Atom topic feed | site map | contact | login | Protection des données personnelles | Powered by FluxBB | réalisation artaban
You are not logged in.
Pages: 1
Hi All,
I am new here (and to Salome-Meca/Code_Aster). My intentions are to use the package for detailed FE calculations of tubular joints with regards to stress concentration factors used for fatigue life assessment.
Currently I am trying to determine how to evaluate the stresses in the quadratic shell elements (Coque_3D), as this is essential to my task at hand.
My starting point is the simple tutorial found here; a simply supported plate of dimensions 1.000x1.000x0.001m. The model is meshed with quad8 elements.
My command file can be seen below. This enables me to plot/preview deformations, but not stresses. I have tried various approaches, from different tutorials or examples found on the web (e.g. here), but none have worked so far.
I am using Salome-Meca 2013.2 with Code_Aster 11.4 (The newest package downloadable from www.code-aster.org).
My question/plea is then if anyone has any constructive input to the approach I need to take ?
DEBUT();
th = 0.001;
steel=DEFI_MATERIAU(ELAS=_F(E=2.100e11,
NU=0.30,
RHO=7850,),);
initMesh=LIRE_MAILLAGE(FORMAT='MED',
INFO=1,);
cocMesh=CREA_MAILLAGE(MAILLAGE=initMesh,
MODI_MAILLE=_F(TOUT='OUI',
OPTION='QUAD8_9',),);
intModel=AFFE_MODELE(MAILLAGE=initMesh,
AFFE=_F(TOUT='OUI',
PHENOMENE='MECANIQUE',
MODELISATION='3D',),);
cocModel=AFFE_MODELE(MAILLAGE=cocMesh,
AFFE=_F(TOUT='OUI',
PHENOMENE='MECANIQUE',
MODELISATION='COQUE_3D',),);
shellch=AFFE_CARA_ELEM(MODELE=cocModel,
COQUE=_F(GROUP_MA='shell',
EPAIS=th,
VECTEUR=(1,0,0,),
COQUE_NCOU=1,),);
material=AFFE_MATERIAU(MAILLAGE=cocMesh,
AFFE=_F(TOUT='OUI',
MATER=steel,),);
Load=AFFE_CHAR_MECA(MODELE=cocModel,
DDL_IMPO=(_F(GROUP_MA='Linex0',
DX=0,
DZ=0,),
_F(GROUP_MA='Liney0',
DY=0,
DZ=0,),
_F(GROUP_MA='Linex1',
DZ=0,),
_F(GROUP_MA='Liney1',
DZ=0,),),
PRES_REP=_F(GROUP_MA='shell',
PRES=-1000,),);
RESU=MECA_STATIQUE(MODELE=cocModel,
CHAM_MATER=material,
CARA_ELEM=shellch,
EXCIT=_F(CHARGE=Load,),
OPTION='SIEF_ELGA',);
RESU=CALC_CHAMP(reuse =RESU,
RESULTAT=RESU,
TOUT='OUI',
CONTRAINTE=('SIGM_ELGA','SIGM_ELNO',),);
proj_res=PROJ_CHAMP(PROJECTION='OUI',
RESULTAT=RESU,
MODELE_1=cocModel,
MODELE_2=intModel,);
IMPR_RESU(FORMAT='MED',
RESU=_F(RESULTAT=proj_res,),);
FIN();
Offline
hello
with a pressure stresses in the neutral fiber are null
this adds calculation for the top face
RESU=CALC_CHAMP(
...................
);
#on the top face
resu2=POST_CHAMP(
RESULTAT=RESU,
EXTR_COQUE=_F(
NUME_COUCHE=1,
NIVE_COUCHE='SUP',
NOM_CHAM=('SIGM_ELNO',),
),
);
#invariants
resusup=CALC_CHAMP(
RESULTAT=resu2,
CRITERES=('SIEQ_ELNO','SIEQ_NOEU',),
);
jean pierre aubry
consider reading my book
freely available here https://framabook.org/beginning-with-code_aster/
Offline
Hoi
that example is for pre C-A11.4.
These may be used with C-A11.X, depending on what postprocessor you like [postpro or paravis]:
http://www.caelinux.org/wiki/index.php/ … /plotcoq3d
or
http://www.caelinux.org/wiki/index.php/ … q3dparavis
Last edited by keeswouters (2013-10-21 20:15:11)
kind regards - kees
--
I a parallel univers the laws of mechanics may be different.
Offline
Attached some file that can help you.
Ciao
Jacopo
Salome-Meca 2017.02 (Intel Xeon 8 Core x 2 RAM 32GiB) Ubuntu 16.04 LTS
Offline
Thank you all for the helpful replies, they are muchly appreciated!
@keetwouters:
I have used post-pro, but only because the first tutorial I tried used that, I have no preference as such...
I have tried to follow the example you set forth in http://www.caelinux.org/wiki/index.php/ /plotcoq3d, but generating the geometry through Salome-meca. I have furthermore disabled some of the more advanced functions (variable thickness, multiple load cases).
I am able to run the model and import the results into post-pro, but then for some reason, I am only able to plot the results on the edges (See attached: PostPro.png - Note how I have three groups on my mesh, the two edges for BCs, and then the shell, but in post pro only the two edge groups remain). I am not able to plot results onto the wireframe mesh, or onto the surface.
Any ideas what I may have done wrong, or why I experience this issue?
/BR
Anders
Last edited by anders82 (2013-10-22 09:05:00)
Offline
I figured it out. Due to my inexperience with the software, I didn't realize that I needed to specifiy result files for 81 and 82 as well.
Once again, thank you all for the input and help.
/BR
Anders
Offline
Hoi Anders
I figured it out. Due to my inexperience with the software, I didn't realize that I needed to specifiy result files for 81 and 82 as well.
That should be noticed by a copy error in the *.mess file.
Postpro is not available anymore in Salome7.X. So paraviz will be the future I presume.
kind regards - kees
--
I a parallel univers the laws of mechanics may be different.
Offline
Pages: 1