Validation of an Automatic Mesh Generation Technique in Engine Simulations
|
|
- Madlyn McCarthy
- 5 years ago
- Views:
Transcription
1 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 Wang, Devin Hodgson, Ellen Meeks Reaction Design FORTÉ CFD software is designed for multidimensional reactive flow simulations, especially for engine applications. Such applications intrinsically contain moving boundaries and often contain complex geometries, such as poppet valves. This makes mesh generation a challenging task. The latest FORTÉ software features automatic mesh generation that is based on an immersed boundary method. With this technique, computational meshes are generated on the fly based on the instantaneous shape of the computational domain. Dynamic mesh refinement can be used to create higher mesh resolution at system boundaries or in regions of interest at certain periods during the simulation. The flow and physical-model equations are solved using a perfectly orthogonal Cartesian grid in the interior of the computational domain. Special algorithms have been developed to handle the solution in immersed-boundary cells at open boundaries, as well as static or moving wall boundaries. This paper presents the validation of this automatic meshing technique in both diesel engine and spark ignition engine simulations.. Introduction The numerical method used for solving the basic fluid dynamics equations in FORTÉ is similar to that used by KIVA-V []. Specifically, the state variables and velocities are discretized using a staggered scheme; the solution procedure follows the ALE (Arbitrary Lagrangian Eulerian) method; the solution of the pressure-linked equations is patterned after the SIMPLE method; and the convection terms are solved using a quasi-second-order upwind differencing method. The need to generate a body-fitted, block-structured mesh has been a major limitation of the KIVA-V code when applied to complex engine geometries. Not only is the initial mesh creation time-consuming and expertise-intensive, but determining a robust meshmoving control algorithm often requires tedious trial-and-error iterations. In addition, highly distorted cells can introduce inaccuracy and convergence issues into the numerical solution. In FORTÉ, we have developed an automatic mesh generation technique that is based on immersed boundary method and is compatible with the staggered discretization scheme. The automatic meshing technique in FORTÉ starts with a CAD-generated geometry file (such as a file in STL format), which defines the physical boundary surfaces of the computational domain. This imported geometry serves as the starting surface mesh, which can be transformed using several basic geometrymanipulation functions. From this surface mesh, a Cartesian computational mesh is created to cover the physical domain, based on user-specified cell size constraints. Different cell sizes can be specified at different boundary surfaces to provide appropriate resolution for local geometry structures. Subsequently, the Cartesian cells whose centers lie outside of the physical boundary will be eliminated from the Cartesian mesh. The resulting mesh serves as the background framework of the flow solution. In cases that have moving boundaries, the surface mesh (which represents the physical boundary of the domain) is adjusted according to the moving surface velocities for each timestep. Correspondingly, cells are activated or deactivated in the Cartesian mesh depending on how the Cartesian mesh intersects the physical boundary. The general methodology and preliminary results of using this automatic meshing technique have been reported previously []. In this work we discuss several important technical aspects and verification results. The technical topics to be described include ) formulation of the boundary control volume for maintaining mass and energy conservation; ) application of forcing term at moving wall boundaries; and ) mesh refinement capability. These improvements will then be demonstrated by several unit tests and engine simulations.
