CFD SIMULATIONS OF HORIZONTAL AXIS WIND TURBINE (HAWT) BLADES FOR VARIATION WITH WIND SPEED
|
|
- Harry Booth
- 6 years ago
- Views:
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.
Application of STAR-CCM+ to Helicopter Rotors in Hover
Application of STAR-CCM+ to Helicopter Rotors in Hover Lakshmi N. Sankar and Chong Zhou School of Aerospace Engineering, Georgia Institute of Technology, Atlanta, GA Ritu Marpu Eschol CD-Adapco, Inc.,
More informationIntroduction to ANSYS CFX
Workshop 03 Fluid flow around the NACA0012 Airfoil 16.0 Release Introduction to ANSYS CFX 2015 ANSYS, Inc. March 13, 2015 1 Release 16.0 Workshop Description: The flow simulated is an external aerodynamics
More informationIntegration of an unsteady nonlinear lifting line free wake algorithm in a wind turbine design framework
Integration of an unsteady nonlinear lifting line free wake algorithm in a wind turbine design framework Introduction D. Marten, G. Pechlivanoglou, C. N. Nayeri, C. O. Paschereit TU Berlin, Institute of
More informationNumerische Untersuchungen von Windkraftanlagen: Leistung, Wake und Steuerungsstrategien
Fachtagung Lasermethoden in der Strömungsmesstechnik 8. 10. September 2015, Dresden Numerische Untersuchungen von Windkraftanlagen: Leistung, Wake und Steuerungsstrategien Numerical Investigations of Wind
More informationNUMERICAL 3D TRANSONIC FLOW SIMULATION OVER A WING
Review of the Air Force Academy No.3 (35)/2017 NUMERICAL 3D TRANSONIC FLOW SIMULATION OVER A WING Cvetelina VELKOVA Department of Technical Mechanics, Naval Academy Nikola Vaptsarov,Varna, Bulgaria (cvetelina.velkova1985@gmail.com)
More informationCFD Study of a Darreous Vertical Axis Wind Turbine
CFD Study of a Darreous Vertical Axis Wind Turbine Md Nahid Pervez a and Wael Mokhtar b a Graduate Assistant b PhD. Assistant Professor Grand Valley State University, Grand Rapids, MI 49504 E-mail:, mokhtarw@gvsu.edu
More informationAxisymmetric Viscous Flow Modeling for Meridional Flow Calculation in Aerodynamic Design of Half-Ducted Blade Rows
Memoirs of the Faculty of Engineering, Kyushu University, Vol.67, No.4, December 2007 Axisymmetric Viscous Flow Modeling for Meridional Flow alculation in Aerodynamic Design of Half-Ducted Blade Rows by
More informationNASA Rotor 67 Validation Studies
NASA Rotor 67 Validation Studies ADS CFD is used to predict and analyze the performance of the first stage rotor (NASA Rotor 67) of a two stage transonic fan designed and tested at the NASA Glenn center
More informationThe Spalart Allmaras turbulence model
The Spalart Allmaras turbulence model The main equation The Spallart Allmaras turbulence model is a one equation model designed especially for aerospace applications; it solves a modelled transport equation
More informationEnhancement of wind turbine aerodynamic performance by a numerical optimization technique
Journal of Mechanical Science and Technology 26 (2) (202) 455~462 www.springerlink.com/content/738-494x DOI 0.007/s2206-0-035-2 Enhancement of wind turbine aerodynamic performance by a numerical optimization
More informationCFD Modeling of a Radiator Axial Fan for Air Flow Distribution
CFD Modeling of a Radiator Axial Fan for Air Flow Distribution S. Jain, and Y. Deshpande Abstract The fluid mechanics principle is used extensively in designing axial flow fans and their associated equipment.
