I’ve just commissioned a Grblweb instance on a Raspberry Pi 2. It allows me to connect to it and upload the gcode to the pi without having to leave my computer constantly connected to the X-Carve.
http://xyzbots.com/grblweb.html
I’ve only had it running for a few hours and I haven’t cut with it yet but it shows promise as a way to run the system in a headless fashion.
Your circle.gcode file does not specify relative vs absolute coordinates. That’s of grave concern because if you leave your machine in relative mode (G90 vs G91) and run this file, it will shoot off into lala land by about line 10 where it is now 20 inches into the positive Y territory, i.e. the back of your machine. That sounds like what you described. So, the question is where did you create this file?
If this worked differently in UGS vs ChiliPeppr it’s simply a fluke based on what mode your Grbl device was in. I’m guessing after Grbl resets it defaults to absolute mode. BTW, when you jog in ChiliPeppr it swaps to relative mode but then auto-swaps back to absolute mode. However, if you probe it may leave you in relative mode.
All good CAM apps will specify G90 or G91 at the start of the Gcode file. It’s about as fundamental as issuing the units at the start of a Gcode file.
I used aspire to create the circle and generate the gcode. It worked perfectly in UGS but not in chilipeppr. I ran both with the exact same file. The only difference is that I used a z zero touch plate to set my z to zero in chilipeppr.
You just got lucky. It was random whether you were in incremental or absolute mode.
Can you, for the sake of the folks reading this forum, run your Gcode file from ChiliPeppr again but make sure you type G90 into the serial port console first? You’ll see it runs fine. Or perhaps just make line 1 of your Gcode file say G90.
Thanks
I ran the gcode file again without any changes. It worked perfect. The only thing I can think of is that I may not have exited completely out of the touch plate tab if that is possible. Also, I noticed that the touch plate inputs are in MM and I had my jog units set in inches. When running the touch plate scheme it always came up short of going to zero. I changed my jog console area to mm and tried it again and it zero’d perfectly. Then I ran the gcode for the circle and it worked as it should.
Your Gcode file specifies inches on line 3 (as any good gcode file should) so the units don’t matter because the moment you go to send your file it puts Grbl into the correct units mode independent of anything you did prior. Truly, your file not specifying G90 is a real problem and you should be blaming Aspire on that one.
I’ve added explicit G90’s to the header of the Grbl posts for Aspire & VCarve now to correct things if the toolpath is run with the incorrect state - these will be included in the next patch. In the meantime you can modify your installed Grbl_mm/inch.pp files yourselves if you like. Find the following block of text and modify accordingly:
±--------------------------------------------------
begin HEADER
“T1”
“G17”
“G20”/“G21” <- this setting will be according to the file’s units
“G90” <- insert the G90 here
“G0[ZH]”
“G0[XH][YH][S]M3”
I hope this helps.
Cheers,
Edward
I had to also modify the pp file to add the “M5” command at the end to turn off the spindle.
Original file contents:
+---------------------------------------------------
+ Commands output at the end of the file
+---------------------------------------------------
begin FOOTER
"G0 [ZH]"
"G0 [XH] [YH]"
"M30"
I edited this to include M5 as below:
+---------------------------------------------------
+ Commands output at the end of the file
+---------------------------------------------------
begin FOOTER
"G0 [ZH]"
"M5" (I added this line to turn off the spindle)
"G0 [XH] [YH]"
"M30"