Numerical study and optimization of a GT car Rear-Wing aerodynamics

NUMERICAL STUDY and OPTIMIZATION of a GT Car Rear-Wing Aerodynamics by Masoud Arianezhad Diploma Thesis for Degree Master in Aerospace Science and Technology at Universitat Polit`ecnica de Catalunya Advisor: FERNANDO P. MELLIBOVSKY ELSTEIN Barcelona ,March 2015 Dedicated to my mother The most beautiful woman I have ever seen in my life. She is, to me, my rock. She is by far the strongest woman I have ever known. Abstract Race car performance significantly depends on elements such as the engine, tires, suspension, road, aerodynamics, and of course the driver. Although human factors are frequently publicized as the reason behind the success or failure of one racing team or another, engine power, tire adhesion, chassis design, and, aerodynamics probably play a more important role in winning the technology race. In recent years, however, vehicle aerodynamics gained increased attention, mainly due to the utilization of the negative lift (downforce) principle, yielding several important performance improvements. Various methods exist to generate downforce such as inverted wings, diffusers, and vortex generators. Some cars like McLaren P1 are able to produce 600kg of downforce at well below maximum speed (257 km/h=161 mph) in Race mode, which is considerably higher than most other high performance supercars, and more in line with the levels of downforce generated by a GT3 racing car. This downforce improves the car s cornering ability, especially in high speed corners. Balance, agility and controllability are all outstanding. This work briefly explains the significance of the aerodynamic downforce by using multi-element airfoils. After a short introduction, the philosophies behind the high-lift airfoils design are discussed and finally the CFD simulation of multi-element is performed and the resultant data is compared and investigated. The first idea for this work was to design a new airfoil or optimize an available high-lift airfoil according to our requirements but since it needed to have a powerful inverse airfoil design software like Profoil, which is not easy to access, and in addition the user should have a deep knowledge of aerodynamics, we decided to choose some high-lift airfoils as the base and use their combination for CFD simulations. Unfortunately CFD simulations are so time consuming, for this reason many researchers try to simulate the multi-element airfoils in codes like MSES which is a numerical airfoil development system. It includes capabilities to analyze, modify and optimize single and multi-element airfoils. But since we could not afford buying this relatively software, we tried to go directly through CFD simulation of multi-element airfoils. Unfortunately, it is hard to find empirical data about rear wing of race cars because normally they are confidential piece of information of big car companies. On the other hand it is so rare to find a similar wind tunnel or CFD simulation of the same selected multi-element airfoils and what can be found is almost always empirical data of single element airfoils. All these things make it hard to have a reliable CFD results as long as there is no evaluation of results with the real world information. It would be interesting that in the future someone use information of this work as a reference to compare with wind tunnel or CFD simulations. Contents 1 Introduction 9 1.1 Aerodynamic Downforce . . . . . . . . . . . . . . . . . . . . . . . . . 9 1.2 Airfoil Force and Moment Coefficients . . . . . . . . . . . . . . . . . 11 1.2.1 TypesofDrag .......................... 12 1.3 Technical Regulations for Grand Touring Cars . . . . . . . . . . . . 13 1.4 Structure of the Thesis . . . . . . . . . . . . . . . . . . . . . . . . . . 13 2 Design Methodology 15 2.1 High Lift Design Philosophy . . . . . . . . . . . . . . . . . . . . . . . 16 2.2 S1223 High Lift Section . . . . . . . . . . . . . . . . . . . . . . . . . 18 2.3 EpplerE420airfoil............................ 19 2.4 Blunt or Flatback Trailing Edge . . . . . . . . . . . . . . . . . . . . 20 2.5 S1223 (with blunt trailing edge) Performance . . . . . . . . . . . . . 20 2.6 Multi-element Airfoils . . . . . . . . . . . . . . . . . . . . . . . . . . 21 2.6.1 TheFlapEffect.......................... 23 2.6.2 Fresh Boundary-Layer Effect . . . . . . . . . . . . . . . . . . 24 2.7 Boundary-Layer Separation . . . . . . . . . . . . . . . . . . . . . . . 25 3 Computational Fluid Dynamics (CFD) Modeling 27 3.1 Geometry ................................. 27 3.2 TurbulenceModel ............................ 28 3.2.1 SST k-ωModel.......................... 30 3.3 GridGeneration ............................. 31 3.3.1 Structured or Unstructured Grids? . . . . . . . . . . . . . . . 31 3.3.2 Boundary Layer and Estimation of First Cell Height for correct y+(WallUnit) ....................... 32 3.3.3 Grid Resolution for RANS Models . . . . . . . . . . . . . . . 34 3.3.4 Domain Boundaries and Grids . . . . . . . . . . . . . . . . . 35 3.3.5 Near-wall Mesh Generation . . . . . . . . . . . . . . . . . . . 36 3.4 Multi-Element Airfoil Configuration . . . . . . . . . . . . . . . . . . 38 3.5 Set up the solver (Ansys Fluent) and physical models . . . . . . . . 40 ii CONTENTS 3.5.1 The Pressure-Based Segregated Algorithm . . . . . . . . . . . 41 3.5.2 Transient Solution . . . . . . . . . . . . . . . . . . . . . . . . 42 4 CFD Simulation Results 45 4.1 2DSingleAirfoil ............................. 46 4.1.1 Boundary Conditions . . . . . . . . . . . . . . . . . . . . . . 46 4.1.2 Results .............................. 46 4.1.3 Grid Independence Study . . . . . . . . . . . . . . . . . . . . 47 4.2 2D Multi-element Airfoil . . . . . . . . . . . . . . . . . . . . . . . . . 49 4.2.1 Flap Deflection αf= 40o: .................... 49 4.2.2 Flap Deflection αf= 35o: .................... 49 4.3 Discussion................................. 52 4.3.1 Effect of Turbulence Models on the Results . . . . . . . . . . 58 4.3.2 Separation Bubbles . . . . . . . . . . . . . . . . . . . . . . . . 59 4.3.3 Variation of Angle of Attack and Multi-element Airfoil Performance............................... 62 4.3.4 K´arm´an vortex street . . . . . . . . . . . . . . . . . . . . . . 65 4.3.5 Effect of Variation of Sportscar Speed . . . . . . . . . . . . . 65 5 Conclusions 69 5.1 Futureworks ............................... 71 5.1.1 3D Wing Simulation . . . . . . . . . . . . . . . . . . . . . . . 71 5.1.2 Analysis of Twisted Wing . . . . . . . . . . . . . . . . . . . . 72 Conclusions 69 A Some Aerodynamics Definitions 73 Acknowledgments I would like to thank my family and specially my beloved mother for their constant support. Without their help it would impossible to continue my study here in Spain and overcome a challenging student s life in a foreign country on a limited budget and many other emotional and social difficulties. Nobody would understand the toughness of living abroad until they try it. Unfortunately my father is not among us anymore. I also like to thank him for bringing me up like a strong man. May God bless his soul and rest him in peace I would also like to appreciate all kind helps of my supervisor FERNANDO MELLIBOVSKY ELSTEIN. Without his supervision and great recommendations this project could go to a wrong direction. I would also like to thank my friends for their support during my staying in Spain. They help me to feel like I am in my own country. List of Figures 1.1 Variation of the one-lap record speed at the Indianapolis Speedway.[1] 9 2.1 A graph demonstrates the Interrelation between boundary layer control efforts and consequences. . . . . . . . . . . . . . . . . . . . . . . 17 2.2 Pressure distribution vectors computed from XFOIL for α= 5oshow airfoil loading. Note that the vectors with arrows pointed outward correspond to relatively negative pressure. . . . . . . . . . . . . . . . 18 2.3 Trends in low Reynolds number airfoil characteristics as functions of the pitching moment and type of upper-surface pressure recovery distributions. (adopted from [2]) . . . . . . . . . . . . . . . . . . . . 19 2.4 Plot comparing modified T.E airfoil with original S1223 airfoil. . . . 21 2.5 A Comparison between lift coefficient of original S1223 airfoil and S1223 with trailing edge gap of 0.5% of the chord length.(The viscous analysis has been done in XFOIL for Re=800,000) ............... 22 2.6 Performance polar for the S1223 with blunt T.R at Re=1,067,000 computedbyXFOIL........................... 23 2.7 Performance comparison in different Reynolds numbers computed by XFOIL................................... 24 2.8 Typical boundary-layer behavior for a three-element airfoil.[3] . . . . 25 2.9 Flap effect (modeled by a vortex) on the velocity distribution over the mainwing. ................................ 26 2.10 Boundary layer developing around an airfoil. . . . . . . . . . . . . . 26 3.1 A Screen shot from XFOIL of Mark Drela showing its root menu . . 29 3.2 Transition process in boundary layer on a flat plate . . . . . . . . . 33 3.3 Domain boundary distances were chosen as 16.5×(total Chord Length) for the inlet and 30×(total Chord Length) for the outlet . . . . . . . 36 3.4 Hybrid mesh used as the first attempt for creating grids in which the majority of it (except close to multi-element airfoil) contains structured mesh, however finally a completely unstructured mesh was chosen. 37 3.5 Division of domain into smaller parts. . . . . . . . . . . . . . . . . . 38 Chapter 1 Introduction 1.1 Aerodynamic Downforce Since the early days of the automobile and of motor racing, engine, tire, and suspension technology have gradually developed. In most of these disciplines the advances were reasonably gradual, leading to increased race car performance, higher speeds, and lower lap times. This trend is demonstrated by Fig 1.1 , which shows the history of the one-lap record speed at the Indianapolis Speedway. As can be seen, the biggest jump in speed occurred in 1972 with the first efficient use of front and rear wings.[1] Figure 1.1: Variation of the one-lap record speed at the Indianapolis Speedway.