COMPUTATIONAL MODELING OF WIND ENERGY SYSTEMS
|
|
- Virginia Andrews
- 5 years ago
- Views:
Transcription
1 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, Mechanical Engineering, IIT Gandhinagar, GJ, India, - tapanshah@iitgn.ac.in 2 Graduate Student, Mechanical Engineering, IIT Gandhinagar, GJ, India, - rachit.prasad@iitgn.ac.in 3 Professor, Mechanical Engineering, IIT Gandhinagar, GJ, India, - murali@iitgn.ac.in ABSTRACT Computational modeling of flow fields in the vicinity of the blades of the low cost horizontal axis wind turbine (HAWT) and vertical axis wind turbine (VAWT) windmills are outlined in this paper. Computed pressure fields, wakes, vorticity structures for an assumed free stream velocity and as well as for a assumed atmospheric boundary layer profile are shown along with estimates of time variation of the torque generated by the windmill as it rotates in a time varying free stream velocity. These models form the basis for the design optimization of the blade profiles which would ensure as close to an uniform output of the torque around the axis of rotation in the presence of the temporal and spatially varying wind speeds that prevail over the area where the windmills are sited in order to improve the performance of the windmill by examining its performance metrics in the next phase of work. Keywords:- HAWT, VAWT, CFD, Atmospheric Boundary Layer. 1. Introduction Harnessing wind energy for domestic needs has been an age old tradition not only in India, but around the world. Modern design techniques using Computational Fluid Dynamics (CFD) are rapidly replacing the traditional approaches of designing multi-purpose wind turbines. The aim of this work is to use CFD to compute the aerodynamics of Horizontal Axis Wind Turbine (HAWT) and a Vertical Axis Wind Turbine (VAWT) designs for low-cost rural applications such as pumping of brine water, irrigation, and electricity generation. The model will also serve as a basis for examining the aerodynamic considerations for the placement of wind turbines in a wind farm and the blade wake interactions from these turbines. The approaches have been used to model wind turbine characteristics using CFD in the past fall into low-order models, or steady, non-rotating two dimensional studies and three-dimensional flows. While low-order and two-dimensional models provide useful insight, important flow physics associated with complex three-dimensional flows are usually lost. There are also efforts to study the time accurate aerodynamic characteristics of wind turbines. Benjanirat and Sankar (2003) have carried out a comparison between different turbulence models and their performance in predicting wind turbine characteristics. Sezer-Uzol and Long (2006) have carried out a time accurate, unsteady, inviscid computation of a two blade wind turbine. Turbine blades under yawed flow have been addressed in Tongchitpakdee et al. (2005). Experimental and computational study of VAWT was carried out by Howell et al. (2005). However there is a paucity of discussions on how the free stream wind conditions affect the rate of rotation of the turbine. HAWT and VAWT are mounted on structural frameworks (henceforth referred as structure) and most studies have only focused on the blades isolated from the framework. The present study aims to compute steady and unsteady viscous threedimensional blade rotation rate and hence the torque which is the output required to drive useful wind powered applications in the presence of the structural mount. The aerodynamic characteristics and flowfield of a HAWT was first studied in isolation without presence of the Proc. of the 8th Asia-Pacific Conference on Wind Engineering Nagesh R. Iyer, Prem Krishna, S. Selvi Rajan and P. Harikrishna (eds) Copyright c 2013 APCWE-VIII. All rights reserved. Published by Research Publishing, Singapore. ISBN: doi: /
2 structure. Then the impact of including the structure on the HAWT aerodynamics is assessed. A standard practice is to compute the torque acting on the turbine rotating at a fixed rotation rate. In the actual scenario, the rotation of the turbine is a function of the aerodynamic moment acting on it, which depends on the free stream wind speed and direction. In this study the torque generated is estimated from the rotation of the turbine induced by the wind speed which may be steady or unsteady. The standard atmospheric boundary layer (ABL) profile described in Garratt et al. (1982) is used in place of uniform velocity profiles which are used for turbine alone studies in literature since wind turbines are mounted on structural frameworks mounted on the ground. 