using tool comp on 5axis

[JCarlucci1]

I am running 5axis curves (thru holes with tight dimensions) that need tool comp. I keep getting an alarm 2062 TCPC or DWO, incompatible code. The machine this on is a UMC1000. 

How can I , OR can I use tool comp. 

[JParis]

Unless Haas is doing something new, cutter comp on 5 axis paths is no bueno

 

[JCarlucci1]

I didn't think so, It was just a shot in the dark. Thanks anyway. Oh and I saw your avatar over there....

[nickbe10]

1 hour ago, JCarlucci1 said:

How can I , OR can I use tool comp.

You need to manipulate from within the Operation (Stock or Cutter definition).

For most material / tolerance combinations this is sufficient....note I said most....

[JCarlucci1]

That's what I've been doing. It's a hassle to do it that way 

[Colin Gilchrist]

There is no "real 5-Axis cutter compensation" available on the Haas Control.

Your best bet would be to re-program the same feature, but use G268 instead of G234. This would allow you to still program using a single "work offset location" for setting your initial zero point, but the "feature" location and rotation are controlled by the G268, which references both your Work Offset location, and your MRZP (Setting 300-305 values).

By using G268, you are "rotating the G17 plane", from the Work Offset View (G54, G55, Etc.), onto the new rotated work plane.

This would allow you to use Cutter Compensation and regular TLO (G43) with your program.

------------

Another option is similar to G268, but is Dynamic Work Offset (G254). This codes allows you to program a "tool plane" in Mastercam, but only have to set a single Work Offset (like G54) in the control. The control takes care of the math to move the offset value to the zero point, as the B/C values change.

Using a Tool Plane, with a work offset, means you could then program standard Cutter Comp, and not be in TCPC mode.

-------------

If that just won't work, and you're stuck on using G234 to cut this feature, then your only real option to control feature size, is to setup multiple paths inside Mastercam.

I typically will create 6-10 "finish" Operations, where each OP is only removing 0.001-0.002 of material for finishing. This allows me to cut the feature slightly undersized, and then run a particular subroutine for finishing. If that doesn't get close enough, I can then keep running the "next finish sub", in sequential order, until I've hit the tolerance I'm seeking.