zhyang-dev/openfoam
1
0
Fork 0
mirror of https://develop.openfoam.com/Development/openfoam.git synced 2025-11-28 03:28:01 +00:00
Code Issues Actions Packages Projects Releases Wiki Activity

postProcessing: Replaced 'foamCalc' and the 'postCalc' utilities

Browse Source 
with the more general and flexible 'postProcess' utility and '-postProcess' solver option

Rationale
---------

Both the 'postProcess' utility and '-postProcess' solver option use the
same extensive set of functionObjects available for data-processing
during the run avoiding the substantial code duplication necessary for
the 'foamCalc' and 'postCalc' utilities and simplifying maintenance.
Additionally consistency is guaranteed between solver data processing
and post-processing.

The functionObjects have been substantially re-written and generalized
to simplify development and encourage contribution.

Configuration
-------------

An extensive set of simple functionObject configuration files are
provided in

OpenFOAM-dev/etc/caseDicts/postProcessing

and more will be added in the future.  These can either be copied into
'<case>/system' directory and included into the 'controlDict.functions'
sub-dictionary or included directly from 'etc/caseDicts/postProcessing'
using the '#includeEtc' directive or the new and more convenient
'#includeFunc' directive which searches the
'<etc>/caseDicts/postProcessing' directories for the selected
functionObject, e.g.

functions
{
    #includeFunc Q
    #includeFunc Lambda2
}

'#includeFunc' first searches the '<case>/system' directory in case
there is a local configuration.

Description of #includeFunc
---------------------------

    Specify a functionObject dictionary file to include, expects the
    functionObject name to follow (without quotes).

    Search for functionObject dictionary file in
    user/group/shipped directories.
    The search scheme allows for version-specific and
    version-independent files using the following hierarchy:
    - \b user settings:
      - ~/.OpenFOAM/\<VERSION\>/caseDicts/postProcessing
      - ~/.OpenFOAM/caseDicts/postProcessing
    - \b group (site) settings (when $WM_PROJECT_SITE is set):
      - $WM_PROJECT_SITE/\<VERSION\>/caseDicts/postProcessing
      - $WM_PROJECT_SITE/caseDicts/postProcessing
    - \b group (site) settings (when $WM_PROJECT_SITE is not set):
      - $WM_PROJECT_INST_DIR/site/\<VERSION\>/caseDicts/postProcessing
      - $WM_PROJECT_INST_DIR/site/caseDicts/postProcessing
    - \b other (shipped) settings:
      - $WM_PROJECT_DIR/etc/caseDicts/postProcessing

    An example of the \c \#includeFunc directive:
    \verbatim
        #includeFunc <funcName>
    \endverbatim

postProcess
-----------

The 'postProcess' utility and '-postProcess' solver option provide the
same set of controls to execute functionObjects after the run either by
reading a specified set of fields to process in the case of
'postProcess' or by reading all fields and models required to start the
run in the case of '-postProcess' for each selected time:

postProcess -help

Usage: postProcess [OPTIONS]
options:
  -case <dir>       specify alternate case directory, default is the cwd
  -constant         include the 'constant/' dir in the times list
  -dict <file>      read control dictionary from specified location
  -field <name>     specify the name of the field to be processed, e.g. U
  -fields <list>    specify a list of fields to be processed, e.g. '(U T p)' -
                    regular expressions not currently supported
  -func <name>      specify the name of the functionObject to execute, e.g. Q
  -funcs <list>     specify the names of the functionObjects to execute, e.g.
                    '(Q div(U))'
  -latestTime       select the latest time
  -newTimes         select the new times
  -noFunctionObjects
                    do not execute functionObjects
  -noZero           exclude the '0/' dir from the times list, has precedence
                    over the -withZero option
  -parallel         run in parallel
  -region <name>    specify alternative mesh region
  -roots <(dir1 .. dirN)>
                    slave root directories for distributed running
  -time <ranges>    comma-separated time ranges - eg, ':10,20,40:70,1000:'
  -srcDoc           display source code in browser
  -doc              display application documentation in browser
  -help             print the usage

