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.
ABSTRACT The studies described in this report focus on the short-term structural performanceof a new replacement Kealakaha Bridge scheduled for construction in Fall 2003. A new three span, 220-meter concrete bridge will be built to replace an existingsix span concrete bridge spanning the Kealakaha Stream on the island of Hawaii. Duringand after construction, fiber optic strain gages, accelerometers, Linear VariableDisplacement Transducers (LVDTs) and other instrumentation will be installed tomonitor the structural response during ambient traffic and future seismic activity. Thiswill 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 deformationsunder thermal and static truck loading. Mode shapes and modal periods are also studiedto see how the bridge would react under seismic activity. Using SAP2000, a finiteelement program, a 2-D bridge model was created to perform modal analysis, and studyvertical deformations due to static truck loads. A 3-D bridge model was also created inSAP2000 to include the horizontal curve and vertical slope of the bridge. This model iscompared with the 2-D SAP2000 model to evaluate the effect of these and otherparameters on the structural response.In addition, a 3-D Solid Finite Element Model was created using ANSYS to studythermal loadings, longitudinal strains, modal analysis, and deformations. This model wascompared with the SAP2000 model and generally shows good agreement under statictruck loading and modal analysis. In addition, the 3-D ANSYS solid finite element modelgave reasonable predictions for the bridge under thermal loadings. These models will beused as a reference for comparison with the measured response after the bridge is built. iii
3.
ACKNOWLEDGEMENTS This report is based on a Masters Plan B report prepared by Jennifer Chang underthe 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 BridgeResearch and Construction (IBRC) as part of the seismic instrumentation of theKealakaha Stream Bridge. This support is gratefully acknowledged. The content of thisreport reflects the views of the authors, who are responsible for the facts and the accuracyof the data presented herein. The contents do not necessarily reflect the official views orpolicies of the State of Hawaii, Department of Transportation, or the Federal HighwayAdministration. This report does not constitute a standard, specification or regulation. iv
4.
TABLE OF CONTENTSAbstract…………………………………………………………………………. iiiAcknowledgements……………………………………………………………… ivTable of Contents……………………………………………………………….. vList of Tables……………………………………………………………….…… viiList of Figures…………………………………………………………………… viiiChapter 1 INTRODUCTION…..…………………………………………… 1 1.1 Project Description……………………………………………….. 1 1.2 Project Scope……………………………………………………… 5Chapter 2 DESIGN CRITERIA FOR KEALAKAHA BRIDGE…………… 7 2.1 Geometric Data…………………………………………………… 7 2.2 Linear Soil Stiffness Data………………………………………… 7 2.3 Material Properties………………………………………………… 11 2.4 Boundary Conditions of Bridge…………………………………… 11 2.5 Bridge Cross Section……………………………………………… 11Chapter 3 SAP2000 FRAME ELEMENT MODELS ……………………… 13 3.1 Development of SAP2000 Frame Element Models……………… 13 3.2 Element Sizes used for SAP2000 Models………………………… 16 3.3 Results of Frame Element Model Comparisons…………………… 18 3.3.1 Natural Frequencies…………………………………………18 3.3.2 Static Load Deformations………………………………….. 18Chapter 4 ANSYS SOLID MODEL ………………………………………… 25 4.1 ANSYS Solid Model Development………………………………. 25 4.2 Finite Element Analysis: ANSYS, an Overview ..……………….. 26 4.3 Solid Model Geometry…………………………………………… 26 4.4 Development of Solid Model Geometry…………………………. 29 4.5 Meshing in ANSYS………………………………………………. 33 4.6 Test Beam: Determining Finite Element Type and Mesh for Thermal Loading…………………………………………………. 34 4.7 Analytical Solution For Test Beam………………………………. 37 4.8 Comparison of ANSYS to Theoretical Result: Thermal Loading… 38 4.9 Comparison of ANSYS to Theoretical Result: Static Point Loading.39 4.10 Mesh Generation for Kealakaha Bridge Model……………………. 42 4.11 Convergence of 4 Meter Mesh…………………………………….. 42Chapter 5 ANSYS SOLID MODEL ANALYSIS …………………………… 45 5.1 Truck Loading Conditions…………………………………………. 45 5.2 Truck Loading Results…………………………………………….. 46 5.2.1 Single 320 kN (72 Kip) Point Load……………………….. 46 5.2.2 Distributed Single Truck Load……………………………. 48 5.2.3 2x2 Truck Loading……………………………………….. 50 v
5.
5.2.4 4 Truck Loading Creating Torsion Effects………………… 52Chapter 6 TEMPERATURE ANALYSIS …………………………………… 57 6.1 Temperature Gradient……………………………………………… 57 6.2 Results of Temperature Gradient………………………………….. 58 6.3 Strain Distribution…………………………………………………. 64Chapter 7 MODAL ANALYSIS …………………………………………….. 67 7.1 Modal Periods……………………………………………………… 67 7.1.1 Modal Periods: 2-D vs. 3D Models…….…………………. 67 7.1.2 Modal Periods: Gross Section vs. Transformed Section….. 68 7.1.3 Modal Periods: Linear Soil Spring vs. Fixed Support….… 68 7.1.4 Modal Periods: SAP2000 vs. ANSYS….…………………. 69 7.2 Mode Shapes………………………………………………………. 70Chapter 8 CONCLUSIONS AND SUMMARY……………………………… 79 8.1 Summary………………….………………………………………. 79 8.2 Conclusions……………………………………………………….. 79 8.3 Sources of Possible Error………………………………………….. 80 8.4 Suggestions for Further Study…………………………………….. 81References …………………………………………………………………….. 83Appendix A – Model Input Data ………………………………………………… 85 Coordinates of SAP2000 2-D Model …………………………………….. 85 Coordinates of SAP2000 3-D Model …………………………………….. 86 SAP2000 Cross Section Properties ………………………………………. 88 Material Properties used in SAP2000 ……………………………………. 89 ANSYS Solid Model – Coordinates ……………………………………… 90 ANSYS Solid Model – Cross-Section Depths …………………………… 91 vi
6.
