N..

P

Q

N50

G70

P55

Q70

N55
N60
N65

G0
G1
G2

G42 X..
Z-..
X.. Z..

N70
N..

G1

G40

X..
31

R..

TRAINING

G71
+X

W+
N75

N60

R U
U+
N70

N65

+Z

-Z

-X

N..

P

Q

N50

G71

U..

R..

N55

G71

P60

Q75

N60
N65
N70

G0
G1
G2

G42 X..
Z-..
X.. Z-..

N75
N..

G1

G40

X..

32

U+..

R..

W+..

TRAINING
G71(STOCK REMOVAL IN TURNING)
G71 U( ¡ d) R(e) :
G71 P

Q

U( ¡ u) W( ¡ w) F :
P : Start sequence no.
C
(R)
(R)

e

(F)

Q : Final sequence no.

A

∆d

B

U( ¡ d) : Cut volume of one time(Designate

45°

the radius.

(F)

R(e) : Escape volume(Always 45) escape

(F) : Cutting feed
(R) : Rapid traverse

U( ¡ u) : Finishing tolerance in X axis

∆u/2

Program command

W( ¡ w) : Finishing tolerance in Z axis

A`

F(f) : Cutting feedrate

∆w

40
60
70
90
110
140

33

Ø80

Ø60

Ø50

Ø40

20

Ø30

Example of program

TRAINING
(G70, G71)
N10 G50 S1500 T0101 :
G96 S180 M03 :
G00 X85.0 Z5.0 M08 :
Z0 :
G01 X-1.6 F0.25 :
G00 X83.0 Z2.0 :
G71 U3.0 R1.0 :
G71 P20 Q30 U0.5 W0.1 F0.27 :
N20 G42 G00 X30.0 :

G71 CYCLE CUTTING FEED

G01 Z-20.0 F0.17 :
G70 CYCLE CUTTING FEED
X40.0 Z-40.0 :
Z-60.0 :
X50.0 Z-70.0 :
Z-90.0 :
X60.0 Z-110.0 :
Z-140.0 :
X80.0 :
N30 G40 :
G70 P20 Q30 : (When using the same bite)
G00 X200.0 Z200.0 T0100 :
M30 :

¡¯ When finishing, if a different bite is used
G00 X200.0 Z200.0 T0100 :
M01 :
N40 G50 S2000 T0303 :
G96 S200 M03 :
G00 X83.0 Z2.0 M08 :
G70 P20 Q30 :
G00 X200.0 Z200.0 T0300 :
M30 :

34

TRAINING
Examples of program
Stock Removal in Turning(G71) (Type I)

X

40

20 2010 20 30

100
80

Ø40

Ø60

Ø100

Ø140

2

7

Start point
End point

Z

30 10 2
100

(Diameter designation, metric input)
N010 G00 X200.0 Z100.0 :
N011 G00 X160.0 Z10.0 :
N012 G71 U7.0 R1.0 :
N013 G71 P014 Q021 U4.0 W2.0 F0.3 S550 :
N014 G00 G42 X40.0 S700 :
N015 G01 W-40.0 F0.15 :
N016

X60.0 W-30.0 :

N017

W-20.0 :

N018

X100.0 W-10.0 :

N019

W-20.0 :

N020

X140.0 W-20.0 :

N021

G40 U2.0 :

N022 G70 P014 Q021 :
N023 G00 X200.0 Z100.0 :
M30 :

35

TRAINING
G72(STOCK REMOVAL IN FACING)
G72 W( ¡ d) R(e) :
G72 P_ Q_ U( ¡ u) W( ¡ w) F :
U( ¡ d) : Cut volume of one time

∆d
A`

R(e) : Escape volume

C
A

P : Start sequence No.
Tool path

Q : Final sequence No.

(F)

e
(R)

U( ¡ u) : Finishing in clearance X axis(Diameter

(R)

∆u/2

command)
45°
(F)

Program command

W( ¡ w) : Finishing in clearance Z axis

B

F(f) : Cutting feedrate
∆w

C

1

Example of program

X40.0 Z-15.0 :
X30.0 :

C

1

Z-1.0 :

Ø80

Ø60

Ø45

15

Ø40

30
50

Ø30

X26.0 Z1.0 :
N14 G40 :
G70 P12 Q14 :
G00 X200.0 Z200.0 T0100 :
M30 :

N10 G50 S2000 T0100 :

¡¯(When finishing with a different tool)

G96 S180 M03 :

G00 X200.0 Z200.0 T0100 :

G00 X85.0 Z5.0 T0101 :

M01 :

Z0 :

N16 G50 S2500 T0300 :

G01 X-1.6 F0.2 :
G00 X85.0 Z1.0 :

G96 S200 M03 :

G72 W2.0 R1.0 :

G00 X85.0 Z5.0 T0303 :

G72 P12 Q14 U0.5 W0.2 F0.25 :

G70 P12 Q14 :

N12 G00 G41 Z-51.0 :

G00 X200.0 Z200.0 T0300 :

G01 X80.0 F0.2 :

M30 :

X78.0 W1.0 :
X60.0 :
Z-45.0 :

36

TRAINING
Examples of program
Stock Removal in Pacing(G72)

7
X

60

Ø40

Ø80

Ø120

Ø160

88
110

Start point

101010 20 20

Z

2
60

(Diameter designation, metric input)
N010 G00 X220.0 Z60.0 :
N011 G00 X176.0 Z2.0 :
N012 G72 W7.0 R1.0 :
N013 G72 P014 Q021 U4.0 W2.0 F0.3 S550 :
N014 G00 G41 Z-70.0 S700 :
N015 X160.0 :
N016 G01 X120.0 Z-60.0 F0.15 :
N017

W10.0 :

N018

X80.0 W10.0 :

N019

W20.0 :

N020

X36.0 W22.0 :

N021

G40 :

N022 G70 P014 Q021 :
N023 G00 X220.0 Z60.0 :
N024 M30 :

37

TRAINING
G73(PATTEN REPEATING)
G73 U( ¡ i) R(d) W( ¡ k) :
G73 P Q U( ¡ u) W( ¡ w) F :

U( ¡ i) : Excape distance and direction in X axis
(Designated the radius)
W( ¡ k) : Escape distance and direction in Z axis

∆k+∆w
∆w

R(d) : Repeating time

D
∆i+∆u/2

C
A

(R)

(It is conneeted with the cut volume of each time)

∆u/2

P : Start sequence No.

B

Q : Final sequence No.

∆u/2
A`

∆w

U( ¡ u) : Finishing in clearance X axis(Radius designated)
W( ¡ w) : Finishing in clearance Z axis
F(f) : Cutting feedrate

10

20

10

Ø60

Ø40

Ø20

R

∆u

Example of program

20

50

N10 G50 S2000 T0300 :
G96 S200 M03 :

N12 G00 G42 X20.0 Z2.0 :
G01 Z-10.0 F0.15 :

G00 X35.0 Z5.0 T0303 :
G02 X40.0 Z-20.0 R10.0 :
Z0 :
G01 Z-30.0 :
G01 X-1.6 F0.2 :
X60.0 Z-50.0 :
G00 X70.0 Z10.0 :
N16 G40 U1.0 :
G73 U3.0 W2.0 R2 :
G70 P12 Q16 :
G73 P12 Q16 U0.5 W0.1 F0.25 :
G00 X200.0 Z200.0 T0300 :
M30 :
38

TRAINING
Examples of program
Pattern Repeating(G73)
16

16

Start point

Ø80

Ø120

Ø160

Ø180

110

2

14

130

X

Z

2

14

20

R

60

10

40 10 20
220

(Diameter designation, metric input)
N010 G00 X260.0 Z80.0 :
N011 G00 X220.0 Z40.0 :
N012 G73 U14.0 W14.0 R3 :
N013 G73 P014 Q020 U4.0 W2.0 F0.3 S0180 :
N014 G00 G42 X80.0 Z2.0 :
N015 G01 W-20.0 F0.15 S0600 :
N016 X120.0 W-10.0 :
N017 W-20.0 S0400 :
N018 G02 X160.0 W-20.0 R20.0 :
N019 G01 X180.0 W-10.0 S0280 :
N020 G40 :
N021 G70 P014 Q020 :
N022 G00 X260.0 Z80.0 :
N023 M30 :

39

40

TRAINING

G74
+X

-Z

+Z

Q

-Z
-X

N40
N50

G74
G74

R..
Z-..

