×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Problem with static structural analysis

Problem with static structural analysis

Problem with static structural analysis

(OP)
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.

RE: Problem with static structural analysis

have you looked in the f06 file, there's more description about the error codes there.

how have you joined your two parts together ?

another day in paradise, or is paradise one day closer ?

RE: Problem with static structural analysis

(OP)
Yes I connected the two parts.
Even when I delete the part that's not causing any problems , and run analysis with only the part causing the problem , i still get the same error.

in f06 there's a message "nogo encountered in subdmap semg."

But I really don't understand the problem.
Maybe the part has edges or faces causing problems for femap ?
Can you recommend a tolls or a way to check my part and fix it ? (But again,the part performed normally in solidworks)

thanks a lot for your reply

RE: Problem with static structural analysis

"subdmap" ? ... doesn't sound like a simple linear run.

how's the connection between the pieces modelled ? are the connections inline (like a hinge) ? are the connections springs ? If a model is supported only by springs it'll fail (constraint 1 node in 6dof to take out rigid body motion)

you think the problem is in one piece ? can you run the model with only the piece you think works ? can you run the other piece on it's own with the connects remodelled as constraints ? what if you "weld" the pieces together (change the element nodes, yes?) ?

a pic might help ?

another day in paradise, or is paradise one day closer ?

RE: Problem with static structural analysis

(OP)
Yes the problem is in one piece, because if I run the good piece alone , it works. While when I run run the "faulty" piece alone it fails.

Also when I mesh the faulty piece , I can read that the mesher skipped a few degenerate surfaces.And they also say that there are duplicate faces somewhere.(Eventhough when I check the model,I can't find the duplicate faces).

I will attach the file in a bit.

RE: Problem with static structural analysis

i don't know what a .x_t file is, and neither does my computer ... how about a screen shot ?

another day in paradise, or is paradise one day closer ?

RE: Problem with static structural analysis

Try the File / Rebuild and list here the error messages.
If there are some duplicate surfaces then their IDs will be printed in the message box.

Seif Eddine Naffoussi, Stress Engineer
www.Innovamech.com
33650 Martillac û France

RE: Problem with static structural analysis

(OP)
@compositecurves well after meshing I get the following : "Tet mesh was created but problems were reported " "...4 nodes causing the problem"

If I look into the comment box : >>> Warning : Found duplicate face : 96 2168 97
>>> Warning : Found duplicate face : 96 2214 2168

These two sets of 3 numbers each , are coordinates or IDs ? So there's 2 faces or 6 faces causing the problem ?How can I delete them ?Or should I leave some of them ?

RE: Problem with static structural analysis

(OP)
Because if I do Geometry->Solid>Remove Face and Type "96" for example or even "96-97-2168" they say "0 face was selected"

RE: Problem with static structural analysis

duplicate face for a tet would suggest the three numbers are node IDs.

have you tried the coincident node check ?

can you view these nodes or elements (using "show entities") ?

another day in paradise, or is paradise one day closer ?

RE: Problem with static structural analysis

(OP)
No I can't see them in "show entities" .
It's really complicated it seems.
Do you think I should not use parasolids ?
What's the best file format for FEMAP ?(I'm new to femap as you can see).

Thanks a lot for your time btw

RE: Problem with static structural analysis

if it exists in the modfem, it'll show in "show entities" .... have you checked the boxes "transparent highlight" and "label with ID". you can also use "list, model"

another day in paradise, or is paradise one day closer ?

RE: Problem with static structural analysis

I've already encountered this kind of issue but forgot how I solve it.
Export a ".dat" and import it in a new Femap then see what errors will be shown.
Otherwise, you should clean up your geometry before meshing it. There are a lot of capability under Femap to solve geometry issue.
Use the meshing toolbox to identify small edges and surfaces...

Regards,

Seif Eddine Naffoussi, Stress Engineer
www.Innovamech.com
33650 Martillac û France

RE: Problem with static structural analysis

"I've already encountered this kind of issue but forgot how I solve it." ... damn ! don't you just hate that !

another day in paradise, or is paradise one day closer ?

RE: Problem with static structural analysis

(OP)
Hope you remember ! Because I think I'm hopeless with this assembly .

RE: Problem with static structural analysis

Could you drop the CAD if it is not confidential? or just the part causing problem?

Seif Eddine Naffoussi, Stress Engineer
www.Innovamech.com
33650 Martillac û France

RE: Problem with static structural analysis

I read the X_T model and it looks like your model has some cavities (no pun intended). The crown has some holes, near the edges. You will need to fix that but i don't think this can be done automatically. The error most likely is in the program determing/scanning the geometry.

RE: Problem with static structural analysis

I've run into this before. The 3D model probably has "weird" geometry that is causing issues. You need to change the accuracy of the model in solid works. I'm not sure how to do this but there is a setting to do this. The model will likely fail at the bad geometry and then you can fix the issue and export. Hope this helps.

RE: Problem with static structural analysis

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

RE: Problem with static structural analysis

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:

CODE -->

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.

CODE -->

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/

RE: Problem with static structural analysis

(OP)
@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.

RE: Problem with static structural analysis

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/

RE: Problem with static structural analysis

(OP)
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 ?

RE: Problem with static structural analysis

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/

RE: Problem with static structural analysis

(OP)
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

RE: Problem with static structural analysis

(OP)
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?

RE: Problem with static structural analysis

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/

RE: Problem with static structural analysis

(OP)
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.


RE: Problem with static structural analysis

(OP)
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.

RE: Problem with static structural analysis

(OP)
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 ?

RE: Problem with static structural analysis

(OP)
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 ?

RE: Problem with static structural analysis

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/

RE: Problem with static structural analysis

(OP)
this is very helpful.thank you .

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources