[mahaputra]

Dear All


does anybody know, how to make a 2d mesh in Salome and can be recognized by OpenFOAM ?


many thanks

[gschaider]

Originally Posted by mahaputra

does anybody know, how to make a 2d mesh in Salome and can be recognized by OpenFOAM ?

I assume that the converter (ideasUnvToFoam) fails. Probably (haven't checked) it doesn't support 2D-Meshes. The easiest thing (unless you want to rewrite the convert) is to extrude in Salome the mesh to a 3D-mesh that is 1 layer thick and export that. Just the thing the convert would do to get a Foamish 2D-mesh

Bernhard

[mahaputra]

Originally Posted by gschaider

I assume that the converter (ideasUnvToFoam) fails. Probably (haven't checked) it doesn't support 2D-Meshes. The easiest thing (unless you want to rewrite the convert) is to extrude in Salome the mesh to a 3D-mesh that is 1 layer thick and export that. Just the thing the convert would do to get a Foamish 2D-mesh

Bernhard

Thanks Bernhard


so, could you please suggest me, some option to make a 2D mesh (exclude using blockMeshDict or any commercial software) ?

by the way, out of the topic, i have a problem related to dieselFoam, please spend a while your time to see my case in : http://www.cfd-online.com/Forums/ope...tml#post216606

i really need some suggestion and help


Thousand Thanks


Nugroho Adi S

[nimasam]

Originally Posted by gschaider

The easiest thing (unless you want to rewrite the convert) is to extrude in Salome the mesh to a 3D-mesh that is 1 layer thick and export that.

Dear Bernard

i follow this suggestion, now it can be converted with ideasUnvToFoam, but it returns patches as default faces and it can not recognize patches, do you have any idea how i can keep patches name in conversion from salome

[gschaider]

Originally Posted by nimasam

Dear Bernard

i follow this suggestion, now it can be converted with ideasUnvToFoam, but it returns patches as default faces and it can not recognize patches, do you have any idea how i can keep patches name in conversion from salome

Have you named the patches in Salome?

[nimasam]

well, my steps in salome:
1- create 2D sketch
2-create face
3-explod face to edges
4-creates groups
5- mesh face (2D mesh)
6- extrude it
it fails to recognize my groups

then i changed my approach,
1- create 2D sketch
2-create face
3- extrude face to create volume
4- explode volume
6- create groups
7- create mesh
3D project with 2D-1D netgen element
but OpenFOAM can not recognize the elements

any idea how i can create one cell thickness for 2D simulation in OpenFOAM with Salome and with known patches ?

[gschaider]

Originally Posted by nimasam

well, my steps in salome:
1- create 2D sketch
2-create face
3-explod face to edges
4-creates groups
5- mesh face (2D mesh)
6- extrude it
it fails to recognize my groups

then i changed my approach,
1- create 2D sketch
2-create face
3- extrude face to create volume
4- explode volume
6- create groups
7- create mesh
3D project with 2D-1D netgen element
but OpenFOAM can not recognize the elements

any idea how i can create one cell thickness for 2D simulation in OpenFOAM with Salome and with known patches ?

If I remember it correctly you've got to create mesh groups or so (not sure of the nomenclature, don't want to start Salome and it is done in one of the basic tutorials on Salome anyway) from the geometry groups.

[startingWithCFD]

Geometry module
1) create 2D sketch
2) create face
3) extrude face to create volume
4) use propagate on the extrusion (operations -> blocks -> propagate) to create groups ("compounds") of edges that have the same discretization
5) create face groups

Mesh module
6) create mesh for the extrusion
7) create a sub-mesh for the extrusion at the compound containing edges you want to discretize with only one interval. Algorithm: wire discretization. New hypothesis: nb. of segments = 1
8) compute the mesh

[startingWithCFD]

Sorry, forgot these last steps:
9) Right click on mesh, create group, face, group on geometry. Geometrical object: direct geometry selection and choose the groups on the geometry.
10) Right click on the mesh and export to UNV

That's all folks!

[hsmao]

Originally Posted by startingWithCFD

Geometry module
1) create 2D sketch
2) create face
3) extrude face to create volume
4) use propagate on the extrusion (operations -> blocks -> propagate) to create groups ("compounds") of edges that have the same discretization
5) create face groups

Mesh module
6) create mesh for the extrusion
7) create a sub-mesh for the extrusion at the compound containing edges you want to discretize with only one interval. Algorithm: wire discretization. New hypothesis: nb. of segments = 1
8) compute the mesh

Thanks! This worked perfectly.