Example_Aerodynamics

SRN: 14149217
Investigation of the aerodynamics of a wing under various conditions
BEng Automotive Engineering with Motorsports
UNIVERSITY OF HERTFORDSHIRE
Abstract
This paper aims to investigate the
aerodynamic properties of a 3D wing. A
model wing was used in the University of
Hertfordshire's open jet wind tunnel and
surface pressure measurements were taken
at various angles of attack (0°,5°,10°,15°).
These values were then compared to those
obtained through CFD analysis using Star-
CCM+. The results show that there is good
correlation between both methods at
certain points on the wing, as long as the
experimental conditions are precisely
defined in the numerical model.
Introduction
Computational Fluid Dynamics, or CFD,
has become an important tool in the
automotive and aerospace industries to
simulate the flow of fluids around a vehicle
body. The improvement in computational
models mean that wind tunnel testing can
be kept to a minimum to reduce costs.
However wind tunnels still play a major
role in validating the theoretical results.
That's why all the following CFD results
were compared to values obtained in the
university's subsonic open-jet wind tunnel
to ensure that the numerical results were
realistic.
Pre-analysis of the aerofoil
Before starting to simulate the wing under
Star-CCM+, the wing was assumed to be a
flat plate in order to determine the nature
of the flow at 25m/s. The Reynolds
number is an non-dimensional number that
helps to define the nature of a flow and is
governed by:
𝑅𝑒 =
𝜌. 𝑈. 𝐿
𝜇
Where μ is the dynamic viscosity of air in
kg/m.s, ρ is the density of air in kg/m3
, U is
the velocity of air in m/s and L is the
reference length of the wing in m. The
Reynolds number was approximated to be:
𝑅𝑒 =
1.226 ∗ 25 ∗ 1
18.27 ∗ 10−6
= 1.68 ∗ 106
With this number being higher than 4800,
which is deemed a critical number for
turbulence, the flow around the wing will
be assumed to be turbulent and the physics
model was chosen accordingly.
Another important point when using a
CFD package is the use of wall treatments
to determine the near wall conditions
without a very fine mesh. These functions
only work within a certain range of y+
values. The wall y+ can be defined as a
non-dimensional number that defines the
distance of the first mesh grid point to the
wall. Star-CCM+ offers three types of wall
treatment options. A high-y+ wall
treatment used with a coarse mesh, where
the first grid point is located above the
viscous sub layer. A low-y+ wall treatment

SRN: 14149217 2
for when the mesh is fine enough to
resolve the viscous sublayer and must have
between 10 & 20 prism layers to be
effective. The final option is the All-y+
wall treatment which combines both of the
previous options and should give accurate
results. It is this final option that was
chosen for the near wall treatment of the
wing. Moreover, a wall y+ value of 0.3
was chosen and the domain was meshed
accordingly. The first cell height was
estimated at 0.0044mm and the total height
of the prismatic layer was 0.094mm. The
y+ height, viscous sublayer and turbulent
region can be seen in the following image:
Mesh (domain, wing, close-ups)
The previous image shows the overall
polyhedral mesh of the domain, with a
volumetric control around the wing. This
allows to have a high concentration of cells
around the wing to increase the precision
of the results, whilst having larger cells in
the far field regions to speed up the
computing process. The following images
are close-ups of the volumetric controlled
meshed area and wing surface:
A trim mesh was found to be up to five
times faster to compute than a polyhedral
mesh with the same cell count. The
trimmer option allows a finer control of
each cell size in the three dimensions of
space. The following image shows a trim
mesh with 12 prismatic cells on the surface
of the wing and a volumetric control of the
leading edge:

SRN: 14149217 3
Meshing parameters
Parameter Value
Base size 0.1 m
Number of prism layers 12 around the wing
Surface relative size
(Domain)
25%
Surface relative target
size (Domain)
100%
Number of cells <1.5 million
The domain size was taken to be 7m above
and below the wing, 3m in front and 6m
behind. Lower walls were tested but were
found to interfere with the results because
of the formation of a boundary layer on the
horizontal walls. Research showed that a
bullet shaped domain with a c-grid mesh
around the aerofoil is best suited for
studying external flows around an aerofoil,
but wasn't put into application because of
time constraints.
Physics conditions
Parameter Value
Space 3D
Time Steady
Fluid Gas
Equation of state Constant density
Viscous regime Turbulent
Model k-ε
Velocity 25 m/s
Pressure 101325 Pa
Fluid density 1.226 kg/m3
(constant)
Kinematic viscosity 1.83e-3 Pa.s
Reynolds 1.68e6
Surface area 1 m²
Flow Segregated
Before comparing initial aerodynamic
properties of the wing, the mesh and
physics had to be validated in order to
insure correlation between the numerical
and wind tunnel models. The mesh was
deemed valid if the maximum dynamic
pressure was equal to the experimental
value of 374Pa. Then to validate a certain
mesh and physic property combination, a
more refined mesh was simulated with the
same physics conditions in order to
determine if the solution was mesh
dependant. If the results changed
drastically, that meant that the initial mesh
was not refined enough. This procedure
ensured that the amount of cells in the
mesh was reduced as much as possible so
that computational times were kept at a
minimum without compromising the end
result.
Convergence of results
The results were accepted once the values
in the residual panel decreased below 10-4
and stayed there for over 150 iterations.
Extra checks were performed on the values
of Cd and Cl to see that there was less than
1% change over 150 iterations. This was to
insure that the results were stable. A
typical converged residual plot for a k-ε
model looks like this:
However when simulating the wing at 15°
of AoA, the residuals wouldn't descend
below 10-2
. Moreover, inspection of the lift
and drag plots showed pseudo-sine wave
after a certain amount of iterations.
This suggested that the flow around the
wing was unstable and the ups-and-downs

SRN: 14149217 4
on the graph indicated that a phenomenon
of vortex shedding was occurring. In order
to obtain a constant value for Cd & Cl, the
physics conditions were switched to
'Implicit Unsteady'. This meant that the
transit time of the fluid over the wing had
to be defined. At 25m/s and with a chord
length of 1m, the transit time was found to
be 0.04s. To make sure the simulation
didn't run too long, a max time of 0.6s was
chosen. The drag and lift curves were
monitored and the simulation was stopped
when the average of both values changed
within 1% over a span of 100 iterations.
Plots of velocity contours
Velocity contour around the wing at 5°
AoA: (note how the flow stays attached to
the profile of the wing)
Velocity contour around the trailing edge
at 10° AoA: (notice how the flow is
starting to detach from the wing at the
trailing edge)
Velocity contour around the wing at 15°
AoA:
This image shows that the air flow has
detached from the upper surface of the
wing, thus creating a turbulent flow. The
following image shows in red the point
where the air flow separates from the wing
body and the subsequent region of
circulating flow beyond:
Experimental & numerical results
Experimental & numerical pressure
distribution at 0° AoA:
-250
-200
-150
-100
-50
0
50
0 0,2 0,4 0,6 0,8 1
Numerical Experimental

SRN: 14149217 5
As we can see from the curves, the
correlation at 0° of angle of attack (AoA)
is not good, with only the trailing edge
giving satisfactory results. This can be
explained mainly by the roughness of the
CAD wing model. However, the upper
portion of the curves at 5°,10° and 15°,
which correspond to the lower part of the
wing, are very closely matched. The
differences with the upper surface are more
critical, but the trend seems to be well
established. We should note that at
𝑥
𝑐
<
0.2, the numerical model seems to
contradict the wind tunnel values for the
upper surface. The leading edge of the
wing being a sensitive area, a slight
difference in the position of the localised
negative pressure are will fundamentally
change the results obtained. This is
especially true at 15° of AoA because the
pressure gradients imposed on the
boundary layers become more severe and
separation on the upper layer occurs. This
means that the wing has stalled and a
region of circulating flow is formed over
the upper surface of the wing.
The following results show the variation of
the coefficients of lift (Cl) and drag (Cd)
versus different angles of attack.
The graph shows that both coefficients
grow in a linear fashion up to around 10°
AoA. Then between 10° and 15° AoA, the
lift coefficient drops as the drag coefficient
increases substantially. This illustrates the
region where the wing stalls, meaning that
there is a loss of lift capacity and an
increase in drag. Further evidence of this
phenomenon can be found in the following
-600
-400
-200
0
200
0 0,2 0,4 0,6 0,8 1
-1400
-900
-400
100
600
0 0,2 0,4 0,6 0,8 1
-1750
-1250
-750
-250
250
0 0,2 0,4 0,6 0,8 1

