Optimization of under-relaxation factors. and Courant numbers for the simulation of. sloshing in the oil pan of an automobile
|
|
- Osborn Lewis
- 6 years ago
- Views:
Transcription
1 Optimization of under-relaxation factors and Courant numbers for the simulation of sloshing in the oil pan of an automobile Swathi Satish*, Mani Prithiviraj and Sridhar Hari⁰ *National Institute of Technology, Surathkal, Karnataka, CD-adapco, Bangalore, Karnataka, ⁰ CD-adapco, Bangalore, Karnataka,
2 INDEX I. List of Figures II. List of Tables Abstract Background Introduction Geometry modelling and simulation Results and Discussion Conclusion References Figures Tables
3 I. List of Figures 1. Illustration of grids that are unsuitable (left) and suitable (right) for two-phase flows using the VOF model. 2. 3D model of the oil pan. 3. Section plane showing the polyhedral mesh generated. 4. Scalar scene after initialization showing the 6 point probes. 5. Scalar scene after the attainment of steady state. 6. (a) Trimmer mesh with base size 8 mm, (b) Trimmer mesh with base size 4 mm. 7. Plots of URF values versus simulation time at the 6 probe points. 8. Plot of (a) Volume fraction of Oil at the 6 probe points versus the simulation time, (b) Pressure at the pressure outlet versus the simulation time for a Velocity URF Plot of (a) Volume fraction of Oil at the 6 probe points versus the simulation time, (b) Pressure at the pressure outlet versus the simulation time for a Pressure URF Plot of (a) Volume fraction of Oil at the 6 probe points versus the simulation time, (b) Pressure at the pressure outlet versus the simulation time for a Segregated VOF URF Plot of (a) Volume fraction of Oil at the 6 probe points versus the simulation time, (b) Pressure at the pressure outlet versus the simulation time for a K-ɛ turbulence URF Plot of Courant number versus simulation time for a polyhedral mesh. 13. Plot of Courant number versus simulation time for a trimmer mesh of base size 8 mm. 14. Plot of Courant number versus simulation time for a trimmer mesh of base size 4 mm. 3
4 II. List of Tables 1. Meshing parameters for the polyhedral mesh. 2. Physics models. 3. Material properties in the multiphase mixture. 4. Meshing parameters for the two trimmer meshes. 5 (a). Convergence time for different values of Velocity URF at the 6 probe points. (b). Convergence time for different values of Pressure URF at the 6 probe points. (c). Convergence time for different values of Segregated VOF URF at the 6 probe points. (d). Convergence time for different values of K-ε turbulence URF at the 6 probe points. 4
5 Abstract The phenomenon of sloshing in the oil pan of an automobile moving with a constant acceleration of 3 m/s^2 has been simulated in STAR-CCM+ v , a multi-disciplinary engineering simulation tool. The Volume Of Fluid multiphase model has been used for the same. This study consists of two parts, the first one being, optimization of the underrelaxation factors (URFs) involved in the flow simulation. The optimum values for the velocity URF, pressure URF, segregated VOF URF, K-Epsilon turbulence URF and K- Epsilon turbulent viscosity URF have been obtained. The maximum, mean and minimum Courant numbers for the optimum case have been found out. The second part of the study is the analysis of the variation of the maximum, mean and minimum Courant numbers with a change in mesh type from polyhedral to trimmer mesh. This has been performed on two cases of the trimmer mesh, with base mesh sizes of 8 mm and 4 mm respectively. The results obtained show that the Courant numbers decrease when the mesh type is changed from polyhedral to trimmer. Also, the Courant numbers are lower for the trimmer mesh with 4 mm base mesh size as compared to the trimmer mesh with 8 mm base mesh size. Therefore, according to the requirements of the user, a balance can be achieved between mesh type, mesh size and Courant numbers. 1. Background Oil pans are major engine cooling system parts. They are usually constructed of thin steel and shaped into a deeper section to fully perform its function. It is also where the oil pump is placed. When an engine is not running or at rest, oil pans collect the oil as it flows down from the sides of the crankcase. In other words, oil pans that are mounted at the bottom of the crankcase serves as an oil reservoir. They also act as a source of structural strength for 5
6 the crank case. Engine oil is used for the lubrication, cooling, and cleaning of internal combustion engines [1-2]. At the bottom of the pan is the oil drain plug that can be usually removed to allow old oil to flow out of the car during an oil exchange. After the used oil drains out, the plug is screwed back into the drain hole. Drain plugs are often made with a magnet in it, collecting metal fragments from the oil. Some contains a replaceable washer to avoid leakage caused by corrosion or worn threads in the drain hole. An oil pan is more prone to leaking compared to any other car part. It is because it holds oil which is being thrown around due to sloshing. Sloshing refers to the movement of liquid inside another object (which is, typically, also undergoing motion). Here, sloshing of oil occurs in the oil pan of an automobile that is under motion. The dynamics of the oil interact with the pan to alter the system dynamics significantly. Other examples include propellant slosh in spacecraft tanks and rockets (especially upper stages), and cargo slosh in ships and trucks transporting liquids (for example oil and gasoline). 2. Introduction The phenomenon of sloshing in the oil pan of an automobile is a multiphase flow problem. It consists of two phases, air and oil. Multiphase flow refers to the flow and interaction of several phases within the same system where distinct interfaces exist between the phases. Multiphase flows can be modelled using the Lagrangian approach or the Eulerian approach. For simulating sloshing in an oil pan, Volume Of Fluid (VOF) approach is used [3]. The VOF model is used for immiscible fluids and makes use of Eulerian phases. It is well suited for problems where each phase constitutes a large structure, with relatively small 6
