Computer Modeling of the Proposed Kealakaha Stream Bridge

Transcription

1 Computer Modeling of the Proposed Kealakaha Stream Bridge Jennifer B.J. Chang Ian N. Robertson Research Report UHM/CEE/03-03 May 2003

2

3 ABSTRACT The studies described in this report focus on the short-term structural performance of a new replacement Kealakaha Bridge scheduled for construction in Fall A new three span, 220-meter concrete bridge will be built to replace an existing six span concrete bridge spanning the Kealakaha Stream on the island of Hawaii. During and after construction, fiber optic strain gages, accelerometers, Linear Variable Displacement Transducers (LVDTs) and other instrumentation will be installed to monitor the structural response during ambient traffic and future seismic activity. This will be the first seismic instrumentation of a major bridge structure in the State of Hawaii. The studies reported here use computer modeling to predict bridge deformations under thermal and static truck loading. Mode shapes and modal periods are also studied to see how the bridge would react under seismic activity. Using SAP2000, a finite element program, a 2-D bridge model was created to perform modal analysis, and study vertical deformations due to static truck loads. A 3-D bridge model was also created in SAP2000 to include the horizontal curve and vertical slope of the bridge. This model is compared with the 2-D SAP2000 model to evaluate the effect of these and other parameters on the structural response. In addition, a 3-D Solid Finite Element Model was created using ANSYS to study thermal loadings, longitudinal strains, modal analysis, and deformations. This model was compared with the SAP2000 model and generally shows good agreement under static truck loading and modal analysis. In addition, the 3-D ANSYS solid finite element model gave reasonable predictions for the bridge under thermal loadings. These models will be used as a reference for comparison with the measured response after the bridge is built. iii

4 ACKNOWLEDGEMENTS This report is based on a Masters Plan B report prepared by Jennifer Chang under the direction of Ian Robertson. The authors wish to express their gratitude to Drs Si- Hwan Park and Phillip Ooi for their effort in reviewing this report. This project was funded by the Hawaii Department of Transportation (HDOT) and the Federal Highway Administration (FHWA) program for Innovative Bridge Research and Construction (IBRC) as part of the seismic instrumentation of the Kealakaha Stream Bridge. This support is gratefully acknowledged. The content of this report reflects the views of the authors, who are responsible for the facts and the accuracy of the data presented herein. The contents do not necessarily reflect the official views or policies of the State of Hawaii, Department of Transportation, or the Federal Highway Administration. This report does not constitute a standard, specification or regulation. iv

5 TABLE OF CONTENTS Abstract. Acknowledgements Table of Contents.. List of Tables. List of Figures iii iv v vii viii Chapter 1 INTRODUCTION Project Description Project Scope 5 Chapter 2 DESIGN CRITERIA FOR KEALAKAHA BRIDGE Geometric Data Linear Soil Stiffness Data Material Properties Boundary Conditions of Bridge Bridge Cross Section 11 Chapter 3 SAP2000 FRAME ELEMENT MODELS Development of SAP2000 Frame Element Models Element Sizes used for SAP2000 Models Results of Frame Element Model Comparisons Natural Frequencies Static Load Deformations.. 18 Chapter 4 ANSYS SOLID MODEL ANSYS Solid Model Development Finite Element Analysis: ANSYS, an Overview Solid Model Geometry Development of Solid Model Geometry Meshing in ANSYS Test Beam: Determining Finite Element Type and Mesh for Thermal Loading Analytical Solution For Test Beam Comparison of ANSYS to Theoretical Result: Thermal Loading Comparison of ANSYS to Theoretical Result: Static Point Loading Mesh Generation for Kealakaha Bridge Model Convergence of 4 Meter Mesh.. 42 Chapter 5 ANSYS SOLID MODEL ANALYSIS Truck Loading Conditions Truck Loading Results Single 320 kn (72 Kip) Point Load Distributed Single Truck Load x2 Truck Loading.. 50 v

6 Truck Loading Creating Torsion Effects 52 Chapter 6 TEMPERATURE ANALYSIS Temperature Gradient Results of Temperature Gradient Strain Distribution. 64 Chapter 7 MODAL ANALYSIS Modal Periods Modal Periods: 2-D vs. 3D Models Modal Periods: Gross Section vs. Transformed Section Modal Periods: Linear Soil Spring vs. Fixed Support Modal Periods: SAP2000 vs. ANSYS Mode Shapes. 70 Chapter 8 CONCLUSIONS AND SUMMARY Summary Conclusions Sources of Possible Error Suggestions for Further Study.. 81 References.. 83 Appendix A Model Input Data 85 Coordinates of SAP D Model.. 85 Coordinates of SAP D Model.. 86 SAP2000 Cross Section Properties. 88 Material Properties used in SAP ANSYS Solid Model Coordinates 90 ANSYS Solid Model Cross-Section Depths 91 vi

7 LIST OF TABLES 2.1 Kealakaha Bridge Geometric Data Linear Soil Stiffness Data Comparison of Vertical Deflections For Fixed Support Comparison between Fixed Supports and Soil Springs Vertical Deflection at Midspan on Test Beam: Thermal Loading Vertical Deflection at Midspan on Test Beam: 10 N Point Load Comparison between Four and Six Meter Mesh for ANSYS Model Results of Single 320 kn Truck Point Load Vertical Deflection at Center of Bridge due to Single Truck Load (Actual Wheels Modeled) Vertical Deflection of Bridge due to 2x2 Truck Load (Actual Wheels Modeled) Vertical Deflection of Bridge due to 4 Truck Loading at Edge of Bridge (Actual Wheels Modeled) Vertical Deflection due to Temperature Gradient Modal Periods: 2-D vs. 3D Modal Periods: Gross Section vs. Transformed Section Modal Periods: Linear Soil Spring Support vs. Fixed Supports Modal Periods: SAP2000 vs. ANSYS 69 vii

8 LIST OF FIGURES 1.1 Location of Project Elevation, Section and Plan of Kealakaha Bridge UBC 1997 Seismic Zonation Horizontal Ground Acceleration (% g) at a 0.2 Second Period with 2% Probability of Exceedance in 50 Years Horizontal Ground Accelerations (% g) at a 0.2 Second Period with 10% Probability of Exceedance in 50 Years Lateral Stiffness (Longitudinal Direction) Lateral Stiffness (Transverse Direction) Rotational Stiffness (Longitudinal Direction) Rotational Stiffness (Transverse Direction) Design Cross Section of Kealakaha Bridge SAP D Frame Element Model (Schematic) SAP D Frame Element Model (Screen Capture) SAP D Frame Element Model (Schematic) SAP D Frame Element Model (Screen Capture) Element Lengths in SAP2000 Models Convergence of Original and Half Size Finite Elements Schematic Drawing of a Single HS20 Truck Load Single HS20 Truck Load used in Chapter Deformed Shape due to Single Truck Load Comparisons Between 2-D and 3-D Model Comparison of Gross and Transformed Section Properties for 2-D Model Results Comparison of Gross and Transformed Section Properties for 3-D Model Results Difference Between Fixed Support and Soil Springs: 2-D Model Difference Between Fixed Support and Soil Springs: 3-D Model Side View of a Portion of the Kealakaha Bridge Design Cross Section Simplified Cross Section ANSYS Solid Model Cross Section View before Meshing Kealakaha Bridge before Meshing, Elevation Kealakaha Bridge before Meshing, Isometric View Solid 45, Eight Node Structural Solid (ANSYS) Solid 92, Ten Node Tetrahedral Structural Solid (ANSYS) Square Test Beam Thermal Loading Thermal Distribution in Test Beam Test Beam Deflection under 10 C Temperature Gradient (Auto Mesh) Square Test Beam Point Loading Four Meter Mesh Size, Kealakaha Bridge (Part of Bridge) Six Meter Mesh Size, Kealakaha Bridge (Part of Bridge) Convergence of Four and Six Meter Mesh for ANSYS Model Distribution of Truck Loads.. 45 viii

