Post Processor for LinuxCNC and PlasmaC

I looked in sheetcam and I have that f3.nnn called out as plunge speed . And above it I have 100in/sec cut speed. So that is why it was plunging so slow and arcing out. I kinda worked around the problem of diving down while cutting holes. My temp solution was to set THC delay just long enough for it to complete the hole befor it turns it on.

In that case you can edit the post processor to output a more reasonable feed speed.

JTknives

You really need to fix your material/tool files. No PP that is made to work with Plasmac will work unless you do. Your band aid is a poor work around at best. To realize the full potential of the Plasmac branch you must fix this. Sorry you are trying to use an experimental branch with advanced features that aren't well documented yet, it is a very steep hill to climb.

You need to edit your imperial_plasmac_material.cfg file for all the materials (tools) you use and have a corresponding tool number in your Sheetcam tool list. The example for editing your material file is in the file. Make a material entry for each material and cutting condition you will need. So for me I have a 14ga HRstl Finecut, 14ga HRstl Finecut openlines and 14ga HRstl holes. All for cutting 14ga HR steel at 45A with Finecut consumables. I have many others for different materials that I build when I need them. Build your files one set of cutting parameters at a time as you need them, it is much easier that way.

I have a new PP that appears to work from code inspection that will not put in extra feed rate commands either for plunging or cutting. I may get to to test actual cutting tomorrow. I spent the day chasing a SheetCam "feature" that inserts an extra do nothing G0 block in the code when you change tools. It must be hard coded some where in the tool change code because it is totally nonmodal and doesn't have any effect on the modality of the following code. I traced this back for the last couple of years after a few more gray hairs and there aren't many left. I couldn't get the parking from SheetCam to work with the features I want so the parking position must be set in your copy of the PP (or you can comment out my code and use the SheetCam parking position).

John

Is it possible to turn on and off the THC from Gcode with Plasmac?

If not why not? It really comes in handy to be able to use the Sheetcam rules to turn off the THC before the end of a cut, Also as the others mentioned on holes having two tools. it would be easier to just have one tool rather than having multiple tools, As Tom and Rod pointed out in another thread, There is lots of reasons to have multiple tools. Like different amps, shields, nozzles,gases, cutting speeds etc, If we need to have another set of tools for THC enable and THC disabled it is going to be a nightmare to get set up.

I had an idea but I can't see it would work now I looked at the plasmac config as the pin I want to use is in use.

Phill, some questions:

1. could you confirm the motion.adaptive feed pin is used by reverse run?
2. Is reverse run only in use when the program is paused? eg. halui.program.is-paused is true?

What I had in mind was to reduce the feedrate using a sheetcam code snippet using adaptive feed and use a motion.analog-out.nn pin to set the adaptive feed pin from gcode using m67/m68. Plasmac's corner lock would halt the THC action when the speed was reduced.

This might be able to be done if a mux component could select between the plasmac pin and the analog pin based on the machine state (eg is paused).

This would allow some cutting rules to be set for holes in the sheetcam post processor.

But in the mean time, I might look at seeing if I can add a flag in the post processor that determines if the plasmac or sheetcam feed rate is used.

But the plasmac way would be to create a second materials set that has the thc disabled as Islander261 does. Then its just a matter of moving your holes to a different layer using the different tool.

Incidentally, this highlights the importance of the Linuxcnc state tags branch for plasma operations. The real problem is that Linuxcnc is never told what the commanded feedrate is. If state tags were implemented, plasmac would be able to know what the commanded feed rate is and it could be set in Sheetcam with no problems.

JTK's issue also highlights the need for the ability to enable and disable the THC from gcode. This would avoid using 2 plasmac tools and also avoid the need for layers as sheetcam code snippets could control settings for holes. An additional external THC hold pin would be very nice.

'03

Yes you can. I did it before the material change from Sheetcam feature became available. You will need to have a post GUI hal file and break the link from the GUI to the Plasmac component and put an OR component in there. Your Plasmac material in the GUI will always have the THC disabled. You will then control the THC with a bit setting/clearing M code. Sorry the examples I have are so out of date they are useless now. I am not sure about THC or ARC early off. THC is easy as corner hold will freeze the cut height. I think the M codes may cause the blending to break. Usually for lasers there are special M codes that allow early off for the beam but they aren't implemented in the standard LinuxCNC releases.

You are quickly heading into decisions made to keep plasmac self contained and not dependent on any specific PP or CAM program. I didn't make those decisions so I just rolled with the punches and am still thrilled with the result.

John