7 contact area between the phases (Figure 1). It acts as an efficient tool for tracking and locating the position and shape of the fluid-fluid interface. Under-relaxation factors are significant parameters affecting the convergence of a numerical scheme. They represent the fraction of the solution being carried forward from one iteration to the next for the various equations being solved during the simulation. The Courant number expresses the ratio of the distance travelled by a disturbance in one time step to the length of a computational distance step. It influences the accuracy and stability of the solution. The phenomenon of sloshing in the oil pan of an automobile has been a topic of intense research, as can be seen evinced from even a cursory glance at literature [4-8]. The current exercise has been undertaken with an objective to optimize the values of the various under-relaxation factors as well as the Courant numbers involved in the simulating sloshing in an oil pan in order to minimize the simulation time and hence the cost of the simulation. 3. Geometry modelling and simulation The geometry of the oil pan was created using the STAR-CCM+ 3D-CAD modeller. The dimensions of the model are shown in Figure 2. The oil pan has a length 59 cm, width 28 cm and height 19 cm. The base of the pan has three steps at depths of 9 cm, 13 cm and 19 cm. A pressure outlet is present on the top face of the oil pan in order to simulate the atmospheric pressure acting on the oil surface. The reference pressure was taken as Pa and all the pressure values were specified with respect to this value. The mesh generation process was performed with a base size of 8 mm using polyhedral cells with a prism layer mesh at the boundaries (Figure 3). The surface remesher was used to improve the quality of the mesh. The meshing parameters used for the process are shown in Table 1. The physics models were specified to the region as shown in Table 2. 7
8 A 3-dimensional, implicit unsteady model was chosen the VOF method was selected as the multiphase flow model. The material for the region was specified as a multiphase mixture consisting of Air and Oil, whose material properties are shown in Table 3. The RANS k- epsilon turbulence model was used for the simulation along with the additional gravity model. Initial and boundary conditions were assigned as follows. The initial level of oil in the pan was specified as 7 cm from the top surface. The oil pan was given an initial acceleration of 3 m/s in the forward direction as shown in Figure 2. The pressure at the pressure outlet was taken as 0 Pa with respect to the reference pressure. Six point probes were created as shown in Figure 4 to monitor the volume fraction of oil at the points. Pressure at the pressure outlet was also monitored. Plots were created for the above two quantities versus simulation time. The solver parameters included an implicit unsteady time-step of 0.03 s and maximum inner iterations of 20. The tolerance value for determining steady-state was taken as for 100 iterations, that is, the change in the value of the physical quantity should be less than for 100 iterations. The flow was simulated until steady state was obtained (Figure 5). The process of optimization of the URFs includes varying the value of one URF, while keeping the others constant and selecting the value for which the simulation time is the least. This was carried out for the velocity URF, pressure URF, segregated VOF URF, K- Epsilon turbulence URF and K-Epsilon turbulent viscosity URF. The maximum, mean and minimum Courant numbers were then determined for the polyhedral mesh. The mesh type was changed from polyhedral to trimmer and the maximum, mean and minimum Courant numbers were found out for two trimmer meshes, one with a base size 8 mm and the other with a base size 4 mm (Figure 6). The meshing parameters for the two 8
9 trimmer meshes are shown in Table 4. The flow was simulated with the default values of URFs provided by STAR-CCM+. 