How to fix / Smooth Multiple Surfaces, Faces or Edges

[REDesigner09]

Hi,

I have a couple of NX 6 CAD models that has multiple (solid) surfaces, faces or edges - See attachment & pictures. I'm told that if these CAD models are left "As Is", then the CAD models will be more difficult for ANSYS & Tool Programming Engineers to work with.

I'm working with another Engineer to try to resolve or recreate the model, hopefully without having to do a lot of re-work.

Any suggestions would be appreciative. Please see attached pics.

Thanks

 

[REDesigner09]

Oops,

Looks like I did not complete the attachment process. Here's the attachment or pictures.

 

[JohnRBaker]

Before I did anything else, I would first perform a...

Insert -> Combine -> Join Face...

...operation selecting the 'On Same Surface' option. This may help to remove any unnecessary edges ('seams') between smooth faces.

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.com/museum/

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

 

[REDesigner09]

Hi John,

Thanks for the suggestion. As soon as I can get my NX to stop updating, I'll give this a try.


During feature creation & with a bunch of spline profiles, which NX feature will provide better results?

Will the Through Curve, Through Curve Mesh, Swept or any other feature provide more precision & "cleaner" geometry?

What are the dependencies to get "transition" areas to transition well - Twist areas or Thick to Thin areas, etc. Any CAD examples would be great too.

Thanks again.

 

[JohnRBaker]

All other things being equal, Through Curve generally result in the smoothest and simplist faces, while Swept would be next, with Through Curve Mesh after that. Now there ARE reasons why we provide multiple methods because each one has certain characteristics in how they utilize input curves which allows different ways of controlling the final shape, thus if you're dealing with complex curves or you desire more control, you may need to use a more complex function. It's not always possible or practical to always use the 'cleanest' approach when your requirements are complex or requires high degrees of control over the shape of the model.

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.com/museum/

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

 

[REDesigner09]

Hi John & Others,

I tried using the, Insert -> Combine -> Join Face... commands & found this under the, Insert -> Trim -> Join Face...

Regardless, I can't seem to get this command to work for me. On slide 1, there's an area on the middle upper middle let with multiple faces on it.

I have another area similar to this, but with less multiple faces in which I tried the command - Not pictured.

Tried using the Join Face, but the command wants to pick the whole body. Also tried using Sew feature, but missing a step somewhere.

What are you suggestions or steps to get this to work?

Thanks

 

[JohnRBaker]

It will only Join faces which when the edge (seam) is removed would form a single face of the same type and continuity. If the original model was built using suitable tools, often there are NO redundant or unneeded edges in the model. I only recommended performing this operation as it's easy to use and if there are cases which it can clean-up, it's the best way to do so. Aother thing that you might consider, if the model is no made up of features (i.e., the solid models are dumb), you could use the...

Export -> Heal Geometry...

...function which will produce a copy of the part file with the model 'cleaned-up' removing small faces, edges and filling gaps and so on. Often, this will improve the quality and performance of subsequent meshing operations.

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.com/museum/

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

 

[Xwheelguy]

I'm a former NX user and I used to define the outer boundary of a group of sewn surfaces and then use Quilt to combine them into a single sheet. I would remove the parameters (usually a transform with copy) of the Quilt and then recreate with any continuity that may be needed.

You'll probably find yourself building surfaces, deleting and rebuilding surfaces to fine tune the continuities.

Get familiar with extracting the UV curves, trimming them and using Bridge Curves (non-associative) to get the continuities where you need them. Watch your gap & angle tolerances. Don't make them too large and never mix them - pick one and stick with it.

HTH & good luck.

Tim Flater
Senior Designer

 

[DaSalo]

Tim,
Could you elaborate a bit more on what you mean when you say you remove parameters of the quilt and then recreate? I'm not following exactly what you are doing here and why it would be necessary to use transform. I understand what it means to remove parameters and how all of the individual tools you mention work but I'm not quite grasping what the work flow looks like.
Thanks for your time.

-Jeff

 

[mlamping]

I thought I would chime in with respect to the ANSYS thread. Have you considered meshing the geometry in NX? NX has an ANSYS environment as well, so there's potential for you to do all of your pre/post processing work with ANSYS as the solver.

