LARGE-EDDY SIMULATION OF AN URBAN CANOPY USING A SYNTHETIC TURBULENCE INFLOW GENERATION METHOD
|
|
- Asher Parks
- 6 years ago
- Views:
Transcription
1 Annual Journal of Hydraulic Engineering, JSCE, Vol.**, 2015, February LARGE-EDDY SIMULATION OF AN URBAN CANOPY USING A SYNTHETIC TURBULENCE INFLOW GENERATION METHOD Tobias GRONEMEIER 1, Atsushi INAGAKI 2, Micha GRYSCHKA 3 and Manabu KANDA 4 1Member of JSCE, M. Sc., Institute of Meteorology and Climatology, Leibniz Universität Hannover (Herrenhäuser Straße 2, Hannover, Germany) 2Member of JSCE, Ph. D., Department of International Development Engineering, Tokyo Institute of Technology (12-1, Ookayama 2, Meguro-ku, Tokyo 152, Japan) 3Ph. D., Institute of Meteorology and Climatology, Leibniz Universität Hannover (Herrenhäuser Straße 2, Hannover, Germany) 4Member of JSCE, Ph. D., Professor, Department of International Development Engineering, Tokyo Institute of Technology (12-1, Ookayama 2, Meguro-ku, Tokyo 152, Japan) When simulating the turbulent flow around urban structures with large-eddy simulation models it is often necessary to use non-cyclic boundary conditions in streamwise direction. In such cases a turbulent inflow condition at the inlet is favored although it is highly difficult to obtain. A synthetic turbulence generator, modelling turbulence statistics and correlations, is used to generate a turbulent inflow for large-eddy simulations. Results are compared with simulations using laminar inflow. An artificial urban canopy consisting of aligned buildings with cubical shape was used. Two simulations contained one additional tall building located at the center of the domain. The turbulence statistics show a well-developed urban boundary layer above the building arrays for each simulation. Higher turbulence intensity was found when using the turbulence inflow method resulting in faster development of an urban boundary layer. Key Words : large-eddy simulation, synthetic turbulence, turbulent inflow, urban canopy 1. INTRODUCTION When using large-eddy simulation (LES) models it is a common technique to use cyclic boundary conditions for the horizontal boundaries of the simulation domain. However, if a structure such as a single building is present in the simulation domain, cyclic boundaries would cause that the simulated flow will see an infinite array of the same building in each horizontal direction rather than a single building. So, if the flow around an isolated structure like a single building or a part of a real urban canopy needs to be simulated, open boundary conditions rather than cyclic conditions have to be used in the LES model. Open boundaries, however, have the disadvantage that the user has to define the inflow. The easiest way to define an inflow condition would be a constant non-turbulent flow. But, to get realistic results for the turbulent motions around the obstacles of interest, the flow has to be turbulent, as it would be the case in a real atmospheric situation, before it hits those obstacles. Therefore, a wide turbulence generation area has to be added to the simulation domain in front of the obstacles of interest where the laminar flow from the inflow boundary forms into a well-developed turbulent flow. Hence, laminar inflow conditions require a distinct larger domain which leads to a significant increase of computation time and cost. In the past many studies were carried out to find a way to provide a realistic turbulent flow at the inflow boundary to minimize the needed simulation domain and therefore the computation time and so the cost of a simulation. In this study a synthetic turbulence inflow generation method designed by Xie and Castro 1) and optimized by Kim et al. 2) will be used to simulate an urban boundary layer over an array of cubes and one tall building in the center of the domain with noncyclic boundary conditions. The objective of this study is to show the advantages of using this synthetic turbulence inflow generator over a laminar inflow.
