Description🔗

The flowRateInletVelocity is a velocity boundary condition that either corrects the extrapolated velocity or creates a uniform velocity field normal to the patch adjusted to match the specified flow rate. The condition is a wrapper around the fixedValue condition.

Usage🔗

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

Boundary file🔗

<patchName>
{
    type            patch;
    ...
}

Field file🔗

<patchName>
{
    // Mandatory entries
    type                flowRateInletVelocity;

    // Conditional entries

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

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

    // Optional entries
    rho                 <word>;
    rhoInlet            <scalar>;
    extrapolateProfile  <bool>;

    // Inherited entries
    ...
}

where:

The inherited entries are elaborated in:

• Foam::fixedValueFvPatchField

• Foam::Function1

• For a mass-based flux input:
  • 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 inlet density using the rhoInlet entry.
• For a volumetric-based flux:
  • The flow rate is in [m^3/s].

A uniform plug flow is set by default. To set the profile according to the downstream cells:

extrapolateProfile  yes;

To convert from a mass flow rate to a volumetric flow rate:

rho                 rho;

To convert from a mass flow rate to a volumetric flow rate for incompressible flows:

rhoInlet            1.0;

Further information🔗

Tutorial:

• $FOAM_TUTORIALS/compressible/rhoPimpleFoam/laminar/helmholtzResonance
• $FOAM_TUTORIALS/incompressible/porousSimpleFoam/angledDuct

Source code:

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

API:

• Foam::flowRateInletVelocityFvPatchVectorField

History:

• Introduced in version 1.5