Atom topic feed | site map | contact | login | Protection des données personnelles | Powered by FluxBB | réalisation artaban

You are not logged in.

- Topics: Active | Unanswered

**astercode****Member**- Registered: 2019-06-15
- Posts: 29

Hi everyone,

I have modeled a simple plate with quadrilateral shell elements of DKT type (5x5 quads).

I have set the thickness (EPAIS) and the orientation vector (VECTEUR).

Then I constrained the nodes on the left side and applied a nodal force

on the nodes on the right side.

Here are some lines from the .comm file (I have skipped unnecessary lines and focused on the keywords):

CALC_CHAMP -> CONTRAINTE=('SIEF_ELNO', 'SIGM_ELNO', 'SIGM_ELGA')

bottom results: POST_CHAMP(EXTR_COQUE=_F(NIVE_COUCHE='INF', NOM_CHAM=('SIGM_ELNO', 'SIGM_ELGA'), NUME_COUCHE=1)

CALC_CHAMP(CRITERES=('SIEQ_ELNO', 'SIEQ_NOEU')

tpp results: POST_CHAMP(EXTR_COQUE=_F(NIVE_COUCHE='SUP', NOM_CHAM=('SIGM_ELNO', 'SIGM_ELGA'), NUME_COUCHE=1)

CALC_CHAMP(CRITERES=('SIEQ_ELNO', 'SIEQ_NOEU')

IMPR_RESU(NOM_CHAM=('SIEQ_NOEU', ), NOM_CMP=('VMIS', )...)

Then I loaded the results in Paravis.

I repeated the same analysis with a commercial solver with exactly the same mesh/boundary conditions/etc.

The displacements are very close with Code Aster with a difference < 0.5 mm.

But the Von Mises stresses in Paravis and Gmsh are almost twice as high.

E.g. the commercial solver gives ~160 MPa while Code Aster gives ~220 Mpa.

What causes this big difference? Any help would be appreciated.

Offline

**jeanpierreaubry****Guru**- From: nantes (france)
- Registered: 2009-03-12
- Posts: 3,638

hello

it would be nice to have the full command file and maybe the mesh

as a few [common] mistakes may be hidden in the non submitted part

nevertheless it is a good idea to make an IMPR_RESU with ASCII values and VALE_MIN and VALE_Max to check out the calculations

as a few other [common] mistakes may be in the handling of Paravis or Gmsh

the above procedure is a must in my own opinion as it is pretty easy to get a post pro viewer to show on the screen values with strange relation to the calculated ones

jean pierre aubry

consider reading my book

freely available here https://framabook.org/beginning-with-code_aster/

Offline

**astercode****Member**- Registered: 2019-06-15
- Posts: 29

Hi Jean-Pierre,

thanks for your prompt reply!

Indeed this is a "must" before anything else.

Please check the attached mesh & command file.

With a commercial version of Nastran with CQUAD4, SPC1, FORCE, I get the following results:

displacement = 0.759 mm

vmis top = vmis bottom = 166 MPa

With code aster I get the following results:

displacement = 0.738 mm

vmis top = vmis bottom = 224 MPa

Also the results of code aster in the ASCII file that I output, agree with the results I see in Paravis.

Any idea what causes this difference?

*Last edited by astercode (2019-10-07 20:46:28)*

Offline

**astercode****Member**- Registered: 2019-06-15
- Posts: 29

Attaching the command file also.

Offline

**AsterO'dactyle****Administrator**- Registered: 2007-11-29
- Posts: 312

Check HOW the von Mises stress is evaluated by other software.

Real stresses are at integration points (SIEQ_ELGA in code_aster), not at nodes.

Code_Asterの開発者

Offline

**astercode****Member**- Registered: 2019-06-15
- Posts: 29

From the command file and the mesh, do you confirm that the above calculation is correct?

Or is there an error in model setup?

Offline

**jeanpierreaubry****Guru**- From: nantes (france)
- Registered: 2009-03-12
- Posts: 3,638

Compound_Mesh_1.sauv is not a .med mesh file

i cannot open it

is it CASTEM2000 ?

consider reading my book

freely available here https://framabook.org/beginning-with-code_aster/

Offline

**astercode****Member**- Registered: 2019-06-15
- Posts: 29

I tested it in Salome-Meca. You can import it in Mesh Module.

