[giammy92]

Hi foamers, my case case sists in a airfoil 2D with a chord lenght of 0.5459 m. I have found this formula in this site for mixing lenght http://www.cfd-online.com/Wiki/Turbulence_length_scale

Do you think it is correct for my case?

[giammy92]

Hi foamers, my case consists in airfoil 2D with a chord lenght 0.5459 m in a flow of air with a U=41.511 m/s, M=0.12, Re=1.5e6, turbulent intensity(%)=0.1, turbulent viscosity ratio=0.1 and angle of attack=13°. My model of turbulence is k-omega SST. Report my 0 directory:

EPSILON

dimensions      [0 2 -3 0 0 0 0];

internalField   uniform 0.397998;

boundaryField
{
    FAR_FIELD
    {
        type            turbulentMixingLengthDissipationRateInlet;
        mixingLength    5.42e-5;
        value           uniform 0.397998;
    }

    TRAILING_EDGE
    {
        type            epsilonWallFunction;
        value           uniform 0.397998;
    }
   
    SUCTION_SIDE
    {
        type            epsilonWallFunction;
        value           uniform 0.397998;
    }

    PRESSURE_SIDE
    {
       type            epsilonWallFunction;
       value           uniform 0.397998;
    }

    frontAndBackPlanes
    {
        type            empty;
    }
}

K

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

internalField   uniform 0.0025847;

boundaryField
{
    FAR_FIELD
    {
        type            turbulentIntensityKineticEnergyInlet;
        intensity       0.001;
        value           uniform 0.0025847;
    }

    TRAILING_EDGE
    {
        type            kqRWallFunction;
        value           uniform 0.0025847;
    }

    SUCTION_SIDE
    {
        type            kqRWallFunction;
        value           uniform 0.0025847;
    }

    PRESSURE_SIDE
    {
       type            kqRWallFunction;
       value           uniform 0.0025847;
    }
    
    frontAndBackPlanes
    {
        type            empty;
    }
}

NUT

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

internalField   uniform 1.51e-6;

boundaryField
{
    FAR_FIELD
    {
        type            freestream;
        freestreamValue uniform 1.51e-6;
    }

    TRAILING_EDGE
    {
        type            nutkWallFunction;
        value           uniform 0;
    }

    SUCTION_SIDE
    {
        type            nutkWallFunction;
        value           uniform 0;
    }
    
    PRESSURE_SIDE
    {
        type            nutkWallFunction;
        value           uniform 0;
    }

    frontAndBackPlanes
    {
        type            empty;
    }
}

OMEGA

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

internalField   uniform 1710.91;

boundaryField
{
    FAR_FIELD
    {
        type            turbulentMixingLengthFrequencyInlet;
        mixingLength   5.42e-5;
        value           uniform 1710.91;
    }

    TRAILING_EDGE
    {
        type            omegaWallFunction;
        value           uniform 1710.91;
    }

    SUCTION_SIDE
    {
        type            omegaWallFunction;
        value           uniform 1710.91;
    }

   PRESSURE_SIDE
   {
        type            omegaWallFunction;
        value           uniform 1710.91;
    }

     frontAndBackPlanes
    {
        type            empty;
    }
}

P

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

internalField   uniform 0;

boundaryField
{
    FAR_FIELD
    {
        type            freestreamPressure;
    }

    TRAILING_EDGE
    {
        type            zeroGradient;
    }

    SUCTION_SIDE
    {
        type            zeroGradient;
    }
    
    PRESSURE_SIDE
    {
        type            zeroGradient;
    }

    frontAndBackPlanes
    {
        type            empty;
    }
}

U

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

internalField   uniform (40.447 9.338 0);

boundaryField
{
    FAR_FIELD
    {
        type            freestream;
        freestreamValue uniform (40.447 9.338 0);
    }

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

    SUCTION_SIDE
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    
    PRESSURE_SIDE
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }

    frontAndBackPlanes
    {
        type            empty;
    }
}

So, how do you valutate my data and boundary conditions?

[giammy92]

I would especially confirmations for nut and for mixing lenght

[giammy92]

my problem is I can't obtain Cl of about 1.2-1.3, that is the right value comparing with experimental results, instead i obtain Cl of about 1.5. What could be cause of this?

[rupole1185]

There are many things that could influence your result ..what is your y+ around the airfoil?

[giammy92]

this is a good question i don't know this because i'm using a mesh created by another student that rans this case with fluent. Can i occur y+ for example with a checkmesh?

[rupole1185]

Y+ is something you can calculate once you have completed the simulation. Depending on your openfoam version you may run yPlus or yPlusRas

[giammy92]

Good i have ran yPlus and it has created field yPlus for every time directory. Now which value of yPlus i have to read? That in directory 0, min, max or average?

[taxalian]

Hi,
Having a look at you boundary conditions and the Cl value you are getting seems to be normal. Obviously if you need to compare your results with the experiments.
Prior to that you need to make sure that you have done grid independent study and secondly make sure that if you want to use the wallfunction approach, as you are, the yPlus value should be within a range of 30-150 or if you use a very good mesh that resolves till the airfoil surface then you should have average yPlus of about 1.
Another important thing to check is the "fvSchemes" and "fvSolution" dicitionaries.
That if you are using 1st order or 2nd order schemes this could also cause an overprediction of Cl.
If you experimental pressure coefficient plot, then its worth comparing with it too.

best of luck.

[rupole1185]

Since you are using komegasst it is recommended to maintain y+ between 1 and 5 let's say ...

