Simulations and Analysis of Fuel Flow in an Injector Including Transient Needle Effects
|
|
- Wesley Norton
- 6 years ago
- Views:
Transcription
1 ILASS-Americas 24th Annual Conference on Liquid Atomization and Spray Systems, San Antonio, TX, May 2012 Simulations and Analysis of Fuel Flow in an Injector Including Transient Needle Effects K.D. Neroorkar 1, C.E. Mitcham II 2, A.H. Plazas 3, R.O. Grover, Jr 3 and D.P. Schmidt 1 1 University of Massachusetts Amherst 2 General Motors Powertrain 3 General Motors Research and Development Abstract A fully parallelized, 3 dimensional, transient flow solver based on the Homogeneous Relaxation Model was developed for modeling and analyzing flash boiling flows in fuel injectors. This model has been validated in past work on both cavitating and flash boiling flows in real injector geometries. The ability of this model to be coupled with different fluids has also been demonstrated. The focus of the current work is to analyze the flow of diesel fuel in a 5-hole microsac injector with tapered holes. Transient needle effects are captured by providing an initial mesh, and moving the needle through mesh topological changes involving addition and deletion of mesh cell layers. The experimental needle lift profile is used to impose the needle motion, and model validation is conducted against measurements of the injected mass flow profile over the injection duration. Additionally, it is observed that the transient motion of the needle greatly influences the characteristics of the internal flow. Corresponding Author: kneroork@engin.umass.edu
2 Introduction The performance of an internal combustion engine is greatly affected by the characteristics of the fuel injection system. The highly transient nature of the flow through these systems and their small size makes these systems extremely difficult to analyze experimentally. This difficulty is further compounded by the occurrence of multiphase phenomena like cavitation in diesel and flash boiling in gasoline injectors. Hence computational fluid dynamics (CFD) is often used to model the flow through fuel injectors and to provide insight into the physical processes taking place inside these systems [1, 2, 3, 4, 5, 6]. In the past, most of the CFD analyses of fuel injectors has been limited to steady state flows assuming the needle to be fixed at a given location due to the complexity of including the moving needle. Very limited studies have been presented to analyze these transient effects. The work of Margot et al. [7] and Payri et al. [8] used a method with pure mesh motion without changing the number of cells in the domain. They used the STAR-CD solver for their flow simulations. Lee and Reitz [9] used KIVA, which uses a snapper algorithm for needle motion similar to the method presented in the current paper. In KIVA, a structured hexahedral mesh is required in the entire flow domain which significantly increases the difficulty of mesh generation when considering arbitrary shaped injectors. The current work involves using the Homogeneous Relaxation Model (HRM), which was incorporated in the OpenFOAM CFD library for analyzing the flow of diesel fuel through a 5-hole microsac injector. The HRM was originally developed for flash boiling flows in gasoline injectors. However, its applicability to diesel flow has been validated in recent publications [10, 11]. The transient needle motion is captured by addition and removal of cell layers by using OpenFOAM s dynamic mesh library. An important feature of the OpenFOAM library is its ability to be used with polyhedral meshes. Model Formulation and Numerical method The flow solver used in the current work is called HRMFoam, and its detailed formulation and numerical method is presented in past work [12, 13, 14]. For the transient needle cases, the first order upwind method was used for the divergence terms in order to increase stability, and slip walls were assumed in the nozzles to allow for a coarser mesh to reduce computation time. A steady needle simulation at 1200 bar injection and 60 bar back pressure showed a mass flow rate decrease of 5% when boundary conditions were changed from slip to no-slip. The transient cases will therefore show a slightly higher mass flow rate due to the slip-wall assumption. Additionally, laminar flow was considered as a first step to investigate the effect of the transient needle on the flow. Results and Discussions Experimental data: The 5 hole microsac geometry simulated in the current work was taken from Payri et al. [15] and Benajes et al [16] and is shown in Fig. 1. The data presented in the work of Payri et al. included two configurations as shown in the figure: without needle (data from steady state flow test rig) and with needle (data from the Injection Discharge Rate Curve Indicator (IDRCI) using the Bosch method [17]). The injector holes are tapered with a k factor of 1.5. For the case without the needle, the injection pressure was 10 and 20 MPa, and the back pressure was varied to see the effect on mass flow rate. For the case with the needle, for different injection and back pressures, the energizing time was changed from 0.25 ms to 3ms. The lower energizing times (less than 1ms) demonstrate the injection rate curve in an injection event representative of an engine. The longer energizing times produce the steady results at full needle lift. In addition to the injection rate curves, the needle lift profiles were also recorded by Payri et al. [15] by using an injector holder fitted with a needle lift sensor. These profiles were used in the current study to govern the needle motion in the injector. Steady flow results: The diesel fuel was simulated using a surrogate obtained from the work of Weber et al. [18]. The comparison of the properties of this surrogate with industrial diesels was presented in Neroorkar et al. [11], and it was found that the density and vapor pressure were within the range of the industrial diesels. However, the variability in properties of diesel from region to region implies that the properties of the surrogate may not match exactly with the diesel used in any experiments. For example, it was found that the density of the diesel used in the experiments by Payri et al. [15] was different from the surrogate s density by around 1.5%. Also, it must be noted that the steady flow results still incorporate the transient terms from the transport equations however the boundaries are stationary. For the steady flow cases, a polyhedral mesh was generated in STARCCM+ with around 225,000 cells. The Fig. 2 shows the mass flow rate comparisons for the steady flow cases with and without the needle. The experimental results for the cases with the needle represent the stable mass flow rate obtained from 2
3 (a) with needle (a) with needle (b) without needle Figure 1. Geometry of microsac injector simulated in the current study the injection rate curves for the high energizing time case (3ms). From Bernoulli s equation, for non cavitating cases, the mass flow rate should be directly proportional to the square root of pressure drop. This behavior is well represented in both experimental and simulation results for both sets of cases. However, the absolute values are different and this can be due to the difference in the fuel properties, or some minor differences in the actual hydrogrinding radius of the nozzle versus the CAD model generated. The steady state results are important because they indicate that the HRMFoam model satisfactorily reproduces the data at full needle lifts for the microsac injector which will be used for transient calculations. It must be noted that the discrepancy in the mass flow rate seen in Fig. 2 will also affect the predictions for the transient cases when at full lift. Transient needle effects: The mesh for the transient cases was generated in two parts. The first part included the needle and seat region and was composed of hexahedral cells. The second part included the sac region along with the nozzles and was a tetrahedral mesh. Both these parts were gener- (b) without needle Figure 2. Mass flow rates for steady flow cases ated in the software ICEM CFD and are shown in Fig. 3. This configuration is used for the following reasons: since the needle motion is achieved by addition/deletion of cell layers in the mesh, a layered hexahedral mesh is required around the needle, however, the extension of this hexahedral mesh into the sac and nozzle regions for a multi-hole injector is non-trivial. It is believed that the current method can be applied to arbitrary injector designs due to the lack of constraint on the nozzle/sac mesh. Once the two parts of the mesh were generated, they were connected using the generalized grid interface (GGI) feature in OpenFOAM [19] which allows the coupling of two non-conformal regions through an interface similar to the one shown in Fig. 3. The initial mesh was generated with the needle being close to the seat to represent the fully closed position. In past work by Margot et al [7] and Lee and Reitz [9], the needle had to maintain a minimum lift from the seat in order to prevent degener- 3
4 Case a b Pinj (bar) Pback (bar) Pulse width (ms) Table 1. Test cases considered for transient simulations ate cells from forming. In the current work, a minimum lift of 25 microns was assumed. The current formulation allows the needle to be moved by providing a file of time versus the required displacement from the initial position. As the needle moves, the hexahedral cell layer closest to the needle boundary gets stretched or compressed, and when the cell layer size goes outside a user-specified bound, a new cell layer is introduced or deleted adjacent to the needle. It must be noted that the mesh motion is limited to the cells at the boundary, and no motion equation is solved for the interior points in the mesh. This improves the speed of the computations by avoiding the solution of an additional equation. Secondly, the mesh motion can distort the interior mesh and increase skewness for large displacements. In the current method, a good mesh resolution can