[treem22]

Fellow foamers,

I'm attempting to simulate wing in-ground effects on a 2D airfoil over an air-water interface. I want to assign a specific waveform to the interface, but the waveform is changing shape as it progresses through the domain. I recognize that the presence of the airfoil will affect the waveform shape, but I'm seeing waveform changes as soon as one period after the boundary, which is ~9 chord lengths upstream of the airfoil.

Picture1 shows the initial setup.

Picture2 shows the first period of the wave from the boundary condition and highlights an indentation at the wave peak.

Picture3 shows the first several periods and the change in waveform shape as it progresses through the domain.

Does anyone have ideas on how I can better control the waveform shape that reaches the airfoil?

Here are my pertinent input files:

controlDict

application       interFoam;

startFrom         latestTime; //startTime;

startTime	  0.;

stopAt            nextWrite; //endTime;

endTime	          0.31896; // 60 periods (3x flow-throughs)

deltaT 	          1e-6;

writeControl      adjustableRunTime;

writeInterval	  2.658e-4; // 20 steps per period

purgeWrite	  0;

writeFormat	  binary;

writePrecision	  6;

writeCompression  off;

timeFormat	  general;

timePrecision	  6;

runTimeModifiable yes;

adjustTimeStep	  on;

maxCo	          3.;

maxAlphaCo	  1.;

maxDeltaT         1.;

fvSchemes

ddtSchemes
{
    default         Euler;
}

gradSchemes
{
    default         Gauss linear;
    limitedGrad     cellLimited Gauss linear 1;
}

divSchemes
{
    div(rhoPhi,U)   Gauss linearUpwind grad(U);
    div(phi,alpha)  Gauss vanLeer;
    div(phirb,alpha) Gauss linear;
    div(phi,k)      Gauss linearUpwind limitedGrad;
    div(phi,omega)  Gauss linearUpwind limitedGrad;
    div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
    default         Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}

wallDist
{
    method          meshWave;
}

fvSolution

solvers
{
    "alpha.water.*"
    {
        nAlphaCorr      3;
        nAlphaSubCycles 1;
        cAlpha          1;
        icAlpha         0;

        MULESCorr       yes;
        nLimiterIter    15;
        alphaApplyPrevCorr  yes;

        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-10;
        relTol          0;
        minIter         1;
    }

    "pcorr.*"
    {
        solver          GAMG;
        smoother        DIC;
        tolerance       1e-3;
        relTol          0;
    };

    p_rgh
    {
        solver          GAMG;
        smoother        DIC;
        tolerance       5e-8;
        relTol          0;
    };

    p_rghFinal
    {
        $p_rgh;
        relTol          0;
    }

    "(U|k|omega).*"
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
        nSweeps         1;
        tolerance       1e-7;
        relTol          0;
        minIter         1;
    };
}

PIMPLE
{
    momentumPredictor no;

    nOuterCorrectors 2;
    nCorrectors      2;
    nNonOrthogonalCorrectors 0;

    correctPhi      yes;
    moveMeshOuterCorrectors no;
    turbOnFinalIterOnly yes;
}

relaxationFactors
{
    equations
    {
        ".*" 1;
    }
}

cache
{
    grad(U);
}

0/U:

Umean   100;

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

internalField   uniform ($Umean 0 0);

boundaryField
{
	front_and_back
	{
		type  empty;
	}
        inlet
        {
                type            fixedValue;
                value           $internalField;
        }
        outlet
        {
                type            outletPhaseMeanVelocity;
                alpha           alpha.water;
                Umean           $Umean;
                value           $internalField;
        }
	top
	{
                type                pressureInletOutletVelocity;
                tangentialVelocity  $internalField;
                value               uniform (0 0 0);
	}
	bottom
	{
                type                pressureInletOutletVelocity;
                tangentialVelocity  $internalField;
                value               uniform (0 0 0);
	}
	wing
	{
		type  noSlip;
	}
}

0/p_rgh:

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

internalField   uniform 0;

boundaryField
{
	front_and_back
	{
		type  empty;
	}
	bottom
	{
		type  totalPressure;
		p0    uniform 0;
	}
	wing
	{
		type   fixedFluxPressure;
		value  $internalField;
	}
	outlet
	{
		type   zeroGradient;
	}
	top
	{
		type  totalPressure;
		p0    uniform 0;
	}
	inlet
	{
		type   fixedFluxPressure;
		value  $internalField;
	}
}

0/alpha.water:

dimensions      [0 0 0 0 0 0 0];

internalField   uniform 0;

boundaryField
{
	front_and_back
	{
		type  empty;
	}
	bottom
	{
		type        inletOutlet;
		inletValue  uniform 1;
		value       $internalField;
	}
	wing
	{
		type  zeroGradient;
	}
	outlet
	{
		type        variableHeightFlowRate;
		lowerBound  0;
		upperBound  1;
		value       $internalField;
	}
	top
	{
		type        inletOutlet;
		inletValue  $internalField;
		value       $internalField;
	}
	inlet
	{
		type   uniformFixedValue;
		value  $internalField;
		uniformValue
		{
			type expression;
			variables
			(
			        "orig_h = -0.1329"
				// wave amplitude
				"a = 0.045"
				// wave speed (match velocity inlet)
				"Vg = 100"
				// wavelength
				"l = 0.5316"
				// wave height
				"eta = -a*cos(2*pi()*Vg*time()/l)"
			);
			expression
                        #{
				// if the y position is less than or equal to
				// the original water level plus the wave
				// height then set the alpha value to 1; if not
				// set the alpha value to 0
				(pos().y() <= orig_h + eta) ? 1 : 0
                        #};
		}
	}
}

Any help is most appreciated!

[Alczem]

Hey!


You could use the file waveProperties with the waveVelocity and waveAlpha boundary conditions to generate waves. They tend to be stable in my experience. There are some examples in the interFoam tutorials.


Other than that, maybe turning off the turbulence will help because turbulence will introduce dissipation depending on the scale of the simulation. And I always turn off alphaApplyPrevCorr in fvSolution, my simulations are more unstable more often than not (although I may be using it when it is not applicable). Just a thing that you could also try


And finally, if you use setFields, add an hRef file in constant with your initial water level. It helps with the water leaving properly at the outlet.