CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Interior surfaces in OpenFOAM

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   April 19, 2011, 11:48
Default Interior surfaces in OpenFOAM
  #1
Member
 
Claudio
Join Date: Mar 2010
Posts: 57
Rep Power: 7
claco is on a distinguished road
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
claco is offline   Reply With Quote

Old   April 20, 2011, 02:56
Default
  #2
Senior Member
 
Gijsbert Wierink
Join Date: Mar 2009
Posts: 383
Rep Power: 9
gwierink is on a distinguished road
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!
__________________
Regards, Gijs
gwierink is offline   Reply With Quote

Old   April 20, 2011, 03:13
Default
  #3
Member
 
Claudio
Join Date: Mar 2010
Posts: 57
Rep Power: 7
claco is on a distinguished road
Quote:
Originally Posted by gwierink View Post
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
claco is offline   Reply With Quote

Old   April 20, 2011, 03:30
Default
  #4
Senior Member
 
Gijsbert Wierink
Join Date: Mar 2009
Posts: 383
Rep Power: 9
gwierink is on a distinguished road
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 .
__________________
Regards, Gijs
gwierink is offline   Reply With Quote

Old   April 20, 2011, 05:30
Default
  #5
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 471
Rep Power: 11
bastil is on a distinguished road
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
bastil is offline   Reply With Quote

Old   April 20, 2011, 06:03
Default
  #6
Member
 
Claudio
Join Date: Mar 2010
Posts: 57
Rep Power: 7
claco is on a distinguished road
Quote:
Originally Posted by bastil View Post
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
claco is offline   Reply With Quote

Old   July 23, 2012, 14:51
Default
  #7
Member
 
Kalyan
Join Date: Oct 2011
Location: Columbus, Ohio
Posts: 53
Blog Entries: 1
Rep Power: 5
kalyangoparaju is on a distinguished road
Claudio,

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

Kalyan
kalyangoparaju is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Cross-compiling OpenFOAM 1.7.0 on Linux for Windows 32 and 64bits with Mingw-w64 wyldckat OpenFOAM Announcements from Other Sources 3 September 8, 2010 06:25
Modified OpenFOAM Forum Structure and New Mailing-List pete Site News & Announcements 0 June 29, 2009 05:56
64bitrhel5 OF installation instructions mirko OpenFOAM Installation 2 August 12, 2008 18:07
Adventure of fisrst openfoam installation on Ubuntu 710 jussi OpenFOAM Installation 0 April 24, 2008 14:25
OpenFOAM Debian packaging current status problems and TODOs oseen OpenFOAM Installation 9 August 26, 2007 13:50


All times are GMT -4. The time now is 03:47.