AERODYNAMIC DEVELOPMENT OF THE SEGURACING F1-R01 PROTOTYPE USING CFD

Undergraduate thesis
AERODYNAMIC DEVELOPMENT OF THE SEGURACING F1-R01 PROTOTYPE USING CFD
Mouhamed Akrem Mouffouk
University H.L of Batna
Department of Mechanical Engineering
Specialty Aeronautical Engineering
2013/2014
Batna Algeria
Copyright this thesis cannot be reproduced or quoted extensively from without first obtaining permission in writing from the author, the content must not be changed in any way without the formal permission from the auther.
Author email: mouffoukma@hotmail.fr

ACKNOWLEDGEMENTS:
First i would like to thank my partner in this work Jose Gallego Segura for giving me the opportunity to work on full car and for his efficient help and for sharing a lot of ideas in the design of F1 car
I would also like to give my most sincere thank to Romuald Bavar my technical support from CD-adapco and for all the CD-adapco team (Satish Bonthu, Tammy deBoer ...) for giving me the opportunity to run STAR-CCM+ on my laptop so i could work from home.
Without forgetting my dear friends from F1 industry Luca Furbatto, Leigh Evans, Frédéric Jean-Laurent, Abderrahmane Fiala, Eelke De Groot, Nicolas Perrin, Mattia Brenner. And special thank to my university family specially to Pr Kamel Zidani for supporting me during all the undergraduate degree period,and my supervisor Dr Messaoudi Laïd, Dr Nabil Bessanane, Dr Ghazaly Mebarki, Pr Mohamed Si-Ameur. And in the end many thanks to my wonderful family my dear parents my dear sister and brother not only for their support on this project but also to understand my passion and dedication to Motorsport industry, also my dear friends Salah Benyahia and Rami Yousfie Tarek Jomaa and all who has supported me during this work.

Abstract
Over the past 30 years, the race car industry has become a leader of technology innovation, a training ground for highly qualified engineers in the different disciplines from all over the world, an integral part of the high tech engineering industry. The nature of the industry is such that there is a constant need for performance improvement. Among the various factors which influence the performance of a car, such as powertrain, driver, weight, tires and aerodynamics, aerodynamics represents a major area that a constructor can invest in, and improve the car performanc.
During this thesis we will understand the CFD development of a Formula 1 car step by step.

Contents
I. F1 Aerodynamics
1 What is Formula 1 Aerodynamics. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .9
2 Why F1 aerodynamics?. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10
2.1 Wind Tunnels. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10
2.2 CFD. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11
2.3 Project cycle. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .13
II. Preprocessing
3 Introduction. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .15
4 Surface repair. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .16
5 Computational domain creation. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .20
6 Mesh generation. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .21
6.1 Gridtype. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 22
6.2 Cell aspect ratio. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .22
6.3 Cell skewness.. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .22
7 Turbulent flows. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 23
7.1 Turbulent near wall flow. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .23
7.1.1 Linear or viscous sublayer. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .24
7.1.2 Log-law layer. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 24
7.1.3 Outer layer. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .24
7.2 Near wall treatment. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .25
7.2.1 Near wall function. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .25
7.2.2 Wall functions. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .25
8 Volumetric mesh. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ...26
8.1 General purpose of the mesh types. . . . . . . . . . . . . . . . . . . . . . . . . . . . .28
8.1.1 Tetrahedral meshes. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 28
8.1.2 Polyhedral meshes. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 28
8.1.3 Trimmed cell meshes. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 28

8.2 Specific regions mesh refinement. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 28
8.3 Mesh setting. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 29
8.3.1 Prism Layer Settings. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .29
8.3.2 Aero Surfaces. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .29
8.3.3 Ground.. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .29
9 Mesh analysis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .31
9.1 Volume change. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .31
9.2 Skewness angle. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .31
9.3 Wall treatment Y+. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 33
10 Imposing boundary conditions. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 34
10.1 Boundary conditions. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 34
10.1.1 Windtunnel inlet. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 34
10.1.2 Windtunnel outlet. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .34
10.1.3 Walls. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 34
10.1.4 Symmetry. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35
10.1.5 Fluids. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .35
10.2 Setting boundary conditions. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35
10.2.1 Inlet. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .35
10.2.2 Outlet. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 36
10.2.3 Floor. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 36
10.2.4 Symmetry. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .36
10.2.5 Tire. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 36
10.2.5.1 ROTATING WALL . . . . . . . . . . . . . . . . . . . . . . . 36
10.2.5.2 MULTIPLE REFERENCE FRAMES. . . . . . . . . . . .36
10.2.6 Front wheel. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 37
10.2.7 Rear wheel. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .37
III. Solver
11 Numerical methods. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 39
12 Turbulence models settings. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 39
12.1 Turbulence Models & Settings. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .41

12.1.1 K-Epsilon. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 41
12.1.2 K-Omega. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 41
12.1.3 Spalart-Allmaras. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .41
13 The solver. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .41
13.1 The segregated solver. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 42
13.2 The coupled solver. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .43
14 Judging convergence. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 44
IV. Postprocessing
15 Introduction. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 47
16 The Front Wing(FW) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .50
16.1 How important is the front wing? . . . . . . . . . . . . . . . . . . . . . . . . 50
16.2 Initial front wing. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .53
16.3 Updated front wing. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 55
17 Front tires. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 57
17.1 The wake of the front tire. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 57
17.2 The wake in the Z direction. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 59
17.3 Wake controle. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .61
17.4 Front tire aero values. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 62
18 Floor. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 63
19 Rear Wing (RW) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 64
20 Full car analysis.. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .67
21 Car rear wake. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .68
22 Conclusion. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .73
23 Recommendations. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .74
24 References. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 75

AERODYNAMIC DEVELOPMENT OF THE SEGURACING F1-R01 PROTOTYPE USING CFD 9
1 What is Formula 1 Aerodynamics:
Weighing just 605 kilograms in race trim, propelled by an engine that delivers in excess of 800 horsepower, a Formula 1 car is regularly subjected to braking and cornering forces in excess of 5g, The maximum speed depends on aerodynamic setup, which changes from circuit to circuit, but is usually around 340 kph, At that speed, the geometry of the car produces downforce of around two tons,This invisible force pushes the car into the ground, increasing traction and allowing the car to maintain higher cornering speeds and generate greater braking force. Since both lift (in this case negative lift) and drag are functions of velocity squared, the ability to deliver an efficient aerodynamic package on raceday is a critical ingredient in reducing individual lap times by the fractions of a second that combined are the difference between winning and losing the race. With engine development now frozen and only one tyre manufacturer supplying the whole grid, the aerodynamic package has become a single most important component of race car performance, The development of a car’s aerodynamic package typically relies on an extensive wind tunnel programme, conducted in parallel with, and to some extent driven by, an even more extensive Computational Fluid Dynamics (CFD) programme. In this mode CFD is largely used as a coarse filter, examining many possible design variants, from which only the best will be tested in the wind-tunnel [1].

