CFD PREDICTION OF WIND PRESSURES ON CONICAL TANK
|
|
- Isabella Greene
- 5 years ago
- Views:
Transcription
1 CFD PREDICTION OF WIND PRESSURES ON CONICAL TANK T.A.Sundaravadivel a, S.Nadaraja Pillai b, K.M.Parammasivam c a Lecturer, Dept of Aeronautical Engg, Satyabama University, Chennai, India, aerovelu@yahoo.com b PhD Research Scholar, WERC, Tokyo Polytechnic University, Japan. c JSPS fellow, WERC, Tokyo Polytechnic University, Japan ABSTRACT Computational analysis was performed using versatile fluid analysis software. The analysis was made in an unsteady three-dimensional turbulent flow with SST k-? as a turbulence model. Wind pressures on a conical tank have been predicted from this study. On the leeward side, strong intensity of RMS pressures are observed. This is consistent with RMS velocities on the same section. Conical water tank has a complex geometry, for which CFD is applied and results are validated with the experimental data for the mean pressure coefficients. Predicted mean pressure coefficients from the computational study were found to be in reasonably good agreement with experimental values for the tank, except in wake regions. Key Words: Computational analysis, Fluent 6.2, SST k-? model, Pressure?uctuations, conical water tank INTRODUCTION Developments in software and computer hardware have given increased impetus to the use of computer modeling research in recent years. If numerical simulations are used, need for validation arises for the results to be of practical use. Predictions can be validated against analytical solutions or data taken from experiments. Analytical solutions to standard problems can be found in the literature for many cases but to?nd existing experimental data that suit the problem under study can be difficult. However, for most practical problems no standard analytical solution exists and recourse to experimental data is required. Pressure?uctuations on bluff bodies have received a great deal of attention in recent years because they cause wind noise and structural damage. The knowledge can be obtained by experimental studies or computational studies. Performing an experimental study to understand the nature of pressure?uctuations is hard due to the sensitivity of pressure?uctuations to the size of the probe. An alternative approach is to develop a computational model that can simulate the?ow and predict the parameters of interest. Water tanks are tall, slender, non aerodynamic bodies with large mass on top and they are erected in all kinds of terrains to ensure adequate water supply to homes and industrial buildings. Scant information is available so far for 1
2 evaluation of the flow field and the aerodynamic loads on water tank towers or similar tall structures of variable cross section. Nowadays Computational modeling has become a powerful tool for wind engineering studies, which provides more precise information about the flow field over the complete structure. Moreover the flow field can be visualized and a better understanding can be gained using the CFD in addition to the wind tunnel tests. Flow field behind the structures such as the manner of vortex shedding etc can be better visualized in CFD studies. In the last three decades, extensive research work has been reported in the literature on flow past non-streamlined bodies because of its wide spread application in variety of engineering problems. Computational Wind Engineering has evolved as a new branch of Computational Fluid Dynamics (CFD) in the last two decades for evaluation of the interaction between wind and buildings numerically through mathematical modeling. THE EXPERIMENTAL STUDY Conical water tank towers were chosen for this study because of their failure due to cyclones on Shriharikota Island in Venkateswaralu et. al. (2007) discussed the reasons for the failure of the water tank on Sriharikota from the structural design viewpoint. In the experiments carried out by Parammasivam etal (2005 & 2007) in a boundary layer wind tunnel having a test section of 2.2m W x 1.8m H x 19m L, free stream velocity was fixed at 10 m/s at the tip of the water tower model and the corresponding Reynolds Number was based on the shaft diameter for a = The conical tower model was fabricated from acrylic material to a 1:200 scale with 168 pressure taps on 11 levels along the height of the tower as shown in Fig. 1(84 on both shaft-bottom and top-cone sections). It was reported that Cp rms in the stagnation