See discussions, st ats, and author pr ofiles f or this public ation at : https:www .researchgate.ne tpublic ation326583896 [625171]

See discussions, st ats, and author pr ofiles f or this public ation at : https://www .researchgate.ne t/public ation/326583896
CFD Simulation of the Air Flow arou nd a Car Model (Ahmed Body)
Article · July 2018
DOI: 10.29322/IJSRP .8.7.2018.p7979
CITATIONS
2READS
519
2 author s, including:
Some o f the author s of this public ation ar e also w orking on these r elat ed pr ojects:
Information T echnolog y View pr oject
Measuring the Cost and Benefit of L earning English at Priv ate Univ ersities in K urdist an View pr oject
Thabit Hassan Thabit
Nine vah Univ ersity
51 PUBLICA TIONS    42 CITATIONS    
SEE PROFILE
All c ontent f ollo wing this p age was uplo aded b y Thabit Hassan Thabit on 04 A ugust 2018.
The user has r equest ed enhanc ement of the do wnlo aded file.

International Journal of Scientific and Research Publications, Volume 8, Issue 7, July 2018 517
ISSN 2250 -3153
http://dx.doi.org/10.29322/IJSRP.8.7.2018.p7979 www.ijsrp.org CFD Simulation of the Air Flow around a Car
Model (Ahmed Body)

Senan Thabet*, Thabit H. Thabit**

*University of South Wales, Cardiff, UK
**Ninevah University, Mosul, Iraq

DOI: 10.29322/IJSRP.8.7.2018.p7979
http://dx.doi.org/10.29322/IJSRP.8.7.2018.p7979

Abstract — this paper describes the flow simulation focuses on
the simulation around Ahmed body car with slant angle of 40°.
Computational Fluid Dynamics (CFD) is the proper approach to
deal with these complicated equations and obtain the numerical
solutions of these complicated flows equations .
The researchers conclude that CFD simulation has been carried
out to investigate the flow characteristics over a model car (Ahmed Body). The aim was to calculate the aerodynamic coefficients from
the CFD simulation and compared them with t he available
expe rimental data. The numerical results are agreed in decent way
with experimental data.

Keywords — CFD , Ahmed Body , Air Flow , Simulation
INTRODUCTION
This paper is investigating the flow simulation focuses on
the s imulation around Ahmed body car with a slant angle of
40° (CL= 0.037, CD = 0.32 & CM= 0.036).
From the literature review, slant angle of 40° is not the ideal
angle for Ahmed car body. However, the literature shows that
the proper angles lie between 10 -25°.
In this analysis, a realizable k -ε mod el with 2nd order
accuracy. The flow governing equations within a CFD solver
(ANSYS -Fluent) will be applied.
These are the continuity, momentum and energy equations.
These equations are non -linear, partial differential equations
(PDE’s) and high orders, h ence the analytical solution is
impossible to obtain, (Saad & Ragavan, 2013) . Computational
Fluid Dynamics (CFD) is the proper approach to deal with these complicated equations and obtain the numerical
solutions of these compl icated flows equations (Kuzmin,
2010) .
CFD
APPROACH AS DESIGN TOOL IN AUTOMOTIVE INDUSTRY
CFD simulations is an efficient tool in automatic industry
used extensively for design. This allows the designers to
obtain a quick and proper analysis before go ahead to the final step. Recently, CFD approach has been adopted effectively
within the automotive industry, with several new methods for car design (Smith, 2008) .
CFD analysis in car industry is used in the determination of
the applied forces and that of the vehicles wake during
moving. CFD also is used to analyze the effect of wake on the
vehicle’s efficiency and capability in comparison with other
cars (Thabet and Thabit, 2018) . Figure 1 is an e xample that
indicating how CFD can be used effectively in the context of vehicle design. It shows the flow paths (in terms of velocity magnitude) emanating from the wing -mirror structure of the
Formula -1 racing car, and how it flows over the whole
geometry .

