Numerical optimization of the guide vanes of a biradial self-rectifying air turbine.
|
|
- Ralf Jacobs
- 5 years ago
- Views:
Transcription
1 Numerical optimization of the guide vanes of a biradial self-rectifying air turbine. André Ramos Maduro andre.maduro@ist.utl.pt Instituto Superior Técnico, University of Lisbon,Av. Rovisco Pais, Lisboa, Portugal July 2016 Abstract The focus of this paper is the design and optimization of the guide-vane system of a self-rectifying biradial air turbine for use in oscillating water column systems for wave energy conversion. Since the turbine is required to be self-rectifying, there are two sets of guide-vanes, placed symmetrically on both sides of the rotor, instead of a single set (as in the conventional turbines). The efficiency of the biradial turbine with fixed guide-vanes is affected by the losses at the entry to the downstream row of guide-vanes, due to the misalignment between the flow direction and the exit guide-vanes. A problem also shared with other self-rectifying axial-flow impulse turbines. The goal of this paper is to perform a numerical optimization of the guide-vane system geometry so as to increase the turbine efficiency by reducing the losses at the exit guide-vane system, while ensuring the required flow deflection at the inlet guide-vane system. Time dependent flow calculations are performed to assess the performance and to evaluate the pressure losses for each guide-vane system configuration, due to the relatively large separated region at the exit guide-vane system. Finally, the turbine operating curves are obtained by calculating the three-dimensional flow through the complete turbine. Keywords: Biradial turbine, guide-vane design, optimization, blade cascade, wave energy. 1. Introduction 1 Self-rectifying impulse turbines (including the biradial turbine) have severe limitations in efficiency due to low aerodynamic performance of the second stator, positioned downstream of the rotor. Since this type of turbines are required to be selfrectifying, there are two sets of guide-vanes placed symmetrically on both sides of the rotor instead of a single set (as in conventional turbines). The guide-vanes, designed to guarantee the desired flow deflection at the impeller inlet, are the main cause of the poor performance of such turbines in the variant of fixed guide-vanes. When the flow exits the rotor, the existing misalignment between the guide-vanes of the downstream stator and the flow direction makes these behave as bluff-bodies. This effect promotes flow separation on the surface of the blades
2 2 and increases drastically the pressure loss in the exit stator. If this misalignment is too high, the flow passage between the guidevanes is strongly obstructed. Thus further increasing the loss and consequently reducing the turbine performance. In 2009, the Portuguese company Kymaner developed a new system of guidevanes in multiples cascades for the axialflow turbine that bridges the effect of the downstream stator [1, 2]. In this case, the inlet flow deflection is divided in stages by the use of several rows of guide-vanes, strategically positioned at a given rotor distance in order to increase the free space between blades (see Fig. 1). This deflection strategy and preferential positioning between sets of guide-vanes allows to increase the passage of outflow and consequently increase the efficiency of the turbine. Company data shows that this strategy guaranteed an increase of 20% in peak efficiency of the axial turbine in comparison with the case of a single row of guide-vanes. The biradial turbine [3], being also a impulse turbine, has the same problem with the downstream stator. Several projects related with the design of guide-vanes had been developed for this turbine [4, 5], but none had addressed the effect of multiple cascades. Therefore the purpose of this paper is to apply this stator design concept to the biradial turbine and evaluate the benefits of it implementation (see Fig. 2). The aim is to assure the deflection of the inflow, without introducing large losses in the inlet stator, and reduce the outflow obstruction with the introduction of multiple cascades. The number of cascades it is a parameter to determine through the downstream stator performance evaluation for a given rotor operation conditions. The guide-vane sections were designed using a thickness and camber distribution optimization that respects the restriction of preferential position to assure minimum outflow obstruction. This numerical geometry optimization problem is solved with the gradient-free Differential Evolution (DE) method [6]. The DE method is a metaheuristic algorithm that solves the optimization problem by iterative improving a candidate solution through the use of genetic operations. To validate the optimized geometries, time dependent calculations are performed through the downstream stator to evaluate the pressure drop. Finally a 3D flow analysis through the complete turbine will define the performance of this stator concept. Figure 1: Stator of the self-rectifying impulse turbine developed by Kymaner for the ModOndas national project (reproduced from [1]). 1 st row of guide-vanes 2 nd row of guide-vanes Radial flow Rotor Figure 2: Flow representation for exit guide-vane system of the biradial turbine.