2 Why F1 aerodynamics?
It is not immediately obvious how the intense aerodynamic development of small racing cars, festooned as they are with drag producing wings, can be of any relevance to society. However, the investment that the teams have made in aerodynamic development continues to drive technology that is of significant environmental importance.
All the teams make a large investment in aerodynamic competence as the car with the best aerodynamic package generally wins the championship. Although our racing cars look nothing like road cars, buildings, wind generators or aeroplanes, all of these fields require significant aerodynamic expertise, and all of them benefit to some degree from the rapid development of aerodynamic understanding that Formula 1 engenders. For example:
2.1 Wind Tunnels:
For many years, to be successful, a Formula 1 team must have mastered the skills necessary to maximise the “ground effect” downforce that can be generated between the underside of the car and the road. Pursuit of this downforce has given rise to many, many millions of pounds of investment by the teams in wind tunnel technology that allows this tricky area of design to be accurately exploited. Although neglected for many years by the mainstream road car industry, the aerodynamic importance of the region between the underside of the car and the ground has recently come to the fore, as it is clear that careful design in this region can yield substantial fuel consumption benefits through drag reduction. Major road car manufacturers are now using precisely the same wind tunnel technology pioneered and perfected by Formula 1 ten years earlier to allow them to exploit this benefit [2].
Figure 1: Sauber F1 team Wind Tunnel facility.

2.2 CFD:
The development of Wind Tunnel technology, important though it has been, pales into insignificance alongside the rapid growth of Computational Fluid Dynamics (CFD). With a wind tunnel, experiments are made by blowing wind over a real object in a controlled environment and measuring the aerodynamic forces that arise. In CFD, the same experiment may be conducted in the form of a computer simulation. Although the equations that govern these computations have been understood since the 1930s, they are complex to solve and require the sort of computing power that has only become truly practical in the last 15 years or so.
A huge range of industries benefit from the mastery of aerodynamic design that a successful CFD programme enables. It is probably no surprise that the aerospace, road car and wind turbine industries use CFD in their design process. It might be less obvious that it also brings significant advantage in hundreds of other industries. In fact, in any application where there is any sort of fluid (gas or liquid) flow, CFD can bring benefit. Climate modelling, the force of wind on a building, the way in which medicine is distributed in an inhaler, efficient air conditioning design, transport of gas or liquids in pipelines; the list of applications is truly enormous.
All of these applications benefit, to a greater or lesser extent from the investment that Formula 1 has made in the growing technology of CFD. For a sustained period of around 20 years, the teams in Formula 1 have ploughed money into the development of CFD ,as it has been clear for a long time that mastery of this tool would be a prerequisite for success in the sport. Teams have sponsored the development of improved CFD techniques at top universities and they have also put money directly with the providers of commercial CFD codes to ensure that the considerable challenge of accurately simulating the aerodynamic behaviour of a Formula 1 car has turned from an aspiration to a reality. It would be wrong to pretend that the development of subsonic CFD codes has been the sole responsibility of the Formula 1 industry, but no serious observer of the industry would deny that the combined investment of the teams has been very significant. An example of the positive role that Formula 1 plays in this field can be seen in the relationship that Lotus F1 Team enjoys with Boeing and CD-adapco.
For example at Lotus F1 Team, the aero department makes use of two sets of CFD codes to run virtual simulations on the cars. One code is commercially available from CD-adapco, while the other code is available through the partnership with Boeing.
The Boeing code is highly specific and used for the design of aircraft, but it has significant application within Formula 1. Development of this code at Lotus F1 Team, in partnership with Boeing, has produced industry-leading optimisation software. The potential benefit to Boeing of this development is not trivial: For example, a 1% reduction in drag will reduce an airline’s direct operating costs by 14% due to reduced fuel usage will result in lower CO2 emissions.

The competitive nature of Formula 1 and the desire to extract greater levels of performance from the car has undoubtedly helped to develop the capabilities of CFD software at an everincreasing rate Methods developed by Formula 1 teams for applying CFD to simulate performance can be seen filtering down into passenger car development where more complete and detailed simulations are helping to improve safety at the same time as efficiency.” and from this paragraph we can see clearly how much the F1 is involved in the development of CFD and the specific relation with aeronautical and aerospace engineering [2].
Figure 2: Lotus F1 computational aerodynamic center ENSTONE.
Figure 3: Lotus F1 super computer.

2.3 Project cycle:
The goal of this thesis was developing the aero package of an Formula 1 car prototype using CFD, all the computational process was done using CD-adapco STAR-CCM+ from the geometry preparation and mesh generation through the solver and finley the result analysis.
Another important part of this thesis is the modification of the geometry of the SEGURACING F1-R01. Upon completion of data processing on the vehicle certain key areas have to be pin pointed that require improvement. These changes to the geometry shall be performed by using the CATIA V5 Computer Aided Design (CAD) software package.
From the original model to the final one we have designed more than 30 differents configurations and looking to the large parameters that you can play on we have specified our modifications on the most influenced parts.Front wing Nose and Sidepod.
It should be clear that the SEGURACING F1-R01 undergoes a cycle during which numerous changes to its geometry are made until we achieve the best design. For the sake of clarity, the complete cycle including its stages is set out in figure.
Figure 4: Working method.

II. Preprocessing

3 Introduction:
The main important phase in the CFD it's the mesh, and for this reason i spent a lot of time to generate high quality mesh, in this chapter we will get a look about how we can generate high quality mesh using CD-Adapco STAR-CCM+ from poor CAD geometry.
But before discussing the grid generation process, it should be noted that there has to be a geometric model of the car, This model should be some sort of digital file that can be processed by the grid generation package of interest, there is many different files format can be procedure using mesh generation software the popular one are IGES or STEP and many other from my experience i find that STEP is the best one becouse they protect the model data.
For this work the 3D CAD model is designed using CATIA V5, one of the most popular and advanced softwares in the field of design and many F1 teams use this software to designing there own cars.
The car design is based on the FIA F1 2012 rules (the original model designed by Mr Jose Gallego Segura lead design engineer with several F1 teams), it's full car 1/1 scale with all the extrnal details as shown in figure 5.
Figure 5: Perspective picture of the initial CAD model.

