User Manual - PEER - University of California, Berkeley

BridgePBEE: OpenSees 3D Pushover and
Earthquake Analysis
of Single-Column 2-span Bridges
User Manual (Beta 1.0)
http://peer.berkeley.edu/bridgepbee/
Jinchi Lu, Kevin Mackie, and Ahmed Elgamal
December 2011
Table of Contents
Introduction ............................................................................................................................. 1 1.1 Overview .......................................................................................................................... 1 1.2 System Requirements ....................................................................................................... 2 1.3 Acknowledgments ............................................................................................................ 3 1.4 Units ................................................................................................................................. 4 2 Getting Started ........................................................................................................................ 5 2.1 Start-Up ............................................................................................................................ 5 2.2 Interface ............................................................................................................................ 5 2.2.1 Menu Bar .................................................................................................................. 6 2.2.2 Model Input Window ................................................................................................ 7 2.2.3 Finite Element Mesh Window .................................................................................. 8 3 Bridge Model .......................................................................................................................... 9 3.1 Column Parameters ........................................................................................................ 10 3.1.1 Column Linear Material Properties ........................................................................ 11 3.1.2 Nonlinear Fiber Section .......................................................................................... 12 3.1.3 Column below Grade .............................................................................................. 17 3.2 Bridge Deck Parameters ................................................................................................. 17 3.3 Embankment Parameters ................................................................................................ 18 3.4 Abutment Parameters ..................................................................................................... 19 3.4.1 Elastic Abutment ..................................................................................................... 19 3.4.2 Roller Model ........................................................................................................... 21 3.4.3 Simplified Model (SDC 2004) ................................................................................ 22 3.4.4 Spring Model .......................................................................................................... 26 3.4.5 SDC (2010) Sand .................................................................................................... 30 3.4.6 SDC (2010) Clay..................................................................................................... 30 3.4.7 EPP-Gap Model ...................................................................................................... 30 3.4.8 HFD Model ............................................................................................................. 32 4 Soil Parameters ..................................................................................................................... 32 5 Pushover & Eigenvalue Analyses ......................................................................................... 37 5.1 Load Pattern ................................................................................................................... 37 5.1.1 Pushover by User-Defined Load Pattern (U-Push) ................................................. 38 5.2 Output for Pushover Analysis ........................................................................................ 40 5.2.1 Column Response Time Histories and Profiles ...................................................... 41 5.2.2 Column Response Relationships............................................................................. 41 5.2.3 Abutment Force-Displacement and Response Time Histories ............................... 42 5.2.4 Deformed Mesh ...................................................................................................... 42 5.3 Eigenvalue Analysis ....................................................................................................... 43 6 PBEE Analysis (Ground Shaking) ........................................................................................ 45 6.1 Theory and Implementation of PBEE Analysis ............................................................. 45 6.2 Input Necessary for User-defined PBEE Quantities ...................................................... 48 6.3 Definition/specification of PBEE input motion ensemble (suite) .................................. 49 6.3.1 Available Ground Motions ..................................................................................... 49 6.3.2 Specifications of PBEE Input Motions ................................................................... 50 1 i
6.4 Save Model and Run Analysis ....................................................................................... 54 6.5 PBEE Analysis ............................................................................................................... 55 6.5.1 PBEE Quantities ..................................................................................................... 56 6.5.2 Compute Repair Cost & Time ................................................................................ 58 6.5.3 Compute Hazard Curves ......................................................................................... 59 6.5.4 Compute Disaggregation ........................................................................................ 60 7 Time History and PBEE Output ........................................................................................... 61 7.1 Time History Output Quantities ..................................................................................... 61 7.1.1 Column Response Time Histories and Profiles ...................................................... 64 7.1.2 Column Response Relationships............................................................................. 70 7.1.3 Abutment Responses Time Histories ...................................................................... 73 7.1.4 Deformed Mesh ...................................................................................................... 76 7.1.5 Soil Response Time Histories ................................................................................. 77 7.1.6 PBEE Output Quantities ......................................................................................... 81 7.1.7 Bridge Peak Accelerations for All Motions ............................................................ 88 7.1.8 Maximum Column & Abutment Forces for All Motions ....................................... 90 7.2 PBEE Outcomes ............................................................................................................. 93 7.2.1 Repair Cost & Time ................................................................................................ 93 7.2.2 Hazard Curves ......................................................................................................... 96 7.2.3 Disaggregation ...................................................................................................... 100 7.2.4 EPS Version of All PBEE Figures ........................................................................ 102 8 Appendix A: How to Define the Soil Finite Element Mesh ............................................... 104 9 Appendix B: Simple Pushover Examples (Bridge on Rigid Ground) ................................ 113 10 Appendix C: How to Incorporate User-defined Motions ................................................... 118 11 Appendix D: Calculation of Steel and Concrete Material Properties ................................. 122 12 Appendix E: Customization of PBEE Quantities ............................................................... 127 13 References ........................................................................................................................... 132 ii
List of Figures
Fig. 1. Coordinate system in BridgePBEE...................................................................................... 3 Fig. 2. BridgePBEE main window.................................................................................................. 5 Fig. 3. BridgePBEE’s menu and submenu bars: a) menu bar; b) menu File; c) menu Execute; d)
menu Display; and e) menu Help.................................................................................................... 6 Fig. 4. BridgePBEE copyright and disclaimer window .................................................................. 7 Fig. 5. Buttons available in the Finite Element Mesh window ....................................................... 8 Fig. 6. BridgePBEE main window (defining a bridge model) ........................................................ 9 Fig. 7. Bridge Model window ....................................................................................................... 10 Fig. 8. Steps to define the elastic properties of the column .......................................................... 11 Fig. 9. Steps to define a nonlinear Fiber Section .......................................................................... 12 Fig. 10. Fiber Section window ...................................................................................................... 13 Fig. 11. Column fiber section (based on PEER best modeling practices report, Berry and
Eberhard, 2007)............................................................................................................................. 13 Fig. 12. Stress-strain curve for Steel02 material (default values employed; “C” represents
compression and “T” represents tension) ..................................................................................... 15 Fig. 13. Stress-strain curve of Concrete02 material for the core concrete (default values
employed; “C” represents compression and “T” represents tension) ........................................... 15 Fig. 14. Stress-strain curve of Concrete02 material for the cover concrete (default values
employed; “C” represents compression and “T” represents tension) ........................................... 16 Fig. 15. Moment-curvature response for the column (with default steel and concrete parameters,
and the deck weight 11,915 kN applied at the column top).......................................................... 16 Fig. 16. Steps to define the deck geometrical configuration and material properties ................... 17 Fig. 17. Elastic abutment model ................................................................................................... 19 Fig. 18. Steps to define Elastic abutment model ........................................................................... 20 Fig. 19. Longitudinal force-displacement relationship for the Elastic abutment model ............... 20 Fig. 20. Roller abutment model .................................................................................................... 21 Fig. 21. Steps to define a Roller abutment model ......................................................................... 21 Fig. 22. Longitudinal force-displacement relationship for the Roller abutment model................ 22 Fig. 23. General scheme of the Simplified abutment model (Aviram et al., 2008) ...................... 22 Fig. 24. Longitudinal backbone curve force-displacement relationship (two on each end of the
bridge; Caltrans SDC, 2004) ......................................................................................................... 23 Fig. 25. Steps to define the Simplified abutment model. .............................................................. 24 Fig. 26. Longitudinal force-displacement relationship for the Simplified abutment model: a)
longitudinal direction; b) transverse direction .............................................................................. 25 Fig. 27. General scheme of the Spring abutment model (Aviram et al. 2008) ............................. 27 Fig. 28. Steps to define a Spring abutment model ........................................................................ 28 Fig. 29. Force-displacement relationship for the Spring abutment model: a) longitudinal direction;
b) transverse direction. .................................................................................................................. 29 Fig. 30. Steps to define a SDC 2010 Sand abutment model ......................................................... 30 Fig. 31. Steps to define a SDC 2010 Clay abutment model ......................................................... 31 Fig. 32. Steps to define an EPP-Gap abutment model .................................................................. 31 Fig. 33. Steps to define a HFD abutment model: a) choosing HFD model at the bridge model
window; b) HFD model window .................................................................................................. 33 iii
Fig. 34. Analysis options .............................................................................................................. 34 Fig. 35. Beam-column element types available for column ......................................................... 34 Fig. 36. Rayleigh damping coefficients ........................................................................................ 35 Fig. 37. Soil strata definition......................................................................................................... 35 Fig. 38. User-defined clay material U-Clay2 ................................................................................ 36 Fig. 39. Steps to define a load pattern for pushover analysis ....................................................... 37 Fig. 40. Load pattern for pushover analysis .................................................................................. 38 Fig. 41. Steps to define a user-defined load pattern (U-Push) ...................................................... 39 Fig. 42. Example of user-defined pushover load pattern (U-Push) .............................................. 40 Fig. 43. Response time histories and profiles for column (and pile shaft) ................................... 41 Fig. 44. Response relationships for column (and pile shaft)......................................................... 41 Fig. 45. Abutment response time histories.................................................................................... 42 Fig. 46. Deformed mesh and contour fill ...................................................................................... 42 Fig. 47. Steps to perform an Eigenvalue analysis ......................................................................... 43 Fig. 48. Sample output for an Eigenvalue analysis ....................................................................... 44 Fig. 49. Schematic procedure of the LLRCAT methodology for a single bridge component ...... 46 Fig. 50. Steps to define PBEE motions ......................................................................................... 51 Fig. 51. PBEE input motions widow ............................................................................................ 52 Fig. 52. Intensity measures, time histories and response spectra of individual record ................. 53 Fig. 53. Histogram and cumulative distribution for the whole input motion set .......................... 53 Fig. 54. Intensity Measures (IM) table for the whole input motion set ........................................ 54 Fig. 55. Options to change number of records to be run at the same time ................................... 54 Fig. 56. OpenSees analysis in progress......................................................................................... 55 Fig. 57. PBEE analysis window .................................................................................................... 55 Fig. 58. Damage states window .................................................................................................... 56 Fig. 59. Repair quantities window ................................................................................................ 57 Fig. 60. Unit Costs window .......................................................................................................... 57 Fig. 61. Production Rates window ................................................................................................ 58 Fig. 62. Post-processing capabilities (menu options) available in a pushover analysis ............... 62 Fig. 63. Post-processing capabilities (menu options) available in a base shaking analysis.......... 62 Fig. 64. Analysis options in BridgePBEE..................................................................................... 63 Fig. 65. Steps to display output for a different input motion: a) click menu Display (Fig. 3); b)
select an input motion ................................................................................................................... 64 Fig. 66. Menu items to access the column response time histories and response profiles ........... 66 Fig. 67. Response time histories and profiles for column (and pile shaft): displacement is shown
at the nodes (only one element is used above ground). ................................................................ 67 Fig. 68. Bending moment profile in the longitudinal plane .......................................................... 67 Fig. 69. Response summary .......................................................................................................... 68 Fig. 70. Column longitudinal displacement response time histories: a) response profiles at
specific load steps; b) response time histories at different elevations .......................................... 69 Fig. 71. Column longitudinal acceleration response time histories at different elevations (freefield and input accelerations are also included) ............................................................................ 70 Fig. 72. Menu items to access the column response relationships................................................ 71 Fig. 73. Column response output options ..................................................................................... 71 Fig. 74. Load-displacement curve at column top .......................................................................... 72 Fig. 75. Moment-curvature curve at column top .......................................................................... 72 iv
Fig. 76. Menu items to access the abutment responses................................................................. 73 Fig. 77. Menu items to access the abutment responses................................................................. 74 Fig. 78. Abutment response time histories (scroll down to see all directions): a) abutment forcedisplacement relationships; b) relative deck-end/abutment displacement time histories; c)
resisting force time histories; and d) abutment pile cap time histories ......................................... 75 Fig. 79. Menu items to access the deformed mesh ....................................................................... 76 Fig. 80. Deformed mesh................................................................................................................ 77 Fig. 81. Menu items to access the soil responses .......................................................................... 78 Fig. 82. Response options for soil time histories .......................................................................... 79 Fig. 83. Planes for locations of the soil response time histories ................................................... 79 Fig. 84. Locations of soil response time histories ......................................................................... 80 Fig. 85. Soil settlement time histories under abutment ................................................................. 80 Fig. 86. Finite element mesh in BridgePBEE: Node O – Column base node (at ground surface);
Node A – Column top node; Node B – Deck-end node; Node C – Abutment top node (having
the same coordinates as Node B); Nodes B are C are connected by an abutment model; Node D
– Abutment pile cap node ............................................................................................................. 82 Fig. 87. Code snippet to calculate the tangential drift ratio of column ......................................... 83 Fig. 88. Menu items to access the PG quantities for all motions .................................................. 85 Fig. 89. PG quantities for all motions (scroll down to see all 11 PGs) ......................................... 86 Fig. 90. Converting figures to EPS format ................................................................................... 86 Fig. 91. Lognormal standard deviations (beta values) for each PG: a) table format; b) bar graph
format ............................................................................................................................................ 87 Fig. 92. Menu items to access bridge peak accelerations for all motions ..................................... 88 Fig. 93. Bridge peak accelerations for all motions: a) maximum bridge accelerations; b)
maximum column base accelerations; and c) maximum free-field accelerations ........................ 90 Fig. 94. Menu items to access maximum column & abutment forces for all motions ................. 91 Fig. 95. Maximum column & abutment forces for all motions: a) maximum column shear forces;
b) maximum column bending moments; and c) maximum abutment forces................................ 92 Fig. 96. Contribution to expected repair cost ($) from each performance group ......................... 93 Fig. 97. Total repair cost ratio (%) as a function of intensity ....................................................... 94 Fig. 98. Contribution to expected repair cost ($) from each repair quantity ................................ 94 Fig. 99. Contribution to repair cost standard deviation ($) from each repair quantity ................. 95 Fig. 100. Total repair time (CWD: Crew Working Day) as a function of intensity ..................... 95 Fig. 101. Contribution to expected repair time (CWD) from each repair quantity ...................... 96 Fig. 102. Mean annual frequency of exceedance (ground motion) .............................................. 97 Fig. 103. Return period against total repair cost ratio................................................................... 98 Fig. 104. Mean annual frequency of exceedance (loss) against total repair cost ratio ................. 98 Fig. 105. Return period against total repair time .......................................................................... 99 Fig. 106. Mean annual frequency of exceedance (loss) against total repair time ......................... 99 Fig. 107. Disaggregation of expected cost by performance group ............................................. 100 Fig. 108. Disaggregation of expected repair cost by repair quantities........................................ 101 Fig. 109. Disaggregation of expected repair time by repair quantities ....................................... 102 Fig. 110. Converting all PBEE figures to EPS format ................................................................ 103 Fig. 111. Schematic view of an idealized single bent bridge system ......................................... 104 Fig. 112. General meshing controlling parameters (default values) ........................................... 105 Fig. 113. Meshing controlling parameters for horizontal direction (default values) .................. 106 v
Fig. 114. Adjusting mesh near embankment: a) before adjusting; b) after adjusting ................. 107 Fig. 115. Meshing controlling parameters for vertical direction (default values) ...................... 108 Fig. 116. Finite element mesh created with default values ......................................................... 109 Fig. 117. Mesh refinement example 1: a) Change “Num of Slices” to 32; b) the resulting mesh
..................................................................................................................................................... 110 Fig. 118. Mesh refinement example 2: a) Change “Number of Mesh Layers” in the vertical
direction; b) the resulting mesh................................................................................................... 111 Fig. 119. Mesh refinement example 3: a) Change meshing controlling parameters in the
horizontal direction; b) the resulting mesh ................................................................................. 112 Fig. 120. Cantilever beam simulation using BridgePBEE .......................................................... 114 Fig. 121. Fixed-end beam simulation using BridgePBEE .......................................................... 115 Fig. 122. Deck deformation under gravity (the maximum displacement is 0.0372 m) .............. 116 Fig. 123. Fixed end-roller beam analytical solution (from efunda.com) .................................... 116 Fig. 124. Longitudinal pushover ................................................................................................. 117 Fig. 125. Transverse pushover .................................................................................................... 117 Fig. 126. Choosing PBEE motion set ......................................................................................... 119 Fig. 127. Directory structure of PBEE motion set ...................................................................... 120 Fig. 128. Sample .info file .......................................................................................................... 120 Fig. 129. Sample .data file .......................................................................................................... 121 Fig. 130. Example of user-defined motion ................................................................................. 121 Fig. 131. Visual Studio file PBEE.SLN ...................................................................................... 128 Fig. 132. Modifying file PBEE.CPP ........................................................................................... 129 Fig. 133. Building PBEE.DLL in Visual Studio 2005................................................................ 130 Fig. 134. Replacing file PBEE.DLL under the installation folder .............................................. 131 vi
List of Tables
Table 1. Default Values for Column RC Section Properties ........................................................ 14 Table 2. Default Values for Steel02 Material Properties .............................................................. 14 Table 3. Default values for Concrete02 Material Properties ........................................................ 14 Table 4. Default Values for Bridge Deck ..................................................................................... 18 Table 5. Default Values for Deck Material Properties ................................................................. 18 Table 6. Geometric and Material Properties of a Bearing Pad ..................................................... 27 Table 7. Spring Abutment Model Properties ................................................................................ 28 Table 8. Abutment Configurations ............................................................................................... 28 Table 9. Clay material properties .................................................................................................. 36 Table 10. PBEE Repair Quantities................................................................................................ 59 Table 11. PBEE Performance Groups .......................................................................................... 81 vii
1 Introduction
1.1 Overview
BridgePBEE is a PC-based graphical pre- and post-processor (user-interface) for conducting
Performance-Based Earthquake Engineering (PBEE) studies for bridge-ground systems. The user
interface allows for:
 Management of ground motions
 Simplified structure and soil mesh generation
 Simplified assignment of material properties for both the soil and structure
 Time history and PBEE analyses
 Visualization of output data
The interface is unique because it enables complete PBEE studies in a single GUI-driven
package. The PBEE implementation employed is based on Pacific Earthquake Engineering
Research (PEER) Center’s performance-based earthquake engineering framework (Cornell and
Krawinkler, 2000). The framework includes several building blocks (intermediate probabilistic
models) that allow the user to generate probabilistic estimates of repair cost and repair time
(consequences or decision variables) directly. These results are obtained seamlessly in the
interface alongside more traditional outputs such as displacements, strains, etc.
The intermediate models require:
 Hazard model that uses earthquake ground motion data to determine an intensity measure
(IM)
 Demand model uses response from dynamic analysis to determine an engineering
demand parameter (EDP)
 Damage model connects the EDP to a damage measure (DM) or discrete set of damage
states (DS)
 Repair model describes repair methods and repair quantities (Q) necessary to return the
DSs to original functionality
 Loss model links Qs to consequences that are termed the decision variables (DV). Repair
cost and repair time can be thought of as two possible decision variable (DV) outcomes
characterized probabilistically by the framework.
The models are required for each performance group (PG). PGs represent a collection of
structural components that act as a global-level indicator of structural performance and that
contribute significantly to repair-level decisions. Performance groups are not necessarily the
same as load-resisting structural components. The complete analysis is accomplished using the
local linearization repair cost and time methodology (LLRCAT), detailed more in Chapter 6. The
interface handles all of the above-mentioned intermediate models and provides default data for
the case of reinforced concrete box girder bridges.
The decision variables that can be generated as output are the repair cost ratio (RCR), or the ratio
of repair cost to replacement cost, and the repair time (RT) or repair effort, measured in terms of
1
crew working days (CWD). These outcomes are presented graphically as loss models
conditioned on earthquake intensity. In addition, site-specific ground motion hazard can be
specified, and the user-interface will then also generate loss hazard curves (mean annual
frequencies of exceeding different loss levels). The loss hazard curves are presented graphically
as mean annual frequencies or return periods.
An important feature of the interface is that the PBEE analysis can be executed sequentially:
ground motion selection, time history analysis, loss modeling, hazard, and visualization.
However, once a final selection of geometry and materials has been made (the FEA model is not
changing), the time history analyses do not need to be repeated. These are the most time and
resources intensive portions of the complete analyses. Once the time history results are computed,
the user may perform what-if scenarios by changing any of the parameters of the intermediate
damage, loss, and hazard models. The PBEE portions of the analysis do not require recomputing
the time history results unless the model is changed or a new selection of ground motions is
made.
Finite element computations are conducted using OpenSees (http://opensees.berkeley.edu,
Mazzoni et al. 2009), an open source framework developed by the Pacific Earthquake
Engineering Research (PEER) Center. The current version of the interface is limited to ordinary
bridge overpasses with two spans and a single-column bent. The analysis options available in
BridgePBEE include:
 Pushover Analysis
 Modal Analysis
 Single 3D Base Input Acceleration Analysis
 Full Performance-Based Earthquake Engineering (PBEE) Analysis
This document describes how to conduct the above analyses in BridgePBEE. For information on
how to download and install BridgePBEE, please visit the BridgePBEE website
(http://peer.berkeley.edu/bridgepbee/).
The coordinate system employed in BridgePBEE is shown in Fig. 1. The origin is located at the
column base (the ground surface).
1.2 System Requirements
BridgePBEE runs on PC compatible systems using Windows (NT V4.0, 2000, XP, Vista or
Windows 7). The system should have a minimum hardware configuration appropriate to the
particular operating system.
Internet Explorer 3.0 or above (or compatible Browser) with Java Applet enabled is needed to
view the graphic results. For best results, your system’s video should be set to 1024 by 768 or
higher.
2
Transverse axis: Y
Vertical axis: Z
Longitudinal axis: X
Fig. 1. Coordinate system in BridgePBEE
1.3 Acknowledgments
This research was funded in part by the Pacific Earthquake Engineering Research (PEER) Center
Transportation Program (Dr. Stephen Mahin, Director and Dr. Yousef Bozorgnia, Executive
Director). Dr. Steven Kramer (U. of Washington, Seattle) coordinated a review process of
BridgePBEE. Feedback and suggestions provided by Dr. Kramer and the anonymous reviewers
are greatly appreciated.
OpenSees (currently ver. 2.1.0 is employed) is a software framework (Mazzoni et al. 2009) for
developing applications to simulate the performance of structural and geotechnical systems
subjected to earthquakes (for more information, visit http://opensees.berkeley.edu/). Throughout,
Dr. Frank McKenna was always generous and gracious with his assistance in matters related to
OpenSees. The employed OpenSees geotechnical simulation capabilities were developed by Dr.
Zhaohui Yang and Dr. Ahmed Elgamal. For more information, please visit
http://cyclic.ucsd.edu/opensees/. The implemented PBEE analytical framework is provided by Dr.
Kevin Mackie (U. Central Florida). For questions or remarks, please send email to Dr. Jinchi Lu
(jinlu@ucsd.edu), Dr. Kevin Mackie (Kevin.Mackie@ucf.edu), or Dr. Ahmed Elgamal
(elgamal@ucsd.edu).
BridgePBEE is written in Microsoft Visual C++ 2005 with Microsoft Foundation Class (MFC)
Library version 8.0. The Java Applet package used to display graphical results in BridgePBEE
3
is obtained from the website http://ptolemy.eecs.berkeley.edu/. GIF images are generated with
GNUPLOT for MS-Windows 32 bit Version 3.7, available at http://www.gnuplot.org/.
1.4 Units
The SI unit system is used throughout the user interface. For conversion between SI and English
Units, please check:
http://www.unit-conversion.info/
Some commonly used quantities can be converted as follows:
 1 kPa =
0.14503789 psi
 1 psi =
6.89475 kPa
 1m =
39.37 in
 1 in =
0.0254 m
4
2 Getting Started
2.1 Start-Up
On Windows, start BridgePBEE from the Start button or from an icon on your desktop. To Start
BridgePBEE from the Start button:
1. Click Start, and then select Programs.
2. Select the BridgePBEE folder
3. Click on BridgePBEE
The BridgePBEE main window is shown in Fig. 2.
Fig. 2. BridgePBEE main window
2.2 Interface
There are 3 main regions in the BridgePBEE window – menu bar, the model input window, and
the finite element mesh window.
5
2.2.1 Menu Bar
The menu bar, shown in Fig. 3, offers rapid access to most BridgePBEE main features.
a)
b)
c)
d)
e)
Fig. 3. BridgePBEE’s menu and submenu bars: a) menu bar; b) menu File; c) menu Execute; d)
menu Display; and e) menu Help
6
BridgePBEE’s main features are organized into the following menus:
 File: Controls reading, writing and printing of model definition parameters, and exiting
BridgePBEE.
 Execute: Controls running analyses.
 Display: Controls displaying of the analysis results.
 Help: Visit the BridgePBEE website and display the copyright/Disclaimer message (Fig. 4).
Fig. 4. BridgePBEE copyright and disclaimer window
2.2.2 Model Input Window
The model input window controls definitions of the model and analysis options, which are
organized into three regions (Fig. 2):
 Step 1: Define Model: Controls analysis types (pushover analysis, eigenvalue analysis or
ground shaking) and analysis options; also controls definitions of bridge and soil strata
including material properties. Meshing parameters are also defined.
7
 Step 2: Execute FE Analysis: Controls execution of the finite element analysis and display the
progress bar.
 Step 3: Compute Repair Cost: Controls the PBEE analysis.
2.2.3 Finite Element Mesh Window
The finite element mesh window (Fig. 2) displays the generated mesh. In this window, the mesh
can be rotated by dragging the mouse, moved in 4 directions by pressing keys of LEFT ARROW,
RIGHT ARROW, UP ARROW or DOWN ARROW respectively. The view can be zoomed in
(by pressing key ‘F9’), out (by pressing key ‘F10’) or frame (by pressing key ‘F11’).
To display a 2D view, press key ‘F2’ (for Plane XY, where X is the longitudinal direction, Y the
transverse direction), ‘F3’ (for Plane YZ, where Z is the vertical direction) or ‘F4’ (for Plane XZ).
An isometric view of the mesh can be achieved by pressing key ‘F5’.
Alternatively, users can use the corresponding buttons shown in Fig. 5.
Fig. 5. Buttons available in the Finite Element Mesh window
8
3 Bridge Model
To define a bridge model, click Bridge Parameters in the Model Input window (Fig. 6).
Fig. 7 displays the Bridge Model window. For a single-bent bridge, essentially four parts are
needed to define: column, deck, embankment and abutment.
Fig. 6. BridgePBEE main window (defining a bridge model)
9
Column parameters
Embankment parameters
Deck parameters
Abutment parameters
Fig. 7. Bridge Model window
3.1 Column Parameters
Parameters to define the geometrical configurations of the column include (refer to Fig. 7):
 Circular: column cross section type. Currently only circular cross section is available.
 Diameter: column diameter, which is 1.22 m by default.
 Total Column Length: the total length of the column including the pile shaft below
grade. The default value is 12 m.
 Column Length above Grade: the length of the column above grade. The default value
is 6.71 m.
To define the material properties of the column, click Column Properties. There are 2 scenarios
in this case:
1) Linear material properties will be defined if Linear Column is checked.
2) Nonlinear Fiber Section will be defined if Linear Column is unchecked.
Please see next section for detailed information.
10
3.1.1 Column Linear Material Properties
To define the linear material properties of the column, follow the steps shown in Fig. 8.
Parameters to define a linear column include (Fig. 8):
 Young’s Modulus: Young’s Modulus of the column. The default value is 3 × 107 kPa.
 Moment of Inertia @ Transverse Axis: the default value I = πD4/64 = 0.108745 m4
(where D -- column diameter, D = 1.22 m by default). The default value is for the gross
moment of inertia; it can be reduced as desired by the user to better capture cracked
column properties.
 Moment of Inertia @ Longitudinal Axis: calculation for the default value is the same
as the above.
 Cross-Section Area: the default value (0.7854 m2) is calculated based on the circular
cross-section with a diameter of 1.22 m.
 Mass Density: the mass density of the column. The default value is 2.4 ton/m3.
Elastic beam-column elements (elasticBeamColumn, Mazzoni et al. 2009) are used for the
column in this case.
Step 2: Click Column
Properties
Step 1: check Linear
Column
Step 3: Define values in
this window
Fig. 8. Steps to define the elastic properties of the column
11
3.1.2 Nonlinear Fiber Section
To define the nonlinear Fiber section for the column, follow the steps shown in Fig. 9. The
window to define the Fiber section is shown in Fig. 10. Nonlinear beam-column elements with
fiber section (Fig. 11) are used to simulate the column/pile shaft in this case. Forced-based beamcolumn elements (nonlinearBeamColumn, Mazzoni et al. 2009) are used for the column (1
element, number of integration points = 5) as well as the pile shaft below grade (number of
integration points = 3). The default values for the material properties of the column/pile shaft are
shown in Tables 1-3.
Step 2: Click Column
Properties.
Step 1: make sure Linear
Column is unchecked.
Fig. 9. Steps to define a nonlinear Fiber Section
By default, the Steel02 material in OpenSees (Mazzoni et al. 2009) is employed to simulate the
steel bars and Concrete02 material is used for the concrete (core and cover). Steel02 is a uniaxial
Giuffré-Menegotto-Pinto material that allows for isotropic strain hardening. Concrete02 is a
uniaxial material with linear tension softening. The default values for the material properties of
the Fiber section are listed in Table 2 for Steel02 and Table 3 for Concrete02 (core and cover).
The Concrete02 material parameters were obtained from the Mander (1988) constitutive
relationships for confined and unconfined concrete. More details on the derivation of the default
values and the OpenSees uniaxialMaterial definitions used for each material are shown in
Appendix D.
12
Fig. 10. Fiber Section window
Fig. 11. Column fiber section (based on PEER best modeling practices report, Berry and
Eberhard, 2007)
13
Table 1. Default Values for Column Reinforced Concrete (RC) Section Properties
Parameter
Value
Longitudinal bar size (US #)
10
Longitudinal steel %
2
Transverse bar size (US #)
7
Transverse steel %
1.6
3
Steel unit weight (kN/m )
77
Steel yield strength (kPa)
460,000
3
22.8
Concrete unit weight (kN/m )
Concrete unconfined strength (kPa)
27,600
Table 2. Default Values for Steel02 Material Properties
Parameter
Value
Typical range
Steel yield strength (kPa)
460,000
345,000-470,000
Young’s modulus (MPa)
200,000
Strain-hardening ratio*
0.01
0.005-0.025
Controlling parameter R0**
15
10-20
Controlling parameter cR1**
0.925
-Controlling parameter cR2**
0.15
-*The strain-hardening ratio is the ratio between the post-yield stiffness and the initial elastic
stiffness.