region is approximately proportional to the turbulence intensity of the approaching flow for smooth cylindrical surface, and has a peak at a point around the minimum pressure coefficient. The Cp (mean and rms) distributions for the conical water tank at various levels plotted from experimental data are shown in Figs. 2 to 5. THE COMPUTATIONAL STUDY The model used by Parammasivam et. al. (2005 & 2007) for the experiment is used for the present computational study, in which the SST k-? turbulence model is a two-equation eddy viscosity model which has become very popular. The use of k-? formulation in the inner parts of the boundary layer makes it directly usable all the way down to the wall through the viscous sub layer. Hence the SST k-? model can be used as a low Reynolds Number turbulence model without any extra damping functions. The SST formulation also switches to a k-e behavior in the free stream and thereby avoids the common k-? problem that the model is too sensitive to inlet free stream proprieties. Authors 2
3 who use the SST k-? model often merit it for its good behavior in adverse pressure gradients and separating flow. The SST k-? model produces a bit too large turbulence levels in regions with normal strain, like stagnation regions and regions with strong acceleration. In the conical tower surface and wall, the velocity components u, v & w are set to zero. At Inlet 1, u = U1 and at Inlet 2, u = U. At the outlet of the mesh, pressure is set to zero, which denotes the atmospheric pressure. Were u = Velocity component in the x-direction, v = Velocity component in the y-direction, w = Velocity component in the z-direction, U1= velocity profile corresponding to 0.27 power law coefficient & U = constant velocity. The computational domain is discretized in to 6, 52, 875 nodes, 6, 29, 676 cells and 19, 12, 006 faces. The inlet of the computational domain is discretized into two sections as inlet 1 and inlet 2. Inlet 1 is used to introduce the velocity profile using an UDF (User Defined Function) corresponding to the power law coefficient of 0.27 and inlet 2 has uniform velocity as obtained from the inlet 1 at corresponding height. The computational domain for the study is shown in Fig. 6. The shaft portion is divided into 36 divisions circumferentially and 25 divisions longitudinally. The cone section is divided into 36 divisions circumferentially and 15 divisions longitudinally. Finer mesh is made near the model and the coarseness of the mesh is increased away from the model as shown in Fig. 7. CFD PREDICTION OF WIND PRESSURES In spite of vast research material available on flow past simple circular cylinder, our understanding of the complex fluid mechanics for flow past circular cylinders at Reynolds numbers in excess of a few hundred thousand still remains incomplete. The computational analysis was performed using the versatile fluid analysis software package Fluent 6.2 using the finite volume method. The analysis was made in unsteady three-dimensional turbulent flow. The SST k-? model was used as a turbulent model for the present study. The existing experimental data by Parammasivam et. al. (2005 & 2007) has been used for the comparison of the CFD data. At the inlet, the velocity profile was introduced with the power law coefficient of 0.27, same as in the experiments. At the base of the shaft two clear symmetrical vortices are observed in contour plots as shown in Figs. 8 and 9 with less intensity of fluctuating velocities. It is expected that the flow is symmetrical with respect to the low velocity at the bottom of the model. The two vortices are formed at the leeward face of the model. It is clearly observed from Figs. 10 and 11. Vortices get mixed as the shaft height increases and near shaft-cone intersection (z/h = 0.73) two vortices are formed along with the shear layers from the cone. The predicted pressure coefficients and the RMS pressures on the conical tank are shown as contour plots in Figs. 12 and 13. On the leeward side of 3
