Urea Injection Simulation with Adaptive Mesh Refinement for Engine Aftertreatment
|
|
- David Lambert
- 6 years ago
- Views:
Transcription
1 ILASS Americas 26th Annual Conference on Liquid Atomization and Spray Systems, Portland, OR, May 2014 Urea Injection Simulation with Adaptive Mesh Refinement for Engine Aftertreatment Scott A. Drennan Convergent Science, Inc E. Common Street, Suite 1204 New Braunfels, TX USA Abstract Controlling NOx emissions from vehicles is a key aspect of meeting new regulations for cars and trucks across the world. Selective Catalytic Reduction (SCR) is an NOx reduction option that many engine manufacturers are adopting. The performance of urea injection and mixing upstream of an SCR catalyst is critical in obtaining reliable NOx reduction. Computational Fluid Dynamic (CFD) simulations of urea injection systems have become an important development and diagnostic tool for designers. Designers are interested in applying more accurate spray and kinetic models to their CFD simulations and in reducing mesh generation time. This paper presents the application of an automatically generated Cartesian meshing approach to a urea liquid injection system with RANS CFD simulation. Investigations of the impact of injection and mesh refinement strategy with RANS simulation is presented for a commonly accepted urea injected validation case. A modified cut-cell Cartesian method is used that eliminates the need for the computational grid to be morphed with the geometry of interest while still representing the true boundary shape. This approach allows for the use of simple orthogonal grids and completely automates the mesh generation process. The meshing approach also utilizes Adaptive Mesh Refinement (AMR) to resolve the domain near geometric features and in regions near the spray. AMR allows the use of a very fine grid in the vicinity of the spray while keeping the overall cell count relatively low.
2 Introduction Today s global regulations have made engine aftertreatment a necessity rather than an option for on and off-road powertrain systems. Engine aftertreatment for NOx in diesel fueled systems is looking to urea injection and Selective Catalytic Reduction (SCR) to achieve NOx reduction. The urea injection and SCR systems is often combined with a NOx trap. The urea injection/scr system is then operated when the NOx trap flushes itself and a large amount of NOx is emitted. The application of urea injection and SCR for NOx treatment is not new. Power boilers have used both urea injection with and without SCR for more than 10 years. The efficacy of the NOx reduction of a urea injection/scr system is often linked to the uniformity of the distribution of ammonia (NH3) upstream of the catalyst. The engine aftertreatment designer rarely has the ability to influence the surface chemistry inside of the SCR catalyst as these are most often supplied by third party vendors. However, the engine aftertreatment designer has control over the injection and atomization of the urea and how that urea decomposes into ammonia and is mixed prior to entering the SCR. The urea injection/scr system designer is working to balance the competing objectives of generating a uniform ammonia distribution upstream of the SCR catalyst and the overall pressure drop associated with the mixing strategy and the capital, operational and maintenance costs of the unit. Good urea/water injection and mixing is critical to produce the HCNO and NH3 gas phase mixture and then to promote decomposition of the HCNO into NH3. Substantial effort is expended to develop static mixers that are good a mixing the flow at a low pressure drop and are inexpensive to manufacture. Typical urea injection/scr mixers are complicated geometries yet simple in design; such as stamped thin metal plates with variations in all three directions. Background Computational Fluid Dynamics (CFD) offers the designer a valuable tool in the design and analysis of urea injection/scr systems. However, traditional CFD approaches use complex meshes that must be created in advance and can add weeks to the CFD simulation timeframe. It is also imperative the CFD analysis use the proper mesh and atomization models to capture spray behavior correctly. Finally, thin and complicated mixer plate designs add complexity and require more effort to mesh. Mesh generation represents a large portion of the CFD design flow in order to accommodate complex combustor and fuel injector geometries. Additionally, highly skewed non-orthogonal meshes slow CFD simulations while introducing computational errors. It is not uncommon for non-orthogonal, polyhedral meshes to have cells with negative volume. The optimal mesh for CFD simulation numerical accuracy and computational speed is Cartesian. The approach presented in this paper uses a Cartesian mesh that is automatically generated from combustor geometry and uses Adaptive Mesh Refinement (AMR) to deliver the required mesh resolution for the model being used. Modeling Approach In this work, the CONVERGE CFD software package [1] is used as the computational framework for running the spray and combustion simulations. CON- VERGE is a general purpose CFD code for the calculation of three-dimensional, incompressible or compressible, chemically-reacting fluid flows in complex geometries with stationary or moving boundaries. CON- VERGE can handle an arbitrary number of species and chemical reactions, as well as transient liquid sprays, and laminar or turbulent flows. CONVERGE uses an innovative modified cut-cell Cartesian method that eliminates the need for the computational grid to be morphed with the geometry of interest while still precisely representing the true boundary shape. This approach allows for the use of simple orthogonal grids and completely automates the mesh generation process. This section presents a brief overview of the mesh manipulation, numerical algorithms, and physical submodels used in the current work as these elements all contribute to the grid convergence behavior achieved. Fixed Embedding and AMR It is often desirable to add grid resolution locally in critical flow sections of the domain while leaving less critical sections