2. Computational Modeling of HAWT and VAWT Aerodynamics Time accurate unsteady flow past a HAWT and VAWT is computed by solving the unsteady incompressible Reynolds Averaged Navier-Stokes (RANS) equations using a finite volume based method within the framework of Star-CCM+(2012) which is a commercial CFD software package. The incompressible RANS model in finite-volume formulation is given as: ( b U U ) ds = 0 (1(a)) S d ρ UdV + U ( U U b). nds = pnds + (( μ + μt ) τ) nds + ρ f dv dt V S S S V 1(b)) where the vector U defines the velocity field, p is the pressure field and U b is the velocity of the moving mesh boundary. From the CAD drawings of a full scale model of the HAWT, a three-dimensional CAD model is first constructed. Similarly a VAWT model is also developed as a starting design, keeping in mind the small scale and economical application in the rural sector. The computational mesh is then created within the computational domain of interest where the RANS model is solved by appropriate spatial and temporal discretization schemes to compute the unsteady evolution of the flow field which provides insight into the flow patterns and structures in the wake region of the turbine. Composite grids involving arbitrary moving mesh to facilitate free rotation of the mesh around and fixed to the turbines blades which moves relative to the rest of the computational mesh. The exchange of information between the moving and the stationary regions is done using a sliding mesh technique. The convective flux in the momentum equation Eqn. (1(b)) is discretized using the second order upwind scheme. The flow variables are then advanced in time with the help of implicit time stepping scheme. The mesh that had been created has been refined near the turbine blade surfaces and also in the wake region to effectively capture the wakes created by the turbine motion (rotation in case of VAWT, rotation and yaw in case of HAWT). The flow is assumed to be turbulent; the turbulence has been modeled using the Spalart-Allmaras (1992) turbulence model which solves a transport equation to determine the turbulent dynamic viscosity T which is added to the laminar viscosity.in order to resolve the boundary layer at the ground and wing surface, a thin conformal structured prismatic mesh consisting of 15 layers of structured cells have been created over the wall surface in order to obtain a y+ value of 11.4 is created along the ground and blade surfaces. 2.1 Computational Domain and Boundary Conditions Figure 1 shows the computational domains used for this study pertaining to unsteady aerodynamics of HAWT and VAWT. At the inflow boundary, the velocity is set to the free stream velocity. At the outflow, the pressure is interpolated from within the domain by setting 1239
3 the pressure gradient to zero. The no slip boundary condition is specified on the blade surfaces and one the ground plane. At the far field boundary, the pressure is set to the free stream value. The structure is considered as a wall and no slip condition has been set there. In the case of HAWT with the complete structure, portions of the structure have been modeled as porous surfaces to account for airflow through framework strut gaps which will be outlined in the full paper. The initial conditions for the different cases have been discussed in the method of approach section. Figure 1: Computational Domain used for the study of HAWT 2.2 Mesh Generation The computational domain is discretized into a mesh of polygonal elements using the mesh generator in the within the framework of the commercial CFD software Star-CCM+ (2012). The mesh refinement to resolve the flow structures in the vicinity of the HAWT and in the evolving wake region where the mesh has been refined in the region downstream of the turbine in order to capture the wake patterns effectively are shown in Fig. 2. (a) Mesh used for the study of HAWT with structure. (b) Zoomed in view of the mesh created HAWT. (c) Prism layer on the turbine blade surface to capture near wall flows (d) Mesh used for the computational study of VAWT (e) Zoomed in view of the mesh near VAWT. Figure 2: Computational Meshes (f) Perspective view of the mesh for VAWT 1240
4 The total number of mesh elements in the domain varies from case to case; however the order of mesh elements used in these studies runs into approximately a million elements. The rotation of the turbine blades is handled by rotating the cylindrical region encompassing the blade and the mesh generated within it relative to the rest of the stationary mesh outside the cylinder. In the case of the HAWT the yawing motion of the directional vane fixed to the turbine is also accounted for. The computed flow variables are interpolated in a conservative manner across the boundaries of the stationary and rotating regions of the domain using the sliding mesh technique. Details of the interpolation of flow variables to ensure conservation across the sliding mesh interface can be found in the work of Steijl et al. (2008). The mesh in the computational domain has been refined on similar lines as it has been done so in the case shown previously Method of Approach The unsteady computations carried out in this study, for both HAWT and VAWT, have been done in three different phases. Each phase uses the result from the previous phase as its initial condition. In the first phase, a preliminary steady flow field is generated by rotating the turbine at a fixed rotation determined from field data obtained from a rural