Large Eddy Simulation of a Turbulent Jet Impinging on a Flat Plate at Large Stand-off Distance
|
|
- Darcy Robinson
- 5 years ago
- Views:
Transcription
1 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 Engineering, University of Windsor, Windsor, N9B 3P4, Ontario, Canada 2 Professor, Department of Civil and Environmental Engineering, University of Windsor, Windsor, N9B 3P4, Ontario Canada 3 Professor, Department of Mathematics & Statistics, University of Windsor, Windsor, N9B 3P4, Ontario Canada shadema@uwindsor.ca ABSTRACT Large Eddy Simulation (LES) has been performed to evaluate the characteristics of a turbulent impinging jet with large nozzle height-to-diameter ratio. Dynamic Smagorinsky model was employed to simulate the subgrid scale stresses resulting from the filtering of the governing equations. The Reynolds number considered is about 28,000 based on the jet exit velocity and nozzle diameter. Results of the mean normalized centreline velocity in both free jet and impingement regions and also pressure distribution over the plate show good agreement with experimental data. According to this analysis, simulation of the impinging jet using LES can improve the accuracy of the results as compared to the previous RANS simulations, however more computational resource is required. The current comparison presents a robust CFD approach for evaluating the flow characteristics of turbulent impinging jets with large stand-off distance. 1. INTRODUCTION Circular jets impinging on flat surfaces have many practical applications. Most of the experiments on impinging jets have been performed for short stand-off distances, i.e., with an impingement height (H) to nozzle diameter (D) ratio of less than six. Cooper et al. [1] carried out experiments on a jet impinging on a large plane surface and measured the mean and turbulence quantities in different regions of the jet. They considered two Reynolds numbers, 23,000 and 70,000, while the H/D ratio varied from two to ten, with particular focus between two and six. For H/D < 6 the core of the jet is still developing when it reaches the surface (Nishino et al. [2], Hadziabdic and Hanjalic [3]). For larger impingement heights (H/D > 8.3), Beltaos and Rajaratnam [4,5] classified the flow into three different regions: the free jet portion (region I), the impingement zone (region II), and the axisymmetric wall jet portion (region III) as illustrated in Fig. 1. Giralt et al. [6] experimentally evaluated axisymmetric turbulent impinging jets with H/D ratios ranging from 3 to 25, and Re varying from 34,000 up to 80,000. Based on their experimental data, they developed a conceptual model for submerged, axisymmetric, turbulent impinging jets which can be used to analyze the effect of increasing the nozzle height from the plate. In addition to the experiments by Beltaos and Rajaratnam [4,5], Rajaratnam et al. [7] recently performed experiments on an impinging jet with a higher H/D ratio of 18.5 at Re = 100,000 (based on the nozzle exit velocity and diameter) and evaluated the turbulence characteristics in the different regions of the jet. Numerical simulation of a round jet impinging on a flat surface using Reynolds Averaged Navier-Stokes (RANS) simulations has been the subject of extensive research, forming part of the 2nd ERCOFTAC-IAHR Workshop on Refined Flow Modelling [8]. Subsequently, Craft et al. [9] published their research using different turbulence models to analyze the heat transfer in the impingement region of the jet, i.e., region II. They observed that the results were not in good agreement with experimental data, and attributed this to the weakness associated with the eddy viscosity stressstrain relationship in the turbulence models used. They also implemented second-moment closure models. Due to the incorrect response of the wall reflection process, the eddy viscosity model (k - ε) and the basic Reynolds Stress Model (RSM) failed to produce reasonable results while an improved Reynolds Stress Model which takes into account the wall reflection effects generated satisfactory results. Clearly, to analyze a complex fluid
2 flow problem such as an impinging jet, direct numerical simulation (DNS) or large eddy simulation (LES) seem to be the more accurate approaches. However, in order to resolve all scales of motion in DNS, the number of grid points should be of the order of Re 9/4 as suggested by Piomelli [10]. This is a limitation which currently makes DNS practical only for low Reynolds number flows with simple geometries. For example, Chung et al. [11] used DNS to simulate an unsteady slot jet with H/D = 10 and Re = 300, 500 and 1,000. Hattori and Nagano [12] simulated the plane impinging jet using DNS at Re = 9,120 for values of H/D = 0.5, 1 and 2. Both plane and round impinging jets with H/D = 10 were investigated by Tsubokura et al. [13] using DNS for