Coque3D / von Mises

Hello.

I am modelling using exclusively Coque3D elements and I would like a presentation of the von Mises reference stress.

The only thing that seems to work for me seems to be the SIEF_ELGA_DEPL which gives the stresses/shears in the global coordinate system.

CoqSolu=CALC_ELEM(reuse =CoqSolu,
RESULTAT=CoqSolu,
OPTION=('SIEF_ELGA_DEPL',),);

I am not entirely sure what this CALC_ELEM should actually request calculated to obtain the von Mises. Can anyone help me, please.

Further I have generated the triangular elements using Salomé 2nd order triangles and have Aster calculate new elements of type TRIA7 using the TRIA6_7 option of CREA_MAILLAGE. Will Salomé be able to postprocess the output from the TRIA7?

Thanks for your responses.

Hi Kees Wouters. Thank you very much for your input. After some additional reading of your contributions I have found much inspiration here: www.caelinux.org/wiki/index.php/Contrib:KeesWouters/stress_2D3D .

Calculation of von Mises stresses is very well done with the CALC_ELEM command and output can be listed by writing output to the list output file but not be written to a MED file.

Up to now I was not aware of possibility of using the CALC_NO command to transform the "element output" structure to a "node output" structure. Both commands are needed. First the CALC_ELEM and then the CALC_NO.

U4.81.02 - Opérateur CALC_NO says it very clearly on the front page: Enrichir une structure de données resultat par des options de post-traitement. Il s'agit notamment des options forces nodales, réactions d’appui et plus généralement toutes les options de grandeurs élémentaires aux nœuds (options xxxx_NOEU_xxxx) transformant un cham_elem aux nœuds en un chamno.


My working Aster command file is:

[code:1]DEBUT();

Coque6=LIRE_MAILLAGE(UNITE=20,
FORMAT='MED',);

Coque7=CREA_MAILLAGE(MAILLAGE=Coque6,
MODI_MAILLE=_F(TOUT='OUI',
OPTION='TRIA6_7',),);

Coq7Mod=AFFE_MODELE(MAILLAGE=Coque7,
AFFE=_F(TOUT='OUI',
PHENOMENE='MECANIQUE',
MODELISATION='COQUE_3D',),);

Steel=DEFI_MATERIAU(ELAS=_F(E=210000000000.0,
NU=0.28,),);

CoqMat=AFFE_MATERIAU(MAILLAGE=Coque7,
MODELE=Coq7Mod,
AFFE=_F(TOUT='OUI',
MATER=Steel,),);

CoqCara=AFFE_CARA_ELEM(MODELE=Coq7Mod,
COQUE=_F(GROUP_MA='GR_1_Fac',
EPAIS=10.0,),);

CoqMeca=AFFE_CHAR_MECA(MODELE=Coq7Mod,
DDL_IMPO=(_F(GROUP_NO='Edge_19',
LIAISON='ENCASTRE',),
_F(GROUP_NO='Edge_20',
LIAISON='ENCASTRE',),
_F(GROUP_NO='Edge_21',
LIAISON='ENCASTRE',),
_F(GROUP_NO='Face_1',
DZ=0.0,),),
FORCE_NODALE=_F(GROUP_NO='Vertex_12',
FY=-19452.0,),);

CoqSolu=MECA_STATIQUE(MODELE=Coq7Mod,
CHAM_MATER=CoqMat,
CARA_ELEM=CoqCara,
EXCIT=_F(CHARGE=CoqMeca,),
OPTION='SANS',);

CoqSolu=CALC_ELEM(reuse =CoqSolu,
MODELE=Coq7Mod,
RESULTAT=CoqSolu,
OPTION=('SIGM_ELNO_DEPL','EQUI_ELNO_SIGM',),);

CoqSolu=CALC_NO(reuse =CoqSolu,
RESULTAT=CoqSolu,
OPTION=('SIGM_NOEU_DEPL','EQUI_NOEU_SIGM',),);

IMPR_RESU(MODELE=Coq7Mod,
FORMAT='MED',
UNITE=80,
RESU=_F(RESULTAT=CoqSolu,
TOUT_CHAM='OUI',
TOUT='OUI',),);

FIN(FORMAT_HDF='OUI',);[/code:1]
Thanks again, Kees Wouters, for the great help.<br /><br />Post edited by: Torben, at: 2010/11/03 23:03