Description🔗

The fanPressure is a pressure boundary condition to assign either a pressure inlet or outlet total pressure condition for a fan. The condition sets the static pressure from a definition of the total pressure and pressure drop as a function of volumetric flow rate across the patch.

The non-dimensional flux is calculated as follows:

\[phi = \frac{4 \dot{m}}{\rho \pi^2 d_m^3 \omega}\]

The non-dimensional flux is calculated as follows:

\[\Psi = \frac{2 \Delta P}{\rho (\pi \omega d_m)}\]

The non-dimensional table should be given as \(\Psi = F(\phi)\).

The condition sets the static pressure at the patch \(p_p\) based on a specification of the total pressure, \(p_0\), and pressure drop, \(p_d\), specified as a function of the volumetric flow rate.

\[p_p = p_0 - p_d\]

Usage🔗

The condition requires entries in both the boundary and field files.

Boundary file🔗

<patchName>
{
    type            patch;
    ...
}

Field file🔗

<patchName>
{
    // Mandatory entries
    type            fanPressure;
    fanCurve        <Function1<scalar>>;
    direction       <word>;

    // Optional entries
    nonDimensional  <bool>;

    // Conditional entries

      // if 'nonDimensional' is true
      rpm           <Function1<scalar>>;
      dm            <Function1<scalar>>;

    // Inherited entries;
    ...
}

where:

Options for the direction entry:

The inherited entries are elaborated in:

• Foam::totalPressureFvPatchScalarField

• Foam::Function1

• For compatibility with older versions (OpenFOAM-v2006 and earlier), a missing fanCurve keyword is treated as a tableFile and makes the file keyword mandatory.

Further information🔗

Tutorial:

• $FOAM_TUTORIALS/incompressible/pimpleFoam/RAS/TJunctionFan

Source code:

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

API:

• Foam::fanPressureFvPatchScalarField

History:

• Introduced in version 1.5