VALIDATION OF A CFD MODEL IN RECTANGULAR SETTLING TANKS
|
|
- Edmund York
- 6 years ago
- Views:
Transcription
1 Proceedings of the 13 th International Conference on Environmental Science and Technology Athens, Greece, 5-7 September 2013 VALIDATION OF A CFD MODEL IN RECTANGULAR SETTLING TANKS A. GKESOULI 1, A. I.STAMOU 1, M. XANTHAKI 2 and S. GEORGIADIS 2 1 School of Civil Engineering, Department of Water Resources and Environmental Engineering, National Technical University of Athens, Iroon Polytechniou 5, Athens, Greece. 2 E.Y.D.A.P. S.A., Oropou 156, Athens, Greece. gkesouli@central.ntua.gr EXTENDED ABSTRACT Sedimentation is one of the most important treatment processes in conventional Water Treatment Plants and it is performed in settling tanks, whose investment in treatment plants usually accounts for the one third of the total investment; a significant percentage of suspended solids settles by gravity and therefore, influences the degree of treatment in the downstream units and the removal efficiency of the plant. Subsequently, the determination of the removal efficiency of a sedimentation tank has been the subject of numerous theoretical and experimental studies. The removal efficiency depends on the physical characteristics of the suspended solids, as well as on the flow field and the mixing regime in the tank. Flow field and mixing can strongly affect the settling efficiency through flocculation, breakup or re-entrainment of solid particles. Therefore, the determination of the flow field and mixing characteristics, which can be determined with the use of simple or sophisticated mathematical models, is essential for the prediction of the tank efficiency. Since the flow in settling tanks is fully turbulent, in sophisticated mathematical models, a turbulence model is usually employed for the determination of the eddy viscosity and the description of turbulent mixing. In addition to turbulent mixing, large-scale mixing occurs in zones with flow recirculation, which are present even at the simplest settling tank geometries. It is obvious that simple models ignore these zones and therefore are inadequate in predicting even approximately the flow and mixing in settling tanks. The validity of a mathematical model for settling tanks can be checked by comparison with experimental data that may include flow velocity profiles, streamline patterns, size of recirculation regions, dispersion or flow-through curves, profiles of concentration of suspended solids and removal efficiencies. In the present work a Computational Fluid Dynamics model was formulated, calibrated and applied in the settling tanks of the old unit of the Water Treatment Plant of Aharnes of EYDAP SA in Attica. Calculations showed that (1) flow fields are 3-D and complex, especially in the region of the inlet of the tank, with three large recirculation areas, and (2) concentration fields depend strongly on the flow fields. In the recirculation areas (where mixing is intense) the concentrations are uniformly distributed; moreover, with increasing flow rate the suspended solids iso-concentration lines are shifted to the right (towards the outlet of the tank), the outlet concentration increases and the efficiency of the tank is reduced. The model was calibrated and verified successfully using experimentally determined removal efficiency values. Keywords: settling tank, water treatment plant, CFD modeling, suspended solids, removal efficiency 1. INTRODUCTION Sedimentation is one of the most important treatment processes in conventional Water Treatment Plants; a significant percentage of suspended solids, which is formed by the aggregation of particles in the untreated water with flocculants, settles by gravity and
2 therefore, influences the degree of treatment in the downstream units (usually filtration and disinfection) and the removal efficiency of the plant. Sedimentation is performed in settling tanks, whose investment in treatment plants usually accounts for the one third of the total investment. Subsequently, the determination of the removal efficiency of a sedimentation tank has been the subject of numerous theoretical and experimental studies. The removal efficiency depends on the physical characteristics of the suspended solids (e.g. particle size, density and settling velocity), as well as on the flow field and the mixing regime in the tank. Flow field and mixing can strongly affect the settling efficiency through flocculation (Lyn et al., 1992), breakup or re-entrainment of solid particles. Therefore, the determination of flow and mixing characteristics is essential for the prediction of the tank efficiency (Stamou et al., 2009). Flow and mixing characteristics can be determined with the use of mathematical models. A mathematical model can be simple (Stamou et al., 2008) or sophisticated (Stamou et al., 2000); for example in a simple model a prescribed shape (logarithmic, uniform, parabolic) for velocity that is based on a set of mean flow equations, which are solved numerically, can be adopted. Since the flow in settling tanks is fully turbulent, a turbulence model is usually employed for the determination of eddy viscosity and the description of turbulent mixing (Stamou, 1991). In addition to turbulent (small scale) mixing, large-scale (and usually intense) mixing occurs in zones with flow recirculation, which are present even at the simplest settling tank geometries with inlet baffles; see for example Krebs et al. (1996) and Stamou (1994). It is obvious that simple models ignore these zones and therefore are inadequate in predicting even approximately the flow and mixing in settling tanks. The validity of a mathematical model for settling tanks can be checked by comparison with experimental data (Stamou, 2007); these data may include flow velocity profiles, streamline patterns, size of recirculation regions, dispersion or flow-through curves (Stamou and Noutsopoulos, 1994), profiles of concentration of suspended solids (Stamou et al., 1989) and removal efficiencies (Stamou et al., 1989). In 2011 a research project was initiated at the NTUA aiming at proposing measures for the settling tanks of the Water Treatment Plant of Aharnes (WTPA) of EYDAP SA in Attica, including the use of deflectors, that are expected to reduce the detrimental effect of wind on the settling efficiency of the tanks, improve their hydrodynamic conditions and their efficiency, and thus reduce the cost of treatment. The investigation was performed with the use of a mathematical Computational Fluid Dynamics (CFD) model (Stamou, 2006) that was formulated, calibrated and applied in the settling tanks. The present paper demonstrates briefly the first part of this investigation, which is the calibration and the verification of the model, which was performed with experimental data that were obtained during the project. 2. CHARACTERISTICS OF THE SETTLING TANKS There are sixteen rectangular settling tanks in the "old unit" of the WTPA with the following dimensions: width w=14.4 m, length L=73.2 m and average water depth H=3.5 m; the design flow rate to each tank ranges from 0.25 m 3 /s to 0.31 m 3 /s. The water enters into the settling tank from the flocculation tank via four rectangular openings and exits the tank via a series of V-notch weirs installed at the outlet channels. The suspended solids at the inlet were divided into four classes, whose characteristic diameters were determined (APHA, AWWA and WEF, 2005) equal to 41 μm, 17 μm, 9.5 μm and 5 μm; for each class the settling velocity (V set) was calculated using the Stokes Law. The turbidity of the water at the inlet of the tank ranges from 2.0 to 20.0 NTU and the daily average value is calculated equal to 5.0 NTU; these turbidity values correspond to a range of concentrations of suspended solids from 2.5 mg/l to 29.4 mg/l and an average value equal to S in=7.0 mg/l. Correspondingly, the turbidity measurements at the outlet of the tank range from 0.4 to 3.8 NTU and the daily average value is equal to 1.4