2 . Methodology The approaches to handling immersed boundary cells of a Cartesian grid can be largely classified into two groups in the literature: cut-cell approach and ghost-cell approach [-6]. In a cut-cell approach, the Cartesian boundary cells are reshaped to fit the local geometry, and the flow solution numerical algorithms are modified to handle the irregular shaped cut cell faces and volumes. The cut-cell approach tries to reconstruct the physical computational domain for each timestep and thus it tracks the mass and energy contained in the physical domain accurately. However, implementation of an exact cut-cell approach for D problems is complicated and the cell reshaping may result in tiny cells. It also imposes stringent requirement for the quality of the STL surface mesh. In a ghost-cell approach, the boundary cells keep their hexahedron shape. The variables at the ghost cell centers or ghost vertices are defined through interpolation. Thus the flow equations are solved on the Cartesian grid directly. In this approach, the variable interpolation must be precise enough to maintain strict mass and energy conservation inside the system boundary. The immersed boundary method used in FORTÉ combines features of both ghost-cell and cut-cell approaches. Specifically, the momentum equation is solved on the Cartesian grid directly. Since the momentum equation involves only intensive variables (such as pressure, gas density, specific energy) instead of extensive variables (mass and total energy) and there is no mass crossing cell or system boundaries during this step, it is not critical to track the location of the system boundary precisely and solve the equation on reshaped cut cells. However, when solving terms that involve mass or energy transfer across the system boundary, the cut-cell approach is employed. Next, we briefly discuss a few technical topics involved in this hybrid approach used in FORTÉ.. Formulation of boundary control volumes In FORTÉ, the Cartesian cells whose cell centers lie inside the system boundary are defined as fluid cells, and the fluid cell domain is wrapped by a layer of ghost cells. When the flow solution involves mass or energy transfer across the system boundaries or cell boundaries, a cut-cell boundary control volume is formulated and tracked for each boundary cell. This is done by splitting the physical volume contained in ghost cells into their neighboring fluid cells. In this way, the total volume of the system can be recovered by the cut-cell control volumes of all the boundary cells plus the volumes of the interior fluid cells. In the example shown in Fig., the cut-cell control g Interior Fluid 4 g Figure. Cut-cell boundary control volumes volumes for fluid cells -6 correspond to the respective volumes encompassed by the red segments. The physical volume contained in ghost cell g is shared by the control volumes of cells and. Similarly, the physical boundary area contained in the ghost cells are also shared by their neighboring fluid cells. Using the wall heat transfer calculation as an example, the heat transfer amount across each cut-cell control volume is calculated as the local heat flux times the physical wall area contained in the control volume. Then this delta of energy is added to the total energy contained in the control volume (instead of the Cartesian boundary cell). This in turn changes the specific internal energy of the gas inside this control volume. The calculation of mass and energy exchange between a vaporizing spray particle and the gas in a boundary cell is another example.. Forcing term at moving wall boundary At moving wall boundaries, the transport equations are solved using the ALE procedure. During the Lagrangian stage, the fluid cells float with the fluid and consequently change their location, shape and volume. The moving wall cell faces of the Cartesian grid also move to a new location according to the moving velocity of the wall boundary. The motion of the moving walls imposes a pushing or pulling force on the interior fluid. In the method used by FORTÉ, the Cartesian boundary cells at moving wall boundary will resume their hexahedral shape after each time step, meaning that the wall boundary will always impose the force at the Cartesian wall boundary. The purpose for doing this is to avoid changing the boundary cell volumes continuously and thus greatly simplify the numerical algorithm of the ALE procedure. However, since the pushing or pulling force is not applied at the exact system boundary location, the force (and consequently the moving velocity) of the Cartesian moving cell faces must be adjusted continuously in order 5 6
