[Zymorui]

Dear Foamers,
I'm conducting a transient study of a fluidic oscillator with water at 20°C (corresponding to nu=1.004e-6). For this I'm using the SpalartAllmarasIDDES turbulence model and the pisoFoam-solver. The Mean Courant Number is 0.1 and the maximum about 7. I average the pressure over a diameter slice in each feedback loop and use the pressure difference between both to calculate a sinoid signal containing the oscillation frequency of the jet for the particular inlet velocity.

My problem is that the CFD oscillation frequency of the jet is almost the double of experimental values. The problem persists for all flow rates even in the laminar regime (where I used no turbulence model). As I have double checked the geometry, the Mesh should be fine (checkMesh):
- 1mio Cells
- blockMesh generated
- y+=1
- cell-to-cell-exp-ratio at the wall is about 1.2
- Non-Ortho-Max 58
- Max aspect ratio 152
- Max skewness 1.7

So I guess there must be something wrong with my fvSchemes or fvSolutions. Does anyone have suggestions what part of the simulation could make the oscillation frequency getting over estimated that strong?

Kind regards,
Hendrik


fvSchemes

/*--------------------------------*- 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      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default backward;
}

d2dt2Schemes
{
}

gradSchemes
{
    default         cellLimited Gauss linear 1; //Gauss linear;

    //grad(nuTilda)   cellLimited Gauss linear 1;
    //grad(U)         cellLimited Gauss linear 1;
}

divSchemes	// convection
{
    default         none;

    div(phi,U)      Gauss linearUpwind grad(U); // LUST unlimitedGrad(U);
    div(phi,k)      Gauss limitedLinear 1;
    div(phi,nuTilda) Gauss limitedLinear 1;

    div((nuEff*dev2(T(grad(U))))) Gauss linear;
}

laplacianSchemes   // diffusion
{
    default         Gauss linear limited corrected 0.33;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         limited corrected 0.33;
}

wallDist
{
    method meshWave;
}


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

fvSolution

/*--------------------------------*- 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      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    p
    {
        solver          GAMG;
        tolerance       1e-5;
        relTol          0.05;
        smoother        GaussSeidel;
	//nSweeps			1;
	nPreSweeps		0;
	nPostSweeps		2;
	nFinestSweeps		2;
        nCellsInCoarsestLevel 50;
	//maxIter			50;
    }

    pFinal
    {
        $p;
	tolerance       1e-5;
        relTol          0;
	//maxIter		100;
    }

    "(U|k|B|nuTilda)"
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
	nSweeps		1;
        tolerance       1e-5;
        relTol          0;
    }
}

PISO
{
    nCorrectors     3;
    nNonOrthogonalCorrectors 1;
}

relaxationFactors
{
	p	1;
    "U.*"               1;
    "nuTilda.*"         1;
}


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

[sati]

Hi,

A Courant number of 7 is way too high. You should decrease your time step to reach a maxCo < 1.

[Zymorui]

It took me some time but I've narrowed the issue down to the outlet boundary condition. I did a quick run with fluent and got the right frequency right away. (transient kOmega simulation). But fluent gave the 'A wall has been set at portions of an outlet'-notice. My fixedValue=0 pressure condition at the outlet created backflow, as the vortice cores in the outlet channel were at p<0.

I experimented with advective -> phi, BC for velocity and fixedMean for pressure but it's not quite right yet.

Does anyone have some experience with the backflow issue? Is there a BC that does something similar as fluent does?