Re = 2,000 and LES for Re = 6,000. In LES, only the large and high energy-containing eddies are resolved and the small ones are modeled. This method demands reasonably fine meshes at higher Reynolds numbers. Most LES jet studies have only dealt with simple plane jets at low Reynolds numbers as, for example, the LES studies on plane impinging jets by Voke and Gao [14] at Re = 6,500, and by Beaubert and Viazzo [15] at Re = 3,000 and 7,500. Recently, Hadziabdic and Hanjalic [3] have investigated the circular impinging jet at Re = 20,000 and H/D = 2 using LES. Based on a review of the literature, there is an apparent lack of information regarding the numerical simulation of turbulent impinging jets with large H/D ratios. Moreover, there is an increasing number of practical applications in which the value of H/D is large. Therefore, it is of interest to evaluate the performance of LES method for modelling the impinging jets with high H/D ratios. In this study, LES was carried out for H/D = 20 at Re = 28,000. The experiments performed by Rajaratnam et al. [7] have been used as the benchmark to validate the numerical model. Experimental data from Bradshaw and Love [16] and Shinneeb et al. [17] have also been used to assess the accuracy of the results. 2. GEOMETRY MODELLING In this simulation, the nozzle exit diameter is 10 mm and the distance between the nozzle and the plate is 20 cm resulting in a H/D ratio of 20. The water jet velocity exiting the nozzle is 2.86 m/s which corresponds to a Reynolds number of 28,000. To ensure that the location of the outlet boundary has negligible influence on the pressure and velocity fields, the computational domain is taken to have a radius of 0.2 m along the plate. In order to mimic the experimental setup, the water is allowed to escape to the ambient through the side boundaries of the computational domain. Therefore, these boundaries are set as pressure outlets. The plate is considered to be a no slip boundary. Three different mesh sizes were used to satisfy the mesh requirement for LES, as discussed below. Details of the computational domain and mesh generated for one of the LES cases are shown in Figs. 2, 3, and 4. The full 3D geometry including the boundary conditions are illustrated in Fig. 2. The fully structured mesh system and surface mesh over the plate are shown in Fig. 3 and 4, respectively. The flow over the wall can be either resolved or modeled in LES by using different mesh resolution close to the wall. Since, in the current simulations, the analysis of the impingement zone is of primary interest, more emphasis is considered on the resolution of the mesh close to the wall. Chapman [18] determined that the resolution needed for the outer layer of a boundary layer is proportional to Re 0.4, while for the wall layer the number of grid points required increases by Re 1.8. The wall surface area increases rapidly with increase of the radial coordinate, resulting in a larger domain and consequently more cells. However, in the area of interest (r/d < 4.0), the mesh resolution is close to the generally approved LES criteria for wall-attached flows suggested by Piomelli and Chasnov [19], which requires that r + < 100, (r θ) + < 20 and z + < 2. The mesh resolution quality can also be evaluated by comparing the mesh size = ( r r θ z) 1/3 to the Kolmogorov length scale η = (ν 3 /ε) 1/4. Here ν is the molecular viscosity and ε is the dissipation rate estimated from our previous RANS simulation using the Realizable k ε turbulence model. For isotropic turbulence, Pope [20] has shown that a grid spacing of 12η is required in order to resolve the major contributions to the dissipation. Therefore, in the current study, attempts were made to keep the Δ/η value less than 12 in regions of interest. Further, using the recommendations from previous studies (Hadziabdic and Hanjalic [3], Piomelli [10]), three types of mesh resolution were generated. Mesh #1 includes 300 points in the axial direction, 120 points in the circumferential direction and 150 points in the radial direction. Mesh #2 contains 400 points in the axial direction, with grid points in the circumferential and radial directions kept the same as Mesh #1. Mesh #3 includes 400 grid points in axial direction, 160 points in circumpherential direction and 150 in radial direction. In all three meshes, in the radial direction, the expansion is 1.04 towards the centerline, while in circumferential direction a uniform distribution is used. The total number of cells in the three meshes is 5,400,000, 7,200,000 and 10,600,000 respectively. The simulations on three different highdensity grids require a large computational effort. The averaged time used for each simulation for each mesh on the Shared Hierarchical Academic Research Computing Network (SHARCNET) clusters was about 2 months using 28 (2.2 GHz AMD Opteron) CPUs.
