CFD SIMULATIONS OF HORIZONTAL AXIS WIND TURBINE (HAWT) BLADES FOR VARIATION WITH WIND SPEED

Transcription

1 2 nd National Conference on CFD Applications in Power and Industry Sectors January 28-29, 2009, Hydrabad, India CFD SIMULATIONS OF HORIZONTAL AXIS WIND TURBINE (HAWT) BLADES FOR VARIATION WITH WIND SPEED Sagar S. Deshpande Computational Research Laboratory Ltd. Pune, India Raashid Baig Computational Research Laboratory Ltd. Pune, India Rajesh Ranjan Computational Research Laboratory Ltd. Pune, India Kishor S. Nikam Computational Research Laboratory Ltd. Pune, India Rajendra K. Lagu Computational Research Laboratory Ltd. Pune, India ABSTRACT Steady state CFD simulations have been carried out for Horizontal Axis Wind Turbine (HAWT) aerodynamics using commercial code CFD++. Pressure coefficient have been computed and compared with the wind-tunnel data of National Renewable Energy Laboratory (NREL) phase VI experiments. The wind velocity ranging from 8 m/s to 15 m/s has been considered for the present work. The pitch angle of 3 0 has been chosen for upwind type of configuration. The results have been validated with the experimental results for C P, velocity decay and Mach number at r/r of 0.3, 0.45, 0.61, 0.8 and The results are found in good agreement with the experimental data available in the literature. The wake analysis has been studied for vortex variation in the flow, which is essential for wind farm design. 1. INTRODUCTION Wind mill optimization has gathered an attention of scientific and industrial community, being a renewable energy resource. The design process of a wind turbine blade involves accurate and reliable predictions of wind turbine rotor performance for the wind mill s full range of operating conditions. This is mainly because it is a low density source of power and terrain based wind flow is a critical factor. CFD analysis is therefore essential in order to study the local flow field and pressure exerted on blades for power optimization and to reduce empiricism in the design process. Accurate prediction of wind turbine aerodynamics is still considered challenging mainly due to computational limitations and complex flow behavior both near the turbine blades and in far field [1]. The flow near the rotor root region is strongly three-dimensional and traditionally more difficult to predict computationally. Here, the effects due to centrifugal and coriolis forces in boundary delay stall by which much higher lift is achieved compared to the same obtained by two-dimensional study [2]. Similarly aerodynamics of wind turbine wake is difficult to analyze due to presence of rotor support tower and tip vortices. Nevertheless wind turbine wake region is important in case where wind turbines are placed in clusters, like wind farms. Due to difficulty in conducting aerodynamic analysis of wind farms experimentally, numerical studies offer a good alternative. Accurate aerodynamic analysis and modeling was partly limited due to high computational costs of using Navier-Stokes solver, in the entire computational domain. Several hybrid models were developed with combined near-field Navier-Stokes analysis with a far field representation by potential and vortex methods [3-5]. With the availability of modern supercomputers the computational bottleneck is removed and full Navier- Stokes analysis with sufficiently dense grid can be carried out for large number of wind mill configurations. Therefore, in the present work, CFD analysis has been carried out for the NREL Phase-VI experimental cases in order to validate the aerodynamic phenomena [6]. An investigation has been carried out for the wind speeds in the range 8m/sec-15m/sec with an emphasis on flow behavior in root section and wake region of rotor blade. 2. METHODOLOGY In the present study, wind tunnel experimental data of National Renewable Energy Laboratory (NREL) Phase VI experiments available in the literature has been considered as reference. The experiment has been carried out for the two bladed rotor made of S809 airfoil (relative thickness 21%) with a diameter (D) of m. The blade has a taper with a maximum chord of 0.735m and a tip chord of 0.061m. The twist between normalized radial distance (r/r) of 0.30 and 0.95 is 15.8 deg, while the overall twist is 22.5 deg. The analysis has been carried out for wind velocity ranging from 8m/s to 15m/s. In experimental setup, one blade of the turbine rotor is fitted with pressure transducers which are

