NUMERICAL SIMULATION AND EXPERIMENTAL INVESTIGATION OF THE FLOW IN AN AXIAL TURBINE
|
|
- Virgil Bishop
- 6 years ago
- Views:
Transcription
1 IAHR OCTOBER 27-31, FOZ DO IGUASSU RESERVED TO IAHR NUMERICAL SIMULATION AND EXPERIMENTAL INVESTIGATION OF THE FLOW IN AN AXIAL TURBINE J.-M. Gagnon, C. Deschênes, G.D. Ciocan, M. Iliescu LAMH, 1065, avenue de la médecine, Québec, Canada, G1V 0A6, Canada (418) jean-mathieu.gagnon.1@ulaval.ca ABSTRACT In this paper, a numerical simulation of the flow in a complete model of an axial turbine is performed to investigate circumferential non-uniformities in the distributor and at stay vanes inlet. This phenomenon is of prime importance since it is directly related to torque and power fluctuations of the runner output. Simulations involving a distributor section of the hydraulic machine cannot assess the non-uniformities that mainly take place in the admission channel and spiral casing. Therefore, the admission, distributor and draft tube sections of the model axial turbine are meshed and combined via general grid interfaces for complete machine simulations. Design and off-design operating conditions are simulated with a standard k-epsilon turbulence model and stationary RANS equations. Circumferential non-uniformities of the flow field and effect on stay vanes are investigated for the different operating regimes. Analyses for the conical diffuser are done for sections that have been measured experimentally and where information on the flow field is available. Then, simulations are compared for the different cross sections against experimental results. 3-D PIV and 2-D LDV investigations give insight on the accuracy of the numerical simulations of the flow fields. It is shown that the region near the admission pile has a different velocity distribution than the region away from the pile in the semispiral casing. This indicates non-uniformity at the distributor inlet that may propagate downstream in the runner. Further investigation with 2-D LDV and simulated cases at the runner outlet shows that the vortex rope is playing an important role in the flow rates for different quadrants of the machine. This study took place within the Consortium on Hydraulic Machines held at the Hydraulic Machinery Laboratory of Laval University. KEY WORDS: axial turbine, circumferential non-uniformities, stereo PIV, 2-D LDV, velocity profile, cone, draft tube.
2 INTRODUCTION It is not obvious to determine whether circumferential non-uniformities of the flow at the cone outlet section originate from the spiral casing or from the draft tube pile of a hydraulic machine. There is a strong acceleration of the flow in the distributor and runner that acts as a mixing device enforcing diffusion and stretching of velocity gradients. Furthermore, laser measurements such as PIV or LDV after the guide vanes and at the runner inlet section are not an easy task to perform because of visual obstruction from the stay vanes, guide vanes and upper distributor that limit optical access. Numerical simulation of the flow is an interesting way to investigate azimuthal non-uniformity phenomena. However, some practical considerations must be taken, in order to prevent a time consuming experience that would give no results on non-uniformities. First, complete machine simulations are necessary to initiate the non-uniformities in the spiral casing and at the outlet of the runner since the admission and the draft tube channel are the main actors of the phenomena [1]. Second, grid and interface should be carefully built and placed to avoid the dampening effect brought on by non-conformal mesh at mating surfaces and accelerating flow [2, 3]. This paper presents a methodology that combines numerical simulations and experimental measurements to study flow phenomena in an axial hydraulic turbine. 2-D LDV and 3-D PIV measurements are presented for two operating points and compared with stationary numerical simulations. METHODOLOGY 2-D LDV AND 3-D PIV MEASUREMENTS 2-D LDV and stereo PIV measurements are done in the conical diffuser of the hydraulic machine and illustrated in Fig. 1 below. Figure 1. LDV measurement setup (left) and stereo PIV setup (right) at the runner outlet section of the axial hydraulic machine model. Details of measurement techniques can be found in [4]. In this paper, further azimuthal positions were studied with 2-D LDV to assess circumferential nonuniformities of the flow at the runner outlet. Fig. 2 shows the global coordinates system 2