**The constants R0, cR1 and cR2 are parameters to control the transition from elastic to plastic
branches.
Table 3. Default values for Concrete02 Material Properties
Parameter
Core
Cover
Elastic modulus (MPa)
25,312
25,312
Compressive strength (kPa)
-46,457
-27,600
Strain at maximum strength
-0.00367
-0.002
Crushing strength (kPa)
-44,979
0
Strain at crushing strength
-0.036
-0.006
Ratio between unloading slope
0.1
0.1
Tensile strength (kPa)
6504
3864
Tensile softening stiffness (kPa) 1,771,820
1,932,000
Figs. 12-14 show the stress-strain curves for the steel, core, and cover concrete materials,
respectively. These plots can be obtained for updated material properties directly from the
interface by clicking on the corresponding View Stress-Strain buttons in the Column Material
Properties window (Fig. 10). The moment-curvature response for the column is shown in Fig. 15
(generated with consideration of the overall deck weight 11,915 kN applied at the column top).
14
Fig. 12. Stress-strain curve for Steel02 material (default values employed; “C” represents
compression and “T” represents tension)
Fig. 13. Stress-strain curve of Concrete02 material for the core concrete (default values
employed; “C” represents compression and “T” represents tension)
Important note: The above-displayed graphics applet allows for mouse-driven zoom
capability (To zoom, just left-click and drag at the desired location)
15
Fig. 14. Stress-strain curve of Concrete02 material for the cover concrete (default values
employed; “C” represents compression and “T” represents tension)
Fig. 15. Moment-curvature response for the column (with default steel and concrete parameters,
and the deck weight 11,915 kN applied at the column top)
16
3.1.3 Column below Grade
If Use Different Properties for Column below Grade is checked (Fig. 7), the column below
grade can be different from the portion above grade. In this case, the column below grade is
assumed to be elastic only. The column diameter and the Young’s Modulus are required to
define (Fig. 7) the properties of this elastic column below grade.
3.2 Bridge Deck Parameters
To define the deck, please follow the steps shown in Fig. 16. The default values are listed in
Tables 4 and 5 below. The default values were obtained from a two-cell reinforced concrete box
girder deck configuration.
Step 2: click Deck
Properties.
Step 3: define deck
properties.
Step 1: define deck
length, width and depth.
Fig. 16. Steps to define the deck geometrical configuration and material properties
17
Table 4. Default Values for Bridge Deck
Parameter
Value
Deck length (m)
90.0
Deck width (m)
11.9
Deck depth (m)
1.83
Table 5. Default Values for Deck Material Properties
Parameter
Value
Elastic modulus (MPa)
28,000
Shear modulus (MPa)
11,500
Cross-section area (m2)
5.72
Moment of inertia @
2.81
transverse axis (m4)
Moment of inertia @ vertical
53.9
axis (m4)
Weight per unit length (kN/m) 130.3
3.3 Embankment Parameters
The geometric configuration of the embankments is shown in Fig. 2 by the triangular shapes to
the right and left of the bridge deck. These geometric triangular configurations are simply
represented by relatively rigid beam-column elements. This simple idealization of the
embankment allows for (Fig. 7) representation of the distributed self-weight of soil embankment
(if present) and a depth of embankment/abutment foundation into the soil mesh. The user will
specify the embankment length in the longitudinal bridge direction, depth of the embankment
below grade, and total weight of the embankment (the user must calculate this parameter to
match the mass of the actual soil embankment). The embankment parameters will have no effect
in the rigid ground simulation cases, but will contribute when the bridge is supported on soil
mesh.
In addition, a single pile represented only by beam-column elements (i.e., cross-sectional
geometry of the pile is not represented) may be included by the user (Fig. 7) to further support
the embankment/abutment. The single pile is positioned below the embankment geometric
configuration (closest to the bridge, and aligned with the bridge longitudinal axis). This option is
activated by selecting the checkbox Activate Abutment Pile. Length of this additional pile can
be specified as well as its diameter. The material properties of this pile can be the same as the
bridge’s central column, or can be defined independently by clicking “Define” as shown in Fig.
7. Upon clicking define, a window similar to that of Fig. 10 will open and the user can follow the
procedures associated with Fig. 10 as described earlier.
18
3.4 Abutment Parameters
Abutment behavior, soil-structure interaction, and embankment flexibility have been found by
post-earthquake reconnaissance reports to significantly influence the response of the entire
bridge system under moderate to strong intensity ground motions. Specifically, for Ordinary
Standard bridge structures in California with short spans and relatively high superstructure
stiffness, the embankment mobilization and the inelastic behavior of the soil material under high
shear deformation levels dominate the response of the bridge and the intermediate column bents
(Kotsoglu and Pantazopoulou, 2006, and Shamsabadi et al. 2007, 2010). Seven abutment models
are implemented in BridgePBEE. The abutment models are defined as Elastic, Roller, Simplified
(SDC 2004), Spring (SDC 2004), SDC 2010 Sand, SDC 2010 Clay, and EPP-Gap abutment
models.
3.4.1 Elastic Abutment
The elastic abutment model (Fig. 17) consists of a simple set of 6 translational elastic springs at
each end of the bridge (see schematic below): 2 longitudinal, 2 transverse, and 2 vertical springs.
By default, no additional rotational springs are specified, but can be added by the user.
Fig. 17. Elastic abutment model
To define an Elastic abutment model, please follow the steps shown in Fig. 18. The typical forcedisplacement curve for the Elastic abutment model is shown in Fig. 19.
19
Step 3: enter parameters
for Elastic abutment
model
Step 1: select Elastic.
Step 2: click Define.
Fig. 18. Steps to define Elastic abutment model
Fig. 19. Longitudinal force-displacement relationship for the Elastic abutment model
20
3.4.2 Roller Model
The roller abutment model (Fig. 20) consists of rollers in the transverse and longitudinal
directions, and a simple boundary condition module that applies single-point constraints against
displacement in the vertical direction (i.e., bridge and abutment are rigidly connected in the
vertical direction). These vertical restraints also provide a boundary that prevents rotation of the
deck about its axis (torsion).
Fig. 20. Roller abutment model
This model can be used to provide a lower-bound estimate of the longitudinal and transverse
resistance of the bridge, that may be displayed through a pushover analysis. To define a Roller
abutment model, please follow the steps shown in Fig. 21. The typical force-displacement curve
for the Roller abutment model is shown in Fig. 22.
Step 3: enter
parameters for Roller
b t
t
d l
Step 1: select
Step 2: click Define.
Fig. 21. Steps to define a Roller abutment model
21
Fig. 22. Longitudinal force-displacement relationship for the Roller abutment model
3.4.3 Simplified Model (SDC 2004)
The simplified model of the embankment-abutment system provides several nonlinear springs to
better represent abutment-bridge interaction that is neglected with the elastic or roller abutment
models. The general scheme of the simplified model is presented in Fig. 23. It consists of a rigid
element of length dw (superstructure width), connected through a rigid joint to the superstructure
centerline, with defined longitudinal, transverse and vertical nonlinear response at each end.
Fig. 23. General scheme of the Simplified abutment model (Aviram et al., 2008)
22
The longitudinal response defined for the simplified model accounts only for the gap and the
embankment fill response, where passive pressures are produced by the abutment back wall (Fig.
23). The shear resistance of bearing pads connecting the bridge to the abutment wall is ignored.
In the longitudinal direction (Fig. 23), a gap element is assigned an elastic-perfectly-plastic (EPP)
backbone curve after gap closure with abutment stiffness ( K abut ) and ultimate strength ( Pabut )
obtained from section 7.8.1 of the Caltrans SDC (2004), see Fig. 24. There is no stiffness in the
longitudinal direction when the deck pulls away from the abutment.
The stiffness and strength are calculated using the SDC equations:
 h 
K abut  11500 .0 w

 1 .7 
(1)
 h 
Pabut  239.0 wh

 1 .7 
(2)
Where w is the width of the back wall (unit: m) and h is the height of the back wall (unit: m). In
the current implementation, the width of the back wall is taken as the bridge deck width minus
twice of the bridge deck depth. The units of K abut and Pabut are kN/m and kN, respectively.
Fig. 24. Longitudinal backbone curve force-displacement relationship (two on each end of the
bridge; Caltrans SDC, 2004)
In the transverse direction, a zero-length element is defined at each end of the rigid link with an
assigned Elastic perfectly plastic (EPP) backbone curve representing the wing wall and pile
resistance, similar to the longitudinal backbone. The transverse backbone is obtained by
multiplying the longitudinal backbone by CL = 2/3 and CW = 4/3 and is mobilized immediately
(there is no gap in the transverse direction). The resistance of the brittle shear keys and
distributed bearing pads is ignored in this model for simplicity. Skew changes the orientation of
the rigid link at the end of the deck segment.
23
In the vertical direction, an elastic spring is defined at each end of the rigid link, with a stiffness
corresponding to the vertical stiffness of the embankment soil mass. The embankment is
assumed to have a trapezoidal shape and based on the effective length formulas from Zhang and
Makris (2002), the vertical stiffness ( K v , unit: 1/m) can be calculated from (Zhang and Makris,
2002):
E sl d w
Kv 
z H
(3)

z 0 ln 0
 z0 
Where H is the embankment height, d w is the deck width, z 0  0.5d w S , S is the embankment
slope (parameter in window, see Fig. 20), E sl  2.8G , G  V s 2 ,  and Vs are the mass density
and the shear wave velocity of the embankment soil, respectively (parameters in window, see Fig.
25).
To define a Simplified abutment model, please specify the parameters shown in Fig. 25. The
typical force-displacement curve for the Simplified abutment model is shown in Fig. 26.
Fig. 25. Steps to define the Simplified abutment model.
24
a)
b)
Fig. 26. Longitudinal force-displacement relationship for the Simplified abutment model: a)
longitudinal direction; b) transverse direction
25
3.4.4 Spring Model
A more complex abutment model was developed by Mackie and Stojadinovic (2006), including
sophisticated longitudinal, transverse, and vertical nonlinear abutment response, as well as a
participating mass corresponding to the concrete abutment and mobilized embankment soil. A
system of zero-length elements is distributed along two rigid elements oriented in the transverse
bridge direction. The discrete zero-length elements represent each component of the abutment
that contributes to the combined behavior and allow for differential response in each element as
the superstructure rotates about the vertical bridge axis. A general scheme of this abutment
model is presented in Fig. 27. The bearing pads create a series system between the two transverse
rigid elements (Rigid element 1 and 2 in Fig. 27). Rigid element 1 is connected to the deck end
by a rigid joint. The longitudinal elastomeric bearing pad response and gap closure behavior are
illustrated by L1 in Fig. 27. The number and distribution of the bearing pads is defined according
to the number and location of the girders in the box, with plan and thickness dimensions
according to plans or specifications. The longitudinal backfill, back wall, and pile system
response are accounted for by the two zero-length elements at the extreme locations of rigid
element 2, designated as L2.
Longitudinal response: The longitudinal response is based on the system response of the
elastomeric bearing pads, gap, abutment back wall, abutment piles, and soil backfill material.
Prior to impact or gap closure, the superstructure forces are transmitted through the elastomeric
bearing pads to the stem wall, and subsequently to the piles and backfill, in a series system. After
gap closure, the superstructure bears directly on the abutment back wall and mobilizes the full
passive backfill pressure.
Transverse Response: The transverse response is based on the system response of the
elastomeric bearing pads, exterior concrete shear keys, abutment piles, wing walls, and backfill
material. The bearing pad model discussed above is used with uncoupled behavior with respect
to the longitudinal direction. The constitutive model of the exterior shear keys is derived from
experimental tests (Megally et al., 2003). The parallel system of transverse bearing pads and
shear keys are labeled T1 in Fig. 27.
Vertical Response: The vertical response of the abutment model includes the vertical stiffness
of the bearing pads (V1) in series with the vertical stiffness of the trapezoidal embankment (V2).
The user can modify the vertical tensile force factor for the bearing pads (multiplier on the
vertical bearing strength). The embankment stiffness per unit length of embankment was
obtained from Zhang and Makris (2000) and modified using the critical length to obtain a
lumped stiffness.
Model Characteristics
Each bearing pad has a height (h) of 0.0508 m (2 in) and a side length (square) of 0.508 m (20
in). The properties of a bearing pad are listed in Table 6.
The abutment is assumed to have a nominal mass proportional to the superstructure dead load at
the abutment, including a contribution from structural concrete as well as the participating soil
26
mass. An average of the embankment lengths obtained from Zhang and Makris (2002) and
Werner (1994) is included in the calculation of the participating mass due to the embankment of
the abutment. The user can modify the lumped mass through the soil mass.
Fig. 27. General scheme of the Spring abutment model (Aviram et al. 2008)
Table 6. Geometric and Material Properties of a Bearing Pad
Shear Modulus G
1034.2 kPa (0.15 ksi)
Young’s Modulus E
34473.8 kPa (5 ksi)
Yield Displacement
150% shear strain
GA
(where A is the cross-section area and h is the height)
Lateral Stiffness
h
EA
Vertical Stiffness
h
Vertical Tearing Stress
15513.2 kPa (2.25 ksi)
To define a Spring abutment model, please follow the steps shown in Fig. 28. The default values
for the Spring abutment model are shown in Tables 7 & 8. The typical force-displacement curve
for the Spring abutment model is shown in Fig. 29.
27
Fig. 28. Steps to define a Spring abutment model
Table 7. Spring Abutment Model Properties
Parameter
Value
Soil mass (Mg)
150
Skew angle (degree)
0
Soil shear wave velocity (m/s) 150
Embankment slope
2
3
Soil mass density (kg/m )
1,760
Longitudinal gap (m)
0.1016
Table 8. Abutment Configurations
Parameter
Value
Number of bearings
3
Bearing height (m)
0.051
Number of shear keys
2
Shear key height (m)
1.83
28
a)
b)
Fig. 29. Force-displacement relationship for the Spring abutment model: a) longitudinal direction;
b) transverse direction.
29
3.4.5 SDC (2010) Sand
This model is similar to the Simplified (SDC 2004) abutment model, but employs the parameters
of the most recent SDC (2010) for a sand backfill Embankment. To define a SDC 2010 Sand
abutment model, please follow the steps shown in Fig. 30.
3.4.6 SDC (2010) Clay
This model is similar to the Simplified (SDC 2004) abutment model, but employs the parameters
of the most recent SDC (2010) for a Clay backfill Embankment. To define a SDC 2010 Clay
abutment model, please follow the steps shown in Fig. 31.
Fig. 30. Steps to define a SDC 2010 Sand abutment model
3.4.7 EPP-Gap Model
This model is similar to the Simplified (SDC 2004) abutment model, but employs user defined
parameters for the stiffness, maximum resistance, and gap size between bridge-deck and backwall. To define an EPP-Gap abutment model, please follow the steps shown in Fig. 32.