2 connected to 5 span-wise positions equipped with the pressure orifices at r/r=0.3, 0.47, 0.63, 0.80 and The pressure data obtained has been compared with CFD results. In this case, Sequence-S of experiment is considered for CFD Validation in which an upwind, rigid turbine with 0 o cone angle is tested. The blade pitch angle is set at 3 0 and yaw angle case of 0 o has been considered [6]. The wind tunnel rotor is modeled without nacelle and tower to reduce the computational overhead and simplify the flow physics. The first quarter rotor plane experimental results were chosen for comparing CFD simulation results where there are negligible tower effects, blade vibrations and variation in pressure distribution.[7] The two meshes have been concatenated at common zonal interfaces in the solver as described in the subsection 2.2. This has been done purposely as gives ease in parametric study wherein various combinations for the rotating zone configurations can be studied while keeping the mesh of static zone same. The surface mesh has been generated in HyperMesh and volume mesh is generated in parallel mode. The volume mesh was decomposed on 8 processors into 128 domains using parallel metis algorithm to be used in the solvers Figure 1 Flow domain and wind turbine geometry 2.1 Mesh Details The computational domain has been split into two zones, namely, rotating zone which consists of wind blades and a static hemispherical zone surrounding the rotating zone. The rotating zone contains the centrally placed turbine which involves hub, blade roots and the blades. (Figure 1) The cylindrical zonal boundary of diameter 1.1D has been used, and height of the section has been set to be 0.4D. The surface mesh of 0.3 million rightangled triangular has been generated on each blade [see Figure 2], while hub as well as zonal sections have been set to be triangular. The volume mesh involves prism mesh in the boundary layer with first grid location at y + ~ 10 [see Figure 2]. The boundary layer has been generated such that the connection between prisms and tetrahedral mesh is maintained with the ratio of 1.1. The growth ratio of 1.1 has been set in the bulk region for tetrahedral mesh also [Figure 2]. The rotating zone consists of a total of 28 million mesh. The radius of spherical domain (static zone) is kept 30 times the blade diameter in order to thoroughly analyze flow in the downstream region. To capture the wake phenomena well, the surface mesh on downstream zonal interface has been extruded up to 10.0D. Grid for wake region has been generated in the form of diffuser section with maximum diameter of 3.0D as shown in Figure 3. The total volume mesh of 7.5 million has been generated in the wake section, while the remaining hemispherical section consists of approximately 4.5 million cells. Figure 2 Mesh details; R-tria mesh on blade surface Boundary layer Mesh section

3 Figure 3 Wake region meshing 2.2 Solver setup and turbulence models For modeling turbine rotor blades, moving frame of reference (MRF) approach has been used, where the rotor blades were kept fixed and the fluid zone has been solved in rotating frame of reference by adding source terms in the governing equations. The blade geometry is placed inside a hemispherical stationary zone. Upstream of this stationary domain undisturbed inlet velocity is specified. A density based solver has been used to solve the continuity and momentum equations. Preconditioning has been turned on after 20 iterations in order to capture the incompressible flow conditions. Preconditioning factor has been decided based on the 5 percent of the maximum velocity in the domain. The k-ε-rt turbulence model has been used in order to account for surface separation. The advanced two layer blended wall functions have been used in order to account for the near wall turbulence. The steady state simulations have been carried out with implicit pseudo time marching. The simulations have been carried out on 128 processors on Eka supercomputer (3.0GHz Xeon processors, each with 2GB of memory). Each simulation converged in approximately 250 implicit iterations and 3.5 hours, with residual convergence of RESULTS AND DISCUSSIONS The simulations have been carried out for the wind velocity U 0 = 8, 10 and 15 m/s in order to validate with the NREL experimental data sets available [7]. The analysis has been performed to find the effect of velocity on various parameters such as C P and wake dynamics. In the present discussion, the central region of turbine (i.e., smaller r/r) is referred as inboard section, blade side on upstream where the stagnation occurs is mentioned as the pressure side, while back side is mentioned as suction side. 3.1 Comparison of Pressure Distribution The pressure coefficients (C P ) have been evaluated at each section of the blade (r/r) based on the wind velocity (U 0 ) and rotational velocity (Ω) as: C P P P = (1) ρVRe f where, P is dynamic pressure distribution at each section of the blade r/r, V f = U + ( Ωr is the resultant Re 0 ) reference velocity, P 0 is the base pressure and ρ is the fluid density. Figures 4-4 show the comparison of C P vs. dimensionless chord length (x/c) for U 0 = 10 m/s at r/r = 0.3, 0.47, 0.63, 0.8 and The pressure side (as shown by positive C P values in Figure 4) of the blade on the all the sections show good predication as compared to the experimental values. The main deviation is observed on the suction side where the flow is accelerated. The inboard section shows the maximum deviation near the leading edge [Figure 4 and 4]. However, the overall trend has been predicted accurately on suction side (as shown by negative C P values) as well. This can be seen by same value of the integration of predicted as well as experimental values of C P across the section. Thus, the resultant forces exerted have been predicted correctly. Also, the maximum values of the C P predictions as well as the experimental values show declining trend in the sections r/r= This indicates the flow distinction at these locations as compared to the inboard section. Figures 4 - show very good agreement of pressure distribution on the blade section towards the tip section. At 10 m/s [Figure 5-5], the contours illustrate the predominately attached flow and in the blade downstream (i.e., wake region) at r/r= The peak of the C P at r/r = 0.47 is also reflected in the circular concentrated region of acceleration zone on leading surface at each section. This region is observed to be expanded towards the tip from Figures 5-5. Figures 6 and 7 show the C P distribution and the velocity contour plots for U 0 = 15 m/s at r/r = 0.3, 0.47, 0.63, 0.8 and 0.95, respectively. A reasonably good agreement has been observed at all locations except at r/r=0.3. This may be because of the insufficient grid resolution to capture flow separation near wall in this region. At r/r=0.47, the predictions reflected the trend of experimental pressure dynamics very closely. The trend of C P profile is found to be different from 8 m/s and 10 m/s cases where, inboard region shows flat distribution. This pattern indicates the occurrence of regime change over the blades. To analyze the pattern critically, the velocity magnitudes have been compared at the respective sections as shown in Figure 7-7. Figure 7 shows the wave

