April 13, 2019 at 11:11 pm #96960
So far I’ve been working by homing my machine, then moving to the point on the stock where I want to mill and resetting the coordinates to zero. Works great, but the problem is, this loses me the actual table coordinates so I can’t move to a safe spot on the table automatically after it’s done. I just know one of these days I’ll get busy reading a book or something and the 20 minute timeout will disengage the steppers and send the spinning bit right into my work.
Is there some way to use WCS coordinates to preserve my original coordinates without having to zero everything where I want to mill? It looked like maybe someone tried adding support for this into the marlin firmware but I can’t figure out how to use it.
GregApril 14, 2019 at 12:22 am #96964
Just recently the G53 – G59 have been repaired in Marlin. Recently, like three days ago: https://github.com/MarlinFirmware/Marlin/pull/13654
You can wait for it to make it into Ryan’s version, or you can try to patch the code yourself and re-flash the firmware.
Once these commands are available, you can allocate one coordinate system for machine coordinates and another for your workpiece. This would mean:
- Home your machine
- Invoke G54 to switch to machine coordinates
- Perform G92 to set the home position to 0,0 in machine coordinates
- Jog to your workpiece origin
- Start your g-code after adding these to your start/end g-code:
- Perform G55 to switch to workpiece coordinates
- Perform G92 to set your current position to 0,0 in workpiece coordinates
- Run your CAM commands (runs in workpiece coordinates)
- After finishing, perform G54 to switch back to machine coordinates
- Move to your safe machine location in a safe way, e.g. G1 Z100 (or whatever your maximum height) followed by G1 X0 Y0
If you have trouble patching the firmware, let me know and we can work through it or pester Ryan to pull from upstream.April 14, 2019 at 5:52 am #96970
That’s great. That is the thing I miss most from grbl.April 14, 2019 at 9:07 am #96977
Great stuff! I have my own fork of the firmware for dual endstops on the Rambo mini that I updated from latest marlin a few weeks ago but I couldn’t figure out why WCS wasn’t working. I’ll update again and give it another shot.April 14, 2019 at 9:13 am #96978
Oh wow that got pulled so fast! I really need to update the firmware ASAP. Thanks againApril 14, 2019 at 4:06 pm #96999
FYI I updated to the latest marlin. Good news is that WCS works perfectly just like Jamie describes. Bad news is my cut that used to take 10 minutes now takes 30 minutes because it’s going extremely slowly around the curves. I noticed some pulls related to arcs so I don’t know if it’s related or I’m just doing something dumb. Before the simulated time in fusion matched the actual cut pretty closely but not anymore.
I’ll probably revert my changes and just include the one pull related to WCS.
You must be logged in to reply to this topic.