ScienceDirect. Vibration Response Prediction of the Printed Circuit Boards using Experimentally Validated Finite Element Model
|
|
- Ruby Armstrong
- 6 years ago
- Views:
Transcription
1 Available online at ScienceDirect Procedia Engineering 144 (2016 ) th International Conference on Vibration Problems, ICOVP 2015 Vibration Response Prediction of the Printed Circuit Boards using Experimentally Validated Finite Element Model Somashekar V.N a, Harikrishnan S b, PSM Aejaz Ahmed c, Kamesh D d a,d SRG, ISRO Satellite Centre, Bengaluru , India b,c SaiVidya Institute of Technology, Bengaluru , India Abstract A spacecraft consists of a number of mechanical and electronic sub-assemblies. An electronic package is consists of printed circuit boards placed in mechanical housings which are stacked together. Electronic components are mounted on the printed circuit board (PCB). A spacecraft experiences various types of mechanical loads during its launch such as vibration, acoustic and shock loads. The understanding of dynamic behaviour provides valuable insight to a design engineer, to improve the mechanical design and product reliability when used in harsh vibration condition. Generally electronic package design for vibration loads is verified by conducting tests on actual hardware. This paper addresses on using basic FEA tool to accurately investigate the dynamic characteristics of the PCB and avoid costly testing methods which require hardware. Here the normal modes & frequency response functions (FRF) of PCB are determined and validated using vibration test on PCB. The validated model is used to predict vibration response for random vibration input. It is shown here how the responses are accurately predicted for random vibration input for a design parameter variation of PCB. The results are also validated using vibration test on PCB The Authors. Published by Elsevier by Elsevier Ltd. Ltd. This is an open access article under the CC BY-NC-ND license ( Peer-review under responsibility of the organizing committee of ICOVP Peer-review under responsibility of the organizing committee of ICOVP 2015 Keywords:Printed Circuit Board (PCB); Spacecraft;Vibration Response. * Corresponding author. Tel.: / address: krishnan1993@gmail.com, aejazahmed93@gmail.com The Authors. Published by Elsevier Ltd. This is an open access article under the CC BY-NC-ND license ( Peer-review under responsibility of the organizing committee of ICOVP 2015 doi: /j.proeng
2 V.N. Somashekar et al. / Procedia Engineering 144 ( 2016 ) Introduction A spacecraft experiences various types of dynamic loads during its launch such as vibration, acoustic and shock loads. The electronic packages are designed to withstand the launch vibration environment. The mechanical design of electronicpackages is verified by subjecting to vibration testing. The electronic component failures have been observed whenever there is change in its location on the PCB due to electrical design requirements. The basic failure modes of components mounted on PCB due to random vibration environment are the results of the following conditions: high acceleration levels,high stress levels,large displacement amplitudes andelectrical signals out of tolerance [1]. The design failures during test and evaluation process have resulted in delay in the project schedule. An effective methodology to verify the design other than testing has to be evolved and finite element (FE) analysis has been an effective tool in predicting results. The FE analysis of electronic packages has a lot difficulties due to many low mass individual elements present in it. Electronic systems are often simulated using simple masses, springs and dampers to estimate the dynamic characteristics of the system. Simple one and two degree of freedom systems are used to approximate the electronic systems. More complicated finite element models of electronic systems are created to study the dynamic characteristics of the system and to estimate the fatigue life of critical components mounted on the PCB. Finite element models can be either simplified or detailed. Detailed finite element models are built by modeling the PCB and the components. However, this approach is rarely used as it is time consuming and expensive. Instead, simplified models of PCB are created where the components geometry is neglected. The component effects are included by increasing the Young's modulus and density of the PCB FE model, so it effectively behaves as if components were present. The simple geometry of the board is modeled and meshed using 2-D finite elements (i.e. by using flat shell elements). Sensitivity analysis of PCB finite element models was carried out by Amy et al. [2]. They determined the factors of safety by using different simplification methods of modeling the PCB. Printed circuit boards are multi-layered structures with complex material properties that make the simulation of their dynamic behavior complicated and hence to simplify this, a number of parameters affecting the PCB s dynamics have been studied through experimentation. Dynamic responses such as accelerations, strains are to be closely monitored and controlled to achieve test results which are consistent and predict the structural behavior in reality [3]. Printed circuit boards with multiple layers are suitable candidates preferable for high speed and high density applications. In order to design electronic packaging systems for safety and standards criterion, the accurate modeling of components influence on the multi-layered PCB becomes critical and complex due to various reasons. Numerical model using finite element technique was developed to simulate the mechanical behavior of multilayered PCB and physical tests were conducted to validate the impact performance [4]. In this paper, vibration analysis of a typical PCB used for space applications is carried out. The normal modes & frequency response functions (FRF) of bare PCB (without components) are determined and validated using vibration test on PCB. The validated model is used to predict vibration response for random vibration input. It is shown here how the responses are accurately predicted for random vibration input for a design parameter change of PCB. The results are also validated using vibration test on PCB. 2. Vibration Response Prediction of PCB using FEM In this study, a six layer PCB used for space applications is considered. The PCB is modelled as isotropic plate with equivalent material properties such as Young s modulus, Poisson s ratio and mass density. FEA simulations of PCB dynamics are made using MSC.PATRAN as pre-processor and MSC.NASTRAN as solver for bare PCB and PCBwith components. Finite Element model consists of 3364 quadrilateral shell elements. Young s modulus of elasticity for PCB is obtained as 15 GPa by conducting a three point bending test for three different samples of PCB. The PCB properties are given in Table (1). The FE model of bare PCB is analysed and validated for two different boundary conditions i.e., i) PCB fixed/clamped at nine mounting locations shown in Figure (1) and ii) PCB with fixed at eight mounting locations shown in Figure (2).
