Surface Delete in NX6 1

[maxxforce23]

Hi NX6 Users,

How to delete a surface(s) in a 3D part w/o using synchronous tech.?

Thanks - Maxxforce23

 

[cowski]

Any particular reason that you have to avoid synchronous? The delete face will work in history based mode and will show up as a feature in the tree, you don't have to go into history free mode to use most of the synchronous modeling commands (there are a few exceptions).

 

[maxxforce23]

Thanks, Cowski!

There's no reason at all, I have try the regular way and using synchronous but it delete the whole feature every time rather than just a single surface that I want. I have used IDEAS for the past 15 yrs and it very easy to delete a surface(s) and I tried it in NX6 and have a problem doing so. I know there's an easy way but can't figured it out.

 

[hudson888]

Are you talking about a sheet body as in surface or do you mean one face of a solid body?

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[maxxforce23]

Hi Hudson.

I tried to delete one face of a solid body. Thanks!

Maxxforce23

 

[hudson888]

Okay then you would use Delete Face as Cowski suggested if it gives you an unexpected result try reversing the vector.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[maxxforce23]

Thanks for your help, everyone!

I will try it out and let you know later...

Maxxforce23

 

[cowski]

Also, on the selection toolbar make sure it is set to single face and not something like 'tangent faces' (unless that is what you want, of course).

 

[JohnRBaker]

OK, since you mentioned Ideas I suspect that what you want to do is LITERALLY 'delete' one of the faces of a solid body like you could could before. The traditional NX 'Delete Face' command won't work for you since you don't really want a nice cleaned up solid body as a result but rather a body with a 'hole' where the face used to be which you just 'deleted', correct?

If so, try going to...

Insert -> Combine Bodies -> Unsew...

...and selecting the face(s) you wish to 'delete'. After you hit OK, while it may not look like anything happened, the solid has been 'split' into two 'sheet bodies', so just hide the portion which you no longer need (but don't try to actually delete it since it's now actually a feature and not really a separate sheet body).

Anyway, give that a shot and she if that was what you were looking for.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[maxxforce23]

Hi John,

This is the exact answer that I'm looking for, I have try it in NX6 and it works great. Thanks to other users that have shared their opinions regarding to my question.

Regards,

Maxxforce23