2 The following chapter will give a short introduction to the used LES model and the synthetic turbulence inflow generator. In chapter 3 the simulation setup is described and the results of four cases differing in inflow conditions and topography are shown. At the end the conclusions will be drawn in chapter SIMULATION TECHNIQUE (1) PALM The parallelised LES model PALM 3), version 3.10 revision 1466, was used to carry out the simulations for this study. PALM is open source software and the code can be accessed under palm.muk.uni-hannover.de/browser/?rev=1466. The model solves the non-hydrostatic incompressible Boussinesq equations using a fifth-order advection scheme of Wicker and Skamarock 4) and a third-order Runge-Kutta 5) scheme for time step. Topography is added by using a masking method based on the method of Kanda et al. 6). At first the prognostic equations are solved without considering the topography and in a second step the wall-normal velocities at the edge of the obstacles are set to zero 7). (2) Inflow method A synthetic turbulence inflow generation method developed by Xie and Castro 1) is used for the inflow boundary condition. At the inlet unscaled turbulent disturbances u i containing correlations in space and time are added to the mean wind velocity profiles U i u i = U i + a ij u j, (1) where i, j {1,2,3}, u i is the instantaneous wind velocity, and a ij is the amplitude tensor derived from the Reynolds stress tensor R ij by a transformation after Lund et al. 8) a ij = (2) 0.5 R ( 1 R 21 a 11 (R 22 a 2 21 ) ). 1 1 R 31 a 11 (R 32 a 21 a 31 )a 22 (R 33 a 2 31 a 2 32 ) 0.5 The turbulent disturbances were derived using a filter function 2n 0.5 b i = b i ( 2 b k ), (3a) k= 2n b k = exp ( π k ), (3b) n where n = L / Δx, Δx is the grid size, and L is the length scale. A spatial correlation for a two dimensional slice at the inlet is then generated by 2n 2n ψ m,l = b j b k r m+j,l+k, (4) j= 2n k= 2n where r m,l is a set of random number with zero mean and unit variance. The two dimensional data ψ m,l is then correlated in time with the disturbance of the previous time step forming the new velocity disturbance u i (t + t) = u i (t) exp ( π t 2T ) + ψ i (t) [1 exp ( π t T )] 0.5, (5) where T is the Lagrangian time scale. The modification Kim et al. 2) provided for this method is the mass flux correction, so that the bulk velocity will not change throughout the simulation. This is important for models using incompressible assumptions such as PALM does. The velocity at the inflow is corrected with the ratio of the prescribed bulk velocity u b and u b,t = S 1 S u n,t ds, (6) which is the bulk velocity calculated with the uncorrected velocity normal to the inlet u n,t at the inlet, where S is the surface area of the inlet. The corrected velocity at the inlet follows as u b u i = u u i,t, (7) b,t where u i,t is the uncorrected velocity. The synthetic turbulence inflow generator needs in total 18 profiles as input profiles, which are the six components of R ij, the mean velocity profiles U i, and the length scale for each of the three velocity components in both orthogonal directions of the flow direction as well as the Lagrangian time scale along the flow direction. These input profiles can be derived from a precursor simulation or even by measurements. 3. SIMULATIONS WITH AND WITHOUT SYNTHETIC TURBULENCE (1) Simulation setup Four cases were simulated and will be presented in this study. Two cases using a homogeneous building array consisting of aligned cubes. A single tall building was added to the building array for the other two cases. In either case a laminar inflow condition and for the other case the synthetic turbulence inflow generator was applied for each urban canopy. The setup for each simulation contains a strict neutral stratified atmosphere without heating from the
3 ground. The atmosphere was assumed to be dry, so no humidity effects were considered. Surface conditions were non-slip for the surface and each wall boundary while the top boundary condition of the domain was slip. Cyclic boundary conditions were used in spanwise (y) direction while in streamwise (x) direction the synthetic turbulence inflow generator at the inflow and an open boundary at the outflow were used. The domain size was set to 1440m in streamwise and 480m in spanwise direction and 240m in vertical (z) direction (see Fig. 1). An isotropic grid was used with a grid spacing of 2m. The topography consists of an aligned array of cubes with an edge length of h = 24m and a distance between cubes of also h in x and y direction. The first and last row of cubes have a distance of 6h and 7h to the inlet and outlet, respectively, which corresponds to the absence of the first and last 3 rows of buildings. This results into a homogeneous grid of building cubes as shown in figure 1. For the latter two cases, one tall building with a horizontal width and depth of 3h and a height of 4h was added at the center of the domain. These cases will therefore be named TB_l (tall building case, laminar inflow) and TB_t (tall building case, turbulent inflow) while the other two cases without the tall building will be named HB_l (homogeneous building case, laminar inflow) and HB_t (homogeneous building case, turbulent inflow) hereafter. Results obtained from a simulation with cyclic boundaries with flat topography were used for the input of the turbulence generator. The domain height in this preliminary simulation was set to 200m and the profiles were later set to constant values above this height to match the new domain height. Only the mean wind profile was used as input for HB_l and TB_l. The simulation time was set to two hours. A dynamic time-step was used, which fulfilled the Courant-Friedrichs-Levy criterion. After the first hour of simulation time the flow reached a quasisteady state and therefore only the second hour of each simulation is used for analysis. (2) Results First results of the two cases with homogeneous buildings will be compared. Both cases HB_l and HB_t show the development of an urban boundary layer. Figure 2 shows the vertical profile of the wind speed component in x direction (u), averaged over the last hour of the simulation and spatially averaged over the building area as indicated in figure 1. The solid line represents the HB_l case while the longdashed line shows the HB_t case. Also the input profile for the turbulence generator (stars) and the profile for the TB_t case, which will be discussed later, are shown. The height is normalized by the domain height H. The building layer reaching up to 0.1H is clearly visible in the HB_l and HB_t case by the decelerating of the wind speed. On top of the buildings the wind speed accelerates faster with height than the input profile. Similar behavior of u was also observed by Kanda et al. 6) for a flow over a homogeneous cubical array. However, the flow inside the building layer is slightly faster for HB_t than for HB_l and above the building layer HB_t is slightly slower until 0.4H. Figure 3 shows the normalized and time averaged profiles of u 2 and w 2, which are the variances of wind speed in x and z direction, respectively, as well as the vertical momentum flux w u. Profiles were normalized by the friction velocity u. The shape of the variance profiles and also of the vertical momentum flux are comparable between both cases and also to those reported by Kanda et al. 6) giving confidence in the turbulence produced by the new inflow method. However, w 2 and w u reach higher values Fig.1 Domain specifications. The grey shaded tall building is only included in the TB cases. The averaging area shows the area used for horizontal averaging of profiles. Fig.2 Spatially and time-averaged u profiles.
