nutURoughWallFunctionFvPatchScalarField.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) 2011-2023 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::nutURoughWallFunctionFvPatchScalarField
 
Description
    This boundary condition provides a turbulent kinematic viscosity condition
    when using wall functions for rough walls, based on velocity.  The
    condition manipulates the E parameter to account for roughness effects.
 
    Reference:
    \verbatim
        Cebeci, T., & Bradshaw, P. (1977).
        Momentum transfer in boundary layers.
        Washington, DC, Hemisphere Publishing Corp.; New York,
        McGraw-Hill Book Co., 1977. 407 p.
    \endverbatim
 
Usage
    \table
        Property     | Description             | Required    | Default value
        Ks           | sand-grain roughness height | yes     |
        Cs           | roughness constant      | yes         |
    \endtable
 
    Parameter ranges
    - roughness height (Ks) = sand-grain roughness (0 for smooth walls)
    - roughness constant (Cs) = 0.5 - 1.0
 
    Example of the boundary condition specification:
    \verbatim
    <patchName>
    {
        type            nutURoughWallFunction;
        Ks              uniform 1e-5;
        Cs              uniform 0.5;
        value           uniform 0;
    }
    \endverbatim
 
See also
    Foam::nutUWallFunctionFvPatchScalarField
 
SourceFiles
    nutURoughWallFunctionFvPatchScalarField.C
 
\*---------------------------------------------------------------------------*/
 
#ifndef nutURoughWallFunctionFvPatchScalarField_H
#define nutURoughWallFunctionFvPatchScalarField_H
 
#include "nutUWallFunctionFvPatchScalarField.H"
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
namespace Foam
{
 
/*---------------------------------------------------------------------------*\
           Class nutURoughWallFunctionFvPatchScalarField Declaration
\*---------------------------------------------------------------------------*/
 
class nutURoughWallFunctionFvPatchScalarField
:
    public nutUWallFunctionFvPatchScalarField
{
    // Private Data
 
        //- Roughness height
        scalarField Ks_;
 
        //- Roughness constant
        scalarField Cs_;
 
 
protected:
 
    // Protected Member Functions
 
        //- Calculate yPLus
        virtual tmp<scalarField> yPlus(const scalarField& magUp) const;
 
        //- Calculate the turbulence viscosity
        virtual tmp<scalarField> nut() const;
 
 
public:
 
    //- Runtime type information
    TypeName("nutURoughWallFunction");
 
 
    // Constructors
 
        //- Construct from patch, internal field and dictionary
        nutURoughWallFunctionFvPatchScalarField
        (
            const fvPatch&,
            const DimensionedField<scalar, volMesh>&,
            const dictionary&
        );
 
        //- Construct by mapping given
        //  nutURoughWallFunctionFvPatchScalarField
        //  onto a new patch
        nutURoughWallFunctionFvPatchScalarField
        (
            const nutURoughWallFunctionFvPatchScalarField&,
            const fvPatch&,
            const DimensionedField<scalar, volMesh>&,
            const fieldMapper&
        );
 
        //- Disallow copy without setting internal field reference
        nutURoughWallFunctionFvPatchScalarField
        (
            const nutURoughWallFunctionFvPatchScalarField&
        ) = delete;
 
        //- Copy constructor setting internal field reference
        nutURoughWallFunctionFvPatchScalarField
        (
            const nutURoughWallFunctionFvPatchScalarField&,
            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 nutURoughWallFunctionFvPatchScalarField(*this, iF)
            );
        }
 
 
    // Member Functions
 
        // Access functions
 
            //- Return the roughness height
            const scalarField& Ks() const
            {
                return Ks_;
            }
 
            //- Return reference to the roughness height to allow adjustment
            scalarField& Ks()
            {
                return Ks_;
            }
 
 
            //- Return the roughness constant scale
            const scalarField& Cs() const
            {
                return Cs_;
            }
 
            //- Return reference to the roughness constant to allow adjustment
            scalarField& Cs()
            {
                return Cs_;
            }
 
 
        // Mapping functions
 
            //- Map the given fvPatchField onto this fvPatchField
            virtual void map(const fvPatchScalarField&, const fieldMapper&);
 
            //- Reset the fvPatchField to the given fvPatchField
            //  Used for mesh to mesh mapping
            virtual void reset(const fvPatchScalarField&);
 
 
        // I-O
 
            //- Write
            virtual void write(Ostream& os) const;
};
 
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
} // End namespace Foam
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#endif
 
// ************************************************************************* //