3 with investigated axes. Axis 5a, 5b and 5c correspond to three vertical optical accesses. These accesses were then rotated with the cone to allow measurements at different circumferential positions as illustrated on the right of the figure. Obstruction from the lower distributor casing limits measurements to Axis 5b and 5c for circumferential positions 1 and 3. Distributor Oz Admission Circumferential positions Z ref Ox Cone O Axis 5a Axis 5b Axis 5c Draft tube 2D-LDV Probe Ox Cone 60 Oy Figure 2. Global coordinates system and axis vertical and circumferential positions. Stereo PIV measurements are made for a plane at the runner outlet that is orthogonal to circumferential position 2 of LDV measurements. NUMERICAL SIMULATIONS The commercial solver ANSYS CFX was run on parallel processors for all simulations. In Fig. 3, the hydraulic machine geometry and mesh are split into four domains: the admission channel including 24 stay vanes (1), the distributor (2), the runner (3) and the draft tube (4) Interface Figure 3. - Left. Domains definition. Right. Tetra and o-grid meshes around stay vanes, spiral tongue and guide vanes with the interface limit (dashed line). A total of 3,700,000 elements are needed to respect a good aspect ratio in near wall elements. This is important to ensure good accuracy when switching from wall laws to 3
4 the k-epsilon turbulence model. Tetra meshing is used in the admission domain whereas block structured meshes and an o-grid are used in the other domains. Boundary conditions are a steady flow rate at the inlet and zero average static pressure at the draft tube outlet. Grid interfaces are needed to connect meshes from adjacent domains. For steady simulations, it is possible to use a standard grid interface or a circumferential averaging grid interface that allows for connecting domains with different mating areas. Both types of interfaces are used for the runner. In the circumferential averaging case, a section presenting a single blade (out of 6 for the runner) is used to limit the runner mesh size. A total of four simulations were done to compare two operating points and two interface types with LDV and PIV measurements. The chosen turbine regimes were optimum and overload conditions with respective guide vane opening angles of α=33 and α=38 degrees. Convergence of simulations is assumed when the hydraulic efficiency reaches a constant asymptotic value. For each domain, momentum and pressure equation residuals drop under rms values except for the draft tube where residual reaches The global machine RMS residuals are therefore limited to for all simulations. Specific draft tube flow phenomena with different time scales are supposed to be at the source of this low convergence. In the post-processing step, planes are built at the same location as the LDV axes presented in Fig. 2 and are used for comparisons in the following section. ANALYSIS ADMISSION AND DISTRIBUTOR Numerical simulations are used to assess flow non-uniformities in the admission duct and distributor. Figure 4 shows the location of the planes utilized for non-uniformity analysis. Plane 1 Plane 2 Figure 4. Planes location for analysis of admission and distributor. Static pressure results on plane 2 at overload condition for both types of interface are illustrated in figure 5. Plane 2 is a XY plane located at 75% height in the distributor section. One should note that there is almost no difference between left and right figures 4