More informationCFD Analysis of 2-D Unsteady Flow Past a Square Cylinder at an Angle of Incidence
CFD Analysis of 2-D Unsteady Flow Past a Square Cylinder at an Angle of Incidence Kavya H.P, Banjara Kotresha 2, Kishan Naik 3 Dept. of Studies in Mechanical Engineering, University BDT College of Engineering,
More informationDevelopment and application of a dynamic stall model for rotating wind turbine blades
Journal of Physics: Conference Series OPEN ACCESS Development and application of a dynamic stall model for rotating wind turbine blades To cite this article: B F Xu et al 4 J. Phys.: Conf. Ser. 54 33 View
More informationCFD wake modeling using a porous disc
CFD wake modeling using a porous disc Giorgio Crasto, Arne Reidar Gravdahl giorgio@windsim.com, arne@windsim.com WindSim AS Fjordgaten 5 N-325 Tønsberg Norway Tel. +47 33 38 8 Fax +47 33 38 8 8 http://www.windsim.com
More informationHigh-Lift Aerodynamics: STAR-CCM+ Applied to AIAA HiLiftWS1 D. Snyder
High-Lift Aerodynamics: STAR-CCM+ Applied to AIAA HiLiftWS1 D. Snyder Aerospace Application Areas Aerodynamics Subsonic through Hypersonic Aeroacoustics Store release & weapons bay analysis High lift devices
More informationPotsdam Propeller Test Case (PPTC)
Second International Symposium on Marine Propulsors smp 11, Hamburg, Germany, June 2011 Workshop: Propeller performance Potsdam Propeller Test Case (PPTC) Olof Klerebrant Klasson 1, Tobias Huuva 2 1 Core
More information3D Aerodynamic Optimization of NREL VI Wind Turbine Blade for Increased Power Output and Visualization of Flow Characteristics
Dissertations and Theses Spring 2014 3D Aerodynamic Optimization of NREL VI Wind Turbine Blade for Increased Power Output and Visualization of Flow Characteristics Tsewang Rabga Shrestha Embry-Riddle Aeronautical
More informationAshwin Shridhar et al. Int. Journal of Engineering Research and Applications ISSN : , Vol. 5, Issue 6, ( Part - 5) June 2015, pp.
RESEARCH ARTICLE OPEN ACCESS Conjugate Heat transfer Analysis of helical fins with airfoil crosssection and its comparison with existing circular fin design for air cooled engines employing constant rectangular
More informationEstimating Vertical Drag on Helicopter Fuselage during Hovering
Estimating Vertical Drag on Helicopter Fuselage during Hovering A. A. Wahab * and M.Hafiz Ismail ** Aeronautical & Automotive Dept., Faculty of Mechanical Engineering, Universiti Teknologi Malaysia, 81310
More informationCFD MODELING FOR PNEUMATIC CONVEYING
CFD MODELING FOR PNEUMATIC CONVEYING Arvind Kumar 1, D.R. Kaushal 2, Navneet Kumar 3 1 Associate Professor YMCAUST, Faridabad 2 Associate Professor, IIT, Delhi 3 Research Scholar IIT, Delhi e-mail: arvindeem@yahoo.co.in
More informationMULTI-SCIENCE PUBLISHING COMPANY. Teymour Javaherchi, Sylvain Antheaume and Alberto Aliseda
Hierarchical Methodology for the Numerical Simulation of the Flow Field around and in the Wake of Horizontal Axis Wind Turbines: Rotating Reference Frame, Blade Element Method and Actuator Disk Model by
More informationMcNair Scholars Research Journal
McNair Scholars Research Journal Volume 2 Article 1 2015 Benchmarking of Computational Models against Experimental Data for Velocity Profile Effects on CFD Analysis of Adiabatic Film-Cooling Effectiveness
More informationCOMPUTATIONAL FLUID DYNAMICS ANALYSIS OF ORIFICE PLATE METERING SITUATIONS UNDER ABNORMAL CONFIGURATIONS
COMPUTATIONAL FLUID DYNAMICS ANALYSIS OF ORIFICE PLATE METERING SITUATIONS UNDER ABNORMAL CONFIGURATIONS Dr W. Malalasekera Version 3.0 August 2013 1 COMPUTATIONAL FLUID DYNAMICS ANALYSIS OF ORIFICE PLATE
More informationUnsteady Hybrid Navier-Stokes/Vortex Model Applied to Wind Turbine Aerodynamics under Yaw Conditions
