Problem with static structural analysis

[holmesss]

Hello,

I recently started using femap 11.1 and I've been having a problem for the past two weeks that I can't solve.

I have a simple assembly of two parts that I exported as a parasolid ( .x_t) from solidworks.
When I run the FEA static analysis in solidworks simulation , it works with no errors.
When I open the parasolid assembly in femap , and when I run the analysis I get a fatal error 9031 (ERRPH1) .
I tried reducing the size of the mesh, I ended up with more errors.
I tried to check element quality ,I ended up with missing surfaces.
Only one of the two parts is causing the problem,is there a way or program to fix the part?It's really frustrating.
Any ideas why the same assembly works on solidworks simulation but not on femap ?

Thank you very much.

 

[holmesss]

@compositcurves Please find the assembly already uploaded in a previous post.
I will also try to upload it again.

 

[holmesss]

@rob768 @Kwan thank you for your tips, I will try to apply them now.

 

[BlasMolero]

Dear Holmess,
Well, you will agree with me that the geometry is quite strange to mesh with FE, it seems a StereoLithography source. If I use command GEOMETRY > SOLID > CLEANUP I see that many sliver surfaces exist:

Solid Cleanup
1 Solid(s) Selected...
Found Sliver Surface ID - 9438
Found Sliver Surface ID - 9440
Found Sliver Surface ID - 9442
Found Sliver Surface ID - 10477
Found Sliver Surface ID - 11073
Found Sliver Surface ID - 14014
Found Sliver Surface ID - 14936
Found Sliver Surface ID - 14955
Found Sliver Surface ID - 14973
Found Sliver Surface ID - 14992
Found Sliver Surface ID - 18176
Found Sliver Surface ID - 18177
Found Sliver Surface ID - 18286
Found Sliver Surface ID - 18302
Found Sliver Surface ID - 18339
Found Sliver Surface ID - 18346
Found Sliver Surface ID - 18347
Found Sliver Surface ID - 18348
Found Sliver Surface ID - 18349
Found Sliver Surface ID - 18350

If I plot the surface geometry in detail I see thefollowing:

Also, I see I am able to cut the solid body using command "Geometry > Solid > SLICE":

I will try to mesh playing with the "Mesh > Geometry Preparation" command (the hidden jeweld of FEMAP!!). In fact, I am OK, but you can see many messages with degenerated surfaces. Also, the resulting mesh has a TET collapse of 111, this is brutal.

Tet Mesh Solid
1 Solid(s) Selected...
Material 1 Created.
Meshing Surfaces...
Meshing Skipped on Degenerate Surface 12852.
Meshing Skipped on Degenerate Surface 13143.
Meshing Skipped on Degenerate Surface 14955.
Meshing Skipped on Degenerate Surface 18890.
Meshing Skipped on Degenerate Surface 18897.
Merging...
0 Node(s) Merged.
Loading Elements...
  MESHING SOLID 2        ______________________________________________________
  -- SURFACE MESH       108572 Triangles
 
  -- SURFACE MESH QUALITY
     MINIMUM ANGLE _____________________
      60.0 > A > 40.0     77391 Elements
      40.0 > A > 25.0     26576 Elements
      25.0 > A > 15.0      4241 Elements
      15.0 > A > 10.0       290 Elements
      10.0 > A >  5.0        54 Elements
       5.0 > A >  2.0        19 Elements
       2.0 > A >  1.0         1 Elements
 
     Worst Angle    = 1.759     Element 104227 (53031 597 596)
     Shortest Edge  = 0.00439   Element 811 (597 584 596)
     Longest Edge   = 0.262     Element 107404 (32221 53000 32222)
>>>  Warning : Found duplicate face :    30597    30599    30598 
>>>  Warning : Found duplicate face :      150      152      151 
>>>  Warning : Found duplicate face :      363      395      394 
 
  -- TETRAHEDRAL MESH QUALITY
     ASPECT RATIO / COLLAPSE ___________   JACOBIAN ___________________________
         1 < C <    2    357065 Elements     0.00 < J < 0.10    346864 Elements
         2 < C <    3    531332 Elements     0.10 < J < 0.20    386938 Elements
         3 < C <    5     55158 Elements     0.20 < J < 0.40    205336 Elements
         5 < C <   10       998 Elements     0.40 < J < 0.60      5120 Elements
        10 < C <   20       177 Elements     0.60 < J < 0.80       427 Elements
        20 < C <  100        58 Elements     0.80 < J < 0.90        81 Elements
       100 < C < 1000         2 Elements     0.90 < J < 0.95        17 Elements
      1000 < C                0 Elements     0.95 < J                7 Elements
 
     Worst Collapse = 111.      Element 123632 (12423 54262 12410 53376)
     Worst Jacobian = 0.978     Element 293495 (10747 10749 10748 53388)
     Shortest Edge  = 0.00439   Element 131907 (53031 596 597 584)
     Longest Edge   = 0.385     Element 110593 (54517 54519 55628 55438)
 
  -- TETRAHEDRAL MESH   944790 Tets

Here you are the finished model: more than 1.3 million of nodes. In summary, reducing the element size you can reduce as well the mesh distortion and arrive to a valid TET10 mesh, OK?.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[holmesss]

@BlasMolero Thank you for your input. You are right the model derives from STL.
I didn't quite understand your conclusion : Did you mean that I can mesh the model as it is right now if I choose a very small mesh size?(What size?)And will the analysis run after it?
If you had to correct this model,so you could then be able to use a mesh size a little bigger so that it wouldn't take hours to run the analysis, what would you do?
Because the cleanup is unable to correct all the errors . Is there any tool that you think would be efficient to adjust the geometry and make it pass?
My target is to use a mesh size of around 0.04 .

Thanks again.

