Autoleveller

I have just noted that the autoleveller does not handle the Linuxcnc G82 command (Drilling Cycle, Dwell) correctly. This command will retract the tool after the drilling operation to the Z level before the execution of the command.

The following is an extract from the original G-code file:
G00 Z1.0000
G82 X33.0200 Y78.7400 Z-0.2540 F144.00 R1.0000 P1.000000
G00 X33.0200 Y7.6200
G01 Z-0.2540 F144.00

and results in:
G00 Z1.0000
#102=[#522+0.24983*#519-0.24983*#522]
#101=[#523+0.24983*#520-0.24983*#523]
#100=[#102+0.33282*#101-0.33282*#102]
G82 X33.0200 Y78.7400 Z[#100+-0.2540] F144.00 R1.0000 P1.000000
#102=[#522+0.70683*#519-0.70683*#522]
#101=[#523+0.70683*#520-0.70683*#523]
#100=[#102+0.33282*#101-0.33282*#102]
G00 X33.02000 Y73.74000Z[#100+-0.2540] ;segmented line. Max segment length set to 5

which will mill the surface rather than move above it. This is also shown in the attached picture, indicated by the red arrow.

The way I read this is the first part of the command adjusts for the height of the surface (#100) and then it will drill down the 0.2540 depth and then dwell the required time and return to the proper height.

The problem is the G0 move on the last line of the code extract that is done at #100+-0.254:
G00 X33.02000 Y73.74000Z[#100+-0.2540] ;segmented line. Max segment length set to 5

It should be:
G00 X33.02000 Y73.74000Z[#100+1.000] ;segmented line. Max segment length set to 5

since the retract (R) in the G82 line is set to 1.0:
G82 X33.0200 Y78.7400 Z-0.2540 F144.00 R1.0000 P1.000000

Hi yes I think I can see the cause of the problem. Autoleveller does its levelling business on any line that it thinks Z is negative. On the G82 line it drills down to a negative value but actually will pop back up to a positive value at the end, but this line doesnt explicitly state this. Therefore in the next G0 line, Autoleveller still thinks Z is negative and will attempt to level Z, whereas Z is not really negative and should be left alone.

Thanks for pointing this out and I will try to publish a fix for this. In the meantime though, I suppose the easiest workaround is to ensure your drill holes are "deep enough" and not run Autoleveller on this drill file, only on the milling files.

EDIT: So what I mean is that even though the R / retract value is set to 1.000000, Autoleveller ignores the R value and just looks at Z. So when it gets to the next G0 line it thinks Z is still a negative value and Z will need to be levelled and set explicitly, which of course is not the case.

Thanks for your attention to this issue.

Actually it's not a drill file, it's an etch file created with Eagle and the pcb-gcode ulp. There is an option to spot all hole positions with the engraving tool so a tiny drill won't wander off and break when the drill operation is executed.

I think the easy, short term fix, in my case is to omit the spot drilling option and hope for the best when I run the drill file.

Ah yes, I forgot about the spot drilling option. Its been a while since I used eagle to be honest.

Heres another option then, you could insert a quick G0 line immediatly after G82 lines. i.e.

G00 Z1.0000
G82 X33.0200 Y78.7400 Z-0.2540 F144.00 R1.0000 P1.000000
G00 Z1.0000
G00 X33.0200 Y7.6200
G01 Z-0.2540 F144.00

Your tool wont move as it should be at 1.0000 anyway, but it should stop Autoleveller thinking Z is negative and so the following line wont be touched by Autoleveller and you wont mill into the surface.

You could use a text editor to search for all the G82 lines in your original gcode and insert the highlighted line after each one, then run it through Autoleveller as normal. I think that will work. Just an option.