Seventh International Conference on Computational Fluid Dynamics (ICCFD7), Big Island, Hawaii, July 9-13, 2012 ICCFD7-3501 Unsteady Hybrid Navier-Stokes/Vortex Model Applied to Wind Turbine Aerodynamics
More informationAccurate and Efficient Turbomachinery Simulation. Chad Custer, PhD Turbomachinery Technical Specialist
Accurate and Efficient Turbomachinery Simulation Chad Custer, PhD Turbomachinery Technical Specialist Outline Turbomachinery simulation advantages Axial fan optimization Description of design objectives
More informationDebojyoti Ghosh. Adviser: Dr. James Baeder Alfred Gessow Rotorcraft Center Department of Aerospace Engineering
Debojyoti Ghosh Adviser: Dr. James Baeder Alfred Gessow Rotorcraft Center Department of Aerospace Engineering To study the Dynamic Stalling of rotor blade cross-sections Unsteady Aerodynamics: Time varying
More informationNUMERICAL SIMULATIONS OF FLOW THROUGH AN S-DUCT
NUMERICAL SIMULATIONS OF FLOW THROUGH AN S-DUCT 1 Pravin Peddiraju, 1 Arthur Papadopoulos, 2 Vangelis Skaperdas, 3 Linda Hedges 1 BETA CAE Systems USA, Inc., USA, 2 BETA CAE Systems SA, Greece, 3 CFD Consultant,
More informationEstimation of Flow Field & Drag for Aerofoil Wing
Estimation of Flow Field & Drag for Aerofoil Wing Mahantesh. HM 1, Prof. Anand. SN 2 P.G. Student, Dept. of Mechanical Engineering, East Point College of Engineering, Bangalore, Karnataka, India 1 Associate
More informationDYNAMICS OF A VORTEX RING AROUND A MAIN ROTOR HELICOPTER
DYNAMICS OF A VORTEX RING AROUND A MAIN ROTOR HELICOPTER Katarzyna Surmacz Instytut Lotnictwa Keywords: VORTEX RING STATE, HELICOPTER DESCENT, NUMERICAL ANALYSIS, FLOW VISUALIZATION Abstract The main goal
More informationKeywords: CFD, aerofoil, URANS modeling, flapping, reciprocating movement
L.I. Garipova *, A.N. Kusyumov *, G. Barakos ** * Kazan National Research Technical University n.a. A.N.Tupolev, ** School of Engineering - The University of Liverpool Keywords: CFD, aerofoil, URANS modeling,
More informationSimulation of Turbulent Flow around an Airfoil
1. Purpose Simulation of Turbulent Flow around an Airfoil ENGR:2510 Mechanics of Fluids and Transfer Processes CFD Lab 2 (ANSYS 17.1; Last Updated: Nov. 7, 2016) By Timur Dogan, Michael Conger, Andrew
More informationUsing Multiple Rotating Reference Frames
Tutorial 9. Using Multiple Rotating Reference Frames Introduction Many engineering problems involve rotating flow domains. One example is the centrifugal blower unit that is typically used in automotive
More informationInvestigation of cross flow over a circular cylinder at low Re using the Immersed Boundary Method (IBM)
Computational Methods and Experimental Measurements XVII 235 Investigation of cross flow over a circular cylinder at low Re using the Immersed Boundary Method (IBM) K. Rehman Department of Mechanical Engineering,
More informationNumerical and theoretical analysis of shock waves interaction and reflection
Fluid Structure Interaction and Moving Boundary Problems IV 299 Numerical and theoretical analysis of shock waves interaction and reflection K. Alhussan Space Research Institute, King Abdulaziz City for
More informationExperimental and numerical investigations of aerodynamic loads and 3D flow over non-rotating MEXICO blades
WIND ENERGY Wind Energ. 2017; 20:585 600 Published online 5 September 2016 in Wiley Online Library (wileyonlinelibrary.com)..2025 RESEARCH ARTICLE Experimental and numerical investigations of aerodynamic
More informationIntroduction to CFX. Workshop 2. Transonic Flow Over a NACA 0012 Airfoil. WS2-1. ANSYS, Inc. Proprietary 2009 ANSYS, Inc. All rights reserved.
Workshop 2 Transonic Flow Over a NACA 0012 Airfoil. Introduction to CFX WS2-1 Goals The purpose of this tutorial is to introduce the user to modelling flow in high speed external aerodynamic applications.