be maintained at minimum lift as well as at full lift conditions since the cell sizes will always be within the user-specified bound. However, the addition and deletion of layers leads to small localized disturbances in the flow solution which get smoothed out during consecutive time steps, and do not affect the overall solution. The transient simulations were run in parallel on 4 processors. Transient needle simulation results: Two cases were considered as shown in Table 1. The Fig. 4 shows the comparison of the mass flow rate predicted by the model with the injection rate data presented in the work by Payri et al [15]. The point to be noted from the figures is that the simulated needle lift curve flattens at around 10 % of the full lift since this is equal to the minimum lift of 25 µm assumed in this study. It is seen that for the higher energizing time case a, the mass flow rate matches the behavior of the injection rate curve for the part of the profile corresponding to the needle opening. However, it is seen that as the needle closes, the mass flow rate predicted by the model reduces faster than the experimental data which seems to have a small delay. For the smaller energizing time case b, the predictions are very different as compared to the experimental mass flow rates. This can be attributed to the fact that the minimum lift of 25 µm is almost 50 % of the peak lift of the needle for this case which is around 70 µm. Also, past analysis of the (a) Two part mesh for transient simulations (b) Close-up of sac region after assembly Figure 3. Mesh setup for transient needle cases diesel injection system by Seykens et al [20] showed that the needle lift sensor measures the movement of the needle control plunger which may not correspond to the actual movement of the needle tip due to high elastic deformation prior to injection. They reported that the initial deformation of the control plunger and needle can be as high as 36% of the total measured displacement for injection pressures of 1400bar. Additionally, it was observed that the rail pressure also deforms the control plunger and needle from the bottom during injection further affecting the measurement. In the current study, we assume that the data from the needle lift sensor directly correlates to the needle tip movement. For future studies, the method presented by Powell et al [21] which uses X-ray phase-enhanced imaging to resolve the geometry of the needle tip as it moves during an injection event would be more valid for such transient simulations. In general, it is observed that the flow is highly 4
5 (a) needle just opening, time = 0.1ms (a) Case a (b) needle at full lift, time = 0.9ms (c) needle just closed, time = 1.9ms (b) Case b Figure 5. Streamlines colored by velocity at three different times during simulation for case a Figure 4. Comparison of mass flow rate predictions with injection rate data. Dashed lines - Payri et al [15], Solid lines - Simulations M assdispersion = s transient when the needle is at low lifts. This is mainly due to the presence of a swirling flow under these conditions as can be observed from the streamlines for case a shown in Fig. 5. The swirling flow only exists at low lifts when the flow in the nozzles is affected by the fuel in the sac volume. This behavior has also been observed in past work on transient simulations [8, 9]. In case b, due to the low energizing time and low maximum needle lift, the swirling motion exists almost over the entirety of the simulation. As was mentioned earlier, one of the main advantages of the current work is the ability to simulate a full 3D injector. As a result of this, the effect of the swirling flow on the mass flow rate through each nozzle hole can be analyzed. For this, the percent dispersion of mass flow rate was calculated as follows σ= σ 100 M Σ(Mi M )2 N (1) (2) In the above equations, Mi, M and N represent the mass flow rate per hole, the average mass flow rate through all holes at a given time, and the number of nozzles respectively. The Fig. 6 shows the mass dispersion over the entire simulation for the cases a and b. It is clearly observed that the dispersion is very high when the needle is at low lifts, whereas the dispersion reduces to negligible values as the needle approaches the full lift condition for case a. However, case b shows that since the maximum needle lift achieved in this case is small, high dispersion exists over almost the entire simulation. This indicates that in case of pilot injections in engines, large 5