4. Results and discussion a. Optimization of the URFs: (i) Velocity URF: The values of simulation time obtained by varying the value of velocity URF and keeping the other URFs constant (default values) are shown in Table 5.a. The number of iterations taken to attain a steady state is shown is found to be the least for a Velocity URF of 0.9 (Figure 7.a). The same behaviour is observed in the plots obtained for volume fraction of oil at the six probe points and outlet pressure versus simulation time (Figure 8). (ii) Pressure URF: The values of simulation time obtained by varying the value of pressure URF, keeping the value of velocity URF at 0.9 and the other URFs constant (default values) are shown in Table 5.b. The number of iterations taken to attain a steady state is shown is found to be the least for a Pressure URF of 0.5 (Figure 7.b). The same behaviour is observed in the plots obtained for volume fraction of oil at the six probe points and outlet pressure versus simulation time (Figure 9). (iii) Segregated VOF URF: The values of simulation time obtained by varying the value of segregated VOF URF, keeping the value of velocity URF at 0.9, pressure URF at 0.5 and the other URFs constant (default values) are shown in Table 5.c. The number of iterations taken to attain a steady state is shown is found to be the least for a Segregated VOF URF of 0.8 (Figure 7.c). The same behaviour is observed in the plots obtained for volume fraction of oil at the six probe points and outlet pressure versus simulation time (Figure 10). (iv) K-ɛ turbulence URF: The values of simulation time obtained by varying the value of K-ɛ turbulence URF, keeping the value of velocity URF at 0.9, pressure URF at 0.5, segregated 9
10 VOF URF at 0.8 and the K-ɛ turbulent viscosity URF at 1.0 (default value) are shown in Table 5.c. The number of iterations taken to attain a steady state is shown is found to be the least for a K-ɛ turbulence URF of 0.9 (Figure 7.d). The same behaviour is observed in the plots obtained for volume fraction of oil at the six probe points and outlet pressure versus simulation time (Figure 11). b. Variation of Courant numbers with the type and size of mesh: For the polyhedral mesh, using the optimized values of the under-relaxation factors, at the end of 1000 iterations we obtain the following values for the maximum, mean and minimum Courant numbers (Figure 12): Maximum Courant Number = Minimum Courant Number = Mean Courant Number = Total CPU time = 8567 s. For the trimmer mesh with base size 8 mm (Figure 6.a), using the default values of URFs, at the end of 1000 iterations we obtain the following values of maximum, mean and minimum Courant numbers (Figure 13): Maximum Courant Number = Minimum Courant Number = E-4. Mean Courant Number = For the trimmer mesh with base size 4 mm (Figure 6.b), using the default values of URFs, at the end of 2000 iterations we obtain the following values of maximum, mean and minimum Courant numbers (Figure 14): Maximum Courant Number = Minimum Courant Number = E-4. Mean Courant Number =
11 For the two trimmer meshes used, it was observed that the number of iterations required to attain a steady state is more for the trimmer mesh with base size 4 mm. Due to its smaller mesh size, the amount of computation involved is more. The maximum, mean and minimum Courant numbers obtained for this mesh are significantly lower compared to the trimmer mesh with base size 8 mm. 5. Conclusion Optimization of the values of under-relaxation factors was performed for the case of sloshing in the oil pan of an automobile moving with a constant acceleration of 3 m/s 2 was performed and the URF values after optimization were found to be as follows: Velocity URF : 0.9 Pressure URF : 0.5 Segregated VOF URF : 0.8 K-ɛ turbulence URF : 0.9 K-ɛ turbulent viscosity URF : 1.0 (default) The maximum, mean and minimum Courant numbers for a polyhedral mesh were found to be lower than those for a trimmer mesh of the same base mesh size (8 mm). With a decrease in the base size of the trimmer mesh to 4 mm, there was a significant decrease in the Courant numbers. The simulation time, however, was higher. Therefore, according to the requirements of the developer such as mesh type and mesh size, optimum values of Courant numbers are obtained. In terms of future scope, optimization of URFs can be performed for various other conditions such as sloshing in the oil pan during braking, varying accelerations, etc. Optimization is a necessity for almost all simulations and hence the same methodology can be utilized to reduce the simulation time for a variety of problems. 11
12 6. References [1] [2] [3] STAR-CCM+ Code User Manual Version (2012), CD-adapco, NY 11747, USA. [4] E Kopec, W Oberknapp, Slosh baffle for oil pan of internal combustion engine. US Patent 4,449,493, [5] TM Bishop, Oil pan with vertical baffles for oil flow control. US Patent 6,845,743, [6] RK Shier, Engine having oil pan with deflection vanes. US Patent 3,425,514, [7] M Beer, Oil container and a process for the production thereof. US Patent 7,077,285, [8] JR Lang, Oil level sensing apparatus. US Patent 4,091,895,
13 7. Figures Figure 1. Illustration of grids that are unsuitable (left) and suitable (right) for two-phase flows using the VOF model. Figure 2. 3D model of the oil pan Figure 3. Section plane showing the polyhedral mesh generated 13
14 Figure 4. Scalar scene after initialization showing the 6 point probes Figure 5. Scalar scene after the attainment of steady state Figure 6. (a) Trimmer mesh with base size 8 mm, (b) Trimmer mesh with base size 4 mm 14
15 Figure 7. Plots of URF values versus simulation time at the 6 probe points Figure 8. Plot of (a) Volume fraction of Oil at the 6 probe points versus the simulation time, (b) Pressure at the pressure outlet versus the simulation time for a Velocity URF
16 Figure 9. Plot of (a) Volume fraction of Oil at the 6 probe points versus the simulation time, (b) Pressure at the pressure outlet versus the simulation time for a Pressure URF 0.5 Figure 10. Plot of (a) Volume fraction of Oil at the 6 probe points versus the simulation time, (b) Pressure at the pressure outlet versus the simulation time for a Segregated VOF URF
