Description🔗

The freestream is a generic boundary condition that provides a free-stream condition. It is a mixed condition derived from the inletOutlet condition, whereby the mode of operation switches between fixed (free stream) value and zero gradient based on the sign of 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            freestream;

    // Conditional entries

        // Option-1
        freestreamValue        <Field<Type>>;

        // Option-2
        freestreamBC           <fvPatchField<Type>>;

    // Optional entries
    phi             <word>;

    // Inherited entries;
    ...
}

where:

The inherited entries are elaborated in:

• Foam::inletOutletFvPatchField

Further information🔗

Tutorial:

• $FOAM_TUTORIALS/compressible/rhoPimpleFoam/RAS/aerofoilNACA0012
• $FOAM_TUTORIALS/verificationAndValidation/atmosphericModels/atmFlatTerrain

Source code:

• $FOAM_SRC/finiteVolume/fields/fvPatchFields/derived/freestream

API:

• Foam::freestreamFvPatchField

History:

• Introduced in version 1.5