Atom topic feed | site map | contact | login | Protection des données personnelles | Powered by FluxBB | réalisation artaban

You are not logged in.

- Topics: Active | Unanswered

**AlbiBone****Member**- Registered: 2020-10-05
- Posts: 20

Hello,

I want to compute a linear static analysis on a sheet metal component made of steel (fix-force BC).

I decided to model it by using a shell (a 3D modelization is too heavy and not efficient).

I check both DKT modelization (using linear elements) and COCQUE_3D modelization (using bi-quadratic elements), but the simulation continue to fail.

In the mesh there are no double elements or double nodes. In attached the mesh image.

The error that I get is the following:

```
Sur les 21494 mailles du maillage mesh, on a demandé l'affectation de 17800, on a pu en affecter 0
!-------------------------------------------------------------------------!
! <EXCEPTION> <MODELE1_6> !
! !
! Aucune maille du maillage mesh n'a été affectée par des éléments finis. !
!-------------------------------------------------------------------------!
```

It seems that the AFFE_MODELLE is not able to assign the modelisation to the mesh, but I am not sure of this interpretation.

I have some dubt:

Is it correct to use a COCQUE_3D or a DKT for a sheet metal that is oriented on different planes (and curvature radius on the bending lines)?

What's wrong with the model? Have you some suggestion for solve the errors that I encourring?

I am using Salome Meca for Windows 2019. I don't think that using linux official release will solve it, since it is a very simple simulation.

Is it correct to use EXCENTREMENT for "offset" the average plane of the shell with rispect to the mesh plane?

I am not able to upload the entire .hdf model, so I simply attach here the input file.

```
mesh = LIRE_MAILLAGE(FORMAT='MED',
UNITE=2)
mdl_cck3 = AFFE_MODELE(AFFE=_F(GROUP_MA=('Group_surf', ),
MODELISATION=('COQUE_3D', ),
PHENOMENE='MECANIQUE'),
MAILLAGE=mesh)
elemprop = AFFE_CARA_ELEM(COQUE=_F(EPAIS=0.0015,
EXCENTREMENT=-0.00075,
GROUP_MA=('Group_surf', ),
INER_ROTA='OUI'),
MODELE=mdl_cck3)
AISI304 = DEFI_MATERIAU(ELAS=_F(E=190000000000.0,
NU=0.3))
fieldmat = AFFE_MATERIAU(AFFE=_F(MATER=(AISI304, ),
TOUT='OUI'),
MODELE=mdl_cck3)
BC_fix = AFFE_CHAR_MECA(DDL_IMPO=_F(GROUP_NO=('Group_fix', ),
LIAISON='ENCASTRE'),
MODELE=mdl_cck3)
BC_force = AFFE_CHAR_MECA(FORCE_NODALE=_F(FZ=-1.0,
GROUP_NO=('Group_force2', )),
MODELE=mdl_cck3)
reslin = MECA_STATIQUE(CARA_ELEM=elemprop,
CHAM_MATER=fieldmat,
EXCIT=(_F(CHARGE=BC_fix),
_F(CHARGE=BC_force)),
MODELE=mdl_cck3)
reslin = CALC_CHAMP(reuse=reslin,
CONTRAINTE=('SIGM_NOEU', ),
CRITERES=('SIEQ_NOEU', ),
FORCE=('FORC_NODA', 'REAC_NODA'),
RESULTAT=reslin)
#comment: unnamed1 = POST_CHAMP(EXTR_COQUE=_F(NIVE_COUCHE='SUP',
#comment: NOM_CHAM=('SIEQ_ELNO', ),
#comment: NUME_COUCHE=1),
#comment: RESULTAT=reslin)
IMPR_RESU(RESU=_F(RESULTAT=reslin,
TOUT_CHAM='OUI'),
UNITE=80)
```

Thank for the support,

A

*Last edited by AlbiBone (2021-08-26 10:31:18)*

Offline

**laurent****Member**- Registered: 2007-11-22
- Posts: 232

Hi

Could you specify a bit your environment for the CAE in Salome ?

In particular, the number associated to the MED file?

You have

mesh = LIRE_MAILLAGE(FORMAT='MED',

UNITE=2)

If the unit is wrong, it may be that the file is not read at all.

From very old files, i had something like

"

mesh = LIRE_MAILLAGE(identifier='0:1',

FORMAT='MED',

UNITE=20)

mesh = MODI_MAILLAGE(identifier='1:1',

reuse=mesh,

MAILLAGE=mesh,

ORIE_NORM_COQUE=_F(GROUP_MA=('Plate', 'Pipe', 'Chamfer')))

model = AFFE_MODELE(identifier='2:1',

AFFE=_F(MODELISATION=('DKT', ),

PHENOMENE='MECANIQUE',

TOUT='OUI'),

MAILLAGE=mesh) "

Reading of mesh, reorientation, then DKT affectaction.

Given that nothing was assigned in your case, it may be that the mesh file was not read at all.

You could post your CAE file directement, it shouldn't be too big seeing the picture of your mesh.

Regards

Offline

**AlbiBone****Member**- Registered: 2020-10-05
- Posts: 20

Hi Laurent, in attached the FEM model.

I fixed your suggestion about "unit" of the mesh.

However the model still does not work.