4 Surface repair:
But before starting the mesh generation we need to clean up the geometry, but Why do surfaces need to be prepared [3]?
Imported CAD has too many details. Possible surface errors are:
 Volume is not closed.
 Surfaces overlay each other.
 Surfaces intersect each other.
 Volume is not manifold.
Error figures are:
Figure 6.1: An edge of a face that is not joined to another face [3].
Figure 6.2: an edge belonging to a face pieces a different face at any location [3].

Figure 6.3: The ratio of the distance to the nearest neighbor face proportionale to the size of the face [3].
Figure 6.4: A vertex that is sole join between one surface and another [3].
Figure 6.5: A measure of how perfect a face is, with a perfect face being equilatral in shape [3].

And depending on your problem there is some specific tools to repair your model, manual approche or automated approaches:
What type of surface problems can be repaired manually?
 Free edges.
 Zip edges or fill holes with new triangles.
 Intersecting surfaces.
 Intersect, then delete surfaces.
 Imprint surfaces and edges onto target surfaces/bodies.
 Surfaces can be split and combined to create required boundaries.
And all the other problems can be repaired using the second approche automated approach or the surface wrapper
surface wrapper provides the user with a “closed”, “manifold”, “nonintersecting” surface, starting from a poor quality or too complex CAD surface as shown in figure 7.
Problems commonly fixable by surface wrapping:
 Multiple intersecting parts.
 Surface mismatches.
 Double surfaces.
 Overly complex details.
Or we can use remeshing technics.
The surface remesher is used to re-triangulate an existing surface in order to improve the overall quality of the surface and optimize it for the volume mesh models.
Figure 7: The difference between the imported CAD surface after wrapper and before the wrapper [3].

Figure 8.1: Import 3D CAD model the geometry representation
Figure 8.2: Import 3D CAD model before surface wrapper
Figure 8.3: Import 3D CAD model before surface remeshing

5 Computational domain creation:
Then when we create a full clean surfaces all over the car, we can generate the computational domain, the dimensions of this domain are too important, the boundaries should be set up such that the inlet, outlet and sides are quit far from the car model, to make sure that the air flow near to the bondaries will not influence the air flow over the car, and in the same time you need to respect your computational capabilities (hardware) because large domain equal more cells and in consequence more computatioal time.
There is an efficient estimation to estimate how much your domain need to be, this is what we call it the blockage ratio it's the ratio between frontal area of the car and the Cross Sectional Area of the domain as it showing in the equation (1) . It should be always under a 10%. However, keeping it lower than 7.5% is recommended
(1)
In this study the boundaries should be set up such that the inlet, outlet and sides are:
 7 m upstream
 5 m side to side and above
 18 m downstream
Figure 9.1: 3D view of the car inside the computational domain.

Figure 9.2: Top view of the computational domain.
Figure 9.3: Frontal view of the computational domain.
6 Mesh generation:
To illustrate the importance of grid generation, it’s worth mentioning that up to 70% of the time spent on a CFD case is devoted to creating a good grid, The quality of the mesh to a large extent determines the accuracy and stability of the numerical computation.
In this section we will discuss the mesh generation steps using STAR-CCM+ the requirement of a good mesh, and in the same time the criterion that we need to respect.

6.1 Gridtype:
In general there are four ways to discretize a three-dimensional domain:
 Structured grid which consists of hexahedral cells.
 Unstructured grid which is built up from tetrahedral cells.
 Prismatic grid which results from extruding a two-dimensional unstructured grid into space.
 Hybrid grid which is a combination of 1 and 2 and uses tetrahedral and pyramid cells.
And to sum up, which type of grid layout to choose depends on several factors:
 Ease of generation.
 Available computer resources.
 Required numerical accuracy.
 Required flexibility to change (local) cell resolution.
 Model complexity.
6.2 Cell aspect ratio:
The aspect ratio of a cell is a measure of its stretching. Each cell type has its own definition of aspect ratio:
 Quadrilateral cell aspect ratio is computed from the ratio of the average length and average width. The aspect ratio is always greater than or equal to 1 with a value of 1 representing a square.
 Hexahedral cell aspect ratio is computed from the ratio of the maximum of the length, width, andheightandtheminimumofthelength, width, andheight. The aspect ratio is always greater than or equal to 1 with a value of 1 representing a cube.
 Triangular cell aspect ratio is computed as the ratio of the radius of the cell’s circumscribing circle to 2 times the radius of the inscribed circle
 Tetrahedral cell aspect ratio is computed as the ratio of the radius of the cell’s circumscribing sphere to 3 times the radius of the inscribed sphere.
 Prism aspect ratio is the ratio of the average height of the prism and the average length of the base’s (triangle) edges. The aspect ratio of a prism can be less than 1.
 Pyramid aspect ratio is the ratio of the height of the pyramid and the average length of the base’s (quadrilateral) edges. The aspect ratio of a pyramid can be less than1.
6.3 Cell skewness:
Skewness is defined as the difference between the shape of the cell and the shape of an equilateral cell of equivalent volume. Highly skewed cells should be avoided as they can decrease solution accuracy and even destabilize the solution.

7 Turbulent flows:
Properly resolving a boundary layer around any model requires a fine grid resolution close to the model surface. The actual cell density depends on several factors such as the boundary layer type (laminar or turbulent), the near wall model used and, in case of turbulent flow, the implemented turbulence model. Compared with laminar flows, numerical results for turbulent flows are even more dependent on grid density due to the inherent strong interaction of mean flow and turbulence [4].
7.1 Turbulent near wall flow:
When speaking in terms of turbulent boundary layers, it is common practice to work with dimensionless velocity u+ and distance from the wall y+ defined as follows:
(2)
Here uτ is the so-called friction velocity and is defined as:
(3)
It has been empirically acknowledged that the flow near a model surface can be largely subdivided into three regions as depicted in figure10.
Figure 10: A schematic of the velocity profile in a turbulent boundary layer [4].

7.1.1 Linear or viscous sublayer:
Within the viscous sublayer, the flow is dominated by viscous shear due to the fact that very close to the model wall the fluid is stationary causing turbulent eddying motions to stop. The result is a negligible turbulent shear stress within the extremely thin viscous sublayer (y+ < 5).
Furthermore, the shear stress may be assumed to be approximately constant and equal to the wall shear stress τw throughout the layer. The flow within the viscous sublayer is thus nearly laminar. The following relation between velocity and distance holds for the viscous sublayer [4]:
(4)
7.1.2 Log-law layer:
The log-law layer (30 < y+ < 500) lies outside the viscous sublayer and is characterized by both viscous as well as turbulent effects. The shear stress τ within this region is assumed to be constant and equal to the wall shear stress. In between the viscous sublayer and log-law layer (5 < y+ < 60) the buffer layer is distinguishable in which the viscous and turbulent stresses are of equal magnitude. As far as the log-law layer is concerned we have [4]:
(5)
In which κ, B and E are universal constants for turbulent flows that depend on the roughness of the wall. In case of a smooth wall κ = 0.4, B = 5.5 and E = 9.8.
7.1.3 Outer layer:
The outer layer (y+ > 300) is located far away from the wall and contains inertia dominated flow. Viscous effects are negligible. This leads to the following relation between velocity and distance [4]:
(6)
The viscous sublayer, log-law layer and the buffer layer can be taken together forming the inner region, whereby the outer layer forms the outer region. Even so, the inner region forms only 10 to 20% of the total thickness of the wall layer. This already gives an indication of the required mesh resolution close to the model wall if one wants to directly solve for the turbulence equations.