application for brine water pumping in the coastal areas of Gujarat in the presence of the corresponding free stream wind speed or ABL wind profile. This computed steady flow field is then used as initial conditions in the next phase, where the turbine blade is allowed to rotate freely under the influence of the aerodynamic torque acting on it. The purpose of this phase is to have the turbine blades rotate at a steady rotation rate which depends on its shape and free stream velocity. In this study, the angular velocity has been determined implicitly from a 1 DOF dynamics equation, = I, where is the aerodynamic torque acting on the turbine blades, I is the moment of inertia of the turbine about its axis of rotation and is the angular acceleration of the turbine. The torque is estimated using the computed surface pressure distribution on the turbine blades at each time step Δ t. Using a simple first order Euler integration, the relationship between the angular rotation at two consecutive time levels can be established as τ n ωn+ 1 = ωn + Δt (2) I Equation (2) allows the angular speed of the turbine to change at every time step thereby readjusting the aerodynamic torque at each step as well. The third phase is then initiated by varying the free stream velocity of wind, in order to study the unsteady response of the turbine to rapidly changing wind speeds and direction. 3. Results and Discussions 3.1 HAWT (without structure) As mentioned in the previous section, the approach of the computational study involves carrying out the computation in three phases. The free stream velocity, torque experienced by the blade, and the angular velocity of the blade can be seen in Fig. 3 for all the three phases. It can be seen that rotating the turbine at a fixed rotation rate leads to a steady non- zero torque. However, when the rotation rate of the turbine is coupled to the aerodynamic moment experienced by it using Eqn. (2), as in the second phase, both the value of torque and the rotation rate begin to change with time. The rotation rate reaches a steady value, and the torque also reduces to a steady value of zero. This physically makes sense, as for a steady free stream velocity, the turbine will observe a steady rotation rate. From Eqn. (2), in order 1241
5 for the rotation rate to be steady with time, the rate of change of rotation rate will be zero, and thus will also be the torque experienced by the turbine, which is what has been observed. In the third phase, the response of the turbine has been studied to the varying free stream velocity of the wind. From Fig. 3, it can be observed that the wind velocity has been varied piecewise linearly, according to a random distribution. This change in wind velocity disturbs the flow field, giving rise to changes in pressure distribution across the turbine blade surfaces, and hence leading to a non-zero torque, as shown in Fig. 3. From Eqn. (2) it is known, that a non-zero torque changes the angular rotation rate of the turbine which is shown in Fig. 3 as well. Visualization of the flow field obtained at the end of second phase has been displayed in Fig. 4. The swirl of the wake can be clearly seen from the plots of the velocity and vorticity contours on several Trefftz planes in the wake region of the turbine blades. Figure 3: Variation of torque, angular speed of the turbine and free stream velocity of the wind with time across all three phases. (a) Filled velocity contours on a Trefftz plane. (b) Vorticity contours on various Trefftz planes. (c) Velocity contours on a series of Trefftz plane. (d) Pressure distribution on the upstream side of the turbine blades. Figure 4: Computed flowfield patterns for the case involving HAWT without the structure. 3.2 VAWT (without Structure) A similar computational approach has been used to study VAWT flowfields. Initial condition for the 1st phase for VAWT was set up in exactly the same manner as for the HAWT, for the second phase, the torque and rotation rate have been coupled with help of Eqn. (2). Figure 5 shows the computed variation of RPM with time and varying wind velocities. 1242
6 (a) Variation of aerodynamic moment. (b) Variation of rotation rate and velocity Figure 5: Variation of parameters of VAWT with respect to time. From Fig. 5 we see that airflow at a constant velocity over a VAWT produces a torque which is oscillating about a fixed non-zero value. It is also observed that the torque increases with increase in inflow velocity and decreases with a reduction in inflow air velocity. It was observed that unlike the case of HAWT, the torque in VAWT never tends to zero but oscillates about zero value because the VAWT blades observe different angles of attack as they rotate about the vertical axis, whereas in the case of HAWT the blades always see the same angle of attack and velocity. As seen in Fig. 6, it can be seen that the orientation of the VAWT blades changes at every time step. Because of this, the relative angle of attack the blade sees at every time step also changes, and so will the magnitude of the relative wind. At a certain instance of time t n, the blade is at an angle of n with the free stream velocity. At this instance the blade is experiencing a relative wind which is a vector sum of V and n. In order to compute the relative velocity and the relative angle of attack, assume the airfoil to be at a certain orientation as shown in Fig. 6(b). (a) (b) Figure 6: (a) Relative angle of attack for different blade orientation, (b) Vector diagram for relative angle of attack. 1243
