This boundary condition provides a coupled temperature condition between multiple mesh regions. More...

Inheritance diagram for thermalBaffleFvPatchScalarField:

Collaboration diagram for thermalBaffleFvPatchScalarField:

Public Member Functions
	TypeName ("compressible::thermalBaffle")
	Runtime type information. More...

	thermalBaffleFvPatchScalarField (const fvPatch &, const DimensionedField< scalar, volMesh > &)
	Construct from patch and internal field. More...

	thermalBaffleFvPatchScalarField (const fvPatch &, const DimensionedField< scalar, volMesh > &, const dictionary &)
	Construct from patch, internal field and dictionary. More...

	thermalBaffleFvPatchScalarField (const thermalBaffleFvPatchScalarField &, const fvPatch &, const DimensionedField< scalar, volMesh > &, const fvPatchFieldMapper &)
	Construct by mapping given. More...

virtual tmp< fvPatchScalarField >	clone () const
	Construct and return a clone. More...

	thermalBaffleFvPatchScalarField (const thermalBaffleFvPatchScalarField &, const DimensionedField< scalar, volMesh > &)
	Construct as copy setting internal field reference. More...

virtual tmp< fvPatchScalarField >	clone (const DimensionedField< scalar, volMesh > &iF) const
	Construct and return a clone setting internal field reference. More...

virtual void	autoMap (const fvPatchFieldMapper &)
	Map (and resize as needed) from self given a mapping object. More...

virtual void	rmap (const fvPatchScalarField &, const labelList &)
	Reverse map the given fvPatchField onto this fvPatchField. More...

virtual void	updateCoeffs ()
	Update the coefficients associated with the patch field. More...

virtual void	write (Ostream &) const
	Write. More...

Public Member Functions inherited from turbulentTemperatureRadCoupledMixedFvPatchScalarField
	TypeName ("compressible::turbulentTemperatureRadCoupledMixed")
	Runtime type information. More...

	turbulentTemperatureRadCoupledMixedFvPatchScalarField (const fvPatch &, const DimensionedField< scalar, volMesh > &)
	Construct from patch and internal field. More...

	turbulentTemperatureRadCoupledMixedFvPatchScalarField (const fvPatch &, const DimensionedField< scalar, volMesh > &, const dictionary &)
	Construct from patch, internal field and dictionary. More...

	turbulentTemperatureRadCoupledMixedFvPatchScalarField (const turbulentTemperatureRadCoupledMixedFvPatchScalarField &, const fvPatch &, const DimensionedField< scalar, volMesh > &, const fvPatchFieldMapper &)
	Construct by mapping given. More...

	turbulentTemperatureRadCoupledMixedFvPatchScalarField (const turbulentTemperatureRadCoupledMixedFvPatchScalarField &, const DimensionedField< scalar, volMesh > &)
	Construct as copy setting internal field reference. More...

Public Member Functions inherited from temperatureCoupledBase
	temperatureCoupledBase (const fvPatch &patch, const word &calculationMethod, const word &kappaName, const word &alphaAniName, const word &alphaName)
	Construct from patch and K name. More...

	temperatureCoupledBase (const fvPatch &patch, const dictionary &dict)
	Construct from patch and dictionary. More...

	temperatureCoupledBase (const fvPatch &patch, const temperatureCoupledBase &base)
	Construct from patch and temperatureCoupledBase. More...

virtual	~temperatureCoupledBase ()=default
	Destructor. More...

word	KMethod () const
	Method to obtain K. More...

const word &	kappaName () const
	Name of thermal conductivity field. More...

const word &	alphaName () const
	Name of thermal diffusivity field. More...

virtual tmp< scalarField >	kappa (const scalarField &Tp) const
	Given patch temperature calculate corresponding K field. More...

virtual tmp< scalarField >	alpha (const scalarField &Tp) const
	Given patch temperature calculate corresponding alphaEff field. More...

void	write (Ostream &os) const
	Write. More...

Additional Inherited Members
Public Types inherited from temperatureCoupledBase
enum	KMethodType { mtFluidThermo, mtSolidThermo, mtDirectionalSolidThermo, mtLookup }
	Type of supplied Kappa. More...

