This article looks to provide an overview on ANSYS Fluent and its tools to analyze , as well as and optimize, the vehicle's aerodynamic performance.
...
Select "Number of Planes" to 1 and the symmetry plane to be YZPlane. Input the cushion values as seen below.
Click "Generate"
Half the car and wind tunnel should appear. The car body must be subtracted rom the fluid body.
Click "Tools> Boolean". Select "Operation" as "Subtract". Select the wind tunnel and target body and car as tool body. Click "Generate"
Check the workbench to confirm our Geometry stage is "Up to Date".
The geometery is ready to be meshed.
Double click "Mesh" to open Meshing
Meshing
This is the most critical step in the entire process. Building accurate meshes is a massive topic of study. This tutorial hopes to build some intuition of proper meshing techniques specifically for vehicle aerodynamics.
Immeadiately, you can click "Generate Mesh" and build from default properties. This gives us a very poor mesh.
Meshing Intuition: In general, all finite element techniques looks to break down a difficult problem into smaller simpler parts (each part is a "finite element"). Instead of analyzing flow on the entire tunnel at once, the problem is divided into many air parcels connected to other air parcels. Each air parcel is represented as a node on the mesh, and every connection between parcels is an edge between nodes. Notice no nodes inside the car shaped cavity; air flow goes through edges around the car (which is why the car model is subtracted from the fluid model).
Later we will define some nodes to have boundary conditions (ie. the wind tunnel inlet nodes have set velocity and car surface nodes are static walls). When solving begins every node will send and receive information (such as pressure, velocity, volume, momentum, etc.) to and from adjacent nodes through the edges and update itself. ANSYS will solve hundreds-thousands of these equations between nodes for thousands of iterations until a steady state is acheived.
For the CFD technician, this means we want few nodes in locations where accuracy is insignificant and more nodes in important areas to accurately simulate reality while keeping computation time low. As with all FEA, it is easy to get an accurate simulation (simply make the densest mesh possible); however, the computation time would be impossibly long.
The current mesh is unacceptable: the top surface of the car only has a couple of nodes, the bottom of the car to the ground only has one row of nodes and the mesh has no nodes to represent the boundary layer.
Click "Mesh" in the sidebar and expand "Sizing". Change "Advanced Size Function" to "On: Proximity and Curvature". Change "Smoothing" to "High". Change "Num Cells Across Gap" to "5-10"
These are the global mesh controls. They affect everything. Advanced Size Function (On: Proximity and Curvature) is chosen as we want the car's curvature to be accurately represented; as the car is a thickened surface, the proximity portion prevents undesirable geometry. Actual sizing is useful as well, but requires more experimentation to get the best sizing.
To add the inflation layer (to model the boundary layer). Expand Inflation and set "Use Automatic Inflation" to "Program Controlled"
Click Generate Mesh.
This mesh is far better. The bottom has enough cells to appropriately model ground effects. The mesh is denser overall. A boundary layer is added around the entire car.
Bonus: If the model has detailed geometry (ie, small fairings, door detailings, etc.) local meshing controls are handy. To manipulate mesh quality, right click mesh> insert >sizing, then select the geometry you wish the sizing settings to apply to). There is no rule of thumb.
To finish, the mesh components must be labelled.
Highlight and right click the front wall > "Create Named Selection". Name this face "Inlet".
Repeat the process. The wall behind the car is "outlet". The car cavity is "car". The symmetry plane "symmetry". The remaining three walls are "walls".
The mesh is complete. Go back to ANSYS workbench and double click "setup"
Setup/Solution
...
Our computer sucks so keep settings at default and click "ok".
Click Model > Viscous (Laminar) Model. Select k-epsilon and Realizable.
These are different CFD models which can be used to solve the simulation. Realizable k-epsilon is the better ones for our purposes.
Edit boundary conditions for the inlet. 25m/s (90km/h) is used for this simulation.
ANSYS matches named selection to boundary conditions and everything else is already defined by default. A choice can be made for the road wall to be "moving" for the most accurate simulation; however, that is not a major concern for precision.
Next, the projected area of the car is required for the simulation to compute an accurate drag coefficient. If the frontal projected area is already known, the next step can be skipped.
Select Reports>Projected Areas and highlight "car" and compute.
| Expand | ||
|---|---|---|
| ||
 |
Go to "Reference Value" and replace the "Area" with the car frontal area and "Velocity" with the inlet velocity.
| Expand | ||
|---|---|---|
| ||
 |
"Monitors". Here we can add various values to monitor. For this simulation, only the drag coeffient is relevant (we may look at lift/downforce in other simulations).
Click Create>drag. Highlight car and click "OK". Ensure the force vector is pointing in same direction of the car.
Start the simulation: Go to "Run Calculation" and set number of iterations to around 1000. Click "Calculate" and press "Yes".
The simulation will begin to solve. We can cancel at anytime we believe we've hit steady state (when the values converge and graph is horizontal). If the solution hasn't converged by the end of the 1000 iterations, simply add more iterations.
Post Processing
This stage is where we look at out results. What is possible?
Graphical or plots are availible for airflow, pressure, forces, etc.
If you ever lose track of the model, use this button to zoom back to default.