3 Periodic surface 1 st row of guide vanes 2 nd row of guide vanes Periodic surface Figure 3: Computational domain and blades preferential position for purely radial exit flow. LE1 LE2 1 st row 2 nd row TE2 TE1 Figure 4: Blades parameter for a guide-vane system of multiple cascades. 2. Blade cascades design The positioning of the blades is one of the most important geometrical parameters in this stator design. The guide-vanes are placed in a configuration which maximizes the flow free passage between the blades of the downstream stator (see Fig. 3). This configuration is based on the shadow effect provided by the upstream blades when the flow exit the impeller. Thus, the blades rows are placed within the same angular window β relative to the rotor outflow direction. This strategy ensures that downstream blades are in the wake of upstream ones (see Fig. 2). To control the flow free path in the downstream stator it s defined the blockage factor parameter ζ, given in percentage by ζ(%) = β 100%, (1) Θ where Θ corresponds to the row space an- 3 gle between blades, controlled by the number of blades in the circumferential direction (fixed to 57 blades). The blockage factor ζ represents the obstructed path caused by the exit guide-vanes (symmetrical of the inlet) and it s an indicator of how large is going to be the pressure drop in the exit stator. For a given ζ, the leading and trailing edges of each cascade blade are coincident with the lines of constant β (see Fig. 4). Therefore the blades stagger angle and chord are managed simultaneously by the design parameters R that control the radial position between blades edges, making this two variables implicit in the optimization algorithm. The blades thickness distribution is scaled form the NACA 63A012 [7], using a scale factor parameter for each blade. The camber line is set from Bézier curves, defined with 2 control points, to reduce the number of variables
4 per blade. The first and the last point define the beginning and the end of the curve (see Fig. 5), while the intermediate points coordinates (2 and 3) define the design variables for the camber line. A preliminary exploratory work has shown that the use of 2 intermediate points, with a fixed radial position (r LE, r T E ), generate a wide range of geometries for the camber line curvature. The angular position of intermediate points (δ LE, δ T E ) controls the blade inlet/exit angles (ε LE, ε T E ) when placed in the preferential position. However if the exit flow is not purely radial, as shown in Fig. 3, the first blade s wake does not provide a full shadowing effect to the downstream ones. In this case (α 2 90 o ), the blades are positioned between two logarithmic spirals assuming conservation of angular momentum (see Fig. 6). This means that the stator must be optimized with a given rotation λ between cascades, function of the angle α 2, defined by ) λ = cot α 2 ln ( RLE1 R LE2. (2) This rotation between blade cascades does not interfere with the way the blade sections are parameterized. Since the design method repeats itself at each DE optimization step, the parametrization process should be generic, free of discontinuities and also able to keep the number of design parameters as low as possible. In this way, each cascade blade is designed with the same number of optimization parameters (four). Two design variables for the inlet/exit blade angles, one for the thickness scale factor and another one for the chord and stagger angle ( R). When the number of cascades increases one time there are five more variables to optimize (four from the new cascade and one for 4 the radial relative position between blades). In order to reduce even more the number of parameters, the stator to rotor diameter ratio is fixed to R T E /R rotor = 4.65, where R T E is the radial coordinate of the trailing edge of last stator blade, the closest one to the rotor, and R rotor = 244 mm is the rotor radius. LE LE Camber line Figure 5: Bézier curve with 2 control points used to define the camber line. The parameters δ LE and δ T E are related to ε LE and ε T E respectively, that are use as design variables. Relative rotation between radial cas- Figure 6: cades. TE TE TE Logarithmic spiral 3. Computational domain The computational domain used for the flow simulations is set to bi-dimensional and it represents the stator midplane relative to the axial direction. Periodic boundaries are used to reduce the domain size (see Fig. 3) and consequently the computational time. This domain is used for the inflow and outflow calculations, due to the turbine sym-
