Permalink
Switch branches/tags
Find file Copy path
Fetching contributors…
Cannot retrieve contributors at this time
357 lines (283 sloc) 10.1 KB
/*---------------------------------------------------------------------------*\
========= |
\\ / 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 by the dimensions of the pressure field
to which this boundary condition is applied, the \c psi entry and the value
of \c gamma:
\table
Mode | dimensions | psi | gamma
incompressible subsonic | p/rho | |
compressible subsonic | p | none |
compressible transonic | p | psi | 1
compressible supersonic | p | psi | > 1
\endtable
Usage
\table
Property | Description | Required | Default value
U | Velocity field name | no | U
phi | Flux field name | no | phi
rho | Density field name | no | rho
psi | Compressibility field name | no | none
gamma | (Cp/Cv) | no | 1
p0 | Total pressure | yes |
\endtable
Example of the boundary condition specification:
\verbatim
<patchName>
{
type totalPressure;
p0 uniform 1e5;
}
\endverbatim
See also
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
// ************************************************************************* //