I created a 50 star union in Carbide Create and saved the g-code. It's a nc file. When I load the g-code to the open builds control, it shows the preview and simulates but when I click run job, it just sits there. I can jog my machine around no problem, find and set my zeros.
check the gcode for lines, usually comments, that are longer than 80 characters. if they exist, remove them.
Gcode is just short text instructions so you can open the Gcode file in notepad and read it and check for lines that go far off to the right (make sure line wrapping is off)
I think I'm having the same issue. I create a toolpath in Carbide Create and export the .nc file. When I load it into the OB Control software, it shows the toolpath and everything looks good. When I go to run the job, nothing moves. I opened and checked the .nc file, and there are no long comments. I deleted the one short comment, and still the same result. What else could it be?
I may have figured it out. I deleted the M05, M0 ;T301, and M03S18000 commands from the beginning of my gcode. These commands all seems to be for spindle control, which I don't have on my machine. After deleting them, the job runs and I haven't run into any other issues yet. My job is still running, but I think this solves my problems for now.
the 'M0' is the problem, this is a 'pause the job' command. You should be able to turn it off in the Carbide post options. Maybe near the tool options since it appears to be pausing instead of issuing a toolchange command (T301 is commented out by the GRBL does not do toolchange (so no M6 nor Txxx commands) M03 is a valid 'spindle on' command, even if you have no spindle GRBL understands this command. GRBL runs in the BlackBox. S18000 is a valid spindle speed setting discussion here Unnecessary Tool Change grbl postprocessor
when CONTROL encounters an M0 command all motion stops, but is there no indication of the paused status (@Peter Van Der Walt) click 'Pause Job' the || button the button changes to run > click 'run job' the job will continue.
Ya, when this "pause" command comes up mid job, is there any way to pause, change tools, and continue the job in OB Control? I couldn't figure out how to when running a job last night. Ended up just deleting the first half of the gcode so I could start the second half of the job at that point.
Fixed in v1.0.267: When Grbl gets an M0, it goes into "Hold:0" status. Seeing Hold:0, the GUI goes into Pause mode too
