VARIOUS APPROACHES USED IN THE SEISMIC QUALIFICATION OF THE PIPING SYSTEMS IN NUCLEAR FACILITIES. Introduction
|
|
- Darcy Spencer Bridges
- 5 years ago
- Views:
Transcription
1 VARIOUS APPROACHES USED IN THE SEISMIC QUALIFICATION OF THE PIPING SYSTEMS IN NUCLEAR FACILITIES A. Musil, P. Markov Stevenson&Associates, Pilsen, Czech Republic Introduction In the firm Stevenson&Associates the computational system (see Fig. 1) enhancing the efficiency of modeling and evaluation of the piping systems according to the most commonly applied international codes, which are the ASME Boiler and Pressure Vessel Code (ASME BPVC) and the PNAE G in the case of the WWER-type reactors, is being developed at the current time. The paper presents the step-by-step description of the approach applied in the developed computational system when the differences between the versions for the ASME BPVC and the PNAE Code are mentioned. Preprocessing of a pipeline model and computation of the response for the load cases required by the applied code is performed by using ANSYS software. A 3D beam FEM model of the evaluated pipeline is created by using Piping Models module incorporating the macros developed to automate the individual stages of model preprocessing and response computation. Model geometry and response results are exported into data files which are then imported into the evaluation program set up in Mathcad software. Thus the program receives complete information on the FEM model necessary to carry out automatic evaluation in which the stress at all nodes of the model is determined following the guidelines of the applied code. Subsequently, the obtained values are compared with the stress allowable values specified for the material of the pipeline to calculate the safety factor and based on its value to identify the most critical locations within the qualified pipeline. Fig. 1. Scheme of the computation system for the evaluation of piping systems Such procedure makes development of a pipeline model significantly faster, automates the subsequent evaluation process, and minimizes the risk of a human-factor error. FEM Model Numbers of specialized program modules which can have variously close relation to general FEM systems or can be absolutely autonomous have been developed for modeling of piping systems. An example of such modeler is called Piping Models and is incorporated in ANSYS computer code. Such solution is very convenient since the computation models developed by using Piping Models module are standard 3D computational models built-up from one-dimensional finite elements (PIPE16, PIPE18). Piping Models module enables comfortable modeling of straight sections, curved sections, miter bends, valves, flanges, reducers, flexible supports, and supports with gap. In order to model tee connections according to the provisions ASME Code macro tee.mac was developed. It enables to create the model of the tee connection of UFT or WT type into a
2 chosen node of a pipeline, in a similar manner as standard TEE procedure of Piping Models module which models tee connections simpler than the code [1] requires. Modeling of a tee connection in accordance with the PNAE G Code, Appendix 5, is realized by application of standard TEE procedure with certain modifications. The other macros which have been created are beg.mac, rst.mac, and rse.mac. Macro beg.mac serves for proper definition of all input parameters of preprocessor for modeling and computation analysis. It contains material and section properties of the part of the pipeline which will be modeled next. This macro must me modified prior to its execution to correspond to the currently modeled pipeline. After the execution of macro beg.mac the model of the entire piping system can be built using ANSYS Piping Models module interactively in a standard way. Only for tee connection development when the ASME BPVC is applied, macro tee.mac shall be executed instead of standard TEE procedure of Piping Models module. Modeling of Tee Connection According to the Provisions of the ASME Code The ASME Code classifies two types of tee connections (or tee branches) in the piping design. For the computation models of welding tees (WT) it is required that both the run pipe and the branch pipe are extended to the intersection of their centerlines. The intersection is assumed stiff as well as the length of the branch pipe between the intersection and the run pipe surface. The basic model of unreinforced fabricated tee (UFT) is identical. Only an element of negligible length with local bending flexibility shall be added on the surface of the run pipe. For local flexibility both in bending in the plane defined by the run pipe and the branch pipe centerlines and in the plane perpendicular such that: φ = kmd / EI b, (1) where: Φ local rotation of the branch pipe due to acting moment M, k flexibility of the wall of the branch pipe in the defined direction, M bending moment in the defined direction (see Fig. 2), d outer diameter of the branch pipe, E Young elasticity modulus I b cross-sectional moment of inertia of the branch pipe, T b nominal thickness of the branch pipe defined for various types of reinforcement. The values of k x3 related to moment M x3 which acts perpendicularly to the plane defined by the axes of the run pipe and the branch pipe are defined as [1]: 1/ 2 ' [ ] ( T T ) 1.5 ( D / T ) ( T / t )( d / D) k / x = r r n b r (2) and the values of k z3 related to moment M z3 which acts in the plane defined by the axes of the run pipe and the branch pipe are calculated using:
3 1/ 2 ' [ ] ( T T ) ( D / T )( T / t )( d / D) k / z = r r n b r (3) where: D outside diameter of the run pipe, d outside diameter of the branch pipe, T r thickness of the run pipe, t n thickness of the branch pipe with reinforcement according to [1], T b thickness of branch pipe according to [1].. Fig. 2. Tee connection with displayed moments In case of 3D beam elements, the first requirement (rigid connection at the intersection of the run pipe and the branch pipe centerlines) is satisfied automatically due to basic properties of beam elements. In order to satisfy the second and the third requirement it was necessary to develop a specialized procedure. It was realized by creation of macro tee.mac. In this macro the data describing the material properties and geometry of the run pipe and the branch pipe are read as first. After their reading TEE command from Piping Models module is executed to provide the creation of three new elements with a shared node at the intersection of the run pipe and the branch pipe centerlines. These new elements form one PIPE17 element. PIPE17 element is a combination of three uniaxial elastic straight pipe elements (PIPE16) arranged in a tee configuration with tension-compression, torsion, and bending capabilities. One of the parameters specifies whether the branch connection is of UFT type or WT type. The following parameters define the length of the inserted elements modeling the run pipe and the branch pipe. The length of each run pipe element is equal to two diameters of the run pipe which is in accordance with the default value in TEE command. The length of the branch pipe value is set to be equal to one half of that diameter. Thus a new node on the surface of the branch pipe is created which provides that the second requirement of the code is satisfied. Then the properties of the new branch element must be modified. Since it must be rigid, it was chosen E = and ρ = 0. Thus it is achieved that the model becomes even more realistic than is required by the code because any other value of ρ than zero would bring additional mass compared to the real mass of a pipeline. The third requirement was solved by inserting an element of BEAM4 type into the new node on the surface of the run pipe. The length of this element was set equal to one tenth of the diameter d of the branch pipe which is in agreement with the study [2].The inserted BEAM4 element is of rectangular cross section with moments of inertia in bending: I = I (4) b y / k x3 and I = I (5) h y / k z3
4 where I y is cross-sectional moment of inertia in bending of the pipe branch (if it was modeled by PIPE16): I y 4 4 ( D d )/ 6 = π. (6) The computational model of the branch pipe developed by this procedure fully satisfies the requirements of the code [1]. Macro tee.mac will create it at any part of a pipeline where a branch pipe is modeled. The purpose of the use of BEAM4 element is to model the stiffness reduction of branch pipe due to effect of its attachment (weld) to a thin wall of the run pipe. Scheme of UFT type of tee connection according to the provisions of the ASME BPVC is shown in Fig. 3 and the example of the model of such tee connection created by using macro tee.mac is shown in Fig. 4. Fig. 3. Scheme of the model of UFT type of tee connection according to the provisions of the ASME BPVC Fig. 4. Model of UFT type of tee connection created by using macro tee.mac Modeling of Tee Connection According to the Provisions of the PNAE Code As already mentioned, the model of tee connection according to the provision of the PNAE G Code [3] can be developed by using standard TEE procedure from Piping Models module of ANSYS. Since tee connection is evaluated in the sections A, V, B as it is displayed on the scheme in Fig. 5, the only modification is the relocation of the edge nodes of both elements of the run pipe to the location of the sections. This shortens the length of the run pipe elements to be equal to the length of the branch pipe radius. The branch pipe element is modeled to connect the tee intersection with the run pipe surface. Fig. 5 Scheme of tee connection according to the provisions of the PNAE G Code Computation Analyses The resulting product of Piping Models module is a standard computational model of ANSYS code like the example in Fig. 6. After the setting of boundary conditions and static or dynamic loadings, nodal displacements, forces, and moments are computed. Static analyses are performed in a standard way, seismic analyses are performed by automating procedures developed by Stevenson&Associates. For the analysis of the pipeline response on the seismic excitation by using Response Spectrum Method [4] there are several versions of macro rsm.mac available depending on the applied method for the mode response combination, the most typically it can be Complete Quadratic Combination (CQC) or Square-Root-of-Sums-of-
