Welcome to the forums. Please post in English or French.

You are not logged in.

#1 2019-02-19 15:39:13

pironman
Member
Registered: 2018-05-15
Posts: 50

meshing compound: another way?

I made some simulation of large file, made by shells, solids and nodes where I put discrete elements.
My procedure was:

1) Import STEP file
2) Explode it into shells and solids
3) Create vertices where I want the 0D elements
4) Make a partition with all the exploded elements and the vertices
5) Explode again the partition into vertices, solids and shells.
6) Create groups where I want to put LIAISON_SOLIDE, link, forces and so on
7) In the mesh module, I create a "empty" mesh of the partition
8) Then, I create one sub-mesh for each component
9) I compute the main mesh, add the group and so on

After that, I set the simulation in the aster module. All works, no problem.

Now, the problem: After the simulation, I want to modify one component of the geometry. It's ridiculous, because I must repeat the entire procedure, recreate groups and so on. It's more or less 2 hour of work every time.
I've done that 2-3-4 times, but... there is another faster way to do that?

Thank you

Offline

#2 2019-02-26 12:32:49

nirmaljoshi
Member
From: Japan
Registered: 2018-10-12
Posts: 146

Re: meshing compound: another way?

I agree. Its frustrating sometimes. Eventhough the geometries appear linked, the way to update them spontaneously in GUI is not available yet, perhaps.

Python may rescue you in such situation.  One tutorial :  youtube.com/watch?v=h04X7lXMhrc

Offline

#3 2019-02-27 13:54:20

pironman
Member
Registered: 2018-05-15
Posts: 50

Re: meshing compound: another way?

thank you for the tutorial.
I try to do it, but didn't work, maybe because I import step geometry, and don't create geometry directly on geom module.
But it's good food for tought, i'll try again

Offline

#4 2019-02-27 14:13:59

jeanpierreaubry
Guru
From: nantes (france)
Registered: 2009-03-12
Posts: 3,570

Re: meshing compound: another way?

hello

i stopped using salome many years ago for many reasons
and the problem you describe here is one of them

however working with imported CAD file is never very easy as almost everything as to be redone once the CAD file is modified

in the specific case i use gmsh and follows some, but not all, of the steps you describe here

i needs only steps
1,
1bis, cleaning the imported file
3, 6,
9, creating groups and meshing

Gmsh does not need partition

hopefully some of the scripting may not be affected by the CAD modification

when there are several parts i also import and mesh them one by one and join them within code_aster
this makes modification to one part only easier to cope with

last point
please introduce your self in the ad hoc section of the forum

jean pierre aubry

Offline

#5 2019-02-28 13:07:17

Ioannis
Member
Registered: 2016-04-01
Posts: 45

Re: meshing compound: another way?

Hi,

Between steps 5 and 6 I assume you create a compound where you assign all the groups needed?
Perhaps it could help to have each component with the groups defined on its reference object and then create the final compound transferring the groups, which is possible in the latest versions of Salome. In that way may be you could get away with reconstructing only the component you are changing and its surrounding components. But I understand that it could be non-trivial often.

Bear in mind that you can always dump the study to see the commands that you have executed as a python script. This could be of help I believe as some phases of your model construction could be reproducible.


Aether Engineering
- aethereng.com -

Offline

#6 2019-02-28 17:22:06

ppeetteerr
Member
Registered: 2009-06-30
Posts: 234

Re: meshing compound: another way?

A couple of tips I use.

1.) Create Individual Meshes of components and then combine them in code_aster using ASSE_MAILLAGE

mesh = LIRE_MAILLAGE(UNITE=20)

mesh2 = LIRE_MAILLAGE(UNITE=2)

mesh3 = ASSE_MAILLAGE(MAILLAGE_1=mesh,
                      MAILLAGE_2=mesh2,
                      OPERATION='SUPERPOSE')

2.) Define groups based on geometry in salome

Face_X = geompy.MakeFaceHW(40, 40, 2)
aCriteria = [ smesh.GetCriterion(SMESH.FACE,SMESH.FT_BelongToPlane,SMESH.FT_Undefined,Face_X)]
aFilter_1 = smesh.GetFilterFromCriteria(aCriteria)
aFilter_1.SetMesh(Mesh_2.GetMesh())
Group_2 = Mesh_2.GroupOnFilter( SMESH.FACE, 'Face_X', aFilter_1 )

Item 1 prevents you from having to remesh the parts that didn't change.
Item 2 stops you from having to explode the shells everytime.

Offline

#7 2019-03-08 10:00:42

pironman
Member
Registered: 2018-05-15
Posts: 50

Re: meshing compound: another way?

@jeanpierreaubry, @ppeetteerr
create an individual mesh of each component and then combine it in aster, is a beautiful solution. I'll try in this manner

last point
please introduce your self in the ad hoc section of the forum

you're right. Now I'll do it

Offline