4 Figure 4. Cp distribution for U 0 =10 m/s; NREL experiment; CFD simulations; r/r= 0.3 r/r= 0.47 r/r= 0.63 r/r= 0.8 r/r= 0.95 Figure 5. Mach contour for U 0 =10 m/s; r/r= 0.3 r/r= 0.47 r/r= 0.63 r/r= 0.8 r/r= 0.95

5 Figure 6. Cp distribution for U 0 =15 m/s; NREL experiment; CFD simulations; r/r= 0.3 r/r= 0.47 r/r= 0.63 r/r= 0.8 r/r= 0.95 Figure 7. Mach contour for U 0 =15 m/s; r/r= 0.3 r/r= 0.47 r/r= 0.63 r/r= 0.8 r/r= 0.95

6 like patterns on the suction side indicating the flow reversal and early separation of the flow. The velocity contour of Figures 7 and 7 clearly show the full separation of the flow from the surface. The existence of the possibility of more complex flow behavior needs to be checked based on the streamlines over the blades. This has been discussed in the next subsection. A comparison of Figures 5 and 7 show the effect of variation of velocity profile at the section of r/r = 0.47, which indicates a clear distinction in the flow. The flow is found to be attached in Figure 5, while it is seen to be clearly separated in Figure 7. Similar trend is observed for other inboard locations also [Figure 5, 7]. At the tip, natures of both the profiles are observed to be similar with flow being attached to the surface in most of the section. Therefore, on the tip, the qualitative behavior of the contour plots also show similar behavior as shown in Figure 5 and 7. Thus, a comparison of CP and velocity contours show an idea regarding the stall, however, flat nature of CP plots (on the suction side) at the inboard sections [Figure 6-6] can be better understood by visualizing the 3D flow patterns on the offset plane. It is discussed in the next sub-section. 3.2 Flow Distribution Figure 8 and 8 show the streamlines for the wind velocity of U0 = 10 m/s and 15 m/s, respectively. At U0 = 8 m/s (Figure not shown), the streamlines on the suction side show the linear flow attached to the surface, with small separation and cross directional flow near the blade root. On the other hand, for U0 = 15 m/s the streamlines show early separation from the surface as compared to 10 m/s over most of the section of the blade. Also, on the inboard section, large cross streamlines are observed. Figure 9. Surface-restricted streamlines on pressure side of the blade surface for 8 m/s; 10 m/s; 15 m/s. The comparison of velocity contours [Figure 5 and 7] as well as the streamlines [Figure 8] together give more clarity of the flow. For U0 = 8 m/s (Figure not shown) flow is found to be fully attached, while a partly separated flow at the suction side and a fully attached flow at the pressure side is seen for U0 = 10 m/s. At the suction side CFD predicts turbulent separation at approximately 40% chord for the inboard segment and this position moves downstream to about 80% chord at the outboard part. The span segment at r/r = 0.95 however is not exposed to turbulent separation and the flow seems to be fully attached up till the tip. For U0 = 15 m/s, the flow is separated early at around 20 % of the chord for the inboard section [Figure 8]. Figure 9 shows the surface restricted streamlines on the pressure side. At the tip section, the flow on pressure side changes its path because of the tip curvature effect. 3.3 Wake Distribution Figure 8. Streamlines originating from blade surface for U0=10 m/s; U0=15 m/s Figure 10. Wake section details for 10 m/s; Velocity decay Vorticity profile

