kLowReWallFunctionFvPatchScalarField.H

Go to the documentation of this file.

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | www.openfoam.com
     \\/     M anipulation  |
-------------------------------------------------------------------------------
    Copyright (C) 2012-2016, 2019 OpenFOAM Foundation
    Copyright (C) 2019 OpenCFD Ltd.
-------------------------------------------------------------------------------
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::kLowReWallFunctionFvPatchScalarField
 
Group
    grpWallFunctions
 
Description
    This boundary condition provides a wall constraint on turbulent kinetic
    energy, i.e. \c k, for low- and high-Reynolds number turbulence models.
 
    The model operates in two modes, based on the computed viscous-to-turbulent
    switch-over \c y+ value derived from \c kappa and \c E.
 
Usage
    \table
        Property     | Description             | Required    | Default value
        Ceps2        | Model coefficient       | no          |  1.9
        Ck           | Model coefficient       | no          | -0.416
        Bk           | Model coefficient       | no          |  8.366
        C            | Model coefficient       | no          |  11.0
    \endtable
 
    Example of the boundary condition specification:
    \verbatim
    <patchName>
    {
        // Mandatory entries
        type            kLowReWallFunction;
 
        // Optional entries
    }
    \endverbatim
 
Note
    The coefficients \c Cmu, \c kappa, and \c E are obtained from
    the specified \c nutWallFunction in order to ensure that each patch
    possesses the same set of values for these coefficients.
 
See also
    Foam::fixedValueFvPatchField
 
SourceFiles
    kLowReWallFunctionFvPatchScalarField.C
 
\*---------------------------------------------------------------------------*/
 
#ifndef kLowReWallFunctionFvPatchScalarField_H
#define kLowReWallFunctionFvPatchScalarField_H
 
#include "fixedValueFvPatchField.H"
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
namespace Foam
{
 
/*---------------------------------------------------------------------------*\
            Class kLowReWallFunctionFvPatchScalarField Declaration
\*---------------------------------------------------------------------------*/
 
class kLowReWallFunctionFvPatchScalarField
:
    public fixedValueFvPatchField<scalar>
{
protected:
 
    // Protected Data
 
        //- Ceps2 coefficient
        scalar Ceps2_;
 
        //- Ck coefficient
        scalar Ck_;
 
        //- Bk coefficient
        scalar Bk_;
 
        //- C coefficient
        scalar C_;
 
 
public:
 
    //- Runtime type information
    TypeName("kLowReWallFunction");
 
 
    // Constructors
 
        //- Construct from patch and internal field
        kLowReWallFunctionFvPatchScalarField
        (
            const fvPatch&,
            const DimensionedField<scalar, volMesh>&
        );
 
        //- Construct from patch, internal field and dictionary
        kLowReWallFunctionFvPatchScalarField
        (
            const fvPatch&,
            const DimensionedField<scalar, volMesh>&,
            const dictionary&
        );
 
        //- Construct by mapping given kLowReWallFunctionFvPatchScalarField
        //  onto a new patch
        kLowReWallFunctionFvPatchScalarField
        (
            const kLowReWallFunctionFvPatchScalarField&,
            const fvPatch&,
            const DimensionedField<scalar, volMesh>&,
            const fvPatchFieldMapper&
        );
 
        //- Construct as copy
        kLowReWallFunctionFvPatchScalarField
        (
            const kLowReWallFunctionFvPatchScalarField&
        );
 
        //- Construct and return a clone
        virtual tmp<fvPatchScalarField> clone() const
        {
            return tmp<fvPatchScalarField>
            (
                new kLowReWallFunctionFvPatchScalarField(*this)
            );
        }
 
        //- Construct as copy setting internal field reference
        kLowReWallFunctionFvPatchScalarField
        (
            const kLowReWallFunctionFvPatchScalarField&,
            const DimensionedField<scalar, volMesh>&
        );
 
        //- Construct and return a clone setting internal field reference
        virtual tmp<fvPatchScalarField> clone
        (
            const DimensionedField<scalar, volMesh>& iF
        ) const
        {
            return tmp<fvPatchScalarField>
            (
                new kLowReWallFunctionFvPatchScalarField(*this, iF)
            );
        }
 
 
    // Member Functions
 
        // Evaluation functions
 
            //- Update the coefficients associated with the patch field
            virtual void updateCoeffs();
 
 
        // I-O
 
            //- Write
            virtual void write(Ostream&) const;
};
 
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
} // End namespace Foam
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#endif
 
// ************************************************************************* //