relatively coarse. For example, in the present work, extra grid resolution was added to resolve the complex flow behavior at the nozzle exit, while leaving the remaining grid coarse to minimize simulation time. It is important to note that fixed embedding is specified in a small volume close to the nozzle and is only meant to seed the adaptive mesh refinement described below. In most cases, it is difficult to determine a priori where fixed grid embedding should be added. In these cases, Adaptive Mesh Refinement (AMR) can be applied. Ideally, a good AMR algorithm should add embedding where the flow field is most under-resolved or where the sub-grid field is the largest. The current flow solver estimates the magnitude of the sub-grid field to determine where embedding is added. A cell is embedded if the absolute value of the subgrid is above a user-specified value. Conversely, a cell is released (i.e., the embedding is removed) if the absolute value of the sub-grid is below a user-specified value. To limit the number of embedded cells, a maximum overall number of cells can be specified by the
3 user. With this feature, the user can specify the total number of cells desired in the simulation and AMR will determine where to put the embedding to both best resolve the flow field and meet the target number of cells. Numerical Algorithms In the present CFD solver, all computed values are collocated at the center of the computational cell. To prevent checker-boarding, the Rhie-Chow [2] algorithm is employed. The conservation equations are solved using the finite volume method. In the present study a second-order-accurate spatial discretization scheme is used for the governing conservation equations. In order to maintain stability, time accuracy is set to first order by running fully implicit. The transport equations are solved using the Pressure Implicit with Splitting of Operators (PISO) method. A geometric multigrid solver is used for the pressure solution. Variable time-stepping is used in the current study. The time-step is automatically calculated each computational cycle based on maximum allowed Courant-Friedrichs-Lewy (CFL) numbers for convection, diffusion and the speed of sound. Note that these CFL constraints are maintained for accuracy, and not for stability. In addition, spray and evaporation timestep control methods are used in the present simulations. The calculations in this study are run in parallel on distributed memory machines using the Message Passing Interface (MPI). An automatic domain decomposition technique is employed which allows for efficient load balancing throughout the calculation as the distribution of cells can change significantly due to AMR. Approach to Achieving Grid Convergence This section summarizes the key elements of the computational methodology that result in the grid convergent behavior demonstrated below. Specifically, the following items are critical to achieving grid convergence: 1. Adaptive Mesh Refinement (AMR) Demonstration of grid convergence can only be accomplished if cell sizes below the point of convergence can be simulated. AMR allows the use of a very fine grid in the vicinity of the spray while keeping the overall cell count relatively low. (see Figure 1) 2. Fully implicit momentum coupling Grid convergence cannot be adequately demonstrated if running with a fine mesh causes numerical instabilities. As described in [20], previous studies suffered from such instabilities when the cell size was on the order of the nozzle diameter or smaller. The current methodology utilizes a fully implicit liquid-gas momentum coupling approach to keep the simulations stable in the presence of small cells and high liquid volume fractions. Specifically, an iterative technique is used where the drag is calculated for all drops in a cell and the gas phase velocity is updated accordingly. This updated gasphase velocity is used to calculate drag on all of the drops in the cell which is then used to update the gas-phase velocity. This process is repeated until the drop and gasphase velocities converge to the specified tolerance. 3. Improved liquid-gas coupling The current methodology utilizes a Taylor series expansion to calculate the gas-phase velocity in the liquid-gas coupling calculations. 4. Spray-wall interactions Accounting for spraywall interactions is important in urea/water injection systems. Spray-wall interactions account in the CFD code account for droplet impingement, liquid pooling on the wall, pool evaporation along the wall and droplet rebound from the wall. (see Figure 2) 5. Conjugate Heat Transfer (CHT) As urea/water sprays can impact upon surfaces within the exhaust system, the mixer and the SCR catalyst, CHT must be employed to account for local variations in material temperatures that impact vaporization and reactions. The CFD code employs fully-coupled CHT for such analysis. CFD Model Description The CFD model used in the present study has been used extensively by the community as a validation case for urea/water injection and generation of ammonia upstream of a catalyst. The current model is of a simple pipe (300mm dia. vs. 6m long) with simulated exhaust flow at 673K entering from a circular inlet with a constant pressure outlet at 100kPa (Figure 3). Urea/Water spray (40%/60%) is injected with a Rosin-Rammler size distribution and average SMD of 44µm (Figure 4). Secondary breakup is accounted for with TAB breakup. The simulation results provide gas-phase and liquidphase local compositions, temperatures and exit distributions of NH3, HCNO and dispersed phase. Thermolysis of the urea/water spray is modeled where water and urea are evaporated and urea(l) decomposes generating gas-phase NH3 and HCNO. Subsequently, the HCNO converts to NH3 using a detailed chemical mechanism. Adaptive Mesh Refinement surrounding the spray and fixed mesh embedding are used to provide the proper amount of mesh resolution for the spray model. (see Figure 5). Results The urea/water hollow-cone spray exits from the atomizer and spreads nearly two-thirds of the width of the pipe initially (see Figure 6). As the urea/water spray translates down the pipe, the water is initially evaporated and drop size decreasing leaving urea(l) and gaseous ammonia and HCNO (see Figure 7). The impact of the evaporating water is to reduce the local tem-
