1. Design of Cal Poly FSAE Front Wing in CFD
Daniel Stalters 1
California Polytechnic State University, San Luis Obispo, California, 93401
This study seeks to address the lack of recent aerodynamic development of the
aerodynamic devices of the Cal Poly FSAE car using proper tools and techniques to
predict aerodynamic characteristics on the final car. The aerodynamic performance
of wings operating in ground effect on a racecar are analysed and their sensitivity
to certain design parameters are compared. These parameters include ride height and
pitch and their effect on downforce and drag - which are used as the main aerodynamic
performance meters used to "optimize" the design of the front wing.
1 Undergraduate Aerospace Engineer, Aerospace Engineering, 1 Grand Avenue, San Luis Obispo, CA 93401
1

2. Nomenclature
c = Characteristic length [m]
Cd = Coefficient of drag
Cl = Coefficient of lift
k = Turbulent kinetic energy
L = Length [m]
Re = Reynolds number
Rex = Local Reynolds number
Reθ = Momentum thickness Reynolds number
y+ = Non-dimensionalized normal wall distance
α = Angle of Attack [deg.]
αcritical = Critical angle of attack [deg.]
γ = Intermittency
δ = Boundary layer height[m]
= Dissipation of turbulent kinetic energy
ρ = Density [kg/m3
]
ω = Rate of turbulent dissipation
I. Introduction
The FSAE car is a formula-style race car that relies heavily on aerodynamic devices to improve
performance and make the car competitive against others university built race cars at yearly com-
petitions. In years past, aerodynamic development has been largely a second thought without much
emphasis within the team. This situation has been progressing over the last few years, but a com-
prehensive study of past designs and holistic design process encompassing the entire aerodynamic
subsystem on the car has yet to be conducted. This research focusing on the front wing assembly of
the FSAE car is part of a much larger effort to achieve this goal – indicating where improvements
might be made and offering advice to that end. This is in the hope that what results are collected
will improve the performance of the car and team standing on a national level.
2

3. Fortunately there have been many attempts over the years to further research in areas related
to racing performance. Aerodynamic analysis of formula style race cars provide a solid background
in which to compare the results gained here. While methods might be slightly different, overall
trends can be used to provide some validation of results in the absence of reliable test data. In the
future, this data will be available to us through the use of the Cal Poly low speed wind tunnel and
track testing on the new 2016 FSAE car.
Formula 1 is perhaps the most visible and well-funded racing series directly related to the
type of car driven by Cal Poly FSAE, offering numerous examples to inform our own engineering
decisions. However, these cars operate in largely different conditions and are developed with analysis
tools that far exceed those available for use in this report. This lack of direct correlation makes
imitation a foolish decision – resulting in wings/devices designed to operate in entirely different
flow conditions operating somewhere on a performance curve nowhere near optimum. Many papers
relating to Formula 1 or Indy Car design must then be thought of as guides, without the convenience
of directly comparable numeric results to be used as they relate to the FSAE car.
Several papers of particular interest fit into this category with extensive research done for use
in a high performance racing series such as F1. With regard to the front wing of a racing car, these
papers suggest that the best design approach does not include analysis of the wing in isolation, but
that a more holistic approach including a rotating wheel will provide a more optimized system [1].
This is reflected in the analysis of the rotating wheel’s effect on the aerodynamic performance of
the wing and the effect of the wing on the tire. In the case of a rotating wheel, the downforce of
the wing is reduced due to a high pressure region in front of the wheel. This high pressure region
is also affected by the wing vortices generated at the intersection of the wing and the endplate and
the general lower pressure region generated by the wing. The analysis of the wing-tire interaction
indicated there was an optimal configuration, however, of most interest to validating our CFD
models of the FSAE front wing, the pressure distribution over the bottom of the front main element
will indicate whether or not the rotating wheel is interacting in the same way [1]. Another paper
deals with quantification and location of the vortex structures on a simplified tire in isolation.
This study will provide an interesting comparison of vortex structures in an isolated case to those
3

