simpleFoam convergence issue

Harnoor · March 1, 2016, 01:15

I am new to OpenFoam. I am trying to simulate flow over a 3-d wing (sd 6060 airfoil) at Re=80000. I have created my mesh in icem-cfd and imported it in Openfoam. I am using k omega SST model and I have specified all boundary conditions to the best of my knowledge. I am using simpleFoam as the solver. The solution does not converge and I am getting completely wrong results. I am pasting my case files below. Can someone please take a look and tell me where the problem is? Any help would be greatly appreciated.

k
internalField uniform 2.77e-8;

boundaryField
{
near_side
{
type symmetryPlane;
}
far_side
{
type fixedValue;
value uniform 2.77e-8;
}
outlet
{
type fixedValue;
value uniform 2.77e-8;
}
inlet
{
type fixedValue;
value uniform 2.77e-8;
}
wing_surface
{
type kqRWallFunction;
value uniform 1e-11;
}
wing_tip
{
type kqRWallFunction;
value uniform 1e-11;
}
}

omega
internalField uniform 3.28;

boundaryField
{
near_side
{
type symmetryPlane;
}
far_side
{
type fixedValue;
value uniform 3.28;
}
outlet
{
type fixedValue;
value uniform 3.28;
}
inlet
{
type fixedValue;
value uniform 3.28;
}
wing_surface
{
type omegaWallFunction;
value uniform 2.688e6;
}
wing_tip
{
type omegaWallFunction;
value uniform 1.421e3;
}
}

p
internalField uniform 86974;

boundaryField
{
inlet
{
type fixedValue;
value uniform 86974;
}

outlet
{
type fixedValue;
value uniform 86974;
}

wing_surface
{
type zeroGradient;
}

near_side
{
type symmetryPlane;
}

far_side
{
type fixedValue;
value uniform 86974;
}

wing_tip
{
type zeroGradient;
}

}

U
internalField uniform (8.533 0 0);

boundaryField
{
inlet
{
type fixedValue;
value uniform (8.533 0 0);
}

outlet
{
type fixedValue;
value uniform (8.533 0 0);
}

wing_surface
{
type fixedValue;
value uniform (0 0 0);
}

near_side
{
type symmetryPlane;
}

far_side
{
type fixedValue;
value uniform (8.533 0 0);
}

wing_tip
{
type fixedValue;
value uniform (0 0 0);
;
}

}

nut
internalField uniform 8.446e-9;

boundaryField
{
near_side
{
type symmetryPlane;
}
far_side
{
type calculated;
value uniform 8.446e-9;
}
outlet
{
type calculated;
value uniform 8.446e-9;
}
inlet
{
type calculated;
value uniform 8.446e-9;
}
wing_surface
{
type nutkWallFunction;
value uniform 7.73e-12;
}
wing_tip
{
type nutkWallFunction;
value uniform 7.73e-12;
}
}

fvSchemes
ddtSchemes
{
default steadyState;
}

gradSchemes
{
default Gauss linear;
grad(U) cellLimited Gauss linear 1;
}

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

laplacianSchemes
{
default Gauss linear corrected;
}

interpolationSchemes
{
default linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
}

fvSolution
solvers
{
p
{
solver GAMG;
tolerance 1e-7;
relTol 0.01;
smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
cacheAgglomeration on;
agglomerator faceAreaPair;
nCellsInCoarsestLevel 10;
mergeLevels 1;
}

U
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}

k
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}

omega
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}
}

SIMPLE
{
nNonOrthogonalCorrectors 0;
}

potentialFlow
{
nNonOrthogonalCorrectors 10;
}

relaxationFactors
{
fields
{
p 0.2;
}
equations
{
U 0.5;
k 0.5;
omega 0.5;
}
}

cache
{
grad(U);
}

controlDict
deltaT 0.01;

writeControl timeStep;

writeInterval 50;

Pls tell me where the problem is?

ssss · March 1, 2016, 05:26

Increase NonOrthogonalCorrectors to 1
Change div(phi, U) to upwind
Change default gradient scheme to:

default cellMDLimited Gauss linear 0.5;

Do you think that your mesh has enough quality? Do you have tetrahedral elements on the boundary patches? Which is your expected y+?

Harnoor · March 5, 2016, 09:17

I have made the changes in non orthogonal correctors, div(U,phi) scheme and default grad scheme. Now, the results are less crazier than last time. But, the solution is still incorrect. The value of Ux sarts becoming increasingly negative after abut 15 seconds. The order of magnitude of U is becoming very large at certain locations near the outlet. Also, while viewing in paraview, I noticed that the errors originate at the outlet boundary and propagate towards the inlet. So, my intuition is that there is a problem in the boundary conditions. Can someone please check the type and value of my BC's.
To answer your previous question, my mesh quality is fine. My expected y+ value is 1.9. I dont know how to check if my patches are surrounded by tetragonal cells. checkMesh yielded that mesh is fine.
I have attached an image of my geometry, which can be viewed to get an idea of the location of boundary patches.

Kina · March 5, 2016, 12:47

Okay,
just some thoughts you might consider:

you are specifying very many conditions for the initial variables.
Usually, I define the BCs as follows:

U:
Inlet: fixedValue
Outlet: zeroGradient
side walls: slip
airfoil fixedValue 0 0 0

p:
Inlet: zeroGradient
outlet: fixedValue $internalField (value of internal field)
side: zeroGradient
airfoil: zeroGradient

k:
Inlet: either fixedValue or turbulentKineticEnergyinlet
outlet: zeroGradient
side: zeroGradient
airfoil: zeroGradient or kqRWallFunction

omega:
inlet: either fixedValue or turbulentMixingLengthFrequencyInlet
outlet: zeroGradient
side: zeroGradient
airfoil: omegaWallFunction

Also, you might want to set the gradSchemes to cellMDLimited Gauss Linear 0.5

That's all I would change for now just to see if it makes something better.
You could post 3 steps of your log file or attach the whole file if the problem persists. Sometimes, the behavior of the residuals tell the whole story.

Cheers
Alex

Harnoor · March 6, 2016, 09:41

Thanks a ton Alex. It worked like a charm. Just changed the BC's as you suggested.
There was still one slight problem. The pressure wasnt converging completely. After 2 hours, the initial and final residuals were practically constant over time. I stopped the simulation after 3 hours. The pressure results look more or less correct. But, is there something that could be done in this regard? The velocities and other variables have converged without any problem.

Kina · March 6, 2016, 10:26

Could you post your current fvSchemes and fvSolution file? Please post it as <Code> for better overview

Harnoor · March 7, 2016, 12:43

fvsolution

solvers
{
p
{
solver GAMG;
tolerance 1e-7;
relTol 0.01;
smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
cacheAgglomeration on;
agglomerator faceAreaPair;
nCellsInCoarsestLevel 10;
mergeLevels 1;
}

U
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}

k
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}

omega
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}
}

SIMPLE
{
nNonOrthogonalCorrectors 1;
}

potentialFlow
{
nNonOrthogonalCorrectors 10;
}

relaxationFactors
{
fields
{
p 0.2;
}
equations
{
U 0.5;
k 0.5;
omega 0.5;
}
}

cache
{
grad(U);
}

Harnoor · March 7, 2016, 12:44

fvschemes

ddtSchemes
{
default steadyState;
}

gradSchemes
{
default cellMDLimited Gauss linear 0.5;
grad(U) cellLimited Gauss linear 1;
}

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

laplacianSchemes
{
default Gauss linear corrected;
}

interpolationSchemes
{
default linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
}

Kina · March 7, 2016, 13:43

Okay, again some suggestions. For p, change the solver settings (fvSolution) to tolerance 1e-10, nCellsInCoarsestLvl to 120 (speeds up the computation time).
Then, again to the p-GAMG-solver, add: maxIter 500; also a good speed boost, and the 500 additional iterations barely help.
Also, in the SIMPLE settings, add the line nCorrectors 1 and change the nOrthogonalCorrectors to 3.

Then, in fvSchemes, you can change the grad(U) to Gauss Linear and the div(phi,U) term to bounded Gauss linearUpwind grad(U).

If none of those suggestions helps you, you can also try setting the laplacian scheme in the fvSchemes to Gauss linear uncorrected or Gauss linear limited 0.5. This should do the job but I wouldn't recommend it until it's necessary.

Cheers
Alex

Harnoor · March 11, 2016, 10:32

I tried the changes that you suggested but it didn't make much of a difference.
However, I plotted the coefficient of drag and lift vs time for my simulation. I found out that they are converging beautifully (Plots attached below). All variables except p are completely converging. p gets struck at 1 iteration/time step after 20 seconds and then starts oscillating. Now, I have some questions -

1. Since the force coefficients are converging, is it fine to assume that simulation results are correct. Can I neglect the minor issue with p?

2. The values of Coefficient of drag and lift I am getting are 0.025 and 0.123 respectively. The experimental values are 0.018 and 0.121. The coefficient of lift is spot on. But there is a some error in drag coefficient. Can it be attributed to the fact that the experimental free stream turbulence level was 0.5% whereas in the simulation it was 0.001%? How big a deal is this?

