When doing Polar Milling with G12.1 your not allowed to use G0 rapid moves. If your doing a deep pocket and stepping down into it Surfcam always rapids out and then relocates to the next plunge position. I always have to manually edit all of these rapid moves to plunge moves. Is there any way of making Surfcam change these rapid out and in moves to be plunges?

You can play with "cutting control", It had been so long but the first parameter under Cut Control. I'm not sure you have to make the number bigger or smaller....

I'm not familiar with the term G12.1 Polar milling. Could someone enlighten me? Why no rapid moves? For general pocketing, newtexas2006 is has it right.

Polar milling is done on a lathe that doesn't have a Y axis using a Z axis live tool to mill on the face of the part. By rotating the C axis and moving the X up and down you can create square, round or any shape. When you are in this mode the control doesn't allow any rapid moves. It may be because the machine can't keep up, you get pretty strange moves sometimes when positioning before plunging. Some machines limit your feed rate to 10 IPM. I believe what newtexas2006 is referring to is the "Maximum Feed Between", by increasing this it will keep the tool in the pocket. But what if your engraving text and the tool has to rapid out and over to the start of the next letter. You have to edit all of these rapids to plunge moves. I think I'm going to do something with my post, maybe a Replace "G0" with "G1 F30." but then I'll be stuck with deleting G1 F30. everywhere that I don't need it.

Ok, I was afraid that may be the case but thanks for the explanation. We don't do any lathe programming here so I can't help you out. The only thing I can think of to try when engraving, would be to program each letter separately and/or set the maximum feed between to zero and gouge check to single.

G12.1 does allow G0, the only thing funny about it is when the tool advance to X0 the feedrate will increase to infinite so the C spindle will rotate pretty fast.

I dont know what kind of machine you got, but none of them I ve seen allows G0 during G12.1..

in 2axis options:
Max Feed Between - enter large number.
Gouge check : full.

If this is not the problem check your post. The G0 can come from there.
....... Or run it with
:) Mastercam (:

Is there any of you that have a EdgeCAM post. that supports "G12.1"?
Don't know if this is exactly what I need, but I am trying to make a lathe make a hex or any other polygon with the toolaxis paralell to the "Z"-axis.
J.

No need for Edge cam. use the G12.1. Ploar cordinate interpolation.

Program the X axis as Diameter and the C-axis in Radius.
Program it just like a mill and it will convert it to C-axis degreess of rotation.

Mill to Lathe
X= X *2 (Radius*2=Diameter)
Y=C

just remember everything is coming from the center of the chuck (Usually).

Hi JimW

It seem your MT post has the problem when you using the Cview5 Milling!
The post should output G12.1 when read the "Row/Start" command and output G13.1 when "Row/End"
(Some machine using G112 and G113)

You should modify your post!
Are you using SPost for this? Please modify in FIL!

Also, in G12.1 / G13.1 could not have the Cycle G8x code within them!