4 Fig.3 Normalized spatially and time-averaged profiles of u, 2 (b) u, 2 and (c) w. u (a) for HB_t than for HB_l indicating a higher turbulence intensity inside the canopy layer and the urban boundary layer developing on top of the canopy layer. This differences indicate a higher vertical mixing for the HB_t case which causes also the reduced wind speed inside the boundary layer found in figure 2. A vertical slice in streamwise direction of the vertical velocity is shown in figure 4 for HB_l and HB_t. It is clearly visible that in the HB_t case the atmosphere above the canopy layer is turbulent while in the HB_l case it remains laminar above the urban boundary layer. In past studies these turbulent motions above the boundary layer were identified to have a significant influence of the turbulence inside the boundary layer 9) which is also the case in this study as shown in figure 3. Note that the high vertical velocities at the edge of the first building row are caused by the decelerating of the flow due to the buildings. The development of the urban boundary layer along the streamwise direction is shown in figure 5. The boundary layer height (BLH) is defined as the height where the vertical gradient w / z u reaches a value of ms -2. The BLH develops reasonably faster in the HB_t case compared to the HB_l case and the largest values for the HB_l case are reached about 350m further upstream in the HB_t case. This shows that a larger domain size would be necessary to simulate the same BLH with laminar inflow than with the turbulence inflow method. After showing the differences between the cases with homogeneous buildings now the cases including the tall building will be analyzed. The mean wind profile for the TB_t case (fig. 2) is accelerating slower over the small buildings compared to the HB_t case until the rooftop of the tall building at 0.4H, where u reaches higher values for the TB_t case than for the HB_t case. This shows the decelerating effect of the tall building on the flow. Also the turbulence is affected by the single tall building as shown by the profiles in figure 3. In the TB_t case w u (fig. 3c) is equal to the HB_t case inside the canopy layer. However, the profile of u 2 is slightly decreased. This decrease is then compensated of an increase of w 2 inside the canopy layer resulting in equal values for w. u The influence of the tall building causes the profiles of the TB_t case to differ from those of the HB_t case above the lower buildings. However, w u is nearly equal for both cases until 0.27H from whereon the rooftop of the tall building causes stronger turbulent motions in vertical direction and w u increases again. This effect at the rooftop is also visible in the u 2 and w 2 profiles creating another boundary layer. At about 0.6H the profiles of the TB_t case follow those at the input again
5 but are still slightly increased. The boundary layer height caused by the tall building is, therefore, around 0.6H. Figure 6 shows a vertical slice in xz-direction of time-averaged u for case TB_l and TB_t at y = 240m. The different inflow methods used in these two cases cause different influences of the tall building on the flow field. Especially in the leeward area of the building the velocity field is changed significantly. In case TB_l (fig. 6a) a rectangular shaped area of negative u values is located at the leeward side of the building reaching to the first edge of the second small building behind the tall building. When using the more realistic turbulence inflow method this area of negative u velocity has a more triangular shape and reaches slightly farther in x direction close to the ground including the first two building rows behind the tall building. These differences occur because of the higher vertical mixing in case TB_t compared to TB_l. Such significant differences cannot be neglected especially when focusing on the effect of tall buildings on the flow field. 4. CONCLUSIONS The results shown in this paper revealed the feasibility of using the synthetic turbulence inflow method for LES of urban canopies. The shape of the received profiles from the turbulent inflow case were in good agreement with other studies such as Kanda et al. 6) who, used cyclic boundary conditions in their LES, and Nozawa and Tamura 10), who used a turbulence recycling method instead of cyclic boundary conditions along the mean flow to simulate an urban boundary layer over a staggered grid of buildings. Also the advantages of the turbulence inflow method over a laminar inflow were shown. When using the turbulence inflow method stronger turbulent motions Fig.4 Vertical slice of w averaged along y for (a) the HB_l case and (b) the HB_t case at the end of each simulation. Black cubes indicate the positions of buildings. Fig.5 Development of the boundary layer height along the streamwise direction for cases HB_l and HB_t.