[1] In addition to improved cornering speeds, aerodynamics have dramatically improved vehicle stability and high-speed braking as well, which again lead to faster 10 1 Introduction lap times. Nowadays aerodynamics is one of the areas in racecar development where significant improvements can be achieved at a relatively low cost and less additional weight, whether the car is a road-registered car that does track days, or a big horsepower race car which has yet to have much aerodynamic tuning done on it. The effects on stability by the addition of a properly designed rear wing on a road car for example can definitely be felt from the driver’s seat at permitted speeds on the freeway. When it comes to racecars except for drag cars and Bonneville salt flats cars all race cars are required to go around corners. Obviously the faster that a given car can go around the type of corners, the less its lap time will be. There are two reasons for it: •Obviously the faster the vehicle is traveling the less time it will take to cover a given section of race track, either straight or curved. •The second reason is even more important. Considering a car that exits a given corner at, for example, 130Km/h is going to continue its straight movement in less time than the car which exits the same corner at 110Km/h and it’s all because of the less time needs for accelerating from 110 to 130Km/h. In other word, If you can increase your exit speed from key corners on the track, such as the final turn before a main straight, you can also potentially increase your top speed as you reach the end of the straight, and cover the distance of that straight faster. Factors which determine the cornering power of a given race car include: •Cornering capacity of the tires, which is influenced by: –Suspension geometry –Vehicle load transfer characteristics –Vehicle downforce –Size and characteristics of the tires •Vehicle gross weight •Height of the vehicle center of gravity If we put our focus on racecar aerodynamics, then by using lower drag and increased grip via greater downforce, it is potentially possible to add incremental increases in speed through each corner, exiting each corner and on each straight, and those incremental improvements through individual sections of the track can add up to a significantly lower lap time. 1.2 Airfoil Force and Moment Coefficients 11 The first and most obvious approach to create downforce is to use inverted airplane-like wings to create downforce instead of lift. Such inverted wings can be found throughout the whole spectrum of automobile racing. While various components of an aerodynamic package contribute differently to the downforce levels and resulting flow fields, only the front and rear airfoils and wings lend themselves to theoretical aerodynamic analysis methods and techniques for design. Other components and body shape designs still rely on experimental and numerical data at the design stage. 1.2 Airfoil Force and Moment Coefficients A discussion on wings traditionally starts with a discussion on the wing section shape, the airfoil. Following this approach and first demonstrate the aerodynamic significance of the airfoil geometry and its effect on lift and drag. A three-dimensional wing consists of airfoil sections, but the shape of the wing planform in terms of sweep, taper, twist, and other geometrical parameters affects the overall performance as well. In another definition an airfoil is the two-dimensional cross section of a threedimensional wing. The nondimensional quantity called a force coefficient, F/(V2S) where Fis an aerodynamic force and Sis an area. is similar to the type often developed and used in aerodynamics. It is not, however, used in precisely this form. In place of ρV 2 it is conventional for incompressible flow to use 1 2ρV 2, the dynamic pressure of the free-stream flow. The actual physical area of the body, such as the planform area of the wing is usually used for S. Thus the aerodynamic force coefficient is usually defined as follows: CF=F 1 2ρV 2S(1.1) The two most important force coefficients are lift and drag, defined by: Lift Coefficient CL=Lift 1 2ρV 2S(1.2) Drag Coefficient CD=Drag 1 2ρV 2S(1.3) When the body in question is a wing, the area S is almost invariably the planform. Airfoil Moment: The aerodynamic lift and drag are the result of integrating the surface pressure distribution. It is possible to represent the resultant force due to this pressure distribution by a single force F. One of the more interesting conclusions from basic airfoil theory is that this force acts at the quarter chord of a symmetric airfoil and points in the lift direction. Consequently, this point, called the center of pressure. For cambered wings the center of pressure can be in a different location 12 1 Introduction and may vary with angle of attack, whereas the aerodynamic center will be near the quarter chord. For race car applications the location of the aerodynamic center is less significant, while the location of the center of pressure is more important; a small backward shift of the center of pressure on the rear wing of a race car can visibly influence performance. 1.2.1 Types of Drag Total Drag Total drag is formally defined as the force corresponding to the rate of decrease in momentum in the direction of the undisturbed external flow around the body. This decrease is calculated between stations at infinite distances upstream and downstream of the body, so it is the total force or drag in the direction of the undisturbed flow. It is also the total force resisting the motion of the body through the surrounding fluid. There are a number of separate contributions to total drag. As a first step it may be divided by physical effect into pressure drag and skin-friction drag. Skin-Friction Drag (or Surface-Friction Drag:) Skin-friction drag is generated by the resolved components of the traction due to shear stresses acting on the body surface. This traction is due directly to viscosity and acts tangentially at all points on the body surface. At each point it has a component aligned with but opposing the undisturbed flow (i.e., opposite to the direction of flight). The total effect of these components, integrated over the entire exposed surface of the body, is the skin-friction drag. Skin-friction drag cannot exist in an invisicid flow. Pressure Drag: Pressure drag is generated by the resolved components of the forces due to pressure acting normal to the surface at all points. It is computed as the integral of the flight-path direction component of the pressure forces acting on all points on the body. Pressure distribution, and thus pressure drag, has several distinct contributions: •Induced drag (sometimes known as drag due to lift or vortex drag). •Wave drag, when there exists a supersonic region in the flow regardless of the flight Mach number being less than or greater than 1. •Form drag (sometimes known as boundary-layer pressure drag). The Wake: Behind any body moving in air is a wake. Although the wake in air is not normally visible, it may be felt, as when, for example, a bus passes by. The total drag of a body appears as a loss of momentum and an increase of energy in the wake. The loss of momentum appears as a reduction of average flow speed, while the increase of energy is seen as violent eddying (or vorticity). The size and intensity of the wake is therefore an indication of the profile drag of body. 1.3 Technical Regulations for Grand Touring Cars 13 1.3 Technical Regulations for Grand Touring Cars While the benefits of inverted rear and front wings were understood by racers and many racing-sanctioning organizations recognized the strong influence of aerodynamics on lap-speed they attempted to create regulations based on placing limits on the use and size of aerodynamic devices such as inverted wings. Similarly, the ACO ( Automobile Club de l’Ouest) has defined limits and requirements for the aerodynamic devices of LM GTE (Le Mans Grand Touring Endurance) category are as below: •A wing made from one element only is permitted on top of the bodywork provided that: It replaces the original rear wing if one is fitted on the car; •It fits, including end plates and angle bracket, into a volume the dimensions of which are 45 cm (horizontal) x 15 cm (vertical) x 91% of the maximum width of the road car homologated (ACO Homologation Form); •The chord of the wing section not to exceed 30 cm; •It is set forward by 5 cm in relation to the rearmost point of the bodywork. Any bodywork modification or extension the purpose of which is to move the wing backward is prohibited; •It is set 10 cm lower than the highest point of the roof.[4] Despite the above mentioned rules, there are many other categories of GT racecars which have less restrictions and designers are allowed to use multi-element (mostly dual element) wings and different endplate shapes. In this project we try to ignore Le Mans restricted rules for using single-element wing and instead we will design a dual element wing, however the dimensional restrictions will be applied as mandated by ACO. 1.4 Structure of the Thesis In the next chapter firstly the design available philosophies of high-lift airfoil will be discussed and then the two airfoils which are selected as main and flap airfoils for this project will be introduced and compared with other famous high-lift airfoils. In continue of the next chapter the benefit of the blunt trailing edge (T.E) will be explained and the resultant simulation in XFOIL will be discussed. Then, at the end of Chapter 2 we become familiar with multi-element airfoils and the role of slot which is known as slot effect will be explained. Finally we will be introduced to a short explanation about separation of flow on airfoils. Chapter 3 mostly deals with the fundamental works of CFD simulation, however the beginning of this chapter will be the explanation of how the geometries of airfoils 14 1 Introduction were imported to the computer, modified, initially simulated and finally prepared for mesh generator software and CFD solver. Later the most important part of a CFD work which is mesh generation will be discussed and we will realized the advantage and disadvantages of different commonly used meshes (grids) in CFD. After this part which is an introduction to meshing techniques, the method used in this work is explained. Because in this work it is assumed that the freestream is completely turbulent, selection of the turbulence model is of great importance; for this reason the selected turbulence model will be introduced and compared to others. Finally the set-up af the CFD solver and solution method will be described. Chapter 4 which is the most important part of this work, is the result of the CFD simulations. First we see the CFD results of the single element to have a rough guess about the accuracy of the solution, number of cells, solver st-up etc.. Next we start simulation of the multi element airfoil in two different flap deflections, αf= 35oand αf= 40o. When the optimum points of each configuration is obtained, these two point will be compared. In addition accuracy of the simulation will be explained and the method is described. Because of changing in speed of the car and aoa of the upcoming air, rearwing should be able to operate perfectly in different conditions, for this reason, various simulations in different speeds and aoa were performed. Last chapter is the conclusion of the thesis and brief explanation of what has been done in this work. Finally the future works will be suggested. Chapter 2 Design Methodology However in this project the goal is not to design a high-lift airfoil used in race cars, but it is important to have the knowledge of its design so the candidate airfoils will be chosen precisely. Airfoil design methodologies that satisfying complex requirements of racecars wings are confidential pieces of information that teams and other technical organizations rarely publish their precious secrets and experiments in books or journals and as a consequence the wing design in this field is based on theory, experimental data and sometimes guesses. Like most of airfoil design problem, the common goal of a race car wing is to generate as much lift Clmax (actually downforce) as possible within the physical constraints of the permissible dimensions of the wing.