CFD Online URL
[Sponsors]
Home > Forums > OpenFOAM

Downwind

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 29, 2010, 16:40
Question Can you set downwind cell centre value on faces?
  #1
Member
 
Fran
Join Date: Sep 2009
Location: Buenos Aires
Posts: 35
Rep Power: 7
lfbarcelo is on a distinguished road
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 17:04.
lfbarcelo is offline   Reply With Quote

Old   March 30, 2010, 05:29
Default
  #2
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 11
eugene is on a distinguished road
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?
eugene is offline   Reply With Quote

Old   March 30, 2010, 14:11
Default
  #3
Member
 
Fran
Join Date: Sep 2009
Location: Buenos Aires
Posts: 35
Rep Power: 7
lfbarcelo is on a distinguished road
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?
lfbarcelo is offline   Reply With Quote

Old   March 30, 2010, 14:16
Default
  #4
Member
 
Fran
Join Date: Sep 2009
Location: Buenos Aires
Posts: 35
Rep Power: 7
lfbarcelo is on a distinguished road
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
lfbarcelo is offline   Reply With Quote

Old   March 31, 2010, 06:51
Default
  #5
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 11
eugene is on a distinguished road
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;
eugene is offline   Reply With Quote

Old   April 1, 2010, 10:12
Default
  #6
Member
 
Fran
Join Date: Sep 2009
Location: Buenos Aires
Posts: 35
Rep Power: 7
lfbarcelo is on a distinguished road
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.
lfbarcelo 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
Actuator disk model audrich FLUENT 0 September 21, 2009 08:06
Where's the singularity/mesh flaw? audrich FLUENT 3 August 4, 2009 02:07
Compiling with Intel compiler icc90 hjasak OpenFOAM Installation 19 October 27, 2007 12:35
Higher order downwind scheme jelmer OpenFOAM Running, Solving & CFD 4 August 9, 2006 07:43


All times are GMT -4. The time now is 16:00.