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:

Example by using the postProcess utility:

<solver> -postProcess -func wallHeatFlux

Further information

Tutorial:

$FOAM_TUTORIALS/incompressible/pisoFoam/RAS/cavity

Source code:

Foam::functionObjects::wallHeatFlux

History

Introduced in version v1606+

Table of Contents

Description

Operands

Usage

Further information