waveForcing Class Reference

This fvModel applies forcing to the liquid phase-fraction field and all components of the vector field to relax the fields towards those calculated from the current wave distribution. More...

Inheritance diagram for waveForcing:
Collaboration diagram for waveForcing:

Public Member Functions

 TypeName ("waveForcing")
 Runtime type information. More...
 
 waveForcing (const word &name, const word &modelType, const fvMesh &mesh, const dictionary &dict)
 Construct from components. More...
 
virtual ~waveForcing ()
 Destructor. More...
 
virtual bool read (const dictionary &dict)
 Read dictionary. More...
 
virtual wordList addSupFields () const
 Return the list of fields for which the fvModel adds source term. More...
 
virtual void addSup (const volScalarField &alpha, fvMatrix< scalar > &eqn) const
 Source term to VoF phase-fraction equation. More...
 
virtual void addSup (const volScalarField &rho, const volVectorField &U, fvMatrix< vector > &eqn) const
 Source term to momentum equation. More...
 
virtual bool movePoints ()
 Update for mesh motion. More...
 
virtual void topoChange (const polyTopoChangeMap &)
 Update topology using the given map. More...
 
virtual void mapMesh (const polyMeshMap &)
 Update from another mesh using the given map. More...
 
virtual void distribute (const polyDistributionMap &)
 Redistribute or update using the given distribution map. More...
 
virtual void correct ()
 Correct the wave forcing coefficients. More...
 
- Public Member Functions inherited from forcing
 TypeName ("forcing")
 Runtime type information. More...
 
 forcing (const word &name, const word &modelType, const fvMesh &mesh, const dictionary &dict)
 Construct from components. More...
 
virtual ~forcing ()
 Destructor. More...
 
- Public Member Functions inherited from fvModel
 TypeName ("fvModel")
 Runtime type information. More...
 
 declareRunTimeSelectionTable (autoPtr, fvModel, dictionary,(const word &name, const word &modelType, const fvMesh &mesh, const dictionary &dict),(name, modelType, mesh, dict))
 
 fvModel (const word &name, const word &modelType, const fvMesh &mesh, const dictionary &dict)
 Construct from components. More...
 
autoPtr< fvModelclone () const
 Return clone. More...
 
virtual ~fvModel ()
 Destructor. More...
 
const wordname () const
 Return const access to the source name. More...
 
const fvMeshmesh () const
 Return const access to the mesh database. More...
 
const dictionarycoeffs () const
 Return dictionary. More...
 
virtual bool addsSupToField (const word &fieldName) const
 Return true if the fvModel adds a source term to the given. More...
 
virtual scalar maxDeltaT () const
 Return the maximum time-step for stable operation. More...
 
virtual void addSup (fvMatrix< scalar > &eqn) const
 Add a source term to a field-less proxy equation. More...
 
template<class Type >
tmp< fvMatrix< Type > > sourceProxy (const VolField< Type > &eqnField) const
 Add a source term to an equation. More...
 
template<class Type >
tmp< fvMatrix< Type > > source (const VolField< Type > &field) const
 Return source for an equation. More...
 
template<class Type >
tmp< fvMatrix< Type > > sourceProxy (const VolField< Type > &field, const VolField< Type > &eqnField) const
 Return source for an equation. More...
 
template<class Type >
tmp< fvMatrix< Type > > source (const volScalarField &rho, const VolField< Type > &field) const
 Return source for a compressible equation. More...
 
template<class Type >
tmp< fvMatrix< Type > > sourceProxy (const volScalarField &rho, const VolField< Type > &field, const VolField< Type > &eqnField) const
 Return source for a compressible equation. More...
 
template<class Type >
tmp< fvMatrix< Type > > source (const volScalarField &alpha, const volScalarField &rho, const VolField< Type > &field) const
 Return source for a phase equation. More...
 
