Analysis and Optimization for a Focal Plane Mechanism of a Large Sky Area Multi-object Fiber Spectroscopic Telescope
|
|
- Horatio Ethelbert Beasley
- 5 years ago
- Views:
Transcription
1 Analysis and Optimization for a Focal Plane Mechanism of a Large Sky Area Multi-object Fiber Spectroscopic Telescope Abstract Guo-min Wang, Guo-ping Li, Xiang-qun Cui, Zheng-qiu Yao National Astronomical Observatories of Chinese Academy of Sciences Nanjing Institute of Astronomical Optics & Technology The Large Sky Area Multi-object Fiber Spectroscopic Telescope (LAMOST), a national major scientific project in the process of construction in China, is a special reflecting Schmidt telescope with 4- meter aperture and 5 field of view. There are three sub-assemblies: the reflecting Schmidt correcting plate, the focal plane mechanism and the spherical primary mirror. The focal plane mechanism is the assembly by which the physical information of the celestial bodies can be obtained from optical spectroscopies. The static and dynamic performance of the focal plane mechanism have a significant effect on the ability of the telescope to obtain the optical spectra of various celestial bodies. So, with the help of ANSYS, the optimization of the focal plane mechanism according to the static and dynamic characteristics requested by specifications is presented in this paper, along with the analysis of truss number, deformation in different compensation positions and contribution to the total deformation of each component. The results of study show that a feasible and reliable design scheme can be achieved. Introduction This paper describes the results of a finite element analysis in investigating of the focal plane mechanism of LAMOST using the finite element software ANSYS. The static flexures of the structure has a significant effect on the ability of the structure to sustain its precise position. According to Reference [2], the maximum deflection of focal plate, namely, the center of focal plate deflecting the optical axis, is 0.2mm, and the tilt angle caused by the supporting structures is less than 10. These specifications could be met by optimizing the supporting structure, such as the number and section properties of truss, the thickness of the steel plate, and so on. Another design feature that has been investigated in this paper is the dynamic performance of the focal plane mechanism. With a high structure natural frequency (and the associated wider servo bandwidth)the possibility of the structure being dynamically coupled to vibrations generated by the vibration source, such as wind loading, is reduced. A stiff structure will allow higher servo gain and higher acceleration rates giving faster setting times which will increase the efficiency of observing. According to Reference [2],the lowest eigenfequency of the whole mechanism is above 10H Z. Focal Plane Mechanism The focal plane mechanism is shown in Figure1. It consists of five major components: the focal plate, the trusses, the rotating axis, the frame and the base. The focal plate, 2 tons in weight including the fibers and 1.75m in diameter, is supported from the rotating axis by trusses. During the observation, the focal plate will rotate to compensate the rotation of the earth, and when observing different sky area, the focal plate should tilt for a small angle. The rotating axis is supported from frame by bearings and driving rollers which drive the rotating axis to move. The frame is connected to the stiff base which defines the location of the whole mechanism.
2 Figure 1 - The Focal Plane Mechanism Schematically Analysis and Optimization of Focal Plane Mechanism Finite Element Analysis Model With the help of ANSYS parametric design language, the finite element model of the focal plane mechanism has been developed in terms of parameters (variables). Approximately 4486 nodes and 5433 elements are used for the model, using solid45 to simulate the focal plate,drive disc,drive rollers and bearing base, using pipe16 to simulate the trusses and using shell63 to simulate the rotating axis and frame plates, and the element model is shown in Figure 2.
3 Figure 2 - The Finite Element Model Of Local Plane Mechanism Boundary conditions: the rotating axis is supported from the frame by bearings and drive rollers, so the connecting nodes between drive disc and drive rollers are coupled in radial direction, and the connecting nodes between rotating axis and bearing bracket are coupled in axial direction and radial direction. The boundary conditions are shown in Figure 2. Just as Figure 1 shows that the whole focal plane mechanism is supported from the base by three pedals which adjust the position of the focal plane to ensure its center coincides with the optical axis. So three transition degrees of freedom of the nodes connecting to the three pedals in the bottom plate of the frame are constrained. In order to investigate the graviational deformation, a 1.0g gravity field is applied to the finite element model with the whole focal plane mechanism tilting 25 from horizontal direction. Analysis of Truss Number On the basis of the above analysis of the focal plane mechanism, it should be noted that the trusses,supporting the focal plate whose weight is about 2 tons, will tilt under the weight loading of focal plate. This tilt will affect the focal plate position, and result in the deflection and tilt of focal plate. Changing the truss number has a pronounced effect on the deflection and tilt of the focal plate. During the calculation, the focal plate is assumed to be a rigid body because the self-deformation of focal plate due to its own weight has been calculated by others. For simplification, the field rotator is separated from the mechanism and other parameters are assumed to be constants. The element model(solid45, pipe16, shell63, shown in Figure 3, was run with different truss number. The results are given in Table 1.