5 Y Z X metry condition. The only difference between the two domains is the radial size of the upstream block. In the outflow simulation, the exit block is extended due to the large wake and vortices release associated to the flow separation at the blades surfaces. The discretization scheme used for this computational domain is hybrid (see Fig. 7). Around each blade there is a structured block of mesh, in "O" shape, whose construction is based on the surface curvature of the blade [8]. This type of construction assures that the density of points on the surface of the blade is higher in the zones of high curvature, witch is perfect to define the blade trailing edge (see Fig. 8). Involving all the "O" shape meshes there is one unstructured block of mesh whose construction is base on Delaunay triangulations [9]. This block leaves plenty of room for the blade sections to change shape every optimization step, and it s responsible for making the connection between the upstream and the downstream blocks of structured mesh. Figure 7: Mesh blocks. Structured mesh Unstructured mesh Figure 8: Detail of the computational mesh near the blade trailing edge. Y Z X 4. Viscous flow computation The viscous flow simulations were performed using the commercial software FLUENT, that solves the Reynolds- Averaged Navier-Stokes equations (RANS) coupled with a transitional flow k ω SST turbulence model. In this calculations the flow is considered incompressible (Ma<0.3 at T amb = 300K), and the equations are solved using the pressure-based coupled algorithm. The pressure is computed with the 2 nd order scheme and the other equations with the 2 nd order upwind scheme. The inflow conditions are assumed to be steady, while the outflow conditions are considered to be unsteady, due to the relatively large separated flow area at the downstream region of the blades, making this calculations time dependent. The inlet boundary condition for the inflow and outflow calculations is the same. It is imposed as mass flow with turbulence intensity and hydraulic diameter as closure quantities. The turbulence intensity is different for each case, being a higher value estimated for the exit stator due to the passage through the rotor. For both calculations an outflow condition is imposed at the domain exit with the target mass flow equal to the inlet. The blade walls are set to walls with no-slip boundary condition. The working fluid is air with ρ = kg/m 3 and viscosity µ = Pa s. The reference pressure is the standard atmospheric pressure p ref = Pa. The design mass flow rate used for this calculations results from the design conditions at the rotor entrance (V 1t = 2U and α 1 = 30 o ). Combining this conditions with model size Reynolds number Re = ΩR 2 rotor /ν = , where rotation speed Ω = 500 rpm, results the design mass flow rate of 1.49 kg/s. 5
6 5. Optimization strategy The inlet stator blades are optimized through the DE algorithm for a given blockage factor parameter ζ (Eq. 1). This parameter is not a design optimization variable because it is intended, in this paper, to evaluate how it influences the multiple cascades. Therefore blades geometry and position parameters are optimized to guarantee the minimum angle at the rotor entrance (α 1 ) and low pressure losses at the inlet stator. This multi-objective problem can be solved using an objective function F (z) with a weight factor, as the one used in [5]. This weight factor choice is always a difficult decision due to the parameters different nature and because it influences directly the final optimization result. To avoid using a weight factor the pressure drop is estimated through the blade s boundary layer separation. If the flow separates from the surface of any blade, the pressure losses in the inlet stator are considered too high and the tested geometry is discarded from the optimization process. If the flow does not separate, the pressure loss is considered too small to be optimized, and the algorithm is responsible to compute the mean value of the flow angle at the impeller entrance (α 1 ). This pressure losses evaluation strategy allows to set a single term objective function, defined by F (z) = α 1. (3) Since the blades have a rounded trailing edge there is always flow separation in that region. Therefore the flow separation is evaluated in 90% of the line length that defines the suction side of the blade, starting from the leading edge. This means that separation can occur in the last 10% of the 6 line. An acceptable value that assures low pressure losses in the inlet stator. After each geometry calculation the flow separation is evaluated before computing the objective function. To evaluate this, the velocity profiles are analyzed using a local coordinate system on the suction side of the blade (see Fig. 9). Inflection point Flow separation point Reversed flow Zero velocity line Figure 9: Local coordinate system (s x, s y ) on the suction side of a blade. 6. Results In order to determine the effect of the number of cascades Z R in the blockage factor ζ, several optimizations were performed, see Fig. 10. It is chosen to evaluate this effect for three configurations (Z R = 1, 2 and 3 cascades) with the design outflow angle α 2 = 90 o. This means that the outflow is purely radial and it corresponds to the minimum kinetic energy at the rotor exit. For each optimized geometry (point in the graphic), the angle at the rotor entrance α 1 represents the maximum flow deflection that respects the preferential position and separation condition on the surface of the blades, guaranteeing low pressure losses in the inlet stator. As predicted, the blades blockage factor decrease with the increasing number of cascades. For all configurations the flow deflection decreases with the decreasing blockage factor due to the blade load reduction. To check the performance of each configuration, time dependent calculations are performed to evaluate the pressure drop in