*Last edited by AlbiBone (2021-08-24 14:11:21)*

Offline

**ing.nicola****Member**- Registered: 2017-12-11
- Posts: 127

DTK needs quadratic mesh ( QUAD8 )

COQUE_3D needs bi-quadratic mesh ( QUAD9 ).

Salome can do this conversions .

Offline

**AlbiBone****Member**- Registered: 2020-10-05
- Posts: 20

Dear Ing Nicola, I agree with you about COQUE_3D needs bi-quadratic mesh, but I desagree about DTK: it need linear elements (see R3.07.03).

Now I updated the model with bi-quadratic + COQUE_3D, but still I get the following error, but I don't know what write in "ANGL_REP or VECTOR", since the COQUE_3D is on a surface curved with different orientations (see mesh image in the first post).

I attach also the updated FEM model.

```
!-------------------------------------------------------------------------------------------!
! <EXCEPTION> <ELEMENTS_40> !
! !
! - > the reference axis for the computation of the local coordinate system is normal with !
! at least a shell element. !
! - > Risks & !
! advices: !
! It is necessary to modify the reference axis (axis X by defect) by using !
! ANGL_REP or VECTOR. !
! !
! !
! -------------------------------------------- !
! Contexte du message : !
! Option : SIEF_ELGA !
! Type d'élément : MEC3TR7H !
! !
! Maillage : mesh2D !
! Maille : M3494 !
! Type de maille : TRIA7 !
! Cette maille appartient aux groupes de mailles !
! suivants : !
! Group_surf !
! Position du centre de gravité de la maille : !
! x=-0.247265 y=-0.068396 z=-0.019551 !
!-------------------------------------------------------------------------------------------!
```

Offline

**JanBlokes****Member**- From: Koprivnice
- Registered: 2018-09-06
- Posts: 13

Hello,

I think you need to add 'SIEQ_ELNO' before 'SIEQ_NOEU'. Check the book from Jean Pierre Aubry

Jan

Offline

**AsterO'dactyle****Administrator**- Registered: 2007-11-29
- Posts: 384

Hello,

The local reference frame of a plate element is defined by normaland (two) tangents.

The normal is defined by MODI_MAILLAGE/ORIE_COQUE.

The first tangent is, by default, the global X axis.

So, if the plate/shell element is orthogonal to X axis, tangent and normal are colinear. Not possible !

"It is necessary to modify the reference axis (axis X by defect) by using ANGL_REP or VECTOR"

(in AFFE_CARA_ELEM)

NB: SIEQ_ELNO is not necessary in CALC_CHAMP, it's automatic since at least 15 years.

Code_Asterの開発者

Offline

**AlbiBone****Member**- Registered: 2020-10-05
- Posts: 20

Thank you AsterO'dactyle for your suggestion.

It is clear to me that I need to act on ANGL_REP or VECTOR (inside AFFE_CARA_ELEM).

The problem is that my 2D mesh is oriented in many planes since the sheet metal has many bends (see the image of the geometry in the first post). Therefore the mesh belongs at the same time to many planes on XY, YZ, XZ (and also some inclined planes).

So I don't know which value to set on VECTOR.

*Last edited by AlbiBone (2021-08-25 16:01:35)*

Offline

**laurent****Member**- Registered: 2007-11-22
- Posts: 232

Hi

I might have been sloppy but there were discussions about ANGL_REP at some points,

there was a post "How to use angl_rep or vecteur and what they mean" in 2017, from GiuliaM_91 and an answer from Johannes_ACKVA (can not post link in the forums, but you should be able to find)

with

"The problem in your case: V was perpendicular on (at least) 1 surface element, so the projection could not be done. Perhaps you did not use

ANGL_REP nor VECTEUR. In such a case Code-Aster used the default ANGL_REP=(0,0,). Which means that V is the global X-axis. The projection fails then for elements being in the global Y-Z-plane.

The good thing: often you do not need the stresses to be output in a special local coord system. It can be in ANY local coord system. In this case simply change VECTEUR or ANGL_REP in the manner that they do not make the default (which caused your problem). Simply try anything, for example ANGL_REP=(0.11,0.22,).

Also good: The often needed van Mises stress does not depend on the local coord system because it is a tensor invariant of the stress tensor"

and the example

"# Spec of local CoordSys for stress calc in 2 different manners: ANGL_REP or VECTEUR

CarLocal=AFFE_CARA_ELEM(MODELE=dkt,

COQUE=(_F(GROUP_MA='PART_1',

EPAIS=1.0,

ANGL_REP=(0,90,),),"

So, since i wanted Von Mises Stress from my model, i went with something similar from some models.

Please correct if that is wrong (Aster experts)

regards

Offline

**AlbiBone****Member**- Registered: 2020-10-05
- Posts: 20

Thank you so much Laurent, I choosen a "random" values VECTEUR , in order to avoid alignment of local and the global axis, and the simulation give reasonable results!

Thank you again.

*Last edited by AlbiBone (2021-08-26 10:37:58)*

Offline

**sameer21101970****Member**- Registered: 2019-09-06
- Posts: 353

model = AFFE_MODELE(AFFE=_F(MODELISATION=('COQUE_3D', ),

PHENOMENE='MECANIQUE',

TOUT='OUI'),

MAILLAGE=mesh2D)

elemprop = AFFE_CARA_ELEM(COQUE=_F(ANGL_REP=(0.11, 0.22),

EPAIS=0.0015,

GROUP_MA=('Group_surf', )),

MODELE=model)

above changes will work without error

Offline