Sheets to Solids

[drwhitewater]

What is the best way to make a sheet body a solid body? Our designer uses Rhino and then sends us parasolid or iges files, which then require hours of trimming, extending, closing gaps, sewing, offsetting... Is there a tool or feature that does this automatically or at least quicker than having to do each step to every little problem area?

 

[JohnRBaker]

Are you running NX 5? If so, do the following.

Open a new empty part file. Go to File -> Import -> Parasolid... and select the Parasolid Xmt file and hit OK. Do a display fit so that the Parasolid body is shown (you may need to delete or suppress the Datum CSYS to helot see the model better). Now go into Insert -> Combine Bodies -> Unsew... and select any face of the Parasolid body and hit OK. Now go into Insert ->Combine Bodies -> Sew... and select either the 'face' you just 'unsewed' or the main body as the Target and then the other object as the 'Tool' and hit OK. You should now have a valid Solid Body.

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

http://www.siemens.com/plm

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

 

[drwhitewater]

John,

I am using NX4. I didn't see an unsew feature in the Combine Bodies command list. Is it in a different location, or does NX4 not have this feature?

 

[hudson888]

Dr,

I had a look at your model, what John says may work and I may have a chance to verify more about it later on. However the quality of the surfaces is poor, whether to begin with or as a result of the translation. Even after un-trimming several surfaces have smoothness errors that simply should not be there. You're also missing a couple of faces that can at a pinch be supplied using an offset. There is one very tiny face of no value and even if I can achieve a sew the solid is self intersecting.

I presume therefore that John may have been speaking in theory to some extent. I made it into a solid within minutes but after running examine geometry I quickly realized that there is a lot more things wrong with this data than just the sew.

I can see from experience that your Rhino surfacer is doing several things right, so you may just be having problems with the translation.

After I brought the model in at absolute reference co-ordinates look nearby; X = 3775, Y = -784, Z = 1144

There is actually a little area of the visible surface in that region where the highlights run badly. Translator Problem???

The majority of the visible surface is otherwise very good. I therefore doubt there is anything really wrong with the surfacers' knowledge of his/her craft or attention to the task.

I have rarely seen so many technically un-smooth surfaces in a file according to the examine geometry tool in NX. And the edge trims just aren't right as you already know. When you look at the control polygons of these surfaces they're all over the shop and in some cases you're getting multi patch surfaces of up to 16 patches on what are relatively small faces.

Either Rhino isn't doing the job, isn't being used up to scratch or the translator is an evil thing and you need to try one or all of these options to improve the situation. I think you need to sit down with your Rhino guy get the original data sorted out first and seek help with the translations out from Rhino before you worry about anything else. You may just need to impress upon the surfacer that you have certain modeling tolerance requirements that need to be met. Rest assured other CAD systems are much more finicky than NX so it should not be beyond reasonable expectations to achieve +/- 0.010 edge condition.

Best Regards

Hudson

 

[JohnRBaker]

The 'Unsew' function is new for NX 5 (it literally allows you to 'unassemble' a body, including solid bodies, one face at a time if you wish) and was originally added so that Ideas users could duplicate some very effective work-flows in NX.

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

http://www.siemens.com/plm

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

 

[hudson888]

John,

Even with one body for each face selected the unsew would not work. Extract faces still works.

No bad if the original is suspect to begin with.

Best regards

Hudson

 

[Vikingbro]

dr,

Make sure that if your Rhino guy is exporting IGES, he changes the IGES type to either 'Unigraphics solids' or 'Unigraphics surfaces' and that he set the IGES tolerances correctly. This may help in the translation process.

Good luck!


Chris Cooper
Senior CAD Specialist
Cleveland Golf / Never Compromise

http://www.clevelandgolf.com

http://www.nevercompromise.com

 

[drwhitewater]

Thanks for the responses. I am going to see if we can improve the Rhino file and hopefully have a better translation.