The distribution used is available at code-aster-windows dot com

Offline

**jeanpierreaubry****Guru**- From: nantes (france)
- Registered: 2009-03-12
- Posts: 3,638

i use code_aster stand alone v 14.2 linux version

this is the output of the .mess file

if i open the file with a text editor i can see this is surely not a .med file

```
# ------------------------------------------------------------------------------------------
# Commands No: 0002 Concept of the type: maillage_sdaster
# ------------------------------------------------------------------------------------------
mesh = LIRE_MAILLAGE(FORMAT='MED',
UNITE=20,
INFO_MED=1,
INFO=1,
VERI_MAIL=_F(APLAT=1.E-3,
VERIF='OUI',),
)
!-----------------------------------------------------------------!
! <A> <MODELISA9_44> !
! !
! fichier MED : fort.20 maillage : erreur numéro -1 !
! !
! !
! This is a warning. If you do not understand the meaning of this !
! warning, you can obtain unexpected results! !
!-----------------------------------------------------------------!
!-------------------------------------------------------------------------------!
! <EXCEPTION> <PREPOST3_10> !
! !
! either the file does not exist, or it is a bad version of HDF (uses by MED). !
!-------------------------------------------------------------------------------!
```

consider reading my book

freely available here https://framabook.org/beginning-with-code_aster/

Offline

**Volker****Member**- From: Chemnitz
- Registered: 2016-05-23
- Posts: 76

Hi astercode,

have you already compared your numerical solutions with the analytical solution?

A numerical solution is a good start point to investigate commercial and open source software.

Kind regards and good luck Volker

Offline

**astercode****Member**- Registered: 2019-06-15
- Posts: 29

Since the plate is subjected to pure tension, according to the analytical solution:

sigma = F/A

F ~= 600000 Nt

A = 1000 x 5 = 5000 mm^2

so sigma = 120 MPa.

So I should get something close to that (Nastran gives 166MPa), while I get 224 MPa in CodeAster/Paravis.

Here is the Med file (MED version 3.3.1)

Offline

**jeanpierreaubry****Guru**- From: nantes (france)
- Registered: 2009-03-12
- Posts: 3,638

Since the plate is subjected to pure tension, according to the analytical solution:

sigma = F/A

F ~= 600000 Nt

A = 1000 x 5 = 5000 mm^2

so sigma = 120 MPa.

this is only true far away from the boundary conditions

the mesh is quite coarse and

the constrs boundary condition with full "encastre"

lead to a high stress concentration at the corners

*Last edited by jeanpierreaubry (2019-10-09 06:58:56)*

consider reading my book

freely available here https://framabook.org/beginning-with-code_aster/

Offline

**Volker****Member**- From: Chemnitz
- Registered: 2016-05-23
- Posts: 76

Hi Astercode, I compared the results and my conclusion is both numerical solutions are wrong.

What happens if you only set DX of 'NODES_CONSTR' = 0 and an absolutely unimportant node gets the rest (DY, DZ, DRX, DXY, DRZ =0)??

Volker

Offline

**astercode****Member**- Registered: 2019-06-15
- Posts: 29

Hi all,

I read very carefully your replies, because this is very important for me.

I wonder why Nastran gives quite lower stresses for the same mesh

and boundary conditions and everything.

Displacements, Stresses on beams, Reaction Forces in general agree

between Nastran & Code Aster, but stresses on shells really go very high.

I wonder if I have done something wrong in the *.comm file.

Could you please elaborate more on how to get correct results on this case?

Thanks a lot again!

Offline

**Volker****Member**- From: Chemnitz
- Registered: 2016-05-23
- Posts: 76

Hi Astercode,

again, both numerical calculations are wrong (also Nastran). Change the boundary conditions in both systems that you get 120 MPa in both numerical calculations Aster and Nastran. This is very important. Your boundary condition produces a singularity. The correct result should be infinitely in Aster and Nastran !!! ...

Kind regards and good luck Volker

Offline

**astercode****Member**- Registered: 2019-06-15
- Posts: 29

Hi Volker, Jean,

tried the solution suggested:

"What happens if you only set DX of 'NODES_CONSTR' = 0 and an absolutely unimportant node gets the rest (DY, DZ, DRX, DXY, DRZ =0)??"

but nothing changed. I left only DX = 0 to NODES_CONSTR and added an unimportant node with DY, DZ, DRX, DRY, DRZ = 0.