4. observed interacting with a front wing. In addition, the paper indicated that contact patch and
model simplifications had a large impact on the wake structure shed from the wheel and on the
overall lift and drag of the model. These outcomes informed the model generated here, with wheel
hubs included on the inside of the tire to better correlate with experimental evidence [2]. It is also
known from this research, the addition of a rotating wheel will result in higher pressure regions
forward of wheel than observed in the initial mesh convergence simulations.
A. Project Description
The 2015 FSAE front wing has been analysed in the preliminary portion of the project as part
of a mesh convergence study. From here, a design process to determine angle of attack sensitivity
and ride height influence will be conducted to better understand the influence these have on the
performance of the wing. Through this process, an analysis of airfoil types will also be conducted.
On the Cal Poly FSAE car, the flow over the front wing is dominated by 3D effects generated by
the nose-tub assembly occupying over 28% of the span. The wheels occupy 18% of the span altering
the pressure gradients over the region well outside of the immediate region in between them and
the wing. Due to these large 3D influences, any significant use of a 2D approach was deemed to
be ineffective in capturing the most important flow behaviour governing the majority of the front
wing performance. While optimization tools do exist, the more time intensive nature of the adjoint
flow solver has led its exclusion from this design project. Special considerations to this end include
a much finer mesh in the boundary layer next to the wing to better model the viscous effects in the
wing/flap interaction.
In order to simplify the geometry in the mesh convergence study, a simplification block was
made as an extrusion from the back of the FSAE tub to the outlet (figure 1). This eliminated
the large wake that would have formed off the back of the car without the engine and suspension
modelled – a simplification to reduce mesh size. By solving one problem, this approach introduces
other sources of error in the solution. Primary among these is while eliminating the large wake
forming nearer to the wing than experimentally accurate, the simplification block also eliminates
any wake that will form off of the back of the car in normal operating conditions. This leads to an
4

5. overall more ordered flow field and an over prediction of force coefficients.
Fig. 1: Showing the simplification block extending from the tub to the outlet boundary.
The floor of the simulation is set with a tangential velocity component equal to freestream fluid
velocity to model a moving ground. This was chosen over a slip wall condition to allow more accurate
formation of a boundary layer beneath and in front of the front wing. Due to the study of ride height
and its reliance on small ground effects, this method will provide a more realistic result. The inlet
was modelled with a velocity component normal to the plane at a specified magnitude. The FSAE
car operates at an average speed of 35 mph. Therefore the inlet velocity in SI units has been set to
15.6 m/s. Outlet condition was set to accommodate propagated atmospheric conditions. The outer
walls were modelled as a slip condition. This has the potential to act as a flow straightener, but
given the blockage ratio (under 2%) of the model in the fluid domain, the influence of the walls can
be considered negligible. Both the outer walls were set 10m from the symmetry plane and floor.
The inlet was set to 12m in front and the outlet was 30m behind the FSAE car (figure 2). This
was determined to be an adequate compromise between the standard 5-10 characteristic lengths
combination and common sense reasoning length required for wake and forward pressure regions to
damp out. The characteristic length of the model is 5m, but considering the object of interest is
the front wing with chord length .35m, a far field boundary behind the car of 50m seemed excessive
(over 140c). Therefore, a smaller fluid region was determined and was checked to see if there are
any differences in pressure recovery at inlet and outlet boundaries.
Based on results others have obtained examining similar wing/tire configurations in publicly
available papers, there are several trends we are looking to observe in our front wing simulations.
Of particular interest is characterizing the effect of a rotating wheel on the front wing and designing
a wing-flap configuration that works efficiently with the main element. In order to validate results,
we would expect to see vortices formed on the outer endplates traveling into the tire and lowering
5

6. Fig. 2: Showing the entire fluid domain surrounding the FSAE car.
the pressure in front of the tire.
II. Numerical Model
Using the meshing software in Star CCM+, multiple meshes with progressively higher cell counts
and mesh densities were generated around the FSAE car to determine where the solution would
remain unchanged with any further refinement. The variables of primary interest in the design of
the front wing are the lift/downforce generated and the drag produced. The methodology applied
to the mesh convergence study involved stating that a solution was converged if the values reported
in the downforce and drag monitors held a constant 1000th’s place value between two iterations.
It worth noting here that there are several considerations that will affect the size of mesh
selected for further study. Due to limitations on the computing resources available, prism layers were
excluded from some components in the trimmed mesh study, resulting in less accurate simulations
and lower overall cell counts. Rotating tires are also not modelled in the trimmed mesh convergence
study due to limited computer resources. Therefore, it is understood that these results are only a
guide and will provide a base minimum for reasonable results when the final simulations are run.
In the initial simulations conducted on the trimmed mesh, two turbulence models were used in
order to speed up convergence of the flow field. Initially, 200 iterations were run using the standard
k- turbulence model with the high y+
wall treatment boundary condition. After 200 iterations, the
turbulence model was switched to k-ω SST with all y+
wall treatment boundary condition. These
were run with identical turbulence specifications. The length scale was set as 4 percent chord length
(.014m) and the intensity was set at 4 percent to simulate fairly smooth air conditions that might
be experienced while driving the car in clean air.
6

