Comparison of implicit and explicit nite element methods for dynamic problems
|
|
- Bruce Roberts
- 5 years ago
- Views:
Transcription
1 Journal of Materials Processing Technology 105 (2000) 110±118 Comparison of implicit and explicit nite element methods for dynamic problems J.S. Sun, K.H. Lee, H.P. Lee * Department of Mechanical and Production Engineering, National University of Singapore, 10 Kent Ridge Crescent, Singapore , Singapore Received 15 April 1999 Abstract The nite element software ABAQUS offers several algorithms for dynamic analysis. The direct integration methods include the implicit and the explicit methods which can be used for linear and nonlinear problems. The performance of these two methods are compared for several dynamic problems including the impact of an elastic bar and a cylindrical disk on a rigid wall. The advantages of the implicit method for small wavefront problems and the explicit method for short transient problems are veri ed. # 2000 Elsevier Science S.A. All rights reserved. Keywords: Implicit nite element method; Explicit nite element method; Dynamic problems 1. Introduction The nite element method (FEM) has become the most popular method in both research and industrial numerical simulations. Several algorithms, with different computational costs, are implemented in the nite element codes, ABAQUS [1], which is a commonly used software for nite element analysis. Understanding the nature, advantages and disadvantages of these algorithms is very helpful for choosing the right algorithm for a particular problem. Comparison of implicit and explicit methods for ABA- QUS in nonlinear problems has been reported by ReBelo et al. [2]. The unconditionally stable implicit method will encounter some dif culties when a complicated threedimensional model is considered. The reasons are as follows: (i) as the reduction of the time increment continues, the computational cost in the tangent stiffness matrix is dramatically increased and even causes divergence; (ii) local instabilities cause force equilibrium to be dif cult to achieve. The explicit techniques are thus introduced to overcome the disadvantages of the implicit method [3]. For the explicit method, the CPU cost is approximately proportional to the size of the nite element model and does not change as dramatically as the implicit method. * Corresponding author. Tel.: ; fax: address: mpeleehp@nus.edu.sg (H.P. Lee). The drawback of the explicit method is that it is conditionally stable. The stability limit for an explicit operator is that the maximum time increment must be less than a critical value of the smallest transition times for a dilatational wave to cross any element in the mesh. Secondly, the nature of the explicit method limits it to the analysis of short transient problems. If this method is used for quasi-static problems, the inertia effects must be small enough to be neglected. One way to assure this is to set the limit on the kinematic energy to be less than 5% of the strain energy. Another limit is that only the rst-order, displacement methods elements (four-node quadrilaterals, eight-node bricks, etc.) are available for the present version. For dynamic problems, ABAQUS also offers some other methods such as a modal dynamic algorithm. However, only direct integration methods Ð implicit dynamics and explicit methods Ð are suitable for nonlinear problems. Most of the reported works on the comparison of implicit and explicit methods are on quasi-static nonlinear problems [2,3]. In this paper, attention is paid to comparison of the implicit and the explicit method for linear dynamic problems. 2. Solution procedures The implicit procedure uses an automatic increment strategy based on the success rate of a full Newton iterative /00/$ ± see front matter # 2000 Elsevier Science S.A. All rights reserved. PII: S (00)00580-X
2 J.S. Sun et al. / Journal of Materials Processing Technology 105 (2000) 110± solution method: Du i 1 ˆ Du i K 1 t F i I i (1) where K t is the current tangent stiffness matrix, F the applied load vector, I the internal force vector, and Du is the increment of displacement. For an implicit dynamic procedure, the algorithm is de ned by Hilber et al. [4,5]: Mu i 1 1 a Ku i 1 aku i ˆ F i 1 (2) where M is the mass matrix, K the stiffness matrix, F the vector of applied loads and u the displacement vector: u i 1 ˆ u i Dt _u i Dt b u i bu i 1 (3) and _u i 1 ˆ _u i Dt 1 g u i gu i 1 (4) with b ˆ a2 ; g ˆ 1 2 a; 1 3 a 0 (5) a ˆ 0:05 is chosen by default in ABAQUS as a small damping term to quickly remove the high frequency noise without having a signi cant effect on the meaningful, lower frequency response. The explicit procedure is based on the implementation of an explicit integration rule along with the use of diagonal element mass matrices. The equation of motion for the body is integrated using an explicit central difference integration rule: u i 1 ˆ u i Dt i 1 _u i 1 ; _u i 1=2 ˆ _u i 1=2 1 2 Dt i 1 Dt i u i where _u is the velocity, u the acceleration, and i and i 1 2, i 1 2 refer to the increment number and mid-increment numbers. u i ˆ M 1 F i I i (6) where M is the mass ``lumped'' matrix, F the applied load vector and I the internal force vector. As mentioned above, the explicit integration operator is conditionally stable, so that the time increments must satisfy Dt 2 o max where o max is the element maximum eigenvalue. A conservative estimate of the stable time increment is given by the minimum value for all elements. The above stability limit can be written as Dt ˆ min L e c d where L e is the characteristic element dimension and c d the current effective, dilatational wave speed of the material. 3. Example problems 3.1. Impact of an elastic bar against a rigid wall As the rst example, the impact of an elastic bar against a rigid wall is presented. This model is used to compare the results by ABAQUS and the reported results by Zhong [6]. The dimensions of the bar are m 3. Young's modulus is given as Eˆ100 kpa. Possion's ratio is n ˆ 0, and the mass density is r ˆ 0:001 kg m 3. Eighty C3D8 and C3D8R (eight-node bricks) elements are used for the implicit and explicit methods, respectively. An initial velocity of 1 m s 1 is prescribed to the bar striking the rigid wall. The elements of the rigid wall are R3D4. The mesh is shown in Fig. 1. The impact time can be simply estimated by Dt ˆ 2L c where L is the length of the bar, and c the wave speed for this kind p of material, which is determined by E=r ˆ 2: ms 1. For the implicit method, the half-step residual tolerance HAFTOL is a very important parameter to control the computational accuracy [1]. A large value of 10 is set initially. In Fig. 2a, the contact reaction forces are compared. Fig. 1. Mesh of the bar.
