People's Democratic Republic of Algeria. Ministry of Higher Education and Scientific Research. University of Laarbi Tebessi

Transcription

1 People's Democratic Republic of Algeria Ministry of Higher Education and Scientific Research University of Laarbi Tebessi Faculty of Science and Technology Civil Engineering Department A PARAMETRIC COMPARATIVE ASSESSMENT OF THE NONLINEAR BEHAVIORS OF FLEXURAL AND SHEAR LINKS IN EBF STRUCTURES UNDER MONOTONIC CYCLING LOADS TO EC8 AND AISC 2006 INCLUDING THE EFFECT OF STIFFENERS NUMBER AND CONFIGURATION ABU HALAWEH Ahmad Master Academic study Speciality: structures Promo: 2015/2016 Presented and supported publicly in front the examining committee members: President: Dr: Rapporteur: Dr. LABED Abderrahim Examiner: Dr:

2

3 Acknowledgment First and foremost praise to almighty god, this thesis was completed after four months of hard daily continuous work, I dedicate this humble work to my family whom i will always be indebtedness to endure the bitterness of separation, and they was always backing me up with strength and hope, I also want to extend my appreciation to my dearest friend Ossama for his encouragement and support In spite of the vast distance separating us, thanks also must be presented to all my brothers how escort me in the long way of study life Khalil, Ihab, Fakher, and all of my colleagues. l would like to express my sincere thanks to my supervisor, LABED Abderrahim, for his patience, encouragement, kindness and generosity at all stages of my research work. He always found time to share his vast and deep knowledge in a highly intelligible manner with me. Without my supervisor, LABED s support, scientific, moral and monetary, it is highly doubtful that I would have finished this thesis Great thank to all working staff in the department of civil engineering for the support and help in all the course of five years of study. Thanks also to fellows BOUDIAF Taqie and MAJOR Abdel Haliem for their exhausting effort in ABAQUS.

4 Abstract To assess the nonlinear behaviour of seismic links made of hot-rolled IPE 360 and 450 sections were studied by means of the finite element method.based on the specifications and assumptions given in seismic codes (EC8, AISC2006). The nonlinear twenty one models computations were performed using the commercial finite element software package ABAQUS, which has the ability to consider both geometric and material nonlinearities in a given model. These models are series of isolated links belonging to flexural and shear kind. These two sections differ from their slenderness ratios. Due to the high and moderate ductility demand on short and long links respectively, the flange and web area of the link surface (IPE profile) might experience buckling phenomena; therefore it is required to install web stiffeners. These buckling phenomena of links in EBFs cause rapid strength and stiffness degradation, and this significantly impedes the energy dissipation capabilities of the system. Another investigation of the effect of increasing the numbers and changing the intermediate stiffeners configurations has been carried out on the nonlinear behaviour of links. Also, an attempt was made to investigate the role of the shape of the cross section by considering HEB profiles. The finite element model used C3DR 8-nodes elements to represent the webs, flanges, and stiffeners of the link. An element edge length of approximately 20 mm was found to adequately represent the behaviour of the link through a mesh refinement study. The resulting element edge to thickness ratios varied from 1.6 to 3.0. Full cyclic analysis is necessary in this study to consider the effects of local buckling with the associated strength degradation. The link loading protocol used in this study is described in 2005 AISC Seismic Provisions. The loading protocol for long links consisted of 32 cycles, while the loading protocol for short links consisted of 35 cycles. The results from this study show that placing stiffeners with various number and different configuration has a favourable effect on all short links, while for the flexural links, this effect depends on the height of the section. Favourable effect of stiffeners has been found for long links with IPE360, while non-significant effect has been noticed for IPE450. Also, the local buckling from which IPE sections suffer appears to not affecting links made from HEB. Key words: EBF, link, shear, flexural, nonlinear analysis, FEA, ABAQUS, buckling, strength, stiffness.

5 List of symbols A f = Flange area As = Cross-sectional area of the structural steel core Ast = Area of link stiffener Aw = Link web area b = width of the flange b f = Flange width e = link length E= Modulus of elasticity of steel fu= ultimate stress of steel fy = nominal yield strength of steel Iy = Moment of inertia around y-axis Iz = Moment of inertia around z-axis M Ed = the design values of the bending moment in the seismic design situation Mp, link = the bending plastic design resistances of link M pl,rd = design value of plastic moment resistance at end of a member N= Safety factor N Ed = design axial force from the analysis for the seismic design situation N pl,rd = design value of yield resistance in tension of the gross cross-section of a member q = behaviour factor t f = flange thickness of a seismic link t s : Depth of stiffeners t w = web thickness of a seismic link U= energy V= design value of shear resistance of a member Page I

6 List of symbols V Ed = design shear force from the analysis for the seismic design situation Vp, link = the shear plastic design resistances of link Z = Plastic section modulus of a member α1 = multiplier of horizontal design seismic action at formation of first plastic hinge in the system α1= multiplier of horizontal design seismic action at formation of first plastic hinge in the system γov = material over strength factor γ total = Link rotation angle ε= shear stress ε 1, ε 2, ε 3 = shear stress component θp= rotation capacity of the plastic hinge region λp, λps = Limiting slenderness parameter for compact element ρ =Ratio of required axial force Pu to required shear strength Vu of a link σ = normal stress σ 1, σ 2, σ 3 = normal stress corposants υ = Poisson s ratio Ω = multiplicative factor on axial force N Ed,E from the analysis due to the design seismic action, for the design of the non-dissipative members in concentric or eccentric braced frames Ω= Safety factor Page II

7 LIST OF ABBREVIATIONS CBFs = Concentrically braced frames. D= for diagonal stiffeners EBFs = eccentrically braced frames FEA = Finite Element Analysis FEA = Finite Element Analysis FEM = Finite Element Method LL: long link 360 without Stiffeners LLʺ: long link 450 without Stiffeners LL1: long link 360 with two symmetrical transverse stiffeners LL2: long link 360 with two transverse stiffeners associated to two diagonal stiffeners; LL3: long link 360 with three transverse stiffeners (one in mid-span) LL4: long link 360 with three transverse stiffeners associated to two other diagonal stiffeners LL5: long link 450 with two symmetrical transverse stiffeners LL6: long link 450 with two transverse stiffeners associated to two diagonal stiffeners; LL7: long link 450 with three transverse stiffeners (one in mid-span) LL8: long link 450 with three transverse stiffeners associated to two other diagonal stiffeners MRFs = Unbraced or moment-resisting frames NDS: Number Diagonal Stiffeners NTS: Number of Transverse Stiffeners PEEQ = Equivalent Plastic strain PEMAG = Magnitude Plastic strain SL: short link 360without Stiffeners SLʺ: short link 450 without Stiffeners SL1: short link 360 with two symmetrical transverse stiffeners SL2: short link 360 with two transverse stiffeners associated to two diagonal stiffeners; SL3: short link 360 with three transverse stiffeners (one in mid-span) SL4: short link 360 with three transverse stiffeners associated to two other diagonal stiffeners Page III

8 LIST OF ABBREVIATIONS SL5: short link 450 with two symmetrical transverse stiffeners SL6: short link 450 with two transverse stiffeners associated to two diagonal stiffeners; SL7: short link 450 with three transverse stiffeners (one in mid-span) SL8: short link 450 with three transverse stiffeners associated to two other diagonal stiffeners SL9: short link 450 with two transverse stiffeners associated to one diagonal stiffener T= for transverse stiffeners U = Magnitude Displacement Page IV

9 List of tables Title Page Table 1.1 Comparison between MRF and braced frames (CBF and EBF) 2 Table 1.2 Provisions for eccentrically braced frames according to Eurocodes versus 12 AISC ASCE Table 4.1 Geometrical properties of the models 60 Table 4.2 Dimensions and material properties of IPE 63 Table 4.3 Section classes according to EC3 63 Table 4.4 Proposed long link Loading Protocol (IPE360) 65 Table 4.5 Proposed long link Loading Protocol (IPE450) 65 Table 4.6 Proposed Short Link Loading Protocol (IPE360) 65 Table 4.7 Proposed Short Link Loading Protocol (IPE450) 66 Table5.1 Identification of long links models 69 Table5.2 Identification of short links models 69 Table 5.3 Final results given by ABAQUS for Long links 82 Table 5.4 Final results given by ABAQUS for Short links 83 Table 5.5 Comparison between IPE and HEB. 84 Page VI

10 List of figures Title Page Figure 1. 1 Some Eccentrically Brace Frame Configurations in buildings (EBFs). 2 Figure 1. 2 Moment Resisting Frames (MRFs). 3 Figure 1. 3 Typical CBF (Diagonal, Inverted V, V, Chevron and Knee bracing 4 system) Configurations Figure 1. 4 Eccentrically Braced Frames (EBFs). 5 Figure 1 5 Configurations of frames with eccentrically braces. 6 Figure 1. 6 mid span link 7 Figure 1. 7 diagonal EBF 7 Figure 1. 8 Inelastic action locations in MRFs, EBFs and CBFs 8 Figure 1. 9 Variation of elastic lateral stiffness with e/ L for two simple EBFs. 9 Figure Variation of first natural period with e/l for a five-story EBFs 10 Figure Variation of frame plastic capacity with e/l 10 Figure a) The Inelastic behaviour of concentrically braced frames in a major 11 earthquake.b) Plastic deformation of eccentrically braces frames. Figure Energy dissipation mechanisms 11 Figure Inelastic mechanisms for EBF under lateral load 12 Figure 2.1 Inelastic mechanisms for the two bracing systems 16 Figure 2.2 (a) Short Link and b) Long link 16 Figure2.3 Distribution of forces in the link and the beam outside the link for 17 different configurations Figure 2.4 The links free body diagram 18 Figure 2.5 a) Shear yielding. b) Flexural yielding of link 19 Figure 2.6 Link plastic rotation of EBF with a link at the middle of the beam 20 Figure 2.7 Link plastic rotation of D-type EBF with one link next to the column 20 Figure 2.8 Link plastic rotation of EBF with two links next to the columns 20 Figure 2.9 Typical link 21 Figure 2.10 Definition of symbols for I link sections 24 Figure2.11a)Equal moments at link ends b) unequal moments at link ends 25 Figure 2.12 Protocol of 2005 AISC seismic provisions 33 Fig.3.1 Coarse-mesh. Two-dimensional model of a gear tooth. All nodes and 37 elements lie in the plane of the paper Figure 3.2 (a) A general two-dimensional domain of field variable (x, y). (b) A threenode 39 finite element defined in the domain. (c) Additional elements showing a partial finite element mesh of the domain Figure 3.3 Arbitrary curved-boundary domain modeled using square elements. 41 Stippled areas are not included in the model. A total of 41 elements are shown. (b) Refined finite element mesh showing reduction of the area not included in the model, total of 192 elements are shown Figure 3.4 Material failures due to relative sliding of atomic planes 44 Page VII

11 List of figures Figure 3.5 Stress strain curve and the strain energy 46 Figure 4.1 ABAQUS Modules 51 Figure 4.2 Family of element in ABAQUS 53 Figure 4.3 Number of nodes of element in ABAQUS a) Order of interpolation b) 53 Types of integration Figure 4.4 Displacement and Rotational degrees of freedom 54 Figure 4.5 Systems of Units 55 Figure 4.6 Element shapes in ABAQUS: a) Quad, b) Quad-dominated c) Tri, d) 56 Hex, e) Hex-dominated, f) Tet, g) Wedge Figure 4.7 Link geometry without stiffeners: a) long link b) short link 59 Figure 4.8 Types of stiffeners: a) transverse stiffeners b) diagonal stiffeners 59 Figure 4.9 Basic geometry with Stiffeners of models example for a short IPE Figure 4.10 FEM model boundary conditions applied to the links: (a) Initial 63 configuration b) deformed configuration Figure 4.11 The loading protocol 64 Figure 4.12 Meshing type example for a short Figure 5.1 The applied loading protocol 68 Figure 5.2 a) Distributions of stress at 125 increment b) Distributions of displacement magnitude at 125 increment c) Distributions of stress at the increment 170 d) Distributions of displacement magnitude at the increment 170 Figure 5.3 a) Distributions of stress at 147 increment b) Distributions of displacement magnitude at 149 increment c) Distributions of stress at the increment 199 d) Distributions of displacement magnitude at the increment 199 Figure 5.4 a) Distributions of stress at 153 increment b) Distributions of displacement magnitude at 153 increment c) Distributions of stress at the increment 216 d) Distributions of displacement magnitude at the increment 216 Figure 5.5 a) Distributions of stress at 143 increment b) Distributions of displacement magnitude at 143 increment c) Distributions of stress at the increment 197 d) Distributions of displacement magnitude at the increment 197 Figure 5.6 a) Distributions of stress at 153 increment b) Distributions of displacement magnitude at 153 increment c) Distributions of stress at the increment 216 d) Distributions of displacement magnitude at the increment 216 Figure 5.7 a) Distributions of stress at last increment b) Distributions of displacement magnitude at last Figure 5.8 a) Distributions of stress at last increment b) Distributions of displacement magnitude at last increment Figure 5.9 a) Distributions of stress at last increment b) Distributions of displacement magnitude at last increment Figure 5.10 a) Distributions of stress at last increment b) Distributions of displacement magnitude at last increment Page VIII

12 List of figures Figure 5.11 a) Distributions of stress at last increment b) Distributions of 76 displacement magnitude at last increment Figure 5.12 Samples of results for LLʺ model a) Distributions of stress at last 77 increment, b) Distributions of displacement magnitude at last increment Figure 5.13 Samples of results for LL5 model a) Distributions of stress at last 77 increment b) Distributions of displacement magnitude at last increment Figure 5.14 Samples of results for LL6 model a) Distributions of stress at last 78 increment b) Distributions of displacement magnitude at last increment Figure 5.15 Samples of results for LL7 model a) Distributions of stress at last 78 increment b) Distributions of displacement magnitude at last increment Figure 5.16 Samples of results for LL8 model a) Distributions of stress at last 78 increment b) Distributions of displacement magnitude at last increment Figure 5.17 a) Distributions of stress at 108 increment b) Distributions of 79 displacement magnitude at 108 increment c) Distributions of stress at the increment 145 d) Distributions of displacement magnitude at the increment 145. Figure 5.18 a) Distributions of stress at last increment b) Distributions of 80 displacement magnitude at last increment. Figure 5.19 a) Distributions of stress at last increment b) Distributions of 80 displacement magnitude at last increment. Figure 5.20 a) Distributions of stress at last increment b) Distributions of 81 displacement magnitude at last increment. Figure 5.21 a) Distributions of stress at last increment b) Distributions of 81 displacement magnitude at last increment. Figure 5.22 a) Distributions of stress at last increment b) Distributions of 82 displacement magnitude at last increment. Figure 5.23 Samples of results for HEB280 model a) Distributions of stress at last 84 increment b) Distributions of displacement magnitude at last increment Figure 5.24 Samples of results for HEB320 model a) Distributions of stress at last 84 increment b) Distributions of displacement magnitude at last increment Figure 5.25 shear force and the displacement for SL7, SL8 models 85 Page IX

13 Table of contents

14 Table of contents Title Page Acknowledgment / Abstract / List of symbols List of abbreviations List of tables List of figures Table of contents Introduction I III VI VII X A-C CHAPITRE 1: LATERAL SEISMIC STEEL RESISTING SYSTEMS 1 1. Introduction 1 2. Types of steel structures Unbraced or Moment-Resisting Frames (MRFs) Concentrically Braced Frames (CBFs) Eccentrically Braced Frames (EBFs) EBFs design requirements Basic behaviour of EBFs Stiffness and Strength Inelastic response and energy dissipation Overall comparison Table for EBFs according to Eurocodes versus AISC ASCE Conclusion 14 CHAPTER 2: LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC Introduction Links types Distribution of forces in links and beams in different EBF 16 Page X

15 Table of contents configuration 4. Factor affecting the inelastic behaviour of a link Comparison of yielding failure of shear and flexural (long) links Link plastic rotation angle Link of the EBF buildings Design criteria of links Design Criteria to EC According to AISC EBF Structures to AISC Link Stiffeners ProvisionsErreur! Signet non défini Comparison between the codes Monotonic cyclic loadings Introduction Concepts behind development of loading protocols General requirements Examples of loading protocols used presently or in the recent past Moment connections Loading sequence for link-to-column connections 33 CHAPTER 3: NONLINEAR FINITE ELEMENT ANALYSES General introduction to finite element method (FEM) Overview and summary of FEA Historical development of FEM How does the finite element method work? Finite element and exact solutions Basis of FE analysis procedure in ABAQUS 41 Page XI

16 Table of contents 7. Nonlinear finite element analysis Geometrical Nonlinearity Material Nonlinearity Failure Criteria The Maximum - Shear - Stress Theory Distortion-Energy Theory or The Von Mises Theory 45 CHAPTER 4: INELASTIC MODELLING OF LINKS BY ABAQUS Introduction Introduction to ABAQUS Organization of ABAQUS ABAQUS applications capabilities Solution sequence Element type in ABAQUS System of units in ABAQUS Element shapes in ABAQUS Linear and quadratic element types MODELS DESCRIPTION Definition of the models Link geometry Stiffeners geometry Description of Models Material Properties Boundary Conditions Cyclic Loading Meshing 66 CHAPTER 5: RESULTS AND DISCUSSION Page XII

17 Table of contents 1. Introduction Results and detailed discussion Long links IPE 360 ` Short Link IPE Long Links IPE Short Link IPE Full results from ABAQUS Long Link Short links Comparison between tow section HEB and IPE for long link without stiffener 83 Conclusion D-E References / Page XIII

