Description🔗
The flowRateInletVelocity
is a velocity boundary condition that either
corrects the extrapolated velocity or creates a uniform velocity field normal
to the patch adjusted to match the specified flow rate.
The condition is a wrapper around the fixedValue
condition.
Usage🔗
The condition requires entries in both the boundary
and field files.
Boundary file🔗
<patchName>
{
type patch;
...
}
Field file🔗
<patchName>
{
// Mandatory entries
type flowRateInletVelocity;
// Conditional entries
// Option-1
volumetricFlowRate <Function1<scalar>>;
// Option-2
massFlowRate <Function1<scalar>>;
// Optional entries
rho <word>;
rhoInlet <scalar>;
extrapolateProfile <bool>;
// Inherited entries
...
}
where:
Property | Description | Type | Required | Default |
---|---|---|---|---|
type |
Type name: flowRateInletVelocity
|
word | yes | - |
volumetricFlowRate |
Volumetric flow rate | Function1<scalar> | choice | - |
massFlowRate |
Mass flow rate | Function1<scalar> | choice | - |
rho |
Name of density field | word | no | rho |
rhoInlet |
Density initialisation value | scalar | no | -VGREAT |
extrapolateProfile |
Flag to extrapolate the velocity profile from the interior | bool | no | false |
The inherited entries are elaborated in:
- fixedValueFvPatchFields.H
-
Function1.H
- For a mass-based flux input:
- 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 inlet density using the
rhoInlet
entry.
- For a volumetric-based flux:
- The flow rate is in [m^3/s].
A uniform plug flow is set by default. To set the profile according to the downstream cells:
extrapolateProfile yes;
To convert from a mass flow rate to a volumetric flow rate:
rho rho;
To convert from a mass flow rate to a volumetric flow rate for incompressible flows:
rhoInlet 1.0;
Method🔗
N/A
Further information🔗
Tutorial:
- $FOAM_TUTORIALS/compressible/rhoPimpleFoam/laminar/helmholtzResonance
- $FOAM_TUTORIALS/incompressible/porousSimpleFoam/angledDuct
Source code:
API:
History:
- Introduced in version 1.5