[5] While achieving this goal, various other criteria can be taken into account in the design process to guarantee proper functioning of the high downforce system under available constraints associated with motorsports applications. The process is involving of choosing the pressure distribution, particularly that on the upper wing surface, to maximize lift is the base of the high-lift airfoils design. Even when a completely satisfactory answer is found to this rather difficult issue, it still remains to determine the appropriate shape of the airfoil to produce the specified pressure distribution. This second step in the process is the so-called inverse problem of airfoil design. It is much more demanding than the direct problem of determining the pressure distribution for a given airfoil shape.[3] Nevertheless, satisfactory inverse design methods are available, although they will not be discussed here. In broad terms the maximum lift achievable is limited by two factors: •Boundary-layer separation •The onset of supersonic flow As long as here we are only interested in subsonic flow, the second factor will not be discussed.In two-dimensional flow, boundary-layer separation is governed by: •The severity and quality of the adverse pressure gradient 16 2 Design Methodology •The kinetic-energy defect in the boundary layer at the start of the adverse pressure gradient In the next part the practical affect of the quality of adverse pressure and its importance in a good high-lift design philosophy will be discussed more. 2.1 High Lift Design Philosophy The different design philosophies in the low to moderate Reynolds number regime include the approaches used by Liebeck, Eppler, Wortmann and Selig. To study and implement the applicability of aft loading to motorsports applications, it is necessary to understand the interdependence of various airfoil characteristics upon one another. A graphic representation of the various flow boundary layer transition regimes and the performance consequences is demonstrated in Fig 2.1. It is well known that as pitching moment increases, maximum lift coefficient increases along with the pressure recovery becoming convex (Fig 2.3). Other observable trends from the same figure indicate that as an airfoil tends towards a more concave loading, high lift is achievable along with an increase in the rapidity with which stall is reached. Liebeck airfoils are a good example of the first type where a large rooftop/suction level is employed followed by a Stratford pressure recovery (or concave pressure recovery). This leads to hard stall characteristics and high lift with low pitching moment. The second approach is that reflected by some of the Wortmann airfoils where the reliance on a suction peak is reduced and more emphasis is placed on aft loading (convex pressure recovery) in order to provide softer stall characteristics. A third, middle ground, methodology is reflected by the Selig and Eppler high lift airfoils where a combination of the aforementioned design philosophies are utilized in combination to provide high lift at low Reynolds number. The Liebeck airfoils rely on a Stratford boundary-layer inverse solution whereby a pressure recovery distribution can be found that continuously avoids separation of the turbulent boundary layer. It is meant to recover the maximum possible pressure rise in the shortest possible distance. The Stratford recovery also represents the optimum distribution for low profile drag and this leads to some of the highest lift to drag ratios for these class of airfoils. But this makes the boundary layer on the upper surface very sensitive to surface imperfections that may trip the flow. Motorsport applications often have wings positioned close to the ground. Even rear wings have surfaces that are constantly closer to the ground than typically found in aeronautical applications and this makes their surfaces susceptible to various bits of track and tire debris. These particles can potentially act as trips and, in the case of airfoils reliant on Stratford recoveries, may influence the potential to generate high downforce. Eppler argued that the sensitivity of the turbulent boundary layer in a Stratford 2.1 High Lift Design Philosophy 17 distribution, which is on the verge of separation by design, can be a cause of hard stall as the unsteadily moving transition point can change the initial conditions of the pressure recovery such that the turbulent separation is also unsteady. A race car often sees a large variation in speed across a race track which can change the operating Reynolds number. These variations can cause an increase in adverse pressure gradient which then causes a fast moving turbulent separation point. Usually, the sensitivity to the Reynolds number influence can be mitigated by extending the instability range i.e, extending the range of the turbulent boundary layer. Eppler suggested that concave pressure recoveries should be used but they should not be as steep as the Stratford distribution at the beginning. This forms the basis for Eppler and Selig0s high lift airfoil designs where a moderated degree of concavity is allowed into the pressure recovery along with aft loading. The FX63-137 a convex pressure distribution, as seen in Fig 2.2, along with an increase in length of the representative pressure vectors on the lower surface at the aft portion of the airfoil, thus indicating aft loading. Eppler showed that the lift of an airfoil with concave recovery could be improved using aft loading and this was meant to espouse the combined use of concave pressure recovery and aft loading as a means to enhance high lift performance. An example of this design direction is the Wortmann FX74-CL5-140 (Fig 2.2) which is a high lift design. It uses gradual initial pressure recovery compared to Stratford recovery airfoils and also shows aft loading. Selig adapted concave recovery and aft loading to produce airfoils optimized for high lift. The S1223 (Fig 2.2) and the FX74-CL5-140 produce the highest maximum lift currently among airfoils operating in this regime. Figure 2.1: A graph demonstrates the Interrelation between boundary layer control efforts and consequences. 24 2 Design Methodology Figure 2.7: Performance comparison in different Reynolds numbers computed by XFOIL raises the velocity at the trailing edge, thereby reducing the severity of the adverse pressure gradient. The flap has a second beneficial effect, which can be understood from the figure inset. Note that, owing to the velocity induced by the flap at the trailing edge, the effective angle of attack has been increased. If matters were left unchanged, the streamline would not leave smoothly from the trailing edge of the main airfoil, violating the Kutta condition. What must happen is that viscous effects generate additional circulation, so that the Kutta condition is satisfied once again. Thus the presence of the flap leads to enhanced circulation and therefore higher lift. 2.6.2 Fresh Boundary-Layer Effect It is evident from Fig. 2.8 that the boundary layer on each element develops largely independently from the boundary layers on the other airfoil elements. This ensures a fresh thin boundary layer, and therefore a small kinetic-energy defect, at the start 2.7 Boundary-Layer Separation 25 Figure 2.8: Typical boundary-layer behavior for a three-element airfoil.[3] of the adverse pressure gradient on each element. The length of pressure rise that the boundary layer on each element can withstand before separating is thereby maximized. 2.7 Boundary-Layer Separation In chapter 4 we will see that an important thing that effects the production of lift and drag in and airfoil is the separation of the flow. Before the evaluation of CFD results, it is important to know how separation occurs. For explanation of separation process in airfoils and other bodies with rounded leading edges we consider the exaggerated boundary layer over an airfoil in Fig.2.10. The stagnation flow field gives the initial boundary-layer velocity profile in the vicinity of x = 0. The velocity Uealong the edge of the boundary layer increases rapidly away from the fore stagnation point F. At some point, Uereaches a maximum at the point of minimum pressure. From this point onward, the pressure gradient along the surface changes sign to become adverse and begins to slow the boundary-layer flow. A point of inflexion (P2) develops in the velocity profile that moves toward the wall as xincreases. Eventually, the inflexion point reaches the wall itself, the shear stress at the wall falls to zero, reverse flow occurs, and the boundary layer separates from the airfoil surface at point S.[3] 26 2 Design Methodology Figure 2.9: Flap effect (modeled by a vortex) on the velocity distribution over the main wing. Figure 2.10: Boundary layer developing around an airfoil. Chapter 3 Computational Fluid Dynamics (CFD) Modeling This chapter explains the practical approaches for a CFD simulation used in this project, which started by the geometry creation of candidate airfoils and ended up with CFD post-processing of the simulation results. 3.1 Geometry Before starting the CFD modeling of airfoils, it is necessary to generate the airfoil geometries and, if available, it would be a good idea to have a fast and reliable simulation by using meshless computer programs, namely XFOIL for single airfoil design and simulation or MSES for high-lift multi-element airfoil design and optimization or PROFOIL that is a code for inverse design of airfoils. Unfortunately the two latter ones were not used in this project; MSES was not used because of the unaffordable price of the software and in case of PROFOIL because its full version is not available in market or on the internet. For this reason only XFOIL was used as primary software to test and modify candidate airfoils. Below line is a brief explanation about this software. XFOIL: The XFOIL code solves the panel method equations coupled to an integral boundarylayer formulation using a global Newton iteration scheme. The transition model used in XFOIL has been known to be reliable in predicting various airfoil related flow phenomena such as LSB (Laminar Separation Bubble) formations and transition locations accurately. XFOIL has also been used to validate wind tunnel results for other high lift airfoils, NLF airfoils and multiple flap configurations and shows good comparisons. However, it is also known to over predict Cland L/D at post stall values. No grid generation is necessary and the entire solution set is obtained 28 3 Computational Fluid Dynamics (CFD) Modeling in a few seconds even on a desktop computer. XFOIL, an interactive program for the design and analysis of subsonic isolated airfoils written by Mark Drela from MIT University. It consists of collections of menu-driven routines which perform various useful functions for airfoil redesign by interactive modification of geometric parameters such as: •max thickness and camber, highpoint position •LE radius, TE thickness •camber line via geometry specification •camber line via loading change specification •Blending of airfoils •Writing and reading of airfoil coordinates and polar save files One of the many capabilities of XFOIL is to increase the paneling number that is the amount of points by which the coordinate of an airfoil are determined and can result in a smooth and precise airfoil coordinate that is an important factor in CAD design. As long as the airfoils used in this project have a blunt trailing edge, all the trailing edges should be modified in XFOIL. In addition to generating and modifying airfoil geometry, XFOIL was also used as a fast and reliable software to evaluate and compare different candidate airfoils. In the next chapter the simulation, results and comparison between airfoils which performed by XFOIL will be presented. Figure:3.1 shows the environment of XFOIL. The mesh generator of this project (Pointwise) is not able to read airfoil coordinate by importing Excel or DATA files directly. Therefore, after geometry modification in XFOIL, the airfoil is ready to be saved again as a new airfoil and then by performing some basic Office Excel tasks, it will be be imported to CAD software. In this project SolidWorks from Dassault Systemes was used as CAD program. As explained before, the reason of using CAD program is, unlike ICEM CFD, the lack of ability of Pointwise (grid generator program) in reading coordinates data file like *.dat. The generated geometry in Solidworks can be exported in different recognizable formats ( *.iges, *.igs, *.step, *.stp, *.stl, *.sldprt etc. ) for Pointwise and many other mesh generator programs. 