7.2 Near wall treatment:
Generally there is two approaches to treat the near wall flow gradient and every method have a specific mesh requirements.
7.2.1 Near wall function:
When employing the enhanced wall treatment, all flow variables are directly solved for through the entire near wall region. This means the mesh resolution needs to be fine enough in order to resolve the viscous sublayer. The following mesh requirements hold:
1. When the neer wall treatment is employed with the intention of resolvingthe laminar sublayer,y+ at the wall-adjacent cell should be on the order of y+ = 1. However, a highery+ is acceptable as long as it is well inside the viscous sublayer (y+<5).
2. You should have at least 10 cells within the viscosity-affected near-wall region (Rey < 200) to be able to resolve the mean velocity and turbulence quantities within that region [4].
7.2.2 Wall functions:
When using wall functions, the viscous sublayer and buffer layer are not resolved. This way the mesh resolution needn’t be as fine as in the case of the neer wall treatment thus reducing required computational power.
1. For wall functions, each wall-adjacent cell’s centroid should be located within the log-law layer, (30<y+ <300). A y+ value close to the lower bound y+ = 30 is most desirable.
Figure 11: Near wall treatments [4].

And to get the right treatment of the wall function there is a specific mesh for the region near to the wall that we call it the prism layer mesh.
A prism layer mesh is composed of orthogonal prismatic cells grown next to the wall boundaries in the volume mesh, These cells are required to accurately simulate the turbulence and heat transfer close to the walls and the thickness, number of layers and distribution of the prism layer mesh is determined primarily by the turbulence model used.
Figure 12: Prism layer mesh near to the wall of the front wing.
8 Volumetric mesh:
Now for the volumetric mesh there is a different choices and every type have some advantages and disadvantages some models that can be created using STAR-CCM+ are:
Figure 13.1: Tetrahedral Mesh [3].

Figure 13.2: Trimmed Mesh [3].
Figure 13.3: Polyhedral Mesh [3].

8.1 General purpose of the mesh types:
8.1.1 Tetrahedral meshes:
• Very dissipative.
• Convergence can be slow.
8.1.2 Polyhedral meshes:
• More accurate than tetrahedral meshes.
• Faster convergence than tetrahedral meshes.
• Give a conformal mesh at the interface between separate regions.
8.1.3 Trimmed cell meshes:
• Require less memory to generate than polyhedral mesh.
• Do not give conformal mesh at the interface between separate regions.
From this notes we can judge that the polyhedral mesh is the most advanced mesh and can give us a really accurate results in the turbulent flow but unfortunately it demand a really high research capabilities.
And for this reason i decided to work with trimmer mesh because it's more robust than Tetrahedral Mesh and is less computational research demanding as polyhedral model.
8.2 Specific regions mesh refinement:
As we have a complex geometry so we need to have some mesh regions where we need to use a local volumetric controls to captures the flow gradient vortex and wake, some of these important regions are the wake behind tires the wake in the rear end of the car and the underbody.
In these regions we need to make the mesh delicate as possible the picture shown the volumetric control regions.

8.3 Mesh setting:
Base Size 12 mm
Number Points Around Circle 65
Curvature Refinement on Exterior 4-12 mm
Max Cell Size 3600 % Base
Template Growth Rate
Small Cells Fast
Default Size Slow
Cut off Size 50% Base
8.3.1 Prism Layer Settings:
8.3.2 Aero Surfaces:
Prism Layer Thickness 8 mm
Number of Prism Layers 12
8.3.3 Ground:
Prism Layer Thickness 10 mm
Number of Prism Layers 8

Figure 14: Full car high quality mesh with 12 million cells
From the pictures it's clear that we have a refinement of the mesh in the wake zones to capture the perturbation of the wake.

9 Mesh analysis:
The meshes generated by Star-CCM+ can be diagnosed to control the validity of them. There are three main parameters used to control this: the volume change, the maximum skewness angle and the y+ values.
9.1 Volume change:
Figure 15: The results of the mesh diagnostics report.
We can see that topologically the mesh is valid and has no negative volume cells and this is one of the the main parameters that we need to respect to get a validate and good mesh.
9.2 Skewness angle:
Figure 16: The results of diagnostics report Skewness angle.
The second parameter is the skewness angle we can see that the maximum skewness angle is 72.4 degrees. Star-CCM+ help file states that this value should not be higher than 85 degrees for the mesh to be robust. and 72.4 is really good value for the skewness angle, and

to understand this more we can see this more clearly in the pictures showing the distribution of the skewness angle all over the car.
Figure 17: Distribution of the skewness angle and it's a really good value.

9.3 Wall treatment Y+:
To check the Y+ value, the simulation has to be completed first and this make the presse more difficult and too time consuming to get the right value. Then, a scalar scene has to be created to evaluate the Y+ values on the surface of the vehicle
Figure 18: Y+ distribution all over the car.
From the scalar we can see that the values is between 0 to 65 this means we are modeling the buffer layer, it's not the perfect region but still acceptable.