7. The mesh convergence study was conducted on the Cal Poly Low Speed Wind Tunnel computer.
Of interest is the ability to set a solution to solve in parallel on this computer thereby reducing
iteration time and allowing for a greater number of simulations or higher cell resolutions or both.
The largest mesh in the mesh convergence study (14.6 million) took less than 30 minutes to generate
and solving through 500 iterations took less than 2.5 hours.
The selection of turbulence models was in accordance with prevailing advice concerning the
ability to predict separation and model circulating flows in presence of high pressure gradients.
The k-ω SST model is used as a final model with a y+
value of 30-40 over the front wing for
accurate boundary layer modeling. For this level of refinement, the first prism layer will be set to
6.314 × 104
m. Boundary conditions over fluid domain were set to model closely the conditions the
FSAE car would experience when driving at competition. This includes the physics value for shear
condition over the outer walls set to slip to more accurately model the situation where boundary
layers do not form over the road and at the locations of the outer walls. Later tests in the Cal
Poly Wind Tunnel will need a different set of boundary conditions to model the flow over the test
section walls. Turbulence was specified at the inlet and outlet boundaries to closely model expected
turbulence levels when driving. These parameters include an intensity of 4 percent and length scale
of .014m.
A. Grid Description and Refinement
The automated mesh generation tool in Star CCM+ was used to make the meshes used in
this mesh convergence study. Of the three available automated meshers, the tetrahedral mesh
was eliminated due to concerns over the relative quality of the cells. With the tetrahedral mesh
eliminated, there remain two automated meshers to choose from. To show mesh independence
for all subsequent models used in this report, two separate convergence studies were done on two
different mesh types. Using both the polyhedral and trimmed cell meshes in Star CCM+, the
mesh convergence studies were carried out using three meshes of increasing cell count to determine
the sensitivity of lift and drag to the mesh resolution. This was accomplished refining the mesh
around the FSAE car in what will hereafter be call the “refinement box” surrounding the car and
7

8. extending slightly downstream in an effort to capture some of the wake produced by the car. In
these convergence studies, the FSAE car was greatly simplified to speed up simulation times and
to cut down on the memory required to generate the meshes. This simplified geometry mirrors the
initial simplifications made later to study the relative effectiveness of various airfoils. The various
settings of the mesh convergence studies can be seen in tables 1 and 2.
Case 1
Target Surface 2%
Minimum 1%
Surface Growth Rate 1.2
Volume Size 6%
Case 2
Target Surface 3%
Minimum .5%
Volume Size 5%
Case 3
Target Size 1.25%
Minimum .25%
Surface Curv. 100pts.
Volume Size 3%
Table 1: Non-default settings used for the three trimmed mesh cases tested in the mesh
convergence study.
The most influential of the settings were the surface curvature and minimum surface size setting.
Effectively working together, a higher number of points per circle resulted in much finer mesh around
curved surfaces. As long as minimum surface size was low enough, cell faces could be fit to each
line segment, resulting in a denser mesh around the leading edge and tire surfaces – areas of higher
pressure gradients. It is also important to note the surface growth rate was changed in both trimmed
and polyhedral case 1 to promote faster cell growth over surface over the tub given the geometry
that includes several large, planar surfaces bordered with small-radius curvature lines. Changing
the surface growth rate to allow faster growth rates cuts down on the cell count near the surface
and therefore affects how many cells will surround the car in the nearest layers. This one change is
responsible for most of the cell count difference between cases 1 and 2 because the volume control
8

9. Case 1
Target Surface 2%
Minimum .5%
Surface Curvature 50pts.
Case 2
Target Surface 1.5%
Minimum .5%
Volume Size 4%
Surface Curvature 70pts.
Case 3
Target Surface 1.5%
Minimum .4%
Volume Size 3.5%
Surface Curvature 70pts.
Table 2: Non-default settings used for the three polyhedral mesh cases tested in the mesh
convergence study.
region around the car is itself the primary contributor to cell count.
As mentioned previously, prism layers were not included over some components in the mesh
convergence study in an effort to reduce mesh generation and solve times. Prism layers will be
included in subsequent simulations due to the heavily influential boundary layer flows over the main
element and flaps. As will be examined in greater detail later, this exclusion appears to have had
a negative impact on the results gathered. One will also notice that between case 1 and 2 of the
trimmed mesh study, the target surface size changed from 2 to 3 percent. This was a result of
attempting to placate the custom volume mesh control while keeping a smaller surface size. The
issue being the order of preference within the mesh generation solver. This would result in either
the volume mesh determining the surface size over the car or the surface size determining the size
of the volume mesh generated. On potential benefit of this disorder, is the isolation of surface and
“freestream” effects on the prediction of the forces over the front wing.
The same effects are true for the use of the polyhedral mesh in Star CCM+. A polyhedral
mesh is generated by combining tetrahedral cells from an initial mesh into larger polyhedral cells.
The benefit of the polyhedral mesh is the number of faces on each cell. The random nature of the
9