4 perature and increase the concentration of urea(l) in the droplets which inhibits urea(l) thermolysis. The gas-phase reaction converting HCNO to NH3 is temperature and local gas composition dependent. Figure 8 shows side by side comparisons of the local gas-phase temperature, water vapor mole fraction and the NH3 mole fraction. Finally, the distribution of ammonia at the exit of the domain is plotted with the droplet size in Figure 9. Summary A urea/water injection system has been simulated using an approach with automatic mesh generation enhanced with Adaptive Mesh Refinement for gridconvergent CFD. The urea/water system simulated was a 40/60 blend (urea/water) injected through a hollowcone spray with heat transfer and detailed chemical kinetics to account for thermolysis of the urea liquid and decomposition to ammonia. Grid-convergent spray modeling in this application is achieved through the use of fixed mesh embedding and Adaptive Mesh Refinement on spray parameters. The Urea/Water spray was shown to evaporate water first and then urea liquid which then decomposed into HCNO and NH3. The resulting ammonia distribution at the exit was shown to be concentrated around the centerline without the benefit of a mixer. The automatic mesh generation approach with Adaptive Mesh Refinement and grid embedding around sprays and geometric feature can be used to simulate full urea/water systems with complex geometries without user-time spent in mesh generation. Conference, ICEF , Vancouver, Canada, Senecal, P. K., Pomraning, E., Richards, K., and Som, S., An Investigation of Grid Convergence for Spray Simulations using an LES Turbulence Model, SAE , Som S., Longman, D. E., Luo, Z., Plomer, M., Lu, T., Senecal, P. K., and Pomraning, E., Simulating Flame Lift-Off Characteristics of Diesel and Biodiesel Fuels Using Detailed Chemical-Kinetic Mechanisms and Large Eddy Simulation Turbulence Model, J. Energy Resour. Technol., 134, Senecal, P. K., Richards, K. J., Pomraning, E., Yang, T., Dai, M. Z., McDavid, R. M., Patterson, M. A., Hou, S., and Shethaji, T., A New Parallel Cut-Cell Cartesian CFD Code for Rapid Grid Generation Applied to In-Cylinder Diesel Engine Simulations, SAE , Pomraning, E. and Rutland, C. J., Dynamic One- Equation Nonviscosity Large-Eddy Simulation Model, AIAA J., 40, No. 4, April Pomraning, E., Development of Large Eddy Simulation Turbulence Models, Ph.D. Thesis, University of Wisconsin-Madison, J.Y. Kim, S.H. Ryu, and J.S. Ha. Numerical Prediction on the characteristics of spray-induced mixing and thermal decomposition of urea solution in SCR system. In Proc Fall Technical Conference of the ASME Internal Combustion Engine Division, Long Beach, California USA, F. Birkhold, et al. Analysis of the Injection of Urea water solution for automotive SCR DeNOx Systems: Modeling of the Two phase Flow and Spray/Wall Interaction SAE Acknowledgements The author wishes to acknowledge the assistance from colleagues Mingjie Wang, Shaoping Quan, Gaurav Kumar and Peter Kelley Senecal. References 1. Richards, K. J., Senecal, P. K., and Pomraning, E., CONVERGE (Version 2.1.0) Manual, Convergent Science, Inc., Middleton, WI, Rhie, C. M. and Chow, W. L., Numerical Study of the Turbulent Flow Past an Airfoil with Trailing Edge Separation, AIAA J., 21, , Senecal, P. K., Pomraning, E., Richards, K., and Som, S., Grid Convergent Spray Models for Internal Combustion Engine CFD Simulations, Proceedings of the ASME 2012 Internal Combustion Engine Division Fall Technical Figure 1: Adaptive Mesh Refinement of a spray for grid-convergent CFD
5 Figure 2: Spray-Wall interactions with Adaptive Mesh Refinement showing impingement, pooling and rebound Figure 3: Urea/Water injection CFD case Figure 4: Closeup of computational domain showing injector location, spray fixed grid embedding and the surface mesh
6 Figure 5: Closeup of the spray region fixed mesh embedding near the atomizer Figure 6: Droplet near-field in the Urea/Water spray
7 Figure 7: Urea/Water injection simulation results for droplet size and ammonia concentration Figure 8: Simulation results for temperature, water vapor and ammonia concentration
8 Figure 9: Visualization of the Urea/Water spray with ammonia concentration
Numerical study & validation of a complete
Numerical study & validation of a complete SCR system using 1D-3D (CFD) coupling Presenter: Ashish Joshi Manager, Indian Operations Convergent Science Presenting on behalf of: Scott Drennan Director of
More informationPRESSURE DROP AND FLOW UNIFORMITY ANALYSIS OF COMPLETE EXHAUST SYSTEMS FOR DIESEL ENGINES
PRESSURE DROP AND FLOW UNIFORMITY ANALYSIS OF COMPLETE EXHAUST SYSTEMS FOR DIESEL ENGINES André Bergel 1 Edson L. Duque 2 General Motors Global Propulsion Systems South America 12 E-mail: andrebergel84@yahoo.com.br
More informationA Generalized Adaptive Collision Mesh for Multiple Injector Orifices
A Generalized Adaptive Collision Mesh for Multiple Injector Orifices Shuhai Hou, Sasanka Are, David P. Schmidt University of Massachusetts-Amherst ABSTRACT An algorithm for creating a generalized adaptive
More informationModeling Evaporating Liquid Spray
Tutorial 16. Modeling Evaporating Liquid Spray Introduction In this tutorial, FLUENT s air-blast atomizer model is used to predict the behavior of an evaporating methanol spray. Initially, the air flow
More informationModeling Evaporating Liquid Spray
Tutorial 17. Modeling Evaporating Liquid Spray Introduction In this tutorial, the air-blast atomizer model in ANSYS FLUENT is used to predict the behavior of an evaporating methanol spray. Initially, the
More informationKEY STAR TECHNOLOGIES: DISPERSED MULTIPHASE FLOW AND LIQUID FILM MODELLING DAVID GOSMAN EXEC VP TECHNOLOGY, CD-adapco
KEY STAR TECHNOLOGIES: DISPERSED MULTIPHASE FLOW AND LIQUID FILM MODELLING DAVID GOSMAN EXEC VP TECHNOLOGY, CD-adapco INTRODUCTION KEY METHODOLOGIES AVAILABLE IN STAR-CCM+ AND STAR-CD 1. Lagrangian modelling
More informationNUMERICAL VISCOSITY. Convergent Science White Paper. COPYRIGHT 2017 CONVERGENT SCIENCE. All rights reserved.
