Hi Jaydenn, change the corresponding template-part-file in the template-part directory.
Reload the configuration [or just restart] and it should be done.
Depending on how your post-processors are set up, Cutcom and Adjust values equal the tool number on post-processing. Cutcom defines a cutter radius or diameter offset, (depending on how it's defined in your machine controller tool tables), Adjust defines the G43 H value.
Using Cutcom allows some flexibility with regard to tool usage, particularly with machines with limited tool pockets.
For example, let's say you wanted to use tool number 6 for some open limit milling like a rough slot, your cutter radius D register number, (used during cutter compensation paths G41 or G42 in Fanuc code) would equal 6. However, if you wanted to use the same tool later on in the machining process, say to machine a finely toleranced bore diameter feature, you assign a different Cutcom number in order to output the different D register value, (in this example D56). The effect of this in machining land is that you can edit your wear compensation value 56 in the machine tool table to tweak your bore diameter on the fine machining, without affecting the slot width on the first feature.
The post processor will output these values by default.
Unless of course, your post has been altered in some way to remove them.
It's simply a matter of turning on the output (the item this thread is based on...)
and turning cutcom on in the operation. Go to the "NON CUTTING MOVES" dialog and choose the "MORE" tab. You will see the cutcom options.
Turn it on and post! see what happens.
Keep in mind that most machines CANNOT apply D-comp on an arc. You will get CRC alarms on the control.
Be sure the "G41" or "G42" appear on an X Y linear move.
I am familiar with this problem, and fixed it in NX 7.0.
The problem is that the cutcom register output toggle does not turn on automatically when the value is inherited. Once this toggle has been turned off in the operation, it stops inheriting, and it will not turn on by itself again, and there is no UI to turn the inheritance back on. This is why turning it on in the template does not work - it still will not be inherited.
You can fix your parts in NX6 by running the attached vb program - rename it from .txt to .vb.
This will correct the situation in all operations in the work part. I recommend you also open each template part, such as mill_planar.prt, run the program, and save the part, to prevent future problems.
Download the program.
Rename the extension to .vb.
Open the template part mach/resource/template_part/metric/mill_planar.prt.
Go to Tools --> Journal --> Play, Browse, pick the file, and Run.
Save the part.
Repeat for each template part that you use.