10. orientation of the faces with respect to the fluid domain preclude any bias toward flow direction
as is present with the use of the trimmed cell mesh. In addition, fewer cells are needed to follow
the curvature of a surface resulting in a better resolution over highly curved surfaces as are often
present on the FSAE car because the initial mesh is made up of triangulated cells (tetrahedrons).
Fig. 4: These graphs show the convergence of the two separate mesh convergence studies
conducted with the trimmer and polyhedral meshes. The polyhedral study shows a more
promising trend towards a converged mesh.
An issue with every attempt to model a wheel in CFD is the area between the wheel and the
ground plane. Inherently a very acute angle is formed which results in highly skewed cells. These
cells are important when modelling a rotating tire due to vortices generated in the region near the
contact patch. This presents a difficult problem and one that is only surmountable by compromise
between model accuracy and mesh generation requirements. As can be seen in figure 5, the area
between the wheel and the ground has been highlighted in pink, indicating bad cells in the region.
Adding more cells in the region results in a finer mesh and smaller bad cells, ostensibly lessening
the effect of the region. Taken to extremes one can easily understand how foolish it would be to
follow this path. Therefore we must accept some level of skewed cells in the region near the tire and
deem this acceptable given the few alternatives and understanding how little an effect this region
has on the whole front wing assembly. Due to time constraints, a detailed analysis on the effect of
10

11. Fig. 5: Here the bad cells are highlighted in pink. Post-processing the mesh allows areas of less
than desirable cells to be isolated. Shown here is case 1 of the trimmed cell mesh study.
mesh refinement at the intersection of the ground plane and the tire could not be conducted. For
this we turned to available research that indicated a contact region roughly the size of the contact
patch of the FSAE car under normal conditions was adequate for simulating a rotating wheel [2].
In addition to concluding a simulation as near to the modelled conditions as possible is desirable,
the authors analyse common simplifications made in other CFD and wind tunnel models for racing
vehicles involving tires. Here it is found that large reductions in lift are observed when the wheel
hub is modelled as accurately as possible [2].
The Reynolds number of the FSAE front wing main element is 3.737 × 105
. Over the entire car
the Reynolds number becomes 5.338 × 106
. This poses a potential challenge; with the front wing
operating within the transition region, it necessitates the use of a transition model and much higher
cell counts. Within the k-ω SST turbulence model, the γ-Reθ transition model was examined. γ-
Reθ, being a transition model, requires a y+
value around 1 and at least 10 – 20 prism layers within
the boundary layer to capture viscous effects and model transition. For the Cal Poly FSAE car, a
y+
value would be calculated as follows:
lam =
4.91x
Re
1
2
x
(1)
turb =
.16x
Re
1
7
x
(2)
lam =
L(1.3016 × y+
ave)
Re.75
x
(3)
turb =
L(13.1463 × y+
ave)
.875
Re.9
x
(4)
11

12. The front wing operates in the transition region described by a Reynolds number range of 1×105
to 3 × 106
. Because it lies within the transition region but at a Reynolds number below 5 × 105
, we
would choose to model it as a laminar flow. Doing so results in a y+
of 3.014×10−5
m, far too low to
be calculable in the time frame provided by the FSAE team. Because of this practical consideration,
we make the assumption vibrations associated with driving will force transition to occur at a lower
Reynolds number and because the car will be operating in ground effect over an autocross course,
the flow will be turbulent and transition is not a phenomenon of great importance to our model.
This is especially true when considering the number of moving parts around the wing, operating in
conditions far from traditional aerospace freestream conditions. Overall, the prism layer will extend
to the edge of the boundary layer over the front main element with a separate surface control set
for the tub to better model each boundary layer individually. This will control the number of
cells and limit unnecessary cells where the boundary layer is thinner such as over the front wing
assembly. Using the above equations and assuming turbulent boundary layers, the thickness of the
B.L. over the front wing is determined to be 8.956 × 103
m and the thickness over the tub is .0875m.
The difference between the two boundary layer thicknesses is an order of magnitude, showing the
computational savings that will result from separate surface conditions.
B. Boundary Sensitivity
Mentioned earlier in this report was the overall sensitivity of the solution to the boundary
conditions and location away from the FSAE car in the fluid domain. Because of rotating tires and
the bluntness of the obstruction the flow encounters, a large wake is expected to follow behind the car.
This wake has been greatly reduced by the simplification block that extends to the outlet boundary
behind the tub and serves to minimize what would otherwise be a large area of recirculation. From
initial runs using the current boundary conditions and spacing, it is possible to observe a region
of lower pressure air trailing the car that indicated an incomplete pressure recovery that may have
an influence upstream. To determine the effect of this boundary condition of the solution, the
boundaries were moved 10m further back from their current location. This change necessitates the
generation of a new mesh; however, because the area of change is a region of the fluid domain where
12

