Welcome to the forums. Please post in English or French.

You are not logged in.

#1 2019-10-24 14:12:34

marcelo
Member
From: Brazil
Registered: 2017-06-20
Posts: 79

Error generating mesh

Hi,

An error is happening in my mesh and I don't know how I can fix it, could someone help me?

Downloadable file: encurtador.com.br/aBIJ3


Attachments:
error.jpg, Size: 205.02 KiB, Downloads: 266

Offline

#2 2019-10-24 17:01:09

dezsit
Member
Registered: 2012-06-27
Posts: 69
Website

Re: Error generating mesh

Hello,

This geometry cannot be meshed with pure hex (the error relates to this problem). You have to combine Hex(ijk) Extrude3D and finally you will have a part (the corner fillet) what can be meshed with tetras (maybe you have other possibilities to produce some wedges or mixed mesh here, but I did not try it).
Check the attachment (salome 9.3!), it is not so nice, but you can tweak with the sub meshes to produce better results, or make more partitioning.

BR
dezsit


Attachments:
Fadigue_rep.zip, Size: 456.76 KiB, Downloads: 303

Offline

#3 2019-10-24 17:32:35

marcelo
Member
From: Brazil
Registered: 2017-06-20
Posts: 79

Re: Error generating mesh

Hi,

I am very grateful that you had the good will to generate a new mesh, in fact it is not with error. However, there is a detail... according to the International Institute of Welding that conducts studying fatigue in welding, it is recommended a number of elements close to 8, see the image I attached (it is a little befitting the models I was having problems). So I believe it is possible to have a hex mesh, but the strategy for it to be made... I don't know how to follow it.

IMAGE: encurtador.com.br/bryT7

EDIT1: I made a minor case of the region that gives error and it still gives error, I think it is the easiest way to try to visualize how to solve the problem. (.hdf: encurtador.com.br/ozN56)

Last edited by marcelo (2019-10-24 19:07:02)

Offline

#4 2019-10-24 20:25:36

dezsit
Member
Registered: 2012-06-27
Posts: 69
Website

Re: Error generating mesh

Hi,
Actually I'am far from a computer with SalomeMeca, and I was not able to open your files either. Nevertheless I know the guideline you mentioned very well (daily routine almost).

So I have two notes:

1) I tried to sketch what you can do to achieve a hex mesh, supposing that I remember your problem correctly. The key is the partitioning of the eighth sphere at the fillet. You have to make 3 hex like partition in it (red lines), then follow this cuts in the neighboring regions as well. Good luck to it, it will be a lot of work in salome.

2) what kind of approach you are going to follow? I suppose you want to evaluate your welds based on structural stress and stress extrapolation, because as you might possibly know, for local notched based evaluation you have to use fillets at the root of the welds as well. So just do some test how your mesh influence your extrapolated structural stresses, and you will find, that if you can capture the bending part at your evaluation points correctly, then the mesh at the weld representation will not affect your results significantly (at least not as much as other uncertain parameter of your study, eg. how you select a proper FAT class, or other modifiers or even estimation of the loads), so in a real structure, it simply not worth to spend too much time with the meshing, a good quality quadratic tetra will be enough (or sub-modeling). Your real weld will never look like this...

BR,
dezsit


Attachments:
Capture-1.png, Size: 4.6 KiB, Downloads: 236

Offline

#5 2019-10-24 20:51:54

marcelo
Member
From: Brazil
Registered: 2017-06-20
Posts: 79

Re: Error generating mesh

dezsit wrote:

Nevertheless I know the guideline you mentioned very well (daily routine almost).

Very interesting, I'm starting my studies on fatigue now... so I started with an example from the book I found.

1) I tried to sketch what you can do to achieve a hex mesh, supposing that I remember your problem correctly. The key is the partitioning of the eighth sphere at the fillet. You have to make 3 hex like partition in it (red lines), then follow this cuts in the neighboring regions as well. Good luck to it, it will be a lot of work in salome.

I didn't see if you made these steps in the file you sent me. However, reading what you wrote, I do not understand very well how the divisions should be made so that I can make a hex mesh. The interesting thing for me right now is to use the file I created, which has a simpler geometry, and try to reproduce a hex mesh in it.

2) what kind of approach you are going to follow? I suppose you want to evaluate your welds based on structural stress and stress extrapolation, because as you might possibly know, for local notched based evaluation you have to use fillets at the root of the welds as well. So just do some test how your mesh influence your extrapolated structural stresses, and you will find, that if you can capture the bending part at your evaluation points correctly, then the mesh at the weld representation will not affect your results significantly (at least not as much as other uncertain parameter of your study, eg. how you select a proper FAT class, or other modifiers or even estimation of the loads), so in a real structure, it simply not worth to spend too much time with the meshing, a good quality quadratic tetra will be enough (or sub-modeling). Your real weld will never look like this...

Interesting remark! By the way, if you allow me a question ... do you do fatigue analysis using Code_Aster?
This is the example I want to reproduce: researchgate.net/publication/301092698_Case_Study_1_Box_Beam_of_a_Railway_Wagon

Best,
Marcelo

Offline

#6 2019-10-24 21:13:54

dezsit
Member
Registered: 2012-06-27
Posts: 69
Website

Re: Error generating mesh

The suggested partitioning is not part of the model I prepared to you, actually I did not make any new partition, I just used what you created. As I mentioned, I am not able to open your small study (I do not have access to SalomeMeca for a while), and hard to explain the strategy better by words, than I did in the sketch. The key for hex meshing is to produce six sided regions (actually boxes), so you have to cut out 3 six sided regions from the sphere at first, then to make conforming mesh, you have to follow this partitioning lines in all of the connecting regions, and ensure the same number of nodes on every connecting edges.

