This boundary condition provides a velocity boundary condition, derived from the flux (volumetric or mass-based), whose direction is assumed to be normal to the patch. More...

Inheritance diagram for flowRateInletVelocityFvPatchVectorField:

[legend]

Collaboration diagram for flowRateInletVelocityFvPatchVectorField:

[legend]

Public Member Functions
	TypeName ("flowRateInletVelocity")
	Runtime type information. More...

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

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

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

	flowRateInletVelocityFvPatchVectorField (const flowRateInletVelocityFvPatchVectorField &)
	Construct as copy. More...

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

	flowRateInletVelocityFvPatchVectorField (const flowRateInletVelocityFvPatchVectorField &, 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	updateCoeffs ()
	Update the coefficients associated with the patch field. More...

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

Detailed Description

This boundary condition provides a velocity boundary condition, derived from the flux (volumetric or mass-based), whose direction is assumed to be normal to the patch.

For a mass-based flux:

the flow rate should be provided in kg/s
if rho is "none" the flow rate is in m3/s
otherwise rho should correspond to the name of the density field
if the density field cannot be found in the database, the user must specify the inlet density using the rhoInlet entry

For a volumetric-based flux:

the flow rate is in m3/s

Usage

Property	Description	Required	Default value
`massFlowRate`	mass flow rate [kg/s]	no
`volumetricFlowRate`	volumetric flow rate [m3/s]	no
`rhoInlet`	inlet density	no
`extrapolateProfile`	Extrapolate velocity profile	no	false

Example of the boundary condition specification for a volumetric flow rate:

    <patchName>
    {
        type                flowRateInletVelocity;
        volumetricFlowRate  0.2;
        extrapolateProfile  yes;
        value               uniform (0 0 0);
    }

Example of the boundary condition specification for a mass flow rate:

    <patchName>
    {
        type                flowRateInletVelocity;
        massFlowRate        0.2;
        extrapolateProfile  yes;
        rho                 rho;
        rhoInlet            1.0;
        value               uniform (0 0 0);
    }

The flowRate entry is a Function1 of time, see Foam::Function1Types.

Note

rhoInlet is required for the case of a mass flow rate, where the density field is not available at start-up
The value is positive into the domain (as an inlet)
May not work correctly for transonic inlets
Strange behaviour with potentialFoam since the U equation is not solved

See also: Foam::fixedValueFvPatchField Foam::Function1Types

Source files

Definition at line 135 of file flowRateInletVelocityFvPatchVectorField.H.

Constructor & Destructor Documentation

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

Construct from patch and internal field.

Definition at line 35 of file flowRateInletVelocityFvPatchVectorField.C.

Referenced by flowRateInletVelocityFvPatchVectorField::clone(), and flowRateInletVelocityFvPatchVectorField::flowRateInletVelocityFvPatchVectorField().

Here is the caller graph for this function:

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

Construct from patch, internal field and dictionary.

Definition at line 51 of file flowRateInletVelocityFvPatchVectorField.C.

References Foam::exit(), Foam::FatalIOError, FatalIOErrorInFunction, flowRateInletVelocityFvPatchVectorField::flowRateInletVelocityFvPatchVectorField(), dictionary::found(), dictionary::lookupOrDefault(), Foam::New(), List< Type >::size(), and vectorField().

Here is the call graph for this function:

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

Construct by mapping given.

flowRateInletVelocityFvPatchVectorField onto a new patch

Definition at line 102 of file flowRateInletVelocityFvPatchVectorField.C.

References flowRateInletVelocityFvPatchVectorField::flowRateInletVelocityFvPatchVectorField().

Here is the call graph for this function:

flowRateInletVelocityFvPatchVectorField ( const flowRateInletVelocityFvPatchVectorField & ptf )

Construct as copy.

Definition at line 120 of file flowRateInletVelocityFvPatchVectorField.C.

References flowRateInletVelocityFvPatchVectorField::flowRateInletVelocityFvPatchVectorField().

Here is the call graph for this function:

flowRateInletVelocityFvPatchVectorField	(	const flowRateInletVelocityFvPatchVectorField &	ptf,
		const DimensionedField< vector, volMesh > &	iF
	)

Construct as copy setting internal field reference.

Definition at line 135 of file flowRateInletVelocityFvPatchVectorField.C.

References Foam::gSum(), Foam::mag(), n, Foam::operator==(), and rho.

Here is the call graph for this function:

Member Function Documentation

TypeName ( "flowRateInletVelocity" )

Runtime type information.

virtual tmp<fvPatchVectorField> clone ( ) const

inlinevirtual

Construct and return a clone.

Definition at line 205 of file flowRateInletVelocityFvPatchVectorField.H.

References flowRateInletVelocityFvPatchVectorField::flowRateInletVelocityFvPatchVectorField().

Here is the call graph for this function:

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

inlinevirtual

Construct and return a clone setting internal field reference.

Definition at line 222 of file flowRateInletVelocityFvPatchVectorField.H.

References flowRateInletVelocityFvPatchVectorField::flowRateInletVelocityFvPatchVectorField(), flowRateInletVelocityFvPatchVectorField::updateCoeffs(), and flowRateInletVelocityFvPatchVectorField::write().

Here is the call graph for this function:

void updateCoeffs ( )

virtual

Update the coefficients associated with the patch field.

Definition at line 188 of file flowRateInletVelocityFvPatchVectorField.C.

References Foam::exit(), Foam::FatalError, and FatalErrorInFunction.

Referenced by flowRateInletVelocityFvPatchVectorField::clone().

Here is the call graph for this function:

Here is the caller graph for this function:

void write ( Ostream & os ) const

virtual

Write.

Definition at line 228 of file flowRateInletVelocityFvPatchVectorField.C.

References token::END_STATEMENT, Foam::makePatchTypeField(), Foam::nl, fvPatchField< Type >::write(), and Ostream::writeKeyword().

Referenced by flowRateInletVelocityFvPatchVectorField::clone().

Here is the call graph for this function:

Here is the caller graph for this function:

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

src/finiteVolume/fields/fvPatchFields/derived/flowRateInletVelocity/flowRateInletVelocityFvPatchVectorField.H
src/finiteVolume/fields/fvPatchFields/derived/flowRateInletVelocity/flowRateInletVelocityFvPatchVectorField.C

Public Member Functions

Detailed Description

Constructor & Destructor Documentation

Member Function Documentation