13. the cell size is no longer changing – target cell size has already been reached before this point –
there is no significant difference between the new mesh and old.
C. Project Procedure
To generate initial airfoils for use in the CFD simulations, the simulation tool JavaFoil was
used to find L/D and pressure distributions over chord length. All airfoils used were marked on the
UIUC airfoil database as being either low Reynolds number, high lift or low drag. Additionally,
all airfoils were run at α = 0
◦
to reduce potential errors associated with higher angles of attack
where viscous effects might have a larger influence on the L/D ratio. Pressure distributions were
used to differentiate airfoils based on the size and severity of the adverse pressure regions. Because
the wings eventually used on the FSAE car will be operating ahead of high pressure regions and
in high lift configurations, more gradual pressure gradients were favoured for their potential to
promote further aft separation points.
Fig. 6: The hierarchy of the design process is shown. Each stage includes fewer potential designs
and fewer tested parameters until a final design is chosen in stage 4.
This method was chosen for the quickness of the desired results but is understood to have
limitations that ultimately would limit its effectiveness. As a panel method, JavaFoil is left to
approximate drag and the pressure distributions, while roughly correct, will suffer from inaccuracies
due to boundary layer effects. This was minimized as much as possible by simulating freestream
conditions at α = 0
◦
. From this initial selection process, three airfoils were chosen for their gradual
adverse pressure gradients, low peak suctions further from the leading edge, and relatively efficient
13

14. L/D ratios.
The effect of angle of attack of the entire front wing assembly of the FSAE car was carried out
with the three airfoil shapes as the basis for both the wing and flap. For consistency and to fit within
the scope of this report, the main element and the flap share the same shape and a universal set up
was used to measure the lift and drag of each airfoil in a predetermined slotted flap configuration
to allow for more direct comparison between cases.
Fig. 7: This is a graphical representation of the universal configuration that was used to maintain
geometric similarity among the three airfoil-flap configurations.
As described in figure 6, stage two was the first to involve CFD testing and the simplifications
made to the model here are significant. A floating front wing assembly is used with an initial ride
height of .12c at α = 0
◦
. The tub remained in the simulation because it was determined that, while
a relatively streamlined body, its effect should not be neglected – especially over the inner portion of
the main element where there are two converging surfaces formed by the upper surface of the front
main element and the slope of the underside of the nose cone. However, the wheel was excluded due
to the greater complexity of the flow field introduced by the rotating boundary condition and the
large recirculation region that would form in its wake. This effect, while certainly not negligible,
would be identical between each case. And while some airfoil configurations could potentially be
better at delaying separation in front of the wheel, the more important influence is overall flap design,
deflection and size, two variables which are not studied here. Therefore, interactions between the
14

15. wheel and wing were determined to be insignificant at this stage of the project.
Fig. 8: The 2D airfoil shapes examined in in stages 1 and 2 of the project procedure are shown
here for reference.
Star CCM+ allows the user to change “design parameters” in the imported CAD model and
update all features further “downstream” in the meshing pipeline as long as the design parameters
are specified in the CAD model portion of the geometry node. This feature has the potential to
improve case comparisons and limit the amount of time spent inputting new values for subsequent
mesh generations because it changes CAD on the part level and then moves those changes through
the pipeline while keeping the current settings and solutions. Because the settings and solutions are
kept, the solver spends less time converging to a solution, leading to shorter run times with fewer
iterations.
In order to sweep through all angles of attack, two design parameters were set to allow both
rotation about a coordinate system defined at the leading edge of the main element and translation
in the general laboratory frame in Star CCM+. The translation parameter was used to adjust the
height of the assembly when a high angle of attack produced interference between the trailing edge
of the main element and the nose cone. This translation vector would inherently affect the ride
height of the assembly, producing different results than if the ride height was kept at the initial .12c.
This effect could be significant, but the physical limitations experienced in the CFD software are
identical to what would otherwise be experienced on the FSAE car if track testing were conducted.
Because of this, the effect of changing ride height was determined to be an accurate representation
of reality and its effect accounted for in the lift and drag at α = 4
◦
.
15

