CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Verification & Validation

bubble rising grid study problem!

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

Like Tree7Likes
  • 2 Post By mreza_cfd
  • 1 Post By ssss
  • 3 Post By ssss
  • 1 Post By ssss

Reply
 
LinkBack Thread Tools Display Modes
Old   July 16, 2015, 08:44
Default bubble rising grid study problem!
  #1
New Member
 
Mohammad reza
Join Date: Jul 2015
Posts: 7
Rep Power: 3
mreza_cfd is on a distinguished road
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!


Attached Images
File Type: png bubble rising.PNG (24.7 KB, 41 views)
File Type: png Position of bubble.PNG (21.4 KB, 47 views)
File Type: png rise velosity grid 300-600.PNG (14.0 KB, 44 views)
Attached Files
File Type: zip bubble rising.zip (9.4 KB, 19 views)
BlnPhoenix and Sarang like this.
mreza_cfd is offline   Reply With Quote

Old   July 16, 2015, 11:19
Default
  #2
Senior Member
 
anonymous
Join Date: Aug 2014
Posts: 198
Rep Power: 4
ssss is on a distinguished road
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 likes this.
ssss is offline   Reply With Quote

Old   July 17, 2015, 03:49
Default
  #3
New Member
 
Mohammad reza
Join Date: Jul 2015
Posts: 7
Rep Power: 3
mreza_cfd is on a distinguished road
Quote:
Originally Posted by ssss View Post
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

Last edited by mreza_cfd; July 17, 2015 at 04:51.
mreza_cfd is offline   Reply With Quote

Old   July 17, 2015, 04:22
Default
  #4
New Member
 
Mohammad reza
Join Date: Jul 2015
Posts: 7
Rep Power: 3
mreza_cfd is on a distinguished road
by the way, is there a criteria for maxcourant number when we use VOF?
mreza_cfd is offline   Reply With Quote

Old   July 22, 2015, 17:23
Default
  #5
Senior Member
 
anonymous
Join Date: Aug 2014
Posts: 198
Rep Power: 4
ssss is on a distinguished road
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?
liu-t11, mreza_cfd and lowlow like this.
ssss is offline   Reply With Quote

Old   July 25, 2015, 22:46
Default
  #6
New Member
 
Mohammad reza
Join Date: Jul 2015
Posts: 7
Rep Power: 3
mreza_cfd is on a distinguished road
Quote:
Originally Posted by ssss View Post
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!
Attached Images
File Type: png Grid 300-600 max Co=0.01.PNG (17.0 KB, 43 views)
File Type: png Grid 300-600 max Co=0.001.PNG (17.2 KB, 39 views)
mreza_cfd is offline   Reply With Quote

Old   July 25, 2015, 22:49
Default
  #7
New Member
 
Mohammad reza
Join Date: Jul 2015
Posts: 7
Rep Power: 3
mreza_cfd is on a distinguished road
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!!
mreza_cfd is offline   Reply With Quote

Old   July 26, 2015, 09:41
Default
  #8
Senior Member
 
anonymous
Join Date: Aug 2014
Posts: 198
Rep Power: 4
ssss is on a distinguished road
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
mreza_cfd likes this.
ssss is offline   Reply With Quote

Reply

Tags
bubble, bubble rising, interfoam

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
bubble rising grid study problem! mreza_cfd OpenFOAM Running, Solving & CFD 0 July 15, 2015 08:50
Shear rate distribution around rising bubble Agis Fluent Multiphase 0 June 29, 2015 04:19
grid study, important question hamid1 FLUENT 1 August 4, 2013 00:14
Problem of simulating shape oscillations of Bubble - Multiphase flow akash FLUENT 2 January 29, 2013 14:46
Problem with Grid convergence study dialolema CFX 1 June 14, 2010 18:33


All times are GMT -4. The time now is 19:07.