Fig. 1. CFD simulation for Formula- 1 Racing Car (Smith, 2008)
In vehicle’s industry, Ahmed Car Body is the standard
model that can be used as validating case, in industry and CFD simulation (Davis, 2015) . Ahmed Body is a generic car -type
bluff body with a slant back has different angles from 0 – 40
degree. It is usually used as a benchmark test case for simulating the external aerodynamic flow characteristics over a car model (Hinterberger, et al., 2004).
M
AIN COMPONENTS IN A CFD SOLVER
CFD tool has three main components that is used to handle
the object from the start point till analyzing the results (Thabit
and Younus , 2018) These components can be summarized a
follow:
A. Pre-Processing:
This involves creating the geometry, computational domain

International Journal of Scientific and Research Publications, Volume 8, Issue 7, July 2018 518
ISSN 2250 -3153
http://dx.doi.org/10.29322/IJSRP.8.7.2018.p7979 www.ijsrp.org and meshing. Meshing is to discretising the computational
domain into small control volumes, which are known as cells.
The solution accuracy is a function of the number of
generating cells in the computational domain.
B. The Solver:
This is the main part in the CFD simulation, where the flow
governing equations will be discretised and solved.
C. Post-processing:
This is the final step in the CFD simulation process, which
deals with extracting the important flow parameters such as
velocity, density, pressure and forces. The simulation results
will be compared to the experimental data and other numerical
simulations .
AIMS & OBJECTIVES
The aim of this assignment is to perform a mathematical
and CFD analysis on the flow over Ahmed Body and
compared the numerical results with the available
experimental data. The study will be carried out using both Solidworks and ANSY S software to create the geometry and
obtain the numerical solution, respectively.
P
ROBLEM ASSUMPTIONS
From the given data in the assignment, the follow points
will be assumed during the CFD simulation of the present problem. There is no heat transfer be tween the flow and the
geometry. Air velocity at the inlet section is constant value
during the solution. All the object boundaries will be dealt as
walls with no slip shear condition. Because the Mach number is less than 0.3, hence the flow will be assume d as
incompressible flow.
N
UMERICAL METHODS :
D. Governing Equations:
To simulate the incompressible flow, Navier -Stokes
equations for this flow type will be solved. The form of these
equatio ns based on the flow assumption follows:
1) Continuity Equation:

𝜕𝑝
𝜕𝑡+𝜕(𝜌𝑢)
𝜕𝑥+𝜕(𝜌𝑣)
𝜕𝑦+𝜕(𝜌𝑤)
𝜕𝑧=0
For an incompressible flow
∂ρ
∂t=0, ∇∙�ρV��⃗�=0

Thus;
∂u
∂x+∂v
∂y+∂w
∂z=0
Where,
ρ=C, ∇∙V��⃗=0
2) N-S Equations:
a) X-direction component: ∂(ρu)
∂t+∇(ρuV)=−∂p
∂x+∂τxx
∂x+∂τyx
∂y+∂τzx
∂z+ρfx
b) Y-direction component:
𝜕(𝜌𝑣)
𝜕𝑡+∇(𝜌𝑣𝑉 )=−𝜕𝑝
𝜕𝑦+𝜕𝜏𝑦𝑥
𝜕𝑥+𝜕𝜏𝑦𝑦
𝜕𝑦+𝜕𝜏𝑧𝑦
𝜕𝑧+𝜌𝑓𝑦
c) Z-direction component:
𝜕(𝜌𝑤)
𝜕𝑡+𝛻(𝜌𝑤𝑉 )=−𝜕𝑝
𝜕𝑧+𝜕𝜏𝑧𝑥
𝜕𝑥+𝜕𝜏𝑦𝑧
𝜕𝑦+𝜕𝜏𝑧𝑧
𝜕𝑧+𝜌𝑓𝑧