5 except a slightly higher pressure level for simulations at left without averaging interface. The higher pressure on the third quadrant of the distributor plane (top right of planes) indicates pressure non-uniformity in the spiral casing. This non-uniformity originates from one of the channels and is clearly visible from the velocity contour and flow angle of Fig. 6 and left of Fig. 7 where the angle starts from the positive x axis. Integration of the outflow velocity over the area of Plane 1 for each admission channel shows that there is 11% more flow passing in the left channel on the y minus side. P/Pref 3 rd quadrant P/Pref 3 rd quadrant x y Figure 5. Static pressure contour at overload condition for general interface (left) and averaging interface simulations (right). Figure 6. X Velocity contour inside the admission channels at Plane 2. Normalized static pressure corresponding to Fig. 5 is shown in Fig. 7 right. Navg and OLavg acronyms of the legend stand respectively for simulations with the averaging interface at nominal and overload turbine operation. Figure 7. Velocity flow angle and normalized static pressure in the distributor for all four simulation cases. 5
6 From admission and distributor results, it is clear that flow non-uniformities are initiated at the admission duct and are induced by pressure effect. Global pressure effects are reflected in the upstream and downstream flows from the distributor casing by the elliptic nature of the equations. Simulations with the admission and distributor alone have been made and also showed non-uniformities in the distributor section. This leads us to the conclusion that non-uniformities taking place in these two components are build up within them and they do not originate from draft tube or runner pressure effect. The next section will assess azimuthal non-uniformities in the conical diffuser of the hydraulic machine. RUNNER OUTLET Easy optical accesses implementation in the cone of the hydraulic turbine model allowed measuring the flow with PIV and LDV [5]. Comparisons with numerical results give good assesments of the flow behavior as well as quality of simulations. Axial and circumferential averaged velocity profiles at Axis 5b, 5c and at the circumferential position 2 (ref. Fig. 2) are shown in Fig. 8 for both operating points. Exp Num. Exp Num. Exp Num. Exp Num. Figure 8. Axial and circumferential velocity profile comparisons between 2-D LDV measurements and numerical simulations. Even though the velocity amplitude is not perfectly matched to the measurements, the shape and flow behavior is respected for the operating points investigated. In Fig. 9, notice that the azimuthal non-uniformity of the flow is concentrated at half axis 4 6
7 presenting the highest axial velocity differences with respectively 13% and 12% for Axis 5b and Axis 5c Figure 9. Velocity difference compared to crown averaged velocity for Axis 5b and 5c at overload condition. Comparison of the interpolated measured profiles for all operating points and axes is illustrated below. The right color bars show the amplitude of the velocity and qualitative level may be appreciated from the surface plot. Figure 10. Interpolated axial and circumferential velocity profiles for all axes and operating conditions. 7
8 There is not much variation of the velocity amplitude between Axis 5b and 5c. The main differences occur in the circumferential velocity profile of the top and bottom right surfaces, when passing from nominal regime to overload condition. In that case, circumferential velocity tends to increase in the center of the cone as the vortex rope increases in strength. It is hard to infer a clear conclusion on the behavior of the nonuniformity from steady numerical simulations since the vortex rope may take a particular quadrant at the runner outlet. This situation is illustrated in Fig. 10 where the integration of the flow would give biased results for half axis positions 5 and 6 of the simulated case on the right. Unsteady simulations are needed to resolve the unsteady vortex rope precession and flow non-uniformities associated with the averaged velocity profile. Vortex in the 4 th quadrant Figure 11. Experimental velocity contour (left) and simulated results (right) for the axial velocity at overload condition, α=38, Axis 5c. The experimental averaged velocity profile on the left gives same results as the axial flow in Fig. 9, with a slightly darker color in the third quadrant indicating a higher velocity. The stereo PIV plane is located in the cone past the runner hub and the comparison of the measurements and simulations for the steady circumferential and axial velocity is made at nominal condition in Fig. 12 and Fig. 13. Measurements CFD Hub Hub Figure 12. Circumferential velocity obtained from measurements (left) and simulated (right). 8