9 5.2 ANSYS Layout of Single Truck Point Load SAP2000 vs. ANSYS, Single Truck Point Load Viaduct Section Showing Single Truck Load Layout of Wheel Placement for Single Truck SAP2000 vs. ANSYS, Single Truck Modeled with Wheels Location of Axle Loads for the 2x2 Truck Configuration Viaduct Section showing 2x2 Truck Configuration ANSYS Placement of 2x2 Truck Load SAP2000 vs. ANSYS, 2x2 Trucks Modeled with Wheels Location of Axle Loads for Four Trucks in a Row Viaduct Section showing Four Trucks in a Row ANSYS Layout of Four Trucks in a Row Deflected and Non-Deflected Cross Section Torsion Effects, Four Trucks in a Row Isometric View of Vertical Deflection under Torsion Loading ANSYS Applied Temperature Gradient Bridge End Span Showing Effect of Thermal Gradient Deformation due to 10 Degrees Temperature Gradient Isometric View of Bridge Deformation due to Thermal Loading Side View of Bridge Deformation due to Thermal Loading Locations of Reported Deformation due to Thermal Loading Vertical Deflection of Bridge due to Ten Degree Temperature Gradient Combination of Temperature and Truck Loading Strain Distribution through Box Girder Depth near Pier Strain Distribution through Box Girder Depth near Midspan Strain Output Locations Longitudinal Strains at Locations A and B Longitudinal Strains at Locations C and D ANSYS Mode SAP2000 Mode ANSYS Mode SAP2000 Mode ANSYS Mode SAP2000 Mode ANSYS Mode SAP2000 Mode ANSYS Mode SAP2000 Mode ANSYS Mode SAP2000 Mode ANSYS Mode SAP2000 Mode ANSYS Mode SAP2000 Mode ANSYS Mode SAP 2000 Mode ix

10 x

11 CHAPTER 1 INTRODUCTION 1.1 Project Description The project site is located along Mamalahoa Highway (Hawaii Belt Road) over the Kealakaha stream in the District of Hamakua on the Island of Hawaii. The existing bridge, a six span concrete bridge crossing the Kealakaha Stream is scheduled for replacement in Fall The new replacement bridge will be built on the north side of the existing bridge and will reduce the horizontal curve and increase the roadway width of the existing bridge. The new bridge has been designed to withstand the anticipated seismic activity whereas the existing bridge is seismically inadequate. Figure 1.1 shows the location of the project on the Big Island of Hawaii. Figure 1.1: Location of Project 1

12 The new prestressed concrete bridge will be a 3 span bridge and is approximately 220 meters long and 15 meters wide and will be designed to withstand earthquake and all other anticipated loads. The new bridge will consist of three spans supported by two intermediate piers and two abutments (Figure 1.2). The center span will be a cast-inplace concrete segmental span of about 110 meters and the two outside spans will be about 55 meters resulting in a balanced cantilever system. During and after construction, fiber optic strain gages, accelerometers, Linear Variable Displacement Transducers (LVDT s) and other instrumentation will be installed to monitor the structural response during ambient traffic and future seismic activity. This will be the first seismic instrumentation of a major bridge structure in the State of Hawaii. Figure 1.2: Elevation, Section and Plan of Kealakaha Bridge 2

13 The new bridge is in an ideal location for a seismic study because of the earthquake activity on the island of Hawaii. The Island of Hawaii is in zone 4, the highest zone of seismic activity categorized in the 1997 Uniform Building Code. Figure 1.3 shows the map of the UBC 1997 Seismic Zonation for the State of Hawaii. Figure 1.3: UBC 1997 Seismic Zonation Figures 1.4 and 1.5 show the peak ground acceleration maps included in the International Building Code, IBC (2000). These maps are based on the USGS National Seismic Hazard Mapping Project (USGS 1996). The maps show earthquake ground motions that have a specified probability of being exceeded in 50 years. These ground motion values are used for reference in construction design for earthquake resistance. The maps show peak horizontal ground acceleration (PGA) at a 0.2 second period with 5% of critical damping. There are two probability levels: 2% (Fig. 1.4) and 10% (Fig. 1.5) probabilities of exceedence (PE) in 50 years. These correspond to return periods of about 500 and 2500 years, respectively. The maps assume that the earthquake hazard is independent of time. 3

14 The location of the Kealakaha bridge shows approximately 65% g with a 2% probability of exceedance in 50 years (Fig. 1.4) and 35% g with a 10% probability of exceedance in 50 years (Fig. 1.5). The acceleration due to gravity, g, is 980 cm/sec 2. Figure 1.4: Horizontal Ground Acceleration (%g) at a 0.2 Second Period With 2% Probability of Exceedance in 50 Years (USGS, 1996) 4

15 Figure 1.5: Horizontal Ground Acceleration (%g) at a 0.2 Second Period With 10% Probability of Exceedance in 50 Years (USGS 1996) 1.2 Project Scope A number of computer models of the Kealakaha Bridge were created, analyzed and compared to evaluate the structural response of the bridge to various loading conditions. All models were linear elastic simulations in either SAP2000 (CSI 1997) or ANSYS (ANSYS, 2002). 5

16 Frame element models were created in SAP2000 to determine the following: 1) Vertical deflection of the viaduct due to static truck loads. 2) Mode shapes and modal periods. 3) Effects of different degrees of modeling accuracy: a. 3-D model compared with 2-D model. b. Inclusion of linear soil stiffness properties (soil springs vs. fixed supports.) c. Inclusion of prestressing steel (transformed section vs. gross section properties.) d. Beam element size to produce convergence of results. A three-dimensional solid model was created in ANSYS to determine the following: 1) Deformation and strains of the viaduct due to thermal loads. 2) Deformation and strains of the viaduct due to truck loads. 3) Comparison of mode shapes and modal periods, and vertical deformations under truck loads, with the SAP2000 frame element models. 6

17 CHAPTER 2 DESIGN CRITERIA FOR KEALAKAHA BRIDGE The design specifications used for the Kealakaha bridge are the AASHTO LRFD Bridge Design Specification Second Edition (1998) including the 1999 and 2000 interim revisions (AASHTO, 1998). A geotechnical investigation was performed by Geolabs, Inc. in 2001 and the report was available for this study (Geolabs, 2001a).. Structural bridge data was obtained from Sato and Associates, the bridge design engineers, and from the State of Hawaii project plans titled Kealakaha Stream Bridge Replacement, Federal Aid Project No. BR-019 2(26) dated July Geometric Data The geometric data of the Kealakaha bridge are shown in Table 2.1. The bridge radius and slopes were not modeled in the 2-D SAP2000 and the ANSYS models. The bridge radius, longitudinal slope, and cross slope were included in the SAP D model. Table 2.1: Kealakaha Bridge Geometric Data Design Speed 80 km/hour Span Lengths 55 m 110 m 55m Typical Overall Structure Width m (constant width) Bridge Radius constant radius of m Bridge Deck constant cross slope of 6.2% Vertical Longitudinal Slope Vertical curve changing to a constant longitudinal slope of -3.46% 2.2 Linear Soil Stiffness Data The only geotechnical information available for this study was the data provided by Geolabs, Inc. in the project geotechnical report (Geolabs-Hawaii W.O November 17, 1998). The study was done for Sato and Associates, Inc. and the State of 7

18 Hawaii Department of Transportation. The report summarized the findings and geotechnical recommendations based on field exploration, laboratory testing, and engineering analyses for the proposed bridge replacement project. The recommendations were intended for the design of foundations, retaining structures, site grading and pavements. Geolabs, Inc. provided the design engineers with linear soil stiffness during service conditions and extreme earthquake events using the secant modulus (Geolabs, 2001). A future proposed soil investigation and a soil-structure interaction-modeling program will determine the non-linear and dynamic properties of the foundation material. Figures 2.1 to 2.4 show plots of the secant modulus used to determine these linear soil spring stiffness. Figure 2.1 shows the estimated secant modulus for lateral soil stiffness in the bridge longitudinal direction with a lateral deflection of meters and a lateral load of 18,750 kn. Figure 2.2 shows the secant modulus for the transverse direction. The rotational stiffness in the bridge longitudinal direction was determined from the secant modulus at a rotational displacement of rad and a moment of 165,000 kn-m (Figure 2.3). Figure 2.4 shows the secant modulus for the rotational stiffness in the bridge transverse direction. These stiffness values are used for the soil springs in the SAP2000 frame element models at the base of both piers. The values are shown in Table 2.2. Table 2.2: Linear Soil Stiffness Data Lateral Stiffness Longitudinal Transverse Rotational Stiffness Longitudinal Transverse kn/m kn/m kn-m/rad kn-m/rad 8