30
Fig. 31. Steps to define a SDC 2010 Clay abutment model
Fig. 32. Steps to define an EPP-Gap abutment model
31
3.4.8 HFD Model
As suggested by Shamsabadi et al. (2007, 2010), a Hyperbolic Force-Displacement (HFD)
relationship is employed to represent abutment resistance to bridge displacement in the
longitudinal direction (Fig. 33). In this HFD model, resistance appears after a user-specified gap
is traversed (Fig. 33b), and the bridge thereafter gradually mobilizes the abutment’s passive earth
pressure strength. Herein, this strength is specified according to Shamsabadi et al. (2007, 2010)
at 265 kPa (for a nominal 1.7 m bridge deck height), with full resistance occurring at a passive
lateral displacement of 0.09 m (the sand structural backfill scenario). Similarly, abutment
resistance to the transverse bridge displacement is derived from the longitudinal hyperbolic
force-displacement relationship according to the procedure outlined in Aviram et al. (2008).
To define an HFD abutment model, please follow the steps shown in Fig. 33.
4 Soil Parameters
First, some important master control options are defined by clicking “Analysis Options” as
shown in Fig. 6. This will display the interface shown in Fig. 34 below. The following
modifications can be made in this window:
1. Select to keep the soil properties as defined by their linear properties, or opt to conduct
nonlinear soil computations (note that the default is Linear),
2. Select from among a number of available Brick elements in OpenSees,
3. Conduct more than one earthquake simulation at a time when performing a PBEE multi
earthquake record analysis,
4. Apply own weight of the soil using a global lateral stress coefficient, and a single value of
Young’s modulus that is user defined (this will reduce initial shear stresses in the mesh due to
own weight application, but generally may have minimal impact on the subsequent earthquake
computations anyway),
5. by clicking on “Change OpenSees Options” (Fig. 35 you can change the beam-column
element type (advanced feature, please exercise with care), and
6. by clicking on “Change Rayleigh Damping” (Fig. 36) you can change the viscous damping
characteristics of the model.
The soil parameters section (Fig. 37 below) is activated by clicking “Soil Parameters” in Fig. 6. .
Here the horizontally stratified soil profile can be defined layer by layer (as many as 10 layers as
shown in Fig. 37 below). Currently, only the cohesive soils are available to select (e.g., by
clicking on the U-Clay2 section in Fig. 37, and then selecting any of the available soil types (stiff,
medium and soft clay or U-Clay2 in Fig. 38).
32
a)
b)
Fig. 33. Steps to define a HFD abutment model: a) choosing HFD model at the bridge model
window; b) HFD model window
33
Fig. 34. Analysis options
Fig. 35. Beam-column element types available for column
If you select “Activate Tension Cutoff for Cohesive Soil” as shown in Fig. 37, the soil shear
strength will become negligible when volumetric stress is tensile, allowing for instance the pile
to pull away without resistance from the adjacent clay on the side where tension between the pile
and soil might contribute (this is an advanced feature and should be exercised with care).
34
Fig. 36. Rayleigh damping coefficients
Fig. 37. Soil strata definition
35
Fig. 38. User-defined clay material U-Clay2
The properties of the cohesive stiff, medium, and soft clay models are shown in Table 9 below:
Table 9. Clay material properties
Soft Clay
Mass density
1.3
(ton/m3)
Reference shear
1.3x104
modulus (kPa)
Reference bulk
6.5x104 kPa
modulus (kPa)
Cohesion (kPa)
18
Peak shear strain
0.1
Friction angle
0
(degree)
Pressure dependent
0
coefficient
Medium Clay
Stiff Clay
1.5
1.8
6.0x104
1.5x105
3.0x105 kPa
7.5x105
37
0.1
75
0.1
0
0
0
0
The above-mentioned soil models are based on earlier research (Elgamal et al 2003; Elgamal and
Lu 2009; Elgamal et al 2009; Elgamal et al 2009b; Elgamal 2010; Lu 2006; Yang et al 2003).
Finally, the soil meshing procedures are discussed in Appendix A.
36
5 Pushover & Eigenvalue Analyses
To conduct a pushover analysis, a load pattern must be defined (please follow the steps shown in
Fig. 39). The load pattern window is shown in Fig. 40. Please see Appendix B for pushover
examples.
Fig. 39. Steps to define a load pattern for pushover analysis
5.1 Load Pattern
The pushover options include monotonic pushover as well as pushover by a user-defined loading
pattern (U-Push). Please see the next section for how to define a U-Push file.
Two methods of pushover are available (Fig. 40): force-based and displacement-based. If ForceBased Method is chosen, please enter the parameters of force increment (per step):
Longitudinal (X) Force, Transverse (Y) Force, Vertical (Z) Force, Moment @ X, Moment
@ Y, and Moment @ Z.
37
If Displacement-Based Method is chosen, please enter the displacement increment parameters
(per step): Longitudinal Displacement, Transverse Displacement, Vertical Displacement,
Rotation around X, Rotation around Y, and Rotation around Z.
The pushover load/displacement linearly increases with step in a monotonic pushover mode. The
load/displacement is applied at the column top.
Fig. 40. Load pattern for pushover analysis
5.1.1 Pushover by User-Defined Load Pattern (U-Push)
To define your own load pattern (U-Push), please follow the steps shown in Fig. 41. The U-Push
window is shown in Fig. 42. Click Select/Change Pushover File to change file. The userdefined pushover file should contain single-column data.
38
Step 1: click U-Push.
Step 2: click
Define U-Push.
Fig. 41. Steps to define a user-defined load pattern (U-Push)
39
Fig. 42. Example of user-defined pushover load pattern (U-Push)
5.2 Output for Pushover Analysis
Output windows for a pushover analysis include:
 Response time histories and profiles for column (and pile shaft under grade)
 Response relationships (force-displacement as well as moment-curvature) for column
(and pile shaft under grade)
 Abutment response time histories
 Deformed mesh, contour fill, and animations.
40
5.2.1 Column Response Time Histories and Profiles
Fig. 43. Response time histories and profiles for column (and pile shaft)
5.2.2 Column Response Relationships
Fig. 44. Response relationships for column (and pile shaft)
41
5.2.3 Abutment Force-Displacement and Response Time Histories
Fig. 45. Abutment response time histories
5.2.4 Deformed Mesh
Fig. 46. Deformed mesh and contour fill
42
5.3 Eigenvalue Analysis
To conduct an Eigenvalue analysis, please follow the steps shown in Fig. 47 and then click Save
Model & Run Analysis. Fig. 48 shows the output window for an Eigenvalue analysis, which can
be accessed by clicking menu Display (Fig. 3) and then choosing Deformed Mesh.
Fig. 47. Steps to perform an Eigenvalue analysis
43
a)
b)
Fig. 48. Sample output for an Eigenvalue analysis
44
6 PBEE Analysis (Ground Shaking)
To conduct a single earthquake analysis or a full PBEE analysis, the “Ground Shaking” option
under Analysis Type (Fig. 2) is used. For that purpose, the input earthquake excitation(s) must be
specified. Input files at http://peer.berkeley.edu/bridgepbee/ that exercise this option include
Examples 2-5. If only one earthquake record is selected out of a specified ensemble (suite) of
input motions, then a conventional single earthquake analysis will be performed.
6.1 Theory and Implementation of PBEE Analysis
In the user interface, an implementation of the Pacific Earthquake Engineering Research (PEER)
Center’s performance-based earthquake engineering framework (Cornell and Krawinkler, 2000)
is used to generate probabilistic estimates of repair cost and repair time. The PEER PBEE
framework utilizes the total probability theorem to compute the desired probability distributions
by disaggregating the task into several intermediate probabilistic models with different sources
of randomness and uncertainty. The hazard model uses earthquake ground motion data to
determine an intensity measure (IM). The demand model uses response from dynamic analysis to
determine an engineering demand parameter (EDP). The damage model connects the EDP to a
damage measure (DM). Then, the DM is linked to consequences that are termed the decision
variables (DV). Repair cost and repair time can be thought of as two possible decision variable
(DV) outcomes characterized probabilistically by the framework.
The complete analysis is accomplished using the local linearization repair cost and time
methodology (LLRCAT), described by Mackie et al. (2010) and depicted conceptually in Fig. 49.
In the LLRCAT methodology, each bridge system is disaggregated into independent structural or
non-structural components or subassemblies defined as performance groups (PGs) that are
damaged, assessed, and repaired together using a specific combination of different repair
methods. Demands on the bridge system (and components) are determined using 3D nonlinear
time history analysis under multiple-component earthquake excitation. The damage in each of
the PGs is characterized according to several discrete damage states (DSs) that are defined by
distributions of critical EDPs.
A feature of the LLRCAT implementation used is the introduction of a repair model between the
original PEER abstraction of DM and DV. Jumping directly from DMs to repair costs is difficult
to accomplish, because it skips over the details of repair design and the variability of cost and
time estimating. Creating these two additional models makes it easier to implement a step-bystep procedure for defining the models. The repair model and cost model are created through the
process of schematic design of repairs and estimating the costs of those designs. Different repair
methods are employed for the various damage states of each PG or bridge component. The repair
methods for each PG require a combination of several repair quantities (Qs). Repair quantities
for all PGs are then combined with due consideration of the correlation between components.
Repair costs (RC) are obtained through a unit cost (UC). Repair times (RT) are obtained through
a production rate (PR). The PRs are in terms of crew working days (CWD), representing one
working day for a normal sized crew and can be combined later by construction management
experts to obtain total site construction times.
45
Fig. 49. Schematic procedure of the LLRCAT methodology for a single bridge component
The characterization and visualization of the ground motion suites using different choices of IMs
will be discussed in Section 6.3. The FEM, parameter selection, analysis options, and outcomes
that generated EDPs were similarly covered in Section 3. The bridge is then broken down into
performance groups (PGs) for each major bridge superstructure, substructure, and foundation
component. Each performance group represents a collection of structural components that act as
a global-level indicator of structural performance and that contribute significantly to repair-level
decisions. Performance groups are not necessarily the same as load-resisting structural
components. For example, non-structural components may also form a performance group, since
they also suffer damage and contribute to repair costs. The notion of a performance group also
allows grouping several components together for related repair work. For example, it is difficult
to separate all of the individual structural components that comprise a seat-type abutment (shear
key, back wall, bearings, approach slab, etc.) as they all interact during seismic excitation and
their associated repair methods are coupled. Therefore, the abutment repair group incorporates
the fact that repairs to the back wall require excavation of the approach slab.
Performance groups also address the issue of potentially double counting related repair items.
Some repair items require the same preparation work such as soil excavation. For example, both
back wall repair and enlargement of an abutment foundation require at least 4 ft of excavation
behind the back wall. If these repair items were in different PGs, then double counting the
excavation would be a problem. Bundling these related repair methods within a PG allows for
independent consideration of each PG. The correlation between repair items from the PGs is
handled at the demand model level in the methodology. A total of 11 PGs are considered: PG1:
Max column drift ratio; PG2: Residual column drift ratio; PG3: Max relative deck-end/abutment
displacement (left); PG4: Max relative deck-end/abutment displacement (right); PG5: Max
bridge-abutment bearing displacement (left); PG6: Max bridge-abutment bearing displacement
(right); PG7: Approach residual vertical displacement (left); PG8: Approach residual vertical
displacement (right); PG9: Abutment residual pile cap displacement (left); PG10: Abutment
46
residual pile top displacement (right); PG11: Column residual pile displacement at ground
surface.
Discrete DSs are defined for each PG. Damage states are numbered sequentially in order of
increasing severity. The DS0 damage state corresponds to the onset of damage when repair costs
begin to accumulate. An upper limit to the quantities and costs is called DS∞, because it
corresponds to the most severe possible damage state for the elements in a PG. DS∞ usually
corresponds to complete failure and replacement of all the elements in the entire PG. The DSs
are connected to structural demands obtained from finite element analysis results by way of an
EDP specific to each PG. The repair quantities associated with each DS are developed more fully
in the definition of the damage scenarios. All the PGs and DSs are linked to a single EDP in this
implementation.
Based on previous work, the methodology was calibrated for defining post-earthquake
performance of select bridges that fall within the class of ordinary post-tensioned, box girder,
reinforced concrete highway overpasses (Mackie et al. 2011). The three major components
required for this calibration were damage scenarios that describe particular instances of
earthquake damage, schematic design of bridge repairs to address the state of damage in the
scenarios, and the link between repair design, methods and procedures, and subsequent quantities.
There is a direct link between damage scenarios and the repair, i.e., there is a single repair
procedure for a single state of damage. The repair quantity results were parameterized in terms of
basic bridge geometry and properties so that they can be used to extrapolate loss modeling for
other bridges in the same class (such as those that can be built within the user interface).
Data for time and monetary repair costs were obtained by estimating the costs of the damage and
loss scenarios using published Caltrans construction estimation data, case studies from previous
earthquakes, and interviews with Caltrans bridge engineers. Monetary costs were adjusted to
2007 values based on Caltrans cost index data. Repair costs are estimated for each damage
scenario based on quantities of each repair item. Cost estimates accounted for variations in unit
cost, and the details involved in estimating a combination of repairs together. The benefit of
separating the Qs from costs is that the unit cost model is easily updated for new years of data,
local economic conditions, site accessibility, and incentives.
Normalized costs of repair are obtained by using the repair cost ratio (RCR) between the cost of
repair and the cost of replacement cost (does not include demolition). It is shown in %, and it can
range between 0 and some number higher than 100% (there is no reason why it is bounded by
replacement cost; this is purely an owner/operator decision). This ratio is useful for comparing
the performance of different bridge design options for new construction. For the evaluation of
existing structures, the RCR including demolition costs might be more useful. Constructing a
new bridge on the same site after an earthquake would require both demolition of the damaged
bridge and construction of its replacement. The costs of new construction used in the interface
come from Caltrans bridge cost estimates used for planning purposes. They are based on the
deck and type of construction, providing a range of cost/SF of deck area, circa 2007 to be
consistent with the repair data used.
47
Repair time for the bridge can be expressed either as an approximation of repair duration or
repair effort. The repair effort represents the total number of crew-workdays (CWD) required to
complete the task. This is different from repair duration, which counts the total duration of the
repair project. The repair duration includes the effect of scheduling concurrent on-site
construction processes, while the repair effort does not. The repair duration can vary based on
the amount and type of concurrent construction processes, schedule dependencies, availability of
labor, and whether or not contract incentives are provided in order to decrease duration. Repair
times are also computed on the basis of each repair quantity Q. For any repair item, a probability
of 50% that Q > 0 indicates that the associated repair time should be added to the total repair
time for the project.
6.2 Input Necessary for User-defined PBEE Quantities
If the user is interested in providing user- or project-specific information in a PBEE analysis, the
following paragraphs describe the data needed by the interface to execute the PBEE analysis and
post-process the results. Performance groups need to be defined for each important component or
subassembly of the system that has potential repair consequences. Performance groups are
defined in terms of a single EDP that characterizes the response of this PG. Once this EDP
metric has been defined and time history analysis performed to obtain a distribution of EDP
realizations for different ground motions, the PBEE methodology can be implemented. The
PBEE methodology requires definition (by the user) of discrete damage states for each PG, a
repair method with associated repair quantities for each discrete DS for each PG, and the
corresponding costs and times required to execute the repair method.
