Velocity inlet boundary condition either correcting the extrapolated velocity or creating a uniform velocity field normal to the patch adjusted to match the specified flow rate. 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...

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

virtual tmp< fvPatchField< vector > >	clone () const
	Return a clone. More...

virtual tmp< fvPatchField< vector > >	clone (const DimensionedField< vector, volMesh > &iF) const
	Clone with an 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

Velocity inlet boundary condition either correcting the extrapolated velocity or creating a uniform velocity field normal to the patch adjusted to match the specified flow rate.

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
`rho`	density field name	no	rho
`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 Foam::flowRateOutletVelocityFvPatchVectorField

Source files

Definition at line 141 of file flowRateInletVelocityFvPatchVectorField.H.

Constructor & Destructor Documentation

◆ flowRateInletVelocityFvPatchVectorField() [1/5]

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

Construct from patch and internal field.

Definition at line 32 of file flowRateInletVelocityFvPatchVectorField.C.

◆ flowRateInletVelocityFvPatchVectorField() [2/5]

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

Construct from patch, internal field and dictionary.

Definition at line 48 of file flowRateInletVelocityFvPatchVectorField.C.

References dict, Foam::stringOps::evaluate(), Foam::exit(), Foam::FatalIOError, FatalIOErrorInFunction, and Foam::nl.

Here is the call graph for this function:

◆ flowRateInletVelocityFvPatchVectorField() [3/5]

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 96 of file flowRateInletVelocityFvPatchVectorField.C.

◆ flowRateInletVelocityFvPatchVectorField() [4/5]

flowRateInletVelocityFvPatchVectorField ( const flowRateInletVelocityFvPatchVectorField & ptf )

Construct as copy.

Definition at line 114 of file flowRateInletVelocityFvPatchVectorField.C.

◆ flowRateInletVelocityFvPatchVectorField() [5/5]

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

Construct as copy setting internal field reference.

Definition at line 129 of file flowRateInletVelocityFvPatchVectorField.C.

Member Function Documentation

◆ TypeName()

TypeName ( "flowRateInletVelocity" )

Runtime type information.

◆ clone() [1/2]

virtual tmp<fvPatchField<vector> > clone ( ) const

inlinevirtual

Return a clone.

Definition at line 245 of file flowRateInletVelocityFvPatchVectorField.H.

References fvPatchField< Type >::Clone().

Here is the call graph for this function:

◆ clone() [2/2]

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

inlinevirtual

Clone with an internal field reference.

Definition at line 254 of file flowRateInletVelocityFvPatchVectorField.H.

References fvPatchField< Type >::Clone().

Here is the call graph for this function:

◆ updateCoeffs()

void updateCoeffs ( )

virtual

Update the coefficients associated with the patch field.

Definition at line 194 of file flowRateInletVelocityFvPatchVectorField.C.

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

Here is the call graph for this function:

◆ write()

void write ( Ostream & os ) const

virtual

Write.

Definition at line 235 of file flowRateInletVelocityFvPatchVectorField.C.

References os(), fvPatchField< Type >::write(), Ostream::writeEntry(), Ostream::writeEntryIfDifferent(), and fvPatchField< Type >::writeValueEntry().

Here is the call 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

◆ flowRateInletVelocityFvPatchVectorField() [1/5]

◆ flowRateInletVelocityFvPatchVectorField() [2/5]

◆ flowRateInletVelocityFvPatchVectorField() [3/5]

◆ flowRateInletVelocityFvPatchVectorField() [4/5]

◆ flowRateInletVelocityFvPatchVectorField() [5/5]

Member Function Documentation

◆ TypeName()

◆ clone() [1/2]

◆ clone() [2/2]

◆ updateCoeffs()

◆ write()