4 Figure 3 - The Model for Truss Calculation Table 1 - Analysis of Truss Number truss number ρ max θ max (μm) ( ) ρ max deflection of focal plate θ max tilt angle of focal plate Figure 4 shows the curve of the variation of focal plate deflection ρ max and tilt angleθ max with the truss number. It is found that, at first, an increase in the truss number obviously results in a reduction in the deflection ρ max and tilt angleθ max, and then, with the increasing of the truss number, theρ max and θ max are increasing with the truss number. Here, the increasing of truss number has two effects. One is to increase the flexural stiffness of the structure. So the more truss number, the less deflection and tilt angle. On the other hand, with the increasing of truss number, the weight of the structure increases too. The increasing weight results in the increasing of deflection and tilt angle. As can be seen in Figure 4, the curves of the deflection and tilt angle versus the truss number has a minimum. The optimal number of truss is 10.
5 t r uss number Figure 4 - ρ max θ max Versus Truss Number Optimization of Structure Static and Dynamic Characteristics Design Variables (DVs) are independent quantities that are varied in order to achieve the optimum design. The design variables of the focal plane mechanism are given in Table 2 and illustrated in Figure 5. The upper and lower limits are specified to serve as "constraints" on the design variables. Table 2 - Optimization Design Variables DVs name range of variation(mm) memo t2 10~30 thickness of truss tube d2 80~120 outer diameter of truss t4 10~30 thickness of rotation axis tube l6 100~400 length of bearing base t81 10~120 thickness of top frame plate t82 40~120 thickness of lateral frame plate t83 20~120 thickness of middle frame plate t84 40~120 thickness of bottom frame plate top-l 100~800 length of square hole on top frame plate top-w 100~600 width of square hole on top frame plate mid-l 100~800 length of square hole on middle frame plate mid-w 100~1000 width of square hole on middle frame plate lat-l 100~800 length of square hole on lateral frame plate lat-w 100~1000 width of square hole on lateral frame plate
6 Figure 5 - Design Variables Illustration State Variables (SVs) are quantities that constrain the design. State variables are given in Table 3. Table 3 - Optimization State Variables SVs name max. and min. limit memo ρ max 0.02mm maximum deflection θ max 10 maximum tilt angle σ r4 240MPa maximum equivalent stress of whole structure fre1 10H Z first eigenfrequency
7 The total volume of the structure is defined as objective function. Comparing with defining the weight as objective function, defining total volume of the structure as objective function will save some computer time because the mass matrix is not calculated. The subproblem approximation method, described as an advanced zero-order method in that it requires only the values of the dependent variables, and not their derivatives, is used to optimize the parameters. At first, some feasible designs, satisfying all specified constrains on the SVs as well as constrains on the DVs, was generated using random design generation tool which performs 60 analysis loops using random design variable values for each loop, then based on the feasible designs the subproblem approximation method is used to optimize the parameters. The optimization results are given in Table 4. Besides, the initial solution is given in Table 4, too. Table 4 - Optimization Results initial solution optimized solution memo t2(mm) thickness of truss tube d2(mm) outer diameter of truss t4(mm) thickness of rotation axis tube l6(mm) length of bearing base t81(mm) thickness of top frame plate t82(mm) thickness of lateral frame plate t83(mm) thickness of middle frame plate t84(mm) thickness of bottom frame plate top-l(mm) length of square hole on top plate top-w(mm) width of square hole on top plate mid-l(mm) length of square hole on middle plate mid-w(mm) width of square hole on middle plate lat-l(mm) length of square hole on lateral plate lat-w(mm) width of square hole on lateral plate ρ max (μm) maximum deflection θ max ( ) maximum tilt angle σ r4 (MPa) maximum 4th equivalent stress fre1(h Z ) first eigenfrequency volume(m 3 ) total volume weight(t) total weight Comparing the optimized solution with the initial solution. it is clear that the initial solution can not meet all the specifications. Especially, through optimization, the dynamic performance of the structure is improved largely. The first eigenfrequency of the structure increased from 5.09H Z to 11.10H Z.
8 Analysis of Different compensating position Due to the rotation of the earth, the pointing and tracking of the telescope should be done by the rotation in altitude and azimuth of the Schmidt corrector, at the same time the focal plane should be rotated for certain angle to compensate the rotation of the field of view. So the deflection and tilt angle of focal plate are different with the focal plate in different positions. 360range is taken into account and from the position shown in Fig.2 every counter clockwise 27is a calculation position. The finite element model is shown in Fig. 2 and the calculation results are given in Table 5. Figure 6 and Figure7 respectively show the variation of deflection ρ max and tilt angleθ max with the different compensation positions. Table 5 - Deflection And Tilt Angle With Different Compensation Position ρ max (μm) θ max ( ) ρ max (μm) θ max ( ) Table 5 shows that the variation in deflection ρ max and titl angleθ max are little when the focal plate is in different compensation position. Good results are achieved; 0.856μm for deflection and for tilt angle. Figure 6 - Deflection Versus Different Compensation Position
9 Figure 7 - Tilt Angle Versus Different Compensation Position Contribution to Total Deformation from Components The focal plane mechanism mainly consists of focal plate, trusses, rotating axis, bearing base and frame. The role each part played to the total deformation is different. The focal plate is assumed to be a rigid plate, so it has no effect on the total deformation. The deflection and tilt angle arose from each components are investigated and the results are given in Table 6. Table 6 - Contribution To Total Deformation From Substruction substruction name deflection (μm) contribution (%) tilt angle ( ) contribution (%) truss rotating axis bearing base frame total The results in Table 6 show that the role of each part played in the whole deformation are different. The truss, rotating axis and bearing base make the focal plate deflect down and tilt clockwise, while the frame makes the focal plate uplift and tilt count clockwise. So some of the deformation caused by the truss and rotating axis are offset by the deformation caused by the frame. The frame plays an important role in the focal plane mechanism deformation. Investigation of the Mechanism Eigenfrequency The 1st~10th eigenfrequency of the focal plane mechanism are calculated with the design parameters optimized above and the results are given in Table 7. The first four eigenmodes are shown in Figure 8.
