NX CAM motion output 1

[Proizvodnja]

HI!I was trying to program radius milling on 3 axis (Fixed Contour Operation -surface area option) tool path parallel to the Z axis.The problem is:

1.Tool path is going under desired radius, even though there is no stock left there (Done in previous operation.How can I trim in vertical axis how much tool path can go?
2.When I generate tool path over the radius, it's linear and not circular despite the fact it set on arc motion output.SO instead one arc motion it it's 10 or more linear.Why is that?This has nothing to do with the post processor since it showing this in simulation.

I'm using nx10.

Thank you

 

[John_Vincent]

I would recommend Z-Level profile for this operation. I created two sample paths, one with Z-level profile and the other with contour area.

 

[Proizvodnja]

Thank you JV.
I was wondering how to do this with end mill?Can you help me on that?

 

[John_Vincent]

Same operations, just choose a bull nose end mill. See attached file.

 

[Proizvodnja]

This is how I did,but the problem is that radius is linearized on verification ,there is no single arc motion.

 

[John_Vincent]

The toolpath is not in a principle plane (i.e. G17, G18, G19 ) for portions of the cut so linear moves are expected.

Change your Motion Output Type to Arc Prep/Par to Tool and check you CLS file. You will see some CIRCLE records but not for all paths. Your post will have to bet configured to output arcs in G18 and G19 planes to support this. I don't think any OOTB posts are set this way.

 

[Proizvodnja]

Thank you JV.Motion Output Type to Arc Prep/Par to Tool solved.