Field ex: SIEF_NOEU calculation error. It requests for Post_champ

denizckr35

Hello everyone, I am using the windows 2024 version of Salome-Meca.

I am doing non-linear shell plate analysis.
When I start calculation without the results it calculates without any problem.

However when i try with CALC_CHAMP below it request POST_CHAMP.

╔════════════════════════════════════════════════════════════════════════════════════════════════╗
║ <A> <UTILITAI_3> ║
║ ║
║ La conversion d'un champ par éléments aux noeuds en un champ ║
║ aux noeuds a été demandé. ║
║ Or le ║
║ champ par éléments aux noeuds contient des ║
║ sous-points alors qu'un champ aux noeuds ne peut ║
║ pas en contenir. ║
║ Les mailles contenant des sous-points vont être exclues. ║
║ ║
║ Conseil : ║
║ Si ║
║ vous souhaitez convertir le champ sur les mailles ayant des ║
║ sous-points, vous devez d'abord ║
║ extraire le champ par éléments ║
║ aux noeuds sur un sous-point avec la commande POST_CHAMP. ║
║ ║
║ ║
║ Ceci est une alarme. Si vous ne comprenez pas le sens de cette ║
║ alarme, vous pouvez obtenir des ║
║ résultats inattendus ! ║
╚════════════════════════════════════════════════════════════════════════════════════════════════╝

╔════════════════════════════════════════════════════════════════════════════════════════════════╗
║ <EXCEPTION> <CALCULEL4_16> ║
║ ║
║ Erreur d'utilisation : ║
║ L'option SIEF_ELNO est nécessaire pour le calcul de l'option ║
║ SIEF_NOEU. ║
║ Or SIEF_ELNO est un champ qui ne contient que des sous-points, ce cas n'est pas ║
║ traité. ║
║ Vous devez d'abord extraire SIEF_ELNO sur un sous-point avec la commande ║
║ POST_CHAMP.

My CALC_CHAMP file is this.

message.txt

49kB

resnonl = CALC_CHAMP(
CONTRAINTE=('SIEF_ELNO', 'SIGM_ELNO', 'SIGM_ELGA', 'SIEF_NOEU'),
CRITERES=('SIEQ_ELGA', 'SIEQ_ELNO'),
DEFORMATION=('EPSI_ELGA', 'EPSI_ELNO'),
RESULTAT=resnonl
)

Setup file : https://drive.google.com/file/d/17l3ktdnaAlERyJyVL1aosDclfOOk0KNF/view?usp=sharing

2- My second question is when i try to visualize the displacement fields they are fine but when it comes to stress field for example Von mises stresses it does not showing in good graphical way.

I did ELNOtoFieldToSurface command in paraview and it gives me this kind chainy image

It is not smooth looking. How can I solve this?

tpa

Which kind of element (modelisation) do you use ? Coque3d was - and probably still is - a bit special.
If the plate is as flat as it appears you coukd consider dkt/dst element in a trianguler mesh.

denizckr35

tpa I already used DKT element with quadrangular mesh in my simulation. It is a shell ellement for face geometry. Also for triangular mesh result is the same.
I checked the total displacement and it is accurate in terms of result but idk how to display results in a smooth way also need to caclulate SIEF_NOEU

tpa

Plate and shell elements store results in several layers. Bottom (Inf), middle (moy) and top (sup). To display coherent data you need to postprocess the result fields (POST_CHAMP) extract the field for the specific layer separately (EXTR_COQUE) See https://code-aster.org/doc/default/en/man_u/u4/u4.81.05.pdf
It may look something like this:

reslin = MECA_STATIQUE(...)
ResInf = POST_CHAMP( ... ,
                    EXTR_COQUE=_F(NIVE_COUCHE='INF',
                                  NOM_CHAM=('SIEF_ELGA', ),
                                  NUME_COUCHE=1),
                    RESULTAT=reslin)
ResInf = CALC_CHAMP( ... ,
                    reuse=ResInf,
                    CRITERES=('SIEQ_NOEU', ),
                    RESULTAT=ResInf)

and remember to save the results ResInf as well to the output file.