hi everybody

i try to create internalls walls in OF thanks to this thread: http://openfoamwiki.net/index.php/Howto_importing_fluent_mesh_with_internal_wall s

i create my mesh with gambit but when i convert fluent mesh to openfoam it say me "Patch internal is internal to the mesh and is not being added to the boundary." but it don't create a set to use after splitmesh
what am i doing wrong?
what is the easy way to create a faceset ?

bestregards

[gschaider]

With the new versions of fluentMeshToFoam (1.4+ I think) you have to explicitly trigger the writting of the sets with the -writeSets-option.

It has been asked before here. I will modify the Wiki-page accordingly

Bernhard

thanks bernhard

sorry but i have got this error

Create polyMesh for time = 0

#0 Foam::error::printStack(Foam:stream&) in "/home/gui/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigSegv::sigSegvHandler(int) in "/home/gui/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Uninterpreted: [0xffffe420]
#3 Foam::polyMesh::initMesh() in "/home/gui/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#4 Foam::polyMesh::polyMesh(Foam::IOobject const&) in "/home/gui/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#5 main in "/home/gui/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/splitMesh"
#6 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#7 Foam::regIOobject::write() const in "/home/gui/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/splitMesh"
Erreur de segmentation (core dumped)

i suppose it's because startface like it say in the wiki
What mean "current number of faces" for the startface on the wiki?where i can found it?

best regards

[gschaider]

Have a look at the faces-file in polyMesh. At the start of the list it says how many faces are in the list. This is the "current number of faces". Use it for the startFace.

[fra76]

Alternatively, you can try to use fluent3DMeshToFoam shipped with OF 1.4.1.
If the internal walls are correctly set up in Fluent (i.e., with a Shadow face), it should be able to convert the mesh.

Francesco

[gabriel_stokes]

Hi!

I have a GAMBIT mesh with internal walls. I have exported it to a Fluent .msh file, which reads nicely into Fluent. I want it into OpenFOAM. It works beautifully if I do nothing, but naturally the internal walls are missing from the simulation. So,

I did the fluentMeshToFoam . <case> <meshfile.msh> -writeSets

fluentMeshToFoam recognises the internal walls but skips them, as noted by the original poster: "Patch internal is internal to the mesh and is not being added to the boundary."

I have multiple internal walls, defined as separate BC's in Gambit. I am trying to just get one of them active. So, in the boundary-file I add two entries:

InternalA
{
type wall;
nFaces A;
startFace B;
}

InternalB
{
type wall;
nFaces A;
startFace B;
}

I do not think that the question of what values to put A and B to, is clearly defined anywhere, or in the wiki. It is not clear to ignorant little me, at least.

I run the command splitMesh . <case> <gambit_bc_name> InternalA InternalB and it gives various error messages, depending on what values A and B have. Hence I have some questions, and please be accurate and comprehensible :-)


Question 1: I guess A and B has to be the same in InternalA and in InternalB, right?
Question 2: what should A be set to?
Question 3: what should B be set to?

I tried to set A to the first number which occurs in the sets/<gambit_bc_name> file. Makes no sense to me, as splitMesh should be able to read this number.

I tried to set B to the first number which occurs in the faces-file (just after the header). I believe this is the total face count. Makes no sense to me, why I should be using that number, as it should be available to splitMesh already from the faces-file.


Makes no sense, meaning that I do not understand at all what numbers should go in A and B.

Any help is greatly appreciated, thanks a bunch!

/Mads




I got a sets-directory in my polyMesh directory.

[caw]

Hi Mads,

Have you tried fluent3DMeshToFoam, this should do it.

Best regards
Christian

[gabriel_stokes]

Hi Christian,

fluent3dMeshToFoam never worked for me. But, slightly embarrassed I admit, that fluentMeshToFoam now works, it seems. Well, actually it still breaks, but now it ends on "new cannot satisfy memory request". The mesh is probably too big. I have plenty of RAM so I wonder if changing to the 64bit version will alleviate this...?

Just, to clarify, since I may have caused some confusion, entries in the boundary file should read something like this:

InternalA
{
type wall;
nFaces 0;
startFace <facecount>;
}

InternalB
{
type wall;
nFaces 0;
startFace <facecount>;
}

where <facecount> is the total number of faces, found in the file ./<case>/constant/polyMesh/faces as the first entry after the header.

I have two follow-up questions, then.

Q1: will 64-bit version alleviate the memory limit-issue?
Q2: is fluent3DMeshToFoam the preferred choice?

Thanks!

/Mads

[plmauk]

I had the same problem - I should import a fluent-mesh with an internal wall. This never worked with fluentMeshToFoam, but after reading these messages I've tried fluent3DMeshToFoam - and I have to confirm - it works perfectly!!

[gabriel_stokes]

A quick hint on having multiple internal walls (i.e. defined in each own BC set)?

Do I run splitMesh multiple times or do I have to include all internals in one BC set in Gambit?

/Mads