LIST OF TABLES2.1 Kealakaha Bridge Geometric Data……………….……………………….. 72.2 Linear Soil Stiffness Data………………………………………………….. 83.1 Comparison of Vertical Deflections For Fixed Support…………………… 213.2 Comparison between Fixed Supports and Soil Springs ..…………………. 244.1 Vertical Deflection at Midspan on Test Beam: Thermal Loading………….394.2 Vertical Deflection at Midspan on Test Beam: 10 N Point Load…………. 414.3 Comparison between Four and Six Meter Mesh for ANSYS Model……… 445.1 Results of Single 320 kN Truck Point Load ….…………………………… 465.2 Vertical Deflection at Center of Bridge due to Single Truck Load (Actual Wheels Modeled) .………………………………………….. 485.3 Vertical Deflection of Bridge due to 2x2 Truck Load (Actual Wheels Modeled)………………………………………………….. 505.4 Vertical Deflection of Bridge due to 4 Truck Loading at Edge of Bridge (Actual Wheels Modeled)…………………………………………………. 556.1 Vertical Deflection due to Temperature Gradient .……………………….. 627.1.1 Modal Periods: 2-D vs. 3D ……………………………………………… 677.1.2 Modal Periods: Gross Section vs. Transformed Section………………… 687.1.3 Modal Periods: Linear Soil Spring Support vs. Fixed Supports………… 697.1.4 Modal Periods: SAP2000 vs. ANSYS…………………………………… 69 vii
7.
LIST OF FIGURES1.1 Location of Project………………………………………………………… 11.2 Elevation, Section and Plan of Kealakaha Bridge ..….……………………. 21.3 UBC 1997 Seismic Zonation ..…………………….….…………………… 31.4 Horizontal Ground Acceleration (% g) at a 0.2 Second Period with 2% Probability of Exceedance in 50 Years……………….……………………. 41.5 Horizontal Ground Accelerations (% g) at a 0.2 Second Period with 10% Probability of Exceedance in 50 Years……………………………………. 52.1 Lateral Stiffness (Longitudinal Direction)……………………..………….. 92.2 Lateral Stiffness (Transverse Direction)………………………..…………. 92.3 Rotational Stiffness (Longitudinal Direction)…………………..…………. 102.4 Rotational Stiffness (Transverse Direction)……………………..………….102.5 Design Cross Section of Kealakaha Bridge…………………….………….. 123.1 SAP2000 2-D Frame Element Model (Schematic)………………………… 143.2 SAP2000 2-D Frame Element Model (Screen Capture)..………………….. 143.3 SAP2000 3-D Frame Element Model (Schematic)………………………… 153.4 SAP2000 3-D Frame Element Model (Screen Capture).………………….. 153.5 Element Lengths in SAP2000 Models……………………………..….…… 173.6 Convergence of Original and Half Size Finite Elements………….…….…. 183.7 Schematic Drawing of a Single HS20 Truck Load ………………..……… 193.8 Single HS20 Truck Load used in Chapter 3 ………………………..……... 193.9 Deformed Shape due to Single Truck Load ..……………………………… 203.10 Comparisons Between 2-D and 3-D Model .…………………………….... 213.11 Comparison of Gross and Transformed Section Properties for 2-D Model Results ..……………………………………………………………. 223.12 Comparison of Gross and Transformed Section Properties for 3-D Model Results …..…………………………………………………………. 223.13 Difference Between Fixed Support and Soil Springs: 2-D Model …..…… 233.14 Difference Between Fixed Support and Soil Springs: 3-D Model …...…… 244.1 Side View of a Portion of the Kealakaha Bridge……………………….…. 284.2.1 Design Cross Section………………………………………………….…… 304.2.2 Simplified Cross Section……………………………………………….….. 304.3 ANSYS Solid Model Cross Section View before Meshing…………….…. 314.4 Kealakaha Bridge before Meshing, Elevation ……………………………. 324.5 Kealakaha Bridge before Meshing, Isometric View………………………. 324.6 Solid 45, Eight Node Structural Solid (ANSYS) ….……………………… 344.7 Solid 92, Ten Node Tetrahedral Structural Solid (ANSYS) ..…………….. 344.8 Square Test Beam – Thermal Loading ……………………………………. 354.9 Thermal Distribution in Test Beam……………………………………….. 364.10 Test Beam Deflection under 10° C Temperature Gradient (Auto Mesh) … 384.11 Square Test Beam – Point Loading .………………………………………. 394.12 Four Meter Mesh Size, Kealakaha Bridge (Part of Bridge)……………….. 434.13 Six Meter Mesh Size, Kealakaha Bridge (Part of Bridge)…………………. 434.14 Convergence of Four and Six Meter Mesh for ANSYS Model …………… 445.1 Distribution of Truck Loads…………………………………….…………. 45 viii
8.
