NX 5 Sweep Question

[mnd2659]

1)Using a linked sketch as a section for the sweep operator.
2)Using one guide string for direction.
3)Using face as orientation

Sweep is one of the main operators I have been using to create solids for exterior door upper moldings, the 3 steps I take as described above are usually flawless, until today, when I ran the sketch section the sweep didn't reconize sharp corners in section, it gave me a radius as a result. Is there a default setting in the sweep operator that I'm missing? The same section will extrude and give the desired results. Any help would be appreciated!

 

[cowski]

If there is a 'Preserve shape' option for the section, toggle that on (this option is available in NX6, not sure about NX5). If not, reduce the feature tolerance to 0.

 

[hudson888]

Yes cowski sounds right. It has been a quirk of NX that in earlier versions when sweeping you needed to set the tolerance to zero, and in later ones to tick a box called preserve shape. It should always have been that whether there is a tolerance or not you need to tick a box asking for joined curves by default. I know of no cases where I haven't wanted the sectional elements of my sweep per the input curves. The system seems to want to assume that you'd like to join the curves when sweeping sections, which I would have to say is one of the dumber assumptions I have ever encountered.

In your case I suspect that preserve shape may have gotten ticked off in error during a previous attempt to create a sweep.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[JohnRBaker]

Don't discount the notion of combining curves since that often results in a body with only a single face along the length of the sweep. Granted, if the profile has sharp corners then the preserve shape often gives the desired result, but when the profiles curves are smooth yet still distinct, often the desire is for a final result with NO seams. Granted, one could combine the profile curves ahead of time, but that is an extra step which results in extra features and could be seen as adding more steps and complexity than is necessary.

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

 

[mnd2659]

Using Preserve shape corrected the issue, thanks to all for the valuable input. I do agree that the assumption of joining curves by default is just thhe opposite of most desired results.