FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 51

 PROGRAMMING 

B-63944EN/03

 

 

- 364 - 

14. FUNCTIONS TO SIMPLIFY 

PROGRAMMING 

  - Angular displacement R 

A positive angular displacement R indicates a clockwise rotation 
along the axis of rotation.    Specify angular displacement R in 0.001 
degrees within the range of -360000 to 360000. 
To specify angular displacement R in 0.00001 degrees (one 
hundred-thousandth), set bit 0 (FRD) of parameter No. 11630 to 1.  
In this case, angular displacement R is specified within the range of 
-36000000 to 36000000. 
 

  - G codes that can be specified 

The following G codes can be specified in the three-dimensional 
coordinate system conversion mode: 
G00   Positioning 
G01   Linear interpolation 
G02   Circular interpolation (clockwise) 
G03   Circular interpolation (counterclockwise) 
G04   Dwell 
G10   Data setting 
G17   Plane selection (XY) 
G18   Plane selection (ZX) 
G19   Plane selection (YZ) 
G28   Reference position return 
G29   Movement from the reference position 
G30   Second, third, or fourth reference position return 
G53   Selecting the machine coordinate system 
G65   Custom macro call 
G66   Custom macro modal call 
G67   Custom macro modal call cancel 
G40   Canceling tool radius / tool nose radius compensation 
G41   Tool radius / tool nose radius compensation to the left 
G42   Tool radius / tool nose radius compensation to the right 
G73, G74, G76, G80 to G89 Canned cycle for drilling 
 

M

 

G43   Increasing tool length compensation 
G44   Decreasing tool length compensation 
G45   Increasing the tool offset 
G46   Decreasing the tool offset 
G47   Doubling the tool offset 
G48   Halving the tool offset 
G49   Canceling tool length compensation 
G50.1  Canceling programmable mirror image 
G51.1  Programmable mirror image 
G90   Absolute programming 
G91   Incremental programming 
G94   Feed per minute 
G95   Feed per revolution 
G98   Canned cycle (return to the initial level) 
G99   Canned cycle (return to the level of point R) 
 

B-63944EN/03

 PROGRAMMING 

 

 

- 365 - 

14.FUNCTIONS TO SIMPLIFY

PROGRAMMING

T

 

G90   Absolute programming (when G code system B or C is used.) 
G91   Incremental programming (when G code system B or C is 

used.) 

G94   Feed per minute (when G code system B or C is used.) 
G95   Feed per revolution(when G code system B or C is used.) 
G98   Canned cycle (return to the initial level) (when G code system 

B or C is used.) 

G99   Canned cycle (return to the level of point R) (when G code 

system B or C is used.) 

 

 

  - Rapid traverse rate in drilling of a canned cycle for drilling 

In three-dimensional coordinate system conversion mode, rapid 
traverse rate in drilling by a canned cycle for drilling equals the 
cutting feedrate specified in parameter No. 5412. If the parameter is 
set to 0, the rapid traverse rate equals the maximum cutting feedrate. 
 

 - Compensation functions 

M

 

If tool length compensation, tool radius / tool nose radius 
compensation, or tool offset is specified with three-dimensional 
coordinate system conversion, compensation is performed first, 
followed by three-dimensional coordinate system conversion. 
 

T

 

If tool radius / tool nose radius compensation is specified with 
three-dimensional coordinate system conversion, compensation is 
performed first, followed by three-dimensional coordinate system 
conversion. 
 

 

  - Relationship between three-dimensional and two-dimensional coordinate system 

conversion  

Three-dimensional and two-dimensional coordinate system conversion 
use identical G codes (G68 and G69). A G code specified with I, J, 
and K is processed as the command for three-dimensional coordinate 
system conversion. A G code not specified with I, J, and K is 
processed as the command for two-dimensional coordinate system 
conversion. 
 

  - Custom macro system variables 

Coordinates on the workpiece coordinate system are assigned to 
system variables #5041 to #5048 (current position on each axis).     
 