17 Figure 11. Plot of (a) Volume fraction of Oil at the 6 probe points versus the simulation time, (b) Pressure at the pressure outlet versus the simulation time for a K-ɛ turbulence URF 0.8 Figure 12. Plot of Courant number versus simulation time for a polyhedral mesh 17
18 Figure 13. Plot of Courant number versus simulation time for a trimmer mesh of base size 8 mm Figure 14. Plot of Courant number versus simulation time for a trimmer mesh of base size 4 mm 18
19 8. Tables Mesh Parameter Value Base size 8 mm Number of prism layers 2 Prism layer stretching 1.2 Prism layer thickness 4 mm Surface curvature 18 pts/circle Surface growth rate 1.3 Table 1. Meshing parameters for the polyhedral mesh Physics parameter Type of model Space Three dimensional Time Implicit unsteady Material Multiphase mixture Multiphase flow model Volume Of Fluid model Viscous Regime Turbulent Turbulence model RANS K-epsilon turbulence Optional model Gravity Table 2. Physics models Material Density (kg/ ) Viscosity (E-5 Pa.s) Air Oil Table 3. Material properties in the multiphase mixture Mesh Parameters Trimmer mesh with base size 8 mm Trimmer mesh with base size 4 mm Base size 8 mm 4 mm Maximum cell size 10000% of base 100% of base Number of prism layers 2 2 Prism layer stretching Surface curvature 18 pts/circle 36 pts/circle Surface minimum size 2 mm 1 mm Surface target size 8 mm 4 mm Table 4. Meshing parameters for the two trimmer meshes 19
20 Velocity URF Number of iterations for convergence Top1 Top2 Mid1 Mid2 Bottom1 Bottom Table 5. (a) Convergence time for different values of Velocity URF at the 6 probe points Pressure URF Number of iterations for convergence Top1 Top2 Mid1 Mid2 Bottom1 Bottom Table 5. (b) Convergence time for different values of Pressure URF at the 6 probe points Segregated VOF URF Number of iterations for convergence Top1 Top2 Mid1 Mid2 Bottom1 Bottom Table 5. (c) Convergence time for different values of Segregated VOF URF at the 6 probe points k-ε turbulence URF Number of iterations for convergence Top1 Top2 Mid1 Mid2 Bottom1 Bottom Table 5. (d) Convergence time for different values of K-ε turbulence URF at the 6 probe points 20
Tutorial 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 informationUse 6DOF solver to calculate motion of the moving body. Create TIFF files for graphic visualization of the solution.
Introduction The purpose of this tutorial is to provide guidelines and recommendations for setting up and solving a moving deforming mesh (MDM) case along with the six degree of freedom (6DOF) solver and
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 informationEXPERIMENTAL VALIDATION OF STAR-CCM+ FOR LIQUID CONTAINER SLOSH DYNAMICS
EXPERIMENTAL VALIDATION OF STAR-CCM+ FOR LIQUID CONTAINER SLOSH DYNAMICS Brandon Marsell a.i. solutions, Launch Services Program, Kennedy Space Center, FL 1 Agenda Introduction Problem Background Experiment
More informationSTAR-CCM+: Wind loading on buildings SPRING 2018
STAR-CCM+: Wind loading on buildings SPRING 2018 1. Notes on the software 2. Assigned exercise (submission via Blackboard; deadline: Thursday Week 3, 11 pm) 1. NOTES ON THE SOFTWARE STAR-CCM+ generates
More 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 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 informationSteady Flow: Lid-Driven Cavity Flow
STAR-CCM+ User Guide Steady Flow: Lid-Driven Cavity Flow 2 Steady Flow: Lid-Driven Cavity Flow This tutorial demonstrates the performance of STAR-CCM+ in solving a traditional square lid-driven cavity
More informationIsotropic Porous Media Tutorial
STAR-CCM+ User Guide 3927 Isotropic Porous Media Tutorial This tutorial models flow through the catalyst geometry described in the introductory section. In the porous region, the theoretical pressure drop
More informationSimulation of Automotive Fuel Tank Sloshing using Radioss
Simulation of Automotive Fuel Tank Sloshing using Radioss Prashant V. Kulkarni CAE Analyst Tata Motors. Pimpri, Pune - 411018, India Sanjay S. Patil Senior Manager Tata Motors. Pimpri, Pune - 411018, India
More informationPressure Losses Analysis in Air Duct Flow Using Computational Fluid Dynamics (CFD)
International Academic Institute for Science and Technology International Academic Journal of Science and Engineering Vol. 3, No. 9, 2016, pp. 55-70. ISSN 2454-3896 International Academic Journal of Science
More informationCDA Workshop Physical & Numerical Hydraulic Modelling. STAR-CCM+ Presentation
CDA Workshop Physical & Numerical Hydraulic Modelling STAR-CCM+ Presentation ENGINEERING SIMULATION CFD FEA Mission Increase the competitiveness of companies through optimization of their product development
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 informationµ = Pa s m 3 The Reynolds number based on hydraulic diameter, D h = 2W h/(w + h) = 3.2 mm for the main inlet duct is = 359
Laminar Mixer Tutorial for STAR-CCM+ ME 448/548 March 30, 2014 Gerald Recktenwald gerry@pdx.edu 1 Overview Imagine that you are part of a team developing a medical diagnostic device. The device has a millimeter
More informationOffshore Platform Fluid Structure Interaction (FSI) Simulation
Offshore Platform Fluid Structure Interaction (FSI) Simulation Ali Marzaban, CD-adapco Murthy Lakshmiraju, CD-adapco Nigel Richardson, CD-adapco Mike Henneke, CD-adapco Guangyu Wu, Chevron Pedro M. Vargas,
More informationAPPLIED COMPUTATIONAL FLUID DYNAMICS-PROJECT-3
APPLIED COMPUTATIONAL FLUID DYNAMICS-PROJECT-3 BY SAI CHAITANYA MANGAVELLI Common Setup Data: 1) Mesh Proximity and Curvature with Refinement of 2. 2) Double Precision and second order for methods in Solver.
More informationHealthy Buildings 2017 Europe July 2-5, 2017, Lublin, Poland
Healthy Buildings 2017 Europe July 2-5, 2017, Lublin, Poland Paper ID 0122 ISBN: 978-83-7947-232-1 Numerical Investigation of Transport and Deposition of Liquid Aerosol Particles in Indoor Environments
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 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 informationAdvances in Turbomachinery Simulation Fred Mendonça and material prepared by Chad Custer, Turbomachinery Technology Specialist
Advances in Turbomachinery Simulation Fred Mendonça and material prepared by Chad Custer, Turbomachinery Technology Specialist Usage From Across the Industry Outline Key Application Objectives Conjugate
More informationA new meshing methodology for faster simulation of a Body-In-White dipping process
A new meshing methodology for faster simulation of a Body-In-White dipping process Madhusudhan Devanathan MBtech Group GmbH & Co. KGaA, Sindelfingen, Germany STAR Global Conference 19 1 March 01, Amsterdam
More information2-D Tank Sloshing Using the Coupled Eulerian- LaGrangian (CEL) Capability of Abaqus/Explicit
2-D Tank Sloshing Using the Coupled Eulerian- LaGrangian (CEL) Capability of Abaqus/Explicit Jeff D. Tippmann, Sharat C. Prasad 2, and Parthiv N. Shah ATA Engineering, Inc. San Diego, CA 923 2 Dassault
More informationParametric Study of Sloshing Effects in the Primary System of an Isolated LFR Marti Jeltsov, Walter Villanueva, Pavel Kudinov
1 Parametric Study of Sloshing Effects in the Primary System of an Isolated LFR 19.06.2013 Marti Jeltsov, Walter Villanueva, Pavel Kudinov Division of Nuclear Power Safety Royal Institute of Technology
More informationModeling Unsteady Compressible Flow
Tutorial 4. Modeling Unsteady Compressible Flow Introduction In this tutorial, FLUENT s density-based implicit solver is used to predict the timedependent flow through a two-dimensional nozzle. As an initial
More informationS-ducts and Nozzles: STAR-CCM+ at the Propulsion Aerodynamics Workshop. Peter Burns, CD-adapco
S-ducts and Nozzles: STAR-CCM+ at the Propulsion Aerodynamics Workshop Peter Burns, CD-adapco Background The Propulsion Aerodynamics Workshop (PAW) has been held twice PAW01: 2012 at the 48 th AIAA JPC
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 informationInternational Power, Electronics and Materials Engineering Conference (IPEMEC 2015)
International Power, Electronics and Materials Engineering Conference (IPEMEC 2015) Numerical Simulation of the Influence of Intake Grille Shape on the Aerodynamic Performance of a Passenger Car Longwei
More 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 informationProject 2 Solution. General Procedure for Model Setup
Project 2 Solution MAE598 Applied Computational Fluid Dynamics Shashank Kunjibettu General Procedure for Model Setup Step 1: Model the given component using design modeler Step 2: Meshing is done for the
More informationSTAR-CCM+ User Guide 6922
STAR-CCM+ User Guide 6922 Introduction Welcome to the STAR-CCM+ introductory tutorial. In this tutorial, you explore the important concepts and workflow. Complete this tutorial before attempting any others.
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 informationNUMERICAL STUDY OF CAVITATING FLOW INSIDE A FLUSH VALVE
Conference on Modelling Fluid Flow (CMFF 09) The 14th International Conference on Fluid Flow Technologies Budapest, Hungary, September 9-12, 2009 NUMERICAL STUDY OF CAVITATING FLOW INSIDE A FLUSH VALVE
More 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 informationSimulation of a Free Surface Flow over a Container Vessel Using CFD
Simulation of a Free Surface Flow over a Container Vessel Using CFD Krishna Atreyapurapu 1 Bhanuprakash Tallapragada 2 Kiran Voonna 3 M.E Student Professor Manager Dept. of Marine Engineering Dept. of
More informationDirections: 1) Delete this text box 2) Insert desired picture here
Directions: 1) Delete this text box 2) Insert desired picture here Multi-Disciplinary Applications using Overset Grid Technology in STAR-CCM+ CD-adapco Dmitry Pinaev, Frank Schäfer, Eberhard Schreck Outline
More informationExpress Introductory Training in ANSYS Fluent Workshop 07 Tank Flushing
Express Introductory Training in ANSYS Fluent Workshop 07 Tank Flushing Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 - Industry Oriented HPC Simulations,
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 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 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 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 informationTHE APPLICATION OF AN ATMOSPHERIC BOUNDARY LAYER TO EVALUATE TRUCK AERODYNAMICS IN CFD
THE APPLICATION OF AN ATMOSPHERIC BOUNDARY LAYER TO EVALUATE TRUCK AERODYNAMICS IN CFD A SOLUTION FOR A REAL-WORLD ENGINEERING PROBLEM Ir. Niek van Dijk DAF Trucks N.V. CONTENTS Scope & Background Theory:
More informationBest Practices: Electronics Cooling. Ruben Bons - CD-adapco
Best Practices: Electronics Cooling Ruben Bons - CD-adapco Best Practices Outline Geometry Mesh Materials Conditions Solution Results Design exploration / Optimization Best Practices Outline Geometry Solids
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 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 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 and experimental investigations into liquid sloshing in a rectangular tank
The 2012 World Congress on Advances in Civil, Environmental, and Materials Research (ACEM 12) Seoul, Korea, August 26-30, 2012 Numerical and experimental investigations into liquid sloshing in a rectangular
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 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 informationProject #3 MAE 598 Applied CFD
Project #3 MAE 598 Applied CFD 16 November 2017 H.P. Huang 1 Task 1 (a) Task 1a was to perform a transient analysis of a 2-D chamber that is initially filled with air, and has water flowing through the
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 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 informationSolution Recording and Playback: Vortex Shedding
STAR-CCM+ User Guide 6663 Solution Recording and Playback: Vortex Shedding This tutorial demonstrates how to use the solution recording and playback module for capturing the results of transient phenomena.
More 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 informationAccurate and Efficient Turbomachinery Simulation. Chad Custer, PhD Turbomachinery Technical Specialist
Accurate and Efficient Turbomachinery Simulation Chad Custer, PhD Turbomachinery Technical Specialist Outline Turbomachinery simulation advantages Axial fan optimization Description of design objectives
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 informationStratified Oil-Water Two-Phases Flow of Subsea Pipeline
Stratified Oil-Water Two-Phases Flow of Subsea Pipeline Adib Zulhilmi Mohd Alias, a, Jaswar Koto, a,b,*, Yasser Mohamed Ahmed, a and Abd Khair Junaidi, b a) Department of Aeronautics, Automotive and Ocean
More informationCFD Optimisation case studies with STAR-CD and STAR-CCM+
CFD Optimisation case studies with STAR-CD and STAR-CCM+ Summary David J. Eby, Preetham Rao, Advanced Methods Group, Plymouth, MI USA Presented by Fred Mendonça, CD-adapco London, UK Outline Introduction
More informationSTAR-CCM+: Ventilation SPRING Notes on the software 2. Assigned exercise (submission via Blackboard; deadline: Thursday Week 9, 11 pm)
STAR-CCM+: Ventilation SPRING 208. Notes on the software 2. Assigned exercise (submission via Blackboard; deadline: Thursday Week 9, pm). Features of the Exercise Natural ventilation driven by localised
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 Simulation for Stratified Oil-Water Two-Phase Flow in a Horizontal Pipe
CFD Simulation for Stratified Oil-Water Two-Phase Flow in a Horizontal Pipe Adib Zulhilmi Mohd Alias, a, Jaswar Koto, a,b,* and Yasser Mohamed Ahmed, a a) Department of Aeronautics, Automotive and Ocean
More informationAdvances in Cyclonic Flow Regimes. Dr. Dimitrios Papoulias, Thomas Eppinger
Advances in Cyclonic Flow Regimes Dr. Dimitrios Papoulias, Thomas Eppinger Agenda Introduction Cyclones & Hydrocyclones Modeling Approaches in STAR-CCM+ Turbulence Modeling Case 1: Air-Air Cyclone Case