3 578 V.N. Somashekar et al. / Procedia Engineering 144 ( 2016 ) Fig 1. FE model of PCB fixed at 9 mounting locations Fig 2. FE model of PCB fixed at 8 mounting locations Further the analysis is carried out to predict response for random vibration input which is also validated with test results. With these iterations it should be possible to predict the vibration response accurately for any change in the PCB parameters. To meet the requirement of an ongoing project, the existing PCB thickness has to be reduced. The vibration analysis is carried out to predict the responses for the modified design. However, the response prediction by analysis is also validated by conducting test on modified PCB. Fixed/clamped boundary conditions are applied (PCB mounting locations) by arresting six degrees of freedom for the nodes on the boundary of holes in PCB. Table 1. Details of PCB Parameter Value PCB size mm Density of Bare PCB 1985 Kg/m 3 Young s modulus of Bare PCB 15 GPa Poisson s ratio 0.12 Boundary Condition Fixed/clamped 2.1 Finite Element Model Normal mode analyses were carried out to extract first few fundamental natural frequencies for PCB with nine mounting location and eight mounting location. The calculated first few natural frequencies and corresponding test results are given in Table (3) and (4). Mode shapes corresponding first two natural frequencies for both cases are given in Figures (3) to (6). Fig 3. Mode shape of PCB with 9 mounting locations Fig 4. Mode shape of PCB with 9 mounting locations
4 V.N. Somashekar et al. / Procedia Engineering 144 ( 2016 ) Fig 5.Mode shape of PCB with 8 mounting locations for first frequency Fig 6. Mode shape of PCB with 8 mounting locations for second frequency The same FE model was used to obtain frequency response function (FRF) by subjecting it to base excitation of 1g from 5 Hz to 2000 Hz. In this study, a structural damping coefficient of 2% is incorporated in the model. The FRF at a specific location of the PCB are plotted in Figures (7) and (8). These values are then compared with test data obtained from vibration tests. The same FE model (9 mounting location, 2.1 mm thick PCB) was used to obtain vibration response subjected to random vibration input given in Table (2). The random vibration response plot for 2.1mm PCB is given in Figure (9) & (10). In actual case the thickness of the PCB was to be reduced to 1.6 mm and study the response change. The vibration response for the same random vibration input for 1.6mm PCB is given in Figure (11) & (12). Fig 7. Analysis FRF for PCB with 9 mounting location Fig 8. Analysis FRF for PCB with 8 mounting location Table 2. Random vibration specification Frequency (Hz) PSD (g 2 /Hz) Overall grms db/oct db/oct
5 580 V.N. Somashekar et al. / Procedia Engineering 144 ( 2016 ) Fig9. Analysis random vibration response for 2.1 mm PCB location Q3L1 with 9 mounting location Fig 10. Analysis random vibration response for 2.1 mm PCB location Q3L7 with 9 mounting location Fig 11. Analysis random vibration response for 1.6 mm PCB location Q3L1 with 9 mounting location Fig 12. Analysis random vibration response for 1.6 mm PCB location Q3L7 with 9 mounting location 2.2 Experimental Test Setup The vibration test was conducted by mounting the 2.1 mm PCB with screws at nine and eight locations on vibration table as shown in Figure (13) and (14) respectively. Figure (15) shows 1.6 mm PCB mounted on vibration table. Accelerometers are mounted at various locations of the PCB to measure the responses. The vibration test was carried out in the vibration test facility consisting of electro-dynamic shaker, control system, signal conditioners and data acquisition system. The frequency response function (FRF) is obtained by conducting a sine sweep test. In sine sweep test, the input acceleration is given to the test specimen using electro-dynamic shaker and the output acceleration at various desired locations of the test specimen is measured using accelerometer. The ratio of output to input acceleration gives the FRF at that location. The experimental frequency response plots for PCB with screws at nine and eight mounting locations are shown in Figures (16) and (17) respectively. Fig mm PCB with 9 mounting location on vibration table Fig mm PCB with 8 mounting location on vibration table
6 V.N. Somashekar et al. / Procedia Engineering 144 ( 2016 ) Fig mm PCB with 9 mounting location on vibration table The vibration test was carried out to obtain the vibration responses for the random vibration input and is given in Table (5) & (6). The test was carried out for both 2.1 mm and 1.6 mm thickness PCB. The random vibration response obtained from test is given in Figures (18) to (21). Fig 16. Test FRF for PCB with 9 mounting location Fig 17. Test FRF for PCB with 8 mounting location
