totalPressureFvPatchScalarField.H

Go to the documentation of this file.

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2011-2015 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::totalPressureFvPatchScalarField
 
Group
    grpInletBoundaryConditions grpOutletBoundaryConditions
 
Description
    This boundary condition provides a total pressure condition.  Four
    variants are possible:
 
    1. incompressible subsonic:
        \f[
            p_p = p_0 - 0.5 |U|^2
        \f]
        where
        \vartable
            p_p     | incompressible pressure at patch [m2/s2]
            p_0     | incompressible total pressure [m2/s2]
            U       | velocity
        \endvartable
 
    2. compressible subsonic:
        \f[
            p_p = p_0 - 0.5 \rho |U|^2
        \f]
        where
        \vartable
            p_p     | pressure at patch [Pa]
            p_0     | total pressure [Pa]
            \rho    | density [kg/m3]
            U       | velocity
        \endvartable
 
    3. compressible transonic (\gamma <= 1):
        \f[
            p_p = \frac{p_0}{1 + 0.5 \psi |U|^2}
        \f]
        where
        \vartable
            p_p     | pressure at patch [Pa]
            p_0     | total pressure [Pa]
            G       | coefficient given by \f$\frac{\gamma}{1-\gamma}\f$
        \endvartable
 
    4. compressible supersonic (\gamma > 1):
        \f[
            p_p = \frac{p_0}{(1 + 0.5 \psi G |U|^2)^{\frac{1}{G}}}
        \f]
        where
        \vartable
            p_p     | pressure at patch [Pa]
            p_0     | total pressure [Pa]
            \gamma  | ratio of specific heats (Cp/Cv)
            \psi    | compressibility [m2/s2]
            G       | coefficient given by \f$\frac{\gamma}{1-\gamma}\f$
        \endvartable
 
    The modes of operation are set via the combination of \c phi, \c rho, and
    \c psi entries:
    \table
        Mode                    | phi   | rho   | psi
        incompressible subsonic | phi   | none  | none
        compressible subsonic   | phi   | rho   | none
        compressible transonic  | phi   | none  | psi
        compressible supersonic | phi   | none  | psi
    \endtable
 
 
    \heading Patch usage
 
    \table
        Property     | Description             | Required    | Default value
        U            | velocity field name     | no          | U
        phi          | flux field name         | no          | phi
        rho          | density field name      | no          | none
        psi          | compressibility field name | no       | none
        gamma        | ratio of specific heats (Cp/Cv) | yes |
        p0           | total pressure          | yes       |
    \endtable
 
    Example of the boundary condition specification:
    \verbatim
    myPatch
    {
        type            totalPressure;
        U               U;
        phi             phi;
        rho             none;
        psi             none;
        gamma           1.4;
        p0              uniform 1e5;
    }
    \endverbatim
 
Note
    The default boundary behaviour is for subsonic, incompressible flow.
 
SeeAlso
    Foam::fixedValueFvPatchField
 
SourceFiles
    totalPressureFvPatchScalarField.C
 
\*---------------------------------------------------------------------------*/
 
#ifndef totalPressureFvPatchScalarField_H
#define totalPressureFvPatchScalarField_H
 
#include "fixedValueFvPatchFields.H"
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
namespace Foam
{
 
/*---------------------------------------------------------------------------*\
              Class totalPressureFvPatchScalarField Declaration
\*---------------------------------------------------------------------------*/
 
class totalPressureFvPatchScalarField
:
    public fixedValueFvPatchScalarField
{
    // Private data
 
        //- Name of the velocity field
        word UName_;
 
        //- Name of the flux transporting the field
        word phiName_;
 
        //- Name of the density field used to normalise the mass flux
        //  if neccessary
        word rhoName_;
 
        //- Name of the compressibility field used to calculate the wave speed
        word psiName_;
 
        //- Heat capacity ratio
        scalar gamma_;
 
        //- Total pressure
        scalarField p0_;
 
 
public:
 
    //- Runtime type information
    TypeName("totalPressure");
 
 
    // Constructors
 
        //- Construct from patch and internal field
        totalPressureFvPatchScalarField
        (
            const fvPatch&,
            const DimensionedField<scalar, volMesh>&
        );
 
        //- Construct from patch, internal field and dictionary
        totalPressureFvPatchScalarField
        (
            const fvPatch&,
            const DimensionedField<scalar, volMesh>&,
            const dictionary&
        );
 
        //- Construct by mapping given totalPressureFvPatchScalarField
        //  onto a new patch
        totalPressureFvPatchScalarField
        (
            const totalPressureFvPatchScalarField&,
            const fvPatch&,
            const DimensionedField<scalar, volMesh>&,
            const fvPatchFieldMapper&
        );
 
        //- Construct as copy
        totalPressureFvPatchScalarField
        (
            const totalPressureFvPatchScalarField&
        );
 
        //- Construct and return a clone
        virtual tmp<fvPatchScalarField> clone() const
        {
            return tmp<fvPatchScalarField>
            (
                new totalPressureFvPatchScalarField(*this)
            );
        }
 
        //- Construct as copy setting internal field reference
        totalPressureFvPatchScalarField
        (
            const totalPressureFvPatchScalarField&,
            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 totalPressureFvPatchScalarField(*this, iF)
            );
        }
 
 
    // Member functions
 
        // Access
 
            //- Return the name of the velocity field
            const word& UName() const
            {
                return UName_;
            }
 
            //- Return reference to the name of the velocity field
            //  to allow adjustment
            word& UName()
            {
                return UName_;
            }
 
            //- Return the name of the flux field
            const word& phiName() const
            {
                return phiName_;
            }
 
            //- Return reference to the name of the flux field
            //  to allow adjustment
            word& phiName()
            {
                return phiName_;
            }
 
            //- Return the name of the density field
            const word& rhoName() const
            {
                return rhoName_;
            }
 
            //- Return reference to the name of the density field
            //  to allow adjustment
            word& rhoName()
            {
                return rhoName_;
            }
 
            //- Return the name of the compressibility field
            const word& psiName() const
            {
                return psiName_;
            }
 
            //- Return reference to the name of the compressibility field
            //  to allow adjustment
            word& psiName()
            {
                return psiName_;
            }
 
            //- Return the heat capacity ratio
            scalar gamma() const
            {
                return gamma_;
            }
 
            //- Return reference to the heat capacity ratio to allow adjustment
            scalar& gamma()
            {
                return gamma_;
            }
 
            //- Return the total pressure
            const scalarField& p0() const
            {
                return p0_;
            }
 
            //- Return reference to the total pressure to allow adjustment
            scalarField& p0()
            {
                return p0_;
            }
 
 
        // Mapping functions
 
            //- Map (and resize as needed) from self given a mapping object
            virtual void autoMap
            (
                const fvPatchFieldMapper&
            );
 
            //- Reverse map the given fvPatchField onto this fvPatchField
            virtual void rmap
            (
                const fvPatchScalarField&,
                const labelList&
            );
 
 
        // Evaluation functions
 
            //- Inherit updateCoeffs from fixedValueFvPatchScalarField
            using fixedValueFvPatchScalarField::updateCoeffs;
 
            //- Update the coefficients associated with the patch field
            //  using the given patch total pressure and velocity fields
            virtual void updateCoeffs
            (
                const scalarField& p0p,
                const vectorField& Up
            );
 
            //- Update the coefficients associated with the patch field
            virtual void updateCoeffs();
 
 
        //- Write
        virtual void write(Ostream&) const;
};
 
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
} // End namespace Foam
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#endif
 
// ************************************************************************* //