10 Table 7 - First 10 Eigenfrequency Of Mechanism eigenfrequency(h Z ) eigenfrequency(h Z ) Lateral mode H Z Fore-aft mode H Z Torsion mode H Z Lateral mode H Z Figure 8 - First Four Eigenmodes
11 Conclusions The work described here has shown the following: Through optimization, a feasible and reliable design set, meeting all specified static and dynamic characteristics, can be achieved. The lowest eigenfrequencies of local plane mechanism are: (a) the lateral mode of the local plane mechanism, H Z. (b) the fore-aft mode of the local plane mechanism, H Z. (c) the torsional mode of the local plane mechanism, H Z. Because the gravity-deformation of focal plate is calculated respectively by others, the total deformation should be the sum of the deformation calculated in this paper and the focal plate gravity-deformation. The variation in deflection ρ max and titl angleθ max are small when the focal plate is in different compensation position during a full circle. The variation in deflection is 0.856μm and the variation in tilt angle is only The contributions of each component of the mechanism to the total deflection and tilt angle are different. The contribution of truss, rotating axis, bearing base and frame to the total deformation are about 24%, 18%, 3% and 55% respectively. The contribution of truss, rotating axis, bearing base and frame to the total tilt angle are about 17%, 21%, 2% and 60% respectively. That is to say, the frame plays an important role in the focal plane mechanism deformation. References [1]Shou-guan Wang, Ding-qiang Su, Yao-quan Chu, Xiang-qun Cui and Ya-nan Wang, Special configuration of a very large Schmidt telescope for extensive astronomical spectroscopic observation, Applied Optics, Vol. 35, No.25, , 1996 [ 2 ] Guo-ping Li, Focal plane structure, focus control and image plane rotation and compensatory system, LAMOST Technology Report, [3]SAS IP, Inc., ANSYS User's manual for Revision 5.0 Volume Ⅲ Procedures, 1992 [4]SAS IP, Inc., ANSYS Theory Reference, Seventh Edition. [5]K. Raybould, Finite Element Analysis of the UKLT Structure, Oxford Project Team, 11 April 90 [6]Keith Raybould, Paul Gillett, Peter Hatton, Gordon Pentland, Mike Sheehan, Mark Warner, Gemini Telescope Structure Design, 376/SPIE Vol.2199 [7]Xin-he Zhen, Mechanical Optimization Design, Southeast University, [8]Zheng-qiu Yao, Guo-ping Li, The Tracking System of LAMOST Telescope, SPIE, 1998
Wind Vibration Analysis Giant Magellan Telescope
Wind Vibration Analysis Giant Magellan Telescope prepared for Carnegie Observatories 813 Santa Barbara Street Pasadena, CA 91101 prepared by Simpson Gumpertz & Heger Inc. 41 Seyon Street, Building 1, Suite
More informationII. FINITE ELEMENT MODEL OF CYLINDRICAL ROLLER BEARING
RESEARCH INVENTY: International Journal of Engineering and Science ISSN: 2278-4721, Vol. 1, Issue 1 (Aug 2012), PP 8-13 www.researchinventy.com Study of Interval of Arc Modification Length of Cylindrical
More informationSALT TELESCOPE INSTRUMENT STRUCTURE ANALYSIS
CONTRACT NO.: 5258 TASK NO.: 780 SALT TELESCOPE INSTRUMENT STRUCTURE ANALSIS SAI-RPT-438 10/05/01 REVISION 1.0 Prepared by: Swales Aerospace 5050 Powder Mill Road Beltsville, MD 20705 DOCUMENT CHANGE RECORD
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 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 informationNathan Loewen AMEC Dynamic Structures January 17, AMEC Corporate Profile. AMEC Dynamic Structures Ltd:
CCAT Enclosure Nathan Loewen AMEC Dynamic Structures January 17, 2005 AMEC Corporate Profile AMEC Dynamic Structures Ltd: Located in Vancouver, Canada Design/build steel fabricating firm Specialize in
More informationAPPENDIX 4.5.C CONCEPTUAL DESIGN OF PRIMARY MIRROR SEGMENT SUPPORT SYSTEM OF THE GSMT POINT DESIGN
APPENDIX 4.5.C CONCEPTUAL DESIGN OF PRIMARY MIRROR SEGMENT SUPPORT SYSTEM OF THE GSMT POINT DESIGN Report prepared for New Initiatives Office, October 2001. AURA New Initiatives Office 30m Telescope Project
More informationAnalysis of Contact Stress between Cylindrical Roller and Outer Ring Raceway with Taper Error Using ANSYS
; ISSN 1913-1844 E-ISSN 1913-1852 Published by Canadian Center of Science and Education Analysis of Contact Stress between Cylindrical Roller and Outer Ring Raceway with Taper Error Using ANSYS Xintao
More informationStudy on Digitized Measuring Technique of Thrust Line for Rocket Nozzle
Study on Digitized Measuring Technique of Thrust Line for Rocket Nozzle Lijuan Li *, Jiaojiao Ren, Xin Yang, Yundong Zhu College of Opto-Electronic Engineering, Changchun University of Science and Technology,