E. Boundary Conditions
The following boundary conditions are applied during the
solution in ANSYS -Fluent.
• Velocity -inlet BC: Inlet plane.
• Symmetry BC: Enclosure surfaces (no -slip conditions).
• Walls BC: Road and object surfaces.
• Pressure -outlet BC: Outlet plane.
F. Flow Inlet Parameters:
μ=1.789 x 10- 5 kg/m.s.
ν=15.13 x 10- 6 m2/s.
ρ= 1.225 kg/m3.
V = 40m/s.
Re = 768,000 (based on object’s height).
I ≤ 0.25%
G. Car Model Geometry:
Figure 2 shows the layout of the geometry provided in the
assignment cover sheet for Ahmed Body Car with a slant
angle ϕ equals to 40°. From the figure below, the horizontal
length covered by the slant (L) and its height (H) can be calculated as follow:

Fig. 2. Layout of Ahmed Body
𝑐𝑜𝑠𝜑=ℎ𝑜𝑟𝑖𝑧𝑜𝑛𝑡𝑎𝑙 𝑑𝑖𝑠𝑡𝑎𝑛𝑐𝑒 𝑐𝑜𝑣𝑒𝑟𝑒𝑑 𝑏𝑦 𝑠𝑙𝑎𝑛𝑡 (𝐿)
𝑆𝑙𝑎𝑛𝑡 𝑙𝑒𝑛𝑔𝑡 ℎ
𝑐𝑜𝑠40=𝐿
222
𝐿=170 .06 𝑚𝑚
Hence,
𝑥=1044 −170 .06= 873 .94 𝑚𝑚

𝑠𝑖𝑛𝜑=𝑣𝑒𝑟𝑡𝑖𝑐𝑎𝑙 𝑑𝑖𝑠𝑡𝑎𝑛𝑐𝑒 𝑐𝑜𝑣𝑒𝑟𝑒𝑑 𝑏𝑦 𝑠𝑙𝑎𝑛𝑡
𝑠𝑙𝑎𝑛𝑡 𝑙𝑒𝑛𝑔𝑡 ℎ
𝑠𝑖𝑛40=𝐻
222
𝐻=142 .70 𝑚𝑚
Hence,

International Journal of Scientific and Research Publications, Volume 8, Issue 7, July 2018 519
ISSN 2250 -3153
http://dx.doi.org/10.29322/IJSRP.8.7.2018.p7979 www.ijsrp.org 𝑧=288 −142 .70=145 .30 𝑚𝑚
Using Solidworks software, CAD model for Ahmed Body
is created and exported with IGS extension to be dealt in
ANSYS Workbench. Figure 3 shows the Car Model Geometry
for Ahmed Body.

Fig. 3. Ahmed Car Body CAD Model
H. Computational Domain:
ANSYS software tools (workbench, Design Modular,
Meshing tool & Fluent solver) are used to carry out the flow
simulation.
Figures 4 a nd 5 show a screenshot during preparing the
solution and creating the enclosure by using ANSYS
workbench, and Design Modular, respectively.

Fig. 4. Fluent Solver

Fig. 5. Enclosure Option Box
Figure 6 shows the Car Model with the enclosure created in
Design Modular.
Fig. 6. Geometry and Enclosure
Figure 7 shows the Boolean operation on Ahmed Body and
fluid body.

Fig. 7. Boolean operation on Ahmed Body and f luid body
I. Meshing:
The length of the first cell away from the surface (y) to
calculate effectively the wall shear stress during the simulation
should be calculated carefully. To do so, Y+ calculations
should be performed to calculate the value of (y) before start
meshing process .
1) Reynolds Number (Re):
𝑅𝑒= 𝜌𝜈𝑙
𝜇=𝜈𝑙
𝑣
𝑅𝑒= 40×0.288
15×10−6
𝑅𝑒= 768, 000
2) Skin-Friction Coefficient (Cf):
𝐶𝑓=[2𝑙𝑜𝑔 10(𝑅𝑒𝑥)−0.65]−2.3
𝑓𝑜𝑟 𝑅𝑒𝑥<109
𝐶𝑓=[2log 10(768 ,000 )−0.65]−2.3
𝐶𝑓=3.925 ×10−3
3) Wall Shear Stress (τw):
𝜏𝑤=𝐶𝑓×1
2𝜌𝑈𝑓𝑟𝑒𝑒𝑠𝑡𝑟𝑒𝑎𝑚2
𝜏𝑤=(3.295 ×10−3)×12×1.225 ×402