Protected Attributes inherited from temperatureCoupledBase
const fvPatch &	patch_
	Underlying patch. More...

const KMethodType	method_
	How to get K. More...

const word	kappaName_
	Name of thermal conductivity field (if looked up from database) More...

const word	alphaAniName_
	Name of the non-Isotropic alpha (default: Anialpha) More...

const word	alphaName_
	Name of thermal diffusivity. More...

Static Protected Attributes inherited from temperatureCoupledBase
static const Enum< KMethodType >	KMethodTypeNames_

Detailed Description

This boundary condition provides a coupled temperature condition between multiple mesh regions.

The regions are generally referred to as the:

primary region,
and baffle region.

The primary region creates the baffle region and evolves its energy equation either:

1-D, normal to each patch face
2-D, normal and tangential components

The thermodynamic properties of the baffle material are specified via dictionary entries on the master patch.

Usage

Example of the boundary condition specification:

<masterPatchName>
{
    type                compressible::thermalBaffle;

    // Underlying coupled boundary condition
    Tnbr               T;
    kappaMethod        fluidThermo; // or solidThermo
    kappa              none;
    qrNbr              qr;//or none.Name of qr field on neighbourregion
    qr                 none;// or none.Name of qr field on localregion
    value              uniform 300;

    // Baffle region name
    regionName          baffleRegion;
    active              yes;

    // Solid thermo in solid region
    thermoType
    {
        type            heSolidThermo;
        mixture         pureMixture;
        transport       constIso;
        thermo          hConst;
        equationOfState rhoConst;
        specie          specie;
        energy          sensibleEnthalpy;
    }

    mixture
    {
        specie
        {
            molWeight       20;
        }
        transport
        {
            kappa           0.01;
        }
        thermodynamics
        {
            Hf              0;
            Cp              15;
        }
        density
        {
            rho             80;
        }
    }

    radiation
    {
        radiationModel  opaqueSolid;
        absorptionEmissionModel none;
        scatterModel    none;
    }

    // Extrude model for new region

    extrudeModel        linearNormal;
    nLayers             50;
    expansionRatio      1;
    columnCells         false; //3D or 1D
    linearNormalCoeffs
    {
        thickness           0.02;
    }

}

Slave patch on primary region:

<slavePatchName>
{
    type                compressible::thermalBaffle;
    kappaMethod         fluidThermo;
    kappa               none;
    value               uniform 300;

Patches on baffle region:

bottom
{
    type                compressible::thermalBaffle;
    kappaMethod         solidThermo;
    kappa               none;
    value               uniform 300;
}

top
{
    type                compressible::thermalBaffle;
    kappaMethod         solidThermo;
    kappa               none;
    value               uniform 300;
}

See also: Foam::compressible::turbulentTemperatureCoupledBaffleMixedFvPatchScalarField Foam::regionModels::thermalBaffleModels::thermalBaffleModel

Source files

Definition at line 180 of file thermalBaffleFvPatchScalarField.H.

Constructor & Destructor Documentation

◆ thermalBaffleFvPatchScalarField() [1/4]

thermalBaffleFvPatchScalarField	(	const fvPatch &	p,
		const DimensionedField< scalar, volMesh > &	iF
	)

Construct from patch and internal field.

Definition at line 43 of file thermalBaffleFvPatchScalarField.C.

Referenced by thermalBaffleFvPatchScalarField::clone().

Here is the caller graph for this function:

◆ thermalBaffleFvPatchScalarField() [2/4]

thermalBaffleFvPatchScalarField	(	const fvPatch &	p,
		const DimensionedField< scalar, volMesh > &	iF,
		const dictionary &	dict
	)

Construct from patch, internal field and dictionary.

Definition at line 79 of file thermalBaffleFvPatchScalarField.C.

References polyMesh::defaultRegion, dict, objectRegistry::foundObject(), fvMesh::name(), Foam::New(), Foam::foamVersion::patch, regionName, and fvMesh::time().