18 Introduction

19 INTRODUCTION The initial idea of this research was to investigate the nonlinear behaviour of long links we provide some works dealing with this kind of link in the literature. This analysis intended to contribute to a better comprehension of such kind of links. However, when the modelling of such links was successfully made, the idea has come to extend the study to include the shear links and to understand the behaviour of each kind. This attempt was also successful. However, with the huge volume of results coming from ABAQUS for each case raises the difficulties of dealing with them all. It has been decided to take a sample of results including the equivalent stress, the magnitude of displacement as samples of results. Eccentrically braced steel frames (EBFs) are very efficient structures for resisting earthquakes as they combine the ductility of that is characteristic of moment frames (MRFs) and the stiffness associated with concentric braced frames (CBFs). The successful performance of EBFs under seismic loading depends on the stable inelastic rotation of active links while other frame component remain essentially. EBFs are characterized by an isolated segment of beam, which is referred to as link. All inelastic activity is intended to be confined to the properly detailed links. At least one end of each brace intersects a beam at a point offset from the beam intersection with the column or with the opposing brace. Structures suffer significant inelastic deformation under a strong earthquake and dynamic characteristics of the structure change with time so investigating the performance of a structure requires inelastic analytical procedures accounting for these features. An EBF is a steel-braced frame designed in accordance with chapter 8 of the EC8 part 6 and Section 15, Part I, of the AISC Seismic Provisions. The short section of the beam between opposing braces, or between a brace and the beam-column intersection, is called the link beam, and is the element of the frame intended to provide inelastic cyclic yielding. Link beams are the fuses of the EBF structural system, and are to be placed at locations that will preclude buckling of the braces. A link beam must be located in the intersecting beam at least at one end of each brace. In the EBFs inelastic activity is confined to a small length of the floor beams which yields mostly in shear (therefore called the shear link). To take advantage of the ductility of the link, it is important that all related framing elements are strong enough to force the link to yield, and that they maintain their integrity through the range of forces and displacements developed during the yielding of the link. It is desirable that structures are proportioned to yield at locations which are most capable of deforming into inelastic range and sustaining large cyclic inelastic deformations. The aim of the eccentrically braced frame design is to provide a ductile link that will yield in lieu of buckling of its braces when the frame experiences dynamic loads in excess of its elastic strength. As pointed out Page A

20 INTRODUCTION earlier, the reason that inelastic activity should be limited within links is to prevent other elements from yielding. Depending on the section properties of the link, link may yield either in shear extending over the full length of the link or in flexure at the link ends, or the combination of shear and flexural yielding. Yielding mechanism of links depends on material properties of links such as moment capacity, shear capacity, and strain hardening. Link beams can yield in shear, in bending, or in both shear and bending at the same time. Which yield mechanism governs is a function of the relationship of link length to the ratio of its bending strength to shear strength. Since link beams that yield in shear are considered to have the most stable energy-dissipating characteristics, most of the EBF research has tested the cyclic inelastic capacity of link beams with shear yielding at large rotations. Design of EBFs habitually starts by selecting the length of links at all levels based on seismic code criteria such as architectural constraints. After sizing the links, the selected length of link should be checked using material properties in order to satisfy code equations (EC8, AISC) which category the link belongs to (shear yielding, flexural yielding, or combination of shear and flexural yielding). This is the most important step of designing an EBF because strength and ductility of an EBF is closely related to the strength and ductility of the links, and ill-proportioned links along the height of structures can lead to concentration of large inelastic link deformations at some floor levels due to over-strengthening of links at some levels. Furthermore, elements other than the links are designed based on the maximum expected strength of links thus, improper sizing of links can also cause unexpected yielding in those other elements. Equations to determine the length ranges and allowable link inelastic rotation angles have been developed for I sections as specified in EC8 chapter 8 and AISC Seismic Provisions. Link plastic rotation angle ( γp ) can be easily estimated by frame geometry assuming rigidplastic behaviour of the frame members. The rotation demand on the link beam is a multiple of the lateral drift of the frame as a whole. It is important to point out that the EBF structures are not yet covered by the Algerian Seismic Code (RPA 99version 2003). This research work aims to contribute to a better understanding of the performance of such structures in order to come out with some proposals to be integrated in the future version of RPA. In this study, a parametric numerical study was carried out on a series of shear and long links system to investigate their cyclic behaviour. The ABAQUS finite element software was utilized to model the 21 specimens for large-deformation nonlinear analysis. The long and shear links which were expected to behave inelastic manner, were modelled using a C3DR 8-nodes. (ABAQUS) is used with Page B

21 INTRODUCTION geometric and material nonlinearities with large deflection, and large strain capability. This element has six degrees of freedom per node: translations in x, y, z directions, and rotations about x, y, z axes. The objecting of this study was to investigate the rotation demands on short links in eccentrically braced frames under design earthquake loading and develop a loading protocol for experimental link testing that reflects those demands. Organization of Study This study contains five chapters. The introduction chapter involves brief information about the study conducted in this study and the objectives of the study. Details of each chapter are described as follows. A general introduction to EBF structures with some details concerning the links used as segment in different configurations. The objectives of this research are also briefly exposed. Chapter 1 gives a brief overview regarding the seismic steel structures. More details are given for EBF structures with a full description and design philosophy principles along with some historical events. Chapter 2 deals in details different kind of links, their design criteria, forces acting on them along with their failure mechanism according the provisions of Europeans codes 3 and 8, and the American code AISC 2005 are presented. A comparison of the two codes is also given. Details are given on the cyclic loading protocol. Chapter 3 Nonlinear FEA Chapter 4 this chapter gives information about the finite element program ABAQUS, also gives the modelling details of 3D models for two IPE sections (360, and 450) for both short and long links. An additional modelling of two long links made of HEB sections. Chapter 5 Gives the results and their discussion. Finally the conclusion: presents a brief summary of the studies undertaken within the scope of the study and a demonstration of results and concluding remarks and comments on the study. Page C

22 Chapter 1 LATERAL SEISMIC STEEL RESISTING SYSTEMS

23 ABU HALAWEH Ahmad CHAPTER 1 CHAPTER 1: LATERAL SEISMIC STEEL RESISTING SYSTEMS 1. Introduction This chapter presents an overview on the seismic design of steel resisting systems and it emphasizes in particular the seismic design of steel structures. Moment Resisting Frames (MRF) and Concentrically Braced Frames (CBF) and Eccentrically Braced Frames EBF are the most commonly utilized systems in the EC 3, EC8, and ANSI/AISC etc. MRFs have a high level of ductility, making them an excellent option to dissipate energy for high seismic events. However, the high level of ductility comes at a cost: a low level of lateral stiffness. MRFs have a lower level of lateral stiffness than CBFs since they lack braces, and the low lateral stiffness of MRFs can cause story drift at levels exceeding drift limitations. As such, MRFs are designed around drift instead of strength, resulting in reduced economy. Conversely, CBFs have a high level of lateral stiffness and a low level of ductility. For CBFs to be utilized in high seismic regions, special detailing is required to ensure that the frames behave in the prescribed manner. In the 1970s, a new set of frame configurations was proposed for seismic design that would combine the advantages of MRFs and CBFs. The seismic-resisting EBF is the product of decades depicts a modified chevron configuration in which there is one mid-beam link per level; the braces of the above level could be inverted to form a modified two-story X configuration, which would reduce the axial load transferred to the beams. The frame configuration in Figure 3-1b depicts a column-link configuration in which the link is adjacent to one of the frame columns. Figure 3-1c depicts a second modified chevron configuration in which two links are created due to brace-column eccentricity; in this case, one link is considered active and one passive. The passive link can introduce uncertainty in the inelastic behaviour of the frame as the two links do not necessarily equally share the inelastic deformation, as the nomenclature suggests. EBFs successfully combine the high level of ductility of MRFs and the high level of stiffness of CBFs by introducing eccentricity, between a frame cross bracing and column (Popov & Engelhardt, 1988). The cross brace of an EBF provides the elastic stiffness of CBF and the eccentricity of the cross brace creates a link that is responsible for the ductility and, therefore, energy dissipation capacity of MRF. The following sections describe the behaviour of the link of an EBF; all other frame components are intended to remain elastic, and as such as here to conventional elastic behaviours. LATERAL SEISMIC STEEL RESISTING SYSTEMS Page 1

24 ABU HALAWEH Ahmad CHAPTER 1 Figure 1.1 Some Eccentrically Brace Frame Configurations in buildings (EBFs). Table 1.1 Comparison between MRF and braced frames (CBF and EBF) Type Strength Stiffness Ductility MRF good poor excellent CBF good good poor EBF good good good In fact, eccentrically braced frames (EBFs) can be considered as the superposition of two different framing systems: moment-resisting frames (MRF) and concentrically braced frames (CBF). 2. Types of steel structures: The lateral-force-resisting systems for structural steel buildings and structures can generally be categorized into one of three broad classes: 1. Unbraced or moment-resisting frames (MRF). 2. Concentrically braced frames (CBF). 3. Eccentrically braced frames (EBFs) 2.1. Unbraced or Moment-Resisting Frames (MRFs). Moment resisting frames are described as the joining beams and columns in a rectangular shape. In this joining, the beams and columns should be spliced rigidly. The reason of resistance against lateral loads which accounts for the consequent shear forces and bending moments through frame members and joints is the rigidity of the frame behaviour. It is impossible for a moment frame to move horizontally without deforming the beams and columns as a result of the beam-column connections rigidity. The lateral stiffness and strength of the entire structure is generated by the LATERAL SEISMIC STEEL RESISTING SYSTEMS Page 2

25 ABU HALAWEH Ahmad CHAPTER 1 strength of the frames and bending rigidity. No bracing members are present to block the wall openings which provide architectural versatility for space utilization. But, compared to other braced systems moment frames generally required larger member sizes than those required only for strength alone to keep the lateral deflection within code approved drift limits. Again, the inherent flexibility of the system may introduce drift-induced non-structural damage under earthquake excitation than with other stiffer braced systems. Beam, column, and panel zone are the components of the moment frames. In traditional analysis, moment frames were used to be modelled with nodes without dimensions, these nodes were as a matter of fact the intersection of beam to column members. The structural components expected to dissipate hysteretic energy during an earthquake must be detailed to allow the development of large plastic rotations. Plastic rotation demand is typically obtained by inelastic response history analysis. Without considering panel zone plastic deformations it was expected that the largest plastic rotations in the beams are 0.02radian. After the Northridge earthquake the required connection plastic rotation capacity was increased to 0.03radian for new construction and for post-earthquake modification of existing building it was 0.02radian. Figure 1.2 Moment Resisting Frames (MRFs) Concentrically Braced Frames (CBFs). Concentrically braced frames (CBF) is used to control lateral drifts since diagonal braces increase the lateral stiffness of the system, CBFs can resist against lateral forces during minor and moderate earthquakes. Using this kind of structures is generally more economical than increasing element sizes and using doubler plates. However, during a major earthquake, these lateral forces can increase significantly and generally diagonal bracing struts buckle due to the cyclic axial load. The plastic behaviour of bracing struts results in a decrease of buckling strength and energy dissipation capacity after continued load cycles. As a result, an unstable behaviour may be expected in the LATERAL SEISMIC STEEL RESISTING SYSTEMS Page 3

26 ABU HALAWEH Ahmad CHAPTER 1 structure due to the reduction of lateral load carrying capacity. To eliminate this problem, the slenderness ratio of bracings can be increased by using larger sized elements which is also an uneconomical solution. Braces may be made of different shapes and sections such as: I-shaped sections, circular or rectangular tubes, double angle attached together to form a T-shaped section, solid T-shaped sections, single angles, channels and tension only rods and angles. Generally the members of braces are joined to the other members of the framing system by gusset plates which are bolted or welded. Figure 1.3 Typical CBF (Diagonal, Inverted V, V, Chevron and Knee bracing system) Configurations Due to the problems faced in CBFs and MRFs, Popov and his associates at University of California, Berkeley developed an alternative structural system that have large energy dissipation capacity and sufficient stiffness to resist lateral cyclic loads in ductility limits. This system is called Eccentrically Braced Frame (EBF) Eccentrically Braced Frames (EBFs) Definition of EBF: Eccentrically braced frames (EBFs) are a lateral load-resisting system for steel buildings, which are in effect an attempt to combine the individual advantages of moment-resisting frames (MRFs) and concentrically braced frames (CBFs), providing good inelastic capacity for steel structures under large cyclic loading, high elastic stiffness in addition to significant energy dissipation and high degree of ductility at inelastic range. LATERAL SEISMIC STEEL RESISTING SYSTEMS Page 4

27 ABU HALAWEH Ahmad CHAPTER 1 An eccentrically braced frame (EBF) is a type of steel framing system including beams, columns and braces, where these members are arranged in a manner where at least one end of each brace is connected to isolate a segment of the beam called a link. EBFs are typically used as a lateral force resisting system for earthquake loading. Figure 1.4 Eccentrically Braced Frames (EBFs) Historical background of EBFs Development and testing of eccentrically braced frames (EBF) began in the late 1970s, and the early 1980s. When compared to concentrically braced frames and moment resisting frames, EBFs are relatively new. They were adopted into codes in the late 1980s and are now commonly used as the lateral force resisting system for structures in high seismic areas. Egor P. Popov presented the idea of eccentrically braced frames (EBF) in the middle of the 70s to overcome the disadvantages of the conventional methods of lateral force resisting, which are moment resisting (MRFs) and concentrically braced frames (CBF). Moment frame has a proper ductility because of the flexural yielding of beam elements. It has a limited rigidity and also its construction is hard. Conversely converged braced frame has high stiffness but because of diagonal wind-brace buckling its failure is brittle and it has low ductility. Eccentrically braced frames (EBF) have proper stiffness under service loads, which leads to the reduction of deformations in the structure. It also has proper ductility and capability of absorbing energy against immense lateral loads such as strong earthquakes. This guarantees the ductility and the stiffness. Nowadays the use of eccentrically LATERAL SEISMIC STEEL RESISTING SYSTEMS Page 5

28 ABU HALAWEH Ahmad CHAPTER 1 braced frames is widespread especially in the countries which are affected by earthquakes (United States of America, Japan, Iran, Turkey, and Italy) because of high energy absorbing ability at the time of earthquakes, noticeable stiffness and more architectural facilities. Many investigations have been carried out on the behaviour of link beam and its failure mechanism in the two recent decades. The AISC specifications have evolved through numerous versions, an edition concerning Seismic Provisions was published in (2005) as the AISC Seismic Provisions for Structural Steel Buildings (AISC 2005/part I. P 50) which define the design requirements for seismic resistant EBFs in the US. European Code (EC 8) (version 2004) provides details concerning the EBF structures and we will examine the difference in chapter 6, worth mentioning that it was not mentioned in the Algerian seismic regulations (Règles Parasismique Algériennes version 2003, RPA) Eccentrically braced frames types There are many possible framing arrangements for EBFs. The figure 1.5 below shows several possible arrangements for EBFs. Figure 1.5 Configurations of frames with eccentrically braces. LATERAL SEISMIC STEEL RESISTING SYSTEMS Page 6

29 ABU HALAWEH Ahmad CHAPTER EBF Examples in real life: The International Terminal at San Francisco airport An EBF with links at mid-span of the beams Figure 1.6 mid span link A single diagonal EBF is a high-rise steel office building located in Taipei, Taiwan Columns are steel box sections, The link is attached to the steel box column with a fully welded connection. Figure 1.7 diagonal EBF Theoretical background of EBFs EBFs design requirements As described above, the intended behaviour of an EBF subject to earthquake loading is that yielding occurs within the ductile link while the other frame elements remain elastic. To achieve this behaviour, the links must be the weakest elements in the frame and the braces, columns and the beam segment outside the links should therefore be necessarily stronger than the links. It can be said that links are the fuse elements of an EBF. Engelhardt and Popov (1989) constituted a design procedure based on capacity design. According to this method, the dimensions and properties of the link are chosen based on the codes but other elements in the structure are designed for the loads developed in the structure when the link is fully yielded and strain hardened, and where ultimate shear and moment capacity of a frame can be estimated according to Seismic Provisions AISC (2010). Another important issue about eccentrically braced frames is the intersection angle of brace and the beam. Small intersection angles may develop large axial forces outside of the beam. Engelhardt and Popov (1989) indicated that high magnitudes of moment and axial force on the beam cause instability of beam before it reaches its full strength. To avoid this problem, the angle between the beam and brace should not be less than 35. LATERAL SEISMIC STEEL RESISTING SYSTEMS Page 7

30 ABU HALAWEH Ahmad CHAPTER 1 Under the assumption of perfect-plasticity, strain hardening is not observed and shear moment interaction of the link is neglected. According to Engelhardt and Popov (1989), to design a perfectly plastic link, it is important to determine the yield strength of the link. The dimensions of a link are determined so that link does not yield under the shear loads generated by lateral loads specified in codes. Engelhardt and Popov (1989) suggested the equations to determine the shear yield strength Basic behaviour of EBFs EBFs resist lateral load through a combination of frame action and truss action. They can be viewed as a hybrid system between moment resisting frames (MRF) and concentrically braced frames (CBF). EBFs provide high levels of ductility similar to MRFs by concentrating inelastic action in the link, which can be designed and detailed for highly ductile response. Locations where the inelastic action occurs in MRFs, EBFs and CBFs are highlighted in the next Figure1.6at the same time, EBFs can provide high levels of elastic stiffness, similar to that provided by CBFs, and so the code drift requirements can be met economically. Figure 1.8 Inelastic action locations in MRFs, EBFs and CBFs Stiffness and Strength It is instructive to consider the variation of the elastic lateral stiffness of an EBF as a function of the link length e. This variation is illustrated in figure 1.9 for two simple eccentric framing arrangements. For e= L, one has a moment resisting frame and the elastic stiffness is at a minimum. For e/l>0.5, little stiffness is gained from the bracing. However, as the length of the link decreases, a rapid increase in stiffness occurs. Maximum stiffness develops when e=0, corresponding to a concentrically braced frame. It is this situation that EBFs are intended to avoid. When e=0, there is no link present to act as a fuse for brace member forces. Figure 1.9 clearly illustrates that in order to gain maximum possible frame stiffness, the links must be kept short. LATERAL SEISMIC STEEL RESISTING SYSTEMS Page 8

