G992 Setting Temporary WCS

Format

• G992 X_Y_Z_
• G992 I_J_K_

Description

This command is to set temporary WCS and it can be used for realizing array function.

Its function is similar to that of command G92.

The difference between the two: command G92 alters the WCS permanently and takes the same standard to the whole system, while command G992 alters the WCS temporarily and only influences the coordinate parsing of processing command, which will be restored automatically after machining is completed.

The comparison between G992 X_Y_Z_ and G992 I_J_K_ is as follows:

• G992 X_Y_Z_ sets the current point as a specified point in the new coordinate system, while G992 I_J_K_ translates the original coordinate system a specified distance to create a new coordinate system.
• Comparatively speaking, G992 I_J_K_ is more efficient because it avoids the redundant rapid traverse command produced by origin offset, while G992 X_Y_Z_ sets an origin after returning to the original origin.

CAUTION:

During array machining, command G92 should be deleted manually because it is not supported by the system.

Programming Example

To realize array function, do one of the following:

In the methods, the first 4 parameters, i.e., #1=30, #2=40, #3=30, and #4=30, can be adjusted and customized.

• Solution 1: G992_X_Y_Z

  1. Delete command M30 in the processing file.

  2. Add the following contents at the beginning of the processing file:

     #1=30 'X offset value
     

     #2=40 'Y offset value
     

     #3=30 'machining quantity along X axis
     

     #4=30 'machining quantity along Y axis
     

     G65 P3455 L=#4
     

     G00 G90 X=-#1*#3 Y=-#2*#4
     

     G992 X0 Y0
     

     M30
     

     O3455
     

     G65 P3456 L=#3
     

     G00 G90 X=-#1*#3 Y=#2
     

     G906
     

     G992 X0 Y0
     

     M17
     

     O3456
     

  3. Add the following contents at the end of the processing file:

     G00 G90 X=#1
     

     G906
     

     G992 X0
     

     M17
     

• Solution 2: G992 I_J_K_

  1. Delete command M30 in the processing file.

  2. Add the following contents at the beginning of the processing file:

     #1=30 'X offset value
     

     #2=40 'Y offset value
     

     #3=30 'machining quantity along X axis
     

     #4=30 'machining quantity along Y axis
     

     G65 P3455 L=#4
     

     G00 G90 X=-#1*#3 Y=-#2*#4
     

     G992 I=-#1*#3 J=-#2*#4
     

     M30
     

     O3455
     

     G65 P3456 L=#3
     

     G00 G90 X=-#1*#3 Y=#2
     

     G906
     

     G992 I=-#1*#3 J=#2
     

     M17
     

     O3456
     

  3. Add the following contents at the end of the processing file:

     G00 G90 X=#1
     

     G906
     

     G992 I=#1
     

     M17