5 Squares (SRSS). After the completion of the computation analyses, macros rst.mac (for static analysis) or rse.mac (seismic analysis) are executed to generate the output data files containing the model data such as element types, model geometry and results of the computed responses (nodal displacements, forces, and moments). Subsequently, these files are imported into Piping Evaluation program in which the evaluation of the pipeline is carried out in terms of compliance with the acceptance criteria of the applied code. Fig. 6. Computational model of a pipeline Piping Evaluation Piping Evaluation program set up in Mathcad software consists of a number of separated, consequential modules which serve for realization of individual steps during the piping evaluation process. Thanks to the capability of Mathcad to read data form various types of data files (xls, txt, LOTUS, etc.), it is possible to automate the import of the data generated by ANSYS. At the same time, Mathcad also enables to create these types of data files which is utilized both during the data transfer between individual modules and during the generation of output data files containing the results of evaluation. The function of the first module Pipeline Reading is to read the data of all elements of the pipeline FEM model and on the basis of these data (Element Name, Real Constant, KeyOpt) to sort and classify the elements into the groups representing the standardized types of pipeline components (straight pipe, curved pipe, tee connection, flange connection, etc.). At the same time, the elements of the FEM model representing different types of elements which will not be further evaluated (SPRING, LINK, etc.) are filtered out and are not proceeded to the following evaluation steps. The separate tables of the evaluated types of pipeline components containing all data essential for the following evaluation steps are created and exported in the form of Excel sheets. The subsequent module in Piping Evaluation program is Pipeline Response module. This module imports the data files with the response results for the applied loads computed in the FEM model in ANSYS. The evaluation based on the ASME BPVC is carried out for nodal values of moments. The responses on individual seismic load cases are combined the most commonly by applying the SRSS rule and the resultant nodal values of moment then computed. The resultant moments are calculated identically for static loads and the resultant nodal moments for both static and seismic loads are then exported to Stress Evaluation module. For the pipeline evaluation following the PNAE code different version of Pipeline Response module was developed since the stress evaluation is based on the nodal values of Fz (axial force) and moment components Mx, My (bending moments), and Mz (torsional moment). Stress Evaluation module reads both files with the element data of all evaluated types of pipeline components imported from Pipeline Reading module and files with the response results generated by Pipeline Response module. For the case of the pipeline evaluation according to the ASME BPVC code, primary stress intensity S n is determined for the required load case (Service Level) at all nodes of the evaluated types of pipeline components. Provided
6 the PNAE code is applied for the pipeline evaluation, reduced stress (σ) 2 is determined. The results listed in the Excel tables are passed to the last phase of the pipeline evaluation which is performed in Final Evaluation module. Module Allowable Stress contains the procedures for determination of the values of material allowable stress defined by the acceptance criteria of the applied code corresponding to the required load combination. The determined allowable value is exported to the last module which is Final Evaluation. In this module the values of stress computed in Stress Evaluation module are compared with the allowable stress values determined in Allowable Stress module. In Final Evaluation module the parameter called Safety Factor is calculated for all nodes of the evaluated pipeline elements. Its value expresses the safety reserve of the investigated node in the pipeline model under the applied seismic loading compared to the allowable stress value. On the basis of this value, the critical locations of the pipeline are identified. The pipeline satisfies in terms of compliance with the acceptance criteria provided the value of Safety Factor is not lower than 1. If this condition is not met, the seismic reinforcement provisions shall be proposed to achieve the sufficient seismic strength of the pipeline. The results produced by this module are exported as an output file of seismic qualification of the pipeline. Conclusion The presented computational system is prepared for the evaluation of piping according to the ASME BVPC Subsection NB (piping systems of the primary circuit) and Subsection NC (piping systems of the other nuclear facilities) pro Service Levels C, D (normal operation loads + seismic loads). It remains to extend the program to cover the piping evaluation for Service Levels A and B (inclusion of the thermal gradients on elastic stress). Parallelly, the version for the evaluation based on the PNAE G Code [3] has been developed and implemented. This Code is expected to be applied for the piping evaluations in the project of the construction of the 3 rd and 4 th Unit of the Mochovce Nuclear Power Plant in Slovakia. The aim of the current efforts is to develop the complex, universal and effective computational system for the pipeline qualifications with regard to the current needs of the nuclear industry. References 1. ASME Boiler & Pressure Vessel Code, Section III, Division 1. New York, USA, Stress Intensification Factors and Flexibility Factors for Unreinforced Branch Connections. EPRI Report No. TR , Palo Alto, USA, Strength Design Code for Components and Pipelines of Nuclear Power Facilities (PNAE G ). Gosatomenergonadzor of USSR, Energoatomizdat, Moscow, Russia, Gupta, A. K. Response Spectrum Method in Seismic Analysis and Design of Structures. Blackwell scientific Publications, Cambridge, USA, 1990.