16. III. Findings
Several trends are worth noting about the lift and drag data gathered among the three airfoil
shapes and the three tested α’s. The Marske7 airfoil shape was selected because it was a low drag
airfoil that might be of interest for low drag situations or where the necessary downforce required
for aerodynamic balance was less than anticipated. This proved to be an accurate characterization
of the drag performance of the airfoil seeing that it produced the least amount of drag at all α when
compared to the other tested airfoils. It also had the largest α sensitivity to lift, decreasing 60%
over the tested range of 8◦
. Potentially related to this behaviour, the Marske7 airfoil has a smaller
leading edge radius that contributes to a sharpness not generally seen on low Reynolds number
airfoils. From a design perspective, this suggests that there is could be a limited range of α and
that the wing will stall abruptly and completely at αcritical. Because of the observed sensitivity
lift has to α and the resulting potential for abrupt changes in aerodynamic behavior under varying
conditions, the Marske7 was eliminated from further consideration.
Table 3: The differences in predicted lift and drag with three different airfoils at three values of α.
The CH10-48-13 airfoil has the largest camber of the three airfoil shapes used and exhibits
similar behaviour to the FSAE 2015 front wing which too had a large degree of camber. Camber is
often used by race car engineers to move peak suction farther back over the chord length [6]. This is
possible due to lower Reynolds numbers than those experienced by aircraft for which most airfoils
are developed. However, because both the CH10-48-13 and 2015 airfoils are not thick through the
mid-chord, there is a large concave region above the wing which will tend to slow air down as it
passes over the wing. Without a well-designed flap, the air travelling over the wing is brought closer
16

17. to stall and leads to an increase in drag. The recirculation over the top of the wing can also lead to
reduced lift. Considering the lower overall lift and higher drag numbers of the CH10-48-13 it has
been decided that this is a less than desirable set up for the front wing and was scrapped in favour
of the LA203.
Fig. 9: The wall shear stress over the top of the front wing is shown in contours with the darker
blue regions indicating near zero or zero shear stress. The leading edge is oriented towards the
bottom of the figure.
From the three airfoil shapes, the LA203 was selected because it had the highest overall efficiency
(L/D = 11.36) and the highest max downforce at α = 0
◦
. Interestingly, at α = 4
◦
the downforce
decreased while the drag continued to increase – indicating that separation may have occurred over
the flap or some other portion of the wing. It is possible that the flap is operating near its limit and
a high α sensitivity is present. If this were the case, it would be important to test that deflection
of suspension during braking would not induce a pitch angle that would cause the wing to stall.
This could be a difficult task considering the change speeds of the car under braking and the lower
Reynolds number flows the wing would see. However, understanding this interaction would be
critical to prevent possible loss of downforce under braking. A summary of this data is presented
17

18. Fig. 10: The regions of low to near zero shear stress is shown in this image as regions of darker blue
over the underside of the front wing. The leading edge is oriented towards the top of the image.
in figure 3.
Once airfoil geometry was chosen, the ride height sensitivity was studied to determine the best
position of the front wing assembly above the ground. The ride height was initially measured in
SolidWorks as the distance from the ground plane to the lowest point on the airfoil. Once the
geometry was imported into Star CCM+, it was then translated using the same translation design
parameter used when adjusting and sweeping angle of attack. From the data gathered in this stage
of the procedure, .15c is shown to have the highest lift and lowest drag as well as best overall
efficiency as can be seen in table 4. This interaction is difficult to explain and further study would
be necessary to make any conclusions as the the cause of this counter intuitive result. The best
explanation that can be offered at this point of the design process is that there is a balance between
increased lift associated with ground effect and either increased lift or, more likely, decreased drag
produced in the region of convergence between the trailing edge of the main element and the nose
cone. From case studies, it is often the case that there is a trade-off between decreased ride height
and desirable nose-wing interactions as presented by Katz [6]. This would appear to agree with the
observed reaction to increased ride height.
18