Convergent Science White Paper COPYRIGHT 2017 CONVERGENT SCIENCE. All rights reserved. This document contains information that is proprietary to Convergent Science. Public dissemination of this document
More informationApplying Solution-Adaptive Mesh Refinement in Engine Simulations
International Multidimensional Engine Modeling User's Group Meeting April 11, 2016, Detroit, Michigan Applying Solution-Adaptive Mesh Refinement in Engine Simulations Long Liang, Yue Wang, Anthony Shelburn,
More informationIntroduction to C omputational F luid Dynamics. D. Murrin
Introduction to C omputational F luid Dynamics D. Murrin Computational fluid dynamics (CFD) is the science of predicting fluid flow, heat transfer, mass transfer, chemical reactions, and related phenomena
More informationAir Assisted Atomization in Spiral Type Nozzles
ILASS Americas, 25 th Annual Conference on Liquid Atomization and Spray Systems, Pittsburgh, PA, May 2013 Air Assisted Atomization in Spiral Type Nozzles W. Kalata *, K. J. Brown, and R. J. Schick Spray
More informationValidation of an Automatic Mesh Generation Technique in Engine Simulations
International Multidimensional Engine Modeling User's Group Meeting April,, Detroit, Michigan Validation of an Automatic Mesh Generation Technique in Engine s Abstract Long Liang, Anthony Shelburn, Cheng
More informationCold Flow Simulation Inside an SI Engine
Tutorial 12. Cold Flow Simulation Inside an SI Engine Introduction The purpose of this tutorial is to illustrate the case setup and solution of the two dimensional, four stroke spark ignition (SI) engine
More informationClick to edit Master title style
Click to edit Master title style LES LES Applications for for Internal Internal Combustion Engines Engines David Gosman & Richard Johns CD-adapco, June 2011 Some Qs and As Why would we use LES calculations
More informationDeveloping LES Models for IC Engine Simulations. June 14-15, 2017 Madison, WI
Developing LES Models for IC Engine Simulations June 14-15, 2017 Madison, WI 1 2 RANS vs LES Both approaches use the same equation: u i u i u j 1 P 1 u i t x x x x j i j T j The only difference is turbulent
More informationCalculate a solution using the pressure-based coupled solver.
Tutorial 19. Modeling Cavitation Introduction This tutorial examines the pressure-driven cavitating flow of water through a sharpedged orifice. This is a typical configuration in fuel injectors, and brings
More informationICE Roadmap Japanese STAR Conference. Richard Johns
ICE Roadmap Japanese STAR Conference Richard Johns Introduction Top-Level Roadmap STAR-CCM+ and Internal Combustion Engines Modeling Improvements and Research Support Sprays LES Chemistry Meshing Summary
More informationAdjoint Solver Workshop
Adjoint Solver Workshop Why is an Adjoint Solver useful? Design and manufacture for better performance: e.g. airfoil, combustor, rotor blade, ducts, body shape, etc. by optimising a certain characteristic
More informationFluent User Services Center
Solver Settings 5-1 Using the Solver Setting Solver Parameters Convergence Definition Monitoring Stability Accelerating Convergence Accuracy Grid Independence Adaption Appendix: Background Finite Volume
More informationImpact of STAR-CCM+ v7.0 in the Automotive Industry Frederick J. Ross, CD-adapco Director, Ground Transportation
Impact of STAR-CCM+ v7.0 in the Automotive Industry Frederick J. Ross, CD-adapco Director, Ground Transportation Vehicle Simulation Components Vehicle Aerodynamics Design Studies Aeroacoustics Water/Dirt
More informationNumerical Spray Calibration Process. ANSYS Inc. Pune, India. Laz Foley. ANSYS Inc. Evanston, IL
ILASS Americas, 23 rd Annual Conference on Liquid Atomization and Spray Systems, Ventura, CA, May 2011 Numerical Spray Calibration Process Padmesh Mandloi *,Jayesh Mutyal, Pravin Rajeshirke ANSYS Inc.