7 90% 80% Z R =1 Z R =2 Z R =3 4.0 ζ 70% 60% K p Z R =1 Z R =2 Z R =3 50% 40% α 1 [ ] Figure 10: Blockage factor for systems of 1, 2 and 3 cascades optimized for α 2 = 90 o Re Figure 11: Outflow pressure loss for systems of 1, 2 and 3 cascades optimized for α 2 = 90 o. the downstream stator. The selected geometries penalizes this turbine s stator performance. for this calculations match the ro- In this configuration the pressure drop is al- tor entrance operating condition (α 1 = most twice the verified in the other tested 30 o ). The outflow angle is set to the stators design condition (α 2 = 90 o ). Fig. 11 presents the dimensionless pressure drop (Eq. 4) for each selected configuration as function of the Reynolds number (Eq. 5), configurations. Since the 2 and 3 cascades configurations present almost the same exit losses and both fulfill the inlet stator operating condition, it is preferred to adopt the Z R = 2 configuration. This one brings more K p = p benefits from the economical and manufacturing point of view , (4) 2 R TE However, in order to increase the range Re stat = cv of stator candidates the 2 cascade configuration is optimized for two new different R TE. (5) υ angles: α The dimensionless pressure drop K p is 2 = 65 o and 115 o. Which means a rotation of ±λ between the two cascades defined as the total pressure variation across (see Fig. 6). The optimization process is the blades rows p 01 normalized by the dynamic pressure based on the radial compo- replicated from the previous one, used for the design angle α nent of the flow velocity at the last blade 2 = 90 o, and is presented in Fig. 12. In this two new configurations trailing edge radial section (the same for all the blockage factor presents the same evolution as before, but in the particular case configurations). In this case, the Reynolds number is based on the chord c of the last of the α blade and the radial velocity at the same 2 = 65 o configuration, the blockage factor is significantly smaller for the blade trailing edge radial section. same rotor entrance condition (α Due to the extremely turbulent flow 1 ). The reason behind this huge reduction relays on verified at the downstream section of the the way the blades are placed within the blades, the pressure losses are completely lines of constant β. Where the configurations optimized for design angles α independent from the Reynolds number. The high blockage factor observed for 2 closer to the rotor entrance design angle (α the Z R = 1 configuration (70%) severely 1 ) are 7
8 the most benefited. Finally, a set of calculations for different outflow angles were performed to verify if the design angle α 2 of each configuration fulfills the purpose of it optimization (see Fig. 13). This result shows that each optimized configurations assures the best performance for their own design angle (α 2 = α 2 ), and on the other hand shows that all configurations are very sensitive to variations of the outflow angle. ζ 90% 80% 70% 60% 50% 40% 30% 20% α 2 = 65 α 2 = 90 α 2 = % α 1 [ ] Figure 12: Blockage factor for Z R = 2 optimized for α 2 = 90 ± 25 o. K p α 2 = α 2 = 90 α 2 = α 2 [ ] Figure 13: Influence of the angle α 2 in the outflow pressure loss, for Z R = 2 optimized for α 2 = 90 ± 25 o. 7. Turbine performance 7.1. Modeling the three-dimensional flow To have more reliable values of each stator performance, three-dimensional flow calculations through the complete turbine were performed. The aim of this calculations is the validation of the rotor operating conditions, namely the angle at the rotor entrance, and find out which configuration provides more benefit to the turbine. The rotor used for this calculation, as well as the respective meshes, are reported [10]. This rotor was optimized to maximize the total-static efficiency for the design condition α 1 = 30 o, the same angle used to analyze the turbine stators. All the 5 optimized stator configurations were simulated with this rotor. The computational domain is defined by: 2 stators (inlet and exit) and 1 rotor, assuming periodic boundaries (see Fig. 14). The periodicity of the rotor and stators domains are different due to number of blades (11 rotor blades to 57 circumferential stator blade sets). The Mixing Plane model [11] was then used to compute the quantities between domains interfaces. Two rotor connection block were used to avoid intense gradients at the mixing plane. A moving reference frame [11] was used to compute the flow through the rotor. The rotor rotation speed Ω was set to rpm, which respects the full scale Reynolds number of Re = for a rotor diameter of 1.5 m [12] and turbine flow rate Q = 37.1 m 3 /s. The atmospheric static pressure is imposed as boundary condition at the exit surface of the domain. All computations are performed assuming steady incompressible flow. 8