3 for the interior fluid to feel the precise compression or expansion effect due to wall motion. This moving velocity correction will be demonstrated using a unit compression-expansion test case below.. Mesh refinement The Cartesian mesh in FORTÉ follows an octree structure, in which all cells are perfect cubes. When a cell is refined, it will be split into eight smaller cubes evenly. Engine geometries inevitably contain small structures, such as the crevice between valve seats and the cylinder head. Such small fluid passages have to be resolved using very small cells, and it is impractical to use such small cells throughout the computational domain. This makes mesh refinement a necessary capability. In FORTÉ, mesh refinement can be applied on boundary surfaces or in specified regions. Different cell sizes can be specified for different refinement controls, and the refinement can be applied dynamically for certain time or crank angle intervals. As mentioned earlier, FORTÉ uses the staggered discretization scheme in which velocities are defined at vertices. To handle a refined mesh, the momentum control volumes of "hanging" nodes have been properly formulated to avoid "checker-board" patterns of velocity and pressure, which are often seen in CFD applications. In solving the momentum equation, pressure gradient are applied at the corners of each momentum control volume. Thus, pressures need to be interpolated at certain locations inside a bigger cell. Solving the momentum equation on a staggered and refined mesh is more complicated than doing so on a collocated mesh (in which both state variables and velocities are defined at cell centers), but the use of a staggered scheme can avoid the "checker-board" pattern without resorting to any numerical damping (called node coupling) method. The refinement capability will be demonstrated using a flow-through-pipe test case.. Validation Using Unit Tests. Heat transfer in a compression-expansion test The compression and expansion of gas mixture inside the cylinder is a fundamental process in engine operations. In a previous paper [], we demonstrated the effectiveness of formulating cut-cell boundary control volumes by simulating a wall heat transfer problem for a constant volume vessel. In the present work, wall heat transfer is tested in a compression-expansion environment. This test can help validate the technical treatment discussed in sections. and.. The geometry used is a simple cylinder (bore diameter = 6 cm, stroke = 7.5 cm, squish height =.5 cm), which gives a compression ratio (CR) 6:. The calculation is carried out from -5 ATDC to 5 ATDC at 5 RPM. The initial temperature and pressure are 4 K and bar, respectively, and the wall temperature is K. The initial swirl ratio is.5. The results using immersed boundary are benchmarked against results generated using a KIVAV compatible body-fitted mesh. The average grid size of the body-fitted case is cm; the global grid size of the immersed boundary mesh is cm, and the wall boundaries are refined using / size cells. In Fig., the histories of in-cylinder averaged pressures and heat transfer rates are compared between the immersed boundary case and body-fitted case. Very good agreements have been obtained for both parameters. Figure shows the temperature contours on a horizontal cut plane (z=7.5 cm) at - ATDC during the compression. The contours show very similar pattern of temperature stratification. It is worth noting that the immersed boundary method does a better job because the temperature distribution is more axisymmetric. By contrast, the body-fitted case shows some non-axisymmetric pattern due to cell-size variation along the boundary Body-fitted Auto Mesh Wall Heat Transfer Rate (J/deg).6.4. Body-fitted Auto Mesh (a) In-cylinder pressures (b) Wall heat transfer rates Figure Pressure and wall heat transfer rate curves of body-fitted and auto mesh calculations
4 (a) Auto Mesh (b) Body-fitted Figure Computed temperature contours on a horizontal cut plane at z = 7.5 cm and - ATDC. Mesh refinement tests A simple flow-through-square-pipe problem was used to test the accuracy of mesh refinement treatment. The width, height, and length of the square pipe are 5cm 5cm cm, respectively. The geometry is tilted by a 45 angle relative to the horizontal location. The lower left face is the inlet and the upper right face is the outlet. A fixed-velocity inlet boundary condition and an outflow outlet boundary condition are specified. The inlet velocity is m/s and its direction is normal to the inlet face. Freely slipping and adiabatic wall boundary conditions are specified at the pipe walls. In this test, we should expect to see uniform velocities at any cross-sectional plane of the pipe. Two refinement arrangements are tested, both using global grid size =.5 cm. In the first test, a spherical region at the center of the pipe is refined by two levels. In the second test, all the boundaries are refined using / size cells. Figures 4 and 5 show that uniform and smooth velocity patterns could be preserved using both refinement arrangements. This demonstrates the effectiveness of the refinement treatment. (a) t = ms (b) t =.5 ms (c) t = 4 ms Figure 4 Computed velocity contours on a vertical cut plane using interior refinement (a) t = ms (b) t =.5 ms (c) t = 4 ms Figure 5 Computed velocity contours on a vertical cut plane using boundary refinement 4
5 4. Validation in Engine s 4. Diesel engine In a validation test that simulated a diesel engine, only the in-cylinder spray and combustion processes were simulated. The engine modeled is a single-cylinder direct injection optical engine operating at low temperature combustion conditions (CR=6:; bore stroke = ; injection timing = -.5 ATDC) [7]. The simulation is carried out from IVC (-65 ATDC) to EVO (5 ATDC). The global grid size is mm, and the cells along the wall boundaries are refined by / size. The spray breakup models employ gas-jet theory to achieve results that are independent of grid resolution [8-9]. A 5-species n-heptane mechanism is used for chemistry. Using the default values for all model constants, the simulated pressure matches the measured pressure very well, as shown in Fig. 6. Figure 7 shows the simulated spray structures and temperature contours on two cut-planes at selected crank angle locations through the spray and ignition processes Apparent Heat Release Rate (J/deg) Figure 6 In-cylinder pressures and heat release rates of the diesel engine case (a) -7 ATDC (b) - ATDC (c) - 5 ATDC Figure 7 Computed spray structures and temperature contours on cut planes 4. Spark ignition engine A four-valve Ford engine operating in PFI (port fuel injection) mode is simulated to validate the flow and spark ignition and combustion models in the immersed boundary framework. These calculations include the whole engine cycle starting from EVO (6 ATDC). Specifications of the engine and operating conditions include: CR=:; bore stroke = 8.9 cm 7.95 cm; RPM = 5; manifold pressure =.65 bar []. Conditions with a spark timing sweep are modeled. The global grid size of the immersed boundary meshes is set to mm. Dynamic refinement controls are applied at boundary surfaces. For example, cells at the valve surfaces are refined to /4 size when the valves are lifted. The DPIK (discrete particle ignition kernel) model is used to track the flame location of the ignition kernel and the G-equation model is used to simulate the subsequent flame propagation []. Figure 8 shows computed temperature contours on a vertical cut plane across one pair of valves during the exhaust and intake strokes. The four crank angle locations correspond to exhaust valve opening, valve overlap, intake valve opening, and intake valve closing, respectively. Figure 9 shows the temperature contours on a vertical cut plane across the spark plug during ignition and flame propagation. The ignition kernel flame particles are shown on the Fig. 9(a). It can be seen in Fig. 9(c) that /4 level refinement is used at the boundaries in order to resolve the narrow squish region. 5
6 (a) CA = ATDC (b) CA = 4 ATDC (c) CA = 5 ATDC (d) CA = 6 ATDC Figure 8 Computed temperature contours on a vertical cut plane (a) CA = 69 ATDC (b) CA = 7 ATDC (c) CA = 75 ATDC (d) CA = 76 ATDC Figure 9 Temperature contours during spark ignition and flame propagation (spark timing = 68 ATDC) Simulated in-cylinder pressures are compared to the measured data [] in Fig.. The agreement is very good during the exhaust, intake and early compression strokes. Reasonable agreements are also obtained for the ignition and combustion stages and expansion strokes. The trend of peak pressure as function of spark timing is well captured. The normalized NOx emissions are compared between simulation and experiment in Fig.. Again, the trend of NOx as function of spark timing is very well reproduced in the simulation. 6
7 .5 Spark Timing = 676 ATDC.5 Spark Timing = 68 ATDC Spark Timing = 684 ATDC.5 Spark Timing = 688 ATDC NOx (ppm) normalized to Maximum Figure Computed and measured in-cylinder pressures Spark Timing (CA ATDC) (Normalized) Model (Normalized) Figure Computed and measured NOx emissions at EVO Summary An automatic mesh generation technique based on immersed-boundary theory is described. Several key technical aspects of the implementation are discussed. The technique is validated using a few unit tests and both diesel and spark ignition engine simulations. The validation shows that the immersed-boundary method is an effective technique for achieving accuracy in engine CFD simulations without the burden of manual mesh generation. References. A.A. Amsden, et al. (989) KIVA-II manual, LA-56-MS.. L. Liang, et al. () st International Multidimensional Engine Modeling User's Group Meeting.. R. Mittal, et al. (5) Annu. Rev. Fluid Mech., 7: T. Ye, et al. (999) J. Comp. Phys., 56: Y.-H. Tseng, et al. () J. Comp. Phys., 9: J. Yang, et al. (6) J. Comp. Phys., 5: M.P.B. Musculus, (4) SAE N. Abani et al. (8) SAE Y. Wang et al. () SAE R. H. Muñoz, et al. (5) SAE L. Liang, et al. (7) SAE
Applying 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 informationIMPORTANCE OF INTERNAL FLOW AND
IMPORTANCE OF INTERNAL FLOW AND GEOMETRY MODELLING IN THE GM 1.9L LIGHT DUTY ENGINE F. Perini a, P. C. Miles b, R. D. Reitz a a University of Wisconsin-Madison b Sandia National Laboratories ERC Seminar
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 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 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 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 informationCrevice and Blowby Model Development and Application
Crevice and Blowby Model Development and Application Randy P. Hessel University of Wisconsin - Madison Salvador M. Aceves and Dan L. Flowers - Lawrence Livermore National Lab ABSTRACT This paper describes
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 informationCoarse Mesh CFD: Trend Analysis In a Fraction of the Time
Coarse Mesh CFD: Trend Analysis In a Fraction of the Time Y. He, C. J. Rutland, Z. Nagel, R. P. Hessel, R. D. Reitz, D.E. Foster Engine Research Center, University of Wisconsin-Madison In an effort to
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 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 informationANSYS AIM Tutorial Compressible Flow in a Nozzle
ANSYS AIM Tutorial Compressible Flow in a Nozzle Author(s): Sebastian Vecchi Created using ANSYS AIM 18.1 Problem Specification Pre-Analysis & Start Up Pre-Analysis Start-Up Geometry Import Geometry Mesh
More informationFlow in an Intake Manifold
Tutorial 2. Flow in an Intake Manifold Introduction The purpose of this tutorial is to model turbulent flow in a simple intake manifold geometry. An intake manifold is a system of passages which carry
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 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 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 informationcuibm A GPU Accelerated Immersed Boundary Method
cuibm A GPU Accelerated Immersed Boundary Method S. K. Layton, A. Krishnan and L. A. Barba Corresponding author: labarba@bu.edu Department of Mechanical Engineering, Boston University, Boston, MA, 225,
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 informationUsing a Single Rotating Reference Frame
Tutorial 9. Using a Single Rotating Reference Frame Introduction This tutorial considers the flow within a 2D, axisymmetric, co-rotating disk cavity system. Understanding the behavior of such flows is
More informationin:flux - Intelligent CFD Software
in:flux - Intelligent CFD Software info@insightnumerics.com Fire and Gas Mapping. Optimized. Slide 1 Introduction to in:flux in:flux is a CFD software product to be used for dispersion and ventilation
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 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 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 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 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 informationLS-DYNA 980 : Recent Developments, Application Areas and Validation Process of the Incompressible fluid solver (ICFD) in LS-DYNA.
12 th International LS-DYNA Users Conference FSI/ALE(1) LS-DYNA 980 : Recent Developments, Application Areas and Validation Process of the Incompressible fluid solver (ICFD) in LS-DYNA Part 1 Facundo Del
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 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 informationRBF Morph An Add-on Module for Mesh Morphing in ANSYS Fluent
RBF Morph An Add-on Module for Mesh Morphing in ANSYS Fluent Gilles Eggenspieler Senior Product Manager 1 Morphing & Smoothing A mesh morpher is a tool capable of performing mesh modifications in order
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 informationMetafor FE Software. 2. Operator split. 4. Rezoning methods 5. Contact with friction
ALE simulations ua sus using Metafor eao 1. Introduction 2. Operator split 3. Convection schemes 4. Rezoning methods 5. Contact with friction 1 Introduction EULERIAN FORMALISM Undistorted mesh Ideal for
More informationRecent applications of overset mesh technology in SC/Tetra
Recent applications of overset mesh technology in SC/Tetra NIA CFD Seminar October 6, 2014 Tomohiro Irie Software Cradle Co., Ltd. 1 Contents Introduction Software Cradle SC/Tetra Background of Demands
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 informationK3PREP Workshop. This workshop is being offered on. June 22 th, by Engine Research Center University of Wisconsin-Madison
K3PREP Workshop This workshop is being offered on June 22 th, 2000 by Engine Research Center University of Wisconsin-Madison The goal of the workshop is to learn how to use K3PREP for building grids of
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 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 informationFirst Steps - Ball Valve Design
COSMOSFloWorks 2004 Tutorial 1 First Steps - Ball Valve Design This First Steps tutorial covers the flow of water through a ball valve assembly before and after some design changes. The objective is to
More informationModeling and Simulation of Single Phase Fluid Flow and Heat Transfer in Packed Beds
Modeling and Simulation of Single Phase Fluid Flow and Heat Transfer in Packed Beds by:- Balaaji Mahadevan Shaurya Sachdev Subhanshu Pareek Amol Deshpande Birla Institute of Technology and Science, Pilani
More information1.2 Numerical Solutions of Flow Problems
1.2 Numerical Solutions of Flow Problems DIFFERENTIAL EQUATIONS OF MOTION FOR A SIMPLIFIED FLOW PROBLEM Continuity equation for incompressible flow: 0 Momentum (Navier-Stokes) equations for a Newtonian
More informationRotating Moving Boundary Analysis Using ANSYS 5.7
Abstract Rotating Moving Boundary Analysis Using ANSYS 5.7 Qin Yin Fan CYBERNET SYSTEMS CO., LTD. Rich Lange ANSYS Inc. As subroutines in commercial software, APDL (ANSYS Parametric Design Language) provides
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 informationNUMERICAL INVESTIGATION OF THE FLOW BEHAVIOR INTO THE INLET GUIDE VANE SYSTEM (IGV)
University of West Bohemia» Department of Power System Engineering NUMERICAL INVESTIGATION OF THE FLOW BEHAVIOR INTO THE INLET GUIDE VANE SYSTEM (IGV) Publication was supported by project: Budování excelentního
More informationSimulation of Flow Development in a Pipe
Tutorial 4. Simulation of Flow Development in a Pipe Introduction The purpose of this tutorial is to illustrate the setup and solution of a 3D turbulent fluid flow in a pipe. The pipe networks are common
More informationCFD Topology Optimization of Automotive Components
CFD Topology Optimization of Automotive Components Dr.-Ing. Markus Stephan, Dr.-Ing. Dipl.-Phys. Pascal Häußler, Dipl.-Math. Michael Böhm FE-DESIGN GmbH, Karlsruhe, Germany Synopsis Automatic CFD optimization
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 informationCFD Analysis of conceptual Aircraft body
CFD Analysis of conceptual Aircraft body Manikantissar 1, Dr.Ankur geete 2 1 M. Tech scholar in Mechanical Engineering, SD Bansal college of technology, Indore, M.P, India 2 Associate professor in Mechanical
More informationNUMERICAL SIMULATION OF MULTI-CHAMBER PISTON C.I ENGINE
IOSR Journal of Mechanical and Civil Engineering (IOSR-JMCE) ISSN: 2278-1684, PP: 58-65 www.iosrjournals.org NUMERICAL SIMULATION OF MULTI-CHAMBER PISTON C.I ENGINE Mr. ARAHANTH 1, Mr. KARTIKA S.B 2 1
More informationHow to Use the kiva3v_lite Suite
How to Use the kiva3v_lite Suite This document gives an overview of and outlines the steps for using the kiva3v_lite software suite. Other kiva references available are: 1. kiva2, kiva3, kiva3v-release2
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 informationA Simplified CFD Model for Radiative Heat Transfer in Engines
International Multidimensional Engine Modeling User s Group Meeting at the SAE Congress Detroit, MI, 9 April 2018 A Simplified CFD Model for Radiative Heat Transfer in Engines D.C. Haworth and C. Paul
More informationCo-Simulation von Flownex und ANSYS CFX am Beispiel einer Verdrängermaschine
Co-Simulation von Flownex und ANSYS CFX am Beispiel einer Verdrängermaschine Benoit Bosc-Bierne, Dr. Andreas Spille-Kohoff, Farai Hetze CFX Berlin Software GmbH, Berlin Contents Positive displacement compressors
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 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 informationLagrangian methods and Smoothed Particle Hydrodynamics (SPH) Computation in Astrophysics Seminar (Spring 2006) L. J. Dursi
Lagrangian methods and Smoothed Particle Hydrodynamics (SPH) Eulerian Grid Methods The methods covered so far in this course use an Eulerian grid: Prescribed coordinates In `lab frame' Fluid elements flow
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 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 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 informationUse of CFD in Design and Development of R404A Reciprocating Compressor
Purdue University Purdue e-pubs International Compressor Engineering Conference School of Mechanical Engineering 2006 Use of CFD in Design and Development of R404A Reciprocating Compressor Yogesh V. Birari
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 informationExample 13 - Shock Tube
Example 13 - Shock Tube Summary This famous experiment is interesting for observing the shock-wave propagation. Moreover, this case uses the representation of perfect gas and compares the different formulations:
More informationA higher-order finite volume method with collocated grid arrangement for incompressible flows
Computational Methods and Experimental Measurements XVII 109 A higher-order finite volume method with collocated grid arrangement for incompressible flows L. Ramirez 1, X. Nogueira 1, S. Khelladi 2, J.