19 Lateral Stiffness (Longitudinal) Calculating Secant Modulus Data from Geolabs, Inc. 1/29/2001 Lateral Load (kn) kn/m (Extreme Event) kn/m (Service) Fitted Curve Secant Modulus Lateral Deflection (meters) Figure 2.1: Lateral Stiffness (Longitudinal Direction) Lateral Stiffness (Transverse) Calculating Secant Modulus Data from Geolabs, Inc. 1/29/2001 Lateral Load (kn) kn/m (Extreme Event) Secant Modulus Lateral Deflection (meters) Figure 2.2: Lateral Stiffness (Transverse Direction) 9

20 Rotational Stiffness (Longitudinal) Calculating Secant Modulus Data from Geolabs, Inc. 1/29/ kn-m/rad (Extreme Event) Moment (kn-m) kn/m (Service) Fitted Curve Secant Modulus Rotation (Rad) Figure 2.3: Rotational Stiffness (Longitudinal Direction) Rotational Stiffness (Transverse) Calculating Secant Modulus Data from Geolabs, Inc. 1/29/ kn-m/rad (Extreme Event) Moment (kn-m) Rotation (Rad) Secant Modulus Figure 2.4: Rotational Stiffness (Transverse Direction) 10

21 2.3 Material Properties Based on the design documents obtained from Sato and Associates, three different types of concrete were used to model the structure in the frame element models. Superstructure concrete was used for the bridge span, sub-structure concrete was used for the concrete piers and abutments, and weightless concrete was used for the dummy connectors between the pier and the bridge girder in the SAP2000 frame element models. Poisson s ratio of 0.20 was used throughout the bridge. The Elastic Modulus was taken as 2.4 x 10 7 kn/m 2 for the bridge superstructure and 2.1 x 10 7 kn/m 2 for the piers and abutments. 2.4 Boundary Conditions of Bridge For most computer models, the bases of the two piers were modeled as fully fixed. In the SAP2000 soil spring model, rotational, horizontal, and vertical linear soil springs were incorporated at the base of the piers. In all computer models, the abutments at each end of the bridge were modeled as roller supports in the bridge longitudinal direction, free to rotate about all axes, but restrained against vertical and transverse displacement. 2.5 Bridge Cross Section Figure 2.5 shows the design cross section of the Kealakaha bridge box girder. From this cross section, centroidal coordinates, moments of inertia, torsion constants, and cross-sectional areas were calculated for the SAP2000 models. All dimensions are constant throughout the length of the bridge except the box girder depth, h, and the bottom slab thickness, T. These values are listed in Appendix A for the end of each bridge segment. The cross section in Figure 2.5 is referred to as the design cross section. 11

22 Modifications were made to simplify the cross-section for the ANSYS solid model as explained in Chapter 4. Figure 2.5: Design Cross Section of Kealakaha Bridge 12

23 CHAPTER 3 SAP2000 FRAME ELEMENT MODELS 3.1 Development of SAP2000 Frame Element Models SAP2000 (CSI, 1997) was used to create the frame element models. Figures 3.1 and 3.2 show elevation, plan and isometric views of the 2-D model. This model ignores the horizontal curve, longitudinal slope and cross slope. Note that although the roadway is horizontal, the girder frame elements follow the centerline of the varying depth box girder and are therefore curved in the vertical plane. Figures 3.3 and 3.4 show elevation, plan and isometric 3-D views of the 3-D model. In the 3-D model, the horizontal curve with radius of m and the vertical curve are modeled. The vertical curve begins as a varying slope until the center of the bridge where it becomes a constant slope of 3.46 %. To model the bridge deck constant cross slope of 6.2%, moments of inertia, and centerline coordinates were recalculated for the 3-D model. 13

24 Figure 3.1: SAP D Frame Element Model (Schematic) Figure 3.2: SAP D Frame Element Model (Screen Capture) 14

25 Figure 3.3: SAP D Frame Element Model (Schematic) Figure 3.4: SAP D Frame Element Model (Screen Capture) 15

26 Eight frame element models were created based on these 2-D and 3-D geometries. 2-D frame element model (slopes and curve of bridge not considered) 1) Gross section properties neglecting the effect of prestressing steel a) Fixed Supports b) With linear soil springs at base of piers 2) Transformed section properties including prestressing steel a) Fixed Supports b) With linear soil springs at base of piers 3-D frame element model (slopes and curve of bridge included). 1) Gross section properties neglecting the effect of prestressing steel a) Fixed Supports b) With linear soil springs at base of piers 2) Transformed section properties including prestressing steel a) Fixed Supports b) With linear soil springs at base of piers 3.2 Element Sizes used for SAP2000 Models To model the varying cross section along the length of the bridge, the box girder was modeled using frame element segments. Each segment had the same section and properties. The mass of each segment was computed automatically by SAP2000 based the cross sectional area, concrete density, and frame element length. The frame element size was based on the construction segment length throughout the bridge. For the majority of the bridge length, 5.25 meter long elements were used. Three 1.5 meter long elements were used above each pier and abutment, and three 1 meter long 16

27 elements were used at the closure segment at the center of the middle span. Elements used to model the piers varied in length from 1 m to 6.45 m. Figure 3.5 shows the SAP D model. 1m m Figure 3.5: Element Lengths in SAP2000 models These element sizes were small enough to produce valid results. An analysis using finite element sizes 50% smaller produced the same deflection results under a single truck loading and the same modal frequencies. Figure 3.6 shows the results of the vertical deflection under a single truck loading. 17

28 2 Sap2000 Frame Element Model Vertical Deflection with Single Truck Loading at Center Convergence of Original and Half Size Finite Elements 2-D No Steel Model Vertical Deflection (mm) Original Size Elements Half Size Elements Along Length of Bridge (meters) Figure 3.6: Convergence of Original and Half Size Finite Elements 3.3 Results of Frame Element Model Comparisons Natural Frequencies Natural frequencies, modal periods and mode shapes were determined for the first nine modes for each of the eight SAP2000 frame element models. These results are presented in Chapter six along with those from the ANSYS analysis Static Load Deformations In order to evaluate the anticipated structural response to vehicle traffic, a number of truck loading conditions were considered. This section presents the deflected shape resulting from a single AASHTO HS20 truck located at midspan of the center span. This loading condition is used to compare the various SAP2000 models. A single truck weighs a total of 72 Kips or 320 kn. The truck scale dimensions are shown in Figure

29 Figure 3.7: Schematic Drawing of a Single HS20 Truck Load Chapter 4 shows results from modeling each axle or wheel for the HS20 loading of Figure 3.7. In this section, a single point load of 320 kn is used to represent a single truckload for comparisons of different computer modeling techniques as shown in Figure 3.8. Figure 3.8: Single HS20 Truck Load Used in Chapter 3 19

30 Figure 3.9 shows the deflected shape of the bridge when subjected to a single truck load at the center of the middle span using the 2-D SAP2000 model. Figure 3.9: Deformed Shape due to Single Truck Load 20