3. I cant find out a way to set the free stream turbulence intensity to 0.5% in k-omega sst model. This is because of the restrictions imposed on the value of nut infinity in k-omega sst. It must lie between 10^(-5) to 10^(-2) times nu infinity. nu infinity for our case is 1.6^(-5). This restriction puts a bound on the maximum value of TKE and hence on free stream turbulence. Is there any way to solve this problem?

4. After the simulation, I tried to generate the log file by the commands -

foamJob simpleFoam
foamLog log

But, the generated log files only contain the last few timestep data (Around 10 delta t). I have no idea why this is happening. This is the reason that I haven't been able to plot the residuals using gnuplot. Is there anything wrong with my commands?

5. Could the error in the value of drag coefficient be attributed to the fact that I am using a steady state solver? My problem appears to have no transient phenomenon whatsoever.

6. I am trying to simulate flow over a wing on which experiments have already been performed. The paper that I am using only specifies the chord length. It does not specify the wing span. Can I take any arbitrary wing span without effecting the force coefficients? I mean would the end effects (due o wing tips) really have any significant influence on the force coefficients? What is the minimum span that I should keep (In terms of chord length) to avoid errors due to end effects?

Thanks in advance.

Kina · March 12, 2016, 13:08

Quote:

Originally Posted by Harnoor

I tried the changes that you suggested but it didn't make much of a difference.
However, I plotted the coefficient of drag and lift vs time for my simulation. I found out that they are converging beautifully (Plots attached below). All variables except p are completely converging. p gets struck at 1 iteration/time step after 20 seconds and then starts oscillating. Now, I have some questions -

1. Since the force coefficients are converging, is it fine to assume that simulation results are correct. Can I neglect the minor issue with p?

2. The values of Coefficient of drag and lift I am getting are 0.025 and 0.123 respectively. The experimental values are 0.018 and 0.121. The coefficient of lift is spot on. But there is a some error in drag coefficient. Can it be attributed to the fact that the experimental free stream turbulence level was 0.5% whereas in the simulation it was 0.001%? How big a deal is this?

3. I cant find out a way to set the free stream turbulence intensity to 0.5% in k-omega sst model. This is because of the restrictions imposed on the value of nut infinity in k-omega sst. It must lie between 10^(-5) to 10^(-2) times nu infinity. nu infinity for our case is 1.6^(-5). This restriction puts a bound on the maximum value of TKE and hence on free stream turbulence. Is there any way to solve this problem?

4. After the simulation, I tried to generate the log file by the commands -

foamJob simpleFoam
foamLog log

But, the generated log files only contain the last few timestep data (Around 10 delta t). I have no idea why this is happening. This is the reason that I haven't been able to plot the residuals using gnuplot. Is there anything wrong with my commands?

5. Could the error in the value of drag coefficient be attributed to the fact that I am using a steady state solver? My problem appears to have no transient phenomenon whatsoever.

6. I am trying to simulate flow over a wing on which experiments have already been performed. The paper that I am using only specifies the chord length. It does not specify the wing span. Can I take any arbitrary wing span without effecting the force coefficients? I mean would the end effects (due o wing tips) really have any significant influence on the force coefficients? What is the minimum span that I should keep (In terms of chord length) to avoid errors due to end effects?

Thanks in advance.

1. Yes and no

Converging coefficients mean that your solution is stable and the result is the best outcome your setup can produce. Around what value (1e-4, 1e-5) are your pressure residuals oscillating? Is it possible that your residual plot software interprets the 3 nOrthogonalCorrectors as oscillating since the pressure is solved three times in one iteration meaning the GAMG produces three output lines of residuals per iteration?

2. I think the freestream turbulence is a minor issue regarding your simulation results. The problem of OF's kOmegaSST is that it is just in High Re formulation. Can you switch the k-wall BC to kLowReWallFunction? Also, if you are including nut in your /0 folder, you can set the wall BC to nutLowReWallFunction. High-Re kOmegaSST tends to overpredict drag even in Low-Re meshes. Another possibility would be to use the kkLOmega model as it simulates transitional flow. I found it to be performing well when dealing with a transitional boundary layer (I am not sure if that's the case in your simulation)

3. Read about the turbulentIntensityKineticEnergyInlet BC for 0/k. Maybe this is a way for you to define your turbulence values. Or did I misunderstand the question?

4. I am generating my log file by putting an empty text document named "log" in the case directory and starting the simulation with

Code:

simpleFoam >log

This way, the whole simulation is written into this text document. I am not sure if this works for you.