3.2 Turbulence Model There is a crucial difference when modeling the physical phenomena between laminar and turbulent flow. For the latter, the appearance of turbulence eddies occurs over a wide range of length scales so before starting the critical process of mesh generation, it is important to have a good understanding of turbulence and different models used 3.2 Turbulence Model 29 Figure 3.1: A Screen shot from XFOIL of Mark Drela showing its root menu in CFD codes. Knowing pros and cons of each turbulence model and respecting their requirements in choosing a right mesh type and grid resolution especially near the wall is of great importance. The reason why this section is located here, is its close connection with mesh generation process and physics of the problem. The below lines will explain the most widely used turbulence model in industrial and educational fields and then the choice of the best turbulence model among them will be discussed. Aerodynamic flows are usually complex flows characterized by their various Reynolds numbers which are sometimes at the order of million and different range of Mach numbers from subsonic condition. However, in case of motorsports we have to deal with low to moderate Reynolds numbers and flow is almost always subsonic, but its complexity still exists because the flow is either attached or separates at some specific part of airfoil. When the angle of attack is increased large-scale separation or unsteadiness often appear in the flow. In addition to it, CFD modeling of multi-element airfoils is more challenging since the flow field around such airfoil elements is characterized by unsteadiness, regions of separated flow and the confluence of the boundary layer of the downstream element with the wake of the upstream element[6].These phenomena pose significant challenges to CFD simulations. 30 3 Computational Fluid Dynamics (CFD) Modeling The majority of CFD studies would employ Reynolds-Averaged Navier-Stokes (RANS) models. More CPU demanding methods, such as the Unsteady Reynolds-Averaged Navier-Stokes (URANS), Large Eddy Simulation (LES) and Detached Eddy Simulation (DES) have been employed in recent years to model aeronautical flows among many others.[7] RANS models offer the most economic approach for computing complex turbulent industrial flows.Typical examples of such models are the K-εthe K-ωmodels in their different forms. These models simplify the problem to the solution of two additional transport equations and introduce an Eddy-Viscosity (turbulent viscosity) to compute the Reynolds Stresses.[8] 3.2.1 SST k-ωModel The draw-back of some k-εmodels is their insensitivity to adverse pressure gradients and boundary layer separation. They typically predict a delayed and reduced separation relative to observations. This can result in overly optimistic design evaluations for flows which separate from smooth surfaces (aerodynamic bodies, diffusers, etc.). The k-εmodel is therefore not widely used in external aerodynamics.[8] In all the simulations done in this project the turbulence model used is SST k-ω.The SST k-ωturbulence model [Menter 1993] is a two-equation eddy-viscosity model which has become very popular. The Shear Stress Transport (SST) formulation combines the best of two worlds. Below lines is an explanation about this model and the reason of using it as the dominant turbulence model in this thesis project. The ω-equation offers several advantages relative to the ε-equation. The most prominent one is that the equation can be integrated without additional terms through the viscous sublayer. This makes the formulation of robust y+-insensitive Enhanced Wall Treatment (EWT) relatively straightforward. Furthermore, k-ωmodels are typically better in predicting adverse pressure gradient boundary layer flows and separation. The downside of the standard ω-equation is a relatively strong sensitivity of the solution depending on the freestream values of kand ωoutside the shear layer. The use of the standard k-ωmodel is, for this reason, not generally recommended in ANSYS FLUENT. The SST k-ωmodel has been designed to avoid the freestream sensitivity of the standard k-ωmodel, by combining elements of the ω-equation and the εequation. In addition, the SST model has been calibrated to accurately compute flow separation from smooth surfaces. Within the k-ωmodel family, it is therefore recommended to use the SST model. The SST model is one of the most widely used models for aerodynamic flows. It is typically somewhat more accurate in predicting the details of the wall boundary layer characteristics than the Spalart-Allmaras model. The SST model (as all ω-equation based models) uses the enhanced wall treatment as default.[8] For the k-ωmodels, so-called low Reynolds number terms (low Re) have been pro- 3.3 Grid Generation 31 posed by Wilcox. These are available in ANSYS FLUENT as an option. It is important to point out that these terms are not required for integrating the equations through the viscous sublayer. Their main influence lies in mimicking laminarturbulent transition processes. According to Ansys Fluent recommendation usage of the low-Re terms is not encouraged. 3.3 Grid Generation Grid generation is the most time consuming and difficult part of the CFD analysis process. Grid generation often consumes up to 80 percent of the labor hours for a CFD project and is the largest controllable influence on the accuracy of the analysis. Specialized software programs have been developed for the purpose of mesh and grid generation, and access to a good software package and expertise in using this software are vital to the success of a modeling effort. Among all commercial/noncommercial grid generator codes ANSYS ICEM CFD, BETA CAE Systems S.A., Numeca Int., Cambridge Flow Solutions, Ltd., Pointwise, Inc. etc. are the most famous ones. For this project mesh generator of Pointwise Inc. has been used. Some reasons of choosing this software are user-friendliness, precision and easy and fast ways to create hi quality grids both structured and unstructured and then examine the quality of the generated grid by different accepted factors and also repairing bad cells with a single click of mouse. The other fantastic ability of this software is the extrusion of domain from 2D to 3d and creating blocks in different ways like following paths, rotating etc. Another interesting point of it is the possibility to export the generated mesh, connector or database to numerous CAD or CFD programs. In the following sections of this chapter, the grid generation approaches used in the current project will be explained. 3.3.1 Structured or Unstructured Grids? Structured grids can be considered as most natural for flow problems as the flow is generally aligned with the solid bodies and we can imagine the grid lines to follow in some sense the streamlines, at least conceptually, when not possible realistically. It has to be emphasized that structured grids will, compared to unstructured grids, often be more efficient from CFD point of view, in terms of accuracy, CPU time and memory requirement. The reason behind the development of unstructured CFD codes is essentially connected to the time required to generate good quality blockstructured grids on complex geometries. This task, with the best available software tools, can easily take weeks or months of engineering time and the associated engineering costs are considered as prohibitive industrially. Hence, the requirement for automatic grid generation tools has become essential for the further development of industrial CFD. Another drawback of structured grids is a form of stiffness connected to the fact that adding a point locally implies adding lines of each family through 32 3 Computational Fluid Dynamics (CFD) Modeling that point, which will therefore affect the whole domain. In complex geometries, this can be very detrimental and render the grid generation process quite cumbersome. Unstructured meshes are certainly well suited for handling arbitrary shape geometries, especially for domains having high curvature boundaries. Despite its many advantages, CFD users should also be aware of the disadvantages of employing an unstructured mesh for CFD simulations: •In comparison to a structured mesh, the points of an elemental cell for an unstructured mesh generally cannot be simply treated or addressed by double indices (i,j) in two dimensions or triple indices (i,j,k) in three dimensions. An elemental cell may have an arbitrary number of neighboring cells attaching to it, making the data treatment and connection arduously complicated. •Triangular (two-dimensional) or tetrahedral (three-dimensional) cells, in comparison to quadrilateral (two-dimensional) or hexahedral (three-dimensional) cells, are usually ineffective for resolving wall boundary layers. In most cases, the grid yields very long, thin, triangular or tetrahedral cells adjacent to the wall boundaries, thereby creating major problems in the approximation of the diffusive fluxes. •Another disadvantage in connection with data treatment and connectivity of elemental cells is the requirement for more complex solution algorithms to solve the flow field variables. This may result in increased computational times in obtaining a solution and may erode the gains in computational efficiency.