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

Problem running simpleFoam with kOmegaSST turbulence model

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

Like Tree1Likes
  • 1 Post By tomf

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 1, 2012, 08:02
Default Problem running simpleFoam with kOmegaSST turbulence model
  #1
Member
 
MB
Join Date: Sep 2012
Posts: 30
Rep Power: 10
matzbanni is on a distinguished road
Hello,
I'm trying to run a channel-case (4m^2) with a smaller cross-section (0.05m^2) in between. My boundary-conditions are:

Code:
inlet_velocity (0.3 0 0)
inlet_pressure zeroGradient
inlet_k uniform 2e-04
inlet_omega uniform 0.2
inlet_nut uniform 0

outlet_velocity zeroGradient
outlet_pressure uniform 0
outlet_k zeroGradient
outlet_omega zeroGradient
outlet_nut uniform 0

wall_velocity (0 0 0)
wall_pressure zeroGradient
wall_k kqRWallFunction uniform 2e-04
wall_omega omegaWallFunction uniform 0.2
wall_nut nutkWallFunction uniform 0
fvSchemes:

Code:
ddtSchemes
{
    default         steadyState;
}

gradSchemes
{
    default         Gauss linear;
}

divSchemes
{
    default         none;
    div(phi,U)      Gauss linear;
    div(phi,k)      Gauss linear;
    div(phi,omega)  Gauss linear;
    div((nuEff*dev(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
    default         Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default         no;
    p;
}
and finally fvSolution:

Code:
solvers
{
    p
    {
        solver           GAMG;
        tolerance        1e-06;
        relTol           0.01;
		smoother	 DICGaussSeidel;
        cacheAgglomeration on;
		agglomerator	 faceAreaPair;
        nCellsInCoarsestLevel 50;
        mergeLevels      1;
    }
    U
    {
        solver           PBiCG;
		preconditioner	 DILU;        
		tolerance        1e-05;
        relTol           0.1;
    }
    k
    {
        solver           PBiCG;
		preconditioner	 DILU;
        tolerance        1e-05;
        relTol           0.1;
    }

    omega
    {
        solver           PBiCG;
        preconditioner 	 DILU;
		tolerance        1e-05;
        relTol           0.1;
    }
}

SIMPLE
{
    nNonOrthogonalCorrectors 0;
}

potentialFlow
{
    nNonOrthogonalCorrectors 10;
}

relaxationFactors
{
    fields
    {
        p               0.3;
    }
    equations
    {
        U               0.7;
        k               0.7;
		epsilon			0.7;
        omega           0.7;
		nuTilda			0.7;
		R				0.7;
    }
}
The problem is that the calculation diverges with bounding k and omega. Any suggestions?
matzbanni is offline   Reply With Quote

Old   November 1, 2012, 09:23
Default
  #2
Senior Member
 
sail's Avatar
 
Vieri Abolaffio
Join Date: Jul 2010
Location: Always on the move.
Posts: 308
Rep Power: 13
sail is on a distinguished road
can you post images of the mesh? have you tried to visualize where the k and omega rises to high values?
__________________
http://www.leadingedge.it/
Naval architecture and CFD consultancy
sail is offline   Reply With Quote

Old   November 1, 2012, 10:15
Default
  #3
Member
 
MB
Join Date: Sep 2012
Posts: 30
Rep Power: 10
matzbanni is on a distinguished road
Quote:
Originally Posted by sail View Post
can you post images of the mesh? have you tried to visualize where the k and omega rises to high values?
there is no defined location where the k and omega values reach the high values. it depends on the timestep... attached you can find two screenshots of a slice through the fluid domain.
Attached Images
File Type: jpg slice1.jpg (75.6 KB, 51 views)
File Type: jpg slice2.jpg (97.5 KB, 55 views)
matzbanni is offline   Reply With Quote

Old   November 1, 2012, 18:15
Default
  #4
Senior Member
 
sail's Avatar
 
Vieri Abolaffio
Join Date: Jul 2010
Location: Always on the move.
Posts: 308
Rep Power: 13
sail is on a distinguished road
mmm the mesh looks good from here,

are the layers correctly added even in the corners?

maybe increasing the number of nonOrtogonalCorrectors in the simple loop?

if the issue arises in the early timesteps you might want to try to increase the value of the initial omega internal field to artificially stabilize the solution.

this is what comes to mind right now...
__________________
http://www.leadingedge.it/
Naval architecture and CFD consultancy
sail is offline   Reply With Quote

Old   November 2, 2012, 18:31
Default
  #5
Member
 
MB
Join Date: Sep 2012
Posts: 30
Rep Power: 10
matzbanni is on a distinguished road
tried to solve it without turbulence, but also no convergence. I have no idea what the problem is...
matzbanni is offline   Reply With Quote

Old   November 3, 2012, 07:45
Default
  #6
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Breda, Netherlands
Posts: 561
Rep Power: 22
tomf will become famous soon enough
Send a message via MSN to tomf Send a message via Skype™ to tomf
Hi,

Just looking at your fvSchemes, try changing:

Code:
divSchemes
{
    default         none;
    div(phi,U)      Gauss linear;
    div(phi,k)      Gauss linear;
    div(phi,omega)  Gauss linear;
    div((nuEff*dev(T(grad(U))))) Gauss linear;
}
to:

Code:
divSchemes
{
    default         none;
    div(phi,U)      Gauss GammaV 0.5;
    div(phi,k)      Gauss Gamma 0.5;
    div(phi,omega)  Gauss Gamma 0.5;
    div((nuEff*dev(T(grad(U))))) Gauss linear;
}
You are now introducing some filtering, because I doubt that you have the required resolution (Cell Reynolds number <2) for pure central differencing (linear scheme). Or maybe look at limitedLinear instead of Gamma.

You may even want to use upwind for the turbulence variables if that is needed for convergence, to my experience the end result is not affected significantly.

Especially if you have a lot of nonOrthogonality this may help:
Code:
laplacianSchemes
{
    default         Gauss linear limited 0.333;
}
Regards,
Tom
blake likes this.
tomf is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
multiphaseInterFoam for RAS turbulence model chiven OpenFOAM Bugs 8 December 6, 2017 03:08
Turbulence model for mixing problem??? nileshjrane Main CFD Forum 7 September 14, 2010 05:57
Turbulence model for mixing problem nileshjrane OpenFOAM Running, Solving & CFD 1 September 7, 2010 18:48
Implementing and running a new turbulence model svens OpenFOAM 3 August 21, 2009 03:59
Why Turbulence models are not universal. Senthil Main CFD Forum 4 July 5, 2000 05:34


All times are GMT -4. The time now is 09:22.