|
[Sponsors] |
March 29, 2010, 15:40 |
Can you set downwind cell centre value on faces?
|
#1 |
Member
Fran
Join Date: Sep 2009
Location: Buenos Aires
Posts: 37
Rep Power: 17 |
I'm trying to modify the code in one of the solvers to suit it for my particular case.
In order to determine the velocity value in the faces of the finite volumes, the solver interpolates it's value in the cell centres. mesh.Sf() & fvc::interpolate(U) Instead of this interpolated value on the faces I need the downwind value on each face. This means that the face should not take an interpolated value between the cell centres, but the value corresponding to the downwind cell centre. Is there a known function to do this? Thank You. Best Regards. Last edited by lfbarcelo; March 29, 2010 at 16:04. |
|
March 30, 2010, 04:29 |
|
#2 |
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 21 |
Sure,
fvc::interpolate(U, word("Udownwind")); And then add Udownwind downwind; to the interpolationSchemes section of the fvSchemes dictionary. What is this for if I may ask? |
|
March 30, 2010, 13:11 |
|
#3 |
Member
Fran
Join Date: Sep 2009
Location: Buenos Aires
Posts: 37
Rep Power: 17 |
I did everithing you said and the application compiled perfectly but when I try to run the case I get the next error message:
--> FOAM FATAL IO ERROR: attempt to read beyond EOF file: /home/user/OpenFOAM/user-1.6.x/run/tanque/system/fvSchemes::interpolationSchemes::default at line 50. From function ITstream::read(token& t) in file db/IOstreams/Tstreams/ITstream.C at line 84. FOAM exiting Any Ideas? |
|
March 30, 2010, 13:16 |
|
#4 |
Member
Fran
Join Date: Sep 2009
Location: Buenos Aires
Posts: 37
Rep Power: 17 |
sorry, my mistake, this is the error message I get:
--> FOAM FATAL IO ERROR: attempt to read beyond EOF file: /home/user/OpenFOAM/user-1.6.x/run/tanque/system/fvSchemes::interpolationSchemes::Udownwind at line 51. From function ITstream::read(token& t) in file db/IOstreams/Tstreams/ITstream.C at line 84. FOAM exiting |
|
March 31, 2010, 05:51 |
|
#5 |
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 21 |
Normally you get this error if there is a missing entry or ";". The code in downwind.H indicates that you need an entry for the name of the flux:
Udownwind downwind phi; |
|
April 1, 2010, 09:12 |
|
#6 |
Member
Fran
Join Date: Sep 2009
Location: Buenos Aires
Posts: 37
Rep Power: 17 |
Thanks eugene, both answers were really usefull. Downwind is working. I needed it to test different results in drift flux equations. The transport of alpha seems to work better, concerning mass conservation, when useing a downwind scheme.
|
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Actuator disk model | audrich | FLUENT | 0 | September 21, 2009 07:06 |
Where's the singularity/mesh flaw? | audrich | FLUENT | 3 | August 4, 2009 01:07 |
Compiling with Intel compiler icc90 | hjasak | OpenFOAM Installation | 19 | October 27, 2007 11:35 |
Higher order downwind scheme | jelmer | OpenFOAM Running, Solving & CFD | 4 | August 9, 2006 06:43 |