More informationProfile Catalogue for Airfoil Sections Based on 3D Computations
Risø-R-58(EN) Profile Catalogue for Airfoil Sections Based on 3D Computations Franck Bertagnolio, Niels N. Sørensen and Jeppe Johansen Risø National Laboratory Roskilde Denmark December 26 Author: Franck
More informationModeling External Compressible Flow
Tutorial 3. Modeling External Compressible Flow Introduction The purpose of this tutorial is to compute the turbulent flow past a transonic airfoil at a nonzero angle of attack. You will use the Spalart-Allmaras
More informationMOMENTUM AND HEAT TRANSPORT INSIDE AND AROUND
MOMENTUM AND HEAT TRANSPORT INSIDE AND AROUND A CYLINDRICAL CAVITY IN CROSS FLOW G. LYDON 1 & H. STAPOUNTZIS 2 1 Informatics Research Unit for Sustainable Engrg., Dept. of Civil Engrg., Univ. College Cork,
More informationDevelopment of a CFD Capability for Full Helicopter Engineering Analysis
Development of a CFD Capability for Full Helicopter Engineering Analysis George Barakos Department of Engineering University of Liverpool 5/6 April 2006 Loughborough University Collective effort of more
More informationPerformance improvement of a wind turbine blade using a developed inverse design method
energyequipsys/ Vol 4/No1/June 2016/ 1-10 Energy Equipment and Systems http://energyequipsys.ut.ac.ir www.energyeuquipsys.com Performance improvement of a wind turbine blade using a developed inverse design
More informationDeposited on: 7 July 2009
Fletcher, T.M. and Brown, R.E. and Kim, R.E. and Kwon, O.J. (2009 Predicting wind turbine blade loads using vorticity transport and RANS methodologies. In: European Wind Energy Conference 2009, March 2009,
More informationMASSACHUSETTS INSTITUTE OF TECHNOLOGY. Analyzing wind flow around the square plate using ADINA Project. Ankur Bajoria
MASSACHUSETTS INSTITUTE OF TECHNOLOGY Analyzing wind flow around the square plate using ADINA 2.094 - Project Ankur Bajoria May 1, 2008 Acknowledgement I would like to thank ADINA R & D, Inc for the full
More informationCFD Simulations of Flow over Airfoils:
CFD Simulations of Flow over Airfoils: An Analysis of Wind Turbine Blade Aerodynamics By: John Hamilla, Mechanical Engineering Advisor: Maria-Isabel Carnasciali, Ph.D. Abstract Wind turbines are rapidly
More informationUsing Multiple Rotating Reference Frames
Tutorial 10. Using Multiple Rotating Reference Frames Introduction Many engineering problems involve rotating flow domains. One example is the centrifugal blower unit that is typically used in automotive
More informationCOMPUTATIONAL MODELING OF WIND ENERGY SYSTEMS
The Eighth Asia-Pacific Conference on Wind Engineering, December 10 14, 2013, Chennai, India COMPUTATIONAL MODELING OF WIND ENERGY SYSTEMS T. Shah 1, R. Prasad 2 and M. Damodaran 3 1 Project Associate,
More informationDetached Eddy Simulation Analysis of a Transonic Rocket Booster for Steady & Unsteady Buffet Loads
Detached Eddy Simulation Analysis of a Transonic Rocket Booster for Steady & Unsteady Buffet Loads Matt Knapp Chief Aerodynamicist TLG Aerospace, LLC Presentation Overview Introduction to TLG Aerospace
More informationAN EXPERIMENTAL STUDY AND SIMULATION WITH FLUENT
AN EXPERIMENTAL STUDY AND SIMULATION WITH FLUENT OF THE HORIZONTAL AXIS WIND TURBINE (HAWT) BLADE TOWER DYNAMIC INTERACTION V. P. CAMBANIS 1 & H. STAPOUNTZIS 2 Lab. of Fluid Mechanics & Turbomachinery,
More informationExpress Introductory Training in ANSYS Fluent Workshop 04 Fluid Flow Around the NACA0012 Airfoil
Express Introductory Training in ANSYS Fluent Workshop 04 Fluid Flow Around the NACA0012 Airfoil Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 -
More informationON THE NUMERICAL MODELING OF IMPINGING JET HEAT TRANSFER
ON THE NUMERICAL MODELING OF IMPINGING JET HEAT TRANSFER Mirko Bovo 1,2, Sassan Etemad 2 and Lars Davidson 1 1 Dept. of Applied Mechanics, Chalmers University of Technology, Gothenburg, Sweden 2 Powertrain
More informationPossibility of Implicit LES for Two-Dimensional Incompressible Lid-Driven Cavity Flow Based on COMSOL Multiphysics
Possibility of Implicit LES for Two-Dimensional Incompressible Lid-Driven Cavity Flow Based on COMSOL Multiphysics Masanori Hashiguchi 1 1 Keisoku Engineering System Co., Ltd. 1-9-5 Uchikanda, Chiyoda-ku,
More informationProgress and Future Prospect of CFD in Aerospace
Progress and Future Prospect of CFD in Aerospace - Observation from 30 years research - Kozo Fujii Institute of Space and Astronautical Science (ISAS) Japan Aerospace Exploration Agency (JAXA) Japan JAXA:
More informationA STUDY ON THE UNSTEADY AERODYNAMICS OF PROJECTILES IN OVERTAKING BLAST FLOWFIELDS
HEFAT2012 9 th International Conference on Heat Transfer, Fluid Mechanics and Thermodynamics 16 18 July 2012 Malta A STUDY ON THE UNSTEADY AERODYNAMICS OF PROJECTILES IN OVERTAKING BLAST FLOWFIELDS Muthukumaran.C.K.
