Surface Cleanup Wind-Tunnel Setup and CFD Simulation of a Formula-SAE Car Running Over Two Different Tracks

The objective of this project is to perform surface cleanup, boundary flagging, virtual wind tunnel setup, pre-processing, CFD simulation and post-processing of a Formula - SAE Car below, the .STL of which was provided. The project has been divided into two phases:

• Surface Cleanup, Boundary Flagging and Virtual Wind Tunnel Setup
• Pre-Processing or Case Setup
• Post-Processing and Study of Flow Processes Around the FSAE Car

INTRODUCTION:The Formula-SAE car shown above falls under the category of Open-Wheel Race Cars. This vehicle has four exposed wheels that create a lot of drag, a narrow body which does not have an under-body tunnel except the upward bent plate at the rear, but still, the venturi effect produced is nowhere near to an Indy Car. It also has two large wings mounted at the front and rear that generate aerodynamic downforce. The role of aerodynamics in race-cars is to generate downforce and drag wherever necessary and thus help improve vehicle performance. Each and every part of the body is designed to enhance its aerodynamic performance save for the four exposed wheels which lead to separated flows behind them.

The study aims to perform CFD simulation for a Suspension Team of a racing company which needs data on the downforce generated by individual components using a software tool known as Converge and later post-processing it in Paraview. Using this data, the team would decide on the suspension spring stiffness, the types of tyres to be used, improvement of design of suspension control arms and focus on placing center of gravity behind center of pressure to make the car more stable. The company has two races in the upcoming season which have the following track conditions:

Race-1 

• Racing track conditions - Lot of turns
• Average lap speeds - 45kmph
• 70% turns at 45 degrees
• 20% turns at 80 degrees
• 10% turns at 20 degrees

Race-2

• Racing track conditions - Straights
• Average lap speed - 75kmph

Each of these race tracks require different aerodynamic design for the car to work well under and thus the objective has been to generate sufficient downforce and less drag for both the races. The first race has turns of varying degrees and for the tyres to work on the limit of friction ellipse, it is imperative that sufficient downforce be generated at such a speed. How vehicle performance is related to aerodynamics is a topic that has been discussed in the post-processing phase. For the second race, drag minimisation is the number one target.

PHASE I : SURFACE CLEANUP, BOUNDARY FLAGGING AND VIRTUAL WIND-TUNNEL SETUP

• Surface Cleanup: A diagnosis was first run on the .STL file of the FSAE car to check for errors. As seen below, the geometry had 48 Non-Manifold Problems. This error exists when a single edge on the geometry is being shared by more than two triangles. CONVERGE highlighted the problem areas in purple.

1) The first Non-Manifold error was on the triangles situated between the rear wing and air intake area. This section had 12 non-manifold problems. Using Delete and Patch tool the error was resolved.

2) The second non-manifold error occured just behind the air intake triangles as highlighted below. This section had 32 non-manifold errors. Since this portion had the most errors \'show w/nbr\' option had to be used to hide the entire body and only display the errors. This made it easier to resolve errors.

3) The third error was presented between the mounting of the rear wings as shown below. There were 6 Non-Manifold errors that had to be resolved.

•Boundary Flagging: With all the errors resolved the next step was to flag the appropriate boundaries on the car. The objective here was to calculate downforce on individual components which posed a challenge because of the complexity of the geometry. A tool known as Fences was utilised to accomplish this. The rear wing was first flagged. This was made possible by creating fences around the mounting of the wings whose triangles were then selected through boundary fences. The second step was to flag the front and rear wheels individually. In order to achieve this, the interface of suspension links and tie rod to the wheels was fenced thus enabling easier selection of the boundary fences. Next, underbody was flagged, this was simple since the entire surface is almost flat and only angle selection method had to be used. The suspension links were flagged by first flagging the body of the car to a new boundary, cleaning up all the fences and then reconstructing them using existing boundaries. Again, using Boundary Fence Triangle selection method, each side of the links were flagged. The front wing was simple to flag since its fences were created just at the body and wing interface. The human was also flaggged separately. This completed the second portion of the phase.

