turbulentMixingLengthFrequencyInletFvPatchScalarField Class Reference

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

Inheritance diagram for turbulentMixingLengthFrequencyInletFvPatchScalarField:

Collaboration diagram for turbulentMixingLengthFrequencyInletFvPatchScalarField:

Public Member Functions
	TypeName ("turbulentMixingLengthFrequencyInlet")
	Runtime type information. More...
	turbulentMixingLengthFrequencyInletFvPatchScalarField (const fvPatch &, const DimensionedField< scalar, volMesh > &)
	Construct from patch and internal field. More...
	turbulentMixingLengthFrequencyInletFvPatchScalarField (const fvPatch &, const DimensionedField< scalar, volMesh > &, const dictionary &)
	Construct from patch, internal field and dictionary. More...
	turbulentMixingLengthFrequencyInletFvPatchScalarField (const turbulentMixingLengthFrequencyInletFvPatchScalarField &, const fvPatch &, const DimensionedField< scalar, volMesh > &, const fvPatchFieldMapper &)
	Construct by mapping given. More...
	turbulentMixingLengthFrequencyInletFvPatchScalarField (const turbulentMixingLengthFrequencyInletFvPatchScalarField &)
	Construct as copy. More...
virtual tmp< fvPatchScalarField >	clone () const
	Construct and return a clone. More...
	turbulentMixingLengthFrequencyInletFvPatchScalarField (const turbulentMixingLengthFrequencyInletFvPatchScalarField &, 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 specific dissipation, \(\omega\) (omega) inlet condition based on a specified mixing length. The patch values are calculated using:

\[ \omega_p = \frac{k^{0.5}}{C_{\mu}^{0.25} L} \]

where

\( \omega_p \)	=	patch omega 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            turbulentMixingLengthFrequencyInlet;
        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

• turbulentMixingLengthFrequencyInletFvPatchScalarField.H
• turbulentMixingLengthFrequencyInletFvPatchScalarField.C

Definition at line 129 of file turbulentMixingLengthFrequencyInletFvPatchScalarField.H.

Constructor & Destructor Documentation

turbulentMixingLengthFrequencyInletFvPatchScalarField() [1/5]

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

Construct from patch and internal field.

Definition at line 45 of file turbulentMixingLengthFrequencyInletFvPatchScalarField.C.

turbulentMixingLengthFrequencyInletFvPatchScalarField() [2/5]

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

Construct from patch, internal field and dictionary.

Definition at line 75 of file turbulentMixingLengthFrequencyInletFvPatchScalarField.C.

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

Here is the call graph for this function:

turbulentMixingLengthFrequencyInletFvPatchScalarField() [3/5]

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

Construct by mapping given.

turbulentMixingLengthFrequencyInletFvPatchScalarField onto a new patch

Definition at line 61 of file turbulentMixingLengthFrequencyInletFvPatchScalarField.C.

turbulentMixingLengthFrequencyInletFvPatchScalarField() [4/5]

turbulentMixingLengthFrequencyInletFvPatchScalarField

(

const turbulentMixingLengthFrequencyInletFvPatchScalarField &

ptf

)

Construct as copy.

Definition at line 96 of file turbulentMixingLengthFrequencyInletFvPatchScalarField.C.

turbulentMixingLengthFrequencyInletFvPatchScalarField() [5/5]

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

Construct as copy setting internal field reference.

Definition at line 107 of file turbulentMixingLengthFrequencyInletFvPatchScalarField.C.

Member Function Documentation

TypeName()

TypeName

(

"turbulentMixingLengthFrequencyInlet"

)

Runtime type information.

clone() [1/2]

virtual tmp<fvPatchScalarField> clone ( ) const

inlinevirtual

Construct and return a clone.

Definition at line 183 of file turbulentMixingLengthFrequencyInletFvPatchScalarField.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 203 of file turbulentMixingLengthFrequencyInletFvPatchScalarField.H.

updateCoeffs()

void updateCoeffs ( )

virtual

Update the coefficients associated with the patch field.

Definition at line 120 of file turbulentMixingLengthFrequencyInletFvPatchScalarField.C.

References turbulenceModel::coeffDict(), dictionary::getOrDefault(), Foam::constant::atomic::group, IOobject::groupName(), 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 156 of file turbulentMixingLengthFrequencyInletFvPatchScalarField.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/turbulentMixingLengthFrequencyInlet/turbulentMixingLengthFrequencyInletFvPatchScalarField.H
• src/TurbulenceModels/turbulenceModels/RAS/derivedFvPatchFields/turbulentMixingLengthFrequencyInlet/turbulentMixingLengthFrequencyInletFvPatchScalarField.C