7 The angle between the chord of the blade and the free stream velocity n is given by: θ = ω Δ t + θ. (3) ( ) n n 1 n 1 Now, there are two vectors inclined to each other at an angle n, the resultant of these two vectors is given by: 2 2 Rv = ( V ) + ( ω ) + 2V ω cos θ n n n (4) By resolving basic trigonometric relations an expression for the relative angle of attack can be obtained as 1 ωnsinθn α = θn sin ( ) R v (5) From these relations it can be observed that the variation of relative velocity, relative angle of attach and variation of moment for a single rotation of blade is shown by Fig. 7. Similar results can be found in the work carried out by Castelli et al (2011). (a) Relative angle of attack (b) Magnitude of relative velocity (c) Aerodynamic moment Figure 7: Variation with respect to angular position. Flow field about a VAWT can be visualized with the help of Fig. 8. The blade leading edge experiences high pressure coefficient and it goes to maximum when it the blade leading edge faces the inflow velocity. In Fig. 8, the wake generated by VAWT can be seen to extend till the end of the computational domain, and the strength decreasing gradually in the direction downstream of the VAWT. (a) (b) (c) (d) Figure 8: (a) Pressure coefficient on Cut plane through VAWT, (b) Velocity contours on Cross- planes through VAWT, (c) Pressure coefficient on ground and VAWT with velocity contours in downstream region, (d) Vorticity contours in downstream of the VAWT. 1244
8 3.3 HAWT with Structure In this section the effect of including the structure of the wind turbine and make necessary comparisons with results without the structure. As the structure consists of many struts and links an approximation to represent the base structure to be built of porous plates conforming to the shape of the structural framework has been used from the point of view of computational economy. The porosity was estimated as a fraction of empty space and the total space occupied by the struts on the assumed plate and the estimate of the porosity for the supporting structure of the wind turbine was found to be Non-uniform porosity distributions to better represent the approximation are being explored at the moment. Figure 9 shows various computed contours of flow variables in the wake region of the turbine. In Fig. 9(a), the wake from the turbine can be seen to be interacting with the wake from the structure. It can also be seen that the flow velocities near the blade tips are higher than that near the root regions showing typical expected characteristics of rotating bodies. It can be observed from the computations that the structure facing the inflow experiences a higher surface pressure than that of the structure facing downstream. The computations also reveal that since the structure interacts with the wake emerging from the rotating blades, there is a cyclical intermittent fluid-structure interaction taking place between the rotating turbine blades and the structure, the region of this interaction on the structure experiences a higher pressure than that of the rest of the structure as shown in Fig. 9(d). (a) (b) (c) (d) Figure 9: Computed (a) Velocity Contours on a cut section through the HAWT (b) Pressure coefficient contours on the HAWT and Velocity contours in the downstream wake region (c) vorticity contours in the downstream wake region (d) Pressure coefficient contours on the HAWT structure. The impact of the presence of the structure on the HAWT moment and torque variation is shown in Fig. 10 it can be seen that, in the case of the turbine blades with the structure there is a sinusoidal variation in the aerodynamic moment about a mean value. This is due to the pressure rise on the suction side of the blade (Fig. 9(d)) due to the fluid-structure interaction between the moving turbine blade, the static structure and the fluid contained between these two entities, each time the blade passes the structure, thereby giving rise to changes in the surface pressure on the blade. 1245
