[kiski]

Hi,


In simple boundary values, such as fixedValue "value" parameter is well explained even in documentation (for example, command `foamInfo fixedValue` reports its usage).


But in less standard ones information is missing and is sometimes even not consistent. For example, `foamInfo pressureDirectedInletOutletVelocity` reports

...
Usage
\table
Property | Description | Required | Default value
phi | flux field name | no | phi
rho | density field name | no | rho
inletDirection | inlet direction per patch face | yes |
\endtable

Example of the boundary condition specification:
\verbatim
<patchName>
{
type pressureDirectedInletOutletVelocity;
phi phi;
rho rho;
inletDirection uniform (1 0 0);
value uniform 0;
}
\endverbatim
...

Here "value" is not reported, and when using it, it actually requires a vector or it complains, i.e. "value (0 1 0);" The example given in the documentation itself is not working.


The question is, for given pressureDirectedInletOutletVelocity example, what is value doing? I am not able to figure it out from code. Too hard for me. Also, is there any other source of information where I can find this info for other boundaries?

Thank you for your help

[GerhardHolzinger]

The value parameter is part of one of the very base classes of the boundary conditions. So, most boundary conditions inherit it from their ancestry.
However, the more complex classes have no particular use for this parameter, as they compute the boundary value. Thus, the user-provided value value is ignored.

The placeholder comment in some header-descriptions of BCs is an indication.

Class
    Foam::turbulentIntensityKineticEnergyInletFvPatchScalarField

Description
    This boundary condition provides a turbulent kinetic energy condition,
    based on user-supplied turbulence intensity, defined as a fraction of the
    mean velocity:

        \f[
            k_p = 1.5 (I |U|)^2
        \f]

    where

    \vartable
        k_p     | kinetic energy at the patch
        I       | turbulence intensity
        U       | velocity field
    \endvartable

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

Usage
    \table
        Property     | Description             | Required    | Default value
        intensity    | fraction of mean field [0-1] | yes    |
        U            | velocity field name     | no          | U
        phi          | flux field name         | no          | phi
    \endtable

    Example of the boundary condition specification:
    \verbatim
    <patchName>
    {
        type        turbulentIntensityKineticEnergyInlet;
        intensity   0.05;           // 5% turbulence
        value       uniform 1;      // placeholder
    }
    \endverbatim

See also
    Foam::inletOutletFvPatchField

SourceFiles
    turbulentIntensityKineticEnergyInletFvPatchScalarField.C

[kiski]

Thank you for your answer. I just realized that in some of such advanced conditions, the value value is used for initialization, and then ignored I guess.


Cheers