International Journal of Scientific and Research Publications, Volume 8, Issue 7, July 2018 520
ISSN 2250 -3153
http://dx.doi.org/10.29322/IJSRP.8.7.2018.p7979 www.ijsrp.org 𝜏𝑤=3.847 𝑃𝑎
4) Friction Velocity:
𝑢∗=�𝜏𝑤
𝜌
𝑢∗=�3.847
1.225
𝑢∗=1.772 𝑚/𝑠
For most near -wall modeling , Y+ ≈ 1.0. (Salim & Cheah,
2009)
Therefore,
5) Wall Distance (y):
𝑦=𝑦+𝜇
𝜌𝑢∗
𝑦=1.0×(1.789 ×10−5)
1.225 ×1.772
𝑦=8.241 ×10−6 𝑚
Therefore, the boundary layer thickness (wall Distance) for
this analysis is 8.241×10 -6 m.
Figure 8 shows screen shots of the final mesh used in the
present analysis.

Fig. 8. Screen shots of the final mesh
The maximum number of elements (cells) generated in this
grid is about 500,000 cells; since this is the allowable number
of cells you can generate using the student license.
SOLUTION PROCEDURES :
J. CFD Model Set -Up:
Figures 9, 10, and 11 show screen shots of the solution
general setting model selection and turbulence model in
ANSYS Fluent solver for the investigated flow, respectively.
Fig. 9. Solver general setting

Fig. 10. Model selection

International Journal of Scientific and Research Publications, Volume 8, Issue 7, July 2018 521
ISSN 2250 -3153
http://dx.doi.org/10.29322/IJSRP.8.7.2018.p7979 www.ijsrp.org
Fig. 11. Turbulent model selection
Figures 12, 13, and 14 show screen shots for the material
setting boundary conditions and reference values in ANSYS
Fluent solver for the investigated flow respectively.

Fig. 12. Air properties
Fig. 13. Boundary Conditions

Fig. 14. Reference Values
K. Numerical Schemes:
The numerical schemes used in the current simulatio n can
be summarized as follows methods :
• Coupled Scheme: This scheme is used for Pressure –
Velocity Coupling Method, which enables the full
pressure based solver, which has superior
performance.
• Least -Squares Cell -Based: This is used for the
gradients within the interpolation methods. This scheme has the same accuracy as the node -based
gradients, however, is less computationally intensive.
• Second -Order Upwind: The scheme is used for
interpolation process, which pressure, momentum
and turbulence act upon. This will give better accuracy.
L. Solution Controls :
Figures 15, 16 and 17 show screen shots for the solution
control residual monitoring and solution initialization,
respectively.

International Journal of Scientific and Research Publications, Volume 8, Issue 7, July 2018 522
ISSN 2250 -3153
http://dx.doi.org/10.29322/IJSRP.8.7.2018.p7979 www.ijsrp.org
Fig. 15. Solution controls parameters

Fig. 16. Residuals monitoring
Fig. 17. Solution initialisation
RESULTS ANALYSIS :
M. Convergence History:
Figure 18 shows a screen shot from the solution
convergence history at about 250 iterations.

Fig. 18. Convergence history
N. Static Pressure Contours:
Figure 19 shows a screen shot of the static pressure
contours around Ahmed Body. From the figure, it can be seen
that the highest value of static pressure is located at the centre
of the oncoming Ahmed body and the minimum value is
located the separated flow region.

Fig. 19. Static pressure contours
O. Velocity Magnitude
Figure 20 shows a screen shot of the velocity magnitude
pressure contours around Ahmed Body.

International Journal of Scientific and Research Publications, Volume 8, Issue 7, July 2018 523
ISSN 2250 -3153
http://dx.doi.org/10.29322/IJSRP.8.7.2018.p7979 www.ijsrp.org
Fig. 20. Velocity magnitude contours
P. Axial Velocity
Figure 21 shows a screen shot of the contours of axial
velocity component of the flow around Ahmed Body.

