I have a part, ( for training ), that I want to tool-path on top. I need to fill hole's , which I have done , (except for the half-holes on the end's, which I haven't figured out yet how to cover those), by using bounding plane, & covered them. My question is , the part is a solid body, & the holes are covered with a sheet body, will my tool-path ignore the covered hole's, or do I need to go another route ? Also one more question, I would like to create surface's of the entire solid model at once. Maybe window it & create surface's , so I can put my curve's on one layer, solid on another, & my surface's on a third. I like to keep them seperate for tool-pathing. Thank's in advance.

Harold C.

Harold,

Are you working in an assembly or putting the tool paths in the same file as the model?

In NX5 If your in an assembly WAVE Link the solid and use delete face to remove the un-wanted holes.

If your working the the same file use extract and extract a copy of the solid body and use delete face as above.

This will fill in the holes so you can select the faces you want to machine.
Basicly you are modifying the model to what it will look like before the holes are put in.

You can then use the original solid when you want to drill the holes.

e-mail or call me me if you have questions

Thank's for the tip, John. I used cavity mill & that option did ignore the drilled holes, but I did learn some thing's about the option you mentioned, Extract. We don't use an assembly, we put the tool paths in the same file as the model . I am in the drilling segment of myigetit & like being able to select holes & putting into set's but from what I have read & tried NX does not output a G83 cycle, it will a G81, but I like to use a Q value. Any work around ?

Regard's ,
Harold C.

Thank's for the tip, John. I used cavity mill & that option did ignore the drilled holes, but I did learn some thing's about the option you mentioned, Extract. We don't use an assembly, we put the tool paths in the same file as the model . I am in the drilling segment of myigetit & like being able to select holes & putting into set's but from what I have read & tried NX does not output a G83 cycle, it will a G81, but I like to use a Q value. Any work around ?

Regard's ,
Harold C.

Set the cycle to Standard Drill Deep and on the step values enter the Q value you want on the first step parameter. This works for me when I use the default MILL_3_AXIS post
I get

G83 X.2281 Z.7369 R1.863 F9.8 Q.0197

Thank's John. It work's for me with the default MILL_3_AXIS post also & I have a modified 3 axis post a co-worker gave me & it work's in it too.

Regard's
Harold C.