The damage states are discrete and supplied in the form of what is commonly called a fragility
curve. This is a misnomer however, because the information required is the value of the EDP
(not IM) required to trigger different probabilities of exceeding the given discrete DS. It is often
assumed that said curves are well described by the lognormal probability distribution and
therefore, the only parameters required are the two lognormal distribution parameters: lambda
and beta. Lambda is the median and beta is the lognormal standard deviation. A PG can have as
many discrete DS as are required to cover the full range of possible responses experienced by the
PG. These should be input as is shown in Section 6.5.1 below.
Once the different states of damage have been established, damage scenarios need to be
generated that show different possible “snapshots” of damage that the structure may be in after
an earthquake event. Once these scenarios have been generated (note the scenarios need to be
detailed and include exact descriptions of the extent and depth of damage), they can be used to
decide what repair method would be appropriate for each PG or group of PGs. Such information
is specific to the type of structure, the discrete DSs, and the PGs. It is really only obtainable from
experts with past experience designing repair procedures given a damage scenario or snapshot.
Once the repair methods have determined, specific details about the repair quantities (specific
meaning square footage of deck, cubic yards of concrete, etc.) can be specified. The current data
employed in the interface has repair quantities parameterized in terms of the common bridge
design and geometric parameters, making it possible to solve for a variety of bridges within class.
48
However, any changes beyond these configurations would require numerical values for all the
repair quantities to be input.
It is assumed that the repair quantity estimates for each PG and DS are also random quantities
and can be described by a mean (or median) value and a coefficient of variation or lognormal
standard deviation. In the interface, beta has been set as 0.4, but could be modified by the user in
the future (if so desired). The repair quantities may then be handed over to a cost estimator, who
would have the ability to access historical pricing and bid information. In addition, the type and
magnitude of each repair quantity would correspond to standard DOT estimates and
specifications procedures. Each repair quantity can then be bid or an estimation of cost and
effort/time/production rate made. These unit costs and production rates are also random
quantities and can be described by a mean (or median) value and a coefficient of variation or
lognormal standard deviation. The values currently in the interface all have a beta of 0.2, but
could again be set by the user if desired. See more details about PERT criteria for the production
rates in Mackie et al. (2008).
Modifying the default PBEE quantities (repair quantities, unit costs, and production rates) is
detailed in Appendix E.
6.3 Definition/specification of PBEE input motion ensemble (suite)
6.3.1 Available Ground Motions
Four ground motion data sets are available:
Motion Set 1: This PBEE motion ensemble were obtained from the PEER NGA database
(http://peer.berkeley.edu/nga/) and consist of 100 3D input ground motions triplets, sorted into 5
bins. Each motion is composed of 3 perpendicular acceleration time history components (2
lateral and one vertical). These motions were selected through earlier efforts (Gupta and
Krawinkler, 2000; Mackie et al., 2007) to be representative of seismicity in typical regions of
California. The motions are divided into 5 bins of 20 motions each with characteristics: i)
moment magnitude (Mw) 6.5-7.2 and closest distance (R) 15-30 km, ii) Mw 6.5-7.2 and R 30-60
km, iii) Mw 5.8-6.5 and R 15-30 km, iv) Mw 5.8-6.5 and R 30-60 km, and v) Mw 5.8-7.2 and R
0-15 km. The engineering characteristics (IMs and time histories) of each motion and of the
ensemble overall may be viewed directly within BridgePBEE.
Motion Set 2: These motions (160 in total) are developed by Dr. Mackie from the 80 motions of
Motion Set 1 (excluding the 20 motions in bin v) above), to account for the more accurate site
classifications (NEHRP C and NEHRP D) in NGA. The magnitude, distance, and spectral shape
were intended to be similar to the previous bins (and indeed all of the previous motions appear in
either the NEHRP C or NEHRP D bins now). As such, these motions are divided into 8 bins
(compared to the 4 bins of Motion Set 1).
49
Motion Set 3: These motions (80 in total) are labeled Broadband_* (separated into the two bins,
Broadband rock and Broadband soil) as developed by Dr. Jack Baker for PEER. Additional
information about these motions is available at the website:
http://peer.berkeley.edu/transportation/projects/ground-motion-studies-for-transportationsystems/
Motion Set 4: These motions (260 in total) include the above Motion Set 2 and Motion Set 3 as
well as the additional bin v.) (near fault motions) of Motion Set 1.
All of the above 4 ground motion data sets were resampled to a sampling frequency of 50 Hz
(regardless of whether initial sampling frequency was 100 or 200 Hz) due to the computational
demands of running full ground-structure analyses for an ensemble of motions. Standard
interpolation methods were used to resample the time domain signals (so that the signal shape is
preserved). The resampled records were then baselined to remove any permanent velocity and
displacement offsets. Baselining was accomplished using a third order polynomial fitted to the
displacement record.
6.3.2 Specifications of PBEE Input Motions
To conduct a PBEE analysis, input motions must be defined (please follow the steps shown in
Fig. 50). The window to define PBEE input motions is shown in Fig. 51. To unselect all motions,
click De-select All. To see all motions, click Select All (same button as De-select All). The
dropdown list of Randomly Choose Records for Each Bin will randomly select a certain
number of input motions from each bin (the input motions are categorized by bin).
Double-click any record to view its intensity measures and response spectra (Fig. 52). SRSS
stands for Square Root of Sum of Squares of the 2 horizontal components. Click Display
Intensity Measures (Fig. 51) to view the histogram and cumulative distribution plots for whole
input motion set (Fig. 53). The intensity measures include:
 PGA (Peak Ground Acceleration)
 PGV (Peak Ground Velocity)
 PGD (Peak Ground Displacement)
 D5-95 (Strong Motion Duration)
 CAV (Cumulative Absolute Velocity)
 Arias Intensity
 SA (Spectral Acceleration; assuming 1 second period)
 SV (Spectral Velocity), SD (Spectral Displacement)
 PSA (Pseudo-spectral Acceleration)
 PSV (Pseudo-spectral Velocity)
The strong motion duration (D5-95) is defined according to the time domain bounded by the 5%
and 95% cumulative Arias intensity of the record. All of the spectral intensity measures are
defined at an effective viscous damping of 5% unless otherwise noted.
50
In the histogram window (Fig. 53), click Display Intensity Measures Values to view the
intensity measures listed in text format (Fig. 54). The user can copy and paste to her/his favorite
text editor such as MS Excel (in Fig. 54, right-click and then click Select All to highlight, and
then right-click and then click Copy to copy to the clipboard).
To incorporate user-defined input motions, please see Appendix C.
Fig. 50. Steps to define PBEE motions
51
Fig. 51. PBEE input motions widow
52
Fig. 52. Intensity measures, time histories and response spectra of individual record
Fig. 53. Histogram and cumulative distribution for the whole input motion set
53
Fig. 54. Intensity Measures (IM) table for the whole input motion set
6.4 Save Model and Run Analysis
After defining the finite element model, click on “Save model and run analysis”. The finite
element computations will start, for several earthquakes at a time as specified in the “Analysis
Options” (Fig. 55) window below. You can select as many as 8 records to be run at the same
time in order to reduce the overall run time (for dual core machines or better). Fig. 56 shows the
analysis progress for each record.
Fig. 55. Options to change number of records to be run at the same time
54
Fig. 56. OpenSees analysis in progress
6.5 PBEE Analysis
Once the FE analysis of all motions in the ensemble is complete, click PBEE Analysis (Fig. 2)
to display:
Fig. 57. PBEE analysis window
55
6.5.1 PBEE Quantities
In the figure above (Fig. 57), only “Damage States” can be currently modified by the user
directly within the user interface (however, this is an advanced feature that should be exercised
with care, or just left as is). Under Damage States (Fig. 58), Lambda is the median EDP that
defines onset of the damage state and is one parameter of the assumed lognormal distribution of
damage when conditioned in EDP. It has the same units as the EDP for the selected PG. Beta is
the lognormal standard deviation, and is the second parameter of the assumed lognormal
distribution. Hence beta is dimensionless and has a typical range between 0 and 1 (although it is
not bounded by 1). This parameter is closely related to the coefficient of variation (standard
deviation normalized by the mean) under certain conditions (small beta values).
The Repairs, Unit Costs, and Production Rates are displayed in Figs. 59-61, respectively. Users
can customize these PBEE quantities through updating a file named PBEE.DLL which is located
at the installation folder (C:\Program Files\BridgePBEE or C:\Program Files(x86)\BridgePBEE
on a 64bit PC). Please follow the steps described in Appendix E to build an updated PBEE.DLL
file and then replace the one in the installation folder.
Fig. 58. Damage states window
56
Fig. 59. Repair quantities window
Fig. 60. Unit Costs window
57
Fig. 61. Production Rates window
6.5.2 Compute Repair Cost & Time
Now, you can select any of the Intensity Measures (e.g., PGV above), and then click Compute
Repair Cost or Compute Repair Time in Fig. 57 to display the probabilistic repair cost and
Crew Working time in Days (CWD) along with Standard Deviation, displayed for each PG
(eleven of them) and each repair quantity (29 of them, see Table 10), as shown below. See
Section 7.2.1 for the detailed output.
To convert all PBEE figures to the EPS format, click Click Here for EPS Version of All PBEE
Figures. A MS Word window with the EPS figures included in the document will pop up once
the converting is done (please see Section 7.2.4 for the detailed output).
58
Table 10. PBEE Repair Quantities
Item#
Item name
1
Structure excavation
2
Structure backfill
3
Temporary support (superstructure)
4
Temporary support (abutment)
5
Structural concrete (bridge)
6
Structural concrete (footing)
7
Structural concrete (approach slab)
8
Aggregate base (approach slab)
9
Bar reinforcing steel (bridge)
10
Bar reinforcing steel (footing, retaining wall)
11
Epoxy inject cracks
12
Repair minor spalls
13
Column steel casing
14
Joint seal assembly
15
Elastomeric bearings
16
Drill and bond dowel
17
Furnish steel pipe pile
18
Drive steel pipe pile
19
Drive abutment pipe pile
20
Asphalt concrete
21
Mud jacking
22
Bridge removal (column)
23
Bridge removal (portion)
24
Approach slab removal
25
Clean deck for methacrylate
26
Furnish methacrylate
27
Treat bridge deck
28
Barrier rail
29
Re-center column
6.5.3 Compute Hazard Curves
The user is also able to specify a Seismic Hazard for a particular geographic location of this
bridge system in terms of specified values for any IM (e.g., derived from USGS seismicity maps).
The user interface provides default values for site hazard specific to a location in Northern
California. The hazard values are provided at each of the 2%-, 5%-, and 10%-probability of
exceedance in 50 years only for PGA and PGV. The user should input hazard values specific to
the site being studied as well as the intensity measure selected for analysis. If an IM other than
PGA or PGV is selected, the user interface will leave the three hazard level input boxes blank for
user input as there are no readily available hazard maps or conversions from PGA for an
arbitrary IM. The default PGA hazard values were obtained from USGS hazard maps. These
PGA values were converted to PGV values using the firm ground conversion of 48 in./sec/g. It is
59
not meant to imply that switching between PGA and PGV (or any other IM) will yield equal
hazard.
Once a desired local site seismicity is defined, users can click Display Hazard Curves (Fig. 57)
to display the mean annual frequency of exceedance and return period. Please see Section 7.2.2
for the detailed output.
6.5.4 Compute Disaggregation
Users can also click Display Disaggregation (Fig. 57) to display the disaggregation by
performance groups and repair quantities. Please see Section 7.2.3 for the detailed output. Only
the disaggregation of the expected repair cost/time by performance group is possible due to the
LLRCAT formulation. However, both expected and variance disaggregation plots are available
when disaggregating by repair quantity. The user can select the intensity measure and value on
which to disaggregate. The default value is a PGV value equal to the 10% probability of
exceedance in 50 years specified in the previous section.
60
7 Time History and PBEE Output
7.1 Time History Output Quantities
At the end of the FE analysis phase, time histories and bridge responses will be available of the
form:
 Column Response Time Histories and Profiles
 Column Response Relationships
 Abutment Responses
 Deformed Mesh
In addition, for PBEE analysis scenarios, Intensity Measures (IMs) and response spectra for each
input motion are calculated and are available for display in Table and Figure formats.
Performance Group (PG) Quantities and Bridge peak accelerations for all employed shaking
motions are also available for display against any of the computed IMs.
The post-processing capabilities can be accessed from Menu Display (Fig. 3). Fig. 62 and Fig.
63 show the post-processing capabilities available in a pushover analysis and a base shaking
analysis, respectively. Fig. 64 shows the Analysis Options window. Depending on the selection
of the Output Data options (Fig. 64), the menu items shown in Fig. 62 and Fig. 63 may be
enabled or disabled. For example, In order to view column response profiles and response
relationships, Include Column Response Profiles & Relationships (Fig. 64) has to be checked
before analysis (in this case, menu items of Column Response Time Histories & Profiles as
well as Column Response Relationships shown in Fig. 62 and Fig. 63 will be enabled). To
view the deformed mesh (and animation), both Output Data options of Include Column
Response Profiles & Relationships and Include Soil Displacement (Fig. 64) must be checked.
If the user wants to view the deformed mesh for the final step only, check Display Deformed
Mesh for Final Step Only (Recommended for Large Models) (Fig. 64). The option is
particularly useful when the output data is large and all output cannot be loaded into memory.
To display output for a different input motion, please follow steps shown in Fig. 65. The name of
the selected input motion will also appear on the menu items (Fig. 63).
61
Fig. 62. Post-processing capabilities (menu options) available in a pushover analysis
Fig. 63. Post-processing capabilities (menu options) available in a base shaking analysis
62
Fig. 64. Analysis options in BridgePBEE
a)
63
b)
Fig. 65. Steps to display output for a different input motion: a) click menu Display (Fig. 3); b)
select an input motion
7.1.1 Column Response Time Histories and Profiles
The column response time histories and response profiles can be accessed by clicking menu
Display (Fig. 3) and then Column Response Time Histories and Profiles (Fig. 66). The
column response window is shown in Fig. 67. There are 3 dropdown lists available for users to
choose. The contents of the 3 lists are as follows:
Left Dropdown List:
 Response Histories
 Response Profiles
Middle Dropdown List:
 Displacement (relative to base of soil mesh for earthquake excitation scenarios)
 Acceleration (Absolute or Total)
 Rotation
 Bending Moment
 Shear Force
 Pressure
 Response Summary
Right Dropdown List:
 Longitudinal Direction
64


Transverse Direction
Vertical Direction
Please note that the above Middle Dropdown List is only valid for the longitudinal and
transverse directions. If the Vertical Direction in the Right Dropdown List is selected, the Middle
Dropdown List will become (the displacement refers to the one relative to the model base):
 Displacement
 Acceleration
 Rotation
 Torsional Moment (Torque)
 Axial Force
1) Column Response Profiles
The column response profile will be displayed if Response Profiles in the Left Dropdown List
(Fig. 67) is selected. For example, Fig. 68 shows the bending moment in the longitudinal plane.
