Skip to content
Permalink
Fetching contributors…
Cannot retrieve contributors at this time
191 lines (145 sloc) 5.39 KB
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Copyright (C) 2011-2018 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::compressible::alphatWallFunctionFvPatchScalarField
Description
This boundary condition provides a turbulent thermal diffusivity conditon
when using wall functions
- replicates OpenFOAM v1.5 (and earlier) behaviour
The turbulent thermal diffusivity calculated using:
\f[
\alpha_t = \frac{\mu_t}{Pr_t}
\f]
where
\vartable
\alpha_t| turblence thermal diffusivity
\mu_t | turblence viscosity
Pr_t | turblent Prandtl number
\endvartable
Usage
\table
Property | Description | Required | Default value
nut | turbulence viscosity field name | no | nut
Prt | turbulent Prandtl number | no | 0.85
\endtable
Example of the boundary condition specification:
\verbatim
<patchName>
{
type alphatWallFunction;
nut nut;
Prt 0.85;
value uniform 0; // optional value entry
}
\endverbatim
See also
Foam::fixedValueFvPatchField
SourceFiles
alphatWallFunctionFvPatchScalarField.C
\*---------------------------------------------------------------------------*/
#ifndef alphatWallFunctionFvPatchScalarField_H
#define alphatWallFunctionFvPatchScalarField_H
#include "fixedValueFvPatchFields.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
namespace Foam
{
namespace compressible
{
/*---------------------------------------------------------------------------*\
Class alphatWallFunctionFvPatchScalarField Declaration
\*---------------------------------------------------------------------------*/
class alphatWallFunctionFvPatchScalarField
:
public fixedValueFvPatchScalarField
{
// Private data
//- Turbulent Prandtl number (default = 0.85)
scalar Prt_;
public:
//- Runtime type information
TypeName("compressible::alphatWallFunction");
// Constructors
//- Construct from patch and internal field
alphatWallFunctionFvPatchScalarField
(
const fvPatch&,
const DimensionedField<scalar, volMesh>&
);
//- Construct from patch, internal field and dictionary
alphatWallFunctionFvPatchScalarField
(
const fvPatch&,
const DimensionedField<scalar, volMesh>&,
const dictionary&
);
//- Construct by mapping given
// alphatWallFunctionFvPatchScalarField
// onto a new patch
alphatWallFunctionFvPatchScalarField
(
const alphatWallFunctionFvPatchScalarField&,
const fvPatch&,
const DimensionedField<scalar, volMesh>&,
const fvPatchFieldMapper&
);
//- Construct as copy
alphatWallFunctionFvPatchScalarField
(
const alphatWallFunctionFvPatchScalarField&
);
//- Construct and return a clone
virtual tmp<fvPatchScalarField> clone() const
{
return tmp<fvPatchScalarField>
(
new alphatWallFunctionFvPatchScalarField(*this)
);
}
//- Construct as copy setting internal field reference
alphatWallFunctionFvPatchScalarField
(
const alphatWallFunctionFvPatchScalarField&,
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 alphatWallFunctionFvPatchScalarField(*this, iF)
);
}
// Member functions
// Evaluation functions
//- Update the coefficients associated with the patch field
virtual void updateCoeffs();
// I-O
//- Write
virtual void write(Ostream&) const;
};
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
} // End namespace compressible
} // End namespace Foam
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#endif
// ************************************************************************* //
You can’t perform that action at this time.