Create Surface - Thicken and then convert to sheetmetal 3

[oharag11]

Please help me with a problem I'm having with creating a Part using existing an existing Part. I attached a file for your review.

http://files.engineering.com/getfil...3c&file=Create_Surface-thciken-sheetmetal.png

So here is my goal: Create a new part within assembly. Make it the Work Part. Select multiple surfaces on another Part in an assembly and offset the faces by 0 (zero). Then I want to thicken this surface a small amount to create a solid. I would then hope to convert this solid to sheetmetal and hopefully unfold. The issue I'm having is once I activate the Work Part to start selecting surfaces I can not reference other faces in the assembly. The only option I get is Faces/Current Work Part. I even tried copying the part I want to reference into the Work Part and I still cannot select faces. If I work within the referenced Part I of course can select the faces, create a surface. though thicken fails. I went so far to try to copy those features and past into the Work Part, and of course this didn't work. What I need is to separate the created part/features into its own part file for production.

So I also decided to try to create two separate curves between top and bottom surfaces - loft/sweep the two curves and then offset. The problem is the edges are complex due to cut I made (some surfaces are straight cut - the other surface is tapered). I saw a post where someone asked for NX to allow 3D sketches like SW. I agree. In SW I would select the edges - choose convert edge. Is there any function like this in NX? I want to do the first option above, but I'm open to solutions.

Another thing I noticed when selecting faces in Reference Part to create an offset surface NX automatically selects all tangent faces. I want to select only the faces to create a surface. Any help?

What I want to represent with this part is paper being attached to all of the surfaces. I would like to unfold this to create a 2D profile so we can use it as a profile to cutout paper.

Thanks

PS Please help JohnRBaker!!!

 

[emorrison]

Have you tried using WAVE Geometry Linker to select the face(s) from the other part?

 

[fsh27]

Could you send the prt file?



Airin
NX Designer

 

[oharag11]

emorrison

To say I received little or no training is an understatement. But I did figure out wave geometry linker. And it worked.Though thicken is an issue, converting to SM is problematic, and I think unfolding it will not happen.

fsh27 I will try to share prt file though we work in TC and exporting out native NX is extremely confusing and complex. Do you have any tips? I went to Export to local HD, set directory, set naming conventions click execute, and then nothing happens.

 

[Toost]

If you do the export using Parasolids it's very simple. File - Export - Parasolid- SELECT THE SOLID BODY + OK (When NX presents the little dialog "Export parasolid")

Exporting from a TC NX session the way you describe should work equally well but is more complex.
Tick the dry run option before the Execute to see how and what will be exported when you execute without the dry run option.

"So here is my goal: Create a new part within assembly. Make it the Work Part. Select multiple surfaces on another Part in an assembly and offset the faces by 0 (zero)."

I think you have managed to create that new partfile . When the new part is the work part, you want to extract copies of the faces in a different part. Maybe this is done in SW using the offset face command ? - In NX it can be done associative using the Wave link feature, or non associative in a couple of ways. Maybe the simplest is "select the faces you desire, Edit Copy ( Ctrl+C) and paste Ctrl+V"
Offset 0?

"Then I want to thicken this surface a small amount to create a solid. I would then hope to convert this solid to sheetmetal and hopefully unfold."

Make sure these faces connect into a "sheet body" before you do the Thicken . A sheet body is a multi-face surface body. Use "sew" to stitch any separate faces.
When in sheetmetal mode, you might need to cut a few edges to be able to flatten.



"So I also decided to try to create two separate curves between top and bottom surfaces - loft/sweep the two curves and then offset. The problem is the edges are complex due to cut I made (some surfaces are straight cut - the other surface is tapered). I saw a post where someone asked for NX to allow 3D sketches like SW. I agree. In SW I would select the edges - choose convert edge. Is there any function like this in NX? I want to do the first option above, but I'm open to solutions."

In NX you can use these edges directly , without any "convert to" or similar. Start the Through curves feature, select the edges.
You can add/connect curves or sketches to the edges and use the combination of curve/sketch/edge in the surface.
Again you might need to use the wave linker to create associative copies in your work part, or in some other way copy the edges over to your work part.


"Another thing I noticed when selecting faces in Reference Part to create an offset surface NX automatically selects all tangent faces. I want to select only the faces to create a surface. Any help?"

In the middle of the screen ( in NX9 or later) there is a small white field where it says "tangent faces" WHEN you are about to select. ( It's not there if you are doing something which cannot use this selection method) If you have selected already, Right click on the selected object and switch to a different selection method.