The horizontal axis of the plot is the response name (e.g., displacement, bending moment, etc.)
and the vertical axis is the elevation of the column (and the pile shaft below grade). Zero
elevation means the ground surface.
For Displacement, Acceleration and Rotation, two lines are plotted for the response profile
selected (these lines are continuous):
 End: the response profile at the final step
 Max: the response profile at a certain step when the maximum (absolute) value occurs
In the cases of Bending Moment, Shear Force, and Pressure, three lines are plotted:
 End (Envelope): Envelope of the response values at the final step
 End (Element Output): the response values for both nodes (top node/bottom node) of
every element (this line is discontinuous)
 Max: the response profile at a certain step when the maximum (absolute) value occurs
Pressure is the difference of the shear forces at the both ends of each element divided by the
element length.
If Response Summary is selected (the Middle Dropdown List, see Fig. 67), response profiles of
displacement, bending moment, shear force and pressure will be plotted in one window (Fig. 69).
To convert all the plots in the current window to a PDF file (Adobe PDF or similar has to be
available) or send to a printer, click Print located near the top-left corner of the window (this
feature is available in all figure windows in BridgePBEE). To view the data of each plot (this
feature is also available in all plots in BridgePBEE), click the filename (e.g., click momProf.txt
in Fig. 68 and an Internet Explorer window will pop up and display the momProf.txt data file).
2) Column Response Time Histories
65
The column response time history will be displayed if Response Time Histories in the Left
Dropdown List (Fig. 67) is selected. Fig. 70 shows the window for displaying the column
longitudinal displacement time histories. The top plot in the window (Fig. 70a) is the response
profiles for at specific load steps, while the remaining plots are the response time histories at
different depths (Fig. 70b).
In the plot for the Response Profiles for All Steps (Fig. 70a), only 20 steps including the initial
state (Step 0), the first step and the final step are shown if more than 20 steps are simulated.
Step 0 refers to the initial state after application of own weight and before the dynamic run (i.e.,
pushover or earthquake shaking).
If Acceleration is selected, the free-field acceleration response time history and the input
acceleration time history are also plotted (Fig. 71). The free-field location is shown in Fig. 66 (at
the ground surface along the diagonal line of the mesh near the edge corner node).
Fig. 66. Menu items to access the column response time histories and response profiles
66
Fig. 67. Response time histories and profiles for column (and pile shaft): displacement is shown
at the nodes (only one element is used above ground).
Fig. 68. Bending moment profile in the longitudinal plane
67
Fig. 69. Response summary
68
a)
b)
Fig. 70. Column longitudinal displacement response time histories: a) response profiles at
specific load steps; b) response time histories at different elevations
69
b)
Fig. 71. Column longitudinal acceleration response time histories at different elevations (freefield and input accelerations are also included)
7.1.2 Column Response Relationships
The column response relationships can be accessed by clicking menu Display (Fig. 3) and then
Column Response Relationships (Fig. 72). The column response relationships window is
shown in Fig. 73. There are 3 dropdown lists available for users to choose from. The contents of
the 3 lists are as follows:
Left Dropdown List:
 Load-displacement
 Moment-curvature
Right Dropdown List:
 Longitudinal Direction
 Transverse Direction
The Middle Dropdown List includes all elevations (starting from column top). Again, zero
elevation refers to the ground surface.
Fig. 74 shows the longitudinal load-displacement curve at the column top. The load refers to the
shear force of the beam-column element at the specified elevation. Fig. 75 shows the momentcurvature curve at the column top. The vertical axis is the bending moment and the horizontal
70
axis is the curvature. To view the data for the plot, click the .txt filename (e.g., click
curvX_6.71m.txt in Fig. 75).
Fig. 72. Menu items to access the column response relationships
Fig. 73. Column response output options
71
Fig. 74. Load-displacement curve at column top
Fig. 75. Moment-curvature curve at column top
72
7.1.3 Abutment Responses Time Histories
The abutment responses can be accessed by clicking menu Display and then Abutment
Responses (Fig. 76). The abutment responses window includes the following options (Fig. 77):
 Force-Displacement Relationships
 Relative Deck-end/Abutment Displacement Time Histories
 Resisting Force Time Histories
 Pile Cap Displacement Time Histories
where Pile Cap refers to the embankment base right below the deck-end (please see Fig. 86 in
Section 7.1.6).
Three directions (longitudinal, transverse and vertical directions) of the above responses for both
left and right abutments are all displayed. Fig. 78 shows the abutment response time histories.
The force refers to the resisting force acting on deck-end and the displacement refers to the
relative deck-end/abutment displacement.
Fig. 76. Menu items to access the abutment responses
73
Fig. 77. Menu items to access the abutment responses
a)
b)
74
c)
d)
Fig. 78. Abutment response time histories (scroll down to see all directions): a) abutment forcedisplacement relationships; b) relative deck-end/abutment displacement time histories; c)
resisting force time histories; and d) abutment pile cap time histories
75
7.1.4 Deformed Mesh
The deformed mesh can be accessed by clicking menu Display (Fig. 3) and then Deformed
Mesh (Fig. 79). The deformed mesh window is shown in Fig. 80. There are 3 dropdown lists
available for users to choose. The contents of the 3 lists are as follows:
Left Dropdown List:
 Due to gravity (soil only)
 Due to gravity (bridge included)
 Due to pushover (or Due to base shaking)
Middle Dropdown List:
 Deformed mesh
 Disp. contour fill
 X-Disp contour
 Y-Disp contour
 Z-Disp contour
The Right Dropdown List includes options of 3D view as well as 2D views for a number of predefined planes.
To view the bridge structure only, check Bridge Only in the bottom-right corner of the window
(Fig. 80).
Fig. 79. Menu items to access the deformed mesh
76
Fig. 80. Deformed mesh
7.1.5 Soil Response Time Histories
The soil response time histories can be accessed by clicking menu Display (Fig. 3) and then Soil
Response Histories (Fig. 81). The soil response window is shown in Fig. 82. There are 3
dropdown lists available for users to choose. The contents of the 3 lists are as follows:
Left Dropdown List (Fig. 82):
 Longitudinal acceleration time histories
 Longitudinal displacement (rel. to base) histories
 Transverse acceleration time histories
 Transverse displacement (rel. to base) histories
 Vertical acceleration time histories
 Vertical displacement time histories
 Excess pore pressure time histories
 Shear stress (zx) vs. strain & eff. confinement
 Shear stress (yz) vs. strain & eff. confinement
 Longitudinal normal stress time histories
 Transverse normal stress time histories
77
 Shear stress (zx) time histories
 Shear stress (yz) time histories
Right Dropdown List (Fig. 83):
 Longitudinal plane crossing column center
 Transverse plane crossing column center
Distances away from the column center are calculated to match the corresponding soil nodes and
are listed in the Middle Dropdown List (Fig. 84). Fig. 85 is the sample output of the soil
settlement time histories under the left abutment.
Fig. 81. Menu items to access the soil responses
78
Fig. 82. Response options for soil time histories
Fig. 83. Planes for locations of the soil response time histories
79
Fig. 84. Locations of soil response time histories
Fig. 85. Soil settlement time histories under abutment
80
7.1.6 PBEE Output Quantities
At the end of the finite element analysis phase, the following output performance group
quantities (for each earthquake record) are used in the next phase of PBEE analysis:
Table 11. PBEE Performance Groups
Performance Group
Performance group names
(PG) #
1
Maximum column drift ratio
2
Residual column drift ratio
3
Maximum relative deck-end/abutment displacement (left)
4
Maximum relative deck-end/abutment displacement (right)
5
Maximum bridge-abutment bearing displacement (left)
6
Maximum bridge-abutment bearing displacement (right)
7
Approach residual vertical displacement (left)
8
Approach residual vertical displacement (right)
9
Abutment residual pile cap displacement (left)
10
Abutment residual pile top displacement (right)
11
Column residual pile displacement at ground surface
In addition, Intensity Measures for the computed Free Field ground surface acceleration records
are computed, so that outcomes can be either shown against the input base shaking IMs or the
computed ground surface IMs (noted as Free-Field in the user interface). The sections below
detail how the response quantities are obtained for each PG. Refer to Fig. 86 for the annotated
model that is used to describe the location of sampling points during time history analysis.
PG1: Maximum tangential drift ratio SRSS (column)
PG2: Residual tangential drift ratio SRSS (column)
The tangential drift ratio is defined as the maximum of a) displacement above the inflection point
divided by the length of this distance, and b) displacement below the inflection point divided by
the length of this distance. This takes care of rotation at the base, different boundary conditions,
etc., so that the results are consistent when computing damage. The Square Root of Sum of
Squares (SRSS) values of the 2 horizontal components are used. The tangential drift ratios are
combined separately at each time step (to obtain SRSS).
PG1 (Max tangential drift ratio SRSS) is the maximum of the SRSS values of all time steps. PG2
(Residual tangential drift ratio SRSS) is the SRSS value at the last time step. The tangential drift
ratio is in percentage.
To calculate the tangential drift ratio, the following 2 lines were added into the tcl file:
recorder Element -file A-ELC.dft -time -ele $columnEle tangentDrift
recorder Element -file A-ELC.ifp -time -ele $columnEle inflectionPoint
81
where $columnEle is the element # of the column (Only one forced-based beam-column element
nonlinearBeamColumn is used for the column). In the .dft file, there will be 5 columns of data
for each time step and the first column is time. In the .ifp file, there will be 3 columns for each
time step and the first column is also time.
Subsequently, the tangential drift ratio is calculated using the code snippet shown in Fig. 87. For
the tangential drift ratio in the longitudinal direction (X-direction or bridge longitudinal
direction), the tdx1 and tdx2 variables are the second and third column (the first column is time),
respectively, of the tangential drift recorder file (e.g., A-ELC.dft). The tdxi variable is the
second column (the first column is time) of the inflection point recorder file (e.g., A-ELC.ifp).
For the transverse tangential drift ratio, the tdx1 and tdx2 variables are the fourth and fifth
column of the .dft file and the tdxi variable is the third column of the .ifp file.
A
B
O
D
C
E
Fig. 86. Finite element mesh in BridgePBEE: Node O – Column base node (at ground surface);
Node A – Column top node; Node B – Deck-end node; Node C – Abutment top node (having
the same coordinates as Node B); Nodes B are C are connected by an abutment model; Node D
– Abutment pile cap node
82
// tdx1 & tdx2 -- the tangent drift recorder file at time step i
// tdxi -- the inflection point recorder at time step i
// tdx – tangential drift ratio
if( fabs(tdxi) < 1e-20 ) {
tdx = -tdx2/(H - tdxi);
}
else if ( fabs(H-tdxi) < 1e-20 ) {
tdx = -tdx1 / tdxi;
}
else {
tdx = __max(fabs(tdx1/tdxi), fabs(tdx2/(H-tdxi)));
//tdx = -tdx*sgn(tdx2/(H-tdxi));
if( fabs(tdx2/(H-tdxi)) < 1e-20 )
tdx = 0;
else if( (tdx2/(H-tdxi)) > 0)
tdx = -tdx;
}
return tdx;
Fig. 87. Code snippet to calculate the tangential drift ratio of column
PG3: Maximum longitudinal relative deck-end/abutment displacement (left)
PG4: Maximum longitudinal relative deck-end/abutment displacement (right)
These two PGs are intended to address the issue of abutment impact into the backwall, so they
are defined as only the motion of the deck into the abutment. Maximum absolute values in the
longitudinal direction are used.
For example, for the right abutment shown in Fig. 86, it is the relative longitudinal displacement
of node B (deck-end node) in the direction of node C (abutment top node). A zero value is used
for the times during which the deck-end node moves away from the abutment top node.
PG5: Maximum absolute bearing displacement (left abutment)
PG6: Maximum absolute bearing displacement (right abutment)
These two PGs are intended to address bearing damage whether or not an explicit representation
of the bearings is included in the user-selected abutment model. Therefore, the EDP for the PG is
based on the relative displacements of the deck-end node (e.g., Node B for the right abutment
shown in Fig. 86) to the abutment top node (e.g., Node C for right abutment shown in Fig. 86).
The SRSS values of the resulting two relative horizontal displacements is used and both motion
into the backwall and away from the backwall are considered.
PG7: Residual vertical displacement (left abutment)
PG8: Residual vertical displacement (right abutment)
83
This PG is used to gage immediate repairs for rideability, and is not a measure of the permanent
slumping of the embankment (for example). Therefore, the EDP is calculated as the vertical
displacement of the abutment top node (e.g., Node B for the right abutment shown in Fig. 86)
relative to the deck-end node (e.g., Node C for the right abutment shown in Fig. 86). The residual
value is used (value at the final time step).
PG9: Residual pile cap displacement SRSS (left abutment)
PG10: Residual pile cap displacement SRSS (right abutment)
These PGs address possible damage below grade due to lateral translation of the piles and pile
caps. While not a direct measure, pile cap displacement was selected as it would not require
knowledge or observations of piles below grade. The EDP is defined by calculating the SRSS
value of the 2 horizontal displacements of the abutment pile cap node (e.g., Node D for the right
abutment shown in Fig. 86). The residual is obtained from the value at the final time step.
PG11: Residual pile cap displacement SRSS (column)
This quantity is analogous to the two previous PG, but is representative of response and damage
at the abutment foundations. The EDP is obtained by calculating the SRSS value of the 2
horizontal displacements of the column pile cap node (e.g., Node O shown in Fig. 86) and taking
the value at the final time step.
The PG (Performance Group) quantities for all input motions can be accessed by clicking menu
Display (Fig. 3) and then PG Quantities for All Motion (Fig. 88). The window to display PG
quantities is shown in Fig. 89.
The PG quantities are displayed against any of the 22 intensity measures (including 11 for the
input acceleration and the other 11 for the free-field response). The PG quantities for each input
motion are displayed by bin of the motion (see legend in Fig. 89). When an IM is paired with an
EDP and all the individual realizations are plotted, the result is typically termed a demand model,
or probabilistic seismic demand model (PSDM). Previous research has demonstrated that the
central values of PSDMs are often well described using a power-law relationship between EDP
and IM. The parameters of such a power-law fit can be obtained using least squares analysis on
the data. Therefore, when plotted in log-log space (as is shown in Fig. 89), the best-fit, or mean,
relationship is linear.
The mean (in log-log space) is shown along with the standard deviation (also in log-log space) of
the power-law fit. If it is assumed that the EDP responses are lognormally distributed when
conditioned on IM, then these curves can be interpreted as being defined by the two parameters
of a lognormal distribution (the median can be related to the mean of the logarithm of the data
and the lognormal standard deviation is as shown).
84
To convert all figures currently displayed in the window, click Convert Figures to EPS Format.
A MS Word window with the EPS figures included in the document will pop up once the
converting is done (Fig. 90).
To view lognormal standard deviations for each PG (Fig. 91), click View Beta Values in Fig. 89.
The information is tabulated with values in bold indicating the lowest lognormal standard
deviation for all the computed IMs in a given PG. The same information is shown graphically as
a bar chart (separate bar chart for each PG). Such a figure is useful for determining the selection
of optimal IM for a given EDP or PG.