5. I am pretty sure that this is not the case.

6. That is actually a tough question since a too short wing produces too much induced drag compared to the regular drag of the middle section of the wing. If you have information about what kind of airplane this wing could be used for you could make a pretty accurate guess by looking at the technical data of the airplane. If there is nothing mentioned I'd look at typical airplane wingspans. Since the lift is also affected by the wing geometry (e.g. washout), you might have already chosen just the right wingspan.

What is your yPlus value after the simulation?

Code:

yPlus -latestTime

For the kkLOmega you should keep y+<1 and also for the LowReWallFunctions in SST this is a good thing. I found that a too coarse mesh generally overpredicts lift.

Cheers
Alex

Kina · March 12, 2016, 13:12

Oh and for your drag you can also play around with the convection terms:

Code:

div(phi,U)
div(p,U)

I found that the drag coefficient in my simulations with SST changes when changing from upwind to linearUpwind, linear or limitedLinear 1. This is also logical since a 2nd order scheme is more resistant to numerical errors.

mech_engg_swag · March 14, 2016, 01:58

Sir, I am working with Harnoor on this project.

1. The pressure residuals are oscillating between values of the order of 1e-8 to 1e-7. Our number of nOrthogonalCorrectors is 1.

2. We have changed our airfoil, and the values of Cl and Cd at alpha=0 are 0.1 and 0.019 respectively. But, the results we are getting are Cl=0.031 and Cd=0.029. We tried switching the BC's to kLowReWallFunction. There is not much change in the values of our lift and drag co-efficients.

3. Sir you misunderstood the question. We are finding difficulty in determining the values of k and omega to be given in initial conditions. Menter's paper in which he proposed the kOmegaSST model, is on this link : https://drive.google.com/open?id=0B3...GEybXNEMXVmY3c
Menter has suggested the following values for freestream k and omega in equation (A11) :
omegainfinity = e*Uinfinity/L
nutinfinity = nuinfinity*d
kinfinity = omegainfinity*nutinfinity

The values of e and d vary from [1,10] and [1e-5,1e-2] respectively.

I have the following data fixed :

Re=235000
c=0.298m
Freestream Turbulent Intensity=0.1%

How do we choose the values of e,d and L? Also, in equation (A12), what does deltay1 mean? In our simulations, we have chosen the values e=5 and d=1e-2.

6. On most of the airfoil, our y+ value is less than 1. Our mesh contains around 800,000 cells. Is it fine enough?

Thanks in advance.

Mahe88 · November 16, 2016, 09:23

Hi all,

I do need help to set up a Simulation of an Airfoil using SimpleFoam and the KOmegaSST model.
I created all the files needed and the simulation is running. However the C_l and C_d values are around something 3e88. which definitely makes no sense.

Maybe somebody could look through my files and give me some hints what is or could be wrong.

I calculated my yPlus which is ~30.

CONTROL DICT

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.1                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application     simpleFoam;

startFrom       latestTime;

//startTime       0;

stopAt          endTime;

endTime         25;

deltaT          0.1;

writeControl    timeStep;

writeInterval   10;

purgeWrite      0;

writeFormat     ascii;

writePrecision  6;

writeCompression off;

timeFormat      general;

timePrecision   6;

runTimeModifiable true;

adustTimeStep    yes;

maxCo        0.9;



 functions
{
    #include "forceCoeffs"
}
// ************************************************************************* //

FV Solution

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.1                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
//Tutorial 2D Airfoil
solvers
{
    p
    {
        solver          PCG;
    preconditioner  DIC;
        tolerance       1e-06;
        relTol          0.1;
        smoother        GaussSeidel;
    nSweeps         2;
    }
    
 pFinal
    {
        $p;
        relTol          0;
    }

    U
    {
        solver          PBiCG;
    preconditioner  DILU;
        smoother        GaussSeidel;
        nSweeps         2;
        tolerance       1e-08;
        relTol          0.1;
    }

    nuTilda
    {
        solver          PBiCG;
    //preconditioner  DIC;
        smoother        GaussSeidel;
        nSweeps         2;
        tolerance       1e-08;
        relTol          0.1;
    }
    omega
    {
    solver         PBiCG;
    preconditioner  DILU;
    smoother    GaussSeidel;
    nSweeps         2;
    tolerance       1e-08;
    relTol        0.1;
    }      
    k
    {    solver         PBiCG;
        preconditioner  DILU;
    smoother    GaussSeidel;
    nSweeps         2;
    tolerance       1e-08;
    relTol        0.1;
    }   
}