Q..

40

F..

TRAINING
G74(Peck drilling in Z axis divection)
1) Drill cutting cycle
G74 R(e) :
G74 Z(w) Q( ¡ k) F :
∆k`

∆k

∆k

∆k

∆k

R(e) : Retreat volume
Z(w) : Final cutting depth

A
∆i

C

(R)

(R)

Q( ¡ k) : One time cutting depth

(R)

∆d

(R)

(1000=1mm)

(F)

∆i

(F)

F : Cutting feedrate

∆i`

(F)

U/2

(F)
(F)

B
X
e

[0 < ∆i` < ∆i ]

W

(R) : Radius traverse
(F) : Cutting feed

Z

Examples of program

∆k`

∆k

C

∆d

(R)
(F)

N10 G50 S500 T0200 :

(F)

G74 R1.0 :

G97 S280 M03 :

G74 Z-90.0 Q5000 F0.23 :

G00 X0 Z5.0 T0202 M08 :

G00 X200.0 Z150.0 T0200 :

Start point of drilling

M01 :

41

TRAINING
2) Stock removal cycle in side
G74 R(e) :
G74 X(u) Z(w) P( ¡ i) Q( ¡ k) R( ¡ d) F :
∆k`

∆k

∆k

∆k

∆k

A
∆i

C

(R)

(R)

(R)

∆d

(R)

(F)

∆i

(F)

∆i`

(F)

U/2

(F)
(F)

B
X
e
W

[0 < ∆i` < ∆i ]
(R) : Radius traverse
(F) : Cutting feed

Z

R(e) : Retreat volume(Modal command)
P( ¡ i) : Moving volume of X axis
Q( ¡ k) : Cut volume in Z axis(Q5000=5mm)
X(u) : Composition of X axis
Z(w) : Final cutting depth

R( ¡ d) : Escape wlume at the end point of Z axis proess(Designate the symbol and
radius according to the direction of escape)
F : Cutting feedrate

42

10

10

Ø10
Ø30
Ø50

Ø50

Ø20

TRAINING

¡¯ If there is one groove, X(u), P( ¡ i) can be omitted.
(In case of omitting, it shall be done at the same time)
N10

N10 G50 S2000 T0100 :
G00 X20.0 Z1.0 :

G96 S80 M03 :

G74 R1.0 :

G00 X50.0 Z1.0 T0101 :

G74 Z-10.0 Q3000 F0.1 :

G74 R1.0 :

G00 X200.0 Z200.0 :

G74 X10.0 Z-10.0 P10000 Q3000 F0.1 :
G00 X200.0 Z200.0 T0100 :

M30 :

M30 :

Attention
FANUC 0TC
Q3000=3mm

N1 G50 S2000 T0100 :

P10000=10MM

G96 S80 M3 :
G0 X47.0 Z1.0 T0101M8 :
G74 R1.0 :

3

G74 Z-10.0 Q3000 F0.1 :
G0 U-5.0 :
G74 X20.0 Z-10.0 P2500 Q3000 F0.1 :

Ø50

M30 :

Ø50

Ø20

G0 X200.0 Z200.0 T0100 :

10

43

TRAINING

G75
Q)
Z(w) : Z spindle coordinate at the end point of thread process
R(i)

: For omitting, straight thread and R– : X+ and Taper thread
R+ : X– and Taper thread

P(k) : Height of thread(Omit the decimal point P900=0.9mm)

Q(d) : Initial cut volume (Omit the decimal point Q500=Designate) the radius
value
F(f) : Cutting feedrate(Lead)
*P(k) : 0.6 x Pitch = Core diameter of thread
Hikgh value
Midium value = 0.6
Low value
(Exampal1) G76 Compound type thread cycle
E

A

(R)

Tool tip

B

r

C
X

1st
2nd
3rd
nth

d

Z
w

49

∆d

a

k

∆d

D

i

B

(R)

K

(F)

∆d n

U/2

TRAINING
(Exampal1) G76 Compound type thread cycle

Ø60.64

Ø68

1.8

X

Z

6
105

25





,





,


1.8

G00 X80.0 Z130.0 :

3.68

G76 P011060 Q100 R200 :

G76 X60.64 Z25.0 P3680 Q1800 F6.0 ;

M30x2.0

P=1.5

30

50

PROGRAM
N10 G97 S1000 M03
T0100
G00 X50.0 Z5.0 T0101
G76 P021060 Q100 R100
G76 X28.2 Z-32.0 P900 Q500 F1.5
G00 X200.0 Z200.0 T0100
M30
*

TRAINING
(Exampal1) G76 Compound type thread cycle

M40x1.5
M20x1.5

P=1.5
20

P=1.5

25
50

PROGRAM
N10 G97 S800 M03
T0300
G00 X30.0 Z5.0 T0303
G76 P021060 Q100 R100
G76 X18.2 Z-20.0 P900 Q500 F1.5
G00 X50.0 Z-20.0

G76 P021060 Q100 R100
Omissible

G76 X38.2 Z-52.0 P900 Q500 F1.5
G00 X200.0 Z200.0 T0300
M30
*

51

TRAINING

G90
G00
G01

-Z

+Z

50

-X

N1234
N1235
N1236
N1237

G90
G90
U-8
U-8
52

X41

Z-50

Ø25

4 4

+X

TRAINING
G90 Fixed cycle
1) Single fixed cycle for cutting

FORMAT G90 X(U)

Z(W) _R _F_

Taper cutting

X(U)

: X coordinate at the tnd point of Z

Z(W)

: End point

R-

: When cutting from the start point to X+ direction

R+

: When cutting from the start point to X- direction

I/R

: Inclination(Designate the radius value)
G90X(U)

Z(W)

X

F

;

G90X(U)

Z(W)

R

F

;

X

Z

W

3(F)

U/2

U/2

4(R)
1(R)

X/2

Z

X/2

Z

R

2(F)
W

R... Rapid traverse
F... Cutting traverse specified by F code

1. U<0,

W<0, R<0

2. U>0,

W<0, R>0

X

X

W

Z

Z

2(F)
R
1(R)
R

3(F)

U/2

U/2

4(R)

1(R)

3(F)
4(R)

2(F)
W

3. U<0,
at

R

W<0, R>0
U
2

4. U>0,
at

X

R

W<0, R<0
U
2

X
W
Z

Z
R

4(R)
U/2

2(F)

2(F)
3(F)

1(R)

R

U/2

1(R)
3(F)

4(R)

W

53

Z

TRAINING
Example)

X

2

Ø50

Z

Ø30

R
Ø40

Ø60

X

2

Z

40

Ø30

Exampal1) When the taper is R

30

PROGRAM

PROGRAM

G30 U0 W0 :

G30 U0 W0 :

G50 S2000 T0100 :

G50 S2000 T0100 :

G96 S200 M03 :

G96 S200 M03 :

G00 X61.0 Z2.0 T0101 M8 :

G00 X56.0 Z2.0 T0101 M08 :

G90 X55.0 W–42.0 F0.25 :
X50.0 :

G90 X51.0 W-32.0 F0.25 :

X45.0 :

X46.0 :

X40.0 :

X41.0 :

Z-12.0 R-1.75 :

X36.0 :

Z-26.0 R-3.5 :

X31.0 :

Z-40 R-5.25 :

X30.0 :

G30 U0 W0 :

G30 U0 W0 :

M30 :

M30 :

When cutting of inside diame-

ƒT

ter,above format can be used.

54

TRAINING

20
PROGRAM
N10 G50 S2000
G96 S180 M03
T0100
G00 X65.0 Z3.0 T0101
G90 X55.0 Z-20.0 F0.25
X50.0
X45.0
X40.0
X35.0
X30.0
X25.0
X20.5
X20.0
G00 X200.0 Z200.0 T0100
M30
ƒT

55

Ø60

Ø20

(Exampal1) G90 Fixed cycle

TRAINING

Ø55

Ø50

Ø20

(Exampal2) G90 Fixed cycle

20
40
PROGRAM
ex1)

ex2)

N10 G50 S2000

N10 G50 S2000

G96 S180 M03

G96 S180 M3

T0100

T0100

G00 X60.0 Z0 T0101

G0 X60.0 Z5.0 T0101 M8

G01 X-1.6 F0.2

G90 X50.0 Z-40.0 F0.25

G00 X50.0 Z1.0

X45.0 Z-20.0

G01 Z-40.0 F0.25

X40.0

G00 U1.0 Z1.0

X35.0

G90 X45.0 Z-20.0 F0.25

X30.0

X40.0

X25.0

X35.0

X20.0

X30.0

G00 X200.0 Z200.0 T0100

X25.0

M30

X20.5
X20.0
G00 X200.0 Z200.0 T0100
M30
ƒT

56

TRAINING

G92
G00
+X

G01
P3

P0
F

P1

-Z

+Z

5
50

-X

N1234

G92

X40.
57

Z-55.

