FATIGUE ASSESSMENT OF TYPICAL DETAILS OF VLGC
|
|
- Oswin Goodwin
- 5 years ago
- Views:
Transcription
1 FATIGUE ASSESSMENT OF TYPICAL DETAILS OF VLGC P. Cambos, BUREAU VERITAS, France C. Chauviere, BUREAU VERITAS, France SUMMARY This paper mainly focuses on the fatigue assessment of the structural details specific to the large LPG carriers with prismatic tanks. In a first step, are described the method of structural assessment of the hull and the independent tanks of LPG carriers. In a second step, are described more specifically the methodologies developed for the fatigue assessment of structural details specific to LPG carriers, and more particularly to the supports and keys. The paper also integrates the return of experience and mention practical solutions to enhance the fatigue of critical details. 1. INTRODUCTION The world fleet of Liquefied Petroleum Gas (LPG) tankers is more than 1000 vessels. This fleet of LPG carriers is consisting of a large range of ships, different in size, design, and cargo capability. Type of ships is spreading from the coastal fully pressurised butane and propane tankers to the very large fully refrigerated tankers of more than 80,000m3, involved on long trade traffic, and also includes more sophisticated small and medium size tankers, semi pressurised and fully refrigerated, able to carry a wide range of more delicate substances such as ethylene or chemical gases, in addition to the current LPG products. The purpose of this paper is to focus on the segment of large LPG carriers designed with atmospheric type A cargo tanks, in accordance with the definition of the IMO IGC code [1] and to focus on the fatigue assessment of the particular structural details for the hull and containment system of this type of ship. For memory, there are about 100 VLCG on operation worldwide. In accordance with ICG code, independent type A cargo tanks are self supporting tanks designed using recognised ship structural analysis procedures. They are usually gravity tanks made of plane surface and their design vapour pressure is limited to a maximum of 0.7 bars. On the other hand, the latest designs includes more and more high tensile steel (Re = 355MPa), which makes the structure more critical for fatigue point of view, and which makes the fatigue assessment more and more necessary, for the design review of VLCG. BUREAU VERITAS has developed a notation VeriSTAR Hull DFL XX years, with XX is taken between 25 and 40 years, which may be granted to ship subject to the analysis described in this paper. This paper aims at showing on a real example how the methodology was applied on an actual case of a 84000m3 LPG carrier project, recently built under BV classification. 2. DESCRIPTION OF THE STUDIED SHIP The ship subject of the fatigue assessment is a VLCG with a capacity of 84000m3 recently built. The ship is fitted with four independent cargo tanks on the length. The design is fitted with double bottom and single side as shown figure 1on the typical midship section. The independent type A cargo tanks are required to be duplicated with a complete secondary containment system (secondary barrier) able to preserve the integrity of the ship structure in case of leakage of the cargo tanks and to safely keep the cryogenic cargo into the ship within 15 days. Calculation tools implemented by shipyards, design offices and classification societies have largely progressed since the first large independent type A LPG carrier was built in the early 70s. FEM analysis tools and methodologies for fatigue assessment have been more and more user friendly, easier and faster to run and as a consequence, more and more frequently used. Figure 1: Typical midship section
2 The independent tanks are supported and maintained in position within the ship s hold tanks to various types of supports and keys. Cargo tank supports and keys are to be designed and built to : Insulate the cargo tank in order to insure a acceptable boil off rate and to avoid that the temperature of the ship structure in way of the supports & keys is lowered below the values allowed for the steel used. Transmit to the hull structure the loads corresponding to the weight supplemented by the dynamic effects due to the ship motions while limiting the stress concentrations in both the hull and the cargo tank. Allow free contraction due to temperature and free displacement between the cargo tank and the hold due to the wave. The various type of supports and keys, generally fitted with wooden chocks, are: Four rows of vertical supports are located in way of the transverse frame aim at transferring the weight of the tank and cargo to the hull. They are currently different types of such supports able to sustain loads of various ranges from about 400 t to 1000 t. Those fitted in the corner of the cargo tank are generally the more loaded. Anti-rolling keys, preventing from lateral motion of the cargo tanks, are fitted along the centre line, both in way of the upper and lower parts of the cargo tank. Anti-pitching keys, preventing from longitudinal motion of the cargo tanks, are fitted along the transverse line of the cargo tank. They are located at mid span of the cargo tank, generally only in the lower part of the cargo hold. They are also used as anti collision keys. Two rows of anti flotation keys, preventing from lifting of the cargo tank in case of flooding of the cargo hold are located on the top of the cargo tank on each side. 3. CALCULATION PROCEDURES The analysis have been performed with VeriSTAR hull software, developed by BUREAU VERITAS. This computer program has already been subject to several papers [2]. It is a powerfull integrated finite element analysis software enabling to automatically generate and load the model of a ship, with respect to BUREAU VERITAS rule requirements. It includes facilities to perform local refined analysis and fatigue assessment of typical structural details from coarse mesh models. 3.1 COARSE MESH MODEL The main objectives of the coarse mesh analysis are: To determine the stress distribution in the primary supporting members of the cargo tank and the ship structures, To determine the forces in the keys supporting the tanks, To verify that the yielding and buckling strength criteria as given in Rules for the Classification of Steel Ships are complied with, To determine, where necessary, the relevant boundary conditions for finer mesh analyses of the highly stressed areas. As the reaction forces in the supports and keys depends on the stiffness of the ship hull and the stiffness of the cargo tank, the global coarse mesh model is to include both the ship hull and the cargo tank. According to VeriSTAR calculation, the model is to be extended over three cargo tanks. As the structure is generally not symmetrical, both sides are to be modelled. The figure 2 shows a three cargo tank typical VeriSTAR model (half of the model). Z X Figure 2: Y Typical VeriSTAR three cargo tank model The model integrates supports and keys modelled by beams or springs elements having the stiffness of the structure. Different methodologies are proposed to evaluate the stiffness of the supports and keys. In the results of the coarse mesh model, the elements modelling the supports and found in tension are to be deleted. Only the elements in compression are kept.
