mirror of
https://develop.openfoam.com/Development/openfoam.git
synced 2025-11-28 03:28:01 +00:00
280 lines
8.0 KiB
C++
280 lines
8.0 KiB
C++
/*---------------------------------------------------------------------------*\
|
|
========= |
|
|
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
|
|
\\ / O peration |
|
|
\\ / A nd | www.openfoam.com
|
|
\\/ M anipulation |
|
|
-------------------------------------------------------------------------------
|
|
Copyright (C) 2012-2017 OpenFOAM Foundation
|
|
Copyright (C) 2016 OpenCFD Ltd.
|
|
-------------------------------------------------------------------------------
|
|
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::functionObjects::scalarTransport
|
|
|
|
Group
|
|
grpSolversFunctionObjects
|
|
|
|
Description
|
|
Evolves a passive scalar transport equation.
|
|
|
|
- To specify the field name set the \c field entry
|
|
- To employ the same numerical schemes as another field set
|
|
the \c schemesField entry,
|
|
- The diffusivity can be set manually using the 'D' entry, retrieved
|
|
from the turbulence model or specified nut
|
|
- Alternatively if a turbulence model is available a turbulent diffusivity
|
|
may be constructed from the laminar and turbulent viscosities using the
|
|
optional diffusivity coefficients \c alphaD and \c alphaDt (which default
|
|
to 1):
|
|
\verbatim
|
|
D = alphaD*nu + alphaDt*nut
|
|
\endverbatim
|
|
- To specify a transport quantity within a phase enter phase.
|
|
- bounded01 bounds the transported scalar within 0 and 1.
|
|
|
|
Usage
|
|
Example of function object specification to solve a scalar transport
|
|
equation:
|
|
\verbatim
|
|
functions
|
|
{
|
|
scalar1
|
|
{
|
|
type scalarTransport;
|
|
libs ("libsolverFunctionObjects.so");
|
|
|
|
resetOnStartUp no;
|
|
region cabin;
|
|
field H2O;
|
|
|
|
|
|
fvOptions
|
|
{
|
|
...
|
|
}
|
|
}
|
|
}
|
|
\endverbatim
|
|
|
|
Example of function object specification to solve a residence time
|
|
in a two phase flow:
|
|
equation:
|
|
\verbatim
|
|
functions
|
|
{
|
|
sTransport
|
|
{
|
|
type scalarTransport;
|
|
libs ("libsolverFunctionObjects.so");
|
|
|
|
enabled true;
|
|
writeControl outputTime;
|
|
writeInterval 1;
|
|
|
|
field s;
|
|
bounded01 false;
|
|
phase alpha.water;
|
|
|
|
write true;
|
|
|
|
fvOptions
|
|
{
|
|
unitySource
|
|
{
|
|
type scalarSemiImplicitSource;
|
|
enabled true;
|
|
|
|
scalarSemiImplicitSourceCoeffs
|
|
{
|
|
selectionMode all;
|
|
volumeMode specific;
|
|
injectionRateSuSp
|
|
{
|
|
s (1 0);
|
|
}
|
|
}
|
|
}
|
|
}
|
|
|
|
resetOnStartUp false;
|
|
}
|
|
}
|
|
\endverbatim
|
|
|
|
Where the entries comprise:
|
|
\table
|
|
Property | Description | Required | Default value
|
|
type | Type name: scalarTransport | yes |
|
|
field | Name of the scalar field | no | s
|
|
phi | Name of flux field | no | phi
|
|
rho | Name of density field | no | rho
|
|
phase | Name of the phase | no | none
|
|
nut | Name of the turbulence viscosity | no | none
|
|
D | Diffusion coefficient | no | auto generated
|
|
nCorr | Number of correctors | no | 0
|
|
resetOnStartUp | Reset scalar to zero on start-up | no | no
|
|
schemesField | Name of field to specify schemes | no | field name
|
|
fvOptions | List of scalar sources | no |
|
|
bounded01 | Bounds scalar between 0-1 for multiphase | no | true
|
|
phasePhiCompressed | Compressed flux for VOF | no | alphaPhiUn
|
|
\endtable
|
|
|
|
See also
|
|
Foam::functionObjects::fvMeshFunctionObject
|
|
|
|
SourceFiles
|
|
scalarTransport.C
|
|
|
|
\*---------------------------------------------------------------------------*/
|
|
|
|
#ifndef functionObjects_scalarTransport_H
|
|
#define functionObjects_scalarTransport_H
|
|
|
|
#include "fvMeshFunctionObject.H"
|
|
#include "volFields.H"
|
|
#include "fvOptionList.H"
|
|
|
|
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
|
|
|
|
namespace Foam
|
|
{
|
|
namespace functionObjects
|
|
{
|
|
|
|
/*---------------------------------------------------------------------------*\
|
|
Class scalarTransport Declaration
|
|
\*---------------------------------------------------------------------------*/
|
|
|
|
class scalarTransport
|
|
:
|
|
public fvMeshFunctionObject
|
|
{
|
|
// Private data
|
|
|
|
//- Name of the transport field.
