Fanuc G72.2 Linear Copy (Figure Copy Function CNC Mill)

Fanuc G72.2 Linear Copy
Using G72.2 Linear Copy G-code a figure specified by a subprogram can be repeatedly produced with Linear movement.


G72.2 P... L... I... J...


PSubprogram number
LNumber of times the operation is repeated
IShift along X-axis
JShift along Y-axis

G-Code Data

Modal/Non-ModalG-Code Group

Programming Notes


  1. In the G72.2 block, addresses other than P, L, I and J are ignored.
  2. P, I and J must always be specified.
  3. If L is not specified, the figure is copied once.
  4. For shifts (I, J), specify increments. The n-th geometric shift is equal to the specified shift times (n – 1).

First block of the subprogram

Always specify a move command in the first block of a subprogram that performs a linear copy. If the first block contains only the program number such as O00001234; and does not have a move command, movement may stop at the start point of the figure made by the n-th (n = 1,2, 3, …) copying.
Example of an incorrect program

O00001234 ;
G00 G90 X100.0 Y200.0 ;
M99 ;

Example of a correct program

O00001000 G00 G90 X100.0 Y200.0 ;
M99 ;


Specifying two or more commands to copy a figure
G72.2 cannot be specified more than once in a subprogram for making a linear copy (If this is attempted, alarm PS0901 will occur).
In a subprogram that specifies linear copy, however, rotational copy (G72.1) can be specified. Similarly, in a subprogram that specifies rotational copy, linear copy can be specified.

Commands that must not be specified
Within a program that performs a linear copy, the following must not be specified:
Command for changing the selected plane (G17 to G19)
Command for specifying polar coordinates (G16)
Reference position return command(G28)
Axis switching
Coordinate system rotation (G68)
scaling (G51)
programmable mirror image (G51.1)

Single block
Single-block stops are not performed in a block with G721.1 or G72.2.

G72.2 Programming Example

Fanuc G72.2 Linear Copy

Main program

O3000 ;
N10 G90 G00 X-30. Y0 ;
N20 X0 ;
N30 G01 G17 G41 X30. D01 F100 ; (P0)
N40 Y20. ;                      (P1)
N50 X40. ;                      (P2)
N60 G72.2 P3100 L3 I90.0 J0 ;
N70 G90 X310. Y0 ;              (P8)
N80 X0 ;
N90 G40 G00 X-30.0 ;
N100 M30 ;

Sub program

O3100 G91 G01 X20. ; (P3)
N100 Y30. ;          (P4)
N200 G02 X40. I20. ; (P5)
N300 G01 Y-30. ;     (P6)
N400 X30. ;          (P7)
N500 M99 ;