31 ABU HALAWEH Ahmad CHAPTER 1 However, links cannot be made shorter because the inelastic deformation demand on the link becomes excessive. It is also interesting to consider the variation of the fundamental period of vibration of an EBF as a function of link length. Figure 1.10, shows this variation for a five story EBF suggesting the interesting possibility of varying the link length in order to adjust the first period of a building. This concept could be used to move the first period of a building away from a peak in the response spectrum for a particular site. The authors are, however, unaware of any instance of EBFs being used for this purpose. In addition to influencing the elastic stiffness, the link length also significantly affects the strength of an EBF under lateral load. Figure 1.11 shows the ultimate strength of a three-story EBF as a function of el L, assuming elastic-perfectly plastic behavior. Frame capacity is normalized by the quantity 2MP/h which represents the strength of an MRF. Frame strength rapidly increases with decreasing link length, until the frame strength is limited by the fully plastic shear capacity of the links. This region of frame behavior is represented by the horizontal lines in figure Clearly, maximum frame strength is achieved with short links. It must be recognized that the effects of link length shows in, Figure 1.9, 1.10, and 1.11 represent idealized situations for small frames, assuming constant member sizes as e is varied. The actual effects will depend on many factors, including building height and code-imposed drift limitations. However, these figures are representative of the significant trends in behavior as link length is varied. Engelhardt and Popov (1989) Figure 1.9 Variation of elastic lateral stiffness with e/ L for two simple EBFs. LATERAL SEISMIC STEEL RESISTING SYSTEMS Page 9

32 ABU HALAWEH Ahmad CHAPTER 1 Figure 1.10 Variation of first natural period with e/l for a five-story EBFs From Engelhardt and Popov (1989) Figure 1.11 Variation of frame plastic capacity with e/l Inelastic response and energy dissipation Hjelmstad and Popov have said in (1984), another advantage of using EBFs is compliance to architectural requirements while limiting the drifts since the braces can be placed in different variations to allow for architectural openings. The principle that eccentrically braced frames works relies on is the transformation of the moment and shear forces on a segment of the beam through the brace to column or another brace as axial force. This beam segment is referring to as active link or shear link. The link member yields after severe cyclic movement and dissipate large amount of energy (Hjelmstad and Popov (1984)). Comparing the next two Figures the energy dissipation mechanism of EBFs and difference between CBFs and EBFs can be observed more clearly as a result of the differences in the yielding mechanism. LATERAL SEISMIC STEEL RESISTING SYSTEMS Page 10

33 ABU HALAWEH Ahmad CHAPTER 1 Generally, inelastic behaviour of shorter links is dominated by shear yielding of web; however, in longer links, yielding behaviour of the link element is between the shear yielding case in short beams and the flexural yielding case of long beams typically occurring in MRFs. With an optimum design of EBFs, the system can satisfy both ductility and stiffness limits, as well as strength criteria. a b Figure 1.12 a) The Inelastic behaviour of concentrically braced frames in a major earthquake. b) Plastic deformation of eccentrically braces frames. In order to provide sufficient rotational capacity and ductility to shear-link elements, web stiffeners should be used and the dimensions of web and flange of the link are the first parameters that become important in the design. The width to thickness ratio of flanges and webs should satisfy the high ductility requirements. Figure 1.13 Energy dissipation mechanisms Inelastic action during an earthquake is intended to occur within the link of an EBF. Figure 1.14 shows the inelastic mechanism for an EBF. The link can experience very large inelastic rotations. LATERAL SEISMIC STEEL RESISTING SYSTEMS Page 11

34 ABU HALAWEH Ahmad CHAPTER 1 As will be discussed later a well-designed and detailed link should be able to sustain a cyclic inelastic rotation up to ±0.08 rad for a shear link and ±0.02 for flexure link. Figure 1.14 Inelastic mechanisms for EBF under lateral load The excellent ductility of EBFs can be attributed to two factors, First, inelastic activity under severe cyclic loading is restricted primarily to the links, which are designed and detailed to sustain large inelastic deformations without loss of strength. Secondly, braces are designed not to buckle, regardless of the severity of lateral loading on the frame. 3. Overall comparison Table for EBFs according to Eurocodes versus AISC ASCE In the following table Comparison of the capacity design rules according to Euro codes versus AISC ASCE, for the design of EBF, the noticeable features provided by the relevant codes are showed briefly here. Table 3.1 Provisions for eccentrically braced framesa ccording to Eurocodes versus AISC ASCE Description Eurocodes (EC3/EC8) AISC/ASCE Remarks Energy dissipation philosophy EBFs shall be designed so that specific elements or parts of elements called seismic links are able to dissipate energy by the formation of plastic bending and/or EBFs are expected to withstand significant inelastic deformations in the links when subjected to the forces resulting from the motions of the design earthquake. An almost same criterion is considered LATERAL SEISMIC STEEL RESISTING SYSTEMS Page 12

35 ABU HALAWEH Ahmad CHAPTER 1 plastic shear mechanisms Dissipative members Plastic Hinges should take place in links prior to yielding or failure elsewhere. EBFs are expected to withstand significant in-elastic deformations in the links when subjected to forces resulting from the motions of the design earthquake Check to achieve global dissipative behavio ur of the structure Overstrength factor The maximum overstrength Ωi should not differ from the minimum value Ω by more than 25% the minimum value of Ωi = 1,5 Vp, link, i /V Ed, i among all short links, whereas the minimum value of Ωi =1,5 Mp,link,i /M Ed,i among all intermediate and long links; Ω is a multiplicative factor which is the minimum value of Ωi=1.5V p,link,i/v ED, I among all short Ωi=1.5Mp,link,i/ M ED,I among all intermediate and long links Ωo equal to 2 for EBFs is given Ωo in EC8 is (1.1γ ov Ω) Cross section limitations For q > 4 only class 1 sections are allowed, for 2 < q 4 class 1 and class 2 and for 1.5 < q 2 class 1, 2 and 3 are allowed Limits λp to λps, i.e. to use seismically compact section and is obtained by modified slenderness ratio Class 1 and seismically compact sections are unaffected by local buckling Design Checks If N Ed / N pl,r d 0.15 then Check for Design Resistance of Link is V Ed Vp,link Effect of axial force on the link, available shear strength need not be considered if Pu N Ed, M Ed & V Ed respectively are the design axial force, design bending LATERAL SEISMIC STEEL RESISTING SYSTEMS Page 13

36 ABU HALAWEH Ahmad CHAPTER 1 M Ed Mp,link 0.15Py or Pa 0.15/1.5Py moment and design shear at both ends of the link. Seismic load reduction factor A behaviour factor (q) equal to 4 for DCM and5αu/α1 for DCH is provided. A response modification factor (R) equal to 8.0 for EBFs is given An almost same criterion is considered Drift philosophy (Reduction) Spectrum is reduced by 2.0 and 2.5 for importance classes I & II, and III &IV, respectively Reduction factor is (Cd/R) equals (4/8) for EBF Overall EC8 check for drift is more stringent rotation capacity (local ductility concept) Plastic hinge rotation is limited to 35 mrad for structures of DCH and 25 mrad for structures of DCM Link rotation angle shall not exceed (a) 0.08 radians for links of length 1.6Mp/Vp or less and (b) 0.02 radians for links of length 2.6Mp/Vp or greater. For high seismicity it is recommended by both codes to apply ductility concept Links can be short, long and Intermediate. Which fail due to Shear, bending and bending & Shear respectively. V Ed,i, M Ed,i are the design values of the shear force and of the bending moment in Link i in the seismic design situation;vp,link,i, Mp,link,i are the shear and bending plastic design resistances of link i 4. Conclusion In this chapter, some details have been discussed on the lateral seismic resisting systems. Emphasize has been made on the design and the inelastic behaviour of EBFs steel structures, their geometry characteristics, energy dissipation, strength, plastic deformation etc. LATERAL SEISMIC STEEL RESISTING SYSTEMS Page 14

37 Chapter 2 LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC 2005

38 ABU HALAWEH Ahmad CHAPTER 2 CHAPTER 2: LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC Introduction In this chapter, the design criteria, forces acting on a link, the failure mechanism of the link in EBF structures are being discussed according to the provisions of Eurocodes 3 and 8, and the American code AISC Generally speaking, the link which is the part of the beams between the braces are designed to yield during moderate and severe earthquakes. The links can generally be categorized into one of three broad classes: short, long, and intermediate links. Links have very well in high shear, which is constant along the link lengths it also has a very large bending moments, links are subject to reverse curvature bending, with high end moments of opposite sign, and links have seen very low axial forces. The link length (e) is a key parameter that controls inelastic behaviour. Inelastic response of short links is dominated by shear; while the longer links are rather dominated by flexure. Shear yielding of a link will occur when the shear force reaches the fully plastic shear capacity Vp of the link section, flexural yielding will occur at the link ends when the end moment reaches Mp of the link section. The plastic rotation angle γ p is the primary kinematic variable used to characterize inelastic deformation demands on a link. γ p is defined as the inelastic angle between the link and adjoining beam, in a rigid-plastic Experimental previous works have shown that EBF structures exhibit good strength and stiffness in elastic range, so avoiding non-structural element damage, and are also able to provide enough ductility to dissipate large amounts of energy in the inelastic range. It is designed as shear links according to [EN : ]. The active link must be designed in order to obtain that its bending and shear limit strength precedes the attainment of the tension and compression limit strength of other elements. The length of the active link is responsible of the collapse mechanism which dissipates energy. A careful design of seismic links can lead to good hysteresis loops with large stiffness and energy absorption. However, the rest of the structure is designed to remain elastic during the earthquake. Comparing the CBF and EBF behaviour, it can be seen that the inelastic deformations primarily comes from yielding of the tension braces and inelastic buckling of the compression braces. Both inelastic mechanisms are shown in figure 2.1. LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC 2005 Page 15

39 ABU HALAWEH Ahmad CHAPTER 2 a b Figure 2.1 Inelastic mechanisms for the two bracing systems. 2. Links types The length of the active link is responsible of the collapse mechanism which dissipates energy. Short links dissipate energy mainly by inelastic shear deformation in the web and so are called shear links; long links dissipate energy mainly by inelastic normal strain in the flanges and so are called moment links. The links can generallybe categorized into three main categories: 1. Short links dissipate energy mainly by inelastic shear deformation in the web and so are called shear links. 2. Long links: dissipate energy mainly by inelastic normal strain in the flanges and so are called moment links. A careful design of seismic links can lead good hysteresis loops with large stiffness and energy absorption. a b Figure 2.2 (a) Short Link and (b) Long link (b) 3. Distribution of forces in links and beams in different EBF configuration Figure 2.3 below shows qualitatively the distribution of moment, shear and axial force in the link and beam segments outside of the link in an EBF subjected to lateral load, namely earthquake or wind forces. Two common EBF configurations are shown; one with the link at mid-span and the other LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC 2005 Page 16

40 ABU HALAWEH Ahmad CHAPTER 2 with the link connected to the column. The link is generally subject to high shear along its full length, high end moments and low axial force. Yielding within the link can be shear yielding, flexural yielding or a combination of shear and flexural yielding. Forces in the beam segment outside of the link are the more interesting features in Figure below. The beam segment has a high bending moment immediately adjacent to the link. This is because the high moment at the end of the link must be resisted primarily by the beam segment. The figure shows a drop in moment between the end of the link and the adjoining beam segment. This represents the portion of the link end moment transferred to the brace, assuming that moment is transferred between the brace and the link. The beam segment outside of the link is also subjected to high axial force. The brace in an EBF also sees high axial force, and the horizontal component of the brace axial force will generate high axial force in the beam segment. Finally, the shear in the beam segment outside of the link is generally small. Consequently, the force environment for the beam segment outside of the link is dominated by high axial force and high moment. Since earthquake loads are cyclic, the beam segment outside of the link experiences both axial tension and axial compression. Figure 2.3 Distribution of forces in the link and the beam outside the link for different configurations 4. Factor affecting the inelastic behaviour of a link The link length (e) is the major factor on the inelastic performance of a link. As previously mentioned, the link of an EBF can experience three types of forces: shear, axial, and flexural. Axial forces have been shown to be negligible for the case where link required axial strength, is marginal compared to nominal axial yield strength, Depending on the length of the link, either shear or flexural forces will dominate failure behaviour. The standard terminology for links where behaviour is LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC 2005 Page 17

41 ABU HALAWEH Ahmad CHAPTER 2 dominated by shear and flexure is shear links and flexure links, respectively. In addition, and due to inelastic behaviour, a third classification arises that is dominated by a combination of shear and flexural yielding; links of such length are called intermediate links. Figure 2.4 The links free body diagram 5. Comparison of yielding failure of shear and flexural (long) links The figure 2.5shows a free body diagram of a link subjected to a constant shear and equal and opposite end moments. The shorter link length shows better inelastic behaviour as a result the influence of shear forces. Shear yielding has a tendency to occur uniformly alongside of the link. Shear yielding has a high ductility and also significant inelastic performance capacity which is more than that predicted by the structure shear area, if the web is braced enough against buckling. However, longer link lengths allow for greater architectural and functional freedom. Nevertheless, the usage of large values decreased the level of certainty at which engineers could ensure that failure would occur in the prescribed ductile manner. As a result, research into the behaviour and effectiveness of longer links began to appear. At present, long-link behaviour is better understood, allowing for greater architectural and functional freedom with a high level of certainty. Often the behaviour of the links are like short beams which are exposed to equal shear loads applied in opposite directions at the ends of the link. LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC 2005 Page 18

42 ABU HALAWEH Ahmad CHAPTER 2 a b 6. Link plastic rotation angle Figure 2.5 a) Shear yielding. b) Flexural yielding of link. The available ductility of a link is often described by its plastic rotation capacity. The plastic rotation of a link can be denoted as γ p. A goal of EBF design is that the link plastic rotation capacity exceeds the plastic rotation demand of an earthquake. In EBF design, the link plastic rotation can be related for multi-stories structures to the plastic story drift angle, θp, by the geometry of a rigid plastic mechanism. Figures 2.6 through 1.8 show the rigid plastic mechanism for three common EBF geometries with the total beam span denoted as L and the link length denoted as e. Equation 2.1 presents the relationship between link plastic rotation angle and the plastic story drift angle for mechanisms in Figures 1.6 and 1.7while Equation 2.2 presents relationship between link plastic rotation angle and the plastic story drift angle for the mechanism in Figure 1.8. Note that as theratio of span length to link length (L/e) increases, the link rotation angle also increases for a given plastic story drift angle. Consequently, large values of L/e can result in excessive plastic rotation demands on the link. The configuration had shown in Figure 1.6, with two links in each level, places only one-half the plastic rotation demands on the link as compared to the other configurations. γ p =(L/e) x θp (2.1) γ p =(L/2e) x θp (2.2) Where LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC 2005 Page 19

43 ABU HALAWEH Ahmad CHAPTER 2 L = bay width θp = plastic story drift angle, radians (= Δp / h) γ p = link rotation angle e = link length Figure 2.6 Link plastic rotation of EBF with a link at the middle of the beam Figure 2.7 Link plastic rotation of D-type EBF with one link next to the column Figure 2.8 Link plastic rotation of EBF with two links next to the columns LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC 2005 Page 20

44 ABU HALAWEH Ahmad CHAPTER 2 7. Link of the EBF buildings The following figure describes the link segments of the EBF buildings. Figure 2.8 represents, for an EBF building, the connection between the bracing members and the corresponding beam. Figure 2.9 Typical link Link stiffeners and lateral bracing of the link Link stiffeners are needed to prevent web shear buckling of the link. Kasai and Popov proposed a rule for stiffener spacing for shear yielding links based on analytical and experimental results. They used the experimental results of 30 shear yielding links tested upto that date and combined the results with the plastic plate buckling theory to develop stiffener spacing criteria for shear yielding links. Popov and Engelhardt (1989) also observed that the dominant force causing instability on EBFs with long links is not shear but flexure resulting in lateral torsional buckling of the beam and local flange buckling. The results of this investigation revealed that the stiffeners located only at ends of the link are adequate for flexural yielding links. 8. Design criteria of links Whereas short links suffer from high ductility demands, they yield primarily in shear. Experimental evidence (e.g. Hjelmstad and Popov; Kasai and Popov; Engelhardt and Popov) showed that shear link behaviour in steel is superior to that of flexural plastic hinges. However, other considerations such as architectural requirements may necessitate the use of long links. Previous analytical and experimental research has demonstrated that properly designed eccentrically braced frame (EBF) systems can provide the ductility and energy dissipation capacity needed to serve as an effective lateral load resisting system to resist earthquake demands (Hjelmstad and Popov). LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC 2005 Page 21

45 ABU HALAWEH Ahmad CHAPTER Design Criteria to EC8 Introduction According to EC8, all steel buildings shall be assigned to one of the following structural types according to the behaviour of their primary resisting structure under seismic actions. Hence, the moment resisting frames (MRF), in which the horizontal forces are mainly resisted by members acting in an essentially flexural manner. In the other hand, frames with concentrically bracings, in which the horizontal forces are mainly resisted by members subjected to axial forces. Another type of structures, namely frames with eccentrically bracings (EBF), in which the horizontal forces are mainly resisted by axially loaded members, but where the eccentricity of the layout is such that energy can be dissipated in seismic links by means of either cyclic bending or cyclic shear. Inverted pendulum structures in which dissipative zones are located in the columns. Also, structures with concrete with cores or concrete walls, in which horizontal forces are mainly resisted by these cores or walls, are covered. Moment resisting frames combined with concentrically bracings. Moment resisting frames combined with in fills. In moment resisting frames, the dissipative zones should be mainly located in plastic hinges in the beams or the beam-column joints so that energy is dissipated by means of cyclic bending. In frames with concentric bracings, the dissipative zones should be mainly located in the tensile diagonals. The bracings may belong to one of the following categories: Active tension diagonal bracings, in which the horizontal forces can be resisted by the tension diagonals only, neglecting the compression diagonals; V bracings, in which the horizontal forces can be resisted by considering both tension and compression diagonals. The intersection point of these diagonals lies on a horizontal member which must be continuous. K bracings, in which the diagonals intersection lies on a column, may not be used. For frames with eccentric bracings configurations should be used that ensure that all links will be active. Design and detailing rules for links according to Eurocode 8 (version 2004) provides details concerning the link in chapter 8are listed below. LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC 2005 Page 22