F5.

40

P2

TRAINING
G92 Fixed cycle

1) Single fixed cycle for cutting
FORMAT G92 X(U)

Z(W) _R_F_

X(U)

: X axis coordinate of thread process position of each time

Z(W)

: End point

R-

: When cutting form the start point to X+ direction.

R+

: When cutting from the start point to X- direction.

I/R

: Lead(pitch)

Note) Spindle override and feedrate override of cycle distance are disregarded.

G92x(U)

Z(W)

F

G92x(U) _ Z(W)_ F_

; Lead(L) is specified

;

X
X

Z
W
U/2

Z

W
4(R)
3(R)

4(R)

2(F)

1(R)

3(R)

X/2

X/2

R

2(F)

Z

Z

L

45

r

1(R)

L

R... Rapid traverse
F... Thread cutting specified
by F code

58

45
r

TRAINING
Exampal1) When the taper is R

2

60

60

X

Z

5
Ø40

(Ø50.666)
Ø50

6.166

5

30

30

PROGRAM

PROGRAM

G30 U0 W0 :

G30 U0 W0 :

G50 S1000 T0100 :

G50 S1000 T0100 :

G97 S1000 M03 :

G97 S1000 M03 :

G00 X70.0 Z5.0 T0101 M08 :

G00 X60.0 Z5.0 T0101 M08 :

G92 X49.4 Z–32.0 R–6.166 F1.5 :

G92 X49.5 Z–30.0 F1.5 :

X49.0 :

X49.2 :

X48.7 :

X48.9 :

X48.5 :

X48.7 :

-

-

-

-

G30 U0 W0 :

G30 U0 W0 :

M30 :

M30 :

ƒT

ƒT

59

Z

Ø50

F1.5

Example) M50 x 1.5

TRAINING
(Exampal1) G90 Fixed cycle

M30x1.5
P=1.5

30

PROGRAM
N10 G97 S1000 M03
T0300
G00 X35.0 Z5.0 T0303
G92 X29.5 Z-32.0 F1.5
X29.2
X28.9
X28.7
:
G00 X200.0 Z200.0 T0300
M30
ƒT

60

TRAINING
(Exampal2) G92 thread cycle

M40x2.0
M20x2.0

15
30

20

PROGRAM
N10 G97 S1500 M03
T0300
G00 X30.0 Z5.0 T0303
G92 X19.5 Z-15.0 F2.0
X19.2
X18.9
X18.6
X18.4
:
G00 X50.0
Z-25.0 S1000
G92 X39.5 Z-50.0 F2.0
X39.2
X38.9
X38.6
X38.4
G00 X200.0 Z200.0 T0300
M30
∗
61

TRAINING

G94
G00

-Z

+Z

50

-X

N1234

G94

62

X25.

Z-50.

Ø25

+X

G01

TRAINING
G94 (Stock vemoval cycle in facing)
FORMAT G92 X(U)

Z(W)_R_F_

X(U)

: End point

Z(W)

: (End point of inclination)= a point of cycle distance

R-

: program the veal inclined value.

F

: Cutting feedrate

G94X(U)

Z(W)

F

;

G90X(U)

Z(W)

R

F

;

X
X
1(R)
2(F)

X/2

Z

W

4(R)
3(F)

U/2

2(F)

3(F)

W

X/2

1(R)

U/2

4(R)

R
Z

Z

a
Z

R... Rapid traverse
F... Cutting traverse specified by F code

1. U<0,

W<0, R<0

2. U>0,

W<0, R<0

X

X

R

W

Z

Z

3(F)
U/2

U/2

4(R)
1(R)

2(F)
3(F)
R

4(R)

2(F)
1(R)

W

3. U<0,
at

W<0, R>0

R

4. U>0,
at

W

X

W<0, R<0

R

W

X
R

W

Z

Z
3(F)

2(F)

U/2

U/2

1(R)
4(R)

4(R)

2(F)
1(R)

3(F)
R
W

63

TRAINING
Exampal)

Z

20

PROGRAM
G30 U0 W0 :
G50 S2000 T0100 :
G96 S200 M03 :
G00 X85.0 Z2.0 T0101 M08 :
G94 X40.0 Z–2.0 F0.2
Z–4.0 :
Z–6.0 :
Z–8.0 :
Z–10.0 :
Z–12.0 :
Z–14.0 :
Z–16.0 :
Z–18.0 :
Z-19.7 :
Z–20.0 :
G30 U0 W0 :
M30 :
*

64

2

Ø40

Ø83.5

X

TRAINING

8

PROGRAM
N10 G50 S2500
G96 S180 M03
T0100
G00 X55.0 Z2.0 T0101
G94 X15.0 Z-2.0 F0.2
Z-4.0
Z-6.0
Z-8.0
G00 X200.0 Z200.0 T0100
M30
*

65

Ø50

Ø15

(Exampal 1) G94 Stock removal cycle in facing

TRAINING

10

Ø80

Ø40

Ø12

(Exampal 2) G94 Stock removal cycle in facing

7

PROGRAM
ex1)

ex2)

N10 G50 S2500 :

N10 G50 S2500 :

G96 S180 M03 :

G96 S180 M3 :

T0300 :

T0300 :

G00 X85.0 Z2.0 T0303 :

G0 X85.0 Z2.0 T0303 :

G94 X12.0 Z-2.0 F0.2 :

G94 X12.0 Z-2.0 F0.2 :

Z-4.0 :

Z-4.0 :

Z-6.0 :

Z-6.0 :

Z-7.0 :

Z-7.0 :

G00 X85.0 Z-5.0 :

X 40.0 Z-9.0 :

G94 X40.0 Z-9.0 F0.2 :

Z-11.0 :

Z-11.0 :

Z-13.0 :

Z-13.0 :

Z-15.0 :

Z-15.0 :

Z-17.0 :

Z-17.0 :

G0 X200.0 Z200.0 T0300 :

G00 X200.0 Z200.0 T0300 :

M30 :

M30 :

∗

∗

66

TRAINING
G96, G97(Constant travelling speed control ON, OFF)

G Code

Constant travelling
speed control

G 96

ON

To control the travelling speed
constantly

m/min

G 97

OFF

Designate the rotating time of
main spindle

rpm

Meaning

Unit

Example) G96 S100 :
Cutting speed is 100m/min
G97 S100 :
Rotating time of main spindle is 100rpm
G98, G99(Feedrate selection)
G GODE

Meaing

Unit

G 98

Feedrate per minute

mm/min

G 97

Feedrate per rotation

mm/rev

Example) G98 G01 Z100.0 F50.0 :
Feedrate of tool is 50mm per minute.
G97 G01 Z10.0 F0.3 :
Feedrate of tool is 0.3mm per rotation of main spindle.

However, unless there is the G98 command, N.C unit is always in G99 condition.
Therefor it is not necessary to command G99 seperately.