31 Sap2000 Frame Element Model Vertical Deflection with Single Truck loading at center of bridge Fixed Foundation Support Gross Section Properties 2 1 Vertical Deflection (mm) D D Along Length of Bridge (meters) Figure 3.10: Comparison between 2-D and 3-D Models Figure 3.10 shows that differences between the 2-D model and the 3-D model are minimal for static deflections. At the center of the bridge, the maximum deflections differ by only 0.07 mm between the 2-D and 3-D model as shown in Table 3.1. Table 3.1: Comparison of Vertical Deflections For Fixed Support Fixed Support Models 2-D Model (mm) 3-D Model (mm) Effect of Model Type Gross Section (1.2 %) Transformed Section ( 1.3 %) Effect of Prestressing Steel (mm) 0.78 (13.2 %) 0.78 (13.3 %) 21

32 2 2-D Sap2000 Frame Element Model Vertical Deflection With Single Truck Loading at Center Fixed Support Model With (Transformed) or Without (Gross) Prestressing Steel Vertical Deflection (mm) D Model (Gross Section) -6-7 Along Length of Bridge (meters) 2-D Model (Transformed Section) Figure 3.11: Comparison of Gross and Transformed Section Properties for 2-D Model Results 2 3-D Sap2000 Frame Element Model Vertical Deflection With Single Truck Loading at Center Fixed Support Model With (Transformed) or Without (Gross) Prestressing Steel 1 Vertical Deflection (mm) Along Length of Bridge (meters) 3-D Model (Gross Section) 3-D Model (Transformed Section) Figure 3.12: Comparison of Gross and Transformed Section Properties for 3-D Model Results 22

33 When comparing the models with and without the prestressing steel, the differences are more significant. Figures 3.11 and 3.12 show the comparison between gross section and transformed section properties for the 2-D and 3-D models respectively. Table 3.1 lists the maximum midspan deflections for each model showing differences of 0.78 mm (13.2%) and 0.78 mm (13.3%) for the 2-D and 3-D models respectively D Sap2000 Frame Element Model Vertical Deflection with Single Truck Loading at Center of Bridge 2-D Models With or Without Linear Soil Spring Vertical Deflection (mm) Along Length of Bridge (meters) Gross Section Without Linear Soil Springs Gross Section With Linear Soil Springs Figure 3.13: Differences Between Fixed Supports and Soil Springs: 2-D Model 23

34 3-D Sap2000 Frame Element Model Vertical Deflection with Single Truck Loading at Center of Bridge 3-D Models With or Without Linear Soil Springs 2 Vertical Deflection (mm) Along Length of Bridge (meters) Gross Section Without Linear Soil Springs Gross Section With Linear Soil Springs Figure 3.14: Difference Between Fixed Supports and Soil Springs: 3-D Model Figures 3.13 and 3.14 show the differences between the fixed support and linear soil springs used at the foundation of the piers for the 2-D and 3-D model respectively. As stated previously, the soil springs are modeled with linear soil properties, and may not accurately reflect actual soil response to different forces. Table 3.2 shows that there are minimal differences in the vertical deflection between the fixed and spring foundation and minimal differences between the 2-D and 3-D model. For this reason, and to keep the ANSYS solid model under 32,000 nodes, the solid model was generated as a straight model (equivalent to the SAP D fixed geometry) using fixed supports at the piers. Table 3.2: Comparison between Fixed Supports and Soil Springs 2-D Model (mm) 3-D Model (mm) Effect of Model Type Linear Soil Spring (1%) Fixed Foundation 0.07 (1.2%) Effect of Soil Springs 0.06 (1%) 0.07 (1%) 24

35 CHAPTER 4 ANSYS SOLID MODEL 4.1 ANSYS Solid Model Development Reasons for creating a solid model in ANSYS include: More detailed representation than a frame element model Output strain values for use in designing a strain-based deflection system Study torsion effects of eccentric truck loads Predict thermal deformations ANSYS has nonlinear modeling capabilities for use in future seismic analysis. Several software programs were considered for analyzing the solid model. Sap 2000 Version 8 (CSI 2002) ANSYS Version 6.1 (ANSYS Inc, 2002) Abaqus-Standard Version 6.0 (Abaqus, Inc. 2002) I-deas ANSYS was the choice of software for creating the solid model. SAP2000 did not have the capability of creating a box girder bridge with a varying cross section. SAP2000 did not have adequate meshing capabilities and could only mesh solid models in linear elements. I-deas was used previously to create solid bridge models of the H-3 (Ao 1999) but the College of Engineering at the University of Hawaii no longer has a license for I-deas. Between Abaqus and ANSYS, ANSYS appeared to be the more user friendly software with a simple tutorial and CAD input capabilities. 25

36 4.2 Finite Element Analysis: ANSYS, an Overview ANSYS is a finite element analysis program used for solid modeling. It has extensive capabilities in thermal, and structural analysis. The solid model consists of key points/nodes, lines, areas and volumes with increasing complexity in that order. Careful thought needs to be put into the model before building the entire model. Once the model is meshed, volumes, areas, or lines cannot be deleted if they are connected to existing meshed elements. The aspect ratio and type of mesh must also be decided depending on the size and shape of the complete solid model. ANSYS contains many solid finite elements to choose from, each having its own specialty. First, the type of analysis must be chosen which ranges from structural analysis, thermal analysis, or fluid analysis. Once the type of analysis is determined, an element type needs to be chosen ranging from beam, plate, shell, 2-D solid, 3-D solid, contact, couple-field, specialty, and explicit dynamics. Each element has unique capabilities and consists of tetrahedral, triangle, brick, 10 node, or 20 node finite elements both in 2-D or 3-D analysis. 4.3 Solid Model Geometry There are three ways to create a model in any finite element program for solid modeling. 1) Direct (manual) generation Specify the location of nodes Define which nodes make up an element Used for simple problems that can be modeled with line elements (links, beams, pipes) 26

37 For objects made of simple geometry (rectangles) Not recommended for complex solid structures 2) Importing Geometry Geometry created in a CAD system like Autodesk Inventor Saved as an import file such as an IGES file. Inaccuracies occur during the import, and the model may not import correctly. 3) Solid Modeling Approach The model is created from simple primitives (rectangles, circles, polygons, blocks, cylinders, etc.) Boolean operations are used to combine primitives. Direct manual generation was the approach used to create the SAP2000 frame element models. However when creating a solid model that contains over 20,000 nodes, this approach is not recommended. Using a CAD program such as Autodesk Inventor to create the solid model was also investigated. Autodesk Inventor had a very good CAD capability compared to creating the model in the ANSYS CAD environment. However, attempts to import the IGES file into ANSYS were unsuccessful. The model did not import correctly due to software incompatibility. The solid modeling approach was used to create the Kealakaha Bridge. Creating the top slab of the bridge with the extrude command was easy because it was the same shape throughout the bridge. However, when creating the box girder, the cross section varied throughout the length of the bridge. ANSYS did not have good CAD capabilities 27

38 to create many volumes in 3-D space with a varying cross section. When creating the solid volume for the box girder, each solid element had to be created using only 8 nodes at a time by using the create volumes arbitrary by nodes command. Creation of the final bridge model was accomplished by dividing the bridge into many volumes and combining them together. Figure 4.1 shows the side view of portion of the bridge. Each color represents a different area and block volume that had to be created and joined together using the Boolean operation. Due to symmetry, the reflect and copy command was used to create the other half of the bridge. 1 AREAS AREA NUM FEB :00:21 Y Z Figure 4.1: Side View of a Portion of the Kealakaha Bridge 28

39 4.4 Development of Solid Model Geometry The program that was used to analyze the solid model was ANSYS/University High Option, Version 6.1. Limitations to this software include the maximum number of nodes which is set at 32,000 nodes. To keep the number of nodes below this limit, the original cross section could not be used without having a large aspect ratio during meshing. To reduce the amount of nodes as well as computation time, the cross section model had to be simplified. Weng Ao (1999) performed a similar study on the North Halawa Valley Viaduct (NHVV), which is part of the H-3 freeway. The NHVV box girder shape was very similar to the Kealakaha bridge box girder. Ao used simpler cross sections than the original box girder and compared the predicted to measured results. Even with simplification of the cross sections, the analytical results using the I-deas solid modeling program showed good agreement with actual results for both thermal and truck loading conditions. The simplified cross section shown in Figure was created by averaging the top and bottom slab thickness of the design cross section to create an equivalent area in the simplified cross section. The moment of inertia was changed by no more than 3% in the lateral direction and 11% in the vertical direction. Figure shows the design cross section that was used to compute section properties for the frame element models in SAP2000. Figure shows the simplified cross section used for the solid model in ANSYS. The depths and heights that vary are listed in the Appendix. 29