46 ABU HALAWEH Ahmad CHAPTER 2 Frames with eccentrically bracings shall be designed so that specific elements or parts of elements called seismic links are able to dissipate energy by the formation of plastic bending and/or plastic shear mechanisms. The structural system shall be designed so that a homogeneous dissipative behaviour of the whole set of seismic links is realized. The rules given hereafter are intended to ensure that yielding, including strain hardening effects in the plastic hinges or shear panels, will take place in the links prior to any yielding or failure elsewhere. Seismic links may be horizontal or vertical components. Seismic Links Provisions The web of a link should be of single thickness without double plate reinforcement and without a hole or penetration. - Seismic links are classified into 3 categories according to the type of plastic mechanism developed: - Short links, which dissipate energy by yielding essentially in shear; - Long links, which dissipate energy by yielding essentially in bending; - Intermediate links, in which the plastic mechanism involves bending and shear. For I sections, the following parameters are used to define the design resistance sand limits of categories: M p, link = f y b t f (d-t f ) (2.3) V p,link = (fy/ 3) t w (d t f ) (2.4) Where the geometrical parameters are those showed in Figure 2.10 If N Ed /N pl,rd 0.15, the design resistance of the link should satisfy both of the following relationships at both ends of the link: V ED VP, link (2.5) M ED Mp, link (2.6) Where: LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC 2005 Page 23

47 ABU HALAWEH Ahmad CHAPTER 2 Figure 2.10 Definition of symbols for I link sections N Ed, M Ed, V Ed design action effects, respectively design axial force, design bending moment and design shear, at both ends of the link. If N Ed /N Rd 0.15, the link length e should not exceed: e 1,6 Mp,link/Vp,link (2.7) When R = (N Ed.t w.(d 2t f ) / V Ed.A )< 0,3, in which A is the gross area of the link Or e (1,15 0,5 R) 1,6 Mp, link /Vp, link (2.8) When R 0.3. To achieve a global dissipative behaviour of the structure, it should be checked that the individual values of the ratios i Ω =1,5 Vpl,R d,i/ VEd,1 for short link and i Ω =1,5 Mpl,R d,i /M Ed, 1 for long links, do not exceed the minimum value Ω by more than 25%. In design where equal moments would form simultaneously at both ends of the link, links may be classified according to the length e. For I sections, the categories are: Short links e <es = 1.6 Mp, link /Vp, link (2.9) Long links e >e L = 3.0 Mp, link /Vp, link (2.10) Intermediate links es < e < e L (2.11) In design where only one plastic hinge would form at one end of the link, the length e defining the categories of the links is, for I sections: LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC 2005 Page 24

48 ABU HALAWEH Ahmad CHAPTER 2 Short links e < e s = 0.8 (1+α) Mp,link/V p,link (2.12) Long links e > e L = 1.5 (1+α) Mp, link /V p,link (2.13) Intermediate links e s < e < e L. (2.14) Where: α is the ratio of the smaller bending moments M Ed,A at one end of the link in the seismic design situation, to the greater bending moments M Ed,B at the end where the plastic hinge would form, both moments being considered in absolute value. Figure 2.11 a) Equal moments at link ends; b) unequal moments at link ends. The link rotation angle θp between the link and the element outside of the link should be consistent with global deformations. It should not exceed the following values: Short links θp θp R = 0.08 radians (2.15) Long links θp θp R = 0.02 radians (2.16) Intermediate links θp θp R = the value determined by linear interpolation between the above values According to AISC 2005 The AISC Specification for Structural Steel Buildings (ANSI/AISC ) is intended to cover common design criteria. This document, the AISC Seismic Provisions for Structural Steel Buildings (ANSI/AISC ) with Supplement No. 1 (ANSI/AISC 341s1-05) (hereafter referred to as the Provisions) is a separate consensus standard that addresses one such topic: the design and construction of structural steel and composite structural steel/reinforced concrete building systems for high seismic applications. Supplement No. 1 consists of modifications made to Part I, Section 14 of the Provisions after the initial approval had been completed. These Provisions are presented in two parts: Part I is intended for the design and construction of structural steel buildings, and is written in a unified format that addresses both LRFD and ASD; Part II is intended for the design and construction of composite LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC 2005 Page 25

49 ABU HALAWEH Ahmad CHAPTER 2 structural steel/ reinforced concrete buildings, and is written to address LRFD only. In addition, seven mandatory appendices, a list of Symbols, and Glossary are part of this document EBF Structures to AISC Eccentrically braced frames (EBFs) are expected to withstand significant inelastic deformations in the links when subjected to the forces resulting from the motions of the design earthquake. The diagonal braces, columns, and beam segments outside of the links shall be designed to remain essentially elastic under the maximum forces that can be generated by the fully yielded and strain hardened links, except where permitted in this Section. The web of a link shall be single thickness. Doubler-plate reinforcement and web penetrations are not permitted. Shear Strength Except as limited below, the link design shear strength, φ v Vn, and the allowable shear strength, Vn/Ωv, according to the limit state of shear yielding shall be determined as follows: Where Vn = nominal shear strength of the link, equal to the lesser of Vp or 2Mp /e, kips (2.17) Φv = 0.90 (LRFD) Ωv = 1.67 (2.18) Mp = FyZ, kip-in. (N-mm) (2.19) Vp = 0.6 FyAw, kips (N) (2.20) e = link length, in. (mm) (2.21) Aw = (d2t f )t w (2.22) The effect of axial force on the link available shear strength need not be considered If Pu 0.15Py (2.23) Or Pa (0.15/1.5) Py. (2.24) Where P u = required axial strength using LRFD load combinations, kips (N) (2.25) LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC 2005 Page 26

50 ABU HALAWEH Ahmad CHAPTER 2 P a = required axial strength using ASD load combinations, kips (N) (2.26) P y = nominal axial yield strength = FyAg, kips (N) (2.27) If Pu > 0.15Py (2.28) Or Pa > (0.15/1.5)Py, as appropriate, the following additional requirements shall be met: The available shear strength of the link shall be the lesser of ΦvVpa and 2φ v Mpa /e (2.29) Or Vpa / Ωv and 2 (Mpa /e)/ωv, as appropriate (2.30) Where ( ) (2.31) ( ) (2.32) ( ) (2.33) [ ( )] (2.34) ( ) ( ) (2.35) ( ) ( ) (2.36) The length of the link shall not exceed: a) [ ρ (Aw /Ag)]1.6Mp /Vp when ρ (Aw /Ag) 0.3 (2.37) or b) 1.6 Mp /Vp when ρ (Aw /Ag) < 0.3(2.38). Where Aw = (d 2t f ) t w (2.39) ρ = Pr /Vr (2.40) And where Vr = Vu (LRFD) or Va (ASD), as appropriate (2.41) LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC 2005 Page 27

51 ABU HALAWEH Ahmad CHAPTER 2 Vu = required shear strength based on LRFD load combinations, kips (2.42) Va = required shear strength based on ASD load combinations, kips (2.43) The link rotation angle is the inelastic angle between the link and the beam outside of the link when the total story drift is equal to the design story drift, Δ. The link rotation angle shall not exceed the following values: (a) 0.08 radians for links of length 1.6Mp /Vp or less. (2.44) (b) 0.02 radians for links of length 2.6Mp /Vp or greater. (2.45) (c) The value determined by linear interpolation between the above values for links of length between 1.6Mp /Vp and 2.6Mp /Vp. (2.46) Link Stiffeners Provisions Full-depth web stiffeners shall be provided on both sides of the link web at the diagonal brace ends of the link. These stiffeners shall have a combined width not less than (bf _ 2t w ) and a thickness not less than 0.75tw or a in. (10 mm), whichever is larger, where bf and t w are the link flange width and link web thickness, respectively links shall be provided with intermediate web stiffeners as follows: (a) Links of lengths 1.6Mp /Vp or less shall be provided with intermediate web stiffeners spaced at intervals not exceeding (30t w d/5) for a link rotation angle of 0.08 radian or (52t w d/5) for link rotation angles of 0.02 radian or less. Linear interpolation shall be used for values between 0.08 and 0.02radian. (b) Links of length greater than 2.6Mp /Vp and less than 5Mp /Vp shall be provided with intermediate web stiffeners placed at a distance of 1.5 times b f from each end of the link. (c) Links of length between 1.6Mp /Vp and 2.6Mp /Vp shall be provided with intermediate web stiffeners meeting the requirements of (a) and (b) above. (d) Intermediate web stiffeners are not required in links of lengths greater than5mp /Vp. (e) Intermediate web stiffeners shall be full depth. For links that are less than25 in. (635 mm) in depth, stiffeners are required on only one side of the link web. The thickness of one-sided stiffeners shall not be less than t w or a in,(10 mm), whichever is larger, and the width shall be not less than (b f /2) - t w LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC 2005 Page 28

52 ABU HALAWEH Ahmad CHAPTER 2 For links that are 25 in. (635 mm) in depth or greater, similar intermediate stiffeners are required on both sides of the web. The required strength of fillet welds connecting a link stiffener to the link web is AstFy or AstFy/ 1.5 (ASD), as appropriate, where ast is the area of the stiffener. The required strength of fillet welds connecting the stiffener to the link flanges is AstFy/4 (LRFD) or AstFy/) Comparison between the codes 1. Length ratio: in the American code the length ratio is an opened interval unlike the Euro code which provides a precise value. 2. Rotational angle: the rotational angle is the same in codes, 0.02 in the long and 0.08 in the short links, and the code UBC mentioned the angle for the long to have the same as 0.02 but gives the short link a 0.09 rad value. 3. Stiffeners: stiffeners are given the same classification in the two codes. 4. The American code has a protocol for the seismic charge. 5. The link length in the American code is slightly longer than the Euro one, for example the short IPE 360 has a length of 740mm in the Eurocode and an 848mm in the American. In this study, the provisions of EC8 have been used to design the links, while the protocol of cyclic loading used is AISC Monotonic cyclic loadings 9.1. Introduction All structural elements have limited strength and deformation capacities; and collapse safeties as well as damage control are depending on our ability to assess these capacities with some confidence. The structural properties of a structure deteriorate when deformations reach the range of inelastic behaviour. A possible consequence of deterioration of the hysteretic behaviour of a structure is failure of critical elements at deformation levels that are significantly smaller than its ultimate deformation capacity. The aim of the study is to determine the response of short and long links under earthquake loads. Thus, and in order to take into account the deterioration in strength due to plastic local buckling, cyclic analysis was performed using the loading protocol given in Appendix S of the 2005 AISC Seismic Provisions. Monotonic analysis under-predicts buckling amplitudes and strength degradation. Link rotation was defined as the imposed transverse displacement divided by the link LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC 2005 Page 29

53 ABU HALAWEH Ahmad CHAPTER 2 length. We have a maximum rotation of 0.02 rad for the long links and 0.08 rad for the short links. Cyclic displacements were applied to the specimens in the plane of the web of the specimens to simulate earthquake loading. The loading was applied until failure of the specimen initiated. In finite element simulation conducted in this thesis, the displacement is defined in only the y-direction which is normal to the plane of the flanges and displacements in other directions are restraint to illustrate the experimental setup Concepts behind development of loading protocols Present codes, standards, and guidelines make reference to the need for performance assessment through testing in various sections. The actual history for an earthquake, will depend on the intensity and frequency content (magnitude, distance, and soil type dependence) of the ground motion the specific component (or assembly) will be subjected to as part of the structural system. The overriding issue is to account for cumulative damage effects through cyclic loading. If there is no cumulative damage, there is no need for cyclic loading. The number and amplitudes of cycles the component will experience depend on the configuration, strength, stiffness, and modal properties (periods and participation factors) of the structure and on the deterioration characteristics of the structural system components. These cycles applied to the specimen may be derived from analytical studies in which models of representative structural systems are subjected to representative earthquake ground motions and the response is evaluated statistically. Unfortunately, in earthquake engineering, strength and deformation capacities depend (sometimes weakly and sometimes strongly) on cumulative damage, which implies that every component has a permanent memory of past damaging events and at any instance in time it will remember all the past excursions (or cycles) that have contributed to the deterioration in its state of health. Thus, performance depends on the history of previously applied damaging cycles, and the only reasonable way to assess the consequences of history (short of developing complex analytical models that can be used for damage state predictions) is to replicate, to the best we can, the load and deformation histories a component will undergo in an earthquake (or several earthquakes if this is appropriate). The objective of a loading protocol is to achieve this in a conservative, yet not too conservative, manner. Any loading protocol will always be a compromise that will provide deformation histories whose realism will depend on many parameters. LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC 2005 Page 30

54 ABU HALAWEH Ahmad CHAPTER General requirements The objective of a cyclic seismic loading protocol is to simulate the number of inelastic cycles, cumulative inelastic demand, and peak displacement demand associated with a design seismic event. Many loading protocols have been proposed in the literature, and several have been used in multiinstitutional testing programs (Krawinkler et al.), or are contained in standards or are proposed for standards (e.g., FEMA 2007, AISC 2005 (modified in 2006), ASTM 2003, ICBO-ES 2002) Examples of loading protocols used presently or in the recent past Many loading protocols have been used in testing programs or are contained in standards or are proposed for standards (e.g., FEMA 2007, AISC 2005). These protocols recommend somewhat different loading histories, but in most cases they differ more in detail than in concept. One reason may be that for this material analytical methods for performance prediction are rather unreliable, but probably the main reason is that it is cost-effective to test wood panels and connector in great numbers, whereas it is extremely expensive to perform many tests on components of steel or reinforced concrete structures. Thus, for economic reasons, seismic performance acceptance of wood components is based mostly on tests rather than analytical models. It is interesting to note that there appears to be no widely used loading protocol for components of reinforced concrete structures. Steel - ATC-24 Protocol (ATC-24, 1992), Figure 1(a).This protocol, which was specifically developed for components of steel structures, was one of the first formal protocols developed in the U.S. for seismic performance evaluation of components using a cyclic loading history. It uses the yield deformation, γyield, as the reference for increasing the amplitude of cycles. The history contains at least 6 elastic cycles (amplitude <γyield), followed by three cycles each of amplitude (amplitude γyield). There is one more clear difference between the CUREE protocol and the ATC-24 and SAC protocols, which is the presence of trailing cycles. These are the smaller cycles following the preceding larger (primary) cycle at each step. These trailing cycles do less (and often much less) damage than cycles of amplitude equal to the larger one. Time history analysis has shown that the pattern of larger cycles being followed by smaller cycles is indeed justifiable by statistical means. A simplified version of the CUREE protocol makes the amplitude of the trailing cycles equal to that of the preceding primary cycle for simplicity only. LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC 2005 Page 31

55 ABU HALAWEH Ahmad CHAPTER 2 FEMA 461 (FEMA 2007), Figure 1(d).This protocol was developed originally for testing of drift sensitive non-structural components, but is applicable in general also to drift sensitive structural components. It uses a targeted maximum deformation amplitude, γ m, and a targeted smallest deformation amplitude, γ0, as reference values, and a predetermined number of increments, n, to determine the loading history (a value of n 10 is recommended). Two cycles are to be executed for each amplitude. (a) Steel - ATC-24 (ATC-24, 1992) (b) Steel SAC (Clark et al., 1997) (c) Wood ISO (ISO, 1998) (d) FEMA 461 (FEMA, 2007) LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC 2005 Page 32

56 ABU HALAWEH Ahmad CHAPTER 2 Figure 2.12 PROTOCOLS OF 2005 AISC SEISMIC PROVISIONS Moment connections Qualifying cyclic tests of beam-to-column moment connections in special and intermediate moment frames shall be conducted by controlling the inter-story drift angle, θ, imposed on the test specimen, as specified below: (1) 6 cycles at θ = rad (2) 6 cycles at θ = rad (3) 6 cycles at θ = rad (4) 4 cycles at θ = 0.01 rad (5) 2 cycles at θ = rad (6) 2 cycles at θ = 0.02 rad (7) 2 cycles at θ = 0.03 rad (8) 2 cycles at θ = 0.04 rad Continue loading at increments of θ = 0.01 radian, with two cycles of loading at each step Loading sequence for link-to-column connections Qualifying cyclic tests of link-to-column moment connections in eccentrically braced frames LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC 2005 Page 33

57 ABU HALAWEH Ahmad CHAPTER 2 Shall be conducted by controlling the total link rotation angle, γ total, imposed on the test specimen, as follows: (1) 6 cycles at γ total = rad (2) 6 cycles at γ total = rad (3) 6 cycles at γ total = rad (4) 6 cycles at γ total = 0.01 rad (5) 4 cycles at γ total = rad (6) 4 cycles at γ total = 0.02 rad (7) 2 cycles at γtotal = 0.03 rad (8) 1 cycle at γ total = 0.04 rad (9) 1 cycle at γ total = 0.05 rad (10) 1 cycle at γ total = 0.07 rad (11) 1 cycle at γ total = 0.09 rad Continue loading at increments of γ total = 0.02 radian, with one cycle of loading at each step. This procedure is characterized by the control of inter-storey drift angle, imposed on the test specimen, as specified below (θ = chord rotation): 1) 6 cycles with θ = rad 2) 6 cycles with θ = rad 3) 6 cycles with θ = rad 4) 4 cycles with θ = 0.01 rad 5) 2 cycles with θ = rad 6) 2 cycles with θ = 0.02 rad 7) 2 cycles with θ = 0.03 rad 8) 2 cycles with θ = 0.04 rad 9) 1 cycle with θ = 0.05 rad 10) 1 cycle with θ = 0.07 rad LINKS IN EBF STRUCTURES ACCORDING TO EC8 and AISC 2005 Page 34

58 Chapter 3 NONLINEAR FINITE ELEMENT ANALYSES

59 ABU HALAWEH Ahmad CHAPTER 3 CHAPTER 3: NONLINEAR FINITE ELEMENT ANALYSES 1. General introduction to finite element method (FEM). In this chapter, an overview of finite element method (FEM) and finite element analysis (FEA) is presented. Nowadays, the finite element method has become a great tool used by engineers worldwide in most fields of engineering. The FEA has many advantages. It can be used for solving many types of problems. There are no geometric, boundary conditions, loading and material properties restrictions. The Finite element analysis (FEA) is a numerical method for solving complicated structural systems that may be impossible to be solved in the closed form. The finite element analysis may be viewed as a general structural analysis procedure that allows the computation of stresses and deflections in 2D and 3D. The name, finite element analysis, arises because there exists only a finite number of elements in any given model to represent an actual continuum with an infinite number of degrees of freedom. The Finite Element Method (FEM) and its practical applications, often known as Finite Element Analysis (FEA) is a numerical technique for finding approximate solutions of partial differential equations as well as integral equations. The FE method was developed more by engineers using physical insight than by mathematicians using abstract methods. FEM has been applied to a number of physical problems, where the governing differential equations are available. The method consists essentially of assuming the piecewise continuous function for the solution and obtaining the parameters of the functions in a manner that reduces the error in the solution. In solving partial differential equations, the primary challenge is to create an equation that approximates the equation to be studied, but is numerically stable, meaning that errors in the input and intermediate calculations do not accumulate and cause the resulting output to be meaningless. There are many ways of doing this, all with advantages and disadvantages. The finite element method is a good choice for solving partial differential equations over complicated. The finite element method (FEM), sometimes referred to as finite element analysis (FEA), is a computational technique used to obtain approximate solutions of boundary value problems in engineering. Simply stated, a boundary value problem is a mathematical problem in which one or more dependent variables must satisfy a differential equation everywhere within a known domain of independent variables and satisfy specific conditions on the boundary of the domain. Boundary value problems are also sometimes called field problems. The field is the domain of interest and most often represents a physical structure. NONLINEAR FINITE ELEMENT ANALYSES Page 35