3 3. NUMERICAL METHOD The governing equations used in LES are obtained by filtering the unsteady Navier-Stokes equations in Fourier space. In this method small eddies with scales smaller than the filter width are removed. The filtered equations are as following: ρ + ρu t = 0 i t ρu i + ρu i u j = μ σ ij p τ ij (2) In these equations σ ij is the stress tensor, defined by σ ij μ( u i + u j ) 2 3 μ u i δ ij (3) and τ ij is the subgrid-scale stress given by τ ij = ρu i u j ρu i u j (4) The subgrid-scale stresses resulting from the filtering operation are unknown, and require modelling. Therefore, the dynamic Smagorinsky method presented by Germano et al. [21] is used for the modelling of the subgrid-scale stresses in current simulations. Fluent 6.3 [22] was used to solve the governing equations. The third-order accurate upwind scheme QUICK (Leonard [23,24]) has been used to discretize the convective terms in the momentum equations. Timemarching is performed using a fully-implicit secondorder scheme. Based on the mesh topology presented and to satisfy the Courant number less than 1 condition for these simulations, the time step is set to be 5e-5. The time step was kept constant during the simulation. The SIMPLE algorithm was used for coupling velocity and pressure. Mean variables were determined by averaging the instantaneous results long after the simulation was started and the flow was in a fully established condition. 4. RESULTS AND DISCUSSIONS Validation of the numerical results is carried out by comparing the mean quantities with the experimental data. Time-averaging is performed on a sufficient number of periodic oscillations far after the initial condition. Figure 5 compares the normalized mean centreline velocity from the current simulations with experimental results for 10 < x/d < 25. The results from the present simulations and the experimental data follow the expected trend observed for different H/D values. Up to about x/d = 15, the flow does not get influenced by the impingement wall and essentially follows the behavior of a free jet. The model shows good agreement with the experimental data as the flow approaches the plate (region II). Figure 6 compares the mean static pressure distribution along the plate. The static pressure values are normalized by the static pressure at the stagnation point, Ps. The radial direction is normalized with r ½, which is the radial position where P = 0.5Ps. The numerical prediction obtained from the current simulation is in good agreement with the measurements by Bradshaw and Love [16] and Giralt et al. [6]. Results of these simulations show the performance of the LES method in capturing accurate flow characteristics in impinging jets with large stand-off distance. ACKNOWLEDGEMENTS This study was conducted using the facilities of the Shared Hierarchical Academic Research Computing Network (SHARCNET).This research was funded by Ontario Ministry of Research and Innovation through the Ontario Research Fund under the Green Auto Power Train project. REFERENCES [1] D.Cooper, D.C.Jackson, B.E.Launder, and G.X.Liao, "Impinging jet studies for turbulence model assessment - I. Flow-field experiments," Int. J. Heat Mass Transfer 36, 1993, pp [2] K.Nishino, M.Samada, K.Kasuya, and K.Torii, "Turbulence statistics in the stagnation region of an axisymmetric impinging jet flow," Int. J. Heat Fluid Flow 17(3), 1996, pp [3] M.Hadziabdic and K.Hanjalic, "Vortical structures and heat transfer in a round impinging jet," J. Fluid Mech. 596, 2008, pp [4] S.Beltaos and N.Rajaratnam, "Impinging circular turbulent jets,"j. Hydraul. Eng. ASCE 100, 1974,pp [5] S.Beltaos and N.Rajaratnam, "Impingement of axisymmetric developing jets,"j. Hydraul. Res.15(4), 1977, pp [6] F.Giralt, C.Chia, and O.Trass, "Characterization of the impingement region in an axisymmetric turbulent jet," Ind. Eng. Chem. Fund. 16(1), 1977, pp [7] N.Rajaratnam, D.Z.Zhu, and S.P.Rai, "Turbulence measurements in the impinging region of a circular jet," Can. J. Civ. Eng. 37(5), 2010, pp [8] Second ERCOFTAC-IAHR Workshop on Refined Modelling, "Round normally impinging turbulent jet and turbulent flow through tube bank subchannel," 16th Meeting of the IAHR Working Group on Refined Flow Modelling, 1993, University of Manchester Inst. of Sci. and Tech., UK. [9] T.Craft, L.Graham, and B.E.Launder, "Impinging jet studies for turbulence model assessment - II.