9 Figure 10: Variation of torque acting on turbine and free stream velocity with time in the presence of the structure. 3.4 Effect of Atmospheric Boundary Layer(ABL) The results discussed in the previous sections are for a uniform velocity inflow condition. However, in real conditions, a turbine will encounter an atmospheric boundary layer because of its close proximity to the terrain. In order to simulate with parameters closer to the real life atmospheric conditions, the Atmospheric Boundary layer (ABL) outlined in Garratt et al. (1982) has been used as an inflow condition. The ABL used in this study is based on the averaging of wind data provided by various internet sources providing real time and summarized details of wind and temperature conditions in a desired geographical region of α 1 ref India. The ABL flow conditions used as inflow condition is defined as U Z Z, U ref = where α = ln 10 Z o where U is the velocity at the altitude Z, U ref is the reference velocity at reference altitude Z ref, and Zo is the ground roughness length. For this study U ref, Z ref, and Zo are assumed to be 10ms -1, 25 m and 0.02 respectively. Figure 11 shows the variation of the computed velocity profiles in the downstream region of HAWT and VAWT. (a) HAWT (b) VAWT Figure 11: Velocity contours plotted in different Trefftz planes. It can be noted that using the atmospheric boundary layer inflow condition captures the wake patterns in the vicinity of the wind turbine mixing with ABL thereby changing the overall wake patterns as observed in Fig 11, where computed velocity contours are shown on various Trefftz planes in the downstream region of the turbine. Note: Selected animations of selected computed flow field variables past the VAWT and HAWT can be viewed at the YouTube channel by clicking on the following link:
10 4. Conclusion The high fidelity CFD models for assessing the performance of a single HAWT and VAWT in various modes (with and without structural framework) in this study can now be used to assess various performance aspects of wind farms. On the basis of the present work, future effort will be focused on the assessment of fluid- blade surface and structure interaction, studying the interaction of wakes from a wind farm, optimal spacing between the various HAWT/VAWT units and the impact of the wakes on the environment. For this the plan will be to use LES simulations. The models will also serve as the basis for blade design optimization and assessment of power characteristics for various operational applications such as brine water pumping and electricity generation in the rural sector. References Benjanirat, S., Sankar, L. N., & Guanpeng X.. Evaluation of turbulence models for the prediction of wind turbine aerodynamics, AIAA Paper Castelli, R. M., Englaro A., Benini E., The Darrieus wind turbine: Proposal for a new performance prediction model based on CFD, Elseiver, Journal of Energy, 36(8), Howell, R., Qin, N., Edwards, J. and Durrani, N. Wind tunnel and numerical study of a small vertical axis wind turbine. Renewable Energy, 35(2), , Garratt, J. R., Wyngaard, J. C., & Francey, R. J. (1982). Winds in the atmospheric boundary layer-prediction and observation. Journal of Atmospheric Sciences, 39, Sezer-Uzol, N., & Long, L. N. 3-D time-accurate CFD simulations of wind turbine rotor flow fields. AIAA Paper , 44 th Aerospace Sciences Meeting and Exhibit, Reno, NV. Spalart, P.R., and Allmaras S.R., "An one-equation turbulence model for aerodynamic flows." AIAA, Aerospace Sciences Meeting and Exhibit, 30 th, Reno, NV StarCCM+, Computational Fluid Dynamics and Multi-Physics Engineering Software, Version 7.06, (2012) CD-Adapco, Lebanon, NH, USA. Steijl, R., and G. Barakos. "Sliding mesh algorithm for CFD analysis of helicopter rotor fuselage aerodynamics." International journal for numerical methods in fluids 58.5 (2008): Tongchitpakdee, C., Benjanirat, S., & Sankar, L. N. (2005). Numerical simulation of the aerodynamics of horizontal axis wind turbines under yawed flow conditions. Transactions- ASME, Journal of Solar Energy Engineering, 127(4),
CFD 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 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 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 informationReproducibility of Complex Turbulent Flow Using Commercially-Available CFD Software
Reports of Research Institute for Applied Mechanics, Kyushu University, No.150 (60-70) March 2016 Reproducibility of Complex Turbulent Flow Using Commercially-Available CFD Software Report 2: For the Case
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 informationReproducibility of Complex Turbulent Flow Using Commercially-Available CFD Software
Reports of Research Institute for Applied Mechanics, Kyushu University No.150 (47 59) March 2016 Reproducibility of Complex Turbulent Using Commercially-Available CFD Software Report 1: For the Case of
More informationTHE APPLICATION OF AN ATMOSPHERIC BOUNDARY LAYER TO EVALUATE TRUCK AERODYNAMICS IN CFD
THE APPLICATION OF AN ATMOSPHERIC BOUNDARY LAYER TO EVALUATE TRUCK AERODYNAMICS IN CFD A SOLUTION FOR A REAL-WORLD ENGINEERING PROBLEM Ir. Niek van Dijk DAF Trucks N.V. CONTENTS Scope & Background Theory:
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 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 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 informationOpenFOAM capabilities for the analysis of Vertical-Axis Wind Turbine aerodynamics
OpenFOAM capabilities for the analysis of Vertical-Axis Wind Turbine aerodynamics Diego Domínguez 1, a), Daniel Fernández 1, Tim De Troyer 2, Mark C. Runacres 2 1 Aerospace Engineering Area, Universidad