60 ABU HALAWEH Ahmad CHAPTER 3 The field variables in FEM are the dependent variables of interest governed by the differential equation. The boundary conditions are the specified values of the field variables (or related variables such as derivatives) on the boundaries of the field. It was first applied to problems of stress analysis and has since been applied to other problems of fields. In all applications the analyst seeks to calculate a field quantity: in stress analysis it is the displacement field or the stress field; in thermal analysis it is the temperature field or the heat flux; in fluid flow it is the stream function or the velocity potential function; and so on. Results of greatest interest are usually peak values of either the field quantity or its gradients. The FE method is a way of getting a numerical solution to a specific problem. A FE analysis does not produce a formula as a solution, nor does it solve a class of problems. 2. Overview and summary of FEA The advantage of using the finite element analysis is that the errors between the individual structural components and the stresses in the individual structural components can be easily determined. However, the finite element analysis is also having some downsides.it is imperative that the FEA be recognized as simulation, not as reality. Moreover, the obtained output results from the FEA are only approximations. Namely, there is a difference between the finite element solution and the exact solution. The type of the model should be as complex as needed to obtain the required accuracy of the structure, but also as simple as possible to minimize the computational time. For nonlinear FEA analysis details, see section 3.7 The main ideas of the finite element method are in summary, the finite element method has the following three basic features: 1. Divide the whole (i.e. domain) into parts, called finite elements. 2. Over each representative element, develop the relations among the secondary and primary variables (e.g. forces and displacements, heats and temperatures, and so on). 3. Assemble the elements (i.e. combine the relations of all elements) to obtain the relations between the secondary and primary variables of the whole system. An unsophisticated description of the FE method is that it involves cutting a structure into several elements (pieces of the structure), describing the behaviour of each element in a simple way, then reconnecting elements at "nodes" as if nodes were pins or drops of glue that hold elements together Fig This process results in a set of simultaneous algebraic equations. In stress analysis these equations are equilibrium equations of the nodes. There may be several hundred or several thousand such equations, which mean that computer implementation is mandatory. A more sophisticated description of the FE method regards it as piecewise polynomial NONLINEAR FINITE ELEMENT ANALYSES Page 36

61 ABU HALAWEH Ahmad CHAPTER 3 Fig.3.1 Coarse-mesh. Two-dimensional model of a gear tooth. All nodes and elements lie in the plane of the paper The power of the FE method is its adaptability. Surely, the analyzed structure may have an arbitrary shape, arbitrary supports, and arbitrary loads. Such generality does not exist in classical analytical methods. For example, temperature-induced stresses are usually difficult to analyze with classical methods, even when the structure geometry and the temperature field are both simple. The FE method treats thermal stresses as easily as stresses induced by mechanical load, and the temperature distribution itself can be calculated by FE. Using commercial packages dealing with the application of the theory of FE includes matrix manipulations, numerical integration, equation solving, and other procedures carried out automatically by these commercial software s. The user may see only indication of these procedures as the software processes data. The user deals mainly with pre-processing (describing loads, supports, materials, and generating the FE mesh) and post processing (sorting output listing, and plotting of results). In a large software package, such as ABAQUS, LUSAS and ANSYS, the analysis portion is accompanied by the pre-processor and postprocessor portions of the software. There also exist standalone pre- and postprocessors that can communicate with other large programs. Specific procedures of "pre" and "post" are different in different programs. Learning how to perform any type of analysis is often a matter of training, assisted by introductory notes, manuals, and online documentation that accompanies the software. Also, sellers of large-scale programs offer training courses. Fluency with pre- and postprocessors is helpful to the user but is unrelated to the accuracy of FE results produced. First, the quality of the results obtained from FEA depends up on the density of the mesh, element type and the input properties of the element and these modelling aspects usually increases as the structural system become complex. For example, the increase in the number and the variety of structural components and its connections, especially, when the geometric non linearity s and the material non linearity s cannot be neglected. The results become more accurate when the modelling NONLINEAR FINITE ELEMENT ANALYSES Page 37

62 ABU HALAWEH Ahmad CHAPTER 3 shifts from one dimension to three. Also it is very important to validate the modelling and analysis strategies with the classical theories or with experimental testing. The second drawback of the finite element analysis is that the analysis necessitates very powerful software and an individual with strong basics of the finite element theory and the analysis techniques. It can notice that there are many commercial packages available: ABAQUS; ANSYs; LUSAS etc. 3. Historical development of FEM The name "finite element" was first used in The mathematician Courant, described a piecewise polynomial solution for the torsion problem in a publication in His work was not noticed by engineers and the procedure was impractical at that time due to the lack of digital computers. In the 1950s, the problems imposed on the aircraft industry led to introducing the FE method to work on solving their issuesby practicing engineers. A classic study described FE work that was driven by a need to analyse wings, which are too short for beam theory to be reliable. By 1963, the mathematical reliability of the FE method was worldwide known and the method was extended quickly from its structural beginnings to include heat transfer, ground water flow, magnetic fields, and many other areas that concern every engineer in all branches of engineering. Large generalpurpose FE software began to spread in the 1970s. By the late 1980s the software was available on microcomputers, complete with colour graphics and pre- and postprocessors. By the mid-1990s roughly 40,000 papers and books about the FE method and its applications had been published. 4. How does the finite element method work? In this section, the general techniques and terminology of finite element analysis will be presented with reference to Figure 3.2. The figure describes a number of some material or materials that we already know its physical properties. The bulk represents the domain of a boundary value problem to be solved. For further more simple explanation, we assume a two-dimensional case with a single field variable (x, y) to be determined at every point P(x,y) such that a known governing equation (or equations) is satisfied exactly at every such point. It can be noticed that this implies that an exact mathematical solution is achieved by the FEM; that is, the solution is a closed-form algebraic expression of the independent variables. In the practical problems solved by FEM, the domain may be very complex in its geometrical, their governing equations and the probability of obtaining an exact closed-form solution is very low. Therefore, approximate solutions are frequently obtained in engineering analyses for these complex problems. FEA is a very powerful and useful method to obtain an approximate solution with NONLINEAR FINITE ELEMENT ANALYSES Page 38

63 ABU HALAWEH Ahmad CHAPTER 3 acceptable accuracy. A small triangular element that encloses a finite-sized subdomain of the area of interest is shown in Figure 3.2. b. Figure 3.2 (a) A general two-dimensional domain of field variable (x, y). (b) A three-node finite element defined in the domain. (c) Additional elements showing a partial finite element mesh of the domain. This element is not a differential element of size which makingit a finite element. When wear adopt this example as a two-dimensional problem, it is assumed that the thickness in the z direction is constant and z dependency is not indicated in the differential equation. The vertices of the triangular element are numbered to indicate that these points are nodes. A node is defined as a specific point in the finite element at which the value of the field variable is explicitly going to be calculated. Exterior nodes are located on the boundaries of the finite element and may be used to connect an element to other adjacent finite elements. Nodes that do not lie on element boundaries are interior nodes this means that they cannot be connected to any other element. The triangular element in Figure 3.2b has only exterior nodes. If the values of the field variable are computed only at nodes, the values of the field variable computed at the nodes are used to approximate the values at no nodal points (i.e., in the element interior) by interpolation of the nodal values. For the three-node triangle example, the nodes are all exterior and, at any other point within the element, the field variable is described by the approximate relation where 1, 2, and 3 are the values of the field variable at the nodes, and N1, N2, and N3 are the interpolation functions, also known as shape functions or blending functions. In the finite element approach, the nodal values of the field variable are treated as unknown constants that are to be determined. The interpolation functions are most often polynomial forms of the independent variables, derived to satisfy certain required conditions at the nodes. The major point to be made here is that the NONLINEAR FINITE ELEMENT ANALYSES Page 39

64 ABU HALAWEH Ahmad CHAPTER 3 interpolation functions are predetermined, known functions of the independent variables; and these functions describe the variation of the field variable within the finite element. The triangular element is said to have 3 degrees of freedom, as three nodal values of the field variable are required to describe the field variable everywhere in the element. This would be the case if the field variable represents a scalar field, such as temperature in a heat transfer problem. How does this element-based approach work over the entire domain of interest. As depicted in Figure 3.2c, every element is connected at its exterior nodes to other elements. The finite element equations are formulated such that, at the nodal connections, the value of the field variable at any connection is the same for each element connected to the node. Thus, continuity of the field variable at the nodes is a must. In fact, finite element formulations are such that continuity of the field variable across inters element boundaries is also ensured. Although continuity of the field variable from element to element is essential to the finite element formulation, inter element continuity of derivatives of the field variable does not generally exist. In most cases, such derivatives are of more interesting than the field variable values. For example, in structural problems, the field variable is displacement but. If the domain of Figure 3.2 represents a thin, solid body subjected to plane stress, the field variable becomes the displacement vector and the values of two components must be computed at each node. In the latter case, the threenode triangular element has 6 degrees of freedom. In general, the number of degrees of freedom associated with a finite element is equal to the product of the number of nodes and the number of values of the field variable and its derivatives that must be computed at each node. The true interest of users of FEM is more often in strain and stress. As strain is defined in terms of first derivatives of displacement components, strain is not continuous across element boundaries. However, the magnitudes of discontinuities of derivatives can be used to assess solution accuracy and convergence as the number of elements is increased, as is illustrated by the following example. 5. Finite element and exact solutions Meshing is defined as the process of representing a physical domain with finite elements creating a set of elements known as the finite element mesh. Since the commonly used element have straight sides, if the domain includes curved boundaries it will be impossible to include the entire physical domain in the element mesh. Such a situation is shown in Figure 3.3a, where a curvedboundary domain is meshed using square elements. NONLINEAR FINITE ELEMENT ANALYSES Page 40

65 ABU HALAWEH Ahmad CHAPTER 3 A refined mesh for the same domain is shown in Figure 3.3b, using smaller, more numerous elements of the same type. Note that the refined mesh includes significantly more of the physical domain in the finite element representation and the curved boundaries are more closely approximated. If the interpolation functions satisfy certain mathematical requirements, a finite element solution for a particular problem converges to the exact solution of the problem. That is, as the number of elements is increased and the physical dimensions of the elements are decreased, the finite element solution changes incrementally. The incremental changes decrease with the mesh refinement process and approach the exact solution asymptotically. To illustrate convergence, we consider a relatively simple problem that has a known solution. Figure 3.3 depicts a tapered, solid cylinder fixed at one end and subjected to a tensile load at the other end. Assuming the displacement at the point of load application to be of interest, a first approximation is obtained by considering the cylinder to be uniform, having a cross-sectional area equal to the average area Figure 3.3 Arbitrary curved-boundary domain modelled using square elements. Stippled areas are not included in the model. A total of 41 elements are shown. (b) Refined finite element mesh showing reduction of the area not included in the model. A total of 192 elements are shown. 6. Basis of FE analysis procedure in ABAQUS Any structure may be idealized as a finite number of elements assembled together in a structural system. The structural geometry, material properties, boundary conditions and the loading conditions which change the response of the structure can be quickly established. In this study the modelling and simulation of the steel links has been executed in ABAQUS (Version ) Finite Element Analysis software (ABAQUS/standard) in order to study its behaviour under a specific cyclic loading finally, link elements are also applied. Link elements are used to model structures which have one dimension (length) greater than the other two dimensions of the cross section (slenderness assumption). Moreover, they are used to model structures in which the NONLINEAR FINITE ELEMENT ANALYSES Page 41

66 ABU HALAWEH Ahmad CHAPTER 3 longitudinal stresses is of great importance. When developing a model for the finite element analysis (FEA), a typical analysis process is going to be followed as shown in the next chapter. In fact, using ABAQUS there are three basic phases that make up the finite element analysis procedure: - First phase is structural idealization in which the original system is subdivided into assemblage of discrete elements and is a critical aspect in performing an accurate analysis. This is because for the idealization to provide a reasonable and accurate representation of the actual continuum, each element must be established so that it deforms similarly to the deformations that occur in the corresponding domain of the continuum. Otherwise, as load is applied, the elements would change independently of one another, except at the nodes, and gaps or over lapping would develop along their edges. The idealization would therefore be much more flexible than the continuum. In addition, sharp stress concentrations would develop at each nodal point and the result would be an idealization that poorly resembled the actual structure. Thus, considering the deformation pattern of an element, and ensuring compatibility to adjacent elements patterns, is the most important criterion in performing this first phase. - The second phase consists of the evaluation of the element properties. This is the critical phase of the analysis procedure as it involves the setting up of the force-deflection relationship by use of a flexibility or stiffness matrix. The essential elastic characteristics of an element are represented by this force-displacement relationship which is a means of relating the forces applied at the nodes to the resulting nodal deflections. - The third phase of the finite element analysis procedure is the structural analysis of the element assemblage. As in any analysis, the main problem is to simultaneously satisfy equilibrium, compatibility, and force-deflection relationships. The basic operations for approaching this problem include the use of the displacement method which is easiest for dealing with highly complex structures. 7. Nonlinear finite element analysis In linear analysis, the response is directly proportional to the load. Linearity may be a good representation of reality or may only be inevitable result of assumptions made for the analysis purposes. In linear analysis, the assumption are the displacements and rotations are smaller, stress is directly proportional to strain and the supports do not settle and the loads maintain their original directions as the structural system deforms. The nonlinearity which presents in a structural system makes the problem more complicated because the equations that describe the solutions must incorporate the conditions not fully known until NONLINEAR FINITE ELEMENT ANALYSES Page 42

67 ABU HALAWEH Ahmad CHAPTER 3 the solution is known-the actual structural configurations, loading conditions, state of stresses and the support conditions. The solutions cannot be obtained in a single step of analysis and will take several steps, update the tentative solution after each step and repeating until a convergence is satisfied. There are three basic types of nonlinearity s and they are 1) Geometric non linearity 2) Material non linearity and 3) the boundary nonlinearity. The modelling and the analysis employed for the verification and parametric studies include the geometric non linearity s and the material non linearity s Geometrical Nonlinearity Geometric nonlinearity arises when the deformations are large enough to significantly alter the way load is applied or the way load is resisted by the structural system. Geometric non linearity s should be considered, especially when there is a large deformation and small strain case. Ignoring the effects of geometric non linearity makes the governing kinematic equations linear and thus it is impossible to capture the behaviour such as lateral torsional buckling Material Nonlinearity The stress-strain curve of steel is linearly elastic until some significant point called the yielding point. After the attainment of the yield point, the stress strain curve becomes nonlinear and the strains become partially irrecoverable. In other words when the material behaviour does not fit the elastic model there is a phenomenon of material nonlinearity. Effects due to the constitutive equations (stressstrain relations) that are nonlinear are referred to as material nonlinearities. Material nonlinearity is modelled using ABAQUS standard metal plasticity material model which is based on an incremental plasticity formulation employing associated flow assumptions in conjunction with a Von Mises failure surface whose evolution in stress-strain is governed by a simple isotropic hardening rule Failure Criteria Strength of a material or failure of the material is deduced generally from uniaxial tests from which stress strain characteristics of the material are obtained. In the case of multidimensional stress at a point we have a more complicated situation present. Since it is impractical to test every material and every combination of stresses σ 1, σ 2, and σ 3, a failure theory is needed for making predictions on the basis of material s performance on the tensile test., of how strong it will be under any other conditions of static loading. The theory behind the various failure theories is that whatever is responsible for failure in the standard tensile test will also be responsible for failure under all other conditions of static loading. NONLINEAR FINITE ELEMENT ANALYSES Page 43

68 ABU HALAWEH Ahmad CHAPTER 3 The microscopic yielding mechanism in ductile material is understood to be due to relative sliding of materials atoms within their lattice structure. This sliding is caused by shear stresses and is accompanied by distortion of the shape of the part. Thus the yield strength in shear Ssy is strength parameter of the ductile material used for design purposes. The stress required to break the atomic bond and separate the atoms is called the theoretical strength of the material. It can be shown that the theoretical strength is approximately equal to E/3 where, E is Young s modulus.1 However, most materials fail at a stress about one hundredth or even one thousandth of the theoretical strength. For example, the theoretical strength of aluminium is about 22 GPa. However, the yield strength of aluminium is in the order of 100 MPa, which is 1/220th of the theoretical strength. This enormous discrepancy could be explained as follows. In ductile material yielding occurs not due to separation of atoms but due to sliding of atoms (movement of dislocations) as depicted in Figure 3.4. Thus, the stress or energy required for yielding is much less than that required for separating the atomic planes. Hence, in a ductile material the maximum shear stress causes yielding of the material. In brittle materials, the failure or rupture still occurs due to separation of atomic planes. However, the high value of stress required is provided locally by stress concentration caused by small pre-existing cracks or flaws in the material. The stress concentration factors can be in the order of 100 to 1,000. That is, the applied stress is amplified by enormous amount due to the presence of cracks and it is sufficient to separate the atoms. When this process becomes unstable, the material separates over a large area causing brittle failure of the material. Figure 3.4 Material failures due to relative sliding of atomic planes Generally used theories for Ductile Materials are: Maximum shear stress theory Maximum distortion energy theory.(von Misestheory) The Maximum - Shear - Stress Theory The Maximum Shear Stress theory states that failure occurs when the maximum shear stress from a combination of principal stresses equals or exceeds the value obtained for the shear stress at yielding in the uniaxial tensile test. At yielding, in auni-axial test, the principal stresses are NONLINEAR FINITE ELEMENT ANALYSES Page 44

