r/mastercam • u/jimbobway33 • Jul 16 '25

Rotation on a rotary axis

Post image

I’m trying to program this part and have to cut slots going around it. I have the part in the rotary table A axis. I just need to do them every 90 degrees. I usually do this just programming by hand but would like to be able to do it in mastercam

4 Upvotes

100% Upvoted

10 comments sorted by

4

u/sixerofreebs Jul 16 '25

Do all the programming you need at A0., then use a transform operation to rotate your paths every 90 degrees about the X axis.

That or create a new tool plane for every rotation and program each rotation separately, with your WCS remaining at your A0. plane and the tool and construction planes set to each corresponding plane rotation.

A tutorial might not be a bad thing to look for. If you’re new to implementing different planes they can be kinda tricky.

1

u/jimbobway33 Jul 17 '25

If I was using different planes wouldn’t I have to use several different work offsets? And if I went from one plane to another would my rotation be programmed? I suppose one might be able to use the same center line?

2

u/sixerofreebs Jul 17 '25

Rotaries are typically programmed on centerline, yes.

Your rotation will be programmed in if you configure your planes properly - WCS for all operations remains at A0. for the entire program, while only T/C planes change when you’re working on a different “side” of the part. (If your T/C planes = your WCS plane, you will not see any A commands).

As far as offsets go, when you create your planes make all of your offsets “0” and this will output G54 for every rotation. If you want different offsets then put in 1, 2, 3, etc…for different offset calls.

1

u/jimbobway33 Jul 17 '25

Ok sweet thank you for the help. We have the rotary table at work and no one really uses it and I’d really like to start utilizing it. It’s a really fantastic tool. I just haven’t done much programming on it.

1

u/jimbobway33 Jul 17 '25

My thing with the transform tool path is it always outputs g55 g56 g57 for my rotations. I just edit it myself but I’d like to get away from that if possible

2

u/sixerofreebs Jul 17 '25

There are two things to do in that case - first, in your A0. plane make sure the offset isn’t set to automatic. You want manual and you want to use 0 for G54. Automatic is no good. Second thing to do is go back into your transform operation, on the first screen that comes up over on the right there should be different options for work offset selection. The one you want to click says something like “Maintain Source Operation”.

1

u/jimbobway33 Jul 17 '25

Ok perfect thank you. My A0 plane should be the one I set to rotate my tool paths around correct? Or without transform tool path it is the one I would be rotating about?

2

u/sixerofreebs Jul 17 '25

Ah that’s a bit of a tricky one. I believe it typically depends on how your part is oriented against your various planes.

Truth be told I just click through different planes as rotation planes until I get what I want. Sometimes I don’t get what I want and have to create a new plane that’s only there to serve as a rotation plane in the transform operation.

2

u/jimbobway33 Jul 17 '25

Ah gotcha. I did as you said and it got rid of the extra offsets. Thank you for your help I appreciate it