7 582 V.N. Somashekar et al. / Procedia Engineering 144 ( 2016 ) Fig 18. Test random vibration response for 2.1 mm PCB location Q3L1 with 9 mounting location Fig 19. Test random vibration response for 2.1 mm PCB location Q3L7 with 9 mounting location Fig 20. Test random vibration response for 1.6 mm PCB location Q3L1 with 9 mounting location Fig 21. Test random vibration response for 1.6 mm PCB location Q3L7 with 9 mounting location
8 V.N. Somashekar et al. / Procedia Engineering 144 ( 2016 ) Results and Discussion In this section, the FEM and experimental test results are compared. Analysis and test results for first few fundamental frequencies of the PCB at 9 mounting locations are compared in Table (3) and for PCB at 8 mounting locations are compared in Table (4). The analysis and test results for both the cases are matching well. The random vibration response for 2.1 mm thickness PCB at 9 mounting locations for both analysis and test are compared in Table (5). Table (6) shows the same comparison for 1.6 mm thickness PCB. Here the random vibration response (overall grms) has reduced for 1.6 mm PCB versus 2.1 mm PCB. This is very well evident from analysis and test results. Table 3. Comparison of fundamental frequencies for PCB FEM Fundamental Test Results Percentage Results Frequency (Hz) Difference (Hz) Table 4. Comparison of fundamental frequencies for PCB FEM Fundamental Test Results Percentage Results Frequency (Hz) Difference (Hz) Table 5. Comparison of random vibration responses for 2.1 mm thick PCB with 9 mounting location Location Analysis Results, g RMS Test Results, g RMS Percentage Difference Table 6. Comparison of random vibration responses for 1.6 mm thick PCB with 9 mounting location Location Analysis Results, g RMS Test Results, g RMS Percentage Difference Q3L Q3L Q3L Q3L Q3L Q3L Q3L Q3L Q3L Q3L Conclusions Vibration analysis is carried out using FEM to obtain normal modes & frequency response functions (FRF) of PCB and validated using experimental test on PCB. The validated model is used to predict vibration response for random vibration input. It is shown from analysis that the responses predicted for random vibration input for a design parameter change (thickness reduction) in the PCB are reducing. These results are also validated using vibration test on PCB. The paper presents using FEM instead of test and evaluation method to predict vibration response accurately. The work can be extended for simulating the components on the PCB. References [1] Steinberg, D. S. Vibration Analysis for Electronic Equipment. 3rd ed. New York: John Wiley & Sons Inc.; [2] Amy, R. A., Aglietti, G. S., Richardson, G. Sensitivity analysis of simplified Printed Circuit Board finite element models. Microelectronics Reliability, 2009; Vol. 49, pp [3] Jing-en Luan, Tong Yan Tee, Eric Pek, CheeTeck Lim, ZheoweiZhong. Dynamic responses and solder joint reliability under board level drop test. Microelectronics Reliability, 2007; Vol. 47, pp [4] Yuqi Wang, K.H. Low, H.L.J. Pang, K.H. Hoon, F.X. Che, Y.S. Yong. Modeling and simulation for a drop-impact analysis of multi-layered printed circuit boards. Microelectronics Reliability, 2006; Vol. 46, pp [5] Jayaraman S, Manish Trikha, Somashekar V N, Kamesh D. Vibration Analysis of Printed Circuit Boards. Interbational Journal of Applied Engineering Research, ISSN Vol.10 No.24 (2015)
CHAPTER 5 RANDOM VIBRATION TESTS ON DIP-PCB ASSEMBLY
117 CHAPTER 5 RANDOM VIBRATION TESTS ON DIP-PCB ASSEMBLY 5.1 INTRODUCTION Random vibration tests are usually specified as acceptance, screening and qualification tests by commercial, industrial, and military
More informationMODELING AND VIBRATION ANALYSIS OF ELECTRONIC EQUIPMENT IN AEROSPACE STRUCTURES
Indian Journal of Fundamental and Applied Life Sciences ISSN: 3 6345 Online An Open Access, Online International Journal Available at www.cibtech.org/sp.ed/jls/4/4/jls.htm 4 Vol. 4 S4, pp. 38-388/Zandipour
More informationFinite Element Analysis and Experimental Validation of Lower Control Arm
Finite Element Analysis and Experimental Validation of Lower Control Arm 1 Miss. P. B. Patil, 2 Prof. M. V. Kharade 1 Assistant Professor at Vishweshwaraya Technical Campus Degree wing, Patgaon, Miraj
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 informationStructural re-design of engine components
Structural re-design of engine components Product design cycle Design Development Testing Structural optimization Product knowledge Design freedom 2/18 Structural re-design of engine components Product
