CFD Online Discussion Forums - Fluent result reports

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Post-Processing (https://www.cfd-online.com/Forums/openfoam-post-processing/)

- - Fluent result reports (https://www.cfd-online.com/Forums/openfoam-post-processing/132063-fluent-result-reports.html)

Fluent result reports

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?

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

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.

Quote:

Originally Posted by jherb (Post 498600)

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;

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.