6 Fig.6 Time-averaged vertical slice of u at y = 240m for case (a) TB_l and (b) TB_t. developed inside the boundary layer and the BLH grew faster compared to the laminar case. As a benefit simulation domains can be smaller reducing the time and cost of simulations. When comparing the two TB cases a change of the influence of tall buildings on the flow field was found which can have a high influence on the interpretation of the effects of tall buildings on their surroundings. Simulated pollution emissions adjacent to such a building or calculations of the wind chill might be significantly changed when using laminar instead of turbulent inflow conditions. In the future this synthetic turbulence inflow generation method will be applied to simulations using different urban canopy layers. The influence of tall buildings on the velocity field will be further investigated by a case study with different canopy setups. This case study would highly benefit from the use of the synthetic turbulence inflow generator by reducing the required time for each simulation making it possible to enlarge the number of cases. ACKNOWLEDGMENT: We would like to thank Prof. Satoru Iizuka, Nagoya University, for supporting us in the early beginning of our research. The first author was supported by a grant of the DAAD (German Academic Exchange Service). All computations presented in this study were performed on TSU- BAME2.5 at the Tokyo Institute of Technology, Tokyo, Japan. conditions for large eddy simulation of street-scale flows, Flow Turbulence Combust, Vol.81, pp , ) Kim, Y., Castro, I. P. and Xie, Z.-T.: Divergence-free turbulence inflow conditions for large-eddy simulations with incompressible flow solvers, Computers & Fluids, Vol.84, pp.56-68, ) Raasch, S. and Schröter, M.: Palm a large-eddy simulation model performing on massively parallel computers, Meteorol. Z., Vol.10, pp , ) Wicker, L. J. and Skamarock, W. C.: Time-splitting methods for models using forward time schemes. Mon. Wea. Rev., Vol.130, pp , ) Williamson, J. H.: Low-storage runge-kutta schemes, J. Comput. Phys., 35, pp.48-56, ) Kanda, M., Moriwaki, R. and Kasamatsu, F.: Large eddy simulation of turbulent organized structures within and above explicitly resolved cube arrays, Boundary-Layer Meteorol., Vol.112, pp , ) Letzel, M. O., Krane, M. and Raasch, S.: High resolution urban large-eddy simulation studies from street canyon to neighborhood scale, Atmos. Environ., Vol.42, pp , ) Lund, T., Wu, X. and Squires, D.: Generation of turbulent inflow data for spatially developing boundary layer simulation, J. Comput. Phys., Vol.140, pp , ) Thole, K. A. and Bogard, D. G.: High freestream turbulence effects on turbulent boundary layers, J. Fluids Eng., Vol.118, pp , ) Nozawa, K. and Tamura, T.: Large eddy simulation of the flow around a low-rise building immersed in a rough-wall turbulent boundary layer, J. Wind Eng. Ind. Aerodyn., Vol.90, pp , REFERENCES 1) Xie, Z.-T. and Castro, I. P.: Efficient generation of inflow (Received September 30, 2014)
Numerical 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 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 informationS. Di Sabatino 1, R. Buccolieri 1, P. Paradisi 2, L. Palatella 2, R. Corrado 1,2, E. Solazzo 3
A FAST MODEL FOR FLOW AND POLLUTANT DISPERSION AT THE NEIGHBOURHOOD SCALE S. Di Sabatino 1, R. Buccolieri 1, P. Paradisi, L. Palatella, R. Corrado 1,, E. Solazzo 3 1 Dipartimento di Scienza dei Materiali,
More informationLARGE-EDDY EDDY SIMULATION CODE FOR CITY SCALE ENVIRONMENTS
ARCHER ECSE 05-14 LARGE-EDDY EDDY SIMULATION CODE FOR CITY SCALE ENVIRONMENTS TECHNICAL REPORT Vladimír Fuka, Zheng-Tong Xie Abstract The atmospheric large eddy simulation code ELMM (Extended Large-eddy
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 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 informationProbing urban canopy dynamics using direct numerical simulations (DNS) O. Coceal1a, T.G. Thomas2 & S.E. Belcher1 1Department aemail: of Meteorology, University of Reading, UK, 2School of Engineering Sciences,
More informationINTERACTION BETWEEN TURBULENT DYNAMICAL PROCESSES AND STATISTICS IN DEFORMED AIR-LIQUID INTERFACES, VIA DNS
INTERACTION BETWEEN TURBULENT DYNAMICAL PROCESSES AND STATISTICS IN DEFORMED AIR-LIQUID INTERFACES, VIA DNS Yoshinobu Yamamoto Department of Nuclear Engineering, Kyoto University Yoshida Sakyo Kyoto, 66-85,
