I was thinking about doing something similar, but not using any special CAM for cylindrical work pieces. I figured out that the Y height of whatever I was cutting would be limited to the number of steps it takes to go 360 degrees. Then, from there I just had to divide the number of steps to go 360 degrees by the number of steps per millimeter, and the will always be the height of the canvas in whatever CAM program I use, because no matter the diameter of the work piece, there are still only 360 degrees in a circle.
Since your Y dimension is fixed, you will have to lay whatever you want to cut properly, then stretch it to make it 320mm or 360mmm or whatever the value ends up being when you divide the 6,400 by your chosen $101 value.
These examples are for engraving so that the lettering can be read when the cylinder is sitting on the round end, like this (shamelessly stolen from image search):
If you want to engrave so that the letters can be read like this (not the emboss part, just the text orientation):
@Crispy Chris, the gcode describes exactly what you are seeing on the machine, so the ‘sender’ and machine end of things do appear to be working correctly, and your steps calibration etc OK.
The tool path itself is a LUA Widget (a ‘macro’ in other terms) running inside Aspire. It will ask the Job for the stock size, reference point etc and create the clever tool path for you. I will presume it is capable of coping with being told the square stock is larger than the Aspire Job stock diameter set - it would make sense that it can, and it does output a tool path - the preview shows it is good (as far as Aspire interpreting the tool path is concerned).
The post-processor clearly assumes that Y is the rotary axis, which is correct, but one thing I noticed is that the PP title is ‘Shapeoko (mm)…’ and your Job is in inches… One thing to try would be to select @neilferreri ‘Shapeoko (in)…’ post processor and see if there is some metric/inch translation issue. Perhaps Neil can advise more knowledgeably on this point.
@neilferreri I can do this. Will quickly find a simple rotary job and run it through the PP.
Done. File .nc attached. No issues in VCarve Pro 11.504 seen.
I can see Y numbers ranging from 0 to 359deg. I dropped my own header and footer preferences in, but they don’t affect what is being tried here. I have also attached the VCarve file used, just in case it is useful (a test project to see if I could cut a square onto a round stock and it be accurate, the opposite of what the OP was doing, but the principle is the same).
Got a few mins to experiment, read the LUA code etc and track down cause/effect for this 1355.62 pre-rotation. In my VCarve file, Material Setup dialog, Home/Start Position for X and Y had non-zero numbers entered. No idea where they came from, or whether the Widget sets them.
Setting X and Y to zero stops the pre-rotation. It seems like the VCarve tool path evaluation code that outputs to the post-processor is affected by this negatively…
If I get another few mins, I will try creating a new file and checking these settings before and after running the Widget to see when/if they get set, or whether they are some non-volatile carry-over from the last time I used VCarve.
[Edit - a new file has these X and Y setups at zero, so it looks like a carry-over from some earlier use of VCarve]