4 the cone section strong intensity of RMS pressures are observed. This is consistent with RMS velocities on the cone section. The shear layers over the cone form two distinct vortices on the leeward side of the cone surface and it is shown in the Fig. 13. The plots of mean Cp vs circumferential angle for the 3 typical levels of the shaft (z/h = 0.1, 0.4 & 0.68) are shown in Figs. 14, 15 & 16 and similar plots for the cone sections (z/h = 0.73, 0.91&0.97) are shown in Figs. 17 to 19 along with the experimental results. It is clear that the predicted patterns of pressure coefficients from the computational study are found to be in reasonably good agreement for the conical tower except at circumferential angles from 90 degrees to 270 degrees. At 90 degrees to 270 degrees of the conical tank, the SST k-? model could not match the experimental data due to the vortices and turbulent nature of the flow field and finer mesh is needed at these regions to catch the wake. RMS pressures had peaks on the leeward side of the cone surfaces. The predicted profile coincides with the experimental one in both base levels (Fig. 14) as well as the levels at the cone surfaces (Figs ). The minimum value of mean Cp is found at the two locations approx at 80 degrees and 280 degrees from the wind flow direction. The result indicates that the flow separates from those points (80 degrees and 280 degrees). This agrees with the theory. Flow over the cone section of water tank tower is three-dimensional as against the shaft section, and can be considered as 2-D flow. CONCLUSIONS The adopted solution method for the velocity pressure fields was the SIMPLE Algorithm (Semi-Implicit Method for Pressure Linked Equations). PISO- Pressure Implicit Split operator can be used to improve the accuracy of the pressure filed. Some characteristics of the vertical structures of the shear layer behind the conical tower have been examined and it is found that two strong vortices are formed on the leeward faces. In order to enhance the stability of the solution process, under-relaxation techniques were applied to all the equations. Otherwise iteration may diverge. A finer mesh is required in the vicinity of walls and ground in order to accurately resolve the high-gradient regions of the flow field. One of the main problems in turbulence modeling is the accurate prediction of flow separation from a smooth surface. The k-? based Shear Stress Transport (SST) model was designed to give highly accurate predictions of the onset and the amount of flow separation under adverse pressure gradients by the inclusion of transport effects into the formulation of the eddy- viscosity. Due to the complex nature of the water tank structure and the inlet velocity profile, flow in the leeward side of the model will be highly turbulent and large eddy formation takes place. As mentioned by Lars Davidson (2003), the eddy viscosity models are simple due to the use of an isotropic eddy (turbulent) viscosity and as a consequence of the above; the model is found to be unable to account for curvature effects. So the results show that the k-? based Shear Stress Transport (SST) model is less effective in predicting the wake region in this study. For better accuracy of results, future study can be conducted using 4
5 Reynolds Stress model or LES (with a higher configuration computer system/ workstation) in which the above mentioned problem can be solved with the aid of finer mesh in the vicinity of walls. The mean flow characteristics appear to have been captured by the computational modeling, which attests the reasonability of the approach for the study. NOTATION a Power Law Coefficient u Velocity component in the x direction (m/s) v Velocity component in the y direction (m/s) w Velocity component in the z direction (m/s) mean Cp Mean Coefficient of pressure rms Cp rms coefficient of pressure z/h Ratio of height of a section to overall height of the water tank. REFERENCES 1. Bergstrom, Derksen and Rezkallah (1993), Numerical study of wind flow over a cooling tower J. Wind Eng. Ind. Aerodyn., Vol. 46, pp Fluent, Fluent 6 User s Guide2, Fluent INC., Lebanon, U.S.A, Fujisawa, Asano, Arakawa and Hashimoto (2005), Computational and experimental study on flow around a rotationally oscillating cylinder in a uniform flow J. Wind Eng. Ind. Aerodyn., Vol. 93, Gao and Chow (2005), Numerical studies on airflow around a cube, J. Wind Eng. Ind. Aerodyn., Vol.93, pp Lars Davidson (2003), An Introduction to Turbulence models Publication 97/2, Dept. of Thermo and Fluid Dynamics, Chalmers University of Tech., GÖteborg, Sweden 6. Parammasivam and Yukio Tamura (2007), Aerodynamic characteristics of a conical water tank, Proceedings of 2007 Annual Meeting, Japan Society of Fluid Mechanics, Japan, pp Parammasivam (2005), Wind Tunnel Studies on Water Tank Tower with Terrain Simulation, Ph.D. Thesis, Anna University, Chennai. 8. Paterson (1993), Predicting rms pressure from computed velocities and mean pressures, J. Wind Eng. Ind. Aerodyn., Vol. 46, pp Reichrath and Davies (2002), Computational fluid dynamics simulations and validation of the pressure distribution on the roof of a commercial multi-span venlo-type glass house J.Wind Eng. Ind.Aerodyn.,Vol.90, pp Senthooran,Dong-Dae Lee & Parameswaran (2004), A Computational model to calculate the flow induced pressure fluctuations on buildings J. Wind Eng. Ind. Aerodyn., Vol. 92, Venkateswaralu, Lakshmanan, Shanmugasundaram and Balakrishna Rao (1995), Failure of water tower shafts due to cyclonic winds, 9ICWE, pp