•Virtual Wind-Tunnel Setup: For setting up the wind-tunnel, there are a number of factors that need to be kept in mind. The length of the wind tunnel in front of the car where the flow comes in needs to be such that the boundary layer forms uninterruptedly. The formation shouldn\'t get disturbed by the car. For setting up the wind tunnel which extends all the way from rear of the car to the outflow, the length needs to be such that the wake region doesn\'t interact with the outflow boundary. If the wake region interacts with the the outflow, the pressure will then have to return to atmospheric leading to under-predictions in the wake region. The outflow boundary should also be located such that the pressure returns to atmoshpheric. The width of the tunnel is kept equal to the width of the car on each of the sides whereas the height of the tunnel is kept equal to the length of the car.

PHASE II : CASE SETUP OR PRE PROCESSING With the wind-tunnel setup, boundaries flagged and errors resolved, the next step was to proceed with pre-processing. This stage involved choosing Simulation parameters, setting appropriate Boundary conditions to the assigned boundaries, initializing regions, selecting the right turbulence model, choosing grid size and finally selecting the number of files and variables to post-process.

• Run Parameters: Transient solver with Full-Hydrodynamic mode was chosen.
• Simulation Time Parameters: The end time was chosen as ~`2` times one flow through time. One flow through time is `32.5/12.5 = 2.6 s` and end time is thus chosen as `5.2` seconds for Lots of Turns Track. Whereas for straight track, the end time was chosen as `3.12` seconds based on one flow through time `32.5/20.83 = 1.56 s`.
• Regions and Initialisation: Inlet velocity is also specified here. Temperature is taken as 300K and Pressure as 101325 Pascals. `O_2` with a concentration of `0.23` and `N_2` with a concentration of `0.77` is pulled inside the region. If the velocity is only specified at the inlet and not inside the regions, the solver will take a longer time to run the simulation and compute the velocity and pressure at each cell when the simulation progresses.
• Turbulence Model: Turbulence modelling tries to represent Reynolds stresses in terms of time-averaged velocity components. The common turbulence models are classified on the basis of the number of additional transport equations that need to be seloved along with the RANS equations. For the purpose of this project, Standard `k-omega` model is chosen which solves two extra transport equations to resolve the Reynolds stress tensor. This model is an improvement over the existing `k-epsilon` turbulence model and it addresses some of the key disadvantages associated with `k-epsilon`: Poor predictions for swirling & rotating flows and flows with strong separation, two of the key flow characteristics associated with FSAE car. Moreover, `k-omega` models have an enhanced wall treatment or an Automatic Wall Function. What this does is give a good range of `Y^+` values. `Y^+` is not constant throughout the car but varies at different locations. This is pertaining to the fact that there are many regions where stagnation or suction peak occur and other regions where the velocity is in between these two. These lead to differing values of `Y^+` over the entire geometry. What the chosen turbulence model does is resolve `Y^+` in the range of `0.5-300`. Where Y+ is between 30-100 or in the turbulence, it solves a different set of equations and where Y+ falls below 10 or even below 1 it uses enhanced wall treatment.

• Grid Control: The base grid size is chosen based on the wall-spacing values calculated by taking a desired `Y^+` value. These computations are based on flat-plate boundary layer theory. The inputs required are free-stream velocity, density, characteristic length, desired `Y^+` and dynamic viscosity:http://www.pointwise.com/yplus/ . The following equations are used to arrive at the wall spacing value:

1. Reynolds Number `R_e = (rho*V*L)/mu`.     
2. Skin Friction Co-efficient: It is a non-dimensional number indicating the level of friction between ahmed body and air. `C_f = 0.026/((R_e)^0.142)`.
3. Wall Shear-Stress: It is the surface shear force/unit surface and is given as `tau_w = (C_f*rho*V^2)/2`.
4. Friction Velocity: It gives the rate of increase of turbulent boundary layer. `U_f = (tau_w/rho)^0.2`
5. Wall Spacing, `y = (Y^+*mu)/(U_f*rho)`

Based on these calculations, wall spacing came out to be 0.55 mm for straight track case and 0.89mm for lots of turns track case. Having such a fine grid will lead to the simulation running indefinitely. Since, this mesh size is only required at the FSAE car, so a top-down approach was used to arrive at the values of base grid where the cell would be stretched by 50% in X and Y direction. Thus for the straight track a base mesh of `0.035 m` was taken across Z and `0.035*1.5 = 0.0528 m` across X and Y. Whereas, for lots of turns the base mesh was chosen as `0.057 m` across Z and `0.057*1.5 = 0.085 m` across X and Y.