69 ABU HALAWEH Ahmad CHAPTER 3 σ 1 = Sy; σ 2 = 0 and σ 3 = 0. Therefore the shear strength at yielding Ssy = ([σ 1 - (σ 2 or σ 3 =0)])/2 (3.1) Therefore Ssy = Sy/2 To use this theory for either two or three-dimensional static stress inhomogeneous, isotopic, ductile materials, first compute the three principal stresses (σ 1, σ 2, σ 3 ), and the maximum shear stressτ 13 as τ max = ((σ 1 - σ 2 ) )/2= ((σ p max - σ p min ))/2 (3.2) Then compare the maximum shear stress to the failure criterion. τ max S sy OR (σ p max - σ p min )/2 S sy (3.3) The safety factor for the maximum shear-stress theory is given by N= S sy / τ max (3.4) Distortion-Energy Theory or The Von Mises Theory It has been observed that a solid under hydro-static, external pressure (e.g. volume element subjected to three equal normal stresses) can withstand very large stresses. When there is also energy of distortion or shear to be stored, as in the tensile test, the stresses that may be imposed are limited. Since, it was recognized that engineering materials could with stand enormous amounts of hydro-static pressures without damage, it was postulated that a given material has a definite limited capacity to absorb energy of distortion and that any attempt to subject the material to greater amounts of distortion energy result in yielding failure. Total Strain Energy: Assuming that the stress-strain curve is essentially linear up to the yield point, we can express the total strain energy at any point in that range as: U= 1/2 σε (3.5) Extending this to three dimensional case: U= ½ (σ 1 ε 1 + σ 2 ε 3 + σ 3 ε 3 ) (3.6) Where: σ 1, σ 1, and σ 3 areprincipal stresses and ε 1, ε 2, and ε 3 are principal strains. Expressing strains in terms of stresses as: ε 1 = 1/E {σ 1 - υ (σ 2 + σ 3 )} (3.7) ε 2 = 1/E {σ 2 - υ (σ 1 + σ 3 )} (3.8) ε 3 = 1/E {σ 3 - υ (σ 1 + σ 2 )} (3.9) NONLINEAR FINITE ELEMENT ANALYSES Page 45

70 ABU HALAWEH Ahmad CHAPTER 3 The total energy can be written U= (1/2E) {σ 1 2 +σ σ 3 2-2υ(σ 1 σ 2 + σ 2 σ 3 + σ 3 σ 1 )} (3.10) Figure 3.5 Stress strain curve and the strain energy Let U h be energy due to volume change and U d be energy due to distortion. Then we can express each of the principal stresses in terms of hydrostatic component (σ h ), common to all the faces of volume element and distortion component (σ id ) that is unique to each face. U= U h + U d (3.11) σ 1 =σ h +σ 1d (3.12) σ 2 =σ h +σ 2d (3.13) σ 3 =σ h +σ 3d (3.14) Adding the three principal stresses, gives σ 1 +σ 1 + σ 3 = 3 σ h + (σ 1d +σ 2d +σ 3d ) (3.15) For volumetric change with no distortion, the terms in the bracket of the above equation must be zero. Thus, we have σ h =1/3 (σ1+σ1+ σ3 ) (3.16) Now, U h can be obtained by replacing principal stresses U h = (1/2E) {σ 2 h +σ 2 h + σ 2 h -2υ (σ 2 h + σ 2 h + σ 2 h )} = 3/2 (1-2υ)/Eσ h (3.17) U h = (1-2υ)/E {σ 2 1 +σ σ (σ 1 σ 2 + σ 2 σ 3 + σ 3 σ 1 )} Distortion Energy U= U h - U d (3.18) U d = (1+υ)/E {σ 2 1 +σ σ 2 3 -σ 1 σ 2 + σ 2 σ 3 + σ 3 σ 1 } (3.19) In uniaxial stress-state at yield σ 1 =S y, σ 2 = σ 3 = 0 NONLINEAR FINITE ELEMENT ANALYSES Page 46

71 ABU HALAWEH Ahmad CHAPTER 3 Therefore energy of distortion in uniaxial stress-state 2 U du =(1+υ)/3ES y (3.20) Failure criterion according distortion energy is (1+υ)/3ES 2 y = (1+υ)/3E {σ 2 1 +σ σ 2 3 -σ 1 σ 2 - σ 2 σ 3 - σ 3 σ 1 } (3.21) S y = {σ 2 1 +σ σ 2 3 -σ 1 σ 2 - σ 2 σ 3 - σ 3 σ 1 } 1/2 (3.22) Distortion energy theory states that failure by yielding under a combination of stresses occurs when the energy of distortion equals or exceeds the energy of distortion in the tensile test when the yield strength is reached. According to theory failure criteria is S y = {σ 2 1 +σ σ 2 3 -σ 1 σ 2 - σ 2 σ 3 - σ 3 σ 1 } 1/2 (3.23) For tow dimensional stress-state (σ 2 =0), the equations reduces to S y = {σ σ σ 3 σ 1 } 1/2 (3.24) It is often convenient in situations involving combined tensile and shear stresses acting at a point to define an effective stress that can be used to represent the stress combination. The von-mises effective stress (σ e ) also sometimes referred to as equivalent stress is defined as the uniaxial tensile stress that would create the same distortion energy as is created by the actual combination of applied stresses. σ e ={σ 2 1 +σ σ 2 3 -σ 1 σ 2 - σ 2 σ 3 - σ 3 σ 1 } 1/2 (3.25) σ e = {σ σ σ 3 σ 1 } 1/2 (3.26) In terms of applied stresses in coordinate directions σ e = {σ 2 xx + + σ 2 yy σ xx σ yy +3τ 2 xy } 1/2 (3.27) Safety factor N= S y / σ e (3.28) NONLINEAR FINITE ELEMENT ANALYSES Page 47

72 Chapter 4 INELASTIC MODELLING OF LINKS BY ABAQUS

73 ABU HALAWEH Ahmad CHAPTER 4 CHAPTER 4: INELASTIC MODELLING OF LINKS BY ABAQUS 1. Introduction This chapter is divided into two main topics: First we will present some generalities concerning ABAQUS programme which we are using in this study due to the great abilities that it has especially in dealing with the finite element method, cycling loading, and performing nonlinear analyses. Secondly we are discussing the models that we implemented and tested in the ABAQUS in terms of the cyclic loading, these where 21 IPE links and another 2 HEB links to be compared with, the main aim is to determine the effect of adding stiffeners to a link. 2. Introduction to ABAQUS ABAQUS FEA is a suite of software applications for finite element analysis and computeraided engineering, originally released in The parametric study of any structure can be involved changing the spans, lateral bracing stiffness with the resulting capacities being recorded and analysed. The ABAQUS product suite consists of four core software products. ABAQUS is a suite of powerful engineering simulation programs, based on the finite element method that can solve problems ranging from relatively simple linear analyses to the most challenging nonlinear simulations. ABAQUS contains an extensive library of elements that can model virtually any geometry. It has an equally extensive list of material models that can simulate the behaviour of most typical engineering materials including metals, rubber, polymers, composites, reinforced concrete, crushable and resilient foams, and geotechnical materials such as soils and rock. ABAQUS is a program that having the ability to perform many analysing, it has the ability to consider both geometric and material nonlinearities in a given model, which is an advantage over ANSYS, ANSYS and LUSAS, merging the geometric and material nonlinearities together in the same analysis gives better results. ABAQUS contains an extensive library of elements that can model virtually any geometry. It has an equally extensive list of material models that can simulate the behaviour of most typical engineering materials including metals, rubber, polymers, composites, reinforced concrete, crushable and resilient foams, and geotechnical materials such as soils and rock. Designed as a general-purpose simulation tool, ABAQUS can be used to study more than just structural (stress/displacement) problems. It can simulate problems in such diverse areas as heat transfer, mass diffusion, thermal management of electrical components (coupled thermal-electrical analyses), acoustics, soil mechanics (coupled pore fluid-stress analyses), and piezoelectric analysis. INELASTIC MODELLING OF LINKS BY ABAQUS Page 48

74 ABU HALAWEH Ahmad CHAPTER 4 ABAQUS is simple to use and offers the user a wide range of capabilities. Even the most complicated analyses can be modelled easily. For example, problems with multiple components are modelled by associating the geometry defining each component with the appropriate material models. In most simulations, including highly nonlinear ones, the user need only provide the engineering data such as the geometry of the structure, its material behaviour, its boundary conditions, and the loads applied to it. In a nonlinear analysis ABAQUS automatically chooses appropriate load increments and convergence tolerances. Not only does it choose the values for these parameters, it also continually adjusts them during the analysis to ensure that an accurate solution is obtained efficiently. The user rarely has to define parameters for controlling the numerical solution of the problem. The commercial multipurpose finite element software package ABAQUS (Version ) is employed in this research. ABAQUS software has the ability to treat advanced analysis that may rise in a given structural system: the geometric and material non linearity, cycling loadings, dynamic analysis etc. that may rise in a given structural system. It provides the user with an extensive library of elements that can model virtually any geometry. It has a wide variety of material models that can simulate the behaviour of most typical engineering materials such as metals, composites, reinforced concrete, etc. For the purpose of performing nonlinear analyses ABAQUS software is capable of automatically choosing appropriate load increments and convergence tolerances as well as continually adjusting them during the analysis to ensure that an accurate solution is obtained efficiently. ABAQUS is an environment for modelling, managing, and monitoring analysis and visualize results using a suite of finite element analysis modules. The heart of ABAQUS is the analysis modules, ABAQUS/Standard and ABAQUS/Explicit, which are complementary and integrated analysis tools. 3. Organization of ABAQUS ABAQUS/Standard isa general-purpose, finite element module: ABAQUS/Standard employs solution technology ideal for static and low-speed dynamic events where highly accurate stress solutions are critically important. Examples include sealing pressure in a gasket joint, steady-state rolling of a tire, or crack propagation in a composite airplane fuselage. Within a single simulation, it is possible to analyse a model both in the time and frequency domain. For example, one may start by performing a nonlinear engine cover mounting analysis including sophisticated gasket mechanics. Following the mounting analysis, the pre-stressed natural frequencies of the cover can be extracted, or the frequency domain mechanical and acoustic response of the pre-stressed cover to engine induced INELASTIC MODELLING OF LINKS BY ABAQUS Page 49

75 ABU HALAWEH Ahmad CHAPTER 4 vibrations can be examined. ABAQUS/Standard is supported within the ABAQUS/CAE modelling environment for all common pre- and post-processing needs. ABAQUS/Explicit is an explicit dynamics finite element module: ABAQUS/Explicit is a finite element analysis product that is particularly well-suited to simulate brief transient dynamic events such as consumer electronics drop testing, automotive crashworthiness, and ballistic impact. The ability of ABAQUS/Explicit to effectively handle severely nonlinear behaviour such as contact makes it very attractive for the simulation of many quasi-static events, such as rolling of hot metal and slow crushing of energy absorbing devices. ABAQUS/Explicit is designed for production environments, so ease of use, reliability, and efficiency are key ingredients in its architecture. ABAQUS/Explicit is supported within the ABAQUS/CAE modelling environment for all common pre- and post- processing needs. ABAQUS/CAE incorporates the analysis modules into a Complete ABAQUS: (Complete solution for ABAQUS finite element modelling, visualization, and process automation) with ABAQUS/CAE you can quickly and efficiently create, edit, monitor, diagnose, and visualize advanced ABAQUS analyses. The intuitive interface integrates modelling, analysis, job management, and results visualization in a consistent, easy-to-use environment that is simple to learn for new users, yet highly productive for experienced users. ABAQUS/CAE supports familiar interactive computer-aided engineering concepts such as feature-based, parametric modelling, interactive and scripted operation, and GUI customization. Users can create geometry, import CAD models for meshing, or integrate geometry-based meshes that do not have associated CAD geometry. Associative Interfaces for CATIA V5, Solid Works, and Pro/ENGINEER enable synchronization of CAD and CAE assemblies and enable rapid model updates with no loss of user-defined analysis features. The open customization toolset of ABAQUS/CAE provides a powerful process automation solution, enabling specialists to deploy proven workflows across the engineering enterprise. ABAQUS/CAE also offers comprehensive visualization options, which enable users to interpret and communicate the results of any ABAQUS analysis. 4. ABAQUS applications capabilities ABAQUS is used in the automotive, aerospace, and industrial products industries. The product is popular with academic and research institutions due to the wide material modelling capability, and the program's ability to be customized. ABAQUS also provides a good collection of multiphasic INELASTIC MODELLING OF LINKS BY ABAQUS Page 50

76 ABU HALAWEH Ahmad CHAPTER 4 capabilities, such as coupled acoustic-structural, piezoelectric, and structural-pore capabilities, making it attractive for production-level simulations where multiple fields need to be coupled. ABAQUS was initially designed to address non-linear physical behaviour; as a result, the package has an extensive range of material models such as elastomeric (rubberlike) material capabilities. 5. Solution sequence Every complete finite-element analysis consists of 3 separate stages: Pre-processing or modelling: This stage involves creating an input file which contains an engineer's design for a finite-element analyser (also called "solver"). Processing or finite element analysis: This stage produces an output visual file. Post-processing or generating report, image, animation, etc. from the output file: This stage is a visual rendering stage. ABAQUS/CAE is capable of pre-processing, post-processing, and monitoring the processing stage of the solver; however, the first stage can also be done by other compatible CAD software, or even a text editor. ABAQUS/Standard, ABAQUS/Explicit or ABAQUS/CFD is capable of accomplishing the processing stage. Assault Systems also produces ABAQUS for CATIA for adding advanced processing and post processing stages to a pre-processor like CATIA. As it is shown in the picture, ABACUS CAE has 11 modules which will be used one after the other in order to modelling, loading, defining boundary conditions and finally analysis and after that showing the results, diagrams and etc These11 modules are: Part-Property-Assembely-Step- Intreaction-Load-Mesh-Optimization-Job-Vizualation-Sketch Figure 4.1 ABAQUS Modules INELASTIC MODELLING OF LINKS BY ABAQUS Page 51

77 ABU HALAWEH Ahmad CHAPTER 4 PART MODULE: This module allows you to create the geometry required for the problem. To create a 3-D geometry you first create a 2-D profile and then manipulate it to obtain the solid geometry. PROPERTY MODULE: In this module you define the material properties for your analysis and assign those properties to the available parts. Assembly Module: This module allows you to assemble together parts that you have created. Even if you have a single part you need to include it in your assembly. INTERACTION MODULE: This module allows you to rely different part by Tie, Rigid body, etc. STEP MODULE: This module allows you to select the kind of analysis you want to perform on your model and define the parameters associated with it. You can also select which variables you want to include in the output files in this modules. You apply loads over a step. To apply a sequence of loads create several steps and define the loads for each of them. LOAD MODULE: The Load Module is where you define the loads and boundary conditions for your model for a particular step (indicated in the toolbar above). You can even define loads and boundary conditions as fields like electric potential, acoustic pressure, etc. MESH MODULE: The mesh module controls how you mesh your model the type of element, their size etc. JOB MODULE: This module allows you to submit your model for analysis. VISUALIZATION MODULE: This module allows you to look at your model after deformation. You can also plot values of stress, displacement, reaction forces, etc. as contours on your model surface or as vectors or tensors. 6. Element type in ABAQUS Each element can be differed by family, number of nodes, and Degrees of freedom. Family: solid (Continuum), shell, membrane, rigid, beam, truss elements, etc. INELASTIC MODELLING OF LINKS BY ABAQUS Page 52

78 ABU HALAWEH Ahmad CHAPTER 4 Number of nodes Figure 4.2 Family of element in ABAQUS a) Figure 4.3 Number of nodes of element in ABAQUS a) Order of interpolation b) b) Types of integration INELASTIC MODELLING OF LINKS BY ABAQUS Page 53

79 ABU HALAWEH Ahmad CHAPTER 4 Degrees of freedom 1 Translation towards 1 2 Translation towards 2 3 Translation direction 3 4 rotations around the axis 1 5 rotations around the axis 2 6 rotations around the axis 3 7 buckling in beams elements to open profile 8 Sound pressure, pore pressure, or hydrostatic pressure 9 Electrical potential 10 Temperature Directions 1, 2 and 3 correspond to the global directions 1, 2 and 3, respectively; unless a local coordinate system has been defined at the nodes. Axisymmetric elements exceptionally, the degrees of freedom of movement along and rotation: 1 Translation direction r 2 Translation in the z direction 6 Rotation around the r-z plane r directions (radial) and z (axial) correspond to the global directions 1 and 2, respectively, unless a local coordinate system has been defined at the nodes. Figure 4.4 Displacement and Rotational degrees of freedom INELASTIC MODELLING OF LINKS BY ABAQUS Page 54

80 ABU HALAWEH Ahmad CHAPTER 4 7. System of units in ABAQUS ABAQUS has no built-in system of units. Specify all unit data in consistent units. Some common systems of consistent units: SI: m, N, kg, s, Pa, J, kg/m 3 SI (mm): mm, N, tonne (1000 kg), s, MPa, mj, tonne/mm 3 US Unit (ft): ft, lbf, slug, s, lbf/ft 2, ft lbf, slug/ft 3 Figure 4.5 Systems of Units Each element in ABAQUS has a unique name, such as S4R, B31, M3D4R, C3D8R and C3D4. The element name identifies primary element characteristics. Furthermore it is possible to create new element in FORTRAN and used it in ABAQUS. 8. Element shapes in ABAQUS There are various kinds of element types in ABAQUS: Quad: Use exclusively quadrilateral elements. The following figure shows an example of a mesh that was constructed using this setting. Quad-dominated: Use primarily quadrilateral elements, but allow triangles in transition regions. This setting is the default. The following figure shows an example of a mesh that was constructed using this setting. Tri: Use exclusively triangular elements. The following figure shows an example of a mesh that was constructed using this setting. Hex: Use exclusively hexahedral elements. This setting is the default. The following figure shows an example of a mesh that was constructed using this setting. INELASTIC MODELLING OF LINKS BY ABAQUS Page 55