template<class Type >
tmp< fvMatrix< Type > > sourceProxy (const volScalarField &alpha, const volScalarField &rho, const VolField< Type > &field, const VolField< Type > &eqnField) const
 Return source for a phase equation. More...
 
template<class Type >
tmp< fvMatrix< Type > > source (const volScalarField &alpha, const geometricOneField &rho, const VolField< Type > &field) const
 Return source for a phase equation. More...
 
template<class Type >
tmp< fvMatrix< Type > > source (const geometricOneField &alpha, const volScalarField &rho, const VolField< Type > &field) const
 Return source for a phase equation. More...
 
template<class Type >
tmp< fvMatrix< Type > > source (const geometricOneField &alpha, const geometricOneField &rho, const VolField< Type > &field) const
 Return source for a phase equation. More...
 
template<class Type >
tmp< fvMatrix< Type > > d2dt2 (const VolField< Type > &field) const
 Return source for an equation with a second time derivative. More...
 
virtual void preUpdateMesh ()
 Prepare for mesh update. More...
 
virtual bool write (const bool write=true) const
 Write fvModel data. More...
 
template<class AlphaRhoFieldType , class ... AlphaRhoFieldTypes>
Foam::dimensionSet sourceDims (const dimensionSet &ds, const AlphaRhoFieldType &alphaRhoField, const AlphaRhoFieldTypes &... alphaRhoFields)
 
template<class AlphaRhoFieldType , class ... AlphaRhoFieldTypes>
const Foam::wordfieldName (const AlphaRhoFieldType &alphaRhoField, const AlphaRhoFieldTypes &... alphaRhoFields)
 
template<class AlphaRhoFieldType >
const Foam::wordfieldName (const AlphaRhoFieldType &alphaRhoField)
 
template<class Type , class ... AlphaRhoFieldTypes>
Foam::tmp< Foam::fvMatrix< Type > > sourceTerm (const VolField< Type > &eqnField, const dimensionSet &ds, const AlphaRhoFieldTypes &... alphaRhoFields) const
 
template<class Type >
Foam::tmp< Foam::fvMatrix< Type > > sourceProxy (const VolField< Type > &eqnField) const
 
template<class Type >
Foam::tmp< Foam::fvMatrix< Type > > source (const VolField< Type > &field) const
 
template<class Type >
Foam::tmp< Foam::fvMatrix< Type > > sourceProxy (const VolField< Type > &field, const VolField< Type > &eqnField) const
 
template<class Type >
Foam::tmp< Foam::fvMatrix< Type > > source (const volScalarField &rho, const VolField< Type > &field) const
 
template<class Type >
Foam::tmp< Foam::fvMatrix< Type > > sourceProxy (const volScalarField &rho, const VolField< Type > &field, const VolField< Type > &eqnField) const
 
template<class Type >
Foam::tmp< Foam::fvMatrix< Type > > source (const volScalarField &alpha, const volScalarField &rho, const VolField< Type > &field) const
 
template<class Type >
Foam::tmp< Foam::fvMatrix< Type > > sourceProxy (const volScalarField &alpha, const volScalarField &rho, const VolField< Type > &field, const VolField< Type > &eqnField) const
 
template<class Type >
Foam::tmp< Foam::fvMatrix< Type > > source (const geometricOneField &alpha, const geometricOneField &rho, const VolField< Type > &field) const
 
template<class Type >
Foam::tmp< Foam::fvMatrix< Type > > source (const volScalarField &alpha, const geometricOneField &rho, const VolField< Type > &field) const
 
template<class Type >
Foam::tmp< Foam::fvMatrix< Type > > source (const geometricOneField &alpha, const volScalarField &rho, const VolField< Type > &field) const
 
template<class Type >
Foam::tmp< Foam::fvMatrix< Type > > d2dt2 (const VolField< Type > &field) const
 