 pimpleFoam -postProcess -help

Usage: pimpleFoam [OPTIONS]
options:
  -case <dir>       specify alternate case directory, default is the cwd
  -constant         include the 'constant/' dir in the times list
  -dict <file>      read control dictionary from specified location
  -field <name>     specify the name of the field to be processed, e.g. U
  -fields <list>    specify a list of fields to be processed, e.g. '(U T p)' -
                    regular expressions not currently supported
  -func <name>      specify the name of the functionObject to execute, e.g. Q
  -funcs <list>     specify the names of the functionObjects to execute, e.g.
                    '(Q div(U))'
  -latestTime       select the latest time
  -newTimes         select the new times
  -noFunctionObjects
                    do not execute functionObjects
  -noZero           exclude the '0/' dir from the times list, has precedence
                    over the -withZero option
  -parallel         run in parallel
  -postProcess      Execute functionObjects only
  -region <name>    specify alternative mesh region
  -roots <(dir1 .. dirN)>
                    slave root directories for distributed running
  -time <ranges>    comma-separated time ranges - eg, ':10,20,40:70,1000:'
  -srcDoc           display source code in browser
  -doc              display application documentation in browser
  -help             print the usage

The functionObjects to execute may be specified on the command-line
using the '-func' option for a single functionObject or '-funcs' for a
list, e.g.

postProcess -func Q
postProcess -funcs '(div(U) div(phi))'

In the case of 'Q' the default field to process is 'U' which is
specified in and read from the configuration file but this may be
overridden thus:

postProcess -func 'Q(Ua)'

as is done in the example above to calculate the two forms of the divergence of
the velocity field.  Additional fields which the functionObjects may depend on
can be specified using the '-field' or '-fields' options.

The 'postProcess' utility can only be used to execute functionObjects which
process fields present in the time directories.  However, functionObjects which
depend on fields obtained from models, e.g. properties derived from turbulence
models can be executed using the '-postProcess' of the appropriate solver, e.g.

pisoFoam -postProcess -func PecletNo

or

sonicFoam -postProcess -func MachNo

In this case all required fields will have already been read so the '-field' or
'-fields' options are not be needed.

Henry G. Weller
CFD Direct Ltd.
This commit is contained in:
Henry Weller
2016-05-28 18:58:48 +01:00
parent 6f9573bb12
commit e4dc50dcb0
394 changed files with 1450 additions and 5384 deletions
Download Patch File Download Diff File Expand all files Collapse all files

314
src/functionObjects/solvers/scalarTransport/scalarTransport.C Normal file
View File

