Description🔗
The fluxCorrectedVelocity
is a velocity-outlet boundary condition that
for patches where the pressure is specified. The outflow velocity is obtained
by zeroGradient
and then corrected from the flux.
Usage🔗
The condition requires entries in both the boundary and field files.
Boundary file🔗
<patchName>
{
type patch;
...
}
Field file🔗
<patchName>
{
// Mandatory entries
type fluxCorrectedVelocity;
// Conditional entries
// Option-1
volumetricFlowRate <Function1<scalar>>;
// Option-2
massFlowRate <Function1<scalar>>;
// Optional entries
rho <word>;
rhoOutlet <scalar>;
// Inherited entries
...
}
where:
Property | Description | Type | Required | Default |
---|---|---|---|---|
type |
Type name: fluxCorrectedVelocity
|
word | yes | - |
volumetricFlowRate |
Volumetric flow rate | Function1<scalar> | choice | - |
massFlowRate |
Mass flow rate | Function1<scalar> | choice | - |
rho |
Name of density field | word | no | rho |
rhoOutlet |
Density initialisation value | scalar | no | -VGREAT |
The inherited entries are elaborated in:
- Foam::fixedValueFvPatchField
- For a mass-based flux:
- The flow rate should be provided in [kg/s].
- If
rho
isnone
the flow rate is in [m^3/s]. - Otherwise
rho
should correspond to the name of the density field - If the density field cannot be found in the database, the user must
specify the outlet density using the
rhoOutlet
entry.
- For a volumetric-based flux:
- The flow rate is in [m^3/s].
-
rhoOutlet
is required for the case of a mass flow rate, where the density field is not available at start-up. - The value is positive out of the domain (as an outlet).
- May not work correctly for transonic outlets.
- Strange behaviour with potentialFoam since the U equation is not solved.
Further information🔗
Tutorial:
Source code:
API:
History:
- Introduced in version v1712