9 Hub Hub Figure 13. Radial velocity at runner outlet. Left) Measurements. Right) Simulations. One should note that the velocity amplitudes defined by the colour bars on the right of the simulations match the measurements well. Contours at zero value have been added to all plots to show reversing velocity regions. The radial velocity zero contour plot of Fig. 13 illustrates regions of shear layer mixing and diffusion from blade tip vortices. The velocity distributions in Fig. 12 and Fig. 13 are consistent with the evolution of the stall flow region evidenced on the axial velocity profiles in Fig. 8 top left. The circumferential velocity also indicates the presence of a weak forced vortex near the axis, consistent with the statements in reference [6]. In the experimental case at bottom left, this region moves towards the axis and reaches the centerline at about z/zref= In the simulation case, the same region stays close to the wall and indicates less diffusion and mixing of the blade tip vortex. This phenomenon may be induced either by the mesh, that is changing from the runner to draft tube domains, or by the interface, which needs interpolation and reference frame changes within the solver. The radial and axial perturbation of the vortex core is also shown by the shear layer presence near the diffuser axis. The zero contours of the circumferential and radial velocities crossing the axis illustrate the instability of the forced vortex core. CONCLUSION This paper presents a methodology to assess non-uniformity of the flow in an axial hydraulic turbine. The 3-D PIV and 2-D LDV measurements are compared and analyzed with simulations for two operating conditions. It is found that measured and simulated results match and allow studying circumferential non-uniformities of the flow. However, the steady simulation results exposed in the paper should be taken with care since the vortex rope takes a specific configuration that reduced the axial velocity and flow rates in one quadrant of the hydraulic machine. Finally, the PIV analysis has shown that the interface or mesh has a strong impact on radial velocity distribution. It is most probable that a finer mesh or a different interface location would be needed to account for blade tip vortices and radial velocity diffusion. 9
10 ACKNOWLEDGMENTS The authors would like to thank all the partners of the Consortium on Hydraulic Machines. Special thanks to Hydro-Quebec, Alstom Hydro Canada, Voith Siemens, Va Tech Hydro, CVG Edelca, NRCan, for their support and contribution to this research project. The Canadian Natural Sciences and Engineering Research Council also provided funding for this research. REFERENCES [1] MUNTEAN, S., BALINT, D., SUSAN-RESIGA, R. ANTON and I., DARZAN, C. (2004), 3D Flow analysis in the spiral case and distributor of a Kaplan turbine, 22 nd IAHR Symposium on Hydraulic Machinery and Systems, Stockholm, Sweden [2] GAGNON J.-M., CIOCAN G.D, DESCHÊNES C., ILIESCU M. (2008), "Numerical and Experimental Investigation of Rotor-Stator Interactions in an Axial Turbine: Numerical Interface Assessement", ASME 2008 Fluids Engineering Divisin Summer Meeting, Jacksonville, Florida, USA, August 10-14, FEDSM [3] ANSYS CFX v11.0: Solver Theory Guide [4] GAGNON J.-M., ILIESCU M., CIOCAN G.D, DESCHÊNES C. (2008), Experimental investigation of runner outlet flow in axial turbine with LDV and stereoscopic PIV, 24 nd IAHR Symposium on Hydraulic Machinery and Systems, accepted for publication, Foz do Iguassu, Brazil [5] CIOCAN, G.D., AVELLAN F. and KUENY J.L. (2000), Optical Measurement Techniques for Experimental Analysis of Hydraulic Turbines Rotor-Stator Interaction, Proceeding of the ASME 2000 Fluids Engineering Division Summer Meeting, Boston, MA. [6] BETTOCCHI R., CANTORE L., MAGRI L. and UBALDI M. (1982), Experimental analysis of the flow in the axial region of propeller-turbine admission ducts La Houille Blanche, 7/8 10
Two-way coupled fluid structure interaction simulation of a propeller turbine
IOP Conference Series: Earth and Environmental Science Two-way coupled fluid structure interaction simulation of a propeller turbine To cite this article: H Schmucker et al 2010 IOP Conf. Ser.: Earth Environ.