[?] For single element airfoil it is an almost easy task to create hi-quality C-Type or O-Type structured grids using Pointwise Inc. mesh generator, however in case of multi-element airfoils it could take several days to generate a high quality structured mesh which makes the CFD convergence much faster than unstructured grid. As result, despite all the disadvantages of unstructured mesh mentioned in above lines, to facilitate and increase the mesh generation process, unstructured mesh was chosen for the whole domain except for the boundary layer of airfoils, which are nearly 30 to 50 layers of structured mesh 3.3.2 Boundary Layer and Estimation of First Cell Height for correct y+(Wall Unit) The small layer between solid objects surfaces and the free stream flow represents the boundary layer. The velocity gradient can be visualized as a velocity profile that is mainly governed by friction forces between the shear layers of different velocities. The boundary layer thickness increases with surface roughness and length. Two general types of boundary layers exist as can be seen in Figure 3.2; laminar and turbulent boundary layers. In a laminar boundary layer the flow shows layered behavior, while 3.3 Grid Generation 33 in a turbulent boundary layer the flow is chaotic and can have actuating components in a direction perpendicular to the surface. This causes small scale vortices and leads to an increase in friction drag. Due to instabilities the flow can go from a laminar to a turbulent state at a transition point. On road vehicles most of the boundary layer is turbulent. When the velocity gradient in a turbulent boundary layer becomes too large, the flow can not follow the contour of the surface any more and separates. Separation gives a significant rise in pressure drag. At the very bottom of a laminar boundary layer, the velocity profile is nearly linear Figure 3.2: Transition process in boundary layer on a flat plate and depends only on the wall shear stress and the viscosity, and not directly on the pressure gradient or on anything that happens in the outer part of the layer. In a turbulent boundary layer, the same dependence applies reasonably well to the wall region, which spans the viscous sublayer and the corner region of the velocity profile. In the viscous sublayer, the velocity profile is nearly linear, as it effectively is at the bottom of a laminar boundary layer. [9] The y+value is a non-dimensional distance, based on local cell fluid velocity, from the wall to the first mesh node. To use a wall function approach for a particular turbulence model with confidence, we need to ensure that our y+values are within a certain range. we need to be careful to ensure that our y+values are not so large that the first node falls outside the boundary layer region. If this happens, then the Wall Functions used by our turbulence model may incorrectly calculate the flow properties at this first calculation point which will introduce errors into our pressure drop and velocity results. The upper range of applicability will vary depending on the flow physics and the extent of the boundary layer profile. y+value required is determined by the flow behaviour and the turbulence model being used. If the flow is attached, then generally a Wall Function approach can be used, which means a 40 3 Computational Fluid Dynamics (CFD) Modeling Figure 3.8: Flap gap and overlap definition. 3.5 Set up the solver (Ansys Fluent) and physical models The CFD solver of this work was Ansys Fluent, a software contains the broad physical modeling capabilities needed to model flow, turbulence, heat transfer, and reactions for industrial applications. In order to obtain correct and reliable results, it is important to set-up the solver correctly. Selecting a wrong options even if the problem could converge, would give beautiful but wrong colorful results in post-cfd or in worst case the convergence difficulty or error messages would be probable. The next part will be a brief explanation about each choice was made in this work. Once the geometries and suitable mesh are generated and the boundary conditions are defined, the grids ready to be exported as fluid computational domain file *.cas to be recognized by Ansys Fluent. For a given problem the next step is to open the case file by Fluent. The whole set up procedure is as follow: •Import and check the mesh. •Select the numerical solver (for example, density based, pressure based, unsteady, and so on). •Select appropriate physical models. •Turbulence, combustion, multiphase, and so on. •Define material properties: 3.5 Set up the solver (Ansys Fluent) and physical models 41 –Fluid, Solid or Mixture •Prescribe operating conditions. •Prescribe boundary conditions at all boundary zones. •Provide an initial solution. •Set up solver controls. •Set up convergence monitors. •Initialize the flow field. 3.5.1 The Pressure-Based Segregated Algorithm ANSYS FLUENT allows users to choose one of the two numerical methods: •pressure-based solver •density-based solver Historically speaking, the pressure-based approach was developed for low-speed incompressible flows, while the density-based approach was mainly used for high-speed compressible flows. However, recently both methods have been extended and reformulated to solve and operate for a wide range of flow conditions beyond their traditional or original intent. Since in this project all the simulations have been solved by using the Pressure-Based Segregated Algorithm, the following section will focus on this algorithm. The pressure-based solver employs an algorithm which belongs to a general class of methods called the projection method. In the projection method, wherein the constraint of mass conservation (continuity) of the velocity field is achieved by solving a pressure (or pressure correction) equation.Two pressure-based solver algorithms are available in ANSYS FLUENT: •segregated algorithm •coupled algorithm The pressure-based solver uses a solution algorithm where the governing equations are solved sequentially (that is, segregated from one another). Because the governing equations are non-linear and coupled, the solution loop must be carried out iteratively in order to obtain a converged numerical solution. The segregated solution method is the default method in most commercial finite volume codes. It is best suited for incompressible flows or compressible flows at low Mach number. In the segregated algorithm, the individual governing equations for 42 3 Computational Fluid Dynamics (CFD) Modeling the solution variables (for example u, ν, w, p, T, k, ε etc.) are solved one after another. Each governing equation, while being solved, is decoupled or segregated from other equations, hence its name. The segregated algorithm is memory-efficient, since the discretized equations need only be stored in the memory one at a time. However, the solution convergence is relatively slow, inasmuch as the equations are solved in a decoupled manner. Figure 3.9 illustrates the segregated solution procedure. Unlike the segregated algorithm described above, the pressure-based coupled alFigure 3.9: Segregated Solution Procedure gorithm solves a coupled system of equations comprising the momentum equations and the pressure-based continuity equation. Since the momentum and continuity equations are solved in a closely coupled manner, the rate of solution convergence significantly improves when compared to the segregated algorithm. However, the memory requirement increases by 1.5 to 2 times that of the segregated algorithm since the discrete system of all momentum and pressure-based continuity equations must be stored in the memory when solving for the velocity and pressure fields (rather than just a single equation, as is the case with the segregated algorithm).[8] 3.5.2 Transient Solution Nearly all flows in nature are transient. Steady-state assumption is possible if we ignore transient fluctuations or employ ensemble/time-averaging to remove unsteadiness (this is what is done in averaging to remove unsteadiness (this is what is done in modeling turbulence). In CFD, steady-state methods are preferred because of lower computational cost and easier to post-process and analyze, however many applications like aerodynamics (aircraft, land vehicles, etc.), vortex shedding, rotating machinery (rotor/stator interaction, stall, surge), multiphase flows , free surfaces, bubble dynamics etc. require resolution of transient flow. Time step (∆t) must be small enough to resolve time-dependent features; make sure convergence is reached 3.5 Set up the solver (Ansys Fluent) and physical models 43 within the number of Max Iterations per Time Step. Time step size estimate can be chosen so that the transient characteristics of the flow can be resolved (e.g. flow within a known period of fluctuations) in other word convergence at every time step may not be necessary. Unsteady solution has the same procedure for segregated and coupled solvers (Fig 3.10). Figure 3.10: Transient (Unsteady) Solution Procedure Chapter 4 CFD Simulation Results In this chapter the final results of all the 2D CFD simulations done in this projects will be demonstrated and eventually the optimum point or region for each multielement configuration will be selected. As mentioned before, unfortunately there is no experimental work similar to this project, so the only way to evaluate the results is to first make sure that the turbulent model and its requirements namely y+have been chosen and designed precisely. Then it should be investigated that the solution is grid independent, it means that with increasing the number of cells and creating finer meshes, the results would not change significantly and the difference between results of each mesh refinement and the previous one are in an acceptable range. The last part that probably gives us a feeling that results are almost near to reality would be 3D simulation of the multi-element wing in its optimum point(s) of operation. In this project, since all the works were done on a laptop with Intel Core2 Duo CPU P8400 2.26GHz and only 2 GB RAM available and 3D simulations of this size need at least 5,000,000 cells in order to get a satisfactory result, unfortunately the 3D simulation was not successful and it just postponed to the other time when a powerful computer resource is available. Commercial CFD codes like ANSYSFLUENT incorporates impressive visualization tools within their user-friendly GUIs to allow users to graphically view the results of a CFD calculation at the end of a computational simulation. However, there are also many excellent stand-alone applications of independent computer graphics software packages that the users may opt to utilize for CFD applications. In this work a popular and versatile computer graphics software package, called TECPLOT has been used. Some abilities of this software are X-Y Plots, Vector Plots, Contour Plots, streamlines, triangulation of data, etc. However there are some open sources software like GNUplot but the features used in TECplot are much more powerful than GNUplot. 46 4 CFD Simulation Results 4.1 2D Single Airfoil At the very beginning of this project in order to visualize the flow around the main element airfoil (S1223) and to get a rough idea about the flow around it and also to study the grid dependency of the results, different series of tests were performed. The chord length of the single element is exactly the same as the main airfoil (m.c) in multi-element airfoil (240 mm). The algorithm for the solution of the NavierStokes equations utilized an implicit segregated velocity-pressure formulation, such as the SIMPLE or PISO scheme (Pressure Implicit with Splitting of Operators) which proposed by Issa (1986). This pressure-velocity calculation procedure was originally developed for non-iterative computation of unsteady compressible flows. Nevertheless, it has been adapted successfully for the iterative solution of steadystate problems. PISO is simply an extension of SIMPLE with an additional corrector step that involves an additional pressure correction equation to enhance the convergence. Progress toward a converged solution can be greatly assisted by the careful selection of various under-relaxation factors in order to increase the stability of the numerical procedure and to ensure the convergence of the iterative process. The reason for using the under-relaxation factors into the system of algebraic equations that govern the fluid flow is that they significantly moderate the iteration process by limiting the change in each of the transport variables from one iterative step to the next. However here are no straightforward guidelines for pertinent choices of these factors and it is mostly based on experience. 