3 3.2 LOAD CASES For the yielding and buckling analysis, the internal load cases take into account the following internal load cases: Full load, Ballast, Alternate load case, Non symmetrical case, Damage case tank empty hold flooded. The fatigue analysis is based mainly on full load and ballast load cases. The internal load cases are combined with external sea conditions : Crest of wave head sea, Through of wave beam sea, Maximum internal acceleration, Beam sea external dynamic Beam sea maximum acceleration. 3.4 ASSESSMENT OF THE SUPPORTS & KEYS Each type of supports has been subjected to a detailed FEM analysis. The structural elements surrounding the supports have been analysed on both sides (cargo tank side and hull side) The typical size of the current finite element edge is based on a quarter of a longitudinal spacing. The figures 4a and 4b show the two fine mesh models for the assessment of a typical vertical support. The loads from the coarse mesh are applied on the support, and the friction force is added in longitudinal and transversal directions, as shown figure FINE MESH MODEL Beyond the 3D coarse mesh analysis, several refined analysis are carried out on the basis of 3D fine mesh models, namely: Cargo tank web frames and stringers, Hold typical bottom transverses, bottom girders, transverse bulkhead, knuckles The standard size of elements used for fine meshes is based on the spacing between secondary stiffeners. Displacements from the coarse mesh model are applied as boundary conditions to the fine mesh model. The pressure loads and local forces are applied on the fine mesh model. An example of a fine mesh model of the foot of the transverse bulkhead is shown on the figure 3 below. ( p Y Z X Figure 4a: Example of a fine mesh model of upper part of a typical vertical support Y Y X Z XZ Figure 3: Example of a fine mesh model Figure 4b: Example of a fine mesh model of lower part of a typical vertical support
4 The deterministic methodology has been calibrated using the spectral methodology, described hereafter, as well as return of experience. 4.2 DAMAGE CALCULATION Figure 5: loading of vertical supports In spite of the critics, the only usable damage calculation method for marine structures design is the Miner sum. The method is based on a linear fatigue damage accumulation from a stair representation of the stress long term distribution. An illustration is given on figure 6 and the failure criteria is: n D = i 1 > N i γ where γ is the partial safety coefficient which take into account the uncertainties of the Miner sum, as the value 1 is a mean value at failure of samples. 4. FATIGUE ANALYSIS METHODOLOGY log S S-N curve In the early 1980s, this methodology was introduced with the purpose to assure that the seagoing ships could respect a fatigue life of 20 years, in North Atlantic sea conditions, with a cumulative damage ratio of 1, taking into account the SN curve at minus two standard deviations. S i long term distribution S m N= C n i S m' N= C' (corrosion) These ships were verified by considering mainly two draughts; full and ballast loading cases. At that time, a guidance notes for fatigue assessment have been developed. Figure 6: 10 7 Miner sum principle illustration N i log N The IACS recommendation No56 was published in Fatigue assessment became mandatory, for ships more than 170 m in length, in FATIFUE METHODOLOGY Different approaches for fatigue analysis are available in BV rules. For the case of the LPG carriers, the deterministic methodology was used, calibrated on a hydrodynamic analysis. The stress ranges are calculated based on loads at a probability level of The loads take into account the hull girder ending moment and shear forces, the wave pressure on the shell and the internal tank pressure due to the accelerations, which are taken from rule formula. The distribution of long term stress range assuming a Weibull distribution, and rule formula are used to define the shape parameter. To allow to take into account the welding and/or postweld treatment conditions, Bureau Veritas decided to used the local stress where the crack are expected to occur. Welded joints For welded joints the stress range to be used is the notch stress range, i.e., taking into account the local geometry plus weld toe stress concentration (hot spot stress plus notch effect). This stress range is associated with a unique typical basic material S-N curve with a stress range power m = 3 to respect the weld joint sample test results: S 3 N = (in MPa) This curve is applicable to any steel, mild or high strength, used for floating unit structures. For normal design this design S-N curve is a curve at 2 standard deviations in log(c) below the mean curve. When the structural component is efficiently protected against corrosion a change of m, from 3 to 5, is
