SapRefer3.vp CSi Refer

User Manual: CSiRefer

Open the PDF directly: View PDF .
Page Count: 556

Download
Open PDF In Browser	View PDF

CSI Analysis Reference Manual

CSI Analysis Reference Manual
For SAP2000®, ETABS®, SAFE®
and CSiBridge®

ISO# GEN062708M1 Rev.15
Berkeley, California, USA

July 2016

COPYRIGHT
Copyright © Computers & Structures, Inc., 1978-2016
All rights reserved.
The CSI Logo®, SAP2000®, ETABS®, SAFE®, CSiBridge®, and SAPFire® are
TM
registered trademarks of Computers & Structures, Inc. Model-Alive and Watch
TM
& Learn are trademarks of Computers & Structures, Inc. Windows® is a registered trademark of the Microsoft Corporation. Adobe® and Acrobat® are registered trademarks of Adobe Systems Incorporated.
The computer programs SAP2000®, ETABS®, SAFE®, and CSiBridge® and all
associated documentation are proprietary and copyrighted products. Worldwide
rights of ownership rest with Computers & Structures, Inc. Unlicensed use of these
programs or reproduction of documentation in any form, without prior written authorization from Computers & Structures, Inc., is explicitly prohibited. No part of
this publication may be reproduced or distributed in any form or by any means, or
stored in a database or retrieval system, without the prior explicit written permission of the publisher.

Further information and copies of this documentation may be obtained from:
Computers & Structures, Inc.
www.csiamerica.com
info@csiamerica.com (for general information)
support@csiamerica.com (for technical support)

DISCLAIMER
CONSIDERABLE TIME, EFFORT AND EXPENSE HAVE GONE
INTO THE DEVELOPMENT AND TESTING OF THIS SOFTWARE.
HOWEVER, THE USER ACCEPTS AND UNDERSTANDS THAT
NO WARRANTY IS EXPRESSED OR IMPLIED BY THE DEVELOPERS OR THE DISTRIBUTORS ON THE ACCURACY OR THE
RELIABILITY OF THE PROGRAMS THESE PRODUCTS.
THESE PRODUCTS ARE PRACTICAL AND POWERFUL TOOLS
FOR STRUCTURAL DESIGN. HOWEVER, THE USER MUST EXPLICITLY UNDERSTAND THE BASIC ASSUMPTIONS OF THE
SOFTWARE MODELING, ANALYSIS, AND DESIGN ALGORITHMS AND COMPENSATE FOR THE ASPECTS THAT ARE
NOT ADDRESSED.
THE INFORMATION PRODUCED BY THE SOFTWARE MUST BE
CHECKED BY A QUALIFIED AND EXPERIENCED ENGINEER.
THE ENGINEER MUST INDEPENDENTLY VERIFY THE RESULTS AND TAKE PROFESSIONAL RESPONSIBILITY FOR THE
INFORMATION THAT IS USED.

ACKNOWLEDGMENT
Thanks are due to all of the numerous structural engineers, who over the
years have given valuable feedback that has contributed toward the enhancement of this product to its current state.
Special recognition is due Dr. Edward L. Wilson, Professor Emeritus,
University of California at Berkeley, who was responsible for the conception and development of the original SAP series of programs and
whose continued originality has produced many unique concepts that
have been implemented in this version.

Table of Contents
Chapter I

Introduction
Analysis Features . . . . . . . . . . . .
Structural Analysis and Design . . . . .
About This Manual . . . . . . . . . . .
Topics. . . . . . . . . . . . . . . . . .
Typographical Conventions . . . . . .
Bold for Definitions . . . . . . . .
Bold for Variable Data. . . . . . .
Italics for Mathematical Variables .
Italics for Emphasis . . . . . . . .
Capitalized Names . . . . . . . . .
Bibliographic References . . . . . . . .

Chapter II

1
.
.
.
.
.
.
.
.
.
.
.

.
.
.
.
.
.
.
.
.
.
.

Objects and Elements

2
3
3
3
4
4
4
4
5
5
5

Objects . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7
Objects and Elements . . . . . . . . . . . . . . . . . . . . . . . . . . . 8
Groups . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9

Chapter III

Coordinate Systems
Overview . . . . . . . . . . . . . . . . . . . . .
Global Coordinate System . . . . . . . . . . . .
Upward and Horizontal Directions . . . . . . . .
Defining Coordinate Systems . . . . . . . . . . .
Vector Cross Product . . . . . . . . . . . . .
Defining the Three Axes Using Two Vectors

11
.
.
.
.
.
.

.
.
.
.
.
.

12
12
13
13
13
14

CSI Analysis Reference Manual
Local Coordinate Systems. . . . . . . . . . . . . . . . . . . . . . . . 14
Alternate Coordinate Systems . . . . . . . . . . . . . . . . . . . . . . 16
Cylindrical and Spherical Coordinates . . . . . . . . . . . . . . . . . 17

Chapter IV

Joints and Degrees of Freedom
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . .
Modeling Considerations . . . . . . . . . . . . . . . . . . .
Local Coordinate System . . . . . . . . . . . . . . . . . . .
Advanced Local Coordinate System . . . . . . . . . . . . .
Reference Vectors . . . . . . . . . . . . . . . . . . . .
Defining the Axis Reference Vector . . . . . . . . . . .
Defining the Plane Reference Vector. . . . . . . . . . .
Determining the Local Axes from the Reference Vectors
Joint Coordinate Angles . . . . . . . . . . . . . . . . .
Degrees of Freedom . . . . . . . . . . . . . . . . . . . . . .
Available and Unavailable Degrees of Freedom . . . . .
Restrained Degrees of Freedom . . . . . . . . . . . . .
Constrained Degrees of Freedom. . . . . . . . . . . . .
Mixing Restraints and Constraints Not Recommended .
Active Degrees of Freedom . . . . . . . . . . . . . . .
Null Degrees of Freedom. . . . . . . . . . . . . . . . .
Restraint Supports . . . . . . . . . . . . . . . . . . . . . . .
Spring Supports . . . . . . . . . . . . . . . . . . . . . . . .
Nonlinear Supports . . . . . . . . . . . . . . . . . . . . . .
Distributed Supports . . . . . . . . . . . . . . . . . . . . .
Joint Reactions . . . . . . . . . . . . . . . . . . . . . . . .
Base Reactions . . . . . . . . . . . . . . . . . . . . . . . .
Masses. . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Force Load . . . . . . . . . . . . . . . . . . . . . . . . . .
Ground Displacement Load . . . . . . . . . . . . . . . . . .
Restraint Displacements . . . . . . . . . . . . . . . . .
Spring Displacements . . . . . . . . . . . . . . . . . .
Link/Support Displacements . . . . . . . . . . . . . . .
Generalized Displacements . . . . . . . . . . . . . . . . . .
Degree of Freedom Output . . . . . . . . . . . . . . . . . .
Assembled Joint Mass Output. . . . . . . . . . . . . . . . .
Displacement Output . . . . . . . . . . . . . . . . . . . . .
Force Output . . . . . . . . . . . . . . . . . . . . . . . . .
Element Joint Force Output . . . . . . . . . . . . . . . . . .

21
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

22
23
24
24
25
26
26
27
28
30
31
32
32
32
33
34
34
36
37
38
39
39
40
42
42
43
44
45
45
46
47
47
48
48

Table of Contents
Chapter V

Constraints and Welds
Overview . . . . . . . . . . . . .
Body Constraint . . . . . . . . . .
Joint Connectivity . . . . . .
Local Coordinate System . . .
Constraint Equations . . . . .
Plane Definition . . . . . . . . . .
Diaphragm Constraint . . . . . . .
Joint Connectivity . . . . . .
Local Coordinate System . . .
Constraint Equations . . . . .
Plate Constraint . . . . . . . . . .
Joint Connectivity . . . . . .
Local Coordinate System . . .
Constraint Equations . . . . .
Axis Definition . . . . . . . . . .
Rod Constraint . . . . . . . . . .
Joint Connectivity . . . . . .
Local Coordinate System . . .
Constraint Equations . . . . .
Beam Constraint. . . . . . . . . .
Joint Connectivity . . . . . .
Local Coordinate System . . .
Constraint Equations . . . . .
Equal Constraint. . . . . . . . . .
Joint Connectivity . . . . . .
Local Coordinate System . . .
Selected Degrees of Freedom
Constraint Equations . . . . .
Local Constraint . . . . . . . . . .
Joint Connectivity . . . . . .
No Local Coordinate System .
Selected Degrees of Freedom
Constraint Equations . . . . .
Welds . . . . . . . . . . . . . . .
Automatic Master Joints. . . . . .
Stiffness, Mass, and Loads . .
Local Coordinate Systems . .
Constraint Output . . . . . . . . .

49
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

50
51
51
51
51
52
53
53
53
54
55
55
55
55
56
56
57
57
57
58
58
59
59
59
60
60
60
60
61
61
62
62
62
65
66
66
67
67

iii

CSI Analysis Reference Manual
Chapter VI

Material Properties

Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 70
Local Coordinate System . . . . . . . . . . . . . . . . . . . . . . . . 70
Stresses and Strains . . . . . . . . . . . . . . . . . . . . . . . . . . . 71
Isotropic Materials . . . . . . . . . . . . . . . . . . . . . . . . . . . 73
Uniaxial Materials . . . . . . . . . . . . . . . . . . . . . . . . . . . . 74
Orthotropic Materials . . . . . . . . . . . . . . . . . . . . . . . . . . 75
Anisotropic Materials . . . . . . . . . . . . . . . . . . . . . . . . . . 75
Temperature-Dependent Properties . . . . . . . . . . . . . . . . . . . 76
Element Material Temperature . . . . . . . . . . . . . . . . . . . . . 77
Mass Density . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 77
Weight Density . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 78
Material Damping . . . . . . . . . . . . . . . . . . . . . . . . . . . . 78
Modal Damping . . . . . . . . . . . . . . . . . . . . . . . . . . 79
Viscous Proportional Damping. . . . . . . . . . . . . . . . . . . 80
Hysteretic Proportional Damping . . . . . . . . . . . . . . . . . 80
Nonlinear Material Behavior . . . . . . . . . . . . . . . . . . . . . . 80
Tension and Compression . . . . . . . . . . . . . . . . . . . . . 81
Shear . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 81
Hysteresis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 82
Application . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 83
Friction and Dilitational Angles . . . . . . . . . . . . . . . . . . 84
Hysteresis Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . 85
Backbone Curve (Action vs. Deformation) . . . . . . . . . . . . 86
Cyclic Behavior. . . . . . . . . . . . . . . . . . . . . . . . . . . 86
Elastic Hysteresis Model . . . . . . . . . . . . . . . . . . . . . . 88
Kinematic Hysteresis Model . . . . . . . . . . . . . . . . . . . . 88
Degrading Hysteresis Model . . . . . . . . . . . . . . . . . . . . 89
Takeda Hysteresis Model. . . . . . . . . . . . . . . . . . . . . . 93
Pivot Hysteresis Model . . . . . . . . . . . . . . . . . . . . . . . 94
Concrete Hysteresis Model . . . . . . . . . . . . . . . . . . . . . 95
BRB Hardening Hysteresis Model . . . . . . . . . . . . . . . . . 97
Isotropic Hysteresis Model . . . . . . . . . . . . . . . . . . . . . 99
Modified Darwin-Pecknold Concrete Model . . . . . . . . . . . . . 100
Time-dependent Properties . . . . . . . . . . . . . . . . . . . . . . 101
Properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 101
Time-Integration Control . . . . . . . . . . . . . . . . . . . . . 102
Design-Type . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 102

Table of Contents
Chapter VII

The Frame Element
Overview. . . . . . . . . . . . . . . . . . . . . .
Joint Connectivity . . . . . . . . . . . . . . . . .
Insertion Points . . . . . . . . . . . . . . . .
Degrees of Freedom . . . . . . . . . . . . . . . .
Local Coordinate System . . . . . . . . . . . . .
Longitudinal Axis 1 . . . . . . . . . . . . . .
Default Orientation . . . . . . . . . . . . . .
Coordinate Angle . . . . . . . . . . . . . . .
Advanced Local Coordinate System . . . . . . . .
Reference Vector . . . . . . . . . . . . . . .
Determining Transverse Axes 2 and 3 . . . .
Section Properties . . . . . . . . . . . . . . . . .
Local Coordinate System . . . . . . . . . . .
Material Properties . . . . . . . . . . . . . .
Geometric Properties and Section Stiffnesses.
Shape Type . . . . . . . . . . . . . . . . . .
Automatic Section Property Calculation . . .
Section Property Database Files. . . . . . . .
Section-Designer Sections . . . . . . . . . .
Additional Mass and Weight . . . . . . . . .
Non-prismatic Sections . . . . . . . . . . . .
Property Modifiers . . . . . . . . . . . . . . . . .
Named Property Sets . . . . . . . . . . . . .
Insertion Points . . . . . . . . . . . . . . . . . .
Local Axes . . . . . . . . . . . . . . . . . .
End Offsets. . . . . . . . . . . . . . . . . . . . .
Clear Length. . . . . . . . . . . . . . . . . .
Rigid-end Factor . . . . . . . . . . . . . . .
Effect upon Non-prismatic Elements . . . . .
Effect upon Internal Force Output . . . . . .
Effect upon End Releases . . . . . . . . . . .
End Releases . . . . . . . . . . . . . . . . . . . .
Unstable End Releases . . . . . . . . . . . .
Effect of End Offsets . . . . . . . . . . . . .
Named Property Sets . . . . . . . . . . . . .
Nonlinear Properties . . . . . . . . . . . . . . . .
Tension/Compression Limits . . . . . . . . .
Plastic Hinge . . . . . . . . . . . . . . . . .
Mass . . . . . . . . . . . . . . . . . . . . . . . .
Self-Weight Load . . . . . . . . . . . . . . . . .