3 NTU; the corresponding concentration values for the range and average are mg/l and S out=1.6 mg/l, respectively. Using the average concentration values, the average removal efficiency of the tank is calculated equal to R = ( )/5.0 = 72 %. 3. MATHEMATICAL MODEL 3.1. Equations of the model For the calculation of the 3-D flow and solids concentration fields in the settling tank the equations of continuity, momentum and mass conservation for the solids are solved; these equations are written as follows,: U j = 0 x j (1) Ui UU j i P Ui + = - + ( RTS) + gi t x j xi x j x j (2) S Uj Vset S S + = ( TSS) (3) t x j x j x j where ρ is the density of water, U i and U j are the flow velocities in i and j direction, respectively, x i and x j are the Cartesian coordinates in i and j direction, respectively, t is the time, P is the pressure, μ is the molecular viscosity of the water, g i is the acceleration of gravity and S is the local concentration of suspended solids. The process of settling is modeled as a mass flux of solids in the direction of gravity with a settling velocity equal to V set; this flux that is proportional to V set S is added to the transport term of equation (3). For the calculation of the Reynolds (turbulent) stresses (RTS), the assumption of the isotropic turbulence is applied combined with the Bussinesq approximation, i.e. U x U i j RTS = t( + ) - k j i 3 where μ t is the eddy viscosity, δ ij is the Kronecker delta (δ ij=1 for i=j and δ ij=0 for ij ) and k is the average turbulent kinetic energy per unit mass, given by: 1 2 k = ( U i' ) (5) 2 where U i' 2 are the normal Reynolds stresses in i direction. Similarly, the Turbulent SS Stresses (TSS) are calculated by equation (6). t S TSS (6) S x j where σ s is the turbulent Schmidt number for the solids. In the present work, turbulence is modeled with the Shear Stress Transport (SST) k-ω based model (Menter, 1994). This model combines the standard k-ε model (Rodi, 1980) and the k-ω model (Wilcox, 1988); virtually, it is a transformation of the k-ε to a k-ω formulation and a subsequent addition of certain equations. The standard k-ω model (Wilcox, 1988) relates the eddy viscosity to k and to the turbulence frequency (ω). x 2 ij (4) k t = The k and ω are calculated from the following model transport equations: (7)
4 k U k k t x x x j t ' + = ( ) + G - k j j k j (8) Uj t 2 + = ( ) + G - (9) t x j x j x j k The standard values of the constants of the SST model are β =0.09, α=5/9 and β=3/40, the turbulent Schmidt numbers for k and ω are σ k=2 and σ ω=2, respectively, and G is the production rate of turbulence Numerical code Calculations were performed with the 3-D CFD code CFX 14.0 that uses the finite volume method for the spatial discretisation of the domain ( Equations (1), (2), (3), (8) and (9) are integrated over each control volume, such that the relevant quantity (mass, momentum, S, k and ω) is conserved, in a discrete sense, for each control volume. For the continuity equation (pressure-velocity coupling) a second order central difference approximation is used, modified by a fourth order derivative in pressure, which redistributes the influence of pressure. The second order upwind Euler scheme approximates the transient term. The code employs an automatic, unstructured hybrid element mesh generator with an adaptive mesh refinement algorithm, which permits a very accurate representation of the boundaries. The advantage of using unstructured mesh is the minimization of numerical errors and the consistency of the solution throughout the domain. For the solution of the equations, a scalable and fully implicit coupled solver is used. 4. CALCULATIONS 4.1. Scenarios Calculations were performed for three scenarios with the characteristics that are shown in Table 1; these scenarios were chosen to cover the expected flow rates (Q). Initially, it was assumed that there was no flow or suspended solids in the computational domain (cold start). Transient calculations were run to steady state. Scenario Flow rate Q (m 3 /s) Table 1: Characteristics of the scenarios. Inlet velocity U in (m/s) Mean flow velocity U m (m/s) Theoretical hydraulic time Θ (h) Overflow rate OR (m/h) S S S Numerical grid and boundary conditions The numerical grid that consisted of elements is shown in Figure 1 together with the division of the computational domain into four volumes: inlet, main domain, change of geometry and outlet, with different grid properties. The boundary conditions employed in the model are summarized in Table 2.
5 Figure 1. View of the numerical grid. Location Surface Bottom Walls Symmetry plane Inlet Outlet Table 2: Boundary conditions. Boundary condition Free Slip Wall - No deposition No slip wall - Smooth wall - Deposition No slip wall - Smooth wall - No deposition Symmetry Normal speed = mean inlet velocity Opening - Entrainment (Inlet flow rate = Outlet flow rate) 4.3. Flow field In Figures 2 and 3 the streamlines of the flow field at a plane xy at z = 4 m and the eddies-recirculation areas that are formed in the tank are shown, respectively. Figures 2 and 3 depict that the flow field is 3-D and complex, especially in the region of the inlet of the tank. Three main recirculation areas are observed. The first (R1) is counter-clockwise and is created above the horizontal plane of the inlet jets (y=0.55 m); R1 starts from x=5.0 m and has a length that ranges from 20.0 m (near the symmetry plane) to 40.0 m (near the wall of the tank); this length decreases with increasing flow rate. The second recirculation area (R2) is clockwise (around axis y) and its size increases with increasing flow rate, while the third (R3) is developed near the boundary wall due to the interaction of R1 and R2 with the boundary walls and has a length of approximately 10.0 m. (a) Scenario S1; flow rate Q=0.25 m 3 /s (b) Scenario S2; flow rate Q=0.28 m 3 /s (c) Scenario S3; flow rate Q=0.31 m 3 /s Figure 2. Calculated flow streamlines.