 PROGRAMMING 

B-63944EN/03

 

 

- 366 - 

14. FUNCTIONS TO SIMPLIFY 

PROGRAMMING 

 - Reset 

If a reset occurs during three-dimensional coordinate system 
conversion mode, the mode is canceled and the continuous-state G 
code is changed to G69. 
Bit 2 (D3R) of parameter No. 5400 determines whether just the G69.1 
code is used to cancel the three-dimensional coordinate system 
conversion mode (G68.1). When this setting is selected, a CNC reset 
by a reset operation or by an input signal from the PMC will not 
cancel the three-dimensional coordinate system conversion mode. 
 

  - Absolute position display 

The absolute coordinates based on the program or workpiece 
coordinate system can be displayed in the three-dimensional 
coordinate system conversion mode. Specify a desired coordinate 
system in bit 6 (DAK) of parameter No. 3106. 
 

  - Three-dimensional rigid tapping 

By specifying the rigid tapping command in three-dimensional 
coordinate system conversion mode, tapping can be executed in the 
direction of the angle programmed by the three-dimensional 
coordinate system conversion command. 
In three-dimensional coordinate system conversion mode, "Position 
Error Z", displayed on the spindle adjustment screen, is taken from the 
longitudinal tapping axis after three-dimensional conversion. 
Positioning in three-dimensional coordinate system conversion mode 
must be linear interpolation positioning (bit 1 (LRP) of parameter 
No.1401 is set to 1). 
 

Limitation 
 - Manual intervention 

Three-dimensional coordinate system conversion does not affect the 
degree of manual intervention or manual handle interrupt. 
 

  - Positioning in the machine coordinate system 

Three-dimensional coordinate system conversion does not affect 
positioning in the machine coordinate system (e.g. specified with G28, 
G30, or G53). 

  - Specifying rapid traverse 

Specify linear rapid traverse when three-dimensional coordinate 
system conversion is executed. (Set bit 1 (LRP) of parameter No.1401 
to 1.) 

  - Block with G68 or G69 

In a block with G68 or G69, other G codes must not be specified.  
G68 must be specified with I, J, and K. 
 

  - Position display and compensation 

To display the absolute position when three-dimensional coordinate 
system conversion is executed, set bits 4 to 7 (DRL, DRC, DAL, and 
DAC) of parameters No. 3104 to 0. 
 

B-63944EN/03

 PROGRAMMING 

 

 

- 367 - 

14.FUNCTIONS TO SIMPLIFY

PROGRAMMING

 - Mirror image 

M

 

Programmable mirror image can be specified, but external mirror 
image (mirror image by the mirror image signal or setting) cannot be 
specified. Three-dimensional coordinate system conversion is carried 
out after the programmable mirror image function is executed. 
 

T

 

External mirror image (mirror image by the mirror image signal or 
setting) cannot be specified. 

 

  - Three-dimensional coordinate system conversion and other continuous-state 

commands 

M

 

Canned cycles, G41, G42, or G51.1 must be nested between G68 and 
G69. 
(Example) 

G68 X100. Y100. Z100. I0. J0. K1. R45. ; 
 : 
G41 D01 ; 
 : 
G40 ; 
 : 
G69 ; 

 

T

 

Canned cycles, G41 or G42 must be nested between G68.1 and G69.1. 
(Example) 

G68.1 X100. Y100. Z100. I0. J0. K1. R45. ; 
 : 
G41 X_ Z_ I_ K_ ; 
 : 
G40 ; 
 : 
G69.1 ; 

 

T

 

  - Relationship between three-dimensional coordinate system conversion and tool 

offset 

When using a tool offset command, nest the tool offset command 
within the three-dimensional coordinate system conversion mode. 
(Example) 

G68.1 X100. Y100. Z100. I0. J0. K1. R45. ; 
 : 
T0101; 
 : 
T0100; 
 : 
G69.1 ; 

 PROGRAMMING 

B-63944EN/03

 

 

- 368 - 

14. FUNCTIONS TO SIMPLIFY 

PROGRAMMING 

 

  - PMC axis control 

In the three-dimensional coordinate system conversion mode, PMC 
axis control cannot be performed for the three axes related to the 
conversion (alarm). 
 

 - Manual operation 

When manual feeding is performed during a three-dimensional 
coordinate system conversion, the tangent velocity in the coordinate 
system after conversion (program coordinate system) equals the 
lowest feedrate of those on the selected axes. 
 

  - Workpiece coordinate system 

Avoid changing the workpiece coordinate system in the 
three-dimensional coordinate system conversion mode. 
 

