Nomad + Solidworks CAM GRBL Post Processor (Z limit error)

Hi there,

I’m running a simple carving test via Solidworks CAM using hawkridge’s post processor. Not sure where i made a mistake but the machine (nomad 3) start the code with carbide motion, and after changing tool and starting the spindle, it will attempt an unusually high Z while going to zero (before starting the path).

I had successfully ran code from the same post processor on a different computer, so i’m guessing i set something up wrong on this laptop (maybe tool crib or machine related).

Any suggestions?

Thanks in advance!
cnc_test-01.NC (12.3 KB)

This line in your code

N15 G91 G28 X0 Y0 Z0

G91 incremental with the X0 Y0 Z0 tells the machine to move zero distance from where it’s at. (i.e. don’t move). The G28 tells it to move to a predefined position (Set with G28.1). If the reference point has never been set, then it is likely at Machine X0Y0Z0. This would put the Z axis on the limit switch.
Try MDI G28.1 X-100 Y-100 Z-5. (Or wherever you want your “safety/start point” Once you set this, it should remember it.

Or edit the post (If you can) to leave that line out.

1 Like

Hi Tod!
Thanks a lot for your quick reply!
Should i just MDI from carbide motion to test it first?
Or do you think there’s anything i could change in Solidworks CAM to fix it and re-process? I can’t get around the fact that the same post processor on another computer with Solidworks CAM was not writing the same problem.
I’ll give it a try today!

Perhaps one of those posts was modified, or a newer version of soldworks? No idea, really.

Your G28 only gets output right before a toolchange, so it appears the post is using it as a toolchange position. So perhaps G28.1 X-100 Y-200 Z-5 would be better. (or Front Center on your machine).
If you MDI the G28.1 once, then machine controller should remember it. So any subsequent call to G28 should go to the same position.

No idea about solidworks or the post. If you are using Carbide Motion, it inserts it’s own toolchange position with an M6 command, so the G28 is really unnecessary. If you can configure it to leave the G28 out, it should still be safe.

You mentioned “After the toolchange & spindle on”. The code moves the tool over the first engage point at Z1.0 (1" above the start point).

N5 G20 (Inch)
N10 G90 (Absolute)
N15 G91 G28 X0 Y0 Z0 (Reference point)
N20 M6 T1 (Toolchange)
N25 M3 S12000 (Spindle)
N30 G90 G0 X.7292 Y1.615 Z1. (Clearance point 1" above part)
N35 Z.1 (Rapid to retract height)
N40 G1 Z-.125 F15. (Feed at 15ipm to start of first cut)

Hey Tod,

Thank you so much for all your time on this issue.
Eliminating G28 didn’t really help, machine still hitting hard Z limit.
Would it be possible that the tool length + the 1" Clearance above part is also causing the issue?
Maybe the combination of the two is just over the limit.
I have also got this error sometimes before starting the job:

Should i try 0.5" clearance instead of 1"?

Thank you

Yes, that message is caused by the retract height being greater than the machine can lift from where the origin is set.

This topic was automatically closed after 30 days. New replies are no longer allowed.