CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM (https://www.cfd-online.com/Forums/openfoam/)
-   -   pitzDailyMapped killing fluctuations (https://www.cfd-online.com/Forums/openfoam/182087-pitzdailymapped-killing-fluctuations.html)

Eman. December 30, 2016 14:12

pitzDailyMapped killing fluctuations
 
HI,

I was going through the pitzDailyMapped folder and it is supposed to create a turbulent inflow condition by mapping the velocity at a plane located in the downsteam of the flow back to the inlet plane. I noticed it uses averaging of velocity to maintain the volumetric flux. However, the average vector is (10,0,0), which means it kills the eddies and therefore the fluctuations over time by mapping the Uy and Uz to zero. Isn't it the whole idea of LES to take the fluctuations larger than the filter width into account? I assume the inlet profile would approach that of a laminar flow after enough time steps and if I'm right the whole simulation case of "pitzDailyMapped" makes no sense. Am I missing something here? any idea?

Many thanks in advance.

juho January 2, 2017 08:06

Here you can see how the setAverage works:

https://github.com/OpenFOAM/OpenFOAM...tchFieldBase.C

Code:

  if (setAverage_)
    {
        Type averagePsi =
            gSum(patchField_.patch().magSf()*newValues)
          /gSum(patchField_.patch().magSf());

        if (mag(averagePsi)/mag(average_) > 0.5)
        {
            newValues *= mag(average_)/mag(averagePsi);
        }
        else
        {
            newValues += (average_ - averagePsi);
        }
    }


Eman. January 2, 2017 17:32

Quote:

Originally Posted by juho (Post 631779)
Here you can see how the setAverage works:

https://github.com/OpenFOAM/OpenFOAM...tchFieldBase.C

Code:

  if (setAverage_)
    {
        Type averagePsi =
            gSum(patchField_.patch().magSf()*newValues)
          /gSum(patchField_.patch().magSf());

        if (mag(averagePsi)/mag(average_) > 0.5)
        {
            newValues *= mag(average_)/mag(averagePsi);
        }
        else
        {
            newValues += (average_ - averagePsi);
        }
    }


Thanks a lot for the reply. So, it rescales the velocity to maintain the flow rate. However, I tried to use mapped boundary condition on different geometries (2D and 3D) and everytime turbulence decays and I end up with a laminar velocity profile.

Also here on page 15 you can see:
"Care must be taken not to make the control algorithms too efficient; if the velocity control is too good then it can have the effect of completely destroying fluctuations in the velocity, thus unintentionally relaminarising the flow."

chegdan January 3, 2017 11:44

the way that channelFoam use to work for this type of application was to use a cyclic BC with a pressure gradient to drive the flow in a user-specified direction. Without the pressure gradient -> the flow decays. There is an fvoption in openFOAM-plus for pressure gradient source term to replicate that of channelFoam used like:

Code:

    airDeflection
    {
        type            directionalPressureGradientExplicitSource;
        active          true;

        directionalPressureGradientExplicitSourceCoeffs
        {
            selectionMode  cellZone;
            cellZone        cZone;

            fieldNames  (U);            // Name of the field
            flowDir    (1 1 0);        // Desired flow direction
            faceZone    f0Zone;        // Face zone upstream cell zone
            relaxationFactor    0.3;    // Relaxation factor for flow
                                        // deflection (default 0.3)

            //Pressure drop model [Pa]
            model      volumetricFlowRateTable;//constant;//DarcyForchheimer;

            //DarcyForchheimer model
            // deltaP = (D*mu + 0.5*rho*magUn)*magUn*length_

            D          5e7;
            I          0;
            length      1e-3;

            //constant model
            pressureDrop    40;

            //volumetricFlowRateTable model
            outOfBounds    clamp;
            fileName        "volFlowRateTable";
        }
    }



All times are GMT -4. The time now is 15:54.