5 introduced at N = 10 7 to take into account for the influence of the fatigue limit associated to stress range randomness on the long term Miner sum. When the component is not protected, i.e., is submitted to a free corrosion in marine environment, the S-N curve constant C is divided by 2 and the S-N curve is continuous without any change of m. For normal design and as-welded joints, where the maximum and minimum stress level are not exceeding the yield strength, the influence of the static stress is considered deleted by the welding residual stresses. When extreme stress levels exceed the yield strength particular corrections are necessary and determined case by case. But when post-weld treatments are applied, the weld toe shape and the welding residual stresses are modified. Versus the applied technique the notch concentration factor has to be adjusted, but also the S-N curve power m may have to be changed. For example grinding only requires modifying the notch concentration factor when refusion TIG requires to modify both notch concentration factor and power m values. Non welded areas Hot spots exist also on without weld plate edges and the return experience show that cracks can be observed in such areas (figure 9) In such case there is no more welding residual stresses. The static stress level defined by the R ratio (R = Smin/Smax) influences the S-N curve to be used for the Miner sum calculation. Test results show that the m value and the position of the S-N curve are function of R for N > 104 but that for N < 104 there is no influence, the S-N curve being the same than for R = -1 (see figure 7) 1000 S (MPa) 4.3 FEM MODELS FOR FATIGUE The fine mesh models for the fatigue assessment have a mesh size of the order of magnitude of the plating thickness. The following structural connections of VLCG are candidates to fatigue assessment: Foot of main frames of side shell, Side shell longitudinals with transverse webs, Knuckles between double bottom & hopper tank, Brackets in cargo tank, Supports and keys, Tank dome Most of the structural details in the above list are similar to other vessels. But the support and keys are typical of VLCG. We are going to focus on these structural members in the next chapters. 5. VERTICAL SUPPORTS ASSESSMENT Generally, the fatigue calculations are based on the assumption of continuity and linearity of the phenomena. In case of the supports, there are discontinuities and non linearity of the forces due to the friction, sliding and shifting of the cargo tanks on the supports. It is due to this behaviour that a specific methodology was developed. As there are two friction coefficients, the static and the dynamic friction coefficients, the friction coefficient changes when the sliding appears. The figure 8 shows the histogram of the friction force depending on the probability level. On this figure, we can see the discontinuity in the friction force, which appears at a probability level P. The right side of the histogram is linked to the static coefficient, and the left hand side is linked to the dynamic coefficient. R = -1 R = R = 0.5 R > N Figure 7: S-N curves versus R ratio for non welded areas The Miner sum is therefore calculated with the hot spot stress range associated with a S-N curve determined versus the value of R. These curves allow taking into account for stress extremes greater than the yield strength after correction using the material stress-strain curve. Figure 8: Histogram for fatigue analysis of the supports
6 The probability level p where the sliding appears depends on the position of the studied support. The histogram is to be continuous. Consequently, it is necessary to modify the histogram, to obtain a continuous function of the number of cycle. This modified histogram is shown on the figure 9. The different histograms of sliding distribution are given for different probability of p ng = 1E0 ng = 1E2 ng = 1E4 ng = 1E6 Then two fatigue calculations are carried out and the damage ratio combined. The applied methodology for the fatigue assessment of the support is composed on the following steps, for the cases full load : Step 1: The coarse mesh and fine mesh models are calculated assuming the supports merged, i.e. there is no sliding, as shown on the figures 12 & 13. The part of the support in way of the tank is connected with the part in way of the hull in one unique model E+00 1E+01 1E+02 1E+03 1E+04 1E+05 1E+06 1E+07 1E+08 Figure 9: Modified histogram of supports An alternative to the unique histogram of friction force is to divide the histogram in two parts. On the figure 10, is shown the histogram of the friction force, when there is no sliding. The histogram of the friction force with sliding is shown figure 11. Figure 12: Fine mesh for fatigue assessment of vertical support in longitudinal direction S Static friction S cr stress range P = 1E-6 Probability level P Figure 10: Histogram of friction force without sliding S stress range S cr / 2 Dynamic friction P = 1E-6 Probability level P Figure11: Histogram of friction force when sliding Figure 13: Fine mesh for fatigue assessment of vertical support in longitudinal direction Step 2: Taking into account the results of the coarse mesh with merged supports, the probability level p where the sliding appears is evaluated. Step 3: The supports is calculated in two separates models, with the friction force input. The part of the support in way of the hull and the part of the support in way of the cargo tank are calculated separately. The model of the part of the support in way of the hull is shown on the figure 14. The friction force is introduced in way of the wooden spacer, both in the
