Near Field and Far Field Prediction of Noise in and around a Loudspeaker: A Numerical and Experimental Investigation
|
|
- Della Hines
- 6 years ago
- Views:
Transcription
1 Near Field and Far Field Prediction of Noise in and around a Loudspeaker: A Numerical and Experimental Investigation M. Younsi, V. Morgenthaler ANSYS France SAS, France G. Kergourlay Canon CRF, France Summary This paper aims at studying the acoustic behavior and the noise propagation in and around a loudspeaker Bass-Reflex type when its membrane is excited at low frequency with a harmonic signal. Both numerical simulations and experimental tests have been performed. The near field noise has been predicted on the basis of a direct approach: LES (Large Eddy Simulation) calculation in which acoustic sources and coupling with turbulence are fully represented. For the far field noise, the acoustic analogy method from Ffowcs-Williams and Hawkings (FW-H) has been used. In parallel with this calculation, acoustic measurements at different distances and directions from the loudspeaker have been run in an anechoic environment. The numerical results are compared with the experimental data and a good match is obtained both in behavior and intensity. 1. Introduction 1 In order to enhance low frequency performances of loudspeakers, bass reflex ports are commonly used. The objective of this technique is to extend the low frequency response of loudspeaker systems by creating a Helmholtz resonator. The movement of the air caused by the loudspeaker driver is characterized by a pumping phenomenon through the port. The flow behavior within the port has a significant influence on the system efficiency. At high pressure level, the air velocity within the port increases and creates turbulence structures and vortex shedding which are responsible for the aerodynamic noise generation. For these reasons, the port design optimization is considered as an important step by high quality loudspeakers manufacturers. In an industrial environment, the recent development of Computational Fluid Dynamics (CFD) for 3D viscous flow fields provides an efficient tool for flows analysis and design. There is a continuously increasing demand in all areas of CFD for unsteady flow simulations. Several researchers have made significant contributions to study loudspeakers using different methods. However, little work is available in the literature 1 (c) European Acoustics Association ISSN ISBN concerning the application of CFD techniques in this field. Z. Rapoport and A. Devantier [1] used a 2D axisymmetric model in order to study the unsteady fluid flow in loudspeaker ports. In their work, a commercial code (ANSYS Fluent) was used where the turbulent flow was modeled using LES technique. They studied the effect of the port entrance angle on the flow behavior. By varying this parameter, six geometries were created and their acoustic efficiency were studied and analyzed. The numerical results showed the influence of the entrance angle of the port on the flow. In addition to this, the evidence of vortex shedding was clearly observed. Finally, experimental work based on listening tests was performed in order to confirm the numerical study. N.B Roozen et. al. [2] studied a method to reduce bass-reflex port nonlinearties by optimizing the port geometry. In their study, 2D axisymmetric calculations and measurements are presented for a number of ports geometries. The effect of rounding the port lips and the effect of nozzle in the port on the production of blowing sounds was investigated. Their results showed that the intensity of the unsteady flow separation, as well as the radiation efficiency of the port and the quality factor of the port resonances, altogether determine the level of blowing noise. They concluded that the port contour geometry has an important impact on the blowing sounds intensity. 504
2 Thus, the acoustic losses can be reduced by using a port contour geometry that slowly diverges. In an additional work, N.B Roozen et. al. [3] [4] were interested in observing the response to harmonic excitation using experimental investigations. In the first part of their study, they summarized the dominant physical phenomena and presented the port geometry alterations for minimizing the blowing sound. In the second part, a method to estimate the time-averaged point of separation was performed. Analytic method based on the unsteady Bernoulli equation was used. A direct method for determining the velocity of the air particles in the port was also performed using Laser Doppler Anemometry. 2. 3D Flow Simulation In the present work, a box loudspeaker equipped with a bass-reflex port has been studied. The Computer Aided Design (CAD) and the mesh generation are first performed (section 2.1), along with choice of simulations parameters and boundary conditions. Then the CFD analysis leading to the flow behavior and the acoustic prediction is performed using Ansys Fluent 12 [5] software (sections 2.2, 2.3, 2.4). The flow morphology analysis is detailed (section 2.5). Finally, the pressure signals in and around the loudspeaker are analyzed (section 2.6) Geometry, Mesh and Boundary Conditions Using the initial CAD of the loudspeaker, 3D fluid volume geometry and mesh have been generated with ANSYS Design Modeler and ANSYS Meshing respectively. Figure 1 shows the loudspeaker geometry and the corresponding fluid volume. Due to the geometry complexity, this calculation domain has been divided in several blocks in order to generate a good quality hexahedral mesh. The grid refinement has been studied and adapted to the flow morphology. Thus, a particular attention has been paid to the boundary layer resolution and the mean cell size in the calculation domain has been