CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   compressibleInterDyMFoam on OF1.6 (http://www.cfd-online.com/Forums/openfoam-solving/68148-compressibleinterdymfoam-of1-6-a.html)

lucadauria September 8, 2009 10:03

compressibleInterDyMFoam on OF1.6
 
Has anybody experience with compressibleInterDyMFoam on OF1.6? I was not able to find any specific documentation.

I tried using the dynamicMeshDict in the tutorial damBreakWithObstacle for interDyMFoam but it does not work with compressibleInterDyMFoam.

Thanks

scttmllr February 22, 2010 13:25

Luca: Any luck with compressibleInterDyMFoam? I am having the same problems you described.

scttmllr February 24, 2010 21:18

compressibleInterDyMFoam -- dynamicRefineFvMesh
 
I have found 2 issues that caused problems when trying to use AMR with compressibleInterDyMFoam.

1. There are 3 constructors in createFields.H that need to be modified so that they get updated as the mesh refines: alpha2, rho1, rho2. Example:

//Old:
//volScalarField alpha2("alpha2", scalar(1) - alpha1);

//New:
volScalarField alpha2
(
IOobject
(
"alpha2",
runTime.timeName(),
mesh,
IOobject::NO_READ,
IOobject::NO_WRITE
),
scalar(1) - alpha1
);

2. You cannot use the GAMG solver for p and pFinal. However, as we are not solving a pressure Poisson equation, it should suffice to use a smoothSolver, etc, as multi-grid is more suited to elliptic PDEs. Using GAMG for the pcorr equation is fine here, since we are using an elliptic correction to the flux to ensure continuity when we update the mesh.

Hope this helps.


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