More informationComparison Between Numerical & PIV Experimental Results for Gas-Solid Flow in Ducts
Fabio Kasper Comparison Between Numerical & PIV Experimental Results for Gas-Solid Flow in Ducts Rodrigo Decker, Oscar Sgrott Jr., Henry F. Meier Waldir Martignoni Agenda Introduction The Test Bench Case
More informationFree Convection Cookbook for StarCCM+
ME 448/548 February 28, 2012 Free Convection Cookbook for StarCCM+ Gerald Recktenwald gerry@me.pdx.edu 1 Overview Figure 1 depicts a two-dimensional fluid domain bounded by a cylinder of diameter D. Inside
More informationCOOL-COVERINGS. André Santos, The Netherlands Copyright Active Space Technologies
COOL-COVERINGS André Santos, The Netherlands 21-03-2012 Copyright Active Space Technologies 2004-2011 Young and competent company Started in 2007 in Germany, in 2004 in Portugal Role Support scientific
More informationA study of Jumper FIV due to multiphase internal flow: understanding life-cycle fatigue. Alan Mueller & Oleg Voronkov
A study of Jumper FIV due to multiphase internal flow: understanding life-cycle fatigue Alan Mueller & Oleg Voronkov Case description Main structural dimensions [1]: deformable jumper [2] in Mixture on
More informationCFD Study of a Darreous Vertical Axis Wind Turbine
CFD Study of a Darreous Vertical Axis Wind Turbine Md Nahid Pervez a and Wael Mokhtar b a Graduate Assistant b PhD. Assistant Professor Grand Valley State University, Grand Rapids, MI 49504 E-mail:, mokhtarw@gvsu.edu
More informationComputational Fluid Dynamic Hydraulic Characterization: G3 Cube vs. Dolos Armour Unit. IS le Roux, WJS van der Merwe & CL de Wet
Computational Fluid Dynamic Hydraulic Characterization: G3 Cube vs. Dolos Armour Unit IS le Roux, WJS van der Merwe & CL de Wet Presentation Outline Scope. Assumptions and boundary values. Numerical mesh.
More informationSimulation of the Airflow Characteristic inside a Hard Disk Drive by Applying a Computational Fluid Dynamics Software
Simulation of the Airflow Characteristic inside a Hard Disk Drive by Applying a Computational Fluid Dynamics Software Chanchal Saha, Huynh Trung Luong, M. H. Aziz, and Tharinan Rattanalert Abstract Now-a-days,
More informationIntroduction to CFX. Workshop 2. Transonic Flow Over a NACA 0012 Airfoil. WS2-1. ANSYS, Inc. Proprietary 2009 ANSYS, Inc. All rights reserved.
Workshop 2 Transonic Flow Over a NACA 0012 Airfoil. Introduction to CFX WS2-1 Goals The purpose of this tutorial is to introduce the user to modelling flow in high speed external aerodynamic applications.
More informationBest Practices: Volume Meshing Kynan Maley
Best Practices: Volume Meshing Kynan Maley Volume Meshing Volume meshing is the basic tool that allows the creation of the space discretization needed to solve most of the CAE equations for: CFD Stress
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 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 informationParallelization study of a VOF/Navier-Stokes model for 3D unstructured staggered meshes
Parallelization study of a VOF/Navier-Stokes model for 3D unstructured staggered meshes L. Jofre, O. Lehmkuhl, R. Borrell, J. Castro and A. Oliva Corresponding author: cttc@cttc.upc.edu Centre Tecnològic
More informationShape optimisation using breakthrough technologies
Shape optimisation using breakthrough technologies Compiled by Mike Slack Ansys Technical Services 2010 ANSYS, Inc. All rights reserved. 1 ANSYS, Inc. Proprietary Introduction Shape optimisation technologies
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 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 informationAvailable online at ScienceDirect. Procedia Engineering 136 (2016 ) Dynamic analysis of fuel tank
Available online at www.sciencedirect.com ScienceDirect Procedia Engineering 136 (2016 ) 45 49 The 20 th International Conference: Machine Modeling and Simulations, MMS 2015 Dynamic analysis of fuel tank
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 informationNon-Newtonian Transitional Flow in an Eccentric Annulus
Tutorial 8. Non-Newtonian Transitional Flow in an Eccentric Annulus Introduction The purpose of this tutorial is to illustrate the setup and solution of a 3D, turbulent flow of a non-newtonian fluid. Turbulent
More informationSimulating Sinkage & Trim for Planing Boat Hulls. A Fluent Dynamic Mesh 6DOF Tutorial
Simulating Sinkage & Trim for Planing Boat Hulls A Fluent Dynamic Mesh 6DOF Tutorial 1 Introduction Workshop Description This workshop describes how to perform a transient 2DOF simulation of a planing
More informationPotsdam Propeller Test Case (PPTC)
Second International Symposium on Marine Propulsors smp 11, Hamburg, Germany, June 2011 Workshop: Propeller performance Potsdam Propeller Test Case (PPTC) Olof Klerebrant Klasson 1, Tobias Huuva 2 1 Core
More 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 informationWorkshop 3: Cutcell Mesh Generation. Introduction to ANSYS Fluent Meshing Release. Release ANSYS, Inc.