3 Fig. 2. (a) Contact reaction force RF1 with HAFTOLˆ10; (b) the stress component S11 with HAFTOLˆ10; (c) contact reaction force RF1 with HAFTOLˆ1; (d) the stress component S11 with HAFTOLˆ J.S. Sun et al. / Journal of Materials Processing Technology 105 (2000) 110±118
4 J.S. Sun et al. / Journal of Materials Processing Technology 105 (2000) 110± Fig. 3. Mesh of the cylindrical disk. It only takes 19 steps and less than 1 s CPU time for the explicit method, while it takes 106 s of CPU time for the implicit method. However, under this condition, the accuracy of the results by the explicit method is better than that by the implicit method. Fig. 2b shows the stress component S11. The values of S11 by the implicit method are found to oscillate much more than the corresponding results by the explicit method. From Fig. 2a, the reaction force is found to be about 10 N. In order to secure more accurate results, 10% of the reaction force, 1.0, is set as the revised HAFTOL value. The reaction force and S11 are shown in Figs. 2c and d. The values of S11 by the implicit methods still oscillate more than those by the explicit method, but both the stresses and reaction force oscillate less than the corresponding results for the previous case with HAFTOLˆ10. The CPU time for the implicit method signi cantly increases, from 106 to 524 s. The periods of the FEM deviate from that of the exact solution. As mentioned above, a is set to 0:05 for the implicit method to induce arti cial damping. The numerical dissipation leads to an amplitude decay of 2px [5], where x is the algorithmic damping ratio. This is illustrated in Figs. 2a and c. analyze and predict failure. Comparing the stresses by these two methods is helpful for failure diagnosis. A three-dimensional example is needed for the above purpose. This example is shown in Fig. 3. A cylindrical disk is formed by two cylinders. The radius of the bottom cylinder is 1 m, and the radius of the top cylinder is 0.25 m. The bottom cylinder is of 0.5 m height, and the height of the top one is 0.1 m. The distance between the centers of these two cylinders is 0.31 m. There are 548 eightnode brick elements and 810 nodes for the mesh. Elements 173 and 409 are chosen for the purpose of stress comparison. Nodes 311 and 709 are one of the eight nodes for elements 173 and 409, respectively. The material is ductile steel with a Young's modulus of E ˆ 200 GPa and density of r ˆ 7833 kg m 3. Poisson's ration is taken to be n ˆ 0 in order that the stresses can be simply calculated by s i;j ˆ E i ; i; j ˆ 1; 3 (7) 3.2. Impact of an elastic cylindrical disk against a rigid wall In the rst example, the results for the displacement by both the implicit and explicit method in direction 1 agree very well with the initial velocity in direction 1, which is used to control the movement of the bar. Moreover, the displacements in the other two directions are very small. Actually, this example cannot show the effects of these two methods on the displacements of the other two directions and subsequent effects on the stress distribution. In engineering applications, stress analysis is usually important to Fig. 4. The maximum principal stress SP3 for static contact.
5 114 J.S. Sun et al. / Journal of Materials Processing Technology 105 (2000) 110±118 Fig. 5. (a) The contact reaction force RF2; (b) the displacement component U1 of node 311; (c) the displacement component U2 of node 311; (d) the stress component S11 of element 173; (e) the stress component S22 of element 173; (f) the stress component S33 of element 173.
6 J.S. Sun et al. / Journal of Materials Processing Technology 105 (2000) 110± Fig. 5. (Continued ).
7 116 J.S. Sun et al. / Journal of Materials Processing Technology 105 (2000) 110±118 Fig. 6. (a) The displacement U3 by explicit; (b) the displacement U3 by implicit. in which s i;j are the six independent components of stress, u i are the three components of displacement, and x j are the three coordinates. The maximum principal stresses (SP3) by the static algorithm are shown in Fig. 4. The original gap between the model and the rigid wall is 0.01 m. A static displacement of 0.02 m is applied on the bottom surface of the large cylinder. An initial velocity of 10 m s 1 is prescribed. Fig. 5a shows the agreement of the contact reaction force RF2 for the results by the two methods. The displacements U1, U2 and U3 of node 311 are shown in Figs. 5a±c. U3 shows a large difference, but the absolute value of U3 for node 311 is relatively small because node 311 is on the axisymmetric axis. Due to the fact that the displacement of the rigid body in direction 2 is comparatively large relative to the deformation, U2 shows an insigni cant change, but Figs. 5d±f show apparent differences of stresses of element 173 by these two methods. Although at some region such as node 331, the values of U3 are quite different for the two methods, the whole displacement pattern of U3 is similar, as shown in Figs. 6a and b. On the other hand, the stress components S11, S22 and S33 of another element 409 which connects to the contact surface, show agreement by the two methods in Figs. 7a±c. Displacements have higher accuracy than stresses, thus the three displacements U1, U2 and U3 of node 709 obviously agree. The results are testi ed in Figs. 6a and b. For stress distribution, the regularity is the