67

TRAINING


b

β

∗ Calculation formular of compensation volume
α
a = r(1–tan 2 )

α

a

b = r(1–tan

β
)
2

r = Rvalue of bite
Example)

R3

20

a

b

0.4

0.468

0.234

0.8

0.937

0.468

Ø30

C1

Ø60

R3

NOSE
R=0.8

Bite Nose

23.8
23
20

80

17.8

O0035 :

17
Ø54
Ø36

Ø30
Ø34.4
Ø52.4

N10 G50 S1500 T0100 :

N20 G50 S2000 T0303 :
G96 S180 M03 :
G00 X35.0 Z5.0 M08 :
Z0:

R+r
3+0.8=R3.8

G01 X-1.6 F0.2 :
G00 X25.063 Z1.0 :

R-r
3-0.8=R2.2

G01 X30.0 Z-1.468 F0.17 :
Z-17.8 :
G02 X34.4 Z-20.0 R2.2 :
G01 X52.4 :

Concave R = R–r

G03 X60.0 Z-23.8 R3.8 :

Convex R = R+r

G01 Z-80.0 :

R : Circumference R

G00 X150.0 Z150.0 :

r : Bite r

T0300 :
M30 :
68

TRAINING
Example) PROGRAM

0O
R1 C

A

Ø60

Ø70

B

55
75

CB = (70 – 60) ÷ 2 = 5
OC = R10 – 5 = 5
AO = 10
AC = (AO)2 – (OC)2 28.66
55 – 8.66 = 46.34

G00 X60.0 Z3.0 :
G42 Z1.0 :
G01 Z-46.34 F0.23 :
G02 X70.0 Z-55.0 R10.0 :
I10.0
G01 Z-75.0

69

TRAINING
Example) PROGRAM
80

F
30
R5

D
a
B

C
E

G

C

B

F

E

A
a
R3

20

EF = (100 – 60) ÷ 2 = 20

BF = 20° tan x 15 = 5.45955

OC = 20 x 30 tan = 11.547

α = (180 – 70) ÷ 2 = 55°

α = (180 – 60) ÷ 2 = 60°

BC = 3 x 35° tan = 2.1

AC = BC

AC = AB

AC = 2.887 x 60° sin = 2.5

AE = 2.1 x 70° sin = 1.973

2.887 x 30° cos = 2.5

Ø60

Ø30

Ø100

D

∗ X ¡ 1.973 x 2 = 3.947

∗ X ¡ 2.5 x 2 = 5
CG = 2.887 x 30° sin = 1.444

♠ Coordinate value

2.887 x 60° cos = 1.444

A ¡ X = 60 – 3.947 = 56.053
Z = 5.459 – 0.718 = 4.741

♠ Coordinate value

C ¡ X = 60

A ¡ X = 60

Z = 5.459 + 2.1 = 7.559

Z = 80 – (CE – AC) = 65.566

D ¡ X = R3 – AE ¡ 3 – 1.973 = 2.054

B ¡ X = 60 + BG = 65

Z = BE + BC ¡ 2.1 + 0.718 = 2.816

Z = 68.453 + 1.444 = 69.897
A ¡ X = R5 = 5
Z=0

70

TRAINING

O'
E
R3

R3

O"

E

J

0

D

ø78

C
ø50

H

A
R30

30

G

F

O

ø10
B

A

1)

30
5
0

B

(29.58)

OC = 30, CF = 25

C

2)

(OB)2 = (OA)2- (AB)2 = (30)2 - (5)2 = 875 = 29.58

30

25
F

COF = SIN

O

(16.583)

OF = (50)2 - (25)2 = 16.583

COF = 25 = 56.442O
50

COF =

O'CD

COF =

O'CD

C
30
25
0

X

O'D = 25

DH = O'H - O'D = 30 - 25 = 5

F

O' of

CF = O'D

6D = 25

50 + 25 + 25 = 100

O' of Z

OB + OF + CD = 29.58 + 16.383 + 16.583 = 62.746

O" of X

78 - 6 = 72

O' E =

(100-72)
= 14
2

33

O'
14

O"

O"O' = 3 + 30 = 33
O'E = 14

O"E = 332 - 142 = 29.883

E

E of Z

62.746 + 29.883 = 92.629

I of X

72 + 1.2727 + 1.2727 = 74.5454

I of Z

92.629 - 2.7166 = 89.9124

SIN

O'O"E = 14 = 25.1027O
33
I
3
I J = SIN 25.1027 X 3 = 1.2727
25.1027

O"

O

J O"J = COS 25.1027 X 3 = 2.7166

71

TRAINING
(Example 1)
Process
Dimension
Material

Facing process, Outside diameter process
ø 45 x 60L
S45C

10

15

10

Ø45

Ø40

Ø30

Ø20

Ø10

4-C1

10

60

Condition of using tool

Facing process

Outside diameter process

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

PCLNR/L

Stock removal

PCLNR/L

Stock removal

PCLNR/L–1

Finishing

PCLNR/L–1

Finishing

72

TRAINING
(Example 2)

Material

ø 70 x 100L
S45C

C1

20

40

Ø50

Ø30

C2

20

100

Condition of using tool

Facing process

Outside diameter process

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

PCLNR/L

Stock removal

PCLNR/L

Stock removal

PCLNR/L–1

Finishing

PCLNR/L–1

Finishing

73

Ø70

Dimension

Facing process, Outside diameter taperprocess

Ø60

Process

TRAINING
(Example3)

S45C

Ø20

R2

15

30

C2

15

75

Condition of using tool

Facing process

Outside diameter process

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

PCLNR/L

Stock removal

PCLNR/L

Stock removal

PCLNR/L–1

Finishing

PCLNR/L–1

Finishing

74

Ø60

C1

Ø50

Material

ø 60 x 75L

Ø40

Dimension

Facing process, Outside diameter taper process(Chamfering, R process)

Ø30

Process

TRAINING
(Example4)
Process
Dimension
Material

Facing process, Outside diameter(Groove process, Chamfering R process)
ø 70 x 70L
S45C

R5

4-C1

15

15

15

Ø70

Ø60

Ø50

Ø30

Ø20

3

2

2

3

10

70

Condition of using tool

Facing process

Outside diameter process

Groove process

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

PCLNR/L

Stock removal

PCLNR/L

Stock removal

PCLNR/L

Stock removal + Finishing

PCLNR/L–1

Finishing

PCLNR/L–1

Finishing

PCLNR/L–1

75

TRAINING
(Example5)
Process
Dimension
Material

Facing process, Outside diameter(Groove process, Chamfering R process, Thread process)
ø 90 x 80L
S45C
C1.5

R3

5

10

20

25

80

Condition of using tool
Facing process

Outside diameter process

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

PCLNR/L

Stock removal

PCLNR/L

Stock removal

PCLNR/L–1

Finishing

PCLNR/L–1

Finishing

Groove process

Thread process

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

R/L 154.91

Stock remova + Finishing

R/L 166.0

Stock remova + Finishing

76

Ø90

Ø80

Ø60

Ø40

C2

Ø30

C2

TRAINING
(Example6)

Dimension
Material

Facing process, Outside diameter(Groove process, Thread process, Relief)
ø 65 x 88L
S45C

+

M42 2.0
C1

M42 2.0
+

Process

2-C1.5

R2

10

40

Ø65

Ø55

Ø42

Ø36

1

15

85

Condition of using tool
Facing process

Outside diameter process

Groove process

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

PCLNR/L

Stock removal

PCLNR/L

Stock removal

R/L 154.91

Stock removal + Finishing

PCLNR/L–1

Finishing

PCLNR/L–1

Finishing

Facing process

Thread process

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

Relief

Stock remova + Finishing

R/L 166.0

Stock remova + Finishing

77

TRAINING
(Example7)

R3

R6

S45C

R13

Ø77

Material

ø 80 x 120L

R16

Dimension

Outside diameter R process

Ø80

Process

5.66
5

31

5

25.3

5 11.2 5

120

Condition of using tool

Outside diameter process
TOOL

PROCESS TYPE

SVVBN

Stock removal + Finishing

78

5

TRAINING
(Example8)

S45C

R3

Ø50

5
120

Condition of using tool

Outside diameter circumference process
TOOL

PROCESS TYPE

SVVBN

Stock removal + Finishing

79

Ø10

R3

0

R3
0

Material

ø 82 x 120L

Ø78

Dimension

Outside diameter circumference process

Ø82

Process

TRAINING
(Example9)
Process
Dimension
Material

Outside diameter(Groove process, Thread process, Chamfering R process)
ø 60 x 110L
S45C

