CNC Milling | Fanuc G72.2 Code | Linear Copy

In this article, we describe how to use G72.2 code for linear copy of a figure in CNC milling machines with all details and examples.

0
221

G72.2 Code Introduction

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

G72.2 Code Format

G72.2 P… L… I… J…

Parameters

P : Subprogram number
L : Number of times the operation is repeated
I : Shift along X-axis
J : Shift along Y-axis

Things to Know

  • In the G72.2 block, addresses other than P, L, I and J are ignored.
  • P, I and J must always be specified.
  • If L is not specified, the figure is copied once.
  • 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 ;

You may be interested also:
“Fanuc G72.1 G72.2 Figure Copy Program Example (Bolt Hole Circle)”

Limitation

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 PS0901will 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

G72.2 Programming Example

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 ;


Need to More?

Our volunteers have worked together and carefully prepared the articles published here in their native language without using machine translation. You can search the entire site for more information on the subject. You can start a discussion on CNCarea.com forums and join us to get support, ask questions, improve a published article or give your opinion.


Previous articleHow to Improve Manufacturing Efficiency
Next articleCNC | Principle of Operation of a Numerical Controlled Machine