6 (a) Recirculation area (R1) at z=4.0 m from the boundary wall (b) Recirculation area (R2) at y=0.7 m from the bottom (c) Recirculation area (R3) at z=0.5 m from the boundary wall Figure 3. Main recirculation areas that are formed in the flow field Concentration field of suspended solids The suspended solids iso-concentration contours of Figure 4, which are plotted at the same planes with the flow field plots of Figure 2, show that the concentration fields depend strongly on the flow fields. In the three recirculation areas, where mixing is intense, the concentration profiles are approximately uniform. As expected, with increasing flow rate the iso-concentration lines are shifted to the right (towards the outlet of the tank), the outlet concentration increases and the efficiency of the tank is reduced. (a) Scenario S1; flow rate Q=0.25 m 3 /s (b) Scenario S2; flow rate Q=0.28 m 3 /s (c) Scenario S3; flow rate Q=0.31 m 3 /s Figure 4. Iso-concentration contours of suspended solids Calibration and verification of the model For the calibration of the model the calculated removal efficiency was compared with the experimentally determined efficiency for the flow rate Q=0.27 m 3 /s; model calibration involved the determination of the value of the percentage of the second class of suspended solids for which the calculated by the model removal efficiency coincides with the experimentally determined value (71%). This procedure, which is summarized in Table 3, was performed to take indirectly into account the effect of intense coagulation that occurs in the region of inlet of the settling tank (presence of recirculation areas with favorable velocity gradients), which is not accounted for by the mathematical model. The value of the percentage of the second class of suspended solids was determined equal to 36%. Then, using this value the verification of the model was performed; the model was applied for a flow rate equal to Q=0.31 m 3 /s to determine the removal efficiency of the tank, as shown in Table 4; the calculated efficiency 67 % coincides with the experimental value, thus proving the successful validation of the model.
7 In Tables 3 and 4, the efficiencies for ideal settling (Hendricks, 2011) are shown, respectively, these were found equal to 84% and 80%, i.e. they are significantly higher (by 13%) than the real tank efficiencies and set the upper theoretical limits of the removal efficiency. Table 3: Summary of the calculation of the efficiency of the tank for Q=0.27 m 3 /s (calibration of the model). Class Percentage at inlet S in (mg/l) S out (mg/l) Efficiency V set (m/h) Efficiency of ideal settling Total Table 4: Summary of the calculation of the efficiency of the tank for Q=0.31 m 3 /s (verification of the model). Class Percentage at inlet S in (mg/l) S out (mg/l) Efficiency V set (m/h) Efficiency of ideal settling Total CONCLUSIONS A Computational Fluid Dynamics model was formulated, calibrated and applied in the settling tanks of the old unit of the Water Treatment Plant of Aharnes of EYDAP SA in Attica. Calculations showed that (1) flow fields are 3-D and complex, especially in the region of the inlet of the tank, with three large recirculation areas, and (2) concentration fields depend strongly on the flow fields. In the recirculation areas (where mixing is intense) the concentrations are uniformly distributed; moreover, with increasing flow rate the suspended solids iso-concentration lines are shifted to the right (towards the outlet of the tank), the outlet concentration increases and the efficiency of the tank is reduced. The model was calibrated and verified successfully using experimentally determined removal efficiency values. ACKNOWLEDGEMENT The present work was performed in the NTUA within the framework of the research program entitled "Improving the efficiency of settling tanks of the Water Treatment Plant of EYDAP SA in Aharnes using mathematical models. REFERENCES 1. ANSYS-CFX, Release 14.0, URL: (accessed 10/03/2013). 2. APHA, AWWA and WEF. (2005), Standard Methods for the Examination of Water and Wastewater, 21st ed. American Public Health Association, Washington, D.C.
8 3. Hendricks D. (2011), Fundamentals of Water Treatment Unit Processes: Physical, Chemical and Biological, CRC Press, United States of America. 4. Krebs P., Stamou A.I., Garcia-Heras J.L and Rodi W. (1996), Influence of Inlet and Outlet Configuration on the Flow in Secondary Clarifiers, Wat. Sci. Tech., 34(5-6), Lyn D. A., Stamou A. I. and Rodi W. (1992), Density Currents and Shear Induced Flocculation in Sedimentation Tanks, Journal of Hydraulic Engineering, ASCE, 118(6), Menter F.R. (1994), Two-Equation Eddy-Viscosity Turbulence Models for Engineering Applications, AIAA Journal, 32 (8), Rodi W. (1980), Turbulence Models and Their Application in Hydraulics A State of the Art Review, IAHR, Delft, Netherlands. 8. Stamou A.I., Theodoridis G. and Xanthopoulos K. (2009), Design of Secondary Settling Tanks using a CFD Model, Journal of Environmental Engineering, ASCE, 135 (7), Stamou A.I., Giokas D.L., Kim Y. and Paraskevas P.A. (2008), Validation and Application of a Simple Model for Circular Secondary Settling Tanks, Global Nest the Int. J., 10(1), Stamou A.I. (2007), Discussion of Two-Dimensional Simulation Model of Sediment Removal and Flow in Rectangular Sedimentation Basin, Journal of Environmental Engineering, ASCE, 133(9), Stamou A.I. (2006), A Design Methodology for Settling Tanks using CFD Models, IASME Transactions on Fluid Mechanics, 4(1), Stamou A.I., Latsa M. and Assimacopoulos D. (2000), Design of Two-Storey Final Settling Tanks using Mathematical Models, J. of Hydroinformatics, 2(4), Stamou A.I. and Noutsopoulos G. (1994), Evaluating the Effect of Inlet Arrangement in Settling Tanks Using the Hydraulic Efficiency Diagram, Water SA, 20(1), Stamou A.I. (1994), Discussion of Modelling of Rectangular Settling Tanks, Journal of Hydraulics Engineering, ASCE, 120, Stamou A.I. (1991), On the Prediction of Flow and Mixing in Settling Tanks Using a Curvature Modified k-ε Model, Applied Mathematical Modelling, 15, Stamou A.I., Adams E. A. and Rodi W. (1989), Numerical Modelling of Flow and Settling in Primary Rectangular Clarifiers, J. of Hydr. Res., IAHR, 27(5), Wilcox D.C. (1988), Reassessment of the scale determining equation for advanced turbulence models, AIAA Journal, 26 (11),