same. Figs. 7d and e show that the pattern of stress distribution is similar for most regions, especially at regions where the stresses are compressive and the absolute values are large. This is a compressive model, the absolute values of tensile stresses being much smaller than the compressive stresses. The differences shown in Figs. 7d and e are all in the region of tensile stresses. For this fast impact problem, the total time is usually very short, the computational cost of the explicit begin about one tenth that of the implicit Slow contact between an elastic cylindrical disk and a rigid wall The displacement for the bottom surface of the elastic cylindrical disk is set to be 0.02 m. The total time is 1 s, which is much larger than in the fast case (0.002 s). Fig. 8a shows the displacement U2 of node 311, whilst Fig. 8b shows the stress component S22 of element 173: differences are apparent. Fig. 8b shows the stress component S22 of element 409. The results show good agreement. Figs. 8c and d compare the maximum principal stress SP3. The regularities are the same as mentioned in the last section. The perfect agreement between Fig. 8c and Figs. 6a and b show that the results by implicit methods are very accurate, where under these conditions inertia effects can be neglected. The stable time step for explicit is s for the slow case and 8: s for the fast case. For the slow case, the time increment is much more than that of the fast case. Thus the CPU cost increases dramatically from 7 min to 1 h 17 min. The CPU cost for the implicit method is 10 min. 4. Closure Fast and slow linear contact problems have been analyzed by different methods in ABAQUS. For the fast case, the advantages of the explicit method are apparent within the desirable tolerance. The cost of the explicit method is much less than that of the implicit method. Due to numerical damping, amplitude decay is observed for the implicit method. For the slow case, the solutions are more unstable because high frequency numerical noise becomes more important. The numerical damping induced in the implicit method shows its function to remove the noise and keep the results more accurate. Because the explicit method is conditionally stable, the stable time period is much smaller than that of the
8 J.S. Sun et al. / Journal of Materials Processing Technology 105 (2000) 110± Fig. 7. (a) The stress component S11 of element 409; (b) the stress component S22 of element 409; (c) the stress component S33 of element 409; (d) the maximum principal stress SP3 of the impacting disk by explicit; (e) the maximum principal stress SP3 of the impacting disk by implicit.
9 118 J.S. Sun et al. / Journal of Materials Processing Technology 105 (2000) 110±118 Fig. 8. (Continued ). implicit method. If the whole procedure is very long, it takes many time increments for the explicit method. Thus the advantages of the implicit method are obvious for the slow contact problem. References Fig. 8. (a) The displacement U2 of node 311; (b) the stress component S22 of element 173; (c) the stress component S22 of element 409; (d) the maximum principal stress (SP3) of the slow contact disk by explicit; (e) the maximum principal stress (SP3) of the slow contact disk by implicit. [1] ABAQUS User's Examples and Theory Manual, Version 5.7. Hibbitt, Karlsson & Sorensen Inc., [2] N. Rebelo, J.C. Nagtegaal, L.M. Taylor, Comparison of implicit and explicit nite element methods in the simulation of metal forming processes, in: Chenot, Wood, Zienkiewicz (Eds.), Numerical Methods in Industrial Forming Processes, 1992, pp. 99±108. [3] Hibbitt, Karlsson & Sorensen Inc., Application of implicit and explicit nite element techniques to metal forming, J. Mater. Process. Technol. 45 (1994) 649±656. [4] H.M. Hilber, T.J.R. Hughes, Collocation, dissipation and `overshoot' for time integration schemes in structural dynamics, Earthquake Eng. Struct. Dyn. 6 (1978) 99±117. [5] T.J.R. Hughes, The Finite Element Method Ð Linear Static and Dynamic Finite Element Analysis, Prentice-Hall, Englewood Cliffs, NJ, 07632, [6] Z.H. Zhong, Finite Element Procedures for Contact Ð Impact Problems, Oxford University Press, New York, 1993.
Example 24 Spring-back
Example 24 Spring-back Summary The spring-back simulation of sheet metal bent into a hat-shape is studied. The problem is one of the famous tests from the Numisheet 93. As spring-back is generally a quasi-static
More informationcourse outline basic principles of numerical analysis, intro FEM
idealization, equilibrium, solutions, interpretation of results types of numerical engineering problems continuous vs discrete systems direct stiffness approach differential & variational formulation introduction
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 informationAnalysis of Fluid-Structure Interaction Effects of Liquid-Filled Container under Drop Testing
Kasetsart J. (Nat. Sci.) 42 : 165-176 (2008) Analysis of Fluid-Structure Interaction Effects of Liquid-Filled Container under Drop Testing Chakrit Suvanjumrat*, Tumrong Puttapitukporn and Satjarthip Thusneyapan
More informationES 128: Computer Assignment #4. Due in class on Monday, 12 April 2010
ES 128: Computer Assignment #4 Due in class on Monday, 12 April 2010 Task 1. Study an elastic-plastic indentation problem. This problem combines plasticity with contact mechanics and has many rich aspects.
