pressureDirectedInletVelocity

Description

The pressureDirectedInletVelocity is a velocity boundary condition that calculates inflow velocity from the flux with the specified inlet direction.

Usage

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

Boundary file

<patchName>
{
    type            patch;
    ...
}

Field file

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

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

    // Inherited entries
    ...
}

where:

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

The inherited entries are elaborated in:

• Foam::fixedValueFvPatchField

• If reverse flow is possible or expected use the pressureDirectedInletOutletVelocity condition instead.

Further information

Tutorial:

• N/A

Source code:

• pressureDirectedInletVelocity

API:

• Foam::pressureDirectedInletVelocityFvPatchVectorField

History: Introduced in version 1.5