4.1.1 Boundary Conditions At the inlet, Dirichlet conditions were used for all variables. The inlet velocity based on the free-stream velocity Uref was taken as constant, with values of inlet flow velocity was assumed to be 66.67 m/s which corresponds for 240 km/h and considered as the maximum possible cornering speed of a GT car, or even when it goes through a straight road. The air dynamic viscosity at 288.16oKis 1.7894e−05 and its density equals 1.225kg/m3. Reynolds number based on the inlet velocities and the main airfoil chord length is Remainairfoil ≃1.1×106. At the outlet, zero-gradient conditions were applied for all the transported variables. No-slip wall boundary conditions were applied to the airfoil.As we know on the so-called no-slip condition, the boundary condition on a solid surface assumes zero relative velocity between the surface and the fluid immediately at the surface. Because the turbulence model is SST K-ωit is necessary to have a y+= 1 so the first cell distance next to the airfoil wall should be almost 5 ×10−3mm. 4.1.2 Results Because the main goal of this series of simulations was only visualization of the flow in the same angle of attack that this airfoil is going to be mounted as primarily 4.1 2D Single Airfoil 47 configuration set-up in multi-element airfoil, the angle of attack was remained constant at (aoa=0oand 5o). The domain, as explained before was divided into four unstructured smaller domains, starting close to the airfoil ending up at the inlet and outlet boundaries in addition to one structured domain for capturing viscous layer around the airfoil wall. The turbulent intensity was assumed to be 1% and turbulent viscosity ratio 10 for both velocity inlet and pressure outlet boundary conditions. A summary of the results and corresponding amount of cells is shown in Table 4.1. Airfoil= S1223 (0.5% T.E gap), Chord=240 mm, V∞= 66.67m/s,Re = 1.1×106 Turbulent Intensity= 1%, Turbulent Viscosity Ratio=10 Solver Total Cells Refinement Ratio AoA CL CL difference% CD CD difference% Iterations Fluent 135,037 NA 0o1.1409 NA 0.018643 NA 3605 Fluent 191,445 1.42 0o1.1561 1.3235% 0.018143 2.7184% 9362 Fluent 297,572 1.554 0o1.1561 0% 0.018071 0.3976% 6383 XFOIL NA NA 0o1.2868 NA 0.01271 NA NA Fluent 135,037 NA 5o1.63 NA 0.024947 NA 2329 Fluent 520,941 3.85 5o1.6479 1.0922% 0.024685 1.0558% 3135 Table 4.1: Main airfoil simulations (Single Element S1223) at 0oand 5oand Re=1.1×106 Refinement ratio is defined asNi+1 Niin which Niis the total numbers of cells in each simulation. Difference ratio of CLand CDwas calculated applying simple percentage difference equation: (|V1−V2| (V1+V2) 2 )×100 (4.1) 4.1.3 Grid Independence Study To assess the accuracy of CFD problems for a particular algorithm on a finite-grid one method is to apply it to a related but simplified problem. It means the one that possesses an exact solution. However, accuracy is usually problem-dependent; an algorithm that is accurate for one model problem may not necessarily be as accurate for another, more complicated problem. Another way to assess accuracy is to obtain solutions on successively refined grids (grid convergence) and to check that, with successive refinements, the solution is not changing and is therefore satisfying some predetermined accuracy. This technique assumes that the approximate solutions will converge to the exact solution as the finite quantities diminish, and then the approximate solution on the finest grid can be used in place of the exact solution; a grid-independent solution is thus achieved. Assuming that the accuracy of this approximate solution can be assessed, it is important to consider the related question of how accuracy may be improved. At a specific level, the use of high-order approximation or grid refinement would be expected to produce more accurate solutions. Nevertheless, such choices are meaningful only if they are considered in conjunction with execution time and computational efficiency. It is also important to be aware 48 4 CFD Simulation Results that a converged solution does not necessarily mean an accurate solution. It is desirable that a grid (mesh) independence study is performed to analyze the suitability of the mesh and to yield an estimate of the numerical errors in the solution. In addition, such a study is used to determine the minimum mesh resolution required to generate a solution that is independent of the mesh size used. This is ususally involves monitoring a fluid flow parameter that is of interest of study and how it changes under successive grid refinements. The level of accuracy required from a CFD analysis depends on the desired use of the results. The examination of the spatial convergence of a simulation is a straight-forward method for determining the ordered discretization error in a CFD simulation. The method involves performing the simulation on two or more successively finer grids. The term grid convergence study is equivalent to the commonly used term grid refinement study. As a common practice, before starting any simulation, the values of interest should be defined, and make sure that these values are monitored to ensure that they reach a steady state. It is also much more important to insure that the Residual RMS error values are at least 10(−4). Finally, we need to ensure that the overall imbalance in the domain is less than 1% for all variables. But the outlined approach will result in a single solution for the given mesh that we have used. Although the solution has converged based on RMS Error values, monitor points and imbalances, it is of greatest important to make sure that the solution is also independent of the mesh resolution. Skipping this task and not checking it, is a common cause of erroneous results in CFD, and this process should at least be carried out once for each type of problem, It also helps to have an understanding of the mesh sizing for similar problems in the future. For this reason the simulation firstly is performed using a coarse mesh and the solution is monitored until the convergence achieved. Then the mesh would be globally refined. This refinement rate is normally around 1.3 to 2. It means that the new grid has 1.3 to 2 times more cells that the previous mesh. Again the calculation is run until the signs of convergence appear. Then the computed values are compared. If their difference is big, it means that the grid needs more refinement and the solution is not grid independent. So the next refinement would be done and previous steps are repeated. This procedure continues until the results will not change and their in acceptable range. In this step we check the previous results from the point they started to remain unchanged and the smaller mesh will be chosen for the simulation in order to save CPU times. Considering the table 4.1, by comparing the results it is obvious that with grid refinements, the CLand CDvalues would not change significantly. It means that by using a domain with around 130,000 cells the results would be reliable and the simulation time would be faster. 4.2 2D Multi-element Airfoil 49 4.2 2D Multi-element Airfoil In previous chapter the procedure of simulation was explained in details. As it was mentioned, two general configurations were selected in which the deflection angle of the flap element (Eppler E420) airfoil that its chord length is 35% of the main airfoil (84 mm) was kept fixed at αf= 35oand αf= 40o(relative to main airfoil) while the daoa of the main airfoil was kept at αm= 0o. Then the relative gap and overlap between two elements were changed in increments of 1% to 2% of the main airfoil chord length. As soon as the results started to improve and the values of CL, downforce and especially CL/CDincreased, the increments became shorter in order to find the optimized point. Like previous simulation, characteristics of the inlet and outlet boundaries were remained unchanged. In all simulations it was assumed that the angle of attack of the incoming air from the car is 0ohowever after obtaining the optimum point the angle of attack was changed in order to investigate operative range of the multi-element airfoil. 4.2.1 Flap Deflection αf= 40o: Table 4.3 is a summary of simulations. The values for CL,max. , (CL/CD)max. and Downforcemax are highlighted in the table. As it could be guessed, the optimum operating condition of the multi-element airfoil is located in a region between O.L = 7.08% ∼10% and the Gap = 1.67% ∼2.08%. With manual optimization of the airfoil and having CPU limitation, it is so difficult to find a point in which there is an optimum of aerodynamics coefficients. Also In reality the flow condition around the multi-element airfoil is more complicated that the optimum point would vary every moment, but it is obvious that in a certain region, as pointed before, the multi-element has its best performance for this configuration. In order to have a sense of how the values are distributed in 2D surface an automatic triangulation of obtained values were performed. Figures 4.1 and 4.2 illustrate the contour plots of desired aerodynamics values. From these plots also we can visualize that the optimum operation condition of the multi-element airfoil is located in an area highlighted by pale pink color. 4.2.2 Flap Deflection αf= 35o: In the next configuration, in order to investigate the effect of relative angle of flap on performance of multi-element airfoil, the deflection angle of flap airfoil was changed to αf= 35o, relatively to the main airfoil. All the characteristics of the boundary conditions and average number of cells remained constant. This time by having more experience from the previous simulations, the overlapping and gap distance respectively started at 4.17% and 1.25%. In each fixed overlap, the gap distance was increased and the model was simulated again. This process was continued until 56 4 CFD Simulation Results Figure 4.6: Comparison between relative flow velocity around two multi-element airfoil configurations with flap at 40oand 35o. can be greatly enhanced if the airfoil has multiple elements with favorably configured slots between them. For a slot to be effective in enhancing maximum lift, the general pattern of flow through it must be as shown in Fig.4.7, in which the flow passes smoothly through the slot, from the lower surface to the upper surface, and is directed along the upper surface of the aft element. much of the air passing through the slot is not in the boundary layers and has free stream total-pressure. The same flow pattern which is available from the simulation results is shown in Fig.4.8. How the slot effect really works was explained in chapter 2 by simulating the flap effect as a vortex on trailing edge of the main element. A slotted configuration enhances maximum lift by doing two things: •1) Starting a fresh upper-surface boundary layer at the leading edge of each element. For elements after the first, this means a thinner boundary layer at the start of the pressure rise than would be there if there were no slot. 4.3 Discussion 57 Figure 4.7: Typical features of the flow through an effective high-lift slot. Figure 4.8: Streamlines passing through the slot, resulted from CFD simulation in the current work shows an effective high-lift slot. •2) Slot can provide leading edge suction-peak suppression or trailing-edge dumping-velocity elevation. Slots do this in either of two ways, or both simultaneously, depending on the situation of the given airfoil element. –Leading edge suction-peak suppression: When there is an element ahead essentially by providing some flow turning ahead of the leading edge of the current element, so that the flow does not rush around the leading edge as fast as it otherwise would. –The dumping effect: In this case trailing edge of the forward element (in this project, main airfoil) is placed in a high velocity region near the leading edge of the trailing element (flap airfoil). It results in reducing the velocity at the leading edge of an element and elevating the velocity at the trailing edge of the main airfoil which both reduce the total velocity drop the boundary layer is subjected to.