To obtain a report of mass flow rate, total heat transfer rate, total sensible heat transfer rate, or radiation heat transfer rate on selected boundary zones, use the Flux Reports Dialog Box (Figure 32.19: The Flux Reports Dialog Box).
Results → Reports → Fluxes
Edit...
The steps for generating the report are as follows:
Specify which flux computation you are interested in by selecting one of the following under Options:
Mass Flow Rate
Total Heat Transfer Rate
Total Sensible Heat Transfer Rate
Radiation Heat Transfer Rate
Film Mass Flow Rate (available as an option only when the Eulerian Wall Film model is enabled—see Modeling Eulerian Wall Films)
Film Heat Transfer Rate (available as an option only when the Eulerian Wall Film model is enabled—see Modeling Eulerian Wall Films)
In the Boundaries list, choose the boundary zone(s) on which you want to report fluxes.
You can use Filter Text entry box to filter the Boundaries list to show only the boundary zones that match the pattern you enter. For additional information on using the Filter Text entry box, see Filter Text Entry Boxes.
To create an output parameter for the reported value, click Save Output Parameter.... The Save Output Parameter Dialog Box (Figure 32.20: The Save Output Parameter Dialog Box) will open where you will specify the name of the newly created output parameter, or overwrite an existing output parameter of the same type. ANSYS Fluent automatically creates generic default names for new input and output parameters (for example, parameter-1, parameter-2, and so on).
After the output parameter is created, it is listed in the Parameters Dialog Box, accessed via the Parameters... button in the Reports Task Page. You can create any number of output parameters of this report type.
Note: If you create an output parameter from a flux report and save the case and data (write), an equivalent report definition will be created when you read in the case file.
Click the Compute button to display the results of the selected flux computation for each selected boundary zone. The Net Results field will show the summation of the individual zone flux results.
Important: Additional steps must be taken prior to generating a flux report for an interior boundary zone that has the same fluid defined on either side. In such a case, the area vectors of the cell faces associated with the zone may have been automatically defined in an inconsistent manner when the mesh file was read into the solver. Since the flux for each individual cell face is calculated with respect to its area vector, such an inconsistency leads to inaccurate results when the face fluxes are summed to calculate the total flux of the boundary zone.
To ensure accurate flux results for such an interior zone, you must orient the area vectors by changing the definition of the zone Type to wall. You should then change the Type back to interior and proceed to generate the flux report.
Note that the fluxes are reported exactly as computed by the solver. Therefore, they are inherently more accurate than those computed with the Flow Rate option in the Surface Integrals Dialog Box (described in Surface Integration).