To get to the desired mesh size boundary embedding was done on the car. Also, a box embedding was created around the car whose length would be `2*2.5 = 5 m`, `2.5 m` being the length of car along X. This embedding is provided to capture the physics of the wake region. Wake regions are characterized by low pressures and have very less drag. Having a very large wake region could lead to the trailing car utilizing the less drag and overtaking the car in front. 

Phase III: Post-Processing and Visualisation: The key objectives of this phase is to obtain lift and drag force on every component of the car using the pressure force plots, obtain velocity and pressure contours to visualise the flow around the car and visualise wake structure at the rear end of the body.

→Calculation of Lift and Drag Force for Straight Track Using Paraview:

Drag force acts parallel to the wind flow and opposes the relative motion of the object. A high drag force is an undesirable phenomenon that can lead to the car working to overcome the drag force thus ending up spending fuel.The aerodynamic design of a car is a very big contributor to how much the drag force would oppose the motion of the object. Drag Co-efficient, which is normalized using the drag force gives an indication of how much aerodynamic a certain object is. Drag Co-efficient is calculated as:

`C_d= (2*F_d)/(rho*V^2*A)`,  

`C_d` is the drag coefficient,
`F_d` is the drag force
`rho` is density of the fluid in which the object is moving
`V`    is freestream velocity
`A`    is Frontal Area of the object

Lift force acts perpendicular to the wind flow and is what helps to generate downforce on an object. Cars, on the other hand, are designed in such a way that they produce a negative lift or downforce. This negative lift force helps the car to maintain contact with ground surface even at very high speeds. The lift coefficient is normalized using the lift force formula:                                        

`C_l = (2*L)/(rho*V^2*A)`,

`C_l` is the lift co-efficient

`L` is the lift force

The lift and drag forces and the frontal area of the body were computed using a post-processing tool known as Paraview. For doing this, the first thing that needs to be done is convert the post-processed files using Ensight. A test.case file is generated which can be opened using paraview. Next, the steps below should be followed:

1) Go to \'Filters\' and select \'Extract Block\'. Choose Ahmed Body and Ahmed Body Wheels as the the blocks since this is where lift and drag co-efficients will be calculated.

2) Next, the surface needs to be extracted from the generated block so that normals can be generated. To do this, go to \'Filters\', select \'Extract Surface\' and then click on Apply.

3) After the surface has been generated, the next thing would be to generate surface normals using which drag and lift will be calculated. Again, go to \'Filters\', select \'Generate Surface Normals\' and then check the box \'Compute Cell Normals\'.

4) To compute Lift or Downforce, bring up calculator in Paraview. In the Result Array Name Box, type \'Downforce\', then change the attribute mode to \'Cell Data\'. After that select Pressure from the scalars drop-down menu and multiply it with NormalZ. As seen below, on the top-side there is much larger downforce that is experienced throughout the body whereas on the bottom, the down-force is less than zero. This difference is what keeps the car planted on the ground when it is travelling at a high speed or even taking tight turns.                                                             

5) To compute Drag, bring up calculator in Paraview. In the Result Array Name Box, type \'Drag\', then change the attribute mode to \'Cell Data\'. After that select Pressure from the scalars drop-down menu and multiply it with NormalsX. Notice how most of the drag force is concentrated towards the rear end. The main objective for the straight track is to have as low drag as possible which will allow the car to accelerate faster. For this car, there are certain areas where there is negative drag acting, however the first half of the front wing, mid-section of the rear wing and also the rear portion of the air intake region are generating a significant amount of drag force. These wings are designed to generate downforce and thus there will be some drag generated as a result. However, their design can be optimised for better performance.   

6) Lastly, the drag and lift forces need to be integrated over the entire body using \'Integrate Variables\' Feature. Thus, the following values for drag and lift force were calculated:

The down-force data presents a worrying picture. The car body generates maximum amount of downforce, `121445 N` which is expected of it. However, the front and rear wings fail to generate any significant downforce, courtesy of the poor design. A possible change that can be made is to modify the angle of attack of the front wings. More number of wings can be introduced at the rear or the first wing can be made in such a way that it energises the boundary layer even better.