More informationTop Layer Subframe and Node Analysis
Top Layer Subframe and Node Analysis By Paul Rasmussen 2 August, 2012 Introduction The top layer of the CCAT backing structure forms a critical interface between the truss and the primary subframes. Ideally
More informationASSIGNMENT 1 INTRODUCTION TO CAD
Computer Aided Design(2161903) ASSIGNMENT 1 INTRODUCTION TO CAD Theory 1. Discuss the reasons for implementing a CAD system. 2. Define computer aided design. Compare computer aided design and conventional
More informationOptimization and Simulation of Machining Parameters in Radial-axial Ring Rolling Process
International Journal of Computational Intelligence Systems, Vol.4, No. 3 (May, 0). Optimization and Simulation of Machining Parameters in Radial-axial Ring Rolling Process Shuiyuan Tang, Jiping Lu *,
More informationAssembly of thin gratings for soft x-ray telescopes
Assembly of thin gratings for soft x-ray telescopes Mireille Akilian 1, Ralf K. Heilmann and Mark L. Schattenburg Space Nanotechnology Laboratory, MIT Kavli Institute for Astrophysics and Space Research,
More informationANALYSIS OF BOX CULVERT - COST OPTIMIZATION FOR DIFFERENT ASPECT RATIOS OF CELL
ANALYSIS OF BOX CULVERT - COST OPTIMIZATION FOR DIFFERENT ASPECT RATIOS OF CELL M.G. Kalyanshetti 1, S.A. Gosavi 2 1 Assistant professor, Civil Engineering Department, Walchand Institute of Technology,
More informationTutorial 1: Welded Frame - Problem Description
Tutorial 1: Welded Frame - Problem Description Introduction In this first tutorial, we will analyse a simple frame: firstly as a welded frame, and secondly as a pin jointed truss. In each case, we will
More informationNUMERICAL ANALYSIS OF ROLLER BEARING
Applied Computer Science, vol. 12, no. 1, pp. 5 16 Submitted: 2016-02-09 Revised: 2016-03-03 Accepted: 2016-03-11 tapered roller bearing, dynamic simulation, axial load force Róbert KOHÁR *, Frantisek
More informationDescription of the Optomechanical
Description of the Optomechanical Design for the PFC Project name WEAVE Release Final: Version 1.1 Date: 06 July 2013 Author(s): Owner: Client: Document Number: Kevin Dee Don Carlos Abrams WEAVE Consortium
More informationKISSsoft 03/2013 Tutorial 5
KISSsoft 03/2013 Tutorial 5 Shaft analysis KISSsoft AG Rosengartenstrasse 4 8608 Bubikon Switzerland Tel: +41 55 254 20 50 Fax: +41 55 254 20 51 info@kisssoft.ag www.kisssoft.ag Contents 1 Starting KISSsoft...
More informationFinite Element Analysis Dr. B. N. Rao Department of Civil Engineering Indian Institute of Technology Madras. Module - 01 Lecture - 15
Finite Element Analysis Dr. B. N. Rao Department of Civil Engineering Indian Institute of Technology Madras Module - 01 Lecture - 15 In the last class we were looking at this 3-D space frames; let me summarize
More informationFB-MULTIPIER vs ADINA VALIDATION MODELING
FB-MULTIPIER vs ADINA VALIDATION MODELING 1. INTRODUCTION 1.1 Purpose of FB-MultiPier Validation testing Performing validation of structural analysis software delineates the capabilities and limitations
More informationManual. Ansys Exercise. Offshore Wind Farm Design
Manual for the Ansys Exercise Accompanying the Offshore Wind Farm Design Assignment Contents Contents... i 1. Introduction... 1 2. Brief Overview of ANSYS... 2 3. Overview of the input files for the ANSYS
More information1 P-H tilt 1 mm P-H decenter Coma circle radius ( ) 1 10 Coma circle radius ( µm)
Chapter 28 HRMA Tilts at XRCF William Podgorski In this section we discuss HRMA rigid body misalignments (relative P-H tilt and decenter). Data is presented from the optical alignments at Kodak, from the
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 informationAnalysis of fluid-solid coupling vibration characteristics of probe based on ANSYS Workbench
Analysis of fluid-solid coupling vibration characteristics of probe based on ANSYS Workbench He Wang 1, a, Changzheng Zhao 1, b and Hongzhi Chen 1, c 1 Shandong University of Science and Technology, Qingdao
More informationGEMINI 8-M Telescopes Project
GEMINI 8-M Telescopes Project TN-O-G0022 Report on Deformation of the Primary Mirror Cell and Its Effect on Mirror Figure Assuming the Use of an Overconstrained Axial Defining System Larry Stepp Optics
More informationLS-DYNA s Linear Solver Development Phase1: Element Validation Part II
LS-DYNA s Linear Solver Development Phase1: Element Validation Part II Allen T. Li 1, Zhe Cui 2, Yun Huang 2 1 Ford Motor Company 2 Livermore Software Technology Corporation Abstract This paper continues
More informationInvestigation of Structural Behavior due to. Bend-Twist Couplings in Wind Turbine Blades