SRN: 14149217 6
curve of the maximum velocity around the
wing:
Errors and Limitations
As can be seen in table 1 of the appendix,
the relative precision to the numerical
model varies point to point. Without taking
into account the first two tapping points,
the lowest difference between the two
models can be found at points 18 & 19,
where the margin of error is 1.1% & 4%
respectively. At point 12 there is almost a
60% difference between the values. The
average error over the whole wing in this
configuration is estimated to be 20.7%,
which falls within the 15-30% that was
expected before simulations begun. Errors
are inevitable in experimental and
numerical experiments, but differ in their
nature. The sources of error of this
experimental environment come from the
measurements of the angle of attack, free-
stream velocity and surface pressure
readings from the manometer, as well as
the mounting device of the wing. The
sources of error of the CFD model first
come from the numerical model of the
aerofoil, which didn't have a smooth
profile that created localised negative
pressure zones as seen in the appendix
image 1. The turbulent model chosen is a
secondary source for errors, then the input
parameters, mesh quality and domain size
all contribute in the precision of the CFD
model.
Whilst a wind tunnel model may give
results that closely approach those
expected from a full scale model, the cost
of running these tests have pushed
aerodynamicists to explore the domain of
CFD. Even though no numerical model can
predict air flow with a 100% accuracy rate,
more often than not the results fall within a
satisfactory range to the real model.
However to get good results on complex
structures, the structure has to have a fine
mesh. More often than not, there has to be
a trade off between the number of cells of a
mesh and the computational time required
to simulate the model.
Conclusion
 Computational Fluid Dynamics is a
useful engineering tool for
approximating fluid flows.
 However, the results given need to
be analysed to make sure they
make sense, because different
results can be obtained depending
on the turbulence model you are
using. I found that using a k-ε
turbulence model gives relatively
accurate results in a short amount
of time. Whilst using a more
sophisticated model such as the k-ω
turbulence model requires more
processing power and doesn't
necessarily give better results than
the k-ε model.
 The wing gains lift and drag force
in a linear fashion up to around 10°.
After, lift drops off and drag
increases further, indicating the
stall point of the wing to be
between 10° & 15°.
0
10
20
30
40
50
60
0 5 10 15
Velocity(m/s)
Angle of Attack (deg)
Max Velocity

SRN: 14149217
7
References
Validation of STAR-CCM+ for External
Aerodynamics in the Aerospace Industry,
CD-Adapco
Star South East Asian Conference 2012
Best Practices: Volume Meshing, Kynan
Maley
CFD for aerodynamics (practice) & CFD
for aerodynamics (aerofoil practice)
NACA-4415, Dr. Esteban Ferrer
Convergence Problems in CFD Models: A
Case Study, Gerald Recktenwald
Understanding the Turbulence Models
available in Autodesk Simulation CFD,
https://www.youtube.com/watch?v=Yf2iV
ABc8cg
Appendix A
Point Numerical Experimental Error %
3 -1314,4 -155,7 N/A
4 -990,3 -56,1 N/A
5 -437,9 -921,9 52,5
7 -343,9 -392,4 12,4
8 -278,0 -305,2 8,9
9 -175,2 -255,4 31,4
10 -97,5 -218,0 55,3
11 -19,1 12,5 -53,4
12 17,5 43,6 59,8
13 38,2 68,5 44,3
14 35,6 56,1 36,6
15 27,6 49,8 44,5
16 -21,7 49,8 56,5
17 53,4 37,4 -42,8
18 101,7 105,9 4,0
19 126,0 124,6 -1,1
20 160,5 180,7 11,1
21 229,1 261,6 12,4
22 327,4 373,8 12,4
23 349,8 485,9 28,0
Table 1: Experimental vs Numerical results at 10° AoA

SRN: 14149217
8
Image 1: position of localised negative pressure zones
Image 2: Streamlines at 10° AoA
Image 3: Streamlines at 15° AoA
Image 4: Velocity distribution: evidence of viscous sublayer on top surface

Example_Aerodynamics

Recommended

Recommended

More Related Content

What's hot

What's hot (20)

Similar to Example_Aerodynamics

Similar to Example_Aerodynamics (20)

Example_Aerodynamics