turbulentMixingLengthFrequencyInlet

Description

The turbulentMixingLengthFrequencyInlet is a boundary condition that provides a turbulence specific dissipation, omega inlet condition based on a specified mixing length. The patch values are calculated using:

$$\omega_p = \frac{k^{0.5}}{C_{\mu}^{0.25} L}$$

where:

Property	Description
$\omega_p$	Patch omega values [1/s]
$C_\mu$	Empirical model constant retrived from turbulence model
$k$	Turbulent kinetic energy [m^2/s^2]
$L$	Mixing length scale [m]

Usage

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

Boundary file

<patchName>
{
    type            patch;
    ...
}

Field file

<patchName>
{
    // Mandatory entries
    type            turbulentMixingLengthFrequencyInlet;
    mixingLength    <scalar>;

    // Optional entries
    k               <word>;
    phi             <word>;

    // Inherited entries
    ...
}

where:

Property	Description	Type	Required	Default
type	Type name: turbulentMixingLengthFrequencyInlet	word	yes	-
mixingLength	Mixing length scale [m]	scalar	yes	-
phi	Name of flux field	word	no	phi
k	Name of turbulent kinetic energy field	word	no	k

The inherited entries are elaborated in:

• inletOutletFvPatchFields.H

• In the event of reverse flow, a zero-gradient condition is applied.

Further information

Tutorial:

• verticalChannel

Source code:

• turbulentMixingLengthFrequencyInlet

API:

• Foam::turbulentMixingLengthFrequencyInletFvPatchScalarField

History: Introduced in version 2.2.2