-
Mark OLESEN authored
- this allows more flexibility when defining the location or intensity of sources. For example, { type scalarSemiImplicitSource; volumeMode specific; selectionMode all; sources { tracer0 { explicit { type exprField; functions<scalar> { square { type square; scale 0.0025; level 0.0025; frequency 10; } } expression #{ (hypot(pos().x() + 0.025, pos().y()) < 0.01) ? fn:square(time()) : 0 #}; } } } } ENH: SemiImplicitSource: handle "sources" with explicit/implicit entries - essentially the same as injectionRateSuSp with Su/Sp, but potentially clearer in purpose. ENH: add Function1 good() method to define if function can be evaluated - for example, provides a programmatic means of avoiding the 'none' function
Mark OLESEN authored- this allows more flexibility when defining the location or intensity of sources. For example, { type scalarSemiImplicitSource; volumeMode specific; selectionMode all; sources { tracer0 { explicit { type exprField; functions<scalar> { square { type square; scale 0.0025; level 0.0025; frequency 10; } } expression #{ (hypot(pos().x() + 0.025, pos().y()) < 0.01) ? fn:square(time()) : 0 #}; } } } } ENH: SemiImplicitSource: handle "sources" with explicit/implicit entries - essentially the same as injectionRateSuSp with Su/Sp, but potentially clearer in purpose. ENH: add Function1 good() method to define if function can be evaluated - for example, provides a programmatic means of avoiding the 'none' function
scalarTransport.H 7.88 KiB
/*---------------------------------------------------------------------------*\
========= |
\\ / 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) 2016-2020 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 (solverFunctionObjects);
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 (solverFunctionObjects);
enabled true;
writeControl outputTime;
writeInterval 1;
field s;
bounded01 false;
phase alpha.water;
write true;
fvOptions
{
unitySource
{
type scalarSemiImplicitSource;
enabled true;
selectionMode all;
volumeMode specific;
sources
{
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
// ************************************************************************* //