c-axis milling on face of part

[mmclafferty]

My company has recently purchased a vertical turn/mill with live tooling. The control is a Fanuc 18i-TB. I have MasterCAM version 9.1. When I create toolpath to mill on the face of the part it looks fine on my screen, but nothing seems to work the same at the machine. Has anyone ever successfully used G12.1 and if so what it the secret to it?

[tryon]

THis works on our Hardinge Quest with a Fanuc 16i control. We use G112 instead of G12.1, Maybe your using a different G code group?

 

 

code:

---

N200(C-AXIS FACE CONTOUR)

M98P1

T1010

M23

X2.55Y0.Z.1C0.

M54S2139P3

Z0.

G1G98Z-.5F40.

G112

G1G41X2.25C0.F10.

C-1.125

X-2.25

C1.125

X2.25

C0.

G40U1.

G113

G0Z.1

M98P2

 

---

[Post dept]

I use G12.1 all the time. The big secret....start at C0. So, if you're looking at your part from the right side view, start your lead-in from the positive X axis side. Don't put an arc on your lead-in/out just run a straight line in to the part. if you require an arc, add a perpedicular line before it that is the same langth as the arc rad so again....you'll be starting at C0.

 

If using mplfan, just select the misc int to set G12.1 and away you go.

 

Put your code up here if you like so we can verify.

 

Also note that your cutter comp (rad) must not be active when calling or cancelling G12.1.

[mold100]

Over meh head, but welcome teh best support forum round deh world.

[Harryman]

What's the machine?

[tryon]

Ok how do you get around not being able to start at C0? what if i have two different contours and only one can be started at C0?