The procedure for setting up the WAVE coupling in
FLUENT is presented below.
Read in the mesh file and define the models, materials, and boundary zone types.
Specify the location of the WAVE data and have
FLUENT use them to generate user-defined functions for the relevant boundary conditions (using the
1D Simulation Library panel, shown in Figure
Figure 7.30.1: The
1D Simulation Library Panel with
WAVE in the
1D Library drop-down list.
Specify the name of the WAVE input file in the
1D Input File Name field.
When you click
Start, WAVE will start up and
FLUENT user-defined functions for each boundary in the input file will be generated.
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
7.30.2); this UDF contains all of the conditions at that boundary.
Figure 7.30.2: Using WAVE Data for Boundary Conditions
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
FLUENT and WAVE how often that you want to automatically save your data. You should instruct
FLUENT to automatically save case and data files at specified intervals using the autosave feature.
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
FLUENT and WAVE. For example, if
FLUENT has set the autosave feature to 100, then WAVE must also set the restart file write frequency to 100 as well.
Continue the problem setup and calculate a solution in the usual manner.