[5251]

Hi all,
I am attempting to predict the value of the drag coefficient of a NACA4412 airfoil at a Reynolds number of 3x10^6. I built a case based upon the wingMotion tutorial and I am using pimpleFoam with a variable timestep and the SpalartAllmaras turbulence model to compute results. I have 10 layers on the surface of the wing, with an average y+ of 5.9. Whilst I realise this is not as accurate as it could get, my results are still in magnitude of 100% error when compared to Abbot and Von Doenhoff's Theory of Wing Sections. I suspect this may be due to my boundary conditions, though I am unsure as I am quite new to OpenFOAM. I have attached my U, p, nut and Nutilda files. EDIT: Front and Back patches are defined as empty and the topAndBottom patch is defined as slip.

U:

 
/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  8
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    location    "0";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

#include        "include/initialConditions"

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

internalField   uniform $flowVelocity;

boundaryField
{
    #include "include/fixedInlet"

    outlet
    {
        type            inletOutlet;
        inletValue      uniform (0 0 0);
        value           $internalField;
    }

    wing
    {
        type            movingWallVelocity;
        value           uniform (0 0 0);
    }

    #include "include/frontBackTopBottomPatches"
}

P:

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  8
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

#include        "include/initialConditions"

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

internalField   uniform $pressure;

boundaryField
{
    inlet
    {
        type            zeroGradient;
    }

    outlet
    {
        type            fixedValue;
        value           $internalField;
    }

    wing
    {
        type            zeroGradient;
    }

    #include "include/frontBackTopBottomPatches"
}

nut:

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  8
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform 0;

boundaryField
{
    wing
    {
        type            nutkWallFunction;
        value           uniform 1e-10;
    }

    "(front|back|topAndBottom|inlet|outlet)"
    {
        type            calculated;
        value           uniform 0;
    }
}

nuTilda:

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  8
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      nuTilda;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform 75.5e-06;

boundaryField
{
    inlet
    {
        type            fixedValue;
        value 		 uniform 75.5e-06;
    }

    outlet
    {
        type            fixedValue;
        value		 uniform 75.5e-06;
    }

    wing
    {
        type            fixedValue;
        value           uniform 0;
    }

    frontAndBack
    {
        type            empty;
    }
    
    topAndBottom
    {
    	type		fixedValue;
    	value		uniform 0;	
    }
}

Any help or insights are greatly appreciated! I am not attempting to get exact values of drag, within 30% is sufficient.

[mzzmrt]

First of all, the wall function you used is not correct for SA model, use nutUSpaldingWallFunction instead of nutkWallFunction and see this thread if more details required:

NACA0012 k-OmegaSST simulation

[5251]

Hi mzzmrt,
Thank you very much for your suggestions, that thread was very helpful. Now utilising a USpaldingWallFunction for nut, my drag measurements have improved, though not as far as I would have thought. I am measuring a Cd of ~0.012, when it should be closer to 0.007. I realise that RANS has a tendency to overpredict drag, however I was under the impression this overprediction was in the range of 20-30%, not almost 80%.

Are there other factors that may be contributing to this discrepancy? I am new to OpenFoam (and CDF in general), so apologies if my questions are bit silly.

[mzzmrt]

Mesh quality and resolution may affect the results.
fvSchemes options may also be considered.
A mesh with average yPlus ~1 instead of 5.9 will be better.
For internalField following values;
nut = nu and nuTilda= 5*nu will be better choice, I guess...