Description🔗
The freestreamPressure
is a generic boundary condition that provides
a free-stream condition for pressure. It is an outlet-inlet condition that
uses the velocity orientation to continuously blend between zero gradient for
normal inlet and fixed value for normal outlet flow.
Usage🔗
The condition requires entries in both the boundary
and field files.
Boundary file🔗
<patchName>
{
type patch;
...
}
Field file🔗
<patchName>
{
// Mandatory entries
type freestreamPressure;
freestreamValue <scalarField>;
// Optional entries
U <word>;
// Inherited entries;
...
}
where:
Property | Description | Type | Required | Default |
---|---|---|---|---|
type |
Type name: freestreamPressure
|
word | yes | - |
freestreamValue |
Patch value | scalarField | yes | - |
U |
Name of velocity field | word | no | U |
The inherited entries are elaborated in:
- fvPatchFields.H
- mixedFvPatchFields.H
Method🔗
N/A
Further information🔗
Tutorial:
- $FOAM_TUTORIALS/compressible/rhoPimpleFoam/RAS/aerofoilNACA0012
- $FOAM_TUTORIALS/incompressible/simpleFoam/airFoil2D
Source code:
API:
History:
- Introduced in version 1.5