CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   Running bubbleFoam for turbulent case... (http://www.cfd-online.com/Forums/openfoam/114266-running-bubblefoam-turbulent-case.html)

vishal3 March 8, 2013 01:46

Running bubbleFoam for turbulent case...
 
Hello,

I tried to run bubblefoam for bubble column (the same case with is given in tutorial) simulation for turbulent flow but it is running for some time steps and then diverging. Can anybody help me?????

Bernhard March 8, 2013 04:02

There is probably something wrong with your case.

Sorry, but I can't be more specific than you are. You said you did the tutorial case, but I checked, and that case is laminar, not turbulent.

vishal3 March 8, 2013 07:38

Hey thanks Bernhard

yeah u r right the given case is for laminar. But i changed the model from laminar to kEpsilon in RASproperties in constant (with turbulence on).
Then i added the following schemes for epsilon and k in the fvSchemes:

laplacian(DepsilonEff,epsilon) Gauss linear corrected;
laplacian(DkEff,k) Gauss linear corrected;

after this when i run the simulation again, then it runs for certain timesteps and stops.

I have changed the number of grids from 3000 to 150000. That time also the same thing happens.

Can you suggest something, if possible????

cutter March 8, 2013 09:28

Hi and welcome to the forum,

I also looked into this. The default bubbleFoam tutorial case seems to work fine with kEpsilon turbulence model enabled.

Again, as Berhard already said, be more specific. Which version of OpenFOAM is installed on your machine? What timestep did you use? When does the solution diverge? What changes have you done to the grid? It worked without any modifications for me. We can only assume you somehow changed the discretizations in the blockMeshDict.

By the way, what are grids? At least try to stick to proper english, please.

cutter

vishal3 March 9, 2013 06:25

1 Attachment(s)
Dear Cutter
Currently I am using OpenFOAM 1.6.

For the details of simulation I have attached the files, which are modified accordingly for the case of turbulent.

Please find the attachment and suggest, if any modifications required.

Thankig you.

cutter March 11, 2013 06:41

Ok, that's a really important information. I had no time so far to check your case and OF version. But this what I did to get it running with OpenFOAM 2.1.x (git release):

- use RASModel kEpsilon and enable turbulence in RASProperties
Code:

RASModel  kEpsilon;
turbulence on;

- add laplacian schemes for k and epsilon in fvSchemes (there may be better choices):
Code:

laplacian(DepsilonEff,epsilon) Gauss linear corrected;
laplacian(DkEff,k) Gauss linear corrected;

- add subdictionaries for kFinal and epsilonFinal in fvSolution:
Code:

    kFinal
    {
        $alpha1;
        tolerance      1e-10;
        relTol          0;
    }

    epsilonFinal
    {
        $alpha1;
        tolerance      1e-10;
        relTol          0;
    }


vishal3 March 11, 2013 07:47

Thank you very much for your reply.

I ll try this case with OpenFOAM 2.1

vishal3 March 12, 2013 07:13

Hey dear cutter thank you very much for your suggestion. I think that problem was with OpenFOAM version. I am also getting the results for default case in Version 2.2.

Thanks a lot :)


All times are GMT -4. The time now is 20:17.