CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

interFoam: hydrostatic pressure drives flow in non-orthogonal mesh

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 11, 2010, 05:23
Default interFoam: hydrostatic pressure drives flow in non-orthogonal mesh
  #1
New Member
 
Kasper Kærgaard
Join Date: May 2010
Posts: 5
Rep Power: 7
kaergaard is on a distinguished road
Dear Forum.
I have a problem wiith interFoam. With a plane water surface and no flow trough any boundaries I get a flow along the bottom boundary when the mesh elements near the boundary are non-orthogonal. I expected zero velocity everywhere.
The flow velocity increases as time goes and ends up blowing up the computation. I have attatched an image showing the same simulation with slightly different meshes the top one has a maximum non-orthogonality of 65, the middle 35 and the bottom 15 (mesh is made using snappyMesh). The shown time is 0.01 s.
I would like to be able to run the simulaiton with a larger non-orthogonality since this will describe my bottom better. I have tried
nOrthoCorrectors = 5, with no improvement, I have also tried different combinations of schemes for laplace (MUSCL uncorrected, corrected linear, upwind), and div (MUSCL, upwind, linear). Any ideas are most welcome.

Best regards Kasper


My fvSolution file is:
solvers
{
pcorr PCG
{
preconditioner DIC;
tolerance 1e-10;
relTol 0;
};
p PCG
{
preconditioner DIC;
tolerance 1e-10;
relTol 0;
};
pFinal PCG
{
preconditioner DIC;
tolerance 1e-10;
relTol 0;
};
U PBiCG
{
preconditioner DILU;
tolerance 1e-10;
relTol 0;
};
}

PISO
{
pdRefCell 0;
pdRefValue 0;
momentumPredictor yes;
nCorrectors 3;
nNonOrthogonalCorrectors 5;
nAlphaCorr 1;
nAlphaSubCycles 1;
cAlpha 1;
}
fvSchemes:
ddtSchemes
{
default Euler;
}

gradSchemes
{
default Gauss linear;
grad(U) Gauss linear;
grad(alpha) Gauss linear;
}

divSchemes
{
default Gauss linear;
// div(rho*phi,U) Gauss MUSCL;
// div(phi,alpha) Gauss vanLeer;
// div(phirb,alpha) Gauss interfaceCompression;
}

laplacianSchemes
{
default Gauss upwind phi corrected;
}

interpolationSchemes
{
default linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default yes;
p;
pcorr;
alpha;
}
Attached Images
File Type: jpg image.jpg (23.3 KB, 92 views)
kaergaard is offline   Reply With Quote

Old   September 28, 2010, 12:40
Default
  #2
New Member
 
afshar
Join Date: Jan 2010
Posts: 5
Rep Power: 7
m.afshar is on a distinguished road
Hi Casper

I have faced the same problem as you. The case is a 3D wave tank with a sloping bed. For a simple test (still water in the basin with hydrostatic pressure and no wave) interFoam gives non-physical flows over and around the sloping bed. The DeltaT decreases continuously and finally the run blows up.
Could you please kindly tell me if you have found any way out of this problem?

Best Regards
Mostafa
m.afshar is offline   Reply With Quote

Old   September 29, 2010, 05:17
Default
  #3
New Member
 
Kasper Kærgaard
Join Date: May 2010
Posts: 5
Rep Power: 7
kaergaard is on a distinguished road
As I remember: use quad as grad scheme
kaergaard is offline   Reply With Quote

Old   September 5, 2011, 10:56
Default Could you explain how you solve the problem?
  #4
Member
 
Charlie
Join Date: Dec 2010
Location: 415 Kinross Dr. Newark, DE 19711
Posts: 78
Rep Power: 6
cheng1988sjtu is on a distinguished road
Hi kaergaard,

Could you explain a little bit about the gradScheme : quad?
Since I'm sending wave into a box at one inlet, and top as atmosphere, other 4 walls. however, It keeps blowing up after few seconds of simulation.
Could you share with us how you solve the problem? Thanks !

Zhen

Quote:
Originally Posted by kaergaard View Post
As I remember: use quad as grad scheme
cheng1988sjtu is offline   Reply With Quote

Old   September 6, 2011, 01:09
Default
  #5
New Member
 
Kasper Kærgaard
Join Date: May 2010
Posts: 5
Rep Power: 7
kaergaard is on a distinguished road
An even better solution to solve the original problem in this thread is to upgrade to openfoam 1.7.x where the formulation in interfoam has been changed back so it again (like in 1.5.x) solve for excess pressure. Since I switched to 1.7.x I have not has the problem.

Zhen: I don't think I can help with your wave simulation which is blowing up, but an idea is to use upwing scheme for all your divergence schemes and all your interpolation schemes.
kaergaard is offline   Reply With Quote

Old   September 6, 2011, 07:39
Wink Thanks, runs wells now!
  #6
Member
 
Charlie
Join Date: Dec 2010
Location: 415 Kinross Dr. Newark, DE 19711
Posts: 78
Rep Power: 6
cheng1988sjtu is on a distinguished road
Hi kaergaard,

Thank you very much for your advice!
right now, I'm using CrankNicholson as ddtScheme,
fourth as gradScheme, and Gauss linearUpwind cellLimited Causs linear 1 as div(rho*phi,U) , and it runs well now.


Quote:
Originally Posted by kaergaard View Post
An even better solution to solve the original problem in this thread is to upgrade to openfoam 1.7.x where the formulation in interfoam has been changed back so it again (like in 1.5.x) solve for excess pressure. Since I switched to 1.7.x I have not has the problem.

Zhen: I don't think I can help with your wave simulation which is blowing up, but an idea is to use upwing scheme for all your divergence schemes and all your interpolation schemes.
cheng1988sjtu is offline   Reply With Quote

Reply

Tags
hydrostatic, interfoam, non-orthogonal

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
simple model, difficult outlet Eric CFX 7 May 23, 2014 08:13
mesh file for flow over a circular cylinder Ardalan Main CFD Forum 6 April 17, 2010 23:40
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10
Gas pressure question Dan Moskal Main CFD Forum 0 October 24, 2002 22:02
Hydrostatic pressure in 2-phase flow modeling (CFX4.2) HB &DS CFX 0 January 9, 2000 14:19


All times are GMT -4. The time now is 12:24.