More informationUsing experimental modal analysis to validate a finite element model of a tennis racket
Available online at www.sciencedirect.com Procedia Engineering 34 (2012 ) 688 693 9 th Conference of the International Sports Engineering Association (ISEA) Using experimental modal analysis to validate
More informationFEA and Topology Optimization of an Engine Mounting Bracket
International Journal of Current Engineering and Technology E-ISSN 2277 4106, P-ISSN 2347 5161 2016 INPRESSCO, All Rights Reserved Available at http://inpressco.com/category/ijcet Research Article Sanket
More informationModal Analysis of Intermediate Shaft Used in Automobile Gear Box
Modal Analysis of Intermediate Shaft Used in Automobile Gear Box Mr. Shekhar Dive PG Student, Mechanical Engineering Department, Siddhant College of Engineering, University of Pune, Pune, Maharashtra,
More informationinter.noise 2000 The 29th International Congress and Exhibition on Noise Control Engineering August 2000, Nice, FRANCE
Copyright SFA - InterNoise 2000 1 inter.noise 2000 The 29th International Congress and Exhibition on Noise Control Engineering 27-30 August 2000, Nice, FRANCE I-INCE Classification: 4.7 A HYBRID TOOL FOR
More informationModal Analysis of Exhaust System to Optimize Mounting Hanger Location
Modal Analysis of Exhaust System to Optimize Mounting Hanger Location Chetan D. Gaonkar Assistant Professor, Mechanical Engineering Dpt., DBCE, Margao, Goa Abstract An exhaust system with a superior performance
More informationCrane Hook Design and Analysis
Crane Hook Design and Analysis G Bhagyaraj 1, K Suryaprakash 2, K Subba Rao 3 1M.Tech. CAD/CAM, Godavari Institute of Engineering and Technology, Rajahmundry 2Associate Professor, Godavari Institute of
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 informationCOMPUTER AIDED ENGINEERING. Part-1
COMPUTER AIDED ENGINEERING Course no. 7962 Finite Element Modelling and Simulation Finite Element Modelling and Simulation Part-1 Modeling & Simulation System A system exists and operates in time and space.
More informationRELIABILITY OF THE FEM CALCULATIONS OF THE FRACTURE MECHANICS PARAMETERS
International Conference on Economic Engineering and Manufacturing Systems Braşov, 26 27 November 2009 RELIABILITY OF THE FEM CALCULATIONS OF THE FRACTURE MECHANICS PARAMETERS Galina TODOROVA, Valentin
More informationTHE EFFECT OF THE FREE SURFACE ON THE SINGULAR STRESS FIELD AT THE FATIGUE CRACK FRONT
Journal of MECHANICAL ENGINEERING Strojnícky časopis, VOL 67 (2017), NO 2, 69-76 THE EFFECT OF THE FREE SURFACE ON THE SINGULAR STRESS FIELD AT THE FATIGUE CRACK FRONT OPLT Tomáš 1,2, POKORNÝ Pavel 2,
More informationSmart actuator effectiveness improvement through modal analysis
Smart actuator effectiveness improvement through modal analysis A. Joshi a and S. M. Khot b a Professor, Department of Aerospace Engineering, Indian Institute of Technology, Bombay. b Research Scholar,
More informationNon-Linear Analysis of Bolted Flush End-Plate Steel Beam-to-Column Connection Nur Ashikin Latip, Redzuan Abdulla
Non-Linear Analysis of Bolted Flush End-Plate Steel Beam-to-Column Connection Nur Ashikin Latip, Redzuan Abdulla 1 Faculty of Civil Engineering, Universiti Teknologi Malaysia, Malaysia redzuan@utm.my Keywords:
More informationEffectiveness of Element Free Galerkin Method over FEM
Effectiveness of Element Free Galerkin Method over FEM Remya C R 1, Suji P 2 1 M Tech Student, Dept. of Civil Engineering, Sri Vellappaly Natesan College of Engineering, Pallickal P O, Mavelikara, Kerala,
More informationANSYS Workbench Guide
ANSYS Workbench Guide Introduction This document serves as a step-by-step guide for conducting a Finite Element Analysis (FEA) using ANSYS Workbench. It will cover the use of the simulation package through
More informationInternational Journal of Scientific & Engineering Research, Volume 7, Issue 10, October-2016 ISSN
ISSN 2229-5518 1703 Finite element modeling and its validation using experimental modal analysis Hasan Zakir Jafri, Aas Mohammad Abstract The determination of vibration characteristics of a mechanical
More informationAvailable online at ScienceDirect. Procedia Engineering 160 (2016 )
Available online at www.sciencedirect.com ScienceDirect Procedia Engineering 16 (216 ) 11 18 XVIII International Colloquium on Mechanical Fatigue of Metals (ICMFM XVIII) Characterization of the cyclic
More informationFatigue design of welded bicycle frames using a multiaxial criterion
Available online at www.sciencedirect.com Procedia Engineering 34 (2012 ) 640 645 9 th Conference of the International Sports Engineering Association (ISEA) Fatigue design of welded bicycle frames using