More informationCFD SIMULATIONS OF HORIZONTAL AXIS WIND TURBINE (HAWT) BLADES FOR VARIATION WITH WIND SPEED
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
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 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 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 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 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 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 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 informationApplication 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 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 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 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 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 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 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 informationCFD VALIDATION FOR SURFACE COMBATANT 5415 STRAIGHT AHEAD AND STATIC DRIFT 20 DEGREE CONDITIONS USING STAR CCM+
CFD VALIDATION FOR SURFACE COMBATANT 5415 STRAIGHT AHEAD AND STATIC DRIFT 20 DEGREE CONDITIONS USING STAR CCM+ by G. J. Grigoropoulos and I..S. Kefallinou 1. Introduction and setup 1. 1 Introduction The
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 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 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 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 informationANSYS FLUENT. Airfoil Analysis and Tutorial
ANSYS FLUENT Airfoil Analysis and Tutorial ENGR083: Fluid Mechanics II Terry Yu 5/11/2017 Abstract The NACA 0012 airfoil was one of the earliest airfoils created. Its mathematically simple shape and age
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 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 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 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 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 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 informationDriven Cavity Example
BMAppendixI.qxd 11/14/12 6:55 PM Page I-1 I CFD Driven Cavity Example I.1 Problem One of the classic benchmarks in CFD is the driven cavity problem. Consider steady, incompressible, viscous flow in a square
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 Methods in Aerodynamics. Fluid Structure Interaction. Lecture 4: Fluid Structure Interaction
Fluid Structure Interaction Niels N. Sørensen Professor MSO, Ph.D. Department of Civil Engineering, Alborg University & Wind Energy Department, Risø National Laboratory Technical University of Denmark
More informationDNV GL s 16th Technology Week
OIL & GAS DNV GL s 16th Technology Week Advanced Simulation for Offshore Application: Application of CFD for Computing VIM of Floating Structures 1 SAFER, SMARTER, GREENER OUTLINE Introduction Elements
More informationUnsteady Flow Simulation and Dynamic Stall Behaviour of Vertical Axis Wind Turbine Blades
WIND ENGINEERING VOLUME 35, NO. 4, 2011 PP 511-510 511 Unsteady Flow Simulation and Dynamic Stall Behaviour of Vertical Axis Wind Turbine Blades Ning Qin*, Robert Howell, Naveed Durrani, Kenichi Hamada
More informationSimulation of Flow Development in a Pipe
Tutorial 4. Simulation of Flow Development in a Pipe Introduction The purpose of this tutorial is to illustrate the setup and solution of a 3D turbulent fluid flow in a pipe. The pipe networks are common
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 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 informationWind tunnel study on load combination including torsion for design of medium-rise buildings
The Eighth Asia-Pacific Conference on Engineering, December 10 14, 2013, Chennai, India tunnel study on load combination including torsion for design of medium-rise buildings Mohamed Elsharawy, Ted Stathopoulos,
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 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 information41. Application of the Domain Decomposition Method to the Flow around the Savonius Rotor
12th International Conference on Domain Decomposition Methods Editors: Tony Chan, Takashi Kako, Hideo Kawarada, Olivier Pironneau, c 2001 DDM.org 41. Application of the Domain Decomposition Method to the
More informationSPC 307 Aerodynamics. Lecture 1. February 10, 2018
SPC 307 Aerodynamics Lecture 1 February 10, 2018 Sep. 18, 2016 1 Course Materials drahmednagib.com 2 COURSE OUTLINE Introduction to Aerodynamics Review on the Fundamentals of Fluid Mechanics Euler and
More informationInviscid Flows. Introduction. T. J. Craft George Begg Building, C41. The Euler Equations. 3rd Year Fluid Mechanics
Contents: Navier-Stokes equations Inviscid flows Boundary layers Transition, Reynolds averaging Mixing-length models of turbulence Turbulent kinetic energy equation One- and Two-equation models Flow management
More informationMESH REQUIREMENT INVESTIGATION FOR 2D AND 3D AERODYNAMIC SIMULATION OF VERTICAL AXIS WIND TURBINES
