MODELING AND ANALYSIS OF STEEL GUSSET PLATES IN TRUSS BRIDGES UNDER LIVE LOAD MEGHAN M. MYERS. A thesis submitted to the

Transcription

1 MODELING AND ANALYSIS OF STEEL GUSSET PLATES IN TRUSS BRIDGES UNDER LIVE LOAD by MEGHAN M. MYERS A thesis submitted to the Graduate School - New Brunswick Rutgers, The State University of New Jersey in partial fulfillment of the requirements for the degree of Masters of Science Graduate Program in Civil and Environmental Engineering written under the direction of Dr. Hani Nassif and approved by New Brunswick, New Jersey October, 2011

2 ABSTRACT OF THE THESIS MODELING AND ANALYSIS OF STEEL GUSSET PLATES IN TRUSS BRIDGES UNDER LIVE LOAD By MEGHAN M. MYERS Thesis Director: Dr. Hani Nassif In the aftermath of the collapse of the I-35W over Mississippi River Bridge in Minnesota, the Federal Highway Administration (FHWA) issued a technical advisory to bridge owners to check the status of similarly-designed bridges. It was determined that underdesigned gusset plates contributed to the collapse. This sparked a nationwide effort to investigate the design of these connection members and to develop more detailed specifications for future gusset plate design. In order to thoroughly study complicated bridge elements such as gusset plates, sophisticated analysis techniques are required. One such technique is finite element modeling (FEM), which is used here to identify critical loading cases for typical Warren truss gusset plates. The specific gusset plates studied here are located on two bridges, herein referred to as Bridge A and Bridge B, that are similar in design to the I-35W Bridge. Following the I- 35W collapse, independent investigations, which included finite element analysis, were initiated on both bridges. In this thesis, information from these investigations is used to develop a comprehensive FEM, which facilitates more in-depth analysis of such gusset ii

3 plates. The analysis focuses on the investigation of stresses created in the gusset plates by various types of live loading. The results are compared to the Method of Sections approach recommended by FHWA following the I-35W Bridge collapse to determine if better analysis specifications are needed. Although the results of the finite element analysis and the Method of Sections approach are similar, the authors conclude that the value of the Method of Sections approach is strongly dependent on the accuracy of the load data input. Therefore, more detailed specifications are needed to ensure the accuracy of future gusset plate analysis and design. iii

4 ACKNOWLEDGMENTS I would first like to thank my thesis advisor, Dr. Hani Nassif for giving me the opportunity to conduct this research under him and for his guidance and support during this time. I would also like to thank my committee members, Dr. Kaan Ozbay and Dr. Perumalsamy Balaguru for their useful comments and input. I would like to acknowledge Arora and Associates, P.C. for affording me the opportunity to work on various fatigue-sensitive, fracture-critical steel bridges, which introduced me to the field of gusset plate modeling and analysis. Special thanks are also given to Dr. Nakin Suksawang and Mr. Dan Su for introducing me to other truss bridge evaluations and assisting me in some of my finite element model development. Much of this thesis was supported by previous publications that I would like to acknowledge. My publications submitted to Safety and Reliability of Bridge Structures for the New York City Bridge Conference (Myers 2009a), the NSBA World Steel Bridge Symposium (Myers 2009b), and the NDE/NDT for Highways and Bridges: Structural Materials Technology Conference were largely influential to the development of this thesis. Lastly, I would like to thank my family and friends, and especially my husband Clayton, for their continuous support throughout my time completing the Rutgers University Masters Program. Without their understanding and encouragement during this busy time, my success in this endeavor would not have been possible. iv

5 TABLE OF CONTENTS ABSTRACT OF THE THESIS... ii ACKNOWLEDGMENTS... iv TABLE OF CONTENTS... v LIST OF FIGURES... vii LIST OF TABLES... xi CHAPTER 1. INTRODUCTION Motivation Justification... 3 CHAPTER 2. LITERATURE REVIEW Early Research Current Research CHAPTER 3. INITIAL ANALYSIS Bridge A Project Introduction Method of Sections Analysis Bridge A Finite Element Model Bridge A Instrumentation Bridge A Conclusions CHAPTER 4. MODEL DEVELOPMENT Creating a Model in Abaqus v

6 4.2 Bridge B Research and Model Development Model Integration CHAPTER 5. PARAMETRIC STUDY Varying Plate Thickness Varying Live Load Validating Integrated Plate Model Comparing In-Depth FEM to Method of Sections CHAPTER 6. CONCLUSIONS AND RECOMMENDATIONS REFERENCES vi

7 LIST OF FIGURES Figure 1: Method of Sections notations and section locations... 2 Figure 2: Whitmore Section (Whitmore 1952)... 6 Figure 3: Block Shear sections (Higgins et al. 2010) Figure 4: Bridge A truss geometry for BAR7 model Figure 5: Gusset plate shop drawings for the gusset plates in each category experiencing the highest loads in the BAR7 analysis and used in the hand calculations Figure 6: Typical lower, odd numbered gusset plate type on Bridge A Figure 7: Geometry of Gusset Plate L16 for STAAD model Figure 8: The STAAD finite element model for Gusset Plate L16 depicting nodes and triangular plate elements Figure 9: Stress contours on Gusset Plate L16 from STAAD finite element model Figure 10: Typical section loss in Bridge A gusset plate Figure 11: Sensor locations on Bridge A Gusset Plate L Figure 12: Bridge responses recorded by sensors on Bridge A Gusset Plate L Figure 13: Sensor readings before live loading event for four of the five truss members 31 Figure 14: Sensor readings before live loading event for fifth truss member Figure 15: Sensor readings at peak strain of vertical truss member Figure 16: Sensor readings at peak strain of south diagonal truss member Figure 17: Sensor readings at peak strain of south chord truss member Figure 18: Sensor readings at peak strain of north diagonal truss member Figure 19: Sensor readings at peak strain of north chord truss member vii

8 Figure 20: Example gusset plate for detailed Abaqus finite element model Figure 21: Finite element model of Truss Spans 25, 26, and 27 in Bridge B (Nassif et al. 2007) Figure 22: Integration point of (a) two-node, linear beam (B31) and (b) three-node, quadratic beam (B32) elements along the length of the beam (Abaqus 2010) Figure 23: Four-node (S4) shell element (Abaqus 2010) Figure 24: Typical stress-strain curve of structural steel (Salmon and Johnson 1996) Figure 25: Comparison of stresses in S5-S10 using the FE model and Static Load Test 1 (Nassif et al. 2007) Figure 26: Comparison of stresses in S5-S10 using the FE model and Static Load Test 3 (Nassif et al. 2007) Figure 27: Standard truck configurations used in the calibration of the finite element model (Nassif et al. 2007) Figure 28: Comparison of stresses in S5 using the FE model and the actual field-test data of a 5-axle truck with a GVW of 65 kips traveling WB in Lane 1 (Nassif et al. 2007) Figure 29: Comparison of stresses in S6 using the FE model and the actual field-test data of a 5-axle truck with a GVW of 65 kips traveling WB in Lane 1 (Nassif et al. 2007) Figure 30: Comparison of stresses in S7 using the FE model and the actual field-test data of a 5-axle truck with a GVW of 65 kips traveling WB in Lane 1 (Nassif et al. 2007) viii

9 Figure 31: Comparison of stresses in S8 using the FE model and the actual field-test data of a 5-axle truck with a GVW of 65 kips traveling WB in Lane 1 (Nassif et al. 2007) Figure 32: Comparison of stresses in S9 using the FE model and the actual field-test data of a 5-axle truck with a GVW of 65 kips traveling WB in Lane 1 (Nassif et al. 2007) Figure 33: Comparison of stresses in S10 using the FE model and the actual field-test data of a 5-axle truck with a GVW of 65 kips traveling WB on Lane 1 (Nassif et al. 2007) Figure 34: Bridge B full truss model with gusset plate integration (red circles) in Abaqus Figure 35: Test-truck configuration (top) and information (bottom) for controlled load tests (Nassif et al. 2007) Figure 36: Under-deck view of Span 26 Bay 1 between FB11 and FB12 (Nassif et al. 2007) Note: rectangles represent strain transducers Figure 37: Span 26 sensor layout involving 16 strain gauges and 4 LVDTs (Nassif et al. 2007) Figure 38: Comparison of Abaqus FEM results at Sensor 6 location with and without gusset plate integration Figure 39: Comparison of FEM results at adjacent truss members with and without gusset plate integration Figure 40: Chart graphing plate stress vs. plate thickness Figure 41: Results of varying live load on a gusset plate on Bridge B ix