105
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

106
107
107
108
108
109
109
110
110
112
113
114
115
115
116
116
118
118
118
120
120
123
124
125
126
127
129
129
130
130
130
131
132
132
132
133
133
134
134
134

CSI Analysis Reference Manual
Gravity Load . . . . . . .
Concentrated Span Load .
Distributed Span Load . .
Loaded Length . . .
Load Intensity . . . .
Projected Loads . . .
Temperature Load . . . .
Strain Load . . . . . . . .
Deformation Load . . . .
Target-Force Load . . . .
Internal Force Output . .
Effect of End Offsets
Stress Output . . . . . . .

Chapter VIII

.
.
.
.
.
.
.
.
.
.
.
.
.

135
135
137
137
137
137
140
141
141
142
142
144
144

147
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

The Cable Element
Overview. . . . . . . . . . . .
Joint Connectivity . . . . . . .
Undeformed Length . . . . . .
Shape Calculator . . . . . . . .
Cable vs. Frame Elements.
Number of Segments . . .
Degrees of Freedom . . . . . .

.
.
.
.
.
.
.
.
.
.
.
.
.

Hinge Properties
Overview. . . . . . . . . . . . . . . . . . . . . . .
Hinge Properties . . . . . . . . . . . . . . . . . . .
Hinge Length . . . . . . . . . . . . . . . . . .
Plastic Deformation Curve . . . . . . . . . . .
Scaling the Curve . . . . . . . . . . . . . . . .
Strength Loss . . . . . . . . . . . . . . . . . .
Types of P-M2-M3 Hinges . . . . . . . . . . .
Isotropic P-M2-M3 Hinge. . . . . . . . . . . .
Parametric P-M2-M3 Hinge. . . . . . . . . . .
Fiber P-M2-M3 Hinge . . . . . . . . . . . . .
Hysteresis Models . . . . . . . . . . . . . . . .
Automatic, User-Defined, and Generated Properties
Automatic Hinge Properties . . . . . . . . . . . . .
Analysis Modeling . . . . . . . . . . . . . . . . . .
Computational Considerations . . . . . . . . . . . .
Analysis Results . . . . . . . . . . . . . . . . . . .

Chapter IX

.
.
.
.
.
.
.
.
.
.
.
.
.

147
149
150
150
151
152
153
153
156
156
157
158
159
161
162
163

165
.
.
.
.
.
.
.

.
.
.
.
.
.
.

166
167
167
168
169
170
170

Table of Contents
Local Coordinate System . . . . . . . . . . . . .
Section Properties . . . . . . . . . . . . . . . . .
Material Properties . . . . . . . . . . . . . .
Geometric Properties and Section Stiffnesses.
Mass . . . . . . . . . . . . . . . . . . . . . . . .
Self-Weight Load . . . . . . . . . . . . . . . . .
Gravity Load . . . . . . . . . . . . . . . . . . . .
Distributed Span Load . . . . . . . . . . . . . . .
Temperature Load . . . . . . . . . . . . . . . . .
Strain and Deformation Load . . . . . . . . . . .
Target-Force Load . . . . . . . . . . . . . . . . .
Nonlinear Analysis. . . . . . . . . . . . . . . . .
Element Output . . . . . . . . . . . . . . . . . .

Chapter X

.
.
.
.
.
.
.
.
.
.
.
.
.

The Shell Element
Overview. . . . . . . . . . . . . . . . . . . .
Homogeneous . . . . . . . . . . . . . . .
Layered . . . . . . . . . . . . . . . . . .
Joint Connectivity . . . . . . . . . . . . . . .
Shape Guidelines . . . . . . . . . . . . .
Edge Constraints . . . . . . . . . . . . . . . .
Degrees of Freedom . . . . . . . . . . . . . .
Local Coordinate System . . . . . . . . . . .
Normal Axis 3. . . . . . . . . . . . . . .
Default Orientation . . . . . . . . . . . .
Element Coordinate Angle . . . . . . . .
Advanced Local Coordinate System . . . . . .
Reference Vector . . . . . . . . . . . . .
Determining Tangential Axes 1 and 2 . .
Section Properties . . . . . . . . . . . . . . .
Area Section Type. . . . . . . . . . . . .
Shell Section Type . . . . . . . . . . . .
Homogeneous Section Properties . . . . .
Layered Section Property . . . . . . . . .
Property Modifiers . . . . . . . . . . . . . . .
Named Property Sets . . . . . . . . . . .
Joint Offsets and Thickness Overwrites . . . .
Joint Offsets . . . . . . . . . . . . . . . .
Effect of Joint Offsets on the Local Axes .
Thickness Overwrites . . . . . . . . . . .

170
171
171
172
172
172
173
173
174
174
174
175
175

177
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

178
179
179
180
180
183
184
185
186
186
186
186
188
189
190
190
190
191
193
201
202
203
203
204
205

vii

CSI Analysis Reference Manual
Mass . . . . . . . . . . . . . . .
Self-Weight Load . . . . . . . .
Gravity Load . . . . . . . . . . .
Uniform Load . . . . . . . . . .
Surface Pressure Load . . . . . .
Temperature Load . . . . . . . .
Strain Load . . . . . . . . . . . .
Internal Force and Stress Output.

Chapter XI

.
.
.
.
.
.
.
.

206
206
207
207
208
209
210
210

215
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

The Asolid Element
Overview. . . . . . . . .
Joint Connectivity . . . .
Degrees of Freedom . . .
Local Coordinate System
Stresses and Strains . . .
Section Properties . . . .
Section Type . . . .
Material Properties .
Material Angle . . .

viii

.
.
.
.
.
.
.
.

The Plane Element
Overview. . . . . . . . . . . . . .
Joint Connectivity . . . . . . . . .
Degrees of Freedom . . . . . . . .
Local Coordinate System . . . . .
Stresses and Strains . . . . . . . .
Section Properties . . . . . . . . .
Section Type . . . . . . . . .
Material Properties . . . . . .
Material Angle . . . . . . . .
Thickness . . . . . . . . . . .
Incompatible Bending Modes .
Mass . . . . . . . . . . . . . . . .
Self-Weight Load . . . . . . . . .
Gravity Load . . . . . . . . . . . .
Surface Pressure Load . . . . . . .
Pore Pressure Load. . . . . . . . .
Temperature Load . . . . . . . . .
Stress Output . . . . . . . . . . . .

Chapter XII

.
.
.
.
.
.
.
.

216
217
217
217
217
218
218
219
219
219
220
220
221
221
222
222
223
223

225
.
.
.
.
.
.
.
.
.

.
.
.
.
.
.
.
.
.

226
226
227
227
228
228
228
229
229

Table of Contents
Axis of Symmetry . . . . . . .
Arc and Thickness. . . . . . .
Incompatible Bending Modes .
Mass . . . . . . . . . . . . . . . .
Self-Weight Load . . . . . . . . .
Gravity Load . . . . . . . . . . . .
Surface Pressure Load . . . . . . .
Pore Pressure Load. . . . . . . . .
Temperature Load . . . . . . . . .
Rotate Load . . . . . . . . . . . .
Stress Output . . . . . . . . . . . .

Chapter XIII

.
.
.
.
.
.
.
.
.
.
.

The Solid Element
Overview. . . . . . . . . . . . . . . . . . . . . . . . . . . .
Joint Connectivity . . . . . . . . . . . . . . . . . . . . . . .
Degenerate Solids . . . . . . . . . . . . . . . . . . . . .
Degrees of Freedom . . . . . . . . . . . . . . . . . . . . . .
Local Coordinate System . . . . . . . . . . . . . . . . . . .
Advanced Local Coordinate System . . . . . . . . . . . . . .
Reference Vectors . . . . . . . . . . . . . . . . . . . . .
Defining the Axis Reference Vector . . . . . . . . . . .
Defining the Plane Reference Vector . . . . . . . . . . .
Determining the Local Axes from the Reference Vectors
Element Coordinate Angles . . . . . . . . . . . . . . . .
Stresses and Strains . . . . . . . . . . . . . . . . . . . . . .
Solid Properties . . . . . . . . . . . . . . . . . . . . . . . .
Material Properties . . . . . . . . . . . . . . . . . . . .
Material Angles . . . . . . . . . . . . . . . . . . . . . .
Incompatible Bending Modes . . . . . . . . . . . . . . .
Mass . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Self-Weight Load . . . . . . . . . . . . . . . . . . . . . . .
Gravity Load . . . . . . . . . . . . . . . . . . . . . . . . . .
Surface Pressure Load . . . . . . . . . . . . . . . . . . . . .
Pore Pressure Load. . . . . . . . . . . . . . . . . . . . . . .
Temperature Load . . . . . . . . . . . . . . . . . . . . . . .
Stress Output . . . . . . . . . . . . . . . . . . . . . . . . . .

Chapter XIV

.
.
.
.
.
.
.
.
.
.
.

The Link/Support Element—Basic

230
231
232
232
232
233
233
234
234
234
235

237
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

238
238
239
240
240
240
241
241
242
243
243
246
246
246
246
247
248
248
249
249
249
250
250

251

Overview. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 252

CSI Analysis Reference Manual
Joint Connectivity . . . . . . . . . . . . . . . . . . . . . . . .
Conversion from One-Joint Objects to Two-Joint Elements
Zero-Length Elements . . . . . . . . . . . . . . . . . . . . . .
Degrees of Freedom . . . . . . . . . . . . . . . . . . . . . . .
Local Coordinate System . . . . . . . . . . . . . . . . . . . .
Longitudinal Axis 1 . . . . . . . . . . . . . . . . . . . . .
Default Orientation . . . . . . . . . . . . . . . . . . . . .
Coordinate Angle . . . . . . . . . . . . . . . . . . . . . .
Advanced Local Coordinate System . . . . . . . . . . . . . . .
Axis Reference Vector . . . . . . . . . . . . . . . . . . .
Plane Reference Vector . . . . . . . . . . . . . . . . . . .
Determining Transverse Axes 2 and 3 . . . . . . . . . . .
Internal Deformations . . . . . . . . . . . . . . . . . . . . . .
Link/Support Properties . . . . . . . . . . . . . . . . . . . . .
Local Coordinate System . . . . . . . . . . . . . . . . . .
Internal Spring Hinges . . . . . . . . . . . . . . . . . . .
Spring Force-Deformation Relationships . . . . . . . . . .
Element Internal Forces . . . . . . . . . . . . . . . . . . .
Uncoupled Linear Force-Deformation Relationships . . . .
Types of Linear/Nonlinear Properties. . . . . . . . . . . .
Coupled Linear Property . . . . . . . . . . . . . . . . . . . . .
Fixed Degrees of Freedom . . . . . . . . . . . . . . . . . . . .
Mass . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Self-Weight Load . . . . . . . . . . . . . . . . . . . . . . . .
Gravity Load . . . . . . . . . . . . . . . . . . . . . . . . . . .
Internal Force and Deformation Output . . . . . . . . . . . . .

Chapter XV

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

The Link/Support Element—Advanced
Overview. . . . . . . . . . . . . . . . . . . . .
Nonlinear Link/Support Properties . . . . . . .
Linear Effective Stiffness . . . . . . . . . . . .
Special Considerations for Modal Analyses
Linear Effective Damping . . . . . . . . . . . .
Exponential Maxwell Damper Property . . . . .
Bilinear Maxwell Damper Property . . . . . . .
Friction-Spring Damper Property . . . . . . . .
Gap Property . . . . . . . . . . . . . . . . . . .
Hook Property . . . . . . . . . . . . . . . . . .
Wen Plasticity Property . . . . . . . . . . . . .
Multi-Linear Elastic Property . . . . . . . . . .

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

253
253
253
254
254
255
255
256
256
257
258
259
260
263
264
264
266
267
267
269
270
270
271
272
272
273

275
.
.
.
.
.
.
.
.
.
.
.
.

.
.
.
.
.
.
.
.
.
.
.
.