6 Fig. 4 rms Cp vs Angle for cone section (Experimental Data) Fig. 1 Model Dimensions and Levels Fig. 5 rms Cp vs Angle for shaft section (Experimental Data) Fig. 2 Mean Cp vs Angle for shaft section (Experimental Data) Fig. 6 Computational Domain and Grid System Fig. 3 Mean Cp vs Angle for cone section (Experimental Data) Fig. 7 Mesh Close to the model. 6
7 Fig.8 Contours of Velocity magnitude at z/h=0.73 Fig.9 Contours of Velocity magnitude at z/h=0.1 Fig. 10 Contours of RMS Velocity (m/s) at z/h=0.73 7
8 Fig. 11 Contours of RMS Velocity (m/s) at z/h=0.1 Fig.12 Contours of Pressure Coefficient Fig.13 Contours of RMS Static Pressure (pascal) 8
9 Fig.14 Mean Cp vs Angle at z/h = 0.1 Fig.15 Mean Cp vs Angle at z/h = 0.4 Fig. 16 Mean Cp vs Angle at z/h =
10 Fig. 17 Mean Cp vs Angle at z/h = 0.73 Fig.18 Mean Cp vs Angle at z/h = 0.91 Fig.19 Mean Cp vs Angle at z/h =
CFD 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 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 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 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 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 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 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 informationAssessment of Turbulence Models for Flow around a Surface-Mounted Cube
Assessment of Turbulence Models for Flow around a Surface-Mounted Cube Sercan Dogan, Sercan Yagmur, Ilker Goktepeli, and Muammer Ozgoren Selcuk University, Konya, Turkey Email: {sercandogan, syagmur, ilkergoktepeli}@selcuk.edu.tr
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 informationAnalysis of Wind Forces on a High-Rise Building by RANS-Based Turbulence Models using Computational Fluid Dynamics
Analysis of Wind Forces on a High-Rise Building by RANS-Based Turbulence Models using Computational Fluid Dynamics D.V.V. Rajkamal 1 and Ch. Raviteja 2 1 (Post graduate student, V.R. Siddhartha Engineering
More informationNUMERICAL 3D TRANSONIC FLOW SIMULATION OVER A WING
Review of the Air Force Academy No.3 (35)/2017 NUMERICAL 3D TRANSONIC FLOW SIMULATION OVER A WING Cvetelina VELKOVA Department of Technical Mechanics, Naval Academy Nikola Vaptsarov,Varna, Bulgaria (cvetelina.velkova1985@gmail.com)
More informationNumerical calculation of the wind action on buildings using Eurocode 1 atmospheric boundary layer velocity profiles
Numerical calculation of the wind action on buildings using Eurocode 1 atmospheric boundary layer velocity profiles M. F. P. Lopes IDMEC, Instituto Superior Técnico, Av. Rovisco Pais 149-1, Lisboa, Portugal
More 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 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 informationComputational Simulation of the Wind-force on Metal Meshes
16 th Australasian Fluid Mechanics Conference Crown Plaza, Gold Coast, Australia 2-7 December 2007 Computational Simulation of the Wind-force on Metal Meshes Ahmad Sharifian & David R. Buttsworth Faculty
More informationDetached Eddy Simulation Analysis of a Transonic Rocket Booster for Steady & Unsteady Buffet Loads
Detached Eddy Simulation Analysis of a Transonic Rocket Booster for Steady & Unsteady Buffet Loads Matt Knapp Chief Aerodynamicist TLG Aerospace, LLC Presentation Overview Introduction to TLG Aerospace
More 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 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 informationAERODYNAMICS CHARACTERISTICS AROUND SIMPLIFIED HIGH SPEED TRAIN MODEL UNDER THE EFFECT OF CROSSWINDS
AERODYNAMICS CHARACTERISTICS AROUND SIMPLIFIED HIGH SPEED TRAIN MODEL UNDER THE EFFECT OF CROSSWINDS Sufiah Mohd Salleh 1, Mohamed Sukri Mat Ali 1, Sheikh Ahmad Zaki Shaikh Salim 1, Izuan Amin Ishak 1,
More informationSIMULATION OF PROPELLER-SHIP HULL INTERACTION USING AN INTEGRATED VLM/RANSE SOLVER MODELING.