Investigation of Structural Behavior due to Bend-Twist Couplings in Wind Turbine Blades V.A. Fedorov* 1, N. Dimitrov*, C. Berggreen*, S. Krenk*, K. Branner and P. Berring * Department of Mechanical Engineering,
More informationDRONACHARYA GROUP OF INSTITUTIONS, GREATER NOIDA Department of CIVIL Engineering Semester: III Branch: CIVIL Session: Subject: Surveying Lab
DRONACHARYA GROUP OF INSTITUTIONS, GREATER NOIDA Department of CIVIL Engineering Semester: III Branch: CIVIL Session: 2015-16 Subject: Surveying Lab 1. To measure bearings of a closed traverse by prismatic
More informationNumerical Simulation of Middle Thick Plate in the U-Shaped Bending Spring Back and the Change of Thickness
Send Orders for Reprints to reprints@benthamscience.ae 648 The Open Mechanical Engineering Journal, 2014, 8, 648-654 Open Access Numerical Simulation of Middle Thick Plate in the U-Shaped Bending Spring
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 informationIntroduction to FEM Modeling
Total Analysis Solution for Multi-disciplinary Optimum Design Apoorv Sharma midas NFX CAE Consultant 1 1. Introduction 2. Element Types 3. Sample Exercise: 1D Modeling 4. Meshing Tools 5. Loads and Boundary
More informationMODELING AND ANALYSIS OF LATTICE TOWERS WITH MORE ACCURATE MODELS
Advanced Steel Construction Vol. 3, No. 2, pp. 565-582 (2007) 565 MODELING AND ANALYSIS OF LATTICE TOWERS WITH MORE ACCURATE MODELS Wenjiang Kang 1, F. Albermani 2, S. Kitipornchai 1 and Heung-Fai Lam
More informationDevelopment of Lightweight Engine Mounting Cross Member
Development of Lightweight Engine Mounting Cross Member Nitin Babaso Bodhale Team Lead Tata Technologies Ltd Pimpri Pune-411018, India. nitin.bodhale@tatatechnologies.com Jayeshkumar Raghuvanshi Sr. Team
More informationMAE Advanced Computer Aided Design. 01. Introduction Doc 02. Introduction to the FINITE ELEMENT METHOD
MAE 656 - Advanced Computer Aided Design 01. Introduction Doc 02 Introduction to the FINITE ELEMENT METHOD The FEM is A TOOL A simulation tool The FEM is A TOOL NOT ONLY STRUCTURAL! Narrowing the problem
More informationSolved with COMSOL Multiphysics 4.2
Pratt Truss Bridge Introduction This example is inspired by a classic bridge type called a Pratt truss bridge. You can identify a Pratt truss by its diagonal members, which (except for the very end ones)
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 informationDesign of Arm & L-bracket and It s Optimization By Using Taguchi Method
IOSR Journal of Mechanical and Civil Engineering (IOSR-JMCE) e-issn: 2278-1684,p-ISSN: 2320-334X PP. 28-38 www.iosrjournals.org Design of Arm & L-bracket and It s Optimization By Using Taguchi Method S.
More informationE and. L q. AE q L AE L. q L
STRUTURL NLYSIS [SK 43] EXERISES Q. (a) Using basic concepts, members towrds local axes is, E and q L, prove that the equilibrium equation for truss f f E L E L E L q E q L With f and q are both force
More informationDesign of Low Cost Parabolic Solar Dish Concentrator
ABSTRACT Design of Low Cost Parabolic Solar Dish Concentrator Hamza Hijazi, Ossama Mokhiamar Mechanical Engineering Department, Faculty of Engineering Beirut Arab University Beirut, P.O. Box 11-5020 Reyad
More informationLab#5 Combined analysis types in ANSYS By C. Daley
Engineering 5003 - Ship Structures I Lab#5 Combined analysis types in ANSYS By C. Daley Overview In this lab we will model a simple pinned column using shell elements. Once again, we will use SpaceClaim
More informationGuangxi University, Nanning , China *Corresponding author
2017 2nd International Conference on Applied Mechanics and Mechatronics Engineering (AMME 2017) ISBN: 978-1-60595-521-6 Topological Optimization of Gantry Milling Machine Based on Finite Element Method
More information6th International Conference on Management, Education, Information and Control (MEICI 2016)
The Simulation Study of the Locking Device in Platform Screen Door System Haiying Zhang 1 a, Weiyan Xu 1 b* and Xiangyan Yu 2,c 1 Qingdao Binhai University, Qingdao, China, 266555 2 Qingdao Qian wan Container
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 informationHARP-NEF Front End Assembly
Science Fibers HARP-NEF Front End Assembly Calib Fibers HARPN Front End Assembly ( w/ Partial Cover Plates ) HARPN Front End Assembly 1 HARP-NEF Front End Assembly Roger Eng December 6, 2007 2 HARP-NEF
More informationPTC Newsletter January 14th, 2002
PTC Email Newsletter January 14th, 2002 PTC Product Focus: Pro/MECHANICA (Structure) Tip of the Week: Creating and using Rigid Connections Upcoming Events and Training Class Schedules PTC Product Focus:
More informationDevelopment of Backhoe Machine By 3-D Modelling using CAD Software and Verify the Structural Design By using Finite Element Method
IJIRST International Journal for Innovative Research in Science & Technology Volume 2 Issue 1 June 2015 ISSN (online): 2349-6010 Development of Backhoe Machine By 3-D Modelling using CAD Software and Verify
More informationSAMCEF for ROTORS. Chapter 3.2: Rotor modeling. This document is the property of SAMTECH S.A. MEF A, Page 1
SAMCEF for ROTORS Chapter 3.2: Rotor modeling This document is the property of SAMTECH S.A. MEF 101-03-2-A, Page 1 Table of contents Introduction Introduction 1D Model 2D Model 3D Model 1D Models: Beam-Spring-
More informationN-05 Magnetic Compass
Guideline No.N-05 (201510) N-05 Magnetic Compass Issued date: 20 th October, 2015 China Classification Society Foreword This Guideline is a part of CCS Rules, which contains technical requirements, inspection
More informationHigh Precision Lens Mounting
High Precision Lens Mounting APOMA Tucson Tech Workshop, 10-11 November, 2016 Presentation by Frédéric Lamontagne Institut national d optique (INO) Québec City, Canada 2016 Outline 1. Review of common
More informationMULTI-SPRING REPRESENTATION OF FASTENERS FOR MSC/NASTRAN MODELING
MULTI-SPRING REPRESENTATION OF FASTENERS FOR MSC/NASTRAN MODELING Alexander Rutman, Ph. D, Joseph Bales-Kogan, M. Sc. ** Boeing Commercial Airplane Group Strut Structures Technology MS K95-04 380 South
More informationINNWIND.EU 10MW JACKET INTERFACE DOCUMENT FOR PRELIMINARY JACKET DESIGN
Intended for InnWind.EU Document type Engineering Report Date May 2013 Document no. 341_0001(2) Revision 2 INNWIND.EU 10MW JACKET INTERFACE DOCUMENT FOR PRELIMINAR JACKET DESIGN INNWIND.EU 10MW JACKET
More informationShell-to-Solid Element Connector(RSSCON)
WORKSHOP 11 Shell-to-Solid Element Connector(RSSCON) Solid Shell MSC.Nastran 105 Exercise Workbook 11-1 11-2 MSC.Nastran 105 Exercise Workbook WORKSHOP 11 Shell-to-Solid Element Connector The introduction
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 information11.0 Measurement of Spindle Error Motion
11.0 Measurement of Spindle Error Motion 11.1 Introduction The major spindle error motion is caused by the alignment of the spindle rotational axis, the centerline of the tool holder and the centerline
More informationDesign of a Flexural Joint using Finite Element Method
Design of a Flexural Joint using Finite Element Method Abdullah Aamir Hayat, Adnan Akhlaq, M. Naushad Alam Abstract This paper presents the design and analysis of a compliant mechanism using hyperbolic
More informationKeywords: truck frame, parametric modeling, cross-section.
Key Engineering Materials Online: 2011-01-20 ISSN: 1662-9795, Vols. 460-461, pp 534-539 doi:10.4028/www.scientific.net/kem.460-461.534 2011 Trans Tech Publications, Switzerland A Research and Application
More informationFINITE ELEMENT MODELLING OF A TURBINE BLADE TO STUDY THE EFFECT OF MULTIPLE CRACKS USING MODAL PARAMETERS
Journal of Engineering Science and Technology Vol. 11, No. 12 (2016) 1758-1770 School of Engineering, Taylor s University FINITE ELEMENT MODELLING OF A TURBINE BLADE TO STUDY THE EFFECT OF MULTIPLE CRACKS
More informationIntroduction. Section 3: Structural Analysis Concepts - Review
Introduction In this class we will focus on the structural analysis of framed structures. Framed structures consist of components with lengths that are significantly larger than crosssectional areas. We
More information(Based on a paper presented at the 8th International Modal Analysis Conference, Kissimmee, EL 1990.)
Design Optimization of a Vibration Exciter Head Expander Robert S. Ballinger, Anatrol Corporation, Cincinnati, Ohio Edward L. Peterson, MB Dynamics, Inc., Cleveland, Ohio David L Brown, University of Cincinnati,
More informationOptimal Support Solution for a Meniscus Mirror Blank
Preliminary Design Review Optimal Support Solution for a Meniscus Mirror Blank Opti 523 Independent Project Edgar Madril Scope For this problem an optimal solution for a mirror support is to be found for
More informationLearning Module 8 Shape Optimization
Learning Module 8 Shape Optimization What is a Learning Module? Title Page Guide A Learning Module (LM) is a structured, concise, and self-sufficient learning resource. An LM provides the learner with
More informationDiffraction. Single-slit diffraction. Diffraction by a circular aperture. Chapter 38. In the forward direction, the intensity is maximal.