19. Table 4: The predicted values for lift and drag at three different ride heights.
The Realizable k- model was used with the high y+ wall treatment to better model the large
y+ values that result using the simplified 4 prism cell boundary conditions used over the front wing,
tub and the tires. As a result of limited testing time on the Cal Poly FSAE car, there a no track
testing data points with which to compare the CFD results to. This prevents the validation of
the model needed to fully trust results obtained in Star CCM+ despite all efforts made to properly
define and simulate turbulence parameters and boundary conditions. Because of these interpretation
limits, several turbulence models have been tested to offer a range of potential lift and drag numbers
that could model the flow over the car. This not only provides a better and more encompassing
understanding of how individual turbulence models solve under the same conditions using the same
mesh, but what expected performance might be as a range instead of a singular number. This range
of possible performance is likely to provide a more realistic prediction of actual performance in the
absence of testing data for the FSAE team to use in its decision making process.
The standard k- model was used to see if any benefit was to be gained from simplifying
the mathematical model, especially near the wall, where a high y+
value was being used anyway
and where gains in accuracy associated with using the Realizable model would be unrealized. The
standard model was implemented on a flow field had already been solved using the Realizable model.
The turbulent viscosity was artificially limited on at least one cell in the fluid region indicating
that there is at least one cell with nonphysical turbulent viscosity. However, a larger, abnormally
high region of turbulent viscosity surrounding what is likely a skewed cell negatively impacting
the solution is expected and the results obtained using this model would necessarily need to be
discounted. This would lead to unacceptable and inactionable results and therefore, the standard
k- model was eliminated due to concerns over the robustness of the solver for these boundary
conditions.
19

20. Table 5: The predicted values for lift and drag given by the Realizable k- and k-ω SST turbulence
models.
The k-ω SST model, like the Realizable k- model, is a two equation model. However, it differs
in that it includes the term ω that is intended to better model the dissipation of turbulent energy.
This would potentially lead to differing vortex propagations between models, as suggested by Barber
et al., or a difference in the breakdown of turbulence as the wake is shed off of the tires and tub
[1, 2]. Both the Realizable k- and the k-ω SST models are designed to be used with two layer
wall treatment that resolves both the turbulent boundary layer’s viscous sub-region and the larger
logarithmic growth region. Because the y+
value is large and the high y+ wall treatment is being
appropriately used, the significance of the two models and the treatment of the turbulence in the
boundary layers over the FSAE car will be limited. However, the difference between the two models
is important to understand in the context of modelling the FSAE car. As mentioned earlier, there
is no existing data to validate these results so no determination can be made to the accuracy of the
Realizable k- model and the k-ω SST model. While this is true, the difference in predicted flow
features may still benefit the design process and future data may become available when testing
is finally conducted of the car. As shown in figure 12, there are several differences in predicted
vortex strengths and even location. The k-ω SST model predicts universally higher vortex strengths
indicated by lower pressure regions at the vortex cores. This is due to the mathematical differences
between the two models. It also shows a lower center on the vortex formed beneath the main element
at the intersection of the outer endplate. This larger vortex on the underside of the wing is probably
the cause for the lower prediction of lift over the FSAE front wing design. What is not completely
understood is how this leads to less overall drag. The only explanation that can be offered is the
lower lifting force has a lower induced drag component which outweighs the effect of the increased
vortex strength and size.
With a basic understanding of the best approach for "accurately" modeling the Cal Poly FSAE
20

21. Realizable k-
k-ω SST
Fig. 12: These two images contrast the normalized total pressure immediately behind the front
wing. This shows the difference in vortex strength and location between the two turbulence
models.
car under reasonable time constraints, additional study was conducted on the size of the main
element chord and the shape of the middle section of the main element. From the distribution of
wall shear stress over the under side of the LA203 airfoil used for the main element, a large region
of separation formed over the last 10-15% of the chord. A potential source of this separation was
thought to be a result of the large chord length and the relatively low speeds of the FSAE car that
would allow boundary layer viscosity and skin friction to overcome the momentum of the air near
the wall. To test the effect of shortening the chord length, the overall main element model was
scaled, changing the chord length from .35m to .25m. Unsurprisingly the amount of drag produced
is less on this wing set up than the larger chord length and there was an observed improvement
21