Numerical Investigation of the Flow Dynamics of a Supersonic Fluid Ejector
Proceedings of the International Conference on Heat Transfer and Fluid Flow Prague, Czech Republic, August 11-12, 2014 Paper No. 171 Numerical Investigation of the Flow Dynamics of a Supersonic Fluid Ejector
More informationNext-generation modeling tool helps you get the most from your clarifier
Clarifier Proce Next-generation modeling tool helps you get the most from your clarifier Alonso Griborio, Paul Pitt, and John Alex McCorquodale 52 W E & T w w w. w e f. o r g / m a g a z i n e 2008 Water
More informationCFD Analysis of Pelton Runner
International Journal of Scientific and Research Publications, Volume 4, Issue 8, August 2014 1 CFD Analysis of Pelton Runner Amod Panthee *, Hari Prasad Neopane **, Bhola Thapa ** * Turbine Testing Lab,
More informationPERFORMANCE ANALYSIS OF NATURAL DRAFT WET COOLING TOWER AT OPTIMIZED INJECTION HEIGHT
PERFORMANCE ANALYSIS OF NATURAL DRAFT WET COOLING TOWER AT OPTIMIZED INJECTION HEIGHT 1 ALOK SINGH, 2 SANJAY SONI, 3 R. S. RANA 1 Assistant Professor, 2 Associate Professor, 3 Mechanical Engineering Department
More informationCFD Analysis of Clarifier Performance With and Without Energy Dissipating Inlet
CFD Analysis of Clarifier Performance With and Without Energy Dissipating Inlet Figure 1: Energy Dissipating Inlet (LA-EDI) Introduction To estimate performance enhancements resulting from the use of an
More informationAnalysis of Side Sluice in Trapezoidal Channel
Analysis of Side Sluice in Trapezoidal Channel Dr. L. G. Patil 1, Amol M. Kode 2 1 Associate Professor, Department of Civil Engineering, SGGSIE&T, Nanded 2 M. Tech Student, Department of Civil Engineering,
More informationStudy of water falling film over horizontal drop shaped and inverted drop shaped tubes
Study of water falling film over horizontal drop shaped and inverted drop shaped tubes Vipul Kumar Sharma, Nirmal Kant Singh 2 Dept. of Mechanical Engineering, GLBITM, Greater Noida, U.P, 236, India 2
More informationHeat transfer modelling of slot jet impinging on an inclined plate
Heat transfer modelling of slot jet impinging on an inclined plate A. Ramezanpour 1, H. Shirvani 1 & I. Mirzaee 2 1 School of Design and Communication Systems, APU University, UK 2 CFD Research Centre,
More informationPerformance of an Open Ducted Type Very Low Head Cross- Flow Turbine
Performance of an Open Ducted Type Very Low Head Cross- Flow Turbine Zhenmu Chen, Van Thanh Tien Nguyen, Morihito Inagaki, and Young-Do Choi * Abstract Cross Flow Turbine (CFT) known as a Banki turbine
More informationDerivation of Global Parametric Performance of Mixed Flow Hydraulic Turbine Using CFD. Ruchi Khare, Vishnu Prasad and Sushil Kumar
Derivation of Global Parametric Performance of Mixed Flow Hydraulic Turbine Using CFD Ruchi Khare, Vishnu Prasad and Sushil Kumar Ruchi Khare Vishnu Prasad Sushil Kumar Abstract: The testing of physical
More informationLateral Outflow from Supercritical Channels
Lateral Outflow from Supercritical Channels J. Coonrod 1, J. Ho 2 and N. Bernardo 3 1 Associate Professor, Department of Civil Engineering, University of New Mexico, Albuquerque, NM 87131; PH (505) 277-3233;
More informationCFD Analysis of a Low Head Propeller Turbine with Comparison to Experimental Data By: Artem Ivashchenko, Mechanical Solutions, Inc.
CFD Analysis of a Low Head Propeller Turbine with Comparison to Experimental Data By: Artem Ivashchenko, Mechanical Solutions, Inc. Edward Bennett, Mechanical Solutions, Inc. CFD Analysis of a Low Head
More informationThermal Management of Densely-packed EV Battery Set
EVS28 KINTEX, Korea, May 3-6, 2015 Thermal Management of Densely-packed EV Battery Set Abstract Z. Lu 1, X.Z. Meng 1, W.Y. Hu 2, L.C. Wei 3, L.Y. Zhang 1, L.W. Jin 1* 1 Building Environment and Equipment
More informationCRHT VII. Design and CFD analysis of Pico- hydro Turgo turbine. Paper no. CRHT17-11
Proceedings of the International Symposium on Current Research in Hydraulic Turbines CRHT VII April 04, 2016, Turbine Testing Lab, Kathmandu University, Dhulikhel, Nepal Paper no. CRHT17-11 Design and
More informationScienceDirect. CFD Analysis of a Kerosene Fuel Tank to Reduce Liquid Sloshing
Available online at www.sciencedirect.com ScienceDirect Procedia Engineering 69 ( 2014 ) 1365 1371 24th DAAAM International Symposium on Intelligent Manufacturing and Automation, 2013 CFD Analysis of a
More informationUse of computational fluid dynamics (CFD) for aquaculture raceway design to increase settling effectiveness
Aquacultural Engineering 33 (2005) 167 180 www.elsevier.com/locate/aqua-online Use of computational fluid dynamics (CFD) for aquaculture raceway design to increase settling effectiveness Dania L. Huggins,
More informationCFD analysis of high speed Francis hydraulic turbines
TRANSACTIONS OF THE INSTITUTE OF FLUID-FLOW MACHINERY No. 131, 2016, 111 120 Maciej Kaniecki a, Zbigniew Krzemianowski b CFD analysis of high speed Francis hydraulic turbines a Research and Development
More informationA NEW METHOD FOR EVALUATING PRIMARY CLARIFIERS Alex Ekster and Cristina Pena San Jose/Santa Clara Water Pollution Control Plant City of San Jose
A NEW METHOD FOR EVALUATING PRIMARY CLARIFIERS Alex Ekster and Cristina Pena San Jose/Santa Clara Water Pollution Control Plant City of San Jose ABSTRACT A new method has been developed for evaluating