RF-PIPING. Add-on Modules for PIPELINES. Program Description
Version February 2016 Programs RF-PIPING Add-on Modules for PIPELINES Program Description All rights, including those of translations, are reserved. No portion of this book may be reproduced mechanically,
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 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 informationmidas Civil Advanced Webinar Date: February 9th, 2012 Topic: General Use of midas Civil Presenter: Abhishek Das Bridging Your Innovations to Realities
Advanced Webinar Date: February 9th, 2012 Topic: General Use of midas Civil Presenter: Abhishek Das Contents: Overview Modeling Boundary Conditions Loading Analysis Results Design and Misc. Introduction
More informationFirst Order Analysis for Automotive Body Structure Design Using Excel
Special Issue First Order Analysis 1 Research Report First Order Analysis for Automotive Body Structure Design Using Excel Hidekazu Nishigaki CAE numerically estimates the performance of automobiles and
More informationCOLLAPSE LOAD OF PIPE BENDS WITH ASSUMED AND ACTUAL CROSS SECTIONS UNDER IN-PLANE AND OUT-OF-PLANE MOMENTS
VOL., NO., NOVEMBER 6 ISSN 8968 6-6 Asian Research Publishing Network (ARPN). All rights reserved. COLLAPSE LOAD OF PIPE BENDS WITH ASSUMED AND ACTUAL CROSS SECTIONS UNDER IN-PLANE AND OUT-OF-PLANE MOMENTS
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 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 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 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 informationAUTOPIPE / CAESAR TRANSLATION
AUTOPIPE / CAESAR TRANSLATION CONTENTS AutoPIPE / Caesar Translation... 1 Caesar Neutral File Versions... 2 Transfering Caesar Model to AutoPIPE... 3 Transfer Large Caesar Models... 9 AutoPIPE Configurable
More informationPD2CAEPIPE - Plant Design-to-CAEPIPE Translator
PD2CAEPIPE - Plant Design-to-CAEPIPE Translator (for converting PCF files) 1.0 Installing Program To install PD2CAEPIPE on Windows NT, load the product CD supplied by InfoPlant and run the program "SETUP.EXE"
More informationTechnical Report Example (1) Chartered (CEng) Membership
Technical Report Example (1) Chartered (CEng) Membership A TECHNICAL REPORT IN SUPPORT OF APPLICATION FOR CHARTERED MEMBERSHIP OF IGEM DESIGN OF 600 (103 BAR) 820MM SELF SEALING REPAIR CLAMP AND VERIFICATION
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 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 informationASME Verification and Validation Symposium May 13-15, 2015 Las Vegas, Nevada. Phillip E. Prueter, P.E.
