Description🔗

The pressureDirectedInletOutletVelocity is a velocity inlet/outlet boundary condition that applies zero-gradient condition for outflow (as defined by the flux); and obtains the velocity from the flux with the specified inlet direction for inflow.

Usage🔗

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

Boundary file🔗

<patchName>
{
    type            patch;
    ...
}

Field file🔗

<patchName>
{
    // Mandatory entries
    type            pressureDirectedInletOutletVelocity;
    inletDirection  <vectorField>;

    // Optional entries
    phi             <word>;
    rho             <word>;

    // Inherited entries;
    ...
}

where:

The inherited entries are elaborated in:

• Foam::fvPatchField

• Foam::mixedFvPatchField

• Sign conventions:
  • positive flux (out of domain): apply zero-gradient condition
  • negative flux (into of domain): derive from the flux with specified direction

Further information🔗

Tutorial:

• N/A

Source code:

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

API:

• Foam::pressureDirectedInletOutletVelocityFvPatchVectorField

History:

• Introduced in version 1.5