Centroid Community CNC Support Forum

The diameter references in the tool table on the Centroid will not make any difference because your F360 programs do not enable diameter compensation. There are no G41 or G42 call outs in the .nc file you posted.

I'm starting to under stand that fusion does that if in computer is selected? However I would still like to be able to understand how to input the diameter offsets correctly? I'm a bit thick and can't get it to sink in

When roughing in Fusion, you have to define an allowance, e.g. 0.3mm for 8mm Endmill and activate compensation for finishing. Then G41 or G42 is output for finishing and it takes the diameter of the tool in CNC12. G41 to the left of the workpiece, G42 to the right of the workpiece

I'm trying to understand what numbers to put into the machine control CNC12 for tool diameter offsets? Because I feel they are possibly causing issues when not using compensation with fusion/computer

e.g. in fusion T1 Endmill 12mm dia

in cnc12 T1 12.2mm, the part + size

in cnc12 T1 11.8mm, the part - size

only with compensation on.

?I'm sorry i dont understand that,how do you arrive at those numbers. What drives the numbers? Where and how is it worked out? How do we end 0.2mm?

It depends on if you have your CAM system set up for diameter or wear compensation. If diameter compensation, you put in the effective cutting diameter of your endmill; the diameter it appears to cut at taking grinding tolerances, deflection, and wear into consideration. I.e. a 6mm nominal endmill using diameter compensation might have a tool table entry of 5.976 if if was cutting undersize.

If your CAM system was using wear compensation, that same endmill would have a tool table entry of 0.024.

So Tom, the hypothetical numbers you are using would be what would enter into the diameter offset table?

Yes, but you need to turn cutter diameter compensation on in F360. You also need to verify what type of compensation F360 is using. If you use wear compensation in F360, you need to be aware that Intercon uses diameter compensation and you will have to switch back and forth, or have different tool comp indexes for Intercon and CAM. I e. Tool #1 uses D1 set to 5.976 for Intercon and D101 set to 0.024 for CAM.

Thanks Tom, that's helped
cheers