VVS2015-8015: Comparing Closed-Form Solutions to Computational Methods for Predicting and Validating Stresses at Nozzle-to-Shell Junctions on Pressure Vessels Subjected to Piping Loads ASME Verification
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 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 informationOther Major Component Inspection I
Other Major Component Inspection I Mechanized UT inspections on complex nozzle geometries S. Farley, R. Jansohn, Westinghouse Electric Germany, Germany; H. Ernst, Schweizerischer Verein für technische
More informationStiffness Analysis of the Tracker Support Bracket and Its Bolt Connections
October 25, 2000 Stiffness Analysis of the Tracker Support Bracket and Its Bolt Connections Tommi Vanhala Helsinki Institute of Physics 1. INTRODUCTION...2 2. STIFFNESS ANALYSES...2 2.1 ENVELOPE...2 2.2
More informationGuidelines for proper use of Plate elements
Guidelines for proper use of Plate elements In structural analysis using finite element method, the analysis model is created by dividing the entire structure into finite elements. This procedure is known
More informationTRIFLEX Version Enhancements & Modifications May 2, 2008 Page 1. Enhancements
Page 1 Enhancements 1. One Dimensional Release Elements and Expansion Joints Adding to the versatility of TRIFLEX, this release adds one dimensional release elements and expansion joints that may be specified
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 informationCHAPTER 4. Numerical Models. descriptions of the boundary conditions, element types, validation, and the force
CHAPTER 4 Numerical Models This chapter presents the development of numerical models for sandwich beams/plates subjected to four-point bending and the hydromat test system. Detailed descriptions of the
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 informationTHE COMPUTATIONAL MODEL INFLUENCE ON THE NUMERICAL SIMULATION ACCURACY FOR FORMING ALLOY EN AW 5754
THE COMPUTATIONAL MODEL INFLUENCE ON THE NUMERICAL SIMULATION ACCURACY FOR FORMING ALLOY EN AW 5754 Pavel SOLFRONK a, Jiří SOBOTKA a, Pavel DOUBEK a, Lukáš ZUZÁNEK a a TECHNICAL UNIVERSITY OF LIBEREC,
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 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 information3. Check by Eurocode 3 a Steel Truss
TF 3. Check by Eurocode 3 a Steel Truss Applicable CivilFEM Product: All CivilFEM Products Level of Difficulty: Moderate Interactive Time Required: 40 minutes Discipline: Structural Steel Analysis Type:
More informationDevelopment of Bellows Design Software using MATLAB
Indian Journal of cience and Technology, Vol 8(8), 201 206, April 2015 IN (Print) : 097-686 IN (Online) : 097-565 DOI: 10.1785/ijst/2015/v8i8/70619 Development of Bellows Design oftware using MATLAB ungchul
More informationMANUAL COMPUTERS & STRUCTURES INC.
SAP2000 Integrated Finite Element Analysis and Design of Structures VERIFICATION MANUAL COMPUTERS & STRUCTURES INC. Computers and Structures, Inc. Berkeley, California, USA Version 6.1 Revised July 1997
More informationTutorial on Modeling of Expansion Joints using CAEPIPE
Tutorial on Modeling of Expansion Joints using CAEPIPE The following examples illustrate the modeling of various types of expansion joints in CAEPIPE stress models. Example 1: Tied Bellow (without gaps)
More informationAUTOPIPE NOZZLE. LOCAL STRESS ANALYSIS V8i Release Tutorial with Examples
AUTOPIPE NOZZLE LOCAL STRESS ANALYSIS V8i Release 8.11 Tutorial with Examples 1 Table of Contents List of Examples... 2 Example 1: The basic operating procedures of AutoPIPE Nozzle... 3 Starting AutoPIPE
More informationBuckling Analysis of a Thin Plate
Buckling Analysis of a Thin Plate Outline 1 Description 2 Modeling approach 3 Finite Element Model 3.1 Units 3.2 Geometry definition 3.3 Properties 3.4 Boundary conditions 3.5 Loads 3.6 Meshing 4 Structural
More informationModule 1: Introduction to Finite Element Analysis. Lecture 4: Steps in Finite Element Analysis
25 Module 1: Introduction to Finite Element Analysis Lecture 4: Steps in Finite Element Analysis 1.4.1 Loading Conditions There are multiple loading conditions which may be applied to a system. The load
More informationGBTUL 1.0. Buckling and Vibration Analysis of Thin-Walled Members USER MANUAL. Rui Bebiano Nuno Silvestre Dinar Camotim
GBTUL 1.0 Buckling and Vibration Analysis of Thin-Walled Members USER MANUAL Rui Bebiano Nuno Silvestre Dinar Camotim Department of Civil Engineering and Architecture, DECivil/IST Technical University
More informationGlobal to Local Model Interface for Deepwater Top Tension Risers
Global to Local Model Interface for Deepwater Top Tension Risers Mateusz Podskarbi Karan Kakar 2H Offshore Inc, Houston, TX Abstract The water depths from which oil and gas are being produced are reaching
More informationInstitute of Mechatronics and Information Systems