7 ACKNOWLEDGMENT Authors gratefully acknowledge Metacomp Technologies for valuable technical support. Authors also acknowledge Eka HPC support for the help extended while running the simulations. Figure 11. Isosurface plot of vorticity magnitude of 3 s -1 for U 0 = 10 m/s; Front view showing wake behind blade in rotational plane wake formation on the downstream side of the wind mill. Figure 10 shows the velocity decay behind the blades for 10 m/s. The section shows a stagnation point at pressure side of the turbine followed by the recovery of the energy in the wake region. The conical lower velocity component in the wind flow direction is observed from 1.0D onwards with a cone angle of approximately 300 till around 5.0D and more tangential flow is seen. The vorticity plot in the same section shows evolution of vortex patterns [Figure 10]. The vorticity trend is developed from center towards the tip in the wake region. A 3D isosurface of vorticity magnitude of 3 also shows further insight into the rotational vortex region on the tip which sustains in the wake at the diametrical periphery and decays downstream [Figure 10 and 11]. Thus, vorticity analysis gives additional information regarding the optimization of wind farms wherein the location of subsequent blades have to be fixed based on the vortex patterns for maximization of power output and hence, emerges as the scope for the future work. REFERENCES [1] Schmitz, S., and Chattot, J. J., 2007, Flow Physics and Stokes Theorem in Wind Turbine Aerodynamics, Computers & Fluids, 36, pp [2] Vermeer, L. J., Sorensen, J. N., and Crespo, A., 2003, Wind turbine wake aerodynamics, Progress in Aerospace Sciences, 39, pp [3] Schmitz, S., Chattot, J. J., 2005, A Parallelized Coupled Navier Stokes/Vortex Panel Solver, ASME J Solar Energy Eng, 127, pp [4] Xu, G., Sankar, L. N., 2000, Computational Study of Horizontal Axis Wind Turbines, ASME J Solar Energy Eng, 122, pp [5] Bhagwat, M., Moulton, M. A., and Caradonna, F. X., 2006, Hybrid CFD for Rotor Hover Performance Prediction, AIAA [6] Hand, M. M., Simms, D. A., Fingersh, L. J., Jager, D. W., Cotrell, J. R., Schreck, S., and Larwood, S. M., December 2001, Unsteady Aerodynamics Experiment Phase VI: Wind Tunnel Test Configurations and Available Data Campaigns, NREL/TP [7] Rooij, RPJOMV, Arens, E. A., 2007, Analysis of the Experimental and Computational Flow Characteristics With Respect to the Augmented Lift Phenomenon Caused by Blade Rotation, Journal of Physics: Conference Series, 75, CONCLUSIONS In the present work, the validation of wind mill turbine has been carried out for the various wind speeds namely 8 m/s, 10 m/s and 15 m/s. A total of 40 million grid-points have been generated. The domain has been decomposed in to 128 processors and the runs have been carried out on Eka supercomputer. Following conclusions have been drawn from the study. 1. The C P distribution on the inboard section of blade marginally deviates from experimental values but still able to predict the trend. In this region, the flow is largely separated and its 3 dimensional nature makes it difficult to predict. On the other hand, near the tip, the flow is largely 2 dimensional and C P shows excellent agreement with experimental results. 2. The 3D streamlines show cross-directional circulation flow for U 0 = 15 m/s near the inboard section. This causes the reduction in efficiency of the wind turbine. 3. Wake region just behind the blade shows vortex formation and dissipation and the flow regeneration is observed after approximately 5 blade diameters.