C1
3

20

20

20

15

15

105

Condition of using tool
Facing process

Outside diameter process

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

PCLNR/L

Stock removal

PCLNR/L

Stock removal

PCLNR/L–1

Finishing

PCLNR/L–1

Finishing

Groove process

Thread process

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

R/L 154.91

Stock remova + Finishing

R/L 166.0

Stock remova + Finishing

80

Ø60

3

C1.5

Ø40

C0.5

3

3

C3
R10

Ø20

R3

TRAINING
(Example10)
Process
Dimension
Material

Outside diameter process, Inside diameter process
ø60 x 110L
S45C

20

25

10

10

Ø90

Ø80

Ø70

Ø50

Ø40

Ø30

Ø20

105

10

60

Condition of using tools
Outside diameter process

Facing process

Inside diameter process

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

PCLNR/L

Stock removal

PCLNR/L

Stock removal

S-20S PCLNR/L

Stock removal

PCLNR/L–1

Finishing

PCLNR/L–1

Finishing

S-20S PCNR/L-1

Finishing

81

TRAINING
(Example11)
Process
Dimension
Material

Outside diameter process, Inside diameter process
ø110 x 75L x ø25(Pipe)
S45C

C1

R1
C1

C1

10

10

Ø110

Ø105

Ø90

Ø70

Ø50

Ø40

Ø30

Ø25

C1

10

70
Problem 1) Program when the material is pipe
Problem 2) Program when the material is a round bar

Condition of using tools
Outside diameter process

Facing process

Inside diameter process

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

PCLNR/L

Stock removal

PCLNR/L

Stock removal

S-20S PCLNR/L

Stock removal

PCLNR/L–1

Finishing

PCLNR/L–1

Finishing

S-20S PCNR/L-1

Finishing

82

TRAINING
(Example12)
Process
Dimension
Material

Outside diameter process, Inside diameter process
ø 110 x 75L x ø 25(Pipe)
S45C

10

20
C1

15

15

R5

C1
C0.5

3

C0.5
C1

3

3

3

15

15

12

75

Condition of using tool
Facing process

Outside diameter process

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

PCLNR/L

Stock removal

PCLNR/L

Stock removal

PCLNR/L–1

Finishing

PCLNR/L–1

Finishing

Groove process

Inside diameter process

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

PCLNR/L

Stock remova + Finishing

S-20S PCLNR/L

Stock remova

S-20S PCLNRL-1

Finishing

PCLNR/L–1

83

Ø115

Ø110

Ø100

Ø85

Ø80

Ø40
Ø50

Ø25

C1

Ø20

R2

TRAINING
(Example13)
Process
Dimension
Material

Outside diameter process, Inside diameter process(Chamfering, R, Groove)
ø90 x 60L x ø20(Pipe)
S45C

35

R3

3
2

C1

5

10

20

55
Problem 1) Program when the material is pipe
Problem 2) Program when the material is a round bar

Condition of using tool
Facing process

Outside diameter process

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

PCLNR/L

Stock removal

PCLNR/L

Stock removal

PCLNR/L–1

Finishing

PCLNR/L–1

Finishing

Inside diameter Groove process

Inside diameter process

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

PCLNR/L

Stock remova + Finishing

S-20S PCLNR/L

Stock remova

S-20S PCLNRL-1

Finishing

PCLNR/L–1

84

Ø90

Ø40
Ø50
Ø80

C1

Ø20

R2

Ø25

C1

TRAINING
(Example14)

S45C

15

R2
1

25

10

M8 2.0
+

20

3-C1.5
3

1
3

3

M50 1.5
+

Material

ø110 x 90L x ø20(Pipe)

3 3

Dimension

Outside diameter process(Chamfering, R, Groove, Thread, Relief process)

3

Process

4-C1

M40 1.5

10

10

15

15

90

Problem 1) Program when the material is pipe
Problem 2) Program when the material is a round bar

Condition of using tools
Facing process

Outside diameter process

Inside diameter process

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

PCLNR/L

Stock removal

PCLNR/L

Stock removal

S-20S PCLNR/L Stock removal

PCLNR/L–1

Finishing

PCLNR/L–1

Finishing

S-20S PCNR/L-1

Inside diameter Groove process Vutsude diameter relief process

TOOL

PROCESS TYPE

Finishing

Outside diameter Groove process

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

TOOL

PROCESS TYPE

R/L 154.3

Stock removal + Finishing

PCLNR/L

Stock removal

R/L 154.91

Stock removal + Finishing

PCLNR/L–1

Finishing

85

Ø110

Ø105

Ø80
Ø88
Ø100

Ø35
Ø40
Ø50

Ø25

Ø20

+

R2

TRAINING
Calesslating table of trigonometric function

2

C = A+B

2

Sin D =

A

A

B
A

2

B = A-C

E = 90°−E

2

A
B

B

B

E
90°

90° D

90°

90°

D

C

C

Sin E =

C
A

A = B+C

D = 90°−E

tan D =

A

A

B
C

B

90°

90°

B

E

E

90°

D

90°

C=AxcosD

B=SinDxA

C

B=AxcosE

A

A

B=AxSinE

A

A

90°

D

E

B

B

E
90°

D

C

C

90°

D

90°

C

A= C
SinD

C

A= B

C=BxcotD

A
B

B

90°

D

E

E

B

B

90°

A=BxtanE

cosE

A

90°

90°

D
C

A= C
cosD

C

A= C
SinE

B=CxtanD

A

90°

D

E
B

E

B

90°

90°

90°

D
C

C

B=

B=CxcotE

A

AxSinF
cosD

C

E=180°-(D-F)

AxSinE
B = sinD

B

F

F

tanD = AxSinE
B-AcosE
B

C

D

D

C

D

E

D
E

E
A

A

AxSinE
C = SinD
C

F=180°-(D+E)
D
F

SinF =

F

F

A
2BC

SinD =

B-SinF
A

F=180°-(D+E)

B

B

D

D
F

E
A

E

A

cosD = C+B+A
C

B

D

D
E

2

E=180°-(D+F)

B

D

E

AxBxSinE

BxSinD
A

A

A

86

D
F

E

TRAINING
FORMULA
1. The puthagorean theorem

C

B

C2 = A2 + B2

C = A2 + B2

A2 = C2 – B2

A = C2 – B2

B2 = C2 – A2

B = C2 – A2

A

2. Trigonometric function

C

B

α°

SINα° = B , COSα° = A , TANα° = B
C
C
A
B
TANα°
B = A × TANα°
C= A
COSα°

A = C × COSα°

A

A=

B = C × SINα°
C= B
SINα°
3. SIN law

When finding the length of the two sides(Oneside and two angles are known)
When finding the other angle(Two sides and one angle are know)

γ°
A

B

A = B = C
SINα° SINβ° SINγ°

α°

β°
C
4. COS law

When finding the other side(Two sides and one angle are known)
When finding the other angle(Lengthsof three sides are known)

α°
C

B

A2 = B2 + C2 – 2B.C COSα°
B2 = C2 + A2 – 2C.A COSβ°

β°

γ°

C2 = A2 + B2 – 2A.B COSγ°

A
87

2
2
2
COSα° = B + C – A
2BC
2
2
2
COSβ° = C + A – B
2CA
2
+
B2 – C2
A
COSγ° =
2AB

TRAINING
♠ DECHNICAL GUIDE
CALCULATING FORMULA

♠ Drocess time(sec/ea) =

¥. D. L x 60
Cutting length x 60
=
= sec
100V x F
Arerage of rotating time

♠ Output(8Hrs/day) = 8Hrs x 60 x 60 = ea
Required time per unit

♠ Required day for process =

Object time x Quantity to be processed
=Day
8 x 60
60

2
♠ Surface roughress = Feed volume x 1000 = R.t µm
8 x NOSER

♠ Cutting volume = cm3/min

V = Cutting speed
F = Feed volume(mm/rev)

V. F.D = LT

D = Depth of cutting

ft x W xD
1000

ft = Feedrate(mm/min)

= ML

W= Width of cutting

♠ Cutting condition(Material : AL)
∗ EXTREME – FINISHING

V = 870
F = 0.05~0.15
t = 0.025~2.0

∠ FINISHING

V = 720
F = 0.1~0.3
t = 0.5~2.0

∠ LIGHT
ROUGHING

V = 600
F = 0.2~0.5
t = 2.20~4.0

88

TRAINING
Cutting condition

1. Cutting condition
Material

Classification

Depth of cutting
d(mm)

Cutting speed
v (m/min)

Feedrate
F (mm/rev.)

