fluxCorrectedVelocityFvPatchVectorField Class Reference

This boundary condition provides a velocity outlet boundary condition for patches where the pressure is specified. The outflow velocity is obtained by "zeroGradient" and then corrected from the flux: More...

Inheritance diagram for fluxCorrectedVelocityFvPatchVectorField:

Collaboration diagram for fluxCorrectedVelocityFvPatchVectorField:

Public Member Functions
	TypeName ("fluxCorrectedVelocity")
	Runtime type information. More...
	fluxCorrectedVelocityFvPatchVectorField (const fvPatch &, const DimensionedField< vector, volMesh > &)
	Construct from patch and internal field. More...
	fluxCorrectedVelocityFvPatchVectorField (const fvPatch &, const DimensionedField< vector, volMesh > &, const dictionary &)
	Construct from patch, internal field and dictionary. More...
	fluxCorrectedVelocityFvPatchVectorField (const fluxCorrectedVelocityFvPatchVectorField &, const fvPatch &, const DimensionedField< vector, volMesh > &, const fvPatchFieldMapper &)
	Construct by mapping given fluxCorrectedVelocityFvPatchVectorField. More...
virtual tmp< fvPatchVectorField >	clone () const
	Construct and return a clone. More...
	fluxCorrectedVelocityFvPatchVectorField (const fluxCorrectedVelocityFvPatchVectorField &, const DimensionedField< vector, volMesh > &)
	Construct as copy setting internal field reference. More...
virtual tmp< fvPatchVectorField >	clone (const DimensionedField< vector, volMesh > &iF) const
	Construct and return a clone setting internal field reference. More...
virtual void	evaluate (const Pstream::commsTypes commsType=Pstream::commsTypes::blocking)
	Evaluate the patch field. More...
virtual void	write (Ostream &) const
	Write. More...

Detailed Description

This boundary condition provides a velocity outlet boundary condition for patches where the pressure is specified. The outflow velocity is obtained by "zeroGradient" and then corrected from the flux:

\[ U_p = U_c - n (n \cdot U_c) + \frac{n \phi_p}{|S_f|} \]

where

\( U_p \)	=	velocity at the patch [m/s]
\( U_c \)	=	velocity in cells adjacent to the patch [m/s]
\( n \)	=	patch normal vectors
\( \phi_p \)	=	flux at the patch [m3/s or kg/s]
\( S_f \)	=	patch face area vectors [m2]

where

Property	Description	Required	Default value
phi	name of flux field	no	phi
rho	name of density field	no	rho

Example of the boundary condition specification:

    <patchName>
    {
        type            fluxCorrectedVelocity;
        phi             phi;
        rho             rho;
    }

Note

If reverse flow is possible or expected use the pressureInletOutletVelocity condition instead.

See also

Foam::zeroGradientFvPatchField Foam::pressureInletOutletVelocityFvPatchVectorField

Source files

• fluxCorrectedVelocityFvPatchVectorField.H
• fluxCorrectedVelocityFvPatchVectorField.C

Definition at line 131 of file fluxCorrectedVelocityFvPatchVectorField.H.

Constructor & Destructor Documentation

fluxCorrectedVelocityFvPatchVectorField() [1/4]

fluxCorrectedVelocityFvPatchVectorField	(	const fvPatch &	p,
		const DimensionedField< vector, volMesh > &	iF
	)

Construct from patch and internal field.

Definition at line 37 of file fluxCorrectedVelocityFvPatchVectorField.C.

fluxCorrectedVelocityFvPatchVectorField() [2/4]

fluxCorrectedVelocityFvPatchVectorField	(	const fvPatch &	p,
		const DimensionedField< vector, volMesh > &	iF,
		const dictionary &	dict
	)

Construct from patch, internal field and dictionary.

Definition at line 65 of file fluxCorrectedVelocityFvPatchVectorField.C.

References dict, dictionary::getOrDefault(), word::null, and fvPatchField< vector >::operator=().

Here is the call graph for this function:

fluxCorrectedVelocityFvPatchVectorField() [3/4]

fluxCorrectedVelocityFvPatchVectorField	(	const fluxCorrectedVelocityFvPatchVectorField &	ptf,
		const fvPatch &	p,
		const DimensionedField< vector, volMesh > &	iF,
		const fvPatchFieldMapper &	mapper
	)

Construct by mapping given fluxCorrectedVelocityFvPatchVectorField.

onto a new patch

Definition at line 50 of file fluxCorrectedVelocityFvPatchVectorField.C.

fluxCorrectedVelocityFvPatchVectorField() [4/4]

fluxCorrectedVelocityFvPatchVectorField	(	const fluxCorrectedVelocityFvPatchVectorField &	fcvpvf,
		const DimensionedField< vector, volMesh > &	iF
	)

Construct as copy setting internal field reference.

Definition at line 82 of file fluxCorrectedVelocityFvPatchVectorField.C.

Member Function Documentation

TypeName()

TypeName

(

"fluxCorrectedVelocity"

)

Runtime type information.

clone() [1/2]

virtual tmp< fvPatchVectorField > clone ( ) const

inlinevirtual

Construct and return a clone.

Definition at line 178 of file fluxCorrectedVelocityFvPatchVectorField.H.

clone() [2/2]

virtual tmp< fvPatchVectorField > clone ( const DimensionedField< vector, volMesh > &  iF ) const

inlinevirtual

Construct and return a clone setting internal field reference.

Definition at line 194 of file fluxCorrectedVelocityFvPatchVectorField.H.

evaluate()

void evaluate ( const Pstream::commsTypes  commsType = Pstream::commsTypes::blocking )

virtual

Evaluate the patch field.

Definition at line 97 of file fluxCorrectedVelocityFvPatchVectorField.C.

References Foam::dimArea, Foam::dimDensity, DimensionedField< Type, GeoMesh >::dimensions(), Foam::dimVelocity, Foam::exit(), Foam::FatalError, FatalErrorInFunction, n, Foam::operator==(), and phi.

Here is the call graph for this function:

write()

void write ( Ostream &  os ) const

virtual

Write.

Definition at line 141 of file fluxCorrectedVelocityFvPatchVectorField.C.

References os(), ObukhovLength::write(), and Ostream::writeEntryIfDifferent().

Here is the call graph for this function:

---

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

• src/finiteVolume/fields/fvPatchFields/derived/fluxCorrectedVelocity/fluxCorrectedVelocityFvPatchVectorField.H
• src/finiteVolume/fields/fvPatchFields/derived/fluxCorrectedVelocity/fluxCorrectedVelocityFvPatchVectorField.C