276
276
277
277
278
279
281
282
286
286
287
289

Table of Contents
Multi-Linear Plastic Property . . . . . . . . . . . .
Hysteretic (Rubber) Isolator Property . . . . . . . .
Friction-Pendulum Isolator Property. . . . . . . . .
Axial Behavior . . . . . . . . . . . . . . . . .
Shear Behavior . . . . . . . . . . . . . . . . .
Linear Behavior . . . . . . . . . . . . . . . . .
Double-Acting Friction-Pendulum Isolator Property
Axial Behavior . . . . . . . . . . . . . . . . .
Shear Behavior . . . . . . . . . . . . . . . . .
Linear Behavior . . . . . . . . . . . . . . . . .
Triple-Pendulum Isolator Property. . . . . . . . . .
Axial Behavior . . . . . . . . . . . . . . . . .
Shear Behavior . . . . . . . . . . . . . . . . .
Linear Behavior . . . . . . . . . . . . . . . . .
Nonlinear Deformation Loads . . . . . . . . . . . .
Frequency-Dependent Link/Support Properties . . .

Chapter XVI

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

The Tendon Object
Overview. . . . . . . . . . . . . . . . . . . . . .
Geometry. . . . . . . . . . . . . . . . . . . . . .
Discretization . . . . . . . . . . . . . . . . . . .
Tendons Modeled as Loads or Elements. . . . . .
Connectivity . . . . . . . . . . . . . . . . . . . .
Degrees of Freedom . . . . . . . . . . . . . . . .
Local Coordinate Systems . . . . . . . . . . . . .
Base-line Local Coordinate System . . . . . .
Natural Local Coordinate System . . . . . . .
Section Properties . . . . . . . . . . . . . . . . .
Material Properties . . . . . . . . . . . . . .
Geometric Properties and Section Stiffnesses.
Tension/Compression Limits . . . . . . . . . . .
Mass . . . . . . . . . . . . . . . . . . . . . . . .
Prestress Load . . . . . . . . . . . . . . . . . . .
Self-Weight Load . . . . . . . . . . . . . . . . .
Gravity Load . . . . . . . . . . . . . . . . . . . .
Temperature Load . . . . . . . . . . . . . . . . .
Strain Load . . . . . . . . . . . . . . . . . . . . .
Deformation Load . . . . . . . . . . . . . . . . .
Target-Force Load . . . . . . . . . . . . . . . . .
Internal Force Output . . . . . . . . . . . . . . .

289
291
292
293
294
297
297
297
298
299
299
299
300
304
304
306

309
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

310
310
311
311
311
312
313
313
313
314
314
314
315
316
316
317
318
318
318
319
319
320

CSI Analysis Reference Manual
Chapter XVII Load Patterns

321

Overview. . . . . . . . . . . . . . . . . . . . . . .
Load Patterns, Load Cases, and Load Combinations
Defining Load Patterns . . . . . . . . . . . . . . .
Coordinate Systems and Load Components . . . . .
Effect upon Large-Displacements Analysis. . .
Force Load . . . . . . . . . . . . . . . . . . . . . .
Ground Displacement Load . . . . . . . . . . . . .
Self-Weight Load . . . . . . . . . . . . . . . . . .
Gravity Load . . . . . . . . . . . . . . . . . . . . .
Concentrated Span Load . . . . . . . . . . . . . . .
Distributed Span Load . . . . . . . . . . . . . . . .
Tendon Prestress Load . . . . . . . . . . . . . . . .
Uniform Load . . . . . . . . . . . . . . . . . . . .
Surface Pressure Load . . . . . . . . . . . . . . . .
Pore Pressure Load. . . . . . . . . . . . . . . . . .
Temperature Load . . . . . . . . . . . . . . . . . .
Strain Load . . . . . . . . . . . . . . . . . . . . . .
Deformation Load . . . . . . . . . . . . . . . . . .
Target-Force Load . . . . . . . . . . . . . . . . . .
Rotate Load . . . . . . . . . . . . . . . . . . . . .
Joint Patterns . . . . . . . . . . . . . . . . . . . . .
Mass Source . . . . . . . . . . . . . . . . . . . . .
Mass from Specified Load Patterns . . . . . . .
Negative Mass. . . . . . . . . . . . . . . . . .
Multiple Mass Sources . . . . . . . . . . . . .
Automated Lateral Loads . . . . . . . . . . . .
Acceleration Loads. . . . . . . . . . . . . . . . . .

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

Chapter XVIII Load Cases
Overview. . . . . . . . . . . . .
Load Cases . . . . . . . . . . . .
Types of Analysis . . . . . . . .
Sequence of Analysis . . . . . .
Running Load Cases . . . . . . .
Linear and Nonlinear Load Cases
Linear Static Analysis . . . . . .
Multi-Step Static Analysis . . . .

xii

322
323
323
324
324
325
325
325
326
327
327
327
328
328
328
330
331
331
331
332
332
334
335
336
336
338
338

341
.
.
.
.
.
.
.
.

.
.
.
.
.
.
.
.

342
343
343
344
345
346
347
348

Table of Contents
Linear Buckling Analysis . . . . . . . . . . . . . . .
Functions. . . . . . . . . . . . . . . . . . . . . . . .
Load Combinations (Combos) . . . . . . . . . . . . .
Contributing Cases . . . . . . . . . . . . . . . .
Types of Combos . . . . . . . . . . . . . . . . .
Examples . . . . . . . . . . . . . . . . . . . . .
Correspondence . . . . . . . . . . . . . . . . . .
Additional Considerations. . . . . . . . . . . . .
Global Energy Response . . . . . . . . . . . . . . . .
Equation Solvers . . . . . . . . . . . . . . . . . . . .
Environment Variables to Control Analysis . . . . . .
SAPFIRE_NUM_THREADS. . . . . . . . . . .
SAPFIRE_FILESIZE_MB . . . . . . . . . . . .
Accessing the Assembled Stiffness and Mass Matrices

Chapter XIX

.
.
.
.
.
.
.
.
.
.
.
.
.
.

Modal Analysis
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

Response-Spectrum Analysis
Overview. . . . . . . . . . .
Local Coordinate System . .
Response-Spectrum Function
Damping. . . . . . . . .
Modal Damping . . . . . . .
Modal Combination . . . . .

349
350
351
351
352
353
354
357
357
361
362
362
363
363

365

Overview. . . . . . . . . . . . . . . . . . . . . .
Eigenvector Analysis . . . . . . . . . . . . . . .
Number of Modes . . . . . . . . . . . . . . .
Frequency Range . . . . . . . . . . . . . . .
Automatic Shifting . . . . . . . . . . . . . .
Convergence Tolerance . . . . . . . . . . . .
Static-Correction Modes . . . . . . . . . . .
Ritz-Vector Analysis . . . . . . . . . . . . . . . .
Number of Modes . . . . . . . . . . . . . . .
Starting Load Vectors . . . . . . . . . . . . .
Number of Generation Cycles. . . . . . . . .
Modal Analysis Output . . . . . . . . . . . . . .
Periods and Frequencies . . . . . . . . . . .
Participation Factors . . . . . . . . . . . . .
Participating Mass Ratios . . . . . . . . . . .
Static and Dynamic Load Participation Ratios

Chapter XX

.
.
.
.
.
.
.
.
.
.
.
.
.
.

365
366
367
368
369
369
370
372
373
373
375
375
376
376
377
378

383
.
.
.
.
.
.

.
.
.
.
.
.

383
385
385
386
387
388

xiii

CSI Analysis Reference Manual
Periodic and Rigid Response . .
CQC Method . . . . . . . . . .
GMC Method . . . . . . . . . .
SRSS Method . . . . . . . . . .
Absolute Sum Method . . . . .
NRC Ten-Percent Method . . .
NRC Double-Sum Method . . .
Directional Combination . . . . . . .
SRSS Method . . . . . . . . . .
CQC3 Method . . . . . . . . . .
Absolute Sum Method . . . . .
Response-Spectrum Analysis Output
Damping and Accelerations . . .
Modal Amplitudes. . . . . . . .
Base Reactions . . . . . . . . .

Chapter XXI

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

Linear Time-History Analysis
Overview. . . . . . . . . . . . . . . . . .
Loading . . . . . . . . . . . . . . . . . .
Defining the Spatial Load Vectors . .
Defining the Time Functions . . . . .
Initial Conditions. . . . . . . . . . . . . .
Time Steps . . . . . . . . . . . . . . . . .
Modal Time-History Analysis . . . . . . .
Modal Damping . . . . . . . . . . . .
Direct-Integration Time-History Analysis .
Time Integration Parameters . . . . .
Damping. . . . . . . . . . . . . . . .

397
.
.
.
.
.
.
.
.
.
.
.

.
.
.
.
.
.
.
.
.
.
.

Chapter XXII Geometric Nonlinearity
Overview. . . . . . . . . . . . . . . . . . . . .
Nonlinear Load Cases . . . . . . . . . . . . . .
The P-Delta Effect . . . . . . . . . . . . . . . .
P-Delta Forces in the Frame Element . . . .
P-Delta Forces in the Link/Support Element
Other Elements . . . . . . . . . . . . . . .
Initial P-Delta Analysis . . . . . . . . . . . . .
Building Structures . . . . . . . . . . . . .
Cable Structures . . . . . . . . . . . . . . .
Guyed Towers. . . . . . . . . . . . . . . .
Large Displacements . . . . . . . . . . . . . . .

xiv

388
390
390
390
391
391
391
391
391
392
393
394
394
394
395

398
398
399
400
402
402
403
404
405
406
406

409
.
.
.
.
.
.
.
.
.
.
.

.
.
.
.
.
.
.
.
.
.
.

409
411
413
415
418
419
419
420
422
422
422

Table of Contents
Applications . . . . . . . . . . . . . . . . . . . . . . . . . . . . 423
Initial Large-Displacement Analysis . . . . . . . . . . . . . . . 423

Chapter XXIII Nonlinear Static Analysis
Overview. . . . . . . . . . . . . . .
Nonlinearity . . . . . . . . . . . . .
Important Considerations . . . . . .
Loading . . . . . . . . . . . . . . .
Load Application Control . . . . . .
Load Control . . . . . . . . . .
Displacement Control . . . . . .
Initial Conditions. . . . . . . . . . .
Output Steps . . . . . . . . . . . . .
Saving Multiple Steps . . . . . .
Nonlinear Solution Control . . . . .
Maximum Total Steps . . . . . .
Maximum Null (Zero) Steps . .
Event-to-Event Stepping Control
Nonlinear Iteration . . . . . . .
Line Search Option . . . . . . .
Static Pushover Analysis. . . . . . .
Staged Construction . . . . . . . . .
Stages . . . . . . . . . . . . . .
Changing Section Properties . .
Output Steps. . . . . . . . . . .
Example . . . . . . . . . . . . .
Target-Force Iteration . . . . . . . .

425
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

Chapter XXIV Nonlinear Time-History Analysis
Overview. . . . . . . . . . . . . . . . . . . . .
Nonlinearity . . . . . . . . . . . . . . . . . . .
Loading . . . . . . . . . . . . . . . . . . . . .
Initial Conditions. . . . . . . . . . . . . . . . .
Time Steps . . . . . . . . . . . . . . . . . . . .
Nonlinear Modal Time-History Analysis (FNA)
Initial Conditions . . . . . . . . . . . . . .
Link/Support Effective Stiffness . . . . . .
Mode Superposition . . . . . . . . . . . . .
Modal Damping . . . . . . . . . . . . . . .
Iterative Solution . . . . . . . . . . . . . .

426
426
427
428
428
429
429
430
431
431
433
434
434
434
435
436
437
439
439
442
442
443
444

447
.
.
.
.
.
.
.
.
.
.
.

.
.
.
.
.
.
.
.
.
.
.

448
448
449
449
450
451
451
452
452
454
455

CSI Analysis Reference Manual
Static Period . . . . . . . . . . . . . . . . . . .
Nonlinear Direct-Integration Time-History Analysis
Time Integration Parameters . . . . . . . . . .
Nonlinearity . . . . . . . . . . . . . . . . . . .
Initial Conditions . . . . . . . . . . . . . . . .
Damping. . . . . . . . . . . . . . . . . . . . .
Nonlinear Solution Control . . . . . . . . . . .

.
.
.
.
.
.
.

Chapter XXV Frequency-Domain Analyses

465

Overview. . . . . . . . . . . . . . . .
Harmonic Motion . . . . . . . . . . .
Frequency Domain . . . . . . . . . . .
Damping . . . . . . . . . . . . . . . .
Sources of Damping. . . . . . . .
Loading . . . . . . . . . . . . . . . .
Defining the Spatial Load Vectors
Frequency Steps . . . . . . . . . . . .
Steady-State Analysis . . . . . . . . .
Example . . . . . . . . . . . . . .
Power-Spectral-Density Analysis . . .
Example . . . . . . . . . . . . . .

.
.
.
.
.
.
.
.
.
.
.
.