Fig. 88. Menu items to access the PG quantities for all motions
85
Fig. 89. PG quantities for all motions (scroll down to see all 11 PGs)
Fig. 90. Converting figures to EPS format
86
a)
b)
Fig. 91. Lognormal standard deviations (beta values) for each PG: a) table format; b) bar graph
format
87
7.1.7 Bridge Peak Accelerations for All Motions
The bridge peak accelerations for all input motions can be accessed by clicking menu Display
(Fig. 3) and then Bridge Peak Accelerations for All Motions (Fig. 92). The window to display
the bridge peak accelerations for all motions is shown in Fig. 93. The responses are available in
the longitudinal and transverse directions as well as for the SRSS of the 2 horizontal directions
(Fig. 93).
The figures in this window include (The free-field location is defined in Fig. 66):
 Maximum bridge acceleration
 Maximum column base acceleration
 Maximum free-field acceleration
 Maximum input acceleration
 Bridge peak acceleration / column base peak acceleration
 Column base peak acceleration / input peak acceleration
 Free-field peak acceleration / input peak acceleration
 Bridge peak acceleration / input peak acceleration
Fig. 92. Menu items to access bridge peak accelerations for all motions
88
a)
b)
89
c)
Fig. 93. Bridge peak accelerations for all motions: a) maximum bridge accelerations; b)
maximum column base accelerations; and c) maximum free-field accelerations
7.1.8 Maximum Column & Abutment Forces for All Motions
The maximum column & abutment forces for all input motions can be accessed by clicking
menu Display (Fig. 3) and then Maximum Column & Abutment Forces for All Motions (Fig.
94). The window to display the maximum column & abutment forces for all motions is shown in
Fig. 95. The responses are available in the longitudinal and transverse directions as well as for
the SRSS of the 2 horizontal directions (Fig. 95).
The figures in this window include:
 Maximum column shear forces
 Maximum column bending moments
 Maximum abutment forces (left abutment)
 Maximum abutment forces (right abutment)
90
Fig. 94. Menu items to access maximum column & abutment forces for all motions
a)
91
b)
c)
Fig. 95. Maximum column & abutment forces for all motions: a) maximum column shear forces;
b) maximum column bending moments; and c) maximum abutment forces
92
7.2 PBEE Outcomes
7.2.1 Repair Cost & Time
The final PBEE results will be displayed against any intensity measure (e.g., PGV) in terms of:
 Contribution to expected repair cost ($) from each performance group (Fig. 96)
 Total repair cost ratio (%) (Fig. 97)
 Contribution to expected repair cost ($) from each repair quantity (Fig. 98)
 Contribution to repair cost standard deviation ($) from each repair quantity (Fig. 99)
 Total repair time (CWD) where CWD stands for Crew Working Day (Fig. 100)
 Contribution to expected repair time (CWD) from each repair quantity (Fig. 101)
Fig. 96. Contribution to expected repair cost ($) from each performance group
93
Fig. 97. Total repair cost ratio (%) as a function of intensity
Fig. 98. Contribution to expected repair cost ($) from each repair quantity
94
Fig. 99. Contribution to repair cost standard deviation ($) from each repair quantity
Fig. 100. Total repair time (CWD: Crew Working Day) as a function of intensity
95
Fig. 101. Contribution to expected repair time (CWD) from each repair quantity
7.2.2 Hazard Curves
Based on the local site Seismic Hazard specified, losses are estimated and displayed graphically
as:
 The defined local site hazard curve as a mean annual frequency () of exceedance
(ground motion) (Fig. 102)
 Return period against total repair cost ratio (Fig. 103)
 Mean annual frequency (MAF) of exceedance (loss) against total repair cost ratio RCR
(Fig. 104)
 Return period against total repair time RT (Fig. 105)
 Mean annual frequency (MAF) of exceedance (loss) against total repair time (Fig. 106)
The median ground motion hazard curve is assumed to have a power-law form with two
unknown parameters (k, k0 in Eq. 4) in the range of the ground motion intensities bracketed by
the 2%- and 10%-probability of exceedance IM values (im). The two-parameter fit (linear in log
96
space) to the nonlinear (in log space) hazard curve tends to overpredict frequencies of
exceedance for IM extremes both above and below the range of intensities considered. Therefore,
care should be taken when extrapolating any resultant hazard curves to extremely low (or high)
frequencies of exceedance. Using a least-squares fit in log space, the unknown parameters can be
determined numerically from the three values input by the user (2%-, 5%-, and 10%-probability
of exceedance in 50 years). On the site hazard curves plotted in the interface, both the data points
and the fitted curve are shown (Fig. 102).
 IM im   k 0 im 
k
(4)
The power-law fit to the hazard data is used to compute the loss hazards. The loss model
(probability of exceeding RCR or RT conditioned on intensity levels) is integrated with the
absolute value of the derivative of this IM hazard to obtain the loss hazard curve (MAF of
exceeding either RCR or RT). Details of the numerical integration are presented in Mackie et al.
(2008) and other sources.
The loss hazard curves (both for repair cost and repair time) are further integrated over intensity
to yield mean annual loss. For example, in Fig. 104, the mean annual repair cost ratio expected
for the bridge at the given site is 0.05% of the replacement cost.
Fig. 102. Mean annual frequency of exceedance (ground motion)
97
Fig. 103. Return period against total repair cost ratio
Fig. 104. Mean annual frequency of exceedance (loss) against total repair cost ratio
98
Fig. 105. Return period against total repair time
Fig. 106. Mean annual frequency of exceedance (loss) against total repair time
99
7.2.3 Disaggregation
Figs. 107-109 display the disaggregation (Fig. 57) of expected cost by performance group, the
disaggregation of expected cost by repair quantities, and the disaggregation of expected time by
repair quantities, respectively. In thie figures below, the disaggregation is performed at an
intensity of 100 cm/s (PGV) for all three figures (a user IM and value as shown in Fig. 57). This
IM and its value are shown in the plot titles.
Fig. 107. Disaggregation of expected cost by performance group
100
Fig. 108. Disaggregation of expected repair cost by repair quantities
101
Fig. 109. Disaggregation of expected repair time by repair quantities
7.2.4 EPS Version of All PBEE Figures
A MS Word file contained all PBEE figures in the EPS format can be created as shown below.
102
Fig. 110. Converting all PBEE figures to EPS format
103
8 Appendix A: How to Define the Soil Finite Element Mesh
A bridge and approach embankments supported on a ground strata will be defined. The bridge
configuration is shown below (Fig. 111). In this simple configuration, the approach
embankments are idealized by a rigid triangular configuration employed to exert the self-weight
of these embankments on the supporting ground.
Deck length
Column height above grade
Ground surface
Total column height
Embankment length
Depth of embankment
foundation
Embankment length
Side view
Embankment length
Deck length
Embankment length
Deck width
Plan view
Fig. 111. Schematic view of an idealized single bent bridge system
Step 1
In the user interface, click Bridge Parameters. With reference to Fig. 111, define the following
parameters according to your preference:
Diameter: This is the bridge column outer diameter, which is currently also the pile diameter
(Integral column foundation scenario).
Total Column Length: Starting from the bridge deck all the way to the pile tip
Column Length above Surface: from bridge deck to mud-line
Embankment Length: (in plan view, longitudinally from bridge edge to street level away from
bridge)
104
Depth of Embankment Foundation: Height of approach embankment at bridge edge from the
ground surface to the base of the approach embankment foundation (Fig. 111).
Deck Length: Length of bridge in the longitudinal direction
Soil Parameters: make sure at least the total “Thickness” of soil layers is defined: This is the
total thickness of the ground stratum from the ground surface all the way down to the base of the
soil mesh. Make sure that the column/pile base (tip) is within the defined soil domain depth.
Note: Earthquake input motion is imparted along the base of the soil mesh. This base is assumed
to represent rigid bedrock. As such, this input earthquake excitation constitutes total motion
imparted at this Bedrock level.
Step 2
Click Mesh Parameters to define additional meshing parameters.
Tab “General Definition” (Fig. 112): Make sure “Mesh Scale” is “Full mesh” and “Number of
Slices” is 16 or larger. This parameter refines the mesh by creating additional elements in
horizontal plane of the soil mesh.
Fig. 112. General meshing controlling parameters (default values)
Tab “Horizontal Meshing” (Fig. 113): This section controls mesh refinement along the
horizontal direction. Length of each soil horizontal layer is defined in the left column. Number
105
of mesh elements in each defined is specified in the column “Number of Mesh Layers”. Note
that the first mesh layer is starting from the center of the mesh when the column is located and
the length of the first mesh layer is equal to the column radius. The fourth mesh layer is for the
embankment. Ratio of Element Length over Next is used to obtain a gradually changing
element size within a layer if Uniform Meshing is unchecked (obviously this option is only
valid if the # of mesh layers is 2 or larger).
To obtain a refinement near the embankment (Fig. 114), check Activate Adjusting Mesh beside
Embankment (this option is only valid if Num of Slices is 32 or larger). Then define the size of
the 1st layer as a factor of Deck Width. Fig. 114 shows an example of using this option.
To minimize the number of elements in the horizontal direction, check Minimize Number of
Elements in Horizontal Direction. As a result, all other options defined for the horizontal
meshing will be ignored. This checkbox option is particularly useful when a rigid ground case is
needed.
Fig. 113. Meshing controlling parameters for horizontal direction (default values)
106
a)
b)
Fig. 114. Adjusting mesh near embankment: a) before adjusting; b) after adjusting
Tab “Vertical Meshing” (Fig. 115): This section defines the soil profile (layering) along the
vertical direction starting from the ground surface downwards (looking at the side view from the
top downwards. Height (thickness) of each soil layer is defined in the left column. Number of
mesh elements in each defined is specified in the column “Number of Mesh Layers” (at least
107
equal to 1 to define a soil profile consisting of a single type of soil). Height (thickness) of this
layer must be equal to the entire soil stratum height. Note that the number of mesh layers in the
upper zone (where the pile foundation is embedded) will automatically define the number of
beam column elements of this pile (below ground surface). As such, it is generally advisable to
select an adequate number of mesh layers in this zone. Note: If there is any error during mesh
generation, please follow the error message instructions to adjust the controlling parameters and
then try again.
Note: Element size is a parameter that affects frequency content of the ground response. Smaller
size elements (particularly along the soil domain height), will permit higher frequencies (if
present in the input motion) to propagate to the ground surface with more fidelity.
Fig. 115. Meshing controlling parameters for vertical direction (default values)
The finite element mesh created with the above default values is shown in Fig. 116. Examples of
mesh generation are shown in Figs. 117-119.
108
Fig. 116. Finite element mesh created with default values
109
a)
b)
Fig. 117. Mesh refinement example 1: a) Change “Num of Slices” to 32; b) the resulting mesh
110
a)
b)
Fig. 118. Mesh refinement example 2: a) Change “Number of Mesh Layers” in the vertical
direction; b) the resulting mesh
111
a)
b)
Fig. 119. Mesh refinement example 3: a) Change meshing controlling parameters in the
horizontal direction; b) the resulting mesh
112
9 Appendix B: Simple Pushover Examples (Bridge on Rigid
Ground)
Steps to build a bridge model on a fixed base
In BridgePBEE, a very stiff ground mesh is currently used to simulate a fixed-base scenario.
Simplest Approach:
Start with Example 1 at http://peer.berkeley.edu/bridgepbee/ and modify the bridge model to
match your specifications.
Alternative Approach:
To make the soil very stiff, please follow the steps below:
Step 1: In the main page of the interface (Fig. 2), click File, then New Model, and Yes (to create
a new model).
Step 2: Click Soil Parameters in the main window.
Step 3: Click 22: U-Clay2 from Soil Type dropdown list.
Step 4: Enter a large number for the Shear Wave Velocity (e.g., 10,000 m/sec), and click OK to
close U-Clay2 window.
Step 5: Click OK to close Soil Strata window.
Step 6: Click File, and then Save Model (to save the model).
Simple Verification (Linear column properties)
1. Cantilever Beam with Longitudinal Load at Free End
This case can be obtained by making the bridge deck very flexible (e.g., use a very small value
for the elastic modulus). The Roller abutment model is employed.
The Fiber section with Elastic Material is used to simulate the column. In this case, the
equivalent flexural stiffness is EI = 3375450 kN-m2 (as reported back by the user interface, see
Fig. 10, when “Elastic” is selected).
Load P = 20 kN
Length L = 6.71 m
The end displacement w = PL3/3EI = 5.97 E-04 m
BridgePBEE gives 6.1E-04 m (Fig. 120).
113
Fig. 120. Cantilever beam simulation using BridgePBEE
2. Fixed-end Beam with Point Load
This is a case where the column base is fixed at rigid rock and there is zero rotation at the
column top. This case can be obtained by making the bridge deck very stiff and also applying the
Roller abutment model.
The Fiber section with Elastic material is used to simulate the column. In this case, the
equivalent flexural stiffness EI = 3375450 kN-m2 (as reported by the user interface, when
“Elastic” properties are selected in Fig. 10).
Load P = 40 kN (half load 20 kN is used in the user interface)
Length L = 13.42 m (half length 6.71 m is used in the user interface)
The end displacement w = PL3/12EI = 1.492 E-04 m
BridgePBEE gives 1.496E-04 m (Fig. 121).
114
Fig. 121. Fixed-end beam simulation using BridgePBEE
3. Bridge self-weight with rigid Column & roller abutment model
The distributed load of deck p = 130.3 kN/m
Half of the bridge length L = 45 m
Elastic modulus of deck = 28,000,000 kPa
Moment of Inertia = 2.81 m4
Fig. 122 displays the deformation of bridge deck under gravity. The maximum is 0.0372 m (Fig.
122). The close-form solution gives 0.0368 m (Fig. 123).
115
Fig. 122. Deck deformation under gravity (the maximum displacement is 0.0372 m)
Fig. 123. Fixed end-roller beam analytical solution (from efunda.com)
116
4. Nonlinear-Column Bridge Pushover
a) Longitudinal Pushover (Fig. 124)
Fig. 124. Longitudinal pushover
b) Transverse Pushover (Fig. 125)
Fig. 125. Transverse pushover
117
10 Appendix C: How to Incorporate User-defined Motions
1) Directory Structure of a PBEE Motion Set
To conduct a PBEE analysis, input motions must be defined (please follow the steps shown in
Fig. 50). The window to define PBEE input motions is shown in Fig. 51. Click Browse to select
a PBEE motion set (Fig. 126). Click on the motion set name (e.g., PBEEMotionSet1) and then
click on OK to choose this motion set (Fig. 126).
In BridgeBPEE, the input motions are organized in a format that the program can read.
Specially, the input ground motions are sorted into bins. Fig. 127 shows the directory structure of
a PBEE motion set named PBEEMotionSet1. The second level directories are bins (e.g., LMLR,
LMSR, Near, SMLR, SMSR; see Fig. 126 and Fig. 127). The third level directories are
earthquake names (e.g., there are 3 earthquakes under bin LMLR: BORREGO, LOMAP,
NORTHR; see Fig. 127). And the fourth level directories are the input motion names (e.g., there
is 1 input motion under earthquake BORREGO: A-ELC; see Fig. 127).