Additional Inherited Members

- Static Public Member Functions inherited from fvModel
template<class AlphaRhoFieldType , class ... AlphaRhoFieldTypes>
static dimensionSet sourceDims (const dimensionSet &ds, const AlphaRhoFieldType &alphaRhoField, const AlphaRhoFieldTypes &... alphaRhoFields)
 Return the dimensions of the matrix of a source term. More...
 
static const dimensionSetsourceDims (const dimensionSet &ds)
 Return the dimensions of the matrix of a source term (base. More...
 
template<class AlphaRhoFieldType , class ... AlphaRhoFieldTypes>
static const wordfieldName (const AlphaRhoFieldType &alphaRhoField, const AlphaRhoFieldTypes &... alphaRhoFields)
 Return the name of the field associated with a source term. More...
 
template<class AlphaRhoFieldType >
static const wordfieldName (const AlphaRhoFieldType &alphaRhoField)
 Return the name of the field associated with a source term (base. More...
 
static const wordfieldName ()
 Return the name of the field associated with a source term. Special. More...
 
static autoPtr< fvModelNew (const word &name, const fvMesh &mesh, const dictionary &dict)
 Return a reference to the selected fvModel. More...
 
- Protected Member Functions inherited from forcing
void readCoeffs ()
 Non-virtual read. More...
 
void readLambda ()
 Read the forcing coefficients. More...
 
dimensionedScalar regionLength () const
 Calculate and return the volume average forcing region length. More...
 
void writeForceFields () const
 Optionally write the forcing fields: More...
 
- Protected Member Functions inherited from fvModel
template<class Type >
void addSupType (const VolField< Type > &field, fvMatrix< Type > &eqn) const
 Add a source term to an equation. More...
 
template<class Type >
void addSupType (const volScalarField &rho, const VolField< Type > &field, fvMatrix< Type > &eqn) const
 Add a source term to a compressible equation. More...
 
template<class Type >
void addSupType (const volScalarField &alpha, const volScalarField &rho, const VolField< Type > &field, fvMatrix< Type > &eqn) const
 Add a source term to a phase equation. More...
 
template<class Type , class ... AlphaRhoFieldTypes>
tmp< fvMatrix< Type > > sourceTerm (const VolField< Type > &eqnField, const dimensionSet &ds, const AlphaRhoFieldTypes &... alphaRhoFields) const
 Return a source for an equation. More...
 
- Protected Attributes inherited from forcing
bool writeForceFields_
 Optionally write the forcing fields. More...
 
dimensionedScalar lambda_
 Forcing coefficient [1/s]. More...
 
dimensionedScalar lambdaBoundary_
 Optional boundary forcing coefficient [1/s]. More...
 
autoPtr< Function1< scalar > > scale_
 The scaling function. More...
 
vectorField origins_
 Origins of the scaling coordinate. More...
 
vectorField directions_
 Directions of increasing scaling coordinate. More...
 

Detailed Description

This fvModel applies forcing to the liquid phase-fraction field and all components of the vector field to relax the fields towards those calculated from the current wave distribution.

The force coefficient $\lambda$ should be set based on the desired level of forcing and the residence time the waves through the forcing zone. For example, if waves moving at 2 [m/s] are travelling through a forcing zone 8 [m] in length, then the residence time is 4 [s]. If it is deemed necessary to force for 5 time-scales, then $\lambda$ should be set to equal 5/(4 [s]) = 1.2 [1/s]. If more aggressive forcing is required adjacent to the boundaries, which is often the case if wave boundary conditions are specified at outflow boundaries, the optional lambdaBoundary coefficient can be specified higher than the value of $\lambda$.

Alternatively the forcing force coefficient lambdaCoeff can be specified in which case $\lambda$ is evaluated by multiplying the maximum wave speed by lambdaCoeff and dividing by the forcing region length. lambdaBoundary is similarly evaluated from lambdaBoundaryCoeff if specified.