More informationNumerical Analysis of Effect of Pitch Angle on a Small Scale Vertical Axis Wind Turbine
Numerical Analysis of Effect of Pitch Angle on a Small Scale Vertical Axis Wind Turbine Bose Sumantraa R., Chandramouli S., Premsai T. P., Prithviraj P., Vivek M., V. Ratna Kishore Department of Mechanical
More informationNUMERICAL SIMULATION OF FLOW FIELD IN AN ANNULAR TURBINE STATOR WITH FILM COOLING
24 TH INTERNATIONAL CONGRESS OF THE AERONAUTICAL SCIENCES NUMERICAL SIMULATION OF FLOW FIELD IN AN ANNULAR TURBINE STATOR WITH FILM COOLING Jun Zeng *, Bin Wang *, Yong Kang ** * China Gas Turbine Establishment,
More informationTHE EFFECTS OF THE PLANFORM SHAPE ON DRAG POLAR CURVES OF WINGS: FLUID-STRUCTURE INTERACTION ANALYSES RESULTS
March 18-20, 2013 THE EFFECTS OF THE PLANFORM SHAPE ON DRAG POLAR CURVES OF WINGS: FLUID-STRUCTURE INTERACTION ANALYSES RESULTS Authors: M.R. Chiarelli, M. Ciabattari, M. Cagnoni, G. Lombardi Speaker:
More informationNon-Newtonian Transitional Flow in an Eccentric Annulus
Tutorial 8. Non-Newtonian Transitional Flow in an Eccentric Annulus Introduction The purpose of this tutorial is to illustrate the setup and solution of a 3D, turbulent flow of a non-newtonian fluid. Turbulent
More informationParallelized Coupled Solver (PCS) Model Refinements & Extensions
Parallelized Coupled Solver (PCS) Model Refinements & Extensions Sven Schmitz GE Wind November 29 th, 2007 Greenville, SC University of California, Davis Schmitz GE Wind - PCS 1 Outline 2007 Parallelized
More informationSIMULATION OF PROPELLER-SHIP HULL INTERACTION USING AN INTEGRATED VLM/RANSE SOLVER MODELING.