 

[BlasMolero]

Dear Holmess,
What I try to show you is that you can mesh the model in FEMAP in just a few minutes using the minimum inputs. But if you want to invest time to improve your mesh quality & reduce model size then in FEMAP you have powerful tools to detect & remove very small edges & sliver surfaces: simply go to MESHING TOOLBOX > TOOGLE ENTITY LOCATOR and then you can inspect your full geometry and shearch for "CURVES > SHORT EDGES" or "SURFACES > SLIVER SURFACES, SMALL SURFACES", etc .. You can create groups automatically with the detected geometry and remove them using FEATURE REMOVAL > SURFACES, etc.. Playing with FEMAP Meshing Toolbox will help you to do the cleaning job in deepth, you can perform a "forensic" job with both geometry & mesh!!.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[holmesss]

Thank you all for your tips. It was really helpful . I finally have both parts cleaned and they can be meshed perfectly !
But after cleaning , both parts don't fit one on the other perfectly anymore(There is no congruence , there's voids and intersections when they are assembled one on the other).
If you import both models together, you will see what I mean. Is there a was to remove the intersections and fill the voids between both parts so that they will be adapted perfectly one on the other ?

 

[BlasMolero]

Dear Holmess,
You can remote interferences using "GEOMETRY > SURFACE > NonManifold-Add": first you select thw two solids and perform the solid add, and next you issue the command "Recover NonManifold Add". It´s tricky, the result will be three solids: the two original ones but also the interference(s) as another solid(s). Because you want to avoid interferences, use command GEOMETRY > SOLID > ADD to define a continuos solid, adding the interferences solid to the base one.

To understand the workflow, better define I simply assembly with interferences to see how it runs, OK?.
Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[holmesss]

I give up.When I try to remove the silvers , femap stops working . (1040 slivers detected).
I have to think of another way.
Does femap support ansys meshes ? I mean, if I mesh the models on ansys, can I import them on femap and use the mesh to run the analysis
or will it give me the same problems again ?
Final resort : Does anyone know any freelancer that is familiar with femap?
Btw @BlasMolero your youtube tutorials and blog are helpful , except that they can be applied to simple models with not too much faces and surfaces.
Thank you all for your help

 

[holmesss]

For example one model is perfectly clean. It meshes with no errors,no skipped faces or anything.
And if I do geometry solid cleanup, it says "Solid passes geometry check".
Now when I put some loads and constraints and run the analysis : Fatal error 9031 .


What am I doing wrong ? Should it be that complicated or is it just a learning curve?

 

[BlasMolero]

Dear Holmess,
I am very sorry for the problems you are having, but please note this is not only a problem of FEMAP, this is FEM/FEA where the learning curve take its time. I suggest to contact your local FEMAP VAR/Reseller to ask for a training course from a qualified teacher, fortunately we have an excellent and very good skilled engineers in the FEMAP & NX Nastran network resellers all around the world, then you will understand how to prepare geometry, how to arrive to a quality mesh, how to run the NX NASTRAN solver, etc.. this is the way to became productively immediately, not miracles or magic wand exist.

Back to your problem, I suggest to issue command "TOOLS > CHECK > ELEMENT QUALITY" and check the quality of your FE mesh, specially for TET10 mesh make sure to activate TET COLLAPSE & JACOBIAN ratio. Your mesh could pass the aspect ratio, but jacobian ratio is critial in volumetric mesh.

Fortunately, in the upcoming relase of FEMAP V11.2 we will have a mesh quality check specific for NX NASTRAN solver that will give the user exat information of the quality of your mesh to know in advanced if your FE model can be solved by NX Nastran. Meanwhile, activate the DATA TABLE and this way all the output of check command will go to the DATA TABLE where you can inspect & locate inmediately the more distorted elements.

Also, the upcoming release of FEMAP V11.2 will perform automatically "TET Sliver Removal" during the meshing process, stay tuned!!

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[holmesss]

Thank you for your suggestions.

Is it normal that a model(the working part that I uploaded in the beginning ) has 115 out of 72000 elements that fail the jacobian and still meshes perfectly and the analysis runs smoothly with no errors? And then other models have failing elements but don't mesh properly and give errors on the analysis.

 

[holmesss]

Never mind my last question. I found the answer to that.
Thank you very much once again for your help. This site is really helpful.

 

[holmesss]

I now have the two parts, both in good quality mesh that pass the element quality check and can go through analysis with no errors ,but each separately .
If I put both parts together (assembled) and after doing a non-manifold add , the analysis fails, because the non-manifold add and the recover manifold
gives me a bad mesh again at some regions of the part.
My question is : If I want to obtain congruence on the interface between the two parts , is there a way to do it in femap?
After the non-manifold add and the recover manifold , i get congruence but not on all the part.
Any tips ?

 

[holmesss]

SO this is where I have the problem , it's at this region where the top part ends ,without covering full triangles of the bottom part.
Can I achieve congruence here? because everywhere else in the assembly,Where the top part covers the entire lower part,I have congruence.
Should I just set the connector to surface-edge and node-surface ?

 

[BlasMolero]

Dear Holmess,
The connector "surface-to-surface" runs OK when you have touching faces of geometry, paralell face-to-face, but this is a StereoLithography geometry where everything is caotic. But if you are able to create two groups of nodes becaming to each component then you can use the command "Mesh > Connect > Closest Link ..", is very powerfull, it enables you to choose two sets of nodes, and FEMAP will automatically generate line elements, constraint equa­tions, CGAP node-to-node elements, or rigid RBE2 elements between each node in the first set of nodes (the "Generate From" selection) to the nearest node in the second set of nodes (the "Generate To" selection). This is a useful method to automatically generate a series of connections between two patterns of nodes or between a pattern of nodes and a single node.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[holmesss]

this is very helpful.thank you .