More informationCoustyx Tutorial Indirect Model
Coustyx Tutorial Indirect Model 1 Introduction This tutorial is created to outline the steps required to compute radiated noise from a gearbox housing using Coustyx software. Detailed steps are given on
More informationNX Response Simulation: Structural dynamic response
Response Simulation: Structural dynamic response NX CAE Benefits Reduce costly physical prototypes by using response simulation to improve product performance Gain insight into the dynamic response of
More informationReduction of squeal on laminated brake disc fastened with distributed contact pressure
Recent Researches in Engineering Mechanics, Urban & Naval Transportation and Tourism Reduction of squeal on laminated brake disc fastened with distributed contact pressure Y.KUBOTA, K.OKUBO, T.FUJII Mechanical
More informationMicroelectronics Reliability
Microelectronics Reliability 50 (2010) 1021 1027 Contents lists available at ScienceDirect Microelectronics Reliability journal homepage: www.elsevier.com/locate/microrel Modeling of board-level package
More informationAvailable online at ScienceDirect. Procedia Engineering 99 (2015 )
Available online at www.sciencedirect.com ScienceDirect Procedia Engineering 99 (2015 ) 575 580 APISAT2014, 2014 Asia-Pacific International Symposium on Aerospace Technology, APISAT2014 A 3D Anisotropic
More informationScienceDirect. Forming of ellipse heads of large-scale austenitic stainless steel pressure vessel
Available online at www.sciencedirect.com ScienceDirect Procedia Engineering 81 (2014 ) 837 842 11th International Conference on Technology of Plasticity, ICTP 2014, 19-24 October 2014, Nagoya Congress
More informationUsing Photo Modeling to Obtain the Modes of a Structure
Using Photo Modeling to Obtain the Modes of a Structure Shawn and Mark Richardson, Vibrant Technology, Inc., Scotts Valley, California Photo modeling technology has progressed to the point where a dimensionally
More informationWave Propagation Correlations between Finite Element Simulations and Tests for Enhanced Structural Health Monitoring
6th European Workshop on Structural Health Monitoring - Tu.4.D.4 More info about this article: http://www.ndt.net/?id=14108 Wave Propagation Correlations between Finite Element Simulations and Tests for
More informationThe Vibration Characteristics Analysis of Damping System of Wallmounted Airborne Equipment Based on FEM
IOP Conference Series: Earth and Environmental Science PAPER OPEN ACCESS The Vibration Characteristics Analysis of Damping System of Wallmounted Airborne Equipment Based on FEM To cite this article: Changqing
More informationStatic And Modal Analysis Of Rotating Wheel Rim Using Ansys
International Journal of Engineering Science Invention ISSN (Online): 2319 6734, ISSN (Print): 2319 6726 Volume 3 Issue 9 ǁ September 2014 ǁ PP.18-23 Static And Modal Analysis Of Rotating Wheel Rim Using
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 informationStress Analysis of thick wall bellows using Finite Element Method
Stress Analysis of thick wall bellows using Finite Element Method Digambar J. Pachpande Post Graduate Student Department of Mechanical Engineering V.J.T.I. Mumbai, India Prof. G. U. Tembhare Assistant
More informationISSN: ISO 9001:2008 Certified International Journal of Engineering and Innovative Technology (IJEIT) Volume 2, Issue 3, September 2012
Mitigation Curves for Determination of Relief Holes to Mitigate Concentration Factor in Thin Plates Loaded Axially for Different Discontinuities Shubhrata Nagpal, S.Sanyal, Nitin Jain Abstract In many
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 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 informationAvailable online at ScienceDirect. Procedia Engineering 111 (2015 )
Available online at www.sciencedirect.com ScienceDirect Procedia Engineering 111 (2015 ) 115 120 XXV R-S-P seminar, Theoretical Foundation of Civil Engineering (24RSP) (TFoCE 2015) Numerical simulation
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 information1224. Seismic test and numerical verification of the scaled-down reinforced concrete containment vessel
1224. Seismic test and numerical verification of the scaled-down reinforced concrete containment vessel Yu-Chih Chen 1, Wei-Ting Lin 2, Tung-Liang Chu 3, Yuan-Chieh Wu 4 1 National Center for Research
More informationEVALUATION OF COMMERCIAL LAUNDRY MACHINE IN ROUGH HANDLING LOAD CASE
EVALUATION OF COMMERCIAL LAUNDRY MACHINE IN ROUGH HANDLING LOAD CASE Abhishekh Jadhav 1, Dr. B. S. Manjunath 2 1 M.Tech Student (Design Engineering), KLE. Dr. M.S Sheshgiri College of Engg & Tech, Belagavi,