6 (a) Case a Figure 7. Nozzles showing asymmetric vapor formation in case a when needle is just closed, time = 1.9ms (b) Case b Figure 6. Mass dispersion between holes for the transient cases amount of flow asymmetry can be expected consequently leading to spray asymmetry. It is also observed that the cavitation behavior is very transient and asymmetric under low lift conditions as seen from Fig. 7 which shows the void fraction contour at an instant when the needle is just closed in case a. Since the nozzles are tapered in this case, the amount of cavitation is very limited. On the other hand, it is expected that cylindrical nozzles have a higher amount of cavitation and will potentially show higher transient and asymmetric hole-to-hole behavior. Finally, it is important to note that some amount of asymmetry will exist in the nozzle CAD model and mesh which will potentially drive some asymmetry in the nozzle flow. Additionally, an iterative method is used for obtaining the pressure solution which can cause overshoots and undershoots. Hence, experimental verification of the reported phenomena are required. Conclusions The homogeneous relaxation model was used for simulating the flow through a 5 hole microsac injector, and the results were compared against the experimental data of Payri et al [15]. Steady state simulations were performed for cases without the needle and with the needle fixed at full lift to verify that the model reproduces the experimental data under these conditions. In both cases, the model was able to predict the trends of the experimental results accurately. Two transient cases were simulated and the mass flow rate predictions of the model were compared against injection rate data. In general, it was found that the model captured the trend of the data for an energizing time of 1ms, however, the smaller energizing time of 0.5ms showed large discrepancies. The reason for this can be attributed to the fact that the peak needle lift achieved in this case is just about twice the initial minimum lift assumed in the current study. Future studies will try to include the effect of the minimum needle lift on the predictions. The hole to hole dispersion in mass flow rates was plotted and it was found that the highest values of dispersion existed at low needle lift and could be as high as 10 % even though the injector was symmetric. However, it must be noted that the nozzle CAD model and grid will have some inherent asymmetry which can also drive some hole-hole variations and experimental verification of this phenomena is required. Acknowledgements The authors acknowledge the financial support of General Motors for this work. References [1] F.J. Salvador, S. Hoyas, R. Novella, and J. Martínez-López. Proceedings of the Institu- 6
7 tion of Mechanical Engineers, Part D: Journal of Automobile Engineering, 225: , [2] E. Giannadakis, D. Papoulias, M. Gavaises, C. Arcoumanis, C. Soteriou, and W. Tang. SAE Paper , [3] S Som, S.K. Aggarwal, E.M. El-Hannouny, and D.E. Longman. Journal of Engineering for Gas Turbines and Power, 132(4), [4] F. Peng Kärrholm, Henry Weller, and Niklas Nordin. ASME Conference Proceedings, 2007(42894): , [5] W. Yuan and G.H. Schnerr. Proc. CAV2001: Fourth Intl Symp. Cavitation, Pasadena, CA, [18] J. Weber, N. Peters, R. Diwakar, R.M. Siewert, and A. Lippert. SAE Paper , [19] M. Beaudoin and H. Jasak. Open Source CFD International Conference, Berlin, Germany, [20] X.L.J. Seykens, Somers L.M.T., and R.S.G. Baert. MECCA, III:30 39, [21] C.F. Powell, A.L. Kastengren, Z. Liu, and K. Fezzaa. Journal of Engineering for Gas Turbines and Power, 133, [6] A. Alajbegovic, G. Meister, D. Greif, and B. Basara. Experimental Thermal and Fluid Science, 26(6-7): , [7] X. Margot, S. Hoyas, P. Fajardo, and S. Patouna. Mathematical and Computer Modelling, 52: , [8] F. Payri, X. Margot, S. Patouna, F. Ravet, and M. Funk. SAE Paper , [9] W.G. Lee and R.D. Reitz. Journal of Engineering for Gas Turbines and Power, 132, [10] B. Shields, K. Neroorkar, and D.P. Schmidt. 23rd Annual Conference on Liquid Atomization and Spray Systems, Ventura, CA, May 2011, [11] K. Neroorkar, B. Shields, R.O. Grover jr, A.H. Plazas, and D. P. Schmidt. SAE Paper , [12] S. Gopalakrishnan and D.P. Schmidt. SAE Paper , [13] D.P. Schmidt, S. Gopalakrishnan, and H. Jasak. Intl. J. of Multiphase Flow, 36: , [14] K. Neroorkar, S. Gopalakrishnan, D. Schmidt, and R. O. Grover Jr. Atomization and Sprays, 21(2): , [15] R. Payri, A. Gil, A.H. Plazas, and B Giménez. SAE Paper , [16] J. Benajes, J.V. Pastor, R. Payri, and A.H. Plazas. Journal of Fluids Engineering, 126, [17] W. Bosch. SAE Tech. Paper ,
CFD 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 informationA Generalized Adaptive Collision Mesh for Multiple Injector Orifices
A Generalized Adaptive Collision Mesh for Multiple Injector Orifices Shuhai Hou, Sasanka Are, David P. Schmidt University of Massachusetts-Amherst ABSTRACT An algorithm for creating a generalized adaptive
More 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 information*Sebastian Hensel, Kai Herrmann, Reiner Schulz and German Weisser
Paper templeate (for draft and final papers) Numerical analysis and statistical description of the primary breakup in fuel nozzles of large two stroke engines for the application in CFD engine simulations
More informationURANS and SAS analysis of flow dynamics in a GDI nozzle
, 3rd Annual Conference on Liquid Atomization and Spray Systems, Brno, Czech Republic, September 010 J.-M. Shi*, K. Wenzlawski*, J. Helie, H. Nuglisch, J. Cousin * Continental Automotive GmbH Siemensstr.
