Contour Milling with Right Angle Head

[PBoulanger]

Anybody out there have any tips on programming a simple contour using a right angle head. The contour is a single arc in the YZ plane. The tool axis is parallel to the X-axis. When I set the T/C Plane to the Side view the toolpath looks OK but on posting I get the following error message,

"Only Single-axis rotation is allowed. Angles may be incorrect."

I seem to recall this topic being discussed before but I wasn't able to find anything in the search.

Any and all suggestions are appreciated.

[cadcam]

Are we talking about useing a jhead on a cnc?

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

jay/ aka cadcam

Precision Programming

email: [email protected]

web: www.ppcadcam.com

[ChrisD]

What kind of cutting tool are you using and can you describe the shape you are trying to cut?

[gcode]

If it is a real simple profile, just program

it in the XY plane and change all your x's to Z's.

[Will Slota]

Usually when I encounter "only single axis rotation is allowed its because the positive x and y directions of my tool plane are pointed the wrong way. Try rotating the construction plane about z 90 or 180 degrees

[cadcam]

If you are using a jhead being a 90deg head.

You for say program in a front plan then use edit Nci and flip the nci in tool plan then post and it will swap for say the "Y" & "Z"

for you.

Hope this is coming out right have done this sense version 6 to ver8.

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

jay/ aka cadcam

Precision Programming

email: [email protected]

web: www.ppcadcam.com

[PBoulanger]

Hi Cadcam;

I'm not familiar with the term jhead, but 90deg. head or right angle head are interchangeable.

Hi ChrisD;

Just using a regular flat endmill side cutting on the flutes. The shape is a section of arc drawn in the side Cplane.

Thanks for the suggestions guys but I was hoping for something that didn't require manually editting the NCI or NC files.

We'll probably end up surface milling the feature, just wanted to know if Mastercam could accommodate this kind of tool without too much hazzle.

[Allan Brown]

A variable called 'rotaxtyp' in the post controls internal calculations for the rotary angle. A starting point for angled head applications is to set rotaxtyp to 4, which will map most movements to the top toolplane, using the global XYZ coordinate system on your machine.

[mmonica]

We have programmed right angle heads with mastercam. On the parameter page select T/C plane, tool plane top and construction plane front or side depending on geometry. You can use cutter comp if you choose. Our posts are based on the generic fanuc post. When posted, the code should have a G18 or G19 plane select and K values for the incremental Z. Be careful, some machines do not default to G17 after reset, if restarting the machine, be sure the machine is proper plane or you will be responding to the "big crash" post.

[PBoulanger]

Thanks mmonica. I tried your suggestion and it worked just fine. Of course the orientation of the tool in backplot was wrong but the code generated was bang on. And that's the important thing, right.