SIMULATION OF PROPELLER-SHIP HULL INTERACTION USING AN INTEGRATED VLM/RANSE SOLVER MODELING. M.N.Senthil Prakash, Department of Ocean Engineering, IIT Madras, India V. Anantha Subramanian Department of
More informationRotorcraft Noise Prediction with Multi-disciplinary Coupling Methods. Yi Liu NIA CFD Seminar, April 10, 2012
Rotorcraft Noise Prediction with Multi-disciplinary Coupling Methods Yi Liu NIA CFD Seminar, April 10, 2012 Outline Introduction and Background Multi-disciplinary Analysis Approaches Computational Fluid
More informationDynamic stall for a Vertical Axis Wind Turbine in a two-dimensional study
Dynamic stall for a Vertical Axis Wind Turbine in a two-dimensional study R. Nobile 1,*, M. Vahdati 1, J. Barlow 1, A. Mewburn-Crook 2 1 University of Reading, Reading, UK 2 Wind Dam Renewables Ltd, Swansea,
More informationNumerical analysis of the tip and root vortex position in the wake of a wind turbine
Journal of Physics: Conference Series Numerical analysis of the tip and root vortex position in the wake of a wind turbine To cite this article: S Ivanell et al 2007 J. Phys.: Conf. Ser. 75 012035 View
More informationSmall Height Duct Design for 17 Multicopter Fan Considering Its Interference on Quad-copter
Small Height Duct Design for 17 Multicopter Fan Considering Its Interference on Quad-copter Stremousov K.*, Arkhipov M.* **, Serokhvostov S.* ** * Moscow Institute of Physics and Technology, Department
More informationUnstructured CFD for Wind Turbine Analysis
Unstructured CFD for Wind Turbine Analysis C. Eric Lynch and Marilyn Smith Daniel Guggenheim School of Aerospace Engineering Georgia Institute of Technology Atlanta, USA Wind availability: Egypt Extremely
More informationFLUID DYNAMICS ANALYSIS OF A COUNTER ROTATING DUCTED PROPELLER
FLUID DYNAMICS ANALYSIS OF A COUNTER ROTATING DUCTED PROPELLER Chao Xu, Cees Bil, Sherman CP. Cheung School of Aerospace, Mechanical and Manufacturing Engineering, RMIT University Keywords: Twin counter-rotating
More informationAnalysis of an airfoil
UNDERGRADUATE RESEARCH FALL 2010 Analysis of an airfoil using Computational Fluid Dynamics Tanveer Chandok 12/17/2010 Independent research thesis at the Georgia Institute of Technology under the supervision
More informationSimulations of Flow Over Wind Turbines
University of Massachusetts Amherst ScholarWorks@UMass Amherst Masters Theses 1911 - February 2014 Dissertations and Theses 2010 Simulations of Flow Over Wind Turbines Dnyanesh A. Digraskar University
More informationNumerical Simulation Study on Aerodynamic Characteristics of the High Speed Train under Crosswind
2017 2nd International Conference on Industrial Aerodynamics (ICIA 2017) ISBN: 978-1-60595-481-3 Numerical Simulation Study on Aerodynamic Characteristics of the High Speed Train under Crosswind Fan Zhao,
More informationACTIVE SEPARATION CONTROL WITH LONGITUDINAL VORTICES GENERATED BY THREE TYPES OF JET ORIFICE SHAPE
24 TH INTERNATIONAL CONGRESS OF THE AERONAUTICAL SCIENCES ACTIVE SEPARATION CONTROL WITH LONGITUDINAL VORTICES GENERATED BY THREE TYPES OF JET ORIFICE SHAPE Hiroaki Hasegawa*, Makoto Fukagawa**, Kazuo
More informationDesign and Computational Fluid Dynamics Analysis of an Idealized Modern Wingsuit
Design and Computational Fluid Dynamics Analysis of an Idealized Modern Wingsuit Maria E. Ferguson Washington University in St. Louis Advisor: Dr. Ramesh K. Agarwal Abstract The modern wingsuit has been
More informationTurbocharger Design & Analysis Solutions. Bill Holmes Brad Hutchinson Detroit, October 2012
Turbocharger Design & Analysis Solutions Bill Holmes Brad Hutchinson Detroit, October 2012 Agenda ANSYS overview ANSYS TurboSystem Blade row solutions The ANSYS Transformation methods An example: turbocharger
More informationNUMERICAL AND EXPERIMENTAL ANALYSIS OF A REPRESENTATIVE ADF HELICOPTER FUSELAGE
28 TH INTERNATIONAL CONGRESS OF THE AERONAUTICAL SCIENCES NUMERICAL AND EXPERIMENTAL ANALYSIS OF A REPRESENTATIVE ADF HELICOPTER FUSELAGE Dylan Brunello*, Gareth Clarke, Rami Reddy* *Defence Science Technology
More informationAerodynamic Design Optimization of UAV Rotor Blades using a Genetic Algorithm