estimated in order to capture a maximal frequency of 6 khz. For numerical stability reasons, and to minimize edges effects, the computational domain has been extended downstream. Based on these considerations, 2.6 millions cells have been created in the calculation domain. Figure 1 shows the resulting mesh which is considered to be fine enough to capture the desired flow instabilities and therefore capture the acoustic behavior. The driver geometry has been isolated from the complete domain in order to apply a Moving and Deforming Mesh (MDM) model in ANSYS Fluent solver. Thus, a spring analogy method based on the smoothing algorithm has been applied on this region which allows simulating the sinusoidal movement of the driver. Pressure outlet boundary condition has been applied at the external surfaces of the downstream domain and wall boundary conditions elsewhere. In addition to this, enclosure surfaces have been placed at the port outlet in order to use them as integration surfaces for quadrupole sources calculation in the FW-H model Numerical Modeling Ideal gas state equation has been used in order to describe the thermodynamic behavior of the air in the loudspeaker enclosure. Thus the compressible unsteady flow is generated by the sinusoidal movement of the driver whose velocity is given by the following harmonic equation: X (t) = 0.58 cos (2 π.50.t) (1) The frequency of the driver oscillation is set to 50 Hz and the equation (1) has been implemented in the MDM model using a User Defined Function (UDF) in ANSYS Fluent. As mentioned previously, a smoothing algorithm has been applied in this study particularly because of the driver amplitude displacement which is very small (3.692 mm). Consequently, deleting and creating cells in the domain is not necessary and morphing them is enough. Moreover, this method is less computer time consuming. According to numerical considerations for this simulation, such as Courant number taken in between 1 and 10, a time step of 8 µs has been used. This value is small enough to capture the pressure signal due to the driver excitation and ensure solver stability. Figure 2 illustrates near field and far field sensors locations where the acoustic pressures have been computed. 505
3 2.3.1 The Large Eddy Simulation Model It is possible, in theory, to directly resolve the whole spectrum of turbulent scales using an approach known as Direct Numerical Simulation (DNS). No modeling is required in DNS and might have been successfully used if the solver numerical schemes were accurate enough to generate very limited numerical noises which will not affect the smaller eddies formation. Moreover, the resolution of the whole spectrum eddies requires a finer mesh which would increase the calculation cost dramatically. Figure 1. Geometry and Mesh. P1 14cm 7cm Figure 2. Pressure sensors location 2.3. Turbulence Modeling The flow generated by the loudspeaker is laminar in most of the domain except in the loudspeaker s port were the flow restriction increase the fluid velocity and transition the fluid from a laminar state to a turbulent one. In order to capture correctly all the physics and especially the broadband noise generated by the turbulent part of the flow, a turbulence modeling approach which can work both in laminar and turbulent situation has to be chosen. The largest eddies will be generated here by the jet instability triggered by the port. Large eddies will also be generated inside the boundary layer attached to the port wall. These eddies are responsible for the tonal noise and should be described very precisely as they are bringing energy to turbulence. Turbulence is breaking this large eddies into smaller ones until viscosity dissipate them at the smallest scales. Those intermediaries eddies form the broadband noise. We choose to use the Large Eddy Simulation (LES) approach as often used for aero-acoustic calculations [6]. In this approach, large eddies are resolved directly, while small eddies effects on momentum and mass transport are modeled. As the smaller eddies are modeled, the need of an extremely precise numerical scheme is lessen. Moreover, in this study, only the lower frequencies of the spectrum are considered, which relieves the need for carefully modeling the smaller scales. Several subgrid-scale turbulence models can be used in ANSYS Fluent. We choose the model proposed by Smagorinsky [7]. In the Smagorinsky model is a mixing length model where the mixing length is taken as the filter width. This model suffers from two main drawbacks: the lack of universality of the Smagorinsky constant and the impossibility of treating relaminarization and thus boundary layer. To try and avoid the problem of the classical Smagorinsky model Germano et al. [8] and subsequently Lilly [9] conceived a procedure in which the Smagorinsky model constant, is dynamically computed based on the information provided by the resolved scales of motion. The dynamic procedure thus obviates the need for users to specify the Smagorinsky constant in advance. The obtained constant varies in time and space over a fairly wide range. To avoid numerical instability, in ANSYS Fluent, the result is clipped at zero and 0.23 by default. This approach enables also the Smagorinsky model to reproduce relaminarization with a Smagorinsky constant which naturally soften with a decreasing Reynolds number. 506