7 longitudinal and transversal directions, in two separate load cases. Step 1: The coarse mesh and fine mesh models are run without contact in the upper anti rolling key in ballast and full load conditions. The deflection at the probability level depending on the probability level. The damage ratio is calculated in the critical elements of the keys. Step 2: The probability level where there is contact of the anti rolling key is calculated, Step 3: The calculation is run with anti rolling keys merged. The damage ratio is calculated in the critical elements of the keys. Step 4: The damage is calculated by combining the damage ratio obtained. The figure 16 shows an example of fine mesh for the fatigue assessment of the anti rolling keys. Figure 14: Fine mesh of lower part of vertical support Step 4: The damages ratio obtained in the conditions of the step 1 with the histogram shown on figure 10 and the damage ratio obtained in the condition of the step 3 with the histogram of the figure 11 are combined to obtain the final damage ratio. For the cases in ballast conditions, the damage ratio is calculated with only the self weight of the cargo tank. As in this case, most of the supports are found in tension in coarse mesh model, most of the elements modelling the supports are disconnected. For the calculation of this disconnected supports in the fine mesh model, the damage ratio is calculated as for the step 3, i.e. with the support in two parts. 6. ANTI ROLLING KEYS ASSESSMENT The methodology for the fatigue assessment of the anti rolling keys is very different from the methodology for the vertical supports, due to the fact that there is a gap between the keys. This gap has a significant influence on the fatigue life and is to be taken into account in the fatigue calculation. The figure 11 shows the gap. Figure 15: Gap in the anti rolling keys Due to this gap, the calculation is not linear. Then the methodology for the fatigue assessment includes the following steps: Figure 16: Fine mesh of upper anti rolling key 7. CONCLUSIONS If due to the use of structural scantling optimisation, by computing and the use of high tensile steel, the fatigue cracking has become one of the major failure modes in ship structures. It has to be pointed out that the observed failures inservice concern generally ships which have not been verified in fatigue during their design. Today the fatigue assessment is included in the ship rules. However, the application to structural members as supports and keys of LPG carriers is not easy due to the non linearity and the siding of these particular structures. This paper proposes a methodology for this assessment, published in the rev. 2 of the BV guidance note for structural assessment of LPG carriers. This methodology was applied o a case of a VLCG built recently, and has led to structural improvement has: thickness increment, additional grinding, improved brackets design
8 The accumulated expertise allow Bureau Veritas to help ship designers to improve the fatigue strength of the structures, but also ships operators, to understand inservice observed fatigue cracks, to improve the efficiency of inspection plans, or to propose adequate repair solutions. 8. ACKNOWLEDGEMENTS The authors wish to thank Bureau Veritas for permission to publish this paper. The views expressed are those of the authors and do not necessarily reflect those of Bureau Veritas. 9. REFERENCES 1. IMO, International code for the construction and equipment of Liquefied Gas Carriers, AUTHORS BIOGRAPHIES Philippe CAMBOS is a Naval Architect. He joined Bureau Veritas in 1991, in the calculation team. In 1994 he joined the development team of VeriSTAR software, where he was more specifically in charge of development of the fatigue methodologies. In 1997 he was appointed Head of the liquid in bulk section, in the Paris plan approval office. In 2002 he was appointed head of the Oil & Gas section in the Technical department of Bureau Veritas Marine Division in With his section he is in charge of drawing review for hull part of Oil tankers, Gas carriers and Offshore units. Christophe CHAUVIERE is Naval Architect. He joined BUREAU VERITAS in He worked for 4 years as plan approval surveyor for hull structure. He was appointed head of structural team of the Oil & Gas section of in the Technical department of Bureau Veritas Marine Division in 2002.
Spectral fatigue for FPSO conversion.
Spectral fatigue for FPSO conversion. Vincent Bonniol, Introduction The required time to build a new FPSO leads to more and more conversions from existing tankers. On demand of several oil companies has
More informationPlus - extended fatigue analysis of ship details
CLASS GUIDELINE DNVGLCG0152 Edition April 2016 Plus extended fatigue analysis of ship details The electronic pdf version of this document, available free of charge from http://www.dnvgl.com, is the officially
More informationEMSHIP Erasmus Mundus Master Course in Integrated Advanced Ship Design
EMSHIP Erasmus Mundus Master Course in Integrated Advanced Ship Design Global and Local Strength Analysis in Equivalent Quasistatic Head Waves, for a Tanker Ship Structure, Based on Full Length and 2-3
More informationOverview of the MAESTRO System
Overview of the MAESTRO System 1 Historical Highlights Early Stages of Development and Fielding Professor Owen Hughes conceived and developed MAESTRO Wrote and published (Wylie/SNAME) textbook Ship Structural
More informationLoads Recognition Tools Checks Reports
Loads Recognition Tools Checks Reports SDC Verifier is a powerful postprocessor program with an advanced calculation core which works seamlessly with Siemens multi-solver, FEA software suite Femap. SDC