  - Manual reference position return 

Avoid making a manual reference position return in the 
three-dimensional coordinate system conversion mode. 
 

  - Cs contour axis 

When specifying the Cs contour axis and rapid traverse at the same 
time in the three-dimensional coordinate system conversion mode, 
make a reference position return on the Cs contour axis in advance. If 
a reference position return is made in the first rapid traverse after the 
Cs contour axis is selected (bit 1 (NRF) of parameter No.3700 is set to 
0), avoid specifying the reference position return command in the 
three-dimensional coordinate system conversion mode. 
 

 

B-63944EN/03

 PROGRAMMING 

 

 

- 369 - 

14.FUNCTIONS TO SIMPLIFY

PROGRAMMING

Example 

N1 G90 X0 Y0 Z0 ; 

Carries  out  positioning  to  zero 
point H. 

N2 G68 X10. Y0 Z0 I0 J1 K0 R30. ;   Forms  new  coordinate  system 

X'Y'Z'. 

N3 G68 X0 Y-10. Z0 I0 J0 K1 R-90. ; Forms other coordinate system 

X''Y''Z''.  

 

The origin agrees with (0, -10, 
0) in coordinate system X'Y'Z. 

N4 G90 X0 Y0 Z0 ; 

Carries  out  positioning  to  zero 
point H'' on coordinate system 
X''Y''Z''. 

N5 X10. Y10. Z0 ;   

Carries  out  positioning  to  (10, 
10, 0) on coordinate 

system 

X''Y''Z''. 

 

Y

Y'

H

Z

N4

H'

X'

Y"

N5

Z"

Z'

H"

(10, 10, 0)

10

-10

30

°

30

°

X"

-90

°

 

 

15.COMPENSATION FUNCTION

 PROGRAMMING 

B-63944EN/03

 

 

- 370 - 

15 

COMPENSATION FUNCTION 

 
Chapter 15, "COMPENSATION FUNCTION", consists of the 
following sections: 
 
15.1  TOOL LENGTH COMPENSATION (G43, G44, G49) ........371 
15.2  SCALING (G50, G51) ...........................................................379 
15.3  PROGRAMMABLE MIRROR IMAGE (G50.1, G51.1) ......389 
15.4  NORMAL DIRECTION CONTROL (G40.1,G41.1,G42.1) .391 
15.5  WORKPIECE SETTING ERROR COMPENSATION.........397 

 

B-63944EN/03

 PROGRAMMING 

15.COMPENSATION FUNCTION

 

 

- 371 - 

15.1 

TOOL LENGTH COMPENSATION (G43, G44, G49) 

 
This function can be used by setting the difference between the tool 
length assumed during programming and the actual tool length of the 
tool used into the offset memory. It is possible to compensate the 
difference without changing the program. 
Specify the direction of offset with G43 or G44. Select a tool length 
compensation value from the offset memory by entering the 
corresponding address and number (H code). 

Tool assumed
during programming

Actual tool

Specify this distance as
the value of tool length
compensation.

 

Fig. 15.1 (a)    Tool length compensation 

 

15.1.1 

Overview 

 
The following three methods of tool length compensation can be used, 
depending on the axis along which tool length compensation can be 
made. 
- Tool length compensation A 
  Compensates for the difference in tool length along the basic Z-axis. 
- Tool length compensation B 
  Compensates for the difference in tool length in the direction normal 

to a selected plane. 

- Tool length compensation C 
  Compensates for the difference in tool length along a specified axis. 
 

Format 

Type Format 

Description 

Tool length compensation A 

G43 Z_ H_ ; 
G44 Z_ H_ ; 

Tool length compensation B 

G17 G43 Z_ H_ ;
G17 G44 Z_ H_ ;
G18 G43 Y_ H_ ;
G18 G44 Y_ H_ ;
G19 G43 X_ H_ ;
G19 G44 X_ H_ ;

Tool length compensation C 

G43 

α

_H_ ; 

G44 

α

_H_ ; 

Tool length compensation cancel

G49 ; or H0 ; 

G43 : Positive offset 
G44 : Negative offset 
G17 : XY plane selection 
G18 : ZX plane selection 
G19 : YZ plane selection 

α

 

: Address of a specified axis

H 

: Address for specifying the 

tool length compensation 
value 

X, Y, Z : Offset move command