More informationSimulations of the vortex in the Dellenback abrupt expansion, resembling a hydro turbine draft tube operating at part-load
Simulations of the vortex in the Dellenback abrupt expansion, resembling a hydro turbine draft tube operating at part-load H Nilsson Chalmers University of Technology, SE-412 96 Gothenburg, Sweden E-mail:
More informationUnsteady numerical simulation of the flow in the U9 Kaplan turbine model
IOP Conference Series: Earth and Environmental Science OPEN ACCESS Unsteady numerical simulation of the flow in the U9 Kaplan turbine model To cite this article: Ardalan Javadi and Håkan Nilsson 2014 IOP
More informationLife time assessment and plant operation optimization based on geometry scan and strain gauge testing START/STOP optimization
IGHEM 2014 The 10 th International conference on hydraulic efficiency measurements Itajuba, Brasil September 16 th - 18 th, 2014 XXXXXX Life time assessment and plant operation optimization based on geometry
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 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 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 informationThe ERCOFTAC centrifugal pump OpenFOAM case-study
3 rd IAHR International Meeting of the Workgroup on Cavitation and Dynamic Problems in Hydraulic Machinery and Systems, October 14-16, 009, Brno, Czech Republic The ERCOFTAC centrifugal pump OpenFOAM case-study
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 informationThe effect of runner cone design on pressure oscillation characteristics in a Francis hydraulic turbine
137 The effect of runner cone design on pressure oscillation characteristics in a Francis hydraulic turbine Z D Qian 1 *,WLi 1, W X Huai 1, and YLWu 2 1 State Key Laboratory of Water Resources and Hydropower
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 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 informationComparison of a two-dimensional viscid and inviscid model for rotating stall analysis
Comparison of a two-dimensional viscid and inviscid model for rotating stall analysis S. LJEVAR, H.C. DE LANGE, A.A. VAN STEENHOVEN Department of Mechanical Engineering Eindhoven University of Technology
More informationTurbine-99 unsteady simulations Validation
IOP Conference Series: Earth and Environmental Science Turbine-99 unsteady simulations Validation To cite this article: M J Cervantes et al 2010 IOP Conf. Ser.: Earth Environ. Sci. 12 012014 View the article
More informationEvaluation of an improved mixing plane interface for OpenFOAM
IOP Conference Series: Earth and Environmental Science OPEN ACCESS Evaluation of an improved mixing plane interface for OpenFOAM To cite this article: M Beaudoin et al 2014 IOP Conf. Ser.: Earth Environ.
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 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 informationDetermination of turbine runner dynamic behaviour under operating condition by a two-way staggered fluid-structureinteraction method
IOP Conference Series: Earth and Environmental Science Determination of turbine runner dynamic behaviour under operating condition by a two-way staggered fluid-structureinteraction method To cite this
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 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 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 informationVerification of Laminar and Validation of Turbulent Pipe Flows
1 Verification of Laminar and Validation of Turbulent Pipe Flows 1. Purpose ME:5160 Intermediate Mechanics of Fluids CFD LAB 1 (ANSYS 18.1; Last Updated: Aug. 1, 2017) By Timur Dogan, Michael Conger, Dong-Hwan
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 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 informationTurbocharger Design & Analysis Solutions. Bill Holmes Brad Hutchinson Detroit, October 2012
Turbocharger Design & Analysis Solutions Bill Holmes Brad Hutchinson Detroit, October 2012 Agenda ANSYS overview ANSYS TurboSystem Blade row solutions The ANSYS Transformation methods An example: turbocharger
More 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 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 informationOPTIMIZATION OF AXIAL HYDRAULIC TURBINES RUNNER BLADES USING HYDRODYNAMIC SIMULATION TECHNIQUES
Scientific Bulletin of the Politehnica University of Timisoara Transactions on Mechanics Special issue The 6 th International Conference on Hydraulic Machinery and Hydrodynamics Timisoara, Romania, October
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 informationSimulation of Laminar Pipe Flows
Simulation of Laminar Pipe Flows 57:020 Mechanics of Fluids and Transport Processes CFD PRELAB 1 By Timur Dogan, Michael Conger, Maysam Mousaviraad, Tao Xing and Fred Stern IIHR-Hydroscience & 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 informationRANS COMPUTATION OF RIBBED DUCT FLOW USING FLUENT AND COMPARING TO LES
RANS COMPUTATION OF RIBBED DUCT FLOW USING FLUENT AND COMPARING TO LES Máté M., Lohász +*& / Ákos Csécs + + Department of Fluid Mechanics, Budapest University of Technology and Economics, Budapest * Von
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 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 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 informationApplication of Homogeneous and Inhomogeneous Two-Phase Models to a Cavitating Tip Leakage Vortex on a NACA0009 Hydrofoil
Application of Homogeneous and Two-Phase Models to a Cavitating Tip Leakage Vortex on a NACA0009 Hydrofoil 1 Jonas Wack*; 1 Stefan Riedelbauch 1 University of Stuttgart, Germany Introduction Abstract Two-phase
More informationCFD Modeling of a Radiator Axial Fan for Air Flow Distribution
CFD Modeling of a Radiator Axial Fan for Air Flow Distribution S. Jain, and Y. Deshpande Abstract The fluid mechanics principle is used extensively in designing axial flow fans and their associated equipment.
