I have a Lead 1515 and generated gcode with fusion 360 with the OpenbuildsFusion360PostGrbl.cps V1.0.31. I can't figure out where is it telling it to raise the z axis all the way to the top. The problem is I don't have a limit switch (it broke and I need to replace it), and once it grinds the gears, the axis settings are shot and I need to recalibrate it) I do enter the setting to automatically raise the z axis 24mm (@ 1 inch) just so it never runs across the surface on accident while starting. 24mm is converted to .9449 inches in the gcode where I marked in bold, not the 10 or so inches it is going. Here is the top part of the instructions generated. I attached the whole file. (Made in : Autodesk CAM Post Processor) (G-Code optimized for default controller) (OpenBuilds CNC : GRBL/BlackBox) (Post-Processor : OpenbuildsFusion360PostGrbl.cps V1.0.31) (Units = inch) (Drawing name : LokiKitchen v10) (Program Name : 2-90vbitengrave) (1 Operation (1 : Engrave5) ( Tool 1: Chamfer Mill 2 Flutes, Diam = 0.6875inch, Len = 0.33inch) ( Spindle : RPM = 18000, set router dial to 3.0) ( Machining time : 6 min 19 sec) G90 G94 G17 G20 (Operation 1 of 1 : Engrave5) G54 (This relies on homing, see Search Results for Query: G53 fusion | OpenBuilds ) G53 G0 Z0.9449 G0 X-6.1289 Y5.028 S18000 M3 G4 P1.8 G0 X-6.1289 Y5.028 Z0.6 F40 G1 Z0.2 Z0 F20 X-5.9962 Y4.9597 Z-0.1067 F40
G53 = machine coordinates It does Z-safe moves in Machine Coordinates (not work coordinates) However, the default value in the Post options are -10mm, yours being a positive number indicates you changed that parameter in the Post option. Mouseover over the options, you'll see the tip tells you to only use negative values. Lastly then, it does need you to HOME before setting zero - so that both machine and work coordinate spaces are set correctly. Fix those switches asap, in the meantime, its painful but you'll have to "fake the home" How to 'Fake the home' And some additional reading to understand Machine Coordinates and why that is negative space: Frequently Asked Questions · gnea/grbl Wiki
I let fusion 360 have it's default of -10mm and the problem went away. One thing I discovered is I don't have a problem with the original gcode if I don't start the carving process where the bit is at the xyz zero point. If I just move it to anywhere else, it starts going up the z but only a couple of inches. Thanks for helping the noob.
Are you homing yet? The Machine Coordinate moves relies on it - so it has to be in place - if not you'll see weird behaviour as Z0 in Machine Coordinates is "anywhere"