40 Figure 4.2.1: Design Cross Section Figure Simplified Cross Section 30

41 1 VOLUMES TYPE NUM FEB :02:06 Y Z Figure 4.3: ANSYS Solid Model Cross Section before Meshing Figure 4.3 shows a close up view of the simplified cross section in ANSYS. Figures 4.4 and 4.5 show the completed solid model before meshing. The piers have fixed supports while the abutment ends are restrained against vertical and lateral movement perpendicular to the bridge. 31

42 1 VOLUMES TYPE NUM U FEB :27:15 Y Z Figure 4.4: Kealakaha Bridge before Meshing, Elevation 1 VOLUMES TYPE NUM U FEB :26:02 Y Z Figure 4.5: Kealakaha Bridge before Meshing, Isometric View 32

43 4.5 Meshing in ANSYS Meshing in ANSYS can be applied manually or automatically. The element type selected (Linear vs. Tetrahedral), and the mesh size can affect the accuracy of the results of the analysis. Due to the large model size, automatic meshing was not possible for the entire Kealakaha bridge. In automatic meshing, ANSYS automatically chooses a meshing size based on the shape of the model. This resulted in more elements than permitted by the University High Option of ANSYS. Manual meshing allows the user to define the maximum size of the elements. To guide the selection of element type, a test beam was created in ANSYS to determine what solid finite element produced the best results for deflection under thermal loading. There are two types of elements in ANSYS that have both structural and thermal capabilities for solid modeling. They are Solid 45 which is an eight node brick (cube shaped) element (Fig. 4.6) and Solid 92 which is a 10 node tetrahedral element (Fig. 4.7). These elements were tested under thermal and static loads on a test beam to determine which element produced the best results when compared to the theoretical values. 33

44 Figure 4.6: Solid 45, Eight Node Structural Solid (ANSYS) Figure 4.7: Solid 92, Ten Node Tetrahedral Structural Solid (ANSYS) 4.6 Test Beam: Determining Finite Element Type and Mesh for Thermal Loading Solid 45 and Solid 92 were evaluated using a test beam that was 10 meters long by one meter thick and one meter high. The sample test beam was also created to test the performance of ANSYS under thermal loading conditions. Simply supported end conditions were used for the test beam as shown in Figure

45 10 m 10 Degrees 1 m Temp Gradient Figure 4.8: Square Test Beam-Thermal Loading A 10-degree temperature gradient was produced by applying two different temperatures at the top and bottom surfaces of the beam. A temperature gradient is anticipated for the top slab of the Kealakaha bridge during solar heating similar to the H- 3 study (Ao 1999). The thermal expansion coefficient was arbitrarily chosen as 10-5 per degrees Celsius for this test beam. Figure 4.9 shows the distribution of the temperature that was applied throughout the beam. The red indicates a temperature of 10 degrees C, while the blue represents a temperature of 0 degrees C. The actual thermal expansion coefficient used in the Kealakaha bridge model will be based on concrete cylinder tests and is expected to be in the range of 10 to per degree Celsius. For the thermal analysis performed in this study, a value of per degree Celsius was used for the Kealakaha bridge model. Concrete properties similar to the top slab of the Kealakaha bridge was used for the test beam. 35

46 1 NODAL SOLUTION STEP=1 SUB =1 TIME=1 BFETEMP (AVG) RSYS=0 DM = SM =10 Y FEB :33:04 Z M MN Figure 4.9: Thermal Distribution in Test Beam 36

47 4.7 Analytical Solution For Test Beam The deformation due to a linear temperature change can be expressed as: where v α d dv T = α dx dx h = Vertical Deflection = Coefficient of Thermal Expansion = 10-5 / C in the test beam T = Change in temperature between top and bottom surfaces = 10 C in the test beam h = Depth of the beam = 1 meter in the test beam Therefore, dv dx where A and B are integration constants. T = α x + A h 1 α T 2 v = x + Ax + B 2 h Applying boundary conditions: At x=0, v(0)=0 and at x=10, v(10)=0 and substituting the numerical values into the equation, we obtain: At the midspan, x = 5 meters therefore: v = (50-5x)x*10-5 v = meters There should be a maximum deflection of meters at the center of the test beam. 37

48 Figure 4.10 shows the deflection result of the test beam in ANSYS due to the 10 degrees temperature gradient using the solid 92 element. The automatic meshing tool was used which produced element sizes close to 0.5 meters. 1 DISPLACEMENT STEP=1 SUB =1 TIME=1 DM = FEB :32:31 Y Z Figure 4.10: Test beam deflection under 10 Celcius Temperature Gradient (Automatic Mesh) 4.8 Comparison of ANSYS to Theoretical Result: Thermal Loading Table 4.1 shows the comparison between Solid 45 and Solid 92 for the thermal loading conditions. Varying the element size from 0.25 to 1 meter had very little effect on the vertical deflection under thermal loading. The theoretical result is 1.25 mm for the vertical deflection at midspan. The percentage error in Table 4.1 is the error compared to the theoretical result. 38

49 Table 4.1: Vertical Deflection at Midspan on Test Beam: Thermal Loading Vertical Deflection at Percentage Error Midspan (mm) Theoretical Result Solid45 Eight Node Structural Solid (Brick Node) Solid 92 Ten Node Structural Solid Tetrahedral Shaped % % Solid 92 gave the lowest percentage error of 4.3% when compared with the analytical result. 4.9 Comparison of ANSYS to Theoretical Result: Static Point Loading A static point load of 10 Newton applied to the midspan of the test beam using different element types and sizes as shown in Figure N (at midspan of beam) 1 m 10 m Figure 4.11: Square Test Beam Point Loading 39

50 For a simply supported beam under a midspan point load, the theoretical deflection is: Vertical Deflection 3 PL = 48EI where P = Load at midspan = 10 N on test beam L = Length of beam = 10 m for test beam E = Modulus of Elasticity = kn/m 2 for test beam 3 I = Moment of Inertia = bh 12 = 1 m 4 for test beam 12 Substituting the numerical values produces the following theoretical result: = m down Table 4.2 lists the comparisons between the Solid 45 and Solid 92 elements for the vertical deflection at the midspan due to a 10 N point load. The theoretical result will not match the result from ANSYS because the theoretical result does not include shear deformation. However, the % difference between the theoretical and ANSYS will be used. The results show that Solid 92 consistently predicted deflections close to the theoretical result with the percent difference ranging from 3.2 to 5.4%. The solid 45 results range from 5.76 to 62 percent and are highly dependant on the mesh element size. For this reason, Solid 92 would be the better choice under a static load. 40

51 Table 4.2: Vertical Deflection at Midspan on Test Beam: 10 N Point Load Element Size Solid45 Eight Node Structural Solid (Brick Node) Solid 92 Ten Node Structural Solid Tetrahedral Shaped Vertical Deflection at Midspan (10-7 m) % Difference From Theoretical Vertical Deflection at Midspan (10-7 m) % Difference From Theoretical Automatic Meshing meters meters meter Theoretical Result m m Structural Solid 92 was selected for meshing the Kealakaha Bridge model. Solid 92 has a quadratic displacement behavior and is well suited to model irregular geometries as shown in Figure 4.7. The element can model plasticity, creep, swelling, stress stiffening, large deflection, and large strain conditions. When applying a thermal load, a thermal solid element must also be selected. ANSYS automatically chose Thermal Solid 87 for both test beam and bridge models. Thermal analysis is done separately in ANSYS, and is saved as a.rth file in the working directory. In thermal analysis, one must transfer the element type from a structural element to thermal element so that thermal loads can be applied linearly. This is important because if the program is in structural element mode, the temperatures will only be applied at the surface of the beam, and will not be applied linearly throughout the entire beam. After running the thermal analysis, the.rth file must be imported into the structural element mode with Solid 92 and applied as a temperature from thermal analysis. After running the structural analysis, structural deformation/stress/strain results are produced. 41