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 informationALE and Fluid-Structure Interaction in LS-DYNA March 2004
ALE and Fluid-Structure Interaction in LS-DYNA March 2004 Workshop Models 1. Taylor bar impact 2. One-dimensional advection test 3. Channel 4. Underwater explosion 5. Bar impacting water surface 6. Sloshing
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 informationManipulating the Boundary Mesh
Chapter 7. Manipulating the Boundary Mesh The first step in producing an unstructured grid is to define the shape of the domain boundaries. Using a preprocessor (GAMBIT or a third-party CAD package) you
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 informationTutorial 2. Modeling Periodic Flow and Heat Transfer
Tutorial 2. Modeling Periodic Flow and Heat Transfer Introduction: Many industrial applications, such as steam generation in a boiler or air cooling in the coil of an air conditioner, can be modeled as
More informationFinite Volume Discretization on Irregular Voronoi Grids
Finite Volume Discretization on Irregular Voronoi Grids C.Huettig 1, W. Moore 1 1 Hampton University / National Institute of Aerospace Folie 1 The earth and its terrestrial neighbors NASA Colin Rose, Dorling
More 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 informationSolving Partial Differential Equations on Overlapping Grids
**FULL TITLE** ASP Conference Series, Vol. **VOLUME**, **YEAR OF PUBLICATION** **NAMES OF EDITORS** Solving Partial Differential Equations on Overlapping Grids William D. Henshaw Centre for Applied Scientific
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 informationCFD Topological Optimization of a Car Water-Pump Inlet using TOSCA Fluid and STAR- CCM+
CFD Topological Optimization of a Car Water-Pump Inlet using TOSCA Fluid and STAR- CCM+ Dr. Anselm Hopf Dr. Andrew Hitchings Les Routledge Ford Motor Company CONTENTS Introduction/Motivation Optimization
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 informationExperimental and Numerical Analysis of Near Wall Flow at the Intake Valve and its Influence on Large-Scale Fluctuations
Experimental and Numerical Analysis of Near Wall Flow at the Intake Valve and its Influence on Large-Scale Fluctuations Frank Hartmann, Stefan Buhl, Florian Gleiß, Christian Hasse Philipp Barth, Martin
More informationDevelopment of Adaptive Mesh Refinement Scheme and Conjugate Heat Transfer Model for Engine Simulations
Graduate Theses and Dissertations Graduate College 2009 Development of Adaptive Mesh Refinement Scheme and Conjugate Heat Transfer Model for Engine Simulations Qingluan Xue Iowa State University Follow
More informationStructured Grid Generation for Turbo Machinery Applications using Topology Templates
Structured Grid Generation for Turbo Machinery Applications using Topology Templates January 13th 2011 Martin Spel martin.spel@rtech.fr page 1 Agenda: R.Tech activities Grid Generation Techniques Structured
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 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 informationMAE 3130: Fluid Mechanics Lecture 5: Fluid Kinematics Spring Dr. Jason Roney Mechanical and Aerospace Engineering
MAE 3130: Fluid Mechanics Lecture 5: Fluid Kinematics Spring 2003 Dr. Jason Roney Mechanical and Aerospace Engineering Outline Introduction Velocity Field Acceleration Field Control Volume and System Representation
More informationUrea Injection Simulation with Adaptive Mesh Refinement for Engine Aftertreatment
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
More informationPTE 519 Lecture Note Finite Difference Approximation (Model)
PTE 519 Lecture Note 3 3.0 Finite Difference Approximation (Model) In this section of the lecture material, the focus is to define the terminology and to summarize the basic facts. The basic idea of any