Usage
Example usage:
waveForcing1
{
    type            waveForcing;

    libs            ("libwaves.so");

    liquidPhase     water;

    // Define the line along which to apply the graduation
    origin          (600 0 0);
    direction       (-1 0 0);

    // // Or, define multiple lines
    // origins         ((600 0 0) (600 -300 0) (600 300 0));
    // directions      ((-1 0 0) (0 1 0) (0 -1 0));

    scale
    {
        type        halfCosineRamp;
        start       0;
        duration    300;
    }

    lambdaCoeff     2;   // Forcing coefficient

 // lambdaBoundaryCoeff  10;  // Optional boundary forcing coefficient
                         // Useful when wave BCs are specified at outlets

    // Write the forcing fields: forcing:scale, forcing:forceCoeff
    writeForceFields true;
}
See also
Foam::fv::forcing
Source files

Definition at line 108 of file waveForcing.H.

Constructor & Destructor Documentation

◆ waveForcing()

waveForcing ( const word name,
const word modelType,
const fvMesh mesh,
const dictionary dict 
)

Construct from components.

Definition at line 97 of file waveForcing.C.

References forcing::writeForceFields().

Here is the call graph for this function:

◆ ~waveForcing()

virtual ~waveForcing ( )
inlinevirtual

Destructor.

Definition at line 173 of file waveForcing.H.

Member Function Documentation

◆ TypeName()

TypeName ( "waveForcing"  )

Runtime type information.

◆ read()

bool read ( const dictionary dict)
virtual

Read dictionary.

Reimplemented from forcing.

Definition at line 232 of file waveForcing.C.

References dict, and forcing::read().

Here is the call graph for this function:

◆ addSupFields()

Foam::wordList addSupFields ( ) const
virtual

Return the list of fields for which the fvModel adds source term.

to the transport equation

Reimplemented from fvModel.

Definition at line 122 of file waveForcing.C.

◆ addSup() [1/2]

void addSup ( const volScalarField alpha,
fvMatrix< scalar > &  eqn 
) const
virtual

Source term to VoF phase-fraction equation.

Definition at line 128 of file waveForcing.C.

References alpha(), fvMatrix< Type >::psi(), and Foam::fvm::Sp().

Here is the call graph for this function:

◆ addSup() [2/2]

void addSup ( const volScalarField rho,
const volVectorField U,
fvMatrix< vector > &  eqn 
) const
virtual

Source term to momentum equation.

Definition at line 144 of file waveForcing.C.

References Foam::fvc::ddt(), Foam::fvc::div(), fvMatrix< Type >::psi(), rho, Foam::fvm::Sp(), and U.

Here is the call graph for this function:

◆ movePoints()

bool movePoints ( )
virtual

Update for mesh motion.

Implements fvModel.

Definition at line 170 of file waveForcing.C.

References forcing::scale().

Here is the call graph for this function:

◆ topoChange()

void topoChange ( const polyTopoChangeMap )
virtual

Update topology using the given map.

Implements fvModel.

Definition at line 179 of file waveForcing.C.

References forcing::scale().

Here is the call graph for this function:

◆ mapMesh()

void mapMesh ( const polyMeshMap map)
virtual

Update from another mesh using the given map.

Implements fvModel.

Definition at line 185 of file waveForcing.C.

References forcing::scale().

Here is the call graph for this function:

◆ distribute()

void distribute ( const polyDistributionMap )
virtual

Redistribute or update using the given distribution map.

Implements fvModel.

Definition at line 191 of file waveForcing.C.

References forcing::scale().

Here is the call graph for this function:

◆ correct()

void correct ( )
virtual

Correct the wave forcing coefficients.

Reimplemented from fvModel.

Definition at line 197 of file waveForcing.C.

References Foam::dimless, Foam::dimVelocity, Foam::constant::universal::h, Foam::levelSetAverage(), Foam::levelSetFraction(), and DimensionedField< Type, GeoMesh >::New().

Here is the call graph for this function:

The documentation for this class was generated from the following files: