CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Post-Processing

Fluent result reports

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 25, 2014, 07:08
Default Fluent result reports
  #1
Member
 
Jiri
Join Date: Mar 2014
Posts: 73
Rep Power: 4
Jiricbeng is on a distinguished road
Hello,

after computing pitzDaily case in openfoam I converted the results by using foamMeshToFluent and foamDataToFluent and recieved .msh and .dat. In Fluent I can see velocity vectors and pressure contours. But when I click Report -> Result Reports -> Fluxes and I choose inlet and outlet and push compute, the mass flow through inlet and outlet is zero.
Where is the mistake?
Jiricbeng is offline   Reply With Quote

Old   May 20, 2014, 08:00
Default
  #2
New Member
 
Sylvain Clavreul
Join Date: Apr 2014
Location: France
Posts: 2
Rep Power: 0
SylvainC is on a distinguished road
Hello Foamers,

I have the same problem: converting Foam results with foamDataToFluent gives a zero mass flow rate at inlet and outlet even if the rest of the results looks fine.
The problem for me is that I can't add a UDS transport at the inlet because it is not advected by the flux. It seems like the data conversion missed the flux or the density.

Did anyone face this problem and resolve it?

Thanks
SylvainC is offline   Reply With Quote

Old   June 25, 2014, 07:49
Default
  #3
Senior Member
 
Joachim Herb
Join Date: Sep 2010
Posts: 375
Rep Power: 10
jherb is on a distinguished road
You might have to correct your system/foamDataToFluentDict. What are your settings there?

I use the following
Code:
p               1;

U               2;

U.X             111;
U.Y             112;
U.Z             113;

T               3;

h               4;

k               5;

epsilon         6;

gamma           150;
If you look in OpenFOAM-x.x.x/applications/utilities/postProcessing/dataConversion/foamDataToFluent/fluentUnitNumbers.txt you can see the internal numbers used by fluent. There is also something call XF_RF_DATA_MASS_FLUX=18 which you might need to convert, but this is just a guess.
jherb is offline   Reply With Quote

Old   July 7, 2014, 03:57
Default
  #4
New Member
 
Sylvain Clavreul
Join Date: Apr 2014
Location: France
Posts: 2
Rep Power: 0
SylvainC is on a distinguished road
Quote:
Originally Posted by jherb View Post
You might have to correct your system/foamDataToFluentDict. What are your settings there?

I use the following
Code:
p               1;

U               2;

U.X             111;
U.Y             112;
U.Z             113;

T               3;

h               4;

k               5;

epsilon         6;

gamma           150;
If you look in OpenFOAM-x.x.x/applications/utilities/postProcessing/dataConversion/foamDataToFluent/fluentUnitNumbers.txt you can see the internal numbers used by fluent. There is also something call XF_RF_DATA_MASS_FLUX=18 which you might need to convert, but this is just a guess.
You are right jherb, but even with all correct unit numbers, it doesn't work.

I contacted Ansys Fluent support, and the answer they gave me is that when you convert the data, each cell of the mesh receive its value, but the flux and gradients must be rebuilt, and the only possibility to do that is by restarting the calculation with Fluent.

In short, with OpenFoam results converted to Fluent, we can't have direct access to some result reports such as mass flow through surfaces.
SylvainC 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
How to start Fluent with Matlab?? Jay Hu FLUENT 5 October 9, 2013 14:20
Fluent Vs Star CCM firda Main CFD Forum 3 February 26, 2011 03:51
Setup for Fluent Flux Reports Jallen13a FLUENT 7 November 18, 2010 11:32
few quesions on ANSYS ICEMCFD and FLUENT Prakash.Paudel ANSYS 0 August 12, 2010 12:07
Fluent 6.3.26 vs 12.1 and partition method Anorky FLUENT 0 April 27, 2010 10:55


All times are GMT -4. The time now is 14:59.