As for the drag force it is a completely opposite picture. Where the car body generates least amount of drag, the underbody generates very high drag. This can be attributed to extremely low pressure acting at the bottom whereas extremely high pressures acting on the top thus keeping the car planted on road.

→`Y^+`Visualization: For Law of the Wall Model, `Y^+` should be between `30`-`100` which would indicate that the first cell is in the log-law region. A value lower than that would mean that the cell is in the viscous sub-layer or transition region. The below image shows that `Y^+` isn\'t uniform throughout the body. It varies throughout the body with localized peaks or crest. Localized Regions characterized by low velocity have low Y+ values and the regions where velocity is high like the top portion of the wheels, the Y+ crosses over 100.  

→ Velocity, Vorticity and Wake Contours Visualization: The contours will be visualized around the front wing, rear wing, wheels individually. Since the aerodynamics package as seen above is working very inefficiently, the discussion will also be extended to suggesting improvements on increasing downforce and reducing drag. Also, the interaction of front wing with nose cone is discussed.

→ Wakes: A body moving through air creates a track of disturbed flow region known as wakes. This local disturbance in the flow pattern behind the vehicle causes a momentum loss also known as form drag which extends far behind the vehicle. These have a periodic shape where the counter-rotating vortices are shed in an alternative pattern. The reason why these vortices rotate toward the inside is because the region outside the wake has free-stream velocity whereas the velocity in these seperation zones is near zero. So, the air tries to rush in to fill this vaccuum and thus starts to rotate in counter-clockwise direction. Between the region of the alternating vortices created by wing tips, an upwash or upward flow is induced. Notice how in the vicinity of the car these vortices have a stronger magnitude but as it moves far-field, a vortex burst is experienced.

→ Flow over Wheels: The visualization of air-flow around the wheels is similar to that of a cylinder kept at ground. Since, the wheels in this particular simulation are not moving, the discussion will be limited to stationary wheels. The presence of ground forces a zero speed condition near the tire\'s contact patch which will create lift on the wheel. Periodic vortex shedding occurs behind the wheels because of separated flow. This separation starts just behind the wheel\'s highest point. On the highest point, the air flow experiences a high velocity which is characterized by negative co-efficient of pressure (`V_(i)` `>` V∞). This high velocity is because of the locally attached flow which causes more lift whereas behind this point the additional negative pressure creates a lot of drag.

Suggestion for improving downforce: Ahead of the wheel, a stagnation region of high pressure exists. This high pressure can be utilized to increase downforce by mounting a plate ahead of the wheel and parallel to the ground. As seen in the image below, a low velocity high pressure region is created.

A plate that utlizes this principle on the rear wheels is shown below. Another side plate mounted just in front of the cooling inlet utilizes the same principle to increase downforce on the car. A bargeboard can be installed on the same location that would help prevent the dirty air from the wheels ineract with the clean air entering the cooling inlet.

→ Flow Visualisation over Front Wings: In principle, the front wing behaves in the same manner as an inverted airfoil. There is high pressure on the top whereas low pressure region at the bottom that help create downforce. The front wing shown below has two end plates that are mounted to prevent the formation of vortices. At the tip of the wing, the high pressure air rushes to fill in the low pressure air at the bottom which can create vortices. These vortices will then create additional drag behind the wheels when they interact. So, end plates are a counter measure to these vortices. In the image below, it can be seen that most of the low velocity area is concentrated towards the tip whereas, as we move towards the root, the wing-body interaction decreases the downforce being generated and thus the velocity is a tad bit higher here. An anhedral is used at the root to allow the air flow to the rear of the body. By doing this, some of the ground effect created is lost but pitch sensitivity is reduced. (this refers to the phenomenon when airflow to the rear gets blocked when the nose dives and blocks the air)

Suggestion to improve downforce and decrease drag on the front wing:

• Increasing the camber of the wings especially towards the trailing edge and drooping the leading edge will lead to the air flowing faster under the airfoil and a thinner boundary layer will form because of the sharp leading edge.
• Decreasing the ground clearance of the wing and body will create a ground effect that will eventually lead to higher downforce.
• The wing tip vortices can be avoided by creating narrower front wings and installing flaps which works similar to the principle of increasing camber of the wings. However, these flaps can divert the flow away from the cooling inlet so, a cut-out portion is created at the root of the wing.
• Decreasing thickness of airfoil can decrease the overall drag that the wing produces.