Each motion is composed of 3 perpendicular acceleration time history components (2 laterals
and one vertical). As shown in Fig. 127, each motion folder contains 6 files categorized into 2
file types: the DATA files contain the time history (acceleration unit in g) of a component and
the INFO files contain the characteristics of the corresponding component. Fig. 128 and Fig. 129
displays sample INFO & DATA files. Naming of these files has to follow the format below:
Input motion name + angle (or “–UP” or “–DWN” for vertical component) + “.AT2” + “.data”
(or “.info”)
Note that the filenames with the smaller angle will be used for the longitudinal direction and the
other one (with the larger angle) will be used for the transverse direction.
The first 2 lines of each INFO file must follow the style of the example below:
{Data points NPTS}{4000}
{Sampling period DT (sec)}{0.01}
Where 4000 and 0.01 are the number of data points, and the time step, respectively, of an input
motion component.
2) Steps to Create an Input Motion
Based on the above description for the directory structure of a PBEE motion set, one can easily
create an input motion (Fig. 130):
Step 1: create a folder and rename to your PBEE motion set name (e.g. MotionSet1; see Fig.
130).
118
Step 2: create a folder under the motion set folder and rename to your bin name (e.g., bin1).
Step 3: create a folder under the bin folder and rename to your earthquake name (e.g., Quake1).
Step 4: create a folder under the earthquake name and rename to your input motion name (e.g.
MOTION1).
Step 5: create the 6 files (3 INFO files and 3 DATA files) for this input motion (Fig. 130).
Note: If you download the input motion files from the PEER NGA Database, there is no need to
re-format the data into one column as shown in Fig. 129. Just copy the data points into the
corresponding DATA files. And then make the INFO files containing the number of data points
and the sampling period DT (2 lines) according to the header information.
Motion set name
There are 5 bins in this motion set.
Fig. 126. Choosing PBEE motion set
119
Earthquake name
Vertical component
Motion set name
Bin name
Motion name
Horizontal components
Fig. 127. Directory structure of PBEE motion set
Fig. 128. Sample .info file
120
Fig. 129. Sample .data file
Fig. 130. Example of user-defined motion
121
11 Appendix D: Calculation of Steel and Concrete Material
Properties
Steel Bars
By default, the Steel02 material is used to simulate steel bars. The format of the Steel02
command is as follows (Mazzoni et al. 2009):
uniaxialMaterial Steel02 $matTag $fy $E0 $b $R0 $cR1 $cR2
Where $fy is the steel yield strength (Table 2), $E0 is Young’s modulus of steel, and $b is the
strain-hardening ratio (ratio between post-yield tangent and initial elastic tangent), $R0, $cR1
and $cR2 are parameters to control the transition from elastic to plastic branches.
The number of longitudinal bars is calculated as follows:
# bars 
 s Ac
(5)
Ab
Where  s is the longitudinal steel percentage (Table 1), Ac the column cross-section area, Ab is
the cross-section area of the steel bar.
If the number of longitudinal bars is known, the longitudinal steel percentage (reinforcement
ratio) can be calculated:
s 
As
Ac
(6)
Where As is the area of longitudinal steel, which is equal to the area of each bar times the number
of bars. For example, the diameter of a #18 bar is 2.257 inches, so area is 4 in2. If there are 10
bars in a 36 inch diameter circular column, then
s 
10( 4)

4
36
 0.039
2
or 3.9%.
The transverse steel percentage (reinforcement ratio) for a spirally confined circular column,
currently the only type of column supported in the interface, is
122
t 
 (d db 2 )
(7)
s (d cc )
Where dbt is the diameter of the transverse spiral (always smaller than the diameter of the
longitudinal bars). The spacing between transverse bars is s. The diameter of the confined core is
dcc which is the gross diameter minus twice the cover and minus the diameter of the transverse
bars (see Eq. 10). So for a #5 spiral spaced at 3 inches on center in the same column mentioned
above.
t 
5
8
 ( )2
5
3(36  2(2)  )
8
 0.013
(8)
or 1.3%.
Currently the transverse reinforcement does affect the shear response (through changes in the
uniaxial constitutive model for the concrete core). However, the columns are modeled
considering only flexurally dominated response (i.e., there is no accounting for shear flexibility
or shear degradation directly). Additional relevant details on the parameters used in both the
Cover and Core Concrete are included in Appendix D (below).
Cover concrete
The Concrete02 material is used to simulate the concrete (for both cover and core). The format
of the Concrete02 command is as follows:
uniaxialMaterial Concrete02 $matTag $fpc $epsc0 $fpcu $epsu $lambda $ft $Ets
Where $fpc is the concrete compressive strength, $epsc0 is the concrete strain at maximum
strength, $fpcu is the concrete crushing strength, $epsu is the concrete strain at crushing strength
(all of the above values are entered as negative), $lambda is the ratio between unloading slope at
$epsu and initial slope, $ft is the tensile strength, and $Ets is tension softening stiffness (absolute
value) (slope of the linear tension softening branch).
For cover concrete, $fpc is equal to the concrete unconfined strength in Table 1, $epsc0 = 0.002,
$fpcu = 0.0, $epscu = 0.006, $lambda = 0.1, $ft = (0.14)$fpc, and $Ets = $ft / $epsc0.
Core concrete
i) For core concrete of circular column cross sections according to the Mander model, the
procedure to calculate the confined concrete strength $fpc(= f cc ) is as follows:
123
f cc
f e'
f e'
 f (1.254  2.254 1  7.94 '  2 ' )
fc
fc
'
c
(9)
Where f c' is the unconfined compressive strength and f e' can be obtained from the following
equation:
f e' 
1
K e t f y
2
(10)
Where f y is the steel yield strength,  is the transverse steel percentage, and K e can be
t
obtained from the following equation for spirally confined circular columns:
S' 2
)
2d cc
Ke 
(1   cc )
(1 
(11)
Where:
cc 
As
Acc
(12)
An assumed value of the area of the confined core is used for default values. This area should be
modified based on the expected compressive block in the column during lateral loading.
 (d cc ) 2
(13)
Acc 
4
d bt 2
S 
 t d cc
'
(14)
Where dbt is the transverse bar diameter
d cc  DL  2c  d bt
(15)
Where c is the clear cover (c = 1.5”)
ii) $epsc0
epsc0 
2 f cc
Ec
(16)
124
Where:
Ec  0.043w1.5 f c'
(17)
Where w is the concrete unit weight (unit: kg/m3)
iii) $epsu (= epscu )
epscu  0.004   s
fy
f c'
t
(18)
Where  s is the ultimate steel strain (  s  0.12 )
iv) $fpcu (= f cu )
f cu 
f cc (epscu)
(
(epsc)
(epscr )
)
(epscu) (epscr )
)
(epscr )  1  (
(epsc)
(19)
Where:
epsc  (epsc0)(1  5(
epscr 
f cc
 1))
f c'
(20)
Ec
Ec 
(21)
f cc
(epsc)
_____________________________________________
Notes:
1. The information above is specific to the Steel02 and Concrete02 models of the Fiber section.
Other options include (Fig. 10), Steel01 and Concrete01 (for more information please see the
OpenSees documentation), and Elastic properties for the fibers. These options can be activated
by clicking on the default Steel02 or Concrete02 sections (Fig. 10) and changing these options.
2. A different property may be specified for the Column below grade (for instance to roughly
represent a large pile group as a large single column). If this option is selected (Fig. 7), the
column below grade will have linear properties as specified by its diameter and Young’s
Modulus).
125
3. All the equations presented in this Appendix are based on the Mander model for spiralreinforced circular concrete columns. The user may want to use their own constitutive model or
parameters. In this case, the values of these parameter can be defined directly in Fig. 10.
126
12 Appendix E: Customization of PBEE Quantities
Users can customize PBEE quantities through updating a file named PBEE.DLL which is located
at the installation folder (C:\Program Files\BridgePBEE or C:\Program Files(x86)\BridgePBEE
on a 64bit PC). Please follow the steps below to build an updated PBEE.DLL file and then
replace the one at the installation folder.
Step 1: Download PBEE.ZIP
Please go to the BridgePBEE website to download a source code project file (filename:
PBEE.zip) for Visual Studio. We'll use this one to build the PBEE.DLL file.
Step 2: Open PBEE.SLN File
Unzip PBEE.zip to a certain location and then use Visual Studio (2005 version preferred) to open
a Visual Studio Solution file named PBEE.SLN (Fig. 131).
Open the file named PBEE.CPP and make appropriate changes (Fig. 132).
Step 3: Build PBEE.DLL File
Under Visual Studio 2005, click menu Build and then Build Solution to build an updated
PBEE.DLL file (Fig. 133).
Step 4: Replace PBEE.DLL File
Make sure that BridgeBEEE is not running and then copy the new PBEE.DLL file to the
installation folder and overwrite the old one (Fig. 134).
Step 5: Run BridgePBEE
Start BridgePBEE, the program is now running with the updated PBEE quantities.
127
Fig. 131. Visual Studio file PBEE.SLN
128
Fig. 132. Modifying file PBEE.CPP
129
Fig. 133. Building PBEE.DLL in Visual Studio 2005
130
Fig. 134. Replacing file PBEE.DLL under the installation folder
131
13 References
Aviram, A., Mackie, K.R., and Stojadinovic, B. (2008). Effect of Abutment Modeling on the
Seismic Response of Bridge Structures, Earthquake Engineering and Engineering Vibration
7(4), 395-402.
Berry, M.P., and Eberhard, M.O. (2007). Performance Modeling Strategies for Modern
Reinforced Concrete Bridge Columns, Report No. 2007/07, Pacific Earthquake Engineering
Research Center, University of California, Berkeley, California.
Kotsoglu, A., and Pantazopoulou, S. (2006). Modeling of Embankment Flexibility and Soilstructure Interaction in Integral Bridges, Proceedings of First European Conference on
Earthquake Engineering and Seismology, September 3–8, Geneva, Switzerland.
Caltrans SDC, 2004. Caltrans Seismic Design Criteria, Version 1.3, California Department of
Transportation, Sacramento, California.
Caltrans SDC, 2010. Caltrans Seismic Design Criteria, Version 1.6, California Department of
Transportation, Sacramento, California.
Elgamal, A., Yang, Z., Parra, E., and Ragheb, A. 2003. Modeling of cyclic mobility in saturated
cohesionless soils. International Journal of Plasticity, 19(6), 883-905.
Elgamal, A., and Lu, J. 2009. A Framework for 3D finite element analysis of lateral pile system
response, Proceedings of the 2009 International Foundation Congress and Equipment Expo,
Contemporary Topics in In Situ Testing, Analysis, and Reliability of Foundations, ASCE
GSP 186, M. Iskander, D. F. Laefer, and M. H. Hussein, Editors, Orlando, Florida, March
15–19, pp. 616-623.
Elgamal, A., Jinchi Lu, J., and Forcellini, D. 2009a. Mitigation of liquefaction-induced lateral
deformation in a sloping stratum: 3D numerical simulation, Journal of geotechnical and
geoenvironmental engineering, ASCE, Vol. 135, No. 11, November , 1672–1682.
Elgamal, A., Lu, J., Yang, Z. and Shantz, T. 2009b. Scenario-focused three-dimensional
computational modeling in geomechanics, Alexandria, Egypt, October 3-5, 4 iYGEC'09 - 4th
International Young Geotechnical Engineers' Conference, 2 - 6 October, ISSMGE.
Elgamal, A. (2010). Calibrated 3D computational modeling of soil-structure systems and
liquefaction scenarios, Proc. Fifth Intl. Conf. on Recent Advances in Geotechnical
Earthquake Engineering and Soil Dynamics, May 24-29, San Diego, CA.
Lu J., 2006. Parallel finite element modeling of earthquake site response and liquefaction, PhD
Thesis, Department of Structural Engineering, University of California, San Diego, La Jolla,
CA.
Mackie, K.R., and Stojadinovic, B. (2005). "Fragility basis for California highway overpass
bridge seismic decision making." PEER Report No. 2005/02, Pacific Earthquake Engineering
Research Center, University of California, Berkeley.
Mackie, K. and Stojadinović, B. (2006). Seismic Vulnerability of Typical Multi-span California
Highway Bridges, Proceedings of the Fifth National Seismic Conference on Bridges and
highways, September 18–20, San Francisco.
Mackie, K.R., Wong, J-M., and Stojadinovic, B. (2008). "Integrated probabilistic performancebased evaluation of benchmark reinforced concrete bridges." PEER Report No. 2007/09,
Pacific Earthquake Engineering Research Center, University of California, Berkeley.
132
Mackie, K.R., Wong, J-M., and Stojadinovic, B. (2010). Post-earthquake bridge repair cost and
repair time estimation methodology. Earthquake Engineering and Structural Dynamics,
39(3): 281-301.
Mackie, K.R., Wong, J-M., and Stojadinovic, B. (2011). Bridge damage and loss scenarios
calibrated by schematic design and cost estimation of repairs. Earthquake Spectra, 27: 11271145.
Maroney, B.H., and Chai, Y.H. (1994). Seismic Design and Retrofitting of Reinforced Concrete
Bridges, Proceedings of 2nd International Workshop, Earthquake Commission of New
Zealand, Queenstown, New Zealand.
Mander, J.B., Priestley, M.J.N., and Park, R. (1988). Theoretical Stress–Strain Model for
Confined Concrete, Journal of the Structural Division ASCE, 114, pp. 1804–1826.
Mazzoni, S., McKenna, F., Scott, M. H., Fenves, G. L., et al. (2009). Open System for
Earthquake Engineering Simulation, User Command-Language Manual, Pacific Earthquake
Engineering Research Center, University of California, Berkeley, OpenSees version 2.0, May.
Megally, S.H., Seible, F., Bozorgzadeh, A., Restrepo, J. and Silva, P.F. (2003). Response of
Sacrificial Shear Keys in Bridge Abutments to Seismic Loading, Proceedings of the FIB
Symposium on Concrete Structures in Seismic Regions, May 6-9, Athens, Greece.
Shamsabadi, A., Rollins, K.M, and Kapuskar, M. (2007). Nonlinear Soil–Abutment–Bridge
Structure Interaction for Seismic Performance-Based Design, Journal of Geotechnical and
Geoenvironmental Engineering, 133(6), 707–720, June.
Shamsabadi, A., Khalili-Tehrani, P., Stewart, J.P., and Taciroglu, E. (2010). Validated
Simulation Models for Lateral Response of Bridge Abutments with Typical Backfills, J.
Bridge Eng., 15(3), 302-311, May.
Werner, S.D. (1994). Study of Caltrans' Seismic Evaluation Procedures for Short Bridges,
Proceedings of the 3rd Annual Seismic Research Workshop, Sacramento, California.
Yang, Z., Elgamal, A., and Parra, E. 2003. A computational model for cyclic mobility and
associated shear deformation, Journal of Geotechnical and Geoenvironmental Engineering,
129 (12), 1119-1127.
Zhang, J., and Makris, N. (2002). Kinematic Response Functions and Dynamic Stiffnesses of
Bridge Embankments, Earthquake Engineering & Structural Dynamics, 31(11), pp. 1933–
1966.
133