Chaining code_saturne and code_aster - LIRE_RESU and 'EVOL_CHAR'

ftrillaudp

Dear all,

I am stuck trying too read a result from code_saturne in med format. Code_Aster does not recognizes the component 'PRES':

! !

! Erreur lors de la fabrication d'un champ par éléments : !

! Il manque la composante : PRES sur la maille : M349 !

! Champ : ch_pres .002.000000 !

! !

! Risques et conseils : !

! Si cette erreur se produit lors de l'exécution de la commande PROJ_CHAMP, !

! il est possible de poursuivre le calcul en choisissant PROL_ZERO='OUI'

Here is the *.comm and attached the case study for someone to run it a give it a try:

DEBUT(PAR_LOT='OUI',);

import math

import numpy

############

### MESH ###

############

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

mail_cfd = LIRE_MAILLAGE(UNITE=21, FORMAT='MED',);

################

### MATERIAL ###

################

acier = DEFI_MATERIAU(ELAS = _F(E=190E9, NU=0.3,),);

mat1 = AFFE_MATERIAU(

MAILLAGE = mail_mec,

AFFE = (

_F(GROUP_MA='SSOL001', MATER=acier,),

);

##############

### MODELE ###

##############

mod_cfd = AFFE_MODELE(

MAILLAGE = mail_cfd,

AFFE = _F(TOUT='OUI', PHENOMENE='MECANIQUE', MODELISATION='3D',),

);

mod_mec = AFFE_MODELE(

MAILLAGE = mail_mec,

AFFE = _F(TOUT='OUI', PHENOMENE='MECANIQUE', MODELISATION='3D',),

);

##################

### CHARGEMENT ###

##################

pres_cfd = LIRE_RESU(

TYPE_RESU = 'EVOL_CHAR',

FORMAT = 'MED',

MODELE = mod_cfd,

UNITE = 21,

FORMAT_MED = _F(

NOM_CHAM = 'PRES',

NOM_CMP = 'PRES',

NOM_CHAM_MED = 'Pressure',

NOM_CMP_MED = 'Scalar',

TOUT_ORDRE = 'OUI',

);

ch_pres = PROJ_CHAMP(

METHODE = 'COLLOCATION',

RESULTAT = pres_cfd,

MODELE_1 = mod_cfd,

MODELE_2 = mod_mec,

TOUT_ORDRE = 'OUI',

VIS_A_VIS = _F(

TOUT_1 = 'OUI',

GROUP_MA_2 = 'SFAC001',

);

chg_mec = AFFE_CHAR_MECA(

MODELE = mod_mec,

EVOL_CHAR = ch_pres,

DDL_IMPO = _F(

GROUP_MA = ('SFAC002','SFAC003'),

DX=0, DY=0, DZ=0

);

meca = MECA_STATIQUE(

MODELE = mod_mec,

CHAM_MATER = mat1,

EXCIT = (

_F(CHARGE = chg_mec),

);

meca = CALC_CHAMP(

reuse = meca,

RESULTAT = meca,

CONTRAINTE = 'SIGM_ELNO',

FORCE = 'REAC_NODA',

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

);

## Ne fonctionne pas avec AFFE_CHAR_MECA_F

IMPR_CONCEPT(

UNITE = 81,

FORMAT = 'MED',

VERSION_MED = '4.0.0',

CONCEPT = (_F(CHARGE = chg_mec),),

);

IMPR_RESU(

UNITE = 80,

FORMAT = 'MED',

VERSION_MED = '4.0.0',

RESU= (

_F(

GROUP_MA = 'SSOL001',

RESULTAT = meca,

NOM_CHAM = 'DEPL',

_F(

GROUP_MA = 'SSOL001',

RESULTAT = meca,

NOM_CHAM = 'SIEQ_NOEU',

NOM_CMP = ('VMIS',),

);

FIN();

Best,

Frederic

Attached file:
Share.zip, 323112kb

Johannes_ACKVA

hello

I have never done this. But I see that your task is done in a different way in test case zzzz215c. In the test case the fluid mesh contains only the 2D-border of the fluid volume and the pressure field on the border. Whereas your fluid-mesh and fluid-result contains also the inner (solid) part. Can you try to generate with Code-Saturne only the 2D-border part? l also suppose that the pressure field should be a nodal field

Since I m not sure if I hit it, can you please confirm or deny after trying?

Regards

Johannes_ACKVA

Our next Code-Aster courses:

*** CODE-ASTER DYNAMIC ANALYSIS

19-20 March 2020

*** CODE-ASTER INTRO + CONTACT + MATERIAL

04-08 May 2020

www.code-aster. de

ftrillaudp

Hi,

It took some time but I figured out how to save only the pressure field on the surface of the fluid mesh. However, it did not solve the issue. The same error keeps popping up:

Erreur lors de la fabrication d'un champ par éléments : !

! Il manque la composante : PRES sur la maille : M349 !

! Champ : ch_pres .002.000000 !

I have no idea how to get the name of the component from the *.med file.

I have joined the new surface mesh with the pressure field.