More informationTransactions on Information and Communications Technologies vol 15, 1997 WIT Press, ISSN
Optimization of time dependent adaptive finite element methods K.-H. Elmer Curt-Risch-Institut, Universitat Hannover Appelstr. 9a, D-30167 Hannover, Germany Abstract To obtain reliable numerical solutions
More informationStudy on Shaking Table Test and Simulation Analysis of Graphite Dowel-Socket Structure
Study on Shaking Table Test and Simulation Analysis of Graphite Dowel-Socket Structure Xiangxiong Kong, Tiehua Shi & Shaoge Cheng Institute of Earthquake Engineering, China Academy of Building Research,
More informationUser-defined elements, Section of the Abaqus Analysis User's Manual
1.1.22 UEL User subroutine to define an element. Product: Abaqus/Standard References Overview Warning: This feature is intended for advanced users only. Its use in all but the simplest test examples will
More information17. SEISMIC ANALYSIS MODELING TO SATISFY BUILDING CODES
17. SEISMIC ANALYSIS MODELING TO SATISFY BUILDING CODES The Current Building Codes Use the Terminology: Principal Direction without a Unique Definition 17.1 INTRODUCTION { XE "Building Codes" }Currently
More informationRecent Advances on Higher Order 27-node Hexahedral Element in LS-DYNA
14 th International LS-DYNA Users Conference Session: Simulation Recent Advances on Higher Order 27-node Hexahedral Element in LS-DYNA Hailong Teng Livermore Software Technology Corp. Abstract This paper
More informationIntroduction to 2 nd -order Lagrangian Element in LS-DYNA
Introduction to 2 nd -order Lagrangian Element in LS-DYNA Hailong Teng Livermore Software Technology Corporation Nov, 2017 Motivation Users are requesting higher order elements for implicit. Replace shells.
More informationRevision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering. Introduction
Revision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering Introduction A SolidWorks simulation tutorial is just intended to illustrate where to
More informationEngineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering
Engineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering Here SolidWorks stress simulation tutorials will be re-visited to show how they
More informationFlexible multibody systems - Relative coordinates approach
Computer-aided analysis of multibody dynamics (part 2) Flexible multibody systems - Relative coordinates approach Paul Fisette (paul.fisette@uclouvain.be) Introduction In terms of modeling, multibody scientists
More informationFinite Element Method. Chapter 7. Practical considerations in FEM modeling
Finite Element Method Chapter 7 Practical considerations in FEM modeling Finite Element Modeling General Consideration The following are some of the difficult tasks (or decisions) that face the engineer
More informationExecutive Summary Sefea Basic Theory
Executive Summary Sefea is one of the newest generations of enriched finite element methods. Developed specifically for low-order 4-node tetrahedron and 3-node triangle in the CAE environment, Sefea achieves
More informationChapter 5 Modeling and Simulation of Mechanism
Chapter 5 Modeling and Simulation of Mechanism In the present study, KED analysis of four bar planar mechanism using MATLAB program and ANSYS software has been carried out. The analysis has also been carried
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 informationEXPLICIT DYNAMIC ANALYSIS OF A REINFORCED CONCRETE FRAME UP TO COLLAPSE
EXPLICIT DYNAMIC ANALYSIS OF A REINFORCED CONCRETE FRAME UP TO COLLAPSE ABSTRACT: K. Kocamaz 1, K. Tuncay 2 and B. Binici 3 1 Res. Assist., Civil Eng. Department, Middle East Technical University, Ankara
More informationWorkshop 15. Single Pass Rolling of a Thick Plate
Introduction Workshop 15 Single Pass Rolling of a Thick Plate Rolling is a basic manufacturing technique used to transform preformed shapes into a form suitable for further processing. The rolling process
More informationAnalysis of ANSI W W 6x9-118,
Page 1 of 8 Analysis of ANSI W W 6x9-118,110236220472 Author: Analysis Created: Analysis Last Modified: Report Created: Introduction Administrator, 08:29:09, 08:29:09 09:26:02 Database: Z:\ENGENHARIA\ESTUDOS
More informationDynamic Behaviour of Pile Foundations in
Dynamic Behaviour of Pile Foundations in Layered Soil Half-Space Using Cone Method M.M. Aldimashki 1 and J.M.W. Brownjohn 1, Department of Civil and Structural Engineering, University of Sheffield, Sir
More informationAn Approximate Method for Permuting Frame with Repeated Lattice Structure to Equivalent Beam
The Open Ocean Engineering Journal, 2011, 4, 55-59 55 Open Access An Approximate Method for Permuting Frame with Repeated Lattice Structure to Equivalent Beam H.I. Park a, * and C.G. Park b a Department
More informationFinite Element Analysis of Dynamic Flapper Valve Stresses
Purdue University Purdue e-pubs International Compressor Engineering Conference School of Mechanical Engineering 2000 Finite Element Analysis of Dynamic Flapper Valve Stresses J. R. Lenz Tecumseh Products
More informationA general contact detection algorithm for finite element analysis
A general contact detection algorithm for finite element analysis M.W. Heinstein, S.W. Attaway J.W. Swegle, F.J. Mello Sandia National Laboratories, Albuquerque, Mezzco 27J&5, A contact detection algorithm
More informationINTEGRATION SCHEMES FOR THE TRANSIENT DYNAMICS OF NONLINEAR CABLE STRUCTURES
6th European Conference on Computational Mechanics (ECCM 6) 7th European Conference on Computational Fluid Dynamics (ECFD 7) 1115 June 2018, Glasgow, UK INTEGRATION SCHEMES FOR THE TRANSIENT DYNAMICS OF
More informationValidation of a New Finite Element for Incremental Forming Simulation Using a Dynamic Explicit Approach
Validation of a New Finite Element for Incremental Forming Simulation Using a Dynamic Explicit Approach C. Henrard 1, C. Bouffioux 2, L. Duchêne 3, J.R. Duflou 4 and A.M. Habraken 1 1 Université de Liège,
More informationLS-DYNA s Linear Solver Development Phase 2: Linear Solution Sequence
LS-DYNA s Linear Solver Development Phase 2: Linear Solution Sequence Allen T. Li 1, Zhe Cui 2, Yun Huang 2 1 Ford Motor Company 2 Livermore Software Technology Corporation Abstract This paper continues
More informationThree Dimensional Seismic Simulation of a Two-Bay, Two-Story Reinforced Concrete Building
Three Dimensional Seismic Simulation of a Two-Bay, Two-Story Reinforced Concrete Building Catherine Joseph, REU Student Rachel Howser, Graduate Advisor Dr. Y.L Mo, Faculty Advisor Final Report Department
More informationOrbital forming of SKF's hub bearing units
Orbital forming of SKF's hub bearing units Edin Omerspahic 1, Johan Facht 1, Anders Bernhardsson 2 1 Manufacturing Development Centre, AB SKF 2 DYNAmore Nordic 1 Background Orbital forming is an incremental
More informationMODELLING OF COLD ROLL PROCESS USING ANALYTIC AND FINITE ELEMENT METHODS
MODELLING OF COLD ROLL PROCESS USING ANALYTIC AND FINITE ELEMENT METHODS Yunus Ozcelik, Semih Cakil Borusan R&D Kayisdagi Cad, Defne Sok. Buyukhanli Plaza 34750 Istanbul/Turkey e-mail: yozcelik@borusan.com
More informationOPTIMIZATION OF STIFFENED LAMINATED COMPOSITE CYLINDRICAL PANELS IN THE BUCKLING AND POSTBUCKLING ANALYSIS.