[giammy92]

after running yPlus i have this for time 0:

Create mesh for time = 0

Time = 0
Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RAS
Selecting RAS turbulence model kOmegaSST
Selecting patchDistMethod meshWave
kOmegaSSTCoeffs
{
alphaK1 0.85;
alphaK2 1;
alphaOmega1 0.5;
alphaOmega2 0.856;
gamma1 0.555556;
gamma2 0.44;
beta1 0.075;
beta2 0.0828;
betaStar 0.09;
a1 0.31;
b1 1;
c1 10;
F3 false;
}

Patch 0 named TRAILING_EDGE, wall-function nutkWallFunction, y+ : min: 0.00457196 max: 0.00551105 average: 0.00492616

Patch 1 named SUCTION_SIDE, wall-function nutkWallFunction, y+ : min: 0.00260361 max: 0.0120975 average: 0.00588652

Patch 3 named PRESSURE_SIDE, wall-function nutkWallFunction, y+ : min: 0.00260361 max: 0.0120977 average: 0.00609504

Writing yPlus to field yPlus

[rupole1185]

First run the simulation and then calculate yPlus in the last time directory

[giammy92]

here the last time directory of yplus:

Time = 6500
Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RAS
Selecting RAS turbulence model kOmegaSST
kOmegaSSTCoeffs
{
alphaK1 0.85;
alphaK2 1;
alphaOmega1 0.5;
alphaOmega2 0.856;
gamma1 0.555556;
gamma2 0.44;
beta1 0.075;
beta2 0.0828;
betaStar 0.09;
a1 0.31;
b1 1;
c1 10;
F3 false;
}

Patch 0 named TRAILING_EDGE, wall-function nutkWallFunction, y+ : min: 0.000309772 max: 0.00849312 average: 0.00144718

Patch 1 named SUCTION_SIDE, wall-function nutkWallFunction, y+ : min: 9.736e-05 max: 0.122311 average: 0.0236659

Patch 3 named PRESSURE_SIDE, wall-function nutkWallFunction, y+ : min: 0.000192994 max: 0.117785 average: 0.0205445

Writing yPlus to field yPlus

End

[giammy92]

I have this doubt: for M=0.12, Re=1.5e6 e p=101325 Pa I have calculated a rho=1.1854 and mu=1.7908e-5 considering p=rho*R*T with T=298K.
But, i don't understand because in the precedent study with fluent with same parameters is been used rho=1.225 and mu=1.7894e-5.

[giammy92]

another confirm that i have to ask: in file forces_coeff is right to consider both lref and Aref 0.5459, value of chord lenght?

[giammy92]

these are my fvschemes and mu fv solution:

ddtSchemes
{
default steadyState;
}

gradSchemes
{
default Gauss linear;
}

divSchemes
{
default none;
div(phi,U) bounded Gauss linearUpwind grad(U);
div(phi,k) bounded Gauss upwind;
div(phi,omega) bounded Gauss upwind;
div((nuEff*dev2(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
default Gauss linear corrected;
}

interpolationSchemes
{
default linear;
}

snGradSchemes
{
default corrected;
}

wallDist
{
method meshWave;
}


solvers
{
p
{
solver GAMG;
tolerance 1e-06;
relTol 0.1;
smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
cacheAgglomeration true;
nCellsInCoarsestLevel 10;
agglomerator faceAreaPair;
mergeLevels 1;
}

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

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;
pRefCell 0;
pRefValue 0;

residualControl
{
p 1e-5;
U 1e-5;
k 1e-5;
omega 1e-5;
}
}

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

[giammy92]

I want use k omega SST for high value of reynold even if my y+ around airfoil is <1 because i want a flux turbulent fully developed. So which BC for wall should use?
now i'm using:
k kqRWallFunction
value uniform internalfield

nut nutkwallfunction
value uniform 0

omega omegawallfunction
value uniform internalfield

[giammy92]

My results of Cl, for every BC's that i have tried, still remain about 1.5, but Cl must be about 1.25. How is possible that? I have a mesh very fine with y+ less than 1. I've found a discussion http://www.cfd-online.com/Forums/ope...estigated.html in which is suggested to use follow bc's for wall:
-k, fixed value very small
-nut, calculated
-omega, omegawallfunction
For patch FAR_FIELD i've use:
-k, turbulentIntensityKineticEnergyInlet with value uniform calculated: 1.5(U*I)^2
-nut, calculated with value uniform 0;
-omega, turbulentMixingLengthFrequencyInlet with value uniform: 1/mu*rho*k*(mut/mu)^-1
and mixinglenght calculated from this formula http://www.cfd-online.com/Wiki/Turbulence_length_scale
My angle of attack is 13° so:
liftDir (-0.22495 0.97437 0);
dragDir (0.97437 0.22495 0);
Questions:
1) Do you validate these bc's and formula for my case?
2)Why did i have about same results of Cl with different bc's like nutkwallfunction, nutuspaldingwallfunction, nutlowre for nut and kqrwallfunction for k?
3)Could be the cause in fvschemes or fvsolution?
Please, help me, i have wasted a lot of time for this problem, i can't imagine what else i have to change!!

[anishtain4]

Hi,

I'm not an expert in airfoils but knowing from LES simulations upwind is over diffusive (induces higher viscosity, hence higher coefficients might be expected). You might want to try to run your case with

divSchemes
{
default none;
div(phi,U) Gauss linear;
div(phi,k) Gauss limitedLinear 1;
}

[giammy92]

now i'm trying with this:


ddtSchemes
{
default steadyState;
}

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

divSchemes
{
default none;
div(phi,U) bounded Gauss linear;
div(phi,k) bounded Gauss limitedLinear 1;
div(phi,omega) bounded Gauss limitedLinear 1;
div((nuEff*dev(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
default Gauss linear corrected;
}

interpolationSchemes
{
default linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
}