More 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 informationNumerical analysis of the tip and root vortex position in the wake of a wind turbine
Journal of Physics: Conference Series Numerical analysis of the tip and root vortex position in the wake of a wind turbine To cite this article: S Ivanell et al 2007 J. Phys.: Conf. Ser. 75 012035 View
More informationProceedings of the ASME 2011 International Mechanical Engineering Congress & Exposition IMECE2011 November 11-17, 2011, Denver, Colorado, USA
Proceedings of the ASME 2011 International Mechanical Engineering Congress & Exposition IMECE2011 November 11-17, 2011, Denver, Colorado, USA IMECE2011-65058 THE EFFECT OF BLADE LEAN, TWIST AND BOW ON
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 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 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 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 informationAdvances in Turbomachinery Simulation Fred Mendonça and material prepared by Chad Custer, Turbomachinery Technology Specialist
Advances in Turbomachinery Simulation Fred Mendonça and material prepared by Chad Custer, Turbomachinery Technology Specialist Usage From Across the Industry Outline Key Application Objectives Conjugate
More informationNumerical Modeling of Ship-Propeller Interaction under Self-Propulsion Condition
STAR Global Conference 2014 Vienna, Austria, March 17-19 Numerical Modeling of Ship-Propeller Interaction under Self-Propulsion Condition Vladimir Krasilnikov Department of Ship Technology, MARINTEK Trondheim,
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 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 Post-Processing of Rampressor Rotor Compressor
Gas Turbine Industrial Fellowship Program 2006 CFD Post-Processing of Rampressor Rotor Compressor Curtis Memory, Brigham Young niversity Ramgen Power Systems Mentor: Rob Steele I. Introduction Recent movements
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 informationCOMPUTATIONAL FLUID DYNAMICS USED IN THE DESIGN OF WATERBLAST TOOLING
2015 WJTA-IMCA Conference and Expo November 2-4 New Orleans, Louisiana Paper COMPUTATIONAL FLUID DYNAMICS USED IN THE DESIGN OF WATERBLAST TOOLING J. Schneider StoneAge, Inc. Durango, Colorado, U.S.A.
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 informationMultiphase flow metrology in oil and gas production: Case study of multiphase flow in horizontal tube
Multiphase flow metrology in oil and gas production: Case study of multiphase flow in horizontal tube Deliverable 5.1.2 of Work Package WP5 (Creating Impact) Authors: Stanislav Knotek Czech Metrology Institute
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 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 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 informationITTC Recommended Procedures and Guidelines
Page 1 of 9 Table of Contents 1. OVERVIEW... 2 2. CHOICE OF MODEL OR FULL SCALE... 2 3. NOMINAL WAKE IN MODEL SCALE... 3 3.1 Pre-processing... 3 3.1.1 Geometry... 3 3.1.2 Computational Domain and Boundary
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 informationVerification and Validation of Turbulent Flow around a Clark-Y Airfoil
1 Verification and Validation of Turbulent Flow around a Clark-Y Airfoil 1. Purpose ME:5160 Intermediate Mechanics of Fluids CFD LAB 2 (ANSYS 19.1; Last Updated: Aug. 7, 2018) By Timur Dogan, Michael Conger,
More informationHydro-elastic analysis of a propeller using CFD and FEM co-simulation
Fifth International Symposium on Marine Propulsors smp 17, Espoo, Finland, June 2017 Hydro-elastic analysis of a propeller using CFD and FEM co-simulation Vesa Nieminen 1 1 VTT Technical Research Centre
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 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 informationSimulation of Turbulent Flow over the Ahmed Body
Simulation of Turbulent Flow over the Ahmed Body 58:160 Intermediate Mechanics of Fluids CFD LAB 4 By Timur K. Dogan, Michael Conger, Maysam Mousaviraad, and Fred Stern IIHR-Hydroscience & Engineering