→ Flow visualisation over rear wing: As seen below, the rear wing creates most of the downforce at the center whereas near the tips the downforce created is less. This can be understood by looking at the velocity contours. Wings on a car have very low aspect ratios (chord/span) due to which they produce lift which is lesser than the lift of a 2-D airfoil, `2*pi`.

Due to this low aspect ratio, wing tip vortices get generated because the high pressure air on top rushes to fill in the vacuum of low pressure air. These vortices apart from increasing drag behind the car also create a downwash which also reduces the angle of attack of the free stream air, tilting the lift vector and thus resulting in an induced drag. Induced drag is given by: `C_(Di) = (1/(pi*AR))*C_L^2`. This leads to an important conclusion that the total drag of a finite wing comprises of induced drag (`C_(Di)`) and viscous drag (`C_(Do)`). So, to prevent these two pheonmenon a large end plate is fixed on both ends of the plate. Moreover, these end plates help to push the center of pressure of the car in aft direction which can increase high speed stability. Now, the end plates shown above do not completely prevent the air between the plates to rush outside the plates. So, as a result of this you get vortices coming out of the end plate tips.

Another feature that can be noticed above are the multi-element wings used on the rear wings. Through this, the angle of attack  of the wing is increased. If we used a single element wing, there is a possibility that an adverse pressure gradient can be created at the trailing edge possibly leading to flow separations. So, by identifying the region where there is high pressure on top side, a curved cut-out is made by which the high pressure air rushes through the slot and energises the boundary layer. This energising adds a fresh stream of air which keeps the flow attached. By increasing the angle of attack of the second wind, a larger downforce is thus obtained. 

Suggestion to improve downforce on the rear wing:

• Increasing the height of end plate can prevent the air\'s tendency to rush outside. This relation can better help how larger end plates (within the practical range) can be beneficial: `AR_ep = AR*(1+1.9*h/b)`, where `AR_ep` is the aspect ratio of end plate, `AR` is the aspect ratio of wing, `h` is the height of end plate and `b` is the span of wing.
• Using a wavy trailing edge mixes the turbulent air flow leading to increased downforce and less separation behind the wing.
• By increasing the airfoil\'s thickness, separation can be delayed and downforce can be increased.
• A combination of louvre and a cut-out at the end of the plate can help increase downforce. Since the air between the plates is at higher pressure than the air outside the end plates, a vortex is formed. So, by creating louvres some of the high pressure air can be directed outside. This high pressure air created outside will then create its own vortices and then interact with the wing tip vortices through the cut-outs thus neutralising vortex generation. 

→Under-Body Tunnel: It is a well known fact that if the area of any section is decreased, air molecules are forced at higher speed with a consequential increase in pressure. The underbody tunnels at the bottom of the car run on the same principle. However, regulations do not allow for a full-body tunnel on a F-1 car, so a streamline cut and an upward bent plate at the rear is made. This streamlining ensures that the high pressure air is supplied from the sides into the underbody creating vortices which keep the flow attached inside the tunnels. A closely mounted rear wing is needed to pump the flow under the vehicle.  The fast moving low pressure air encounters the upward bent plate which helps to gradually direct air to the high pressure area at the rear.

→POST-PROCESSING LOTS OF TURNS CASE SETUP:

The normal load that tire experiences during cornering can be increased by utilizing the aerodynamic package of the car. For example, if the normal load is increased by 50%, then the tires would have to slip less to create the same normal force leading to preservation of tire and less heating due to friction. On the same hand, the vehicle will be able to turn faster and brake harder.

The car above was rotated at an angle of `48.3`° which is the side-slip angle. The flow separates at the side of the vehicle which when combined with the separation at the rear end creates a very large separation bubble (see the low velocity region on the right hand side). Thw low pressure in the separated zone and the big frontal area now available increases drag on the vehicle sharply. As can also be seen, there are localied regions of high velocity over the air intake ducts and nose cone as a result of this which can increase lift.  

→Drag and Downforce Distribution:

→ Drag and Downforce distribution Chart

The link below gives the line plots for drag, side and down forces on Indivdual Components of a FSAE Car for Lots of Turns Setup: https://drive.google.com/file/d/1LokSbmG80na0QXRB9Y-NQe0HQ4xdVDFK/view?usp=sharing