22. in the L/D ratio which indicates a higher efficiency possibly due to less extensive separation. The
reduction in drag is accompanied by a decrease in downforce produced. The shorter chord length
also has several advantages over the other in its improved range of rotation which will allow for
more accurate tuning during testing because the wing need not be translated to clear the nose cone
of the car.
By reducing the chord length of the wing, there is shown an improvement in efficiency by limiting
pressure drag created by separation but a region near the center of the span is still shown to have a
significant portion of stagnating air. This again confirms the large impact of the nose cone and tub
geometry over the center of the wing. Considering this, a less cambered airfoil shape was modeled
in this region to reduce the pressure gradient over the latter half of chord. This lower gradient
would inevitably reduce the downforce generated by the main element but has the potential to help
delay separation and therefore reduce drag. To better visualize this, the air travelling over the front
wing is forced downward by the tub geometry and entrains some of the air moving under the wing
inducing a wall normal component of velocity near the lower surface’s trailing edge, increasing the
likelihood of separation. A lower pressure gradient would provide higher velocity air in this region,
reducing the relative impact of the downward, problematic air from the tub.
IV. Conclusion
From these findings, a configuration for the Cal Poly FSAE car front wing has been designed.
While an improvement over the 2015 front wing assembly designed entirely in 2D inviscid flow
modellers, there are aspects of the presented design that will need further analysis and design. It is
uncertain whether the final geometry presented here is an optimal configuration or just the best of
what was tested. In particular, the 2015 FSAE front main element was .35m which posed problems
when trying to adjust angle of attack by inducing interference at the trailing edge of the main
element and the nose cone, limiting α. This was addressed by reducing the main element chord
length to .25m, but values in between these points were not tested due to time constraints.
Another important limitation of the analysis conducted while completing this project is the
treatment of the flaps. The flaps used on the 2015 FSAE car were carried over to this year with
22

23. the only analysis on the flap deflection angles and slot gap spacing. Further testing on the shape of
the flaps would be beneficial but was left to another study due to an expected small return on time
invested.
While certainly true that more work needs to be done, there are several promising trends
presented here. The sensitivity of multiple airfoil shapes in the same configuration to the change in
α shows the importance of checking the induced pitch changes under braking and acceleration which
may have a large impact on aerodynamic performance if operating near peak performance on the
lift curve. The ride height sensitivity of the front wing element has been analysed and presents the
future designer with a better understanding of the FSAE front wing and its more complex interaction
in ground effect and with the higher pressure regions that occur leading at the tub possibly leading
to drag reductions when positioned optimally. With the current geometric set up, the ride heights
tested in the report indicate that a higher location of the front main (.15c) is desirable. Lastly, the
two turbulence models tested show that there are differences in the predicted lift and drag. These
differences are small in comparison to manufacturing and other uncontrollable differences in surface
finish and final airfoil shape when installed on the Cal Poly FSAE car. Therefore, it can be concluded
that the two turbulence models used predict with an equal accuracy (yet undetermined) the expected
lift and drag characteristics of the front wing, suggesting that the final choice of turbulence model
should be made with regard to other considerations. These considerations would include solving
time or preferred model for other systems on the car when inputted to a full car model. Therefore
it is suggested that the k- model is used to reduce solving times and increase simulation capacity.
The decreased chord length on the main element is another positive improvement and confirms the
importance of reducing separation over all lifting surfaces to reduce drag and improve L/D.
23

24. References
[1] Barber, Tracie J., Sammy Diasinos, Graham Doig. “On the Interaction of a Racing Car Front Wing and
Exposed Wheel.” ResearchGate. Journal of Wind Engineering and Industrial Aerodynamics, 15 Aug.
2015. Web. 07 Nov. 2015.
[2] Barber, Tracie J., Sammy Diasinos, Graham Doig. “The Effects of Simplifications on Isolated Wheel
Aerodynamics.” Elsevier.com. Journal of Wind Engineering and Industrial Aerodynamics, 15 Aug. 2015.
Web. 09 Nov. 2015.
[3] Celik, Ismail B. “Introductory Turbulence Modeling.” West Virginia University, Morgantown. Dec. 1999.
Unicamp Faculty of Mechanical Engineering. Web. 2 Nov. 2015.
[4] “Examining Spatial (Grid) Convergence.” Grc.nasa.com. NPARC Alliance, 17 July 2008. Web. 09 Nov.
2015.
[5] “FLUENT 6.3 User’s Guide - 12.4.1 Standard - Model.” UC Davis FLUENT and GAMBIT Help. UC
Davis, Web. 02 Nov. 2015.
[6] Katz, Joseph. Race Car Aerodynamics: Designing for Speed. 2nd ed. Cambridge, MA, USA: R. Bentley,
2006. Print.
[7] Malan, Paul, Keerati Suluksna, and Ekachai Juntasaro. “Calibrating the Îş-ReÎÿ Transition Model for
Commercial CFD.” Cfd.mace.manchester.ac.uk. University of Manchester, 2009. Web. 9 Nov. 2015.
[8] Rumsey, Christopher. “Turbulence Modeling Resource.” Turbulence Modeling Resource. Langley Research
Center, 7 Oct. 2015. Web. 02 Nov. 2015.
[9] Spalart, P.r. “Strategies for Turbulence Modelling and Simulations.” International Journal of Heat and
Fluid Flow 21.3 (2000): 252-63.Elsevier. Web. 2 Nov. 2015.
24