CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Verification & Validation (https://www.cfd-online.com/Forums/openfoam-verification-validation/)
-   -   bubble rising grid study problem! (https://www.cfd-online.com/Forums/openfoam-verification-validation/156963-bubble-rising-grid-study-problem.html)

mreza_cfd July 16, 2015 08:44
bubble rising grid study problem!
 
4 Attachment(s)
Dear Foam Users,


I did a simple run: 2d bubble rising with solver interFoam.
The problem is that when I run on a finer mesh, the results have more error with comparison to Hysing et al.*

Do you know why?!


You can see the code and results in attachment.


Thanks a lot in advance!

ssss July 16, 2015 11:19
Well did you play with the values of cAlpha, nAlphaCorrs, and with the convective scheme? Which is the VOF approximation used in the article of reference? You should also play with the maxCourant number because the compressive VOF scheme used in OpenFOAM is quite dependant on the timestep

mreza_cfd July 17, 2015 03:49
Quote:
Originally Posted by ssss (Post 555758)
Well did you play with the values of cAlpha, nAlphaCorrs, and with the convective scheme? Which is the VOF approximation used in the article of reference? You should also play with the maxCourant number because the compressive VOF scheme used in OpenFOAM is quite dependant on the timestep
I do not exactly know about cAlpha, nAlphaCorr! could you please explain more?
I didn't change setting because I'm not familiar with OpenFoam yet!
but I changed maxCourant number and now I am waiting for the results!

Is it possible for you to recommend me any source or documentation about VOF of OpenFoam.
I know about CFD and VOF method but I am new to OpenFoam!

Thanks

mreza_cfd July 17, 2015 04:22
by the way, is there a criteria for maxcourant number when we use VOF?

ssss July 22, 2015 17:23
You will find plenty of information of the VOF openfoam implementation in the following papers of the splendid guy Santiago Damián Márquez:

http://infofich.unl.edu.ar/upload/3b...7523c8ea52.pdf

https://www.google.es/url?sa=t&rct=j...o5pnjV9r0Whaaw


In OpenFOAM the VOF formulation is treated adding a compressive term to the advection equation of alpha. This term uses a parameter called cAlpha. cAlpha should not be less than 0 and also it shouldn't be bigger than 2 (maybe other values might work for you). Higher values of cAlpha mean that the interface liquid-gas will be thinner, and lower values of cAlpha mean that the interface would be thicker and thus that there would be more cells which define the interface.

The value of nAlphaSubCycles and nAlphaCorrs determine the way in which the MULES approach will be used to solve the advection equation. You might find more information in the forum and in the links I posted. Basically a higher number of nAlphaSubCycles could allow you to use higher Courant number, but it is not always the case.

About the maximun courant number in VOF simulations in OpenFOAM, it depends on the type of simulation. There are lots of papers in which one can see that the VOF approach in OpenFOAM is quite influenced by the maximumCourant number in the domain. In this paper:

Volume of fluid methods for immiscible-fluid and free-surface flows
Vinay R. Gopala ∗, Berend G.M. van Wachem

You will find a comparation of the different VOF techniques and as well, you will see that the compressive VOF is very dependant on the Courant number.

So you should play a lot with the parameters such as maxCo and maxAlphaCo, discretization schemes, etc.

Start using maxCo and maxAlphaCo of 0.1 and then try to up or lower the values and see what happens. Which are you discretization schemes?

mreza_cfd July 25, 2015 22:46
2 Attachment(s)
Quote:
Originally Posted by ssss (Post 556586)
Start using maxCo and maxAlphaCo of 0.1 and then try to up or lower the values and see what happens.
Thanks!
I changed maxCo and maxAlphaCo to 0.1 and the result does not change but when I changed to 0.01 and 0.001 the results improved dramatically!

mreza_cfd July 25, 2015 22:49
my discretization schemes are:
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  2.3.0                                |
|  \\  /    A nd          | Web:      www.OpenFOAM.org                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version    2.0;
    format      ascii;
    class      dictionary;
    location    "system";
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default        Euler;
}

gradSchemes
{
    default        Gauss linear;
}

divSchemes
{
    div(rhoPhi,U)  Gauss linearUpwind grad(U);
    div(phi,alpha)  Gauss vanLeer;
    div(phirb,alpha) Gauss linear;
    div((muEff*dev(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
    default        Gauss linear corrected;
}

interpolationSchemes
{
    default        linear;
}

snGradSchemes
{
    default        corrected;
}

fluxRequired
{
    default        no;
    p_rgh;
    pcorr;
    alpha.water;
}


// ************************************************************************* //
and I didn't change it.
If you have an idea I can test it!!

ssss July 26, 2015 09:41
Well your results seem to be quite similar to the ones in the article so I would not touch more things if you want to validate data from the article.

Anyway you could try to use different schemes for the div(rhoPhi,U) term:

1) vanLeer
2) limitedLinear 0.5
3) limitedLinear 1

Maybe you could also try modifying the fvSolution file, modifying convergence tolerances and the workflow of the PIMPLE algorithm. I can help you with it if you want


All times are GMT -4. The time now is 09:49.