Chapter XXVI Moving-Load Analysis
Overview for CSiBridge . . . . . . .
Moving-Load Analysis in SAP2000 .
Bridge Modeler . . . . . . . . . . .
Moving-Load Analysis Procedure . .
Lanes . . . . . . . . . . . . . . . . .
Centerline and Direction . . . .
Eccentricity . . . . . . . . . . .
Centrifugal Radius . . . . . . .
Width . . . . . . . . . . . . . .
Interior and Exterior Edges . . .
Discretization . . . . . . . . . .
Influence Lines and Surfaces . . . .
Vehicle Live Loads . . . . . . . . .
Distribution of Loads . . . . . .
Axle Loads . . . . . . . . . . .
Uniform Loads . . . . . . . . .
Minimum Edge Distances . . . .

xvi

457
458
458
459
459
459
461

466
466
467
468
468
469
470
471
471
472
473
474

477
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

478
479
480
481
482
482
482
483
483
483
484
485
487
487
487
487
487

Table of Contents
Directions of Loading . . . . . . . . . . . . . . . . .
Restricting a Vehicle to the Lane Length . . . . . . .
Application of Loads to the Influence Surface . . . .
Length Effects. . . . . . . . . . . . . . . . . . . . .
Application of Loads in Multi-Step Analysis . . . . .
General Vehicle . . . . . . . . . . . . . . . . . . . . . .
Specification . . . . . . . . . . . . . . . . . . . . .
Moving the Vehicle . . . . . . . . . . . . . . . . . .
Vehicle Response Components . . . . . . . . . . . . . .
Superstructure (Span) Moment . . . . . . . . . . . .
Negative Superstructure (Span) Moment . . . . . . .
Reactions at Interior Supports . . . . . . . . . . . .
Standard Vehicles . . . . . . . . . . . . . . . . . . . . .
Vehicle Classes . . . . . . . . . . . . . . . . . . . . . .
Moving-Load Load Cases . . . . . . . . . . . . . . . . .
Directions of Loading . . . . . . . . . . . . . . . . .
Example 1 — AASHTO HS Loading. . . . . . . . .
Example 2 — AASHTO HL Loading. . . . . . . . .
Example 3 — Caltrans Permit Loading . . . . . . . .
Example 4 — Restricted Caltrans Permit Loading . .
Example 5 — Eurocode Characteristic Load Model 1
Moving Load Response Control . . . . . . . . . . . . . .
Bridge Response Groups . . . . . . . . . . . . . . .
Correspondence . . . . . . . . . . . . . . . . . . . .
Influence Line Tolerance . . . . . . . . . . . . . . .
Exact and Quick Response Calculation . . . . . . . .
Step-By-Step Analysis . . . . . . . . . . . . . . . . . . .
Loading . . . . . . . . . . . . . . . . . . . . . . . .
Static Analysis. . . . . . . . . . . . . . . . . . . . .
Time-History Analysis . . . . . . . . . . . . . . . .
Enveloping and Load Combinations . . . . . . . . .
Computational Considerations . . . . . . . . . . . . . . .

Chapter XXVII References

.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.

488
492
492
494
495
495
497
498
498
498
499
500
500
508
509
510
512
513
514
516
518
519
519
520
520
521
521
522
522
523
524
524

527

xvii

Chapter I

Introduction
SAP2000, ETABS, SAFE, and CSiBridge are software packages from Computers
and Structures, Inc. for structural analysis and design. Each package is a fully integrated system for modeling, analyzing, designing, and optimizing structures of a
particular type:
• SAP2000 for general structures, including stadiums, towers, industrial plants,
offshore structures, piping systems, buildings, dams, soils, machine parts and
many others
• ETABS for building structures
• SAFE for floor slabs and base mats
• CSiBridge for bridge structures
At the heart of each of these software packages is a common analysis engine, referred to throughout this manual as SAPfire. This engine is the latest and most powerful version of the well-known SAP series of structural analysis programs. The
purpose of this manual is to describe the features of the SAPfire analysis engine.
Throughout this manual reference may be made to the program SAP2000, although
it often applies equally to ETABS, SAFE, and CSiBridge. Not all features described will actually be available in every level of each program.

CSI Analysis Reference Manual

Analysis Features
The SAPfire analysis engine offers the following features:
• Static and dynamic analysis
• Linear and nonlinear analysis
• Dynamic seismic analysis and static pushover analysis
• Vehicle live-load analysis for bridges
• Geometric nonlinearity, including P-delta and large-displacement effects
• Staged (incremental) construction
• Creep, shrinkage, and aging effects
• Buckling analysis
• Steady-state and power-spectral-density analysis
• Frame and shell structural elements, including beam-column, truss, membrane,
and plate behavior
• Cable and Tendon elements
• Two-dimensional plane and axisymmetric solid elements
• Three-dimensional solid elements
• Nonlinear link and support elements
• Frequency-dependent link and support properties
• Multiple coordinate systems
• Many types of constraints
• A wide variety of loading options
• Alpha-numeric labels
• Large capacity
• Highly efficient and stable solution algorithms
These features, and many more, make CSI product the state-of-the-art for structural
analysis. Note that not all of these features may be available in every level of
SAP2000, ETABS, SAFE, and CSiBridge.

Analysis Features

Chapter I

Introduction

Structural Analysis and Design
The following general steps are required to analyze and design a structure using
SAP2000, ETABS, SAFE, and CSiBridge:
1. Create or modify a model that numerically defines the geometry, properties,
loading, and analysis parameters for the structure
2. Perform an analysis of the model
3. Review the results of the analysis
4. Check and optimize the design of the structure
This is usually an iterative process that may involve several cycles of the above sequence of steps. All of these steps can be performed seamlessly using the SAP2000,
ETABS, SAFE, and CSiBridge graphical user interfaces.

About This Manual
This manual describes the theoretical concepts behind the modeling and analysis
features offered by the SAPfire analysis engine that underlies the various structural
analysis and design software packages from Computers and Structures, Inc. The
graphical user interface and the design features are described in separate manuals
for each program.
It is imperative that you read this manual and understand the assumptions and procedures used by these software packages before attempting to use the analysis features.
Throughout this manual reference may be made to the program SAP2000, although
it often applies equally to ETABS, SAFE, and CSiBridge. Not all features described will actually be available in every level of each program.

Topics
Each Chapter of this manual is divided into topics and subtopics. All Chapters begin with a list of topics covered. These are divided into two groups:
• Basic topics — recommended reading for all users

Structural Analysis and Design

CSI Analysis Reference Manual
• Advanced topics — for users with specialized needs, and for all users as they
become more familiar with the program.
Following the list of topics is an Overview which provides a summary of the Chapter. Reading the Overview for every Chapter will acquaint you with the full scope
of the program.

Typographical Conventions
Throughout this manual the following typographic conventions are used.

Bold for Definitions
Bold roman type (e.g., example) is used whenever a new term or concept is defined. For example:
The global coordinate system is a three-dimensional, right-handed, rectangular coordinate system.
This sentence begins the definition of the global coordinate system.

Bold for Variable Data
Bold roman type (e.g., example) is used to represent variable data items for which
you must specify values when defining a structural model and its analysis. For example:
The Frame element coordinate angle, ang, is used to define element orientations that are different from the default orientation.
Thus you will need to supply a numeric value for the variable ang if it is different
from its default value of zero.

Italics for Mathematical Variables
Normal italic type (e.g., example) is used for scalar mathematical variables, and
bold italic type (e.g., example) is used for vectors and matrices. If a variable data
item is used in an equation, bold roman type is used as discussed above. For example:
0 £ da < db £ L

Typographical Conventions

Chapter I

Introduction

Here da and db are variables that you specify, and L is a length calculated by the
program.

Italics for Emphasis
Normal italic type (e.g., example) is used to emphasize an important point, or for
the title of a book, manual, or journal.

Capitalized Names
Capitalized names (e.g., Example) are used for certain parts of the model and its
analysis which have special meaning to SAP2000. Some examples:
Frame element
Diaphragm Constraint
Frame Section
Load Pattern
Common entities, such as “joint” or “element” are not capitalized.

Bibliographic References
References are indicated throughout this manual by giving the name of the
author(s) and the date of publication, using parentheses. For example:
See Wilson and Tetsuji (1983).
It has been demonstrated (Wilson, Yuan, and Dickens, 1982) that …
All bibliographic references are listed in alphabetical order in Chapter “References” (page 527).

Bibliographic References

CSI Analysis Reference Manual

Bibliographic References

C h a p t e r II

Objects and Elements
The physical structural members in a structural model are represented by objects.
Using the graphical user interface, you “draw” the geometry of an object, then “assign” properties and loads to the object to completely define the model of the physical member. For analysis purposes, SAP2000 converts each object into one or more
elements.
Basic Topics for All Users
• Objects
• Objects and Elements
• Groups

Objects
The following object types are available, listed in order of geometrical dimension:
• Point objects, of two types:
– Joint objects: These are automatically created at the corners or ends of all
other types of objects below, and they can be explicitly added to represent
supports or to capture other localized behavior.

Objects

CSI Analysis Reference Manual
– Grounded (one-joint) link/support objects: Used to model special support behavior such as isolators, dampers, gaps, multi-linear springs, and
more.
• Line objects, of four types
– Frame objects: Used to model beams, columns, braces, and trusses
– Cable objects: Used to model slender cables under self weight and tension
– Tendon objects: Used to prestressing tendons within other objects
– Connecting (two-joint) link/support objects: Used to model special
member behavior such as isolators, dampers, gaps, multi-linear springs,
and more. Unlike frame, cable, and tendon objects, connecting link objects
can have zero length.
• Area objects: Shell elements (plate, membrane, and full-shell) used to model
walls, floors, and other thin-walled members; as well as two-dimensional solids (plane-stress, plane-strain, and axisymmetric solids).
• Solid objects: Used to model three-dimensional solids.
As a general rule, the geometry of the object should correspond to that of the physical member. This simplifies the visualization of the model and helps with the design process.

Objects and Elements
If you have experience using traditional finite element programs, including earlier
versions of SAP2000, ETABS, and SAFE, you are probably used to meshing physical models into smaller finite elements for analysis purposes. Object-based modeling largely eliminates the need for doing this.
For users who are new to finite-element modeling, the object-based concept should
seem perfectly natural.
When you run an analysis, SAP2000 automatically converts your object-based
model into an element-based model that is used for analysis. This element-based
model is called the analysis model, and it consists of traditional finite elements and
joints (nodes). Results of the analysis are reported back on the object-based model.
You have control over how the meshing is performed, such as the degree of refinement, and how to handle the connections between intersecting objects. You also
have the option to manually mesh the model, resulting in a one-to-one correspondence between objects and elements.

Objects and Elements

Chapter II

Objects and Elements

In this manual, the term “element” will be used more often than “object”, since
what is described herein is the finite-element analysis portion of the program that
operates on the element-based analysis model. However, it should be clear that the
properties described here for elements are actually assigned in the interface to the
objects, and the conversion to analysis elements is automatic.
One specific case to be aware of is that both one-joint (grounded) link/support objects and two-joint (connecting) link/support objects are always converted into
two-joint link/support elements. For the two-joint objects, the conversion to elements is direct. For the one-joint objects, a new joint is created at the same location
and is fully restrained. The generated two-joint link/support element is of zero
length, with its original joint connected to the structure and the new joint connected
to ground by restraints.

Groups
A group is a named collection of objects that you define. For each group, you must
provide a unique name, then select the objects that are to be part of the group. You
can include objects of any type or types in a group. Each object may be part of one
of more groups. All objects are always part of the built-in group called “ALL”.
Groups are used for many purposes in the graphical user interface, including selection, design optimization, defining section cuts, controlling output, and more. In
this manual, we are primarily interested in the use of groups for defining staged
construction. See Topic “Staged Construction” (page 79) in Chapter “Nonlinear
Static Analysis” for more information.

Groups

CSI Analysis Reference Manual

Groups

C h a p t e r III

Coordinate Systems
Each structure may use many different coordinate systems to describe the location
of points and the directions of loads, displacement, internal forces, and stresses.
Understanding these different coordinate systems is crucial to being able to properly define the model and interpret the results.
Basic Topics for All Users
• Overview
• Global Coordinate System
• Upward and Horizontal Directions
• Defining Coordinate Systems
• Local Coordinate Systems
Advanced Topics
• Alternate Coordinate Systems
• Cylindrical and Spherical Coordinates

CSI Analysis Reference Manual

Overview
Coordinate systems are used to locate different parts of the structural model and to
define the directions of loads, displacements, internal forces, and stresses.
All coordinate systems in the model are defined with respect to a single global coordinate system. Each part of the model (joint, element, or constraint) has its own local coordinate system. In addition, you may create alternate coordinate systems that
are used to define locations and directions.
All coordinate systems are three-dimensional, right-handed, rectangular (Cartesian) systems. Vector cross products are used to define the local and alternate coordinate systems with respect to the global system.
SAP2000 always assumes that Z is the vertical axis, with +Z being upward. The upward direction is used to help define local coordinate systems, although local coordinate systems themselves do not have an upward direction.
The locations of points in a coordinate system may be specified using rectangular
or cylindrical coordinates. Likewise, directions in a coordinate system may be
specified using rectangular, cylindrical, or spherical coordinate directions at a
point.