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 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 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 informationEVALUATION OF A GENERAL CFD-SOLVER FOR A MICRO-SCALE URBAN FLOW
EVALATION OF A GENERAL CFD-SOLVER FOR A MICRO-SCALE RBAN FLOW Jarkko Saloranta and Antti Hellsten Helsinki niversity of Technology, Laboratory of Aerodynamics, Finland INTRODCTION In this work we study
More informationAn Introduction to SolidWorks Flow Simulation 2010
An Introduction to SolidWorks Flow Simulation 2010 John E. Matsson, Ph.D. SDC PUBLICATIONS www.sdcpublications.com Schroff Development Corporation Chapter 2 Flat Plate Boundary Layer Objectives Creating
More informationMeasurements and CFD simulations of flow and dispersion in urban geometries. Valeria Garbero* and Pietro Salizzoni. Lionel Soulhac and Patrick Mejean
Int. J. Environment and Pollution, Vol. x, No. x, xxxx 1 Measurements and CFD simulations of flow and dispersion in urban geometries Valeria Garbero* and Pietro Salizzoni Dipartimento di Ingegneria Aeronautica
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 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 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 informationAdarsh Krishnamurthy (cs184-bb) Bela Stepanova (cs184-bs)
OBJECTIVE FLUID SIMULATIONS Adarsh Krishnamurthy (cs184-bb) Bela Stepanova (cs184-bs) The basic objective of the project is the implementation of the paper Stable Fluids (Jos Stam, SIGGRAPH 99). The final
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 informationOptimizing Building Geometry to Increase the Energy Yield in the Built Environment
Cornell University Laboratory for Intelligent Machine Systems Optimizing Building Geometry to Increase the Energy Yield in the Built Environment Malika Grayson Dr. Ephrahim Garcia Laboratory for Intelligent
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 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 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 informationSolidWorks Flow Simulation 2014
An Introduction to SolidWorks Flow Simulation 2014 John E. Matsson, Ph.D. SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit the following websites
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 informationExamining tree canopy models for CFD prediction of wind environment at pedestrian level
Journal of Wind Engineering and Industrial Aerodynamics 9 (8) 17 177 www.elsevier.com/locate/jweia Examining tree canopy models for CFD prediction of wind environment at pedestrian level Akashi Mochida
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 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 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 informationPARALLEL DNS USING A COMPRESSIBLE TURBULENT CHANNEL FLOW BENCHMARK
European Congress on Computational Methods in Applied Sciences and Engineering ECCOMAS Computational Fluid Dynamics Conference 2001 Swansea, Wales, UK, 4-7 September 2001 ECCOMAS PARALLEL DNS USING A COMPRESSIBLE
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 informationSuper-Parameterization of Boundary Layer Roll Vortices in Tropical Cyclone Models
DISTRIBUTION STATEMENT A. Approved for public release; distribution is unlimited. Super-Parameterization of Boundary Layer Roll Vortices in Tropical Cyclone Models PI Isaac Ginis Graduate School of Oceanography
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 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 informationA Computational Study on the Influence of Urban Morphology on Wind-Induced Outdoor Ventilation
International Environmental Modelling and Software Society (iemss) 2012 International Congress on Environmental Modelling and Software Managing Resources of a Limited Planet, Sixth Biennial Meeting, Leipzig,
More informationLarge eddy simulation for atmospheric boundary layer flow over flat and complex terrains
Journal of Physics: Conference Series PAPER OPEN ACCESS Large eddy simulation for atmospheric boundary layer flow over flat and complex terrains To cite this article: Yi Han et al 2016 J. Phys.: Conf.
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 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 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 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 informationDirect Numerical Simulation of Turbulent Boundary Layers at High Reynolds Numbers.