MESH REQUIREMENT INVESTIGATION FOR 2D AND 3D AERODYNAMIC SIMULATION OF VERTICAL AXIS WIND TURBINES SAMAN NAGHIB ZADEH A Thesis In the Department of Mechanical and Industrial Engineering Presented in Partial
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 informationTutorial 2. Modeling Periodic Flow and Heat Transfer
Tutorial 2. Modeling Periodic Flow and Heat Transfer Introduction: Many industrial applications, such as steam generation in a boiler or air cooling in the coil of an air conditioner, can be modeled as
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 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 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 informationALE Seamless Immersed Boundary Method with Overset Grid System for Multiple Moving Objects
Tenth International Conference on Computational Fluid Dynamics (ICCFD10), Barcelona,Spain, July 9-13, 2018 ICCFD10-047 ALE Seamless Immersed Boundary Method with Overset Grid System for Multiple Moving
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 informationValidation of an Unstructured Overset Mesh Method for CFD Analysis of Store Separation D. Snyder presented by R. Fitzsimmons
Validation of an Unstructured Overset Mesh Method for CFD Analysis of Store Separation D. Snyder presented by R. Fitzsimmons Stores Separation Introduction Flight Test Expensive, high-risk, sometimes catastrophic
More informationMESHLESS SOLUTION OF INCOMPRESSIBLE FLOW OVER BACKWARD-FACING STEP
Vol. 12, Issue 1/2016, 63-68 DOI: 10.1515/cee-2016-0009 MESHLESS SOLUTION OF INCOMPRESSIBLE FLOW OVER BACKWARD-FACING STEP Juraj MUŽÍK 1,* 1 Department of Geotechnics, Faculty of Civil Engineering, University
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 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 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 informationAnalysis of Wind Forces on a High-Rise Building by RANS-Based Turbulence Models using Computational Fluid Dynamics
Analysis of Wind Forces on a High-Rise Building by RANS-Based Turbulence Models using Computational Fluid Dynamics D.V.V. Rajkamal 1 and Ch. Raviteja 2 1 (Post graduate student, V.R. Siddhartha Engineering
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 informationNUMERICAL MODELING STUDY FOR FLOW PATTERN CHANGES INDUCED BY SINGLE GROYNE
NUMERICAL MODELING STUDY FOR FLOW PATTERN CHANGES INDUCED BY SINGLE GROYNE Jungseok Ho 1, Hong Koo Yeo 2, Julie Coonrod 3, and Won-Sik Ahn 4 1 Research Assistant Professor, Dept. of Civil Engineering,
More informationResearch and Design working characteristics of orthogonal turbine Nguyen Quoc Tuan (1), Chu Dinh Do (2), Quach Thi Son (2)
GSJ: VOLUME 6, ISSUE 6, JUNE 018 116 Research and Design working characteristics of orthogonal turbine Nguyen Quoc Tuan (1), Chu Dinh Do (), Quach Thi Son () (1) Institute for hydro power and renewable
More informationComputational Fluid Dynamics modeling of a Water Flow Over an Ogee Profile
FINITE ELEMENT METHOD TECHNICAL REPORT Computational Fluid Dynamics modeling of a Water Flow Over an Ogee Profile ANSYS CFX 12 ENME 547 Dr. Sudak Matias Sessarego Written Report Due Date: Friday December
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 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 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 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 informationA COMPARATIVE STUDY ON INTERFERENCE FACTORS OF BUILDINGS
The Eighth Asia-Pacific Conference on Wind Engineering, December 10 14, 013, Chennai, India A COMPARATIVE STUDY ON INTERFERENCE FACTORS OF BUILDINGS Ankit Singh 1 & S. Mandal 1 IDD (B. Tech. - M.Tech.)
More informationAerodynamicCharacteristicsofaReal3DFlowaroundaFiniteWing
Global Journal of Researches in Engineering: D Chemical Engineering Volume 14 Issue 1 Version 1.0 Year 2014 Type: Double Blind Peer Reviewed International Research Journal Publisher: Global Journals Inc.
More informationMissile External Aerodynamics Using Star-CCM+ Star European Conference 03/22-23/2011
Missile External Aerodynamics Using Star-CCM+ Star European Conference 03/22-23/2011 StarCCM_StarEurope_2011 4/6/11 1 Overview 2 Role of CFD in Aerodynamic Analyses Classical aerodynamics / Semi-Empirical
More informationA simple method for potential flow simulation of cascades
Sādhanā Vol. 35, Part 6, December 2010, pp. 649 657. Indian Academy of Sciences A simple method for potential flow simulation of cascades ARAVIND BHIMARASETTY and RAGHURAMAN N GOVARDHAN Department of Mechanical
More informationSTAR-CCM+: Wind loading on buildings SPRING 2018
STAR-CCM+: Wind loading on buildings SPRING 2018 1. Notes on the software 2. Assigned exercise (submission via Blackboard; deadline: Thursday Week 3, 11 pm) 1. NOTES ON THE SOFTWARE STAR-CCM+ generates
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 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 informationLab 9: FLUENT: Transient Natural Convection Between Concentric Cylinders
Lab 9: FLUENT: Transient Natural Convection Between Concentric Cylinders Objective: The objective of this laboratory is to introduce how to use FLUENT to solve both transient and natural convection problems.
