fluxCorrectedVelocity

Description

The fluxCorrectedVelocity is a velocity-outlet boundary condition that for patches where the pressure is specified. The outflow velocity is obtained by zeroGradient and then corrected from the flux.

Usage

The condition requires entries in both the boundary and field files.

Boundary file

<patchName>
{
    type            patch;
    ...
}

Field file

<patchName>
{
    // Mandatory entries
    type            fluxCorrectedVelocity;

    // Conditional entries

        // Option-1
        volumetricFlowRate      <Function1<scalar>>;

        // Option-2
        massFlowRate            <Function1<scalar>>;

    // Optional entries
    rho             <word>;
    rhoOutlet       <scalar>;

    // Inherited entries
    ...
}

where:

Property	Description	Type	Required	Default
type	Type name: fluxCorrectedVelocity	word	yes	-
volumetricFlowRate	Volumetric flow rate	Function1<scalar>	choice	-
massFlowRate	Mass flow rate	Function1<scalar>	choice	-
rho	Name of density field	word	no	rho
rhoOutlet	Density initialisation value	scalar	no	-VGREAT

The inherited entries are elaborated in:

• Foam::fixedValueFvPatchField
• Foam::Function1

• For a mass-based flux:
  • The flow rate should be provided in [kg/s].
  • If rho is none the flow rate is in [m^3/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 outlet density using the `rhoOutlet` entry.

• For a volumetric-based flux:
  • The flow rate is in [m^3/s].
• rhoOutlet is required for the case of a mass flow rate, where the density field is not available at start-up.
• The value is positive out of the domain (as an outlet).
• May not work correctly for transonic outlets.
• Strange behaviour with potentialFoam since the U equation is not solved.

Further information

Tutorial:

• iobasin

Source code:

• fluxCorrectedVelocity

API:

• Foam::fluxCorrectedVelocityFvPatchVectorField

History: Introduced in version v1712