|
|
word fieldName_;
|
|
|
|
//- Name of flux field (optional)
|
|
word phiName_;
|
|
|
|
//- Name of density field (optional)
|
|
word rhoName_;
|
|
|
|
//- Name of turbulent viscosity field (optional)
|
|
word nutName_;
|
|
|
|
//- Name of phase field (optional)
|
|
word phaseName_;
|
|
|
|
//- Name of phase field compressed flux (optional)
|
|
word phasePhiCompressedName_;
|
|
|
|
//- Diffusion coefficient (optional)
|
|
scalar D_;
|
|
|
|
//- Flag to indicate whether a constant, uniform D_ is specified
|
|
bool constantD_;
|
|
|
|
//- Laminar diffusion coefficient (optional)
|
|
scalar alphaD_;
|
|
|
|
//- Turbulent diffusion coefficient (optional)
|
|
scalar alphaDt_;
|
|
|
|
//- Number of corrector iterations (optional)
|
|
label nCorr_;
|
|
|
|
//- Flag to reset the scalar to zero on start-up
|
|
bool resetOnStartUp_;
|
|
|
|
//- Name of field whose schemes are used (optional)
|
|
word schemesField_;
|
|
|
|
//- Run-time selectable finite volume options, e.g. sources, constraints
|
|
fv::optionList fvOptions_;
|
|
|
|
//- Bound scalar between 0-1 using MULES for multiphase case
|
|
bool bounded01_;
|
|
|
|
|
|
// Private Member Functions
|
|
|
|
//- Return reference to registered transported field
|
|
volScalarField& transportedField();
|
|
|
|
//- Return the diffusivity field
|
|
tmp<volScalarField> D
|
|
(
|
|
const volScalarField& s,
|
|
const surfaceScalarField& phi
|
|
) const;
|
|
|
|
//- No copy construct
|
|
scalarTransport(const scalarTransport&) = delete;
|
|
|
|
//- No copy assignment
|
|
void operator=(const scalarTransport&) = delete;
|
|
|
|
|
|
public:
|
|
|
|
//- Runtime type information
|
|
TypeName("scalarTransport");
|
|
|
|
|
|
// Constructors
|
|
|
|
//- Construct from Time and dictionary
|
|
scalarTransport
|
|
(
|
|
const word& name,
|
|
const Time& runTime,
|
|
const dictionary& dict
|
|
);
|
|
|
|
|
|
//- Destructor
|
|
virtual ~scalarTransport();
|
|
|
|
|
|
// Member Functions
|
|
|
|
//- Read the scalarTransport data
|
|
virtual bool read(const dictionary&);
|
|
|
|
//- Calculate the scalarTransport
|
|
virtual bool execute();
|
|
|
|
//- Do nothing.
|
|
// The volScalarField is registered and written automatically
|
|
virtual bool write();
|
|
};
|
|
|
|
|
|
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
|
|
|
|
} // End namespace functionObjects
|
|
} // End namespace Foam
|
|
|
|
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
|
|
|
|
#endif
|
|
|
|
// ************************************************************************* //
|