[9] This phenomena can be seen in 58 4 CFD Simulation Results Fig.4.9 which is a comparison between single airfoil (main element S1223) and multi-element airfoil. Figure 4.9: Improvement of lift in multi-element airfoil has been compared with single airfoil in two different angles of attack. Leading edge suction-peak suppression of the flap element which increases the energy of boundary layer above what it would have been without a slot and elevating the velocity at the trailing edge of the main airfoil are the two factors by which slot effect helps enhancing the lift created by multi-element airfoil. 4.3.1 Effect of Turbulence Models on the Results In previous chapters it was explained that the he draw-back of some k-εmodels is their insensitivity to adverse pressure gradients and boundary layer separation. They typically predict a delayed and reduced separation relative to observations. This can result in overly optimistic design evaluations for flows which separate from smooth 4.3 Discussion 59 surfaces. The k-εmodel is therefore not widely used in external aerodynamics.[8] The SST k-ωmodel has been designed to avoid the freestream sensitivity of the standard k-ωmodel, by combining elements of the ω-equation and the εequation. In addition, the SST model has been calibrated to accurately compute flow separation from smooth surfaces. Within the k-ωmodel family, it is therefore recommended to use the SST model. The SST model is one of the most widely used models for aerodynamic flows. It is typically somewhat more accurate in predicting the details of the wall boundary layer characteristics than the Spalart-Allmaras model. In order to investigate the difference between these models several simulations were done. Among the models Realizable k-ε, Spalart-Allmaras and SST k-ωwhich was selected as the default turbulence model for this work were used. Results of the simulations are briefly plotted in Fig.4.10 and Fig.4.11 show the difference between the resultant pressure coefficient for a specific multi-element configuration. As it could be predicted there is a close similarity between Spalart-Allmaras and SST k-ω. The main difference between them can be visualized in critical points of the airfoil which are near the leading-edge and trailing-edge. Obviously realizable k-εshows an unreliable result for the simulation. 4.3.2 Separation Bubbles Another interesting phenomenon which may affect race car aerodynamics is a laminar bubble in the boundary layer. The boundary layer that starts at the airfoil’s leading edge is laminar initially but, typically, for Re > 0.2×106a transition to turbulent boundary layers occurs along the upper surface (suction side). On many airfoils with relatively large upper-surface curvatures, high local curvature over the forward part of the chord may initiate a laminar separation when the airfoil is at a moderate angle of incidence. But the increased thickness of the boundary layer results in a transition to a turbulent boundary layer, which is less sensitive to stall. Consequently, the flow reattaches, creating a bubble with an enclosed area of recirculating flow. Small disturbances grow much more readily and at low Reynolds numbers in separated, as compared to attached, boundary layers. Consequently, the separated laminar boundary layer may undergo transition to turbulence with characteristic rapid thickening. This thickening may be sufficient for the lower edge of the now turbulent shear layer to come back into contact with the surface and reattach as a turbulent boundary layer on the surface. In this way, a bubble of fluid is trapped under the separated shear layer between the separation and reattachment points. Within the bubble, the boundary of which is usually the streamline that leaves the surface at the separation point, two regimes exist. In the upstream region, a pocket of stagnant fluid at constant pressure extends back some way; behind this, a circulatory motion develops, as shown in Fig.4.13, with the pressure in this latter region increasing rapidly towards the reattachment point. •A short bubble of the order of 1% of the chord in length that exerts negligible 60 4 CFD Simulation Results Figure 4.10: Investigation of different turbulence models. effect on the peak suction value just ahead of it. •A long bubble that may be of almost any length from a few percent of the chord to almost the entire chord, which exerts a large effect on the value of the peak suction near the airfoil leading edge. Short bubbles exert very little influence on the pressure distribution over the airfoil surface and remain small, with increasing incidence, right up to the stall. In general, they move slowly forward along the upper surface as incidence increases. If a long bubble forms at moderate incidence, its length rapidly increases with increasing incidence, causing a continuous reduction of the leading-edge suction peak. The bubble may ultimately extend to the trailing edge or even into the wake downstream. This condition results in a low lift coefficient and effective stalling of the airfoil. Known as progressive stall, this usually occurs with thin airfoils and is often referred 4.3 Discussion 61 Figure 4.11: Contours of the pressure coefficient show the different between the results of the two turbulence models . Figure 4.12: Laminar separation and turbulent reattachment points. to as thin-airfoil stall. Fig.4.13 illustrates this phenomena for 35oflap deflection while the overlap and gap are respectively 5% and 4.167% of the main element chord. It results in generation of a big wake aft of the multi-element airfoil and a performance (CL/CD) reduction of 17.33% comparing to the optimum performance point which is located at 5% overlap and 1.667% gap. Fig.4.14 is a comparison of pressure coefficient plot of these two cases. 62 4 CFD Simulation Results Figure 4.13: Laminar bubble separation and complete separation of the boundary layer at 5% overlap and 4.167% gap (top) Laminar bubble separation and reattachment of the boundary layer at 5% overlap and 1.667% gap (bottom). 4.3.3 Variation of Angle of Attack and Multi-element Airfoil Performance Even though a motorsports wing does not see large changes in angle of attack during forward motion, it is necessary to have as wide an operating range as possible in order to give the aerodynamicist and the vehicle dynamicist enough options when it comes to car setup. The rear wing is often used to balance the car after the front wing setup has been completed to compensate for any possible undesirable characteristics of the car endowed to it by pre-existing handling traits. Due to the very low aspect ratios of race car wings, the primary source of drag comes from the induced component of overall drag. Therefore the chief concern in motorsports airfoil design is not one of profile drag reduction. Instead it is a maximization of downforce and the ability of the designed airfoil to sustain the highest possible levels of downforce across a wide range of physical and aerodynamic adversities. This way he possibility of slight changes in direction of the upcoming air and the effect of passing cars are taking 4.3 Discussion 63 Figure 4.14: Comparison between the resultant pressure coefficient plot at (5% overlap and 4.167% gap) and t (5% overlap and 1.667% gap). to account, at least in 2D simulation; In 3D simulation this phenomena is more complicated. In this project for both configurations the multi element airfoils were rotated around the leading edge of the main airfoil and the simulation was performed for different aoa increments. The results can be seen in the table 4.5 and table 4.6. Obviously with increase in angle of incidence the drag and lift both will increase, but this increase for lift is not continuously and in some point it starts going down and the airfoil is losing its performance significantly. The main reason of this behavior is the same thing that happens in single element airfoils and it is the moving of separation point toward the leading edge of the airfoil and finally stall of the airfoil. Fig.4.15 shows the turbulent intensity counters combined by streamlines around the airfoil in αf= 40oat different aoa. the flow separating from a body carries vorticity and a deficit in total-pressure, and that downstream of the tail of the body this vortical flow becomes the wake. Wakes take on a wide variety of forms. The wake behind a lifting body in 3D carries strong streamwise vorticity and is called a vortex wake. Wake flow not associated with lift in 3D is referred to as a viscous wake, not because the rest of the flow is not viscous, but because the wake is the part that has felt significant direct effects of viscosity. Vortex and viscous wakes are overlapping categories, and there is no rigorous way to assign a given wake to one or the other. 