FORCE_ARETE applying Moment

die_ca

Hi everyone, I'm not very good at Code aster and I've been trying to apply a moment distributed along an edge of a 3D solid for a while, without success. I created a hollow cylinder. I created two groups: a faces group (constraints, DX=DY=DZ=0) and an edges group (where I would like to apply the moment). when I run it, it doesn't generate an error, but when I open the model in Paraview, the cylinder is completely unloaded (Depl=0, VMIS=0). Can anyone help me? Thank you in advance

mesh = LIRE_MAILLAGE(FORMAT='MED',

                 UNITE=20)

model = AFFE_MODELE(AFFE=_F(MODELISATION=('3D', ),

                        PHENOMENE='MECANIQUE',

                        TOUT='OUI'),

                MAILLAGE=mesh)

mater = DEFI_MATERIAU(ELAS=_F(E=206000.0,

                          NU=0.3))

materfl = AFFE_MATERIAU(AFFE=_F(MATER=(mater, ),

                            TOUT='OUI'),

                    MODELE=model)

mecabc = AFFE_CHAR_MECA(DDL_IMPO=_F(DX=0.0,

                                DY=0.0,

                                DZ=0.0,

                                GROUP_MA=('FIX_SUPPORT', )),

                    MODELE=model)

mecach = AFFE_CHAR_MECA(FORCE_ARETE=_F(GROUP_MA=('EDGE_MOMENT', ),

                                   MY=100.0),

                    MODELE=model)

result = MECA_STATIQUE(CHAM_MATER=materfl,

                   EXCIT=(_F(CHARGE=mecabc),

                          _F(CHARGE=mecach)),

                   MODELE=model)

ris = CALC_CHAMP(CONTRAINTE=('SIGM_ELNO', 'SIGM_NOEU'),

             CRITERES=('SIEQ_ELNO', 'SIEQ_NOEU'),

             RESULTAT=result)

IMPR_RESU(FORMAT='MED',

      RESU=(_F(NOM_CHAM=('SIGM_ELNO', 'SIGM_NOEU', 'SIEQ_ELNO', 'SIEQ_NOEU'),

               RESULTAT=ris),

            _F(NOM_CHAM=('DEPL', ),

               RESULTAT=result)),

      UNITE=80)

IMPR_RESU(FORMAT='RESULTAT',

      RESU=_F(NOM_CHAM=('SIGM_ELNO', 'SIGM_NOEU', 'SIEQ_ELNO', 'SIEQ_NOEU'),

              RESULTAT=ris,

              VALE_MAX='OUI',

              VALE_MIN='OUI'),

      UNITE=8)

FIN()

die_ca

can someone please help me? i need your help. thanks in advance

k_zurawski

Have you looked for the answer in mess file? Alarms are displayed after command that failed. Share your mess file please as an attachment.

die_ca

k_zurawski thanks for you reply. Do you mean this as a message? Tjanks in advance

jacob

https://www.caelinux.org/wiki/images/4/46/ApplyingTorque.pdf

k_zurawski

It seems that's the case. You may as well apply the moment to a POI1 element, as stated in the pdf above. If I need to support the structure or apply distant force I'm using that approach. I'm creating POI1 on orphan node using C_A syntax and tie elements like in your case 'EDGE_MOMENT' to that POI1 element with LIASON_SOLIDE.
You can look at this example:
https://we.tl/t-fEUxIGdzsr
the discussion regarding this example is here:
https://forum.code-aster.org/public/d/27711-distant-supportload-and-coque-3d-in-stat-non-line-grot-gdep

die_ca

Thanks to all for the support. I was able to use the FORCE_NODALE command, applying the desired moment. However, for my case I think it is more correct to use the FORCE_ARETE command. I used a “3D” modeling everywhere and a DIS_TR_DN modeling for the edge on which I want to apply the moment. But even in this case I get inconsistent results (VMIS=0, DEPL=0).

k_zurawski

die_ca share your mesh and comm file please

die_ca

k_zurawski

die_ca

k_zurawski

die_ca

k_zurawski I tried to upload the hdf and .comm file as a rar archive. can you view it?

die_ca

k_zurawski

Hi. No. Use We transfer, Google Drive, oOneDrive or any other online service. It's the only way at the moment.

die_ca

k_zurawski https://we.tl/t-tOLk1N0rs2

k_zurawski

die_ca have you tried PrePoMax? Maybe this software will fit your needs?