Global Coordinate System
The global coordinate system is a three-dimensional, right-handed, rectangular
coordinate system. The three axes, denoted X, Y, and Z, are mutually perpendicular
and satisfy the right-hand rule.
Locations in the global coordinate system can be specified using the variables x, y,
and z. A vector in the global coordinate system can be specified by giving the locations of two points, a pair of angles, or by specifying a coordinate direction. Coordinate directions are indicated using the values ±X, ±Y, and ±Z. For example, +X
defines a vector parallel to and directed along the positive X axis. The sign is required.
All other coordinate systems in the model are ultimately defined with respect to the
global coordinate system, either directly or indirectly. Likewise, all joint coordinates are ultimately converted to global X, Y, and Z coordinates, regardless of how
they were specified.

Overview

Chapter III

Coordinate Systems

Upward and Horizontal Directions
SAP2000 always assumes that Z is the vertical axis, with +Z being upward. Local
coordinate systems for joints, elements, and ground-acceleration loading are defined with respect to this upward direction. Self-weight loading always acts downward, in the –Z direction.
The X-Y plane is horizontal. The primary horizontal direction is +X. Angles in the
horizontal plane are measured from the positive half of the X axis, with positive angles appearing counterclockwise when you are looking down at the X-Y plane.
If you prefer to work with a different upward direction, you can define an alternate
coordinate system for that purpose.

Defining Coordinate Systems
Each coordinate system to be defined must have an origin and a set of three,
mutually-perpendicular axes that satisfy the right-hand rule.
The origin is defined by simply specifying three coordinates in the global coordinate system.
The axes are defined as vectors using the concepts of vector algebra. A fundamental
knowledge of the vector cross product operation is very helpful in clearly understanding how coordinate system axes are defined.

Vector Cross Product
A vector may be defined by two points. It has length, direction, and location in
space. For the purposes of defining coordinate axes, only the direction is important.
Hence any two vectors that are parallel and have the same sense (i.e., pointing the
same way) may be considered to be the same vector.
Any two vectors, Vi and Vj, that are not parallel to each other define a plane that is
parallel to them both. The location of this plane is not important here, only its orientation. The cross product of Vi and Vj defines a third vector, Vk, that is perpendicular
to them both, and hence normal to the plane. The cross product is written as:
Vk = Vi ´ Vj

Upward and Horizontal Directions

CSI Analysis Reference Manual
The length of Vk is not important here. The side of the Vi-Vj plane to which Vk points
is determined by the right-hand rule: The vector Vk points toward you if the acute
angle (less than 180°) from Vi to Vj appears counterclockwise.
Thus the sign of the cross product depends upon the order of the operands:
Vj ´ Vi = – Vi ´ Vj

Defining the Three Axes Using Two Vectors
A right-handed coordinate system R-S-T can be represented by the three mutuallyperpendicular vectors Vr, Vs, and Vt, respectively, that satisfy the relationship:
Vt = Vr ´ Vs
This coordinate system can be defined by specifying two non-parallel vectors:
• An axis reference vector, Va, that is parallel to axis R
• A plane reference vector, Vp, that is parallel to plane R-S, and points toward the
positive-S side of the R axis
The axes are then defined as:
Vr = Va
Vt = Vr ´ Vp
Vs = Vt ´ Vr
Note that Vp can be any convenient vector parallel to the R-S plane; it does not have
to be parallel to the S axis. This is illustrated in Figure 1 (page 15).

Local Coordinate Systems
Each part (joint, element, or constraint) of the structural model has its own local coordinate system used to define the properties, loads, and response for that part. The
axes of the local coordinate systems are denoted 1, 2, and 3. In general, the local coordinate systems may vary from joint to joint, element to element, and constraint to
constraint.
There is no preferred upward direction for a local coordinate system. However, the
upward +Z direction is used to define the default joint and element local coordinate
systems with respect to the global or any alternate coordinate system.

Local Coordinate Systems

Chapter III

Coordinate Systems

Va is parallel to R axis
Vp is parallel to R-S plane
Vr = Va
Vt = Vr x Vp
Vs = Vt x Vr

Vs
Vt

Plane R-S

Cube is shown for
visualization purposes
Vr

Va
Global
X

Figure 1
Determining an R-S-T Coordinate System from Reference Vectors Va and Vp

The joint local 1-2-3 coordinate system is normally the same as the global X-Y-Z
coordinate system. However, you may define any arbitrary orientation for a joint
local coordinate system by specifying two reference vectors and/or three angles of
rotation.
For the Frame, Area (Shell, Plane, and Asolid), and Link/Support elements, one of
the element local axes is determined by the geometry of the individual element.
You may define the orientation of the remaining two axes by specifying a single
reference vector and/or a single angle of rotation. The exception to this is one-joint
or zero-length Link/Support elements, which require that you first specify the local-1 (axial) axis.
The Solid element local 1-2-3 coordinate system is normally the same as the global
X-Y-Z coordinate system. However, you may define any arbitrary orientation for a
solid local coordinate system by specifying two reference vectors and/or three angles of rotation.
The local coordinate system for a Body, Diaphragm, Plate, Beam, or Rod Constraint is normally determined automatically from the geometry or mass distribution of the constraint. Optionally, you may specify one local axis for any Dia-

Local Coordinate Systems

CSI Analysis Reference Manual
phragm, Plate, Beam, or Rod Constraint (but not for the Body Constraint); the remaining two axes are determined automatically.
The local coordinate system for an Equal Constraint may be arbitrarily specified;
by default it is the global coordinate system. The Local Constraint does not have its
own local coordinate system.
For more information:
• See Topic “Local Coordinate System” (page 24) in Chapter “Joints and Degrees of Freedom.”
• See Topic “Local Coordinate System” (page 108) in Chapter “The Frame Element.”
• See Topic “Local Coordinate System” (page 185) in Chapter “The Shell Element.”
• See Topic “Local Coordinate System” (page 217) in Chapter “The Plane Element.”
• See Topic “Local Coordinate System” (page 227) in Chapter “The Asolid Element.”
• See Topic “Local Coordinate System” (page 240) in Chapter “The Solid Element.”
• See Topic “Local Coordinate System” (page 253) in Chapter “The Link/Support Element—Basic.”
• See Chapter “Constraints and Welds (page 49).”

Alternate Coordinate Systems
You may define alternate coordinate systems that can be used for locating the
joints; for defining local coordinate systems for joints, elements, and constraints;
and as a reference for defining other properties and loads. The axes of the alternate
coordinate systems are denoted X, Y, and Z.
The global coordinate system and all alternate systems are called fixed coordinate
systems, since they apply to the whole structural model, not just to individual parts
as do the local coordinate systems. Each fixed coordinate system may be used in
rectangular, cylindrical or spherical form.
Associated with each fixed coordinate system is a grid system used to locate objects
in the graphical user interface. Grids have no meaning in the analysis model.

Alternate Coordinate Systems

Chapter III

Coordinate Systems

Each alternate coordinate system is defined by specifying the location of the origin
and the orientation of the axes with respect to the global coordinate system. You
need:
• The global X, Y, and Z coordinates of the new origin
• The three angles (in degrees) used to rotate from the global coordinate system
to the new system

Cylindrical and Spherical Coordinates
The location of points in the global or an alternate coordinate system may be specified using polar coordinates instead of rectangular X-Y-Z coordinates. Polar coordinates include cylindrical CR-CA-CZ coordinates and spherical SB-SA-SR coordinates. See Figure 2 (page 19) for the definition of the polar coordinate systems.
Polar coordinate systems are always defined with respect to a rectangular X-Y-Z
system.
The coordinates CR, CZ, and SR are lineal and are specified in length units. The coordinates CA, SB, and SA are angular and are specified in degrees.
Locations are specified in cylindrical coordinates using the variables cr, ca, and cz.
These are related to the rectangular coordinates as:
2

cr = x + y
ca = tan -1

y
x

cz = z
Locations are specified in spherical coordinates using the variables sb, sa, and sr.
These are related to the rectangular coordinates as:
2

x +y

sb = tan -1
sa = tan -1
2

z
y
x
2

sr = x + y + z

Cylindrical and Spherical Coordinates

CSI Analysis Reference Manual
A vector in a fixed coordinate system can be specified by giving the locations of
two points or by specifying a coordinate direction at a single point P. Coordinate
directions are tangential to the coordinate curves at point P. A positive coordinate
direction indicates the direction of increasing coordinate value at that point.
Cylindrical coordinate directions are indicated using the values ±CR, ±CA, and
±CZ. Spherical coordinate directions are indicated using the values ±SB, ±SA, and
±SR. The sign is required. See Figure 2 (page 19).
The cylindrical and spherical coordinate directions are not constant but vary with
angular position. The coordinate directions do not change with the lineal coordinates. For example, +SR defines a vector directed from the origin to point P.
Note that the coordinates Z and CZ are identical, as are the corresponding coordinate directions. Similarly, the coordinates CA and SA and their corresponding coordinate directions are identical.

Cylindrical and Spherical Coordinates

Chapter III

Coordinate Systems

+CZ

Z, CZ

+CA

P
+CR

Cylindrical
Coordinates

Y
cr
ca

Cubes are shown for
visualization purposes
Z

+SR
+SA
sb

Spherical
Coordinates

P
sr
+SB
Y

Figure 2
Cylindrical and Spherical Coordinates and Coordinate Directions

Cylindrical and Spherical Coordinates

CSI Analysis Reference Manual

Cylindrical and Spherical Coordinates

C h a p t e r IV

Joints and Degrees of Freedom
The joints play a fundamental role in the analysis of any structure. Joints are the
points of connection between the elements, and they are the primary locations in
the structure at which the displacements are known or are to be determined. The
displacement components (translations and rotations) at the joints are called the degrees of freedom.
This Chapter describes joint properties, degrees of freedom, loads, and output. Additional information about joints and degrees of freedom is given in Chapter “Constraints and Welds” (page 49).
Basic Topics for All Users
• Overview
• Modeling Considerations
• Local Coordinate System
• Degrees of Freedom
• Restraint Supports
• Spring Supports
• Joint Reactions
• Base Reactions

CSI Analysis Reference Manual
• Masses
• Force Load
• Degree of Freedom Output
• Assembled Joint Mass Output
• Displacement Output
• Force Output
Advanced Topics
• Advanced Local Coordinate System
• Nonlinear Supports
• Distributed Supports
• Ground Displacement Load
• Generalized Displacements
• Element Joint Force Output

Overview
Joints, also known as nodal points or nodes, are a fundamental part of every structural model. Joints perform a variety of functions:
• All elements are connected to the structure (and hence to each other) at the
joints
• The structure is supported at the joints using Restraints and/or Springs
• Rigid-body behavior and symmetry conditions can be specified using Constraints that apply to the joints
• Concentrated loads may be applied at the joints
• Lumped (concentrated) masses and rotational inertia may be placed at the
joints
• All loads and masses applied to the elements are actually transferred to the
joints
• Joints are the primary locations in the structure at which the displacements are
known (the supports) or are to be determined
All of these functions are discussed in this Chapter except for the Constraints,
which are described in Chapter “Constraints and Welds” (page 49).

Overview

Chapter IV

Joints and Degrees of Freedom

Joints in the analysis model correspond to point objects in the structural-object
model. Using the SAP2000, ETABS, SAFE, or CSiBridge graphical user interface,
joints (points) are automatically created at the ends of each Line object and at the
corners of each Area and Solid object. Joints may also be defined independently of
any object.
Automatic meshing of objects will create additional joints corresponding to any elements that are created.
Joints may themselves be considered as elements. Each joint may have its own local coordinate system for defining the degrees of freedom, restraints, joint properties, and loads; and for interpreting joint output. In most cases, however, the global
X-Y-Z coordinate system is used as the local coordinate system for all joints in the
model. Joints act independently of each other unless connected by other elements.
There are six displacement degrees of freedom at every joint — three translations
and three rotations. These displacement components are aligned along the local coordinate system of each joint.
Joints may be loaded directly by concentrated loads or indirectly by ground displacements acting though Restraints, spring supports, or one-joint (grounded)
Link/Support objects.
Displacements (translations and rotations) are produced at every joint. Reaction
forces and moments acting at each supported joint are also produced.
For more information, see Chapter “Constraints and Welds” (page 49).

Modeling Considerations
The location of the joints and elements is critical in determining the accuracy of the
structural model. Some of the factors that you need to consider when defining the
elements, and hence the joints, for the structure are:
• The number of elements should be sufficient to describe the geometry of the
structure. For straight lines and edges, one element is adequate. For curves and
curved surfaces, one element should be used for every arc of 15° or less.
• Element boundaries, and hence joints, should be located at points, lines, and
surfaces of discontinuity:
– Structural boundaries, e.g., corners and edges
– Changes in material properties

Modeling Considerations

CSI Analysis Reference Manual
– Changes in thickness and other geometric properties
– Support points (Restraints and Springs)
– Points of application of concentrated loads, except that Frame elements
may have concentrated loads applied within their spans
• In regions having large stress gradients, i.e., where the stresses are changing
rapidly, an Area- or Solid-element mesh should be refined using small elements and closely-spaced joints. This may require changing the mesh after one
or more preliminary analyses.
• More that one element should be used to model the length of any span for
which dynamic behavior is important. This is required because the mass is always lumped at the joints, even if it is contributed by the elements.

Local Coordinate System
Each joint has its own joint local coordinate system used to define the degrees of
freedom, Restraints, properties, and loads at the joint; and for interpreting joint output. The axes of the joint local coordinate system are denoted 1, 2, and 3. By default
these axes are identical to the global X, Y, and Z axes, respectively. Both systems
are right-handed coordinate systems.
The default local coordinate system is adequate for most situations. However, for
certain modeling purposes it may be useful to use different local coordinate systems at some or all of the joints. This is described in the next topic.
For more information:
• See Topic “Upward and Horizontal Directions” (page 13) in Chapter “Coordinate Systems.”
• See Topic “Advanced Local Coordinate System” (page 24) in this Chapter.

Advanced Local Coordinate System
By default, the joint local 1-2-3 coordinate system is identical to the global X-Y-Z
coordinate system, as described in the previous topic. However, it may be necessary to use different local coordinate systems at some or all joints in the following
cases:
• Skewed Restraints (supports) are present
• Constraints are used to impose rotational symmetry

Local Coordinate System

Chapter IV

Joints and Degrees of Freedom

• Constraints are used to impose symmetry about a plane that is not parallel to a
global coordinate plane
• The principal axes for the joint mass (translational or rotational) are not aligned
with the global axes
• Joint displacement and force output is desired in another coordinate system
Joint local coordinate systems need only be defined for the affected joints. The
global system is used for all joints for which no local coordinate system is explicitly
specified.
A variety of methods are available to define a joint local coordinate system. These
may be used separately or together. Local coordinate axes may be defined to be parallel to arbitrary coordinate directions in an arbitrary coordinate system or to vectors between pairs of joints. In addition, the joint local coordinate system may be
specified by a set of three joint coordinate angles. These methods are described in
the subtopics that follow.
For more information:
• See Chapter “Coordinate Systems” (page 11).
• See Topic “Local Coordinate System” (page 24) in this Chapter.

Reference Vectors
To define a joint local coordinate system you must specify two reference vectors
that are parallel to one of the joint local coordinate planes. The axis reference vector, Va , must be parallel to one of the local axes (I = 1, 2, or 3) in this plane and
have a positive projection upon that axis. The plane reference vector, V p , must
have a positive projection upon the other local axis (j = 1, 2, or 3, but I ¹ j) in this
plane, but need not be parallel to that axis. Having a positive projection means that
the positive direction of the reference vector must make an angle of less than 90°
with the positive direction of the local axis.
Together, the two reference vectors define a local axis, I, and a local plane, i-j.
From this, the program can determine the third local axis, k, using vector algebra.
For example, you could choose the axis reference vector parallel to local axis 1 and
the plane reference vector parallel to the local 1-2 plane (I = 1, j = 2). Alternatively,
you could choose the axis reference vector parallel to local axis 3 and the plane reference vector parallel to the local 3-2 plane (I = 3, j = 2). You may choose the plane
that is most convenient to define using the parameter local, which may take on the
Advanced Local Coordinate System

CSI Analysis Reference Manual
values 12, 13, 21, 23, 31, or 32. The two digits correspond to I and j, respectively.
The default is value is 31.

Defining the Axis Reference Vector
To define the axis reference vector for joint j, you must first specify or use the default values for:
• A coordinate direction axdir (the default is +Z)
• A fixed coordinate system csys (the default is zero, indicating the global coordinate system)
You may optionally specify:
• A pair of joints, axveca and axvecb (the default for each is zero, indicating
joint j itself). If both are zero, this option is not used.
For each joint, the axis reference vector is determined as follows:
1. A vector is found from joint axveca to joint axvecb. If this vector is of finite
length, it is used as the reference vector Va
2. Otherwise, the coordinate direction axdir is evaluated at joint j in fixed coordinate system csys, and is used as the reference vector Va

Defining the Plane Reference Vector
To define the plane reference vector for joint j, you must first specify or use the default values for:
• A primary coordinate direction pldirp (the default is +X)
• A secondary coordinate direction pldirs (the default is +Y). Directions pldirs
and pldirp should not be parallel to each other unless you are sure that they are
not parallel to local axis 1
• A fixed coordinate system csys (the default is zero, indicating the global coordinate system). This will be the same coordinate system that was used to define
the axis reference vector, as described above
You may optionally specify:
• A pair of joints, plveca and plvecb (the default for each is zero, indicating joint
j itself). If both are zero, this option is not used.

Advanced Local Coordinate System

Chapter IV

Joints and Degrees of Freedom

For each joint, the plane reference vector is determined as follows:
1. A vector is found from joint plveca to joint plvecb. If this vector is of finite
length and is not parallel to local axis I, it is used as the reference vector V p
2. Otherwise, the primary coordinate direction pldirp is evaluated at joint j in
fixed coordinate system csys. If this direction is not parallel to local axis I, it is
used as the reference vector V p
3. Otherwise, the secondary coordinate direction pldirs is evaluated at joint j in
fixed coordinate system csys. If this direction is not parallel to local axis I, it is
used as the reference vector V p
4. Otherwise, the method fails and the analysis terminates. This will never happen
if pldirp is not parallel to pldirs
A vector is considered to be parallel to local axis I if the sine of the angle between
-3
them is less than 10 .

Determining the Local Axes from the Reference Vectors
The program uses vector cross products to determine the local axes from the reference vectors. The three axes are represented by the three unit vectors V1 , V2 and
V3 , respectively. The vectors satisfy the cross-product relationship:
V1 = V2 ´ V3
The local axis Vi is given by the vector Va after it has been normalized to unit
length.
The remaining two axes, V j and Vk , are defined as follows:
• If I and j permute in a positive sense, i.e., local = 12, 23, or 31, then:
Vk = Vi ´ V p and
V j = Vk ´ Vi
• If I and j permute in a negative sense, i.e., local = 21, 32, or 13, then:
Vk = V p ´ Vi and
V j = Vi ´ Vk
An example showing the determination of the joint local coordinate system using
reference vectors is given in Figure 3 (page 28).

Advanced Local Coordinate System

CSI Analysis Reference Manual
Va is parallel to axveca-axvecb
Vp is parallel to plveca-plvecb
V3 = V a
V2 = V3 x Vp
V1 = V 2 x V3

All vectors normalized to unit length.

Z
plvecb

plveca

Plane 3-1
V3

axveca

Va
Global
axvecb
X

Figure 3
Example of the Determination of the Joint Local Coordinate System
Using Reference Vectors for local=31

Joint Coordinate Angles
The joint local coordinate axes determined from the reference vectors may be further modified by the use of three joint coordinate angles, denoted a, b, and c. In
the case where the default reference vectors are used, the joint coordinate angles define the orientation of the joint local coordinate system with respect to the global
axes.
The joint coordinate angles specify rotations of the local coordinate system about
its own current axes. The resulting orientation of the joint local coordinate system
is obtained according to the following procedure:
1. The local system is first rotated about its +3 axis by angle a
2. The local system is next rotated about its resulting +2 axis by angle b
3. The local system is lastly rotated about its resulting +1 axis by angle c
The order in which the rotations are performed is important. The use of coordinate
angles to orient the joint local coordinate system with respect to the global system is
shown in Figure 4 (page 29).

Advanced Local Coordinate System

Chapter IV

Joints and Degrees of Freedom
Z, 3

a
Step 1: Rotation about
local 3 axis by angle a
2

a
a

1
Z

3
b

Step 2: Rotation about new
local 2 axis by angle b

2
Y

X
b

1
Z
3

Step 3: Rotation about new
local 1 axis by angle c

2
c

Figure 4
Use of Joint Coordinate Angles to Orient the Joint Local Coordinate System

Advanced Local Coordinate System

CSI Analysis Reference Manual

Degrees of Freedom
The deflection of the structural model is governed by the displacements of the
joints. Every joint of the structural model may have up to six displacement components:
• The joint may translate along its three local axes. These translations are denoted U1, U2, and U3.
• The joint may rotate about its three local axes. These rotations are denoted R1,
R2, and R3.
These six displacement components are known as the degrees of freedom of the
joint. In the usual case where the joint local coordinate system is parallel to the
global system, the degrees of freedom may also be identified as UX, UY, UZ, RX,
RY and RZ, according to which global axes are parallel to which local axes. The
joint local degrees of freedom are illustrated in Figure 5 (page 31).
In addition to the regular joints that you explicitly define as part of your structural
model, the program automatically creates master joints that govern the behavior of
any Constraints and Welds that you may have defined. Each master joint has the
same six degrees of freedom as do the regular joints. See Chapter “Constraints and
Welds” (page 49) for more information.
Each degree of freedom in the structural model must be one of the following types:
• Active — the displacement is computed during the analysis
• Restrained — the displacement is specified, and the corresponding reaction is
computed during the analysis
• Constrained — the displacement is determined from the displacements at other
degrees of freedom
• Null — the displacement does not affect the structure and is ignored by the
analysis
• Unavailable — the displacement has been explicitly excluded from the analysis
These different types of degrees of freedom are described in the following subtopics.

Degrees of Freedom

Chapter IV

Joints and Degrees of Freedom

R2
Joint
R1
U1

Figure 5
The Six Displacement Degrees of Freedom in the Joint Local Coordinate System

Available and Unavailable Degrees of Freedom
You may explicitly specify the global degrees of freedom that are available to every
joint in the structural model. By default, all six degrees of freedom are available to
every joint. This default should generally be used for all three-dimensional structures.
For certain planar structures, however, you may wish to restrict the available degrees of freedom. For example, in the X-Y plane: a planar truss needs only UX and
UY; a planar frame needs only UX, UY, and RZ; and a planar grid or flat plate
needs only UZ, RX, and RY.
The degrees of freedom that are not specified as being available are called unavailable degrees of freedom. Any stiffness, loads, mass, Restraints, or Constraints that
are applied to the unavailable degrees of freedom are ignored by the analysis.
The available degrees of freedom are always referred to the global coordinate system, and they are the same for every joint in the model. If any joint local coordinate
systems are used, they must not couple available degrees of freedom with the unavailable degrees of freedom at any joint. For example, if the available degrees of
freedom are UX, UY, and RZ, then all joint local coordinate systems must have one
local axis parallel to the global Z axis.

Degrees of Freedom

CSI Analysis Reference Manual

Restrained Degrees of Freedom
If the displacement of a joint along any one of its available degrees of freedom is
known, such as at a support point, that degree of freedom is restrained. The known
value of the displacement may be zero or non-zero, and may be different in different Load Patterns. The force along the restrained degree of freedom that is required
to impose the specified restraint displacement is called the reaction, and is determined by the analysis.
Unavailable degrees of freedom are essentially restrained. However, they are excluded from the analysis and no reactions are computed, even if they are non-zero.
See Topic “Restraint Supports” (page 34) in this Chapter for more information.

Constrained Degrees of Freedom
Any joint that is part of a Constraint or Weld may have one or more of its available
degrees of freedom constrained. The program automatically creates a master joint
to govern the behavior of each Constraint, and a master joint to govern the behavior
of each set of joints that are connected together by a Weld. The displacement of a
constrained degree of freedom is then computed as a linear combination of the displacements along the degrees of freedom at the corresponding master joint.
If a constrained degree of freedom is also restrained, the restraint will be applied to
the constraint as a whole.
See Chapter “Constraints and Welds” (page 49) for more information.

Mixing Restraints and Constraints Not Recommended
It is not recommended that restrained degrees of freedom also be constrained, although it is permitted. Reactions computed at such degrees of freedom will not include the contributions to the reaction from joints connected by constraints.
Ground displacement loads applied at the constraint will not be applied to the joints
connected by constraint. For better results, use springs or grounded (one-joint)
link/support objects to support joints that are also constrained.
Similarly, it is not recommended, that a given degree of freedom be included in
more than one constraint, although it is permitted. The analysis will attempt to combine the coupled constraints, but the results may not be as accurate as using a single
constraint for all coupled joints, especially for dynamics. For better results, include
all coupled joints in a single constraint whenever possible.

Degrees of Freedom

Chapter IV

Joints and Degrees of Freedom

Note that using fixed degrees of freedom in a link/support property is the same as
specifying a constraint. For this reason, such link/support objects should not be
connected together or connected to constrained joints. In such cases, it is better to
use large (but not too large) stiffnesses rather that fixed degrees of freedom in the
link/support property definition.