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 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 informationExample 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 informationFINITE ELEMENT MODELLING AND ANALYSIS OF WORKPIECE-FIXTURE SYSTEM
FINITE ELEMENT MODELLING AND ANALYSIS OF WORKPIECE-FIXTURE SYSTEM N. M. KUMBHAR, G. S. PATIL, S. S. MOHITE & M. A. SUTAR Dept. of Mechanical Engineering, Govt. College of Engineering, Karad, Dist- Satara,
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 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 informationAvailable online at ScienceDirect. Procedia Engineering 183 (2017 )
Available online at www.sciencedirect.com ScienceDirect Procedia Engineering 183 (2017 ) 369 374 17th International Conference on Sheet Metal, SHEMET17 Reverse analysis of scan strategies for controlled
More informationGUIDED WAVE PROPAGATION IN PLATE HAVING TRUSSED STRUCTURES
Jurnal Mekanikal June 2014, No 37, 26-30 GUIDED WAVE PROPAGATION IN PLATE HAVING TRUSSED STRUCTURES Lee Boon Shing and Zair Asrar Ahmad Faculty of Mechanical Engineering, University Teknologi Malaysia,
More informationModal Analysis of the Light Electric Sanitation Vehicle Frame
GRD Journals- Global Research and Development Journal for Engineering Volume 3 Issue 10 September 2018 ISSN: 2455-5703 Modal Analysis of the Light Electric Sanitation Vehicle Frame Lv Shaobin PG Student
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 informationAvailable online at ScienceDirect. Procedia Engineering 136 (2016 ) Dynamic analysis of fuel tank
Available online at www.sciencedirect.com ScienceDirect Procedia Engineering 136 (2016 ) 45 49 The 20 th International Conference: Machine Modeling and Simulations, MMS 2015 Dynamic analysis of fuel tank
More informationLMS Virtual.Lab Noise and Vibration
LMS Virtual.Lab Noise and Vibration LMS Virtual.Lab Noise and Vibration From component to system-level noise and vibration prediction 2 LMS Virtual.Lab Noise and Vibration LMS Virtual.Lab Noise and Vibration
More informationME Optimization of a Frame
ME 475 - Optimization of a Frame Analysis Problem Statement: The following problem will be analyzed using Abaqus. 4 7 7 5,000 N 5,000 N 0,000 N 6 6 4 3 5 5 4 4 3 3 Figure. Full frame geometry and loading
More informationDesign Optimization of a Weather Radar Antenna using Finite Element Analysis (FEA) and Computational Fluid Dynamics (CFD)
Design Optimization of a Weather Radar Antenna using Finite Element Analysis (FEA) and Computational Fluid Dynamics (CFD) Fernando Prevedello Regis Ataídes Nícolas Spogis Wagner Ortega Guedes Fabiano Armellini
More informationAnalysis of Pile Behaviour due to Damped Vibration by Finite Element Method (FEM)
ISSN 2395-1621 Analysis of Pile Behaviour due to Damped Vibration by Finite Element Method (FEM) #1 L.M.Sardesai, #2 G.A.Kadam 1 sardesaileena@rediffmail.com.com 2 ganeshkadam07@gmail.com #1 Mechanical
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 informationTopology Optimization and Analysis of Crane Hook Model
RESEARCH ARTICLE Topology Optimization and Analysis of Crane Hook Model Thejomurthy M.C 1, D.S Ramakrishn 2 1 Dept. of Mechanical engineering, CIT, Gubbi, 572216, India 2 Dept. of Mechanical engineering,
More informationANALYTICAL MODEL FOR THIN PLATE DYNAMICS
ANALYTICAL MODEL FOR THIN PLATE DYNAMICS Joyson Menezes 1, Kadir Kiran 2 and Tony L. Schmitz 1 1 Mechanical Engineering and Engineering Science University of North Carolina at Charlotte Charlotte, NC,
More informationANALYSIS AND OPTIMIZATION OF FLYWHEEL
Int. J. Mech. Eng. & Rob. Res. 2012 Sushama G Bawane et al., 2012 Research Paper ISSN 2278 0149 www.ijmerr.com Vol. 1, No. 2, July 2012 2012 IJMERR. All Rights Reserved ANALYSIS AND OPTIMIZATION OF FLYWHEEL
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 informationTWO-DIMENSIONAL PROBLEM OF THE THEORY OF ELASTICITY. INVESTIGATION OF STRESS CONCENTRATION FACTORS.
Ex_1_2D Plate.doc 1 TWO-DIMENSIONAL PROBLEM OF THE THEORY OF ELASTICITY. INVESTIGATION OF STRESS CONCENTRATION FACTORS. 1. INTRODUCTION Two-dimensional problem of the theory of elasticity is a particular
More informationIntroduction to Finite Element Analysis using ANSYS
Introduction to Finite Element Analysis using ANSYS Sasi Kumar Tippabhotla PhD Candidate Xtreme Photovoltaics (XPV) Lab EPD, SUTD Disclaimer: The material and simulations (using Ansys student version)
More informationStudy of Convergence of Results in Finite Element Analysis of a Plane Stress Bracket
RESEARCH ARTICLE OPEN ACCESS Study of Convergence of Results in Finite Element Analysis of a Plane Stress Bracket Gowtham K L*, Shivashankar R. Srivatsa** *(Department of Mechanical Engineering, B. M.