4 An examination of the performance of four turbulence models," Int. J. Heat Mass Transfer 36, 1993, pp [10].U.Piomelli, "Large-eddy simulation: achievements and challenges," Progress in Aerospace Sciences 35, 1999, pp [11] Y.M.Chung, K.H.Luo, and N.D.Sandham, "Numerical study of momentum and heat transfer in unsteady impinging jets," Int. J. Heat Fluid Flow 23, 2002, pp [12] H.Hattori and Y.Nagano, "Direct numerical simulation of turbulent heat transfer in plane impinging jet," Int. J. Heat Fluid Flow 25, 2004, pp [13] M.Tsubokura, T.Kobayashi, N.Taniguchi, and W.P. Jones, "A numerical study on the eddy structures of impinging jets excited at the inlet," Int. J. Heat Fluid Flow 24, 2003, pp [14] P.R.Voke and S.Gao, "Numerical study of heat transfer from an impinging jet," Int. J. Heat Mass Transfer 41, 1998, pp [15] F.Beaubert and S.Viazzo, "Large eddy simulation of plane turbulent impinging jets at moderate Reynolds numbers,". Int. J. Heat Fluid Flow 24, 2003, pp [16] P.Bradshaw and E.M.Love, "The normal impingement of a circular air jet over a flat surface,"arc R&M,3205, [17] A.M.Shinneeb, J.D.Bugg, and R. Balachandar, "Quantitative investigation of vortical structures in the near-exit region of an axisymmetric turbulent jet," J. Turbul. 9(19), 2008, pp [18] D.R. Chapman, Computational aerodynamics development and outlook, AIAA J. 17(12), 1979, [19] U. Piomelli and J. R.Chasnov, "Large-eddy simulations: theory and applications. In Transition and Turbulence Modelling," (eds. A. Henningson, K. Hallback, L. Alfredsson & M. Johansson). Kluwer, [20] S.B.Pope, "Turbulent Flows," Cambridge University Press, [21] M. Germano, U. Piomelli, P. Moin, W.H. Cabot, "A dynamic subgrid-scale eddy viscosity model,"phys. Fluids A3, 1991, p [22] FLUENT 6.3 User s Guide, FLUENT Inc., Lebanon, New Hampshire, USA. [23] B.P.Leonard, "A stable and accurate convective modelling procedure based on quadratic upstream interpolation," Comput Meth. Appl. Mech. Engng. 19, 1979, pp [24] B.P.Leonard, "Simple high-accuracy resolution program for convective modelling of discontinuities," Intl J. Numer Meth. Fluids 8, 1988, pp D Jet from nozzle Core jet Free jet region I Impingement region II Wall jet region III Fig. 1. Definition sketch of impinging circular jet Fig. 2. Domain dimensions and boundary conditions
5 P/Ps Fig. 3. Fully structured generated mesh Fig. 4. Generated face mesh over the plate Shinneeb et al. (2008), free jet Rajaratnam et al. (2010), H/D=18.5 LES, mesh #3, H/D=20 U C /U j x/d Fig. 5. Normalized mean centreline velocity r/r 1/2 Fig. 6. Normalized mean static pressure along the wall Bradshaw & Love (1961), H/D=21 Giralt et al. (1977), H/D=22 LES, mesh#3, H/D=20
Large 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 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 informationON THE NUMERICAL MODELING OF IMPINGING JET HEAT TRANSFER
ON THE NUMERICAL MODELING OF IMPINGING JET HEAT TRANSFER Mirko Bovo 1,2, Sassan Etemad 2 and Lars Davidson 1 1 Dept. of Applied Mechanics, Chalmers University of Technology, Gothenburg, Sweden 2 Powertrain
More 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 informationMOMENTUM AND HEAT TRANSPORT INSIDE AND AROUND
MOMENTUM AND HEAT TRANSPORT INSIDE AND AROUND A CYLINDRICAL CAVITY IN CROSS FLOW G. LYDON 1 & H. STAPOUNTZIS 2 1 Informatics Research Unit for Sustainable Engrg., Dept. of Civil Engrg., Univ. College Cork,
More 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 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 informationInviscid Flows. Introduction. T. J. Craft George Begg Building, C41. The Euler Equations. 3rd Year Fluid Mechanics
Contents: Navier-Stokes equations Inviscid flows Boundary layers Transition, Reynolds averaging Mixing-length models of turbulence Turbulent kinetic energy equation One- and Two-equation models Flow management