OPTIMIZATION OF STIFFENED LAMINATED COMPOSITE CYLINDRICAL PANELS IN THE BUCKLING AND POSTBUCKLING ANALYSIS. A. Korjakin, A.Ivahskov, A. Kovalev Stiffened plates and curved panels are widely used as primary
More informationMODELING OF WATERHAMMER EVENTS USING A LAGRANGEAN FORMULATION
Mecánica Computacional Vol XXVIII, págs. 381-391 (artículo completo) Cristian García Bauza, Pablo Lotito, Lisandro Parente, Marcelo Vénere (Eds.) Tandil, Argentina, 3-6 Noviembre 2009 MODELING OF WATERHAMMER
More informationEXACT BUCKLING SOLUTION OF COMPOSITE WEB/FLANGE ASSEMBLY
EXACT BUCKLING SOLUTION OF COMPOSITE WEB/FLANGE ASSEMBLY J. Sauvé 1*, M. Dubé 1, F. Dervault 2, G. Corriveau 2 1 Ecole de technologie superieure, Montreal, Canada 2 Airframe stress, Advanced Structures,
More informationMODELLING OF AN AUTOMOBILE TYRE USING LS-DYNA3D
MODELLING OF AN AUTOMOBILE TYRE USING LS-DYNA3D W. Hall, R. P. Jones, and J. T. Mottram School of Engineering, University of Warwick, Coventry, CV4 7AL, UK ABSTRACT: This paper describes a finite element
More informationScienceDirect. Vibration Response Prediction of the Printed Circuit Boards using Experimentally Validated Finite Element Model
Available online at www.sciencedirect.com ScienceDirect Procedia Engineering 144 (2016 ) 576 583 12th International Conference on Vibration Problems, ICOVP 2015 Vibration Response Prediction of the Printed
More informationA PHYSICAL SIMULATION OF OBJECTS BEHAVIOUR BY FINITE ELEMENT METHOD, MODAL MATCHING AND DYNAMIC EQUILIBRIUM EQUATION
A PHYSICAL SIMULATION OF OBJECTS BEHAVIOUR BY FINITE ELEMENT METHOD, MODAL MATCHING AND DYNAMIC EQUILIBRIUM EQUATION Raquel Ramos Pinho, João Manuel R. S. Tavares FEUP Faculty of Engineering, University
More informationA substructure based parallel dynamic solution of large systems on homogeneous PC clusters
CHALLENGE JOURNAL OF STRUCTURAL MECHANICS 1 (4) (2015) 156 160 A substructure based parallel dynamic solution of large systems on homogeneous PC clusters Semih Özmen, Tunç Bahçecioğlu, Özgür Kurç * Department
More informationTHREE DIMENSIONAL DYNAMIC STRESS ANALYSES FOR A GEAR TEETH USING FINITE ELEMENT METHOD
THREE DIMENSIONAL DYNAMIC STRESS ANALYSES FOR A GEAR TEETH USING FINITE ELEMENT METHOD Haval Kamal Asker Department of Mechanical Engineering, Faculty of Agriculture and Forestry, Duhok University, Duhok,
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 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 informationModeling Strategies for Dynamic Finite Element Cask Analyses
Session A Package Analysis: Structural Analysis - Modeling Modeling Strategies for Dynamic Finite Element Cask Analyses Uwe Zencker, Günter Wieser, Linan Qiao, Christian Protz BAM Federal Institute for
More informationModal Analysis of Three Dimensional Numerical Control Laser Cutting Machine Based on Finite Element Method Yun-Xin CHEN*
Proceedings of the 3rd International Conference on Material Engineering and Application (ICMEA 2016) Modal Analysis of Three Dimensional Numerical Control Laser Cutting Machine Based on Finite Element
More informationSome Aspects for the Simulation of a Non-Linear Problem with Plasticity and Contact
Some Aspects for the Simulation of a Non-Linear Problem with Plasticity and Contact Eduardo Luís Gaertner Marcos Giovani Dropa de Bortoli EMBRACO S.A. Abstract A linear elastic model is often not appropriate
More informationDEPLOYMENT SIMULATIONS OF COMPLEX ANTENNA STRUCTURES USING AN IMPLICIT NON-LINEAR FINITE ELEMENT SOLVER
DEPLOYMENT SIMULATIONS OF COMPLEX ANTENNA STRUCTURES USING AN IMPLICIT NON-LINEAR FINITE ELEMENT SOLVER F. Cugnon (1), D. Granville (1), P. Howard (2), M. Milano (3), J. Santiago Prowald (4) (1) Samtech
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 informationAXIAL OF OF THE. M. W. Hyer. To mitigate the. Virginia. SUMMARY. the buckling. circumference, Because of their. could.
