Stresses higher than yield in post-processing

Caster

Bonjour

I have a question about stresses higher than yield in post-processing. I use ParaView.

Most of the time my models consist of shells and they are either DKT or COQUE_3D elements. My analyses are nonlinear, material is mostly bilinear elastic-perfectly plastic, I use TRACTION in material definition and VMIS_ISOT_TRAC in STAT_NON_LINE. Analysis runs fine and the results make sense.

But I get stresses much higher than set yield limit in ParaView when using PROJ_CHAMP to project the TRI7 or QUAD9 mesh into corresponding linear mesh. See attached picture about what I mean. Stresses in the picture are shell's top-level stresses, I always save all three layers in my .rmed files.

Is there any way to reduce these stresses in post-processing? They are obviously not real stresses but in the attached picture stresses are much higher than set yield limit 355 MPa in a very large area. So even checking stresses a node or two away from the highest peak is still not enough. I understand that these projected stresses are ELNO - fields so there is always being more or less error compared to ELGA - fields.

Please find attached the full command file. It is a test model and I copied several parts from my other models so it might be a little bit cluttered.

I just created this account for the first time, have been reading the forums for some months. Feel free to ask any questions.

Merci d’avance !

stage-1.txt

8kB

jeanpierreaubry

Caster
just one question

why should it be less than yield limit ?

Caster

jeanpierreaubry

Not less but in theory it should be limited to 355 MPa if that is set as a yield limit for perfectly-plastic material. In integration points it shouldn't go over that set limit at all, but I have noticed that sometimes it goes slightly over that even for SIEQ_ELGA - values. But these higher than yield SIEQ_ELGA - values only appear at intersections of shells which I think doesn't contain very meaningful information anyway, I always check a node or two away from those. For this particular example I artificially selected a very thin plate, with realistic plate thickness stresses are much more reasonable. And obviously extrapolation of stresses from integration points to nodes gives error. I have noticed that with DKT there is less discrepancy, I guess I have to get myself more familiar with the formulation of COQUE_3D to better understand it.

AsterO'dactyle

Hello,

Which projection method do you use in PROJ_CHAMP? For ‘ELGA’ fields, the best option is “ECLA_PG”. Transferring ‘ELGA’ fields is a difficult problem.

Caster

AsterO'dactyle

I have opted for only projecting nodal values with PROJ_CHAMP. Very likely that I have had issues when trying to project ELGA - fields when using COQUE_3D. Below example of how I have sometimes extracted maximum/minimum stresses, fields are calculated with CALC_CHAMP.

IMPR_RESU(FORMAT='RESULTAT',
RESU=_F(CARA_ELEM=elemprop,
MAILLAGE=mesh,
NOM_CHAM=('SIEQ_ELGA', ),
NOM_CMP=('VMIS', ),
RESULTAT=resnonl,
VALE_MAX='OUI',
VALE_MIN='OUI'),
UNITE=2)

Below a typical POST_CHAMP - function which I use when dealing with COQUE_3D and DEFORMATION=GROT_GDEP, since results look weird in ParaView with TRI7/QUAD9 mesh. For DKT I usually use linear mesh so there is no need to project really.

sup = POST_CHAMP(EXTR_COQUE=_F(NIVE_COUCHE='SUP',
NOM_CHAM=('SIEQ_ELNO', 'EPEQ_ELNO'),
NUME_COUCHE=1),
RESULTAT=resnonl)

But thank you for mentioning that ECLA_PG, I can do some searching myself how to possibly utilize that. I'm quite novice in manipulating different fields and due to that I posted my original question as well, that perhaps there is a better way to project fields to post-processing.

Sound_Spinning

Caster
Your material features a flat line on NL part? VALE=(0.00169, 355.0, 0.05, 355.0)
Doesn't that mean zero stiffness, and therefore hassles for solvers?
Also, your peak stress levels in pic are at singularity areas, sharp corners, no fillets?

Caster

Sound_Spinning

I changed the material to have a small slope on the plastic part, but it doesn't make a difference, still there is a large area going over 355 MPa, not only the sharp corner nodes (picture attached). So the problem is not the material behaviour law.

Peak stresses are fine since I'm not interested in those corners, this is a global behaviour study of a larger structure. But stresses get gradually lower, at hole edges they are only 20 % more than yield limit, which I think is not unusual amount of difference when extrapolating the stresses from intregration points to nodes.

Obviously if this was a study about fatigue I would need to model the details accurately and have more refined mesh. With 3D modelling I have never noticed any issues with stresses going over the set yield limit at integration points, they always stop precisely at the set limit. For shells even the ELGA - fields sometimes go 10 - 20 % over the yield, which I thought wasn't programmatically possible due to it being a hard limit.

vishwas

I also encountered this issue. With all 3d elements and VMIS_ISOT_TRAC. Code aster coding is going downhill.