5.2 ANSYS Layout of Single Truck Point Load…………………………….… 475.3 SAP2000 vs. ANSYS, Single Truck Point Load…………………...……… 475.4 Viaduct Section Showing Single Truck Load………………………………485.5 Layout of Wheel Placement for Single Truck………………………..……. 495.6 SAP2000 vs. ANSYS, Single Truck Modeled with Wheels…………...….. 495.7 Location of Axle Loads for the 2x2 Truck Configuration ……………..…. 505.8 Viaduct Section showing 2x2 Truck Configuration……………………..… 515.9 ANSYS Placement of 2x2 Truck Load ………………….………………… 515.10 SAP2000 vs. ANSYS, 2x2 Trucks Modeled with Wheels……………….... 525.11 Location of Axle Loads for Four Trucks in a Row………………………....525.12 Viaduct Section showing Four Trucks in a Row…………………..………. 535.13 ANSYS Layout of Four Trucks in a Row………………………….……… 535.14 Deflected and Non-Deflected Cross Section……………………….……… 545.15 Torsion Effects, Four Trucks in a Row………………………………….… 545.16 Isometric View of Vertical Deflection under Torsion Loading………..….. 556.1 ANSYS Applied Temperature Gradient………………………………….... 576.2 Bridge End Span Showing Effect of Thermal Gradient……………….…... 586.3 Deformation due to 10 Degrees Temperature Gradient……………….…... 596.4 Isometric View of Bridge Deformation due to Thermal Loading……....…. 596.5 Side View of Bridge Deformation due to Thermal Loading………..…..…. 606.6 Locations of Reported Deformation due to Thermal Loading…...………... 616.7 Vertical Deflection of Bridge due to Ten Degree Temperature Gradient…. 626.8 Combination of Temperature and Truck Loading…………………………. 636.9 Strain Distribution through Box Girder Depth near Pier………………..… 646.10 Strain Distribution through Box Girder Depth near Midspan……………... 646.11 Strain Output Locations……………………………………………….…… 656.12 Longitudinal Strains at Locations A and B …………………………..…… 666.13 Longitudinal Strains at Locations C and D …………………………..……. 667.1 ANSYS Mode 2……………………………………………………….…… 707.2 SAP2000 Mode 1………………………………………………………..…. 707.3 ANSYS Mode 1………………………………………………………….… 717.4 SAP2000 Mode 2……………………………………………………….….. 717.5 ANSYS Mode 3……………………………………………………………. 727.6 SAP2000 Mode 3……………………………………….……………….…. 727.7 ANSYS Mode 4………………………………………….………………… 737.8 SAP2000 Mode 4………………………………………….…………….…. 737.9 ANSYS Mode 5…………………………………………….……………… 747.10 SAP2000 Mode 5…………………………………………….………….…. 747.11 ANSYS Mode 6……………………………………………….…………… 757.12 SAP2000 Mode 6………………………………………………………..…. 757.13 ANSYS Mode 7……………………………………………….…………… 767.14 SAP2000 Mode 7……………………………………………….……….…. 767.15 ANSYS Mode 8………………………………………………….………… 777.16 SAP2000 Mode 8………………………………………….…………….…. 777.17 ANSYS Mode 9………………………………………….………………… 787.18 SAP 2000 Mode 9……………………………………….……………….… 78 ix
10.
CHAPTER 1 INTRODUCTION1.1 Project Description The project site is located along Mamalahoa Highway (Hawaii Belt Road) overthe Kealakaha stream in the District of Hamakua on the Island of Hawaii. The existingbridge, a six span concrete bridge crossing the Kealakaha Stream is scheduled forreplacement in Fall 2003. The new replacement bridge will be built on the north side ofthe existing bridge and will reduce the horizontal curve and increase the roadway widthof the existing bridge. The new bridge has been designed to withstand the anticipatedseismic activity whereas the existing bridge is seismically inadequate. Figure 1.1 showsthe location of the project on the Big Island of Hawaii. Figure 1.1: Location of Project 1
11.
The new prestressed concrete bridge will be a 3 span bridge and is approximately220 meters long and 15 meters wide and will be designed to withstand earthquake and allother anticipated loads. The new bridge will consist of three spans supported by twointermediate piers and two abutments (Figure 1.2). The center span will be a cast-in-place concrete segmental span of about 110 meters and the two outside spans will beabout 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 responseduring ambient traffic and future seismic activity. This will be the first seismicinstrumentation of a major bridge structure in the State of Hawaii. Figure 1.2: Elevation, Section and Plan of Kealakaha Bridge 2
12.
The new bridge is in an ideal location for a seismic study because of theearthquake activity on the island of Hawaii. The Island of Hawaii is in zone 4, thehighest 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 theInternational Building Code, IBC (2000). These maps are based on the USGS NationalSeismic Hazard Mapping Project (USGS 1996). The maps show earthquake groundmotions that have a specified probability of being exceeded in 50 years. These groundmotion 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 with5% 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 ofabout 500 and 2500 years, respectively. The maps assume that the earthquake hazard isindependent of time. 3
13.
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 ofexceedance in 50 years (Fig. 1.5). The acceleration due to gravity, g, is 980 cm/sec2. Figure 1.4: Horizontal Ground Acceleration (%g) at a 0.2 Second Period With 2% Probability of Exceedance in 50 Years (USGS, 1996) 4
14.
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, analyzedand compared to evaluate the structural response of the bridge to various loadingconditions. All models were linear elastic simulations in either SAP2000 (CSI 1997) orANSYS (ANSYS, 2002). 5
15.
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 thefollowing: 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
16.
CHAPTER 2 DESIGN CRITERIA FOR KEALAKAHA BRIDGE The design specifications used for the Kealakaha bridge are the AASHTO LRFDBridge Design Specification – Second Edition (1998) including the 1999 and 2000interim revisions (AASHTO, 1998). A geotechnical investigation was performed byGeolabs, Inc. in 2001 and the report was available for this study (Geolabs, 2001a).. Structural bridge data was obtained from Sato and Associates, the bridge designengineers, and from the State of Hawaii project plans titled “Kealakaha Stream BridgeReplacement, Federal Aid Project No. BR-019 2(26)” dated July 2001.2.1 Geometric Data The geometric data of the Kealakaha bridge are shown in Table 2.1. The bridgeradius and slopes were not modeled in the 2-D SAP2000 and the ANSYS models. Thebridge radius, longitudinal slope, and cross slope were included in the SAP2000 3-Dmodel.Table 2.1: Kealakaha Bridge Geometric DataDesign Speed 80 km/hourSpan Lengths 55 m – 110 m – 55mTypical Overall Structure Width 14.90 m (constant width)Bridge Radius constant radius of 548.64 mBridge 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 providedby Geolabs, Inc. in the project geotechnical report (Geolabs-Hawaii W.O. 3885-00November 17, 1998). The study was done for Sato and Associates, Inc. and the State of 7
17.