More informationPreliminary Spray Cooling Simulations Using a Full-Cone Water Spray
39th Dayton-Cincinnati Aerospace Sciences Symposium Preliminary Spray Cooling Simulations Using a Full-Cone Water Spray Murat Dinc Prof. Donald D. Gray (advisor), Prof. John M. Kuhlman, Nicholas L. Hillen,
More informationStreamlining Aircraft Icing Simulations. D. Snyder, M. Elmore
Streamlining Aircraft Icing Simulations D. Snyder, M. Elmore Industry Analysis Needs / Trends Fidelity Aircraft Ice Protection Systems-Level Modeling Optimization Background Ice accretion can critically
More informationModeling of a DaimlerChrysler Truck Engine using an Eulerian Spray Model
Modeling of a DaimlerChrysler Truck Engine using an Eulerian Spray Model C. Hasse, S. Vogel, N. Peters Institut für Technische Mechanik RWTH Aachen Templergraben 64 52056 Aachen Germany c.hasse@itm.rwth-aachen.de
More informationExpress Introductory Training in ANSYS Fluent Workshop 02 Using the Discrete Phase Model (DPM)
Express Introductory Training in ANSYS Fluent Workshop 02 Using the Discrete Phase Model (DPM) Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 - Industry
More informationInvestigation of mixing chamber for experimental FGD reactor
Investigation of mixing chamber for experimental FGD reactor Jan Novosád 1,a, Petra Danová 1 and Tomáš Vít 1 1 Department of Power Engineering Equipment, Faculty of Mechanical Engineering, Technical University
More informationreal world design & problems fluid flow engineering solving Computational Fluid Dynamics System
C F D 2 0 0 0 Computational Fluid Dynamics System solving real world engineering design & problems aerospace architecture automotive biomedical chemical processing electrical cooling environmental marine
More informationONE DIMENSIONAL (1D) SIMULATION TOOL: GT-POWER
CHAPTER 4 ONE DIMENSIONAL (1D) SIMULATION TOOL: GT-POWER 4.1 INTRODUCTION Combustion analysis and optimization of any reciprocating internal combustion engines is too complex and intricate activity. It
More informationIntroduction to Computational Fluid Dynamics Mech 122 D. Fabris, K. Lynch, D. Rich
Introduction to Computational Fluid Dynamics Mech 122 D. Fabris, K. Lynch, D. Rich 1 Computational Fluid dynamics Computational fluid dynamics (CFD) is the analysis of systems involving fluid flow, heat
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 informationHIGH PERFORMANCE COMPUTATION (HPC) FOR THE
HIGH PERFORMANCE COMPUTATION (HPC) FOR THE DEVELOPMENT OF FLUIDIZED BED TECHNOLOGIES FOR BIOMASS GASIFICATION AND CO2 CAPTURE P. Fede, H. Neau, O. Simonin Université de Toulouse; INPT, UPS ; IMFT ; 31400
More informationEstimation of Flow Field & Drag for Aerofoil Wing
Estimation of Flow Field & Drag for Aerofoil Wing Mahantesh. HM 1, Prof. Anand. SN 2 P.G. Student, Dept. of Mechanical Engineering, East Point College of Engineering, Bangalore, Karnataka, India 1 Associate
More informationPDF-based simulations of turbulent spray combustion in a constant-volume chamber under diesel-engine-like conditions
International Multidimensional Engine Modeling User s Group Meeting at the SAE Congress Detroit, MI 23 April 2012 PDF-based simulations of turbulent spray combustion in a constant-volume chamber under
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 informationSimulation of In-Cylinder Flow Phenomena with ANSYS Piston Grid An Improved Meshing and Simulation Approach
Simulation of In-Cylinder Flow Phenomena with ANSYS Piston Grid An Improved Meshing and Simulation Approach Dipl.-Ing. (FH) Günther Lang, CFDnetwork Engineering Dipl.-Ing. Burkhard Lewerich, CFDnetwork
More informationAdvanced Applications of STAR- CCM+ in Chemical Process Industry Ravindra Aglave Director, Chemical Process Industry
Advanced Applications of STAR- CCM+ in Chemical Process Industry Ravindra Aglave Director, Chemical Process Industry Outline Notable features released in 2013 Gas Liquid Flows with STAR-CCM+ Packed Bed
More informationCompressible Flow in a Nozzle
SPC 407 Supersonic & Hypersonic Fluid Dynamics Ansys Fluent Tutorial 1 Compressible Flow in a Nozzle Ahmed M Nagib Elmekawy, PhD, P.E. Problem Specification Consider air flowing at high-speed through a
More informationCFD in COMSOL Multiphysics
CFD in COMSOL Multiphysics Christian Wollblad Copyright 2017 COMSOL. Any of the images, text, and equations here may be copied and modified for your own internal use. All trademarks are the property of
More informationModeling Flow Through Porous Media
Tutorial 7. Modeling Flow Through Porous Media Introduction Many industrial applications involve the modeling of flow through porous media, such as filters, catalyst beds, and packing. This tutorial illustrates
More informationCFD Best Practice Guidelines: A process to understand CFD results and establish Simulation versus Reality
CFD Best Practice Guidelines: A process to understand CFD results and establish Simulation versus Reality Judd Kaiser ANSYS Inc. judd.kaiser@ansys.com 2005 ANSYS, Inc. 1 ANSYS, Inc. Proprietary Overview
More information1. TopMath-Workshop Iffeldorf/Osterseen. Liquid Sprays. Ayoub Hmaidi Zentrum Mathematik, TU MÜNCHEN
1. TopMath-Workshop Iffeldorf/Osterseen Liquid Sprays Ayoub Hmaidi Zentrum Mathematik, TU MÜNCHEN What are Liquid Sprays? Why are Sprays important? Sprays occur in a large number of applications: Engines
More informationDevelopment of a CFD methodology for fuel-air mixing and combustion modeling of GDI Engines
Development of a CFD methodology for fuel-air mixing and combustion modeling of GDI Engines T. Lucchini, G. D Errico, L. Cornolti, G. Montenegro, A. Onorati Politecnico di Milano, Dipartimento di Energia,
More informationTutorial: Hydrodynamics of Bubble Column Reactors
Tutorial: Introduction The purpose of this tutorial is to provide guidelines and recommendations for solving a gas-liquid bubble column problem using the multiphase mixture model, including advice on solver
More informationShape Optimization for Aerodynamic Efficiency Using Adjoint Methods
White Paper Shape Optimization for Aerodynamic Efficiency Using Adjoint Methods Adjoint solvers take a Computational Fluid Dynamics (CFD) flow solution and calculate the sensitivity of performance indicators
More informationTransition Flow and Aeroacoustic Analysis of NACA0018 Satish Kumar B, Fred Mendonç a, Ghuiyeon Kim, Hogeon Kim
Transition Flow and Aeroacoustic Analysis of NACA0018 Satish Kumar B, Fred Mendonç a, Ghuiyeon Kim, Hogeon Kim Transition Flow and Aeroacoustic Analysis of NACA0018 Satish Kumar B, Fred Mendonç a, Ghuiyeon
More 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 informationSpeed and Accuracy of CFD: Achieving Both Successfully ANSYS UK S.A.Silvester
Speed and Accuracy of CFD: Achieving Both Successfully ANSYS UK S.A.Silvester 2010 ANSYS, Inc. All rights reserved. 1 ANSYS, Inc. Proprietary Content ANSYS CFD Introduction ANSYS, the company Simulation
More informationTutorial: Modeling Liquid Reactions in CIJR Using the Eulerian PDF transport (DQMOM-IEM) Model
Tutorial: Modeling Liquid Reactions in CIJR Using the Eulerian PDF transport (DQMOM-IEM) Model Introduction The purpose of this tutorial is to demonstrate setup and solution procedure of liquid chemical
More informationSTUDY OF FLOW PERFORMANCE OF A GLOBE VALVE AND DESIGN OPTIMISATION
Journal of Engineering Science and Technology Vol. 12, No. 9 (2017) 2403-2409 School of Engineering, Taylor s University STUDY OF FLOW PERFORMANCE OF A GLOBE VALVE AND DESIGN OPTIMISATION SREEKALA S. K.
More informationExample Simulations in OpenFOAM
Example Simulations in OpenFOAM Hrvoje Jasak h.jasak@wikki.co.uk Wikki Ltd, United Kingdom FSB, University of Zagreb, Croatia 18/Nov/2005 Example Simulations in OpenFOAM p.1/26 Outline Objective Present
More informationLab 9: FLUENT: Transient Natural Convection Between Concentric Cylinders
Lab 9: FLUENT: Transient Natural Convection Between Concentric Cylinders Objective: The objective of this laboratory is to introduce how to use FLUENT to solve both transient and natural convection problems.
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 informationFlow and Heat Transfer in a Mixing Elbow
Flow and Heat Transfer in a Mixing Elbow Objectives The main objectives of the project are to learn (i) how to set up and perform flow simulations with heat transfer and mixing, (ii) post-processing and
More informationCFD VALIDATION FOR SURFACE COMBATANT 5415 STRAIGHT AHEAD AND STATIC DRIFT 20 DEGREE CONDITIONS USING STAR CCM+
CFD VALIDATION FOR SURFACE COMBATANT 5415 STRAIGHT AHEAD AND STATIC DRIFT 20 DEGREE CONDITIONS USING STAR CCM+ by G. J. Grigoropoulos and I..S. Kefallinou 1. Introduction and setup 1. 1 Introduction The
More informationHigh-Lift Aerodynamics: STAR-CCM+ Applied to AIAA HiLiftWS1 D. Snyder
High-Lift Aerodynamics: STAR-CCM+ Applied to AIAA HiLiftWS1 D. Snyder Aerospace Application Areas Aerodynamics Subsonic through Hypersonic Aeroacoustics Store release & weapons bay analysis High lift devices
More informationTurbulent Premixed Combustion with Flamelet Generated Manifolds in COMSOL Multiphysics
Turbulent Premixed Combustion with Flamelet Generated Manifolds in COMSOL Multiphysics Rob J.M Bastiaans* Eindhoven University of Technology *Corresponding author: PO box 512, 5600 MB, Eindhoven, r.j.m.bastiaans@tue.nl
More informationVehicle Cabin Noise from Turbulence Induced by Side-View Mirrors. Hua-Dong Yao, 2018/8/29 Chalmers University of Technology, Sweden
Vehicle Cabin Noise from Turbulence Induced by Side-View Mirrors Hua-Dong Yao, 2018/8/29 Chalmers University of Technology, Sweden An Important Cabin Noise Source Turbulence As the development of quiet
More informationComputational Study of Laminar Flowfield around a Square Cylinder using Ansys Fluent
MEGR 7090-003, Computational Fluid Dynamics :1 7 Spring 2015 Computational Study of Laminar Flowfield around a Square Cylinder using Ansys Fluent Rahul R Upadhyay Master of Science, Dept of Mechanical
More informationComputational Fluid Dynamics (CFD) Simulation in Air Duct Channels Using STAR CCM+
Available onlinewww.ejaet.com European Journal of Advances in Engineering and Technology, 2017,4 (3): 216-220 Research Article ISSN: 2394-658X Computational Fluid Dynamics (CFD) Simulation in Air Duct
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 informationContents Contents Contents... 1 Abstract... 3 Nomenclature... 4 Index of Figures... 6 Index of Tables... 8 Introduction... 9 Theory...
Contents Contents Contents... 1 Abstract... 3 Nomenclature... 4 Index of Figures... 6 Index of Tables... 8 1. Introduction... 9 1.1 Overview... 9 1.2 Task... 10 2. Theory... 11 2.1 Continuity and Momentum
More informationOn the numerical accuracy of particle dispersion simulation in operating theatres
On the numerical accuracy of particle dispersion simulation in operating theatres Wiebe Zoon 1,*, Marcel Loomans 1 and Jan Hensen 1 1 Eindhoven University of Technology, Eindhoven, the Netherlands * Corresponding
More informationNumerical Simulation of Fuel Filling with Volume of Fluid
Numerical Simulation of Fuel Filling with Volume of Fluid Master of Science Thesis [Innovative and Sustainable Chemical Engineering] Kristoffer Johansson Department of Chemistry and Bioscience Division
More informationCFD Project Workflow Guide
CFD Project Workflow Guide Contents Select a problem with known results for proof-of-concept testing... 1 Set up and run a coarse test case... 2 Select and calibrate numerical methods... 3 Minimize & quantify
More informationProgram: Advanced Certificate Program
Program: Advanced Certificate Program Course: CFD-Vehicle Aerodynamics Directorate of Training and Lifelong Learning #470-P, Peenya Industrial Area, 4th Phase Peenya, Bengaluru 560 058 www.msruas.ac.in
More 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 informationA 3D VOF model in cylindrical coordinates
A 3D VOF model in cylindrical coordinates Marmar Mehrabadi and Markus Bussmann Department of Mechanical and Industrial Engineering, University of Toronto Recently, volume of fluid (VOF) methods have improved
More informationSolver Settings. Introductory FLUENT Training ANSYS, Inc. All rights reserved. ANSYS, Inc. Proprietary
Solver Settings Introductory FLUENT Training 2006 ANSYS, Inc. All rights reserved. 2006 ANSYS, Inc. All rights reserved. 5-2 Outline Using the Solver Setting Solver Parameters Convergence Definition Monitoring
More informationNumerical and theoretical analysis of shock waves interaction and reflection
Fluid Structure Interaction and Moving Boundary Problems IV 299 Numerical and theoretical analysis of shock waves interaction and reflection K. Alhussan Space Research Institute, King Abdulaziz City for
More informationFinal drive lubrication modeling
Final drive lubrication modeling E. Avdeev a,b 1, V. Ovchinnikov b a Samara University, b Laduga Automotive Engineering Abstract. In this paper we describe the method, which is the composition of finite
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 informationLES/FMDF of Spray Combustion in Internal Combustion Engines
LES/FMDF of Spray Combustion in Internal Combustion Engines Araz Banaeizadeh *, Harold Schock, and Farhad Jaberi Department of Mechanical Engineering Michigan State University, East Lansing, MI, 48824-1226
More informationUsing the Eulerian Multiphase Model for Granular Flow
Tutorial 21. Using the Eulerian Multiphase Model for Granular Flow Introduction Mixing tanks are used to maintain solid particles or droplets of heavy fluids in suspension. Mixing may be required to enhance
More informationCoupling of STAR-CCM+ to Other Theoretical or Numerical Solutions. Milovan Perić
Coupling of STAR-CCM+ to Other Theoretical or Numerical Solutions Milovan Perić Contents The need to couple STAR-CCM+ with other theoretical or numerical solutions Coupling approaches: surface and volume
More 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 informationNovember c Fluent Inc. November 8,
MIXSIM 2.1 Tutorial November 2006 c Fluent Inc. November 8, 2006 1 Copyright c 2006 by Fluent Inc. All Rights Reserved. No part of this document may be reproduced or otherwise used in any form without
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 informationExpress Introductory Training in ANSYS Fluent Workshop 04 Fluid Flow Around the NACA0012 Airfoil
Express Introductory Training in ANSYS Fluent Workshop 04 Fluid Flow Around the NACA0012 Airfoil Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 -
More informationRecent & Upcoming Features in STAR-CCM+ for Aerospace Applications Deryl Snyder, Ph.D.
Recent & Upcoming Features in STAR-CCM+ for Aerospace Applications Deryl Snyder, Ph.D. Outline Introduction Aerospace Applications Summary New Capabilities for Aerospace Continuity Convergence Accelerator
More informationCoupled Analysis of FSI
Coupled Analysis of FSI Qin Yin Fan Oct. 11, 2008 Important Key Words Fluid Structure Interface = FSI Computational Fluid Dynamics = CFD Pressure Displacement Analysis = PDA Thermal Stress Analysis = TSA
More informationCoupled Simulation of the Fluid Flow and Conjugate Heat Transfer in Press Hardening Processes
13 th International LS-DYNA Users Conference Session: Metal Forming Coupled Simulation of the Fluid Flow and Conjugate Heat Transfer in Press Hardening Processes Uli Göhner 1), Bruno Boll 1), Inaki Caldichouri
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 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 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 informationDesign Modification and Analysis of Two Wheeler Engine Cooling Fins by CFD
Design Modification and Analysis of Two Wheeler Engine Cooling Fins by CFD Mohsin A. Ali and Prof. (Dr.) S.M Kherde Abstract An air-cooled motorcycle engine releases heat to the atmosphere through the
More informationAuto Injector Syringe. A Fluent Dynamic Mesh 1DOF Tutorial
Auto Injector Syringe A Fluent Dynamic Mesh 1DOF Tutorial 1 2015 ANSYS, Inc. June 26, 2015 Prerequisites This tutorial is written with the assumption that You have attended the Introduction to ANSYS Fluent
More informationCIBSE Application Manual AM11 Building Performance Modelling Chapter 6: Ventilation Modelling
Contents Background Ventilation modelling tool categories Simple tools and estimation techniques Analytical methods Zonal network methods Computational Fluid Dynamics (CFD) Semi-external spaces Summary
More informationProgress on Engine LES Using STAR-CD
www.cd-adapco.com Progress on Engine LES Using STAR-CD A D Gosman CD-adapco Japan STAR Conference 2012, Yokohama INTRODUCTION 1. Nature and motivation for LES of engines 2. LES modelling in STAR-CD 3.
