7037737d03
Contributed by Bruno Santos Resolves patch report http://www.openfoam.org/mantisbt/view.php?id=2023 Update online documentation http://openfoam.github.io/Documentation-dev/html/
364 lines
10 KiB
C++
364 lines
10 KiB
C++
/*---------------------------------------------------------------------------*\
|
|
========= |
|
|
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
|
|
\\ / O peration |
|
|
\\ / A nd | Copyright (C) 2011-2016 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 (\f$\gamma <= 1\f$):
|
|
\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 (\f$\gamma > 1\f$):
|
|
\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
|
|
|
|
// ************************************************************************* //
|