|March 11, 2011, 08:08||
Numerical schemes for free surface flows (VOF)
Bo Terp Paulsen
Join Date: Oct 2010
Posts: 11Rep Power: 4
I am currently working with free surface flows using the interFoam solver.
Unfortunately I have some serious problems with violent instabilities in the air phase and wondered however this is related to the numerical schemes? An Example of the instabilities are shown in this figure. In the figure the velocity field is shown with a contour of the VOF-scalar (gamma=0.5) superimposed. As seen from the figure, vortices are created in the air and the free surface surface is highly distorted. The distortion of the free surface is non-physical and ruin the computations.
So, if anyone has experience with the numerical schemes in relation to the interFoam solver and/or the VOF scheme in general, I will appreciate some advice!
Currently I am using the settings from the damBreak tutorial.
Last edited by botp; March 11, 2011 at 09:57. Reason: Additional information added
|March 11, 2011, 11:28||
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 371Rep Power: 11
Hi Bo Terp, I had same problems solving an sloshing case. I've been solving other cases too and my suggestion would be run with this parameters:
-upwind difference scheme for all div terms.
-5 PISO correctors
-nAlphaCorr no more than 1
-nAlphaSubCycles, no more than 1
-Courant number below or equal to 0.2 (use adjustTimeStep to do that)
once you have a very diffusive but bounded solution both in alpha and U, then try increasing cAlpha and changing the div schemes to which are used in interFoam tutorials.
Let me know of your findings, I'm learning too.
Santiago MÁRQUEZ DAMIÁN, Ph.D.
Research Center for Computational Mechanics (CIMEC) - CONICET/FICH-UNL
T.E.: 54-342-4511594 Ext. 1005
Güemes 3450 - (3000) Santa Fe
Santa Fe - Argentina
|March 11, 2011, 15:27||
Join Date: Aug 2009
Location: Wiesbaden, Germany
Posts: 240Rep Power: 6
Properly you have an unstructured mesh which contains non-orthogonal cells. Can you post the current one? I don't know the exact boundary conditions but I would suggest you set something like
div(rho*phi,U) Gauss limitedLinearV 1;
div(phi,alpha) Gauss vanLeer;
div(phirb,alpha) Gauss interfaceCompression 1;
Alternatively, I can recommend
div(phi,alpha) Gauss limitedLinear 1;
div(phi,alpha) Gauss linearUpwind cellMDLimited Gauss linear 1;
Setting cAlpha 0 means no interface compression, take cAlpha 1. Hasn't that work than increase to 2,3,4 etc.
Last edited by idrama; March 12, 2011 at 02:17.
|numerical scheme, openfoam 1.5-dev, vof model|
|Thread||Thread Starter||Forum||Replies||Last Post|
|free surface of VOF and melting model?||wanghong||FLUENT||3||March 13, 2006 09:57|
|Standard for checking and testing numerical schemes?||X. Ye||Main CFD Forum||7||August 31, 1999 17:05|
|Free Surface Flows / Ocean Waves / Far-field boundary conditions||Sundar Prasad||Main CFD Forum||5||May 4, 1999 10:25|
|free surface flows of submerged objects||yogesh amle||Main CFD Forum||1||March 16, 1999 02:05|
|Modeling Free Surface Flows||Elliot Schwartz||Main CFD Forum||5||August 25, 1998 21:03|