Public Member Functions | List of all members
turbulentMixingLengthDissipationRateInletFvPatchScalarField Class Reference
Turbulence models » RAS turbulence » Boundary conditionsBoundary conditions » | Inlet

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...

Inheritance diagram for turbulentMixingLengthDissipationRateInletFvPatchScalarField:
Inheritance graph
[legend]
Collaboration diagram for turbulentMixingLengthDissipationRateInletFvPatchScalarField:
Collaboration graph
[legend]

Public Member Functions

 TypeName ("turbulentMixingLengthDissipationRateInlet")
 
 turbulentMixingLengthDissipationRateInletFvPatchScalarField (const fvPatch &, const DimensionedField< scalar, volMesh > &)
 
 turbulentMixingLengthDissipationRateInletFvPatchScalarField (const fvPatch &, const DimensionedField< scalar, volMesh > &, const dictionary &)
 
 turbulentMixingLengthDissipationRateInletFvPatchScalarField (const turbulentMixingLengthDissipationRateInletFvPatchScalarField &, const fvPatch &, const DimensionedField< scalar, volMesh > &, const fvPatchFieldMapper &)
 
 turbulentMixingLengthDissipationRateInletFvPatchScalarField (const turbulentMixingLengthDissipationRateInletFvPatchScalarField &)
 
virtual tmp< fvPatchScalarField > clone () const
 
 turbulentMixingLengthDissipationRateInletFvPatchScalarField (const turbulentMixingLengthDissipationRateInletFvPatchScalarField &, const DimensionedField< scalar, volMesh > &)
 
virtual tmp< fvPatchScalarField > clone (const DimensionedField< scalar, volMesh > &iF) const
 
virtual void updateCoeffs ()
 
virtual void write (Ostream &) const
 

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
$ k $ = Turbulent kinetic energy [m2/s2]
$ L $ = 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 
)

Definition at line 38 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.C.

◆ turbulentMixingLengthDissipationRateInletFvPatchScalarField() [2/5]

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

Definition at line 72 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.C.

References dict, dictionary::getOrDefault(), fvPatchField::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 
)

Definition at line 56 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.C.

◆ turbulentMixingLengthDissipationRateInletFvPatchScalarField() [4/5]

turbulentMixingLengthDissipationRateInletFvPatchScalarField ( const turbulentMixingLengthDissipationRateInletFvPatchScalarField &  ptf)

Definition at line 98 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.C.

◆ turbulentMixingLengthDissipationRateInletFvPatchScalarField() [5/5]

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

Definition at line 111 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.C.

Member Function Documentation

◆ TypeName()

TypeName ( "turbulentMixingLengthDissipationRateInlet"  )

◆ clone() [1/2]

virtual tmp<fvPatchScalarField> clone ( ) const
inlinevirtual

Definition at line 212 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.H.

◆ clone() [2/2]

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

Definition at line 232 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.H.

◆ updateCoeffs()

void updateCoeffs ( )
virtual

Definition at line 125 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.C.

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

Here is the call graph for this function:

◆ write()

void write ( Ostream &  os) const
virtual

Definition at line 160 of file turbulentMixingLengthDissipationRateInletFvPatchScalarField.C.

References os(), fvPatchField::write(), and Ostream::writeEntry().

Here is the call graph for this function:
The documentation for this class was generated from the following files:

Copyright © 2011-2018  OpenFOAM | OPENFOAM® is a registered trademark of OpenCFD Ltd.

Generated by   doxygen 1.8.17