Multi-Pass Operations Using Subprograms

For multi-pass Pocket and Contouring operations, GO2cam can generate the NC program in decomposed mode or using subprograms. The machining operation does not change; only the NC output generated by the post-processor is different.

Output methods for multi-pass operations

Decomposed output

Decomposed output is the default method. The toolpath coordinates are written again for each machining pass. As a result, the NC program contains repeated coordinate blocks for every machining depth.

Output using subprograms

For Pocket and Contouring operations, GO2cam can write the repeated toolpath coordinates once in a subprogram. The main program then calls the subprogram for each machining pass.

This produces a more compact NC program and avoids repeating the same contour coordinates. The machining result and the operation defined in GO2cam remain unchanged.

Important: Subprogram output requires an adapted post-processor. Customers cannot enable this output method from the machining operation. Contact your GO2cam reseller if you want to use subprogram output. Post-Pro Builder configuration is documented separately in the VAR Area.

NC program comparison

The following examples show the same Contouring operation generated first with decomposed output and then using a subprogram.

Decomposed output

With decomposed output, the toolpath coordinates are written again for each machining pass.

N115 G01 G94 Z-50. F212
N120 X379.886
N125 Y51.5
...
N190 G01 Z-60.
N195 X379.886
N200 Y51.5
...

Output using a subprogram

With subprogram output, the repeated toolpath is defined once and called for each machining pass.

N115 G01 G94 Z-54. F212
N120 M98 P1000
...
N145 G01 Z-68.
N150 M98 P1000
...

The contour itself is then written once in the subprogram:

O1000
N5 G01 G41 D01 X369.886 Y-2. F212
...
N65 M99

What to notice

In the decomposed program, the contour coordinates are repeated for each machining depth.
With subprogram output, the main program contains repeated M98 P1000 calls, one for each machining pass.
The single O1000 block contains the contour coordinates.
M99 returns execution from the subprogram to the main program.

The NC code is included only to demonstrate the difference between the two GO2cam outputs. It is not intended as a detailed explanation of FANUC programming.

For comparison: Download the attached NC files to view the complete output in decomposed mode and using subprograms. Notice the difference in length between the two NC programs: the decomposed output is about 100 lines, while the output using subprograms is about 65 lines.

▶️ This short video shows GO2cam producing multi-pass machining either decomposed or via subprograms, and explains that subprograms keep NC files compact by writing the repeated contour once and calling it for each pass.