9 1 st cascade 2 nd cascade Inlet stator Outlet stator Rotor Periodic surface Rotor connection block turbine torque), Ω is the rotation speed, D is the rotor diameter and p is the pressure head (difference between the turbine inlet total pressure and the exit average static pressure). Rotor blade Figure 14: Turbine computational domain. 80% 75% 70% Z R =1 Z R =2 Z R = Results As expected, Fig. 15 shows that boundary layer on the nozzle walls has a significant effect on the axial distribution of the angle of the absolute flow at the rotor entry. Nevertheless the results indicate that flow incidence to the rotor blades is small in the approximately 60% of the channel height. η 65% 60% 55% 50% Φ Figure 16: Turbine efficiency versus dimensionless flow rate, for systems of 1, 2 and 3 cascades optimized for α 2 = 90 o. 50% 40% 80% 75% 70% α 2 = 65 α 2 = 90 α 2 = 115 Channel height 30% 20% 10% η 65% 60% 55% 50% Φ 0% α 1 [ ] Figure 15: Profile of angle α 1, for the system of 2 cascades optimized for α 2 = 90 o. The turbine total-static efficiency η and the dimensionless flow coefficient Φ plotted in Figs are defined as η = P Q p, (6) Φ = Q ΩD. (7) 3 Here, Q is the volume flow rate, P is the turbine power output (P = ΩT, T as the 9 Figure 17: Turbine efficiency versus dimensionless flow rate, for systems of 2 cascades optimized for α 2 = 90 ± 25 o. For all configurations, the peak efficiencies are very close to the rotor design condition (Φ = 0.19). The large efficiency drop verified for smaller flow rate coefficients is caused by the effect of high negative flow incidence to the rotor blades, and due to the large misalignment between the flow direction and the downstream stator blades (see Fig.18). The smooth efficiency drop for the higher flow rate coefficients is caused by the combined effect of the positive flow
10 incidence to the rotor blades, and the pressure loss in the downstream stator, which is proportional to the square of the flow rate coefficient. α 2 [ ] Z R =1; α 2 = 90 Z R =2; α 2 = 90 Z R =3; α 2 = 90 Z R =2; α 2 = 65 Z R =2; α 2 = Φ Figure 18: Rotor exit angle versus dimensionless flow rate, for all configurations. 8. Conclusions A new stator blades design was presented for the biradial turbine. Several stator configurations were tested in order to evaluate the effect of the number of cascades. The implementation of multiple cascades increased the turbine performance due to the reduction of the downstream stator flow obstruction. Results of numerical flow calculations indicate a total-static peak efficient of 76% for the Z R = 2 configuration, optimized for α 2 = 65 o. This may be compared with the corresponding numerical results for the axially movable guide-vanes biradial turbine [12], which gave 83%. References [1] Luis Trigo. Kymaner presentation - The OWC option. files/04_luis_trigo_kymaner.pdf. Accessed: [2] WavEC - Offshore Renewables. Seminar and B2B meetings "Powering the future - Marine energy opportunities". energy_2009#.vxknuvyrlck. Accessed: [3] AFO Falcao, LMC Gato, and EPAS Nunes. A novel radial self-rectifying air turbine for use in wave energy converters. part 2. results from model testing. Renewable Energy, 53: , [4] J.C.C. Henriques and L.M.C. Gato - Optimization of the guide-vanes of a self-rectifyng biradial turbine, Technical report, IST, [5] T. M. Q. Candeias. Numerial optimization of the upstream stator blades of a self-rectifying biradial turbine. Master s thesis, IST - Technical University of Lisbon, [6] Rainer Storn and Kenneth Price. Differential evolution a simple and efficient heuristic for global optimization over continuous spaces. Journal of global optimization, 11(4): , [7] Ira Herbert Abbott and Albert Edward Von Doenhoff. Theory of wing sections, including a summary of airfoil data. Courier Corporation, [8] Harry L Morgan Jr. A computer program for the analysis of multielement airfoils in twodimensional subsonic, viscous flow. In Aerodynamic Analyses Requiring Advanced Computers, volume 347, page 713, [9] J-D Muller, Philip L Roe, and H Deconinck. A frontal approach for internal node generation in Delaunay triangulations. International Journal for Numerical Methods in Fluids, 17(3): , [10] D. N. Ferreira - Rotor optimization for the self-rectifying biradial air turbine, Technical report, IST/IDMEC, [11] Fluent-Inc. Fluent 6.3 users guide. Fluent documentation, [12] A F O Falcao, LMC Gato, and EPAS Nunes. A novel radial self-rectifying air turbine for use in wave energy converters. Renewable Energy, 50: ,
Axisymmetric 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 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 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 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 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 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 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 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 informationStudy on the Design Method of Impeller on Low Specific Speed Centrifugal Pump
Send Orders for Reprints to reprints@benthamscience.ae 594 The Open Mechanical Engineering Journal, 2015, 9, 594-600 Open Access Study on the Design Method of Impeller on Low Specific Speed Centrifugal
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 informationNUMERICAL ANALYSIS OF CENTRIFUGAL PUMP IMPELLER FOR PERFORMANCE IMPROVEMENT