"What I want to represent with this part is paper being attached to all of the surfaces. I would like to unfold this to create a 2D profile so we can use it as a profile to cutout paper."

Curious, -Why ?

Regards,
Tomas

 

[Toost]

Btw,
John has retired. He will from time to time add in and help. But i do not think he has access to a NX install.
( which is amazing, he should have a "lifetime license in gold" , and the regular gold watch

Regards,
Tomas

 

[oharag11]

Toost

What no more John! He was the main man with all the answers!!! Is there someone else to take his place. I assumed he worked for NX?

A reason why I like SW is due to their VAR setup. You have a problem you contact the local office down the street. If it becomes a bigger problem they contact SW HQ, and resources are applied to your problem. If something is wrong with the SW they submit a SPR and provide the user a reference #. With NX I feel lost. Besides internal help - contacting NX is difficult. I did contact someone and told them my issue. The guy said my request has been on their enhancement list for years. I asked then why not implement. This person said, "We haven't updated Assemblies Functionality since 1974!" Oh boy.

BTW I do like NX. It's more complex then it needs to be. It can be simplified and enhanced. Yes I would argue make it like SW as much as you can without impacting or dumbing down the NX functionality.

 

[oharag11]

Okay

I did the linked faces. I thinkened without issue (0.1mm). I converted to SM. And unfolded just one bend. I attached a Parasolid file for you guys to look at:

http://files.engineering.com/getfil...3-fa68-41e6-9ceb-fb58f4ddf5a6&file=FLATSM.x_t

So I changed how I performed the the cut on the reference part. I did a straight linear cut using an angled plane (5 degrees from normal). Therefore the geometry through the part should be uniform (i.e. radius at start and end should be consistent).

If you look at the attached file I managed to unfold the first bend. Selecting the next bend gives me an error about input face being incorrect please check again. I'm almost there! Any thoughts on how to force bend?

I changed the bend radius to 0.1. Thickness is 0.1. I didn't change the neutral factor at 0.33. I do not know what is causing the error.

 

[oharag11]

Here is a pic of the top profile. I think everything should be arcs and lines and not splines.

 

[oharag11]

Oh and someone asked why paper.

Well we line internal faces with blackout paper to reduce reflections. We do not go out and tool up a die to cutout the profile. I would like to make a 2D Flat profile so our supplier can use it to cutout the flat paper. They can then apply it to the region of interest with confidence. Rather than cutting out a large square material, struggling to get it to lay on a complex surface, and then trimming all the excess off wasting material. I would rather provide what we need before the job is started.

Many people use flat profiles in cad to drive upholstery or cloth. I know SW's goal was to provide an option for their users for this specific reason. Their goal was to allow customers to flatten everything. I do see a need.

 

[Rob_N]

NX11 has a nice forming and flatting tool, of course I don't have the license required for it.

If you have NX4 installed you can use the old fabric flat pattern or Metaform tool. I've been tempted to reinstall NX4 just for that reason. But now I have Autoform to do my one step flat patterns.

 

[JohnRBaker]

John has retired. He will from time to time add in and help. But i do not think he has access to a NX install.
( which is amazing, he should have a "lifetime license in gold" , and the regular gold watch

I did get the "Gold Watch" (but that was actually from EDS, when they sold the company to the venture capitalists but I had enough time with the company to formally retire but deferred the pension, which I'm now receiving). As for having access to the software, when I retired I neither asked for nor was I offered a license of NX. It was by mutual agreement. While it is true that I still follow these forums, both here and on the Siemens PLM Community site, not having the software means that I won't be spending ALL of my time on only those forums ;-) After all, I have other things to occupy my time, such as:

http://www.eng-tips.com/viewthread.cfm?qid=408398

http://www.eng-tips.com/viewthread.cfm?qid=412462

http://www.eng-tips.com/viewthread.cfm?qid=415015

http://www.eng-tips.com/viewthread.cfm?qid=418130

But it hasn't all been fun and games since I retired:

http://www.eng-tips.com/viewthread.cfm?qid=419979

John R. Baker, P.E. (ret)
EX-Product 'Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:

The secret of life is not finding someone to live with
It's finding someone you can't live without

 

[oharag11]

I'm using NX 9.

John I hope all is well with you. Enjoy retirement. You will be sorely missed. Is there anyone else in the NX ranks that is willing to help out us pore soles as much as you did?