possible bug-drill cycle and cutter comp in the same program

[dhanger]

UCCNC 1.2113 Windows 10

I seem to have found a rare bug that has only bitten me a few times in several hundred program runs in UCCNC. Until today I haven't been able to find what triggers it so I haven't bothered to inquire about it but now I have something to report on it. Attached are my profile and three copies of the same program with minor edits between them.

The program has 4 tool changes with 2 drill cycles and a profile cut using cutter comp. In the original program (BOTTOM FINISH) it starts with the profile cut with cutter comp., then on the G53 Z0 block it rapids up to the Z home position and then changes to T4 (spot drill). There is also another drill cycle with a second drill right after that. Randomly one or the other drill cycle, upon running the G53 Z0 block, the Z axis goes all the way to the limit switch instead of stopping at the home position as it normally would. After re-homing Z the program will continue as normal. In the past this has only happened on drill cycles.

I tried various small edits to try to debug. In BOTTOM FINISH (2) I tried moving the first drill cycle to the start of the program and left the second drill cycle later after the profile tool with cutter comp, thinking maybe the 2 drill cycles in consecutive order was triggering it. This produced near disastrous results--at the end of the spot drill cycle, instead of going up to Z home, the tool proceeded to plunge down into the part! Fortunately after the axis motor faulted out I was only left with a broken spot drill and minimal damage to the part. Obviously that was not the solution.

I was about to give up and post a bug report anyway when I got inspired to try one more thing this morning. In BOTTOM FINISH (3) I removed all references to cutter comp. (G40, G41, G42) and at last the problem went away!

Check it out and let me know what you think.

Thanks,
Dan

[cncdrive]

Dezsoe, please test this. Thank you.

[dezsoe]

The problem exists:

[cncdrive]

OK, the bug was found and fixed, now in testing...
The issue was that there were cutter radius compensation in the g-code and the G43H.. did not apply the tool height in time, because there is a lookahead for the cutter compensation and then the G53 movement caused the issue, because it still read the old tool height. The issue did not exist with any other codes then the G53 and the bug was fixed now.

[dhanger]

Okay, thanks guys. Nice to know I'm not losing it, LOL. So for the time being my best idea for a workaround is to just simply not use cutter comp. and drill cycles in the same program, unless you have a better suggestion?

Dan

[cncdrive]

No, not the cutter comp and drilling cycle is fine.
The G53 movement in machine coords is the issue together with the cutter comp, but only when a G43 H.. tool length offset is changed prior to the G53, so it is kind of a special case. Probably this is why nobody else encountered it yet, you were the first however this bug was always there.