fluxCorrectedVelocity

Description

The fluxCorrectedVelocity is a velocity-outlet boundary condition that corrects the extrapolated velocity to match the specified flow rate.

Usage

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

Boundary file

<patchName>
{
    type            patch;
    ...
}

Field file

<patchName>
{
    // Mandatory entries
    type            fluxCorrectedVelocity;

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

    // Inherited entries
    ...
}

where:

Property	Description	Type	Required	Default
type	Type name: fluxCorrectedVelocity	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::fvPatchField
• Foam::zeroGradientFvPatchField

Method

$$\mathbf{u}_p = \mathbf{u}_c - \mathbf{n} (\mathbf{n} \cdot \mathbf{u}_c) + \frac{\mathbf{n} \phi_p}{|\mathbf{S}_f|}$$

where:

Property	Description
$\mathbf{u}_p$	Patch velocity [m/s]
$\mathbf{u}_c$	Velocity in cells adjacent to the patch [m/s]
$\mathbf{u}_c$	Patch-normal vectors [-]
$\phi_p$	Patch flux [m^3/s] or [kg/s]
$\mathbf{S}_f$	Patch face area vectors [m^2]

Further information

Tutorial:

• damBreak4phase

Source code:

• fluxCorrectedVelocity

API:

• Foam::fluxCorrectedVelocityFvPatchVectorField

History: Introduced in version 1.5