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 informationAvailable online at ScienceDirect. Procedia Engineering 161 (2016 ) Bohdan Stawiski a, *, Tomasz Kania a
Available online at www.sciencedirect.com ScienceDirect Procedia Engineering 161 (16 ) 937 943 World Multidisciplinary Civil Engineering-Architecture-Urban Planning Symposium 16, WMCAUS 16 Testing Quality
More informationSimulation of AJWSP10033_FOLDED _ST_FR
Phone: 01922 453038 www.hyperon-simulation-and-cad-services.co.uk Simulation of AJWSP10033_FOLDED _ST_FR Date: 06 May 2017 Designer: Study name: AJWSP10033_FOLDED_STATIC Analysis type: Static Description
More informationDESIGN AND OPTIMIZATION OF ROTARY TURRET PLATE OF POUCHER MACHINE
DESIGN AND OPTIMIZATION OF ROTARY TURRET PLATE OF POUCHER MACHINE Jigar G. Patel Institute of Technology, Nirma University, Ahmedabad 382481, India Email:14mmcc17@nirmuni.ac.in Mitesh B. Panchal Mechanical
More informationFEA Model Updating Using SDM
FEA l Updating Using SDM Brian Schwarz & Mark Richardson Vibrant Technology, Inc. Scotts Valley, California David L. Formenti Sage Technologies Santa Cruz, California ABSTRACT In recent years, a variety
More informationAnalysis of Crank End of Connecting Rod using Finite Element Method
Analysis of Crank End of Connecting Rod using Finite Element Method Mohammad Umair Zaki Faculty of Mechanical Engineering Noida International University Greater Noida, India e-mail-umairzaki@yahoo.com
More informationFinite Element Modal Analysis and Mesh Optimization of a Typical Turbo Fan Engine Fan Hub Frame
Finite Element Modal Analysis and Mesh Optimization of a Typical Turbo Fan Engine Fan Hub Frame Charles.G.Martin 1 and Dr. A. Arokkiaswamy 2 1,2 Department of Aeronautical Engg, DSCE, Shavige Malleshwara
More informationRAPID PROTOTYPING FOR SLING DESIGN OPTIMIZATION
RAPID PROTOTYPING FOR SLING DESIGN OPTIMIZATION Zaimović-Uzunović, N. * ; Lemeš, S. ** ; Ćurić, D. *** ; Topčić, A. **** * University of Zenica, Fakultetska 1, 72000 Zenica, Bosnia and Herzegovina, nzaimovic@mf.unze.ba
More informationTOPOLOGY OPTIMIZATION OF WING RIBS IN CESSNA CITATION
TOPOLOGY OPTIMIZATION OF WING RIBS IN CESSNA CITATION [1],Sathiyavani S [2], Arun K K [3] 1,2 student, 3 Assistant professor Kumaraguru College of technology, Coimbatore Abstract Structural design optimization
More informationEuropean Hyperworks Technology Conference 2010 Mesh and orientation dependance of FE models for dynamic simulations.
European Hyperworks Technology Conference 2010 Mesh and orientation dependance of FE models for dynamic simulations. Sébastien ROTH Jennifer OUDRY Hossein SHAKOURZADEH Influence of mesh density on a finite
More informationExercise 1. 3-Point Bending Using the GUI and the Bottom-up-Method
Exercise 1 3-Point Bending Using the GUI and the Bottom-up-Method Contents Learn how to... 1 Given... 2 Questions... 2 Taking advantage of symmetries... 2 A. Preprocessor (Setting up the Model)... 3 A.1
More informationCHAPTER 8 FINITE ELEMENT ANALYSIS
If you have any questions about this tutorial, feel free to contact Wenjin Tao (w.tao@mst.edu). CHAPTER 8 FINITE ELEMENT ANALYSIS Finite Element Analysis (FEA) is a practical application of the Finite
More informationStatic, Modal and Kinematic Analysis of Hydraulic Excavator
Static, Modal and Kinematic Analysis of Hydraulic Excavator Anil Jadhav Abhijit Kulkarni Tamilnadu,India-632014 Vinayak Kulkarni Prof. Ravi. K Assistant professor Mechanical department Abstract Hydraulic
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 informationAvailable online at ScienceDirect. Procedia Engineering 150 (2016 )
Available online at www.sciencedirect.com ScienceDirect Procedia Engineering 150 (2016 ) 866 870 International Conference on Industrial Engineering, ICIE 2016 Numerical Simulation of the Aluminum 6061-T6
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 informationSTATIC BENDING ANALYSIS OF AN ISOTROPIC CIRCULAR PLATE USING FINITE ELEMENT METHOD
International Journal Modern Trends in Engineering and Research www.ijmter.com e-issn :2349-9745, Date: 28-30 April, 20 STATIC BENDING ANALYSIS OF AN ISOTROPIC CIRCULAR PLATE USING FINITE ELEMENT METHOD
More informationStatic Structural Analysis and Optimization of Engine Mounting Bracket
ISSN 2395-1621 Static Structural Analysis and Optimization of Engine Mounting Bracket #1 Chandrashekhar B Tayde, #2 Prof. D. H. Burande 1 chandrashekhar.tayde@gmail.com 2 dhburande.scoe@sinhgad.edu #12