SIMULATION OF PROPELLER-SHIP HULL INTERACTION USING AN INTEGRATED VLM/RANSE SOLVER MODELING. M.N.Senthil Prakash, Department of Ocean Engineering, IIT Madras, India V. Anantha Subramanian Department of
More 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 informationAshwin Shridhar et al. Int. Journal of Engineering Research and Applications ISSN : , Vol. 5, Issue 6, ( Part - 5) June 2015, pp.
RESEARCH ARTICLE OPEN ACCESS Conjugate Heat transfer Analysis of helical fins with airfoil crosssection and its comparison with existing circular fin design for air cooled engines employing constant rectangular
More 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 informationEstimation of Flow Field & Drag for Aerofoil Wing
Estimation of Flow Field & Drag for Aerofoil Wing Mahantesh. HM 1, Prof. Anand. SN 2 P.G. Student, Dept. of Mechanical Engineering, East Point College of Engineering, Bangalore, Karnataka, India 1 Associate
More informationTutorial 17. Using the Mixture and Eulerian Multiphase Models
Tutorial 17. Using the Mixture and Eulerian Multiphase Models Introduction: This tutorial examines the flow of water and air in a tee junction. First you will solve the problem using the less computationally-intensive
More 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 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 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 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 informationSimulation of Turbulent Flow over the Ahmed Body
Simulation of Turbulent Flow over the Ahmed Body 58:160 Intermediate Mechanics of Fluids CFD LAB 4 By Timur K. Dogan, Michael Conger, Maysam Mousaviraad, and Fred Stern IIHR-Hydroscience & Engineering
More 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 informationSPC 307 Aerodynamics. Lecture 1. February 10, 2018
SPC 307 Aerodynamics Lecture 1 February 10, 2018 Sep. 18, 2016 1 Course Materials drahmednagib.com 2 COURSE OUTLINE Introduction to Aerodynamics Review on the Fundamentals of Fluid Mechanics Euler and
More 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 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 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 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 informationCFD-1. Introduction: What is CFD? T. J. Craft. Msc CFD-1. CFD: Computational Fluid Dynamics
School of Mechanical Aerospace and Civil Engineering CFD-1 T. J. Craft George Begg Building, C41 Msc CFD-1 Reading: J. Ferziger, M. Peric, Computational Methods for Fluid Dynamics H.K. Versteeg, W. Malalasekara,
More 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 informationEffects of Buildings Layout on the Flow and Pollutant Dispersion in Non-uniform Street Canyons ZHANG Yunwei, PhD candidate
Effects of Buildings Layout on the Flow and Pollutant Dispersion in Non-uniform Street Canyons ZHANG Yunwei, PhD candidate May 11, 2010, Xi an, Shannxi Province, China E_mail: zhangyunwe@gmail.com 1 Contents:
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 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 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 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 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 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 informationViscous/Potential Flow Coupling Study for Podded Propulsors
First International Symposium on Marine Propulsors smp 09, Trondheim, Norway, June 2009 Viscous/Potential Flow Coupling Study for Podded Propulsors Eren ÖZSU 1, Ali Can TAKİNACI 2, A.Yücel ODABAŞI 3 1
More 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 informationComparison of CFD Simulation of a Hyundai I20 Model with Four Different Turbulence Models
RESEARCH ARTICLE OPEN ACCESS Comparison of CFD Simulation of a Hyundai I20 with Four Different Turbulence s M. Vivekanandan*, R. Sivakumar**, Aashis. S. Roy*** *(Uttam Industrial Engg. Pvt. Ltd., Tiruchirapalli,
