[nwpukaka]

Hi,

For this outlet boundary condition with backflow, I want to set turbulence kinetic energy and dissipation rate for this backflow, what kind of boundary conditions should I set? and how does the code determine that this is backflow?

Thanks in advance

Kan

[skyinventorbt]

Originally Posted by nwpukaka

Hi,

For this outlet boundary condition with backflow, I want to set turbulence kinetic energy and dissipation rate for this backflow, what kind of boundary conditions should I set? and how does the code determine that this is backflow?

Thanks in advance

Kan

Try inletOutletVelocity BC

--
KANNAN B T

[nwpukaka]

Originally Posted by skyinventorbt

Try inletOutletVelocity BC

--
KANNAN B T

Thank you very much, KANNAN.

About this inletOutlet BC, it says it switches U and p between fixedValue and zeroGradient depending on direction of U, for the direction of U, does that mean the normal direction of velocity of bounding cell?

Kan

[fumiya]

Hi,

The direction of U is determined by the sign of the flux ("phi" field) across the patch faces:

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

template<class Type>
void Foam::inletOutletFvPatchField<Type>::updateCoeffs()
{
    if (this->updated())
    {
        return;
    }

    const Field<scalar>& phip =
        this->patch().template lookupPatchField<surfaceScalarField, scalar>
        (
            phiName_
        );

    this->valueFraction() = 1.0 - pos(phip);

    mixedFvPatchField<Type>::updateCoeffs();
}

On the outlet patches

• positive flux (out of domain) phi>=0: pos(phi)=1 and valueFraction=0 apply zero-gradient condition
• negative flux (into of domain) phi<0: pos(phi)=0 and valueFraction = 1 apply the user-specified fixed value

This switching is performed using the mixedFvPatchField:
https://github.com/OpenFOAM/OpenFOAM...FvPatchField.C

template<class Type>
void mixedFvPatchField<Type>::evaluate(const Pstream::commsTypes)
{
    if (!this->updated())
    {
        this->updateCoeffs();
    }

    Field<Type>::operator=
    (
        valueFraction_*refValue_
      +
        (1.0 - valueFraction_)*
        (
            this->patchInternalField()
          + refGrad_/this->patch().deltaCoeffs()
        )
    );

    fvPatchField<Type>::evaluate();
}

Hope this helps,
Fumiya

[nwpukaka]

Originally Posted by fumiya

Hi,

The direction of U is determined by the sign of the flux ("phi" field) across the patch faces:

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

template<class Type>
void Foam::inletOutletFvPatchField<Type>::updateCoeffs()
{
    if (this->updated())
    {
        return;
    }

    const Field<scalar>& phip =
        this->patch().template lookupPatchField<surfaceScalarField, scalar>
        (
            phiName_
        );

    this->valueFraction() = 1.0 - pos(phip);

    mixedFvPatchField<Type>::updateCoeffs();
}

On the outlet patches

• positive flux (out of domain) phi>=0: pos(phi)=1 and valueFraction=0 apply zero-gradient condition
• negative flux (into of domain) phi<0: pos(phi)=0 and valueFraction = 1 apply the user-specified fixed value

This switching is performed using the mixedFvPatchField:
https://github.com/OpenFOAM/OpenFOAM...FvPatchField.C

template<class Type>
void mixedFvPatchField<Type>::evaluate(const Pstream::commsTypes)
{
    if (!this->updated())
    {
        this->updateCoeffs();
    }

    Field<Type>::operator=
    (
        valueFraction_*refValue_
      +
        (1.0 - valueFraction_)*
        (
            this->patchInternalField()
          + refGrad_/this->patch().deltaCoeffs()
        )
    );

    fvPatchField<Type>::evaluate();
}

Hope this helps,
Fumiya

Thank you very much. Fumiya.

It really helps!

Kan