The fatigue evaluation is a post-processing step (aster has also a dedicated post-processing command for this), so you can produce input to it with any kind of FEA code, so depending on the request we used various FEA codes to get the stresses, then made the post processing evaluation by hand calcs., spreadsheet, python scripts, or dedicated fatigue evaluation tools. But yes, nowadays we working a lot with Aster.
Prof. Fricke is a big name in the field of weld fatigue, I also recommend to carefully read out every IIW recommendations, or the FKM Guideline, ff you have access to it, or the related chapter of pressure vessel codes, (eg. EN13445), or check the available resources of FemFat (or other fatigue tools), you can learn a lot from them.

BR.
dezsit

Last edited by dezsit (2019-10-24 21:15:36)

Offline

#7 2019-10-28 12:31:47

marcelo
Member
From: Brazil
Registered: 2017-06-20
Posts: 79

Re: Error generating mesh

dezsit wrote:

The key for hex meshing is to produce six sided regions (actually boxes), so you have to cut out 3 six sided regions from the sphere at first, then to make conforming mesh, you have to follow this partitioning lines in all of the connecting regions, and ensure the same number of nodes on every connecting edges.

Like this? Link: demonstrations.wolfram.com/DividingARegularTetrahedronIntoFourCongruentPieces/

I also recommend to carefully read out every IIW recommendations, or the FKM Guideline,...

Is the FKM guide you recommend? Link: sciencedirect.com/science/article/pii/S1877705815045932

Sorry for the delay in answering.

Offline

#8 2019-10-31 09:06:48

dezsit
Member
Registered: 2012-06-27
Posts: 69
Website

Re: Error generating mesh

Hello,

hex mesh: yes, for example. You can produce with this a fully structured hex mesh, but will be hard to make the connecting regions properly partitioned and to provide equal mesh seeding on the opposite edges of a block. Really a lot of work.
The solution, what I proposed on my sketch, is giving you more freedom, you can use sweeping techniques (Extrude3D in salome) which not necessarily produce structured mesh, and not necessarily produces full hex mesh (it can, but sometimes some wedges will be also generated), but it definitely will produce tetra free mesh. And with less work, and giving more freedom to change the local mesh density.

FKM: yes, that is what the referenced paper about. You can check it also here for example: vdmashop.de/Research--FKM-/

BR,
dezsit

Offline

#9 2019-10-31 12:17:30

marcelo
Member
From: Brazil
Registered: 2017-06-20
Posts: 79

Re: Error generating mesh

Hello,

Got it,

I am progressing slowly, but progressing. Is there a definition of which hex or tetra mesh are best suited for this type of study? I once read that the Finite Element Method works best with tetra meshes.

By the way, do you have a simple case that performed fatigue analysis? Using Code_Aster ... if you can share the example, I'd be very grateful.

dezsit wrote:

FKM: yes, that is what the referenced paper about. You can check it also here for example: vdmashop.de/Research--FKM-/

Thanks!

Best.

Offline

#10 2019-11-04 22:02:26

dezsit
Member
Registered: 2012-06-27
Posts: 69
Website

Re: Error generating mesh

Hello,

Generally, hex outperforms tetra in mechanics (better mesh convergence with less elements), especially if bending involved. But in some cases hex suffers from various problems (volumetric locking, hourglassing, etc, depending on the numerics behind a specific hex formalism (reduced integration, full integration but linear element, etc.), and how a specific fea package handles this kind of problems (eg. assumed strain as in case of aster) ), you should check the element reference manual of a software package, and do verifications! But sometimes the geometry does not allow to make good hex mesh (or simply the job not worth to spend too much time with mesh preparation) so tetra can be used, but only quadratic for mechanics, and again do verification and mesh convergence study.

Code_aster fatigue case: as I mentioned the fea part of fatigue is "simple" mechanics (statics, dynamics), not aster specific. We do the fatigue evaluation separately, independently from the fea package, so I cant provide an aster specific fatigue evaluation (knowing that aster has in-built fatigue evaluation tool, but we have not used it yet).

BR
dezsit

Last edited by dezsit (2019-11-04 22:22:28)

Offline

#11 2019-11-05 19:21:26

marcelo
Member
From: Brazil
Registered: 2017-06-20
Posts: 79

Re: Error generating mesh

dezsit wrote:

...but only quadratic for mechanics, and again do verification and mesh convergence study.

Interesting to mention this, as Salome allows the use of quadratic, bi-quadratic and linear mesh. However, I haven't studied it yet to know the difference in their use and what it really means.

dezsit wrote:

Code_aster fatigue case: as I mentioned the fea part of fatigue is "simple" mechanics (statics, dynamics), not aster specific. We do the fatigue evaluation separately, independently from the fea package, so I cant provide an aster specific fatigue evaluation (knowing that aster has in-built fatigue evaluation tool, but we have not used it yet).

Yes, you had commented and I kept your words. What happened was my failure to believe that perhaps for some reason you had already done a similar analysis using Aster_Study.

Thank you for your teachings.

Offline