But getting back to your main issue. NX CAE products use a polygon geometry layer that is fed parasolid geometry as input. The polygon geometry is just tessellated data that is ideal for quick/dirty face editing such as removing vertices, edges, collapsing short edges to vertices, and splitting faces and edges. Geometry editing is built into the meshers too. By default NX will try to eliminate all geometry artifacts less than 10% of the global element size defining a mesh. Those slivers you identify in the PPTX could be eliminated automatically by the mesher. Or you could eliminate them manually.

I uploaded a PPTX to this post as well. It contains overview slides of the solver environment and polygon geometry concepts that I described above.

Regards,
Mark

Mark Lamping
CAE Technical Consultant
Siemens PLM Software

 

[Xwheelguy]

Jeff,

Due to the fact that we were working with styled surfaces coming from Alias and we weren't the owners of said design, there wasn't a need for retaining any parameters on the rebuilt surfaces. So when I would recreate them, I would not keep them associative or parametric - a transformed surface (back then) wasn't associative, but just a dumb surface, so after the Quilt, I'd transform it (usually rotate), delete the Quilt, then rotate the dumb surface back to the original position take the place of the Quilt. I could then work on smoothing the surface more (extract UV curves, examine curves, refine/rebuild UV curves, rebuild surface) or work on continuity with adjacent surfaces using the same workflow with the UV curves, only trimming them back to an intersection and filling in the gaps with Bridge Curves.

I hope that gives you a better idea of the workflow.

Tim Flater
Senior Designer

 

[REDesigner09]

Hi John & Others,

I tried the, Export -> Heal Geometry... & this did such a good job that it literally wiped out the model. All its left is the geometry profiles or splines that originally helped created the model & handful of "Body" features.

This definitely does not appear to be my solution.

As for the, Insert -> Combine -> Join Face... commands or Insert -> Trim -> Join Face...

I am getting errors, such as:

Join Faces -> On the Same Surface
Failed to change topology

or

Join Faces -> Convert to B-Curves
Face is not parametrical-retangular


Not sure what these mean & more importantly how to use fix these areas.

I'm assuming I'm not selecting or using this function correctly, but whatever suggestion that can be provided would be appreciative.

Thanks

 

[JohnRBaker]

Those are NOT 'error' messages, but rather simply messages reporting the 'status' of your use of the function.

In first example, where it reported that it "Failed to change topology", this simply means that there were NO edges (seams) which could be removed that would have resulted in creating a single face from multiple faces. It does NOT mean that there was anything wrong with the model, just that it did not find any suitable candidates for performing a 'Join Face' operation on. For example, if I create a block and added an edge blend, and if I then attempted to 'Join' the faces of the block I would have gotten that same message, not because there was anything wrong with the block or any of its faces, just that the faces that it found were inappropriate for the operation requested. Perhaps we could have worded the message better, but it was accurate.

As for the second case, that was simply stating that for the operation which you selected, the software was expecting a face bounded by only 4 sides, a common limitation when created a B-surface of any type.

As for the 'Heal Geometry' result, without actually having access to the part file in question, it's hard to say why you got the result that you did. One thing that may have effected this is the overall SIZE of your model, not the size of the part file but rather the actual PHYSICAL size of the model. Is is VERY SMALL, like features being significantly less than a millimeter in length/width? If so, you may need to change the default settings used by the Heal Geometry command since one of its functions IS to remove very small faces and edges. So if your model is very small with very small faces and edges, and you're using a 'Tiny Tolerance' larger than the majority of the faces/edges in the model then that's exactly what it tried to do, remove those 'tiny' edges and faces.

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.com/museum/

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

 

[REDesigner09]

Hi Everyone,

After additional evaluations, it appears that my profiles splines were imported in sets or segments.

When using anyone of the Through Curve features, does the vector direction(s) have a factor of how well the feature will be created between segmented areas?

Thanks

 

[JohnRBaker]

As long as adjoing curves run in the same 'direction' and the starting points are aligned, you should be OK as the number of segements (as long as they are smooth, if that's the intention) is not all the critical.

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.com/museum/

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

 

[DaSalo]

Tim,

OK, I understand what you are doing now. It seems a little round-about but that is probably because some tools and options that I take for granted haven't really been around that long. I would accomplish the same thing by creating the quilt and then using edit => feature => remove parameters.

Thanks for elaborating.

-Jeff

 

[REDesigner09]

Hi John, DaSalo & Others,

I thin this is part of the CAD construction problem (John) with all these miscellaneous surfaces, faces or edges. These imported profiles or splines has multiple vector directions. This is particularly noticeable when using one of the Through features & trying to "connect" going one imported spline profile segments to another.

The company uses other software called Geomajic, PolyWorks & KeyCreator to define reverse engineering data & to create these various profiles. If the vectors can be controlled in these applications, then I think the root is other engineers weren't aware of this. Now I need to investigate if these vectors can be controlled before importing into NX.


Also, I got the Join Face features to work on areas that had minimal surfaces or faces. The surfaces definitely look better, but in some areas, there are still small bumps or wavy surfaces. I do not see a way to remove these wavy or bumpy surfaces, but they're relatively small & I don't think it will cause downstream issues.

Is this considered a "band aid" fix? Even though the surfaces look good, will ANSYS or Tool Programming still "see" these multiple surfaces?

DaSalo,

Although this model is not 100% parametric, we want to keep this model as parametric as possible. If I'm interpreting your suggestion correctly, your suggestion would remove (more) parameters, which I think would end up being a dumb solid.

Is this your intent or is there a better solution?

Thanks everyone.

 

[JohnRBaker]

I can't speak for the tools used by the ANSYS software, but I know that the meshing tools that we are supplying in NX, as Mark Lamping has already pointed out in an early entry in this thread, has options which allows the creation of meshes which can account for and resolve many of these not-so-ideal models, and as Mark also pointed out, if you still needed to use ANSYS for the actual analysis, the meshes created in NX can be exported to the ANSYS software for solving, and the results can even be brought back into NX so that you see your results displayed with the original geometry making it much easier to make your evaluations as well as detecting whether those small surface anomalies appeared to effect the local results or not.

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.com/museum/

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

 

[Xwheelguy]

Jeff,

No problem. The reason I prefer to rotate is because remove parameters doesn't remove all the original wireframe geometry (curves) that was no longer needed, so I would just do it all in one Delete -> rectangle trap/selection, then rotate the copy back to where it was to be used.

To each their own, that's the beauty of NX; there is usually more than one way to skin a cat.

Tim Flater
Senior Designer

 

[DaSalo]

REDesigner,

Sorry, I think Tim and I were having a small side conversation that has muddied up the thread a bit. I was trying to understand his work flow more clearly because I know from his previous posts that he has a ton of experience working with complex surfaces.

I wasn't specifically recommending that you follow this non-parametric workflow in your specific situation. You can do the same thing parametrically.

The idea is just that you have surface that you is very close to what you want but not exactly; it has these small irregularities. So it follows that you will need to create a new surface that deviates somewhat from your current surface in order to correct these irregularities. How much deviation are you willing to accept? Once you decide on that tolerance zone you can repair your surface by extracting curves, correcting those curves through the use of a variety of tools, creating a new surface using through curves or through curves mesh, and then replacing your original surface with the new surface. You'll be doing plenty of deviation analysis along the way to make sure everything is staying within tolerance. There are parametric and non-parametric ways to do all of these steps. The non-parametric workflow is a lot simpler but if you really need the parameters you could definitely do it in a way that would be parametric.

From what I've read here it sounds like the easiest and most straight-forward solution to your problem is to purchase some additional features for NX and let the software do all, or most of, this work for you in the meshing process.

It isn't even totally clear to me that you would actually have much of a problem if you left things as-is. Speaking as a tooling engineer that deals with exactly this type of product all the time: I could easily work with your model. Would it be a tiny bit easier if everything was perfect? Sure, but I have a skill set that allows me to work through stuff like this and I really don't mind doing it at all. I would guess that most people in tooling or analysis would have a similar skill set.

-Jeff