Aerodynamic Design Optimization of UAV Rotor Blades using a Genetic Algorithm Hak-Min Lee 1), Nahm-Keon Hur 2) and *Oh-Joon Kwon 3) 1), 3) Department of Aerospace Engineering, KAIST, Daejeon 305-600, Korea
More informationComputational Analysis of a Wing Oscillator
Western Michigan University ScholarWorks at WMU Master's Theses Graduate College 8-2012 Computational Analysis of a Wing Oscillator Ryne Derrick Radermacher Western Michigan University, rhyno466@gmail.com
More informationComputational Fluid Dynamics Analysis of an Idealized Modern Wingsuit
Washington University in St. Louis Washington University Open Scholarship Mechanical Engineering and Materials Science Independent Study Mechanical Engineering & Materials Science 12-21-2016 Computational
More informationStrömningslära Fluid Dynamics. Computer laboratories using COMSOL v4.4
UMEÅ UNIVERSITY Department of Physics Claude Dion Olexii Iukhymenko May 15, 2015 Strömningslära Fluid Dynamics (5FY144) Computer laboratories using COMSOL v4.4!! Report requirements Computer labs must
More informationTransition Flow and Aeroacoustic Analysis of NACA0018 Satish Kumar B, Fred Mendonç a, Ghuiyeon Kim, Hogeon Kim
Transition Flow and Aeroacoustic Analysis of NACA0018 Satish Kumar B, Fred Mendonç a, Ghuiyeon Kim, Hogeon Kim Transition Flow and Aeroacoustic Analysis of NACA0018 Satish Kumar B, Fred Mendonç a, Ghuiyeon
More informationICMIEE D CFD Analysis of a Straight-bladed Vertical Axis Wind Turbine Using General Grid Interface Method
International Conference on Mechanical, Industrial and Energy Engineering 2018 23-24 December, 2018, Khulna, BANGLADESH ICMIEE18-319 2D CFD Analysis of a Straight-bladed Vertical Axis Wind Turbine Using
More informationComputational Fluid Dynamics Simulation of a Rim Driven Thruster
Computational Fluid Dynamics Simulation of a Rim Driven Thruster Aleksander J Dubas, N. W. Bressloff, H. Fangohr, S. M. Sharkh (University of Southampton) Abstract An electric rim driven thruster is a
More informationUsing a Single Rotating Reference Frame
Tutorial 9. Using a Single Rotating Reference Frame Introduction This tutorial considers the flow within a 2D, axisymmetric, co-rotating disk cavity system. Understanding the behavior of such flows is
More informationComputational Fluid Dynamics Approach for Wind Turbine Blade Aerodynamics Design
CHAPTER 5 Computational Fluid Dynamics Approach for Wind Turbine Blade Aerodynamics Design R.J. Malloy 1 & R.S. Amano 2 1 Milwaukee Electric Tool Corp. 2 Department of Mechanical Engineering, University
More informationCFD Application in Offshore Structures Design at PETROBRAS
CFD Application in Offshore Structures Design at PETROBRAS Marcus Reis ESSS CFD Director Mooring System Design of Floating Production Systems; Current and Wind Loads; Wave Induced Drag Coefficients. Case
More informationApplication of Parallel Compution on Numerical Simulation for the Fluid Flow Field of Fan
2010 3rd International Conference on Computer and Electrical Engineering (ICCEE 2010) IPCSIT vol. 53 (2012) (2012) IACSIT Press, Singapore DOI: 10.7763/IPCSIT.2012.V53.No.2.73 Application of Parallel Compution
More informationVerification and Validation of Turbulent Flow around a Clark-Y Airfoil
Verification and Validation of Turbulent Flow around a Clark-Y Airfoil 1. Purpose 58:160 Intermediate Mechanics of Fluids CFD LAB 2 By Tao Xing and Fred Stern IIHR-Hydroscience & Engineering The University
More informationEffects of bell mouth geometries on the flow rate of centrifugal blowers
Journal of Mechanical Science and Technology 25 (9) (2011) 2267~2276 www.springerlink.com/content/1738-494x DOI 10.1007/s12206-011-0609-3 Effects of bell mouth geometries on the flow rate of centrifugal
More informationSummary of the main PROBAND project results
Summary of the main PROBAND project results WP2: WP2 was dedicated to the development and validation broadband noise prediction methods. Once validated on non rotating airfoils in WP2, these methods were
More informationApplication of Wray-Agarwal Turbulence Model for Accurate Numerical Simulation of Flow Past a Three-Dimensional Wing-body
