wallHeatFlux

Description

The wallHeatFlux function object computes the wall-heat flux at selected wall patches.

Operands

Operand	Type	Location
input	-	-
output file	dat	$FOAM_CASE/postProcessing/<FO>/<time>/<field>
output field	volScalarField (only boundaryField)	$FOAM_CASE/<time>/<outField>

Usage

Example of the wallHeatFlux function object by using functions sub-dictionary in system/controlDict file:

wallHeatFlux1
{
    // Mandatory entries (unmodifiable)
    type            wallHeatFlux;
    libs            (fieldFunctionObjects);

    // Optional entries (runtime modifiable)
    patches     (<patch1> ... <patchN>); // (wall1 "(wall2|wall3)");
    qr          qr;

    // Optional (inherited) entries
    writePrecision  8;
    writeToFile     true;
    useUserTime     true;
    region          region0;
    enabled         true;
    log             true;
    timeStart       0;
    timeEnd         1000;
    executeControl  timeStep;
    executeInterval 1;
    writeControl    timeStep;
    writeInterval   1;
}

where the entries mean:

Property	Description	Type	Required	Default
type	Type name: wallHeatFlux	word	yes	-
libs	Library name: fieldFunctionObjects	word	yes	-
patches	Names of operand patches	wordList	no	all wall patches
qr	Name of radiative heat flux field	word	no	qr

The inherited entries are elaborated in:

• functionObject
• writeFile

Example by using the postProcess utility:

<solver> -postProcess -func wallHeatFlux

Stored properties

Reduced data

The following data are stored by the function object, and can be used by other function objects:

• min(<patch-name>) : minimum patch value
• max(<patch-name>) : maximum patch value
• int(<patch-name>) : integral patch value

Further information

Tutorial:

• cavity

Source code:

• Foam::functionObjects::wallHeatFlux

API:

• wallHeatFlux

History: Introduced in version v1606+