More informationPIV and LDV measurements behind a backward facing step
PIV and LDV measurements behind a backward facing step M.T. Pilloni, C. Schram, M.L. Riethmulle/^ ^ Mechanical Engineering Department, 09123 Cagliari, Italy ^ von Karman Institute for Fluid Dynamics, 1640
More informationIntroduction to C omputational F luid Dynamics. D. Murrin
Introduction to C omputational F luid Dynamics D. Murrin Computational fluid dynamics (CFD) is the science of predicting fluid flow, heat transfer, mass transfer, chemical reactions, and related phenomena
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 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 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 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 informationStream Function-Vorticity CFD Solver MAE 6263
Stream Function-Vorticity CFD Solver MAE 66 Charles O Neill April, 00 Abstract A finite difference CFD solver was developed for transient, two-dimensional Cartesian viscous flows. Flow parameters are solved
More informationCFD modelling of thickened tailings Final project report
26.11.2018 RESEM Remote sensing supporting surveillance and operation of mines CFD modelling of thickened tailings Final project report Lic.Sc.(Tech.) Reeta Tolonen and Docent Esa Muurinen University 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 informationModeling Evaporating Liquid Spray
Tutorial 17. Modeling Evaporating Liquid Spray Introduction In this tutorial, the air-blast atomizer model in ANSYS FLUENT is used to predict the behavior of an evaporating methanol spray. Initially, the
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 informationPutting the Spin in CFD
w h i t e p a p e r Putting the Spin in CFD insight S U M MARY Engineers who design equipment with rotating components need to analyze and understand the behavior of those components if they want to improve
More informationCFD-1. Introduction: What is CFD? T. J. Craft. Msc CFD-1. CFD: Computational Fluid Dynamics
School of Mechanical Aerospace and Civil Engineering CFD-1 T. J. Craft George Begg Building, C41 Msc CFD-1 Reading: J. Ferziger, M. Peric, Computational Methods for Fluid Dynamics H.K. Versteeg, W. Malalasekara,
More informationOpenFOAM for CFD in water power and for international collaboration
OpenFOAM for CFD in water power and for international collaboration ASSOCIATE PROFESSOR HÅKAN NILSSON Outline of the presentation: OpenFOAM for CFD in water power - Overview of flow in Hydro Power Stations
More informationWe are IntechOpen, the first native scientific publisher of Open Access books. International authors and editors. Our authors are among the TOP 1%
We are IntechOpen, the first native scientific publisher of Open Access books 3,350 108,000 1.7 M Open access books available International authors and editors Downloads Our authors are among the 151 Countries
More informationThree Dimensional Numerical Simulation of Turbulent Flow Over Spillways
Three Dimensional Numerical Simulation of Turbulent Flow Over Spillways Latif Bouhadji ASL-AQFlow Inc., Sidney, British Columbia, Canada Email: lbouhadji@aslenv.com ABSTRACT Turbulent flows over a spillway
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 informationCo-Simulation von Flownex und ANSYS CFX am Beispiel einer Verdrängermaschine
Co-Simulation von Flownex und ANSYS CFX am Beispiel einer Verdrängermaschine Benoit Bosc-Bierne, Dr. Andreas Spille-Kohoff, Farai Hetze CFX Berlin Software GmbH, Berlin Contents Positive displacement compressors
More informationInvestigation of mixing chamber for experimental FGD reactor
Investigation of mixing chamber for experimental FGD reactor Jan Novosád 1,a, Petra Danová 1 and Tomáš Vít 1 1 Department of Power Engineering Equipment, Faculty of Mechanical Engineering, Technical University
More informationEffects of bell mouth geometries on the flow rate of centrifugal blowers