More informationComputational Study of Laminar Flowfield around a Square Cylinder using Ansys Fluent
MEGR 7090-003, Computational Fluid Dynamics :1 7 Spring 2015 Computational Study of Laminar Flowfield around a Square Cylinder using Ansys Fluent Rahul R Upadhyay Master of Science, Dept of Mechanical
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 informationFLOW PAST A SQUARE CYLINDER CONFINED IN A CHANNEL WITH INCIDENCE ANGLE
International Journal of Mechanical Engineering and Technology (IJMET) Volume 9, Issue 13, December 2018, pp. 1642 1652, Article ID: IJMET_09_13_166 Available online at http://www.iaeme.com/ijmet/issues.asp?jtype=ijmet&vtype=9&itype=13
More informationThe viscous forces on the cylinder are proportional to the gradient of the velocity field at the
Fluid Dynamics Models : Flow Past a Cylinder Flow Past a Cylinder Introduction The flow of fluid behind a blunt body such as an automobile is difficult to compute due to the unsteady flows. The wake behind
More informationCFD Analysis of a Fully Developed Turbulent Flow in a Pipe with a Constriction and an Obstacle
CFD Analysis of a Fully Developed Turbulent Flow in a Pipe with a Constriction and an Obstacle C, Diyoke Mechanical Engineering Department Enugu State University of Science & Tech. Enugu, Nigeria U, Ngwaka
More informationNovember c Fluent Inc. November 8,
MIXSIM 2.1 Tutorial November 2006 c Fluent Inc. November 8, 2006 1 Copyright c 2006 by Fluent Inc. All Rights Reserved. No part of this document may be reproduced or otherwise used in any form without
More informationEVALUATION OF A GENERAL CFD-SOLVER FOR A MICRO-SCALE URBAN FLOW
EVALATION OF A GENERAL CFD-SOLVER FOR A MICRO-SCALE RBAN FLOW Jarkko Saloranta and Antti Hellsten Helsinki niversity of Technology, Laboratory of Aerodynamics, Finland INTRODCTION In this work we study
More informationCFD-BASED SIMULATION AND EXPERIMENT IN HELICOPTER AEROMECHANICS. Richard E Brown and Stewart S Houston
CFD-BASED SIMULATION AND EXPERIMENT IN HELICOPTER AEROMECHANICS Richard E Brown and Stewart S Houston Helicopter Aeromechanics: A difficult simulation problem multiple rotors (with multiple blades) attached
More informationWake Flow Simulations for a Mid-Sized Rim Driven Wind Turbine
Wake Flow Simulations for a Mid-Sized Rim Driven Wind Turbine Andrew B. Porteous 1, Bryan E. Kaiser 2, and Svetlana V. Poroseva 3 University of New Mexico, Albuquerque, New Mexico, 87131 Cody R. Bond 4
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 information39th AIAA Aerospace Sciences Meeting and Exhibit January 8 11, 2001/Reno, NV
AIAA 1 717 Static Aero-elastic Computation with a Coupled CFD and CSD Method J. Cai, F. Liu Department of Mechanical and Aerospace Engineering University of California, Irvine, CA 92697-3975 H.M. Tsai,
More informationAPPLICATION OF A NAVIER-STOKES SOLVER TO THE ANALYSIS OF MULTIELEMENT AIRFOILS AND WINGS USING MULTIZONAL GRID TECHNIQUES
APPLICATION OF A NAVIER-STOKES SOLVER TO THE ANALYSIS OF MULTIELEMENT AIRFOILS AND WINGS USING MULTIZONAL GRID TECHNIQUES Kenneth M. Jones* NASA Langley Research Center Hampton, VA Robert T. Biedron Analytical
More informationProgram: Advanced Certificate Program
Program: Advanced Certificate Program Course: CFD-Vehicle Aerodynamics Directorate of Training and Lifelong Learning #470-P, Peenya Industrial Area, 4th Phase Peenya, Bengaluru 560 058 www.msruas.ac.in
More informationNumerical optimization of the guide vanes of a biradial self-rectifying air turbine.
Numerical optimization of the guide vanes of a biradial self-rectifying air turbine. André Ramos Maduro email: andre.maduro@ist.utl.pt Instituto Superior Técnico, University of Lisbon,Av. Rovisco Pais,1049-001
More informationSummary and additional notes for Static ti pressure measurements:
Summary and additional notes for Static ti pressure measurements: Determination of static pressure a) Wall tapping b) static tube Error in pressure is function of: Error in pressure is function of: And
More informationBackward facing step Homework. Department of Fluid Mechanics. For Personal Use. Budapest University of Technology and Economics. Budapest, 2010 autumn
Backward facing step Homework Department of Fluid Mechanics Budapest University of Technology and Economics Budapest, 2010 autumn Updated: October 26, 2010 CONTENTS i Contents 1 Introduction 1 2 The problem
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 information