Hawaii Department of Transportation. The report summarized the findings andgeotechnical recommendations based on field exploration, laboratory testing, andengineering analyses for the proposed bridge replacement project. The recommendationswere intended for the design of foundations, retaining structures, site grading andpavements. Geolabs, Inc. provided the design engineers with linear soil stiffness duringservice conditions and extreme earthquake events using the secant modulus (Geolabs,2001). A future proposed soil investigation and a soil-structure interaction-modelingprogram 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 linearsoil spring stiffness. Figure 2.1 shows the estimated secant modulus for lateral soilstiffness in the bridge longitudinal direction with a lateral deflection of 0.0088 meters anda lateral load of 18,750 kN. Figure 2.2 shows the secant modulus for the transversedirection. The rotational stiffness in the bridge longitudinal direction was determinedfrom the secant modulus at a rotational displacement of 0.0054 rad and a moment of165,000 kN-m (Figure 2.3). Figure 2.4 shows the secant modulus for the rotationalstiffness in the bridge transverse direction. These stiffness values are used for the soilsprings in the SAP2000 frame element models at the base of both piers. The values areshown in Table 2.2.Table 2.2: Linear Soil Stiffness DataLateral StiffnessLongitudinal 2.12 X 106 kN/mTransverse 1.89 X 106 kN/mRotational StiffnessLongitudinal 3.29 X 108 kN-m/radTransverse 3.56 X 108 kN-m/rad 8
20.
2.3 Material Properties Based on the design documents obtained from Sato and Associates, three differenttypes of concrete were used to model the structure in the frame element models. Super-structure concrete was used for the bridge span, sub-structure concrete was used for theconcrete piers and abutments, and weightless concrete was used for the dummyconnectors 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 takenas 2.4 x 107 kN/m2 for the bridge superstructure and 2.1 x 107 kN/m2 for the piers andabutments.2.4 Boundary Conditions of Bridge For most computer models, the bases of the two piers were modeled as fullyfixed. In the SAP2000 soil spring model, rotational, horizontal, and vertical linear soilsprings were incorporated at the base of the piers. In all computer models, the abutmentsat each end of the bridge were modeled as roller supports in the bridge longitudinaldirection, free to rotate about all axes, but restrained against vertical and transversedisplacement.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, andcross-sectional areas were calculated for the SAP2000 models. All dimensions areconstant throughout the length of the bridge except the box girder depth, h, and thebottom slab thickness, T. These values are listed in Appendix A for the end of eachbridge segment. The cross section in Figure 2.5 is referred to as the design cross section. 11
21.
Modifications were made to simplify the cross-section for the ANSYS solid model asexplained in Chapter 4. Figure 2.5: Design Cross Section of Kealakaha Bridge 12
22.
CHAPTER 3 SAP2000 FRAME ELEMENT MODELS3.1 Development of SAP2000 Frame Element Models SAP2000 (CSI, 1997) was used to create the frame element models. Figures 3.1and 3.2 show elevation, plan and isometric views of the 2-D model. This model ignoresthe horizontal curve, longitudinal slope and cross slope. Note that although the roadwayis horizontal, the girder frame elements follow the centerline of the varying depth boxgirder 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-Dmodel. In the 3-D model, the horizontal curve with radius of 548.64 m and the verticalcurve are modeled. The vertical curve begins as a varying slope until the center of thebridge where it becomes a constant slope of –3.46 %. To model the bridge deck constantcross slope of 6.2%, moments of inertia, and centerline coordinates were recalculated forthe 3-D model. 13
23.
Figure 3.1: SAP2000 2-D Frame Element Model (Schematic)Figure 3.2: SAP2000 2-D Frame Element Model (Screen Capture) 14
24.
Figure 3.3: SAP2000 3-D Frame Element Model (Schematic)Figure 3.4: SAP2000 3-D Frame Element Model (Screen Capture) 15
25.
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 piers3.2 Element Sizes used for SAP2000 Models To model the varying cross section along the length of the bridge, the box girderwas modeled using frame element segments. Each segment had the same section andproperties. The mass of each segment was computed automatically by SAP2000 basedthe cross sectional area, concrete density, and frame element length. The frame element size was based on the construction segment length throughout thebridge. For the majority of the bridge length, 5.25 meter long elements were used. Three1.5 meter long elements were used above each pier and abutment, and three 1 meter long 16
26.
elements were used at the closure segment at the center of the middle span. Elementsused to model the piers varied in length from 1 m to 6.45 m. Figure 3.5 shows theSAP2000 2-D model. 1m 1.5 m 5.25 Figure 3.5: Element Lengths in SAP2000 modelsThese element sizes were small enough to produce valid results. An analysis using finiteelement sizes 50% smaller produced the same deflection results under a single truckloading and the same modal frequencies. Figure 3.6 shows the results of the verticaldeflection under a single truck loading. 17
27.
Sap2000 Frame Element Model Vertical Deflection with Single Truck Loading at Center Convergence of Original and Half Size Finite Elements 2 2-D No Steel Model 1 0 Vertical Deflection (mm) 0 50 100 150 200 -1 -2 -3 -4 -5 Original Size Elements -6 Half Size Elements -7 Along Length of Bridge (meters) Figure 3.6: Convergence of Original and Half Size Finite Elements3.3 Results of Frame Element Model Comparisons3.3.1 Natural Frequencies Natural frequencies, modal periods and mode shapes were determined for the firstnine modes for each of the eight SAP2000 frame element models. These results arepresented in Chapter six along with those from the ANSYS analysis.3.3.2 Static Load Deformations In order to evaluate the anticipated structural response to vehicle traffic, a numberof truck loading conditions were considered. This section presents the deflected shaperesulting from a single AASHTO HS20 truck located at midspan of the center span. Thisloading condition is used to compare the various SAP2000 models. A single truck weighsa total of 72 Kips or 320 kN. The truck scale dimensions are shown in Figure 3.7. 18
28.
Figure 3.7: Schematic Drawing of a Single HS20 Truck Load Chapter 4 shows results from modeling each axle or wheel for the HS20 loadingof Figure 3.7. In this section, a single point load of 320 kN is used to represent a singletruckload for comparisons of different computer modeling techniques as shown in Figure3.8. Figure 3.8: Single HS20 Truck Load Used in Chapter 3 19
29.
Figure 3.9 shows the deflected shape of the bridge when subjected to a singletruck 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
30.
