Sheetcam and trying to generate spotting gcode.

Have you tried the magic comment that creates a new tool in the materials file rather than a temporary one?

I haven't looked at that stuff for a long time.

EDIT:
I do have an idea for multiple temporary tools that I will look at down the track, although I am not sure they will be required.
I would imagine that if you had a tool in your CAM then you would want it in the materials file.

After fixing my .ini file so the correct number of SPINDLES was used, I have spotting working. But. If i create a file with both spotting and cutting, it will fail on the first cut attempt with the torch going down, igniting and then going up again, over and over. If I separate the two, then it works fine. I'm using the latest post file from Phil as well as the latest qtplasma. in the attached file, I seem to get to line 4090 at which point it fails.
;begin material setup

N04010 M190 P23 (45 amp 14ga mild steel material)
N04020 M66 P3 L3 Q2 (wait for valid change)
N04030 F#<_hal[plasmac.cut-feed-rate]>
N04040 ;end material setup
N04050 M5 $0(cut stop)
N04060 ;end operation #30, cutting
N04070 ;
N04080 ;begin operation #31, cutting, 1.34"
N04090 G0 X2.76051 Y3.80271

I'm actually thinking that it fails at the M5 $0 which is wrong I think. that should be M5 $2 (spotting)
The second last spotting op that succeeds has a M5 $2 in it, but the last one has a M5 $0.

They all seem to be cutting operations, not spotting.

You need a tool named "Centre Spot" or "Center Spot" and a drill operation, or try the sheetcam post earlier in this thread.

phillc54 wrote:

They all seem to be cutting operations, not spotting.

You need a tool named "Centre Spot" or "Center Spot" and a drill operation, or try the sheetcam post earlier in this thread.

I do have the Center Spot tool defined. And I'm using the latest post from you dated in 2021. I just uploaded the wrong file


Line 4050 is wrong. It should be M5 $2 not $0 and for whatever reason this causes an issue with my Z axis. Basically it will never go past that line.

I am out at the moment, could you post the job file and I will take a peek when I get back home.

sure.

It won't open for me, I get this error messge "This file version is no lomger supported"

I am using SheetCam v7.1.12

That is really weird. I was using 7.1.11 and after updating to 7.1.12, I was able to load the saved job file. There seem to be some issue's with sheetcam. If I use a drilling op instead of the center spot, I can not have both drilling and cutting in the same file. As for the Center Spot op, The last center spot does not have a M5 before the Material Setup. Therefore the M5 attempts to stop a cutting operation instead of a Center Spot operation and of course this is where linuxcnc fails. It really does not like a M5 $0 attempting to stop a M3 $2.

It loads now

Try this:
The last operation you have, "Drill, DRILLING":
change the tool in that to "Center Spot"
change the "Min" and "Max" hole sizes so it covers all the holes
move that job so it is the first job

disable the "No Offset, DRILLING" operation

looks like that will work. I posted on the sheetcam forum, since I believe that the issue shown above is still a bug. Not completing the operation before changing the setup is just wrong.