Fig. 21. Axial- velocity contour
Q. Pressure Coefficient:
Figure 22 shows a screen shot of the pressure coefficient
distribution on the top surface of Ahmed Body .

Fig. 22. Pressure coefficient plot
R. The plot Comparison with Experimental Data
Table 1 shows the values of the important parameters
obtained from the simulation. TABLE I . VALUES OF THE IMPORTANT PAR AMETERS
Outputs Value
Coefficient of Lift 0.036860
Coefficient of Drag 0.32346
Coefficient of Moments 0.035953
Vertex Average of Velocity Magnitude 5.4590 ms -1
K 0.00019799
Epsilon 0.00057902

Table 2, figure 23 and figure 24 show the data from the
experiments.
TABLE II. DATA OF THE EXPERIMENTS .
Rear slant angle
(ᵠ) (In Degrees ) Cd Cl
0 2.50031e -01 -1.17457e -01
5 2.37215e -01 -1.4970 9e-02
7.5 2.34631e -01 2.9214 9e-02
10 2.36738e -01 8.2971 0e-02
12.5 2.41644e -01 1.3248 3e-01
15 2.46833e -01 1.8500 1e-01
20 2.61934e -01 2.8362 2e-01
30 2.97872e -01 3.4778 3e-01
35 2.94980e -01 2.0550 2e-01
40 2.5036 0e-01 8.36791e -01

Fig. 23. Experimental CD (Banga, et al., 2015)