More informationSDC Verifier is a powerful postprocessor program with an advanced calculation core which works seamlessly with Siemens multi-solver, FEA software
SDC Verifier is a powerful postprocessor program with an advanced calculation core which works seamlessly with Siemens multi-solver, FEA software suite Simcenter 3D. SDC Verifier & Simcenter 3D SDC Verifier
More informationCRASHWORTHINESS ANALYSIS OF A LOCK GATE IMPACTED BY THREE DIFFERENT RIVER SHIPS
CRASHWORTHINESS ANALYSIS OF A LOCK GATE IMPACTED BY THREE DIFFERENT RIVER SHIPS Hervé Le Sourne* - Jean-Claude Rodet** - Stéphane Paboeuf* - Guy Babaud* * French Shipbuilding Research Institute- Nantes
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 informationPCTCC vesselss. Sc. Thesiss by. March Centre for Naval Architecture
Racking induced stresses in PCTCC vesselss M. Sc. Thesiss by CARL-JOHAN March 2008 SÖDER Centre for Naval Architecture EXECUTIVE SUMMARY For Pure Car and Truck Carriers (PCTC) the main strength problem
More informationStructural Design Code Verifier. Version 3.0
Structural Design Code Verifier Version 3.0 What is SDC Verifier? The goal of SDC Verifier is checking structures according to standards and report generation. 2 SDC Verifier Embedded into Femap 3 Load
More informationSAFEHULL-DYNAMIC LOADING APPROACH FOR CONTAINER CARRIERS
GUIDANCE NOTES ON SAFEHULL-DYNAMIC LOADING APPROACH FOR CONTAINER CARRIERS (FOR THE SH-DLA CLASSIFICATION NOTATION) APRIL 2005 American Bureau of Shipping Incorporated by Act of Legislature of the State
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 informationEng Ship Structures 1 L E C T U R E 1 0 : F I N I T E E L E M E N T T E C H N I Q U E S I N S H I P S T R U C T U R A L D E S I G N
Eng. 6002 Ship Structures 1 L E C T U R E 1 0 : F I N I T E E L E M E N T T E C H N I Q U E S I N S H I P S T R U C T U R A L D E S I G N Contents Introduction Linear Analysis Static Non-linear Analysis
More informationStructural Design Code Verifier. Be an analyst not an admin
Structural Design Code Verifier Be an analyst not an admin SDC Verifier Embedded 2 Separate GUI What is SDC Verifier? The goal of SDC Verifier is checking structures according to standards and report generation.
More informationStructural Design Codes Verifier
Wouter van den Bos, SDC Verifier Owner Structural Design Codes Verifier Femap Symposium 2014 May 14-16, Atlanta, GA, USA FEMAP SYMPOSIUM 2014 Discover New Insights What is SDC Verifier? The goal of SDC
More informationNAUTICUS HULL RELEASE DOCUMENT
NAUTICUS HULL RELEASE DOCUMENT JANUARY 2013 RELEASE Copyright 2013 Det Norske Veritas AS All rights reserved. No part of this book may be reproduced, in any form or by any means, without permission in
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 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 informationA METHOD OF APPLYING LINEAR SEAKEEPING PANEL PRESSURE TO FULL SHIP STRUCTURAL MODELS
A METHOD OF APPLYING LINEAR SEAKEEPING PANEL PRESSURE TO FULL SHIP STRUCTURAL MODELS Ming Ma - DRS Defence Solutions, USA Chengbi Zhao - SCUT, China Nick Danese - COMPIT 2012 Liège, 16-18 April 2012 /1
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 informationTABLE OF CONTENTS SECTION 2 BACKGROUND AND LITERATURE REVIEW... 3 SECTION 3 WAVE REFLECTION AND TRANSMISSION IN RODS Introduction...
TABLE OF CONTENTS SECTION 1 INTRODUCTION... 1 1.1 Introduction... 1 1.2 Objectives... 1 1.3 Report organization... 2 SECTION 2 BACKGROUND AND LITERATURE REVIEW... 3 2.1 Introduction... 3 2.2 Wave propagation
More informationLATERALLY LOADED PILE GROUPS
LATERALLY LOADED PILE GROUPS Pedro Meneses Key words: Group Interaction, Lateral Response, Piles, p-multipliers, p-y Curves. Introduction The lateral resistance of pile foundations is a particularly important
More informationAutomatic FE modeler using stiffener-based mesh generation algorithm for ship structural analysis
Marine Structures 21 (2008) 294 325 www.elsevier.com/locate/marstruc Automatic FE modeler using stiffener-based mesh generation algorithm for ship structural analysis Beom-Seon Jang a,, Yong-Suk Suh a,
More informationDetail Analysis of Ship Structures
Detail Analysis of Ship Structures By David Heath, Neil Pegg Defence Research Establishment Atlantic, Dartmouth, Nova Scotia, Canada and Aaron Dinovitzer, Robert Walker Fleet Technology Limited, Kanata,
More informationFINITE ELEMENT ANALYSIS OF A COMPOSITE CATAMARAN
NAFEMS WORLD CONGRESS 2013, SALZBURG, AUSTRIA FINITE ELEMENT ANALYSIS OF A COMPOSITE CATAMARAN Dr. C. Lequesne, Dr. M. Bruyneel (LMS Samtech, Belgium); Ir. R. Van Vlodorp (Aerofleet, Belgium). Dr. C. Lequesne,
More informationParamarine Tutorial 5
Paramarine Tutorial 5 In this tutorial we will learn how to perform a longitudinal strength analysis of our design. We will then define the structural elements that comprise the ship structure and check
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 informationLinear Elastic Fracture Mechanics (LEFM) Analysis of Flaws within Residual Stress Fields
Linear Elastic Fracture Mechanics (LEFM) Analysis of Flaws within Residual Stress Fields David Woyak 1, Brian Baillargeon, Ramesh Marrey, and Randy Grishaber 2 1 Dassault Systemés SIMULIA Corporation &
More informationThe part to be analyzed is the bracket from the tutorial of Chapter 3.