IMPROVEMENT OF THE AXIAL BUCKLING CAPACITY OF COMPOSITE ELLIPTICAL CYLINDRICAL SHELLS M. W. Hyer Department of Engineering Science and Mechanics (0219) Virginia Polytechnic Institute and State University
More informationstudying of the prying action effect in steel connection
studying of the prying action effect in steel connection Saeed Faraji Graduate Student, Department of Civil Engineering, Islamic Azad University, Ahar Branch S-faraji@iau-ahar.ac.ir Paper Reference Number:
More informationExam paper: Numerical Analysis of Continua I
Exam paper: Numerical Analysis of Continua I Tuesday April th:. - 2. Code: 8W3, BMT 3. Biomedical Technology Eindhoven University of Technology This is an open book exam. It comprises questions. The questions
More informationDEVELOPMENT OF LEG WHEEL HYBRID HEXAPOD BOT
DEVELOPMENT OF LEG WHEEL HYBRID HEXAPOD BOT Sai Srinivas Nallamothu, Sai Preetham Sata, P. Sateesh Kumar Reddy, B. Jaswanth Babu ABSTRACT The conventional mobile robotic platforms which either uses wheels
More informationComputer Life (CPL) ISSN: Finite Element Analysis of Bearing Box on SolidWorks
Computer Life (CPL) ISSN: 1819-4818 Delivering Quality Science to the World Finite Element Analysis of Bearing Box on SolidWorks Chenling Zheng 1, a, Hang Li 1, b and Jianyong Li 1, c 1 Shandong University
More informationSet No. 1 IV B.Tech. I Semester Regular Examinations, November 2010 FINITE ELEMENT METHODS (Mechanical Engineering) Time: 3 Hours Max Marks: 80 Answer any FIVE Questions All Questions carry equal marks
More informationixcube 4-10 Brief introduction for membrane and cable systems.
ixcube 4-10 Brief introduction for membrane and cable systems. ixcube is the evolution of 20 years of R&D in the field of membrane structures so it takes a while to understand the basic features. You must
More informationSTRUCTURAL ANALYSIS OF Ka-BAND GIMBALED ANTENNAS FOR A COMMUNICATIONS SATELLITE SYSTEM
STRUCTURAL ANALYSIS OF Ka-BAND GIMBALED ANTENNAS FOR A COMMUNICATIONS SATELLITE SYSTEM Hong Su COM DEV Ltd. 155 Sheldon Drive, Cambridge Ontario, Canada N1R 7H6 ABSTRACT This paper presents the FE modeling,
More informationROTATIONAL DEPENDENCE OF THE SUPERCONVERGENT PATCH RECOVERY AND ITS REMEDY FOR 4-NODE ISOPARAMETRIC QUADRILATERAL ELEMENTS
COMMUNICATIONS IN NUMERICAL METHODS IN ENGINEERING Commun. Numer. Meth. Engng, 15, 493±499 (1999) ROTATIONAL DEPENDENCE OF THE SUPERCONVERGENT PATCH RECOVERY AND ITS REMEDY FOR 4-NODE ISOPARAMETRIC QUADRILATERAL
More informationFloating Cylinder. SeaFEM - Validation Case 4
SeaFEM - Validation Case 4 Floating Cylinder Compass Ingeniería y Sistemas, SA T. +34 93 218 19 89 F. +34 93 396 97 46 E. info@compassis.com c/ Tuset, 8 7-2 Barcelona 08006 C.I.F.: A 62485180 1 Validation
More informationMetafor FE Software. 2. Operator split. 4. Rezoning methods 5. Contact with friction
ALE simulations ua sus using Metafor eao 1. Introduction 2. Operator split 3. Convection schemes 4. Rezoning methods 5. Contact with friction 1 Introduction EULERIAN FORMALISM Undistorted mesh Ideal for
More informationLinear and Nonlinear Analysis of a Cantilever Beam
LESSON 1 Linear and Nonlinear Analysis of a Cantilever Beam P L Objectives: Create a beam database to be used for the specified subsequent exercises. Compare small vs. large displacement analysis. Linear
More informationNumerical Calculations of Stability of Spherical Shells
Mechanics and Mechanical Engineering Vol. 14, No. 2 (2010) 325 337 c Technical University of Lodz Numerical Calculations of Stability of Spherical Shells Tadeusz Niezgodziński Department of Dynamics Technical
More informationDynamic Analysis of Air Conditioner Compressor Mounting Bracket
ISSN 2395-1621 Dynamic Analysis of Air Conditioner Compressor Mounting Bracket #1 Vyankatesh D. Pawade, #2 Pushkaraj D. Sonawane 1 vdpawade@gmail.com 2 pushkaraj.sonawane@mitpune.edu.in 1 Student ME Design,
More informationSETTLEMENT OF A CIRCULAR FOOTING ON SAND
1 SETTLEMENT OF A CIRCULAR FOOTING ON SAND In this chapter a first application is considered, namely the settlement of a circular foundation footing on sand. This is the first step in becoming familiar
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 informationStudies in dynamic design of drilling machine using updated finite element models
Studies in dynamic design of drilling machine using updated finite element models R.S. Bais a, *, A.K. Gupta b, B.C. Nakra c, T.K. Kundra c a Bharat Heavy Electricals Limited, Hyderabad, India b Instrument
More informationVehicle Load Area Division Wall Integrity during Frontal Crash
Vehicle Load Area Division Wall Integrity during Frontal Crash H. Türkmen TOFAS Türk Otomobil Fabrikasi A.S. Abstract : This study addresses design efforts of a vehicle load area division wall and the
More informationReduction of Finite Element Models for Explicit Car Crash Simulations
Reduction of Finite Element Models for Explicit Car Crash Simulations K. Flídrová a,b), D. Lenoir a), N. Vasseur b), L. Jézéquel a) a) Laboratory of Tribology and System Dynamics UMR-CNRS 5513, Centrale