More informationAuto Injector Syringe. A Fluent Dynamic Mesh 1DOF Tutorial
Auto Injector Syringe A Fluent Dynamic Mesh 1DOF Tutorial 1 2015 ANSYS, Inc. June 26, 2015 Prerequisites This tutorial is written with the assumption that You have attended the Introduction to ANSYS Fluent
More informationThank you for downloading one of our ANSYS whitepapers we hope you enjoy it.
Thank you! Thank you for downloading one of our ANSYS whitepapers we hope you enjoy it. Have questions? Need more information? Please don t hesitate to contact us! We have plenty more where this came from.
More informationNumerical Spray Calibration Process. ANSYS Inc. Pune, India. Laz Foley. ANSYS Inc. Evanston, IL
ILASS Americas, 23 rd Annual Conference on Liquid Atomization and Spray Systems, Ventura, CA, May 2011 Numerical Spray Calibration Process Padmesh Mandloi *,Jayesh Mutyal, Pravin Rajeshirke ANSYS Inc.
More 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 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 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 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 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 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 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 informationICE Roadmap Japanese STAR Conference. Richard Johns
ICE Roadmap Japanese STAR Conference Richard Johns Introduction Top-Level Roadmap STAR-CCM+ and Internal Combustion Engines Modeling Improvements and Research Support Sprays LES Chemistry Meshing Summary
More informationAurélien Thinat Stéphane Cordier 1, François Cany
SimHydro 2012:New trends in simulation - Hydroinformatics and 3D modeling, 12-14 September 2012, Nice Aurélien Thinat, Stéphane Cordier, François Cany Application of OpenFOAM to the study of wave loads
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 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 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 informationMesh Morphing and the Adjoint Solver in ANSYS R14.0. Simon Pereira Laz Foley
Mesh Morphing and the Adjoint Solver in ANSYS R14.0 Simon Pereira Laz Foley 1 Agenda Fluent Morphing-Optimization Feature RBF Morph with ANSYS DesignXplorer Adjoint Solver What does an adjoint solver do,
More informationOptimization of under-relaxation factors. and Courant numbers for the simulation of. sloshing in the oil pan of an automobile
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,
More informationCFD Simulation of Cavitation in an Internal Gear Pump
CFD Simulation of Cavitation in an Internal Gear Pump Dr. Andreas Spille-Kohoff Jan Hesse CFX Berlin Software GmbH Berlin andreas.spille@cfx-berlin.de Contents Introduction Geometry and mesh Simulation
More informationWebinar: TwinMesh for Reliable CFD Analysis of Rotating Positive Displacement Machines
Webinar: TwinMesh for Reliable CFD Analysis of Rotating Positive Displacement Machines 14.07.2015 Dipl.-Ing. Jan Hesse Jan.hesse@cfx-berlin.de CFX Berlin Software GmbH Karl-Marx-Allee 90 A 10243 Berlin
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 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 informationDeveloping LES Models for IC Engine Simulations. June 14-15, 2017 Madison, WI
Developing LES Models for IC Engine Simulations June 14-15, 2017 Madison, WI 1 2 RANS vs LES Both approaches use the same equation: u i u i u j 1 P 1 u i t x x x x j i j T j The only difference is turbulent
More 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 informationApplications of ICFD /SPH Solvers by LS-DYNA to Solve Water Splashing Impact to Automobile Body. Abstract
Applications of ICFD /SPH Solvers by LS-DYNA to Solve Water Splashing Impact to Automobile Body George Wang (1 ), Kevin Gardner (3), Eric DeHoff (1), Facundo del Pin (2), Inaki Caldichoury (2), Edouard
More informationMarine Hydrodynamics Solver in OpenFOAM
Marine Hydrodynamics Solver in OpenFOAM p. 1/14 Marine Hydrodynamics Solver in OpenFOAM Hrvoje Jasak and Henrik Rusche h.jasak@wikki.co.uk, h.rusche@wikki.co.uk Wikki, United Kingdom and Germany 4 December
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 informationAshwin Shridhar et al. Int. Journal of Engineering Research and Applications ISSN : , Vol. 5, Issue 6, ( Part - 5) June 2015, pp.