More 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 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 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 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 informationLarge Eddy Simulation of Turbulent Flow Past a Bluff Body using OpenFOAM
Large Eddy Simulation of Turbulent Flow Past a Bluff Body using OpenFOAM A Thesis Presented By David Joseph Hensel To The Department of Mechanical and Industrial Engineering in partial fulfillment of the
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 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 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 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 informationInvestigation of cross flow over a circular cylinder at low Re using the Immersed Boundary Method (IBM)
Computational Methods and Experimental Measurements XVII 235 Investigation of cross flow over a circular cylinder at low Re using the Immersed Boundary Method (IBM) K. Rehman Department of Mechanical Engineering,
More informationNumerical 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 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 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 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 informationNear Field and Far Field Prediction of Noise in and around a Loudspeaker: A Numerical and Experimental Investigation
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
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 informationStrömningslära Fluid Dynamics. Computer laboratories using COMSOL v4.4
UMEÅ UNIVERSITY Department of Physics Claude Dion Olexii Iukhymenko May 15, 2015 Strömningslära Fluid Dynamics (5FY144) Computer laboratories using COMSOL v4.4!! Report requirements Computer labs must
More informationDES Turbulence Modeling for ICE Flow Simulation in OpenFOAM
2 nd Two-day Meeting on ICE Simulations Using OpenFOAM DES Turbulence Modeling for ICE Flow Simulation in OpenFOAM V. K. Krastev 1, G. Bella 2 and G. Campitelli 1 University of Tuscia, DEIM School of Engineering
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 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 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 informationMicrowell Mixing with Surface Tension
Microwell Mixing with Surface Tension Nick Cox Supervised by Professor Bruce Finlayson University of Washington Department of Chemical Engineering June 6, 2007 Abstract For many applications in the pharmaceutical
More informationCFD Best Practice Guidelines: A process to understand CFD results and establish Simulation versus Reality
CFD Best Practice Guidelines: A process to understand CFD results and establish Simulation versus Reality Judd Kaiser ANSYS Inc. judd.kaiser@ansys.com 2005 ANSYS, Inc. 1 ANSYS, Inc. Proprietary Overview
More informationCFD STUDY OF MIXING PROCESS IN RUSHTON TURBINE STIRRED TANKS
Third International Conference on CFD in the Minerals and Process Industries CSIRO, Melbourne, Australia 10-12 December 2003 CFD STUDY OF MIXING PROCESS IN RUSHTON TURBINE STIRRED TANKS Guozhong ZHOU 1,2,
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 informationMASSACHUSETTS INSTITUTE OF TECHNOLOGY. Analyzing wind flow around the square plate using ADINA Project. Ankur Bajoria
MASSACHUSETTS INSTITUTE OF TECHNOLOGY Analyzing wind flow around the square plate using ADINA 2.094 - Project Ankur Bajoria May 1, 2008 Acknowledgement I would like to thank ADINA R & D, Inc for the full
More 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 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 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 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 informationLARGE EDDY SIMULATION OF VORTEX SHEDDING WITH TRIANGULAR CYLINDER AHEAD OF A SQUARE CYLINDER