EXERCISE 4 Free vibrations of an electrical machine model Target Getting familiar with the fundamental issues of free vibrations analysis of a simplified model of an electrical machine, with the use of
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 informationMAT-Test A New Method of Thin Film Materials Characterisation. LPCVD silicon nitride film bent through 90º
MAT-Test A New Method of Thin Film Materials Characterisation LPCVD silicon nitride film bent through 90º Introduction Measurements of Thin-Film Materials Properties There is a present and growing need
More informationStructural analysis for in-service gas pipeline lowering using numerical method
Structural analysis for in-service gas pipeline lowering using numerical method Mochamad Safarudin 1*, Joga Dharma Setiawan 2 1 Mechanical Engineering, Sekolah Tinggi Teknologi Mandala, Indonesia 2 Mechanical
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 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 informationModule 1.5: Moment Loading of a 2D Cantilever Beam
Module 1.5: Moment Loading of a D Cantilever Beam Table of Contents Page Number Problem Description Theory Geometry 4 Preprocessor 7 Element Type 7 Real Constants and Material Properties 8 Meshing 9 Loads
More informationDeep Beam With Web Opening
Deep Beam With Web Opening Name: Path: Keywords: DeepBeamWithWebOpening/deepbeam /Examples//DeepBeamWithWebOpening/deepbeam analys: linear static. constr: suppor. elemen: cq16m ct12m pstres. load: force
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 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 informationModeling Foundations in RS
Modeling Foundations in RS 3 Piled Raft Modeling in RS 3 Deep foundation piles are commonly used to increase foundation stability and to increase the bearing capacity of structural systems. The design
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 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 informationBackground CE 342. Why RISA-2D? Availability
Background CE 342 RISA-2D RISA-2D is a structural analysis program, which can model: Beams, frames, trusses and plates. Any linear elastic structural material. Typical supports, such as pins, rollers and
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 informationCoupled Analysis of FSI
Coupled Analysis of FSI Qin Yin Fan Oct. 11, 2008 Important Key Words Fluid Structure Interface = FSI Computational Fluid Dynamics = CFD Pressure Displacement Analysis = PDA Thermal Stress Analysis = TSA
More informationElastic Analysis of a Deep Beam with Web Opening
Elastic Analysis of a Deep Beam with Web Opening Outline 1 Description 2 Finite Element Model 2.1 Units 2.2 Geometry definition 2.3 Properties 2.4 Boundary conditions 2.4.1 Constraints 2.4.2 Vertical load
More informationDETECTION AND QUANTIFICATION OF CRACKS IN PRESSURE VESSELS USING ESPI AND FEA MODELLS
DETECTION AND QUANTIFICATION OF CRACKS IN PRESSURE VESSELS USING ESPI AND FEA MODELLS J GRYZAGORIDIS, DM FINDEIS, JR MYLES Department of Mechanical Engineering University of Cape Town Abstract Non destructive
More informationAdvanced model of steel joints loaded by internal forces from 3D frame structures
Advanced model of steel joints loaded by internal forces from 3D frame structures Lubomír Šabatka, IDEA RS s.r.o František Wald, FSv ČVUT Praha Jaromír Kabeláč, Hypatia Solutions s.r.o Drahoslav Kolaja,
More information1.2 Connection configurations:
1.2 Connection configurations: 1.2.1 Simple connections: Simple connections are assumed to transfer shear only shear at some nominal eccentricity. Therefore such connections can be used only in non-sway
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 information[ Ω 1 ] Diagonal matrix of system 2 (updated) eigenvalues [ Φ 1 ] System 1 modal matrix [ Φ 2 ] System 2 (updated) modal matrix Φ fb
Proceedings of the IMAC-XXVIII February 1 4, 2010, Jacksonville, Florida USA 2010 Society for Experimental Mechanics Inc. Modal Test Data Adjustment For Interface Compliance Ryan E. Tuttle, Member of the
More informationTekla Structures Analysis Guide. Product version 21.0 March Tekla Corporation
Tekla Structures Analysis Guide Product version 21.0 March 2015 2015 Tekla Corporation Contents 1 Getting started with analysis... 7 1.1 What is an analysis model... 7 Analysis model objects...9 1.2 About
More informationModule 3: Buckling of 1D Simply Supported Beam
Module : Buckling of 1D Simply Supported Beam Table of Contents Page Number Problem Description Theory Geometry 4 Preprocessor 7 Element Type 7 Real Constants and Material Properties 8 Meshing 9 Solution
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 informationRevised Sheet Metal Simulation, J.E. Akin, Rice University
Revised Sheet Metal Simulation, J.E. Akin, Rice University A SolidWorks simulation tutorial is just intended to illustrate where to find various icons that you would need in a real engineering analysis.
