pressureInletOutletParSlipVelocity

Description

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

The slip condition is applied tangential to the patch.

Usage

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

Boundary file

<patchName>
{
    type            patch;
    ...
}

Field file

<patchName>
{
    // Mandatory entries
    type            pressureInletOutletParSlipVelocity;

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

    // Inherited entries;
    ...
}

where:

Property	Description	Type	Required	Default
type	Type name: pressureInletOutletParSlipVelocity	word	yes	-
phi	Name of flux field	word	no	phi
rho	Name of density field	word	no	rho

The inherited entries are elaborated in:

• 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:

• oscillatingBox

Source code:

• pressureInletOutletParSlipVelocity

API:

• Foam::pressureInletOutletParSlipVelocityFvPatchVectorField

History: Introduced in version 2.1.0