52 4.10 Mesh Generation for Kealakaha Bridge Model ANSYS has the capability of doing automatic meshing where it automatically picks an element size. However, automatic meshing may not produce the best results and cannot be used for the 220 meter Kealakaha bridge because it will produce over 32,000 nodes which exceeds the University program capability. The mesh tool command must be used to specify the element size. Based on the specified element size, ANSYS will mesh the model to produce the best results. The element size will not be the same for all elements, but all elements will be smaller than the specified size. The mesh size used for the Kealakaha bridge was 4 meters. A similar mesh size of 12 feet was used in the NHVV study by Weng Ao (1999), and produced good results when compared with measured deflections. Figure 4.12 shows the 4 meter mesh for a portion of the bridge. The full bridge consisted of 24,576 nodes and 12,246 elements Convergence of 4 Meter Mesh To confirm that the four-meter mesh converges with a larger size mesh, a six meter mesh was created and the response to a single truck load was compared. See Figure 3.8 for a description of the single truck load. The four-meter mesh is seen in Figure 4.12 and the six-meter mesh is shown in Figure

53 1 ELEMENTS FEB :14:11 Figure 4.12: Four Meter Mesh Size, Kealakaha Bridge (Part of Bridge) 1 ELEMENTS Figure 4.13: Six Meter Mesh Size, Kealakaha Bridge (Part of Bridge) 43

54 2 ANSYS Solid Model Vertical Deflection with Single Truck loading at center of bridge Convergence of Four Meter Mesh Vs. Six Meter Mesh Vertical Deflection (mm) Meter Mesh 6 Meter Mesh Distance Along Bridge (meters) Figure 4.14: Convergence of Four and Six Meter Mesh for ANSYS Model Table 4.3: Comparison between Four and Six Meter Mesh for ANSYS Model Maximum End Span Deflection Maximum Center Span Deflection Six Meter Mesh Vertical Deflection (mm) Four Meter Mesh Vertical Deflection (mm) Difference (%) (2.1%) (0%) The results plotted in Figure 4.14 show convergence between a four meter mesh and a six meter mesh. The results at the maximum deflection for the end span and center span under a single truck loading are shown in Table 4.3. In Table 4.3, there is a 0% difference in the center span deflection, and only a 2.1% difference in the end span deflection. Therefore, a four-meter mesh is adequate for this analysis. 44

55 CHAPTER 5 ANSYS SOLID MODEL ANALYSIS 5.1 Truck Loading Conditions According to the design criteria on the construction plans, a typical truck weighs a total of 320 kn or 72 Kips with the dimensions shown in Figure 5.1. Figure 5.1: Distribution of Truck Loads Each 320 kn truck has six wheels and the load is divided among all six wheels for the ANSYS solid model. The total axle load shown in Figure 5.1 is divided by two to get the load for each wheel. In ANSYS, loads can only be applied to existing nodes produced by the mesh. The mesh size used was 4 meters, so the loads were placed at the closest possible node to produce the actual wheel location. Three different truck-loading conditions were considered in this analysis. In all of these analyses, the truck placement was symmetrical about the midspan of the center span of the bridge. The three loading conditions are: 45

56 Single Truck Load on centerline of roadway Four Trucks (Two rows of two trucks each, 2x2 Truck Load) on centerline of roadway Four Trucks (All four trucks in a single line) at edge of roadway In ANSYS, each wheel was modeled as a load, however in the SAP2000 frame element analysis, each axle was modeled as a load. ANSYS and SAP2000 model results are compared in the following sections. In addition, the SAP2000 frame element model and the ANSYS solid model were also compared when a single 320 kn point load was applied at the center of the roadway at midspan of the center span. 5.2 Truck Loading Results Single 320 kn (72 Kip) Point Load Figure 5.2 shows the single 320 kn truck point load applied to the top slab of the ANSYS model. Figure 5.3 shows a comparison between SAP2000 and ANSYS while Table 5.1 shows the vertical displacement under the 320 kn point load. The maximum deflection from the SAP2000 model is less than the ANSYS model, but at all other nodes the ANSYS model yielded slightly less deflections. The local deformation of the top slab under the single concentrated load does not correctly represent the effect of the truck loading. Table 5.1: Results of Single 320 kn Truck Point Load Sap2000 Single Truck Load ANSYS Single Truck Load Vertical Deflection at Center of Bridge Span (mm) Maximum End Span Deflection (mm) Difference 0.4 (6.7%) 0.03 (2.9%) 46

57 1 2 ELEMENTS ELEMENTS U F U F Z Y 3 ELEMENTS U F Y Z Figure 5.2: ANSYS Layout of Single Truck Point Load SAP2000 Vs. ANSYS Single Truck (Point Load) at Center of Bridge 2 1 Vertical Deflection (mm) Along Length of Bridge (meters) Figure 5.3: SAP2000 vs. ANSYS, Single Truck Point Load ANSYS SAP

58 5.2.2 Distributed Single Truck Load Figure 5.4 shows the viaduct section with a single truck loading placed at the center of the section and at the center span along the length of the bridge. Isometric, top and side views are shown in ANSYS in Figure 5.5. The results for the vertical deflection due to the single truck load are shown in Figure 5.6. Wheels were modeled to conform to Figure 5.1 but dimensions of the truck wheels vary according to the node locations in the solid model. The results for deflections are shown in table 5.2 Table 5.2: Vertical Deflection at Center of Bridge due to Single Truck Load, Actual Wheels Modeled Vertical Deflection at Center of Bridge (mm) SAP2000 Each Axle Modeled ANSYS Each Wheel Modeled Difference (mm) Vertical Deflection at Center of Bridge Span (mm) mm (0.6%) Maximum End Span Deflection (mm) mm (3.2%) Figure 5.4 Viaduct Section Showing Single Truck Load 48

59 1 2 ELEMENTS ELEMENTS U F m 5.25 m U F Z Y 3 ELEMENTS U F Y Z 3.12 m Figure 5.5: Layout of Wheel Placement for Single Truck 2 SAP2000 Vs. Ansys Single Truck Load at Center Of Bridge ANSYS: Each Wheel Modeled SAP2000: Each Axle Modeled Vertical Deflection (mm) Along Length of Bridge (meters) ANSYS SAP2000 Figure 5.6: SAP2000 vs. Ansys, Single Truck Modeled with Wheels 49

60 x2 Truck Loading Figure 5.7 shows the locations of the axles for the 2x2 truck loading. Figure 5.8 shows the viaduct section under the 2x2 truck loading. The trucks are placed symmetrically about the center span to reduce computational time for the analysis and produce symmetrical deflected shapes. The axle spacing is larger than as shown in Figure 5.1 due to limited node locations available for applying the loads. Figure 5.9 shows the layout of the 2x2 truck loading in ANSYS. The vertical deflection results are shown in Figure 5.10 and Table 5.3. Table 5.3: Vertical Deflection of Bridge Due to 2x2 Truck Load (Actual Wheels Modeled) Vertical Deflection at Center of Bridge (mm) Vertical Deflection at Center of Bridge Span (mm) Maximum End Span Deflection (mm) SAP2000 Each Axle Modeled ANSYS Each Wheel Modeled Difference (mm) mm (1.6%) mm (4.2%) Midspan of Bridge Center Span Figure 5.7: Location of Axle Loads for the 2x2 Truck Configuration 50

61 Figure 5.8: Viaduct Section showing 2x2 Truck Configuration 1 2 ELEMENTS ELEMENTS U F U F Z Y 3 ELEMENTS U F Y Z Figure 5.9: ANSYS Placement of 2x2 Truck Load 51

