pressureDirectedInletOutletVelocity

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:

Property	Description	Type	Required	Default
type	Type name: pressureDirectedInletOutletVelocity	word	yes	-
inletDirection	Inlet direction field	vectorField	yes	-
phi	Name of flux field	word	no	phi
rho	Name of density field	word	no	rho

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:

• pressureDirectedInletOutletVelocity

API:

• Foam::pressureDirectedInletOutletVelocityFvPatchVectorField

History: Introduced in version 1.5