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) 0 0 50 100 150 200 -1 -2 -3 -4 -5 2-D -6 3-D -7 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 areminimal for static deflections. At the center of the bridge, the maximum deflectionsdiffer 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 SupportFixed Support 2-D Model 3-D Model Effect of ModelModels (mm) (mm) TypeGross Section 5.92 5.85 0.07 (1.2 %)TransformedSection 5.139 5.07 0.07 ( 1.3 %)Effect ofPrestressing Steel 0.78 (13.2 %) 0.78 (13.3 %)(mm) 21
31.
2-D Sap2000 Frame Element Model Vertical Deflection With Single Truck Loading at Center Fixed Support Model With (Transformed) or Without (Gross) Prestressing 2 Steel 1Vertical Deflection (mm) 0 0 50 100 150 200 -1 -2 -3 -4 2-D Model (Gross Section) -5 -6 2-D Model (Transformed Section) -7 Along Length of Bridge (meters) Figure 3.11: Comparison of Gross and Transformed Section Properties for 2-D Model Results 3-D Sap2000 Frame Element Model Vertical Deflection With Single Truck Loading at Center Fixed Support Model With (Transformed) or Without (Gross) Prestressing 2 Steel 1 0 Vertical Deflection (mm) 0 50 100 150 200 -1 -2 -3 -4 3-D Model (Gross Section) -5 -6 3-D Model (Transformed Section) -7 Along Length of Bridge (meters) Figure 3.12: Comparison of Gross and Transformed Section Properties for 3-D Model Results 22
32.
When comparing the models with and without the prestressing steel, thedifferences are more significant. Figures 3.11 and 3.12 show the comparison betweengross 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 of0.78 mm (13.2%) and 0.78 mm (13.3%) for the 2-D and 3-D models respectively. 2-D Sap2000 Frame Element Model Vertical Deflection with Single Truck Loading at Center of Bridge 2-D Models With or Without Linear Soil Spring 2 1 Vertical Deflection (mm) 0 0 50 100 150 200 -1 -2 -3 -4 -5 Gross Section Without Linear Soil Springs -6 Gross Section With Linear Soil Springs -7 Along Length of Bridge (meters) Figure 3.13: Differences Between Fixed Supports and Soil Springs: 2-D Model 23
33.
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 1 Vertical Deflection (mm) 0 0 50 100 150 200 -1 -2 -3 -4 Gross Section Without Linear -5 Soil Springs -6 Gross Section With Linear Soil Springs -7 Along Length of Bridge (meters) 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 linearsoil 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 notaccurately reflect actual soil response to different forces. Table 3.2 shows that there areminimal differences in the vertical deflection between the fixed and spring foundationand minimal differences between the 2-D and 3-D model. For this reason, and to keep theANSYS solid model under 32,000 nodes, the solid model was generated as a straightmodel (equivalent to the SAP2000 2-D fixed geometry) using fixed supports at the piers.Table 3.2: Comparison between Fixed Supports and Soil Springs 2-D Model 3-D Model Effect of Model (mm) (mm) TypeLinear Soil Spring 5.98 5.92 0.06 (1%)Fixed Foundation 0.07 (1.2%) 5.92 5.85Effect of SoilSprings 0.06 (1%) 0.07 (1%) 24
34.
CHAPTER 4 ANSYS SOLID MODEL4.1 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-deasANSYS was the choice of software for creating the solid model. SAP2000 did not havethe capability of creating a box girder bridge with a varying cross section. SAP2000 didnot have adequate meshing capabilities and could only mesh solid models in linearelements. 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 forI-deas. Between Abaqus and ANSYS, ANSYS appeared to be the more “user friendly”software with a simple tutorial and CAD input capabilities. 25
35.
4.2 Finite Element Analysis: ANSYS, an Overview ANSYS is a finite element analysis program used for solid modeling. It hasextensive capabilities in thermal, and structural analysis. The solid model consists of key points/nodes, lines, areas and volumes withincreasing complexity in that order. Careful thought needs to be put into the modelbefore building the entire model. Once the model is meshed, volumes, areas, or linescannot be deleted if they are connected to existing meshed elements. The aspect ratio andtype of mesh must also be decided depending on the size and shape of the complete solidmodel. ANSYS contains many solid finite elements to choose from, each having its ownspecialty. First, the type of analysis must be chosen which ranges from structuralanalysis, thermal analysis, or fluid analysis. Once the type of analysis is determined, anelement 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 uniquecapabilities and consists of tetrahedral, triangle, brick, 10 node, or 20 node finiteelements both in 2-D or 3-D analysis.4.3 Solid Model GeometryThere 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
36.
• 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 frameelement 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 wasalso investigated. Autodesk Inventor had a very good CAD capability compared tocreating the model in the ANSYS CAD environment. However, attempts to import theIGES file into ANSYS were unsuccessful. The model did not import correctly due tosoftware incompatibility. The solid modeling approach was used to create the Kealakaha Bridge. Creatingthe top slab of the bridge with the “extrude” command was easy because it was the sameshape throughout the bridge. However, when creating the box girder, the cross sectionvaried throughout the length of the bridge. ANSYS did not have good CAD capabilities 27
37.
to create many volumes in 3-D space with a varying cross section. When creating thesolid volume for the box girder, each solid element had to be created using only 8 nodesat a time by using the “create volumes arbitrary by nodes” command. Creation of thefinal bridge model was accomplished by dividing the bridge into many volumes andcombining them together. Figure 4.1 shows the side view of portion of the bridge. Eachcolor represents a different area and block volume that had to be created and joinedtogether using the Boolean operation. Due to symmetry, the reflect and copy commandwas used to create the other half of the bridge. 1 AREAS FEB 19 2003 AREA NUM 11:00:21 Y Z X Figure 4.1: Side View of a Portion of the Kealakaha Bridge 28
38.