SIMPLE
{
    nCorrectors        2;
    nNonOrthogonalCorrectors 1;
    pRefCell        0;
    pRefValue       0;

    residualControl
    {
        p               1e-5;
        U               1e-5;
        nuTilda         1e-5;
    }
}

relaxationFactors
{
    fields
    {
        p               0.3;
    }
    equations
    {
        U               0.7;
        nuTilda         0.7;
    omega        0.7;
    
    }
}

potentialFlow
{
    nNonOrthogonalCorrectors 15;
}

// ************************************************************************* //

FV Schemes

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.1                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default         Euler;
}

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

divSchemes
{
    default                     none;
    div(phi,U)                  Gauss upwind;
    div(phi,k)                  Gauss upwind;
    div(phi,epsilon)            Gauss upwind;
    div(phi,omega)              Gauss limitedLinear 1;
    div(phi,R)                Gauss upwind;
    div(R)                Gauss linear;
    div(phi,nuTilda)            Gauss upwind;
    div((nuEff*dev2(T(grad(U)))))     Gauss linear;
}

laplacianSchemes
{
    default                 none;
    laplacian(nuEff,U)      Gauss linear corrected;
    laplacian((1|A(U)),p)         Gauss linear corrected;
    laplacian(alphaTEff,omega)        Gauss linear corrected;
    laplacian(alphaTEff,kt)        Gauss linear corrected;
    laplacian(nu,kl)            Gauss linear corrected;
    laplacian(DepsilonEff,epsilon)    Gauss linear corrected;
    laplacian(DReff,R)            Gauss linear corrected;
    laplacian(DnuTildaEff,nuTilda)    Gauss linear corrected;
    laplacian(DomegaEff,omega)        Gauss linear corrected;
    laplacian(DkEff,k)            Gauss linear corrected;
}

interpolationSchemes
{
    default             linear;
  interpolate(U)    linear;
}

snGradSchemes
{
    default         corrected;
}

fluxRquired 
{
  default        no;
  p            ;
}
wallDist
{
    method meshWave;
}


// ************************************************************************* //

Transport Properties

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.1                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

transportModel  Newtonian;

nu              [0 2 -1 0 0 0 0] 3.087e-05;
rho         [1 -3 0 0 0 0 0 ] 1.225;


CrossPowerLawCoeffs
{
        nu0                 nu0 [ 0 2 -1 0 0 0 0 ] 1e-06;
       nuInf               nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;
        m                   m [ 0 0 1 0 0 0 0 ] 1;
        n                   n [ 0 0 0 0 0 0 0 ] 1;
}
BirdCarreauCoeffs
{
        nu0                 nu0 [ 0 2 -1 0 0 0 0 ] 1e-06;
        nuInf               nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;
        k                   k [ 0 0 1 0 0 0 0 ] 0;
        n                   n [ 0 0 0 0 0 0 0 ] 1;
    
}


// ************************************************************************* //

Transport Properties

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.1                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      turbulenceProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

simulationType RAS;

RAS
{
    RASModel            kOmegaSST;

    turbulence          on;

    printCoeffs         on;
}

//kOmegaSSTCoeffs
//{
//        alphaK1          0.85034;
//        alphaK2          1.0;
//        alphaOmega1      0.5;
//        alphaOmega2      0.85616;
//        gamma1           0.5532;
//        gamma2           0.4403;
//        beta1            0.0750;
//        beta2            0.0828;
//        betaStar         0.09;
//        a1               0.31;
//        c1               10;
//Cmu              0.09;
//}
//wallFunctionCoeffs
//{
//        kappa            0.4187;
//        E                9;
//}


// ************************************************************************* //

k

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.1                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -2 0 0 0 0];

internalField   uniform 1;

boundaryField
{
    Inlet
    {
    type            turbulentIntensityKineticEnergyInlet;
        intensity       0.000002;
        value           uniform 1;
    }
    
     Outlet
      { type         zeroGradient;
      }
    
    
    Front
      {
       type         empty;//fixed Value,
       //value        uniform 1e-6;
    
      }
    
    
    Back
      {
      type         empty;//fixed Value;
     // value        uniform 1e-6;
      }
    
    
    Wing
    {
      type         kqRWallFunction; 
    }


}


// ************************************************************************* //

nut

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.1                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -1 0 0 0 0];

internalField   uniform 1.54074669e-05;

boundaryField
{
   Inlet
    {
       type            fixedValue;
        value           uniform 1.54074669e-05;
    }

