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

buoyantSimpleFoam velocity oszillation 1.6-ext

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 12, 2011, 03:56
Default buoyantSimpleFoam velocity oszillation 1.6-ext
  #1
Member
 
Stefan
Join Date: Jun 2009
Posts: 67
Rep Power: 8
preibie is on a distinguished road
Hallo user ans developer of OpenFOAM 1.6-ext,

I want to simulate a room without any inlets and outlets only with a heat source on the ground. I choose the buoyantSimpleFoam solver. The steps I had done:
  1. build and mesh the domain with Gambit
  2. checkMesh OK (nonOrthogonality max = 63)
  3. buoyantSimpleFoam: after 200 Iterations there are nonphysical oszillations (+-0.04 m/s) in the velocity fild (picture)
  4. simpleFoam: same mesh the oszilations are very low (+- 1e-7) (picture)

Is this a problem with the mesh ore with buoyantSimpleFoam?

Preibie
Attached Images
File Type: jpg buoyantSimpleFoam.jpg (92.7 KB, 32 views)
File Type: jpg simpleFoam.jpg (87.2 KB, 25 views)
preibie is offline   Reply With Quote

Old   May 13, 2011, 02:54
Exclamation
  #2
Member
 
Stefan
Join Date: Jun 2009
Posts: 67
Rep Power: 8
preibie is on a distinguished road
Some more informations about the last hours:

We tryed something more. We changed the mesh (only the mesh) and used a hex grid. What I can say all was fine, no oscillations.
Why I'm confused: The first mesh passed checkMesh!
Next step: we convert the hex mesh with tetDecomposition into a tet Mesh. This mesh passed also checkMesh (nonOrthogonality max = 44 average = 18). It seems that this mesh is good enough, no oszillations!

Is the threshold (70) of nonOrthogonality to high?
preibie is offline   Reply With Quote

Old   May 13, 2011, 03:49
Default
  #3
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Hi,
you should also list the schemes you are using. On tet meshes you often need to turn on limiters which are off by default in OpenFOAM.
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   May 13, 2011, 03:58
Default
  #4
Member
 
Stefan
Join Date: Jun 2009
Posts: 67
Rep Power: 8
preibie is on a distinguished road
fvSchemes:

Code:
ddtSchemes
{
    default         Euler;
}

gradSchemes
{
    default         Gauss linear;
}

divSchemes
{

    div(phiU,p)                    Gauss upwind;
    //div(phi,U)                     Gauss upwind;
    div(phi,U)                     Gauss reconCentral cellLimited leastSquares 1.0;
    div(phi,h)                     Gauss upwind;
    div(phi,k)                     Gauss upwind;
    div(phi,epsilon)               Gauss upwind;
    div((muEff*dev2(grad(U).T()))) Gauss linear;
}

laplacianSchemes
{
    default         Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
    interpolate(U)  reconCentral phi leastSquares;    //für tetraeder Gitter von Jasak
}

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default         no;
    p               ;
}
preibie is offline   Reply With Quote

Old   May 13, 2011, 04:09
Default
  #5
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
I would try:

Code:
gradSchemes
{
    default         cellLimited leastSquares 1; 
}

divSchemes
{
    div(phi,U)                     Gauss linearUpwindV cellLimited leastSquares 1;
    div(phiU,p)                    Gauss upwind;
    div(phi,h)                      Gauss upwind;
    div(phi,k)                      Gauss upwind;
    div(phi,epsilon)               Gauss upwind;
    div((muEff*dev2(grad(U).T()))) Gauss linear;
}
Note that in your schemes, you are using inconsistent gradient formulations. Additionally, if leastSquares gives you problems, replace it with Gauss linear, which will reduce the accuracy, but tends to be more robust.

I hope this helps.
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Reply

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
help with UDF for contact angle based on contact line velocity gandesk Fluent UDF and Scheme Programming 14 October 29, 2012 14:58
Neumann pressure BC and velocity field Antech Main CFD Forum 0 April 25, 2006 02:15
Velocity Under-relaxation in SIMPLE type methods Matt U. Main CFD Forum 6 July 4, 2005 05:29
Terrible Mistake In Fluid Dynamics History Abhi Main CFD Forum 12 July 8, 2002 09:11
Convection velocity of Coherent structures Jongdae Kim Main CFD Forum 3 February 5, 2002 05:04


All times are GMT -4. The time now is 12:25.