turbulentOmegaFvPatchScalarField.H

Go to the documentation of this file.

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Copyright (C) 2011-2026 OpenFOAM Foundation
     \\/     M anipulation  |
-------------------------------------------------------------------------------
License
    This file is part of OpenFOAM.
 
    OpenFOAM is free software: you can redistribute it and/or modify it
    under the terms of the GNU General Public License as published by
    the Free Software Foundation, either version 3 of the License, or
    (at your option) any later version.
 
    OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
    ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
    FITNESS FOR A PARTICULAR PURPOSE.  See the GNU General Public License
    for more details.
 
    You should have received a copy of the GNU General Public License
    along with OpenFOAM.  If not, see <http://www.gnu.org/licenses/>.
 
Class
    Foam::turbulentOmegaFvPatchScalarField
 
Description
    This boundary condition provides a turbulence specific dissipation,
    \f$\omega\f$ (omega) inlet condition based on a specified mixing length.
    The patch values are calculated using:
 
        \f[
            \omega_p = \frac{k^{0.5}}{C_{\mu}^{0.25} L}
        \f]
 
    where
 
    \vartable
        \omega_p | patch omega values
        C_{\mu} | Model coefficient, set to 0.09
        k       | turbulence kinetic energy
        L       | length scale
    \endvartable
 
Usage
    \table
        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
    \endtable
 
    Example of the boundary condition specification:
    \verbatim
    <patchName>
    {
        type            turbulentOmega;
        mixingLength    0.005;
        value           uniform 200;   // placeholder
    }
    \endverbatim
 
    Note:
        In the event of reverse flow, a zero-gradient condition is applied
 
See also
    Foam::inletOutletFvPatchField
 
SourceFiles
    turbulentOmegaFvPatchScalarField.C
 
\*---------------------------------------------------------------------------*/
 
#ifndef turbulentOmegaFvPatchScalarField_H
#define turbulentOmegaFvPatchScalarField_H
 
#include "inletOutletFvPatchFields.H"
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
namespace Foam
{
 
/*---------------------------------------------------------------------------*\
    Class turbulentOmegaFvPatchScalarField Declaration
\*---------------------------------------------------------------------------*/
 
class turbulentOmegaFvPatchScalarField
:
    public inletOutletFvPatchScalarField
{
    // Private Data
 
        //- Turbulent length scale
        scalar mixingLength_;
 
        //- Name of the turbulent kinetic energy field
        word kName_;
 
        //- Turbulence model coefficient
        scalar Cmu_;
 
 
public:
 
    //- Runtime type information
    TypeName("turbulentOmega");
 
 
    // Constructors
 
        //- Construct from patch, internal field and dictionary
        turbulentOmegaFvPatchScalarField
        (
            const fvPatch&,
            const DimensionedField<scalar, fvMesh>&,
            const dictionary&
        );
 
        //- Construct by mapping given
        //  turbulentOmegaFvPatchScalarField
        //  onto a new patch
        turbulentOmegaFvPatchScalarField
        (
            const turbulentOmegaFvPatchScalarField&,
            const fvPatch&,
            const DimensionedField<scalar, fvMesh>&,
            const fieldMapper&
        );
 
        //- Disallow copy without setting internal field reference
        turbulentOmegaFvPatchScalarField
        (
            const turbulentOmegaFvPatchScalarField&
        ) = delete;
 
        //- Copy constructor setting internal field reference
        turbulentOmegaFvPatchScalarField
        (
            const turbulentOmegaFvPatchScalarField&,
            const DimensionedField<scalar, fvMesh>&
        );
 
        //- Construct and return a clone setting internal field reference
        virtual tmp<fvPatchScalarField> clone
        (
            const DimensionedField<scalar, fvMesh>& iF
        ) const
        {
            return tmp<fvPatchScalarField>
            (
                new turbulentOmegaFvPatchScalarField
                (
                    *this,
                    iF
                )
            );
        }
 
 
    // Member Functions
 
        //- Update the coefficients associated with the patch field
        virtual void updateCoeffs();
 
        //- Write
        virtual void write(Ostream&) const;
 
 
    // Member Operators
 
        //- Inherit assignment
        using inletOutletFvPatchScalarField::operator=;
};
 
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
} // End namespace Foam
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#endif
 
// ************************************************************************* //