Permalink
Switch branches/tags
Find file Copy path
Fetching contributors…
Cannot retrieve contributors at this time
199 lines (153 sloc) 5.97 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::turbulentMixingLengthDissipationRateInletFvPatchScalarField
Group
grpRASBoundaryConditions grpInletBoundaryConditions
Description
This boundary condition provides a turbulence dissipation, \f$\epsilon\f$
(epsilon) inlet condition based on a specified mixing length. The patch
values are calculated using:
\f[
\epsilon_p = \frac{C_{\mu}^{0.75} k^{1.5}}{L}
\f]
where
\vartable
\epsilon_p | patch epsilon values
C_{\mu} | Model coefficient, set to 0.09
k | turbulence kinetic energy
L | length scale
\endvartable
Usage
\table
Property | Description | Required | Default value
mixingLength | Length scale [m] | yes |
phi | flux field name | no | phi
k | turbulence kinetic energy field name | no | k
\endtable
Example of the boundary condition specification:
\verbatim
<patchName>
{
type turbulentMixingLengthDissipationRateInlet;
mixingLength 0.005;
value uniform 200; // placeholder
}
\endverbatim
Note
In the event of reverse flow, a zero-gradient condition is applied
See also
Foam::inletOutletFvPatchField
SourceFiles
turbulentMixingLengthDissipationRateInletFvPatchScalarField.C
\*---------------------------------------------------------------------------*/
#ifndef turbulentMixingLengthDissipationRateInlet_H
#define turbulentMixingLengthDissipationRateInlet_H
#include "inletOutletFvPatchFields.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
namespace Foam
{
/*---------------------------------------------------------------------------*\
Class turbulentMixingLengthDissipationRateInletFvPatchScalarField Declaration
\*---------------------------------------------------------------------------*/
class turbulentMixingLengthDissipationRateInletFvPatchScalarField
:
public inletOutletFvPatchScalarField
{
// Private data
//- Turbulent length scale
scalar mixingLength_;
//- Name of the turbulent kinetic energy field
word kName_;
public:
//- Runtime type information
TypeName("turbulentMixingLengthDissipationRateInlet");
// Constructors
//- Construct from patch and internal field
turbulentMixingLengthDissipationRateInletFvPatchScalarField
(
const fvPatch&,
const DimensionedField<scalar, volMesh>&
);
//- Construct from patch, internal field and dictionary
turbulentMixingLengthDissipationRateInletFvPatchScalarField
(
const fvPatch&,
const DimensionedField<scalar, volMesh>&,
const dictionary&
);
//- Construct by mapping given
// turbulentMixingLengthDissipationRateInletFvPatchScalarField
// onto a new patch
turbulentMixingLengthDissipationRateInletFvPatchScalarField
(
const turbulentMixingLengthDissipationRateInletFvPatchScalarField&,
const fvPatch&,
const DimensionedField<scalar, volMesh>&,
const fvPatchFieldMapper&
);
//- Construct as copy
turbulentMixingLengthDissipationRateInletFvPatchScalarField
(
const turbulentMixingLengthDissipationRateInletFvPatchScalarField&
);
//- Construct and return a clone
virtual tmp<fvPatchScalarField> clone() const
{
return tmp<fvPatchScalarField>
(
new turbulentMixingLengthDissipationRateInletFvPatchScalarField
(
*this
)
);
}
//- Construct as copy setting internal field reference
turbulentMixingLengthDissipationRateInletFvPatchScalarField
(
const turbulentMixingLengthDissipationRateInletFvPatchScalarField&,
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 turbulentMixingLengthDissipationRateInletFvPatchScalarField
(
*this,
iF
)
);
}
// Member functions
//- Update the coefficients associated with the patch field
virtual void updateCoeffs();
//- Write
virtual void write(Ostream&) const;
};
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
} // End namespace Foam
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#endif
// ************************************************************************* //