4.4 Development of Solid Model Geometry The program that was used to analyze the solid model was ANSYS/UniversityHigh Option, Version 6.1. Limitations to this software include the maximum number ofnodes which is set at 32,000 nodes. To keep the number of nodes below this limit, theoriginal cross section could not be used without having a large aspect ratio duringmeshing. To reduce the amount of nodes as well as computation time, the cross sectionmodel had to be simplified. Weng Ao (1999) performed a similar study on the NorthHalawa Valley Viaduct (NHVV), which is part of the H-3 freeway. The NHVV boxgirder shape was very similar to the Kealakaha bridge box girder. Ao used simpler crosssections 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 solidmodeling program showed good agreement with actual results for both thermal and truckloading conditions. The simplified cross section shown in Figure 4.2.2 was created by averaging thetop and bottom slab thickness of the design cross section to create an equivalent area inthe simplified cross section. The moment of inertia was changed by no more than 3% inthe lateral direction and 11% in the vertical direction.Figure 4.2.1 shows the design cross section that was used to compute section propertiesfor the frame element models in SAP2000. Figure 4.2.2 shows the simplified crosssection used for the solid model in ANSYS. The depths and heights that vary are listed inthe Appendix. 29
40.
1 VOLUMES FEB 19 2003 TYPE NUM 11:02:06 Y Z X Figure 4.3: ANSYS Solid Model Cross Section before MeshingFigure 4.3 shows a close up view of the simplified cross section in ANSYS. Figures 4.4and 4.5 show the completed solid model before meshing. The piers have fixed supportswhile the abutment ends are restrained against vertical and lateral movementperpendicular to the bridge. 31
41.
1 VOLUMES FEB 20 2003 TYPE NUM 11:27:15 U Y Z X Figure 4.4: Kealakaha Bridge before Meshing, Elevation1 VOLUMES FEB 20 2003 TYPE NUM 11:26:02 U Y Z X Figure 4.5: Kealakaha Bridge before Meshing, Isometric View 32
42.
4.5 Meshing in ANSYS Meshing in ANSYS can be applied manually or automatically. The element typeselected (Linear vs. Tetrahedral), and the mesh size can affect the accuracy of the resultsof the analysis. Due to the large model size, automatic meshing was not possible for theentire Kealakaha bridge. In automatic meshing, ANSYS automatically chooses ameshing size based on the shape of the model. This resulted in more elements thanpermitted by the University High Option of ANSYS. Manual meshing allows the user todefine the maximum size of the elements. To guide the selection of element type, a test beam was created in ANSYS todetermine what solid finite element produced the best results for deflection under thermalloading. There are two types of elements in ANSYS that have both structural andthermal 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 todetermine which element produced the best results when compared to the theoreticalvalues. 33
43.
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 longby one meter thick and one meter high. The sample test beam was also created to test theperformance of ANSYS under thermal loading conditions. Simply supported endconditions were used for the test beam as shown in Figure 4.8. 34
44.
10 Degrees 10 m1m Temp Gradient Figure 4.8: Square Test Beam-Thermal Loading A 10-degree temperature gradient was produced by applying two differenttemperatures at the top and bottom surfaces of the beam. A temperature gradient isanticipated 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 perdegrees Celsius for this test beam. Figure 4.9 shows the distribution of the temperaturethat 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 expansioncoefficient used in the Kealakaha bridge model will be based on concrete cylinder testsand is expected to be in the range of 10 to 11X10-5 per degree Celsius. For the thermalanalysis performed in this study, a value of 11X10-5 per degree Celsius was used for theKealakaha bridge model. Concrete properties similar to the top slab of the Kealakahabridge was used for the test beam. 35
45.
1 NODAL SOLUTION FEB 19 2003 STEP=1 11:33:04 SUB =1 TIME=1 BFETEMP (AVG) RSYS=0 DMX =.001304 SMX =10 Y MX Z X MN 0 2.222 4.444 6.667 8.889 1.111 3.333 5.556 7.778 10 Figure 4.9: Thermal Distribution in Test Beam 36
46.
4.7 Analytical Solution For Test Beam The deformation due to a linear temperature change can be expressed as: d dv α∆T = dx dx h where v = Vertical Deflection α = 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 beamTherefore, dv α∆T x + A = dx h 1 α∆T 2 v= x + Ax + B 2 hwhere A and B are integration constants.Applying boundary conditions: At x=0, v(0)=0 and at x=10, v(10)=0 and substituting thenumerical values into the equation, we obtain: v = (50-5x)x*10-5 At the midspan, x = 5 meters therefore: v = 0.00125 metersThere should be a maximum deflection of 0.00125 meters at the center of the test beam. 37
47.
Figure 4.10 shows the deflection result of the test beam in ANSYS due to the 10 degreestemperature gradient using the solid 92 element. The automatic meshing tool was usedwhich produced element sizes close to 0.5 meters. 1 DISPLACEMENT FEB 19 2003 STEP=1 11:32:31 SUB =1 TIME=1 DMX =.001304 Y Z X 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 thermalloading conditions. Varying the element size from 0.25 to 1 meter had very little effecton the vertical deflection under thermal loading. The theoretical result is 1.25 mm for thevertical deflection at midspan. The percentage error in Table 4.1 is the error compared tothe theoretical result. 38
48.
Table 4.1: Vertical Deflection at Midspan on Test Beam: Thermal Loading Vertical Deflection at Percentage Error Midspan (mm)Theoretical Result 1.25 -Solid45 1.128 9.8%Eight Node Structural Solid(Brick Node)Solid 92 1.304 4.3%Ten Node Structural SolidTetrahedral ShapedSolid 92 gave the lowest percentage error of 4.3% when compared with the analyticalresult.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 beamusing different element types and sizes as shown in Figure 4.11. 10 N (at midspan of beam)1m 10 m Figure 4.11: Square Test Beam – Point Loading 39
49.
For a simply supported beam under a midspan point load, the theoretical deflection is: Vertical Deflection ∆ = − PL 3 48 EIwhere P = Load at midspan = 10 N on test beam L = Length of beam = 10 m for test beam E = Modulus of Elasticity = 2.4X107 kN/m2 for test beam = Moment of Inertia = bh 3 I 12 = 1 m4for test beam 12Substituting the numerical values produces the following theoretical result: ∆ = 1.041X10-7 m down Table 4.2 lists the comparisons between the Solid 45 and Solid 92 elements forthe vertical deflection at the midspan due to a 10 N point load. The theoretical result willnot match the result from ANSYS because the theoretical result does not include sheardeformation. However, the % difference between the theoretical and ANSYS will beused. The results show that Solid 92 consistently predicted deflections close to thetheoretical result with the percent difference ranging from 3.2 to 5.4%. The solid 45results 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
50.