Workshop 3: Cutcell Mesh Generation 14.5 Release Introduction to ANSYS Fluent Meshing 1 2011 ANSYS, Inc. December 21, 2012 I Introduction Workshop Description: CutCell meshing is a general purpose meshing
More informationTutorial: Riser Simulation Using Dense Discrete Phase Model
Introduction The purpose of this tutorial is to demonstrate the setup of a dense discrete phase model (DDPM) with the example of 2D riser. DDPM is used for the secondary phase that has a particle size
More informationA B C D E. Settings Choose height, H, free stream velocity, U, and fluid (dynamic viscosity and density ) so that: Reynolds number
Individual task Objective To derive the drag coefficient for a 2D object, defined as where D (N/m) is the aerodynamic drag force (per unit length in the third direction) acting on the object. The object
More informationOil Sloshing Simulation for No Leaking Tank Design. Wenyan Ni NACCO Materials Handling Group October 31, 2012
Oil Sloshing Simulation for No Leaking Tank Design Wenyan Ni NACCO Materials Handling Group October 31, 2012 Abstract In fork lift truck operations, hydraulic oil may leak from the air breather when hard
More informationUsing Multiple Rotating Reference Frames
Tutorial 9. Using Multiple Rotating Reference Frames Introduction Many engineering problems involve rotating flow domains. One example is the centrifugal blower unit that is typically used in automotive
More informationTutorial: Simulating a 3D Check Valve Using Dynamic Mesh 6DOF Model And Diffusion Smoothing
Tutorial: Simulating a 3D Check Valve Using Dynamic Mesh 6DOF Model And Diffusion Smoothing Introduction The purpose of this tutorial is to demonstrate how to simulate a ball check valve with small displacement
More informationSPEED-UP GEARBOX SIMULATIONS BY INTEGRATING SCORG. Dr. Christine Klier, Sahand Saheb-Jahromi, Ludwig Berger*
SPEED-UP GEARBOX SIMULATIONS BY INTEGRATING SCORG Dr. Christine Klier, Sahand Saheb-Jahromi, Ludwig Berger* CFD SCHUCK ENGINEERING Engineering Services in computational fluid Dynamics (CFD) 25 employees
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 informationSTAR Global Conference 2012 Noordwijk, March 20-21, The InDesA Virtual Test Bench. Dr. Fabiano Bet Dr. Gerald Seider
STAR Global Conference 2012 Noordwijk, March 20-21, 2012 The InDesA Dr. Fabiano Bet Dr. Gerald Seider Company Profile Consulting- & Engineering Services Simulation and Analysis of complex fluid flow and
More informationMUD DEPOSITION SIMULATION AT THE CRFM OF AN AUTOMOBILE USING CFD
Blucher Engineering Proceedings Agosto de 2014, Número 2, Volume 1 MUD DEPOSITION SIMULATION AT THE CRFM OF AN AUTOMOBILE USING CFD SIMULATION Filipe Fabian Buscariolo¹, Julio Cesar Lelis Alves², Leonardo
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 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 informationFigure 2: Water Into Kerosene, Volume Fraction (Left) And Total Density Of Mixture (Right)
Jared Bottlinger MAE598 Project 3 11/16/17 Task 1 a) Figure 1: Volume Fraction Of Water At 0.4s Task 1 b) Figure 2: Water Into Kerosene, Volume Fraction (Left) And Total Density Of Mixture (Right) Task
More informationSTAR-CCM+ v7 Workflow Process
v7refguide02_2012 STAR-CCM+ v7 Workflow Process From Geometry Creation & Import Import a surface/cad geometry File > Import Surface or Click Import, Edit or Create a New Geometry using 3D-CAD Right click
More informationTHE EFFECTS OF THE PLANFORM SHAPE ON DRAG POLAR CURVES OF WINGS: FLUID-STRUCTURE INTERACTION ANALYSES RESULTS
March 18-20, 2013 THE EFFECTS OF THE PLANFORM SHAPE ON DRAG POLAR CURVES OF WINGS: FLUID-STRUCTURE INTERACTION ANALYSES RESULTS Authors: M.R. Chiarelli, M. Ciabattari, M. Cagnoni, G. Lombardi Speaker:
More informationA Comparison of RANS-Based Turbulence Modeling for Flow over a Wall-Mounted Square Cylinder
A Comparison of RANS-Based Turbulence Modeling for Flow over a Wall-Mounted Square Cylinder P. L. Davis 1, A. T. Rinehimer 2, and M.Uddin 3 N C Motorsports and Automotive Research Center, Department of
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 informationCoupling STAR-CCM+ with Optimization Software IOSO by the example of axial 8-stages jet engine compressor.
Coupling STAR-CCM+ with Optimization Software IOSO by the example of axial 8-stages jet engine compressor. Folomeev V., (Sarov Engineering Center) Iakunin A., (JSC Klimov) 1 Objectives To create the procedure
More information