Int. J. Chem. Sci.: 14(2), 2016, 1148-1156 ISSN 0972-768X www.sadgurupublications.com NUMERICAL ANALYSIS OF CENTRIFUGAL PUMP IMPELLER FOR PERFORMANCE IMPROVEMENT S. KALIAPPAN, M. D. RAJKAMAL and D. BALAMURALI
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 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 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 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 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 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 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 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 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 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 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 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 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 informationMicrowell Mixing with Surface Tension
Microwell Mixing with Surface Tension Nick Cox Supervised by Professor Bruce Finlayson University of Washington Department of Chemical Engineering June 6, 2007 Abstract For many applications in the pharmaceutical
More informationLES Analysis on Shock-Vortex Ring Interaction
LES Analysis on Shock-Vortex Ring Interaction Yong Yang Jie Tang Chaoqun Liu Technical Report 2015-08 http://www.uta.edu/math/preprint/ LES Analysis on Shock-Vortex Ring Interaction Yong Yang 1, Jie Tang
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 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 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 informationComputation of Velocity, Pressure and Temperature Distributions near a Stagnation Point in Planar Laminar Viscous Incompressible Flow
Excerpt from the Proceedings of the COMSOL Conference 8 Boston Computation of Velocity, Pressure and Temperature Distributions near a Stagnation Point in Planar Laminar Viscous Incompressible Flow E. Kaufman
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 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 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 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 informationCompressible Flow in a Nozzle
SPC 407 Supersonic & Hypersonic Fluid Dynamics Ansys Fluent Tutorial 1 Compressible Flow in a Nozzle Ahmed M Nagib Elmekawy, PhD, P.E. Problem Specification Consider air flowing at high-speed through a
More informationOptimization of Hydraulic Fluid Parameters in Automotive Torque Converters
Optimization of Hydraulic Fluid Parameters in Automotive Torque Converters S. Venkateswaran, and C. Mallika Parveen Abstract The fluid flow and the properties of the hydraulic fluid inside a torque converter
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 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 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 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 informationInfluence of Geometric Scaling on Linear Cascade Aerodynamic Performance
Available online at www.sciencedirect.com ScienceDirect Procedia Engineering 00 (2014) 000 000 www.elsevier.com/locate/procedia APISAT2014, 2014 Asia-Pacific International Symposium on Aerospace Technology,
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 informationHYDRAULIC DEVELOPMENT OF A CENTRIFUGAL PUMP IMPELLER USING THE AGILE TURBOMACHINERY DESIGN SYSTEM
HYDRAULIC DEVELOPMENT OF A CENTRIFUGAL PUMP IMPELLER USING THE AGILE TURBOMACHINERY DESIGN SYSTEM Krzysztof Denus CTD Technology ñ Ing. Buro Denus Colin Osborne Concepts NREC 1. INTRODUCTION The impeller
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 informationCalculate a solution using the pressure-based coupled solver.
Tutorial 19. Modeling Cavitation Introduction This tutorial examines the pressure-driven cavitating flow of water through a sharpedged orifice. This is a typical configuration in fuel injectors, and brings
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 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 informationAnalysis of Flow Dynamics of an Incompressible Viscous Fluid in a Channel
Analysis of Flow Dynamics of an Incompressible Viscous Fluid in a Channel Deepak Kumar Assistant Professor, Department of Mechanical Engineering, Amity University Gurgaon, India E-mail: deepak209476@gmail.com
More informationEnhancement of a large injection system for steam turbines
GE Oil & Gas Leonardo Nettis, GE Oil & Gas Enzo Imparato, GE Oil & Gas Lorenzo Cosi, GE Oil & Gas DOWNSTREAM TECHNOLOGY SOLUTIONS PRODUCTS & SERVICES Enhancement of a large injection system for steam turbines
More informationNon Axisymmetric Hub Design Optimization for a High Pressure Compressor Rotor Blade
Non Axisymmetric Hub Design Optimization for a High Pressure Compressor Rotor Blade Vicky Iliopoulou, Ingrid Lepot, Ash Mahajan, Cenaero Framework Target: Reduction of pollution and noise Means: 1. Advanced
More informationSimulation of Turbulent Flow in an Asymmetric Diffuser
Simulation of Turbulent Flow in an Asymmetric Diffuser 1. Purpose 58:160 Intermediate Mechanics of Fluids CFD LAB 3 By Tao Xing and Fred Stern IIHR-Hydroscience & Engineering The University of Iowa C.
