Read a Salome mesh with Code_Saturne and NEPTUNE_CFD

[Hervé Neau]

Hello all,
I'm a user of Code_Saturne and especially of NEPTUNE_CFD 1.08.
I would like to know how to import a SALOME 6.3.1 mesh in Code_Saturne and NEPTUNE_CFD 1.08 (with boundary conditions).
If I use I-DEAS mesh file with ECS 1.2.5.1, the mesh is OK but I don't have any boundary condition.
If I use MED mesh file with ECS 1.2.5.1, I obtain an error : "ecs_prep_med.C:543: Erreur fatale". I think Salome export MED 3.0 and ECS 1.2.5.1 read MED 2.3.6.
Is it possible to use I-DEAS mesh file with boundary conditions?
Is it possible to use ECS 1.2.5.1 with MED 3.0?
Thank you for your answer.
Best regards,
Hervé

 

[Yvan Fournier]

Hello,
You can read I-Deas mesh files with boundary conditions, as long as mesh colors or groups are applied on a "surface coating" of surface elements (colors and groups on nodes are ignored).
Also, what version of I-Deas or other tool do you use ?
As for MED support, Code_Saturne versions 2.0 above can support either MED 2.3 or MED 3 (support for MED 2.3 will be removed at some future point in time, but not before a few months at least). Versions 1.3 and older only support MED 2.3, so they cannot be used with SALOME 6.3.1.
NEPTUNE_CFD 1.2 is up to date with Code_Saturne 2.1, so it can use MED 3.
Best regards,
  Yvan Fournier

[Hervé Neau]

Hello Yvan,

Thank you for your answer.

I use the default I-Deas format of Salome 6.3.1 (export "unv").

I use NEPTUNE_CFD V1.08 (fortran) to simulate with O. Simonin (IMFT) gas-particle flows (fluidized beds). We are not ready use NEPTUNE_CFD V1.2 because we have to translate our gas-particle developpements (C/C++) and to validate this version...

According to your answer, if I read to read with ECS 1.2.5.1 a MED file from Salome I have to use Salome 5.

For I-Deas mesh, I think I don't know how to create mesh colors or groups are applied on a "surface coating" of surface elements with Salome 6.3.1. I have created a cube (geometry) and 6 groups (1 per face). I have meshed this cube with hexaedrons and created 6 groups (1 per face). I export this mesh using "unv" format (cf cube6.unv). I can read this mesh with ECS 1.2.5.1 but boundary conditions are not present (cf listenv_pre). Is it right?

Best regards

Hervé Neau

[Yvan Fournier]

Hello,
The "surface coating" required for I-deas is done automatically by Salome when building groups of faces (the vocabulary is different, but in both cases, faces of the required group are added to the volume mesh).
You "unv" file seems correct: when I read it using the preprocessor from Code_Saturne 2.0 (and even 1.3), the face groups are present, but it seems version 1.2 can only read groups from older variants of the I-deas format (the format has gone through several versions of the "dataset" used for groups, and version 1.2 handles dataset variants 2430, 2432, 2435, 2452, while 1.3 added support for datasets 2467 and 2477 (added with I-deas 12). Support for this was added in the Preprocessor in January 2008 (looking at the ChangeLog), but as version 1.2.0 was released in 2005, that branch is much older...
So I have no good solution for you except to use geometric criteria for your boundary conditions.
Regards,
  Yvan

[Hervé Neau]

Thank you for theses precisions.
Do you think it could be ok using Salome 5 I-Deas format with ECS 1.2.5.1?
 
Regards
 
Hervé
 

[Yvan Fournier]

Hello,
I am not sure (I upgraded to SALOME 6.4, and uninstalled my previous versions), but it might work, so you can try.
You may also try to edit the ECS source code: in src/pre-post/ecs_pre_ideas.c, around line 386, after:
case ECS_IDEAS_DATASET_GROUPS_2452:

add:
case 2467:
case 2477:
so you should have a block looking like:
case ECS_IDEAS_DATASET_GROUPS_2430:
case ECS_IDEAS_DATASET_GROUPS_2432:
case ECS_IDEAS_DATASET_GROUPS_2435:
case ECS_IDEAS_DATASET_GROUPS_2452:
case 2467:
case 2477:

Then simply recompile, and test.
I am not sure it will work, but it is probably as quick to test as reverting a Salome version, and would allow you a better choice of meshers.
Regards,
  Yvan