Description🔗
The pressureDirectedInletOutletVelocity
is a velocity inlet/outlet boundary
condition that applies zero-gradient condition for outflow (as defined by the
flux); and obtains the velocity from the flux with the specified inlet direction
for inflow.
Usage🔗
The condition requires entries in both the boundary and field files.
Boundary file🔗
<patchName>
{
type patch;
...
}
Field file🔗
<patchName>
{
// Mandatory entries
type pressureDirectedInletOutletVelocity;
inletDirection <vectorField>;
// Optional entries
phi <word>;
rho <word>;
// Inherited entries;
...
}
where:
Property | Description | Type | Required | Default |
---|---|---|---|---|
type |
Type name: pressureDirectedInletOutletVelocity
|
word | yes | - |
inletDirection |
Inlet direction field | vectorField | 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
- 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:
- N/A
Source code:
API:
History:
- Introduced in version 1.5