62 5 SAP2000 Vs ANSYS 22 Truck Load, 4 Trucks Total ANSYS: Each Wheel Modeled SAP2000: Each Axle Modeled Vertical Deflection (mm) ANSYS -20 SAP Length Along Bridge (meters) Figure 5.10: SAP2000 vs. ANSYS, 2x2 Truck Modeled with Wheels Truck Loading Creating Torsion Effects. 4 truck loads were placed at the edge of the viaduct cross section to study torsion effects due to eccentric loading. Figure 5.11 shows the locations of the axle loadings for the trucks. The trucks are placed symmetrically about the center span of the bridge to reduce the computational time for the analysis and to generate a symmetrical deflected shape. Midspan of bridge center span Figure 5.11: Location of Axle Loads for Four Trucks in a Row 52

63 The 4 trucks modeled at the right edge of the viaduct section are shown in Figure Figure 5.12 show the locations A, B, and C, where the vertical deflections were recorded. Location C is at the middle of the cross section. Location B is on the side of the truck loading above the box girder stem and location A is on the opposite side above the box girder stem. Figure 5.13 shows the layout of the 4 trucks in ANSYS. The loads are applied at the nodes. Figure 5.12: Viaduct Section showing Four Trucks in a Row 1 2 ELEMENTS ELEMENTS U F U F Z Y 3 ELEMENTS U F Z Y Figure 5.13: ANSYS Layout of Four Trucks in a Row 53

64 Figure 5.14 shows the deflected and non-deflected shape of the cross section modeled in ANSYS at midspan of the center span of the bridge, the legend at the bottom shows the vertical deflection in meters. Locations A, B, and C are shown at the top of the slab (See Figure 5.12 for more precise locations). The result of the vertical deflection due to the truck load are shown in Figure Truck Y Z A C B Figure 5.14: Deflected and Non-Deflected Cross Section 5 ANSYS: Torsion Effects 4 Trucks in a Row at Edge of Bridge ANSYS: Each Wheel Represented By One Load Vertical Deflection (mm) Along Length of Bridge (meters) Location A Location B Location C (Center) Figure 5.15: Torsion Effects, Four Trucks in a Row 54

65 Table 5.4 shows the results of the vertical deflections at locations A, B, and C. The torsion effect shows that there is a 2.43 mm difference between the left and right sides of the bridge cross section at the center span and a 0.57 mm difference in the maximum end span deflections. Table 5.4: Vertical Deflection of Bridge due to 4 Truck Loading at Edge of Bridge (Actual Wheels Modeled) Vertical Deflection in Cross Section Points A and B (mm) ANSYS Location A (Left) ANSYS Location B (Right) % Difference (torsion effect) Vertical Deflection at Center of Bridge Span (mm) (13.0%) Maximum End Span Deflection (mm) (15.4%) Figure 5.16 shows an isometric view of the bridge with color contours for the vertical deflection of the bridge. The torsion effect can be seen by the different colors. The legend shows the deflection in meters. 1 NODAL SOLUTION STEP=1 SUB =1 TIME=1 UY (AVG) RSYS=0 DM = SMN = SM = M MN Y Z Figure 5.16: Isometric View of Vertical Deflection under Torsion Loading

66 56

67 CHAPTER 6 TEMPERATURE ANALYSIS 6.1 Temperature Gradient Figure 6.1: ANSYS Applied Temperature Gradient Figure 6.1 show the temperature gradient applied to the ANSYS solid model. A 10 degrees Celsius linear temperature gradient is applied through the 0.35 m thick top slab. The temperature gradient was based on temperature measurements from the NHVV (Ao, 1999). Below the top slab, the temperature was assumed constant at zero degrees throughout the box girder, and piers. This thermal loading develops by mid afternoon due to solar radiation on the top surface of the bridge. Thermocouples will be installed in the Kealakaha Bridge to record the exact temperature gradients after the bridge is built. The coefficient of thermal expansion used for this analysis was per degrees Celsius. 57

68 1 NODAL SOLUTION STEP=1 SUB =1 TIME=1 BFETEMP (AVG) RSYS=0 DM = SM =10 M Figure 6.2: Bridge End Span Showing Effect of Thermal Gradient 6.2 Results of Temperature Gradient Figure 6.2 shows the temperature gradient applied through the top slab of the bridge and the resulting exaggerated deformed shape. Figure 6.3 shows the deformation of the bridge due to the 10 degree temperature gradient. Figures 6.4 and 6.5 show isometric and side views of the deformation of the bridge. 58

69 1 2 DISPLACEMENT DISPLACEMENT STEP=1 SUB =1 TIME=1 DM = STEP=1 SUB =1 TIME=1 DM = Y Z Y Z 3 4 DISPLACEMENT DISPLACEMENT STEP=1 SUB =1 TIME=1 DM = Y Z STEP=1 SUB =1 TIME=1 DM = Y Z Figure 6.3: Deformation due to 10 Degree Temperature Gradient 1 DISPLACEMENT STEP=1 SUB =1 TIME=1 DM = Y Z Figure 6.4: Isometric View of Bridge Deformation due to Thermal Loading 59

70 1 DISPLACEMENT STEP=1 SUB =1 TIME=1 DM = Y Z Figure 6.5: Side View of Bridge Deformation due to Thermal Loading 60

71 The deflected shape is plotted along the middle of the top slab (location a ), along the top of the box stems ( b ) and along the edge of the top slab cantilevers ( c ). Locations a and c are affected by longitudinal and transverse deformations as seen in Figure 6.5, hence location b, above the box girder stems, is assumed to be the best representation of the deformed shape of the bridge spans. Comparisons with measured deflections based on the field instrumentation will confirm whether these predicted deflections are accurate. Figure 6.6 shows the approximate locations a, b, and c in the cross section view indicated by the circles. b a Y b Z c c E E Figure 6.6: Locations of Reported Deformation due to Thermal Loading 61

72 4 ANSYS Solid Model Vertical Deflection due to Gradient Temperature of 10 Degrees Celcius through top slab Deflection along roadway centerline (a) Vertical Deflection (mm) 2 Deflection above base stems (b) Deflection at end of cantilever (c) Distance Along Bridge (meters) Figure 6.7: Vertical Deflection of Bridge due to Ten Degree Temperature Gradient Table 6.1: Vertical Deflection due to Temperature Gradient Distance Along Bridge (meters) Deflection (mm) Along Roadway Centerline a Deflection (mm) Above Base Stems b Deflection (mm) at End of Cantilever c m and m 110 m Figure 6.7 shows the vertical deflections at points a, b, and c. The results at the center span and maximum deflections in the end spans are shown in Table 6.1. Results show that at 110 meters, the greatest deflection occurs downwards. At and meters, the greatest upward deflection occurs. Location b best represents the deformed shape of the bridge span. The top slab curls upwards at the center a while the left and right cantilevers c deflect downwards due to the temperature applied at the top surface. 62

73 4 ANSYS Solid Model Combination of Temperature and Truck Loading 2 Vertical Deflection (mm) Along Length Of Bridge (meters) Temperature Only (10 Degrees Celcius) One Truck Loading Only Combined Figure 6.8: Combination of Temperature and Truck Loading Figure 6.8 shows the combination of the temperature and the truck loading. Note that the vertical deflection due to thermal gradient of 10 C is similar to that caused by a single truck load. Since, this is a linear elastic analysis, the deformation due to the temperature only and the truck loading only can be added using superpositioning to determine the deformation due to the combined temperature and truck loading. For this reason, any results used from the truck loading analysis in the previous section can be added to the temperature only analysis to get the deformations for both temperature and truck loading simultaneously. While monitoring deflections of the bridge under ambient traffic, it will be necessary also to measure the thermal gradient through the top slab so as to adjust for the deflections due to thermal loading. 63

74 6.3 Strain Distribution The strain distribution through the box girder depth under a single truck load is shown near the pier support in Figure 6.9 and at the midspan of the center span in Figure Strain Distribution Through Box Girder Depth Near Pier Along Length of Bridge (Single Truck Load) 0 Depth of Bridge (m) Tension Compression Microstrain Figure 6.9: Strain Distribution through Box Girder Depth near Pier Strain Distribution Through Box Girder Depth Near Centerspan Along Length of Bridge (Single Truck load) Compression Depth of Bridge (m) Tension Microstrain Figure 6.10: Strain Distribution through Box Girder Depth near Midspan 64