International Journal of Scientific and Research Publications, Volume 8, Issue 7, July 2018 524
ISSN 2250 -3153
http://dx.doi.org/10.29322/IJSRP.8.7.2018.p7979 www.ijsrp.org
Fig. 24. Experimental velocity magnitude (Banga, et al., 2015)
CONCLUSIONS AND RECOMMENDATIONS
CFD simulation has been carried out to investigate the flow
characteristics over a model car (Ahmed Body). The aim was
to calculate the aerodynamic coefficients from the CFD
simulation and compared them with the available experimental
data. The numerical values obtained were; CL=0.0368,
CD= 0.323 and CM= 0.036, respectively. The numerical results
are agreed in decent way with experimental data.
REFERENCES
[1] Anderson, J. D. et al., 2009. Computational Fluid Dynamics: An
Introduction. Berlin: Springer Berlin Heidelberg.
[2] ANSYS, 2006. Modeling Turbulent Flows -Introductory FLUENT
Ttaining. [Online] Available at:
http://www.southampton.ac.uk/~nwb/lectures/GoodPracticeCFD/Article
s/Turbulence_Notes_Fluent- v6.3.06.pdf
[Accessed 19 April 2017].
[3] ANSYS, 2010. Introduction to ANSYS FLUENT – Lecture 5: Solver
Settings. [Online] Available at:
http://imechanica.org/files/fluent_13.0_lecture05 -solver -settings.pdf
[Accessed 20 April 201 7].
[4] Banga, S. et al., 2015. CFD Simulation of Flow around External
Vehicle: Ahmed Body. IOSR Journal of Mechanical and Civil
Engineering, 12(4), pp. 87- 94.
[5] Benson, T., 2014. Boundary Layer. [Online] Available at:
https://www.grc.nasa.gov/WWW/BGH/boundlay. html
[Accessed 18 April 2017].
[6] Thabit, Thabit H., and Younus, Saif Q., 2018, Risk Assessment and Management in Construction Industries, International Journal of
Research and Engineering, Vol. 5, No. 2, pp. 315- 320.
[7] Davis, N., 2015. FLUENT Lab Exercise 10 – Ahmed Car Body, Illinois:
Computational Science and Engineering Illinois.
[8] Dempster, C. M., 2016. Wind Tunnel Testing of a NACA Aerofoil to
Validate CFD Modelling Results Using ANSYS FLUENT, Pontypridd:
University of South Wales.
[9] Dobrev, I. & Massouh, F., 2014. Investigation of Relationship Between
Drag and Lift Coefficients for a Generic Car Model. Sozopol,
BULTRANS. [10] Dumas, L., 2011. CFD -based Optimization for Automotive
Aerodynamics. Paris: Université Pierre et Marie Curie.
[11] Flowmeter Directory, 2017. Reynolds Number Calculator. [Online]
Available at:
http://www.flowmeterdirectory.com/reynolds_calculator.html
[Accessed 18 April 2017].
[12] Hewitt, G. F., 2010. Computational fluid dynamics. [Online] Available
at:
http://www.thermopedia.com/content/279/
[Accessed 13 April 2017].
[13] Hinterberger, C., García -Villalba, M. & Rodi, W., 2004. Large eddy
simulation of flow around the Ahmed Body, Karlsruhe: University of
Karlsruhe.
[14] Kuzmin, D., 2010. A Guide to Numerical Method s for Transport
Equations. Nurenburg: Friedrich -Alexander -Universität Erlangen –
Nürnberg.
[15] Lanfrit, M., 2005. Best Practice Guidelines for Handling Automotive
External Aerodynamics with FLUENT, Darmstadt: Fluent Deutschland
GmbH.
[16] Liu, Y. & Moser, A., 2001. N umerical Modeling of Airflow over the
Ahmed Body, Zentrum: Swiss Federal Institute of Technology.
[17] Meile, W. et al., 2011. Experiments and numerical simulations on the
aerodynamics of the Ahmed body. CFD Letters, 3(1), pp. 32- 39.
[18] Mohamed, M., 2017. NG4H246 -Further Computational Fluid
Dynamics -Car Model Aerodynamics using ANSYS Software Assignment
Cover Sheet, Pontypridd: University of South Wales.
[19] Rakshith, K. N. & Mahesh, T. S., 2015. Computations Study of
Turbulent Flow around a Generic Car Body (Ahmed Bod y).
International Journal for Scientific Research and Development, 3(09), pp. 665- 669.
[20] Saad, T. & Ragavan, S., 2013. Historical perspective. [Online]
Available at:
http://www.cfd -online.com/Wiki/Historical_perspective
[Accessed 21 April 2016].
[21] Salim, S. M . & Cheah, S. C., 2009. Wall y+ Strategy for Dealing with
Wall -Bounded Turbulent Flows. Hong Kong, IMECS.
[22] Sirius CFD, 2012. ANSYS Fluent for Vehicle Aerodynamics. [Online]
Available at:
https://www.youtube.com/user/eoescipy/videos
[Accessed 20 April 2017].
[23] Sleigh, P. A., 2008. Laminar and Turbulent Flow. [Online] Available at:
http://www.efm.leeds.ac.uk/CIVE/CIVE1400/Section4/laminar_turbulen
t.htm
[Accessed 18 April 2017].
[24] Thabet, Senan, and Thabit, Thabit H., 2018, Computational Fluid
Dynamics : Science of the Future, International Journal of Research and
Engineering, Vol.5, No. 6, pp. 430- 433.
[25] Smith, R., 2008. Car Design and CFD. [Online] Available at:
http://www.symscape.com/blog/car -design -cfd
[Accessed 13 April 2017].
[26] The Engineering ToolBox, 2017. Laminar, Transitional or Turbulent
Flow. [Online] Available at:
http://www.engineeringtoolbox.com/laminar -transitional- turbulent -flow-
d_577.html
[Accessed 18 April 2017].
[27] Visavale, G., 2006. Reviewing Governing Equations of Fluid Dynamics. [Online] Available at:
https://www.learncax.com/knowledge- base/blog/by –
category/cfd/reviewing -governing- equations -of-fluid -dynamics
[Accessed 20 April 2017].

International Journal of Scientific and Research Publications, Volume 8, Issue 7, July 2018 525
ISSN 2250 -3153
http://dx.doi.org/10.29322/IJSRP.8.7.2018.p7979 www.ijsrp.org

View publication statsView publication stats