waveTransmissiveFvPatchField.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::waveTransmissiveFvPatchField
 
Description
    This boundary condition provides a wave transmissive outflow condition,
    based on solving DDt(W, field) = 0 at the boundary \c W is the wave velocity
    and \c field is the field to which this boundary condition is applied.
 
    The wave speed is calculated using:
 
        \f[
            w_p = \frac{\phi_p}{|Sf|} + \sqrt{\frac{\gamma}{\psi_p}}
        \f]
 
    where
 
    \vartable
        w_p     | patch wave speed
        \phi_p  | patch face flux
        \psi_p  | patch compressibility
        Sf      | patch face area vector
        \gamma  | ratio of specific heats
    \endvartable
 
Usage
    \table
        Property     | Description             | Required    | Default value
        phi          | flux field name         | no          | phi
        rho          | density field name      | no          | rho
        psi          | compressibility field name | no       | psi
        gamma        | ratio of specific heats (Cp/Cv) | yes |
    \endtable
 
    Example of the boundary condition specification:
    \verbatim
    <patchName>
    {
        type            waveTransmissive;
        phi             phi;
        psi             psi;
        gamma           1.4;
    }
    \endverbatim
 
See also
    Foam::advectiveFvPatchField
 
SourceFiles
    waveTransmissiveFvPatchField.C
 
\*---------------------------------------------------------------------------*/
 
#ifndef waveTransmissiveFvPatchField_H
#define waveTransmissiveFvPatchField_H
 
#include "advectiveFvPatchFields.H"
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
namespace Foam
{
 
/*---------------------------------------------------------------------------*\
                Class waveTransmissiveFvPatchField Declaration
\*---------------------------------------------------------------------------*/
 
template<class Type>
class waveTransmissiveFvPatchField
:
    public advectiveFvPatchField<Type>
{
 
    // Private Data
 
        //- Name of the compressibility field used to calculate the wave speed
        word psiName_;
 
        //- Heat capacity ratio
        scalar gamma_;
 
 
public:
 
    //- Runtime type information
    TypeName("waveTransmissive");
 
 
    // Constructors
 
        //- Construct from patch, internal field and dictionary
        waveTransmissiveFvPatchField
        (
            const fvPatch&,
            const DimensionedField<Type, volMesh>&,
            const dictionary&
        );
 
        //- Construct by mapping given waveTransmissiveFvPatchField
        //  onto a new patch
        waveTransmissiveFvPatchField
        (
            const waveTransmissiveFvPatchField<Type>&,
            const fvPatch&,
            const DimensionedField<Type, volMesh>&,
            const fvPatchFieldMapper&
        );
 
        //- Disallow copy without setting internal field reference
        waveTransmissiveFvPatchField
        (
            const waveTransmissiveFvPatchField&
        ) = delete;
 
        //- Copy constructor setting internal field reference
        waveTransmissiveFvPatchField
        (
            const waveTransmissiveFvPatchField&,
            const DimensionedField<Type, volMesh>&
        );
 
        //- Construct and return a clone setting internal field reference
        virtual tmp<fvPatchField<Type>> clone
        (
            const DimensionedField<Type, volMesh>& iF
        ) const
        {
            return tmp<fvPatchField<Type>>
            (
                new waveTransmissiveFvPatchField<Type>(*this, iF)
            );
        }
 
 
    // Member Functions
 
        // Access
 
            //- Return the heat capacity ratio
            scalar gamma() const
            {
                return gamma_;
            }
 
            //- Return reference to the heat capacity ratio to allow adjustment
            scalar& gamma()
            {
                return gamma_;
            }
 
 
        // Evaluation functions
 
            //- Calculate and return the advection speed at the boundary
            virtual tmp<scalarField> advectionSpeed() const;
 
 
        //- Write
        virtual void write(Ostream&) const;
};
 
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
} // End namespace Foam
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#ifdef NoRepository
    #include "waveTransmissiveFvPatchField.C"
#endif
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#endif
 
// ************************************************************************* //