Caster

vishwas

Do you mean you have encountered this issue in "pure" solid continuum modelling (MODELISATION=3D) or using COQUE_3D? I haven't had this issue with ELGA - fields in MODELISATION=3D, but bear in mind my 3D models have been simple test models.

tpa

vishwas
That was an undocumented and unfair remark.

tpa

With shells in bending it might relate to how conditions are integrated across thickness ? Try to select a different COQUE_NCOU:

8.3.5 Operand COQUE_NCOU
◊ COQUE_NCOU = / N (1), [entirety, defect]
It is amongst layers used for integration in the thickness the hull. The number of layers also
determines the number of under-points of the stress field: 2 n+1 .
Into non-linear, it is necessary to use more than one layer to correctly integrate the constraints in the
thickness, cf. [U2.02.01].

Caster

tpa

I did a few test runs, explained in the pictures attached. Stresses plotted are ELNO - fields. Loading is exactly the same for all cases.

Leftmost picture I used default amount of integration points through thickness (1 mid, 1 inf, 1 sup), as you can see stresses higher than yield are very widespread.

In the second picture I used two extra integration points, but only in the plate. Results are much better, but still there are stresses higher than yield in quite a few nodes, not just only at sharp corners or around the hole edges.

Third picture I got great results by also giving the connected parts two extra integration points. Now the stresses higher than yield are only at the sharp corner nodes an hole edges near these sharp corners.

I knew this feature existed but I never thought it could have this much of effect so I kind of forgot about it. Many thanks for pointing this out!

vishwas

Hi,
I dont understand what do you mean by undocumented and unfair?
In lots of testcases and rmed files created, I definitely found once SIEQ_NOEU for VMIS exceeded the VMIS_ISOT_TRAC limit at nodal values maybe due to back projection algorithms(least square I guess). I did not check for ELGA. I highlighted this issue to people at simvia too.

tpa

Caster I think one has to consider how many points are necessary across thickness to realistically describe the parts which yield and the parts which are below the yield criterion. Further to that I think that for initially plane geometries the problem may be equally well modeled by DST/DKT and maybe a finer mesh in the critical areas. With these modelisations you avoid the middle node and thereby the result projection.
Regarding the values of VonM ... beside the extrapolation aspects mentioned above about it may also be worth checking the principal stresses and check the documentation for the plasticity to see if the stress/strain curve is assumed symmetric or not (i.e. similar behavior in compression and tension).

I really have no experience in elasto-plastic analysis using shell element, so don't trust me, but feel free to be inspired 🙂.

Sound_Spinning

Caster
When I reviewed shells in CA I found out that the drill stiffness value is hard-wired, regardless of units. Did you look into that, if it affects the results? I did a post on the subject on a test model, a bit dangerous that is:
https://forum.code-aster.org/public/d/30049-shells-with-tied-contacts-over-constrain-the-body-rotational-dof

Caster

tpa

I would use DKT but it is not compatible with GROT_GDEP. I model almost explicitly thin-walled steel structures in Code_Aster and it doesn't make sense to consider plasticity only and not large displacements and rotations, since usually in these kind of structures loss of stability is governing, usually well before structure yields anywhere. So that is the reason DKT is pretty much out of the question for me. I think for VMIS_ISOT_TRAC the stress-strain curve must be symmetric, due to the theory of Von Mises yield criterion. Or I must have slept through all of my materials classes if this is not the case 🙂

Sound_Spinning

I have done some testing previously alternating this coefficient. I always thought it was unitless and it doesn't matter which unit system you use. If I read the tables correctly which you linked, there was up to 5 % difference in MOMENT_Y when using 1e-05 and 1e-09? I have always used the default value 1e-05, sometimes I have tried maybe 1e-03, 1e-04, 1e-06... but nothing like four orders of magnitude apart. I guess depending on the application 5 % is not drastically large difference, but obviously it is not entirely negligible either. And the smaller the value is, you should be on a safe side since there is less arbitrary stiffness in your model, at least this is my understanding.

AsterO'dactyle

You are correct. For COQUE_3D it is convenient to project nodal values to linear mesh for post-processing purposes. There is always going to be "error" compared to stresses at Gauss points. My initial question arised since I have also noticed that stress values at ELGA - fields go higher than yield, even though the material is elastic-perfectly plastic. I haven't been able to visualize ELGA - fields for COQUE_3D meshes, I know how to do it for DKT though. So it is difficult to troubleshoot are these higher than yield ELGA-stresses only artefacts at sharp corners and junctions. Printing maximum values to .txt file doesn't give you that information, or at least not easily, since you would need to check are these maximum stresses in a "realistic" place or in sharp corners / junctions where "non-sensible" results are expected.

AsterO'dactyle

Hello,

This is not a bug; it is entirely normal.
Stresses for finite elements formulated in terms of displacement are evaluated at the numerical quadrature points (ELGA). Therefore, examining the stresses at the nodes necessarily involves extrapolation followed by averaging at the nodes, resulting in an inaccurate equivalent von Mises stress value. This error will tend towards zero as the mesh is refined.

This is a well-known phenomenon and is a fairly basic principle. All codes produce these effects. It is, in fact, a very well-known error indicator, one of the first to be published, by Zhu and Zienkiewicz in 1987.