7.8.2 User Inputs

The procedure for setting up the WAVE coupling in ANSYS FLUENT is presented below.

1.   Read in the mesh file and define the models, materials, and boundary zone types.

2.   Specify the location of the WAVE data and have ANSYS FLUENT use them to generate user-defined functions for the relevant boundary conditions (using the 1D Simulation Library dialog box, shown in Figure  7.8.1).

Define $\rightarrow$ User-Defined $\rightarrow$ 1D Coupling...

Figure 7.8.1: The 1D Simulation Library Dialog Box with WAVE Selected

(a)   Select WAVE in the 1D Library drop-down list.

(b)   Specify the name of the WAVE input file in the 1D Input File Name field.

(c)   Click the Start button.

When you click Start, WAVE will start up and ANSYS FLUENT user-defined functions for each boundary in the input file will be generated.

3.   Set boundary conditions for all zones. For flow boundaries for which you are using WAVE data, select the appropriate UDFs as the conditions.

Note that you must select the same UDF for all conditions at a particular boundary zone (as shown, for example, in Figure  7.8.2); this UDF contains all of the conditions at that boundary.

Figure 7.8.2: Using WAVE Data for Boundary Conditions

4.   If you plan to continue the simulation at a later time, restarting from the final data file of the current simulation, you need to instruct both ANSYS FLUENT and WAVE how often that you want to automatically save your data. You should instruct ANSYS FLUENT to automatically save case and data files at specified intervals using the autosave feature.

Calculation Activities(Autosave Case/Data) Edit...

In addition, you should instruct WAVE as to how often it should generate its own restart files. See the WAVE User's Guide for instructions on this feature.

To use the restart feature, the time interval for writing data files must be set to the same value in both ANSYS FLUENT and WAVE. For example, if ANSYS FLUENT has set the autosave feature to 100, then WAVE must also set the restart file write frequency to 100 as well.

5.   Continue the problem setup and calculate a solution in the usual manner.