10 Figure 42: Gusset plate in full bridge model stress contours from Abaqus Figure 43: Individual 3D gusset plate model stress contours from Abaqus x

11 LIST OF TABLES Table 1: Gusset plate categories and worst-case plates for Bridge A Table 2: Summary of D/C ratios calculated under HS20 live loading for all analyzed gusset plates Table 3: Summary of D/C ratios calculated under Permit live loading for all analyzed gusset plates Table 4: Comparing stresses for Horizontal Section A-A of gusset plate L Table 5: Comparing stresses for Vertical Section B-B of gusset plate L Table 6: Comparison between hand calculation results using the sensor data and the BAR7 data Table 7: Truck configuration (Nassif et al. 2007) Table 8: Configuration for various trucks used for live loading in model (italics indicate estimations) Table 9: Stress comparisons between plate models Table 10: Plate stresses using Method of Sections xi

12 1 CHAPTER 1. INTRODUCTION 1.1 Motivation At 6:05 P.M. EST on Wednesday, August 1, 2007, the bridge over the Mississippi River between University Avenue and Washington Avenue on highway I-35W in Minneapolis, MN, collapsed. Numerous vehicles were on the bridge at the time, and, as is well known, there was a tragic loss of life and a vital transportation link was severed. At the time, in light of the uncertainty surrounding the cause of the collapse, the Federal Highway Administration (FHWA) advised all State Transportation Agencies and other bridge owners to immediately re-inspect all steel deck truss bridges with fracture critical members or at a minimum to review inspection reports, including those for routine, indepth, fracture critical, and underwater, to determine whether more detailed inspections were warranted. It was later discovered that under designed gusset plates were a contributing cause of the collapse. After this discovery, interest in analyzing existing gusset plates on other similar bridges was generated. This sparked a nation-wide interest in looking deeper into the design of these connection members and the possibility of developing new procedures for future use in such design. In 2008, an investigation was initiated on a bridge henceforth referred to as Bridge A due to its similarity to the I-35W Bridge. The gusset plates on the bridge were to be analyzed to determine whether they were adequate to carry the current loads that were being seen on the bridge. This investigation initiated the development of a finite element model to

13 2 predict the stresses in typical gusset plates on such a bridge. This bridge consists of a continuous haunched Warren deck truss that makes up the three main spans of the bridge. To begin this investigation, documents regarding the bridge geometry and history were collected and reviewed. Using information found in these documents, the bridge was analyzed and loads were generated that represent the current state of stress on the truss. The gusset plates were then investigated using the analysis techniques presented in the FHWA Turner-Fairbank Highway Research Center report on the I-35W Bridge dated January 11, This analysis consisted of a method of sections calculation, where equilibrating loads are calculated for a horizontal and vertical section through a gusset plate to balance the applied loads from the connecting truss members. These sections can be seen in Figure 1 below. Figure 1: Method of Sections notations and section locations After hand calculations were performed to analyze the stresses in the above defined sections, a finite element model was created using STAAD PRO 2005 software to calculate similar stresses. This was done to try to verify the results of the hand calculations. As an extension of the Bridge A analysis, the authors of this paper used

14 3 some of the information found from the investigation of Bridge A as a starting point for a more in-depth analysis. This more in-depth analysis focused on the integration of an individual gusset plate finite element model (FEM) into a 3D full truss bridge FEM. Once the integrated model was complete, variations of live loading that may be experienced by a bridge of this type were applied to the model to determine the stress on gusset plates under such loading. Comparisons were also made between the integrated FEM and the Method of Sections calculations suggested by FHWA. 1.2 Justification Gusset plate connections are very complicated bridge elements. For this reason, many researchers have looked into using finite element modeling in order to really determine how these connections behave. However, since these connections need to be investigated and analyzed often by bridge owners, especially in the last few years, more simplified methods are needed. Development of good, detailed finite element models is too time consuming to be used frequently by these agencies. Though, for research purposes, FEM is a useful tool in learning more about the behavior of these members. As such, the research presented in this paper uses finite element models to find out critical loading cases for typical Warren truss gusset plates. As a focus, this research investigates various types of live loading and how the truss member reactions from these trucks affect the stresses in the gusset plate. For instance, the permit trucks used in typical analyses and ratings of bridges are normally heavy trucks that are also longer than the typical HS20 live load case specified by the American

15 4 Association of State Highway and Transportation Officials (AASHTO). These permit trucks are meant to represent the largest legal trucks allowed on roads. However, there could be heavier trucks that make it onto roads unnoticed. Also, in some cases, trucks that are slightly less heavy, or maybe just as heavy as permit trucks, but are much shorter in length, such as full dump trucks, may end up creating a more critical reaction in trusses since the heavy load would be carried by fewer truss members. These are the types of concepts investigated in this study.

16 5 CHAPTER 2. LITERATURE REVIEW 2.1 Early Research Some of the previous research done specifically to evaluate locations and magnitudes of stress in gusset plates, and to derive a simple way to determine maximum stresses for designing these structural members was performed by Whitmore (Whitmore 1952). In his investigation, Whitmore mainly studied the joints in Warren type truss configurations, one of the most common truss types. For the gusset plates tested, he determined that maximum tension and compression forces were located around the ends of the diagonal members and maximum shearing stresses were located near the chord member and toward the center of the plate, with much lower stresses toward the edge of the plate. The results of this analysis contradicted what had been the regularly assumed distribution of stresses in such gusset plates. Whitmore then found that the maximum stresses at the ends of the diagonal members could be approximated by dividing the force from the truss member by an area equal to the width of the plate multiplied by a length measured perpendicular to the truss member axis along the bottom row of bolts and between two lines measured 30 degrees from the outside columns of bolts along the truss member axis. This section, known now as the Whitmore Section, can be seen in Figure 2 below.

17 6 Figure 2: Whitmore Section (Whitmore 1952) The Whitmore Section analysis became the more widely used procedure to design and check gusset plates until the development of the block shear analysis method. In the 1980 s there were a number of analyses performed in order to further understand the specific stress devices working in typical gusset plate configurations. As mentioned above, Warren, along with Pratt, trusses are the most common truss shapes. Yamamoto, Akiyama, and Okumura (Yamamoto et al. 1985) performed experiments and theoretical analyses on elastic stress distributions in gusset plates of these common truss configurations. The paper stated that at that time the design of gusseted joints is based on rather simple methods of analyses and current design specifications hardly establish definite rules about gusset plate thickness. This is attributed to the general lack of experimental research available on the design of gusset plates. This idea that current design standards do not adequately deal with design of gusset plates is still somewhat relevant today, as will be discussed later in this section. Yamamoto et al. proposes formulae to calculate the design thickness of gusset plates. These formulae establish

18 7 rules for calculating required gusset plate thickness to transmit axial forces and bending moments and transmit shear forces. Another consideration within the study of gusset plates is the evaluation of fatigue and fracture. A study performed under the National Cooperative Highway Research Program (NCHRP) Project (Fisher et al. 1987) researched these mechanisms in riveted connections on bridges. It was confirmed through this study, which examined data from a Department of Transportation (DOT)-sponsored research study, as well as other studies and full-scale tests, that the type of riveted connection does not affect resistance to fatigue stresses in any significant way. It also confirmed that primary members in these riveted bridges are not expected to develop fatigue cracks, though the study did not cover gusset plates specifically. Fatigue stresses were also studied by Kitzawa, Kanaji, Ohminami, and Furukawa (Kitazawa et al. 1994), though with slightly different results. Kitazawa et al. found that the fatigue strength of the gusset plates on the cable-stayed Higashi-Kobe Bridge were not sufficient to resist the largest stresses from live loading. These differing results may very well be attributed to the design standards in Japan versus the United States and the difference between stresses in the types of bridges (cable-stayed versus riveted connections in other kinds of bridges). An aspect of analyzing bridges that has not been considered in many truss analyses is the specific differences that may result from various types of live loads passing over the bridge, specifically, heavier trucks than the standard permit trucks used for rating bridges. One such research project that was conducted on this topic was by Laman, Pechar, and

19 8 Boothby (Laman, et al. 1999). This study looked at the affect of bridge component type, component peak static stress, live load type, and live load speed on the dynamic stresses in steel through-truss bridges. The results do not seem to conclude anything specific about the live load type, and the gusset plates on the bridge were not one of the components analyzed. This leaves some gaps in the topic of truss live load analysis for consideration in future research. In 2006, a Rutgers University team performed field tests, analysis, simulations, and laboratory tests in order to identify if cracking in the deck of a bridge (herein referred to as Bridge B) is caused by shrinkage or by live load vibrations (Nassif 2007). To accurately measure the loads that were crossing the bridge, multiple sensors were installed on the bridge, including a portable Weigh-in-Motion (WIM) system and two piezo-axle sensors connected to a main data collection unit. Using these sensors to measure live load on the bridge, as well as other sensors to measure bridge response, it was possible to create accurate, calibrated finite element models to determine the overall impact of the live load on the bridge, though the gusset plates in particular were not studied at this time. In 2006 Huns et al. conducted research with the objective of developing a finite element model that could predict the tension and shear block failure of gusset plates and conducting a reliability analysis of existing test results to evaluate current design equations and propose new limit state design equations. The current practices in North America, Europe, and Japan for tension and shear block design (Kulak and Grondin