The Eighth Asia-Pacific Conference on Wind Engineering, December 10 14, 2013, Chennai, India LARGE EDDY SIMULATION OF VORTEX SHEDDING WITH TRIANGULAR CYLINDER AHEAD OF A SQUARE CYLINDER Akshoy Ranjan Paul
More 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 informationComparison Between Numerical & PIV Experimental Results for Gas-Solid Flow in Ducts
Fabio Kasper Comparison Between Numerical & PIV Experimental Results for Gas-Solid Flow in Ducts Rodrigo Decker, Oscar Sgrott Jr., Henry F. Meier Waldir Martignoni Agenda Introduction The Test Bench Case
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 informationCFD SIMULATION OF FLOW OVER CONTRACTED COMPOUND ARCHED RECTANGULAR SHARP CRESTED WEIRS
INTERNATIONAL JOURNAL OF OPTIMIZATION IN CIVIL ENGINEERING Int. J. Optim. Civil Eng., 2014; 4(4):549-560 CFD SIMULATION OF FLOW OVER CONTRACTED COMPOUND ARCHED RECTANGULAR SHARP CRESTED WEIRS A. Samadi
More informationDevelopment of New Method for Flow Computations in Vehicle Ventilation
2005:110 CIV MASTER S THESIS Development of New Method for Flow Computations in Vehicle Ventilation FRIDA NORDIN MASTER OF SCIENCE PROGRAMME Luleå University of Technology Department of Applied Physics
More informationNumerical Simulation of Flow around a Spur Dike with Free Surface Flow in Fixed Flat Bed. Mukesh Raj Kafle
TUTA/IOE/PCU Journal of the Institute of Engineering, Vol. 9, No. 1, pp. 107 114 TUTA/IOE/PCU All rights reserved. Printed in Nepal Fax: 977-1-5525830 Numerical Simulation of Flow around a Spur Dike with
More informationInvestigation of the Effect of a Realistic Nozzle Geometry on the Jet Development
Investigation of the Effect of a Realistic Nozzle Geometry on the Jet Development Mehmet Onur Cetin a, Matthias Meinke a,b, Wolfgang Schröder a,b Abstract Highly resolved large-eddy simulations (LES) of
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 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 informationComputational Fluid Dynamics (CFD) for Built Environment
Computational Fluid Dynamics (CFD) for Built Environment Seminar 4 (For ASHRAE Members) Date: Sunday 20th March 2016 Time: 18:30-21:00 Venue: Millennium Hotel Sponsored by: ASHRAE Oryx Chapter Dr. Ahmad
More informationModeling and Simulation of Single Phase Fluid Flow and Heat Transfer in Packed Beds
Modeling and Simulation of Single Phase Fluid Flow and Heat Transfer in Packed Beds by:- Balaaji Mahadevan Shaurya Sachdev Subhanshu Pareek Amol Deshpande Birla Institute of Technology and Science, Pilani
More informationMESHLESS SOLUTION OF INCOMPRESSIBLE FLOW OVER BACKWARD-FACING STEP
Vol. 12, Issue 1/2016, 63-68 DOI: 10.1515/cee-2016-0009 MESHLESS SOLUTION OF INCOMPRESSIBLE FLOW OVER BACKWARD-FACING STEP Juraj MUŽÍK 1,* 1 Department of Geotechnics, Faculty of Civil Engineering, University
More informationPressure Drop Evaluation in a Pilot Plant Hydrocyclone
Pressure Drop Evaluation in a Pilot Plant Hydrocyclone Fabio Kasper, M.Sc. Emilio Paladino, D.Sc. Marcus Reis, M.Sc. ESSS Carlos A. Capela Moraes, D.Sc. Dárley C. Melo, M.Sc. Petrobras Research Center
More information3D-Numerical Simulation of the Flow in Pool and Weir Fishways Hamid Shamloo*, Shadi Aknooni*
XIX International Conference on Water Resources CMWR 2012 University of Illinois at Urbana-Champaign June 17-22, 2012 3D-Numerical Simulation of the Flow in Pool and Weir Fishways Hamid Shamloo*, Shadi
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 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 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 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 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 informationWALL Y + APPROACH FOR DEALING WITH TURBULENT FLOW OVER A SURFACE MOUNTED CUBE: PART 2 HIGH REYNOLDS NUMBER
