FluentMeshToFoam errorplease help me
 

http://www.cfd-online.com/OpenFOAM_D...ges/1/1897.jpg
This is a 2D centeralpump model.
When simulate it in Fluent, I set with two fluid zones, one is stationary and the other is rotating(reference).
But when I import the mesh to OpenFOAM,
errors appears as following:
/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.2 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

Exec : fluentMeshToFoam /home/andycong/OpenFOAM/andycong-1.2/run/tutorials/simpleFoam 2Dcenteralpump /home/andycong/2Dcenteralpump/pump_mesh.msh
Date : Mar 02 2006
Time : 09:09:01
Host : linux
PID : 10727
Root : /home/andycong/OpenFOAM/andycong-1.2/run/tutorials/simpleFoam
Case : 2Dcenteralpump
Nprocs : 1
Create time

Dimension of grid: 2
Number of points: 2567
Reading points
number of faces: 7263
Reading mixed faces
Reading mixed faces
Reading mixed faces
Reading mixed faces
Reading mixed faces
Reading mixed faces
Number of cells: 4690
Reading uniform cells
Reading uniform cells
Reading zone data
Reading zone data
Reading zone data
Reading zone data
Reading zone data
Reading zone data
Reading zone data
Reading zone data


FINISHED LEXING


dimension of grid: 2
Grid is 2-D. Extruding in z-direction by: 14.4162
Creating shapes for 2-D cells
Creating patch for zone: 4 start: 1 end: 173 type: wall name: wall_3
Creating patch for zone: 5 start: 174 end: 263 type: wall name: wall_2
Creating patch for zone: 6 start: 264 end: 479 type: wall name: wall_1
Creating patch for zone: 7 start: 480 end: 498 type: outflow name: outlet
Creating patch for zone: 8 start: 499 end: 546 type: velocity-inlet name: inlet
Creating patch for zone: 10 start: 547 end: 7263 type: interior name: default-interior
Patch 10 contains solid or internal faces. Not added to boundary
Not adding to internal boundaries
Creating patch for front and back planes

Default patch type set to empty


--> FOAM FATAL ERROR : Trying to specify a boundary face 4(0 1 2568 2567) on the face on cell 399 which is either an internal face or already belongs to some other patch. This is face 0 of patch 1 named wall_2.

From function polyMesh::polyMesh
(
const IOobject& io,
const pointField& points,
const cellShapeList& cellsAsShapes,
const faceListList& boundaryFaces,
const wordList& boundaryPatchTypes,
const wordList& boundaryPatchNames,
const word& defaultBoundaryPatchType
)
in file meshes/polyMesh/createPolyMesh.C at line 375.

FOAM aborting

Aborted


Could anyone tell my what's the matter?

I have the same problem. I thi
 

I have the same problem. I think it is related to the zone interfaces. Will be looking into it soon.

Hi Andy, The only Fluent me
 

Hi Andy,

The only Fluent mesh I have that has this problem consists of 13million cells. As you can imagine it is a bit hard to find the problem when the core dump takes 10 mins. Could I please have a copy of your mesh to do my testing on?

Of cource it is OK. Now I wil
 

Of cource it is OK.
Now I will attach it in this board.
Yestoday when I searched the messages before, I found it seemed that OpenFOAM does not support rotating machine, what do you think of that?

Of cource it is OK. Now I wil
 

Of cource it is OK.
Now I will attach it in this board.
Yestoday when I searched the messages before, I found it seemed that OpenFOAM does not support rotating machine, what do you think of that?
I have sent the mesh to your Email.

Thanks, got it. Will post the
 

Thanks, got it. Will post the fix when I find it.

Hi Andy. As far as I can t
 

Hi Andy.

As far as I can tell the problem seems to be that you have an 'interior wall' (see http://www.cfd-online.com/OpenFOAM_D...ges/1/364.html)

What you have to do is define it as INTERNAL in Gambit and export the mesh again. The wall becomes a faceSet. Then use splitMesh to construct two walls from that faceSet (there is a reference to a more detailed description in the thread I referenced above)

Thank you, I will try it.
 

Thank you, I will try it.

http://www.cfd-online.com/Ope
 

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif fluentMeshToFoam.L

This is still work in progress, but if you compile this instead of the default it will basically ignore internal boundaries (it will however writes them as faceSets). Should take care of all the problems posted above.