More informationQuantification of diffuse dust emissions from open air sources on industrial sites
Proc. of the 3rd IASME/WSEAS Int. Conf. on Energy, Environment, Ecosystems and Sustainable Development, Agios Nikolaos, Greece, July 24-26, 2007 276 Quantification of diffuse dust emissions from open air
More informationCFD/FEM Based Analysis Framework for Wind Effects on Tall Buildings in Urban Areas
2017 2nd International Conference on Industrial Aerodynamics (ICIA 2017) ISBN: 978-1-60595-481-3 CFD/FEM Based Analysis Framework for Wind Effects on Tall Buildings in Urban Areas Qiao Yan, Dalong Li,
More informationThree-Dimensional Numerical Simulation of a Model Wind Turbine
Three-Dimensional Numerical Simulation of a Model Wind Turbine N. Tabatabaei 1, M.J. Cervantes 1,2, C. Trivedi 2, J-O Aidanpää 1 1 Luleå University of Technology, Sweden 2 Norwegian University of Science
More informationInternational Symposium on Current Research in HydraulicTurbines DESIGN AND CFD ANALYSIS OF PICO HYDRO TURGO TURBINE
Kathmandu University International Symposium on Current Research in HydraulicTurbines (CRHT-VII) DESIGN AND CFD ANALYSIS OF PICO HYDRO TURGO TURBINE Sudish Gyanwali 1*, Kush Kuikel 1 and Abinath Thapa
More informationEvaluation of the Flow Characteristics in the Intake Structure and Pump Sumps Using Physical Model
International Journal of Engineering Research and Technology. ISSN 0974-3154 Volume 7, Number 1 (2014), pp. 79-91 International Research Publication House http://www.irphouse.com Evaluation of the Flow
More informationCOOLING EFFECT ENHANCEMENT IN MAGNETRON SPUTTERING SYSTEM
Fifth International Conference on CFD in the Process Industries CSIRO, Melbourne, Australia 13-15 December 2006 COOLING EFFECT ENHANCEMENT IN MAGNETRON SPUTTERING SYSTEM Jae-Sang BAEK and Youn J. KIM*
More informationCFD simulation on the turbulent mixing flow performance of the liquid-liquid ejector
IOP Conference Series: Materials Science and Engineering PAPER OPEN ACCESS CFD simulation on the turbulent mixing flow performance of the liquid-liquid ejector To cite this article: W Z An et al 2016 IOP
More informationImproving Performance of Large Rectangular Secondary Clarifiers
Improving Performance of Large Rectangular Secondary Clarifiers S. Zhou, C. Vitasovic (Reid Crowther), J.A. McCorquodale (Univ. of New Orleans) and S. Lipke (Passaic Valley Sewerage Com.), M. DeNicola,
More informationAn Investigation of Oxide Layer Impact on Heat Transfer in a Fuel Element of the MARIA Reactor
Open Access Journal Journal of Power Technologies 93 (4) (2013) 247 256 journal homepage:papers.itc.pw.edu.pl An Investigation of Oxide Layer Impact on Heat Transfer in a Fuel Element of the MARIA Reactor
More informationNumerical Investigation of the Integration of Heat Transfer Devices into Wind Towers
A publication of CHEMICAL ENGINEERING TRANSACTIONS VOL. 34, 2013 Guest Editors: Neven Duić, Petar Sabev Varbanov Copyright 2013, AIDIC Servizi S.r.l., ISBN 978-88-95608-25-9; ISSN 1974-9791 The Italian
More informationApplication of CFD for Analyzing Quenching and Quench System Design. Andrew L. Banka
Application of CFD for Analyzing Quenching and Quench System Design Andrew L. Banka Purpose Quenching - one of last (and more dramatic) steps in heat treat process Poor quench? Distortion Part to part
More informationOptimization of embedded Heat Exchanger in a flat plate Integrated Collector Storage Solar Water Heater (ICSSWH), with indirect heat withdrawal.
World Renewable Energy Congress (WRECX) Editor A. Sayigh 2008 WREC. All rights reserved. 1815 Optimization of embedded Heat Exchanger in a flat plate Integrated Collector Storage Solar Water Heater (ICSSWH),
More informationNumerical Investigation of the Flow Structure in a Kaplan Draft Tube at Part Load
IOP Conference Series: Earth and Environmental Science PAPER OPEN ACCESS Numerical Investigation of the Flow Structure in a Kaplan Draft Tube at Part Load To cite this article: R Maddahian et al 2016 IOP
More informationFlow and Heat Transfer Characteristics in High Porosity Metal Foams
Proceedings of the World Congress on Mechanical, Chemical, and Material Engineering (MCM 2015) Barcelona, Spain July 20-21, 2015 Paper No. 333 Flow and Heat Transfer Characteristics in High Porosity Metal
More informationTheory Comparison between Propane and Methane Combustion inside the Furnace
International Journal of Current Engineering and Technology E-ISSN 2277 4106, P-ISSN 2347 5161 2015 INPRESSCO, All Rights Reserved Available at http://inpressco.com/category/ijcet Research Article Theory
More informationSimulation of the Flow in a Packed-Bed with and without a Static Mixer by Using CFD Technique
Simulation of the Flow in a Packed-Bed with and without a Static Mixer by Using CFD Technique Phavanee Narataruksa, Karn Pana-Suppamassadu, Sabaithip Tungkamani Rungrote Kokoo, and Prayut Jiamrittiwong
More informationComputer modelling of a convective steam superheater
Computer modelling of a convective steam superheater MARCIN TROJAN* Institute of Thermal Power Engineering, Faculty of Mechanical Engineering Cracow University of Technology Al. Jana Pawła II 37, 31-864
More informationLiquid-Solid Phase Change Modeling Using Fluent. Anirudh and Joseph Lam 2002 Fluent Users Group Meeting
Liquid-Solid Phase Change Modeling Using Fluent Anirudh and Joseph Lam 2002 Fluent Users Group Meeting Solidification Model FLUENT can be used to solve fluid flow problems involving both solidification
More informationPrediction of Pollutant Emissions from Industrial Furnaces Using Large Eddy Simulation
Paper # B03 Topic: Turbulent Flames 5 th US Combustion Meeting Organized by the Western States Section of the Combustion Institute and Hosted by the University of California at San Diego March 25-28, 2007.
