I don't quite know how to say this right... I'd like to be able to tell Grbl where my end mill is. For example: If I'm 5mm above Z0, I'd like to be able to tell it that i'm 5.2mm, so that the next cut goes 0.2mm deeper. Reason: I zero to the work surface & cut parts out of a sheet of acrylic. For some reason (maybe my wasteboard swelled a bit, or maybe because of where I zeroed on the wasteboard) it might not cut quite deep enough & leave a thin layer of material in the cut in places. If I can manually edit the position, I can recut & clean up the material that's on the machine, then be in the right place for the next cut. Hope that made sense. Thanks...
You can use either G10 L2, G10 L20, or G92. I'd recommend Googling all three and seeing which one makes the most sense to your brain and/or workflow.
I can't jog down. Z0 is at my wasteboard & my material is on top of it. G10 L2 or G10 L20 seem like the way to go. I need to play with them at the machine, see what happens & which is best.
Cool just offering more ideas. Internally that uses G10 anyway But if you can't jog down, that cut down is also then a "can't"?
Jog/rezero was my first thought, but if zero is set at the spoilboard (and there's no available location outside of the spoilboard area), jogging down is "impossible". Obviously not 0.2mm with MDF, but it's still technically a crash so not a good habit to form in general. Going into the spoilboard *whilst the spindle is on* is technically not a crash, it's just "using the spoilboard". Learning the real commands makes more sense in this instance and is a better long-term habit for everyone.
I'm not quite sure what you mean by this. I'm usually cutting parts (profiles) out of a flat sheet of acrylic. If I remove the part I could jog to Z0 where the part was, but I'm usually wanting to 'clean up' the cut, so I wouldn't want to remove the part. Or I could jog to Z0 if I lined the end mill up with the cut path but that would suck, plus I still couldn't jog down from zero because I'd be into my wasteboard. My workaround has been to move the spindle off to the side of the wasteboard, but i'm tight on space & only a few mm from my limit switches. BTW - more nice updates to CONTROL! For some reason I'm not getting prompted to update, but I saw it today & grabbed it. NIce.
Next time you create a toolpath, measure the thickness of the material and add 0.05mm. When creating toolpaths, Z zero should be at the top of the material, not at the waste board.
I am a fan of Z zero at the waste board if it is surfaced so it is parallel with the X. You cut completely through your material without damaging the waste board. @brrian -The question I have is did the waste board get surfaced by a surfacing endmill? If not, that may be your main problem and you may not have to guess at depth anymore.
I would echo those comments. Peter is also correct. If brrian's wasteboard is not flat and level (as witnessed by the uneven cut) then he will have no option but to cut into the wasteboard.
I surface my wasteboard. It doesn't stay perfectly flat, I assume because of moisture, humidity or whatever changing the dimension. Right after surfacing I could probably zero just about anywhere & get a consistent cut everywhere, but as days go by it changes. It's not really a big deal... i just check the first cut & adjust, but the process has been a little trickier than what I was used to on my Shapeoko. Once I'm able to do it with code, it'll be easy again.
Winner: G10 L20 P0 Z## So if i'm not cutting through in places, I move to a known height (say, 10mm) then add to that the extra distance I need. If it's 0.2mm, I'd use: G10 L20 P0 Z10.2 The DRO updates correctly to show Z 10.2mm; I cut again & check. If the cut is good, good. If not, repeat. It would be cool if someday a macro would take user input... it could ask me how much to adjust by, I'd enter 0.2mm and it would calculate the value & send the command. But this will do for now. Thanks to all for the help...
This seems to be broken in 1.0.238. See below. If for example I'm at Z10mm, & send G10 L20 P0 Z10.25, the DRO updates to 260.35mm, not 10.25mm. Screenshots below. It's changing it in inches. if you flip to the inch-mode tab, you'll see 10.25 inches. Before: After:
Not a version related thing... You probably had a G20 earlier (from a job for example) that put Grbl in inch mode, so any commands you send after that is in inches. If you are sending manual commands (or creating macros), always preface a G20/G21 to ensure its in the correct mode you expect/depend on Actually any modals you depend on, never assume, set explicitly G17/18/19, G20/21, G53/54-59.1, G90/91, Spindle on/off etc From gnea/grbl Note: the UI mm/inch tabs just affects UI, not Grbl's modes Our goal is to interfere with Grbl as little as possible. Send it commands, tell you what it replies, minimum interference