4 2.4. Far Field Noise Prediction Acoustic analogy based on the FW-H model has been used in this simulation in order to predict the acoustic pressures in far field region (P10 and P11 in Figure 2). The FW-H model [10, 11] is essentially an inhomogeneous wave equation that can be derived by manipulating the continuity equation and the Navier-Stokes equation. Based on its mathematical structure, this equation takes into account the source terms which are monopole (thickness), dipole (loading) and quadrupole sources. The monopole source term models the noise generated by the displacement of fluid as the body passes. The dipole or loading source term models the noise that results from the unsteady motion of the force distribution on the body surface. Both of these sources are surface sources. The quadrupole represent volume sources in the region outside the source surface. The contribution of the volume integrals becomes small when the flow is low subsonic. Once the statistical stability is reached on the variables provided by the LES calculation, the fluctuating pressure and velocity upon the integration surfaces can be extracted for time steps. Then, the sound pressure signals are computed at the receiver locations using the source data collected during the unsteady aerodynamic computations CFD Results and Discussion Figure 3 shows the instantaneous velocity field at the middle plan. By analyzing this result, a complex flow can be observed at the port inlet and outlet. It is shown clearly that the driver sinusoidal movement combined with the contraction of the flow sections induces a vortex shedding phenomenon. Thus, turbulent structures are generated at each mid-period at upstream and downstream alternately. In the pressure field, a non homogenous pressure distribution is observed, particularly around the port outlet. Using an animation, a pumping phenomenon occurring at 50 Hz can be observed between the driver zone and the enclosure zone Pressure Signals Analysis The fluctuating pressures post-processing has been done after the stability of the unsteady variables. The time histories of the pressure fluctuations at point P10 is shown in Figure 4. All the obtained signals are regular and a period of 0.02 s can be observed clearly. Compared to the far field region, the signal amplitude is higher at sensor P1, which is closer to the driver. Figure 3. Instantaneous velocity (a), pressure fields (b) Pressure [Pa] (ms -1 ) Pa (b) (a) Figure 4. Computed fluctuating pressure signal at P10 3. Experimental Work Time [s] Figure 5 shows the test bench which has been realized accordingly to the simulated system: a 25 cm- driver is placed in the front plate of a ventedbox of 48 liters equipped with an 11cm-length vent of diameter 18mm located at its back plate. Free-field acoustic measurements have been performed in an anechoic room. The driver is excited by a constant voltage signal of intensity U=8.55V at a frequency of 50 Hz. This voltage enables getting a driver membrane velocity of 580 mm/s, which has been carefully measured by laser vibrometry. 507
5 Figure 5. Test facility in anechoic room 4. Test Analysis Correlation Figures 6 and 7 give the test-analysis correlation performed on the simulated and measured data for points 7 and 10 respectively. The upper part of the Figures corresponds to the superposition of the pressure fluctuations in the temporal domain. The lower part corresponds to the spectral analysis of the signals: a fast Fourier transform has been done on 8.65 periods of the windowed time signals for both numerical and experimental data. The four experimental data superimposed rather well, which shows the reproducibility and repeatability of the test. Figure 7. Test-analysis correlation at Point 10 Up: Fluctuations of pressure (Pa) as function of time Bottom: spectral analysis 20Hz-20 khz 5. Discussion and Conclusion Good qualitative and quantitative results have been found with the chosen CFD approach compared to measurements. The comparison between the computed and measured temporal signals both in near and far fields region shows a good agreement in frequency. Moreover, in the far field the amplitude is also the same. At this location, the signal is obtained using the FW-H acoustic analogy. This result illustrates the quality of the noise sources prediction provided by the LES calculation. However, a 30% discrepancy in the near field signals amplitude can be observed. This difference may be explained by an experimental bias due to the microphone intrusion which interacts frontally with the air flow. In the spectral analysis, the measured and computed results show similar overall behavior for low frequencies until 200 Hz. At higher frequencies, the spectra are different. This discrepancy could be justified by: - The numerical dissipation which becomes predominant at very low pressure levels. - The mesh coarsening far from the source which has an impact on the frequencies interval modeled. Figure 6. Test-analysis correlation at Point 7 Up: Fluctuations of pressure (Pa) as function of time Bottom: spectral analysis 20Hz-20 khz - The acoustic reflections at far field location which are not taken into account in the FW- H model. 508
6 - The quality and the size of the microphone dynamics: The 1/f noise level should be decreased. The analyses performed at the different control points in near-field and in far-field give first conclusions. The following ways to improve the correlation were suggested: - Finer grid mesh should be used in order to reduce the numerical dissipation. - A stronger excitation should be used in order to increase the signal to noise ratio. The limitation is to change the turbulence regime (Mach and Reynolds number). The velocity of the membrane was chosen in order to be close to the turbulence regime observed with the analyzed high-quality speaker in usual listening conditions. - The sensor appears to be intrusive in nearfield: use of a ¼ or even 1/8 one instead of a ½ microphone. Hot-wire probes that are less intrusive could also be used to correlate non-stationary velocity simulations and experimental data. In this