@ -0,0 +1,314 @@
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | Copyright (C) 2012-2016 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/>.
\*---------------------------------------------------------------------------*/
#include "scalarTransport.H"
#include "surfaceFields.H"
#include "dictionary.H"
#include "fixedValueFvPatchFields.H"
#include "zeroGradientFvPatchFields.H"
#include "fvScalarMatrix.H"
#include "fvmDdt.H"
#include "fvmDiv.H"
#include "fvcDiv.H"
#include "fvmLaplacian.H"
#include "fvmSup.H"
#include "turbulentTransportModel.H"
#include "turbulentFluidThermoModel.H"
#include "addToRunTimeSelectionTable.H"
// * * * * * * * * * * * * * * Static Data Members * * * * * * * * * * * * * //
namespace Foam
{
namespace functionObjects
{
defineTypeNameAndDebug(scalarTransport, 0);
addToRunTimeSelectionTable
(
functionObject,
scalarTransport,
dictionary
);
}
}
// * * * * * * * * * * * * * Private Member Functions * * * * * * * * * * * //
Foam::wordList Foam::functionObjects::scalarTransport::boundaryTypes() const
{
const volVectorField& U = mesh_.lookupObject<volVectorField>(UName_);
wordList bTypes(U.boundaryField().size());
forAll(bTypes, patchi)
{
const fvPatchField<vector>& pf = U.boundaryField()[patchi];
if (isA<fixedValueFvPatchVectorField>(pf))
{
bTypes[patchi] = fixedValueFvPatchScalarField::typeName;
}
else
{
bTypes[patchi] = zeroGradientFvPatchScalarField::typeName;
}
}
return bTypes;
}
Foam::tmp<Foam::volScalarField> Foam::functionObjects::scalarTransport::DT
(
const surfaceScalarField& phi
) const
{
typedef incompressible::turbulenceModel icoModel;
typedef compressible::turbulenceModel cmpModel;
if (userDT_)
{
return tmp<volScalarField>
(
new volScalarField
(
IOobject
(
"DT",
mesh_.time().timeName(),
mesh_.time(),
IOobject::NO_READ,
IOobject::NO_WRITE
),
mesh_,
dimensionedScalar("DT", phi.dimensions()/dimLength, DT_)
)
);
}
else if (mesh_.foundObject<icoModel>(turbulenceModel::propertiesName))
{
const icoModel& model = mesh_.lookupObject<icoModel>
(
turbulenceModel::propertiesName
);
return model.nuEff();
}
else if (mesh_.foundObject<cmpModel>(turbulenceModel::propertiesName))
{
const cmpModel& model = mesh_.lookupObject<cmpModel>
(
turbulenceModel::propertiesName
);
return model.muEff();
}
else
{
return tmp<volScalarField>
(
new volScalarField
(
IOobject
(
"DT",
mesh_.time().timeName(),
mesh_.time(),
IOobject::NO_READ,
IOobject::NO_WRITE
),
mesh_,
dimensionedScalar("DT", phi.dimensions()/dimLength, 0.0)
)
);
}
}
// * * * * * * * * * * * * * * * * Constructors * * * * * * * * * * * * * * //
Foam::functionObjects::scalarTransport::scalarTransport
(
const word& name,
const Time& runTime,
const dictionary& dict
)
:
fvMeshFunctionObject(name, runTime, dict),
DT_(0.0),
nCorr_(0),
fvOptions_(mesh_),
T_
(
IOobject
(
name,
mesh_.time().timeName(),
mesh_,
IOobject::READ_IF_PRESENT,
IOobject::AUTO_WRITE
),
mesh_,
dimensionedScalar("zero", dimless, 0.0),
boundaryTypes()
)
{
read(dict);
if (resetOnStartUp_)
{
T_ == dimensionedScalar("zero", dimless, 0.0);
}
}
// * * * * * * * * * * * * * * * * Destructor * * * * * * * * * * * * * * * //
Foam::functionObjects::scalarTransport::~scalarTransport()
{}
// * * * * * * * * * * * * * * * Member Functions * * * * * * * * * * * * * //
bool Foam::functionObjects::scalarTransport::read(const dictionary& dict)
{
fvMeshFunctionObject::read(dict);
phiName_ = dict.lookupOrDefault<word>("phi", "phi");
UName_ = dict.lookupOrDefault<word>("U", "U");
rhoName_ = dict.lookupOrDefault<word>("rho", "rho");
userDT_ = false;
if (dict.readIfPresent("DT", DT_))
{
userDT_ = true;
}
dict.lookup("resetOnStartUp") >> resetOnStartUp_;
dict.readIfPresent("nCorr", nCorr_);
dict.lookup("autoSchemes") >> autoSchemes_;
fvOptions_.reset(dict.subDict("fvOptions"));
return true;
}
bool Foam::functionObjects::scalarTransport::execute(const bool postProcess)
{
Info<< type() << " output:" << endl;
const surfaceScalarField& phi =
mesh_.lookupObject<surfaceScalarField>(phiName_);
// calculate the diffusivity
volScalarField DT(this->DT(phi));
// set schemes
word schemeVar = T_.name();
if (autoSchemes_)
{
schemeVar = UName_;
}
word divScheme("div(phi," + schemeVar + ")");
word laplacianScheme("laplacian(" + DT.name() + "," + schemeVar + ")");
// set under-relaxation coeff
scalar relaxCoeff = 0.0;
if (mesh_.relaxEquation(schemeVar))
{
relaxCoeff = mesh_.equationRelaxationFactor(schemeVar);
}
if (phi.dimensions() == dimMass/dimTime)
{
const volScalarField& rho =
mesh_.lookupObject<volScalarField>(rhoName_);
// solve
for (label i = 0; i <= nCorr_; i++)
{
fvScalarMatrix TEqn
(
fvm::ddt(rho, T_)
+ fvm::div(phi, T_, divScheme)
- fvm::laplacian(DT, T_, laplacianScheme)
==
fvOptions_(rho, T_)
);
TEqn.relax(relaxCoeff);
fvOptions_.constrain(TEqn);
TEqn.solve(mesh_.solverDict(schemeVar));
}
}
else if (phi.dimensions() == dimVolume/dimTime)
{
// solve
for (label i = 0; i <= nCorr_; i++)
{
fvScalarMatrix TEqn
(
fvm::ddt(T_)
+ fvm::div(phi, T_, divScheme)
- fvm::laplacian(DT, T_, laplacianScheme)
==
fvOptions_(T_)
);
TEqn.relax(relaxCoeff);
fvOptions_.constrain(TEqn);
TEqn.solve(mesh_.solverDict(schemeVar));
}
}
else
{
FatalErrorInFunction
<< "Incompatible dimensions for phi: " << phi.dimensions() << nl
<< "Dimensions should be " << dimMass/dimTime << " or "
<< dimVolume/dimTime << endl;
}
Info<< endl;
return true;
}
bool Foam::functionObjects::scalarTransport::write(const bool postProcess)
{
return true;
}
// ************************************************************************* //