10 Imposing boundary conditions:
This part deals with imposing required boundary conditions to wind tunnel walls and vehicle boundaries. Boundary conditions (and initial values) are generally required in any numerical simulation to obtain a unique solution.
10.1 Boundary conditions:
STAR-CCM+ offer a wide variety of boundary conditions,this section will throw a light on the boundary conditions that should be specified in simulating the flow around the F1 car applies to any incompressible ground vehicle external aerodynamics.
10.1.1 Windtunnel inlet:
At the windtunnel inlet, velocity inlet boundary conditions are used to define the free stream flow velocity in the computational windtunnel, apart from the flow velocity, other relevant scalar flow properties at the inlet are also defined (such as temperature, pressure, turbulence quantities etc) the following flow properties have to be defined at the velocity inlet:
1. Velocity magnitude and direction.
2. Turbulence quantities (depending on the applied turbulence model).
10.1.2 Windtunnel outlet:
Pressure outlet boundary conditions are used to specify the static pressure at the wind tunnel outlet boundary. The value of the specified static pressure is used only in case of subsonic flow. When locally, the flow becomes supersonic, the pressure as well as all flow quantities will be extrapolated from the flow in the interior. The following flow variables have to be fixed at the pressure outlet boundary:
1. Pressure magnitude.
2. Turbulence quantities.
10.1.3 Wall:
Wall boundary conditions are used to model impenetrable regions in the flow. When modelling viscous flows, the no-slip boundary condition should be enforced at the walls. Flow details in the local flow field determine the calculated shear stress and heat transfer between fluid and wall. Modelling a moving wall is done by specifying the magnitude and direction of its velocity.The following information should be put in with respect to wall boundary conditions:
1. Type of flow (viscous or inviscid).
2. Wall translational and/or rotational velocity magnitude and direction.

3. Wall roughness in case of turbulent flows (optional).
10.1.4 Symmetry:
Symmetry boundary conditions are used when modelling geometrically symmetric objects that reflect an equally symmetric flow solution. As such, symmetry boundary conditions can reduce computational costs significanty, symmetry boundary conditions do not require specification of any flow variable computational interpretation of symmetry boundary conditions is as follows:
1. Zero normal velocity at a symmetry plane.
2. Zero normal gradients of all variables at a symmetry plane
10.1.5 Fluids:
A fluid zone is a group of cells for which all active equations are solved. The only input requires for a fluid zone is the type of fluid material in order to properly set the material properties.
10.2 Setting boundary conditions:
Figure 19: Domain bondaies
10.2.1 Inlet:
 Velocity inlet boundary condition
 Velocity normal to boundary Vinlet = 77.77m/s
 Turbulence intensity I = 1%
 Turbulent viscosity ratio μt/μ = 10

10.2.2 Outlet:
 Pressure outlet boundary condition
 Pressure at boundary p = 0 Pa
 Turbulence intensity I = 1%
 Turbulent viscosity ratio μt/μ = 10
10.2.3 Floor:
 Wall boundary condition
 Translational velocity vector component u = 77.77m/s
10.2.4 Symmetry:
For the sides and the roof we use symmetry condition and we split the domain in the middle of the car and we put symmetry condition in the middle.
10.2.5 Tire:
The turbulence that is caused by the rotating tire during a vehicle cruising could have a large effect on the flow field around the car. In steady-state analysis two different approaches can be chosen: rotating wall or the multiple reference frames.
10.2.5.1 ROTATING WALL APPROACH:
The simplest approach that you can use for modeling a rotating wheel is to assign a tangential velocity to the wall boundaries faces forming the wheel.
10.2.5.2 MULTIPLE REFERENCE FRAMES APPROACH:
A second approach for modeling a rotating wheel in steady-state analysis is the multiple reference frame (MRF). In this approach a separate region enclosing the entire wheel (including rims, spokes, whatever) must be defined and a rotating reference frame must be assigned to that region. This method assumes that all the fluid cells located in that region are rotating.
And looking to our research capabilities we will focus on the first approach because the MRF is more time consuming .
To apply this method:
1. Define a local coordinate system respect to which the wheel is rotating.
2. Assign a tangential velocity to the wall boundary.

10.2.5.3 Front wheel:
 Wheel radius r = 325mm
 Rotation axis (x,y,z) =(0,0,1) for local coordinate system.
 Angular velocity ω = V/r = 239.316rad/s
10.2.5.4 Rear wheel:
 Wheel radius r = 325mm
 Rotation axis (x,y,z) =(0,0,1) for local coordinate system.
 Angular velocity ω = V/r = 239.316rad/s

III. Solver

11 Numerical methods:
The governing equations for the time dependent three-dimensional fluid flow and heat transfer around a body are the continuity equation, momentum equations and energy equation . The general approach in road vehicle external aerodynamics is to assume incompressible and isothermal flow (we neglect the thermal effect of the engine and brake discs), the flow can be considered incompressible when Ma < 0.3, which is in the vicinity of 100m/s at sea-level and it is unlikely that the flow will reach this velocity anywhere in the domain. Thus the energy equation can be neglected and the momentum- and continuity equations can be written on incompressible form, neglecting the density terms. The continuity equation is thus written [5].
The continuity equation is thus written:
(7)
And the momentum equations:
(8)
The momentum equations 8, are normally referred to as the Incompressible Flow Navier- Stokes equations. They are second order non-linear partial differential equations with only a few known analytical solutions. The main problem in solving the Navier-Stokes equations is that account has to be taken to the turbulence in order for the solution to match the physical flow accurately.
12 Turbulence models settings:
In this study we will use RANS (Reynolds Averaged Navier Stokes) to model the turbulent flow. The most common and simplest way to model the Navier Stokes equations is using what is often referred to as the Reynolds Decomposition. This approach consists of rewriting the terms in the equations as time-averaged terms. For example the time average of the turbulent function u(x,y,z,t), which is the velocity in the x-direction.

(9)
where The fluctuating term u' is defined as the deviation of u compared to the time averaged value.
(10)
where all properties are split into mean and fluctuating parts.
(11)
Substituting these into equations 7 and 8 and taking the time mean of each equation yields in the x-direction for the momentum equations.
(12)

The rewritten Navier-Stokes equations contains only time-averaged terms and fluctuating terms, the latter are normally referred to as turbulent stresses. This formulation is called Reynolds Averaged Navier-Stokes, abbreviated RANS. The turbulent stresses cannot be solved analytically but requires modelling using turbulence models this is often referred to as the closure problem [5].
12.1 Turbulence Models & Settings:
In race car aerodynamics, there are three popular turbulence models: K-Epsilon, K-Omega and Spalart-Allmaras. The main characteristics of the models are:
12.1.1 K-Epsilon:
 Two equation model
 Standard turbulence model for most industrial flows.
 Poor treatment of strong adverse pressure gradients, particularly with regard to the
 under-prediction of separation.
 Poor development of boundary layer around leading edges and bluff bodies.
 Capable to deal with less accurate mesh/boundary condition simulations
12.1.2 K-Omega:
 Two equation model
 Excellent treatment of boundary layers, especially for high adverse pressure-gradients.
 Excellent for external aerodynamics.
12.1.3 Spalart-Allmaras:
 One-equation model
 Faster than k-omega.
 More robust than k-omega.
 Deals well with external aerodynamic flows, especially adverse pressure gradients.
 Smooth transition between laminar and turbulent flow.
 Poor treatment of separation/wake formation when compared with k-omega.
From this point we have decided to use K-Omega as turbulence model because it's more suitable for our study
13 The solver:
We have the choice between two numerical methods:
1. Segregated solver.
2. Coupled solver.