Active Degrees of Freedom
All available degrees of freedom that are neither constrained nor restrained must be
either active or null. The program will automatically determine the active degrees
of freedom as follows:
• If any load or stiffness is applied along any translational degree of freedom at a
joint, then all available translational degrees of freedom at that joint are made
active unless they are constrained or restrained.
• If any load or stiffness is applied along any rotational degree of freedom at a
joint, then all available rotational degrees of freedom at that joint are made active unless they are constrained or restrained.
• All degrees of freedom at a master joint that govern constrained degrees of
freedom are made active.
A joint that is connected to any element or to a translational spring will have all of
its translational degrees of freedom activated. A joint that is connected to a Frame,
Shell, or Link/Support element, or to any rotational spring will have all of its rotational degrees of freedom activated. An exception is a Frame element with only
truss-type stiffness, which will not activate rotational degrees of freedom.
Every active degree of freedom has an associated equation to be solved. If there are
N active degrees of freedom in the structure, there are N equations in the system,
and the structural stiffness matrix is said to be of order N. The amount of computational effort required to perform the analysis increases with N.
The load acting along each active degree of freedom is known (it may be zero). The
corresponding displacement will be determined by the analysis.
If there are active degrees of freedom in the system at which the stiffness is known
to be zero, such as the out-of-plane translation in a planar-frame, these must either
be restrained or made unavailable. Otherwise, the structure is unstable and the solution of the static equations will fail.
For more information:
• See Topic “Springs” (page 36) in this Chapter.
Degrees of Freedom

CSI Analysis Reference Manual
• See Topic “Degrees of Freedom” (page 108) in Chapter “The Frame Element.”
• See Topic “Degrees of Freedom” (page 170) in Chapter “The Cable Element.”
• See Topic “Degrees of Freedom” (page 181) in Chapter “The Shell Element.”
• See Topic “Degrees of Freedom” (page 217) in Chapter “The Plane Element.”
• See Topic “Degrees of Freedom” (page 227) in Chapter “The Asolid Element.”
• See Topic “Degrees of Freedom” (page 240) in Chapter “The Solid Element.”
• See Topic “Degrees of Freedom” (page 253) in Chapter “The Link/Support Element—Basic.”
• See Topic “Degrees of Freedom” (page 312) in Chapter “The Tendon Object.”

Null Degrees of Freedom
The available degrees of freedom that are not restrained, constrained, or active, are
called the null degrees of freedom. Because they have no load or stiffness, their displacements and reactions are zero, and they have no effect on the rest of the structure. The program automatically excludes them from the analysis.
Joints that have no elements connected to them typically have all six degrees of
freedom null. Joints that have only solid-type elements (Plane, Asolid, and Solid)
connected to them typically have the three rotational degrees of freedom null.

Restraint Supports
If the displacement of a joint along any of its available degrees of freedom has a
known value, either zero (e.g., at support points) or non-zero (e.g., due to support
settlement), a Restraint must be applied to that degree of freedom. The known
value of the displacement may differ from one Load Pattern to the next, but the degree of freedom is restrained for all Load Patterns. In other words, it is not possible
to have the displacement known in one Load Pattern and unknown (unrestrained) in
another Load Pattern.
Restraints should also be applied to any available degrees of freedom in the system
at which the stiffness is known to be zero, such as the out-of-plane translation and
in-plane rotations of a planar-frame. Otherwise, the structure is unstable and the solution of the static equations will complain.
Restraints are always applied to the joint local degrees of freedom U1, U2, U3, R1,
R2, and R3. Examples of Restraints are shown in Figure 6 (page 35).

Restraint Supports

Chapter IV

Joints and Degrees of Freedom

7
8
Joint
1
2
3
4

5
6
3

Fixed

Restraints
U1, U2, U3
U3
U1, U2, U3, R1, R2, R3
None

4
1 Hinge

Spring
Support
2

Rollers

Global

3-D Frame Structure
Notes: Joints are indicated with dots:
Solid dots indicate moment continuity
Open dots indicate hinges
All joint local 1-2-3 coordinate systems are
identical to the global X-Y-Z coordinate system

Joint
All
1
2
3

Restraints
U2, R1, R3
U3
U1, U3, R2
U1, U3
Z

Roller

Fixed

Global

Hinge

2-D Frame Structure, X-Z plane

Figure 6
Examples of Restraints

Restraint Supports

CSI Analysis Reference Manual
If a restraint is applied to an unavailable degree of freedom, it is ignored. The displacement will be zero, but no reaction will be computed.
In general, you should not apply restraints to constrained degrees of freedom. However, if you do, the analysis will attempt to automatically rewrite the constraint
equations to accommodate the restraint. Reactions computed at such degrees of
freedom will not include the contributions to the reaction from joints connected by
constraints. Ground displacement loads applied at the constraint will not be applied
to the joints connected by constraint. For better results, use springs or grounded
(one-joint) Link/Supports to support joints that are also constrained.
For more information:
• See Topic “Degrees of Freedom” (page 30) in this Chapter.
• See Topic “Restraint Displacement Load” (page 42) in this Chapter.

Spring Supports
Any of the six degrees of freedom at any of the joints in the structure can have translational or rotational spring support conditions. These springs elastically connect
the joint to the ground. Spring supports along restrained degrees of freedom do not
contribute to the stiffness of the structure.
Springs may be specified that couple the degrees of freedom at a joint. The spring
forces that act on a joint are related to the displacements of that joint by a 6x6 symmetric matrix of spring stiffness coefficients. These forces tend to oppose the displacements.
Spring stiffness coefficients may be specified in the global coordinate system, an
Alternate Coordinate System, or the joint local coordinate system.
In a joint local coordinate system, the spring forces and moments F1, F2, F3, M1, M2
and M3 at a joint are given by:
ì F1 ü
é u1 u1u2 u1u3 u1r1 u1r2 u1r3 ù ì u1 ü
ïF ï
ê
u2
u2u3 u2r1 u2r2 u2r3 ú ï u 2 ï
ï 2 ï
ê
úï ï
u3
u3r1 u3r2 u3r3 ú ï u 3 ï
ï F3 ï
ê
í
ý=-ê
í ý
M
r1
r1r2 r1r3 ú ï r1 ï
1
ï
ï
ê
ú
ïM 2 ï
sym.
r2
r2r3 ú ï r2 ï
ê
ïM ï
ê
r3 úû ïî r3 ïþ
î 3þ
ë

Spring Supports

(Eqn. 1)

Chapter IV

Joints and Degrees of Freedom

where u1, u2, u3, r1, r2 and r3 are the joint displacements and rotations, and the terms
u1, u1u2, u2, ... are the specified spring stiffness coefficients.
In any fixed coordinate system, the spring forces and moments Fx, Fy, Fz, Mx, My and
Mz at a joint are given by:
ì Fx ü
é ux
ïF ï
ê
ï yï
ê
ï Fz ï
ê
í
ý=-ê
M
ï xï
ê
ïM yï
ê
ïM ï
ê
î zþ
ë

uxuy uxuz uxrx
uy
uyuz uyrx
uz
sym.

uzrx
rx

uxry uxrz ù ì u x ü
uyry uyrz ú ï u y ï
úï ï
uzry uzrz ú ï u z ï
í ý
rxry rxrz ú ï rx ï
ú
ry
ryrz ú ï r y ï
rz úû ïî r z ïþ

where ux, uy, uz, rx, ry and rz are the joint displacements and rotations, and the terms
ux, uxuy, uy, ... are the specified spring stiffness coefficients.
For springs that do not couple the degrees of freedom in a particular coordinate system, only the six diagonal terms need to be specified since the off-diagonal terms
are all zero. When coupling is present, all 21 coefficients in the upper triangle of the
matrix must be given; the other 15 terms are then known by symmetry.
If the springs at a joint are specified in more than one coordinate system, standard
coordinate transformation techniques are used to convert the 6x6 spring stiffness
matrices to the joint local coordinate system, and the resulting stiffness matrices are
then added together on a term-by-term basis. The final spring stiffness matrix at
each joint in the structure should have a determinant that is zero or positive. Otherwise the springs may cause the structure to be unstable.
The displacement of the grounded end of the spring may be specified to be zero or
non-zero (e.g., due to support settlement). This spring displacement may vary
from one Load Pattern to the next.
For more information:
• See Topic “Degrees of Freedom” (page 30) in this Chapter.
• See Topic “Spring Displacement Load” (page 43) in this Chapter.

Nonlinear Supports
In certain versions of the program, you may define nonlinear supports at the joints
using the Link/Support element. Nonlinear support conditions that can be modeled
Nonlinear Supports

CSI Analysis Reference Manual
include gaps (compression only), multi-linear elastic or plastic springs, viscous
dampers, base isolators, and more.
This Link/Support can be used in two ways:
• You can add (draw) a one-joint object, in which case it is considered a Support
object, and it connects the joint directly to the ground.
• The object can also be drawn with two joints, in which case it is considered a
Link object. You can use a Link object as a support if you connect one end to
the structure, and fully restrain the other end.
Both methods have the same effect. During analysis, one-joint Support objects are
converted to two-joint Link elements of zero length, and connected to a generated
joint that is fully restrained.
Multiple Link/Support elements can be connected to a single joint, in which case
they act in parallel. Each Link/Support element has its own element local coordinate system that is independent of the joint local coordinate system.
Restraints and springs may also exist at the joint. Of course, any degree of freedom
that is restrained will prevent deformation in the Link/Support element in that direction.
See Chapters “The Link/Support Element – Basic” (page 251) and “The Link/Support Element – Advanced” (page 275) for more information.

Distributed Supports
You may assign distributed spring supports along the length of a Frame element, or
over the any face of an area object (Shell, Plane, Asolid) or Solid element. These
springs may be linear, multi-linear elastic, or multi-linear plastic. These springs are
converted to equivalent two-joint Link/Support elements acting at the joints of the
element, after accounting for the tributary length or area of the element. The generated Link/Support elements are of zero length, with one end connected to the parent
object, and the other end connected to a generated joint that is fully restrained.
Because these springs act at the joints, it may be necessary to mesh the elements to
capture localized effects of such distributed supports. The best way to do this is
usually to use the automatic internal meshing options available in the graphical user
interface. This allows you to change the meshing easily, while still being able to
work with large, simpler model objects.

Distributed Supports

Chapter IV

Joints and Degrees of Freedom

It is not possible to assign distributed restraint supports directly. However, when
using automatic internal meshing, you may optionally specify that the meshed elements use the same restraint conditions that are present on the parent object.
For more information, see Topics “Restraint Supports” (page 34), “Spring Support” (page 36), “Nonlinear Supports” (page 37) in this Chapter, and also Chapter
“Objects and Elements” (page 7.)

Joint Reactions
The force or moment along the degree of freedom that is required to enforce any
support condition is called the reaction, and it is determined by the analysis. The
reaction includes the forces (or moments) from all supports at the joint, including
restraints, springs, and one-joint Link/Support objects. The tributary effect of any
distributed supports is included in the reaction.
If a one-joint Link/Support object is used, the reaction will be reported at the original joint connected to the structure, not at the restrained end of the generated
two-joint Link/Support element. The reaction at the generated joint will be reported
as zero since it has been transferred to the original joint.
For more information, see Topics “Restraint Supports” (page 34), “Spring Support” (page 36), “Nonlinear Supports” (page 37), and “Distributed Supports” (page
38) in this Chapter.

Base Reactions
Base Reactions are the resultant force and moment of all the joint reactions acting
on the structure, computed at the global origin or at some other location that you
choose. This produces three force components and three moment components. The
base forces are not affected by the chosen location, but the base moments are. For
seismic analysis the horizontal forces are called the base shears, and the moments
about the horizontal axes are called the overturning moments.
Base reactions are available for all Load Cases and Combos except for Moving-Load Load Cases. The centroids (center of action) are also available for each
force component of the base reactions. Note that these are the centroids of the reactions, which may not always be the same as the centroids of the applied load causing the reaction.
For more information, see Topic “Joint Reactions” (page 39) in this Chapter.
Joint Reactions

CSI Analysis Reference Manual

Masses
In a dynamic analysis, the mass of the structure is used to compute inertial forces.
Normally, the mass is obtained from the elements using the mass density of the material and the volume of the element. This automatically produces lumped (uncoupled) masses at the joints. The element mass values are equal for each of the three
translational degrees of freedom. No mass moments of inertia are produced for the
rotational degrees of freedom. This approach is adequate for most analyses.
It is often necessary to place additional concentrated masses and/or mass moments
of inertia at the joints. These can be applied to any of the six degrees of freedom at
any of the joints in the structure.
For computational efficiency and solution accuracy, SAP2000 always uses lumped
masses. This means that there is no mass coupling between degrees of freedom at a
joint or between different joints. These uncoupled masses are always referred to the
local coordinate system of each joint. Mass values along restrained degrees of freedom are ignored.
Inertial forces acting on the joints are related to the accelerations at the joints by a
6x6 matrix of mass values. These forces tend to oppose the accelerations. In a joint
local coordinate system, the inertia forces and moments F1, F2, F3, M1, M2 and M3 at
a joint are given by:
0
0 0 0 0 ù ì u&&1 ü
ì F1 ü
é u1
ïF ï
ê
u2
0 0 0 0 ú ï u&&2 ï
ï 2 ï
ê
úï ï
u3 0 0 0 ú ï u&&3 ï
ï F3 ï
ê
í
ý=-ê
í ý
M
r1 0 0 ú ï &&
r
1
ï
ï
ê
ú 1ï
ïM 2 ï
sym.
r2 0 ú ï &&
r2 ï
ê
ïM ï
ï
ê
ú
r3 û î &&
r3 ïþ
î 3þ
ë
where u&&1 , u&&2 , u&&3 , &&
r1 , &&
r2 and &&
r3 are the translational and rotational accelerations at
the joint, and the terms u1, u2, u3, r1, r2, and r3 are the specified mass values.
Uncoupled joint masses may instead be specified in the global coordinate system,
in which case they are transformed to the joint local coordinate system. Coupling
terms will be generated during this transformation in the following situation:
• The joint local coordinate system directions are not parallel to global coordinate directions, and
• The three translational masses or the three rotational mass moments of inertia
are not equal at a joint.