165
src/functionObjects/solvers/scalarTransport/scalarTransport.H Normal file
View File

@ -0,0 +1,165 @@
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | Copyright (C) 2012-2016 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::functionObjects::scalarTransport
Group
grpSolversFunctionObjects
Description
This function object evolves a passive scalar transport equation. The
field in ininitially zero, to which sources are added. The field name
is assigned the name of the function object. Boundary conditions are
automatically applied, based on the velocity boundary conditions.
- the field can be zeroed on start-up using the resetOnStartUp flag
- to employ the same numerical schemes as the flow velocity, use the
autoSchemes flag
- the diffusivity can be set manually using the DT entry, or retrieved
from the turbulence model (if applicable)
SeeAlso
Foam::functionObjects::fvMeshFunctionObject
SourceFiles
scalarTransport.C
\*---------------------------------------------------------------------------*/
#ifndef functionObjects_scalarTransport_H
#define functionObjects_scalarTransport_H
#include "fvMeshFunctionObject.H"
#include "volFields.H"
#include "surfaceFieldsFwd.H"
#include "fvOptionList.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
namespace Foam
{
namespace functionObjects
{
/*---------------------------------------------------------------------------*\
Class scalarTransport Declaration
\*---------------------------------------------------------------------------*/
class scalarTransport
:
public fvMeshFunctionObject
{
// Private data
//- Name of flux field (optional)
word phiName_;
//- Name of velocity field (optional)
word UName_;
//- Name of density field (optional)
word rhoName_;
//- Diffusion coefficient (optional)
scalar DT_;
//- Flag to indicate whether user DT_ is used
bool userDT_;
//- Flag to reset scalar field on start-up
bool resetOnStartUp_;
//- Number of corrector iterations (optional)
label nCorr_;
//- Flag to employ schemes for velocity for scalar transport
bool autoSchemes_;
//- Run-time selectable finite volume options, e.g. sources, constraints
fv::optionList fvOptions_;
//- The scalar field
volScalarField T_;
// Private Member Functions
//- Return the boundary types for the scalar field
wordList boundaryTypes() const;
//- Return the diffusivity field
tmp<volScalarField> DT(const surfaceScalarField& phi) const;
//- Disallow default bitwise copy construct
scalarTransport(const scalarTransport&);
//- Disallow default bitwise assignment
void operator=(const scalarTransport&);
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(const bool postProcess = false);
//- Do nothing.
// The volScalarField is registered and written automatically
virtual bool write(const bool postProcess = false);
};
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
} // End namespace functionObjects
} // End namespace Foam
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#endif
// ************************************************************************* //