    Outlet
    {
         type            zeroGradient;
    }

    Front
    {
        type            empty;
    }

    Back
    {
        type            empty;
    }

    Wing
    {
        type            nutkWallFunction;
        value           uniform 1.54074669e-05;
    }


}


// ************************************************************************* //

nuTilda

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.5                                   |
|   \\  /    A nd           | Web:      http://www.OpenFOAM.org               |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      nuTilda;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -1 0 0 0 0];

internalField   uniform 242;

boundaryField
{
    Outlet
    {
        type            zeroGradient;
    }
    Inlet
    {
        type            fixedValue;
        value           uniform 242;
    }
    Wing
    {
        type            fixedValue;
        value           uniform 242;
    }
    Front
    {
        type            empty;
    }
    Back
    {
        type            empty;
    }
}


// ************************************************************************* //

omega

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.1                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      omega;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 -1 0 0 0 0];

internalField   uniform 30;//5.135822;

boundaryField
{

    Inlet
    {
      type         fixedValue;
      value        uniform 30;//5.135822;
      }

    Outlet
    {
       type         zeroGradient;
    }

    Front
    {
      type         empty;
      }

    Back
    {
      type         empty;
      }

    Wing
    {
     type         omegaWallFunction;
     value        uniform 30;//5.135822;
    }


}


// ************************************************************************* //

P

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.1                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -2 0 0 0 0];

internalField   uniform 0;

boundaryField
{
   Inlet
    {
        type            zeroGradient; //freestreamPressure;
    }

    Outlet
    {
        type            fixedValue;
    value         uniform 0;
    }

    Front
    {
        type            empty;
    }

    Back
    {
        type            empty;
    }

    Wing
    {
      type        zeroGradient;
    }
}

// ************************************************************************* //

U

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.1                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    location    "0";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (92.61 0 0);

boundaryField
{
    Outlet
    {
        type            freestream;
        freestreamValue uniform (92.61 0 0);
    }

    //ObenAndUnten
    //{
    //    type            symmetry;
    //}

    Inlet
    {
        type            freestream;
        freestreamValue           uniform (92.61 0 0);
    }

    Wing
    {
        type            fixedValue;
        value        uniform (0 0 0);
    }

    Front
    {
        type            empty;
    }
    Back
    {
        type            empty;
    }    
}


// ************************************************************************* //

Any help is appreciated!!!

Thanks!

March 1, 2016, 01:15	simpleFoam convergence issue	#1
Harnoor New Member Harnoor Singh Join Date: Jan 2016 Posts: 14 Rep Power: 10	I am new to OpenFoam. I am trying to simulate flow over a 3-d wing (sd 6060 airfoil) at Re=80000. I have created my mesh in icem-cfd and imported it in Openfoam. I am using k omega SST model and I have specified all boundary conditions to the best of my knowledge. I am using simpleFoam as the solver. The solution does not converge and I am getting completely wrong results. I am pasting my case files below. Can someone please take a look and tell me where the problem is? Any help would be greatly appreciated. k internalField uniform 2.77e-8; boundaryField { near_side { type symmetryPlane; } far_side { type fixedValue; value uniform 2.77e-8; } outlet { type fixedValue; value uniform 2.77e-8; } inlet { type fixedValue; value uniform 2.77e-8; } wing_surface { type kqRWallFunction; value uniform 1e-11; } wing_tip { type kqRWallFunction; value uniform 1e-11; } } omega internalField uniform 3.28; boundaryField { near_side { type symmetryPlane; } far_side { type fixedValue; value uniform 3.28; } outlet { type fixedValue; value uniform 3.28; } inlet { type fixedValue; value uniform 3.28; } wing_surface { type omegaWallFunction; value uniform 2.688e6; } wing_tip { type omegaWallFunction; value uniform 1.421e3; } } p internalField uniform 86974; boundaryField { inlet { type fixedValue; value uniform 86974; } outlet { type fixedValue; value uniform 86974; } wing_surface { type zeroGradient; } near_side { type symmetryPlane; } far_side { type fixedValue; value uniform 86974; } wing_tip { type zeroGradient; } } U internalField uniform (8.533 0 0); boundaryField { inlet { type fixedValue; value uniform (8.533 0 0); } outlet { type fixedValue; value uniform (8.533 0 0); } wing_surface { type fixedValue; value uniform (0 0 0); } near_side { type symmetryPlane; } far_side { type fixedValue; value uniform (8.533 0 0); } wing_tip { type fixedValue; value uniform (0 0 0); ; } } nut internalField uniform 8.446e-9; boundaryField { near_side { type symmetryPlane; } far_side { type calculated; value uniform 8.446e-9; } outlet { type calculated; value uniform 8.446e-9; } inlet { type calculated; value uniform 8.446e-9; } wing_surface { type nutkWallFunction; value uniform 7.73e-12; } wing_tip { type nutkWallFunction; value uniform 7.73e-12; } } fvSchemes ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; grad(U) cellLimited Gauss linear 1; } divSchemes { default none; div(phi,U) bounded Gauss linearUpwindV grad(U); div(phi,k) bounded Gauss upwind; div(phi,omega) bounded Gauss upwind; div((nuEff*dev(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } fluxRequired { default no; p; } fvSolution solvers { p { solver GAMG; tolerance 1e-7; relTol 0.01; smoother GaussSeidel; nPreSweeps 0; nPostSweeps 2; cacheAgglomeration on; agglomerator faceAreaPair; nCellsInCoarsestLevel 10; mergeLevels 1; } U { solver smoothSolver; smoother GaussSeidel; tolerance 1e-8; relTol 0.1; nSweeps 1; } k { solver smoothSolver; smoother GaussSeidel; tolerance 1e-8; relTol 0.1; nSweeps 1; } omega { solver smoothSolver; smoother GaussSeidel; tolerance 1e-8; relTol 0.1; nSweeps 1; } } SIMPLE { nNonOrthogonalCorrectors 0; } potentialFlow { nNonOrthogonalCorrectors 10; } relaxationFactors { fields { p 0.2; } equations { U 0.5; k 0.5; omega 0.5; } } cache { grad(U); } controlDict deltaT 0.01; writeControl timeStep; writeInterval 50; Pls tell me where the problem is?