Direct Numerical Simulation of Turbulent Boundary Layers at High Reynolds Numbers. G. Borrell, J.A. Sillero and J. Jiménez, Corresponding author: guillem@torroja.dmt.upm.es School of Aeronautics, Universidad
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 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 informationMAE 3130: Fluid Mechanics Lecture 5: Fluid Kinematics Spring Dr. Jason Roney Mechanical and Aerospace Engineering
MAE 3130: Fluid Mechanics Lecture 5: Fluid Kinematics Spring 2003 Dr. Jason Roney Mechanical and Aerospace Engineering Outline Introduction Velocity Field Acceleration Field Control Volume and System Representation
More informationINTRODUCTION TO POLLUTANT DISPERSION IN URBAN STREET CANYONS MUHAMMAD NOOR AFIQ WITRI
INTRODUCTION TO POLLUTANT DISPERSION IN URBAN STREET CANYONS MUHAMMAD NOOR AFIQ WITRI 1 CONTENTS 1.Motivation 2.Introduction 3.Street canyon characteristics 4.Wind field models 5.Dispersion models 1.Future
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 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 informationNumerical Study of a Separated Boundary Layer Transition over Two and Three Dimensional Geometrical Shapes
Numerical Study of a Separated Boundary Layer Transition over Two and Three Dimensional Geometrical Shapes 1 HAYDER AZEEZ DIABIL, 1 XIN KAI LI, 2 IBRAHIM ELRAYAH ABDALLA 1 Engineering Science and Advanced
More informationCharacterisation of the interaction between a boundary layer and a cavity using Digital Particle Velocimetry with Optical Flow
Characterisation of the interaction between a boundary layer and a cavity using Digital Particle Velocimetry with Optical Flow G. Quénot*, A. Rambert**, P. Gougat**, T. Kowalevski*** *CLIPS-IMAG, Grenoble,
More information9.9 Coherent Structure Detection in a Backward-Facing Step Flow
9.9 Coherent Structure Detection in a Backward-Facing Step Flow Contributed by: C. Schram, P. Rambaud, M. L. Riethmuller 9.9.1 Introduction An algorithm has been developed to automatically detect and characterize
More informationNUMERICAL SIMULATION OF THE SHALLOW WATER EQUATIONS USING A TIME-CENTERED SPLIT-IMPLICIT METHOD
18th Engineering Mechanics Division Conference (EMD007) NUMERICAL SIMULATION OF THE SHALLOW WATER EQUATIONS USING A TIME-CENTERED SPLIT-IMPLICIT METHOD Abstract S. Fu University of Texas at Austin, Austin,
More informationINTERNATIONAL JOURNAL OF CIVIL AND STRUCTURAL ENGINEERING Volume 2, No 3, 2012
INTERNATIONAL JOURNAL OF CIVIL AND STRUCTURAL ENGINEERING Volume 2, No 3, 2012 Copyright 2010 All rights reserved Integrated Publishing services Research article ISSN 0976 4399 Efficiency and performances
More informationStudy and Compare of Heat Transfer Enhancement in Interrupted Louvered Fins and Rectangular Fins
Study and Compare of Heat Transfer Enhancement in Interrupted Louvered Fins and Rectangular Fins Amit Kumar Bansal 1, Chander Kishore 2, Vikrant Chandel 3 1 Director/Principal, Shiva Institute of Engineering
More informationMesh Adaptive LES for micro-scale air pollution dispersion and effect of tall buildings.