More informationFinite Element Analysis Using NEi Nastran
Appendix B Finite Element Analysis Using NEi Nastran B.1 INTRODUCTION NEi Nastran is engineering analysis and simulation software developed by Noran Engineering, Inc. NEi Nastran is a general purpose finite
More informationElement Order: Element order refers to the interpolation of an element s nodal results to the interior of the element. This determines how results can
TIPS www.ansys.belcan.com 鲁班人 (http://www.lubanren.com/weblog/) Picking an Element Type For Structural Analysis: by Paul Dufour Picking an element type from the large library of elements in ANSYS can be
More informationGeneric Neutral Files
Chapter 8 Interfaces 8-57 Generic Neutral Files CAESAR II Neutral File Interface The general neutral file can be used to send data either in to or out of the standard CAESAR II binary input file, otherwise
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 informationOPTFAIL Manual. A1.1 Introduction. APPENDIX 1 SPROPS, PROFAIL, and
APPENDIX 1 SPROPS, PROFAIL, and OPTFAIL Manual A1.1 Introduction OPTFAIL is a computer code written in FORTRAN developed by Woodson (1994) to optimize circular frames laminated from uniaxial tape composites
More informationSAFI Sample Projects. Design of a Steel Structure. SAFI Quality Software Inc. 3393, chemin Sainte-Foy Ste-Foy, Quebec, G1X 1S7 Canada
SAFI Sample Projects Design of a Steel Structure SAFI Quality Software Inc. 3393, chemin Sainte-Foy Ste-Foy, Quebec, G1X 1S7 Canada Contact: Rachik Elmaraghy, P.Eng., M.A.Sc. Tel.: 1-418-654-9454 1-800-810-9454
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 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 informationIntroduction to Nastran SOL 200 Design Sensitivity and Optimization
Introduction to Nastran SOL 200 Design Sensitivity and Optimization PRESENTED BY: CHRISTIAN APARICIO The Nastran Engineering SOL 200 questions? Lab Email me: christian@ the-engineering-lab.com Motivation
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 informationPRE-DESIGN OF SEMI-RIGID JOINTS IN STEEL FRAMES
PRE-DESIGN OF SEMI-RIGID JOINTS IN STEEL FRAMES Martin Steenhuis ( ), Nol Gresnigt ( ), Klaus Weynand ( 3 ) Keywords: steel, joints, frames, semi-rigid, pre-design, stiffness, classification Abstract The
More informationReinforced concrete beam under static load: simulation of an experimental test
Reinforced concrete beam under static load: simulation of an experimental test analys: nonlin physic. constr: suppor. elemen: bar cl12i cl3cm compos cq16m interf pstres reinfo struct. load: deform weight.
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 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 informationA05 Steel Catenary Riser Systems
A05 Steel Catenary Riser Systems Introduction This example contains three examples of steel catenary risers (SCRs). These are: Catenary with Spar Catenary with SemiSub Lazy Wave with FPSO The example also
More informationUsing three-dimensional CURVIC contact models to predict stress concentration effects in an axisymmetric model
Boundary Elements XXVII 245 Using three-dimensional CURVIC contact models to predict stress concentration effects in an axisymmetric model J. J. Rencis & S. R. Pisani Department of Mechanical Engineering,
More informationNEW WAVE OF CAD SYSTEMS AND ITS APPLICATION IN DESIGN
Vol 4 No 3 NEW WAVE OF CAD SYSTEMS AND ITS APPLICATION IN DESIGN Ass Lecturer Mahmoud A Hassan Al-Qadisiyah University College of Engineering hasaaneng@yahoocom ABSTRACT This paper provides some lighting
More informationThe CAESAR II Piping Model. How Good Is It?