More informationVOLCANIC DEFORMATION MODELLING: NUMERICAL BENCHMARKING WITH COMSOL
VOLCANIC DEFORMATION MODELLING: NUMERICAL BENCHMARKING WITH COMSOL The following is a description of the model setups and input/output parameters for benchmarking analytical volcanic deformation models
More informationThe Dynamic Response of an Euler-Bernoulli Beam on an Elastic Foundation by Finite Element Analysis using the Exact Stiffness Matrix
Journal of Physics: Conference Series The Dynamic Response of an Euler-Bernoulli Beam on an Elastic Foundation by Finite Element Analysis using the Exact Stiffness Matrix To cite this article: Jeong Soo
More informationExample 12 - Jumping Bicycle
Example 12 - Jumping Bicycle Summary The purpose of this example is to illustrate how to use the RADIOSS description when resolving a demonstration example. The particularities of the example can be summarized
More informationDynamics Response of Spatial Parallel Coordinate Measuring Machine with Clearances
Sensors & Transducers 2013 by IFSA http://www.sensorsportal.com Dynamics Response of Spatial Parallel Coordinate Measuring Machine with Clearances Yu DENG, Xiulong CHEN, Suyu WANG Department of mechanical
More informationCrashbox Tutorial. In this tutorial the focus is on modeling a Formula Student Racecar Crashbox with HyperCrash 12.0
Crashbox Tutorial In this tutorial the focus is on modeling a Formula Student Racecar Crashbox with HyperCrash 12.0 (Written by Moritz Guenther, student at Altair Engineering GmbH) 1 HyperMesh* 1. Start
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 informationLinear Elastic Fracture Mechanics (LEFM) Analysis of Flaws within Residual Stress Fields
Linear Elastic Fracture Mechanics (LEFM) Analysis of Flaws within Residual Stress Fields David Woyak 1, Brian Baillargeon, Ramesh Marrey, and Randy Grishaber 2 1 Dassault Systemés SIMULIA Corporation &
More informationAn explicit feature control approach in structural topology optimization
th World Congress on Structural and Multidisciplinary Optimisation 07 th -2 th, June 205, Sydney Australia An explicit feature control approach in structural topology optimization Weisheng Zhang, Xu Guo
More informationIntroduction. Co-rotational Concept
1 2D Co-rotational Truss Formulation by Louie L. Yaw Walla Walla University April 23, 29 key words: geometrically nonlinear analysis, 2d co-rotational truss, corotational truss, variationally consistent,
More information3D Finite Element Software for Cracks. Version 3.2. Benchmarks and Validation
3D Finite Element Software for Cracks Version 3.2 Benchmarks and Validation October 217 1965 57 th Court North, Suite 1 Boulder, CO 831 Main: (33) 415-1475 www.questintegrity.com http://www.questintegrity.com/software-products/feacrack
More informationCHAPTER 6 EXPERIMENTAL AND FINITE ELEMENT SIMULATION STUDIES OF SUPERPLASTIC BOX FORMING
113 CHAPTER 6 EXPERIMENTAL AND FINITE ELEMENT SIMULATION STUDIES OF SUPERPLASTIC BOX FORMING 6.1 INTRODUCTION Superplastic properties are exhibited only under a narrow range of strain rates. Hence, it
More informationCONTACT STATE AND STRESS ANALYSIS IN A KEY JOINT BY FEM
PERJODICA POLYTECHNICA SER. ME CH. ENG. VOL. 36, NO. 1, PP. -15-60 (1992) CONTACT STATE AND STRESS ANALYSIS IN A KEY JOINT BY FEM K. VARADI and D. M. VERGHESE Institute of Machine Design Technical University,
More informationA Multiple Constraint Approach for Finite Element Analysis of Moment Frames with Radius-cut RBS Connections
A Multiple Constraint Approach for Finite Element Analysis of Moment Frames with Radius-cut RBS Connections Dawit Hailu +, Adil Zekaria ++, Samuel Kinde +++ ABSTRACT After the 1994 Northridge earthquake
More informationmachine design, Vol.9(2017) No.1, ISSN pp
machine design, Vol.9(2017) No.1, ISSN 1821-1259 pp. 29-34 Research paper DYNAMIC ANALYSIS AND PARAMETRIC OPTIMISATION OF THE CONNECTING ROD USING AUTODESK INVENTOR Vasile George CIOATĂ 1, * - Imre KISS
More informationModelling Flat Spring Performance Using FEA
Modelling Flat Spring Performance Using FEA Blessing O Fatola, Patrick Keogh and Ben Hicks Department of Mechanical Engineering, University of Corresponding author bf223@bath.ac.uk Abstract. This paper
More informationSeismic Soil-Structure Interaction Analysis of the Kealakaha Stream Bridge on Parallel Computers
Seismic Soil-Structure Interaction Analysis of the Kealakaha Stream Bridge on Parallel Computers Seung Ha Lee and Si-Hwan Park Department of Civil and Environmental Engineering University of Hawaii at
More informationChapter 7 Practical Considerations in Modeling. Chapter 7 Practical Considerations in Modeling
CIVL 7/8117 1/43 Chapter 7 Learning Objectives To present concepts that should be considered when modeling for a situation by the finite element method, such as aspect ratio, symmetry, natural subdivisions,
More informationChapter 1 Introduction