HARMO17, Budapest, 9 12 May, 2016. Mesh Adaptive LES for micro-scale air pollution dispersion and effect of tall buildings. Elsa Aristodemou, Luz Maria Boganegra, Christopher Pain, Alan Robins, and Helen
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 informationLarge Eddy Simulation Applications to Meteorology
Large Eddy Simulation Applications to Meteorology Marcelo Chamecki Department of Meteorology The Pennsylvania State University Tutorial School on Fluid Dynamics: Topics in Turbulence May 27 th 2010, College
More informationMicrometeorology and Ecology
Monique Y. Leclerc Thomas Foken Footprints in Micrometeorology and Ecology With Contributions by M. J. Savage and M. Gockede 4^1 Springer 1 History and Definition 1 1.1 Micrometeorological Measurements
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 informationNUMERICAL ANALYSIS OF WIND EFFECT ON HIGH-DENSITY BUILDING AERAS
NUMERICAL ANALYSIS OF WIND EFFECT ON HIGH-DENSITY BUILDING AERAS Bin ZHAO, Ying LI, Xianting LI and Qisen YAN Department of Thermal Engineering, Tsinghua University Beijing, 100084, P.R. China ABSTRACT
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 informationNumerical Simulations of Granular Materials Flow around Obstacles: The role of the interstitial gas
Numerical Simulations of Granular Materials Flow around Obstacles: The role of the interstitial gas Avi Levy, Dept. Mech. Eng., Ben Gurion University, Beer Sheva, Israel. Mohamed Sayed, CHC, National Research
More informationDEPARTMENT OF FLUID DYNAMICS CFD SIMULATION OF FLOW OVER A MOCK URBAN SETTING USING OPENFOAM
DEPARTMENT OF FLUID DYNAMICS Budapest University of Technology and Economics CFD SIMULATION OF FLOW OVER A MOCK URBAN SETTING USING OPENFOAM Anikó Rákai Gergely Kristóf, Ph. D. 5th OpenFOAM Workshop Gothenburg
More informationContinued Investigation of Small-Scale Air-Sea Coupled Dynamics Using CBLAST Data
Continued Investigation of Small-Scale Air-Sea Coupled Dynamics Using CBLAST Data Dick K.P. Yue Center for Ocean Engineering Department of Mechanical Engineering Massachusetts Institute of Technology Cambridge,
More informationLARGE EDDY SIMULATION OF OPEN-CHANNEL FLOW OVER A LAYER OF SPHERES
Proceedings of 31th IAHR Congress, Seoul, September 11-16, 2005. LARGE EDDY SIMULATION OF OPEN-CHANNEL FLOW OVER A LAYER OF SPHERES THORSTEN STOESSER 1, WOLFGANG RODI 2, JOCHEN FRÖHLICH 3 1 Post Doctoral
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 informationAerodynamic effect of overhang on a turbulent flow field within a two-dimensional street canyon
九州大学学術情報リポジトリ Kyushu University Institutional Repository Aerodynamic effect of overhang on a turbulent flow field within a two-dimensional street canyon Mohamad, Mohd Faizal Universiti Teknologi MARA Department
More informationFAST ALGORITHMS FOR CALCULATIONS OF VISCOUS INCOMPRESSIBLE FLOWS USING THE ARTIFICIAL COMPRESSIBILITY METHOD
TASK QUARTERLY 12 No 3, 273 287 FAST ALGORITHMS FOR CALCULATIONS OF VISCOUS INCOMPRESSIBLE FLOWS USING THE ARTIFICIAL COMPRESSIBILITY METHOD ZBIGNIEW KOSMA Institute of Applied Mechanics, Technical University
More informationJ. Vira, M. Sofiev SILAM winter school, February 2013, FMI
Numerical aspects of the advection-diffusion equation J. Vira, M. Sofiev SILAM winter school, February 2013, FMI Outline Intro Some common requirements for numerical transport schemes Lagrangian approach
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 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 informationSTAR-CCM+: Wind loading on buildings SPRING 2018
STAR-CCM+: Wind loading on buildings SPRING 2018 1. Notes on the software 2. Assigned exercise (submission via Blackboard; deadline: Thursday Week 3, 11 pm) 1. NOTES ON THE SOFTWARE STAR-CCM+ generates
More informationAn explicit and conservative remapping strategy for semi-lagrangian advection
An explicit and conservative remapping strategy for semi-lagrangian advection Sebastian Reich Universität Potsdam, Potsdam, Germany January 17, 2007 Abstract A conservative semi-lagrangian advection scheme
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 informationKey words: OML, AERMOD, PRIME, MISKAM, AUSTAL2000, model comparison, wind tunnel, stack-building configuration
H13-163 COMPARISON OF GROUND-LEVEL CENTRELINE CONCENTRATIONS CALCULATED WITH THE MODELS OML, AERMOD/PRIME, MISKAM AND AGAINST THE THOMPSON WIND TUNNEL DATA SET FOR SIMPLE STACK-BUILDING CONFIGURATIONS
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 informationFinite Volume Discretization on Irregular Voronoi Grids
Finite Volume Discretization on Irregular Voronoi Grids C.Huettig 1, W. Moore 1 1 Hampton University / National Institute of Aerospace Folie 1 The earth and its terrestrial neighbors NASA Colin Rose, Dorling
More informationAerodynamic loads on ground-mounted solar panels: multi-scale computational and experimental investigations
Aerodynamic loads on ground-mounted solar panels: multi-scale computational and experimental investigations * Aly Mousaad Aly ) and Girma Bitsuamlak 2) ) Louisiana State University, Baton Rouge, Louisiana
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 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 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 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 informationCFD PREDICTION OF WIND PRESSURES ON CONICAL TANK
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
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 informationMesh techniques and uncertainty for modelling impulse jetfans. O. A. (Sam) Alshroof. CFD manager Olsson Fire and Risk
Mesh techniques and uncertainty for modelling impulse jetfans O. A. (Sam) Alshroof CFD manager Olsson Fire and Risk Email: Sam.Alshroof@olssonfire.com Abstract This study presents the numerical modelling
More informationMathematical Modeling of Drag Coefficient Reduction in Circular Cylinder Using Two Passive Controls at Re = 1000
Mathematical and Computational Applications Article Mathematical Modeling of Drag Coefficient Reduction in Circular Cylinder Using Two Passive Controls at Re = 1000 Chairul Imron 1, *, Lutfi Mardianto
More informationJunhong Wei Goethe University of Frankfurt. Other contributor: Prof. Dr. Ulrich Achatz, Dr. Gergely Bölöni
Efficient modelling of the gravity-wave interaction with unbalanced resolved flows: Pseudo-momentum-flux convergence vs direct approach Junhong Wei Goethe University of Frankfurt Other contributor: Prof.