More informationInvestigation of Surface Vortex Formation at Pump Intakes in PWR
Investigation of Surface Vortex Formation at Pump Intakes in PWR P. Pandazis 1, A. Schaffrath 1, F. Blömeling 2 1 Gesellschaft für Anlagen- und Reaktorsicherheit (GRS) ggmbh, Munich 2 TÜV NORD SysTec GmbH
More informationAn overview of CFD applications in flow assurance From well head to the platform. Simon Lo
An overview of CFD applications in flow assurance From well head to the platform Simon Lo Contents From well head to the platform Heat transfer in Christmas tree Multiphase flow in long pipe Severe slugging
More informationLocal Single- and Two-Phase Heat Transfer from an Impinging Cross-Shaped Jet
Purdue University Purdue e-pubs CTRC Research Publications Cooling Technologies Research Center 2014 Local Single- and Two-Phase Heat Transfer from an Impinging Cross-Shaped Jet M. J. Rau Purdue University
More informationCFD modeling of airflows and contaminant transport in an aircraft cabin
20th International Congress on Modelling and Simulation, Adelaide, Australia, 1 6 December 2013 www.mssanz.org.au/modsim2013 CFD modeling of airflows and contaminant transport in an aircraft cabin Jiuzhou
More informationNumerical Investigation of the Combustion of Methane Air Mixture in Gas Turbine Can-Type Combustion Chamber
International Journal of Scientific & Engineering Research, Volume 3, Issue 10, October-2012 1 Numerical Investigation of the Combustion of Methane Air Mixture in Gas Turbine Can-Type Combustion Chamber
More informationDEVELOPMENT AND PERFORMANCE TESTS OF A SEPARATOR FOR REMOVAL OF PHYSICALLY EMULSIFIED AND FREE OILS FROM WASTEWATERS
010-019 develop&perform 9/4/06 10:01 AM Page 10 DEVELOPMENT AND PERFORMANCE TESTS OF A SEPARATOR FOR REMOVAL OF PHYSICALLY EMULSIFIED AND FREE OILS FROM WASTEWATERS Law Puong Ling, Ngu Lock Hei, Wong Kien
More informationCFD ANALYSIS OF MINI CHANNEL HEAT EXCHANGER USING WATER AS A WORKING FLUID
CFD ANALYSIS OF MINI CHANNEL HEAT EXCHANGER USING WATER AS A WORKING FLUID Bhavesh K. Patel 1, Ravi S. Engineer 2, Mehulkumar H. Tandel 3 1 Assistant Professor, Mechanical Engineering, Government Engineering
More informationImpellers of low specific speed centrifugal pump based on the draughting technology
IOP Conference Series: Earth and Environmental Science Impellers of low specific speed centrifugal pump based on the draughting technology To cite this article: C Hongxun et al 2010 IOP Conf. Ser.: Earth
More informationOn Wave-Defect Interaction in Pressurized Conduits
IAHR-HK Student Research Forum, November 17, 2012 On Wave-Defect Interaction in Pressurized Conduits Moez LOUATI, Prof. Mohamed S. GHIDAOUI Department of Civil and Environmental Engineering, Hong Kong
More information40-Ton Articulated Truck Cooling System Modelling Using STAR-CCM+
40-Ton Articulated Truck Cooling System Modelling Using STAR-CCM+ Gary Yu, Martin Timmins and Mario Ciaffarafa DENSO Marston Ltd, Bradford, BD17 7JR, UK DENSO Marston Founded in 1904 Acquired by DENSO
More informationAbstract. Nomenclature. A Porosity function for momentum equations L Latent heat of melting (J/Kg) c Specific heat (J/kg-K) s Liquid fraction
Enthalpy Porosity Method for CFD Simulation of Natural Convection Phenomenon for Phase Change Problems in the Molten Pool and its Importance during Melting of Solids Abstract Priyanshu Goyal, Anu Dutta,
More informationComparison of RANS, URANS and LES in the Prediction of Airflow and Pollutant Dispersion
Comparison of RANS, URANS and LES in the Prediction of Airflow and Pollutant Dispersion S. M. Salim, K. C. Ong, S. C. Cheah Abstract The performance of three different numerical techniques, i.e. RANS,
More informationNumerical study of the influence of injection/production well perforation location on CO 2 -EGS system
Available online at www.sciencedirect.com Energy Procedia 00 (2013) 000 000 www.elsevier.com/locate/procedia GHGT-11 Numerical study of the influence of injection/production well perforation location on
More informationInternational Journal of Engineering Research & Technology (IJERT) ISSN: Vol. 2 Issue 9, September
Towards a First C.F.D. Study of Innovative Archimedean Inclined Axis Hydropower Turbines Alkistis Stergiopoulou Ph.D. Candidate, M.Sc., National Technical University of Athens, Department of Water Resources
More informationModeling Flow through a Lock Manifold Port
Modeling Flow through a Lock Manifold Port by Richard L. Stockstill and E. Allen Hammack BACKGROUND: Manifolds are essential components of a navigation lock s filling and emptying system. They are used
More informationTask 1 For Task 1, the outlet was set as a zero-gauge pressure outlet, which is the same outlet condition as the five smaller pipes.
Jacob Schichtel Project 2 Page 1 of 9 Setup The geometry was created in ANSYS Design modeler as specified in the report instructions. A plane of symmetry was used to reduce the computation time and to
More informationOPTIMIZED DESIGN FOR HEAVY MOUND VENTURI
THERMAL SCIENCE, Year 2017, Vol. 21, No. 4, pp. 1873-1878 1873 OPTIMIZED DESIGN FOR HEAVY MOUND VENTURI by Futang XING *, Yuheng LI, Dan MEI, Shunfeng GUI, and Liya WANG Hubei Key Laboratory for Efficient
More informationProject Title: Development of a High-Resolution Virtual Wind Simulator for Optimal Design of Wind Energy Projects
Twin Cities Campus Saint Anthony Falls Laboratory Engineering, Environmental, Biological and Geophysical Fluid Dynamics College of Science and Engineering Mississippi River at 3 rd Avenue S.E. Minneapolis,
More informationHydraulic performance of a low specific speed centrifugal pump with Spanwise-Slotted Blades
IOP Conference Series: Materials Science and Engineering OPEN ACCESS Hydraulic performance of a low specific speed centrifugal pump with Spanwise-Slotted Blades To cite this article: D X Ye et al 2013
More informationDetermination of Wall Pressure and Stress an Blast Furnace using Finite Element and SPH Method
Determination of Wall Pressure and Stress an Blast Furnace using Finite Element and SPH Method Mukul Mandal Bhaskar Sengupta Manager, Tech cell Head, Tech cell M&M, L&T Construction M&M, L&T Construction
More informationPerformance Analysis for Natural Draught Cooling Tower & Chimney through Numerical Simulation
Performance Analysis for Natural Draught Cooling Tower & Chimney through Numerical Simulation Kanteyya A 1, Kiran Kumar Rokhade 2 Assistant Professor, Department of Mechanical Engineering, HKESSLN College
More informationAgenda. Background Validation studies. 3D application. Co-simulation. Summary. Espedal stratified flow. StatOil wavy-slug flow.
