QTPlasmaC with fourth axis - rotary

How about this. It was written for LinuxCNC without QTPlasmaC.

Because the circle is wrapped around 3 faces it is broken into lots of short line segments. If it was on one face it would be output as an arc. Before anyone asks, the feed rates are correct. To maintain the correct surface speed the machine needs to move very fast when cutting around corners.

Thanks for that, I have got a bit done on it today. I could possibly push a preliminary test branch tomorrow sometime.

Torch On, Arc OK, and Pierce Delay are still controlled by plasmac.
THC is disabled.
Height Override is still available during the cut.

I also made some changes to the G-code parser so it was happy with not using the material parameters for the feed rate. The only material parameter used is Pierce Delay.

Changes to the G-code were:
add the magic comment #<keep-z-motion>=1
change all M03 to M03 $3 S1
change all M05 to M05 $3
remove all G04 P0.5

A couple of things I am unsure about:
This G-code has no probing so I haven't done anything with probing yet.
The G92 offsets on the Z and A axes grow a bit on each run, Z eventually fails due to the increased height. I have never really used G92 offsets so I am not sure of the purpose for it here or whether it should be reset at the end/beginning of each run.

Looking at the code I'm not sure why it is using G28.1. G38.2 straight probe would make more sense. I'll have to check back in my records to see if I can find out what is going on there. Most of my plasma posts use G38 followed by G92 to set the reference height.
As SheetCam is controlling all of the other cutting parameters I think it would make sense for it to control the pierce delay as well.
Is plasma on/off always spindle 3? Does PlasmaC use any other spindle outputs?
If the machine is fast enough around the corners it should be possible to keep THC on.

It currently uses the following spindles:
0 = Torch - normal cut
1 = Scribe
2 = Torch - spotting

I am intending to use 3 for Torch - tube cut

As SheetCam is controlling all of the other cutting parameters I think it would make sense for it to control the pierce delay as well.

I wasn't sure which way to go here, by getting plasmac to do it then it is able to ensure the arc is valid before proceeding rather than just relying on a G-code delay. This also allows multiple arc start attempts depending on the arc fail parameters.
 

What difference is there between normal cut and tube cut?

I agree PlasmaC should wait for the arc OK signal and retry if needed. Those are settings you would not normally need to change in the tool table.

I was referring to the pause after the arc has established. This varies with material thickness so is in the tool table. As SheetCam has it's own tool table and manages all of the rest of the cutting parameters it makes sense that it controls pierce delay as well. If I remember correctly there is a way to create a temporary table entry from g-code. I could use that to set the pierce delay.

Does scribe automatically apply an X,Y,Z offset for the scribe head?

The different spindles are so the plasmac component knows what type of job to perform. So for a tube cut the component won't do any probing nor move to pierce height, puddle jump height or pierce cut height.

Using a scribe requires a M6 tool change and a G43 as well as the spindle number difference.
linuxcnc.org/docs/devel/html/plasma/qtpl...c.html#plasma:scribe


 

Les, I've attached a very old pre-plasmac touch_off routine if it helps. There is a bit of Dewey Garret's work in there.
It uses g38.2 straight probe then g38.5 to probe away to give a more accurate material height. QTplasmac does the same thing.
Your existing Sheetcam plasmac post should support the magic comments subject to a variable set at the top..

snowgoer540 You are correct for normal flat cutting. However QTPlasmaC is not set up for 4-axis tube cutting. By using the magic comment #<keep-z-motion>=1, SheetCam bypasses a lot of the built in functionality which would interfere with tube cutting. As it takes over feed rate, pierce height, cut height etc there isn't much left in the material table that can be used.

Is there any way to just call PlasmaC's touch-off routine without firing the torch?