Introduction to Solid Modeling Using SolidWorks 2007 COSMOSWorks Tutorial Page 1 In this tutorial, we will use the COSMOSWorks finite element analysis (FEA) program to analyze the response of a component
More informationSDC Verifier is a powerful post-processor extension for Simcenter 3D which automates the full FEA workflow.
SDC Verifier is a powerful post-processor extension for Simcenter 3D which automates the full FEA workflow. SDC Verifier & Simcenter 3D SDC Verifier is a powerful post-processor program that is used to
More informationRevision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering. Introduction
Revision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering Introduction A SolidWorks simulation tutorial is just intended to illustrate where to
More informationEngineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering
Engineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering Here SolidWorks stress simulation tutorials will be re-visited to show how they
More informationOTC MS. Abstract
This template is provided to give authors a basic shell for preparing your manuscript for submittal to a meeting or event. Styles have been included to give you a basic idea of how your finalized paper
More informationA dynamic model for lifting heavy modules between two floating offshore structures
A dynamic model for lifting heavy modules between two floating offshore structures Radboud R.T. van Dijk Maritime Research Institute Netherlands (MARIN), Netherlands Alex A. Hendriks Heerema Marine Contractors
More informationDESIGNING FIBER OPTIC DYNAMIC RISER CABLES FOR OFFSHORE APPLICATIONS
DESIGNING FIBER OPTIC DYNAMIC RISER CABLES FOR OFFSHORE APPLICATIONS Jon Steinar Andreassen (Nexans Norway) Email: Nexans Norway AS, P.O Box 645 Etterstad, N-65 Oslo,
More informationLECTURE 1a Introduction to ship structural design
LECTURE 1a Introduction to ship structural design A very competitive ship market and emergence of novel concepts, including advanced marine vehicles, has created a need for improvements in design methods.
More informationSDC. Engineering Analysis with COSMOSWorks. Paul M. Kurowski Ph.D., P.Eng. SolidWorks 2003 / COSMOSWorks 2003
Engineering Analysis with COSMOSWorks SolidWorks 2003 / COSMOSWorks 2003 Paul M. Kurowski Ph.D., P.Eng. SDC PUBLICATIONS Design Generator, Inc. Schroff Development Corporation www.schroff.com www.schroff-europe.com
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 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 informationComparative Analysis of Marine Structural End Connections
University of New Orleans ScholarWorks@UNO University of New Orleans Theses and Dissertations Dissertations and Theses 12-20-2009 Comparative Analysis of Marine Structural End Connections Bret Silewicz
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 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 informationSolid design. Reliable pipelines. Simulation results can be viewed and printed in different formats in tables, graphs and in 3D illustrations.
Bringing added value to pipeline engineers worldwide SAGE Profile has been specifically designed to assist pipeline engineers in the design, installation and analysis of offshore pipelines. The powerful
More informationThe Role of Finite Element Analysis in Light Aircraft Design and Certification
The Role of Finite Element Analysis in Light Aircraft Design and Certification Nigel Bamber Wey Valley Aeronautics Ltd www.weyvalleyaero.co.uk Engineering Consultancy Civil and Military Aerospace and Motorsport
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 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 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 informationStructural Nonlinear Analysis of a Disconnector Pelikelo (a kind of hook) using ANSYS/Workbench
Structural Nonlinear Analysis of a Disconnector Pelikelo (a kind of hook) using ANSYS/Workbench Mário Coutinho MCS Engineering LTDA. Fátima Souza, M.Sc., Gabriel Silva e Decio Paiva SOFTEC Software Technology
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 informationStrength investigation of a small size floating dock unit by 3D-FEM models in head design waves
IOP Conference Series: Materials Science and Engineering PAPER OPEN ACCESS Strength investigation of a small size floating dock unit by 3D-FEM models in head design waves To cite this article: E Burlacu
More informationCE Advanced Structural Analysis. Lab 4 SAP2000 Plane Elasticity
Department of Civil & Geological Engineering COLLEGE OF ENGINEERING CE 463.3 Advanced Structural Analysis Lab 4 SAP2000 Plane Elasticity February 27 th, 2013 T.A: Ouafi Saha Professor: M. Boulfiza 1. Rectangular
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 informationCONSTRUCT USER S MANUAL. Conceptual Structural Design Software REVISION 1.0 ( )