www.cd-adapco.com Computational Flow Assurance Recent progress in modelling of multiphase flows in long pipelines Simon Lo, Abderrahmane Fiala (presented by Demetris Clerides) Subsea Asia 2010 Agenda Background
More informationDevelopment of Wind Tunnel for Ultrafine Palm Oil Fuel Ash Separator
Development of Wind Tunnel for Ultrafine Palm Oil Fuel Ash Separator Sylvester Kenneth Sedah 1, Ana Sakura Zainal Abidin 1,a, A. Rigit 1, Mohd Azlan Ismail 2, Raudhah Ahmadi 3, and Md Abdul Mannan 3 1
More informationELBE RIVER MODEL: UVP FLOW MAPPING
ELBE RIVER MODEL: UVP FLOW MAPPING Vojtech Bares 1 and Prof. Vojtech Broza 2 1 Doctorand, Czech Technical University in Prague, Faculty of Civil Engineering, Laboratory of Ecological Risks in Urban Drainage,
More informationOptimization of abrasive waterjet nozzle design for precision and reduced wear using compressible multiphase CFD modelling
Optimization of abrasive waterjet nozzle design for precision and reduced wear using compressible multiphase CFD modelling C. Narayanan, D. Caviezel, D. Lakehal ASCOMP AG Technoparkstrasse 1, 8005 Zurich,
More informationHeat Storage Performance of a Honeycomb Ceramic Monolith
Send Orders for Reprints to reprints@benthamscience.ae The Open Fuels & Energy Science Journal, 2014, 7, 113-120 113 Heat Storage Performance of a Honeycomb Ceramic Monolith Xiaoni Qi * and Yongqi Liu
More informationA NOVEL TECHNIQUE FOR EXTRACTION OF GEOTHERMAL ENERGY FROM ABANDONED OIL WELLS
A NOVEL TECHNIQUE FOR EXTRACTION OF GEOTHERMAL ENERGY FROM ABANDONED OIL WELLS Seyed Ali Ghoreishi-Madiseh McGill University 3450 University St., Room 125 Montreal, QC, Canada H3A2A7 e-mail: seyed.ghoreishimadiseh
More informationFINITE ELEMENT MODELLING OF ELECTRIC CURRENTS IN AC SUBMERGED ARC FURNACES
FINITE ELEMENT MODELLING OF ELECTRIC CURRENTS IN AC SUBMERGED ARC FURNACES I. Mc Dougall CSIR, P. O. Box 395, Pretoria, 0001, South Africa E-mail: imcdougall@csir.co.za ABSTRACT Finite element models were
More informationVortex Separator. May be more cost-effective pre-treatment devices than traditional wet or dry basins.
Description Vortex separators: (alternatively, swirl concentrators) are gravity separators, and in principle are essentially wet vaults. The difference from wet vaults, however, is that the vortex separator
More informationDESIGN, SIMULATION AND ANALYSIS OF A HYBRID-TYPE (PV/T) SOLAR AIR HEATER FOR HIGH PERFORMANCE
DESIGN, SIMULATION AND ANALYSIS OF A HYBRID-TYPE (PV/T SOLAR AIR HEATER FOR HIGH PERFORMANCE Pramod kumar N Research Scholar, Department of Mechanical Engineering, VVCE, Msuru B. Sadashive Gowda Principal,
More informationSmoke Dispersion from Stacks on Pitched-Roof Buildings: Model Calculations Using MISKAM in Comparison with Wind Tunnel Results
Smoke Dispersion from Stacks on Pitched-Roof Buildings: Model Calculations Using MISKAM in Comparison with Wind Tunnel Results Konstantinos E. Kakosimos 1 Marc J. Assael 1 Matthias Ketzel 2 Helge Rørdam
More informationSanitary and Environmental Engineering I (4 th Year Civil)
Sanitary and Environmental Engineering I (4 th Year Civil) Prepared by Dr.Khaled Zaher Assistant Professor, Public Works Engineering Department, Faculty of Engineering, Cairo University Wastewater Flow
More informationComparison between 2D and 3D Hydraulic Modelling Approaches for Simulation of Vertical Slot Fishways
5 th International Symposium on Hydraulic Structures Brisbane, Australia, 25-27 June 2014 Hydraulic Structures and Society: Engineering Challenges and Extremes ISBN 9781742721156 - DOI: 10.14264/uql.2014.49
More informationField and CFD Analysis of Jet Aeration and Mixing
Field and CFD Analysis of Jet Aeration and Mixing Randal W. Samstag 1 *, Edward A. Wicklein 1, Roderick D. Reardon 2, Robert J. Leetch 3, R. (Robbie) M. Parks 3, and Colin D. Groff 3 1 Carollo Engineers,
More informationCFD Analysis of Mixing in Large Aerated Lagoons
Engineering Applications of Computational Fluid Mechanics ISSN: 1994-2060 (Print) 1997-003X (Online) Journal homepage: http://www.tandfonline.com/loi/tcfm20 CFD Analysis of Mixing in Large Aerated Lagoons
More informationWATER QUALITY MODELING FOR BOD and COD CONTROL STRATEGIES FOR THE BURIGANGA RIVER OF BANGLADESH
Proceedings of the 13 th International Conference of Environmental Science and Technology Athens, Greece, 5-7 September 13 WATER QUALITY MODELING FOR BOD and COD CONTROL STRATEGIES FOR THE BURIGANGA RIVER
More informationLarge Scale Outdoor Flammable & Toxic Gas Dispersion Modelling in Industrial Environments.
Excerpt from the Proceedings of the COMSOL Conference 2009 Milan Large Scale Outdoor Flammable & Toxic Gas Dispersion Modelling in Industrial Environments. A. Hallgarth* 1, A. Zayer 1, A. Gatward 2 and
More informationModeling and experimental results of heavy oil injection into a high pressure entrained flow gasifier
Modeling and experimental results of heavy oil injection into a high pressure entrained flow gasifier André Bader 1, Paul Tischer 1, Peter Seifert 1, Andreas Richter 2, Bernd Meyer 1 Institute of Energy
More informationORCHID Turbine. Fluid-dynamic design and characterization of a mini-orc turbine for laboratory experiments
Prof. ORCHID Turbine Fluid-dynamic design and characterization of a mini-orc turbine for laboratory experiments M. Pini, C. De Servi, M. Burigana, S. Bahamonde, A. Rubino, S. Vitale, P. Colonna ORC2017-14/09/2017
More informationCombustion in anode baking furnaces: Comparison of two modeling approaches to predict variability
338 Proceedings of Combustion Institute Canadian Section Spring Technical Meeting Université Laval May 13-16, 2013 Combustion in anode baking furnaces: Comparison of two modeling approaches to predict
More informationThermal Dispersion Model for Cooling Water of Thermal Power Plant System
International Journal of Current Engineering and Technology E-ISSN 2277 4106, P-ISSN 2347 5161 2015INPRESSCO, All Rights Reserved Available at http://inpressco.com/category/ijcet Research Article Thermal
More informationFluid dynamics of a post-combustion chamber in electric arc steelmaking plants
Computational Methods and Experimental Measurements XV 205 Fluid dynamics of a post-combustion chamber in electric arc steelmaking plants L. Labiscsak 1, G. Straffelini 1, C. Corbetta 2 & M. Bodino 2 1
More informationEFFECT OF THE NOZZLE EXIT POSITION ON THE EFFICIENCY OF EJECTOR COOLING SYSTEM USING R134A
EFFECT OF THE NOZZLE EXIT POSITION ON THE EFFICIENCY OF EJECTOR COOLING SYSTEM USING R134A K. Sopian 1, B. Elhub 1, Sohif Mat 1, A. N. Al-Shamani 1, AM Elbreki 1, Azher M. Abed 1, Husam Abdulrasool Hasan
More informationNumerical Modelling of Air Distribution in the Natatorium Supported by the Experiment
Proceedings of the World Congress on Mechanical, Chemical, and Material Engineering (MCM 2015) Barcelona, Spain July 20-21, 2015 Paper No. 277 Numerical Modelling of Air Distribution in the Natatorium
More informationNew Developments in Design and Application of Long-Throated Flumes
New Developments in Design and Application of Long-Throated Flumes Tony L. Wahl (1), John A. Replogle (2), Brian T. Wahlin (3), and James A. Higgs (4) (1) Hydraulic Engineer, U.S. Bureau of Reclamation,
More informationAnalysis of the corrosion test process for heat exchangers in corrosion test chambers by CFD simulation
Analysis of the corrosion test process for heat exchangers in corrosion test chambers by CFD simulation STAR Global Conference, Wien, March 17-19, 2014 R. Stauch, F. Brändle, M. Pfitzer, W. Kühnel MAHLE
More informationComparison of experimental results of horizontal kaplan turbine with computational fluid dynamics
University of Iowa Iowa Research Online Theses and Dissertations Summer 2012 Comparison of experimental results of horizontal kaplan turbine with computational fluid dynamics Vijaya Bijukchhe University
More informationHigh Performance. Uniform Distribution
Water Technologies Peripheral Feed - Peripheral Take-Off Clarifier Middle East Project was able to reduce the number of clarifier units from ten to six, providing a significant savings in capital cost.
