inletOutletFvPatchField.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) 2011-2022 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::inletOutletFvPatchField
 
Description
    This boundary condition provides a generic outflow condition, with
    specified inflow for the case of return flow.
 
Usage
    \table
        Property     | Description             | Required    | Default value
        phi          | Flux field name         | no          | phi
        inletValue   | Inlet value for reverse flow | yes    |
    \endtable
 
    Example of the boundary condition specification:
    \verbatim
    <patchName>
    {
        type            inletOutlet;
        phi             phi;
        inletValue      uniform 0;
        value           uniform 0;
    }
    \endverbatim
 
    The mode of operation is determined by the sign of the flux across the
    patch faces.
 
    Note:
        Sign conventions:
      - Positive flux (out of domain): apply zero-gradient condition
      - Negative flux (into of domain): apply the "inletValue" fixed-value
 
See also
    Foam::mixedFvPatchField
    Foam::zeroGradientFvPatchField
    Foam::outletInletFvPatchField
 
SourceFiles
    inletOutletFvPatchField.C
 
\*---------------------------------------------------------------------------*/
 
#ifndef inletOutletFvPatchField_H
#define inletOutletFvPatchField_H
 
#include "mixedFvPatchField.H"
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
namespace Foam
{
 
/*---------------------------------------------------------------------------*\
                   Class inletOutletFvPatchField Declaration
\*---------------------------------------------------------------------------*/
 
template<class Type>
class inletOutletFvPatchField
:
    public mixedFvPatchField<Type>
{
 
protected:
 
    // Protected data
 
        //- Name of flux field
        word phiName_;
 
 
public:
 
    //- Runtime type information
    TypeName("inletOutlet");
 
 
    // Constructors
 
        //- Construct from patch and internal field
        inletOutletFvPatchField
        (
            const fvPatch&,
            const DimensionedField<Type, volMesh>&
        );
 
        //- Construct from patch, internal field and dictionary
        inletOutletFvPatchField
        (
            const fvPatch&,
            const DimensionedField<Type, volMesh>&,
            const dictionary&
        );
 
        //- Construct by mapping given inletOutletFvPatchField onto a new patch
        inletOutletFvPatchField
        (
            const inletOutletFvPatchField<Type>&,
            const fvPatch&,
            const DimensionedField<Type, volMesh>&,
            const fvPatchFieldMapper&
        );
 
        //- Disallow copy without setting internal field reference
        inletOutletFvPatchField(const inletOutletFvPatchField<Type>&) = delete;
 
        //- Copy constructor setting internal field reference
        inletOutletFvPatchField
        (
            const inletOutletFvPatchField<Type>&,
            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 inletOutletFvPatchField<Type>(*this, iF)
            );
        }
 
 
    // Member Functions
 
        // Attributes
 
            //- Return true: this patch field is altered by assignment
            virtual bool assignable() const
            {
                return true;
            }
 
            //- Return the flux-field name
            const word& phiName() const
            {
                return phiName_;
            }
 
            //- Return access to the flux-field name
            word& phiName()
            {
                return phiName_;
            }
 
 
        //- Update the coefficients associated with the patch field
        virtual void updateCoeffs();
 
        //- Write
        virtual void write(Ostream&) const;
 
 
    // Member Operators
 
        virtual void operator=(const fvPatchField<Type>& pvf);
};
 
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
} // End namespace Foam
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#ifdef NoRepository
    #include "inletOutletFvPatchField.C"
#endif
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#endif
 
// ************************************************************************* //