case, transient non-stationary velocities [m/s] have to be saved in addition to static pressure [Pa] for near-field points (all points except points 10 and 12). Harmonic Excitation and remedial Measures, J. Acoust. Soc. Am [4] N. B. Roozen, M. Bockholts, P. V. Eck, A. Hirschberg, Vortex Sound in Bass-reflex Ports of Loudspeakers. Part II. A Method to Estimate the Point of Separation, J. Acoust. Soc. Am [5] Ansys Inc. Copyright [6] C. Wagner, T. Hüttl, P. Sagaut, Large-Eddy Simulation for Acoustics, Cambridge University Press, [7] Smagorinsky, J., General circulation experiments with the primitive equations. The Basic Experimental Monthly Weather Revision, Vol. 91, pp [8] Germano, M., Piomelli, U., Moin, P. and Cabot, W. H., A Dynamic Subgrid-Scale Eddy Viscosity Model, Physics of Fluids A, Vol. 3, No. 7, pp [9] Lilly, D. K., A Proposed Modification of the Germano Subgrid-Scale Closure Method, Physics of Fluids A, Vol. 4, No. 3, pp [10] J. E. Ffowcs Williams and D.L. Hawkings, Sound generation by turbulence and surfaces in arbitrary motion, Philosophical Transactions of the Royal Society of London. Series A, vol. 264, no. 1151, pp , 1969 [11] K. S. Brentner and F. Farassat, Analytical comparison of the acoustic analogy and Kirchhoff formulation for moving surfaces, AIAA Journal, vol. 36, no. 8, pp , Acknowledgement The authors wish to thank Mr. Pierre-Yves Diquelou from Cabasse company located in Brest (France) for his help doing acoustic measurements. 7. References [1] Z. Rapoport, A. Devantier, Method for Predicting Loudspeaker Port Performance and Optimizing Loudspeaker Port Designs Utilizing Bi-directional Fluid Flow Principles, PCT, 2006 [2]N.B. Roozen, J.E.M. Vael, J.A.M, Reduction of Bass-Reflex Port Nonlinearities by Optimizing the Port Geometry, Audio Engineering Society, 1998 [3]N. B. Roozen, M. Bockholts, P. V. Eck, A. Hirschberg, Vortex Sound in Bass-reflex Ports of Loudspeakers. Part I. Observation of Response to 509
Modeling 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 informationOn the flow and noise of a two-dimensional step element in a turbulent boundary layer
On the flow and noise of a two-dimensional step element in a turbulent boundary layer Danielle J. Moreau 1, Jesse L. Coombs 1 and Con J. Doolan 1 Abstract This paper presents results of a study on the
More informationTransition Flow and Aeroacoustic Analysis of NACA0018 Satish Kumar B, Fred Mendonç a, Ghuiyeon Kim, Hogeon Kim
Transition Flow and Aeroacoustic Analysis of NACA0018 Satish Kumar B, Fred Mendonç a, Ghuiyeon Kim, Hogeon Kim Transition Flow and Aeroacoustic Analysis of NACA0018 Satish Kumar B, Fred Mendonç a, Ghuiyeon
More informationAdvanced ANSYS FLUENT Acoustics
Workshop Modeling Flow-Induced (Aeroacoustic) Noise 14.5 Release Advanced ANSYS FLUENT Acoustics 2011 ANSYS, Inc. November 7, 2012 1 Introduction This tutorial demonstrates how to model 2D turbulent flow
More informationLarge Eddy Simulation of Flow over a Backward Facing Step using Fire Dynamics Simulator (FDS)
The 14 th Asian Congress of Fluid Mechanics - 14ACFM October 15-19, 2013; Hanoi and Halong, Vietnam Large Eddy Simulation of Flow over a Backward Facing Step using Fire Dynamics Simulator (FDS) Md. Mahfuz
More informationA Coupling Method for Hybrid CFD-CAA Simulations using a Dual Mesh Approach. Matthias Tautz
A Coupling Method for Hybrid CFD-CAA Simulations using a Dual Mesh Approach Matthias Tautz München, 21. November 2013 Content 1. Motivation Problem Description 2. Analytical Approach 3. Experiments 4.
More informationRotorcraft Noise Prediction with Multi-disciplinary Coupling Methods. Yi Liu NIA CFD Seminar, April 10, 2012
Rotorcraft Noise Prediction with Multi-disciplinary Coupling Methods Yi Liu NIA CFD Seminar, April 10, 2012 Outline Introduction and Background Multi-disciplinary Analysis Approaches Computational Fluid
More informationSimulation of Turbulent Axisymmetric Waterjet Using Computational Fluid Dynamics (CFD)
Simulation of Turbulent Axisymmetric Waterjet Using Computational Fluid Dynamics (CFD) PhD. Eng. Nicolae MEDAN 1 1 Technical University Cluj-Napoca, North University Center Baia Mare, Nicolae.Medan@cunbm.utcluj.ro
More informationDevelopment of an Integrated Computational Simulation Method for Fluid Driven Structure Movement and Acoustics
Development of an Integrated Computational Simulation Method for Fluid Driven Structure Movement and Acoustics I. Pantle Fachgebiet Strömungsmaschinen Karlsruher Institut für Technologie KIT Motivation
More informationNUMERICAL MODELING AND EXPERIMENTAL EVALUATION OF AN HIGH-SPEED TRAIN PANTOGRAPH AERODYNAMIC NOISE
NUMERICAL MODELING AND EXPERIMENTAL EVALUATION OF AN HIGH-SPEED TRAIN PANTOGRAPH AERODYNAMIC NOISE D. SIANO 1, M. VISCARDI 2, F. DONISI 2 P. NAPOLITANO 2 1 CNR (National Research Council of Italy) - Istituto
More informationThe second part of the tutorial continues with the subsequent ANSYS Mechanical simulation steps:
Tutorial: Simulation of aero-vibro-acoustic phenomena using ANSYS Fluent and ANSYS Mechanical. Test case: Noise inside a cavity with a vibrating wall, caused by the external turbulent flow. Introduction
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 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 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 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 informationVerification and Validation in CFD and Heat Transfer: ANSYS Practice and the New ASME Standard
Verification and Validation in CFD and Heat Transfer: ANSYS Practice and the New ASME Standard Dimitri P. Tselepidakis & Lewis Collins ASME 2012 Verification and Validation Symposium May 3 rd, 2012 1 Outline
More informationAero-Vibro Acoustics For Wind Noise Application. David Roche and Ashok Khondge ANSYS, Inc.