81 ABU HALAWEH Ahmad CHAPTER 4 Hex-dominated: Use primarily hexahedral elements, but allow some triangular prisms (wedges) in transition regions. The following figure shows an example of a mesh that was constructed using this setting. Tet: Use exclusively tetrahedral elements. The following figure shows an example of a mesh that was constructed using this setting. Wedge: Use exclusively wedges elements. The following figure shows an example of a single-element mesh that was constructed using this setting. Figure 4.6 Element shapes in ABAQUS: a) Quad b) Quad-dominated c) Tri d) Hex e) Hex-dominated f) Tet g) Wedge. 9. Linear and quadratic element types The choice of the elements depends on the type of problem and the material. In General, the Quadratic meshes give more accurate results than the Linear meshes. But the quadratic elements should NOT be used for the faces coming in contact. This will produce unrealistic jump in Contact Pressure values. In that case, better to refine the mesh and use linear elements. INELASTIC MODELLING OF LINKS BY ABAQUS Page 56

82 ABU HALAWEH Ahmad CHAPTER 4 Many non-linear problems use nearly incompressible materials. Usage of Fully Integrated Elements in this case will lead to volumetric locking and therefore excessive stiffness. Usage of Reduced Integration elements (e.g. C3D8R) will relax it and provide more realistic results. But, one should be careful with the effect of hour glassing (Hour glassing is a phenomenon that creates an artificial stress field on the top of the real field. Therefore you see geometric stress patterns that do not have any physical basis. Hour glassing causes problem in accuracy. The way to check for hour glassing is to look at the artificial energy and compare it to strain energy. The ratio should not exceed 1%) when using Linear Reduced Integration Elements. Hour glassing is the phenomena of elements distorting in such a way that there is no change in Strain Energy. It behaves like a rigid body mode. One should be concerned with hour glassing effect only in Linear Reduced Integration elements. In Quadratic Reduced Integration Elements, Hour glassing doesn't propagate and therefore has no big effect. Most of the times, hour glassing can be controlled by using enhanced hour glass stiffness option. When using hour glass stiffness one must keep an eye on the artificial energy created in the system and make sure it is low. 10. MODELS DESCRIPTION Eccentrically Braced Frames (EBFs) are a type of lateral resistance system in which the Link Beam behaves as dissipated part of structure. The study conducted in this thesis basically focuses on the use of 3-D finite element models uses a previously developed mid-span (frame) finite element. In this study, a total of 21 IPE models isolated links of different shear and long (flexural) links have been studied and another 2 HEB links. A commercially available finite element package ABAQUS which is a suite of finite element analysis modules was used to conduct the detailed threedimensional finite element analysis of the seventeen models. ABAQUS finite element analysis is used to study the elastic and inelastic behaviour under a protocol (AISC 2006) monotonic cycling loadings has been used. Two types of sections have been used, namely IPE360 and IPE450. The length of each model has been designed to EC8 provisions. Many factors have been shown to affect the active link of the member, including the width-tothickness ratio, the effective slenderness ratio, the width-to-depth ratio, and the mechanical properties INELASTIC MODELLING OF LINKS BY ABAQUS Page 57

83 ABU HALAWEH Ahmad CHAPTER 4 of the steel. Also, the effect of stiffeners in the post-elastic range with different configuration, either transverse or diagonal or a combined case: transverse and diagonal stiffeners are considered. A general view of models and materials is shown below. The finite elements method using solid elements is used to analyse these models. The cyclic loading sequence provided in Appendix S of the 2006 AISC Seismic Provisions (Displacement / Plastic rotation control) was used for all analytical models. To investigate the inelastic behaviour of IPE link beams, a nonlinear inelastic finite-element model is developed based on the specifications and assumptions given in the following sections. Full cyclic analysis is necessary in this study to consider the effects of local buckling and associated strength degradation. The link loading protocol in Appendix S of the 2005 modified in 2006 AISC Seismic Provisions was used for the study. Link rotation was defined as the imposed transverse displacement divided by the link length. The material properties used for all models considered herein are: the modulus of elasticity of steel was assumed to be 200 GPa and the Poisson s ratio was assumed to be 0.3.The nonlinear material behaviour was modelled using Von Mises and Tresca yield criterion Definition of the models We have used two types of sections in our study, IPE360 and IPE450. All elements lengths were been designed to meet EC8 provisions. The meshing element C3D8R (an 8-node linear brick, reduced integration, hourglass control), which represents a3d, hexahedral element with eight nodes where specially chosen from the ABAQUS element library because it s the most suitable one for our study Link geometry Each (sub-section) of IPE, namely IPE360 and 450, contains 4 short links having the same length, and differs in the number and location of stiffeners their configuration. Also, seemlier4 long links having the same length, and differ in the stiffener place, and an IPE 450 short having a special stiffener model, this special stiffener was placed in a Diagonal way connecting both ends. The following models have been created to examine problems emerged when the links are subjected to cyclic load. The geometrical characteristics of the links are provided below. INELASTIC MODELLING OF LINKS BY ABAQUS Page 58

84 ABU HALAWEH Ahmad CHAPTER 4 a b Figure 4.7 Link geometry without stiffeners: a) long link b) short link Stiffeners geometry Stiffeners are usually required to control buckling effects from shear stresses in steel members. They are added to a slender girder to ensure that the web panel is able to develop its shear strength and shear buckling resistance. In conclusion, the typical web stiffeners aim to limit buckling in the link web. Types of Stiffeners: transverse stiffeners diagonal stiffeners a b Figure 4.8 Types of stiffeners: a) transverse stiffeners b) diagonal stiffeners. INELASTIC MODELLING OF LINKS BY ABAQUS Page 59

85 ABU HALAWEH Ahmad CHAPTER 4 Transverse Stiffeners: To investigate the possibility of increasing the rotation capacity of the links, besides the stiffeners at a distance 1.5b f from each end of the link, additional stiffeners were placed at a distance of 1.5b f from the side, conducted an analytical study to investigate the behaviour and performance of 21 links, eight of which were nine long, and eight short. In this study, those links were simulated and analysed with additional stiffeners (placed at a distance 1. 5b f ) from the two ends, we have also added another stiffener exactly in the middle of the link. Since, in some old researched specimens local buckling was observed in the flange of the beam in the brace connection panel, in some of these specimens, besides the link beam, the brace connection panels were also modelled at the ends of the link beams. Based on seismic provisions, lateral bracing was located at the two ends of the links to prevent lateral torsional buckling. Diagonal stiffeners: The impact on rotation capacity when using two diagonal stiffeners at link ends was investigated. These stiffeners are embedded at a distance of 1.5b f at two ends of the link on one side. In this section, to investigate the behaviour of links with this type of stiffener, all specimens considered in the above section are analysed, with and without modelling the brace connection panels having diagonal stiffeners. To prevent penetration of the local buckling into the brace connection panel, the diagonal stiffeners are also placed in brace connection panels symmetrically with the same dimensions. Table 4.1 Geometrical properties of the models Web stiffeners Type e mm NTS NDS t s mm LL / LL / SL / SL / LL LL LL LL INELASTIC MODELLING OF LINKS BY ABAQUS Page 60

86 ABU HALAWEH Ahmad CHAPTER 4 LL LL LL LL SL SL SL SL SL SL SL SL SL Where: LL: long link 360 without Stiffeners LLʺ: long link 450 without Stiffeners SL: short link 360without Stiffeners SLʺ: short link 450 without Stiffeners LL1: long link 360 with two symmetrical transverse stiffeners LL2: long link 360 with two transverse stiffeners associated to two diagonal stiffeners; LL3: long link 360 with three transverse stiffeners (one in mid-span) LL4: long link 360 with three transverse stiffeners associated to two other diagonal stiffeners LL5: long link 450 with two symmetrical transverse stiffeners LL6: long link 450 with two transverse stiffeners associated to two diagonal stiffeners; LL7: long link 450 with three transverse stiffeners (one in mid-span) LL8: long link 450 with three transverse stiffeners associated to two other diagonal stiffeners SL1: short link 360 with two symmetrical transverse stiffeners SL2: short link 360 with two transverse stiffeners associated to two diagonal stiffeners; SL3: short link 360 with three transverse stiffeners (one in mid-span) SL4: short link 360 with three transverse stiffeners associated to two other diagonal stiffeners SL5: short link 450 with two symmetrical transverse stiffeners SL6: short link 450 with two transverse stiffeners associated to two diagonal stiffeners; SL7: short link 450 with three transverse stiffeners (one in mid-span) SL8: short link 450 with three transverse stiffeners associated to two other diagonal stiffeners SL9: short link 450 with two transverse stiffeners associated to one diagonal stiffeners INELASTIC MODELLING OF LINKS BY ABAQUS Page 61

87 ABU HALAWEH Ahmad CHAPTER 4 e: is link length designed according to the eurocode NTS: Number of Transverse Stiffeners NDS: Number Diagonal Stiffeners t s : Depth of stiffeners Figure 4.9 Basic geometry with Stiffeners of models example for a short IPE Description of Models Material Properties There are number of different parameters that affect the nonlinear material behaviour of a structure. At different load levels, as the stiffness of the structure changes, the response of the structure will be different. The steel used in this work is of grade s235. The mechanical properties used in all models are listed below including the nominal values of yield strength fy and ultimate tensile strength fu. The FEM-material has following properties: Density, p=7850 Kg/m3. Young s Modulus, E= MPa. Poisson s ratio, υ = 0.3. The max value of plastic strain ε pl =0.25 fy = 235MPa Fu = 360MPa INELASTIC MODELLING OF LINKS BY ABAQUS Page 62

88 ABU HALAWEH Ahmad CHAPTER 4 Class of sections to EC3 Table 4.2 Dimensions and material properties of IPE type b f mm d mm t f mm t w mm Iy cm 4 Iz Iy/Iz fy cm 4 MPa IPE IPE fu MPa Table 4.3 Section classes according to EC3 IPE t f c c/t f Flange classes d t w d/t w Web classes Section classes Therefore, the cross section belongs to class 1 with respect to bending and to class 2 with respect to compression Boundary Conditions In this study, the behaviour of isolated link beams is investigated, boundary conditions are shown in figure 3.4; nodes on the left end were restrained against all degrees of freedom except horizontal translation. Nodes on the right end were restrained against all degrees of freedom except vertical translation. Transverse loading was applied as displacements to the right end nodes. These boundary conditions lead to constant shear along the length of the link, with equal end moments and no axial forces. Figure4.10 FEM model boundary conditions applied to the links: (a) Initial configuration (b) deformed configuration INELASTIC MODELLING OF LINKS BY ABAQUS Page 63

89 ABU HALAWEH Ahmad CHAPTER Cyclic Loading The aim of the study is to determine the response of short and long links under earthquake loads. Thus, In order to take into account the deterioration in strength due to plastic local buckling, cyclic analysis was performed using the loading protocol given in Appendix S of the 2005 AISC Seismic Provisions. Monotonic analysis under-predicts buckling amplitudes and strength degradation. Link rotation was defined as the imposed transverse displacement divided by the link length. We have a maximum rotation of 0.02 rad for the long links and 0.08 rad for the short links. Cyclic displacements were applied to the specimens in the plane of the web of the specimens to simulate earthquake loading. The loading was applied until failure of the specimen initiated. In finite element simulation conducted in this thesis, the displacement is defined in only the y-direction which is normal to the plane of the flanges and displacements in other directions are restraint to illustrate the experimental setup. Figure4.11 The loading protocol INELASTIC MODELLING OF LINKS BY ABAQUS Page 64

90 ABU HALAWEH Ahmad CHAPTER 4 Table 4.4 Proposed long link Loading Protocol (IPE360) Load step break link rotation angle rad Displacement mm Table 4.5 Proposed long link Loading Protocol (IPE450) Load step break link rotation angle rad Displacement mm Table 4.6 Proposed Short Link Loading Protocol (IPE360) Load Break link Displacement step rotation angle rad mm INELASTIC MODELLING OF LINKS BY ABAQUS Page 65

91 ABU HALAWEH Ahmad CHAPTER 4 Table 4.7 Proposed Short Link Loading Protocol (IPE450) Load step Break link rotation angle rad Displacement mm Meshing Meshing is the way to divide the study subject (links) into small particles with the exact same properties (size, type, geometry, etc.) to examine each particle alone. Combining all these small particles give us the mesh. In this study we have used a Hex-dominated which uses hexahedral elements, providing six degrees of freedom per node and provides accurate solutions for most relevant applications, and also allow some triangular prisms (wedges) in transition regions. Namely C3D8R (an 8-node linear brick, reduced integration, hourglass control), this special configuration where chosen from the ABAQUS element library due to the facility of applying and retrieving results with the minor errors. Figure 4.12 Meshing type example for a short 360. INELASTIC MODELLING OF LINKS BY ABAQUS Page 66

92 Chapter 5 RESULTS AND DISCUSSION

93 ABU HALAWEH Ahmad CHAPTAER 5 CHAPTER 5: RESULTS AND DISCUSSION 1. Introduction Chapter 5 describes the evaluation of the study EBFs using extensive inelastic behaviour of links. The study parameters included: length of links, geometrical properties of links, slenderness rations of web and flanges, plastic displacements. This chapter is devoted to the results coming up from 21 models analysed with a brief discussion. It discusses the parameters of the parametric study, an overview of the isolated links within the study, the results of study, and general conclusions resulting from the study. Also, additional results of the HEB section without stiffeners will be discussed and compared to investigate the effect of the shape section on the nonlinear behaviour of links. These models are series of isolated links belonging to flexural and shear kind. These two sections differ from their slenderness ratios. The nonlinear twenty one models computations were performed using the commercial finite element software package ABAQUS, as has the ability to consider both geometric and material nonlinearities in a given model with large deflection, and large strain capability. All of these models where modelled in the ABAQUS finite element software using the C3D8R (an 8-node) model that is implanted in ABAQUS to mesh the links. This mesh type where specially used because it is suitable for complex plastic buckling behaviour and has six degrees of freedom per node and provides accurate solutions to most relevant applications. Flanges were modelled with 10 elements across the width and 14 elements were used throughout the web height for IPE360 and 18 elements were used throughout the web height for IPE450. Boundary conditions for each and every link are the same. These boundary conditions preventing axial deformation of the link while allow translation at both ends. The typical value for the modulus of elasticity (E= MPa) is considered. Nominal yield stress (fy) and ultimate stress (fu) values of steel S235 are specified as of 235 and 360 MPa, respectively. It should be noted that the effects of residual stresses and low-cycle fatigue (brittle failure mode) were not considered in this work. Full cyclic analysis is necessary in this study to consider the effects of local buckling with the associated strength degradation. The link loading protocol used in this study is described in 2005 AISC Seismic Provisions. The loading protocol consisted of 32 cycles of increasing displacement amplitude ranging from 5.4 mm up to 32 mm. According to this procedure the link is subjected to several loading cycles by controlling the total link rotation angle ( total).in our study we have used two protocols for two sets of links. First set the short links where we imposed total as follows: 6 cycles at total= rad; 6 cycles at total=0.005 rad; 6 cycles at total= rad; 6 cycles at total=0.01 rad; 4 cycles at total=0.015 rad; 4 RESULTS AND DISCUSSION Page 67

94 ABU HALAWEH Ahmad CHAPTAER 5 cycles at total=0.02 rad; 2 cycles at total=0.03 rad; 1 cycle at total=0.04 rad; 1 cycle at total=0.05 rad; 1 cycle at total=0.07 rad; 1 cycle at total=0.09 rad;and continue at loading increments of total=0.01 rad, with one cycle of loading at each step. Second set the long links where we imposed total as follows: 6 cycles at total= rad; 6 cycles at total=0.005 rad; 6 cycles at total= rad; 6 cycles at total=0.01 rad; 4 cycles at total=0.015 rad; 4 cycles at total=0.02 rad; and continue at loading increments of total=0.01 rad, with one cycle of loading at each step. The early cycles usually produce elastic response of the link. The applied loading procedure is given in Figure below: Figure 5.1 The applied loading protocol The link stiffeners were placed on both sides of the link according to EC8 provisions. For each model analysed in this work, five cases have been studied, namely: - - the link without stiffeners; - with two symmetrical transverse stiffeners; - with three transverse stiffeners (one in mid-span), - with two transverse stiffeners associated to two diagonal stiffeners; - with three transverse stiffeners associated to two other diagonal stiffeners It can be noted that the thicknesses of stiffeners are 8 mm and 9.5 for IPE360 and IPE450 respectively for all models (long or short links). RESULTS AND DISCUSSION Page 68

95 ABU HALAWEH Ahmad CHAPTAER 5 Table5.1 Identification of long links models Model LL LL1 LL2 LL3 LL4 LLʺ LL5 LL6 LL7 LL8 IPE Stiffeners 0 2T 2T+2D 3T 3T+2D 0 2T 2T+2D 3T 3T+2D Table5.2 Identification of short links models Model SL SL1 SL2 SL3 SL4 SLʺ SL5 SL6 SL7 SL8 SL9 IPE Stiffeners 0 2T 2T+2D 3T 3T+2D 0 2T 2T+2D 3T 3T+2D 2T+1D IPE1 = IPE360 IPE2 = IPE450 T= for transverse stiffeners D= for diagonal stiffeners To ensure the link would achieve the required rotation angle end, stiffeners were to be employed at the link ends. The initial link investigation utilized numerical modelling software to model a variety of link end stiffener configurations. Several quantities were monitor during a typical analysis for each model. These include results of equivalent stress from Von Mises, and Tresca criterion, the magnitude of displacement U, magnitude of plastic strain PEMAG, Equivalent Plastic strain PEEQ. The results include elastic energy dissipation, Active yield flag, Logarithmic strain components LE, and Plastic strain components etc. 2. Results and detailed discussion Structures suffer significant inelastic deformation under a strong earthquake and dynamic characteristics of the structure change with time so investigating the performance of a structure requires inelastic analytical procedures accounting for these features Long links IPE 360 For LL the long link without stiffeners, it can be seen from figure 5.2 that the first buckling appears in both the flange and the web in the same location that is the mid-span at the 125 increment under an equivalent stress according to Von Mises criterion of 237 MPa roughly the yielding stress and a displacement magnitude of 17 mm. At the increment 170, the magnitude increases to 19.8 mm with a stress equal to 279 MPa which represents an increase of 17 % in stress and displacement values. RESULTS AND DISCUSSION Page 69

