ANSYS

This article looks to provide an overview on ANSYS Fluent tools to analyze and optimize, the vehicle's aerodynamic performance.

Prerequisites:

An aerobody model (solidworks, step, parasolid) which can be knitted and thickened to at least 10mm (higher is better).
Lots of patience and something to kill time with as ANSYS loads and solves

CFD Overview

We want to calculate what air particles are doing around our car. Essentially we are looking to build a virtual wind tunnel and shoot air at our car to see how it reacts. To do so we must:

Geometry: Load our car aerobody CAD and define our wind tunnel dimensions
Mesh: Build an accurate mesh that represents reality
Solution: Define parameters to solve

The Process

This is ANSYS workbench. ANSYS's Fluent Module is used to perform the analysis.

0.0) Double click on "Fluid Flow "Fluent" to load the module.

ANSYS Fluent Screenshot

The module contains five parts: geometry, mesh, setup, solution and results. Each have their respective status symbol.

Up To Date: This is the goal. It indicates the step is complete and we can move on.

Unfullfilled: The previous step is incomplete and "upstream" data is missing

Attention Required: Previous step is complete, but action needs to be taken to proceed.

Update Required: Something in a previous step was changed and the step needs to be updated.

Refresh Required: For our pruposes, its the same as update required.

Our current module has everything unfulfilled and attention is required on the geometry step. Each cell must be "Up to Date" before starting the next step. If "Update Required" ever appears, simply press "Update Project".

0.1) Right click on geometry to open the Geometry Modeller (not Space Claim).

Geometry

In this step we will load in the car model and build our "wind tunnel". Additionally, since the car is symmetrical, we will slice and simulate with only half the car model and wind tunnel in half. This reduces our calculation time by over 50%!

Note that the simulation will have the air move around the car (as opposed to car moving thorugh air). For a fully accurate representation, the ground can be simulated to be moving; but this is not worth the additional complexity and solving time (the accuracy improvements is marginal).

1.1) To load the model: Click "File > Import External Geometry File", then click "Generate".

Generate Button Location

You should be able to see the model appear in the window:

We can proceed to build the wind tunnel to contain our "air" (and cut in car in half in the same step).

1.2) Click "Tools>Enclosure"

Under details view, you can select how large the wind tunnel should be by changing values of the cushion. The cushion is the shortest distance between the wall and any part of the car. Input the desired cushion values. Note that the -Y value in this case represents the cushion distance to the ground, this value will depend on the suspensions and wheels (how far the bottom of the aerobody sits away from the ground).

How to Size the Wind Tunnel?

The sizing of the wind tunnel is a challenge: if the wall cushion is too small then the "air" will interact with the wind tunnel walls and give us undesirable results, but if the wall cushion is too large it will take heavy computation time to solve the system.

From personal experience and results from other CFD specialist, it is seen that walls around 5-10 times the car dimensions is the sweet spot between acuracy and computation time (ie. if the car is 2m wide, the total cushion in the width direction is 10-20m).

In reality, the optimal cushion value will depend on many factors. For example, the area of interest: if you care about how the fluid is behaving at the front of the car, then the rear outlet wall can be placed very close. If the mesh can be manipulated to be fine around important regions and coarser in unimportant regions (such as a point far away from the rear of the car), then it may become more beneficial to have a large wind tunnel but a coarser mesh.

If many iterations are being done for aerodynamics optimization, it is worth the time to determin the best cushion values through experimentation (run the same setup with varying cushion values to see how close the walls can get before the results changes drastically).

Our car is symmetrical about the YZ plane (this may vary for other models), so a symmetry plane will be

1.3) Select "Number of Planes" to 1 and the symmetry plane to be YZPlane. Input the cushion values as seen below.

1.4) Click "Generate"

Half Wind Tunnel and Car Screenshot

Half the car and wind tunnel should appear. The car body needs to be subtracted from the fluid body (it'll be clear why during meshing).

1.5) Click "Create> Boolean". Select "Operation" as "Subtract". Select the wind tunnel and target body and car as tool body. Click "Generate"

Boolean Subtract Screenshot

Check the workbench to confirm our Geometry stage is "Up to Date".