Aero-Vibro Acoustics For Wind Noise Application David Roche and Ashok Khondge ANSYS, Inc. Outline 1. Wind Noise 2. Problem Description 3. Simulation Methodology 4. Results 5. Summary Thursday, October
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 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 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 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 informationPossibility of Implicit LES for Two-Dimensional Incompressible Lid-Driven Cavity Flow Based on COMSOL Multiphysics
Possibility of Implicit LES for Two-Dimensional Incompressible Lid-Driven Cavity Flow Based on COMSOL Multiphysics Masanori Hashiguchi 1 1 Keisoku Engineering System Co., Ltd. 1-9-5 Uchikanda, Chiyoda-ku,
More informationSolution Recording and Playback: Vortex Shedding
STAR-CCM+ User Guide 6663 Solution Recording and Playback: Vortex Shedding This tutorial demonstrates how to use the solution recording and playback module for capturing the results of transient phenomena.
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 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 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 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 informationNumerical Simulation of Coastal Wave Processes with the Use of Smoothed Particle Hydrodynamics (SPH) Method
Aristotle University of Thessaloniki Faculty of Engineering Department of Civil Engineering Division of Hydraulics and Environmental Engineering Laboratory of Maritime Engineering Christos V. Makris Dipl.
More informationMODELLING THE FLOW AROUND AN ISLAND AND A HEADLAND: APPLICATION OF A TWO MIXING LENGTH MODEL WITH TELEMAC3D. Nicolas Chini 1 and Peter K.
MODELLING THE FLOW AROUND AN ISLAND AND A HEADLAND: APPLICATION OF A TWO MIXING LENGTH MODEL WITH TELEMAC3D Nicolas Chini 1 and Peter K. Stansby 2 Numerical modelling of the circulation around islands
More informationPreliminary investigation into two-way fluid structure interaction of heliostat wind loads Josh Wolmarans
Preliminary investigation into two-way fluid structure interaction of heliostat wind loads Josh Wolmarans Supervisor: Prof Ken Craig Clean Energy Research Group (CERG), Department of Mechanical and Aeronautical
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 informationAvailable online at ScienceDirect. The 2014 conference of the International Sports Engineering Association.
Available online at www.sciencedirect.com ScienceDirect Procedia Engineering 72 ( 2014 ) 768 773 The 2014 conference of the International Sports Engineering Association Simulation and understanding of
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 informationParametric Study of Sloshing Effects in the Primary System of an Isolated LFR Marti Jeltsov, Walter Villanueva, Pavel Kudinov
1 Parametric Study of Sloshing Effects in the Primary System of an Isolated LFR 19.06.2013 Marti Jeltsov, Walter Villanueva, Pavel Kudinov Division of Nuclear Power Safety Royal Institute of Technology
More informationA B C D E. Settings Choose height, H, free stream velocity, U, and fluid (dynamic viscosity and density ) so that: Reynolds number
Individual task Objective To derive the drag coefficient for a 2D object, defined as where D (N/m) is the aerodynamic drag force (per unit length in the third direction) acting on the object. The object
More informationAuto Injector Syringe. A Fluent Dynamic Mesh 1DOF Tutorial
Auto Injector Syringe A Fluent Dynamic Mesh 1DOF Tutorial 1 2015 ANSYS, Inc. June 26, 2015 Prerequisites This tutorial is written with the assumption that You have attended the Introduction to ANSYS Fluent
More informationSimulating Sinkage & Trim for Planing Boat Hulls. A Fluent Dynamic Mesh 6DOF Tutorial
Simulating Sinkage & Trim for Planing Boat Hulls A Fluent Dynamic Mesh 6DOF Tutorial 1 Introduction Workshop Description This workshop describes how to perform a transient 2DOF simulation of a planing
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 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 informationAerodynamic Study of a Realistic Car W. TOUGERON
Aerodynamic Study of a Realistic Car W. TOUGERON Tougeron CFD Engineer 2016 Abstract This document presents an aerodynamic CFD study of a realistic car geometry. The aim is to demonstrate the efficiency
More informationAurélien Thinat Stéphane Cordier 1, François Cany
SimHydro 2012:New trends in simulation - Hydroinformatics and 3D modeling, 12-14 September 2012, Nice Aurélien Thinat, Stéphane Cordier, François Cany Application of OpenFOAM to the study of wave loads
More informationFFOWCS WILLIAMS-HAWKINGS ACOUSTIC ANALOGY FOR SIMULATION OF NACA 4-(3)(08)-03 PROPELLER NOISE IN TAKE-OFF CONDITION
ASME-ATI-UIT 1 Conference on Thermal and Environmental Issues in Energy Systems 16 19 May, 1, Sorrento, Italy FFOWCS WILLIAMS-HAWKINGS ACOUSTIC ANALOGY FOR SIMULATION OF NACA 4-(3)(8)-3 PROPELLER NOISE