Best,

Frederic

Attached file:
results_pressure_surface.med, 150560kb

AsterO'dactyle

Hello,

At first glance, maybe try PROl_ZERO='OUI'

ch_pres = PROJ_CHAMP(

METHODE = 'COLLOCATION',

RESULTAT = pres_cfd,

MODELE_1 = mod_cfd,

MODELE_2 = mod_mec,

TOUT_ORDRE = 'OUI',

PROL_ZERO='OUI',

VIS_A_VIS = _F(

TOUT_1 = 'OUI',

GROUP_MA_2 = 'SFAC001',

);

Johannes_ACKVA

ok, obviously the mesh and result coming from Code-Saturne must be only a 2D-mesh which is at the same place as the surface border elements of the mechanical mesh. With LIRE_RESU the pressure result coming from Code-Saturne is read. The pressure field is an element field (1 value per surface element). With the command PROJ_CHAMP the pressure field is projected onto the mechanical mesh. This is done "piecewise" using keyword COLLOCATION with VIS_A_VIS. Only one "piece" is defined: TOUT_1 = 'OUI' from the cfd-model is projected to GROUP_MA_2 = 'SFAC001' of the mechanical model. The pieces (only 1) do not cover the whole model so the command PROJ_CHAMP is not happy. It bleats:

ch_pres = PROJ_CHAMP(RESULTAT=pres_cfd, METHODE='COLLOCATION', MODELE_1=mod_cfd, MODELE_2=mod_mec, VIS_A_VIS=_F(TOUT_1='OUI', GROUP_MA_2=('SFAC001', ),), ALARME='OUI', PROL_ZERO='NON', TOUT_ORDRE='OUI', PROJECTION='OUI', INFO=1,) !----------------------------------------------------------------------------! ! <A> <CALCULEL_58> ! ! ! ! Erreur lors de la fabrication d'un champ par éléments : ! ! Il manque la composante : PRES sur la maille : M349 ! ! Champ : ch_pres .002.000000 ! ! ! ! Risques et conseils : ! ! Si cette erreur se produit lors de l'exécution de la commande PROJ_CHAMP, ! ! il est possible de poursuivre le calcul en choisissant PROL_ZERO='OUI' ! ! ! ! ! ! Ceci est une alarme. Si vous ne comprenez pas le sens de cette ! ! alarme, vous pouvez obtenir des résultats inattendus ! !

!----------------------------------------------------------------------------!

M349 is the 1st element of the mechanical model which is a surface element and which is not part of GROUP_MA_2 = 'SFAC001'.

When using PROJ_CHAMP(.. PROL_ZERO='OUI' ..) as AsterO'dactyle indicated then to all elements which are not part of GROUP_MA_2 = 'SFAC001' the value zero is assigned.

I printed the field resulting with PROL_ZERO='OUI' and see that it does not comprise all 12975 elements of the mec model but only 2550 elements (see attached .resu). This is the number of the 2D-elements of the mechanical model ( TRIA3: 1650, QUAD4: 900, see .mess-file). So the projection command works in the manner that a pressure field is projected only on face elements (for other fields there is not this special behaviour). In .resu we see that 1650 of these elements have the value 0 (got because PROL_ZERO='OUI'), the other 2550-1650=900 surface elements have a meaningful pressure value. 900 is the number of elements pf GROUP_MA 'SFAC001'.

Regards

Johannes_ACKVA

Our next Code-Aster courses:

*** CODE-ASTER DYNAMIC ANALYSIS

19-20 March 2020

*** CODE-ASTER INTRO + CONTACT + MATERIAL

04-08 May 2020

www.code-aster. de

Johannes_ACKVA

here the attachment

Attached file:
read_pressure_from_saturne.zip, 400424kb

ftrillaudp

Dear AsterO'dactyle and Johannes_ACKVA,

Thanks to take the time to look at my issue. My knowledge of Code_aster is quite limited and the explaining is much appreciated.

My goal is to couple code_saturne and code_Aster so that one can evaluate the deformation of the walls on the fluid behavior. Some way to go still. If I manage, I will post the model on the forum.

Thanks again, best regards

Frederic

ftrillaudp

Dear all,

I have a working example of coupling code_saturne v6 and code_aster v14.4. I am joining the full folder including the code_saturne case coupled to the code_aster case.

The meshes for the fluid and for the solid surrounding the fluid are done in Salome platform and exported in med format.

The python main.py must be run to chain the CFD and structural computations.

The case study is setup through fictitious material properties so that there is enough deformation to impact the fluid but not enough to lead to large deformations. Large deformations may require a different mechanical solver as well as recompute the meshes (regularization as elements with negative volume may arise due to gherkin's large deformation).

Best regards,

Frederic

Attached file:
CodeSaturne-CodeAster.zip, 768283kb

Shayor

Hello ftrillaudp Sir.Thank you so much for the case.

Could you tell me in brief what the model is for and the objective of the simulation?It would really help me.I was trying to do a simulation of blood flow in artery with flexible walls.It seems the ALE (deformable mesh) and internal coupling option can't do it.

Also if possible could you provide sources to learn how to carry out this process in steps from zero?(Please note I know Code Saturne well) or if you could explain the procedure to me here or in mail(if possible in short).

Thank You in advance.Would really appreciate the help.

The Admins here can also help.As ofcourse you are the primary source.I really need the help.Please.I want to publish using Code Aster and Code Saturne my paper.I am really near.

ftrillaudp

Dear Shayor,

I am very sorry to reply after so many months considering you were under some deadline as far as I understood. I have not used Code_Aster for some time and did not bother to look at this post thinking it was closed. Only by curiosity, I went back to it having discussed this case study with a former student of mine.

I have to get back to it to refresh my mind. If you still need some help, I may be able to provide at least on setting up a case study.

I did this example to understand how to simulate fluid-structure interaction. The case study is random. However, it allowed me to play with the material properties to see the range of values permissible until the coupling fails. If the deformation is relatively small, it works very well.

Best,

Frederic