RESEARCH ARTICLE OPEN ACCESS Conjugate Heat transfer Analysis of helical fins with airfoil crosssection and its comparison with existing circular fin design for air cooled engines employing constant rectangular
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 informationExtension and Validation of the CFX Cavitation Model for Sheet and Tip Vortex Cavitation on Hydrofoils
Extension and Validation of the CFX Cavitation Model for Sheet and Tip Vortex Cavitation on Hydrofoils C. Lifante, T. Frank, M. Kuntz ANSYS Germany, 83624 Otterfing Conxita.Lifante@ansys.com 2006 ANSYS,
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 informationKEY STAR TECHNOLOGIES: DISPERSED MULTIPHASE FLOW AND LIQUID FILM MODELLING DAVID GOSMAN EXEC VP TECHNOLOGY, CD-adapco
KEY STAR TECHNOLOGIES: DISPERSED MULTIPHASE FLOW AND LIQUID FILM MODELLING DAVID GOSMAN EXEC VP TECHNOLOGY, CD-adapco INTRODUCTION KEY METHODOLOGIES AVAILABLE IN STAR-CCM+ AND STAR-CD 1. Lagrangian modelling
More 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 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 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 informationApplying a new dispersion model to turbulent premixed flames
Applying a new dispersion model to turbulent premixed flames Federico Ghirelli Fifth OpenFOAM Workshop Gothenburg, 21 24 June 2010 Point source in steady homogeneous turbulence Fundamental experiment:
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 informationTurbulent Premixed Combustion with Flamelet Generated Manifolds in COMSOL Multiphysics
Turbulent Premixed Combustion with Flamelet Generated Manifolds in COMSOL Multiphysics Rob J.M Bastiaans* Eindhoven University of Technology *Corresponding author: PO box 512, 5600 MB, Eindhoven, r.j.m.bastiaans@tue.nl
More informationValidation of an Automatic Mesh Generation Technique in Engine Simulations
International Multidimensional Engine Modeling User's Group Meeting April,, Detroit, Michigan Validation of an Automatic Mesh Generation Technique in Engine s Abstract Long Liang, Anthony Shelburn, Cheng
More 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 informationInfluence of mesh quality and density on numerical calculation of heat exchanger with undulation in herringbone pattern
Influence of mesh quality and density on numerical calculation of heat exchanger with undulation in herringbone pattern Václav Dvořák, Jan Novosád Abstract Research of devices for heat recovery is currently
More informationImplementation of Transport Model into CavitatingFoam to simulate the Cavitation in Diesel Injector Nozzle
Implementation of Transport Model into CavitatingFoam to simulate the Cavitation in Diesel Injector Nozzle Barış BİÇER Energy and Fluid Science Lab. Graduate School of Maritime Sciences, Kobe University,
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 informationThis tutorial illustrates how to set up and solve a problem involving solidification. This tutorial will demonstrate how to do the following:
Tutorial 22. Modeling Solidification Introduction This tutorial illustrates how to set up and solve a problem involving solidification. This tutorial will demonstrate how to do the following: Define a
More informationThe Spalart Allmaras turbulence model
The Spalart Allmaras turbulence model The main equation The Spallart Allmaras turbulence model is a one equation model designed especially for aerospace applications; it solves a modelled transport equation
More informationProgram: Advanced Certificate Program
Program: Advanced Certificate Program Course: CFD-Vehicle Aerodynamics Directorate of Training and Lifelong Learning #470-P, Peenya Industrial Area, 4th Phase Peenya, Bengaluru 560 058 www.msruas.ac.in
More 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 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 informationApplying Solution-Adaptive Mesh Refinement in Engine Simulations
International Multidimensional Engine Modeling User's Group Meeting April 11, 2016, Detroit, Michigan Applying Solution-Adaptive Mesh Refinement in Engine Simulations Long Liang, Yue Wang, Anthony Shelburn,
More 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 informationObject-Oriented CFD Solver Design
Object-Oriented CFD Solver Design Hrvoje Jasak h.jasak@wikki.co.uk Wikki Ltd. United Kingdom 10/Mar2005 Object-Oriented CFD Solver Design p.1/29 Outline Objective Present new approach to software design
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 informationDevelopment of an Integrated Computational Simulation Method for Fluid Driven Structure Movement and Acoustics
Development of an Integrated Computational Simulation Method for Fluid Driven Structure Movement and Acoustics I. Pantle Fachgebiet Strömungsmaschinen Karlsruher Institut für Technologie KIT Motivation
More informationLab 9: FLUENT: Transient Natural Convection Between Concentric Cylinders
Lab 9: FLUENT: Transient Natural Convection Between Concentric Cylinders Objective: The objective of this laboratory is to introduce how to use FLUENT to solve both transient and natural convection problems.