20 9 2000, 2001) were reviewed and it was discovered that the equations give a satisfactory prediction of capacity of gusset plates, but do not predict the failure mode as well. Some other studies were conducted in search of similar results. Chakrabarti and Bjorhovde (1983) and Hardash and Bjorhovde (1984) studied inelastic behavior of gusset plates in tension, Hu and Cheng (1987) and Yam and Cheng (1993) studied gusset plates in compression, and Rabinovitch and Cheng (1993), Walbridge et al. (1998), and Nast et al. (1999) studied gusset plates under cyclic loading. The conclusions of the Huns et al. research state that the existing literature as well as the finite element analysis performed in this study indicate that tension fracture always occurs before shear rupture. It also indicates that most of the connections showed the full capacity of the gusset plate being reached before the rupture occurs. It was determined through the reliability analysis that equations posed by Hardash and Bjorhovde (1984) and Driver et al. (2004) provide a good prediction of the test results of the gusset plates, where the equations in the design standards were overly conservative and in some cases did not predict the failure mode accurately. Also in 2006, Li, Zhou, Chan, and Yu (Li et al. 2006), published a paper on their research in multi-scale numerical analysis on long-span bridges. This research focused on local damage and dynamic responses in such bridges and used the stiffening truss of a suspension bridge in China as a case study. Li et al. believe that the most effective way to analyze such a complicated structure is through models that account for damage and deterioration and the behavior of the connections between main structural elements. This study concluded that such multi-scale modeling was necessary for the evaluation of long-

21 10 span bridges and the effects of damage on them. A discrete evaluation of the structural elements in such a bridge cannot adequately evaluate more complex responses such as fatigue in the trusses of these bridges, although this simpler form of analysis can be useful in that it can be easily applied for quicker analyses. 2.2 Current Research A variety of topics in the realm of truss or gusset plate analysis were discussed in the previous section. These connections have always been a somewhat lesser understood element, in that their responses and reactions are complex and are many times designed to well exceed necessary capacity in order to assure that they are not the first thing to fail on the bridge. However, in 2007, the collapse of the I-35W Bridge over the Mississippi River in Minneapolis, Minnesota brought the topic of truss analysis to the forefront of structural engineering research. Many studies were performed and papers were written on the analysis of the collapse of the I-35W Bridge (e.g. Holt & Hartmann 2008, Minmao et al. 2009, Hao 2010, Liao et al. 2011). Through the forensic structural analyses performed, it was determined that underdesigned gusset plates were a contributing cause of the collapse of the bridge. The inadequate gusset plates were yielded at the time of the collapse, and increased weight on the bridge due to construction on the deck (materials, equipment, etc.) caused the failure of the plate and the collapse of the bridge. In July of 2009, the FHWA issued a publication entitled Load Rating Guidance and Examples for Bolted and Riveted Gusset Plates in Truss Bridges. This publication was produced in order to give guidance to bridge owners on how to analyze and load rate

22 11 gusset plates. This publication and its guidelines were based on the existing practices and knowledge in the field. However, these guidelines could be updated with information received from a current study that is underway. This study is being conducted by FHWA and is being sponsored jointly by FHWA and AASHTO through the NCHRP. In 2010, Higgins et al. performed a study to compare the methods of block-shear (depicted in Figure 3 below) and Whitmore Section stress evaluation on truss gusset plates. As noted earlier, these kinds of studies became more prevalent after the collapse of the I-35W Bridge. Block shear and Whitmore section analyses are two of the most prevalent methods of gusset plate analysis, which is why these were the two compared in this study. The specific failure mode in a gusset plate will depend on the geometry, distribution of loads, and material properties for that specific gusset plate. This is why there are many failure planes in the block shear method. Higgins et al. found that using the block-shear method on plates that were originally designed with the Whitmore section methods and allowable stress design will produce rating factors below 1.0. They also determined that gusset plates made from higher yield strength steel and those with more bolts produce lower rating factors with the block-shear method. Figure 3: Block Shear sections (Higgins et al. 2010)

23 12 From the current AASHTO bridge specifications, Article states, Gusset or connection plates should be used for connecting main members, except where the members are pin-connected. The fasteners connecting each member shall be symmetrical with the axis of the member, so far as practicable, and the full development of the elements of the member should be given consideration. The comments to this article state that, Following the 2007 collapse of the I-35W Bridge in Minneapolis, the traditional procedures for designing gusset plates, including the provisions of this Article, have been under extensive review. As of Spring 2008, new design procedures have not been codified. Guidance from FHWA is expected shortly. Designers are advised to obtain the latest approved recommendations from Owners. This comment coincides with the statement made by FHWA on their website that was mentioned in the above. When the joint study between FHWA and AASHTO has been completed, it is expected that new guidelines will be given in AASHTO as to how to go about designing future truss bridge gusset plates. This same article also describes the design equations as follows, The maximum stress from combined factored flexural and axial loads shall not exceed φ f Fy based on the gross area. The maximum shear stress on a section due to the factored loads shall be φ v Fy/ 3 for uniform shear and φ v 0.74 Fy/ 3 for flexural shear computed as the factored shear force divided by the shear area. If the length of the unsupported edge of a gusset plate exceeds 2.06(E/Fy) 1/2 times its thickness, the edge shall be stiffened. Stiffened and unstiffened gusset edges shall be investigated as idealized column sections. Besides the reference that is given to the more general Sections and in AASHTO (Block Shear Rupture Resistance and Connection Elements), these are the only guidelines for specific design of gusset plates. This shows the relative uncertain nature of gusset plate design to this point. Obviously the topic of gusset plate analysis is a broad and complex one. This paper focuses on the topic of varying live load cases and their impact on truss gusset plates.

24 13 CHAPTER 3. INITIAL ANALYSIS 3.1 Bridge A Project Introduction As mentioned before, many authorities began investigations of their bridges with similar details to the I-35W Bridge after its collapse. In particular, Bridge A was the subject of such gusset plate analyses. Bridge A is a five-span bridge consisting of a continuous haunched Warren deck truss, which makes up the three main spans, and two deck girder side spans. The overall bridge span is approximately 740 ft, and its width is 61 ft 6 in. The longest of the five spans is the center span, which is 280 ft long. To initiate this analysis, a review of the bridge inspection reports, design calculations, photograph logs, and plans was performed, and a detailed history of the bridge was compiled considering its structural configuration, modifications made through rehabilitation and maintenance contracts, and the condition of the primary members. This was helpful in determining what changes had been made to the structure since the original design and construction and the current state of stress in each of the primary members and, hence, the gusset plates. Using the information found in these documents, the most recent computer analysis run performed on this structure was reviewed and updated. The rating program BAR7 was used to reanalyze the bridge and generate new loads that represent the current state of stress on the truss. Based on the results and the gusset plate geometry detailed in the original shop drawings, the gusset plates were grouped into categories for further analysis. The gusset plates were then investigated

25 14 using the analysis techniques presented in the FHWA Turner-Fairbank Highway Research Center report on the I-35W Bridge dated January 11, 2008 (FHWA 2008). 3.2 Method of Sections Analysis The model that was used to analyze the three-span, continuous deck truss unit is shown in Figure 4. Figure 4: Bridge A truss geometry for BAR7 model With revised input and an updated model, BAR7 was run and new member forces were generated. The live load cases considered were HS20 and Permit loadings. For the Permit live load run, it was assumed that there were three lanes loaded with 100%, 55%, and 55% of the truck load respectively. The two 55% lanes approximate the force of an HS20 live load, while the 100% represents the one lane of Permit truck loading. There are 58 gusset plates in each of the deck trusses. Rather than analyze every gusset plate, a representative sample of gusset plates with worst-case scenario loads and geometry was selected for analysis. The first step was to split the plates into categories

26 15 based on their thickness and their location on the truss. This resulted in 9 different categories. Within each of the categories, the worst-case location was determined using the forces calculated in the new BAR7 run. Table 1 lists the various categories by which each gusset plate could be identified and the gusset plate(s) chosen for analysis for each category. Gusset Plate Worst-Case Gusset Plates Categories High Loads Other 5/8 Upper Chord U7 11/16 Upper Chord U9 3/4 Upper Chord U13 1/2 Upper Chord U14 U8 3/4 Lower Chord L0 L28 11/16 Lower Chord L14 1/2 Lower Chord L15 L7 5/8 Lower Chord L16 Multiple Gussets L8 Table 1: Gusset plate categories and worst-case plates for Bridge A One of these categories ( Multiple Gussets ) consisted solely of the panel points at the pier supports. These panel points contain 4 gusset plates stacked together and represent a unique and important situation. In some categories, two gusset plates were analyzed due to the large differences in force direction (tension vs. compression) and geometry of the connecting truss members (right angles vs. more extreme angles). In the end, the 58 gusset plates in each truss were narrowed down to only 12 that were analyzed. The shop drawing for the high-load gusset plates in each category is shown in Figure 5 below.