k_zurawski

First thing is that you have mixed mesh version (without POI1 element) and added tied connection between edge and that non existing POI1. DIS_TR can be applied to POI1 element, not edge, as you have in comm file:
_F(GROUP_MA=('moment', ),

                         MODELISATION='DIS_TR',

                         PHENOMENE='MECANIQUE')),

It's a good practice to check what's wrong in message window or message file:

Commande #0003 de fort.1, ligne 33

model = AFFE_MODELE(AFFE=(_F(MODELISATION='3D',
PHENOMENE='MECANIQUE',
TOUT='OUI'),
F(GROUP_MA='moment',
MODELISATION='DIS_TR',
PHENOMENE='MECANIQUE')),
DISTRIBUTION=F(METHODE='SOUS_DOMAINE',
PARTITIONNEUR='METIS'),
INFO=1,
MAILLAGE=mesh,
VERI_JACOBIEN='OUI',
VERI_NORM_IFS='OUI')

Sur les 17661 mailles du maillage 00000001, on a demandé l'affectation de 17661, on a pu en affecter
17661.
Modélisation Formulation Type maille Élément fini Nombre
_ _ SEG2 MECA_ARETE2 179
DIS_TR _ SEG2 MECA_DIS_TR_L 18 -<THIS IS WRONG
_ _ TRIA3 MECA_FACE3 5280
3D _ TETRA4 MECA_TETRA4 12184
2 Calculs elementaires et assemblages CPU (USER+SYST/SYST/ELAPS): 0.00 0.00 0.00
Résultat commande #0003 (AFFE_MODELE): model ('<00000002>') de type <Model>
Dépend de :

mesh ('<00000001>') de type <Mesh>
Mémoire (Mo) : 767.11 / 766.55 / 47.81 / 38.57 (VmPeak / VmSize / Optimum / Minimum)
Fin commande #0003 user+syst: 0.02s (syst: 0.00s, elaps: 0.03s)
----------------------------------------------------------------------------------------------

and later on you have:
╔════════════════════════════════════════════════════════════════════════════════════════════════╗
║ <A> <CALCULEL_40> ║
║ ║
║ Erreur possible d'utilisation: ║
║ Vous avez affecté des données sur certaines mailles mais ces données ║
║ n'ont pas de signification pour les éléments finis portés par ces mailles. ║
║ Il s'agit peut-être d'une erreur d'affectation. ║
║ ║
║ Champ : '00000005.CHME.F1D3D' ║
║ Commentaire sur ce champ : ║
║ Grandeur : FORC_R Composante non reconnue : MZ ║
║ ║
║ Ce problème concerne 18 mailles ║
║ Les premières mailles concernées sont imprimées ci-dessous. ║
║ Type de l'élément affecté sur la première maille imprimée : MECA_DIS_TR_L ║
║ ║
║ ║
║ This is a warning. If you do not understand the meaning of this ║
║ warning, you can obtain unexpected results! ║
╚════════════════════════════════════════════════════════════════════════════════════════════════╝

Mesh : M1. This mesh belongs to GROUP_MA : moment

Mesh : M2. This mesh belongs to GROUP_MA : moment

Mesh : M3. This mesh belongs to GROUP_MA : moment

Mesh : M4. This mesh belongs to GROUP_MA : moment

Mesh : M5. This mesh belongs to GROUP_MA : moment ****

Which Googler translator gives you:
Possible usage error: ║
║ You have assigned data to some meshes but this data ║
║ has no meaning for the finite elements carried by these meshes. ║
║ This may be an assignment error.
Which points to mesh group GROUP_MA: moment

k_zurawski

But nevertheless, it seems that FORCE_ARETE isn't working in this case.
Please define node in centre of the hole, add POI1 element there, name that POI1 as group_ma "load".
Create NODAL group of POI1 also called "load".
Add DIS_TR to POI1, define characteristics.
Add LIASON_SOLIDE between moment and load MESH groups.
Apply FORCE_NODALE to the NODAL group "load"
https://code-aster.org/doc/v15/fr/man_u/u4/u4.44.01.pdf
Should work this way.

mf

k_zurawski
Indeed, it does, but the result is highly influenced by the mesh around it:

If I choose a higher scale factor, the bore does not remain at the center. The original moment of 1E6 is completely crazy.

Mario.

runcase-1-stage-1.txt

4kB

k_zurawski

I changed a lot in the study that was shared, but run into some syntax and naming problems. So I decided to do it from scratch, changed MZ to 100 and the result is: