Public Member Functions | List of all members
flowRateInletVelocityFvPatchVectorField Class Reference

Velocity inlet boundary condition creating a velocity field with optionally specified profile normal to the patch adjusted to match the specified mass flow rate, volumetric flow rate or mean velocity. More...

Inheritance diagram for flowRateInletVelocityFvPatchVectorField:
Inheritance graph
[legend]
Collaboration diagram for flowRateInletVelocityFvPatchVectorField:
Collaboration graph
[legend]

Public Member Functions

 TypeName ("flowRateInletVelocity")
 Runtime type information. 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 fieldMapper &)
 Construct by mapping given. More...
 
 flowRateInletVelocityFvPatchVectorField (const flowRateInletVelocityFvPatchVectorField &)=delete
 Disallow copy without setting internal field reference. More...
 
 flowRateInletVelocityFvPatchVectorField (const flowRateInletVelocityFvPatchVectorField &, const DimensionedField< vector, volMesh > &)
 Copy constructor 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 map (const fvPatchVectorField &, const fieldMapper &)
 Map the given fvPatchField onto this fvPatchField. More...
 
virtual void reset (const fvPatchVectorField &)
 Reset the fvPatchField to the given fvPatchField. 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 creating a velocity field with optionally specified profile normal to the patch adjusted to match the specified mass flow rate, volumetric flow rate or mean velocity.

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 [m^3/s] no
meanVelocity Mean velocity [m/s] no
profile Velocity profile no
rho Density field name no rho
rhoInlet Inlet density no
alpha Volume fraction field name no

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

    <patchName>
    {
        type                flowRateInletVelocity;
        volumetricFlowRate  0.2;
        profile             laminarBL;
    }

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

    <patchName>
    {
        type                flowRateInletVelocity;
        massFlowRate        0.2;
        profile             turbulentBL;
        rho                 rho;
        rhoInlet            1.0;
    }

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

    <patchName>
    {
        type                flowRateInletVelocity;
        meanVelocity        5;
        profile             turbulentBL;
    }

The volumetricFlowRate, massFlowRate or meanVelocity entries are Function1 of time, see Foam::Function1s.

The profile entry is a Function1 of the normalised distance to the wall. Any suitable Foam::Function1s can be used including Foam::Function1s::codedFunction1 but Foam::Function1s::laminarBL and Foam::Function1s::turbulentBL have been created specifically for this purpose and are likely to be appropriate for most cases.

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::Function1s::laminarBL Foam::Function1s::turbulentBL Foam::Function1s Foam::flowRateOutletVelocityFvPatchVectorField
Source files

Definition at line 168 of file flowRateInletVelocityFvPatchVectorField.H.

Constructor & Destructor Documentation

◆ flowRateInletVelocityFvPatchVectorField() [1/4]

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

Construct from patch, internal field and dictionary.

Definition at line 137 of file flowRateInletVelocityFvPatchVectorField.C.

References UPstream::blocking, dict, DimensionedField< Type, GeoMesh >::dimensions(), Foam::dimless, Foam::dimMassFlux, Foam::dimVelocity, Foam::dimVolumetricFlux, Foam::evaluate(), Foam::exit(), Foam::FatalIOError, FatalIOErrorInFunction, Function1< Type >::New(), and p.

Referenced by flowRateInletVelocityFvPatchVectorField::clone().

Here is the call graph for this function:
Here is the caller graph for this function:

◆ flowRateInletVelocityFvPatchVectorField() [2/4]

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

Construct by mapping given.

flowRateInletVelocityFvPatchVectorField onto a new patch

Definition at line 227 of file flowRateInletVelocityFvPatchVectorField.C.

◆ flowRateInletVelocityFvPatchVectorField() [3/4]

flowRateInletVelocityFvPatchVectorField ( const flowRateInletVelocityFvPatchVectorField &  )
delete

Disallow copy without setting internal field reference.

◆ flowRateInletVelocityFvPatchVectorField() [4/4]

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

Copy constructor setting internal field reference.

Definition at line 254 of file flowRateInletVelocityFvPatchVectorField.C.

Member Function Documentation

◆ TypeName()

TypeName ( "flowRateInletVelocity"  )

Runtime type information.

◆ clone()

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

Construct and return a clone setting internal field reference.

Definition at line 272 of file flowRateInletVelocityFvPatchVectorField.H.

References flowRateInletVelocityFvPatchVectorField::flowRateInletVelocityFvPatchVectorField().

Here is the call graph for this function:

◆ map()

void map ( const fvPatchVectorField &  ptf,
const fieldMapper &  mapper 
)
virtual

Map the given fvPatchField onto this fvPatchField.

Definition at line 276 of file flowRateInletVelocityFvPatchVectorField.C.

◆ reset()

void reset ( const fvPatchVectorField &  ptf)
virtual

Reset the fvPatchField to the given fvPatchField.

Used for mesh to mesh mapping

Definition at line 294 of file flowRateInletVelocityFvPatchVectorField.C.

◆ updateCoeffs()

void updateCoeffs ( )
virtual

Update the coefficients associated with the patch field.

Definition at line 311 of file flowRateInletVelocityFvPatchVectorField.C.

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

Here is the call graph for this function:

◆ write()

void write ( Ostream &  os) const
virtual

Write.

Definition at line 341 of file flowRateInletVelocityFvPatchVectorField.C.

References word::null, Foam::unitAny, fvPatchField< Type >::write(), and Foam::writeEntry().

Here is the call graph for this function:
The documentation for this class was generated from the following files: