2D Numerical Simulation Study of Airfoil Performance

The aerodynamic characteristics of DTU-LN221 airfoil is studied. ANSYS Fluent is used to simulate the airfoil performance with seven different turbulence models. The simulation results for the airfoil with different turbulence models are compared with the wind tunnel experimental data performed under the same operating conditions. It is found that there is a good agreement between the computational fluid dynamics (CFD) predicted aerodynamic force coefficients with wind tunnel experimental data especially with angle of attack between -5o to 10o. RSM is chosen to investigate the flow field structure and 10 the surface pressure coefficients under different angle of attack between -5o to 10o. Also the effect of changing air temperature, velocity and turbulence intensity on lift and drag coefficients/forces are examined. The results show that it is recommended to operate the wind turbines airfoil at low air temperature and high velocity to enhance the performance of the wind turbines.


Introduction 15
The trend of using renewable energy resources has increases significantly during the past decade. The using of wind power is a promising power generation technology that can help the world to eliminate the dependency on the fuel based sources such as oil and gas. It also helps the environment to be flourished without greenhouse effects or other pollutants. The wind turbine technology offers electrical energy with lower installation and maintenance costs unlike the other energy sources. It is clean, eco-friendly and prime national security at a time when the decreasing global reserves of fossil fuels is an eminent danger in 20 the sustainability of global economy (N. Karthikeyan, 2015).
Airfoil is a basic element of a wind turbine blade, and its aerodynamic characteristics have a major influence on the wind energy conversion efficiency. Airfoil is the cross section of a wind turbine blade which is used to generate mechanical force due to the motion of air around the airfoil. The design of wind turbine airfoils is a basic but important task for designing optimal wind turbine rotors. Different types of airfoils are used along the blades in order to generate energy from the wind. 25 The pressure differences in the airfoil cause a force with two main components: Lift force: it the component of force that acts on the vertical direction of oncoming airflow. It is a result of the unequal pressure on the upper and lower airfoil surfaces. It is given by: Where CL is the lift force coefficient  is the density of air, A is the projected airfoil area (Chord x span), V is the velocity of 30 the undistributed air flow and (½AV 2 ) is the dynamic force Drag Force: it the component of force that acts in the parallel direction of oncoming airflow. It is a result of both viscous friction forces at the surface of the airfoil and the unequal pressure on the upper and lower airfoil surfaces. It is given by: Where CD is the drag force coefficient and (½AV 2 ) is the dynamic force 35 Lift and drag forces on an airfoil are influenced by the angle of attack, AOA, which is the angle between the distributed wind direction and the chord of the airfoil (Namiranian, 2011). In order to get more performance from the rotor, it is required to maximize the lift force and minimize the drag force.by optimize the angle of attack to obtain the best performance. https://doi.org/10.5194/wes-2021-45 Preprint. Discussion started: 21 May 2021 c Author(s) 2021. CC BY 4.0 License. Junwei Yang et al., (Yang et al., 2020) investigate experimentally the effect of turbulent flow on an airfoil with a Gurney flap.
The wind tunnel experiments were performed for the DTU-LN221 airfoil under different turbulence level. The results 40 demonstrate that under low turbulent inflow condition, the maximum lift coefficient of the airfoil with flaps increased by 8.47% to 13.50% (i.e., thickness of 0.75%), and the Gurney flap became less effective after stall angle. Other studies are performed to Study of a Gurney Flap implementation both experimentally and numerically using RANS based numerical simulations (Iñigo Aramendia 2019).
The different turbulence models have significant impacts on the aerodynamic performance of wind turbine blade airfoil. The 45 numerical simulation method of investigation the behavior of flow around the airfoil has a strong adaptability of time-saving, low cost, easy to reveal the details of the flow field, compared with wind tunnel experiment.
H. Wang et. al., (Hao Wang, Augest, 2014) compared the aerodynamic simulation results with the theoretical values of the lift coefficients, drag coefficients and the ratio of lift coefficient to drag coefficient for the forecast of best angle of attack, the effects of these three turbulence models on the blade airfoil aerodynamic performance were estimated. They used three 50 different turbulence models which are S-A, k-εRNG, k-ωSST on the aerodynamic performance of wind turbine airfoil under different attack angles. Their simulation results demonstrate that, for the selected blade airfoil, using S-A turbulence model before the best attack angle and k-εRNG turbulence model after the best attack angle respectively.
Two dimensional airfoil's aerodynamic performance was simulated numerically by Ji Yaoa et al. (Ji Yaoa, 2012). The control equations were Navier-Stokes equations, and four turbulence models were applied: Standard k- model of two equations, RNG found to be in good agreement. This Study clearly shows that capturing the transition behaviour, for low Reynolds numbers flows, needs an accurate turbulence model. In the present case, γ-Reθ SST is preferred model as it predicts the flow behaviour both at low and high AoA, accurately and in a short duration of time. 65 Unsteady aerodynamic characteristics is studied by G. H. Yu et.al. (G. H. Yu, 2010). They used using two-dimensional CFD with Menter's transition corrected K− SST turbulence model for various reduced frequencies. They observed that flow separation is delayed to higher angles of attack compared with the static stall case, and the lift force is found to increase far beyond that at the static stall angle. Reduced frequency is observed to have a significant impact on the aerodynamic forces and the pitching moment. The peak in the lift force coefficient appears at a higher angle of attack with increasing reduced 70 frequency.
The turbulence model has a definitely great influence on the numerical simulation results of wind turbine blade airfoil.
Traditional numerical simulation process did not consider the impacts of the changed angle of attack on the simulation results, no matter how much the angle of attack is, only one single kind of turbulence model was applied to simulate the aerodynamic performance of wind turbine blade airfoil. This simulation method for airfoil aerodynamic performance has a large error result 75 (Hao Wang, Augest, 2014).
This work aims to simulate the behavior and performance of airfoil under different working conditions. A 2D model is considered in Ansys Fluent CFD simulation of DTU-LN221 airfoil. Seven different turbulence models are used to perform the simulation. The simulation results are compared with the experimental data to choose the suitable turbulence model to continuing the investigation of the flow characteristics over the airfoil. The effect of the angle of attack of lift and drag 80 https://doi.org/10.5194/wes-2021-45 Preprint. Discussion started: 21 May 2021 c Author(s) 2021. CC BY 4.0 License. coefficients is investigated. The pressure coefficient is monitored at different angles of attack. The effect of temperature, air velocity and turbulence intensity on the airfoil performance is demonstrated.

Physical Model
The DTU-LN221 airfoil have been designed according to the requirements provided by LM and tested in the LM wind tunnel 85 (2015a; Cheng et al., 2014). The design of such type of wind turbine rotors have aerodynamically high efficiency, low cost and low noise emission (Jt Cheng, 2014).
The DTU-LN221 airfoil model (Cheng, 2013;Sessarego, 2016;Yang et al., 2020;2015a), as shown in Figure 1, was adopted which has a chord length of 0.6 m and a span length of 1.5 m. The airfoil model was vertically placed in the test section. The bottom part of the airfoil section was connected by the rotating shaft, which was fixed on a rotational plate. Therefore, the 90 angle of attack can be remotely controlled via a shaft connection with a motor below the wind tunnel. The airfoil model was made of aluminum alloy.
In the experiment, the free stream flow velocity was 37.5 m/s, and the corresponding Reynolds number based on the airfoil chord length was 1.5 x 10 6 , although wind turbines often operate at wind speed below 37.5 m/s, but the magnitude of the Reynolds number was up to an order of 10 6 . Therefore, the experimental value of the Reynolds number was chosen to approach 95 an order of magnitude corresponding to those obtained from full-scale wind turbines (Yang et al., 2020; Roha. Lswt Campaign Report on Dtu-C21; Lm Internal Report: Jupitervej).
The full description of the design of the airfoil profile is described in details in (Sessarego, 2016;Yang et al., 2020). Table 1 show the basic data for the airfoil and operating conditions of the experimental data (Sessarego, 2016;Yang et al., 2020). 100 Inviscid flow analyses neglect the effect of viscosity on the flow and are appropriate for high-Reynolds-number applications where inertial forces tend to dominate viscous forces. The inviscid is appropriate flow calculations of high-speed aerodynamic analysis as the pressure forces on the body will dominate the viscous forces. Hence, an inviscid analysis will give you a quick estimate of the primary forces acting on the body. After the body shape has been modified to maximize the lift forces and 110 minimize the drag forces, you can perform a viscous analysis to include the effects of the fluid viscosity and turbulent viscosity on the lift and drag forces.
For inviscid flows, ANSYS Fluent solves the Euler equations. The mass conservation equation is the same as for a laminar flow, but the momentum and energy conservation equations are reduced due to the absence of molecular diffusion.

-The Mass Conservation Equation: 115
The equation for conservation of mass, or continuity equation, can be written as follows: The source Sm is the mass added to the continuous phase from the dispersed second and any user-defined sources.
-Momentum Conservation Equations: Conservation of momentum is described by: 120 where p is the static pressure and g and F are the gravitational body force and external body forces respectively. F also contains other model-dependent source terms such as porous-media and user-defined sources.
-Energy Conservation Equation: Conservation of energy is described by: 125

Reynolds Average Navier Stoke(RANS)
In CFD, RANS is the most widely used turbulence modelling approach. In this approach, the Navier Stokes equations are split into mean and fluctuating components. The total velocity ui is a function of the mean velocity ūi and the fluctuating velocity úi as shown in the equation below (Hinze, 1975). 130 The continuity and momentum equation incorporating these instantaneous flow variables are given by: These above equations (in Cartesian tensor form) are known as RANS equations, and the additional Reynolds stress terms 135 −́ ́ need to be modelled. The Boussinesq hypothesis is applied in relating the Reynolds stress and mean velocity:

Spallart Allmars (S-A)
The S-A turbulence model is a one-equation model, designed for aerospace applications. It is quite robust and effective in modelling the flow on an airfoil, with adverse pressure gradients in the boundary layer (Allmaras, 1992;W., 2007). The Gv is the production of turbulent viscosity and Yv is the destruction of turbulent viscosity.
The turbulent viscosity is calculated as shown The fv1 is the viscous damping function = It has been reported that this model is effective for low Reynolds number cases, provided that the mesh resolution is super fine with a wall Y +  1 (2015b; 2015c).

Standard k-ε Model 150
Two-equation turbulence models allow the determination of both, a turbulent length and time scale by solving two separate transport equations. The standard -model in ANSYS Fluent falls within this class of models and has become the workhorse of practical engineering flow calculations in the time since it was proposed by Launder and Spalding (Spalding, 1972).
Robustness, economy, and reasonable accuracy for a wide range of turbulent flows explain its popularity in industrial flow and heat transfer simulations. It is a semi-empirical model, and the derivation of the model equations relies on 155 phenomenological considerations and empiricism.
The standard k-ε model (Spalding, 1972) is a model based on model transport equations for the turbulence kinetic energy (k) and its dissipation rate (ε). The model transport equation for k is derived from the exact equation, while the model transport equation for ε was obtained using physical reasoning and bears little resemblance to its mathematically exact counterpart.
In the derivation of the k-ε model, the assumption is that the flow is fully turbulent, and the effects of molecular viscosity are 160 negligible. The standard k-ε model is therefore valid only for fully turbulent flows.
The turbulence kinetic energy, k, and its rate of dissipation, ε, are obtained from the following transport equations: Where Gk represents the generation of turbulence kinetic energy due to the mean velocity gradients, Gb is the generation of turbulence kinetic energy due to buoyancy, YM represents the contribution of the fluctuating dilatation in compressible turbulence to the overall dissipation rate, C1 , C2 , and C3 are constants. k and  are the turbulent Prandtl numbers for k and , respectively. Sk and S are user-defined source terms.
The turbulent viscosity, t , is computed by combining k and  as follows: Where C is a constant.
The default values of the model constants are (Spalding, 1972):

The RNG -model 175
The RNG -model was derived using a statistical technique called renormalization group theory. It is similar in form to the standard k- model, but includes the following refinements: -The RNG model has an additional term in its equation that improves the accuracy for rapidly strained flows. https://doi.org/10.5194/wes-2021-45 Preprint. Discussion started: 21 May 2021 c Author(s) 2021. CC BY 4.0 License.
-The effect of swirl on turbulence is included in the RNG model, enhancing accuracy for swirling flows.
-The RNG theory provides an analytical formula for turbulent Prandtl numbers, while the standard k- model uses user-180 specified, constant values.
-While the standard k- model is a high-Reynolds number model, the RNG theory provides an analytically-derived differential formula for effective viscosity that accounts for low-Reynolds number effects. Effective use of this feature does, however, depend on an appropriate treatment of the near-wall region.
These features make the RNG k- model more accurate and reliable for a wider class of flows than the standard k- model. 185 The RNG-based k- turbulence model is derived from the instantaneous Navier-Stokes equations, using a mathematical technique called "renormalization group" (RNG) methods. The analytical derivation results in a model with constants different from those in the standard k- model, and additional terms and functions in the transport equations for k and . A more comprehensive description of RNG theory and its application to turbulence can be found in (S. A. Orszag, 1993).

Standard k-ω Model 190
The standard k-ω model in ANSYS Fluent is based on the Wilcox k-ω model (Wilcox, 1998), which incorporates modifications for low-Reynolds number effects, compressibility, and shear flow spreading. One of the weak points of the Wilcox model is the sensitivity of the solutions to values for k and ω outside the shear layer (freestream sensitivity). While the new formulation implemented in ANSYS Fluent has reduced this dependency, it can still have a significant effect on the solution, especially for free shear flows (Menter, 2009). 195 The standard k-ω model is an empirical model based on model transport equations for the turbulence kinetic energy (k) and the specific dissipation rate (ω), which can also be thought of as the ratio of ω to k (Wilcox, 1998).
As the k-ω model has been modified over the years, production terms have been added to both the k and ω equations, which have improved the accuracy of the model for predicting free shear flows.
The turbulence kinetic energy, k, and the specific dissipation rate, ω, are obtained from the following transport equations: 200 And Where Gk represents the generation of turbulence kinetic energy due to mean velocity gradients. G represents the generation of . k and  represent the effective diffusivity of k and , respectively. Yk and Y represent the dissipation of k and  due 205 to turbulence. All of the above terms are calculated as described below. Sk and S are user-defined source terms.

Shear-Stress Transport (SST) k-ω model
The shear-stress transport (SST) k-ω model was developed by Menter (Menter, 1994). It is a combination of the Wilcox K-ω and the standard K-ε model. It is so named because the definition of the turbulent viscosity is modified to account for the transport of the principal turbulent shear stress. The standard K-ε is transformed to K-ω by substituting ε = Kω (W., 2007). It 210 has feature that gives the SST k-ω model an advantage in terms of performance over both the standard k-ω model and the standard k-ε model. Other modifications include the addition of a cross-diffusion term in the ω equation and a blending function to ensure that the model equations behave appropriately in both the near-wall and far-field zones (2015b; 2015c).
The SST k-ω model has a similar form to the standard k-ω model. The turbulence kinetic energy, k, and the specific dissipation rate, ω, are obtained from the following transport equations: 215 where Gk represents the generation of turbulence kinetic energy due to mean velocity gradients. G represents the generation of ω. 220 k and  represent the effective diffusivity of k and ω, respectively. Yk and Y represent the dissipation of k and ω due to turbulence. D represents the cross-diffusion term. Sk and S are user-defined source terms. Calculations for all previous terms have been fully described in (2015b; 2015c).

The Reynolds stress model (RSM)
The Reynolds stress model (RSM) (B. E. Launder, 1975;Launder, 1989;Launder, 1978) is the most elaborate type of RANS 225 turbulence model that ANSYS Fluent provides. Abandoning the isotropic eddy-viscosity hypothesis, the RSM closes the Reynolds-averaged Navier-Stokes equations by solving transport equations for the Reynolds stresses, together with an equation for the dissipation rate. This means that five additional transport equations are required in 2D flows, in comparison to seven additional transport equations solved in 3D.
Since the RSM accounts for the effects of streamline curvature, swirl, rotation, and rapid changes in strain rate in a more 230 rigorous manner than one-equation and two-equation models, it has greater potential to give accurate predictions for complex flows. However, the fidelity of RSM predictions is still limited by the closure assumptions employed to model various terms in the exact transport equations for the Reynolds stresses. The modeling of the pressure-strain and dissipation-rate terms is particularly challenging, and often considered to be responsible for compromising the accuracy of RSM predictions.

Numerical Simulation (Model Setup)
Generating the right computational domain for a Fluid Dynamic problem is an important task of the modeling process. It is necessary to take into account different requirements (J., 2015). The domain should not be too small to correctly reproduce the flow around the airfoil and it should not be too large to not uselessly increase cells number of the grid and hence computation time (Rosario Lanzafame). It is preferable to do independency study to select the suitable domain/grid for your case of study. 245 It should to be taken into account the requirements of the meshing in terms of quality and first cell positioning near the airfoil.

Results and Discussions
The Ansys R17 package is used to simulate the air flow characteristics over DTULN221 airfoil. The 2-D Design Modeler (DM) is used to draw the airfoil profile by using the coordinates of 300 points to guarantee the smoothness and accuracy of the airfoil profile. The computational domain is composed an upstream C-shape, half of circle, in which the airfoil is included. 250 The airfoil end is located at the center of the semicircle. The diameter of the semicircle is 10 times the chord of the airfoil (Schepers J. G., 2004). The downstream domain is a square with side length equals the circle diameter as shown in Fig. 2

Model Validation (Turbulence Models Comparison)
To validate the simulation of the DTULN221 airfoil, seven turbulence models are applied to numerically simulate under the same conditions of Re number, temperature, and turbulence intensity. The air velocity is 37.5 m/s which generates a turbulence with Re of 1.8x10 6 . 2D, Double Precession, serial processing options are chosen. Density based, SIMPLE algorithm is used in processing coupling problems of speed and pressure in FLUENT solver. The second-order upwind scheme is used to discrete. 270 The Energy Equation is on and Air is considered as a real gas. The initial and boundary conditions are shown in Table 2.

Lift and Drag Coefficients
Seven viscous models are used to simulate the flow over DTULN221 airfoil. These models are Inviscid, Spalart-Allmaras, k-275 , RNG k-, k-, SST k- and RSM. The lift and drag coefficients are monitored for each simulation. The results are compared with the experimental findings in (Roha. Lswt Campaign Report on Dtu-C21; Lm Internal Report: Jupitervej; Yang et al., 2020). Their experimental measured data of the airfoil were corrected by after the reference (Allen, 1944). The experimental values of the lift and drag coefficients of the selected airfoil are compared with the simulated lift and drag coefficients of the seven turbulence models respectively. 280

Pressure Coefficient 325
The pressure coefficient Cp on the airfoil surface is defined as: is produced. It could be seen from this figure that the airfoil leading edge had a larger curvature, the flow on the airfoil surface would have a large acceleration, then the static pressure would lower on the airfoil's surface. With the increase of the angle of attack, the differences become more larger at the leading edge. 335 There was an anti-curvature shrinking section on the airfoil rear edge pressure side, which could lower the velocity and increase the pressure as shown also in Fig. 6, so the pressure coefficient of rear edge pressure side had an obvious inclination.
The figure showed that the distribution of pressure on the airfoil's surface varied largely under different attack angle. When the attack angle was less than zero, the pressure coefficient of airfoil's upper surface was positive and lower surface was negative, indicated that at this time lift force of airfoil pointed below. It could be seen from Fig. 6 that the larger attack angle, 340 the greater difference of pressure coefficient between upper and lower surface. For DTULN221 airfoil, the difference of pressure coefficient on the airfoil's front edge was much larger, while on the rear edge was much lower, indicated that the lift force of airfoil mainly come from front edge. For that type of airfoil, when the attack angle was zero, the pressure coefficient of airfoil's upper and lower surface is not equal, as the DTULN221 airfoil is not symmetry. And when the attack angle was larger than zero, the pressure coefficient of airfoil's upper surface was negative and lower surface was positive, indicated that 345

Effect of Air Speed
RSM is used to investigate the effect of changing air speed on the airfoil characteristics. Both lift and drag coefficients are 365 monitored at different air velocity. The velocities are (10, 20, 30, 37.5 and 50) m/s. Air temperature remains constant with a value of 293 K and turbulence intensity of 0.0011. Fig. 11 shows the comparison of lift coefficient under different air velocity.
The lift coefficient increases with the increase of air velocity. The percentage in the increase of the lift coefficients at an angle of attack of 10 o is more significant compared with the change of lift coefficient at lower angles of attack. There is a small change in the drag coefficients with the variation of air velocity as shown in fig. 12. 370

Conclusion
A numerical simulation study of the aerodynamic performance of DTU-LN221 airfoil is presented. The turbulence model has 390 a definitely great influence on the numerical simulation results of wind turbine blade airfoil. Seven turbulence models are used to simulate the flow over the airfoil. These models are Inviscid, Spalart-Allmaras, k-, RNG k-, k-, SST k- and RSM.
The lift and drag coefficients delivered from the simulation are compared with the wind tunnel experimental data. The range of the AOA of this simulation was between -10 o to 20 o . There was no a general model which can be called the best over the range of study. But RSM presented a good results over the other turbulence models especially in the range of AOA between -395 5 o to 10 o .
The RSM is selected to investigate the effect of changing AOA, air temperature, velocity and turbulence intensity on the characteristics of the airfoil. The following points can be concluded: -By increasing the AOA (within the range of study -between -5 o to 10 o ), The pressure in the lower side of the air foil increases while the velocity decreases. 400 -The larger attack angle, the greater difference of pressure coefficient between upper and lower surface.
-Even the change in lift and drag coefficients is very small with the variation of air temperature, there was a noticeable change in the lift and drag forces.
-The lift force decreases with the increase of air temperature.
-The lift coefficient increases with the increase of air velocity. 405 -The lift force increases rapidly with the increase of air velocity.
-The lift and drag forces does not change significantly with the change of the turbulence intensity.