Is there any way to create an angular work offset such that you can measure how “out-of-tram” a part is relative to the machine and correct for it in the toolpath? You’d essentially have a zero for X, Y, Z, and theta (angle about z axis).
If it can’t be done natively, are there any g-codes that would work (either in Motion or a 3rd party sender). If not, any workaround in CAM using Fusion360?
If the machine and part are square and it’s just that the part is rotated around the Z axis then you can be selective about the CAD object vs. CAM zero coordinates in Fusion 360 but this would mean regenerating all your toolpaths each time. I’ve found it quicker and easier to stick a dial indicator in the collet and square up the part than faff about with the CAM though.
While not directly an answer to the question, there also is the concept of “autoleveling” that some CNC senders support (e.g. bCNC) and that is usually utilized when milling PCB tracks, when the job is extremely sensitive to any subtle variation in Z height.
There is always some kind of contact probe involved, with the machine scanning the height across multiple points of the work area, computing a height map, and THEN auto-modifying the gcode of a job on the fly to compensate for the machine/stock non-perfect geometry.
This can also be used for milling/engraving non-flat objects.
Coming back to your point: such a (complex) system could be used to map out how much the machine is out of tram, and automatically compensate at gcode execution time. Honestly, it’s much much simpler to just tram your machine, but this can be a geeky solution as an alternative to handling this in CAM.
This would typically be done with G68/69 - coordinate system rotation. GRBL does not support these G codes, so you’d need a fancier controller which probably isn’t worth the expense/effort. For regular stock a squaring pass on a fence or L-bracket may provide adequate registration surface. For work in process you can mill a fixture in place to ensure the workpiece is aligned. Otherwise I would follow the advise of @LiamN and tap it in.
One work around could be a software feature that calculates the work piece angle for us prior to posting the NC code. This would allow us to rotate the tool path in Carbide Create to the same angle of rotation of our work piece. When finding X, Y and Z zero with or without the BitZero, we would be prompted to probe or center over a second X and Y location. When we hit measure, it would calculate the angle between the two points. (simple trig for a computer) Now we do a simple rotate about our Tool Path Zero and post. Ctrl Z after posting so we are back to our original orientation.
“Tap it in” for most inexperienced people can be very frustrating. I have taught many machinist over the years on how to tram a head or indicate a vise and it takes time and patience for both teacher and student. (indicating center is always fun too) G68 is the cleanest solution but we need to work with what we have.
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.