Table 4.2: Vertical Deflection at Midspan on Test Beam: 10 N Point Load Solid45 Solid 92Element Size Eight Node Structural Solid Ten Node Structural Solid (Brick Node) Tetrahedral Shaped Vertical % Vertical % Deflection at Difference Deflection at Difference Midspan From Midspan From -7 -7 (X10 m) Theoretical (X10 m) TheoreticalAutomatic Meshing 1.128 8.3 1.09 4.70.25 meters 1.178 13.2 1.08 3.70.5 meters 0.961 7.7 1.09 4.71 meter 0.472 55 1.1 5.6Theoretical Result 1.041 X10-7m 1.041 X10-7m Structural Solid 92 was selected for meshing the Kealakaha Bridge model.Solid 92 has a quadratic displacement behavior and is well suited to model irregulargeometries 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 workingdirectory. In thermal analysis, one must transfer the element type from a structuralelement to thermal element so that thermal loads can be applied linearly. This isimportant because if the program is in structural element mode, the temperatures willonly be applied at the surface of the beam, and will not be applied linearly throughout theentire beam. After running the thermal analysis, the .rth file must be imported into thestructural element mode with Solid 92 and applied as a “temperature from thermalanalysis.” After running the structural analysis, structural deformation/stress/strain resultsare produced. 41
51.
4.10 Mesh Generation for Kealakaha Bridge Model ANSYS has the capability of doing automatic meshing where it automaticallypicks an element size. However, automatic meshing may not produce the best results andcannot be used for the 220 meter Kealakaha bridge because it will produce over 32,000nodes which exceeds the University program capability. The “mesh tool” command mustbe used to specify the element size. Based on the specified element size, ANSYS will mesh the model to produce thebest results. The element size will not be the same for all elements, but all elements willbe smaller than the specified size. The mesh size used for the Kealakaha bridge was 4 meters. A similar mesh sizeof 12 feet was used in the NHVV study by Weng Ao (1999), and produced good resultswhen compared with measured deflections. Figure 4.12 shows the 4 meter mesh for aportion of the bridge. The full bridge consisted of 24,576 nodes and 12,246 elements.4.11 Convergence of 4 Meter Mesh To confirm that the four-meter mesh converges with a larger size mesh, a sixmeter mesh was created and the response to a single truck load was compared. SeeFigure 3.8 for a description of the single truck load. The four-meter mesh is seen inFigure 4.12 and the six-meter mesh is shown in Figure 4.13. 42
52.
1 ELEMENTS FEB 20 2003 11:14:11Figure 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
53.
ANSYS Solid Model Vertical Deflection with Single Truck loading at center of bridge Convergence of Four Meter Mesh Vs. Six Meter Mesh 2 1 Vertical Deflection (mm) 0 0 50 100 150 200 -1 -2 -3 -4 -5 4 Meter Mesh -6 6 Meter Mesh -7 Distance Along Bridge (meters) Figure 4.14: Convergence of Four and Six Meter Mesh for ANSYS ModelTable 4.3: Comparison between Four and Six Meter Mesh for ANSYS Model Six Meter Mesh Four Meter Mesh Difference (%) Vertical Vertical Deflection Deflection (mm) (mm) Maximum End 0.94 0.96 0.02 (2.1%)Span DeflectionMaximum Center -5.73 -5.73 0 (0%)Span Deflection The results plotted in Figure 4.14 show convergence between a four meter meshand a six meter mesh. The results at the maximum deflection for the end span and centerspan 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 spandeflection. Therefore, a four-meter mesh is adequate for this analysis. 44
54.
CHAPTER 5 ANSYS SOLID MODEL ANALYSIS5.1 Truck Loading Conditions According to the design criteria on the construction plans, a typical truck weighs atotal 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 forthe ANSYS solid model. The total axle load shown in Figure 5.1 is divided by two to getthe load for each wheel. In ANSYS, loads can only be applied to existing nodesproduced by the mesh. The mesh size used was 4 meters, so the loads were placed at theclosest possible node to produce the actual wheel location. Three different truck-loading conditions were considered in this analysis. In all ofthese analyses, the truck placement was symmetrical about the midspan of the center spanof the bridge. The three loading conditions are: 45
55.
• 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 frameelement analysis, each axle was modeled as a load. ANSYS and SAP2000 model resultsare compared in the following sections. In addition, the SAP2000 frame element model and the ANSYS solid model werealso compared when a single 320 kN point load was applied at the center of the roadwayat midspan of the center span.5.2 Truck Loading Results5.2.1 Single 320 kN (72 Kip) Point Load Figure 5.2 shows the single 320 kN truck point load applied to the top slab of theANSYS model. Figure 5.3 shows a comparison between SAP2000 and ANSYS whileTable 5.1 shows the vertical displacement under the 320 kN point load. The maximum deflection from the SAP2000 model is less than the ANSYSmodel, but at all other nodes the ANSYS model yielded slightly less deflections. Thelocal deformation of the top slab under the single concentrated load does not correctlyrepresent the effect of the truck loading.Table 5.1: Results of Single 320 kN Truck Point Load Sap2000 ANSYS Difference Single Truck Load Single Truck LoadVertical Deflection at 0.4Center of Bridge Span (mm) -5.92 -6.32 (6.7%)Maximum End Span 0.03Deflection (mm) 1.04 1.01 (2.9%) 46
56.
1 2 ELEMENTS ELEMENTS U U F F Z Y X 3 ELEMENTS U F Y Z X Figure 5.2: ANSYS Layout of Single Truck Point Load SAP2000 Vs. ANSYS Single Truck (Point Load) at Center of Bridge 2 1Vertical Deflection (mm) 0 0 50 100 150 200 -1 -2 -3 -4 -5 ANSYS -6 SAP2000 -7 Along Length of Bridge (meters) Figure 5.3: SAP2000 vs. ANSYS, Single Truck Point Load 47
57.