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 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 informationTurbulencja w mikrokanale i jej wpływ na proces emulsyfikacji
Polish Academy of Sciences Institute of Fundamental Technological Research Turbulencja w mikrokanale i jej wpływ na proces emulsyfikacji S. Błoński, P.Korczyk, T.A. Kowalewski PRESENTATION OUTLINE 0 Introduction
More informationOpenFOAM: Open Platform for Complex Physics Simulations
OpenFOAM: Open Platform for Complex Physics Simulations Hrvoje Jasak h.jasak@wikki.co.uk, hrvoje.jasak@fsb.hr FSB, University of Zagreb, Croatia Wikki Ltd, United Kingdom 18th October 2007 OpenFOAM: Open
More informationOverview and Recent Developments of Dynamic Mesh Capabilities
Overview and Recent Developments of Dynamic Mesh Capabilities Henrik Rusche and Hrvoje Jasak h.rusche@wikki-gmbh.de and h.jasak@wikki.co.uk Wikki Gmbh, Germany Wikki Ltd, United Kingdom 6th OpenFOAM Workshop,
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 informationON THE NUMERICAL MODELING OF IMPINGING JET HEAT TRANSFER
ON THE NUMERICAL MODELING OF IMPINGING JET HEAT TRANSFER Mirko Bovo 1,2, Sassan Etemad 2 and Lars Davidson 1 1 Dept. of Applied Mechanics, Chalmers University of Technology, Gothenburg, Sweden 2 Powertrain
More informationCFD Modelling in the Cement Industry
CFD Modelling in the Cement Industry Victor J. Turnell, P.E., Turnell Corp., USA, describes computational fluid dynamics (CFD) simulation and its benefits in applications in the cement industry. Introduction
More informationAxisymmetric Viscous Flow Modeling for Meridional Flow Calculation in Aerodynamic Design of Half-Ducted Blade Rows
Memoirs of the Faculty of Engineering, Kyushu University, Vol.67, No.4, December 2007 Axisymmetric Viscous Flow Modeling for Meridional Flow alculation in Aerodynamic Design of Half-Ducted Blade Rows by
More informationENERGY-224 Reservoir Simulation Project Report. Ala Alzayer
ENERGY-224 Reservoir Simulation Project Report Ala Alzayer Autumn Quarter December 3, 2014 Contents 1 Objective 2 2 Governing Equations 2 3 Methodolgy 3 3.1 BlockMesh.........................................
More informationOverview of Traditional Surface Tracking Methods
Liquid Simulation With Mesh-Based Surface Tracking Overview of Traditional Surface Tracking Methods Matthias Müller Introduction Research lead of NVIDIA PhysX team PhysX GPU acc. Game physics engine www.nvidia.com\physx
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 informationBACK AND FORTH ERROR COMPENSATION AND CORRECTION METHODS FOR REMOVING ERRORS INDUCED BY UNEVEN GRADIENTS OF THE LEVEL SET FUNCTION
BACK AND FORTH ERROR COMPENSATION AND CORRECTION METHODS FOR REMOVING ERRORS INDUCED BY UNEVEN GRADIENTS OF THE LEVEL SET FUNCTION TODD F. DUPONT AND YINGJIE LIU Abstract. We propose a method that significantly
More informationVerification and Validation of Turbulent Flow around a Clark-Y Airfoil
Verification and Validation of Turbulent Flow around a Clark-Y Airfoil 1. Purpose 58:160 Intermediate Mechanics of Fluids CFD LAB 2 By Tao Xing and Fred Stern IIHR-Hydroscience & Engineering The University
More 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 informationAerodynamic Study of a Realistic Car W. TOUGERON
Aerodynamic Study of a Realistic Car W. TOUGERON Tougeron CFD Engineer 2016 Abstract This document presents an aerodynamic CFD study of a realistic car geometry. The aim is to demonstrate the efficiency
More 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 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 informationIntegrated analysis of the scavenging process in marine two-stroke diesel engines
Integrated analysis of the scavenging process in marine two-stroke diesel engines Gothenburg regional OpenFOAM user group meeting. 13 november 2013 Fredrik H. Andersen, Industrial Ph.D. student Process
More information