USER S MANUAL Conceptual Structural Design Software REVISION 1.0 (24.01.2010) Aalto University School of Science and Technology Department of Applied Mechanics Marine Technology Table of Contents TABLE
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 informationA Solution to Robust Shaft Alignment Design
A Solution to Robust Shaft Alignment Design Prepared for SNAME Propellers/Shafting Symposium, Virginia Beach- September 12-13, 2006 Davor Šverko, American Bureau of Shipping, Houston Originally presented
More informationReview on Design Optimization of Liquid Carrier Tanker for Reduction of Sloshing Effects
IOSR Journal of Mechanical and Civil Engineering (IOSR-JMCE) e-issn: 2278-1684,p-ISSN: 2320-334X, Volume 6, Issue 3 (May. - Jun. 2013), PP 15-24 Review on Design Optimization of Liquid Carrier Tanker for
More informationAnalysis of ANSI W W 6x9-118,
Page 1 of 8 Analysis of ANSI W W 6x9-118,110236220472 Author: Analysis Created: Analysis Last Modified: Report Created: Introduction Administrator, 08:29:09, 08:29:09 09:26:02 Database: Z:\ENGENHARIA\ESTUDOS
More informationWORKSHOP 6.4 WELD FATIGUE USING HOT SPOT STRESS METHOD. For ANSYS release 14
WORKSHOP 6.4 WELD FATIGUE USING HOT SPOT STRESS METHOD For ANSYS release 14 Objective: In this workshop, a weld fatigue analysis on a VKR-beam with a plate on top using the nominal stress method is demonstrated.
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 informationPennDOT e-notification Bureau of Business Solutions and Services Highway/Engineering Applications Division
PennDOT e-notification Bureau of Business Solutions and Services Highway/Engineering Applications Division STLRFD No. 013 October 17, 2016 Release of Version 2.4.0.0 The Department s LRFD Steel Girder
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 informationInteraction of design and analysis, integration of CAD and FEA U. Rabien & R. Bronsart Germanischer Lloyd, Vorsetzen 32, Hamburg, Germany
Interaction of design and analysis, integration of CAD and FEA U. Rabien & R. Bronsart Germanischer Lloyd, Vorsetzen 32, 20459 Hamburg, Germany ABSTRACT This paper describes an implemented strategy for
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 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 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 informationSOLIDWORKS Simulation
SOLIDWORKS Simulation Length: 3 days Prerequisite: SOLIDWORKS Essentials Description: SOLIDWORKS Simulation is designed to make SOLIDWORKS users more productive with the SOLIDWORKS Simulation Bundle. This
More informationVALIDATION METHODOLOGY FOR SIMULATION SOFTWARE OF SHIP BEHAVIOUR IN EXTREME SEAS
10 th International Conference 409 VALIDATION METHODOLOGY FOR SIMULATION SOFTWARE OF SHIP BEHAVIOUR IN EXTREME SEAS Stefan Grochowalski, Polish Register of Shipping, S.Grochowalski@prs.pl Jan Jankowski,
More informationDARWIN 8.1 Release Notes
DARWIN 8.1 Release Notes March 2015 Southwest Research Institute Summary of New Capabilities DARWIN 8.1 includes the following new features: Autozoning with inspection Random FE residual stress Anomaly
More informationComparison of 3-D Fracture Analysis Methods Based on ANSYS Workbench
International Conference on Material Science, Energy and Environmental Engineering (MSEEE 2017) Comparison of 3-D Fracture Analysis Methods Based on ANSYS Workbench Dejun Liua, Fang Xieb and Ningbo Gaoc
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 informationBehaviour of cold bent glass plates during the shaping process
Behaviour of cold bent glass plates during the shaping process Kyriaki G. DATSIOU *, Mauro OVEREND a * Department of Engineering, University of Cambridge Trumpington Street, Cambridge, CB2 1PZ, UK kd365@cam.ac.uk
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 informationAISIBEAM User's Manual (Version 3.0)
AISIBEAM User's Manual (Version 3.0) Shabin Taavoni, Ph.D., PE, title Structural Software Inc. location John C. Huang Ph.D., PE, Principal CHC Engineering, LLC Herndon, VA Scope of Software The software
More informationDifficulties in FE-modelling of an I- beam subjected to torsion, shear and bending
DEGREE PROJECT, IN STEEL STRUCTURES, SECOND LEVEL STOCKHOLM, SWEDEN 2015 Difficulties in FE-modelling of an I- beam subjected to torsion, shear and bending MIRIAM ALEXANDROU KTH ROYAL INSTITUTE OF TECHNOLOGY
More informationExperimental and numerical study of sloshing and swirling in partially filled membrane-type LNG tanks
Maritime Transportation and Harvesting of Sea Resources Guedes Soares & Teixeira (Eds) 2018 Taylor & Francis Group, London, ISBN 978-0-8153-7993-5 Experimental and numerical study of sloshing and swirling
More informationEmbedded Reinforcements
Embedded Reinforcements Gerd-Jan Schreppers, January 2015 Abstract: This paper explains the concept and application of embedded reinforcements in DIANA. Basic assumptions and definitions, the pre-processing