27 Figure 5: Gusset plate shop drawings for the gusset plates in each category experiencing the highest loads in the BAR7 analysis and used in the hand calculations 16

28 17 Calculations were performed to analyze the representative gusset plates to determine the forces and stresses acting on them. The calculations and methods used were based on the reconstructed design calculations for the I-35W over Mississippi River Bridge illustrated in the FHWA report (FHWA 2008). The procedure that was used makes two cuts in the plate, one horizontal, just above or below the horizontal member (section A-A) and one vertical, just next to the vertical member (section B-B), as shown in Figure 1 in the introduction section of this paper. Based on the truss member forces found from BAR7, equilibrating axial, shear, and moment forces are calculated to balance the truss member forces from one side of the cut plane. Then the axial (f a = P/A), flexural (f b = M/S), and shear (f v-avg = V/A) stresses along the section and the principal tension and compression stresses are calculated, taking into account any splice plates that contribute to the gusset plate section properties. For this analysis, the principal stresses were taken at either the section neutral axis or at the edge of the plate depending on which was greater. The neutral axis principal stresses were calculated by 2 2 fa fa 3 f ten / comp fv avg (1) and the principal stresses at the edge of the gusset plate were calculated by f ten / comp fa fb (2) The plus or minus was applied in each of these equations to create the biggest tension and compression stresses for each case. For the final step in this procedure, a

29 18 Demand/Capacity (D/C) ratio is produced using AASHTO allowable stresses as the capacities. The review of the available bridge plans and documents did not reveal which edition of AASHTO was used to perform the original bridge design or what grade of steel was used. Therefore, the AASHTO Manual for Condition Evaluation of Bridges, Second Edition was used to determine the allowable stresses. In the Manual, there is a category for unknown steel constructed between 1936 and 1963, which specifies Grade 33 steel. Since the bridge was designed in 1954 and constructed in 1957, Grade 33 steel was assumed in order to determine the allowable stresses for these calculations. For Inventory Rating (IR) compression allowable stress, the AASHTO Manual for Condition Evaluation of Bridges formula for compression in concentrically loaded columns for bridges built between 1936 and 1963, 2 KL F comp 15, (3) r was used, since the FHWA procedure models the edge of the gusset plate as a column. It is noted that the 1949 version of AASHTO uses 2 1 L F comp 15, (4) r for compression in concentrically loaded columns having values of L/r not greater than 140 and with riveted ends. The differences between Equation 3 and Equation 4 would not have significantly changed the results of the analysis. Therefore, the AASHTO

30 19 Manual equation (Eq. 3) was the one chosen, since it is a more general guideline. The Operating Rating (OR) equation for compression allowable stress that was used is 2 KL F comp 19, (5) r The AASHTO Manual was also consulted to determine the allowable stresses for tension (F ten = 18,000 psi for IR and 24,500 psi for OR) and shear (F v-avg = 11,000 psi for IR and 15,000 psi for OR). The same allowable stresses used for tension were also used for the bending allowable stresses, F b. Based on the calculated stresses and D/C ratios, it was evident which gusset plates would require further investigation. There is one D/C ratio over 1.00 for the HS20 live load case, which occurs for f comp. The ratio occurs in gusset plate U13 (1.03 at Section B-B). The gusset plates in the table that have NOT APPLICABLE written in the Section B-B columns are placed at the intersection of a vertical web truss member and a chord truss member. These are located at the centers of continuous chord members and are therefore not carrying much, if any, of the horizontal load. Also, as the gusset plates at these locations are only slightly wider than the vertical truss member, the location of the vertical section would effectively be at the edge of the plate and would not reveal internal gusset plate forces and stresses. This is why the vertical cut was not considered applicable for the analysis. An example of one of these thinner gusset plates can be seen in Figure 6 below.

31 20 Figure 6: Typical lower, odd numbered gusset plate type on Bridge A A summary of the analysis results is shown in Table 2 and Table 3 below for HS20 and Permit loading, respectively. HS20 Section A-A Section B-B f b f v-avg f ten f comp f b f v-avg f ten f comp U U NOT APPLICABLE U U * U NOT APPLICABLE L L NOT APPLICABLE L L L NOT APPLICABLE L L *Case where D/C ratio is greater than 1.0. Table 2: Summary of D/C ratios calculated under HS20 live loading for all analyzed gusset plates

32 21 Permit Section A-A Section B-B f b f v-avg f ten f comp f b f v-avg f ten f comp U U NOT APPLICABLE U U U NOT APPLICABLE L L NOT APPLICABLE L L L NOT APPLICABLE L L Table 3: Summary of D/C ratios calculated under Permit live loading for all analyzed gusset plates Even though the stresses under Permit live loading are larger, the D/C ratios that were calculated were lower than those under HS20 live loading. This was a result of the fact that the Permit live load stresses were compared to Operating Rating allowable stresses. Unsupported edge length adequacy was also studied. Only one of the applicable gusset plates (gusset plates connecting diagonal members) investigated did not comply with the unsupported edge limit, expressed by Unsupported Edge 11,000 Limit F y platethickness (6) This equation is for the unstiffened unsupported edge limit from the AASHTO Standard Specifications for Highway Bridges, Ninth Edition. The gusset plate that did not comply with this limit is located at panel point U9. Since the long unsupported edge of this gusset plate is in tension, it was concluded that all the gusset plates on the bridge were adequate to meet the criteria for unsupported edge length limit.

33 Bridge A Finite Element Model For this investigation of Bridge A, analyses were taken a step beyond the FHWA suggested procedure. As a verification of the hand calculations, a 2D finite element model using STAADPRO 2005 software was developed. Interior gusset plate L16 was chosen as a representative example for this model. The gusset plate dimensions, connection configuration and the limits of splice plates were confirmed after a review of the original shop drawings and were input into the FE model. A copy of the original shop drawing for gusset plate L16 depicting its geometry can be seen in Figure 7 below. Figure 7: Geometry of Gusset Plate L16 for STAAD model Nodes (joints) were generated to define boundaries for the gusset plate, limits of splice plates, and locations of the fasteners in each of the five connections. For simplicity, the

34 23 connection holes in the gusset plate were not modeled. After these fixed nodes were established, a 4 x 4 grid of nodes was placed over the model to fill in the areas between these key points. The node geometry was reviewed and joints from the 4 x 4 grid that conflicted with any of the initially determined fixed nodes were deleted. Locations of conflict were determined by engineering judgment. Triangular plate elements were then generated between the remaining nodes. Figure 8 shows the layout of the nodes and triangular plate elements. Figure 8: The STAAD finite element model for Gusset Plate L16 depicting nodes and triangular plate elements The triangular plate elements within the limits of the splice plate were assigned the thickness of the combined gusset and splice plates (2 ), while elements outside this area were assigned the thickness of the gusset plate alone (5/8 ). The basic geometry model was analyzed for the two sections evaluated with the hand calculations. For the horizontal Section A-A, truss member forces from members B, D, and E were applied to

35 24 the plate. For vertical Section B-B, the member forces from members A and C were applied. Support conditions for the finite element model were given careful consideration. Axial forces taken from the BAR7 output are envelope forces; they represent the maximum values in a given member, but do not necessarily occur under the same loading conditions or at the same time. As a result, the gusset plate as an individual free body is not in equilibrium when these maximum loads are applied simultaneously. Therefore, separate support conditions were established to develop equilibrating forces in the truss members that did not have their maximum forces applied to the model. This was accomplished by placing additional nodes in line with the fasteners of the existing connection and just beyond the gusset plate boundary. These nodes were assigned the properties of a pinned support. From these supports, truss elements were generated in the model to connect each of the fastener nodes in the adjacent connection to the new virtual pinned support. These additional truss elements were assigned a proportion of the area of the corresponding truss member. Loads were applied to the remaining connector nodes depending upon which section of the gusset plate was being evaluated. For example: When evaluating vertical Section B-B, forces from truss members A and C were applied to the model and supports were generated at additional nodes located in line with the existing connections of truss members B, D and E. Unit (1 kip) axial forces, resolved into components along the global X- (horizontal) and Y- (vertical) axes, were applied to each of the fastener nodes. Component values were