Both methods apply the finite-volume method approach to solve the flow equations in the following way:
1. Dividing the grid into discrete control volumes.
2. Integrating the governing flow equations over the individual control volumes thus
constructing algebraic equations for the discrete dependent variables such as velocity and pressure.
3. Linearizing the discretized equations and subsequently solving them to obtain updated values of the unknowns.
as it knowing that the coupled solver is too time consuming and looking to our research capabilities, we will focus on the segregated solver in this simulation
13.1 The segregated solver:
The segregated solver is characterized by the fact that the governing equations are solved one at a time. Due to the non-linear and coupled nature of the flow equations, they have to be linearized and solved iteratively. A schematic overview of one iteration is shown in figure20 each iteration is composed of the following steps [4]:
Figure 20: Breakdown of one segregated solver iteration [4].
1. Fluid properties are updated from the previous solution. The previous solution is either obtained through initialization of the flow field to start the calculation or else it’s the solution obtained from the previous iteration.

2. Velocity field is updated through consecutive solving of the momentum equations using the current values for pressure and face mass fluxes.
3. In order for the velocities obtained in Step 2 to satisfy the continuity equation, a pressure correction is derived from the continuity equation and the linearized momentum equations. The pressure correction equation is then solved to yield the correction that is required by the pressure and velocity fields and the face mass fluxes in order to satisfy continuity.
4. Turbulence equations are solved using the updated variables.
5. Checking to see whether the specified convergence criteria are met.
13.2 The coupled solver:
Unlike the segregated solver, the coupled solver solves the continuity and momentum equations simultaneously. then the turbulence equations and other scalar equations however, will be solved sequentially in the same way as is done by the segregated solver. Again due to the coupled and non-linear nature of the flow equations, the solution has to be obtained in an iterative manner after linearizing the flow equations. As shown in figure each [4].
Figure 21: Breakdown of one coupled solver iteration [4].
Iteration is composed of the following steps:
1. Fluid properties are updated from the previous solution. The previous solution is either obtained through initialization of the flow field to start the calculation or else it’s the solution obtained from the previous iteration.
2. The continuity and momentum equations are solved simultaneously.

3. Turbulence equations are solved using the updated variables.
4. Checking to see whether the specified convergence criteria are met.
Looking to our research capabilities we will use segregated solver because the couple solver is more time consuming.
14 Judging convergence:
knowing when the solution has indeed converged is an important point for the accuracy of the result and to save time. STAR-CCM+ offers a number of ways to keep track of the solution progression to help determine whether the calculation has converged. During the calculation, it’s possible to keep an eye on solution residuals statistics (residual is a measure of the solution error) or force values. The solution will be evaluated by monitoring solution residuals and the lift- and drag-coefficients,CL andCD respectively.
Figure 22.1: solution residuals plot
Figure 22.2: Drag plot in function of iterationDrag plot in function of iteration

Figure 22.3: Downforce plot in function of iterationDrag plot in function of iteration
Note: the plots are not for the current simulation.

IV. Postprocessing

15 Introduction:
This chapter will give an overview of some post processing techniques the same techniques used in the field of F1 industry looking to the huge number of configuration that we have test it, we will focus our analysis just on the original and the final updated design.
The goal of this thesis is to improve the aerodynamics of the SGURACING F1-R01 car by making changes to the car’s geometry. So we will compare the original model and the final update model from the front to the end step by step.
The original design model:
The original model is designed for medium downforce circuit, the car is completely designed by Jose Gallego Segura
The final update design:
Our modification was based especially on the front wing nose and sidepod as it clear from the two pictures.

The original Front Wing and Nose:
The final update Front Wing and Nose:
The both front wings have the same main wing the modification was done in the sides of the front wing especially in the end plate due to the importance of this part in the wing on the the performance of the car, the cascade element was completely redesigned to increase the downforce of the car, and other parameter is the nose the new one looks more higher to penetrate more easily in the air and of course the pillars that support the front wing have designed to get the right interaction with the new design

The original Sidepod:
The final update Sidepod:
Another modifications was done on the side of the car, we have redesigned the side pod area with different design approaches we have changed the side pod completely and in result new engine cover, and new exhaust pipe, the new side pod looks more lower to direct the maximum quantity of air underneath the rear wing to increase the downforce of the rear wing and in the same time to reduce the stagnation pressure on the rear tire.

16 The Front Wing(FW):
In this section we will focus on the front wings results for the both models and the interaction with tire than. 16.1 How important is the front wing? Since the technical regulations were shaken up at the end of the 2008, the new lower and wider front wings for 2009 and beyond make up about a third of the overall downforce produced by the entire car. The wings are profiled to perform the job of an upside down aircraft wing. While an aircraft’s wing is used to produce lift, the front wing (and rear wing) of an F1 car is used to force the car into the track as much as possible, providing high levels of grip, traction and helping the tyres stay in contact with the track surface. The front wing, unlike the rear, does not just provide downforce. As it is the aerodynamic device that precedes the entire car, it is also responsible for directing airflow back towards the rest of the car. The optimal direction of this airflow is of critical importance to the overall downforce levels produced by the entire car. One very important part of the front wing is the endplate design. The endplate is used to redirect the airflow around the front tyres; the tyres are certainly not designed to be aerodynamically efficient and can create a lot of drag. By directing the oncoming airflow around the front tyres, this minimises the amount of drag resistance produced and allows the airflow to continue back to the sidepods and the cars floor. The upper and main flap also helps direct airflow over the front tyres, reducing drag as well as producing airflow towards the rest of the car. looking to this importance we have worked a lot to improve the performance of our front wing maximum as we can and our improvement can be clearly remarked when we compare the two values of downforce coefficient of the two front wing. Front wing
Original design Updated design
Downforce coefficient Cz
0.49
0.68
Drag coefficient Cx
0.12
0.14
Efficiency Cz/Cx
4.08
4.85

From the previous table we can see clearly that we have optimised the front wing, and this is due the remarkable gain of efficiency, we have gain of 15.8%,that's right it looks small but on the truck this optimization can boost the car with some millisecond and these millisecond can make the difference between winning and losing the race. ( A) (B) (C) Figure 23: The distribution of the Cp over the initial front wingFrom figure we can see clearly the distribution of the Cp over the initial front wing where the picture (A) shows the

perspective view of the front wing where the figure (B) shows the top view of the front wing where we have high pressure, and the last one (C) represent the bottom view where we have low pressure area and this variation of the pressure between the top side and the bottom side of the front wing creat the downforce effect the same effect as lift (airplane) but upside down. (A)
(B)
(C)
Figure 24: The distribution of the Cp over the iupdated front wing