More 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 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 informationCFD Modeling of a Radiator Axial Fan for Air Flow Distribution
CFD Modeling of a Radiator Axial Fan for Air Flow Distribution S. Jain, and Y. Deshpande Abstract The fluid mechanics principle is used extensively in designing axial flow fans and their associated equipment.
More informationAnalysis Comparison between CFD and FEA of an Idealized Concept V- Hull Floor Configuration in Two Dimensions
2010 NDIA GROUND VEHICLE SYSTEMS ENGINEERING AND TECHNOLOGY SYMPOSIUM MODELING & SIMULATION, TESTING AND VALIDATION (MSTV) MINI-SYMPOSIUM AUGUST 17-19 DEARBORN, MICHIGAN Analysis Comparison between CFD
More informationCFD grid generation and analysis of screw compressor with variable geometry rotors
CFD grid generation and analysis of screw compressor with variable geometry rotors S Rane, A Kovacevic, N Stosic, M Kethidi City University London, Centre for Positive Displacement Compressor Technology,
More informationAn Investigation on the Geometric Effects of a Vertical-Downward Elbow on Two-Phase Flow
An Investigation on the Geometric Effects of a Vertical-Downward Elbow on Two-Phase Flow Philip Graybill Grove City College Mechanical Engineering Andrew Hardison Robert Morris University Mechanical Engineering
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 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 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 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 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 informationLaser speckle based background oriented schlieren measurements in a fire backlayering front
Laser speckle based background oriented schlieren measurements in a fire backlayering front Philipp Bühlmann 1*, Alexander H. Meier 1, Martin Ehrensperger 1, Thomas Rösgen 1 1: ETH Zürich, Institute of
More informationSimulation of Fuel Sloshing Comparative Study
3. LS-DYNA Anwenderforum, Bamberg 2004 Netfreie Verfahren Simulation of Fuel Sloshing Comparative Study Matej Vesenjak 1, Heiner Müllerschön 2, Alexander Hummel 3, Zoran Ren 1 1 University of Maribor,
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 informationFLUENT Secondary flow in a teacup Author: John M. Cimbala, Penn State University Latest revision: 26 January 2016
FLUENT Secondary flow in a teacup Author: John M. Cimbala, Penn State University Latest revision: 26 January 2016 Note: These instructions are based on an older version of FLUENT, and some of the instructions
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 informationTHERMAL OPTIMIZATION OF GENSET CANOPY USING CFD
International Journal of Mechanical and Production Engineering Research and Development (IJMPERD) ISSN(P): 2249-6890; ISSN(E): 2249-8001 Vol. 5, Issue 3, Jun 2015, 19-26 TJPRC Pvt. Ltd. THERMAL OPTIMIZATION
More informationApplication of Finite Volume Method for Structural Analysis
Application of Finite Volume Method for Structural Analysis Saeed-Reza Sabbagh-Yazdi and Milad Bayatlou Associate Professor, Civil Engineering Department of KNToosi University of Technology, PostGraduate
More informationSIMULATION OF FLOW FIELD AROUND AND INSIDE SCOUR PROTECTION WITH PHYSICAL AND REALISTIC PARTICLE CONFIGURATIONS
XIX International Conference on Water Resources CMWR 2012 University of Illinois at Urbana-Champaign June 17-22, 2012 SIMULATION OF FLOW FIELD AROUND AND INSIDE SCOUR PROTECTION WITH PHYSICAL AND REALISTIC
More informationEulerian Modeling of Fully-Coupled Diesel Injector Flow and Spray MA, 01002, USA
ILASS Americas th Annual Conference on Liquid Atomization and Spray Systems, Portland, OR, May Eulerian Modeling of Fully-Coupled Diesel Injector Flow and Spray Q. Xue, M. Battistoni, S.P. Quan, P. K.
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 steady-state Eulerian-Lagrangian solver for non-reactive sprays
ICLASS 212, 12 th Triennial International Conference on Liquid Atomization and Spray Systems, Heidelberg, Germany, September 2-6, 212 A steady-state Eulerian-Lagrangian solver for non-reactive sprays A.
