turbulentMixingLengthDissipationRateInletFvPatchScalarField Class Reference

This boundary condition provides a turbulence dissipation, \(\epsilon\) (epsilon) inlet condition based on a specified mixing length. The patch values are calculated using: More...

Inheritance diagram for turbulentMixingLengthDissipationRateInletFvPatchScalarField:

Collaboration diagram for turbulentMixingLengthDissipationRateInletFvPatchScalarField:

Public Member Functions
	TypeName ("turbulentMixingLengthDissipationRateInlet")
	Runtime type information. More...
	turbulentMixingLengthDissipationRateInletFvPatchScalarField (const fvPatch &, const DimensionedField< scalar, volMesh > &)
	Construct from patch and internal field. More...
	turbulentMixingLengthDissipationRateInletFvPatchScalarField (const fvPatch &, const DimensionedField< scalar, volMesh > &, const dictionary &)
	Construct from patch, internal field and dictionary. More...
	turbulentMixingLengthDissipationRateInletFvPatchScalarField (const turbulentMixingLengthDissipationRateInletFvPatchScalarField &, const fvPatch &, const DimensionedField< scalar, volMesh > &, const fvPatchFieldMapper &)
	Construct by mapping given. More...
	turbulentMixingLengthDissipationRateInletFvPatchScalarField (const turbulentMixingLengthDissipationRateInletFvPatchScalarField &)
	Construct as copy. More...
virtual tmp< fvPatchScalarField >	clone () const
	Construct and return a clone. More...
	turbulentMixingLengthDissipationRateInletFvPatchScalarField (const turbulentMixingLengthDissipationRateInletFvPatchScalarField &, const DimensionedField< scalar, volMesh > &)
	Construct as copy setting internal field reference. More...
virtual tmp< fvPatchScalarField >	clone (const DimensionedField< scalar, volMesh > &iF) const
	Construct and return a clone setting internal field reference. More...
virtual void	updateCoeffs ()
	Update the coefficients associated with the patch field. More...
virtual void	write (Ostream &) const
	Write. More...

Detailed Description

This boundary condition provides a turbulence dissipation, \(\epsilon\) (epsilon) inlet condition based on a specified mixing length. The patch values are calculated using:

\[ \epsilon_p = \frac{C_{\mu}^{0.75} k^{1.5}}{L} \]

where

\( \epsilon_p \)	=	patch epsilon values
\( C_{\mu} \)	=	Model coefficient, set to 0.09
\( k \)	=	turbulence kinetic energy
\( L \)	=	length scale

Usage

Property	Description	Required	Default value
mixingLength	Length scale [m]	yes
phi	flux field name	no	phi
k	turbulence kinetic energy field name	no	k

Example of the boundary condition specification:

    <patchName>
    {
        type            turbulentMixingLengthDissipationRateInlet;
        mixingLength    0.005;
        value           uniform 200;   // placeholder
    }

Note

In the event of reverse flow, a zero-gradient condition is applied

See also

Foam::inletOutletFvPatchField

Source files

• turbulentMixingLengthDissipationRateInletFvPatchScalarField.H
• turbulentMixingLengthDissipationRateInletFvPatchScalarField.C

Definition at line 128 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.H.

Constructor & Destructor Documentation

turbulentMixingLengthDissipationRateInletFvPatchScalarField() [1/5]

turbulentMixingLengthDissipationRateInletFvPatchScalarField	(	const fvPatch &	p,
		const DimensionedField< scalar, volMesh > &	iF
	)

Construct from patch and internal field.

Definition at line 44 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.C.

turbulentMixingLengthDissipationRateInletFvPatchScalarField() [2/5]

turbulentMixingLengthDissipationRateInletFvPatchScalarField	(	const fvPatch &	p,
		const DimensionedField< scalar, volMesh > &	iF,
		const dictionary &	dict
	)

Construct from patch, internal field and dictionary.

Definition at line 76 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.C.

References dict, dictionary::lookupOrDefault(), fvPatchField< scalar >::operator=(), and p.

Here is the call graph for this function:

turbulentMixingLengthDissipationRateInletFvPatchScalarField() [3/5]

turbulentMixingLengthDissipationRateInletFvPatchScalarField	(	const turbulentMixingLengthDissipationRateInletFvPatchScalarField &	ptf,
		const fvPatch &	p,
		const DimensionedField< scalar, volMesh > &	iF,
		const fvPatchFieldMapper &	mapper
	)

Construct by mapping given.

turbulentMixingLengthDissipationRateInletFvPatchScalarField onto a new patch

Definition at line 61 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.C.

turbulentMixingLengthDissipationRateInletFvPatchScalarField() [4/5]

turbulentMixingLengthDissipationRateInletFvPatchScalarField

(

const turbulentMixingLengthDissipationRateInletFvPatchScalarField &

ptf

)

Construct as copy.

Definition at line 98 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.C.

turbulentMixingLengthDissipationRateInletFvPatchScalarField() [5/5]

turbulentMixingLengthDissipationRateInletFvPatchScalarField	(	const turbulentMixingLengthDissipationRateInletFvPatchScalarField &	ptf,
		const DimensionedField< scalar, volMesh > &	iF
	)

Construct as copy setting internal field reference.

Definition at line 110 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.C.

Member Function Documentation

TypeName()

TypeName

(

"turbulentMixingLengthDissipationRateInlet"

)

Runtime type information.

clone() [1/2]

virtual tmp<fvPatchScalarField> clone ( ) const

inlinevirtual

Construct and return a clone.

Definition at line 182 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.H.

clone() [2/2]

virtual tmp<fvPatchScalarField> clone ( const DimensionedField< scalar, volMesh > &  iF ) const

inlinevirtual

Construct and return a clone setting internal field reference.

Definition at line 202 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.H.

updateCoeffs()

void updateCoeffs ( )

virtual

Update the coefficients associated with the patch field.

Definition at line 123 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.C.

References turbulenceModel::coeffDict(), Foam::constant::atomic::group, IOobject::groupName(), dictionary::lookupOrDefault(), Foam::foamVersion::patch, Foam::pos0(), Foam::pow(), turbulenceModel::propertiesName, and Foam::sqrt().

Here is the call graph for this function:

write()

void write ( Ostream &  os ) const

virtual

Write.

Definition at line 159 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.C.

References fvPatchField< scalar >::write(), and Ostream::writeEntry().

Here is the call graph for this function:

---

The documentation for this class was generated from the following files:

• src/TurbulenceModels/turbulenceModels/RAS/derivedFvPatchFields/turbulentMixingLengthDissipationRateInlet/turbulentMixingLengthDissipationRateInletFvPatchScalarField.H
• src/TurbulenceModels/turbulenceModels/RAS/derivedFvPatchFields/turbulentMixingLengthDissipationRateInlet/turbulentMixingLengthDissipationRateInletFvPatchScalarField.C