Public Member Functions | List of all members
turbulentOmegaFvPatchScalarField 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 turbulentOmegaFvPatchScalarField:
Inheritance graph
[legend]
Collaboration diagram for turbulentOmegaFvPatchScalarField:
Collaboration graph
[legend]

Public Member Functions

 TypeName ("turbulentOmega")
 Runtime type information. More...
 
 turbulentOmegaFvPatchScalarField (const fvPatch &, const DimensionedField< scalar, fvMesh > &, const dictionary &)
 Construct from patch, internal field and dictionary. More...
 
 turbulentOmegaFvPatchScalarField (const turbulentOmegaFvPatchScalarField &, const fvPatch &, const DimensionedField< scalar, fvMesh > &, const fieldMapper &)
 Construct by mapping given. More...
 
 turbulentOmegaFvPatchScalarField (const turbulentOmegaFvPatchScalarField &)=delete
 Disallow copy without setting internal field reference. More...
 
 turbulentOmegaFvPatchScalarField (const turbulentOmegaFvPatchScalarField &, const DimensionedField< scalar, fvMesh > &)
 Copy constructor setting internal field reference. More...
 
virtual tmp< fvPatchScalarField > clone (const DimensionedField< scalar, fvMesh > &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
Cmu Turbulence model coefficient no 0.09

Example of the boundary condition specification: 

    <patchName>
    {
        type            turbulentOmega;
        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

Definition at line 129 of file turbulentOmegaFvPatchScalarField.H.

Constructor & Destructor Documentation

◆ turbulentOmegaFvPatchScalarField() [1/4]

turbulentOmegaFvPatchScalarField ( const fvPatch &  p,
const DimensionedField< scalar, fvMesh > &  iF,
const dictionary &  dict 
)

Construct from patch, internal field and dictionary.

Definition at line 40 of file turbulentOmegaFvPatchScalarField.C.

References dict, DimensionedField< Type, GeoMesh, PrimitiveField >::dimensions(), fvPatchField< Type >::operator, and p.

Here is the call graph for this function:

◆ turbulentOmegaFvPatchScalarField() [2/4]

turbulentOmegaFvPatchScalarField ( const turbulentOmegaFvPatchScalarField &  ptf,
const fvPatch &  p,
const DimensionedField< scalar, fvMesh > &  iF,
const fieldMapper &  mapper 
)

Construct by mapping given.

turbulentOmegaFvPatchScalarField onto a new patch

Definition at line 66 of file turbulentOmegaFvPatchScalarField.C.

◆ turbulentOmegaFvPatchScalarField() [3/4]

turbulentOmegaFvPatchScalarField ( const turbulentOmegaFvPatchScalarField &  )
delete

Disallow copy without setting internal field reference.

◆ turbulentOmegaFvPatchScalarField() [4/4]

turbulentOmegaFvPatchScalarField ( const turbulentOmegaFvPatchScalarField &  ptf,
const DimensionedField< scalar, fvMesh > &  iF 
)

Copy constructor setting internal field reference.

Definition at line 82 of file turbulentOmegaFvPatchScalarField.C.

Member Function Documentation

◆ TypeName()

TypeName ( "turbulentOmega"  )

Runtime type information.

◆ clone()

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

Construct and return a clone setting internal field reference.

Definition at line 186 of file turbulentOmegaFvPatchScalarField.H.

◆ updateCoeffs()

void updateCoeffs ( )
virtual

Update the coefficients associated with the patch field.

Definition at line 98 of file turbulentOmegaFvPatchScalarField.C.

References Foam::neg(), Foam::pow(), and Foam::sqrt().

Here is the call graph for this function:

◆ write()

void write ( Ostream &  os) const
virtual

Write.

Definition at line 120 of file turbulentOmegaFvPatchScalarField.C.

References fvPatchField< Type >::write(), and Foam::writeEntry().

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