More informationVehicle Cabin Noise from Turbulence Induced by Side-View Mirrors. Hua-Dong Yao, 2018/8/29 Chalmers University of Technology, Sweden
Vehicle Cabin Noise from Turbulence Induced by Side-View Mirrors Hua-Dong Yao, 2018/8/29 Chalmers University of Technology, Sweden An Important Cabin Noise Source Turbulence As the development of quiet
More informationDesign Optimization of a Weather Radar Antenna using Finite Element Analysis (FEA) and Computational Fluid Dynamics (CFD)
Design Optimization of a Weather Radar Antenna using Finite Element Analysis (FEA) and Computational Fluid Dynamics (CFD) Fernando Prevedello Regis Ataídes Nícolas Spogis Wagner Ortega Guedes Fabiano Armellini
More informationSecond Symposium on Hybrid RANS-LES Methods, 17/18 June 2007
1 Zonal-Detached Eddy Simulation of Transonic Buffet on a Civil Aircraft Type Configuration V.BRUNET and S.DECK Applied Aerodynamics Department The Buffet Phenomenon Aircraft in transonic conditions Self-sustained
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 informationInfluence of mesh quality and density on numerical calculation of heat exchanger with undulation in herringbone pattern
Influence of mesh quality and density on numerical calculation of heat exchanger with undulation in herringbone pattern Václav Dvořák, Jan Novosád Abstract Research of devices for heat recovery is currently
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 informationEXPERIMENTAL INVESTIGATION OF THE FLOW PATTERN BEHIND CYLINDER. Ing. Rut Vitkovičová, Ing. Vladislav Skála, Ing. Jan Čížek Ph.D.
EXPERIMENTAL INVESTIGATION OF THE FLOW PATTERN BEHIND CYLINDER Ing. Rut Vitkovičová, Ing. Vladislav Skála, Ing. Jan Čížek Ph.D. Abstract Investigation of the flow behind bluff bodies, especially for cylinder,
More informationA STUDY ON THE UNSTEADY AERODYNAMICS OF PROJECTILES IN OVERTAKING BLAST FLOWFIELDS
HEFAT2012 9 th International Conference on Heat Transfer, Fluid Mechanics and Thermodynamics 16 18 July 2012 Malta A STUDY ON THE UNSTEADY AERODYNAMICS OF PROJECTILES IN OVERTAKING BLAST FLOWFIELDS Muthukumaran.C.K.
More informationTurbulencja w mikrokanale i jej wpływ na proces emulsyfikacji
Polish Academy of Sciences Institute of Fundamental Technological Research Turbulencja w mikrokanale i jej wpływ na proces emulsyfikacji S. Błoński, P.Korczyk, T.A. Kowalewski PRESENTATION OUTLINE 0 Introduction
More informationTime-resolved PIV measurements with CAVILUX HF diode laser
Time-resolved PIV measurements with CAVILUX HF diode laser Author: Hannu Eloranta, Pixact Ltd 1 Introduction Particle Image Velocimetry (PIV) is a non-intrusive optical technique to measure instantaneous
More informationJournal of Fluid Science and Technology
Science and Technology Direct Numerical Prediction of Aerodynamic Noise Emitted from a Generic Automobile Rear-View Mirror* Katsunori DOI**, Masaya MIYOSHI***, Naoki HAMAMOTO**** and Yoshiaki NAKAMURA*****
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 informationDYNAMICS OF A VORTEX RING AROUND A MAIN ROTOR HELICOPTER
DYNAMICS OF A VORTEX RING AROUND A MAIN ROTOR HELICOPTER Katarzyna Surmacz Instytut Lotnictwa Keywords: VORTEX RING STATE, HELICOPTER DESCENT, NUMERICAL ANALYSIS, FLOW VISUALIZATION Abstract The main goal
More informationUsing a Single Rotating Reference Frame
Tutorial 9. Using a Single Rotating Reference Frame Introduction This tutorial considers the flow within a 2D, axisymmetric, co-rotating disk cavity system. Understanding the behavior of such flows is
More informationComputational 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 informationDirect numerical simulations of flow and heat transfer over a circular cylinder at Re = 2000
Journal of Physics: Conference Series PAPER OPEN ACCESS Direct numerical simulations of flow and heat transfer over a circular cylinder at Re = 2000 To cite this article: M C Vidya et al 2016 J. Phys.:
More informationShape optimisation using breakthrough technologies
Shape optimisation using breakthrough technologies Compiled by Mike Slack Ansys Technical Services 2010 ANSYS, Inc. All rights reserved. 1 ANSYS, Inc. Proprietary Introduction Shape optimisation technologies
More informationKeywords: flows past a cylinder; detached-eddy-simulations; Spalart-Allmaras model; flow visualizations
A TURBOLENT FLOW PAST A CYLINDER *Vít HONZEJK, **Karel FRAŇA *Technical University of Liberec Studentská 2, 461 17, Liberec, Czech Republic Phone:+ 420 485 353434 Email: vit.honzejk@seznam.cz **Technical
More informationInvestigation of cross flow over a circular cylinder at low Re using the Immersed Boundary Method (IBM)
Computational Methods and Experimental Measurements XVII 235 Investigation of cross flow over a circular cylinder at low Re using the Immersed Boundary Method (IBM) K. Rehman Department of Mechanical Engineering,
More 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 informationNumerical Analysis of a Blast Wave Using CFD-CAA Hybrid Method
