Example: Vehicle Aerodynamics

Example: Vehicle Aerodynamics#

This example demonstrates a complete external aerodynamics workflow — meshing and simulating airflow around a car to calculate drag and lift coefficients and visualize the flow field.

Objective#

  • Generate a mesh around a car geometry with boundary layers

  • Run a RANS simulation at highway speed (30 m/s / ~110 km/h)

  • Calculate drag coefficient (Cd) and lift coefficient (Cl)

  • Visualize pressure distribution, wake structure, and streamlines

Step 1: Create a Meshing Project#

  1. Dashboard → New Project → Meshing

  2. Name: “Car Aerodynamics”

  3. Upload your car geometry file (STEP format recommended)

Step 2: Geometry Check#

Navigate to the Geometry tab and run analysis:

  • Verify the geometry is watertight (no gaps)

  • Check for manifold issues

  • If using STL, run vertex welding to clean up any gaps

Tip

If your car model has open wheel arches or an open underbody, the mesher will struggle. Ensure the geometry is a closed, solid body. The AI Assistant can help identify and fix issues.

Step 3: Domain Configuration#

In the Setup tab:

  1. Select External Flow domain type

  2. Enable Ground Plane — the car should sit on a flat surface

  3. Configure the wind tunnel dimensions:

Parameter

Value

Reasoning

Upstream

1.5× car length

Allow flow to develop before reaching the car

Downstream

3.0× car length

Capture the full wake structure

Sides

1.5× car width

Avoid blockage effects

Top

2.0× car height

Allow flow over the roof to develop

Bottom

0 (ground plane)

Car sits on the ground

Step 4: Refinement Zones#

Add refinement zones to capture key flow features:

Wake Zone#

  • Shape: Box

  • Position: Behind the car, extending 2× car length downstream

  • Width: 1.5× car width

  • Height: 1.5× car height

  • Cell size: 2× finer than base mesh

Underbody Zone#

  • Shape: Box (flat)

  • Position: Under the car, from bumper to bumper

  • Height: Ground to car floor + 0.1 m

  • Cell size: 2× finer than base mesh

Wheel Zones (if applicable)#

  • Shape: Cylinder

  • Position: Around each wheel

  • Radius: 1.5× wheel radius

  • Cell size: 3× finer than base mesh

Step 5: Surface Naming#

In the Surfaces tab, name key boundaries:

Surface

Name

Type

Car body

car_body

Wall

Front wheels

wheel_front

Wall (or rotating wall)

Rear wheels

wheel_rear

Wall (or rotating wall)

Wind tunnel inlet

inlet

Inlet

Wind tunnel outlet

outlet

Outlet

Ground

ground

Moving wall

Top

top

Slip wall

Sides

side_left, side_right

Slip wall

Step 6: Mesh Settings#

Parameter

Value

Target cell size

0.1 m (for a ~4.5 m car)

Min cell size

0.005 m

Refinement levels

8

Boundary layers

Enabled

Number of layers

10

First layer height

0.001 m (y+ ≈ 30)

Growth rate

1.2

Step 7: Generate Mesh#

Click Generate Mesh and wait for completion. Typical cell counts:

Resolution

Approximate Cells

Coarse

2 – 5 million

Medium

5 – 15 million

Fine

15 – 50 million

Check mesh quality in the Mesh Quality tab. Target:

  • Skewness < 0.85

  • Non-orthogonality < 70°

Step 8: Create a CFD Project#

  1. Return to Dashboard → New Project → CFD

  2. Name: “Car CFD”

  3. Select the mesh from your meshing project

Step 9: Simulation Setup#

In the Simulation tab:

Setting

Value

Turbulence model

k-ω SST

Inlet velocity

30 m/s (X-direction)

Outlet pressure

0 Pa

Car body

No-slip wall

Ground

Moving wall (30 m/s in X)

Top, sides

Slip wall

Turbulence intensity

1%

Max iterations

1000

Ground Boundary Condition

For vehicle aerodynamics, the ground must be a moving wall at the same speed as the freestream. This simulates the car moving through still air, rather than air blowing over a stationary car on a stationary floor (which would create an unrealistic ground boundary layer).

Step 10: Run and Monitor#

  1. Click Run Simulation and confirm

  2. Monitor the residual plot — look for all residuals dropping below 1e-4

  3. Check the logs for any warnings

A typical vehicle RANS simulation converges in 300–800 iterations.

Step 11: Results Analysis#

Drag and Lift Coefficients#

  1. In the Results tab, click Forces

  2. Select the car_body surface

  3. Set reference values:

    • Reference velocity: 30 m/s

    • Reference area: Frontal area of the car (approximately width × height, e.g., 2.2 m²)

  4. Read off Cd and Cl

Vehicle Type

Expected Cd Range

Sedan

0.25 – 0.35

SUV

0.35 – 0.45

Sports car

0.28 – 0.35

Truck / Box shape

0.6 – 0.8

Pressure Distribution#

  1. Select Pressure field

  2. Enable surface coloring on car_body

  3. Look for:

    • High pressure (red) at the front stagnation point

    • Low pressure (blue) on the roof and sides where flow accelerates

    • Pressure recovery toward the rear

Wake Visualization#

  1. Add a slice plane at Y = 0 (centerline) colored by velocity magnitude

  2. The wake behind the car appears as a low-velocity region

  3. Add streamlines seeded from the inlet to see flow paths around the car

Underbody Flow#

  1. Add a horizontal slice plane at the underbody height

  2. Color by velocity to see flow acceleration under the car

  3. This reveals ground effect patterns

Using the AI Assistant#

You can set up this entire example through conversation:

You: “I’ve uploaded a sedan CAD file. Set up an external aero mesh for highway speed analysis.”

Assistant: Analyzes geometry dimensions, suggests domain box, recommends mesh settings, boundary layers, and refinement zones. Presents configuration for your approval.

You: “Run a simulation at 30 m/s with k-omega SST”

Assistant: Configures boundary conditions, sets inlet velocity, applies moving ground, and runs the simulation with your confirmation.

You: “What’s the drag coefficient?”

Assistant: Calculates forces on the car body surface and reports Cd and Cl.

Contents