More informationDimensioning and Airflow Simulation of the Wing of an Ultralight Aircraft
Dimensioning and Airflow Simulation of the Wing of an Ultralight Aircraft Richárd Molnár 1 Gergely Dezső 2* Abstract: Increasing interest to ultralight aircrafts usually made of composite materials leads
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 informationAEROELASTICITY IN AXIAL FLOW TURBOMACHINES
von Karman Institute for Fluid Dynamics Lecture Series Programme 1998-99 AEROELASTICITY IN AXIAL FLOW TURBOMACHINES May 3-7, 1999 Rhode-Saint- Genèse Belgium CASE STUDIES IN TURBOMACHINERY AEROELASTICITY
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 informationInvestigation of the critical submergence at pump intakes based on multiphase CFD calculations
Advances in Fluid Mechanics X 143 Investigation of the critical submergence at pump intakes based on multiphase CFD calculations P. Pandazis & F. Blömeling TÜV NORD SysTec GmbH and Co. KG, Germany Abstract
More informationAdvanced Turbomachinery Methods. Brad Hutchinson ANSYS, Inc. Industry Marketing
Advanced Turbomachinery Methods 1 Brad Hutchinson ANSYS, Inc. Industry Marketing Presentation Overview 1. Turbomachinery challenges 2. ANSYS TurboSystem 3. 2 Blade row fluid dynamics solution methods Available
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 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 informationDesign and Optimization of Contra-Rotating Fans
Abstract Axial, contra-rotating fans can be one solution for compact, efficient, powerful air movement technology especially if the speed of each Impeller can be controlled independently. No additional
More informationAIRFOIL SHAPE OPTIMIZATION USING EVOLUTIONARY ALGORITHMS
AIRFOIL SHAPE OPTIMIZATION USING EVOLUTIONARY ALGORITHMS Emre Alpman Graduate Research Assistant Aerospace Engineering Department Pennstate University University Park, PA, 6802 Abstract A new methodology
More informationCFD ANALYSIS Of COMBINED 8-12 STAGES Of INTERMIDIATE PRESSURE STEAM TURBINE
CFD ANALYSIS Of COMBINED 8-12 STAGES Of INTERMIDIATE PRESSURE STEAM TURBINE 1st Author name : SHIVAKUMAR VASMATE, 2nd Author name : KAMALADEVI ANANDE. 1 Department of Mechanical Engineering, India 2 Department
More informationParametric design of a Francis turbine runner by means of a three-dimensional inverse design method
IOP Conference Series: Earth and Environmental Science Parametric design of a Francis turbine runner by means of a three-dimensional inverse design method To cite this article: K Daneshkah and M Zangeneh
More informationDesign optimization method for Francis turbine
IOP Conference Series: Earth and Environmental Science OPEN ACCESS Design optimization method for Francis turbine To cite this article: H Kawajiri et al 2014 IOP Conf. Ser.: Earth Environ. Sci. 22 012026
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 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 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 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 informationUse of CFD in Design and Development of R404A Reciprocating Compressor
Purdue University Purdue e-pubs International Compressor Engineering Conference School of Mechanical Engineering 2006 Use of CFD in Design and Development of R404A Reciprocating Compressor Yogesh V. Birari
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 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 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 informationNUMERICAL STUDY OF CAVITATING FLOW INSIDE A FLUSH VALVE
Conference on Modelling Fluid Flow (CMFF 09) The 14th International Conference on Fluid Flow Technologies Budapest, Hungary, September 9-12, 2009 NUMERICAL STUDY OF CAVITATING FLOW INSIDE A FLUSH VALVE
More informationNUMERICAL INVESTIGATION OF THE FLOW BEHAVIOR INTO THE INLET GUIDE VANE SYSTEM (IGV)
University of West Bohemia» Department of Power System Engineering NUMERICAL INVESTIGATION OF THE FLOW BEHAVIOR INTO THE INLET GUIDE VANE SYSTEM (IGV) Publication was supported by project: Budování excelentního
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 informationA Comparative CFD Analysis of a Journal Bearing with a Microgroove on the Shaft & Journal
Proceedings of International Conference on Innovation & Research in Technology for Sustainable Development (ICIRT 2012), 01-03 November 2012 182 A Comparative CFD Analysis of a Journal Bearing with a Microgroove
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 informationCFD design tool for industrial applications
Sixth LACCEI International Latin American and Caribbean Conference for Engineering and Technology (LACCEI 2008) Partnering to Success: Engineering, Education, Research and Development June 4 June 6 2008,