Chapter 1 Introduction GTU Paper Analysis (New Syllabus) Sr. No. Questions 26/10/16 11/05/16 09/05/16 08/12/15 Theory 1. What is graphic standard? Explain different CAD standards. 2. Write Bresenham s
More informationImpact and Postbuckling Analyses
ABAQUS/Explicit: Advanced Topics Lecture 8 Impact and Postbuckling Analyses ABAQUS/Explicit: Advanced Topics L8.2 Overview Geometric Imperfections for Postbuckling Analyses ABAQUS/Explicit: Advanced Topics
More informationA Locking-free Smoothed Finite Element Formulation (Modified Selective FS/NS-FEM-T4) with Tetrahedral Mesh Rezoning for Large Deformation Problems
A Locking-free Smoothed Finite Element Formulation (Modified Selective FS/NS-FEM-T4) with Tetrahedral Mesh Rezoning for Large Deformation Problems Yuki ONISHI, Kenji AMAYA Tokyo Institute of Technology
More informationDesign optimization of C Frame of Hydraulic Press Machine
IOSR Journal of Computer Engineering (IOSR-JCE) e-issn: 2278-0661,p-ISSN: 2278-8727 PP 79-89 www.iosrjournals.org Design optimization of C Frame of Hydraulic Press Machine Ameet B. Hatapakki 1, U D. Gulhane
More informationMixed Mode Fracture of Through Cracks In Nuclear Reactor Steam Generator Helical Coil Tube
Journal of Materials Science & Surface Engineering Vol. 3 (4), 2015, pp 298-302 Contents lists available at http://www.jmsse.org/ Journal of Materials Science & Surface Engineering Mixed Mode Fracture
More informationEffect of Three-Dimensional Geometry on the Sloshing Behavior of Rectangular Concrete Tanks
Effect of Three-Dimensional Geometry on the Sloshing Behavior of Rectangular Concrete Tanks I. Tavakkoli Avval Departmnet of Civil Engineering, Ryerson University, Canada M.R. Kianoush Departmnet of Civil
More informationDesign procedures of seismic-isolated container crane at port
Design procedures of seismic-isolated container crane at port T.Sugano 1, M.Takenobu 1, T.Suzuki 1, and Y.Shiozaki 2 1 Port and Airport Research Institute,Yokosuka, Japan 2 JFE R&D Corporation,Kawasaki,Japan
More informationStructural Analysis of an Aluminum Spiral Staircase. EMCH 407 Final Project Presented by: Marcos Lopez and Dillan Nguyen
Structural Analysis of an Aluminum Spiral Staircase EMCH 407 Final Project Presented by: Marcos Lopez and Dillan Nguyen Abstract An old aluminum spiral staircase at Marcos home has been feeling really
More informationCHAPTER-10 DYNAMIC SIMULATION USING LS-DYNA
DYNAMIC SIMULATION USING LS-DYNA CHAPTER-10 10.1 Introduction In the past few decades, the Finite Element Method (FEM) has been developed into a key indispensable technology in the modeling and simulation
More informationDevelopment of the Compliant Mooring Line Model for FLOW-3D
Flow Science Report 08-15 Development of the Compliant Mooring Line Model for FLOW-3D Gengsheng Wei Flow Science, Inc. October 2015 1. Introduction Mooring systems are common in offshore structures, ship
More informationEffect of Diagonal Modes on Response Spectrum Analysis
Effect of Diagonal Modes on Response Spectrum Analysis T. Naga Manikanta & O. R. Jaiswal Department of Applied Mechanics Visvesvaraya National Institute of Technology, Nagpur, Maharashtra, India Summary:
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 informationMutltiphysics for Ironcad Demonstration Models (Rev. 1.1)
Centrifuge Model The centrifuge model demonstrates how to perform a rotational spinning centrifugal load analysis. It also demonstrates how to group different parts with/without the intended initial bonding
More informationUsing MSC.Nastran for Explicit FEM Simulations
3. LS-DYNA Anwenderforum, Bamberg 2004 CAE / IT III Using MSC.Nastran for Explicit FEM Simulations Patrick Doelfs, Dr. Ingo Neubauer MSC.Software GmbH, D-81829 München, Patrick.Doelfs@mscsoftware.com Abstract:
More informationA large number of user subroutines and utility routines is available in Abaqus, that are all programmed in Fortran. Subroutines are different for
1 2 3 A large number of user subroutines and utility routines is available in Abaqus, that are all programmed in Fortran. Subroutines are different for implicit (standard) and explicit solvers. Utility
More informationOptimization to Reduce Automobile Cabin Noise
EngOpt 2008 - International Conference on Engineering Optimization Rio de Janeiro, Brazil, 01-05 June 2008. Optimization to Reduce Automobile Cabin Noise Harold Thomas, Dilip Mandal, and Narayanan Pagaldipti
More informationFORMING SIMULATION USING RIGID-PLASTIC MATERIAL MODEL IN MARC
SESSION TITLE WILL BE COMPLETED BY MSC SOFTWARE FORMING SIMULATION USING RIGID-PLASTIC MATERIAL MODEL IN MARC Gary Huang, Simufact-Americas LLC April 8, 2013 SUMMARY When simulating large deformation in
More informationAny analysis, static or dynamic, in a FEM follows a standard procedure as defined in fig.(9.1):
Chapter 9 Model definition 9.1 Main features 9.1.1 Introduction Any analysis, static or dynamic, in a FEM follows a standard procedure as defined in fig.(9.1): The experimental sequence to perform in the
More information