Still Nastran gives ~166 MPa and Code Aster gives ~224 MPa.

Any idea?

Offline

Hi,

could you post two pictures about your results (with legend and mesh)? One for the nastran, one for aster. Depending on your post processing options in nastran, and used post-processor software setup, nastran can show you eg element centroid results, which can be much smaller (especially around BCs with large element size) than the extrapolated (and averaged) nodal ones , what (I suppose) you use from aster (_NOEU).

Just to emphasize AsterO'dactyle's post about the comparison of the right values.

BR,

dezsit

Offline

**jeanpierreaubry****Guru**- From: nantes (france)
- Registered: 2009-03-12
- Posts: 3,638

@astercode

can you contact me by email

consider reading my book

freely available here https://framabook.org/beginning-with-code_aster/

Offline

Ok, as you can see on the nastran_vmises_centroid, the nastran reports 166[MPa?], as element centroid value, and actually the same on the nastran_vmises_averaged. Why: because in this case the element centroid values are simply copied to the nodes, then averaged, but at the corner node there is no other node than one, so it simply gets the element centroid value!

In case of aster SIEQ_NOEU, the values from gauss points are extrapolated (so depending on the results, they can become higher at the nodes than at the gauss points) to element nodes (_ELNO). Then they are averaged to _NOEU. So in case of the corner nodes the high value (224.2) is an extrapolated value from the GP. (as far as I remember the nastran centroid is the average of the element GP results). You try to compare wrong values.

You have to change your nastran setup (POST and STRESS in the case section) to print out the element corner (element nodal) values, than your post processor will average them, or compare the GP values, or element nodal values, etc.

An other thing, which was emphasized on this forum many times: you should not evaluate stresses at BCs, they are meaning less, especially the averaged nodal values. The element centroid or GP results can have meaning, depending on your problem.

BR,

dezsit

*Last edited by dezsit (2019-10-10 08:04:44)*

Offline

**astercode****Member**- Registered: 2019-06-15
- Posts: 29

Hi dezsit,

your reply is very very clear. Thank you for this clarification. I will check it in detail.

I have some further questions:

1. Is it possible in CodeAster/Paravis to get the same method as with Nastran?

i.e.

a. get values at element centroids?

b. use these values to copy to nodes, then average?

c. If I use SIGM_ELGA can I view the results in Paravis?

2. THe SIGM is enough to get the stress tensor?

Thank you all for your guidance and help!

Offline

Hi,

First, you should print out your SIEQ_ELGA results to the med file.

Then in Salome9.2,3 we have a new filter: Filter->Mechanics->ELGA field to Surface (cell averaged),

and you should see something like on the attached picture, which is already quite close to the nastran results, except around the fixed BC. I think this is an answer to your a,b,c points . If you use older Salome version, then without this filter, it is more complicated I think.

SIGM (or others eg, SIEF, etc.) can have different meaning, depending your modelisation, check the manuals U2.01.04/05) but in your case SIGM is ok.

BR

dezsit

Offline

**Volker****Member**- From: Chemnitz
- Registered: 2016-05-23
- Posts: 76

Hi Astercode,

I tested my suggestion and now I get exactly the same result as in the analytical calculation with Sigma = 120 MPa .

Have you already achieved the same in Nastran?

I attach my .comm file for comparing. Kind regards Volker

Offline

**Volker****Member**- From: Chemnitz
- Registered: 2016-05-23
- Posts: 76

here is the .comm file:

Offline

**astercode****Member**- Registered: 2019-06-15
- Posts: 29

@dezsit: I have output the SIEQ_ELGA and read in Salome 9.3.0 and they agree indeed with Nastran and are about ~166 MPa. So for the Gauss points at least we get the same results. The nodal averaging differs but ok, I understand well that this is also affected by the boundary conditions, density of mesh, etc.

@volker: I tried your comm file and indeed by using DX=0 and all the rest (except RZ) on one node, this gives the expected results i.e. 120 MPa. However I had done this already. What made difference this time was the LIAISON_UNIF to uniformly move the edge. Also compared the results in Paravis and again they agree with Nastran (using RBE2 also there).

Thank you all for contributing your knowledge on this important subject.

Offline