Seventh International Conference on CFD in the Minerals and Process Industries CSIRO, Melbourne, Australia 9- December 9 WALL Y + APPROACH FOR DEALING WITH TURBULENT FLOW OVER A SURFACE MOUNTED CUBE: PART
More informationISSN(PRINT): ,(ONLINE): ,VOLUME-1,ISSUE-1,
NUMERICAL ANALYSIS OF THE TUBE BANK PRESSURE DROP OF A SHELL AND TUBE HEAT EXCHANGER Kartik Ajugia, Kunal Bhavsar Lecturer, Mechanical Department, SJCET Mumbai University, Maharashtra Assistant Professor,
More 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 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 informationReproducibility of Complex Turbulent Flow Using Commercially-Available CFD Software
Reports of Research Institute for Applied Mechanics, Kyushu University No.150 (71 83) March 2016 Reproducibility of Complex Turbulent Flow Using Commercially-Available CFD Software Report 3: For the Case
More 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 informationModeling a Nozzle in a Borehole
Modeling a Nozzle in a Borehole E. Holzbecher, F. Sun Georg-August Universität Göttingen *Goldschmidtstr. 3, 37077 Göttingen, GERMANY; E-mail: eholzbe@gwdg.de Abstract: A nozzle, installed in an injecting
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 informationOPTIMISATION OF PIN FIN HEAT SINK USING TAGUCHI METHOD
CHAPTER - 5 OPTIMISATION OF PIN FIN HEAT SINK USING TAGUCHI METHOD The ever-increasing demand to lower the production costs due to increased competition has prompted engineers to look for rigorous methods
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 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 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 informationSimulation and Validation of Turbulent Pipe Flows
Simulation and Validation of Turbulent Pipe Flows ENGR:2510 Mechanics of Fluids and Transport Processes CFD LAB 1 (ANSYS 17.1; Last Updated: Oct. 10, 2016) By Timur Dogan, Michael Conger, Dong-Hwan Kim,
More informationTHE APPLICATION OF AN ATMOSPHERIC BOUNDARY LAYER TO EVALUATE TRUCK AERODYNAMICS IN CFD
THE APPLICATION OF AN ATMOSPHERIC BOUNDARY LAYER TO EVALUATE TRUCK AERODYNAMICS IN CFD A SOLUTION FOR A REAL-WORLD ENGINEERING PROBLEM Ir. Niek van Dijk DAF Trucks N.V. CONTENTS Scope & Background Theory:
More informationDriven Cavity Example
BMAppendixI.qxd 11/14/12 6:55 PM Page I-1 I CFD Driven Cavity Example I.1 Problem One of the classic benchmarks in CFD is the driven cavity problem. Consider steady, incompressible, viscous flow in a square
More informationALE Seamless Immersed Boundary Method with Overset Grid System for Multiple Moving Objects
Tenth International Conference on Computational Fluid Dynamics (ICCFD10), Barcelona,Spain, July 9-13, 2018 ICCFD10-047 ALE Seamless Immersed Boundary Method with Overset Grid System for Multiple Moving
More informationPUBLISHED VERSION. Originally Published at: PERMISSIONS. 23 August 2015
PUBLISHED VERSION Yinli Liu, Hao Tang, Zhaofeng Tian, Haifei Zheng CFD simulations of turbulent flows in a twin swirl combustor by RANS and hybrid RANS/LES methods Energy Procedia, 2015 / Jiang, X., Joyce,
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 informationSIMULATION OF FLOW AROUND KCS-HULL
SIMULATION OF FLOW AROUND KCS-HULL Sven Enger (CD-adapco, Germany) Milovan Perić (CD-adapco, Germany) Robinson Perić (University of Erlangen-Nürnberg, Germany) 1.SUMMARY The paper describes results of
More informationA Study of the Development of an Analytical Wall Function for Large Eddy Simulation of Turbulent Channel and Rectangular Duct Flow
University of Wisconsin Milwaukee UWM Digital Commons Theses and Dissertations August 2014 A Study of the Development of an Analytical Wall Function for Large Eddy Simulation of Turbulent Channel and Rectangular