36 25 calculated based upon the geometry of the individual connection. The forces from each truss member were considered as a separate load case. The live and dead load axial force values obtained from the BAR7 analysis were divided equally amongst the number of connectors in each member. This per connector value was then applied as a factor to the unit load cases in the Load Combination command. Stresses were checked using the feature in STAAD that allows the user to define a cutting plane. Using this STAAD command, horizontal and vertical cutting planes were established at the same locations in the model that were evaluated in the hand calculations. The stresses are summarized in Table 4 and Table 5 below. Positive values represent tensile stresses; negative values represent compressive stresses. Section A-A Left Side of Plate Right Side of Plate ksi ksi Hand Calculations STAAD Model Table 4: Comparing stresses for Horizontal Section A-A of gusset plate L16 Section B-B Top of Plate Bottom of Plate ksi ksi Hand Calculations STAAD Model Table 5: Comparing stresses for Vertical Section B-B of gusset plate L16 Qualitatively, the STAAD model yields results that match those of the hand calculations. However quantitatively there are differences, especially in section A-A. The difference in the stress values for the Section A-A model is attributed to local effects due to the

37 26 support conditions. It is also noted that when the forces in members B and D are in tension, as they are in Figure 9, they have a tendency to want to become parallel, creating a lower tensile area in the right side of the gusset plate along Section A-A (between members B and D). This secondary effect is not accounted for in the hand calculations and would be an area for consideration in future study. Figure 9: Stress contours on Gusset Plate L16 from STAAD finite element model The model for evaluating Section B-B provides stresses that are in general agreement with the hand calculations. Also of note is the distribution of the stresses in the gusset plate. The larger stresses are found to occur at the edges of the cut section and reduce substantially towards the center of the plate. See Figure 9 for stress contours on the gusset plate.

38 27 After the initial FE analysis was done on the gusset plate, the model was modified to account for the section loss in the gusset plate that was documented in the latest available bridge inspection report. Inspection photos reveal that the typical corrosion on the plate occurs just above the bottom chord members, as can be seen in Figure 10. Based upon a review of this information, the gusset plate elements just above the limit of the splice plates were reduced in thickness from 5/8 to 1/2. The model was reanalyzed and it is found that the section loss raises the stresses in the gusset plate by approximately 20% in the area of the section loss. Figure 10: Typical section loss in Bridge A gusset plate

39 Bridge A Instrumentation Recognizing that the recommended analysis procedure includes a number of assumptions that may be overly conservative, it was decided that continuous monitoring would offer data necessary to quantitatively evaluate the actual behavior of the bridge, and allow for a more informed decision making process regarding the bridge operation and any rehabilitation needs. In April 2009, a continuous monitoring program was implemented to gather additional information on the behavior of the gusset plates through sensors installed on the representative gusset plate L16 used in the finite element analysis. 12 strain gauges were installed on various locations on and around the gusset plate. Five extensometers were installed on the truss members, one on each member just beyond the limits of the plate, and seven extensometers were installed on the plate itself at various locations of high stress, as determined by the STAAD FEA. The sensors were installed and monitored continuously for one year by Osmos USA. The yearlong monitoring cycle allowed for all seasonal variations and traffic cycles to be observed. See Figure 11 for sensor locations.

40 29 Figure 11: Sensor locations on Bridge A Gusset Plate L16 In order to manage the sheer volume of available data, the software which was used to record, view, and download the information from the bridge was programmed to save measurements that exceeded a certain threshold. The real-time data could be viewed through a web browser to allow the user to see the bridge s response while the structure was subjected to live load. Alternatively, the historical data that has been downloaded and archived can be reviewed through a program installed on the user s personal computer. The historical data can be organized and viewed in various formats, useful for comparing readings from different sensors at concurrent times. The following screen

41 30 shots depict data that was collected to compare against the results from the hand calculations and finite element model. Figure 12 shows approximately four minutes of monitoring in dynamic mode for the bridge. This information represents the results for four of the truss member sensors. Figure 12: Bridge responses recorded by sensors on Bridge A Gusset Plate L16 Figure 13 and Figure 14 below show a zoomed-in view of the five truss member sensors (four sensors in Figure 13, the fifth sensor in Figure 14) over a time period of less than one minute. The black vertical line represents the cursor function in the data program. The numbers displayed in the bottom left corner of each screen represent the strain recorded by each sensor at the time indicated by the cursor. The various colors in the bottom left corner correspond to the sensor color in the graph. The sensor name is displayed in line with the readings below the graph at the center of the screen.

42 31 Figure 13: Sensor readings before live loading event for four of the five truss members Figure 14: Sensor readings before live loading event for fifth truss member The strain values in the above figures provide a base reading against which to compare the readings from the following set of figures. It can be seen that the responses depicted

43 32 in the graphs above (Figure 13 and Figure 14) occur just before the live loading event and therefore represent the approximate sensor readings when the truss members are subjected only to dead load. Figure 15 below depicts the sensor strain readings of all five truss members at the time when the vertical truss member (green) is experiencing a peak reading. Figure 15: Sensor readings at peak strain of vertical truss member As can be seen, the peak values for each truss member do not occur at the same time, which is consistent for a truss bridge subjected to a moving load. Below are four other screen shots (Figure 16 through Figure 19) depicting the same live load event as Figure 12. In each graph, the cursor has been located at the peak value of a

44 33 different truss member sensor. Therefore, the strains recorded by all five sensors are displayed for the time period corresponding to each of these peak sensor values. Figure 16: Sensor readings at peak strain of south diagonal truss member

45 34 Figure 17: Sensor readings at peak strain of south chord truss member Figure 18: Sensor readings at peak strain of north diagonal truss member

46 35 Figure 19: Sensor readings at peak strain of north chord truss member The data from Figure 18 represented by the pink line (from the sensor affixed to the 45 degree member extending from the gusset plate to the north) suggests that there may have been loosening of the bolted connection that attaches the sensor mounting plate to the member based on the excessive vibrations. The results may not be 100% accurate, but do show the increased strain value during the live load event. The actual strains in each member were found by taking the readings of the peak values on these graphs, subtracting the value at the flat line area of the graph occurring just before the live load event, and dividing the difference by 2000 mm, which is the length of the sensors on the truss members. These strains were then converted to stresses and forces in order to be substituted into the spreadsheets created for the hand calculations. Table 6 compares the final total stresses resulting from using the sensor live load data

47 36 with the total stresses obtained from BAR7. Since it is assumed that the sensor data is only detecting live load strains, the live load stress values obtained from the sensors are added to the dead load stresses calculated in BAR7. Section Location on Plate A-A B-B Sensor Data SC Peak S45 Peak VM Peak N45 Peak NC Peak BAR7 HS20 Left Side of Plate Right Side of Plate Top of Plate Bottom of Plate Table 6: Comparison between hand calculation results using the sensor data and the BAR7 data P82 From the data that has been obtained, it appears that the actual loads and strains experienced by the bridge are significantly less than the hand calculations would predict. The stresses calculated from the sensor data appear to be at most about 75% of the stresses calculated using the envelope forces in BAR7. When comparing the live load forces alone from the sensors to the live load forces from BAR7, the live load forces seen by the sensors are much smaller than those calculated from BAR Bridge A Conclusions The hand calculation analysis of the Bridge A gusset plates reveal only one location with a Demand/Capacity Ratio greater than 1.0, which is at Gusset Plate U13 where the D/C Ratio is A finite element analysis of the Gusset Plate L16 was performed, and the resultant maximum principal stress is found to be 3% above the allowable value. The finite element analysis of the L16 plate indicates that a 20% loss in plate thickness

48 37 occurring just above the bottom chord, which is typically where the gusset plate section loss occurs on the Bridge A structure, results in a 20% increase in stress at the reduced area. However, these stresses are still below the yield strength of the material. The results of the analysis indicate that the gusset plates that do not exhibit significant section loss have adequate capacity to support the current dead load and design live loads on the bridge. Instrumentation of the bridge provides more data regarding the actual state of stress of the gusset plates on Bridge A. Since the actual strains and resulting stresses/forces are far below those obtained from both the hand calculations and FE model, it can be concluded that the structure has adequate capacity.