Diffraction Chapter 38 Huygens construction may be used to find the wave observed on the downstream side of an aperture of any shape. Diffraction The interference pattern encodes the shape as a Fourier
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 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 informationANSYS AIM Tutorial Structural Analysis of a Plate with Hole
ANSYS AIM Tutorial Structural Analysis of a Plate with Hole Author(s): Sebastian Vecchi, ANSYS Created using ANSYS AIM 18.1 Problem Specification Pre-Analysis & Start Up Analytical vs. Numerical Approaches
More informationWP1 NUMERICAL BENCHMARK INVESTIGATION
WP1 NUMERICAL BENCHMARK INVESTIGATION 1 Table of contents 1 Introduction... 3 2 1 st example: beam under pure bending... 3 2.1 Definition of load application and boundary conditions... 4 2.2 Definition
More informationA study on automation of modal analysis of a spindle system of machine tools using ANSYS
Journal of the Korea Academia-Industrial cooperation Society Vol. 16, No. 4 pp. 2338-2343, 2015 http://dx.doi.org/10.5762/kais.2015.16.4.2338 ISSN 1975-4701 / eissn 2288-4688 A study on automation of modal
More informationLecture 17. ENGR-1100 Introduction to Engineering Analysis CENTROID OF COMPOSITE AREAS
ENGR-00 Introduction to Engineering Analysis Lecture 7 CENTROID OF COMPOSITE AREAS Today s Objective : Students will: a) Understand the concept of centroid. b) Be able to determine the location of the
More informationA numerical study of multi-pass design based on Bezier curve in conventional spinning of spherical components
A numerical study of multi-pass design based on Bezier curve in conventional spinning of spherical components Tian Gan 1, Qingshuai Kong 1, Zhongqi Yu 1, Yixi Zhao 1 and Xinmin Lai 1 1 Shanghai Jiao Tong
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 informationCylinders in Vs An optomechanical methodology Yuming Shen Tutorial for Opti521 November, 2006
Cylinders in Vs An optomechanical methodology Yuming Shen Tutorial for Opti521 November, 2006 Introduction For rotationally symmetric optical components, a convenient optomechanical approach which is usually
More informationarxiv: v1 [astro-ph.im] 2 May 2018
Research in Astronomy and Astrophysics manuscript no. (L A TEX: ms-raa-- R.tex; printed on May, ; :) arxiv:.v [astro-ph.im] May Investigating the Efficiency of the Beijing Faint Object Spectrograph and
More information2: Static analysis of a plate
2: Static analysis of a plate Topics covered Project description Using SolidWorks Simulation interface Linear static analysis with solid elements Finding reaction forces Controlling discretization errors
More informationA Six Degree of Freedom, Piezoelectrically Actuated Translation Stage
A Six Degree of Freedom, Piezoelectrically Actuated Translation Stage Richard M. Seugling, Roy H.R. Jacobs, Stuart T. Smith, Lowell P. Howard, Thomas LeBrun Center for Precision Metrology, UNC Charlotte,
More informationChapter 3 Analysis of Original Steel Post
Chapter 3. Analysis of original steel post 35 Chapter 3 Analysis of Original Steel Post This type of post is a real functioning structure. It is in service throughout the rail network of Spain as part
More informationEngineering Optimization
Engineering Optimization Most engineering design involves using optimization software which minimizes or maximizes a merit or objective function while satisfying functional constraints (such as stress
More informationNew modeling method of spiral bevel gears with spherical involute based on CATIA
New modeling method of spiral bevel gears with spherical involute based on CATIA HONG Zhaobin, YANG Zhaojun, ZHANG Xuecheng, WANG Yankun College of Mechanical Science and Engineering, Jilin University,
More informationA comparison between large-size shaking table test and numerical simulation results of subway station structure
October 127, 28, Beijing, China A comparison between large-size shaking table test and numerical simulation results of subway station structure ABSTRACT : CHEN Guo-xing 1, ZUO Xi 1, ZHUANG Hai-yang 1,
More informationPredicting the mechanical behaviour of large composite rocket motor cases
High Performance Structures and Materials III 73 Predicting the mechanical behaviour of large composite rocket motor cases N. Couroneau DGA/CAEPE, St Médard en Jalles, France Abstract A method to develop
More information359. Parametrization-based shape optimization of shell structures in the case of free vibrations
359. Parametrization-based shape optimization of shell structures in the case of free vibrations D. Dagys 1, V. Ostasevicius 2, R. Gaidys 3 1,2,3 Kaunas University of Technology, K. Donelaicio 73, LT-44029,
More informationDesign Analysis Of Industrial Gear Box Casing.
