CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Interior surfaces in OpenFOAM (http://www.cfd-online.com/Forums/openfoam-solving/87405-interior-surfaces-openfoam.html)

claco April 19, 2011 11:48

Interior surfaces in OpenFOAM
 
Dear Sirs,

I have created a mesh with a commercial grid generator. Its format is .msh
(Fluent format). Then I have imported it into OpenFOAM environment.
The problem lies in that the internal surfaces can be imported with fluent3DMeshToFoam, but once imported, I have to declare a specific boundary condition for those.
Is there a procedure that allows me to declare those surfaces as "interior" (as in Fluent) surfaces?

Yours Sincerely,

Claudio

gwierink April 20, 2011 02:56

Dear Claudio,

I have had a similar problem and using fluentMeshToFoam instead of fluent3DMeshToFoam, with the -writeSets and -writeZones options, worked for me.

Code:

Usage: fluentMeshToFoam <Fluent mesh file> [-writeSets] [-writeZones] [-scale scale factor] [-case dir]  [-help] [-doc] [-srcDoc]
That is, for myMesh.msh in millimeters, I do:

Code:

fluentMeshToFoam myMesh.msh -writeSets -writeZones -scale 0.001
Hope it's of any help!

claco April 20, 2011 03:13

Quote:

Originally Posted by gwierink (Post 304334)
Dear Claudio,

I have had a similar problem and using fluentMeshToFoam instead of fluent3DMeshToFoam, with the -writeSets and -writeZones options, worked for me.

Code:

Usage: fluentMeshToFoam <Fluent mesh file> [-writeSets] [-writeZones] [-scale scale factor] [-case dir]  [-help] [-doc] [-srcDoc]
That is, for myMesh.msh in millimeters, I do:

Code:

fluentMeshToFoam myMesh.msh -writeSets -writeZones -scale 0.001
Hope it's of any help!


Thank You very much gwierink.

One question: with the -writeSets -writeZones options, are these interior faces retained or discarded? Because I need they are present during simulation since I make use of them during postprocessing.

In fact, I know that fluentMeshToFoam usage (alone, without any additional options) does not allow to retain interior surfaces.

Yours sincerely,

Claudio

gwierink April 20, 2011 03:30

Hi Claudio,

If your mesh contains sets of vertices/edges describing faces, then it should work. Have a try. Also, have a look at this thread, where fluentMeshToFoamWithInternals is discussed. The thread is pretty old, so I think it is included in the standard converter now, but I'm not sure. Just have a go :).

bastil April 20, 2011 05:30

Well....

default interiors which you do not need for postprocessing can be ignored using fluent3DMeshToFoam. The one you want to keep for postprocessing, ... need to be defined as a "fan" B.C. type in the grid generator BEFORE running fluent3DMeshToFoam. All the other "interior" types will be skipped by the converter.
Afterwards you need to define them as a "cyclic" B.C. in OpenFOAM.

Hope this helps.

Regards Bastian

claco April 20, 2011 06:03

Quote:

Originally Posted by bastil (Post 304363)
Well....

default interiors which you do not need for postprocessing can be ignored using fluent3DMeshToFoam. The one you want to keep for postprocessing, ... need to be defined as a "fan" B.C. type in the grid generator BEFORE running fluent3DMeshToFoam. All the other "interior" types will be skipped by the converter.
Afterwards you need to define them as a "cyclic" B.C. in OpenFOAM.

Hope this helps.

Regards Bastian


Thank You Bastian,

if I have understood correctly, if I want to make an internal surface "transparent" to the flux I have simply to define for it a "type cyclic" b.c. in files p, U, T k omega..?

Yours Sincerely,


Claudio

kalyangoparaju July 23, 2012 14:51

Claudio,

I know it is too late but did that suggestion help? i.e. setting them to cyclic.

Kalyan


All times are GMT -4. The time now is 12:20.