Numerical Analysis of a Blast Wave Using CFD-CAA Hybrid Method In Cheol Lee * and Duck-Joo Lee. Korea Advanced Institute of Science and Technology, Daejeon, 305-701, Republic of Korea Sung Ho Ko and Dong
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 informationExpress Introductory Training in ANSYS Fluent Workshop 08 Vortex Shedding
Express Introductory Training in ANSYS Fluent Workshop 08 Vortex Shedding Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 - Industry Oriented HPC Simulations,
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 informationUsage of CFX for Aeronautical Simulations
Usage of CFX for Aeronautical Simulations Florian Menter Development Manager Scientific Coordination ANSYS Germany GmbH Overview Elements of CFD Technology for aeronautical simulations: Grid generation
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 informationExpress Introductory Training in ANSYS Fluent Workshop 04 Fluid Flow Around the NACA0012 Airfoil
Express Introductory Training in ANSYS Fluent Workshop 04 Fluid Flow Around the NACA0012 Airfoil Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 -
More informationANSYS Fluid Structure Interaction for Thermal Management and Aeroelasticity
ANSYS Fluid Structure Interaction for Thermal Management and Aeroelasticity Phil Stopford Duxford Air Museum 11th May 2011 2011 2010 ANSYS, Inc. All rights reserved. 1 ANSYS, Inc. Proprietary Fluid Structure
More informationFluid-Structure Interaction Modeling of High-Aspect Ratio Nuclear Fuel Plates using COMSOL
Fluid-Structure Interaction Modeling of High-Aspect Ratio Nuclear Fuel Plates using COMSOL Franklin Curtis 1 Kivanc Ekici 1 James Freels 2 1 University of Tennessee, Knoxville, TN 2 Oak Ridge National
More informationNumerical Study of Turbulent Flow over Backward-Facing Step with Different Turbulence Models
Numerical Study of Turbulent Flow over Backward-Facing Step with Different Turbulence Models D. G. Jehad *,a, G. A. Hashim b, A. K. Zarzoor c and C. S. Nor Azwadi d Department of Thermo-Fluids, Faculty
More informationTutorial: Simulating a 3D Check Valve Using Dynamic Mesh 6DOF Model And Diffusion Smoothing
Tutorial: Simulating a 3D Check Valve Using Dynamic Mesh 6DOF Model And Diffusion Smoothing Introduction The purpose of this tutorial is to demonstrate how to simulate a ball check valve with small displacement
More informationModeling Unsteady Compressible Flow
Tutorial 4. Modeling Unsteady Compressible Flow Introduction In this tutorial, FLUENT s density-based implicit solver is used to predict the timedependent flow through a two-dimensional nozzle. As an initial
More informationLarge Eddy Simulation of a Turbulent Jet Impinging on a Flat Plate at Large Stand-off Distance
Large Eddy Simulation of a Turbulent Jet Impinging on a Flat Plate at Large Stand-off Distance M. Shademan 1, R. Balachandar 2 and R.M. Barron 3 1 PhD Student, Department of Mechanical, Automotive & Materials
More informationNumerical Simulation Study on Aerodynamic Characteristics of the High Speed Train under Crosswind
2017 2nd International Conference on Industrial Aerodynamics (ICIA 2017) ISBN: 978-1-60595-481-3 Numerical Simulation Study on Aerodynamic Characteristics of the High Speed Train under Crosswind Fan Zhao,
More information4D-PIV advances to visualize sound generation by air flows
4D-PIV advances to visualize sound generation by air flows Fulvio Scarano Delft University of Technology Aerospace Engineering Department Aerodynamics Section f.scarano@tudelft.nl Aero-acoustics Investigation
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 informationFlow and Heat Transfer in a Mixing Elbow
Flow and Heat Transfer in a Mixing Elbow Objectives The main objectives of the project are to learn (i) how to set up and perform flow simulations with heat transfer and mixing, (ii) post-processing and
More informationUSING CFD SIMULATIONS TO IMPROVE THE MODELING OF WINDOW DISCHARGE COEFFICIENTS
USING CFD SIMULATIONS TO IMPROVE THE MODELING OF WINDOW DISCHARGE COEFFICIENTS Erin L. Hult 1, Gianluca Iaccarino 2, and Martin Fischer 2 1 Lawrence Berkeley National Laboratory, Berkeley, CA 2 Stanford
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 informationDirect Numerical Simulation of a Low Pressure Turbine Cascade. Christoph Müller
Low Pressure NOFUN 2015, Braunschweig, Overview PostProcessing Experimental test facility Grid generation Inflow turbulence Conclusion and slide 2 / 16 Project Scale resolving Simulations give insight
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 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 informationComputational Study of Unsteady Flows around Dragonfly and Smooth Airfoils at Low Reynolds Numbers
46th AIAA Aerospace Sciences Meeting and Exhibit 7 - January 8, Reno, Nevada AIAA 8-85 Computational Study of Unsteady Flows around Dragonfly and Smooth Airfoils at Low Reynolds Numbers H. Gao, Hui Hu,
More informationIntroduction to CFX. Workshop 2. Transonic Flow Over a NACA 0012 Airfoil. WS2-1. ANSYS, Inc. Proprietary 2009 ANSYS, Inc. All rights reserved.