More informationVI. WATER QUALITY MODELING
VI. WATER QUALITY MODELING As was mentioned previously in Chapter V, the Hamblin Pond/Jehu Pond and Quashnet River sub-systems of Waquoit Bay were a part of the larger hydrodynamic model of the Waquoit
More informationHeat Transfer Simulation of Impinging Jet with Finned Heat Sink
Heat Transfer Simulation of Impinging Jet with Finned Heat Sink Shivakumar H 1, Krishnamurthy K N 2, Akashdeep B.N 3 Department of Thermal power Engineering, M.Tech student 1, Assistant professor 2, VTU
More informationIDENTIFICATION OF VENTILATION PROBLEMS IN AN UNDERGROUND BUS TERMINAL IN KOREA
IDENTIFICATION OF VENTILATION PROBLEMS IN AN UNDERGROUND BUS TERMINAL IN KOREA H Han 1* and Y-I Kwon 2 1 Dept. Of Mechanical Engineering, Kookmin University, Korea 2 Dept. Of Building Mechanical Engineering,
More informationDevelopment of hydraulic tanks by multi-phase CFD simulation
Group M - Hydraulic Components Paper M-4 619 Development of hydraulic tanks by multi-phase CFD simulation Dipl.-Ing. Thees Vollmer Institute for Mobile Machines and Commercial Vehicles (IMN), Technische
More information7.0 GROUNDWATER AND STABILIZER TRANSPORT MODELING
7.0 GROUNDWATER AND STABILIZER TRANSPORT MODELING 7.1 Introduction The concept of passive site remediation is the slow injection of stabilizing materials at the up gradient edge of a site and delivery
More informationComputational Fluid Dynamic Analysis of Cross Flow Turbine
Computational Fluid Dynamic Analysis of Cross Flow Turbine Mrudang Patel, Nirav Oza, Karna Patel U.G. Student, Department of Mechanical Engineering, NIRMA University, Ahmedabad, Gujarat, India ABSTRACT:
More informationThe Influence of Hydrodynamics on the Spread of. Pollutants in the Confluence of two Rivers
Applied Mathematical Sciences, Vol. 7, 13, no. 123, 6115-6123 HIKARI Ltd, www.m-hikari.com http://dx.doi.org/.12988/ams.13.39527 The Influence of Hydrodynamics on the Spread of Pollutants in the Confluence
More informationEXPERIMENTAL STUDY OF EFFECT OF END SILL ON STILLING BASIN PERFORMANCE
EXPERIMENTAL STUDY OF EFFECT OF END SILL ON STILLING BASIN PERFORMANCE H.L.Tiwari Department of Civil Engineering, Maulana Azad National Institute of Technology, Bhopal, Madhya Pradesh INDIA Arun Goel
More informationCFD on Small Flow Injection of Advanced Accumulator in APWR
54 CFD on Small Flow Injection of Advanced Accumulator in APWR TOMOSHIGE TAKATA TAKAFUMI OGINO TAKASHI ISHIBASHI TADASHI SHIRAISHI The advanced accumulator in the advanced pressurized-water reactor is
More informationCFD Simulation Studies on Integrated Approach of Solar Chimney and Earth Air Tunnel Heat Exchanger for Building Space Conditioning
International Journal of Economy, Energy and Environment 2017; 2(3): 32-39 http://www.sciencepublishinggroup.com/j/ijeee doi: 10.11648/j.ijeee.20170203.11 CFD Simulation Studies on Integrated Approach
More informationComparison Between PIV Measurements and CFD Simulation on a Model of GT Annular Burner
Comparison Between PIV Measurements and CFD Simulation on a Model of GT Annular Burner D. Giordano, S. Giammartini, M. Rufoloni, G. Calchetti, F. Manfredi, E. Giacomazzi ENEA - C. R. Casaccia Sec. ENE-IMP
More informationAerodynamic Design of 2.5 MW Horizontal Wind Turbine Blade in Combination with CFD Analysis
Aerodynamic Design of 2.5 MW Horizontal Wind Turbine Blade in Combination with CFD Analysis Seul-Ki Yeom *, Tae-Jin Kang *, Warn-Gyu Park 1) School of Mechanical Engineering, Pusan National University,
More informationSimulation of Engine Flow with Swirl Using Re-Stress Turbulence Model in KIVA Code
Simulation of Engine Flow with Swirl Using Re-Stress Turbulence Model in KIVA Code S. L. Yang, * Y. K. Siow, and B. D. Peschke Michigan Technological University and R. R. Tacina NASA John H. Glenn Research
More informationA Modeling of Biomass Fast Pyrolysis using CFD in a fluidized bed reactor
Ref: C0273 A Modeling of Biomass Fast Pyrolysis using CFD in a fluidized bed reactor Young Min Ju, Department of Biosystems Engineering, Kangwon National University, Hyoja 2 Dong, 192-1 Chuncheon, Republic
More information