It's really important to make sure that the flow over the front wing is attached to the surface of the wing. Because the detachment of the boundary layer from the wing will creat many problems affect directly the the performance of the win. In reality there is some techniques to investigate this like the FLOWVIS technique.
Flow visualization or flow visualisation in fluid dynamics is used to make the flow patterns visible, in order to get qualitative or quantitative information on them.
Figure 25: flow visualisation paint on the STR front wing
In CFD too there is the same technique to investigate the direction of the flow and the separation zones like we will see in the next figures.
16.2 Initial front wing:
Figure 26.1: The flowvis over the initial front wing

Figure 26.2: Tthe picture shows in details the direction of the flow on the top of the front wing and shows unexpected recirculation zones and this will influence the performance of the car
Figure 26.3: From the side view to (the end plate) the flow looks irregular and completely perturbed and this effect of the end plate have a direct influence on the tire flow because there is an interaction between end plate and tires.

Figure 26.4: From the bottom view the flow is completely destroyed and this will decrease the downforce of the wing.
16.3 Updated front wing:
Figure 27.1: The flowvis over the updated front wing

Figure 27.2: The flow over the updated front wing looks completely streamlined and attached to the surface of the wing without any separation zone, just with small perturbation in the cascade element due to a more incidence angle for the first element.
Figure 27.3: From the side view (end plate) too the flow is too clean without any perturbation this will help to control the flow outside the tires to reduce the drag effect of wheels.

Figure 27.4: for the bottom side we still have some recirculation zones and this zones are created from the interaction with the ground and looks too complicated to eliminate it completely.
17 Front tires:
One of the main problems for an F1 aerodynamicist is tire, Formula 1 is an open wheel car this means that the tires are exposed to the air , and we know that one of the most complicated flows is the flow around rotating tire in contact with ground, because the tire are buffer bodies and the wake of thies bodies as too complicated three dimensional and unsteady, and in Formula 1 approximately 40% of the total drag of the car is created by the tire.
Due to this importance we will consist this part to investigate some effects of tires.
17.1 The wake of the front tire:
As we have mentioned the wake of tires is too complicated in this short section we will try to investigate this effect.
The wake in the X direction
(A) X=0m (B) X=-0.05m

(C) X=-0.1m (D)=-0.15m
(E) X=-0.2m (F) X=-0.25m
(G) X=-0.3m (H) X=-0.35m
(I) X=-0.4 m (J) X=-0.45m

From the previous pictures we can understand the development of the front tire wake in the X direction, the complexity of this wake is proportional to the interaction with the ground where we have two vortex created in the bottom sides of the tire, these to vortices have a direct influance on the flow underside the car and for this reason we try to deflect this wake away from the car and we will talk about this later.
Another factors that we can talk about it is the section is the detachment of the flow in the top side of the tire this detachment is influenced by two factors the roughness of the tire surface and the temperatur of the tire two, and unfortunately these two factors are neglected from this simulation, and we can see that the flow detachment is started from X=- 0.15m approximately, this point of attachment is too important and have an influence of the tire drag.
17.2 The wake in the Z direction:
(A) Z=-0.3m (B) Z=-0.25m
(C) Z=-0.2m (D) Z=-0.15m

(E) Z=-0.1m (F) Z=-0.05m
(G) Z=0m (H) Z=0.05m
(I) Z= 0.1m (J) Z=0.15m
(K) Z=0.2m (L) Z= 0.25m

The previous picture shows the tire wake structure in the Z direction and it's remarkable that we have a large wake in the contact patch area between the tire and the ground, this large wake will have an influence on the rest of the car.
Figure 28: 3D view of the wake structure Q-criterion iso surface colored by Cp
17.3 Wake controle:
And like we have mentioned that there is an interaction between the front wing and front tire this means that we can control this wake away using the front wing design.
Figure 29.1: The original design tires wake

Figure 29.2: The updated design tires wake
From the figure we can see that the wake of the front tires is directed directly to the car (side pod area), this wake will perturb the flow in this area and due to the importance of this area in the performance of an F1 car, this effect will reduce the performance of the car and can perturb the stability of the car, create problems in the cooling of the engine and too.
In the other hand the updated design have a good capability to deflect the wake of the front tire away from the body and this will increase the performance of the car.
17.4 Front tire aero values:
After the simulation we can see that we have reduced the drag effect of tires by 50% and this achievement is due to the right instruction with the front wing , to be honest the drag values of the tire still quite far from the realistic results, and this because we have simplified the geometry of the tire we don't have the internal systems like the brake system and the cooling of the brake of the tire, this will reduce the drag automatically.
Figure 30.1: Original design Frontal area of the front tire and the Cp distribution Cx=0.12.

Figure 30.2: Updated design Frontal area of the front tire Cx=0.062.
18 Floor:
The floor or the underbody flow is too important factor to get high performance car, the floor is a plan surface work in ground effect with the ground, this part of the car have two roles the first one is to accelerate the air flow under the body maximum as you can to decrease the pressure under the car, and i consequence increasing the downforce of the car.
And in the other hand we need to converge the maximum possible of the flow to the diffuser area
Figure 31.1: Original design underbody flow

Figure 31.2: Original design underbody flow
It's clear that the updated design work more better than the original one, and from the Figures we can see that the updated design help the flow to converge more better to the diffuser area
19 Rear Wing (RW):
As we have the same rear wing for the both cars so we will focus just for one of them and let's take the rear wing equipped the updated design. The rear wing is a crucial component for the performance of a Formula One racecar. These devices contribute to approximately a third of the car's total down force, while only weighing about 10 kg. Usually the rear wing is comprised of two sets of aerofoils connected to each other by the wing endplates. The upper aerofoil, consisting of one element, provides the most downforce, and varied from race to race. The lower aerofoil, consisting of one element, it is smaller and provides some downforce. However, the lower aerofoil creates a low-pressure region just below the wing to help diffuser create more downforce below the car. The rear wing, same as front wing, is varied from track to track because of the trade off between downforce and drag. More wing angle increases the downforce and produces more drag, thus reducing the cars top speed. So when racing on tracks with long straights and few turns, like Monza, it is better to adjust the wings to have small angles. Opposite to that, when racing on tracks with many turns and few straights, like Austria, it is better to adjust the wings to have large angles.