Workshop 2 Transonic Flow Over a NACA 0012 Airfoil. Introduction to CFX WS2-1 Goals The purpose of this tutorial is to introduce the user to modelling flow in high speed external aerodynamic applications.
More informationProfile Catalogue for Airfoil Sections Based on 3D Computations
Risø-R-58(EN) Profile Catalogue for Airfoil Sections Based on 3D Computations Franck Bertagnolio, Niels N. Sørensen and Jeppe Johansen Risø National Laboratory Roskilde Denmark December 26 Author: Franck
More informationRBF Morph An Add-on Module for Mesh Morphing in ANSYS Fluent
RBF Morph An Add-on Module for Mesh Morphing in ANSYS Fluent Gilles Eggenspieler Senior Product Manager 1 Morphing & Smoothing A mesh morpher is a tool capable of performing mesh modifications in order
More informationOzenCloud Case Studies
OzenCloud Case Studies Case Studies, April 20, 2015 ANSYS in the Cloud Case Studies: Aerodynamics & fluttering study on an aircraft wing using fluid structure interaction 1 Powered by UberCloud http://www.theubercloud.com
More informationQuantifying the Dynamic Ocean Surface Using Underwater Radiometric Measurement
DISTRIBUTION STATEMENT A. Approved for public release; distribution is unlimited. Quantifying the Dynamic Ocean Surface Using Underwater Radiometric Measurement Lian Shen Department of Mechanical Engineering
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 informationEffect of initial turbulence intensity and velocity profile on liquid jets for IFE beamline protection
Effect of initial turbulence intensity and velocity profile on liquid jets for IFE beamline protection A. Konkachbaev, N.B. Morley and M. A. Abdou Mechanical and Aerospace Engineering Department, UCLA
More informationPulsating flow around a stationary cylinder: An experimental study
Proceedings of the 3rd IASME/WSEAS Int. Conf. on FLUID DYNAMICS & AERODYNAMICS, Corfu, Greece, August 2-22, 2 (pp24-244) Pulsating flow around a stationary cylinder: An experimental study A. DOUNI & D.
More informationFlow Field of Truncated Spherical Turrets
Flow Field of Truncated Spherical Turrets Kevin M. Albarado 1 and Amelia Williams 2 Aerospace Engineering, Auburn University, Auburn, AL, 36849 Truncated spherical turrets are used to house cameras and
More informationTurbulence Modeling. Gilles Eggenspieler, Ph.D. Senior Product Manager
Turbulence Modeling Gilles Eggenspieler, Ph.D. Senior Product Manager 1 Overview The Role of Steady State (RANS) Turbulence Modeling Overview of Reynolds-Averaged Navier Stokes (RANS) Modeling Capabilities
More informationCloud Cavitating Flow around an Axisymmetric Projectile in the shallow water
Cloud Cavitating Flow around an Axisymmetric Projectile in the shallow water 1,2 Chang Xu; 1,2 Yiwei Wang*; 1,2 Jian Huang; 1,2 Chenguang Huang 1 Key Laboratory for Mechanics in Fluid Solid Coupling Systems,
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 informationSupersonic Flow Over a Wedge
SPC 407 Supersonic & Hypersonic Fluid Dynamics Ansys Fluent Tutorial 2 Supersonic Flow Over a Wedge Ahmed M Nagib Elmekawy, PhD, P.E. Problem Specification A uniform supersonic stream encounters a wedge
More informationExperimental Data Confirms CFD Models of Mixer Performance
The Problem Over the years, manufacturers of mixing systems have presented computational fluid dynamics (CFD) calculations to claim that their technology can achieve adequate mixing in water storage tanks
More informationTHERMAL OPTIMIZATION OF GENSET CANOPY USING CFD
International Journal of Mechanical and Production Engineering Research and Development (IJMPERD) ISSN(P): 2249-6890; ISSN(E): 2249-8001 Vol. 5, Issue 3, Jun 2015, 19-26 TJPRC Pvt. Ltd. THERMAL OPTIMIZATION
More information