49 38 CHAPTER 4. MODEL DEVELOPMENT 4.1 Creating a Model in Abaqus In order to perform a more refined analysis of gusset plates in a typical Warren deck truss, multiple steps must be taken beyond the above discussed hand calculations and simple FEM. As a first step, it is decided that a more comprehensive finite element model program should be used. Abaqus is the program chosen to advance the gusset plate analysis. A similar gusset plate to the one that was used in the previous FE model is used for the Abaqus model. However, since the Abaqus model uses live loads measured on Bridge B (discussed later in this paper), a high-loaded gusset plate from the truss on that bridge (Panel Point L10) is chosen for the Abaqus FEM. In order to improve upon the simple FEM developed in the initial analyses, the Abaqus model is created as a 3D model. Given the complicated shape of gusset plates, it is decided that the Abaqus CAE will be used to develop the model. As stated on the Simulia website, With Abaqus/CAE you can quickly and efficiently create, edit, monitor, diagnose, and visualize advanced Abaqus analyses. The intuitive interface integrates modeling, analysis, job management, and results visualization in a consistent, easy-to-use environment that is highly productive. Abaqus/CAE supports familiar interactive computer-aided engineering concepts such as feature-based, parametric modeling, 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. With the visualizations and multiple manipulation tools, it is easy to create a more complex model.

50 39 Figure 20: Example gusset plate for detailed Abaqus finite element model Abaqus defines its models beginning with parts. The gusset plate model being created in this step of the analysis is based off of the shop drawing shown in Figure 20 above and consists of just one part: the gusset plate. The gusset plate is approximately 73.5 wide by approximately 45.1 tall and is 5/8 thick. At one point, it was considered to refine this model compared to the previous one by modeling the rivet holes in the gusset plate. There are a total of 125 rivets that connect the gusset plate to the truss members. Each of the rivet holes are 1 1/6 in diameter for 1 rivets. Each one of the holes for these rivets could have been included in the gusset plate. However, since in the actual field condition the rivets effectively fill out the voided area of the plates, it was decided that the rivet holes would not be included.

51 40 After each of these parts are modeled and input into Abaqus, the next step is to create a material for the plates, the type of material being steel. In Abaqus, the density is input as kips per cubic inch. The grade of steel for Bridge B (as well as many other similar truss bridges) is Grade 36 (36ksi yield strength). Therefore, this yield strength is input into the Abaqus model. Elastic material properties are then input into the program for the material. A Young s Modulus of 29,000 ksi is used, as well as a Poisson s Ratio of 0.3. This material is then applied to the parts of the model through the use of sections. A section is created as a solid, homogeneous type with the steel material previously defined. The next step to the model development is to create an assembly. The assembly function in Abaqus uses instances of the parts created in order to create a completed model. There can be more than one instance of a part, and any changes made to the part are made to the instance automatically. In the model under discussion here, only one instance of the plate part is used in the assembly. In actuality, these kinds of gusset plate connections are typically double gusset plates. This means that there are symmetrical gusset plates on either side of the truss members. However, since it is assumed that these gusset plates would carry the same stresses as each other on either side of the truss, it is decided that only one gusset plate will be modeled and simply half of the loads felt by the truss members will be transferred to the gusset plate model. After the assembly is positioned correctly, the steps for the model run are created. For this model, three steps are created. The first step, called the Initial step, is created

52 41 automatically for every model developed in the Abaqus CAE. This step applies the boundary conditions, which will be discussed below. The second step created is called the Contact step. This step establishes the contact for the loads carried by the truss members under truck live loading. The third and final step is called the Load step. This step applies the loading itself in iterative steps as defined in the input. Next, the boundary conditions are applied to the model assembly. It is decided that the nodes at the bottom of the vertical truss member will function as the pinned supports for the plate with rotation allowed in all directions, but no translation allowed. After boundary conditions are established, the individual part is meshed to create the finite elements that are to be analyzed during the model run. The first step to the meshing function is to seed the part. For the gusset plate, a maximum deviation factor of 0.1 is tried to limit the size of the finite elements. An approximate global size of 5 is input to accompany the deviation factor. Then, the mesh controls are established. The element shape tested is a Wedge, or a six-node linear triangular prism. This is chosen since the 2D STADD model had used a triangular plate element. This results in an appropriately sized mesh with similarly sized elements in a sweep across the plate that will both give good resolution to the model, but will not take an unreasonably long time to run. Defining the mesh is the last main step in the development of the gusset plate finite element model. The next step is to analyze the truss model developed by the research team at Rutgers, The State University of New Jersey, for Bridge B.

53 Bridge B Research and Model Development As discussed previously in the Literature Review, a team of researchers at Rutgers University performed tests and analysis to determine the cause of cracking in the deck of what is here referred to as Bridge B. As part of this effort, a detailed 3-D finite element model was created to help process the results and conclusions. The model used beam and shell elements. The model was validated using results from field tests that were performed on the bridge. These tests were performed using a test-truck of known axle weights and consisted of taking measurements through sensors installed on the bridge, which included a portable Weigh-in-Motion (WIM) system and two piezo-axle sensors connected to a data collection unit. The finite element model was developed to examine the behavior of the bridge structure at various loading stages. Just as was the decision for the gusset plate model described in the previous section, Abaqus was used for developing the model of Bridge B. The program was chosen here because of its vast materials and elements library that is suited for civil engineering applications. Figure 21 shows part of this full truss model.

54 43 Figure 21: Finite element model of Truss Spans 25, 26, and 27 in Bridge B (Nassif et al. 2007) Various element types were used to model the bridge. The various element types are described in detail. Moreover, the description of the boundary conditions, loads, and constraints are also detailed in the following paragraphs. The beam element is used to assemble the trusses, floor beams, and stringers. It is a onedimensional line element that cannot deform in its own plane; under bending the plane sections remain plane. Two types of beam elements were chosen for the analysis: twonode, linear beam (B31) and three-node, quadratic beam (B32) elements (Figure 22a&b respectively). Both beam elements were modeled in spaces with six degrees of freedom at each node. Abaqus also includes an I-beam section in the beam element cross-section library. The advantage of using the cross-section library is that the moment of inertia and

55 44 torsional rigidity are automatically calculated. The user only needs to input the dimensions of the I-beam. (a) Figure 22: Integration point of (a) two-node, linear beam (B31) and (b) three-node, quadratic beam (B32) elements along the length of the beam (Abaqus 2010) (b) The shell element is used to model the concrete slab on the bridge. It was used because the concrete slab has one dimension that is significantly smaller than the others (i.e., thickness of the slabs is smaller than its width and length). Abaqus contains a vast library of shell elements, but the most common and general type of shell element is the fournode shell element (S4). This element is a fully integrated, general purpose, finitemembrane-strain shell element that allows in-plane bending (Abaqus 2010). The S4 element has six degrees of freedom at each node. Figure 23 shows S4 element.

56 45 Figure 23: Four-node (S4) shell element (Abaqus 2010) Bridge piers and abutments were idealized using boundary conditions to represent the actual bearings used in the field. Piers and abutment were assumed not to be affected by the live load (i.e., no settlement or side-sway) in the FEM model. The bridge model consists of multiple parts that needed to be joined together to construct the entire bridge structure. This is achieved using constraint elements, specifically a multi-point constraint (MPC). In Abaqus, there are predefined MPCs, including BEAM and PIN. The BEAM MPC provides a rigid beam between two nodes to constrain the displacement and rotation at the first node to the displacement and rotation at the second node (Abaqus 2010). It is mainly used for constraining the slab nodes to the stringer nodes for composite action. For non-composite or zero moment connection, such as the connection between the stringers and floor beams, PIN MPC is used. PIN MPC provides a pin connection between two nodes.

57 46 In addition to the constraints, there were some members that shared the same nodes (e.g. the diaphragms and the stringers). Abaqus assumes a rigid connection if the same initial or terminal node of two elements is used. Thus, to model the diaphragm connections, the rotation of the starting and ending nodes of the diaphragms (that are connected to the stringer) needed to be released. This was done using the RELEASE commands specified by Abaqus. Three different types of steel properties were used in the finite element model: structural steel, reinforcing steel, and prestressing steel. The structural steel (I-girder and diaphragms) is subdivided into two grades: A36 carbon steel and A572 high-strength, low-alloy carbon steel. The A36 carbon steel has a minimum yield strength of 36,000 lb/in 2, where the ultimate strength varies between 58,000 lb/in 2 to 80,000 lb/in 2. The A572 high-strength, low-alloy carbon steel has a minimum yield strength of 50,000 psi, where the ultimate strength varies between 70,000 lb/in 2 to 100,000 lb/in 2. A36 carbon steel was used in most older bridges. A572 high-strength, low-alloy carbon steel is used for newly constructed bridges. Figure 24 shows a typical stress-strain curve of the two grades of steel used in the FE model.

