No matter how many times I reference the machine and zero the tool height on the workpiece when I run the program the X and Y move to the correct location but the spindle rises up then back down and begins its programmed depth moves but the tool is just over 2 inches above the work.
What is going on? It references correctly, stops at all the right places but only wants to cut air. Any suggestions?
What does the code you are running look like? There is only a handful of options, G54 is set wrong, Tool length is set wrong, or the programmed depth is off in the program.
Are you sure you have the right tool and tool offset selected? Beyond what @SamBollen mentioned, I’ve seen it quite a bit where the height offset number in the program doesn’t match the selected tool.
So for instance your tool change line should look like this (for tool 5):
M06 T5 G43 H5
but instead has a different number after the H, for instance:
M06 T5 G43 T1
Another possibility is the tool you have selected when zeroing to the material is not the tool that the program is looking for.
Is this a hand-written program? I once inadvertently put a Z location in a hand-written program before the G43 or the G54 commands, so the spindle acted like it was in G91 (incremental) and went up 1 inch instead of moving to 1 inch above my part. In my situation, on a different machine and control, it went on and did everything else just fine. Ive not made this same mistake with ParhPilot (yet), so i dont know how it would respond. Best of luck!
That is exactly what caused the problem. I was using a 1/8 2 flute flat tool as tool 2, for some reason Pathpilot kept calling for tool 11 which was automatically listed as a Tormach tool but in my tool list tool 11 is a drill. When I reviewed the code I would manually change T11 to T2 but apparently it would not “stick”. The only problem remaining is every hole I produce with a boring operation ends up .035 larger than drawn.
Many thanks to those who responded! I am new at this and between Fusion and general ignorance of CNC machining it makes for hours and hours of total frustration … especially Fusion which appears to make the simplest of things severely over complicated.
If the holes are bigger than drawn there’s a couple possible issues. Wrong tool number is a possibility here as well though given the offset I wouldn’t expect that to be the real problem. More likely your diameter offset for the selected tool is incorrect by .035 in pathpilot or the tool definition in fusion is wrong, again by that amount.
I bungled this a few times when I first got started so I want to double check that when you are manually changing the tool number in the gcode are you also changing the height offset being called?
In Ian’s example from above, if you only change the T1 value and not the H1 in that line then you will tell pathpilot that you want to use the tool 2 but use the height offset (length) of tool 1. When you manually change a tool number in a program you have to change both values.
M06 T11 G43 H2 = use tool 11 with the length of tool 2
M06 T11 G43 H11 = use tool 11 with the length of tool 11
Ah so! Thank you very much, I had no idea of that factor.
Thanks, I will look at that. It is definitely a CAM thing since I test those parts by 3d printing before committing to metal and the dimensions were perfect.
You nailed it! I measured what was supposed to be a .125 tool and found it to be .155!
Thank you for your input, silly me trusting the label on the package.