CFD Online Discussion Forums - pitzDailyMapped killing fluctuations

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)

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.

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);

        }

    }

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."

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";

        }

    }

Quote:

Originally Posted by Eman. (Post 631822)

Hello Eman,

Did you solve this issue? The problem in which you get laminar flow when applying the mapped velocity boundary condition. I am trying to simulate a pipe flow using this method and all I get is a averaged-looked profile instead of a fluctuating one.

Thank you,

Sina