More informationAERODYNAMIC DESIGN OF FLYING WING WITH EMPHASIS ON HIGH WING LOADING
AERODYNAMIC DESIGN OF FLYING WING WITH EMPHASIS ON HIGH WING LOADING M. Figat Warsaw University of Technology Keywords: Aerodynamic design, CFD Abstract This paper presents an aerodynamic design process
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 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 informationFlow Field Analysis of Turbine Blade Modeling Based on CFX-Blade Gen
Flow Field Analysis of Turbine Blade Modeling Based on CFX-Blade Gen Liguang Wang 1, 2, a, *, Zhijun Li 1, 2, b, Yu Wang 1, 2, c, Baolin Liu 1, 2, Qin Zhou 1, 2 1 School of Engineering and Technology,
More informationISSN(PRINT): ,(ONLINE): ,VOLUME-1,ISSUE-1,
NUMERICAL ANALYSIS OF THE TUBE BANK PRESSURE DROP OF A SHELL AND TUBE HEAT EXCHANGER Kartik Ajugia, Kunal Bhavsar Lecturer, Mechanical Department, SJCET Mumbai University, Maharashtra Assistant Professor,
More informationAdvanced Computation in the design and development of aircraft engines. Serge Eury SNECMA
Advanced Computation in the design and development of aircraft engines 1 Serge Eury SNECMA Advanced Computation in the design and development of aircraft engines Introduction Some examples Conclusions
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 informationComputational Fluid Dynamics (CFD) for Built Environment
Computational Fluid Dynamics (CFD) for Built Environment Seminar 4 (For ASHRAE Members) Date: Sunday 20th March 2016 Time: 18:30-21:00 Venue: Millennium Hotel Sponsored by: ASHRAE Oryx Chapter Dr. Ahmad
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 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 informationAN INVESTIGATION TO IMPROVE GAS TURBINE ENGINE PERFORMANCE THROUGH THE USE OF SPLITTERED ROTORS
AN INVESTIGATION TO IMPROVE GAS TURBINE ENGINE PERFORMANCE THROUGH THE USE OF SPLITTERED ROTORS JONATHAN McGLUMPHY, Graduate Researcher DR. WING FAI-NG, Research Advisor Department of Mechanical Engineering
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 informationTutorial 17. Using the Mixture and Eulerian Multiphase Models
Tutorial 17. Using the Mixture and Eulerian Multiphase Models Introduction: This tutorial examines the flow of water and air in a tee junction. First you will solve the problem using the less computationally-intensive
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 informationLecture 2.2 Cubic Splines
Lecture. Cubic Splines Cubic Spline The equation for a single parametric cubic spline segment is given by 4 i t Bit t t t i (..) where t and t are the parameter values at the beginning and end of the segment.
More informationTHE INFLUENCE OF ROTATING DOMAIN SIZE IN A ROTATING FRAME OF REFERENCE APPROACH FOR SIMULATION OF ROTATING IMPELLER IN A MIXING VESSEL
Journal of Engineering Science and Technology Vol. 2, No. 2 (2007) 126-138 School of Engineering, Taylor s University College THE INFLUENCE OF ROTATING DOMAIN SIZE IN A ROTATING FRAME OF REFERENCE APPROACH
More informationDevelopment of Hybrid Fluid Jet / Float Polishing Process
COMSOL Conference - Tokyo 2013 Development of Hybrid Fluid Jet / Float Polishing Process A. Beaucamp, Y. Namba Dept. of Mechanical Engineering, Chubu University, Japan Zeeko LTD, United Kingdom Research
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 informationNumerical Modeling Study for Fish Screen at River Intake Channel ; PH (505) ; FAX (505) ;
Numerical Modeling Study for Fish Screen at River Intake Channel Jungseok Ho 1, Leslie Hanna 2, Brent Mefford 3, and Julie Coonrod 4 1 Department of Civil Engineering, University of New Mexico, Albuquerque,
More informationA Comparison of Panel Method and RANS Calculations for a Ducted Propeller System in Open-Water
Third International Symposium on Marine Propulsors smp 13, Launceston, Tasmania, Australia, May 2013 A Comparison of Panel Method and RANS Calculations for a Ducted Propeller System in Open-Water J. Baltazar
More informationSolved with COMSOL Multiphysics 4.0a. COPYRIGHT 2010 COMSOL AB.
Journal Bearing Introduction Journal bearings are used to carry radial loads, for example, to support a rotating shaft. A simple journal bearing consists of two rigid cylinders. The outer cylinder (bearing)
More informationCFD studies of a 10 MW turbine equipped with trailing edge flaps
CFD studies of a 10 MW turbine equipped with trailing edge flaps 10th EAWE PhD Seminar on Wind Energy in Europe 28-31 October 2014, Orléans, France Dipl.-Ing. Eva Jost e.jost@iag.uni-stuttgart.de Overview
More information