[gabrielfelix]

Hi folks

I'm simulating a propeller in steady-state compressible flow using rhoSimpleFoam and I was using the kEpsilon turbulence model with the same boundary conditions as the pimpleFoam marine propeller tutorial. I wanted to run my case with the Spalart-Allmaras turbulence model and I faced some problems to which I could not find a direct guide to overcome them. I saw that there are many posts concerning the same problems I had, and I decided to create this guide, now that I managed to succesfully run my case with SA model.

I believe this guide will work for both compressible or incompressible conditions. I'm not expert on this SA model, so the solutions I will come up here might not be the most adequate ones, but rather the ones I managed to run my case with.

1. Change turbulence model in turbulenceProperties file:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2012                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      turbulenceProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

simulationType  RAS;

RAS
{
    RASModel        SpalartAllmaras;

    turbulence      on;

    printCoeffs     on;
}


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

2. Modify 0/nut and create 0/nuTilda file

The nut represents the turbulent kinematic viscosity boundary conditions and nuTilda is similar to nut, but is the variable that the SA model actually iterates.

The [1] NASA Turbulence Modelling Resource and the document [2] Changes and Settings for Standard Turbulence Model Implementation in OpenFOAM suggest using the following viscosity ratios:
- nuTilda/nu = 3
- nut/nutTilda = 0.07

So if you are running a simulation at sea level rho = 1.225 and mu = 1.8e-5. Hence, nu =~ 1.5e-5. Therefore, using the viscosity ratios above, you should use nuTilda = 4.5e-5 and nut = 3.15e-6.

I configured nut and nuTilda files according to [2] boundary tables.

In nut file you must change wall boundary type to nutUWallFunction. I you are using other turbulence models there will be other variables such as nutkWallFunction. If you dont do this there will be errors on execution.

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2012                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform 3.15e-6;

boundaryField
{
    #includeEtc "caseDicts/setConstraintTypes"

    inlet
    {
        type            calculated;
        value           uniform 3.15e-6;
    }

    outlet
    {
        type            zeroGradient;
    }

    wall
    {
        type            nutUWallFunction;
        value           uniform 0;
    }
}


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

In nuTilda you must not have any type calculted boundary conditions to avoid the following error massage when executing solver:

You are probably trying to solve for a field with a default boundary condition

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2012                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      nuTilda;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform 4.5e-5;

boundaryField
{
    #includeEtc "caseDicts/setConstraintTypes"

    inlet
    {
        type            fixedValue;
        value           uniform 4.5e-5;
    }

    outlet
    {
        type            zeroGradient;
    }

    wall
    {
        type            fixedValue;
        value           uniform 0;
    }
}


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

3. Add nuTilda and R variables to fvSolution and fvSchemes files

When configuring these files you dont need to remove other turbulence model variables such as k, epsilon and omega. You can also keep their 0/ files.

I don't know what the R variable means, but if you dont add it to the files you will get the following warning on solver execution:

Turbulence kinetic energy not defined for Spalart-Allmaras model. Returning zero field

According to what I researched in other threads, you should not worry about this warning, however is better if can get rid of it.

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2012                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default         steadyState;
}

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

divSchemes
{
    default         none;

    div(phi,U)      bounded Gauss linearUpwind limited;

    turbulence      bounded Gauss upwind;
    energy          bounded Gauss linearUpwind limited;

    div(phi,k)      $turbulence;
    div(phi,omega)  $turbulence;
	div(phi,epsilon)  $turbulence;

    div(phi,e)      $energy;
    div(phi,K)      $energy;
    div(phi,Ekp)    $energy;

    div(phid,p)     Gauss upwind;
    div((phi|interpolate(rho)),p)  bounded Gauss upwind;
	
	div(phi,nuTilda) bounded Gauss linearUpwind grad(nuTilda);
    div(((rho*nuEff)*dev2(T(grad(U)))))    Gauss linear;
	
	div(phi,R) bounded Gauss upwind;
	div(R) Gauss linear;
}

laplacianSchemes
{
    default         Gauss linear limited corrected 0.33;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         limited corrected 0.33;
}

wallDist
{
    method meshWave;
}


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

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2012                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    "pcorr.*"
    {
        solver          GAMG;
        tolerance       1e-2;
        relTol          0;
        smoother        DICGaussSeidel;
        cacheAgglomeration no;
        maxIter         50;
    }

    p
    {
        $pcorr;
        tolerance       1e-5;
        relTol          0.01;
    }

    pFinal
    {
        $p;
        tolerance       1e-6;
        relTol          0;
    }

    "(U|k|epsilon|e|nuTilda)"
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-6;
        relTol          0.1;
    }

    "(U|k|epsilon|e|nuTilda)Final"
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-6;
        relTol          0;
    }
	
	R
	{
		solver PBiCG;
		preconditioner DILU;
		tolerance 1e-20;
		relTol 0;
	}
}

SIMPLE
{
    //correctPhi          no;
    //nOuterCorrectors    2;
    //nCorrectors         1;
    nNonOrthogonalCorrectors 1;
	
	// Set up residual controls. Simulation stops when residual target is reached
	residualControl
	{
		p					1e-6;
		//U					1e-4;
		//"(k|epsilon)"		1e-4;
	}
}

potentialFlow
{
    nNonOrthogonalCorrectors 1;
}

relaxationFactors
{
	fields
	{
		p 0.3 ;
		rho 0.01 ;
	}
	equations
	{
		U 0.7 ;
		e 0.7 ;
		k 0.7 ;
		omega 0.7 ;
		nuTilda 0.7 ;
		R 0.7;
	}
}

cache
{
    grad(U);
}


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

4. Define nu value in transportProperties files

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2012                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

transportModel  Newtonian;

rho             1.225;

nu              1.5e-05;

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

[Jonathan]

Very clear and very good. Thanks for documenting / sharing