Here is the call graph for this function:

◆ thermalBaffleFvPatchScalarField() [3/4]

thermalBaffleFvPatchScalarField	(	const thermalBaffleFvPatchScalarField &	ptf,
		const fvPatch &	p,
		const DimensionedField< scalar, volMesh > &	iF,
		const fvPatchFieldMapper &	mapper
	)

Construct by mapping given.

thermalBaffleFvPatchScalarField onto a new patch

Definition at line 57 of file thermalBaffleFvPatchScalarField.C.

◆ thermalBaffleFvPatchScalarField() [4/4]

thermalBaffleFvPatchScalarField	(	const thermalBaffleFvPatchScalarField &	ptf,
		const DimensionedField< scalar, volMesh > &	iF
	)

Construct as copy setting internal field reference.

Definition at line 122 of file thermalBaffleFvPatchScalarField.C.

Member Function Documentation

◆ TypeName()

TypeName ( "compressible::thermalBaffle" )

Runtime type information.

◆ clone() [1/2]

virtual tmp<fvPatchScalarField> clone ( ) const

inlinevirtual

Construct and return a clone.

Reimplemented from turbulentTemperatureRadCoupledMixedFvPatchScalarField.

Definition at line 247 of file thermalBaffleFvPatchScalarField.H.

References thermalBaffleFvPatchScalarField::thermalBaffleFvPatchScalarField().

Here is the call graph for this function:

◆ clone() [2/2]

virtual tmp<fvPatchScalarField> clone ( const DimensionedField< scalar, volMesh > & iF ) const

inlinevirtual

Construct and return a clone setting internal field reference.

Reimplemented from turbulentTemperatureRadCoupledMixedFvPatchScalarField.

Definition at line 264 of file thermalBaffleFvPatchScalarField.H.

References thermalBaffleFvPatchScalarField::thermalBaffleFvPatchScalarField().

Here is the call graph for this function:

◆ autoMap()

void autoMap ( const fvPatchFieldMapper & m )

virtual

Map (and resize as needed) from self given a mapping object.

Definition at line 139 of file thermalBaffleFvPatchScalarField.C.

◆ rmap()

void rmap	(	const fvPatchScalarField &	ptf,
		const labelList &	addr
	)

virtual

Reverse map the given fvPatchField onto this fvPatchField.

Definition at line 148 of file thermalBaffleFvPatchScalarField.C.

◆ updateCoeffs()

void updateCoeffs ( )

virtual

Update the coefficients associated with the patch field.

Reimplemented from turbulentTemperatureRadCoupledMixedFvPatchScalarField.

Definition at line 243 of file thermalBaffleFvPatchScalarField.C.

References polyMesh::defaultRegion, fvMesh::name(), Foam::foamVersion::patch, and turbulentTemperatureRadCoupledMixedFvPatchScalarField::updateCoeffs().

Here is the call graph for this function:

◆ write()

void write ( Ostream & os ) const

virtual

Write.

Reimplemented from turbulentTemperatureRadCoupledMixedFvPatchScalarField.

Definition at line 261 of file thermalBaffleFvPatchScalarField.C.

References polyMesh::defaultRegion, dictionary::get(), fvMesh::name(), Foam::nl, Foam::foamVersion::patch, dictionary::subDict(), turbulentTemperatureRadCoupledMixedFvPatchScalarField::write(), Ostream::writeEntry(), and Ostream::writeKeyword().

Here is the call graph for this function:

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

src/regionModels/thermalBaffleModels/derivedFvPatchFields/thermalBaffle/thermalBaffleFvPatchScalarField.H
src/regionModels/thermalBaffleModels/derivedFvPatchFields/thermalBaffle/thermalBaffleFvPatchScalarField.C

Public Member Functions

Additional Inherited Members

Detailed Description

Constructor & Destructor Documentation

◆ thermalBaffleFvPatchScalarField() [1/4]

◆ thermalBaffleFvPatchScalarField() [2/4]

◆ thermalBaffleFvPatchScalarField() [3/4]

◆ thermalBaffleFvPatchScalarField() [4/4]

Member Function Documentation

◆ TypeName()

◆ clone() [1/2]

◆ clone() [2/2]

◆ autoMap()

◆ rmap()

◆ updateCoeffs()

◆ write()