Material of tool

Carbon steel

Stock vemoval

3~5

180 ~ 200

0.3 ~ 0.4

P 10 ~ 20

2~3

200 ~ 250

0.3 ~ 0.4

P 10 ~ 20

0.2 ~ 0.5

250 ~ 280

0.1 ~ 0.2

P 01 ~ 10

60kg/mm
(Tensile
Finishing

strength)

Thread

124 ~ 125

Grooving

90 ~ 110

0.08 ~ 0.2

P 10 ~ 20

Center drill

1000 ~ 1600 rpm

0.08 ~ 0.15

SKH 2

0.08 ~ 0.2

SKH9

~ 25

Drill
Alloy steel
140kg/mm

P 10 ~ 20

Stock removal

3~4

150 ~ 180

0.3 ~ 0.4

P10 ~ 20

Finishing

0.2 ~ 0.5

200 ~ 250

0.1 ~ 0.2

P 10 ~ 20

70 ~ 100

0.08 ~ 0.2

P 10 ~ 20

2

Grooving
Castiron

Stock removal

3~4

200 ~ 250

0.3 ~ 0.5

K 10 ~ 20

HB 150

Finishing

0.2 ~ 0.5

250 ~ 280

0.1 ~ 0.2

K 10 ~ 20

100 ~ 125

0.08 ~ 0.2

K 10 ~ 20

Grooving
Aluminum

Stock removal

2~4

400 ~ 1000

0.3 ~ 0.5

K 10

Finishing

0.2 ~ 0.5

700 ~ 1600

0.1 ~ 0.2

K 10

350 ~ 1000

0.1 ~ 0.2

K 10

Grooving
Bronge
Brass

Stock removal

3~5

150 ~ 300

0.2 ~ 0.4

K 10

Finishing

0.2 ~ 0.5

200 ~ 500

0.1 ~ 0.2

K 10

150 ~ 200

0.1 ~ 0.2

K 10

Grooving
Staialess steel

Stock removal

2~3

150 ~ 180

0.2 ~ 0.35

P 10 ~ 20

Finishing

0.2 ~ 0.5

180 ~ 200

0.1 ~ 0.2

P 01 ~ 10

60 ~ 90

Grooving

~ 0.15

(Note) 1) Conditions for tools coated
2) Cutting condition shall be changed by the shape and angle of tools

89

P 10 ~ 20

TRAINING
2. Cutting time of thread process(For thread precessing with the S 45 C)

H/8

0.072P

H1 H2

R
P

H

H/4

PITCH

P1.0

1.0

1.25

1.5

1.75

2.0

2.5

3.0

3.5

4.0

4.5

5.0

CUTTING DEPT

H2

0.6

0.74

0.89

1.05

1.19

1.49

1.79

2.08

2.38

2.68

2.98

CORNER ROUND

R

0.07

0.09

0.11

0.13

0.14

0.18

0.22

0.25

0.29

0.32

0.36

1

0.25

0.30

0.30

0.30

0.30

0.30

0.35

0.35

0.35

0.40

0.45

2

0.20

0.20

0.20

0.25

0.25

0.28

0.30

0.35

0.35

0.35

0.35

3

0.10

0.11

0.14

0.16

0.20

0.24

0.26

0.30

0.30

0.30

0.32

4

0.05

0.08

0.12

0.12

0.14

0.20

0.22

0.25

0.26

0.28

0.30

0.05

0.08

0.10

0.11

0.15

0.18

0.20

0.23

0.25

0.25

0.05

0.07

0.08

0.11

0.13

0.15

0.20

0.22

0.25

0.05

0.06

0.09

0.10

0.12

0.17

0.20

0.20

0.05

0.07

0.08

0.10

0.14

0.15

0.17

0.05

0.07

0.08

0.10

0.12

0.15

10

0.05

0.05

0.10

0.10

0.15

11

0.05

0.05

0.08

0.08

0.10

0.05

0.05

0.08

0.10

0.05

0.05

0.08

14

0.05

0.06

15

0.05

0.06

5
SCREW
CUTTING

6
7
8

NUMBER OF
TIMES

9

12
13

90

TRAINING

+X

-Z

+Z

W

M

WORK SHIFT VALUE

-X

OFFSET / GEOMETRY
NO.
X
1.000
10.000
G 01
-49.561
1.486
G 02
-49.561
1.486
G 03
0.000
0.000
G 04
-49.561
1.486
G 05
-49.561
1.486
G 06
-49.561
1.486
G 07
-49.561
1.486
G 08
ACT. POSITION(RELATIVE)
U
0.000
NUM.
MZ
120.

WEAR

GEOM

RESET

O1000
Z
0.000
0.000
0.000
0.000
0.000
0.000
0.000

W
S MDI

CURSOR

0.000
0T

N0000
R

T
0
0
0
0
0
0
0

7
O

8
N

9
G

ALTER

4
X

5
Y

6
Z

INSRT

1
H

2
F

3
R

DELET

–
M

0
S

.
T

/ #
EOB

4t h
B

K
J
I

Q
P

CAN

PAGE
POS

PRGRM

MENU
OFSET

INPUT

DGNOS
PARAM

OPR
ALARM

AUX
GRAPH

OUTPT
START

W.SHIFT MRCRO

91

NO.

TRAINING

RESET

WORK SHIFT
(SHIFT VALVE)
X
0.000
Z 23.061

CURSOR

ACT. POSITION(RELATIVE)
U
0.000
ADRS.

GEOM

8
N

9
G

ALTER

4
X

5
Y

6
Z

INSRT

1
H

2
F

3
R

DELET

–
M

0
S

.
T

/ #
EOB

4t h
B

K
J
I

Q
P

CAN

NO.

PAGE

MDI

WEAR

7
O

POS

PRGRM

MENU
OFSET

INPUT

DGNOS
PARAM

OPR
ALARM

AUX
GRAPH

OUTPT
START

W.SHIFT MRCRO

Work shift method using the tool measure

1.Return to the reference manually.
2. Install the work piece to the JAW and move the TURRET to appropriate position, and then prepare the basic tools to work.
3. On the section of material, TOUCH of process in facing the basic tool
∴At this, it is absolutely not allowed to move the Z spindle.
4. Select WORK/SHIFT screen.
PAGE

Method) MENU
OFSET

Push the bottun to select the WORK/SHIFT

5. Inpit the DATA.
Method) M

W

5
Z

DATA push bottuns one by one, and push MEASURE on the

console, and push INPUT , then identify the input.
∗ DATA

Z coordinate value in the program (Touched position)

∗ After input, Z value on the screen of WORK/SHIFT is automatically calculated and input.
6. As the input is completed,
PAGE

Push

to select the OFFSET screen.

92

TRAINING

Offs.
+X

+Z

-Z

60
80

-X

OFFSET / GEOMETRY
NO.
X
1.000
10.000
G 01
-49.561
1.486
G 02
-49.561
1.486
G 03
0.000
0.000
G 04
-49.561
1.486
G 05
-49.561
1.486
G 06
-49.561
1.486
G 07
-49.561
1.486
G 08
ACT. POSITION(RELATIVE)
U
0.000
NUM.
MZ
120.

WEAR

GEOM

RESET

O1000
Z
0.000
0.000
0.000
0.000
0.000
0.000
0.000

W
S MDI

CURSOR

0.000
0T

N0000
R

T
0
0
0
0
0
0
0

7
O

8
N

9
G

ALTER

4
X

5
Y

6
Z

INSRT

1
H

2
F

3
R

DELET

–
M

0
S

.
T

/ #
EOB

4t h
B

K
J
I

Q
P

CAN

PAGE
POS

PRGRM

MENU
OFSET

INPUT

DGNOS
PARAM

OPR
ALARM

AUX
GRAPH

OUTPT
START

W.SHIFT MRCRO

93

NO.

TRAINING

OFFSET / GEOMETRY
NO.
0.000
G 01
0.000
G 02
0.000
G 03
0.000
G 04
0.000
G 05
0.000
G 06
0.000
G 07

Z

GEOM

W

N0000
R

T
0
0
0
0
0
0
0

0.000
0.000
0.000
0.000
0.000
0.000
0.000

0.000
0.000
0.000
0.000
0.000
0.000
0.000

ACT. POSITION(RELATIVE)
U
0.000
NUM.
MZ
120.

WEAR

RESET

O1000
X

CURSOR

0.000

S MDI

7
O

8
N

9
G

ALTER

4
X

5
Y

6
Z

INSRT

1
H

2
F

3
R

DELET

–
M

0
S

.
T

/ #
EOB

4t h
B

K
J
I

Q
P

CAN

NO.

PAGE

0T

POS

PRGRM

MENU
OFSET

INPUT

DGNOS
PARAM

OPR
ALARM

AUX
GRAPH

OUTPT
START

W.SHIFT MRCRO

OFFSET method using Tool measure
Z axis OFFSET
1. After selecting OFFSET screen
CURSOR

push

to move the OFFSET No. of the basic tool .

∗ In gereral, tool no. and OFFSET No. shall be the same
2. After selecting numbers, input the coordinate value of Z in the current position which is touched.
The method shall be the same as work shift. For summary,

M

W

5
Z

DATA

MEASURE

INPUT
Located in the console

Touched currend position is the Z coordinate value in the program.
Select Z axis. In case of X axis,

4
X

should be pushed.

Indicates the initial “M” of measure.
After input as above, Z value of OFFSET selected by the cursor is automatically input, but the
basic tool becomes “ 0 ”(zero). If another value is given, start from the begining again.(Work shift
end)
X axis OFFSET
3. Continuously, process the outside diameter with the basic tool, and retreat the Z spindle to +
direction(right hand), stop rotating, then measure the processed outside diameter(Xvalue). If the
measured value is ø52.34, the position of tool is X52.34 therefor, input the X value.

M

5
Z

DATA

MEASURE
5

2

¡⁄

INPUT
3

4

94

TRAINING
∗ As you input with above method, X value on OFFSET screen is automatically input.
4. prepare another tool which you want to OFFSET to the work position.
5. Touch slightly on the section of the material.
6. If you input with the same method as finding the OFFSET value of Z spindle written previously, Z
OFFSET value of this tool is autonatically input. (Difference of length compared with the basic
tool)
7. Find the X OFFSET value with the same method as 3.
8. For all other tools, OFFSET with repeating above method(1~3).
(Attention)
1. On WORK/SHIFT screen, input only Z value, not X value.
(∗ Except the GANG TYPE)
2. For the drill and a kind of center drill, input only the OFFSET of Z spindle, leave the X value as
“ 0 ”.
3. Above explanation to find the value of OFFSET is the method when input only the Z value on
WORK/SHIFT screen.
If you input the X axis with the Z axis on WORK/SHIFT screen, you should input the OFFSET
value of X spindle for all tools which are processed in the center of main spindle like the drill
and the center drill.
5. If you OFFSET with above method with using the function of tool measure, you don,t have to
designate the coordinate as G50 during the programming.
Example)
(When using TOOL MEASURE)
O 3333 :
N1 G50 T0100 S1800 M42 :
G96 S100 M03 :
(When not using TOOL MEASURE)
O 3334 :
N1 G50 T100. Z100. T0100 S1800 M42 :
G96 S170 M03 :

95

TRAINING
M-FUNCTION
M00 : PROGRAM STOP
When M00 is commanded in automatic operation mode(MDI or MEM mode), the automatic operation will stop after completion of the command in the block containing M00.
When the machine is stopped by M00 code. Manual operation can be done if the mode selector
switch is turned to JOG position.
To restart cycle, select the mode selector switch to previous automatic operation mode and then
depress the CYCLE START button.
NOTE1)
Spindle stops after completion of M00, then chuck open-close can be done by manual without
changing the MODE.
M01 : OPTIONAL STOP
This command is used to stop the machine temporarily by slash(/) and check workpiece at the
end of each tool operations. OPTIONAL STOP switch(toggle switch) is used to selection this
code.
M02 : END OF PROGRAM
This code is used in the last block of chucking work part program to end the program.
When this code occurs during the automatic operation of the machine, the program returns to
the head after performing the other command in the block, the control is reset, this automatic
mode ends and the machine stop.
M03 : MAIN-SPINDLE FORWARD DIRECTION
Specifies to start the main spindle rotation in counterclockwise direction. S code should be specified in the same block or previous.
If M03 code is specified when the chuck is open, the sequence error will occur.
M04 : MAIN-SPINDLE REVERSE DIRECTION
Specifies to start the main spindle rotation in clockwise direction. S code should be specified in
the same block or previous.
If M04 code is specified when the chuck is open, the sequence error will occur.
M05 : MAIN-SPINDLE STOP
Specifies to stop the main spindle rotation. Even M05 is specified, the command spindle speed
remains effective. Therefore, if M03 or M04 is specified again, the spindle will rotate by the same
speed as the previous speed.
M07 : HIGH PRESSURE COOLANT ON (optional)
Specifies to start the high pressure coolant pump.
M08 : COOLANT ON
Specifies to start the coolant pump. The coolant pump will start when the COOLANT switch on
the operating panel is set to ON position.
M09 : COOLANT OFF
Specifies to stop the high pressure coolant pump and coolant pump.
M10: PART CATCHER1 ADVANCE (optional)
This command moves the part catcher1 advance.
96

TRAINING
M11 : PART CATCHER1 RETRACT (optional)
This command moves the part catcher1 retract.
M13 : AIR BLOW FOR TURRET (optional)
Air blow for turret when M13 is commanded.
M14 : AIR BLOW FOR MAIN SPINDLE (optional)
Air blow for main spindle when M14 is commanded.
M15 : AIR BLOW OFF (optional)
Air blowing stops.
This command is available on M13, M14.
M17 : MACHINE LOCK ON
Specifies to machine lock on. This command is specified only MDI mode.
M18 : MACHINE LOCK OFF
Specifies to machine lock off. This command is specified only MDI mode.
M19 : MAIN- SPINDLE ORIENTATION (optional)
This code stops main-spindle at fixed angle.
M19 Sxxx : Main-spindle multi orientation (ORIENTATION “B”)
When M19 code and S code should be specified in the same block, the spindle stops position is
determined by S code.
M24 : CHIP CONVEYOR RUN (optional)
Specifies to run the chip conveyor.
M25 : CHIP CONVEYOR STOP (optional)
Specifies to stop the chip conveyor.
M30 : PROGRAM END & REWIND (continuous running)
Return to head of the memory by M30 command, reset and stop.
The program is restarted by cycle start and specifies at last block.
M31: INTERLOCK BY-PASS (MAIN-SPINDLE & TAILSTOCK)
This code is used when cycle start is available the spindle unclamp and the tail stock quill operation during spindle rotating
M32 : STEADY REST CLAMP/UNCLAMP DURING SPINDLE ROTATION
This code is interlock by-pass of spindle rotating when STEADY REST is used.
STEASY REST clamp(M38 or M58) and unclamp(M39 & M59) is valid during spindle rotating
with M66.
M33 : REVOLVING TOOL-SPINDLE FORWARD DIRECTION
Revolving tool-spindle starts forward rotation.
M34 : REVOLVING TOOL-SPINDLE REVERSE DIRECTION
Revolving tool-spindle starts reverse rotation.
M35 : REVOLVING TOOL STOP
Revolving tool-spindle stops.
97

TRAINING
M38 : STEADY REST CLAMP(optional-right side), M58 : STEADY REST CLAMP(optional-left side)
Specifies to clamp the steady rest.

M39 : STEADY REST CLAMP(optional-right side), M59 : STEADY REST CLAMP(optional-left side)
Specifies to unclamp the steady rest.
M40 : GEAR CHANGE NEUTRAL
M41 : GEAR CHANGE LOW
M42 : GEAR CHANGE MIDDLE
M43 : GEAR CHANGE HIGH
Specifies to change the each gear range.
M46 : Prog. TAIL STOCK BODY UNCLAMP & TRACTION BAR ADVANCE (optional)
Simultaneous start of prog. Tail stock body unclamp and traction bar retract with this
command.
M47 : Prog. TAILSTOCK BODY CLAMP & TRACTION BAR RETRACT (optional)
Simultaneous start of prog. Tail stock body clamp and traction bar advance with this
command.
M50 : BAR FEEDING (optional)
When automatic bar feeder is attached, feed of material is performed.
M52 : SPLASH GUARD DOOR OPEN (optional)
The splash guard is opened with this command.
M53: SPLASH GUARD DOOR CLOSE (optional)
The splash guard is closed with this command.
M54 : PARTS COUNT (optional)
When M54 is commanded, pieces counter.
M61 : SWITCHING LOW SPEED (only aP60)
When the aP60 spindle motor is use, output torque and speed range of spindle is difference by power line switching. M61 is used to low speed rpm(Y-CONNECTION). 400 ˜
500 rpm(18.5kw)
M62 : SWITCHING HIGH SPEED (only aP60)
M62 is used to high speed rpm(

