Solidworks Cam Multiple parts

[Raymond1432]

Hi there,
I'm trying to make cam paths for multiple parts, i got as far as making a grid of parts in an assembly, and was able to create toolpaths for all.
The thing is, it will make a pretty good nc file, with the right toolpaths, but it will actually only create one full toolpath, then for each duplicate of the part it will reference to the toolpath, instead of having a toolpath for each part.
Now this wouldn't normally be a problem, but my cnc software (planet-cnc) doesn't know how to handle it.

This is the nc code i'm getting:
https://pastebin.com/iyVD636A
If viewed on ncviewer.com you can see what i mean. It will mvoe to the position of the next part, but you don't see the toolpath for that position, which planet-cnc doesn't know how to deal with.

I hope i have been clear in my explanation, if not, i can always elaborate, or give some screenshots.

EDIT: So i've done some more digging, what i was reffering to are subroutines, now i found that planetcnc doesn't use the regular subroutines code (M98) But uses the O-codes.
Maybe someone is familair with planet-cnc, abecause i have edited the code to correspond with their O-codes, but now an error is thrown that there are "Too many subroutine levels" now i can't find anything about that, and am not sure what they mean by that.

Similar Threads:

• multiple parts
• Multiple parts in one set up...?
• Multiple Parts In M.C.
• Multiple Parts

[c9k]

This looks like something your post processor is doing. It's doing coordinate system shifts, then running the shape programs at each location. The reason to do this (instead of just putting the whole shape gcode every time, with the X,Y,Z numbers changed appropriately) is if you like hand editing the shape, or if your controller has limited memory and can't load a program that has the shape written out for every transformation.

So you'll have to have the post tweaked to either stop making sub program callouts, or to make them in the way your machine likes.

"Too many subroutine levels" likely means you accidentally set it up into a loop where it goes into a subroutine, then calls another, and keeps doing that. Typically you can only nest around 7 times, meaning you have the "main program", then it can call a subroutine, then that sub routine can call another one, and that can keep going on for 7 levels. When the 7th subroutine tries calling another you'll get an error like "Too many subroutine levels". I'm guessing the problem is not ending the subroutines properly.

From the page here: https://planet-cnc.com/using-o-words...e-subroutines/ , to get your program working for now you need to change the start of the subroutines from "O0002" to "O0002 sub", then change the M99 to "O0002 endsub." Then change every M98 callout to be like "O0002 call" instead of "M98 P0002"