Forgot to mention, this is for
 

Forgot to mention, this is for 1.3, don't know if it will work for 1.2.

Hi Eugene, I tried compilin
 

Hi Eugene,

I tried compiling your file with 1.2.1, but I miss the repatchPolyTopoChanger.H file:

fluentMeshToFoam.L:56:36: error: repatchPolyTopoChanger.H: No such file or directory.

Hi, I have read several for
 

Hi,

I have read several forum messages about fluenMeahToFoam, and I am still quite confused.

I have a mesh created with fluent (.msh file)
with some of the boudaries declared as "interior".
Is is the first time I am using such
complex grid and I couldn't well understand the
steps to correctly apply fluentMeshToFoam.

First, compiling the above FluentMeshToFoam.L,
with OpenFoam 1-3 gives me the following error compilation:

----
fluentMeshToFoam.L: In function 'int main(int, char**)':
fluentMeshToFoam.L:1506: error: 'repatchPolyTopoChanger' was not declared in this scope
fluentMeshToFoam.L:1506: error: expected `;' before 'repatcher'
fluentMeshToFoam.L:1509: error: 'repatcher' was not declared in this scope
make: *** [Make/linuxGcc4DPOpt/fluentMeshToFoam.o] Error 1
----


Then, reading older forum messages I could
see that this could be dealt with splitMesh, but
it is still very confusing for me the steps to follow.


Thanks you if you could help,

PS: I have also simply applied the original version of the fluentMeshToFoam application and have the following message:

------------------------
Patch 23 contains solid or internal faces. Not added to boundary
Not adding to internal boundaries

Default patch type set to empty
Checking mesh
Writing mesh
Only one cell group: no set written


Anne

Hello again, Well I have fo
 

Hello again,

Well I have found on wiki server the
information for dealing with interior cell.

BUT, the problem I have is that fluentMeshToFoam
does not create any faceSet, which means no
subdirectory sets in the constant/polyline/
so that when running splitMesh the name of the interior BC from Gambit is not given.


I have OpenFoam 1.3 from a linux binary package.


Why the subdirectory is not created ?
n my previous mail I made a copy of the
.msh file and there is one interior BC.


Thanks if you can help with this,


anne

What is the output of fluentMe
 

What is the output of fluentMeshToFoam?

In the distributed version if your "interior wall" has been set in Gambit to one of the types "interior", "internal", "solid", "fan", "radiator" or "porous-jump" a faceSet should be generated.

The last few lines of the MSH-file would be helpful to diagnose the problem(the ones starting with '(0 "Zones:")')

Hello Bernhard, I have now
 

Hello Bernhard,

I have now fixed the problem.
Having seen zones declared as "interior" in my .msh
I have read all th threat around.
However, they were not wall BC but, a zone that
is created by default with Gambit (it was the first I used it).

This zone is actually ignored by fluentMeshToFoam and I could run my job .


Thanks you for anser,


Anne

I use a membrane in my reactor
 

I use a membrane in my reactor. It is an internal wall declared as INTERNAL, because I know that Foam don't accept a internal wall. In Fluent my mesh "reactor.msh" with two different zones is good. But when I convert it by fluentMeshToFoam I can't see the membrane (it is an internal wall
declared as INTERNAL). when I check for
faceSet in order to make the steps written
by "Bernhard Gschaider", I don't find it.
Please can you tel me what should I do step
by step?
1) fluentMeshToFoam . reactor reactor.msh (no problem)
2)??
3)??
Thanks

Is it a 3D mesh? If so, set u
 

Is it a 3D mesh?
If so, set up as usual the Fluent case (with shadow surfaces), save the case in ascii and use the new "fluent3DMeshToFoam" (OpenFOAM 1.4.1) instead.
It should cope with this kind of meshes, now...

Francesco

Hi Danielle! In recent vers
 

Hi Danielle!

In recent versions of fluentMeshToFoam you have to trigger the writing of sets (or zones) with the option -writeSets (or -writeZones). Have you done that? (It's usually a good idea to have a look at the available options with -h if a command does not behave as expected)

Bernhard

PS: liked the quotes around my name which suggest that I'm a fictitious person. Damn, my secret has been revealed ;)

Hi Bernhard and Francesco, Th
 

Hi Bernhard and Francesco,
Thank you for yours answers.
IT WORK NOW!
to Bernhard you are the real one in the Matrix :-)