Human-Powered Vehicle Fairing CFD Analysis
Human-Powered Vehicle Fairing CFD Analysis
Embedded Files
SolidWorks | ANSYS Fluent | Computational Fluid Dynamics
SolidWorks | ANSYS Fluent | Computational Fluid Dynamics
Working on Cal Poly's Human Powered Vehicles Fairing team, I developed a CFD workflow to evaluate the aerodynamic performance of the vehicle fairing and identify opportunities for reducing drag. The workflow uses SolidWorks for fairing geometry development and ANSYS Fluent for meshing, flow simulation, and aerodynamic analysis.
The current simulation establishes a baseline design and CFD methodology that will be used to guide future fairing iterations.
Engineering Objective
Engineering Objective
The objective of the fairing is to reduce aerodynamic drag while maintaining the packaging, visibility, ground-clearance, and manufacturing constraints of the human-powered vehicle.
CFD was used to evaluate the baseline geometry, identify high-drag and separated-flow regions, and determine which areas of the fairing should be modified in future CAD iterations.
CFD Workflow
CFD Workflow
SolidWorks CAD → CFD Domain → Mesh → Fluent Solution → Flow Analysis → CAD Revision
SolidWorks CAD → CFD Domain → Mesh → Fluent Solution → Flow Analysis → CAD Revision
Simulation Setup
Simulation Setup
As seen in the image, the simulation is set up such that the flow enters in the negative x-direction towards the nose of the fairing, exiting towards the pressure outlet. The plane facing towards the screen in the image splits the fairing directly in half, reducing mesh and simulation processing time. This is a reasonable simplification since the fairing is symmetric about this plane, and there are single-line, zero-yaw conditions assumed during the race. The fairing's wheels sit slightly below the ground to model tire deformation while the fairing hits its top speed. Lastly, the ground in the simulation is set to move at the same speed as the velocity inlet. This correctly represents the relative motion between the vehicle and road and prevents an artificial boundary layer from developing.
Mesh Strategy
Mesh Strategy
The mesh was created such that both aerodynamic accuracy and computation time are reasonable due to repeated geometry iterations. Local refinement was added to the fairing and wheel surfaces to improve mesh quality. The current mesh contains around 1 million cells, providing a reasonable baseline for CAD iteration.
Mesh quality was evaluated using orthogonal quality, skewness, and wall y+. The overall mesh quality is acceptable, yet several regions could use improvement, specifically in near-wall resolution and maximum skewness. Future design goals include conducting a mesh independence study to improve simulation accuracy and consistency.
A mesh independence study was conducted to ensure reliable CFD results throughout CAD iteration. Four progressively refined meshes: fine (M1), medium (M2), coarse (M3), and extra-coarse (M4) were generated using scaled surface, volume, and boundary-layer mesh settings, ranging from 1.48 to 5.05 million cells. Richardson extrapolation and the Grid Convergence Index (GCI) method were used to evaluate discretization uncertainty by comparing drag and lift coefficients against estimates for an infinitely fine mesh. Results showed that drag coefficients became increasingly consistent with refinement, with only a 1.1% difference between the medium and fine meshes, while lift coefficients differed by less than 0.1%. Across all four meshes, lift coefficients varied by less than 0.3%, indicating lower sensitivity to mesh resolution. These results provided a quantitative basis for evaluating the tradeoff between computational cost and accuracy during subsequent CAD iterations.
Simulation
Simulation
The simulation was run using the SST k-omega RANS turbulence model, with a no-slip boundary condition on the fairing and ground. The ground was set to a moving wall with the same velocity as the inlet, and the following reference values were used for the simulation:
The simulation was run using the SST k-omega RANS turbulence model, with a no-slip boundary condition on the fairing and ground. The ground was set to a moving wall with the same velocity as the inlet, and the following reference values were used for the simulation:
The simulation was initialized and then run until convergence, where the drag coefficient was also stabilized:
The simulation was initialized and then run until convergence, where the drag coefficient was also stabilized:
Residuals
Residuals
The residuals of continuity, x-velocity, y-velocity, z-velocity, k, and omega converged after 83 iterations, as shown in the next image.
Convergence
Convergence
This simulation ran over 83 iterations before the residuals converged on the final solution based on both residual and output parameter set convergence criteria.
Drag Coefficient
Drag Coefficient
This plot shows the drag coefficient over the 83 iterations, becoming approximately constant around 35 iterations. A convergence criteria of 1E-6 for drag coefficient was set and monitored throughout the simulation to ensure the solution was reletively reliable and not only dependent on residual convergence.
y+
y+
To confirm the inflation layers were correctly applied and ensure a reletively accurate representation of skin friction, the y+ was checked along the fairing body. The goal was to ensure y+ <5 which is where SST-k-omega can successfully model near wall effects. This was achieved as shown in the plot with y+ <2.5.
CFD Results
CFD Results
Once reaching convergence, the final drag force and coefficient were obtained as seen in the image above. Along with this, the following graphics were produced to understand our geometry:
Velocity Magnitude Contour
Velocity Magnitude Contour
The solution identifies the low-velocity wake behind the fairing and regions of accelerated flow around the upper surface.
Static Pressure Contour
Static Pressure Contour
High pressure at the nose transitions into lower-pressure regions along the fairing, allowing pressure recovery and potential separation to be evaluated.
Velocity Streamlines
Velocity Streamlines
Streamlines were used to evaluate flow attachment and identify regions where geometry changes may reduce separation.
CFD-Driven Design Findings
CFD-Driven Design Findings
The baseline CFD solution was used to identify areas of the fairing that have the greatest potential for aerodynamic improvement. Velocity, pressure, and streamline results were evaluated for flow separation, wake development, and pressure recovery.
Future geometry changes will focus on rear taper, wheel fairing transitions, and wake reduction while maintaining the packaging and manufacturing constraints.
Studies
Studies
After creating this baseline method for meshing and simulation, various geometry studies were conducted and more will continue to be conducted as we reach a finalized fairing desig. Click the links below to see their results:
Next Steps
Next Steps
Future work will focus on further reducing aerodynamic drag through continued CAD iteration and CFD analysis. The vehicle model is being refined using 3D scans of the riders, chassis, and drivetrain components to better represent the final vehicle geometry. Incorporating these details will allow for more realistic simulations and help identify additional opportunities to reduce drag through fairing modifications, improved component integration, and optimized airflow around the vehicle.
Page updated
Google Sites
Report abuse