-CONNECTION). 750 ˜ 4500 rpm(22kw)

M63 : MAIN-SPINDLE CW & COOLANT ON
Simultaneous start of main-spindle forward rotation and coolant.
Spindle forward and coolant are preformed by one(M63) command. Coolant comes out
only when operation panel switch is “on”.
M64 : MAIN-SPINDLE CCW & COOLANT ON
Simultaneous start of main-spindle reverse rotation and coolant.
Spindle reverse and coolant are preformed by one(M64) command. Coolant comes out
only when operation panel switch is “on”.
98

TRAINING

M65 : MAIN-SPINDLE & COOLANT STOP
Stop of main-spindle rotation, coolant is stopped by one command.
M66 : DUAL CHUCKING LOW CLAMP (optional)
Main-chuck is closed by low pressure.
M67 : DUAL CHUCKING HIGH CLAMP (optional)
Main-chuck is closed by high pressure.
M68 : MAIN-SPINDLE CLAMP
Specified to open the main-chuck automatically such as bar work.
M69 : MAIN-SPINDLE UNCLAMP
Specified to close the main-chuck automatically such as bar work.
M70 : DUAL TAILSTOCK LOW ADVANCE (optional)
Tailstock bar is advanced by low pressure.
M74 : ERROR DETECT ON
When M74 is in effect, the control proceed to the next block regardless of the pulse lag of
servo between block for liner and circular interpolation except positioning (G00).
The permits the machine to move smoothly between blocks.
However, the corner of the workpiece may not be quite sharp.
M74 command is modal, and it will remain effective until M75 is command.
M75 : ERROR DETECT OFF
Specifies to release the state of error detection ON. When the power is turned on, M75
will be in effect, and it will remain effective until M74 is command.
M76 : CHAMFERING ON
When M76 is specified before the command of thread cutting cycle G76 or G92, the
threading tool will pull out at the terminating thread portion.
M77 : CHAMFERING OFF
Cancel the command of pull out threading function which as specified by M77 code.
M77 code is the modal code.
M78 : TAIL STOCK QUILL ADVANCE
The tail stock quill is advanced with this command.
M79 : TAIL STOCK QUILL RETRACT
The tail stock quill is retracted with this command.
M80 : QUICK-SETTER SWING ARM DOWN (optional)
Specifies to up the quick-setter swing arm.
M81 : QUICK-SETTER SWING ARM UP (optional)
Specifies to up the quick-setter swing arm.
99

TRAINING

M82 : MIRROR IMAGE ON
Specifies to mirror image on.
M83 : MIRROR IMAGE OFF
Specifies to mirror image off.
M84 : TURRET CW ROTATION
This code is used to switch the direction of turret indexing to CW when it is set in the
automatic selection mode.
As this code is as non-modal code, it should be used in the same block the T-code.
M85 : TURRET CCW ROTATION
The turret indexes in clockwise by specifying M85 in the same block of T-code.
This M85 is a non-modal code.
M86 : TORQUE SKIP ACT
This code is used to skip the torque of moving axis.
As this code is a modal code until M87 command, only valid the sub-spindle with B-axis.
EX) G00 B-500.0 ;
M86 ;
G98 G31 P99 V-20.0 F100.0 ;
G01 B-500.0 ;
M87 ;
M87 : TORQUE SKIP CANCEL
This code is used to cancel torque skip function of M86.
M88 : C-AXIS LOW CLAMP
Specified to clamp the C-axis by low pressure.
Only valid the C-axis control.
M89 : C-AXIS HIGH CLAMP
Specified to clamp the C-axis by high pressure.
Only valid the C-axis control.
M90 : C-AXIS UNCLAMP
Specified to unclamp the C-axis.
Only valid the C-axis control.
M91,M92,M93,M94 : EXTERNAL M-CODE COMMAND (optional)
There code spare M code.
M98 : SUB-Prog. CALL
This code is used to enter a sub-program.
M99 : END OF SUB-PROGRAM
This code shows the end of a sub-program.
Executing M99 take the control back to the main program.

100

TRAINING

M103 : SUB-SPINDLE FORWARD DIRECTION
Specifies to start the sub spindle rotation in counterclockwise direction. S code should
be specified in the same block or previous.
If M103 code is specified when the sub-chuck is open, the sequence error will occur.
M104 : SUB-SPINDLE REVERSE DIRECTION
Specifies to start the sub spindle rotation in clockwise direction. S code should be specified in the same block or previous.
If M04 code is specified when the sub-chuck is open, the sequence error will occur.
M105 : SUB-SPINDLE STOP
Specifies to stop the sub spindle rotation. Even M05 is specified, the command spindle
speed remains effective. Therefore, if M103 or M104 is specified again, the spindle will
rotate by the same speed as the previous speed.
M110 : PART CATCHER2 ADVANCE (optional)
This command moves the part catcher2 advance.
M111 : PART CATCHER2 RETRACT (optional)
This command moves the part catcher2 retract.
M114 : AIR BLOW FOR SUB SPINDLE (optional)
Air blow for sub spindle when M114 is commanded.
M119 : SUB-SPINDLE ORIENTATION (optional)
This code stops sub-spindle at fixed angle.
M119 Sxxx : sub-spindle multi orientation (ORIENTATION “B”)
When M19 code and S code should be specified in the same block, the spindle tops
position is determined by S code.
M131 : INTERLOCK BY-PASS (SUB-SPINDLE)
This code is used when cycle start valid on sub spindle unclamp.
M163 : SUB-SPINDLE CW & COOLANT ON
Simultaneous start of sub spindle forward rotation and coolant.
Spindle forward and coolant are preformed by one(M163) command. Coolant comes out
only when operation panel switch is “on”.
M164 : SUB-SPINDLE CW & COOLANT ON
Simultaneous start of sub spindle forward rotation and coolant.
Spindle forward and coolant are preformed by one(M164) command. Coolant comes out
only when operation panel switch is “on”.
M165 : SUB-SPINDLE & COOLANT STOP
The sub spindle rotation & coolant is stopped by one command.
M168 : SUB-SPINDLE CLAMP
Specifies to open the sub-chuck automatically such as bar work.

101

TRAINING

M169 : SUB-SPINDLE UNCLAMP
Specified to close the sub-chuck automatically such as bar work.
M203 : FORWARD SYNCHRONOUS COMMAND
Main and sub spindle start simultaneously for forward rotation.
It is synchronized with forward rotation of main and sub spindle.
M204 : REVERSE SYNCHRONOUS COMMAND
Main and sub spindle start simultaneously for reverse rotation.
It is synchronized with reverse rotation of main and sub spindle.
M205 : SYNCHRONOUS STOP
The synchronous rotation of main and sub spindle is stop.
M206 : SPINDLE ROTATION RELEASE
Specified to release the speed control of main and sub spindle.
If you want to the main and sub spindle is rotate by difference rpm, M206 is commanded before
S-code. Spindle override on operating panel valid last selected spindle.
EX) M03 S1000 ;
M206 ;
M103 S500 ;

102



---

Source Exif Data:

File Type                       : PDF
File Type Extension             : pdf
MIME Type                       : application/pdf
PDF Version                     : 1.3
Linearized                      : No
Page Mode                       : UseOutlines
XMP Toolkit                     : 3.1-702
Create Date                     : 1998:05:15 13:39:14Z
Creator Tool                    : FrameMaker 5.5
Modify Date                     : 2006:07:22 15:56:21-04:00
Metadata Date                   : 2006:07:22 15:56:21-04:00
Format                          : application/pdf
Creator                         : JR Walcott - Georgia Machine Tool Resources
Title                           : Fanuc OT G-Code Training Manual
Description                     : Training
Producer                        : Acrobat Distiller 3.01 for Power Macintosh
Document ID                     : uuid:2ef4dd67-e44c-45bc-ae39-b39bcb7032f4
Instance ID                     : uuid:890f34df-05dd-49da-8700-dca63e4d0353
Page Count                      : 104
Subject                         : Training
Author                          : JR Walcott - Georgia Machine Tool Resources

EXIF Metadata provided by EXIF.tools