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 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 informationLES Applications in Aerodynamics
LES Applications in Aerodynamics Kyle D. Squires Arizona State University Tempe, Arizona, USA 2010 Tutorial School on Fluid Dynamics: Topics in Turbulence Center for Scientific Computation and Mathematical
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 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 informationModeling Evaporating Liquid Spray
Tutorial 16. Modeling Evaporating Liquid Spray Introduction In this tutorial, FLUENT s air-blast atomizer model is used to predict the behavior of an evaporating methanol spray. Initially, the air flow
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 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 informationAN EXPERIMENTAL STUDY AND SIMULATION WITH FLUENT
AN EXPERIMENTAL STUDY AND SIMULATION WITH FLUENT OF THE HORIZONTAL AXIS WIND TURBINE (HAWT) BLADE TOWER DYNAMIC INTERACTION V. P. CAMBANIS 1 & H. STAPOUNTZIS 2 Lab. of Fluid Mechanics & Turbomachinery,
More informationCFD 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 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 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 informationComputational Flow Analysis of Para-rec Bluff Body at Various Reynold s Number
International Journal of Engineering Research and Technology. ISSN 0974-3154 Volume 6, Number 5 (2013), pp. 667-674 International Research Publication House http://www.irphouse.com Computational Flow Analysis
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 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 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 informationNumerical Study of Low Rise Building in ANSYS Fluent Ekta N Soni 1 Satyen Ramani 2
IJSRD - International Journal for Scientific Research & Development Vol. 3, Issue 03, 2015 ISSN (online): 2321-0613 Numerical Study of Low Rise Building in ANSYS Fluent Ekta N Soni 1 Satyen Ramani 2 1
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 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 informationNumerische Untersuchungen von Windkraftanlagen: Leistung, Wake und Steuerungsstrategien
Fachtagung Lasermethoden in der Strömungsmesstechnik 8. 10. September 2015, Dresden Numerische Untersuchungen von Windkraftanlagen: Leistung, Wake und Steuerungsstrategien Numerical Investigations of Wind
More informationCFD Analysis of conceptual Aircraft body
CFD Analysis of conceptual Aircraft body Manikantissar 1, Dr.Ankur geete 2 1 M. Tech scholar in Mechanical Engineering, SD Bansal college of technology, Indore, M.P, India 2 Associate professor in Mechanical
More informationCFD wake modeling using a porous disc
CFD wake modeling using a porous disc Giorgio Crasto, Arne Reidar Gravdahl giorgio@windsim.com, arne@windsim.com WindSim AS Fjordgaten 5 N-325 Tønsberg Norway Tel. +47 33 38 8 Fax +47 33 38 8 8 http://www.windsim.com
More informationACTIVE SEPARATION CONTROL WITH LONGITUDINAL VORTICES GENERATED BY THREE TYPES OF JET ORIFICE SHAPE
24 TH INTERNATIONAL CONGRESS OF THE AERONAUTICAL SCIENCES ACTIVE SEPARATION CONTROL WITH LONGITUDINAL VORTICES GENERATED BY THREE TYPES OF JET ORIFICE SHAPE Hiroaki Hasegawa*, Makoto Fukagawa**, Kazuo
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 informationIncompressible Viscous Flow Simulations Using the Petrov-Galerkin Finite Element Method
Copyright c 2007 ICCES ICCES, vol.4, no.1, pp.11-18, 2007 Incompressible Viscous Flow Simulations Using the Petrov-Galerkin Finite Element Method Kazuhiko Kakuda 1, Tomohiro Aiso 1 and Shinichiro Miura
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 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 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 informationReproducibility of Complex Turbulent Flow Using Commercially-Available CFD Software