More informationON THE NUMERICAL MODELING OF IMPINGING JET HEAT TRANSFER
ON THE NUMERICAL MODELING OF IMPINGING JET HEAT TRANSFER Mirko Bovo 1,2, Sassan Etemad 2 and Lars Davidson 1 1 Dept. of Applied Mechanics, Chalmers University of Technology, Gothenburg, Sweden 2 Powertrain
More informationURANS and SAS analysis of flow dynamics in a GDI nozzle
, 3rd Annual Conference on Liquid Atomization and Spray Systems, Brno, Czech Republic, September 010 J.-M. Shi*, K. Wenzlawski*, J. Helie, H. Nuglisch, J. Cousin * Continental Automotive GmbH Siemensstr.
More informationSIMULATION OF PROPELLER-SHIP HULL INTERACTION USING AN INTEGRATED VLM/RANSE SOLVER MODELING.
SIMULATION OF PROPELLER-SHIP HULL INTERACTION USING AN INTEGRATED VLM/RANSE SOLVER MODELING. M.N.Senthil Prakash, Department of Ocean Engineering, IIT Madras, India V. Anantha Subramanian Department of
More informationSmoothing the Path to Simulation-Led Device Design
Smoothing the Path to Simulation-Led Device Design Beverly E. Pryor 1, and Roger W. Pryor, Ph.D. *,2 1 Pryor Knowledge Systems, Inc. 2 Pryor Knowledge Systems, Inc. *Corresponding author: 4918 Malibu Drive,
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 informationMultiphase Interactions: Which, When, Why, How? Ravindra Aglave, Ph.D Director, Chemical Process Industry
Multiphase Interactions: Which, When, Why, How? Ravindra Aglave, Ph.D Director, Chemical Process Industry Outline Classification of Multiphase Flows Examples: Free Surface Flow using Volume of Fluid Examples:
More informationExperimental and Numerical Study of Fire Suppression Performance of Ultral-Fine Water Mist in a Confined Space
Available online at www.sciencedirect.com Procedia Engineering 52 ( 2013 ) 208 213 Experimental and Numerical Study of Fire Suppression Performance of Ultral-Fine Water Mist in a Confined Space LIANG Tian-shui
More informationMicrowell Mixing with Surface Tension
Microwell Mixing with Surface Tension Nick Cox Supervised by Professor Bruce Finlayson University of Washington Department of Chemical Engineering June 6, 2007 Abstract For many applications in the pharmaceutical
More informationOptimizing Bio-Inspired Flow Channel Design on Bipolar Plates of PEM Fuel Cells
Excerpt from the Proceedings of the COMSOL Conference 2010 Boston Optimizing Bio-Inspired Flow Channel Design on Bipolar Plates of PEM Fuel Cells James A. Peitzmeier *1, Steven Kapturowski 2 and Xia Wang
More informationUSAGE OF ANSA S AUTOMATED VOLUME MESHING-METHODS IN THE RAPID PRODUCT DEVELOPMENT PROCESS OF DIESEL ENGINES
USAGE OF ANSA S AUTOMATED VOLUME MESHING-METHODS IN THE RAPID PRODUCT DEVELOPMENT PROCESS OF DIESEL ENGINES Günther Pessl *, Dr. Robert Ehart, Gerwin Bumberger BMW Motoren GmbH, Austria KEYWORDS - ANSA,
More informationA COUPLED FINITE VOLUME SOLVER FOR THE SOLUTION OF LAMINAR TURBULENT INCOMPRESSIBLE AND COMPRESSIBLE FLOWS
A COUPLED FINITE VOLUME SOLVER FOR THE SOLUTION OF LAMINAR TURBULENT INCOMPRESSIBLE AND COMPRESSIBLE FLOWS L. Mangani Maschinentechnik CC Fluidmechanik und Hydromaschinen Hochschule Luzern Technik& Architektur
More informationA steady-state Eulerian-Lagrangian solver for non-reactive sprays
ICLASS 212, 12 th Triennial International Conference on Liquid Atomization and Spray Systems, Heidelberg, Germany, September 2-6, 212 A steady-state Eulerian-Lagrangian solver for non-reactive sprays A.
More informationCOMPUTATIONAL FLUID DYNAMICS ANALYSIS OF ORIFICE PLATE METERING SITUATIONS UNDER ABNORMAL CONFIGURATIONS
COMPUTATIONAL FLUID DYNAMICS ANALYSIS OF ORIFICE PLATE METERING SITUATIONS UNDER ABNORMAL CONFIGURATIONS Dr W. Malalasekera Version 3.0 August 2013 1 COMPUTATIONAL FLUID DYNAMICS ANALYSIS OF ORIFICE PLATE
More information