From these results the rear wing looks good and for this reason we have keep it.
Figure 32: The distribution of the pressure over the rear wing.
The distribution of the pursuer over the rear wing it's uniform distribution and this will result a stable rear wing.
.
Rear Wing
Drag coefficient CX
0.2
Downforce coefficient Cz
0.93
Efficiency Cz/Cx
4.65

Figure 33.1: Flow vis on the top of the rear wing.
Figure 33.2: Flow vis on the bottom of the rear wing.
Figure 33.3: Flow vis on the side of the rear wing (end plate).
As the front wing the flow over the rear wing is completely clean and attached to the surface of the wing.

20 Full car analysis:
As we have mentioned in the previous paragraph we have optimised the car maximum as we can looking to our research capabilities, in this short section we will show you some results of the full car and in the same timei will present you some thechnique used by the F1 aerodynamicist.
In the end, and from this results we can say that we have achieved our goal and we have increased the efficiency of our car by 12.5%, and this is a really good result, by decreasing the drag effect and increasing the downforce of the car that's right 12.5% looks not too large, but this gain will make the car more faster during the race and because in Formula 1 the difference between winning or losing the race is by some millisecond so this gain is too important for an F1 aerodynamicist.
Another really important factor for the stability of the car is the aero balance. the aero balance is the distribution of the downforce between the front axle and the rear axle of the car and we take in consideration the distribution of the original weight of the car to, the perfect aero bance is to get 45% of downforce in the front and 55% of the rest downforce in the rear without this balance the car will be undriveable and the pilot will have a difficulties in the curves (oversteering or understeering).
Figure 34: the aerobalance
Original SEGURACING F1- R01 design
Updated Seguracing F1-R01 design
Drag coefficient
Cx
1.121
1.097
Downforce coefficient
Cz
1.604
1.744
Efficiency
Cz/Cx
1.43
1.59

Front Downforce
Rear Downforce
Original SEGURACING F1- R01 design
36.12%
63.88%
Updated Seguracing F1-R01 design
38.99 %
61.01%
From the results we can say that we have optimised the balance of your car but still not perfect, and with more work on the front area we can achieve the perfect balance.
21 Car rear wake:
The understand of the car rear wake is too important to reduce the drag effect because this wake have a direct effect on the drag of the car in this section we will talk about the rear wake of an F1 car.
(A) X=3.7m

(B) X=3.8m
(C) X=3.9m
(D) X=4m

(E) X=4.1m
(C) X=4.2m
(E) X=4.3m

(F) X=4.4m
(G) X=4.5m
(H) X=4.6m

The previous figures shows in details the development of the rear F1 car wake. The complexity of this wake is due to interaction between different wakes rear tires wake rear wing vortex and the diffuser wake in the figure (A) the flow start to detach from the rear tires and in the same time the development of rear wing vortex ,and from 4m the tires wake start to mix with the diffuser flow this mix create low total pressure zone or with other words drag zone and then from 4.5m this flow transformed to vortices.
And we can see these vortices in this figure shows the Q-criterion isosurface colored by Cp.
Figure 35.1: Rear end vortices Q-criterion isosurface.
Figure 35.2: Rear wing Vortex.

22 Conclusion:
In the end of this project we can say that we have achieved our goal successfully and we have optimize the performance of our car, but this work still amateur work because the Formula 1 aerodynamics is much more complicated than this.
this work demand a lot of research capabilities, and looking to our capabilities this is the maximum that we can offer of course the doors of this project still opened and we still do more work on the car.
in the continued development of this project we try to investigate the interaction between two cars or more in the overtaking, this subject is a major problem for the F1 aerodynamicists, and i hope our university will help us to run this work because it's to time demanding.
the content of this work can used as guideline for any low speed ground vehicle aerodynamics investigation and in the same time for validation.

23 Recommendations:
Make sure that your computational domain is larger as possible and don't hesitate to use the blockage ratio (equation 1), in the same time you need to respect your computational capabilities (Hardware).
As mentioned earlier, the mesh is one of the most important factors in CFD to get a good results, so please be careful when you generate the mesh try to follow the same steps mentioned in this thesis and never run your simulation without validate your mesh (section 9 Mesh analysis).
Never plot or create any scalar scan without achieving the convergence then your results will be incorrect make sure that you have achieved the convergence to judge the results this please follow (section 4 Judging convergence) from this thesis.
To accelerate your convergence you can use the 1st order discretization scheme for 150 to 200 iteration then upgrade it to 2ed order and never analysing your results whn you are on the 1st order.
Looking to the variety of parameters that you can analyze i suggest you these ones and are the same quantities used by F1 team specific quantities to help better understand the results. These consist of: 1. Surface data. Use a clear legend colour scheme. 1. Surface Pressure in terms of pressure coefficient Cp 2. Surface skin friction in tems of skin friction coefficient Cf 3. surface streaklines 2. Flowfield data; x-normal cross sections, with scales that allow to show flow strudtures properly. 1. Total pressure coefficient Cp_t 2. pressure coefficient Cp 3. y and z compoents of velocity; to examine outwash and downwash 4. vorticity or helicity 3. Isosurfaces of negative velocity (as geometry scene) v=-0.1 or -0.01 m/s to show the wakes behind the different parts of the front wing and especially the front tyre wake.
And for any questions or advices related to the field of ground vehicles or motor sport please don't hesitate contact me on:
http://cfd2012.com/formula-1-cfd-expert.html

24 References:
[1] CD-adapco DYNAMICS magazine issue 30.
[2] Lotus F1 Team and the Environment brochure.
[3] CD-adapco Global academic program CD Adapco STAR CCM+ foundation training material.
[4] Adil el Ouazizi, CFDBASEDAERODYNAMIC REDESIGNOFAMARCOSLM600 Delft University of Technology/Aerospace Engineering Department/Chair of Aerodynamics, Master’s Thesis.
[5] JOHANCEDERLUND, JACOBVIKSTRÖM TheAerodynamicInfluenceofRim Design on a Sports Car and its Interaction with the Wing and Diffuser Flow Department of Applied Mechanics, Division of Vehicle Engineering and Autonomous Systems, CHALMERS UNIVERSITY OF TECHNOLOGY Master’s Thesis.

AERODYNAMIC DEVELOPMENT OF THE SEGURACING F1-R01 PROTOTYPE USING CFD

Recommended

Recommended

More Related Content

What's hot

What's hot (20)

Viewers also liked

Viewers also liked (20)

Similar to AERODYNAMIC DEVELOPMENT OF THE SEGURACING F1-R01 PROTOTYPE USING CFD

Similar to AERODYNAMIC DEVELOPMENT OF THE SEGURACING F1-R01 PROTOTYPE USING CFD (20)

Recently uploaded

Recently uploaded (20)

AERODYNAMIC DEVELOPMENT OF THE SEGURACING F1-R01 PROTOTYPE USING CFD