Reports of Research Institute for Applied Mechanics, Kyushu University No.150 (47 59) March 2016 Reproducibility of Complex Turbulent Using Commercially-Available CFD Software Report 1: For the Case of
More 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 informationTutorial 1. Introduction to Using FLUENT: Fluid Flow and Heat Transfer in a Mixing Elbow
Tutorial 1. Introduction to Using FLUENT: Fluid Flow and Heat Transfer in a Mixing Elbow Introduction This tutorial illustrates the setup and solution of the two-dimensional turbulent fluid flow and heat
More informationAnalysis of Flow through a Drip Irrigation Emitter
International OPEN ACCESS Journal Of Modern Engineering Research (IJMER) Analysis of Flow through a Drip Irrigation Emitter Reethi K 1, Mallikarjuna 2, Vijaya Raghu B 3 1 (B.E Scholar, Mechanical Engineering,
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 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 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 informationEffect of suction pipe leaning angle and water level on the internal flow of pump sump
IOP Conference Series: Earth and Environmental Science PAPER OPEN ACCESS Effect of suction pipe leaning angle and water level on the internal flow of pump sump To cite this article: Z-M Chen et al 216
More informationSimulation of 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 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 informationReproducibility of Complex Turbulent Flow Using Commercially-Available CFD Software
Reports of Research Institute for Applied Mechanics, Kyushu University, No.150 (60-70) March 2016 Reproducibility of Complex Turbulent Flow Using Commercially-Available CFD Software Report 2: For the Case
More informationChapter 4: Immersed Body Flow [pp (8e), or (9e)]
Chapter 4: Immersed Body Flow [pp. 445-459 (8e), or 374-386 (9e)] Dr. Bing-Chen Wang Dept. of Mechanical Engineering Univ. of Manitoba, Winnipeg, MB, R3T 5V6 When a viscous fluid flow passes a solid body
More informationInternational Power, Electronics and Materials Engineering Conference (IPEMEC 2015)
International Power, Electronics and Materials Engineering Conference (IPEMEC 2015) Numerical Simulation of the Influence of Intake Grille Shape on the Aerodynamic Performance of a Passenger Car Longwei
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 informationUniversity of Southampton Fluid-Structure Interactions Group OpenFOAM Research
2 nd Gothenburg OpenFOAM user-group meeting Chalmers University, 14 th November 2012 University of Southampton Fluid-Structure Interactions Group OpenFOAM Research Tom Lloyd T.P.Lloyd@soton.ac.uk Marion
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 informationWONG HSI, J. J. MIAU,
Flow Separation Control with a Truncated Ellipse Airfoil in Cycling Aerodynamics WONG HSI, J. J. MIAU Department of Aeronautics and Astronautics (DAA), National Cheng Kung University, Tainan, Taiwan (R.O.C)
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 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 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 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 informationEXPERIMENTAL VALIDATION OF STAR-CCM+ FOR LIQUID CONTAINER SLOSH DYNAMICS
EXPERIMENTAL VALIDATION OF STAR-CCM+ FOR LIQUID CONTAINER SLOSH DYNAMICS Brandon Marsell a.i. solutions, Launch Services Program, Kennedy Space Center, FL 1 Agenda Introduction Problem Background Experiment
More informationAnalysis of an airfoil
UNDERGRADUATE RESEARCH FALL 2010 Analysis of an airfoil using Computational Fluid Dynamics Tanveer Chandok 12/17/2010 Independent research thesis at the Georgia Institute of Technology under the supervision
More informationHigh-Lift Aerodynamics: STAR-CCM+ Applied to AIAA HiLiftWS1 D. Snyder
High-Lift Aerodynamics: STAR-CCM+ Applied to AIAA HiLiftWS1 D. Snyder Aerospace Application Areas Aerodynamics Subsonic through Hypersonic Aeroacoustics Store release & weapons bay analysis High lift devices
More information