VALIDATION OF CFD METHODS FOR DOWNWIND SAIL DESIGN

High Performance Yacht Design Conference Auckland, 4-6 December,2002 VALIDATION OF CFD METHODS FOR DOWNWIND SAIL DESIGN Stephen Collie 1, steve.collie@xtra.co.nz Peter Jackson 2, p.jackson@auckland.ac.nz Margot Gerritsen 3, margot.gerritsen@stanford.edu Abstract. The suitability of CFD codes based on the Reynolds Averaged Navier Stokes equations is investigated for use in downwind sail design. Simulations are performed using CFX5 and are validated using wind tunnel experiments carried out at the Auckland Yacht Research Unit. Due to the complexity of the downwind flow situation the simulations are limited to two-dimensional analysis. The complex separated flow around downwind sails is heavily dependent on the choice of turbulence model. Accurate prediction of separation points is difficult and turbulence models typically delay separation and thus underestimate the size of the wake which has a large influence on lift and drag calculations. The SST k-omega model was found to be the most suitable model available in CFX for separated flows. In the wind tunnel experiments, the spinnaker geometry is approximated by a circular arc with 24.7% camber. Force measurements were taken through a range in angle of attack from 5 to 30 degrees. At all angles of attack the flow is unsteady and periodic vortex shedding is evident. Through flow visualisation it is apparent that three-dimensionalities exist in the separated wake. Additional validation work has also been carried out using a 10% camber section which has a flow that is nominally two dimensional and is steady and predominantly attached at low angles of attack. NOMENCLATURE c Chord length ε Dissipation of turbulent kinetic energy k Turbulent kinetic energy ρ Density ω Specific rate of dissipation of turbulent kinetic energy τ w Wall shear u τ Friction Velocity (u τ = (τ w /ρ) 1/2 ) ν Kinematic viscosity y + Non-dimensional measure of distance to the nearest wall (y + = u τ y/ν) 1. INTRODUCTION This paper is part of a larger research effort to assess the practicality of CFD usage for reliable and accurate downwind sail design and performance analysis. With the rapid advancement and increasing affordability of high-end computers, engineers and designers are increasingly tempted to invest in CFD methods. However applying CFD methods to separated flows is a challenging task due to the inadequate performance of many turbulence models. It is unwise to embark upon a computational design program for a flow as complex as a downwind sail configuration without first exploring the suitability of the solution method. In order to be confident of results and understand their limitations it is necessary to first validate the method carefully and develop a good understanding of the physics involved. It is common for sail designers to rely almost entirely on computational approaches in the design of upwind sails. Wind tunnel tests are inaccurate for upwind studies due to difficulties in producing a realistic inflow and trimming the sails accurately. Upwind sails involve predominantly attached flow for which computational methods are well established. Conversely in downwind sail design CFD methods are in relative infancy and wind tunnel testing is the primary tool in aerodynamic analysis. Upwind sail design codes are most commonly based on the vortex lattice method [1] and can provide three-dimensional solutions for the flow past genoa - mainsail configurations in less than a minute on a common desktop PC. Consequently extensive parametric design studies can be carried out using a large number of design variables. However panel codes are only valid for close-hauled sailing conditions where the flow remains attached. In fact their inability to predict leading edge and trailing edge separation makes the application of panel methods for performance prediction questionable even in close hauled conditions. Consequently they are seldom used in velocity prediction programs (VPPs). In order to simulate viscous flows involving separation it is necessary to model the boundary layer of the sail. Bailey [2] developed upon the work of Jackson and Fiddes [3] using a two-dimensional panel code coupled to integral boundary layer methods to compute twodimensional sail flows. Bailey s model was capable of predicting turbulent transition, leading edge separation and boundary layer separation. However it was found that the methods used were only applicable to low camber sails at moderate angles of attack. Unfortunately extension of such a coupled method to three dimensions is a difficult and as yet unexplored task. The downwind flow regime is complex. Not only is there extensive separation but the wake system is unstable with vortices shed alternatively from the leeward and windward surfaces of the sail. Karman vortex streets 1 Graduate Student, Department of Mechanical Engineering and Department of Engineering Science, University of Auckland 2 Professor, Department of Mechanical Engineering, University of Auckland 3 Assistant Professor, Department of Petroleum Engineering, Stanford University

have been observed in the wake of downwind sails in wind tunnel flow visualisation (smoke streams). To further complicate the flow all sail flows involve leading edge separation due to the sharp leading edge. To the knowledge of the Authors there have been no publications to date on the validation of computational analysis for highly cambered sail flows that involve significant trailing edge separation. In fact it is difficult to find a flow case that involves the typical flow features of downwind sail flows. Other high-lift foils such as aircraft take-off and landing configurations and front and rear wings on race cars involve the same design goal of maximising lift while ignoring the influence of drag. However these foils are allowed to have slots to sustain attached flow. Downwind sail flows resemble flows past circular cylinders more closely than most high-lift devices. Milgram [4] gathered force measurements for several thin cambered plates with 12, 15 and 18% camber. Unfortunately the models all have lower camber than typical downwind sails. Two dimensional mast-sail combinations were studied by Wilkinson [5]. These sections were typical of upwind sail shapes and did not produce the large amounts of boundary layer separation typical in downwind configuration. 2. THE TWO-DIMENSIONAL SAIL MODEL Real sail flows are intrinsically three-dimensional. Through smoke visualisation streams have been observed to pass a gennaker to weather approximately a third of the height up the luff, then drop dramatically and exit approximately midway along the foot. To leeward the opposite occurs; smoke streams passing the luff near the foot leave the sail well up the leech. Even near mid height there is considerable cross flow. A schematic of the flow past a gennaker is provided in Figure 1 illustrating cross flow on the sail surface and the development of tip vortices around the head and foot. Figure 1. Schematic of the flow past a gennaker. Leeward streamlines - - - Windward streamlines Despite the fact that real sail flows are strongly threedimensional, two-dimensional sail flow solutions are still valuable. They provide a useful tool for a designer to explore the influence of design parameters such as camber and draft position. This type of analysis is valuable both as a tool to provide force output and performance analysis but also to visualise the consequences of design changes. Two-dimensional simulations are also valuable for validation of three-dimensional simulations. From a turbulence modelling perspective the two-dimensional simulations present many of the same difficulties as the three-dimensional problem: leading edge separation, reattachment, boundary layer recovery, separation and the formation of an unsteady wake. The only additional complexity in the three-dimensional case is the development of tip vortices that involve large streamline curvature. However for validation of the ability of turbulence models to predict separation and the resulting unsteady wake, two-dimensional sail flows provide a good test case. A typical two-dimensional downwind sail flow is illustrated in Figure 2. For simplicity we have chosen not to include the mainsail in the simulations as its addition adds no complexity, at least from a turbulence modelling perspective. Figure 2. A two-dimensional downwind sail flow. Real sails are flexible and flying shapes are considerably different to the unloaded shapes (design shapes). The sails are dynamic, moving under the changing onset and hence the fixed sail approximation is not a correct representation of the real, dynamic situation. To predict the flying shape computationally requires coupling of the CFD solver to a Finite Element Analysis (FEA) tool. Because the aim of the current study is to investigate and validate turbulence models, we use fixed sail shapes and ignore the shape changes that are likely to occur under the dynamic loading of the wind. Turbulence models will perform no differently for flexible membranes than for fixed shapes. 3. WIND TUNNEL EXPERIMENTS Wind tunnel experiments were carried out at the De Bray tunnel in the University of Auckland s Yacht Research Unit. The Tunnel is a low-speed, closed loop facility with a test section of dimensions 768mm 615mm. The tunnel has a maximum speed of 60m.s -1 and a maximum turbulence intensity of 1%. The wind tunnel model is positioned on aerodynamic struts above the force balance (see Figure 3). The model was constructed out of rolled 1mm steel plate to a radial tolerance of less than 3mm ( 0.6% camber). The designed curve has a camber of 24.7%, a radius of 200mm and a chord length (c) of 319mm. Steel strengthening sections were soldered to the underside of the model in order to minimize deflection under load and transmit the loads to the struts.

Figure 3. Wind tunnel model. The pivot point of the model (front struts) is 311mm above the tunnel floor and 77mm back along the chord from the leading edge. Consequently the position of the leading edge moves with angle of attack. The model was tested through a range of angles from 5 through to 30 at 2.5 intervals. A second model with a camber of 10% was also tested through a range of angles from -4 to 18 at 2 intervals. This second model has identical dimensions asides from camber. At each end of the model end plates are positioned that span the height of the tunnel. They are 1478 mm long, with the front of the end plates 448 mm in front of the leading edge of the model. The end plates are positioned 165.5mm inside the side walls of the tunnel to allow the tunnel s boundary layer to pass without influencing the model. The model is 435mm (1.37c) wide and small gaps (~2mm) exist between the tips of the model and the end plates. Tape and petroleum jelly were used to limit tip leakage through the small gaps. Particular care was taken to ensure that friction between the model and the side walls did not influence force measurements. This was verified by measuring the forces when fixed weights were applied to the model. The model was tested at an inlet speed of 25m.s -1 which corresponds to a Reynolds number of 5.25 10 5. This Reynolds number is significantly lower than the typical Reynolds number range of 2-3 million for IACC sail flows. However at these Reynolds numbers it is believed that the flow is reasonably independent of Reynolds number. Sail flows exhibit knife edge separation at the leading edge, forming a subsequent recirculating separation bubble. Consequently the boundary layer reattachment process is always turbulent and fairly independent of Reynolds number. In the experimental study of flat plate leading edge bubbles of Crompton and Barrett the shear layer was observed to develop turbulent traits shortly after detachment at the leading edge [6]. Reynolds number independent results were obtained above a Reynolds number of 2.2 10 5. 4. SOLVER DETAILS CFX5 is a general purpose CFD solver capable of solving incompressible and compressible flows, multiphase flows and flows involving heat transfer, combustion and radiation. CFX5.5 uses the Finite Volume Method to solve the Reynolds averaged Navier- Stokes (RANS) equations. The mass and momentum equations are coupled together and solved using incomplete lower upper factorisation accelerated using additive correction algebraic multigrid [7]. The differential equations are discretised using the bounded second order NAC (Numerical Advection Correction) scheme. The solution is advanced using backward Euler time integration. For unsteady simulations a series of inner iterations are required at each time step in order to remove errors associated with the linearisation of the advection term. A convergence study was carried out investigating the influence of the number of inner iterations and it was found that 4 inner iterations was most suitable. Using more than 4 inner iterations proved to make solution times too long and decreasing the time step size was a more appropriate means for reducing these non-linearity errors. For unsteady computations second-order Euler time stepping was used. The following turbulence models are compared in this paper: Standard k-ε [8], Standard k-ω [9] and SST k-ω [10]. An in depth review of turbulence modelling for sail flows is given in [11]. Through this study it was apparent that the SST model holds distinct advantages over other two-equation turbulence models. Alternative models such as Reynolds stress models are significantly more complicated and capture more of the physics. However there is no evidence that such models offer substantial improvement for separated flows. With an increase in sophistication comes an increase in computational cost making Reynolds stress models impractical for our purposes. The Standard k-ε model has been the most commonly used turbulence model over the past 30 years. Consequently its shortcomings are well known. One of its drawbacks is that it is inaccurate (without viscous modifications) when integrated through the near wall of a boundary layer. It is also difficult to impose a boundary condition on ε at the wall. Consequently boundary conditions are usually applied at the first grid point off the wall using the log-law of the wall. This approach is known as the wall function approach and is the implementation used in CFX. The Standard k-ε model is also notorious for overpredicting the eddy-viscosity in adverse pressure gradients and separated flow regions. Consequently separation is almost always delayed. The Standard k-ω model can be integrated through boundary layers without modification. The model also performs much better in adverse pressure gradients and separated regions. However the model is known to be particularly sensitive to free stream turbulence levels. This potentially poses a problem as it is difficult to correctly specify free stream turbulence using far-field boundary conditions since turbulence naturally decays

through the domain. The turbulence levels in the current simulations are low and are not expected to have an adverse influence on the turbulence model comparisons. The SST model is a blend between the strengths of the k- ε model and the k-ω model. The k-ω model is used in the boundary layer and the model blends to k-ε (in a ω formulation) at the outer edge of the layer. In this fashion free stream dependence is avoided and the benefits of k- ω in the boundary layer are retained. The SST model also uses a limiter on the eddy viscosity to aid performance in regions of large mean shear. Consequently it is less likely to inhibit separation of boundary layers subject to adverse pressure gradients. 5. RESULTS AND DISSCUSSION 5.1 CFD Pre-Processing A schematic of the domain is illustrated in Figure 4. The inlet is positioned 2.75c upstream of the sail section and the outlet is positioned 6.69c downstream of the leading edge. The side walls are positioned corresponding to the roof and floor of the tunnel following the dimensions given in section 2. Free-slip boundary conditions are used on the side walls. It is felt that it is necessary to include these walls due to their close proximity to the sail model. Due to the presence of the side walls a new grid is required for each new angle of attack. Grids were generated using ICEM-HEXA, a block-structured grid generator which is available as an add on to CFX. The grids have considerable refinement near the sail surface in order to adequately resolve the boundary layer. Considerable streamwise refinement is also used at the leading and trailing edges and cell stretching in these areas is limited to an aspect ratio of 2.5. An identical setup was used for both the high and low camber tests. 5.2 Grid Convergence Study Three different grids were used in the grid refinement study. At each refinement the grid spacing was reduced to approximately half across the entire domain. These grids are summarised in table 1. The Coarse grid is illustrated in Figure 5. The grid convergence study was performed only with the SST turbulence model, and only for the 15 degrees case. Figure 6 shows the calculated force coefficients for the three grids. 1/N is a measure of the gird spacing and is calculated as (number of cells) -1/ 2. Each of the solutions are computed using a time step of 0.0125s and 4 inner iterations. The medium grid produced a lift coefficient that was 1.6% smaller than the fine grid result. Unfortunately halving the grid spacing again would result in a grid that would be impractical with regards to memory requirements and solution time. However for practical purposes the medium grid is acceptable and within 3% of the extrapolated value for lift. INLET SAIL SECTION Figure 4. The flow domain. SIDE WALLS Table 1. Grid Details (Angle of attack =15 ) Grid Cells Average y+ Coarse 8496 2.5042 Medium 28912 1.2128 Fine 120482 0.6106 Figure 5. The coarse grid (angle of attack = 15 degrees). Cl Cd 2.94 2.91 2.88 2.85 2.82 2.79 0.40 0.38 0.36 0.34 0.32 0.30 OUTLET 0.000 0.004 1/N 0.008 0.012 0.000 0.004 1/N 0.008 0.012 Figure 6. Grid Convergence of the time averaged lift and drag coefficients. A convergence study was also carried out on the time step. Solutions were compared using time steps of 0.025s, 0.0125s and 0.00625s. The lift coefficient calculated using the medium timestep was just 0.65% higher than the lift coefficient calculated using the short time step. For all simulations the 0.0125s was used for the timestep, this corresponds to approximately 32 iterations per period of vortex shedding.

5.3 Wind Tunnel Comparison (high camber tests) CFD and wind tunnel force coefficients are presented in Figure 7. In the experimental data a peak in the lift coefficient exists at 10 degrees. This is the so-called ideal angle of incidence where there is no leading edge bubble disrupting the flow. There is a small drop off in lift above 10 degrees associated with the formation of the leading edge bubble. Above 15 degrees the lift starts to increase again. At 30 degrees the model is fully stalled (totally separated flow) and above this angle the lift coefficient is expected to drop off once more. The same trends are evident in the CFD results. The ideal angle of incidence is slightly lower (around 8 degrees) in the CFD, and at 30 degrees the lift curve for the SST model is starting to level off. At this angle the leading edge bubble detaches and reattaches in a semi-chaotic manner. At lower angles vortex shedding is regular and a Karman vortex sheet exist in the wake (see Figure 8). Downwind sails are trimmed to the lowest possible angle achievable without the luff collapsing due to stagnation on the leeward side of the leading edge. Due to the random nature of the wind it is impossible to trim sails to ideal incidence and instead the sails are generally set at 5 15 degrees above ideal angle of attack. If we assume an apparent wind of 90 so that we are looking to maximise lift while paying little attention to drag, then Figure 7 would indicate that the sails should be trimmed to much higher angles of attack. However for the threedimensional case there is considerable downwash due to tip vortices, consequently the ideal angle of attack is much higher and is closer to the angle of attack where real sails are fully separated (stalled). For real sails maximum lift occurs at ideal angle of attack. 4.5 Cl 4 3.5 3 2.5 2 2 Cd 1.5 1 0.5 0 0 10 alpha 20 30 0 10 alpha 20 30 Figure 7. Force coefficients versus angle of attack. Data, SST, + k omega, k epsilon Observations from smoke visualisation indicate that 3D downwind sails generally separate at approximately 40-50% along the chord. 2D CFD results (without mainsail) indicate that angles of attack of between 20 and 25 degrees are required in order to obtain this degree of separation. In this range of angles the CFD results compare more favourably with the wind tunnel than at lower angles. The lift forces are overpredicted by CFD which is a commonly reported shortcoming of turbulence modelling. Overprediction of lift is due to large values of the eddy viscosity causing the boundary layer to remain attached in adverse pressure gradients that would normally cause separation. This effect has been documented for many similar flows such as the NACA 4412 airfoil at maximum lift [12]. However in such highlift validation studies comparisons between CFD and experiment have shown much better agreement than the current comparison. In our case the primary source of the error is attributed to three-dimensionality in the wind tunnel tests. Surface oil Figure 8. Velocity contours and streamlines. Angle of attack = 15. visualisation shows spanwise variation of the separation point. Surface tufts illustrated cross-flow in the separated region near the trailing edge. Upstream of separation the flow was nominally two-dimensional, although surface oil streams did bend slightly immediately upstream of the separation line. The three-dimensional structures present in the wake originate at the tunnel walls. The boundary layer on the wind tunnel wall interacts with the boundary

layer on the sail creating a horseshoe vortex around the leading edge of the sail. Consequently there is a greater degree of flow separation near the tunnel walls. This effect influences the wake right across the span of the sail. A basic sketch of the flow structure is illustrated in Figure 9. On the left hand side of the foil the flow visualisation results are illustrated with the arrows representing the directions of surface tufts. Oil streaklines are also shown, upstream of the separation line. On the right hand side of the foil a schematic of the wake structure is illustrated. At approximately quarter and three-quarter span longitudinal vortices exist in the wake. This vorticity develops from the second (lower) separation bubble of the vortex pair. This wake structure was confirmed using a threedimensional CFD model. The wake streamlines from the CFD simulation are illustrated in Figure 10. The grid was based upon the coarse grid from the two-dimensional study, with 60 grid points in the spanwise direction and a symmetry plane at midspan. The surface plots of pressure and shear stress in Figure 11 illustrate spanwise variations. The shear stress contours closely follow the separation line patterns observed in the surface oil visualisation. The presence of the longitudinal counter rotating vortex pair causes downwash near mid span and upwash near the tunnel walls. Through examination of the streamlines upstream of the foil it is clear that the net effect of the three-dimensional wake is to reduce the effective angle of attack to the leading edge. Figure 9. The three-dimensional wake. Figure 10. Three dimensional wake structure, angle of attack =15 (image reflected through symetry plane) Figure 11. Suction side surface shear stress (top) and pressure coefficient (bottom). The leading edge bubble in the three-dimensional simulation is nominally two-dimensional and of almost constant length across 90% of the foil s span (the bubble breaks down near the side walls). At this angle of attack (15 ) the leading edge bubble reattaches at 0.033c, for the equivalent two-dimensional simulation reattachment occurred at 0.077c. The small leading edge separation bubble in the three-dimensional simulation is due to the lower effective angle of attack imposed by the threedimensionality of the wake. From Figure 7 it is evident that the wind tunnel predicts the ideal angle of attack (indicated in the lift curve by a local maxima) to be approximately 2 degrees higher than the CFD results indicate. This higher ideal angle of attack is due to downwash induced by the threedimensional wake. Despite using tape to seal of the tips between the model the side walls, there is still likely to be a small amount of tip leakage. Flow visualisation was performed without tape sealing the tips and considerably more three-dimensionality was observed. Force measurements were also taken with the tape removed and the discrepancies with the CFD results were greater.

Notably the ideal angle of attack was approximately 2.5 degrees higher than the previous wind tunnel experiments. Unfortunately the errors caused by the threedimensionality of the wind tunnel results are too large to allow reliable evaluation of the relative performances of the turbulence models. Efforts were made, but without success, to reduce the wake cross flow using straightening plates attached to the rear half of the model on the suction side. The forces from the three-dimensional CFD results (at 15 ) were in better agreement with the wind tunnel experiments than the two-dimensional simulations. The lift was just 2.5% lower than the experimental results and the drag was 9.3% lower. However the grid was relatively coarse and no refinement studies were performed. The grid refinement study in Figure 6 indicates that the forces can be expected to rise with grid refinement. The three-dimensional simulations were performed primarily for visualisation and to aid understanding of this complex three-dimensional flow. To draw stronger conclusions would require a more indepth study. It is highly likely that the section data presented by Milgram in [4] is affected by similar three-dimensional effects. Milgram notes that wall effects are neglected and that it was impossible to estimate the influence that nonuniform flow separation would have on the results. Milgram s model had a aspect ratio of just 2.21 and had 1.6mm gaps at the tips. Based on the results of the current study it is clear that Milgram s results are adversely affected by wall effects and tip leakage. 5. 4 Low Camber Model Tests The CFD model uses grids from the high camber model mapped onto the new (low camber) geometry. A grid refinement study was performed at an angle of attack of 8 degrees. Results indicated satisfactory grid convergence for the medium grid, with both lift and drag within 1.6% of the fine grid solution. Results for the lift coefficient are given in Figure 12. Below 4 degrees the comparison is good with both the wind tunnel and CFD results starting to level off due growth of the trailing edge separation region. Even at 4 degrees there is a small amount of trailing edge separation, however the bubble is small. Above 4 degrees the CFD results continue to level off while the experimental results start to climb. The lift coefficient in the experimental results continues to increase, surprisingly close to the theoretical lift curve. Maximum lift occurs at approximately 14 degrees with a lift coefficient of 2.33. At above 14 degrees fully reversed flow was observed on the suction side of the model and there was no evidence of periodic reattachment. 3.0 Cl 2.5 2.0 1.5 1.0 0.5 0.0-5 0 5 Alpha 10 15 20 Figure 12. Lift coefficient versus angle of attack. Data, Potential flow theory, SST, + k omega 0.8 Cl 0.6 0.4 0.2 0.0-5 0 5 Alpha 10 15 20 Figure 13. Drag coefficient versus angle of attack. Data, SST, + k omega The CFD results remain steady up to 12 degrees when the leading edge bubble starts to periodically detach from the surface. In this mode the flow oscillates between fully stalled and attached flow. Large lift coefficients are generated in the attached part of the shedding period and subsequently the average lift coefficient starts to increase. However this is a very complex bluff body flow involving considerable influence from the side walls. The flow is dramatically different to real sail flows and not suitable for validation purposes. Flow visualisation indicated that between 4 and 14 degrees the wind tunnel model had only small amounts of flow separation if any at all. At no angle of attack was periodic detachment of the leading edge bubble evident. It is believed that the wind tunnel model is more resistant to flow separation due to interaction with the tunnel wall above the model. The flow is forced to accelerate around the leading edge due to the presence of the wall above the model. This acceleration enhances the ability of the boundary layer to withstand the adverse pressure gradient at the trailing edge. In the CFD model the side walls were modelled using free-slip boundary layers. Simulations were also performed using non-slip conditions and the lift coefficients were found to increase, however not to the magnitude of the wind

tunnel results. Ideally the experiments need to be repeated in a larger tunnel where influence of the tunnel walls can be ignored. Results for the drag coefficient are given in Figure 13. At low angles of attack the drag in the wind tunnel experiments is considerably higher than the CFD results. However it is encouraging that the drag curves follow the same shape and the offset can be partially explained by interference drag associated with the end plate boundary layer, and drag due to three dimensional effects. Three dimensional CFD simulations were carried out and again significant three dimensionalities were apparent. At 2 there was cross flow and early separation of the flow near the side walls, however for approximately half the foils span the flow was nominally two-dimensional. At 8 three-dimensionalities of the type illustrated in Figures 9 and 10 existed although they were less severe than in the high camber case. For the 2 case the drag increased by 25.8% over the 2D simulations and the lift decreased by 3.5%. For the 8 case drag increased by 16% and the lift decreased by 9%. Therefore three-dimensional effects cannot explain the high lift coefficients at high angles. The increased drag at low angles can only be partially accounted for by junction drag and three-dimensional effects 6. CONCLUSIONS Comparisons between wind tunnel data and CFD results have been made for cambered plates designed to represent two-dimensional sail shapes. For the low camber section the comparison is good for low angles of attack, where the rear separation region is small. The CFD results past stall are poor, however this is not surprising considering the complexity of the flow and this is not a flow regime commonly encountered in real sail flows. For the high camber section comparison was made difficult due to the three-dimensional effects in the wake of the wind tunnel model. These three-dimensional structures dramatically alter the flow and induce downwash across the model. Consequently drag is increased and lift decreased. A CFD simulation was performed in order to help visualise the stall cell structure. The three-dimensional CFD results agreed well with the flow visualisation performed in the wind tunnel. Due to an inability to produce nominally twodimensional flow the high camber section is not a good test case for the validation of turbulence models. Moreover it is questionable whether a there is such a thing as a separated wake that is truly two-dimensional. While the SST model is perceived to be the most suitable turbulence model for flows with mild separation, little can be said about its suitability for highly separated flows. Validation of turbulence models for bluff body flows requires a three-dimensional test case. References 1. Katz, J. & Plotkin (1991), Low-Speed Aerodynamics. From Wing Theory to Panel Methods. McGraw-Hill Book Co, New York, USA. 2. Bailey, K. I. (1999), The Aerodynamic Analysis of Two-Dimensional Yacht Mast and Sail Configurations, PhD thesis, Department of Mechanical Engineering, University of Auckland. 3. Jackson, P. S. & Fiddes. S. P. (1995) Twodimensional viscous flow past flexible sail sections close to ideal incidence, Aeronautical Journal, 99 (986), 217-225. 4. Milgram, J. H. (1971), Section data for thin highly cambered airfoils in incompressible flow, NASA CR-1767, National Aeronautics and Space Administration, Washington D.C. 5. Wilkinson, S. (1984), "Partially separated flow around masts and sails", PhD Thesis, University of Southampton, Ship Science Dpt. 6. Crompton, M. J. & Barrett, R. V. (2000), Investigation of the separation bubble formed behind the sharp leading edge of a flat plate at incidence, Proceedings of the Institution of Mechanical Engineers Part G, 214, 157-176. 7. Raw M. (1996), Robustness of coupled Algebraic Multigrid for the Navier-Stokes equations, AIAA Paper 96-0297, AIAA, Aerospace Sciences Meeting and Exhibit, 34th, Reno, NV, Jan. 15-18. 8. Jones, W. P. & Launder, B. E. (1972) Prediction of Labialisation with a two-equation model of turbulence, International Journal of Heat and Mass Transfer, 15, 301-314. 9. Wilcox, D. C. (1988) Reassessment of the scaledetermining equation for advanced turbulence models AIAA Journal, 26 (11), 1299-1310. 10. Menter, F. R. (1993) Zonal two-equation k-ω turbulence models for aerodynamic flows, AIAA Paper 93-2906, AIAA. 11. Collie, S. J., Gerritsen M. & Jackson P. S. (2001), A review of turbulence modelling for use in sail flow analysis, School of Engineering Report 603, University of Auckland, NZ. 12. Menter, F. R. (1996) Comparison of some recent eddy-viscosity turbulence models Journal of Fluids Engineering, Transactions of the ASME, 118, 514-519.