March 6, 2016, 09:41	simpleFoam convergence	#5
Harnoor New Member Harnoor Singh Join Date: Jan 2016 Posts: 14 Rep Power: 10	Thanks a ton Alex. It worked like a charm. Just changed the BC's as you suggested. There was still one slight problem. The pressure wasnt converging completely. After 2 hours, the initial and final residuals were practically constant over time. I stopped the simulation after 3 hours. The pressure results look more or less correct. But, is there something that could be done in this regard? The velocities and other variables have converged without any problem.

March 7, 2016, 12:43	fvsolution	#7
Harnoor New Member Harnoor Singh Join Date: Jan 2016 Posts: 14 Rep Power: 10	fvsolution solvers { p { solver GAMG; tolerance 1e-7; relTol 0.01; smoother GaussSeidel; nPreSweeps 0; nPostSweeps 2; cacheAgglomeration on; agglomerator faceAreaPair; nCellsInCoarsestLevel 10; mergeLevels 1; } U { solver smoothSolver; smoother GaussSeidel; tolerance 1e-8; relTol 0.1; nSweeps 1; } k { solver smoothSolver; smoother GaussSeidel; tolerance 1e-8; relTol 0.1; nSweeps 1; } omega { solver smoothSolver; smoother GaussSeidel; tolerance 1e-8; relTol 0.1; nSweeps 1; } } SIMPLE { nNonOrthogonalCorrectors 1; } potentialFlow { nNonOrthogonalCorrectors 10; } relaxationFactors { fields { p 0.2; } equations { U 0.5; k 0.5; omega 0.5; } } cache { grad(U); }

March 7, 2016, 12:44	fvschemes	#8
Harnoor New Member Harnoor Singh Join Date: Jan 2016 Posts: 14 Rep Power: 10	fvschemes ddtSchemes { default steadyState; } gradSchemes { default cellMDLimited Gauss linear 0.5; grad(U) cellLimited Gauss linear 1; } divSchemes { default none; div(phi,U) bounded Gauss upwind; div(phi,k) bounded Gauss upwind; div(phi,omega) bounded Gauss upwind; div((nuEff*dev(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } fluxRequired { default no; p; }

March 7, 2016, 13:43		#9
Kina Senior Member Alex Join Date: Jan 2014 Posts: 126 Rep Power: 12	Okay, again some suggestions. For p, change the solver settings (fvSolution) to tolerance 1e-10, nCellsInCoarsestLvl to 120 (speeds up the computation time). Then, again to the p-GAMG-solver, add: maxIter 500; also a good speed boost, and the 500 additional iterations barely help. Also, in the SIMPLE settings, add the line nCorrectors 1 and change the nOrthogonalCorrectors to 3. Then, in fvSchemes, you can change the grad(U) to Gauss Linear and the div(phi,U) term to bounded Gauss linearUpwind grad(U). If none of those suggestions helps you, you can also try setting the laplacian scheme in the fvSchemes to Gauss linear uncorrected or Gauss linear limited 0.5. This should do the job but I wouldn't recommend it until it's necessary. Cheers Alex 96faizizzuddin and zyzycomcn like this.

