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:

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:

• $FOAM_TUTORIALS/multiphase/interIsoFoam/iobasin

Source code:

• $FOAM_SRC/finiteVolume/fields/fvPatchFields/derived/fluxCorrectedVelocity

API:

• Foam::fluxCorrectedVelocityFvPatchVectorField

History:

• Introduced in version v1712