This boundary condition provides an inlet condition for turbulent kinetic energy dissipation rate, i.e. epsilon, based on a specified mixing length. The patch values are calculated using: More...

#include <turbulentMixingLengthDissipationRateInletFvPatchScalarField.H>

Inheritance diagram for turbulentMixingLengthDissipationRateInletFvPatchScalarField:

[legend]

Collaboration diagram for turbulentMixingLengthDissipationRateInletFvPatchScalarField:

[legend]

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

Detailed Description

This boundary condition provides an inlet condition for turbulent kinetic energy dissipation rate, i.e. epsilon, 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 [m2/s3]
$C_\mu$	=	Empirical model constant retrived from turbulence model
	=	Turbulent kinetic energy [m2/s2]
	=	Mixing length scale [m]

Usage

Example of the boundary condition specification:

<patchName>
{
    // Mandatory entries (unmodifiable)
    type            turbulentMixingLengthDissipationRateInlet;

    // Mandatory entries (runtime modifiable)
    mixingLength    0.005;

    // Optional entries (runtime modifiable)
    Cmu             0.09;
    k               k;
    phi             phi;

    // Placeholder
    value           uniform 200;
}

where the entries mean:

Property	Description	Type	Req'd	Dflt
`mixingLength`	Mixing length scale [m]	scalar	yes	-
`Cmu`	Empirical model constant	scalar	no	0.09
`phi`	Name of flux field	word	no	phi
`k`	Name of turbulent kinetic energy field	word	no	k

Note

The boundary condition is derived from inletOutlet condition. Therefore, in the event of reverse flow, a zero-gradient condition is applied.
The order of precedence to input the empirical model constant Cmu is: turbulence model, boundary condition dictionary, and default value=0.09.
The empirical model constant Cmu is not a spatiotemporal variant field. Therefore, the use of the boundary condition may not be fully consistent with the turbulence models where Cmu is a variant field, such as realizableKE closure model in this respect. Nevertheless, workflow observations suggest that the matter poses no importance.

See also: Foam::inletOutletFvPatchField

Source files

Definition at line 155 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 36 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.C.

References p, and Foam::Zero.

Referenced by turbulentMixingLengthDissipationRateInletFvPatchScalarField(), turbulentMixingLengthDissipationRateInletFvPatchScalarField(), turbulentMixingLengthDissipationRateInletFvPatchScalarField(), and TypeName().

Here is the caller graph for this function:

◆ 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 70 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.C.

References dict, IOobjectOption::MUST_READ, p, and Foam::Zero.

◆ 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 54 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.C.

References p, and turbulentMixingLengthDissipationRateInletFvPatchScalarField().

Here is the call graph for this function:

◆ turbulentMixingLengthDissipationRateInletFvPatchScalarField() [4/5]

turbulentMixingLengthDissipationRateInletFvPatchScalarField ( const turbulentMixingLengthDissipationRateInletFvPatchScalarField & ptf )

Construct as copy.

Definition at line 96 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.C.

References turbulentMixingLengthDissipationRateInletFvPatchScalarField().

Here is the call graph for this function:

◆ turbulentMixingLengthDissipationRateInletFvPatchScalarField() [5/5]

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

Construct as copy setting internal field reference.

Definition at line 109 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.C.

References turbulentMixingLengthDissipationRateInletFvPatchScalarField().

Here is the call graph for this function:

Member Function Documentation

◆ TypeName()

TypeName ( "turbulentMixingLengthDissipationRateInlet" )

Runtime type information.

References turbulentMixingLengthDissipationRateInletFvPatchScalarField().

Here is the call graph for this function:

◆ clone() [1/2]

virtual tmp< fvPatchField< scalar > > clone ( ) const

inlinevirtual

Return a clone.

Definition at line 239 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.H.

References fvPatchField< Type >::Clone().

Here is the call graph for this function:

◆ clone() [2/2]

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

inlinevirtual

Clone with an internal field reference.

Definition at line 247 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.H.

References fvPatchField< Type >::Clone().

Here is the call graph for this function:

◆ updateCoeffs()

void updateCoeffs ( )

virtual

Update the coefficients associated with the patch field.

Definition at line 125 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.C.

References turbulenceModel::coeffDict(), dictionary::getOrDefault(), IOobject::groupName(), Foam::neg(), Foam::pow(), and turbulenceModel::propertiesName.

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 os(), fvPatchField< Type >::write(), and fvPatchField< Type >::writeValueEntry().

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

Public Member Functions

Detailed Description

Constructor & Destructor Documentation

◆ turbulentMixingLengthDissipationRateInletFvPatchScalarField() [1/5]

◆ turbulentMixingLengthDissipationRateInletFvPatchScalarField() [2/5]

◆ turbulentMixingLengthDissipationRateInletFvPatchScalarField() [3/5]

◆ turbulentMixingLengthDissipationRateInletFvPatchScalarField() [4/5]

◆ turbulentMixingLengthDissipationRateInletFvPatchScalarField() [5/5]

Member Function Documentation

◆ TypeName()

◆ clone() [1/2]

◆ clone() [2/2]

◆ updateCoeffs()

◆ write()