Journal of Mechanical Science and Technology 25 (9) (2011) 2267~2276 www.springerlink.com/content/1738-494x DOI 10.1007/s12206-011-0609-3 Effects of bell mouth geometries on the flow rate of centrifugal
More informationDEVELOPMENT OF HIGH SPECIFIC SPEED FRANCIS TURBINE FOR LOW HEAD HPP
Engineering MECHANICS, Vol. 20, 2013, No. 2, p. 139 148 139 DEVELOPMENT OF HIGH SPECIFIC SPEED FRANCIS TURBINE FOR LOW HEAD HPP JiříObrovský*, Hana Krausová*, Jiří Špidla*, Josef Zouhar* Nowadays we can
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 informationOptimization of Appendages Using RANS-CFD-Methods
-Methods HENDRIK VORHOELTER, STEFAN KRUEGER, Hamburg University of Technology Numerical Towing Tank Symposium, Hamburg 2007 There has been a lot of development on RANS- CFD-methods in the past years. The
More informationWind Tunnel Validation of Computational Fluid Dynamics-Based Aero-Optics Model
Wind Tunnel Validation of Computational Fluid Dynamics-Based Aero-Optics Model D. Nahrstedt & Y-C Hsia, Boeing Directed Energy Systems E. Jumper & S. Gordeyev, University of Notre Dame J. Ceniceros, Boeing
More informationViscous/Potential Flow Coupling Study for Podded Propulsors
First International Symposium on Marine Propulsors smp 09, Trondheim, Norway, June 2009 Viscous/Potential Flow Coupling Study for Podded Propulsors Eren ÖZSU 1, Ali Can TAKİNACI 2, A.Yücel ODABAŞI 3 1
More informationExpress Introductory Training in ANSYS Fluent Workshop 06 Using Moving Reference Frames and Sliding Meshes
Express Introductory Training in ANSYS Fluent Workshop 06 Using Moving Reference Frames and Sliding Meshes Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School
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 informationS-ducts and Nozzles: STAR-CCM+ at the Propulsion Aerodynamics Workshop. Peter Burns, CD-adapco
S-ducts and Nozzles: STAR-CCM+ at the Propulsion Aerodynamics Workshop Peter Burns, CD-adapco Background The Propulsion Aerodynamics Workshop (PAW) has been held twice PAW01: 2012 at the 48 th AIAA JPC
More informationDetached-Eddy Simulation of a Linear Compressor Cascade with Tip Gap and Moving Wall *)
FOI, Stockholm, Sweden 14-15 July, 2005 Detached-Eddy Simulation of a Linear Compressor Cascade with Tip Gap and Moving Wall *) A. Garbaruk,, M. Shur, M. Strelets, and A. Travin *) Study is carried out
More informationThe Great Mystery of Theoretical Application to Fluid Flow in Rotating Flow Passage of Axial Flow Pump, Part I: Theoretical Analysis
Proceedings of the 2nd WSEAS Int. Conference on Applied and Theoretical Mechanics, Venice, Italy, November 20-22, 2006 228 The Great Mystery of Theoretical Application to Fluid Flow in Rotating Flow Passage
More informationCFD Verification and Investigation on Building Geometries with BAWT
CFD Verification and Investigation on Building Geometries with BAWT Jed I. Tapiador 1*, Aristotle T. Ubando 1 and Gerardo L. Augusto 1 1 Mechanical Engineering Department, De La Salle University Manila
More informationModeling Supersonic Jet Screech Noise Using Direct Computational Aeroacoustics (CAA) 14.5 Release
Modeling Supersonic Jet Screech Noise Using Direct Computational Aeroacoustics (CAA) 14.5 Release 2011 ANSYS, Inc. November 7, 2012 1 Workshop Advanced ANSYS FLUENT Acoustics Introduction This tutorial
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 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 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 informationEffect of suction pipe leaning angle and water level on the internal flow of pump sump
IOP Conference Series: Earth and Environmental Science PAPER OPEN ACCESS Effect of suction pipe leaning angle and water level on the internal flow of pump sump To cite this article: Z-M Chen et al 216
More informationSimulation of Turbulent Flow around an Airfoil
Simulation of Turbulent Flow around an Airfoil ENGR:2510 Mechanics of Fluids and Transfer Processes CFD Pre-Lab 2 (ANSYS 17.1; Last Updated: Nov. 7, 2016) By Timur Dogan, Michael Conger, Andrew Opyd, Dong-Hwan
More information