58 47 Figure 24: Typical stress-strain curve of structural steel (Salmon and Johnson 1996) Depending on the age of concrete, the deck slab typically has a design compressive strength ranging from 4,000 lb/in 2 to 6,000 lb/in 2. The compressive strength of the deck slab was assumed to be 5,000 lb/in. 2. As mentioned earlier, the modulus of elasticity and Poison s ratio need to be specified in the model for elastic analysis. Unlike steel, the modulus of elasticity of concrete varies significantly with compressive strength, types of aggregates, paste content, and admixture. For simplicity, a relationship between the modulus of elasticity and compressive strength has been established. The American Concrete Institute (ACI) Building Code (ACI 318 Article 8.5.1, 2005) gives the modulus of elasticity, E c, as follows:

59 48 E c 33w c 1.5 f c for 90 w c 155 lb/ft 3 (7) or for normal-strength concrete: E c 57,000 f c (8) where, w c and f c are the unit weight (lb/ft 3 ) and compressive strength (lb/in. 2 ) of concrete, respectively. The tensile strength of concrete was also considered in the FEM model. A good approximation of the tensile strength of concrete is 10% to 20% of the compressive strength (Nawy, 2005). However, if subjected to bending, the modulus of rupture rather than the tensile strength should be used. ACI 318 Article specifies the modulus of rupture of concrete, f r, for normal-weight concrete as follows: f 7. 5 (9) r f c The FE model was validated by comparing it to both the static and dynamic field load tests. The FE model was validated with the static load test results by doing the following: A 3-axle dump truck with a gross vehicle weight (GVW) of 67 kips was positioned at the center of S8 (Stringer 8) (i.e., the left and right wheels of the truck were evenly distributed to the north and south of S8). A diagram depicting the location of S8 on the bridge can be seen in Figure 37 below. The test was controlled and isolated from other trucks traveling over the bridge. It was also unaffected by the dynamic impact factor since the test-truck was moving at a relative low speed (<10 mph).

60 49 Figure 25 and Figure 26 show the comparison of stresses in S5 through S10 from the field test results and the FE model for static load tests 1 and 3, respectively. In the figures, the field test data is denoted by EXP and represented with a red solid line, and the FE model is denoted as FEM with a blue dashed line. Overall, the FE model correlated well with the field test results with variations within 15% of the field test results. The FE model does provide an accurate stress-strain calculation and represents the actual bridge very well.

61 Figure 25: Comparison of stresses in S5-S10 using the FE model and Static Load Test 1 (Nassif et al. 2007) 50

62 Figure 26: Comparison of stresses in S5-S10 using the FE model and Static Load Test 3 (Nassif et al. 2007) 51

63 52 The dynamic load tests were also used for validating the FE model. The dynamic field tests were conducted using the actual truck traffic traveling on the bridge. Three dynamic load cases were used for the comparison. These cases consisted of three 5-axle trucks with gross vehicle weights of 65, 55, and 42 kips. Figure 27 and Table 7 show the configuration of the most common truck used for the FE model. Figure 28 through Figure 33 illustrate the comparison of the dynamic load test of the 5- axle trucks with GVW of 65 kips for S5 through S10, respectively. Overall, the FE model correlated well with the field test results for the maximum stresses, having only a 2% variation. At lower stresses, especially over S8, S9, and S10, the variation is significantly high, which could have been for multiple reasons A B C D Figure 27: Standard truck configurations used in the calibration of the finite element model (Nassif et al. 2007)

64 53 Truck GWV (kips) 65.2 Axle 1 (kip) 9.2 Axle 2 (kip) 13.3 Axle 3 (kip) 12.4 Axle 4 (kip) 15.1 Axle 5 (kip) 15.2 Spacing A (ft) 17.4 Spacing B (ft) 4.3 Spacing C (ft) 35.9 Spacing D (ft) 4.1 Table 7: Truck configuration (Nassif et al. 2007) Figure 28: Comparison of stresses in S5 using the FE model and the actual field-test data of a 5-axle truck with a GVW of 65 kips traveling WB in Lane 1 (Nassif et al. 2007)

65 54 Figure 29: Comparison of stresses in S6 using the FE model and the actual field-test data of a 5-axle truck with a GVW of 65 kips traveling WB in Lane 1 (Nassif et al. 2007) Figure 30: Comparison of stresses in S7 using the FE model and the actual field-test data of a 5-axle truck with a GVW of 65 kips traveling WB in Lane 1 (Nassif et al. 2007)

66 55 Figure 31: Comparison of stresses in S8 using the FE model and the actual field-test data of a 5-axle truck with a GVW of 65 kips traveling WB in Lane 1 (Nassif et al. 2007) ) i s k ( s e s s e r t S S9-EXP S9-FEM Time (1/100 s) Figure 32: Comparison of stresses in S9 using the FE model and the actual field-test data of a 5-axle truck with a GVW of 65 kips traveling WB in Lane 1 (Nassif et al. 2007)

67 56 ) i s k ( s e s s e r t S S10-EXP S10-FEM Time (1/100 s) Figure 33: Comparison of stresses in S10 using the FE model and the actual field-test data of a 5-axle truck with a GVW of 65 kips traveling WB on Lane 1 (Nassif et al. 2007) Multiple simulations representing various load cases were made using the FE model. Two actual trucks obtained from the portable WIM system were used for the simulations: 78.7 kip, 4-axle and 50 kip, 3-axle dump trucks. These types of trucks cause the highest stress range and also represent approximately 20% of the average daily traffic. Multiple simulations were performed with these two truck types: Loading the WB left lane with a 78.7 kip, 4-axle dump truck Loading the EB left lane with a 50 kip, 3-axle dump truck Loading the WB right lane with a 78.7 kip, 4-axle dump truck Loading the WB lanes with two 78.7 kip, 4-axle dump trucks side-by-side

68 57 Loading the WB left lane with a 50 kip, 3-axle dump truck Loading the EB left lane with a 50 kip, 3-axle dump truck Two impact factors, 1.33 and 1.5, are used in the analyses for trucks traveling WB and EB, respectively. The 1.33 impact factor is based on dynamic test results as well as the recommendation of the AASHTO LRFD Standard Specification. It was noted that the observed impact factor of dynamic test-trucks traveling EB was as high as 2.0. However, a conservative value of 1.5 was used since the dynamic impact factor from heavier trucks will be lower and will vary from truck to truck. 4.3 Model Integration In order to complete the final steps of the analysis for this thesis research, the individual gusset plate finite element model that was developed based on the Bridge B as built drawings is integrated into the truss model developed by the Rutgers team described in the previous section. This allows the stresses in the gusset plate to develop under actual loading conditions in a calibrated model. As a first step, it is decided to convert the 3D model into a 2D shell element in order to more closely transition to the 1D beam elements used for the truss members. The Abaqus CAE model for the gusset plate is used to export an input file to define the coordinates of all of the points in the gusset plate FE mesh. The coordinates from one side of the 3D gusset plate are then added as new nodes into the truss model with the appropriate offsets to the base coordinate system in the truss bridge model. The gusset plate coordinates are

69 58 integrated into the truss model at 4 symmetric locations, two on each truss, where this type of gusset plate is located on the bridge. The elements are then created between each node by copying the element definitions from one side of the gusset plate model. The carbon steel material used for some of the members in the truss is applied to the integrated plate. The thickness of each element in the plate is then defined. In the areas connected to truss members, the thickness is increased to account for the two gusset plates as well as the truss member. In the areas in between, the thickness is simply the two gusset plates. In order to insert the gusset plate into the truss, some sections of the truss member are removed around the associated node. Then the connection between the remaining truss members and the nodes at the corresponding edge of the plate are established by using the same node for both the end of the member and the center of the plate edge. A kinematic coupling restraint is also established between the connector node and the adjacent node on the plate edge to establish that the whole edge of the plate at the truss member would move as one. Figure 34 below shows the full bridge model with gusset plate integration. This figure also displays the stress results of the bridge being loaded with a heavy live load, the results of which will be discussed in the next section.

70 59 Figure 34: Bridge B full truss model with gusset plate integration (red circles) in Abaqus Now the model is ready to be loaded. The test live load case shown in Figure 35 below is used on the new combined model as well as the original truss bridge model without the gusset plates. Both models are run with the live load and the results are compared to validate that the gusset plates in the new model do not significantly affect the outcome compared to the original model.

