This boundary condition provides a temperatue interface to an external application. More...

#include <externalCoupledTemperatureMixedFvPatchScalarField.H>

Detailed Description

This boundary condition provides a temperatue interface to an external application.

Values are transferred as plain text files, where OpenFOAM data are written as follows:

    # Patch: <patch name>
    <magSf1> <value1> <qDot1> <htc1>
    <magSf2> <value2> <qDot2> <htc2>
    <magSf3> <value3> <qDot3> <htc2>
    ...
    <magSfN> <valueN> <qDotN> <htcN>

and received as the constituent pieces of the `mixed' condition, i.e.

    # Patch: <patch name>
    <value1> <gradient1> <valueFracion1>
    <value2> <gradient2> <valueFracion2>
    <value3> <gradient3> <valueFracion3>
    ...
    <valueN> <gradientN> <valueFracionN>

Data is sent/received as a single file for all patches from the directory

    $FOAM_CASE/<commsDir>

At start-up, the boundary creates a lock file, i.e..

    OpenFOAM.lock

... to signal the external source to wait. During the boundary condition update, boundary values are written to file, e.g.

    <fileName>.out

The lock file is then removed, instructing the external source to take control of the program execution. When ready, the external program should create the return values, e.g. to file

    <fileName>.in

... and then reinstate the lock file. The boundary condition will then read the return values, and pass program execution back to OpenFOAM.

To be used in combination with the functionObjects::externalCoupled functionObject.

Usage

Property	Description	Required	Default
`outputTemperature`	Output temperature: fluid/wall	yes
`htcRefTemperature`	Fluid temperature for htc: cell/user	no	cell
`Tref`	Reference temperature [K] for htc	conditional

The user-specified reference temperature Tref is specified as a Foam::Function1 of time but spatially uniform.

See also: externalCoupledFunctionObject mixedFvPatchField externalCoupledMixedFvPatchField

Source files

*/

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

namespace Foam {

/*—————————————————————————*\ Class externalCoupledTemperatureMixedFvPatchScalarField Declaration \*—————————————————————————

The documentation for this class was generated from the following file:

src/functionObjects/field/externalCoupled/externalCoupledTemperatureMixed/externalCoupledTemperatureMixedFvPatchScalarField.H