[ishan_ae]

Hello.

I am trying to initialize my rhoSimpleFoam solution with simpleFoam solution.

My geometry is part of a compressible subsonic flow in a duct on which experimental tests were made.

At the inlet I am totalPressure and at outlet I am using flowRateOutletVelocity. On the wall, for omega omegaWallFunction is being used.


I am not sure what's going wrong with my simpleFoam setup, because while the residuals and solution monitors are all-right, but the y+ values are extremely low. I was expecting the values close to 1.

I have the U magnitude contour plots and it is as if the flow is stuck in the core region of the duct with close to zero velocity near the walls. The flow accelerates in the duct core region because it is a nozzle like geometry overall but that's it.

Has anyone ever encountered such low order y+ values before while using sstkOmega model in OpenFOAM v6 ?

I have attachedthe fvSchemes, fvSolution and my residual plots. The peaks are where I stopped and started the solution to make some changes.

ddtSchemes
{
    default         steadyState;
}

gradSchemes
{
    default         Gauss linear;
}

divSchemes
{
    default         none;
    div(phi,U)      bounded Gauss linearUpwindV grad(U);

    div(div(phi,U))   Gauss linear;

    //for kinetic energy
    //div(phi,k)      bounded Gauss upwind;
    div(phi,k)        Gauss linearUpwind grad(k);
    
     //for omega
    div(phi,omega)  bounded Gauss upwind;

    
    //for energy 
    div(phi,e)    Gauss linear; //from U-bend tutorial

    //for epsilon
    div(phi,epsilon)  bounded Gauss upwind;


   // div(phi,nuTilda) Gauss linear;

    //div(phi,Ekp)        Gauss linear;

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

}

laplacianSchemes
{
    default         Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}


fluxRequired
{
    default         no;
    p;
}

wallDist
{
    method meshWave;
}

solvers
{

"p.*" 
{
        solver           GAMG;
        tolerance        1e-10;
        relTol           0.05;
        smoother         GaussSeidel;
        nPreSweeps       0;
        nPostSweeps      2;
        cacheAgglomeration on;
        agglomerator     faceAreaPair;
        nCellsInCoarsestLevel 10;
        mergeLevels      1;
        maxIter         20;
}

"U.*"
{
        solver           smoothSolver;
        smoother         GaussSeidel;
        tolerance        1e-10;
        relTol           0.1;
        nSweeps          1;
}

Phi
{
  $p;
}
 
"(k|epsilon|omega|nuTilda|kFinal|epsilonFinal|omegaFinal|e|rho)"
{
        solver           smoothSolver;
        smoother         GaussSeidel;
        tolerance        1e-10;
        relTol           0.1;
        nSweeps          1;
	maxIter		200;
}


}
 
SIMPLE
{
    nNonOrthogonalCorrectors 2;
    residualControl
    {
        p               1e-5;
        U               1e-4;
        k               1e-4;
        omega           1e-4;
	nuTilda         1e-4;
//	e		1e-3;
    }
}


relaxationFactors
{
    fields
    {
        p               0.3;
      //  rho             0.3;
    }
    equations
    {
        U               0.7;
        k               0.7;
        omega           0.3;
	 epsilon        0.3;
//	nuTilda         0.3;
        //e		0.3;
    }
}

cache
{
    grad(U);
}

[Carlo_P]

How is the yPlus in the simpleFoam?


Are you talking about the max, min or average yPlus?


The min can be very near zero, if the velocity is near zero.

[ishan_ae]

Maybe I was not clear enough. Sorry about that. The yplus values I am referring to are for simpleFoam simulation. They lie between 1e-5 and 1e-3.

As you mentioned, the velocities are zero but they shouldn't be. The max velocity is centered around the center of the duct, and decreases to zero as you move closer to the walls. Also, I am using zero velocities on the wall, so on the wall zero velocity is ok.

[Carlo_P]

Ah okok..


Can you attache the log file of the simulation?
Where you see that the yplus has that values?


Did you mesh by yourself?


How you decide the first layer hegth? Can you check how much is it?


Try here: https://www.cfd-online.com/Tools/yplus.php and check the values

[ishan_ae]

I used postProcess to calculate the y+ values. Unfortunately, I cannot show the yplus contour images at the moment. But these low values are on all the wall patches of the geometry.

Yes. I used a pre-processor for generating tet mesh all around. My first layer height(~2e-3 millimetres ) estimations are actually in-line with those estimated by multiple references who are using the same geometry for simulations with the same values for BC.

The mesh quality is also all-right with max non-ortho of 66 and max skewness =2.5, and max aspect ratio of 3600 close to the walls.

[Carlo_P]

Probably...are you calculating the yPlus for the las titeration or only for the first one?


Otherwise, should be nice to have some pics about yplus and velocity and mesh.


Probably can be a mesh problem? Not quality, but first height?

[ishan_ae]

I think I may have just found the mistake w.r.t my y+ values and possibly also the entire simpleFoam simulation.

I was checking the transportProperties file and noticed that the format was this:

nu nu[0 2 -1 0 0 0 0] 10.48e-6;

It should have been this:

nu [0 2 -1 0 0 0 0] 10.48e-6;


It looks like because of extra nu the values were never being read ? Not sure though.

However, now I have the expected flow pattern and y+ values close to 0.7.

I am not sure what it is going on in the background, but I really want to know about it. I broke my head for almost a week trying to figure it out. This maybe calls for a separate post and I will do that soon.