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 ANSYS Difference Axle Modeled Each Wheel (mm) ModeledVertical Deflection at Centerof Bridge Span (mm) -5.69 -5.73 0.04 mm (0.6%)Maximum End SpanDeflection (mm) 0.98 0.97 0.2 mm (3.2%) Figure 5.4 Viaduct Section Showing Single Truck Load 48
58.
1 2 ELEMENTS ELEMENTS U U F 5.25 m F 10.38 m Z Y X 3 ELEMENTS U F Y Z X 3.12 m Figure 5.5: Layout of Wheel Placement for Single Truck SAP2000 Vs. Ansys Single Truck Load at Center Of Bridge ANSYS: Each Wheel Modeled SAP2000: Each Axle Modeled 2 1Vertical Deflection (mm) 0 0 50 100 150 200 -1 -2 -3 -4 -5 ANSYS -6 SAP2000 -7 Along Length of Bridge (meters) Figure 5.6: SAP2000 vs. Ansys, Single Truck Modeled with Wheels 49
59.
5.2.3 2x2 Truck Loading Figure 5.7 shows the locations of the axles for the 2x2 truck loading. Figure 5.8shows the viaduct section under the 2x2 truck loading. The trucks are placedsymmetrically about the center span to reduce computational time for the analysis andproduce symmetrical deflected shapes. The axle spacing is larger than as shown inFigure 5.1 due to limited node locations available for applying the loads. Figure 5.9shows the layout of the 2x2 truck loading in ANSYS. The vertical deflection results areshown 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) SAP2000 Each ANSYS Difference Axle Modeled Each Wheel (mm) ModeledVertical Deflection atCenter of Bridge Span -19.49 -19.17 0.32 mm (1.6%)(mm)Maximum End SpanDeflection 3.77 3.61 0.16 mm (4.2%)(mm) Midspan of Bridge Center Span Figure 5.7: Location of Axle Loads for the 2x2 Truck Configuration 50
60.
Figure 5.8: Viaduct Section showing 2x2 Truck Configuration1 2 ELEMENTS ELEMENTS U U F F Z Y X 3 ELEMENTS U F Y Z X Figure 5.9: ANSYS Placement of 2x2 Truck Load 51
61.
SAP2000 Vs ANSYS 2X2 Truck Load, 4 Trucks Total ANSYS: Each Wheel Modeled SAP2000: Each Axle Modeled 5 0 Vertical Deflection (mm) 0 50 100 150 200 -5 -10 -15 ANSYS -20 SAP2000 -25 Length Along Bridge (meters) Figure 5.10: SAP2000 vs. ANSYS, 2x2 Truck Modeled with Wheels5.2.4 4 Truck Loading Creating Torsion Effects. 4 truck loads were placed at the edge of the viaduct cross section to study torsioneffects due to eccentric loading. Figure 5.11 shows the locations of the axle loadings forthe trucks. The trucks are placed symmetrically about the center span of the bridge toreduce the computational time for the analysis and to generate a symmetrical deflectedshape. Midspan of bridge center span Figure 5.11: Location of Axle Loads for Four Trucks in a Row 52
62.
The 4 trucks modeled at the right edge of the viaduct section are shown in Figure5.12. Figure 5.12 show the locations “A,” “B,” and “C,” where the vertical deflectionswere recorded. Location “C” is at the middle of the cross section. Location “B” is on theside of the truck loading above the box girder stem and location “A” is on the oppositeside 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 U F F Z Y X 3 ELEMENTS U F Y Z X Figure 5.13: ANSYS Layout of Four Trucks in a Row 53
63.
Figure 5.14 shows the deflected and non-deflected shape of the cross section modeled inANSYS at midspan of the center span of the bridge, the legend at the bottom shows thevertical deflection in meters. Locations “A,” “B,” and “C” are shown at the top of theslab (See Figure 5.12 for more precise locations). The result of the vertical deflectiondue to the truck load are shown in Figure 5.15. 1 Truck Y Z X A C B -.02163 -.015896 -.010162 -.004427 .001307 -.018763 -.013029 -.007295 -.00156 .004174 Figure 5.14: Deflected and Non-Deflected Cross Section ANSYS: Torsion Effects 4 Trucks in a Row at Edge of Bridge ANSYS: Each Wheel Represented By One Load 5 0 Vertical Deflection (mm) 0 50 100 150 200 -5 -10 Location A Location B -15 Location C (Center) -20 Along Length of Bridge (meters) Figure 5.15: Torsion Effects, Four Trucks in a Row 54
64.
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 andright sides of the bridge cross section at the center span and a 0.57 mm difference in themaximum 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 ANSYS % Difference Location A Location B (torsion effect) (Left) (Right)Vertical Deflection at Centerof Bridge Span (mm) -16.20 -18.63 2.43 (13.0%)Maximum End SpanDeflection (mm) 3.71 3.14 0.57 (15.4%) Figure 5.16 shows an isometric view of the bridge with color contours for thevertical 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 MX DMX =.021714 SMN =-.02163 SMX =.004174 MN Y Z X -.02163 -.015896 -.010162 -.004427 .001307 -.018763 -.013029 -.007295 -.00156 .004174 Figure 5.16: Isometric View of Vertical Deflection under Torsion Loading 55
66.
CHAPTER 6 TEMPERATURE ANALYSIS6.1 Temperature Gradient Figure 6.1: ANSYS Applied Temperature Gradient Figure 6.1 show the temperature gradient applied to the ANSYS solid model. A10 degrees Celsius linear temperature gradient is applied through the 0.35 m thick topslab. The temperature gradient was based on temperature measurements from the NHVV(Ao, 1999). Below the top slab, the temperature was assumed constant at zero degreesthroughout the box girder, and piers. This thermal loading develops by mid afternoondue to solar radiation on the top surface of the bridge. Thermocouples will be installed inthe Kealakaha Bridge to record the exact temperature gradients after the bridge is built. The coefficient of thermal expansion used for this analysis was 11X10-5 perdegrees Celsius. 57
Be the first to comment