64 4 CFD Simulation Results The total drag of a body appears as a loss of momentum and an increase of energy in the wake. The loss of momentum appears as a reduction of average flow speed, while the increase of energy is seen as violent eddying (or vorticity). The size and intensity of the wake is therefore an indication of the body s profile drag. The wake of the multielement is growing and becomes more turbulent as the angle of attack increases. This is the main reason of more drag force and losing the performance. If the airfoil incidence is sufficiently large, separation takes place not far downstream of the maximum suction point, and a very large wake develops. This causes such a marked redistribution of the flow over the airfoil that the large area of low pressure near the upper-surface leading edge is seriously reduced, with the result that the lift force is also greatly reduced. This condition is referred to as stall.However as we can see the performance of the multi element airfoil is still good and reliable. Clearly the αf= 40oconfiguration shows a better performance by increasing the aoa, however the αf= 35oconfiguration has also good downforce in different aoa. Since the αf= 35oconfiguration was of the most interest, more simulations were performed to see its behavior in larger angles of incidence. Results of these series of simulations will be discussed in the next section. αf= 40oO.L=7.5% Gap=1.67% V∞= 66.67m/s,ReM≃1.37 ×106,Turbulent Intensity= 1%, Turbulent Viscosity Ratio=10 αmultielement CLCD Downforce (N) Drag (N) CL/CD 0o2.998 0.0512 2387.960 40.81 58.52 2o3.076 0.058 2449.454 46.51 65.55 4o3.10 0.0708 2466.180 56.29 66.29 5o3.073 0.0755 2439.55 40.70 65.41 . Table 4.5: CFD simulation results of Multi-element airfoil with flap position at αf= 40o, in different aoa while both airfoils are rotated around the leading edge of the main element airfoil αf= 35oO.L=5% Gap=1.67% V∞= 66.67m/s,ReM≃1.37 ×106,Turbulent Intensity= 1%, Turbulent Viscosity Ratio=10 αmultielement CLCD Downforce (N) Drag (N) CL/CD 0o2.833 0.042 2331.16 34.42 67.73 2o2.95 0.0478 2420.44 39.24 61.68 4o3.025 0.055 2483.96 45.182 54.98 6o3.054 0.0643 2506.72 52.79 47.48 8o3.026 0.0803 2463.63 65.39 37.68 . Table 4.6: CFD simulation results of Multi-element airfoil with flap position at αf= 35o, in different aoa while both airfoils are rotated around the leading edge of the main element airfoil 4.3 Discussion 65 4.3.4 K´arm´an vortex street In previous section the results of simulations of the multielement airfoil in both configurations were introduced and discussed. An interesting result of increasing the angle of incidence for the αf= 35oconfiguration occurs at αmultielement = 10oand it is similar to what is called K´arm´an vortex street or Von K´arm´an vortex sheet behind a cylinder or sphere which is a repeating pattern of swirling vortices caused by the unsteady separation of flow of a fluid around blunt bodies. The vortices are generated periodically on alternate sides of the horizontal axis through the wake, and in this way a row of vortices is formed. The row persists a very considerable distance downstream. This phenomenon was first explained theoretically by Von K´arm´an in the first decade of the twentieth century. A vortex is generated in the region behind the separation point on one side, and a corresponding vortex on the other side breaks away from the airfoil and moves downstream in the wake. When the attached vortex reaches a particular strength, it in turn breaks away and a new vortex begins to develop, again on the second side, and so on. The wake thus consists of a procession of equal-strength vortices, equally spaced but alternating in sign. During the formation of any single vortex while it is bound to the airfoil, an increasing circulation exists about the airfoil and generates a transverse (lift) force. With the development of each successive vortex. That is the main reason for oscillation of aerodynamic coefficients during the CFD simulation. This force changes sign, giving rise to an alternating transverse force on the airfoil at the same frequency as that of the vortex shedding. If the frequency happens to coincide with the natural frequency of the wing s oscillation, however it may be supported, appreciable vibration may result.[3] As mentioned in above lines the most important signs for detection of this behavior in CFD are oscillation in aerodynamic coefficients and not convergence of the problem after the long time. 4.3.5 Effect of Variation of Sportscar Speed Like other vehicles and even more critically, racecars have to operate in different speeds and as a result the rearwing must show a stable and satisfactory performance in these varying conditions. New luxury sport cars benefit from the smart computerized control variable rearwings however according to competition rules of GT cars usage of this type of wing is still prohibited. In this work in order to observe the performance of the multi-element airfoil, three series of simulation were done in three different speeds: 66.67m/s, 55.56m/s and 44.67m/s for the αf= 35oconfiguration at its optimum point . The results can be seen in table4.7. By visualizing the results we can understand that in spite of the proportional reduction in downforce and drag with reduction in speed, the aerodynamic coefficients and performance of the airfoil have remained unchanged which is a good news for this multi-element configuration. 72 5 Conclusions Figure 5.2: 3D domain around 25% of the wing including the endplate. 5.1.2 Analysis of Twisted Wing Due to the shape of the roof-line, the airflow over the center of the car will hit the wing at a steeper angle of attack than the airflow to the outer ends of the wing. The airflow over the center of the car flows over the roof then turns downward towards the boot lid or trunk. The airflow to the left and right ends of the wing is at an angle closer to horizontal than the airflow to the center of the wing. A twisted element wing allows for the varying angles of attack of the airflow on a racecar, as the air flows over the roof-line and over the sides of the car. So if a straight element wing is run at an angle of attack where you are close to the stall angle at the left and right ends of the wing, then center of the wing is seeing a greater relative angle of attack, which can prematurely stall the center of the wing. However according to the racecar aerodynamicist pioneer, Simon McBeath, what this twist at the center of the wing also does is to reduce the wing’s downforce potential at more moderate angles. The center section of the wing on a closed car already generates less downforce than the outer sections, because the air that encounters the center part of the wing has had to do some work in passing over the car’s upper surface, and it loses energy during this passage. The wing cannot therefore develop the same magnitude of low pressure on its central underside, or indeed magnitude of raised pressure on its central upper surface, as the relatively undisturbed air that encounters the wing’s outer sections. In spite of this, it would be interesting to study pros and cons of twisted wing in 3D CFD environment. Appendix A Some Aerodynamics Definitions This appendix presents some of the common words and expressions used in this work. The reason of putting them in appendix section is to reduce the amount of unnecessary texts in the main sections of the thesis and focus on the main items, so if the reader is interested to become familiar with some theories or technical words might refer to this part. •Airfoil Geometry: If a horizontal wing is cut by a vertical plane parallel to the centerline, the shape of the resulting section is usually like that Fig. A.2. This is an airfoil section, which for subsonic use almost always has a rounded leading edge Figure A.1: Airfoil (wing section) geometry and definitions. •Two-Dimensional Flow: Consider flow in two dimensions only. It is the same as that between two planes set parallel and a little distance apart. The 74 A Some Aerodynamics Definitions fluid can then flow in any direction between and parallel to the planes but not at right angles to them. This means that in the subsequent mathematics there are only two space variables: xand yin Cartesian (or rectangular) coordinates or rand θin polar coordinates. For convenience, a unit length of the flow field is assumed in the z direction perpendicular to xand y. This simplifies the treatment of two-dimensional flow problems. •Pressure Distribution on an Airfoil: The pressure on the surface of an airfoil in flight is not uniform. Fig. shows typical pressure distributions for a given section at various angles of attack. It is easier to deal with nondimensional pressure differences using p∞, the pressure far upstream, as the datum. Thus the coefficient of pressure is introduced as Looking at the sketch for zero incidence (α= 0), we see that there are small regions at the nose and tail where Cpis positive but that over most of the section it is negative. At the trailing edge the pressure coefficient comes close to +1 but does not actually reach it. The reduced pressure on the upper surface is tending to draw the section upward while that on the lower surface has the opposite effect. With the pressure distribution as sketched, the effect on the upper surface is larger, and there is a resultant upward force on the section, that is, the lift. Figure A.2: Typical pressure distributions on an airfoil section. •Suction Peak: There is a decrease in pressure as we move away from the stagnation point of attachment near the leading edge, and a minimum pressure called the suction peak, which can be very close to the leading edge or farther back, depending on the airfoil shape and the angle of attack. (Figure A.3) •Pressure Recovery: The suction peak is followed by an increase in pressure, 75 or pressure recovery from the suction peak to the trailing edge.The recovery region is where the pressure gradient is adverse.In general, a streamlined body with thickness in attached flow must have a recovery region at the rear. (Figure A.3) [9] Figure A.3: Pressure Distribution over NACA 4410 airfoil at α= 2◦ •Canonical Pressure Coefficient (Cp): In his classic Wright Brothers lecture on high-lift aerodynamics, Smith (1975) suggested that plotting recovery pressure distributions in what he called canonical form, in terms of a pressure coefficient relative to the suction-peak pressure and normalized by the peak dynamic pressure, reduces the variation in ∆Cpbetween the suction peak and separation and makes the separation trends easier to see. The canonical pressure coefficient Cpis thus defined and related to conventional Cpby: Cp≡P−P0 1 2ρu02 = 1 −(ue u0 )2= (u∞ u0 )2(Cp−1) + 1 = Cp−Cp0 1−Cp0 (A.1) where the subscript o denotes conditions at the suction peak, which we will take as the start of the recovery. Note that Cpat the suction peak is zero by definition, and it takes on only positive values in the recovery. Separation of a turbulent boundary layer generally occurs at Cpvalues between 0.4 and 0.9, a much smaller range than we would see in terms of conventional ∆Cp. •Rooftop: Rooftop is part of the pressure distribution of upper part of an airfoil ahead of the pressure recovery point. Rooftop pressure distribution 76 A Some Aerodynamics Definitions have a gradually changing or approximately constant upper surface pressure over the forward part of the section. Bibliography [1] Joseph Katz, Race Car Aerodynamics, Designing for Speed. Bently Publishers, 1995. [2] Michael S. Selig and James J. Guglielmo, “High-lift low reynolds number airfoil design,” journal of Aircract, vol. 34, 1997. [3] Houghton E. L., Carpenter P. W. , Steven H. Collicott, Daniel T. Valentine, Aerodynamics for Engineering Students, 6th Edition. Elsevier, 2013. [4] LE MANS GRAND TOURISME ENDURANCE 2014, Technical Regulations for Grand Touring Cars. FIA Sports, 2013. [5] Liebeck, R. H., “Subsonic airfoil design,” Progress in Astronautics and Aeronautics: Applied Computational Aerodynamics AIAA, vol. 125, pp. 133–165, 1990. edited by P. A. Henne. [6] van Dam, C. P., “The aerodynamic design of multi-element high-lift systems for transport airplanes,” journal of Progress in Aerospace Sciences, vol. 38, pp. 101– 144. [7] B. Zhong , F. Scheurich, V. Titarev and D. Drikakis , “Turbulent flow simulations around a multi-element airfoil using URANS, DES and ILES approaches,” 19th AIAA, 22-25 June 2009. [8] ANSYS FLUENT USER’S GUIDE, “Ansys 14.5 help.”. [9] Doug McLean, Understanding Aerodynamics (ARGUING FROM THE REAL PHYSICS). Wiley, 2013.