The geometery is ready to be meshed.

1.6) 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 (many workshops and tutorials based on only meshing). This tutorial hopes to build basic intuition of proper meshing techniques specifically for vehicle aerodynamics.

Meshing and CFD Intuition

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 a network of many 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; this forces air flow to 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/receive information (such as pressure, velocity, volume or momentum) to/from adjacent nodes through the edges and update itself. For example, if a high pressure parcel is connected to a low pressure parcel, it is not in equilibrium; thus, there must be some movement (mass flow or velocity change) from the high to low pressure nodes. ANSYS will solve hundreds-thousands of these equations between nodes for thousands of iterations until a steady state is acheived. (Note: This is NOT the full story, but an easy way to imagine what's happening inside the simulation)

For the CFD technician, this means we want few nodes in locations where accuracy is insignificant and more nodes in important areas (orientated and positioned in a way to accurately simulate reality). As with all FEA, it is easy to get an accurate simulation (simply make the densest mesh possible and have it solve for three weeks); however, being proficient at CFD means being able to create a minimal mesh which keep computational time low and providing meaningful and accurate results.

You can click "Generate Mesh" and mesh based on default properties (click Show Mesh to view the mesh). This gives us a very poor mesh.

The current mesh is unacceptable: the top surface of the car only has a handful of nodes, the bottom of the car to the ground only has one row of cells and the mesh has no nodes to represent the boundary layer.

Let us improve the mesh quality to more accurately resemble reality.

2.1) 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"

Mesh Sizing Screenshot

These are the global mesh controls. These settings affect everything in our geometry. 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.

2.2) To add the inflation layer (to model the boundary layer). Expand Inflation and set "Use Automatic Inflation" to "Program Controlled"

Inflation Layer Screenshot

Or Highlight Surface of Car

Create Named Selection → label "car"

Use "All Faces in Chosen Name Selection" (vs Program Controlled) → select "car"

2.3) Click Generate Mesh.

This mesh is far better than the default settings. The bottom has enough cells to appropriately model ground effects. The mesh is denser overall to provide higher resolution and accurately represent the geometry. A boundary layer is added around the entire car.

Aside: Local Mesh Parameters

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.

2.4) Highlight and right click the front wall > "Create Named Selection". Name the face "Inlet".

Named Selection Screenshot

2.5) 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".

2.6) The mesh is complete. Go back to ANSYS workbench and double click "setup" to begin setting up boundary conditions and solution parameters.

Setup/Solution

3.1) Our computer sucks so keep settings at default and click "ok".

Fluent Launcher Screenshot

3.2) Click Model > Viscous (Laminar) Model. Select k-epsilon and Realizable.

Models Screenshot

These are different CFD models which can be used to solve the simulation. Realizable k-epsilon is the better ones for our purposes.

3.3) Edit boundary conditions for the inlet. 25m/s (90km/h) is used for this simulation.

Inlet Boundary Conditions Screenshot

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.

3.4) Select Reports>Projected Areas and highlight "car" and compute.

Projected Area Screenshot

3.5) Go to "Reference Value" and replace the "Area" with the car frontal area and "Velocity" with the inlet velocity.

Reference Values Screenshot

3.6) "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.

Solution > Report Definitions > Drag

Drag Monitor Screenshot

3.7) Start the simulation: Go to "Run Calculation" and set number of iterations to around 1000. Click "Calculate" and press "Yes".

Run Calculation Screenshot

The simulation will begin to solve. We will wait for the solution to converge. If the solution hasn't converged by the end of the 1000 iterations, simply add more iterations.

Solving and Converged Screenshot

Post Processing

This stage is where we look at out results. What is possible?

Graphical or plots are availible for airflow, pressure, forces, etc.

Results → Reports → Forces → Direction Vector (in direction of air movement) → Print

Graphics → Pathlines → More Steps = Longer Line (500 - 2000) → Make sure to start with some path skips (i.e. 20) and lower as needed

Select Options → Draw Mesh (to see mesh) with path lines (select car)

You can view pathlines for entire car or for a specific line

Line/Rake → select endpoints for line

If you ever lose track of the model, use this button to zoom back to default.