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 informationSIMULATION CAPABILITIES IN CREO
SIMULATION CAPABILITIES IN CREO Enhance Your Product Design with Simulation & Using digital prototypes to understand how your designs perform in real-world conditions is vital to your product development
More informationScienceDirect. Study of the Cardan Cross Using the Experimental and Analytical Method
Available online at www.sciencedirect.com ScienceDirect Procedia Engineering 100 (2015 ) 499 504 25th DAAAM International Symposium on Intelligent Manufacturing and Automation, DAAAM 2014 Study of the
More information1.992, 2.993, 3.04, 10.94, , Introduction to Modeling and Simulation Prof. F.-J. Ulm Spring FE Modeling Example Using ADINA
1.992, 2.993, 3.04, 10.94, 18.996, 22.091 Introduction to Modeling and Simulation Prof. F.-J. Ulm Spring 2002 FE Modeling Example Using ADINA H Hgρ w ργ H = B = 10 m g = 9.81 m/s 2 ρ = 2400 kg/m 3 ρ w
More informationUsing Computer Aided Engineering Processes in Packaging Design Development
Using Computer Aided Engineering Processes in Packaging Design Development Jose Martinez, Miguel Angel Garcia Jose Luis Moreno Vicencio & Hugo Miranda Mabe, Mexico Mahesh Patel, Andrew Burkhalter, Eric
More informationIJREAS VOLUME 6, ISSUE 4 (April, 2016) (ISSN ) International Journal of Research in Engineering and Applied Sciences (IMPACT FACTOR 6.
THICKNESS OPTIMIZATION OF CAR FRAME FOR STRENGTH Manoj Kumar Singh 1 R.Hussain Vali 2 P.Yagnasri 3 Associate Professor Assistant Professor Assistant Professor ABSTRACT Department of mechanical engineering,,
More informationPerformance of railway track system under harmonic loading by finite element method
Performance of railway track system under harmonic by finite element method Ammar Shuber 1, Mohammed Hamood 1, * and Walaa Jawad 1 1 Building and Construction Engineering Department, University of Technology,
More informationDesign of three-dimensional photoelectric stylus micro-displacement measuring system
Available online at www.sciencedirect.com Procedia Engineering 15 (011 ) 400 404 Design of three-dimensional photoelectric stylus micro-displacement measuring system Yu Huan-huan, Zhang Hong-wei *, Liu
More informationStress Concentration Factors
CONSEIL INTERNATIONAL DES MACHINES A COMBUSTION INTERNATIONAL COUNCIL ON COMBUSTION ENGINES CO-ORDINATING WORKING GROUP "CLASSIFICATION SOCIETIES DIESEL" (WG2) Proposal by CIMAC WG4 11th May 2012 IACS
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 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 informationFinite Element Modeling and Multiphysics Simulation of Air Coupled Ultrasonic with Time Domain Analysis
More Info at Open Access Database www.ndt.net/?id=15194 Finite Element Modeling and Multiphysics Simulation of Air Coupled Ultrasonic with Time Domain Analysis Bikash Ghose 1, a, Krishnan Balasubramaniam
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 informationRobust Design Methodology of Topologically optimized components under the effect of uncertainties
Robust Design Methodology of Topologically optimized components under the effect of uncertainties Joshua Amrith Raj and Arshad Javed Department of Mechanical Engineering, BITS-Pilani Hyderabad Campus,
More informationNew paradigm for MEMS+IC Co-development
New paradigm for MEMS+IC Co-development MEMS 진보된스마트세상을만듭니다. Worldwide First MEMS+IC Co-development Solution New paradigm for MEMS+IC Co-development A New Paradigm for MEMS+IC Development MEMS design
More informationA design influence on the mechanical compliance and fracture resistance of railway wheel
Applied and Computational Mechanics 5 (2011) 197 204 A design influence on the mechanical compliance and fracture resistance of railway wheel P. Navrátil a,,p.janíček a, L. Brabenec a, M. Matug a, P. Marcián
More informationCombine Harvester Engine Mounting Frame Optimization
ISSN 2395-1621 Combine Harvester Engine Mounting Frame Optimization #1 Ravikumar Anburaj 1 ravikumar4026@gmail.com # 1Alard College of Engineering and Management, pune, India M. E. (Design Engineering),
More informationIMPROVED SIF CALCULATION IN RIVETED PANEL TYPE STRUCTURES USING NUMERICAL SIMULATION
26 th ICAF Symposium Montréal, 1 3 June 2011 IMPROVED SIF CALCULATION IN RIVETED PANEL TYPE STRUCTURES USING NUMERICAL SIMULATION S.C. Mellings 1, J.M.W. Baynham 1 and T.J. Curtin 2 1 C.M.BEASY, Southampton,
More information