More informationJ4.3 LARGE-EDDY SIMULATION ACROSS A GRID REFINEMENT INTERFACE USING EXPLICIT FILTERING AND RECONSTRUCTION
J4.3 LARGE-EDDY SIMULATION ACROSS A GRID REFINEMENT INTERFACE USING EXPLICIT FILTERING AND RECONSTRUCTION Lauren Goodfriend 1, Fotini K. Chow 1, Marcos Vanella 2, and Elias Balaras 2 1 Civil and Environmental
More informationLATTICE-BOLTZMANN METHOD FOR THE SIMULATION OF LAMINAR MIXERS
14 th European Conference on Mixing Warszawa, 10-13 September 2012 LATTICE-BOLTZMANN METHOD FOR THE SIMULATION OF LAMINAR MIXERS Felix Muggli a, Laurent Chatagny a, Jonas Lätt b a Sulzer Markets & Technology
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 informationSolving non-hydrostatic Navier-Stokes equations with a free surface
Solving non-hydrostatic Navier-Stokes equations with a free surface J.-M. Hervouet Laboratoire National d'hydraulique et Environnement, Electricite' De France, Research & Development Division, France.
More informationThin Film Simulation on a Rotating Wafer. B. Gschaider, D. Prieling, H. Steiner, P. Vita
Thin Film Simulation on a Rotating Wafer B. Gschaider, D. Prieling, H. Steiner, P. Vita Topics Motivation Finite Area Method Thin Film Model Impinging Jet Polydual Mesh Comparison with 3D Solution Conclusion
More informationRealistic Animation of Fluids
Realistic Animation of Fluids p. 1/2 Realistic Animation of Fluids Nick Foster and Dimitri Metaxas Realistic Animation of Fluids p. 2/2 Overview Problem Statement Previous Work Navier-Stokes Equations
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 informationAalborg Universitet. Numerical 3-D Modelling of Overflows Larsen, Torben; Nielsen, L.; Jensen, B.; Christensen, E. D.
Aalborg Universitet Numerical 3-D Modelling of Overflows Larsen, Torben; Nielsen, L.; Jensen, B.; Christensen, E. D. Published in: Confernce Proceedings : 11th International Conference on Urban Drainage
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 informationComputational Fluid Dynamics modeling of a Water Flow Over an Ogee Profile
FINITE ELEMENT METHOD TECHNICAL REPORT Computational Fluid Dynamics modeling of a Water Flow Over an Ogee Profile ANSYS CFX 12 ENME 547 Dr. Sudak Matias Sessarego Written Report Due Date: Friday December
More informationTYPE 529: RADIANT SLAB
TYPE 529: RADIANT SLAB General Description This component is intended to model a radiant floor-heating slab, embedded in soil, and containing a number of fluid filled pipes. The heat transfer within the
More informationPARAMETERIZATION OF DRAG FORCES IN URBAN CANOPY MODELS USING MICROSCALE-CFD MODELS FOR DIFFERENT WIND DIRECTIONS
PARAMETERIZATION OF DRAG FORCES IN URBAN CANOPY MODELS USING MICROSCALE-CFD MODELS FOR DIFFERENT WIND DIRECTIONS J. L. Santiago 1, O. Coceal 2 and A. Martilli 1 1 Atmospheric Pollution Division, Environmental
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 informationTHE FLUCTUATING VELOCITY FIELD ABOVE THE FREE END OF A SURFACE- MOUNTED FINITE-HEIGHT SQUARE PRISM
THE FLUCTUATING VELOCITY FIELD ABOVE THE FREE END OF A SURFACE- MOUNTED FINITE-HEIGHT SQUARE PRISM Rajat Chakravarty, Noorallah Rostamy, Donald J. Bergstrom and David Sumner Department of Mechanical Engineering
More information