I confirm that in this way also the averages stresses on nodes agree.

Wonderful!

Congratulations to all of you for sharing so much!

Thanks

of course if the basis (GP results) are the same, then your averaged nodal values have to be the same (more or less, depending on your post processing software)

The problem is nastran specific, which uses element centroid for averaging by default, while other solvers (eg. ansys, abaqus and aster as well), using extrapolated element nodal results.

To achieve the same averaged results you have two options:

1) change your nastran setup (POST and STRESS case commands as far as I remember) to print out element nodal values and use these results in your postprocessing software for averaging

2) use the method mentioned above to create cell averaged GP results in paravis (= element centroid), then use Cell data to Point data filter to get averaged nodal values from that. It should be the same (more or less) as the ones on picture nastran_vmises_averaged

BR

dezsit

@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.

]]>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]]>

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

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!

]]>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

can you contact me by email

]]>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

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?

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]]>

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!

]]>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]]>