Post Processor for LinuxCNC and PlasmaC
One issue I can see is that SheetCam outputs compensated code. It does not currently support G41/G42. The main reason for this is because some of the things it does are hard to make work correctly with compensation. For instance wiggle piercing can't work with G41/G42.
motion has a pin motion.motion−type which tells you what the g code is doing at any time. One of the states is set when you are cutting an arc. This definitely works. There is a thread here somewhere where Andy helped me come up with a couple of algorithims which in theory should have allowed you to calculate the arc radius. But I did not have any wins. so I don't know why. My maths?? My coding?? the algorithims???
This is where I think state tags in conjunction with a plasmatask module might be able to help.
Sheetcam has an onArc() method where you can determine the arc length and generate code to suit. Perhaps Fusion has something similar.
Attached are the file and instructions (sort of). The .py file needs to be executable.
You enable it in the ini file and you can also select between holes or all arcs.
It works for absolute mode, G91 will not work yet.
Eventually it will be in PlasmaC because I am selfish and that is what I intend to use as I will be using dxf2gcode which doesn't have any plasma related stuff.
Edit: When it does make it into PlasmaC I imagine that the options will be available on the GUI somewhere
This may not be pretty under the hood but it is working. If you want to spot holes create and use a special tool called centerpunch with a drill operation and you will see the tools change while running
File Attachment:File Name: SpaceShipP...post.txt
File Size:23 KB
Is this "rev 6" still the latest plasmac/sheetcam post processor?
Follow up questions:
1. Does plasmac or sheetcam handle kerf offset?
2. Plasmac overrides sheetcam's feedrates, right?
3. Center spotting: I do see there is example code in the user guide. But what's the best way to implement this from sheetcam? (video series linked below covers it but he's not using plasmac)
I know it's asking a lot but a plasmac specific sheetcam user guide would be super helpful for us newbies. I've found a series of video tutorials for sheetcam by Arclight Dynamics that was very helpful on learning the basics of sheetcam, but I don't know what applies or doesn't apply to PlasmaC.
Just create your cut chart as a Sheetcam toolset, export it and import it into Plasmac via the materialverter if thats what Phill still calls it.
And tell Sheetcam to make .ngc files in the settings
1. Sheetcam creates code compensated for the kerf width. Plasmac/Linuxcnc can use a tool offset for kerf compensation (tool width) but that is not required with Sheetcam. I think the POST for fusion360 does it this way and its discussed in the manual
2. The postprocesser here just uses the tool number in sheetcam and retrieves the Plasmac tool number and then reads and sets the Plasmac feedrate.
3. Create a tool called centerpunch and export to Plasmac with the others.. Copy holes to a new layer and create a drilling operation using the centerpunch tool. Set the dimensions for the holes in the operation window to make sure the holes you are drilling are in the min and max range. Make this the first operation in the list.
The arclight demos are very good but ignore all the stuff about code snippets and the like. These are not required with plasamc becasue it has the antidive/corner lock feature and a Hole mode too I think now. There is not really anything special about using Linuxcnc with sheetcam as the post processor handles all the Linuxcnc/Plasmac specific stuff without you needing to worry about it.
I did get Les Newell the Sheetcam developer to agree to write a post for Plasmac quite a while ago but it was so actively under development it was too premature. Now things have stablised in the feature set, perhaps its time to do that. That way, the POST would be distributed with sheetcam.I have not added code for the pneumatic marker which Stephan has pioneered or the Hypertherm RS485 control he is working on with Phill. Perhaps we should do it after that is in the production system.
the cool bit is Sheetcam runs on Linux and Windows but I run it from my Linuxcnc box.
Don't be afraid to edit the POST. Its pretty easy really. Its just a programming language called Lua, a number of methods that are called at specific times and (eg onPenDown) where the controller specific code goes. This code simply outputs text commands to the GCODE file.
This project is not really the right place to ask about sheetcam as its a commercial app in its own right. They run their own forum and also the plasmaspider forum has a wealth of info.
Will it be possible to have a flowchart combining all the different "modules/software/processor" needed to have a CNC plasma running, starting with the DXF file and having as output the end process (the cutting of the part ?
It might sound stupid but when starting from scratch there are some things that are not easy to figure out