March 1, 2016, 05:26		#2
ssss Senior Member anonymous Join Date: Aug 2014 Posts: 205 Rep Power: 13	Increase NonOrthogonalCorrectors to 1 Change div(phi, U) to upwind Change default gradient scheme to: default cellMDLimited Gauss linear 0.5; Do you think that your mesh has enough quality? Do you have tetrahedral elements on the boundary patches? Which is your expected y+?

March 5, 2016, 12:47		#4
Kina Senior Member Alex Join Date: Jan 2014 Posts: 126 Rep Power: 12	Okay, just some thoughts you might consider: you are specifying very many conditions for the initial variables. Usually, I define the BCs as follows: U: Inlet: fixedValue Outlet: zeroGradient side walls: slip airfoil fixedValue 0 0 0 p: Inlet: zeroGradient outlet: fixedValue $internalField (value of internal field) side: zeroGradient airfoil: zeroGradient k: Inlet: either fixedValue or turbulentKineticEnergyinlet outlet: zeroGradient side: zeroGradient airfoil: zeroGradient or kqRWallFunction omega: inlet: either fixedValue or turbulentMixingLengthFrequencyInlet outlet: zeroGradient side: zeroGradient airfoil: omegaWallFunction Also, you might want to set the gradSchemes to cellMDLimited Gauss Linear 0.5 That's all I would change for now just to see if it makes something better. You could post 3 steps of your log file or attach the whole file if the problem persists. Sometimes, the behavior of the residuals tell the whole story. Cheers Alex

March 6, 2016, 10:26		#6
Kina Senior Member Alex Join Date: Jan 2014 Posts: 126 Rep Power: 12	Could you post your current fvSchemes and fvSolution file? Please post it as <Code> for better overview

March 12, 2016, 13:12		#12
Kina Senior Member Alex Join Date: Jan 2014 Posts: 126 Rep Power: 12	Oh and for your drag you can also play around with the convection terms: Code: div(phi,U) div(p,U) I found that the drag coefficient in my simulations with SST changes when changing from upwind to linearUpwind, linear or limitedLinear 1. This is also logical since a 2nd order scheme is more resistant to numerical errors.

March 14, 2016, 01:58		#13
mech_engg_swag New Member Parth Thakkar Join Date: Mar 2016 Posts: 7 Rep Power: 10	Sir, I am working with Harnoor on this project. 1. The pressure residuals are oscillating between values of the order of 1e-8 to 1e-7. Our number of nOrthogonalCorrectors is 1. 2. We have changed our airfoil, and the values of Cl and Cd at alpha=0 are 0.1 and 0.019 respectively. But, the results we are getting are Cl=0.031 and Cd=0.029. We tried switching the BC's to kLowReWallFunction. There is not much change in the values of our lift and drag co-efficients. 3. Sir you misunderstood the question. We are finding difficulty in determining the values of k and omega to be given in initial conditions. Menter's paper in which he proposed the kOmegaSST model, is on this link : https://drive.google.com/open?id=0B3...GEybXNEMXVmY3c Menter has suggested the following values for freestream k and omega in equation (A11) : omegainfinity = eUinfinity/L nutinfinity = nuinfinityd kinfinity = omegainfinity*nutinfinity The values of e and d vary from [1,10] and [1e-5,1e-2] respectively. I have the following data fixed : Re=235000 c=0.298m Freestream Turbulent Intensity=0.1% How do we choose the values of e,d and L? Also, in equation (A12), what does deltay1 mean? In our simulations, we have chosen the values e=5 and d=1e-2. 6. On most of the airfoil, our y+ value is less than 1. Our mesh contains around 800,000 cells. Is it fine enough? Thanks in advance.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Convergence issue with continuity equation	Jake	FLUENT	8	June 6, 2018 04:41
convergence issue laplacianFoam	Shakil Masum	OpenFOAM Running, Solving & CFD	1	September 9, 2014 14:03
Convergence issue for high speed combustion with radiation.	Goutham cet	FLUENT	2	July 30, 2014 08:22
SimpleFoam convergence problem with really simple simulation	mayank.dce2k7	OpenFOAM Running, Solving & CFD	2	November 19, 2013 06:28
simpleFoam: simple 1-D channel flow, yet very strange convergence behavior	kishpishar	OpenFOAM Running, Solving & CFD	2	June 20, 2013 14:55