More informationMilovan Perić CD-adapco. Use of STAR-CCM+ in Marine and Offshore Engineering and Future Trends
Milovan Perić CD-adapco Use of STAR-CCM+ in Marine and Offshore Engineering and Future Trends Introduction CD-adapco is developing simulation capabilities in STAR-CCM+ specifically for marine and offshore
More informationCOMPARISON OF FULL-SCALE MEASUREMENTS WITH CALCULATED MOTION CHARACTERISTICS OF A WEST OF AFRICA FPSO
Proceedings of OMAE3 ND International Conference on Offshore Mechanics and Arctic Engineering June 8 3, 3, Cancun, Mexico OMAE3-378 COMPARISON OF FULL-SCALE MEASUREMENTS WITH CALCULATED MOTION CHARACTERISTICS
More informationUSER S MANUAL OF FORMWORKS PLUS FOR
USER S MANUAL OF FORMWORKS PLUS FOR VECTOR5 by Kyle Blosser Serhan Guner Frank J. Vecchio May 2016 Copyright by K. Blosser, S. Guner, F. J. Vecchio (2016) TABLE OF CONTENTS 1. Introduction... 4 2. Create
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 informationList of forms CLAP/WGP by subject /68/UE
List of forms CLAP/WGP by subject - 2014/68/UE Subject Assembly - Assembly including an item of pressure equipment placed on the market before 29 May 2002 in compliance with national pre-ped regulations
More informationOPTIMIZATION OF STIFFENED LAMINATED COMPOSITE CYLINDRICAL PANELS IN THE BUCKLING AND POSTBUCKLING ANALYSIS.
OPTIMIZATION OF STIFFENED LAMINATED COMPOSITE CYLINDRICAL PANELS IN THE BUCKLING AND POSTBUCKLING ANALYSIS. A. Korjakin, A.Ivahskov, A. Kovalev Stiffened plates and curved panels are widely used as primary
More informationStatic and dynamic simulations for automotive interiors components using ABAQUS
Static and dynamic simulations for automotive interiors components using ABAQUS Mauro Olivero, Vincenzo Puleo, Massimo Barbi, Fabrizio Urbinati, Benedetta Peyron Fiat Research Centre Giancarlo Luciani,
More informationRobustness analysis of metal forming simulation state of the art in practice. Lectures. S. Wolff
Lectures Robustness analysis of metal forming simulation state of the art in practice S. Wolff presented at the ICAFT-SFU 2015 Source: www.dynardo.de/en/library Robustness analysis of metal forming simulation
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 informationModeling Strategies for Dynamic Finite Element Cask Analyses
Session A Package Analysis: Structural Analysis - Modeling Modeling Strategies for Dynamic Finite Element Cask Analyses Uwe Zencker, Günter Wieser, Linan Qiao, Christian Protz BAM Federal Institute for
More informationCFD Application in Offshore Structures Design at PETROBRAS
CFD Application in Offshore Structures Design at PETROBRAS Marcus Reis ESSS CFD Director Mooring System Design of Floating Production Systems; Current and Wind Loads; Wave Induced Drag Coefficients. Case
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 informationComputer Aided Ship Design. Part II. Curve and Surface Modeling
Naval Architecture & Ocean Engineering Computer Aided Ship Design Part II. Curve and Surface Modeling Ch. 1 Introduction September, 213 Prof. Myung-Il Roh Computer Aided Ship Design Lecture Note Department
More informationSIMPLIFIED FATIGUE ANALYSIS BASED ON ABS GUIDE FOR " FATIGUE ASSESSMENT OF OFFSHORE STRUCTURE" WITH 2 SEGMENT SN CURVE
Welcome to this application for Simplified Fatigue Analysis based on ABS Rules What this program does? This program can be used to assess the Fatigue Strength of an Offshore Structure based on ABS Rules
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 informationEngineering Analysis
Engineering Analysis with SOLIDWORKS Simulation 2018 Paul M. Kurowski SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit the following websites
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 informationIntroduction to the Finite Element Method (3)
Introduction to the Finite Element Method (3) Petr Kabele Czech Technical University in Prague Faculty of Civil Engineering Czech Republic petr.kabele@fsv.cvut.cz people.fsv.cvut.cz/~pkabele 1 Outline
More informationInvestigation of the behaviour of single span reinforced concrete historic bridges by using the finite element method
Structural Studies, Repairs and Maintenance of Heritage Architecture XI 279 Investigation of the behaviour of single span reinforced concrete historic bridges by using the finite element method S. B. Yuksel
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 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 informationValidating Finite Element Model with Field Data Joint Rail Conference 2014 Colorado Springs, CO 4 March 2014
Validating Finite Element Model with Field Data Joint Rail Conference 2014 Colorado Springs, CO 4 March 2014 Professor Bassem Andrawes and George Zhe Chen Slide 2 Outline Role of Finite Element (FE) analysis
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 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 information