96 ABU HALAWEH Ahmad CHAPTAER 5 a b c d Figure 5.2 a) Distributions of stress at 125 increment b) Distributions of displacement magnitude at 125 increment c) Distributions of stress at the increment 170 d) Distributions of displacement magnitude at the increment 170. For LL1 the long link with two transverse stiffeners, it can be seen from figure 5.2 that the first buckling appears in both the flange and the web in the same location that is the mid-span for LL1at the 147 increment under an equivalent stress according to Von Mises criterion of 291 MPa greater than the elastic stress and an equivalent displacement of 18 mm. This means that the link behaves already is in the plastic range. At the increment 199, the value of applied stress raised to be 325 MPa, which represents the ultimate value of the stress along with a 19.5 mm, which represents an increase of 12 % in stress and 8 % in the displacement values. This shows the favourable effect of the stiffeners to delay the buckling phenomenon to occur. a b RESULTS AND DISCUSSION Page 70

97 ABU HALAWEH Ahmad CHAPTAER 5 c d Figure 5.3 a) Distributions of stress at 147 increment b) Distributions of displacement magnitude at 149 increment c) Distributions of stress at the increment 199 d) Distributions of displacement magnitude at the increment 199. For LL2 the long link with two transverse stiffeners associated with two diagonal stiffeners, it can be seen from figure 5.4 that the first buckling appears in both the flange and the web. However, the location of the buckling area occurs in left side of the link. The area between seems to be not concerned by any buckling phenomena. At the 153 increment the first buckling appears under an equivalent stress according to Von Mises criterion of 245 MPa corresponding to mm in magnitude. At increment 216, the equivalent stress reaches the value of 342 MPa. This means that the link behaves already is in the plastic range. At the increment 199, the value of applied stress raised to be 325 MPa, which represents roughly the ultimate value of the stress along with a mm magnitude, which represents an increase of 39 % in stress and 4 % in the displacement values. This shows the effect of diagonal stiffeners to delay the buckling phenomenon to occur and changing the location of the buckling area. a b RESULTS AND DISCUSSION Page 71

98 ABU HALAWEH Ahmad CHAPTAER 5 c d Figure 5.4 a) Distributions of stress at 153 increment b) Distributions of displacement magnitude at 153 increment c) Distributions of stress at the increment 216 d) Distributions of displacement magnitude at the increment 216. For LL3 the long link with three transverse stiffeners, it can be seen from figure 5.5 that the first buckling appears in both the flange and the web. At the 143 increment the first buckling appears under an equivalent stress according to Von Mises criterion of 250 MPa, which means that the link behaves already, is in the plastic range with corresponding magnitude of 17.4 mm in magnitude. At increment 197, the equivalent stress reaches the value of 294 MPa with represents a stress less than the ultimate value of the stress. The overall view shows that the left hand side of the link is more concerned with the buckling than it is for the right hand side. a b c d RESULTS AND DISCUSSION Page 72

99 ABU HALAWEH Ahmad CHAPTAER 5 Figure 5.5 a) Distributions of stress at 143 increment b) Distributions of displacement magnitude at 143 increment c) Distributions of stress at the increment 197 d) Distributions of displacement magnitude at the increment 197. For LL4 the long link with three transverse stiffeners associated with two diagonal stiffeners, it can be seen from figure 5.6that the first buckling appears in both the flange and the web. The first bucking appears at 153 increments with equivalent stress equal to 302 MPa corresponding to a magnitude of 19.3 mm. The same remarks can be said as LL2, The location of the buckling area occurs in left side of the link. The area on the right side of the link seems to be not concerned by any buckling phenomena. At increment 216, the equivalent stress reaches the value of 346 MPa, which represents roughly the ultimate value of the stress. That means that the link behaves already is in the plastic range. The corresponding is 21.5 mm, which represents an increase of 14% in stress and 3 % in the displacement values. This shows the effect of diagonal stiffeners to delay the buckling phenomenon to occur and changing the location of the buckling area decreases and negligible decrease of displacement. a b c d Figure 5.6 a) Distributions of stress at 153 increment b) Distributions of displacement magnitude at 153 increment c) Distributions of stress at the increment 216 d) Distributions of displacement magnitude at the increment 216. RESULTS AND DISCUSSION Page 73

100 ABU HALAWEH Ahmad CHAPTAER Short Link IPE 360 For SL the short link without stiffeners, it can be seen from figure 5.7 that the buckling does not appear. However, the flanges seem to undergo more plastic stresses and strains as it is for the web area in which the maximum stresses appear to act diagonally. While and as far as the displacement is concerned, a value of mm which represents 10 times less than it is in LL. A value exceeding the yield stresses 272 MPa on the top and bottom flange and the web. It can be concluded that a short link without stiffeners is more stable than a long one. a b Figure 5.7 a) Distributions of stress at last increment b) Distributions of displacement magnitude at last SL1 the short link with two symmetrical transverse stiffeners, it can be seen from figure 5.8 that a small buckling of the on the top and bottom of the flange appear. Both the flanges and web undergo plastic stresses and strains as it is for the web area in which the maximum stresses are spread uniformly through the web. a b Figure 5.8 a) Distributions of stress at last increment b) Distributions of displacement magnitude at last increment RESULTS AND DISCUSSION Page 74

101 ABU HALAWEH Ahmad CHAPTAER 5 SL2 the short link with two symmetrical transverse stiffeners associated with two diagonal stiffeners. As it can be seen from figure 5.9 a small buckling of the bottom flange appears. Comparing to LL1, the moving location of buckling area does not appear for this case. Both the flanges and web undergo plastic stresses and strains as it is for the web area in which the maximum stresses are spread uniformly through the web. The presence of these additional diagonal stiffeners does not seem to improve the buckling behaviour of the link. a b Figure 5.9 a) Distributions of stress at last increment b) Distributions of displacement magnitude at last increment SL3 the short link with three transverse stiffeners. As it can be seen from figure 5.10 a small buckling between the stiffeners of the bottom and the top flange appears under the roughly the same value of the stress. Comparing to LL1, the moving location of buckling area does not appear for this case. Both the flanges and web undergo plastic stresses and strains as it is for the web area in which the maximum stresses are spread uniformly through the web. The presence of these additional diagonal stiffeners does not seem to improve the buckling behaviour of the link. a b Figure 5.10 a) Distributions of stress at last increment b) Distributions of displacement magnitude at last increment RESULTS AND DISCUSSION Page 75

102 ABU HALAWEH Ahmad CHAPTAER 5 SL4 the short link with three transverse stiffeners associated with two diagonal stiffeners figure The same conclusions can be drawn as it is for the previous case. That is as, it can be noticed a small buckling of the bottom flange appears. Comparing to LL4, the moving location of buckling area does not appear for this case. Both the flanges and web undergo plastic stresses and strains as it is for the web area in which the maximum stresses are spread uniformly through the web. The presence of these additional diagonal stiffeners does not seem to improve the buckling behaviour of the link. a b Figure 5.11 a) Distributions of stress at last increment b) Distributions of displacement magnitude at last increment 2.3. Long Links IPE 450 For the case of long links made of IPE450, an overall discussion will be held. The numerical nonlinear analysis shows practically no differences in the obtaining results. As it can be noticed from figures presented below, that the installation of transverse stiffeners does not contribute significantly to improve the strength of the links neither their capacity to resist any kind of buckling. Indeed, the local buckling occurs at mid-span in the top and the bottom of the flange regardless whether the link has or not transverse stiffeners. As it can be seen from m figures, the web is slightly affected by the local buckling in the vicinity of junction with the flange. This is due principally to the ratio slenderness 20.1 which is higher that it is for the case of IPE360 which is Another parameter which seems to be decisive is the length of the link in a nonlinear behaviour of the long link. However, for the case of LL6 (450), with two diagonal stiffeners, as for the case of IPE360, the buckling area has moved to the left hand side of the link. With an increasing of the stress to reach 360 MPa which is in turn the ultimate yield stress and with a decreasing in displacement about 10%. RESULTS AND DISCUSSION Page 76

103 ABU HALAWEH Ahmad CHAPTAER 5 a b Figure 5.12 Samples of results for LLʺ model a) Distributions of stress at last increment, b) Distributions of displacement magnitude at last increment a b Figure 5.13 Samples of results for LL5 model a) Distributions of stress at last increment b) Distributions of displacement magnitude at last increment a RESULTS AND DISCUSSION Page 77 b

104 ABU HALAWEH Ahmad CHAPTAER 5 Figure 5.14 Samples of results for LL6 model a) Distributions of stress at last increment b) Distributions of displacement magnitude at last increment a b Figure 5.15 Samples of results for LL7 model a) Distributions of stress at last increment b) Distributions of displacement magnitude at last increment a b Figure 5.16 Samples of results for LL8 model a) Distributions of stress at last increment b) Distributions of displacement magnitude at last increment 2.4. Short Link IPE 450 For SLʺ the short link without stiffeners, it can be seen from figure 5.17(a) - (d) that the buckling appear in both web and flange of the section, especially in flange and web junction under equivalent stress of about 287 MPa with exceed largely the yielding stress of the material. The magnitude of displacement reaches the value of 14. The first bucking seems to occur at the increment 108 under a stress of 269 MPa, which means that the link behaves already in plastic range with corresponding displacement of 9.45mm. An increase of 7% in stress is responsible for a growth of 58% in displacement. This is due to the rapid decreasing of the stiffness of the link. RESULTS AND DISCUSSION Page 78

105 ABU HALAWEH Ahmad CHAPTAER 5 a b c d Figure 5.17 a) Distributions of stress at 108 increment b) Distributions of displacement magnitude at 108 increment c) Distributions of stress at the increment 145 d) Distributions of displacement magnitude at the increment 145. SL5 the short link with two symmetrical transverse stiffeners, it can be seen from figure 5.18 that a significant buckling of the whole of the link can noticed. Both the flanges and web undergo plastic stresses and strains as it is for the web area in which the maximum stresses are spread uniformly through the web. The value of displacement decreases to be 4.6 which represent 30 % the displacement discussed above. This is certainly due to the transverse web stiffeners which delay the occurrence of local buckling. RESULTS AND DISCUSSION Page 79

106 ABU HALAWEH Ahmad CHAPTAER 5 a b Figure 5.18 a) Distributions of stress at last increment b) Distributions of displacement magnitude at last increment SL6 the short link with two symmetrical transverse stiffeners associated with two diagonal stiffeners. As it can be seen from figure 5.19 a small buckling of the bottom flange appears between the stiffeners. The buckling occurs approximately at mid span of the top flange and near the left hand side of right transverse stiffener. The presence of diagonal stiffeners seems to contribute poorly to the strength and stiffness as the ultimate displacement with a value of 5.37 greater than the previous case. a b Figure 5.19 a) Distributions of stress at last increment b) Distributions of displacement magnitude at last increment SL7 the short link, with three transverse stiffeners. As it can be seen from figure 5.20 the value of displacement of 4.7 mm is comparable to the previous case, with a stress exceeding 300 MPa which can be explained by the fact that this configuration confers more strength and more stiffness to the link. RESULTS AND DISCUSSION Page 80

107 ABU HALAWEH Ahmad CHAPTAER 5 a b Figure 5.20 a) Distributions of stress at last increment b) Distributions of displacement magnitude at last increment SL8 the short link with three transverse stiffeners associated with two diagonal stiffeners figure 5.21 the link seems to be not concerned with buckling problems. The Comparing to value of the displacement falls to the value of 3 mm. This means that this configuration is better than the previous. a b Figure 5.21 a) Distributions of stress at last increment b) Distributions of displacement magnitude at last increment SL9 the short link with three transverse stiffeners associated with one diagonal stiffener figure Both the flanges and web undergo plastic stresses and strains as it is for the web area in which the maximum stresses of 300 MPa are spread uniformly through the web. This particular configuration shows a buckling of the stiffer itself. This is due essentially to the slenderness ratio of the stiffener. The presence of this single stiffener seems to have a better performance than the SL2. RESULTS AND DISCUSSION Page 81

108 ABU HALAWEH Ahmad CHAPTAER 5 a b Figure 5.22 a) Distributions of stress at last increment b) Distributions of displacement magnitude at last increment Comparing to LL1, the moving location of buckling area does not appear for this case. Both the flanges and web undergo plastic stresses and strains as it is for the web area in which the maximum stresses are spread uniformly through the web. The presence of these additional diagonal stiffeners does not seem to improve the buckling behaviour of the link. 3. Full results from ABAQUS 3.1. Long Link Table 5.3 Final results given by ABAQUS for Long links parameters LL LL1 LL2 LL3 LL4 LLʺ LL5 LL6 LL7 LL8 Mises Tresca PEEQ PEMAG U Short links The table below presents the ABAQUS results for all the short links created in the study. RESULTS AND DISCUSSION Page 82

109 ABU HALAWEH Ahmad CHAPTAER 5 Table 5.4 Final results given by ABAQUS for Short links parameters SL SL1 SL2 SL3 SL4 SLʺ SL5 SL6 SL7 SL8 SL9 Mises Tresca PEEQ PEMAG U Comparison between tow section HEB and IPE for long link without stiffener The idea was to assess the influence of section shape on the nonlinear behaviour of the link under cyclic loading. Based on similar geometric characteristics of sections, it has been found that IPE 360 is approximately equivalent to HEB 280, while IPE450 is equivalent to HEB 320. Two models have been implanted in ABAQUS, in the same manner as it was for the other models, with the same conditions. Models studied are those without stiffeners to demonstrate the basic case. The results have shown a better performance of models made from HEB compared to IPE ones. HEB sections have the advantages of such sections have been pointed out with reference to the link lengths and according to EC8 and EC3, all HEB sections have sufficient local ductility for use in high-ductility structures. The local buckling from which IPE sections suffer appears to not affect links made from HEB. This is due essentially to the shape of HEB section with approximately moment of inertia in the principle directions. Also, it can be noticed that the displacements fall dramatically for HEB compared to those obtained in similar conditions for IPE sections. The table below shows sample of the results (i.e., Von Mises, Tresca) criteria, Equivalent Plastic strain, Magnitude Plastic strain, and Magnitude Displacement. Comparing the IPE to the HEB, without stiffeners in any of these sections. RESULTS AND DISCUSSION Page 83

110 ABU HALAWEH Ahmad CHAPTAER 5 Table 5.5: Comparison between IPE and HEB. model HEB280 LL HEB320 LLʺ Mises Tresca PEEQ PEMAG U a b Figure 5.23 Samples of results for HEB280 model a) Distributions of stress at last increment b) Distributions of displacement magnitude at last increment a b Figure 5.24 Samples of results for HEB320 model a) Distributions of stress at last increment b) Distributions of displacement magnitude at last increment RESULTS AND DISCUSSION Page 84

111 shear force(kn) ABU HALAWEH Ahmad CHAPTAER 5 Remark: Figure below shows the shear force (KN) and the displacement (mm), this loop curve is a result of a cyclic charge. We have met two problems getting this result First time: which is the main problem in this whole study. Second the curve was nut complete due to the insufficient capabilities of EXCEL. Figure 5.25 represent all the shear force and the displacement for SL7, SL8 models Série1 Série Displacement (mm) Figure 5.25 Shear force and the displacement for SL7, SL8 models. The green loops represent SL7 The blue loops represent SL8 RESULTS AND DISCUSSION Page 85

112 Conclusion

113 CONCLUSION The initial idea of this research was to investigate the nonlinear behaviour of long links as few works dealing with this kind of link are available in the literature. By this analysis, the intention was to contribute to a better comprehension of such kind of links. However, when the modelling of such links was successfully made, the idea has come to extend the study to include the shear links and to understand the behaviour of each of kind. This attempt was also successful. However, with the huge volume of results coming from ABAQUS for each case raises the difficulties of dealing with them. It has been decided to take a sample of results including the equivalent stress, the magnitude of displacement as samples of results. The remaining results are left to future analysis and discussion. In this thesis, a parametric numerical study was carried out on a series of shear and long links system to investigate their cyclic behaviour using the AISC2006 loading protocol. The long and shear links which were expected to behave inelastic manner, were modelled using a C3D8R (an 8-node) (ABAQUS) is used with geometric and material nonlinearities with large deflection, and large strain capability. Results of 22 numerical nonlinear models implanted in ABAQUS are being presented in this study. The results coming up from this work have shown parameters which significantly affect the performance of flexural and shear links. These parameters such as the geometrical properties IPE (360 and 450), including the slenderness ratios of flange and the web. Obviously, the thickness of flange and thickness of web is kept constant in this analysis because it cannot be modified in the field due to the applied IPE hot-rolled profiles which are given by default from the factory. Some other parameters can be cited: the geometric and the configuration of the stiffener thickness. Therefore this research analysis topic is focused on the effect of transverse and including diagonal stiffeners and vertical stiffener where those parameters could be modified easily to increase theoretically the performance of flexural and shear links. The influence of section shape has roughly being investigated. These parameters are the flange and web thicknesses, the number, location and configuration of stiffeners. Unfortunately, the total results which are huge coming from this nonlinear analysis cannot be discussed because of short of time. Such discussion normally leads to a better understanding of the performance of these kinds of links. Nevertheless, some conclusions can be drawn from the study presented herein, while waiting for a full discussion of overall results to be done. Page D

114 CONCLUSION 1. Results from this study of the links made from IPE, and regardless the height of the section, show that short links are more stable than the long ones as that the former have more sensitivity to buckling problems. 2. Despite the number and the configuration of stiffeners, their effects on IPE 450 Long links do not appear to be significant. However for short links, stiffeners seem to increase the strength and especially stiffness of the links. 3. The installation of stiffeners decreases the magnitude of displacement and the diagonal stiffeners have favourable effect on plastic strains. 4. Stiffeners control the location of the area of local buckling. 5. For all models considered in this work and due to their high ductility, the links can undergo high level of stresses and strains, exceeding the yield stress and beyond the ultimate stress of the material. 6. The local buckling from which IPE sections suffer appears to not affecting links made from HEB. This is due essentially to the shape of HEB section with approximately moment of inertia in the principle directions. Also, it can be noticed that the displacements fall dramatically for HEB compared to those obtained in similar conditions for IPE sections. Page E

115 REFERENCES