71 60 August/Sept Test-truck 3-axle single body dump truck Gross Vehicle Weight = 53.7k Axles Weights 15.5k 19.1k 19.1k Spacing ft 5.0 ft Figure 35: Test-truck configuration (top) and information (bottom) for controlled load tests (Nassif et al. 2007) After consulting the results from the Rutgers study, the node corresponding to the location of the sensor on S6 (as shown in Figure 36 and Figure 37) in both models is chosen to generate the validation data, since this has the highest responses from the dynamic tests.

72 61 Figure 36: Under-deck view of Span 26 Bay 1 between FB11 and FB12 (Nassif et al. 2007) Note: rectangles represent strain transducers Toward River 6534 S S Top S Bot Top 6536 Bot. S S S6 S S4 Pier 25 FB10 FB11 FB12 S1 FB9 Bay 4 Bay 3 Bay 2 Bay 1 End of 4 span stringer Bottom flange only Top & Bot Flange S3 S2 LVDT vert. or horizontal Figure 37: Span 26 sensor layout involving 16 strain gauges and 4 LVDTs (Nassif et al. 2007)

73 62 The results from the integration points at the bottom of the stringer S6 in both models are shown in Figure 38 below. Figure 38: Comparison of Abaqus FEM results at Sensor 6 location with and without gusset plate integration As can be seen, the results are nearly identical. The models are also compared with respect to the response of the truss members immediately around the gusset plate location. The following images (Figure 39) show the responses of these truss members with and without the plate integrated into the model.

74 63 Member A w/plate Member A w/o Plate Member B w/plate Member B w/o Plate Member C w/ Plate Member C w/o Plate Member D w/plate Member D w/o Plate Member E w/plate Member E w/o Plate Figure 39: Comparison of FEM results at adjacent truss members with and without gusset plate integration

75 64 In general, the results of these comparisons show that the member stresses with or without the gusset plates are similar. The various lines on each chart are the different integration points within the section of the member. There is some difference in the magnitude of the stresses for Member B (horizontal), though the general response shape is the same and is deemed to be similar enough to continue with the model including the plate. This allows us to follow through using the new model to start analyzing the gusset plate stresses under various live loads.

76 65 CHAPTER 5. PARAMETRIC STUDY 5.1 Varying Plate Thickness In this step of the research, a parametric study is conducted to compare the gusset plate responses under various conditions. The first step is to simply see how the response of the gusset plate will change under two lanes of the test dump truck live load that was used in the static analysis of Bridge B with varying plate thickness. The graph also shows the relationship of the gusset plate stress to thickness under two lanes of the AASHTO defined HL-93 standard design live loading. According to as-build drawings of Bridge B, the test gusset plates chosen for this analysis are each 5/8 thick. In each separate finite element run, the thickness is decreased by an additional 1/16 down to 5/16 each, which is the minimum thickness for any steel members, as defined in the AASHTO Bridge Design Specifications. The results of this parametric study are shown in Figure 40 below.

77 66 Figure 40: Chart graphing plate stress vs. plate thickness As would be expected, the stress in the plate increases as the plate thickness decreases under both live loading cases. These graphs follow power trends, approaching infinity when the gusset plate thickness approaches zero (0.0). It can be seen in the graph that the HL-93 loading case is the far more critical case for this type of comparison. And although the stresses for both live loads increase, they do not reach a critical level for steel with a yield strength of 36ksi, even at the minimum plate thickness. This is considered a good result, since it is undesirable for gusset plates to approach failure under any live loading. Gusset plates are typically designed such that they are not the most critical members on a bridge, as is the case with any connection point between main bridge members.

78 Varying Live Load The second parametric study that is performed for this research involves using the original integrated FEM with the as-build gusset plate thickness and varying the live load according to the WIM data that was collected by the Rutgers team during the Bridge B Deck Evaluation. The test dump truck is the first and smallest load applied. However, instead of running one lane of the load down the center of the bridge model, two lanes of the live load are placed along the edge of the deck, with the first lane located approximately 2-0 from the edge of the parapet, and the second lane located 10 feet from the first, as per AASHTO standard specifications. The next largest live load that is tested is an HS20 AASHTO design live load. Again, two lanes of the load are placed on the bridge at the same location as the dump truck case. The third live load that is used is the 78.7-kip Short Heavy Vehicle recorded by the WIM data in the Rutgers study. This truck is coupled with a second lane of the test dump truck. The fourth load is an approximation of the heaviest load measured by the Rutgers WIM system. This is a kip, 6-axle vehicle. The spacing of the wheels is assumed to be approximately 5 feet between each of the back 5 axles under a heavy load and an approximately 16 between the front axle and the first of the back axles. The distribution of the weight is assumed to be 15.8 kips on the front axle and 18 kips on each of the back axles. This truck is then also paired with a second lane of the dump truck. The final and heaviest live load used for this study is a Permit load, representing the largest legal live load allowed on the bridge. This load is coupled with the AASHTO HS20 truck in the second lane to represent the most probable configuration of permit live loading on a bridge per

79 68 AASHTO Bridge Design Specifications. The spacing between and load on each of the axles for all of the above mentioned live loads are listed in the table below. LL Case Test Dump Truck HS20 SHV Max WIM NJ Permit PA Permit Axle 1 Load (kips) Space (ft) Axle 2 Load (kips) Space (ft) Axle 3 Load (kips) Space (ft) Axle 4 Load (kips) Space (ft) Axle 5 Load (kips) Space (ft) Axle 6 Load (kips) Space (ft) Axle 7 Load (kips) Space (ft) Axle 8 Load (kips) Table 8: Configuration for various trucks used for live loading in model (italics indicate estimations) After each of these live load cases are created and the FE models are run for each case, the results are graphed on the chart in Figure 41 below. The results shown are the Tresca

80 69 stresses in the node with the maximum stress in the gusset plate, which happens to be at the edge of the plate next to the vertical truss member. Figure 41: Results of varying live load on a gusset plate on Bridge B The results of this parametric study comparison are as would be expected for the respected live load cases. The test dump truck, which is the lightest of the vehicles produces the smallest stresses, with the maximum stress (when the centroid of the truck is placed over the location of the gusset plate) being 3.41kips. The HS-20 live load case and the 4-axle short heavy vehicle produce very similar results, which makes sense since the loads of these trucks are less than 10% different from each other. However, the

81 70 second lanes for these live load cases are more significantly different. The HS20 second lane is another HS-20 truck, whereas the SHV second lane is the test dump truck, which is only 53.7 kips, compared to the 72 kip HS20. Despite this difference, the stress results still come out similarly, with the maximum stress for the HS20 being slightly higher. This could indicate that a shorter vehicle which fits entirely between two stringers on a truss bridge could have a similar or possibly even more critical reaction in gusset plates than a longer vehicle with a larger load. The load case with the next largest stress is the heavier vehicle with a longer assumed total length. When comparing this longer vehicle with the short heavy vehicle (both with the test dump truck in the second lane), a 20% increase in the total live load on the bridge results in an increase in stress of only 11%. This again indicates that the length of the vehicle can have an inverse effect on the gusset plate stress. However, it does appear that the effect is not so great as to cause concern about using the HS20 vehicle vs. anything much shorter than that. Especially when all of these loading cases are compared to the Permit load, also specified by AASHTO to be used for design of bridges. The Permit truck produces a peak stress that is more than 50% larger than the next largest peak stress. Although in the AASHTO design specifications these types of Permit loads are scaled down compared to a more typical HS20 truck load, the fact that these trucks are used for the design of bridges indicates that most of the largest stresses experienced by gusset plates due to live load are being covered in current designs.

82 Validating Integrated Plate Model One final comparison of the FEM results in order to validate the models used to analyze gusset plates in the future is to compare the results of an individual plate model with the results from the plate shell element integrated into a full truss model. To do this, the stresses in the truss elements of the full bridge model without the gusset plates are found and converted to forces. Then these forces are applied as pressure uniformly to the edges of the plate within the limits of the truss member width. Figure 42 and Figure 43 below show the gusset plate stress distribution on the gusset plate in the truss model and the 3D individual plate model, respectively. Figure 42: Gusset plate in full bridge model stress contours from Abaqus

83 72 Figure 43: Individual 3D gusset plate model stress contours from Abaqus At first glance, these results look very different, but when analyzed more closely, they seem to be much more similar than may be first assumed. The most obvious difference between the two is the added thickness of the plate in the bridge model to account for the truss members that were removed from the original Rutgers bridge model. These locations of the gusset plate model will not experience nearly as large of a stress as the individual model will. It is probably most accurate from a tension/compression stress standpoint that the gusset plate would not fail where it is closely connected to the truss member. Therefore, we can focus mostly on the other locations within the individual model.