75 Figure 6.11: Strain Output Locations Figure 6.11 shows the locations where future strain gages will be installed after the bridge is built to monitor longitudinal strain in the box girder. These gages will be used in a strain based deflection system under development at the University of Hawaii (Fung, 2003). The gages selected for this system must have sufficient resolution to monitor the anticipated strains. The locations are represented with the letters A, B, C, and D. Locations A and B are at the inside top of the box girder, while locations C and D are located at the inside bottom of the box girder. The longitudinal strains due to a single truck at midspan of the center span and due to a 10 degree temperature gradient throughout the top slab are shown in Figures 6.12 and In order to measure these strains, the gages will need a production of 1 microstrain. It will also be important to monitor the slab temperature so as to separate the thermal effects from the loading effects. 65

76 ANSYS Solid Model Longitudinal Strain at Location A and B Along Length of Bridge Longitudinal Strain (Compression +) (microstrain) Along Length of Bridge (meters) Temperature Only (10 Degrees Celcius) One Truck Loading Only Combined Figure 6.12: Longitudinal Strains at Locations A and B ANSYS Solid Model Longitudinal Strain at Location C and D Along Length Of Bridge Longitudinal Strain (compression +) microstrain Temperature Only (10 Degrees Celcius) Truck Loading Only Combined Along Length of Bridge (meters) Figure 6.13: Longitudinal Strains at Locations C and D 66

77 CHAPTER 7 MODAL ANALYSIS 7.1 Modal Periods The first nine modal periods of the Kealakaha bridge were obtained from the SAP2000 and ANSYS models. The objective of this study was to obtain the basic mode shapes to confirm the locations of the strain gages and accelerometers during the construction of the bridge. The accelerometers and strain gages will measure structural response to ambient traffic, thermal loading, and seismic activity. The modal periods from the different SAP2000 models are compared in Tables 7.1.1, 7.1.2, and Table shows the comparison between the SAP2000 model and the equivalent ANSYS model. The mode shapes are shown in Figures 7.1 to Modal Periods: 2-D vs. 3-D Models Table shows the comparison of modal periods between the 2-D and 3-D models for the SAP2000 frame element models, using the gross section properties. There was less than a 1% difference in periods between the 2-D and 3-D models. Table 7.1.1: Modal Periods: 2-D vs. 3-D Mode 2-D no steel 3-D no steel % Difference

78 7.1.2 Modal Periods: Gross Section vs. Transformed Section As seen in Table 7.1.2, there is also very little difference between modal periods for models with gross section (no prestressing steel) and transformed properties including (prestressing steel). Therefore, including the prestressing steel resulted in less than 2.2% difference in the modal periods. Table 7.1.2: Modal Periods: Gross Section vs. Transformed Section Mode 2-D no steel 2-D with steel % Difference Modal Periods: Linear Soil Spring vs. Fixed Support Table shows the modal period comparison between the 2-D SAP2000 model with linear soil springs versus fixed supports. For most mode shapes, the modal periods were similar for the SAP2000 models with or without linear soil springs. However, in modes with significant transverse pier displacement, the modal periods for models with soil springs were up to 21% larger than models without soil springs. There was a high percent difference in modes 3, 5 and 7 which are shown in Figures 7.6, 7.10, and 7.14 respectively. This is due to the lateral soil springs, which are less stiff than the fixed supports. It will be important in future studies to determine the nonlinear and dynamic properties of the soil to obtain the accurate soil stiffness for seismic analysis. 68

79 Table 7.1.3: Modal Periods: Linear Soil Spring Supports vs. Fixed Support 2-D no steel, 2-D no steel, Mode Fixed Support Soil Springs % Difference Modal Periods, SAP2000 vs. ANSYS Table shows the comparison between SAP2000 and ANSYS for the first 9 mode shapes. Mode 1 from the ANSYS model corresponds to mode 2 from SAP2000. There is a significant difference in modal periods for mode shapes 5,7 and 9, which have substantial torsion in the box girder as detected in the ANSYS runs. The torsional crosssection properties used in the SAP2000 models may not accurately represent the boxgirder. Table 7.1.4: Modal Periods, SAP2000 vs. ANSYS Mode SAP2000 ANSYS % Difference (sec.) (sec.) Mode Shapes The first nine mode shapes obtained from the SAP2000 and ANSYS models are shown in Figures 7.1 to

80 1 2 DISPLACEMENT DISPLACEMENT STEP=1 SUB =2 FREQ=1.124 RSYS=0 DM =.420E-03 STEP=1 SUB =2 FREQ=1.124 RSYS=0 DM =.420E-03 Z Y Z Y 3 DISPLACEMENT STEP=1 SUB =2 FREQ=1.124 Y RSYS=0 DM =.420E-03 Z Figure 7.1: ANSYS Mode 2 Figure 7.2: SAP2000 Mode 1 70

81 1 2 DISPLACEMENT DISPLACEMENT STEP=1 SUB =1 FREQ=1.11 RSYS=0 DM =.931E-03 STEP=1 SUB =1 FREQ=1.11 RSYS=0 DM =.931E-03 Z Y Z Y 3 DISPLACEMENT STEP=1 SUB =1 FREQ=1.11 RSYS=0 Y DM Z=.931E-03 Figure 7.3: ANSYS Mode 1 Figure 7.4: SAP2000 Mode 2 71

82 1 2 DISPLACEMENT DISPLACEMENT STEP=1 SUB =3 FREQ=1.423 RSYS=0 DM =.778E-03 STEP=1 SUB =3 FREQ=1.423 RSYS=0 DM Z=.778E-03 Y Z Y 3 DISPLACEMENT STEP=1 SUB =3 FREQ=1.423 Y RSYS=0 DM Z=.778E-03 Figure 7.5: ANSYS Mode 3 Figure 7.6: SAP2000 Mode 3 72

83 1 2 DISPLACEMENT DISPLACEMENT STEP=1 SUB =4 FREQ=2.394 RSYS=0 DM =.636E-03 STEP=1 SUB =4 FREQ=2.394 RSYS=0 DM =.636E-03 Z Y Z Y 3 DISPLACEMENT STEP=1 SUB =4 FREQ=2.394 RSYS=0 Y DM Z=.636E-03 Figure 7.7: ANSYS Mode 4 Figure 7.8: SAP2000 Mode 4 73

84 1 2 DISPLACEMENT DISPLACEMENT STEP=1 SUB =5 FREQ=2.495 RSYS=0 DM =.683E-03 STEP=1 SUB =5 FREQ=2.495 RSYS=0 DM =.683E-03 Z Y Z Y 3 DISPLACEMENT STEP=1 SUB =5 FREQ=2.495 RSYS=0 Y DM Z=.683E-03 Figure 7.9: ANSYS Mode 5 Figure 7.10: SAP2000 Mode 5 74

85 1 2 DISPLACEMENT DISPLACEMENT STEP=1 SUB =6 FREQ=2.996 RSYS=0 DM =.910E-03 STEP=1 SUB =6 FREQ=2.996 RSYS=0 DM =.910E-03 Z Y Z Y 3 DISPLACEMENT STEP=1 SUB =6 FREQ=2.996 RSYS=0 Y DM Z=.910E-03 Figure 7.11: ANSYS Mode 6 Figure 7.12: SAP2000 Mode 6 75

86 1 2 DISPLACEMENT DISPLACEMENT STEP=1 SUB =7 FREQ=3.031 RSYS=0 DM =.722E-03 STEP=1 SUB =7 FREQ=3.031 RSYS=0 DM =.722E-03 Z Y Z Y 3 DISPLACEMENT STEP=1 SUB =7 FREQ=3.031 RSYS=0 Y DM Z=.722E-03 Figure 7.13: ANSYS Mode 7 Figure 7.14: SAP2000 Mode 7 76