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 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 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 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 informationNumerical Simulation of Fuel Filling with Volume of Fluid
Numerical Simulation of Fuel Filling with Volume of Fluid Master of Science Thesis [Innovative and Sustainable Chemical Engineering] Kristoffer Johansson Department of Chemistry and Bioscience Division
More informationAssessment of the numerical solver
Chapter 5 Assessment of the numerical solver In this chapter the numerical methods described in the previous chapter are validated and benchmarked by applying them to some relatively simple test cases
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 informationEffect of Turbulence Model in Numerical Simulation of Single Round Jet at Low Reynolds Number
ISSN (e): 2250 3005 Volume, 07 Issue, 03 March 2017 International Journal of Computational Engineering Research (IJCER) Effect of Turbulence Model in Numerical Simulation of Single Round Jet at Low Reynolds
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 informationNUMERICAL SIMULATION OF THE WIND FLOW AROUND A CUBE IN CHANNEL
BBAA VI International Colloquium on: Bluff Bodies Aerodynamics & Applications Milano, Italy, July, 0-4 008 NUMERICAL SIMULATION OF THE WIND FLOW AROUND A CUBE IN CHANNEL Mohammad Omidyeganeh and Jalal
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 informationRANSE Simulations of Surface Piercing Propellers
RANSE Simulations of Surface Piercing Propellers Mario Caponnetto, Rolla Research, mariocaponnetto@hotmail.com RANSE methods have been applied to the analysis of ship propellers in open-water condition
More informationVI Workshop Brasileiro de Micrometeorologia
Validation of a statistic algorithm applied to LES model Eduardo Bárbaro, Amauri Oliveira, Jacyra Soares November 2009 Index Objective 1 Objective 2 3 Vertical Profiles Flow properties 4 Objective 1 The
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 informationDispersion of rod-like particles in a turbulent free jet
Test case Dispersion of rod-like particles in a turbulent free jet 1. MOTIVATION: Turbulent particle dispersion is a fundamental issue in a number of industrial and environmental applications. An important
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 informationQUASI-3D SOLVER OF MEANDERING RIVER FLOWS BY CIP-SOROBAN SCHEME IN CYLINDRICAL COORDINATES WITH SUPPORT OF BOUNDARY FITTED COORDINATE METHOD
QUASI-3D SOLVER OF MEANDERING RIVER FLOWS BY CIP-SOROBAN SCHEME IN CYLINDRICAL COORDINATES WITH SUPPORT OF BOUNDARY FITTED COORDINATE METHOD Keisuke Yoshida, Tadaharu Ishikawa Dr. Eng., Tokyo Institute
More informationTutorial 2. Modeling Periodic Flow and Heat Transfer
Tutorial 2. Modeling Periodic Flow and Heat Transfer Introduction: Many industrial applications, such as steam generation in a boiler or air cooling in the coil of an air conditioner, can be modeled as
More informationA Framework for Coupling Reynolds-Averaged With Large-Eddy Simulations for Gas Turbine Applications
J. U. Schlüter X. Wu S. Kim S. Shankaran J. J. Alonso H. Pitsch Center for Turbulence Research and Aerospace Computing Lab, Stanford University, Stanford, CA 94305-3030 A Framework for Coupling Reynolds-Averaged
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 informationProgram: Advanced Certificate Program
Program: Advanced Certificate Program Course: CFD-Vehicle Aerodynamics Directorate of Training and Lifelong Learning #470-P, Peenya Industrial Area, 4th Phase Peenya, Bengaluru 560 058 www.msruas.ac.in
More informationLarge Eddy Simulation (LES) for Steady-State Turbulent Flow Prediction
Large Eddy Simulation (LES) for Steady-State Turbulent Flow Prediction T. Ganesan and M. Awang Abstract The aim of this work is to simulate a steady turbulent flow using the Large Eddy Simulation (LES)
More information