More informationApplication of a FEA Model for Conformability Calculation of Tip Seal in Compressor
Purdue University Purdue e-pubs International Compressor Engineering Conference School of Mechanical Engineering 2008 Application of a FEA Model for Conformability Calculation of Tip Seal in Compressor
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 informationFOUR WHAT S NEW IN THIS VERSION? 4.1 FLOW-3D Usability CHAPTER
CHAPTER FOUR WHAT S NEW IN THIS VERSION? FLOW-3D v11.2.0 continues to streamline engineers simulation workflows by enabling them to more quickly set up simulations, avoid common errors, identify and enter
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 informationUse of STAR-CCM+ in Marine and Off-Shore Engineering - Key Features and Future Developments - M. Perić, F. Schäfer, E. Schreck & J.
Use of STAR-CCM+ in Marine and Off-Shore Engineering - Key Features and Future Developments - M. Perić, F. Schäfer, E. Schreck & J. Singh Contents Main features of STAR-CCM+ relevant for marine and offshore
More informationLATTICE-BOLTZMANN METHOD FOR THE SIMULATION OF LAMINAR MIXERS
14 th European Conference on Mixing Warszawa, 10-13 September 2012 LATTICE-BOLTZMANN METHOD FOR THE SIMULATION OF LAMINAR MIXERS Felix Muggli a, Laurent Chatagny a, Jonas Lätt b a Sulzer Markets & Technology
More informationCOMPUTATIONAL FLUID DYNAMICS USED IN THE DESIGN OF WATERBLAST TOOLING
2015 WJTA-IMCA Conference and Expo November 2-4 New Orleans, Louisiana Paper COMPUTATIONAL FLUID DYNAMICS USED IN THE DESIGN OF WATERBLAST TOOLING J. Schneider StoneAge, Inc. Durango, Colorado, U.S.A.
More informationInfluence of geometric imperfections on tapered roller bearings life and performance
Influence of geometric imperfections on tapered roller bearings life and performance Rodríguez R a, Calvo S a, Nadal I b and Santo Domingo S c a Computational Simulation Centre, Instituto Tecnológico de
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 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 informationModelling of Impact on a Fuel Tank Using Smoothed Particle Hydrodynamics
Modelling of Impact on a Fuel Tank Using Smoothed Particle Hydrodynamics R. Vignjevic a, T. De Vuyst a, J. Campbell a, N. Bourne b School of Engineering, Cranfield University, Bedfordshire, MK43 0AL, UK.
More informationNumerische Untersuchungen von Windkraftanlagen: Leistung, Wake und Steuerungsstrategien
Fachtagung Lasermethoden in der Strömungsmesstechnik 8. 10. September 2015, Dresden Numerische Untersuchungen von Windkraftanlagen: Leistung, Wake und Steuerungsstrategien Numerical Investigations of Wind
More informationFree Surface Flow Simulations
Free Surface Flow Simulations Hrvoje Jasak h.jasak@wikki.co.uk Wikki Ltd. United Kingdom 11/Jan/2005 Free Surface Flow Simulations p.1/26 Outline Objective Present two numerical modelling approaches for
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 informationCHAPTER 1. Introduction
ME 475: Computer-Aided Design of Structures 1-1 CHAPTER 1 Introduction 1.1 Analysis versus Design 1.2 Basic Steps in Analysis 1.3 What is the Finite Element Method? 1.4 Geometrical Representation, Discretization
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 informationPressure Drop Evaluation in a Pilot Plant Hydrocyclone
Pressure Drop Evaluation in a Pilot Plant Hydrocyclone Fabio Kasper, M.Sc. Emilio Paladino, D.Sc. Marcus Reis, M.Sc. ESSS Carlos A. Capela Moraes, D.Sc. Dárley C. Melo, M.Sc. Petrobras Research Center
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 informationSimulations of the vortex in the Dellenback abrupt expansion, resembling a hydro turbine draft tube operating at part-load
Simulations of the vortex in the Dellenback abrupt expansion, resembling a hydro turbine draft tube operating at part-load H Nilsson Chalmers University of Technology, SE-412 96 Gothenburg, Sweden E-mail:
More informationAnalysis of Flow through a Drip Irrigation Emitter
International OPEN ACCESS Journal Of Modern Engineering Research (IJMER) Analysis of Flow through a Drip Irrigation Emitter Reethi K 1, Mallikarjuna 2, Vijaya Raghu B 3 1 (B.E Scholar, Mechanical Engineering,
More information