Design Analysis Of Industrial Gear Box Casing. Balasaheb Sahebrao Vikhe 1 1 Assistant Professor, Dept. of Mechanical Engineering, SVIT College Nasik, Maharashtra, India ---------------------------------------------------------------------***---------------------------------------------------------------------
More informationChallenge Problem 5 - The Solution Dynamic Characteristics of a Truss Structure
Challenge Problem 5 - The Solution Dynamic Characteristics of a Truss Structure In the final year of his engineering degree course a student was introduced to finite element analysis and conducted an assessment
More informationAdvanced Multi-Body Modeling of Rotor Blades Validation and Application
Advanced Multi-Body Modeling of Rotor s Validation and Application For efficient wind turbine energy production, larger rotors are required for which slender blades with increased flexibility are often
More informationANSYS Element. elearning. Peter Barrett October CAE Associates Inc. and ANSYS Inc. All rights reserved.
ANSYS Element Selection elearning Peter Barrett October 2012 2012 CAE Associates Inc. and ANSYS Inc. All rights reserved. ANSYS Element Selection What is the best element type(s) for my analysis? Best
More information3D Coordinate Transformation Calculations. Space Truss Member
3D oordinate Transformation alculations Transformation of the element stiffness equations for a space frame member from the local to the global coordinate system can be accomplished as the product of three
More informationMaster and Slave Nodes (Rigid Link Function)
Master and Slave Nodes (Rigid Link Function) The rigid link function specified in Model>Boundaries>Rigid Link constrains geometric, relative movements of a structure. Geometric constraints of relative
More informationGabby Kroes Lars Venema, Ramón Navarro ICSO 2012 AJACCIO GABBY KROES PAPER 0013
Gabby Kroes Lars Venema, Ramón Navarro CONTENT Issues cryogenic transmission optics mounts Concepts Compensation mount Ground based application examples INSTRUMENTATION FOR INFRA RED Instrumental background
More informationOptimization of Tapered Cantilever Beam Using Genetic Algorithm: Interfacing MATLAB and ANSYS
Optimization of Tapered Cantilever Beam Using Genetic Algorithm: Interfacing MATLAB and ANSYS K R Indu 1, Airin M G 2 P.G. Student, Department of Civil Engineering, SCMS School of, Kerala, India 1 Assistant
More information16 SW Simulation design resources
16 SW Simulation design resources 16.1 Introduction This is simply a restatement of the SW Simulation online design scenarios tutorial with a little more visual detail supplied on the various menu picks
More informationD DAVID PUBLISHING. Stability Analysis of Tubular Steel Shores. 1. Introduction
Journal of Civil Engineering and Architecture 1 (216) 563-567 doi: 1.17265/1934-7359/216.5.5 D DAVID PUBLISHING Fábio André Frutuoso Lopes, Fernando Artur Nogueira Silva, Romilde Almeida de Oliveira and
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 informationHigh Performance, Full-Digital Control on the LMT and KVN Telescopes
High Performance, Full-Digital Control on the LMT and KVN Telescopes David R. Smith (MERLAB), alpha@merlab.com Kamal Souccar (UMass), David Gale (INAOE), F. Peter Schloerb (Umass), David Hughes (INAOE)
More informationME 475 FEA of a Composite Panel
ME 475 FEA of a Composite Panel Objectives: To determine the deflection and stress state of a composite panel subjected to asymmetric loading. Introduction: Composite laminates are composed of thin layers
More information25 The vibration spiral
25 The vibration spiral Contents 25.1 The vibration spiral 25.1.1 Zone Plates............................... 10 25.1.2 Circular obstacle and Poisson spot.................. 13 Keywords: Fresnel Diffraction,
More informationAbout the Author. Acknowledgements
About the Author Dr. Paul Kurowski obtained his MSc and PhD in Applied Mechanics from Warsaw Technical University. He completed postdoctoral work at Kyoto University. Dr. Kurowski is an Assistant Professor
More informationA Quadratic Pipe Element in LS-DYNA
A Quadratic Pipe Element in LS-DYNA Tobias Olsson, Daniel Hilding DYNAmore Nordic AB 1 Bacground Analysis of long piping structures can be challenging due to the enormous number of shell/solid elements
More informationSizing Optimization for Industrial Applications
11 th World Congress on Structural and Multidisciplinary Optimisation 07 th -12 th, June 2015, Sydney Australia Sizing Optimization for Industrial Applications Miguel A.A.S: Matos 1, Peter M. Clausen 2,
More informationANALYSIS AND OPTIMIZATION OF CONNECTING ROD BY FEA
ANALYSIS AND OPTIMIZATION OF CONNECTING ROD BY FEA 1 Mr.Ajit Lonkar 1 M-Tech Student dept CAD/CAM 1 Narayana Technical Campus, Telangana, India[Affiliated to JNTU, Approved by AICTE] ABSTRACT: The automobile
More information25 METER - MIJ/LIKETER WAVE'TELESCOPE MEMO // 3 4
25 METER - MIJ/LIKETER WAVE'TELESCOPE MEMO // 3 4 Specification for Prototype Surface Panels for 25 m Diameter mm Wave Radio Telescope October 20, 1975 I. General The National Radio Astronomy Observatory
More informationLS-DYNA s Linear Solver Development Phase 1: Element Validation
LS-DYNA s Linear Solver Development Phase 1: Element Validation Allen T. Li 1, Zhe Cui 2, Yun Huang 2 1 Ford Motor Company 2 Livermore Software Technology Corporation Abstract LS-DYNA is a well-known multi-purpose
More information