...
Once ANSYS is open, drag Fluent into the Project Schematic area.
Right click geometry and import your file. Once complete a green check mark will populate next to Geometry. Next, double click Mesh to open the Mesh editor. You should see you geometry. Right click Mesh and click Generate Mesh. With any luck, you'll get something that looks like this (this is a cross section of the volume mesh):
Some features will not be well-resolved with the default mesh settings. For instance, the Nose Cone Tip of this example model is quite jagged.
Click Mesh and open up the various subsections in settings to access different Mesh settings. Some useful global features are "Defeature Size" and "Curvature Min Size". For refining near specific features of interest, there are other tools such as "Refinement".
Once satisfied with the Mesh, minimize the Mesh Editor, right click Mesh, and click Update. You should see a green check mark in the Workbench area.
If you want to look at quantities on specific regions of the model, you'll need to set up Named Selections. To do this, go back into the Mesh Editor. Set the view to Wirerframe (see below).
To create a Named Selection, hide one side of the volume mesh wall by right clicking and selecting Hide Face. Now you can access internal faces. Hold the Control Key and select all internal faces in the group (which should all be highlighted in green), then right click anywhere, and click "Create Named Selection". If you accidentally hide a face, show all faces with Ctrl + F8, and similarly Ctrl + F9 to show all hidden bodies.
Add regions for Inlet, Outlet, and Side of Boundary regions along with the features of interest.
Right click Setup and click Edit, which will open Fluent. You'll be presented with the Fluent Launcher – allocate a good portion of your cores to the Solver to help speed up simulations (I've allocated 16 of my 24 here).
Under General, select Density-Based (for supersonic CFD; Pressure-based for subsonic).
Under Models, select your preffered model for each part of the phsyics. For high-speed CFD (Reynolds No. > 10^6), Invsicid is a strong first option to get an estimate of forces and moments. When one runs Viscous CFD, meshing becomes exponentially more important (and complex) as the boundary layer must be resolved. Turn on Energy for supersonic flow.
Ensure the fluid is Air, as an ideal gas, as shown below:
For supersonic CFD, double-click boundary conditons and set all fluid boundaries to pressure-far-field and the operating conditon (make sure they all match):
For the first iterations, use the following settings in Solution Methods:
Initialize the solution with hybrid initialization selected. Before running the solver, set up necessary residual monitors and probes of forces/moments/pressures/other quantities of interest.
