The reason I use G53 in the post-processor is to lift the spindle in machine coordinates : whatever your work-coordinates settings, the spindle will go up to the maximum z-axis.
If after homing you are at 0,0,0 (with the spindle up), then G53 G0 Z0 will lift the spindle to this home z -position.
Typically GRBL stays a few mm away from machine 0,0,0 in order to not cause false limit switch triggers.
So if your machine home is 0,0,0, and you stay 10mm safe, then your safe home position is -10,-10,-10
@Strooom I don’t think @KikoLobo is using your post processor. Wouldn’t he raise Z and THEN move XY if that was the case? The error he did a screen capture of is not due to the G54, although it appears that way. He probably has an M6 on the preceding line which throws that error in cncjs.
So yes, I am using @Strooom pre-processor in Fusion360. I think my mistake is using the easel pre-processor and not the OpenbuildsGRBL one… In the repository it comes with two files. I am using: f360-easel.cps … Will try OpenBuildsGRBL.cps instead.
Here is the first section in the .nc file. As can see in the screenshot there’s both G54 and M8T1 near line 9 [where the controller reports the error]. If the error comes from M8T1, then the error is not the causing issue of the movement beyond the end stop in the Z Axis.
I am switching to OpenBuildsGRBL Pre-Processor. Will let you know if issue persists.
No problem. Again, use default grbl post, and share your Fusion file if you have more questions. With just over 7mm of clearance over your stock, you’ll need to pay close attention to your CAM settings.
No, G28.1 creates a G28 position which could be used for any number of reasons. A WCS zero is set with a G92 (temporary) or G10L20 (persistent). Without homing switches, it all needs to be reset every power cycle.
Not true, if my spindle is at Z-20 a move to Z-15 is a move up.
Without homing switches, your machine position is arbitrary. Don’t use it in commands.
G0 Z-10 is a standalone command that could have different results.
If the motion mode is absolute:
If there is a G53 preceding it, on the same line, it is a move to MACHINE Z-10. (could be up)
Otherwise it is a move to WCS Z-10. (could be up)
If the motion mode is incremental:
It will move the Z down 10 from where it is.