The CAESAR II Piping Model How Good Is It? Quick Agenda Introduction The digital model What s missing in our CAESAR II model? Model precision and construction tolerances Engineering Sensitivity Boundary
More informationThis is NOT a truss, this is a frame, consisting of beam elements. This changes several things
CES 44 - Stress Analysis Spring 999 Ex. #, the following -D frame is to be analyzed using Sstan (read the online stan intro first, and Ch-6 in Hoit) 5 k 9 E= 9000 ksi 8 I= 600 in*in*in*in 5 A= 0 in*in
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 informationLateral Loading of Suction Pile in 3D
Lateral Loading of Suction Pile in 3D Buoy Chain Sea Bed Suction Pile Integrated Solver Optimized for the next generation 64-bit platform Finite Element Solutions for Geotechnical Engineering 00 Overview
More informationQuarter Symmetry Tank Stress (Draft 4 Oct 24 06)
Quarter Symmetry Tank Stress (Draft 4 Oct 24 06) Introduction You need to carry out the stress analysis of an outdoor water tank. Since it has quarter symmetry you start by building only one-fourth of
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 informationCase Study - Vierendeel Frame Part of Chapter 12 from: MacLeod I A (2005) Modern Structural Analysis, ICE Publishing
Case Study - Vierendeel Frame Part of Chapter 1 from: MacLeod I A (005) Modern Structural Analysis, ICE Publishing Iain A MacLeod Contents Contents... 1 1.1 Vierendeel frame... 1 1.1.1 General... 1 1.1.
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 informationLindab We simplify construction. Table of contents
Table of contents 1 General information... 3 1.1 Platforms... 3 1.2 Licensing... 3 1.3 Database properties... 3 2 Display language... 4 3 Interface... 5 3.1 General Settings... 5 3.1.1 Country... 6 3.1.2
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 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 informationComputer modelling and simulation of the mechanical response of composite lattice structures
22nd International Congress on Modelling and Simulation, Hobart, Tasmania, Australia, 3 to 8 December 2017 mssanz.org.au/modsim2017 Computer modelling and simulation of the mechanical response of composite
More informationDEVELOPMENT OF THE THIN-WALL-2 PROGRAM FOR BUCKLING ANALYSIS OF THIN-WALLED SECTIONS UNDER GENERALISED LOADING
Eighth International Conference on ADVANCES IN STEEL STRUCTURES Lisbon, Portugal, July 22-24, 2015 DEVELOPMENT OF THE THIN-WALL-2 PROGRAM FOR BUCKLING ANALYSIS OF THIN-WALLED SECTIONS UNDER GENERALISED
More informationGeneral Applications
Chapter General Applications The general analysis modules can be used to calculate section properties, wind pressures on buildings and evaluate drainage systems of building roofs. General Applications
More informationModule 1.2: Moment of a 1D Cantilever Beam
Module 1.: Moment of a 1D Cantilever Beam Table of Contents Page Number Problem Description Theory Geometry Preprocessor 6 Element Type 6 Real Constants and Material Properties 7 Meshing 9 Loads 10 Solution
More informationRISA 3D. Verification Problems. Rapid Interactive Structural Analysis 3 Dimensional
RISA 3D Rapid Interactive Structural Analysis 3 Dimensional Verification Problems 26632 Towne Centre Drive, Suite 210 Foothill Ranch, California 92610 (949) 951 5815 (949) 951 5848 (FAX) www.risatech.com
More informationcheckstress [for Intergraph's PDS]
checkstress [for Intergraph's PDS] Introduction Under the checkstress brand name, three products are available namely checkstress (which generates only CAEPIPE input file), checkstress II (which generates
More informationCHAPTER 5 USE OF STL FILE FOR FINITE ELEMENT ANALYSIS
CHAPTER 5 USE OF STL FILE FOR FINITE ELEMENT ANALYSIS 5.1 Introduction: Most CAD software in the market can generate STL files, and these are generally used for prototyping and rendering purposes. These
More informationTutorial for Response Spectrum Analysis using CAEPIPE
Tutorial for Response Spectrum Analysis using CAEPIPE The following are the Steps for performing the Response Spectrum Analysis using CAEPIPE. General The Response Spectrum is a plot of the maximum response
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 information