Washington University in St. Louis Washington University Open Scholarship Mechanical Engineering and Materials Science Independent Study Mechanical Engineering & Materials Science 4-28-2016 Application
More informationDetermination of Angle of Attack (AOA) for Rotating Blades
Downloaded from orbit.dtu.dk on: Sep 1, 218 Determination of Angle of Attack (AOA) for Rotating Blades Shen, Wen Zhong; Hansen, Martin Otto Laver; Sørensen, Jens Nørkær Published in: Wind Energy Publication
More informationEffect of Position of Wall Mounted Surface Protrusion in Drag Characteristics At Low Reynolds Number
ISSN (e): 2250 3005 Volume, 07 Issue, 11 November 2017 International Journal of Computational Engineering Research (IJCER) Effect of Position of Wall Mounted Surface Protrusion in Drag Characteristics
More informationFAR-Wake Workshop, Marseille, May 2008
Wake Vortices generated by an Aircraft Fuselage : Comparison of Wind Tunnel Measurements on the TAK Model with RANS and RANS-LES Simulations T. Louagie, L. Georges & P. Geuzaine Cenaero CFD-Multiphysics
More informationNumerical calculation of the wind action on buildings using Eurocode 1 atmospheric boundary layer velocity profiles
Numerical calculation of the wind action on buildings using Eurocode 1 atmospheric boundary layer velocity profiles M. F. P. Lopes IDMEC, Instituto Superior Técnico, Av. Rovisco Pais 149-1, Lisboa, Portugal
More informationNear Wake RANS Predictions of the wake Behind the MEXICO Rotor in Axial and Yawed Flow Conditions
Near Wake RANS Predictions of the wake Behind the MEXICO Rotor in Axial and Yawed Flow Conditions Niels N. Sørensen, A. Bechmann, P-E. Réthoré, F. Zahle DTU Wind Energy, Technical Uni. Denmark DK- Roskilde,
More informationAnalysis of Flow through a Drip Irrigation Emitter
International OPEN ACCESS Journal Of Modern Engineering Research (IJMER) Analysis of Flow through a Drip Irrigation Emitter Reethi K 1, Mallikarjuna 2, Vijaya Raghu B 3 1 (B.E Scholar, Mechanical Engineering,
More informationLARGE EDDY SIMULATION OF VORTEX SHEDDING WITH TRIANGULAR CYLINDER AHEAD OF A SQUARE CYLINDER
The Eighth Asia-Pacific Conference on Wind Engineering, December 10 14, 2013, Chennai, India LARGE EDDY SIMULATION OF VORTEX SHEDDING WITH TRIANGULAR CYLINDER AHEAD OF A SQUARE CYLINDER Akshoy Ranjan Paul
More informationCoupling of STAR-CCM+ to Other Theoretical or Numerical Solutions. Milovan Perić
Coupling of STAR-CCM+ to Other Theoretical or Numerical Solutions Milovan Perić Contents The need to couple STAR-CCM+ with other theoretical or numerical solutions Coupling approaches: surface and volume
More informationReproducibility of Complex Turbulent Flow Using Commercially-Available CFD Software
Reports of Research Institute for Applied Mechanics, Kyushu University No.150 (71 83) March 2016 Reproducibility of Complex Turbulent Flow Using Commercially-Available CFD Software Report 3: For the Case
More informationTHE INFLUENCE OF MESH CHARACTERISTICS ON OPENFOAM SIMULATIONS OF THE DRIVAER MODEL
6 th BETA CAE International Conference THE INFLUENCE OF MESH CHARACTERISTICS ON OPENFOAM SIMULATIONS OF THE DRIVAER MODEL Grigoris Fotiadis *, Vangelis Skaperdas, Aristotelis Iordanidis BETA CAE Systems
More informationOPEN-WATER COMPUTATIONS OF A MARINE PROPELLER USING OPENFOAM
Open water computations of a marine propeller using OpenFOAM 11th World Congress on Computational Mechanics (WCCM XI) 5th European Conference on Computational Mechanics (ECCM V) 6th European Conference
More informationWind tunnel experiments on a rotor model in yaw
Nord-Jan ermeer Faculty of Civil Engineering and Geosciences Stevinweg 8 CN Delft The Netherlands Tel: + 78 Fax: + 78 7 E-mail: n.vermeer@ct.tudelft.nl http://www.ct.tudelft.nl/windenergy/ivwhome.htm The
More informationFinite Element Flow Simulations of the EUROLIFT DLR-F11 High Lift Configuration
Finite Element Flow Simulations of the EUROLIFT DLR-F11 High Lift Configuration Kedar C. Chitale MANE Dept., Rensselaer Polytechnic Institute, NY 12180 Michel Rasquin Leadership Computing Facility, Argonne
More information