Masses

Chapter IV

Shape in
plan

Joints and Degrees of Freedom

Mass Moment of Inertia about vertical axis
(normal to paper) through center of mass

Formula

Rectangular diaphragm:
Uniformly distributed mass per unit area
Total mass of diaphragm = M (or w/g)

2
2
MMIcm = M ( b +d )
12

Triangular diaphragm:
Uniformly distributed mass per unit area
Total mass of diaphragm = M (or w/g)

Use general
diaphragm formula

Circular diaphragm:
Uniformly distributed mass per unit area
Total mass of diaphragm = M (or w/g)

2
MMIcm = Md
8

d
c.m.
Y
c.m.
X

X
Y

d
c.m.

Y
c.m.
X

General diaphragm:
Uniformly distributed mass per unit area
Total mass of diaphragm = M (or w/g)
Area of diaphragm = A
Moment of inertia of area about X-X = IX
Moment of inertia of area about Y-Y = IY

MMIcm =

M ( IX+IY)
A

Line mass:
Uniformly distributed mass per unit length
Total mass of line = M (or w/g)

2
MMIcm = Md
12

c.m.

Axis transformation for a mass:
If mass is a point mass, MMIo = 0

MMIcm = MMIo + MD2

c.m.

Figure 7
Formulae for Mass Moments of Inertia

Masses

CSI Analysis Reference Manual
These coupling terms will be discarded by the program, resulting in some loss of
accuracy. For this reason, it is recommended that you choose joint local coordinate
systems that are aligned with the principal directions of translational or rotational
mass at a joint, and then specify mass values in these joint local coordinates.
Mass values must be given in consistent mass units (W/g) and mass moments of in2
ertia must be in WL /g units. Here W is weight, L is length, and g is the acceleration
due to gravity. The net mass values at each joint in the structure should be zero or
positive.
See Figure 7 (page 41) for mass moment of inertia formulations for various planar
configurations.
For more information:
• See Topic “Degrees of Freedom” (page 30) in this Chapter.
• See Topic “Mass Source” (page 334) in Chapter “Load Patterns”.
• See Chapter “Static and Dynamic Analysis” (page 341).

Force Load
The Force Load is used to apply concentrated forces and moments at the joints.
Values may be specified in a fixed coordinate system (global or alternate coordinates) or the joint local coordinate system. All forces and moments at a joint are
transformed to the joint local coordinate system and added together. The specified
values are shown in Figure 8 (page 43).
Forces and moments applied along restrained degrees of freedom add to the corresponding reaction, but do not otherwise affect the structure.
For more information:
• See Topic “Degrees of Freedom” (page 30) in this Chapter.
• See Chapter “Load Patterns” (page 321).

Ground Displacement Load
The Ground Displacement Load is used to apply specified displacements (translations and rotations) at the grounded end of joint restraints, joint spring, and
one-joint Link/Support objects. Displacements may be specified in a fixed coordinate system (global or alternate coordinates) or the joint local coordinate system.

Force Load

Chapter IV

Joints and Degrees of Freedom

uz
r2

Z
rz

r1
u1
Joint

Joint
rx
uy

ux
u3
Joint Local Coordinates

Global Coordinates
Global
Origin
Y

Figure 8
Specified Values for Force Load and Ground Displacement Load

The specified values are shown in Figure 8 (page 43). All displacements at a joint
are transformed to the joint local coordinate system and added together.
Restraints may be considered as rigid connections between the joint degrees of
freedom and the ground. Springs and one-joint Link/Support objects may be considered as flexible connections between the joint degrees of freedom and the
ground.
It is very important to understand that ground displacement load applies to the
ground, and does not affect the structure unless the structure is supported by restraints, springs, or one-joint Link/Supports in the direction of loading!

Restraint Displacements
If a particular joint degree of freedom is restrained, the displacement of the joint is
equal to the ground displacement along that local degree of freedom. This applies
regardless of whether or not springs are present.

Ground Displacement Load

CSI Analysis Reference Manual

The vertical ground settlement, UZ = -1.000,
is specified as the restraint displacement.

The actual restraint displacement that is
imposed on the structure is U3 = -0.866.

GLOBAL
X

3
1

The unrestrained displacement, U1, will be
determined by the analysis.

30°

U3 = -0.866
UZ = -1.000

Figure 9
Example of Restraint Displacement Not Aligned with Local Degrees of Freedom

Components of ground displacement that are not along restrained degrees of freedom do not load the structure (except possibly through springs and one-joint links).
An example of this is illustrated in Figure 9 (page 44).
The ground displacement, and hence the joint displacement, may vary from one
Load Pattern to the next. If no ground displacement load is specified for a restrained
degree of freedom, the joint displacement is zero for that Load Pattern.

Spring Displacements
The ground displacements at a joint are multiplied by the spring stiffness coefficients to obtain effective forces and moments that are applied to the joint. Spring
displacements applied in a direction with no spring stiffness result in zero applied
load. The ground displacement, and hence the applied forces and moments, may
vary from one Load Pattern to the next.
In a joint local coordinate system, the applied forces and moments F1, F2, F3, M1, M2
and M3 at a joint due to ground displacements are given by:

Ground Displacement Load

Chapter IV

Joints and Degrees of Freedom

0
0 0 0 0 ù ì u g1 ü
ì F1 ü
é u1
ïF ï
ê
u2
0 0 0 0 ú ïug 2 ï
ï
ï 2 ï
ê
úï
u3 0 0 0 ú ï u g 3 ï
ï F3 ï
ê
í
ý=-ê
í
ý
r1 0 0 ú ï rg 1 ï
ï M1 ï
ê
ú
ïM 2 ï
sym.
r2 0 ú ï rg 2 ï
ê
ïM ï
ê
r3 úû ïî rg 3 ïþ
î 3þ
ë

(Eqn. 2)

where u g1 , u g 2 , u g 3 , rg1 , rg 2 and rg 3 are the ground displacements and rotations,
and the terms u1, u2, u3, r1, r2, and r3 are the specified spring stiffness coefficients.
The net spring forces and moments acting on the joint are the sum of the forces and
moments given in Equations (1) and (2); note that these are of opposite sign. At a
restrained degree of freedom, the joint displacement is equal to the ground displacement, and hence the net spring force is zero.
For more information:
• See Topic “Restraints and Reactions” (page 34) in this Chapter.
• See Topic “Springs” (page 36) in this Chapter.
• See Chapter “Load Patterns” (page 321).

Link/Support Displacements
One-joint Link/Support objects are converted to zero-length, two-joint Link/Support elements. A restrained joint is generated and the ground displacement is applied as a restraint displacement at this generated joint.
The effect of the ground displacement on the structure depends upon the properties
of the Link/Support element connecting the restrained joint to the structure, similar
to how springs supports work, except the Link/Support stiffness may be nonlinear.

Generalized Displacements
A generalized displacement is a named displacement measure that you define. It is
simply a linear combination of displacement degrees of freedom from one or more
joints.
For example, you could define a generalized displacement that is the difference of
the UX displacements at two joints on different stories of a building and name it
Generalized Displacements

CSI Analysis Reference Manual
“DRIFTX”. You could define another generalized displacement that is the sum of
three rotations about the Z axis, each scaled by 1/3, and name it “AVGRZ.”
Generalized displacements are primarily used for output purposes, except that you
can also use a generalized displacement to monitor a nonlinear static analysis.
To define a generalized displacement, specify the following:
• A unique name
• The type of displacement measure
• A list of the joint degrees of freedom and their corresponding scale factors that
will be summed to created the generalized displacement
The type of displacement measure can be one of the following:
• Translational: The generalized displacement scales (with change of units) as
length. Coefficients of contributing joint translations are unitless. Coefficients
of contributing joint rotations scale as length.
• Rotational: The generalized displacement is unitless (radians). Coefficients of
joint translations scale as inverse length. Coefficients of joint rotations are
unitless.
Be sure to choose your scale factors for each contributing component to account for
the type of generalized displacement being defined.

Degree of Freedom Output
A table of the types of degrees of freedom present at every joint in the model is
printed in the analysis output (.OUT) file under the heading:
DISPLACEMENT DEGREES OF FREEDOM

The degrees of freedom are listed for all of the regular joints, as well as for the master joints created automatically by the program. For Constraints, the master joints
are identified by the labels of their corresponding Constraints. For Welds, the master joint for each set of joints that are welded together is identified by the label of
one of the welded joints. Joints are printed in alpha-numeric order of the labels.
The type of each of the six degrees of freedom at a joint is identified by the following symbols:
(A)
(-)

Active degree of freedom
Restrained degree of freedom

Degree of Freedom Output

Chapter IV
(+)
( )

Joints and Degrees of Freedom

Constrained degree of freedom
Null or unavailable degree of freedom

The degrees of freedom are always referred to the local axes of the joint. They are
identified in the output as U1, U2, U3, R1, R2, and R3 for all joints. However, if all
regular joints use the global coordinate system as the local system (the usual situation), then the degrees of freedom for the regular joints are identified as UX, UY,
UZ, RX, RY, and RZ.
The types of degrees of freedom are a property of the structure and are independent
of the Load Cases, except when staged construction is performed.
See Topic “Degrees of Freedom” (page 30) in this Chapter for more information.

Assembled Joint Mass Output
You can request assembled joint masses as part of the analysis results. The mass at a
given joint includes the mass assigned directly to that joint as well as a portion of
the mass from each element connected to that joint. All mass assigned to the elements is apportioned to the connected joints, so that this table represents the total
mass of the structure. The masses are always referred to the local axes of the joint.
If multiple Mass Sources have been specified, the assembled joint mass output is
provided for each Mass Source that was actually used in the analysis.
For more information:
• See Topic “Masses” (page 40) in this Chapter.
• See Topic “Mass Source” (page 334) in Chapter “Load Patterns”.
• See Chapter “Load Cases” (page 341).

Displacement Output
You can request joint displacements as part of the analysis results on a case by case
basis. For dynamic Load Cases, you can also request velocities and accelerations.
The output is always referred to the local axes of the joint.
• See Topic “Degrees of Freedom” (page 30) in this Chapter.
• See Chapter “Load Cases” (page 341).

Assembled Joint Mass Output

CSI Analysis Reference Manual

Force Output
You can request joint support forces as part of the analysis results on a case by case
basis. These support forces are called reactions, and are the sum of all forces from
restraints, springs, or one-joint Link/Support objects at that joint. The reactions at
joints that are not supported will be zero.
Note that reactions for one-joint Link/Support objects are not reported at the original joint, but rather at a generated joint at the same location with an identifying
label.
The forces and moments are always referred to the local axes of the joint. The values reported are always the forces and moments that act on the joints. Thus a positive value of joint force or moment would tend to cause a positive value of joint
translation or rotation along the corresponding degree of freedom if it were not supported.
For more information:
• See Topic “Degrees of Freedom” (page 30) in this Chapter.
• See Chapter “Load Cases” (page 341).

Element Joint Force Output
The element joint forces are concentrated forces and moments acting at the joints
of the element that represent the effect of the rest of the structure upon the element
and that cause the deformation of the element. The moments will always be zero for
the solid-type elements: Plane, Asolid, and Solid.
A positive value of force or moment tends to cause a positive value of translation or
rotation of the element along the corresponding joint degree of freedom.
Element joint forces must not be confused with internal forces and moments which,
like stresses, act within the volume of the element.
For a given element, the vector of element joint forces, f, is computed as:
f =K u -r
where K is the element stiffness matrix, u is the vector of element joint displacements, and r is the vector of element applied loads as apportioned to the joints. The
element joint forces are always referred to the local axes of the individual joints.
They are identified in the output as F1, F2, F3, M1, M2, and M3.

Force Output

Chapter V

Constraints and Welds
Constraints are used to enforce certain types of rigid-body behavior, to connect together different parts of the model, and to impose certain types of symmetry conditions. Welds are used to generate a set of constraints that connect together different
parts of the model.
Basic Topics for All Users
• Overview
• Body Constraint
• Plane Definition
• Diaphragm Constraint
• Plate Constraint
• Axis Definition
• Rod Constraint
• Beam Constraint
• Equal Constraint
• Welds

CSI Analysis Reference Manual
Advanced Topics
• Local Constraint
• Automatic Master Joints
• Constraint Output

Overview
A constraint consists of a set of two or more constrained joints. The displacements
of each pair of joints in the constraint are related by constraint equations. The types
of behavior that can be enforced by constraints are:
• Rigid-body behavior, in which the constrained joints translate and rotate together as if connected by rigid links. The types of rigid behavior that can be
modeled are:
– Rigid Body: fully rigid for all displacements
– Rigid Diaphragm: rigid for membrane behavior in a plane
– Rigid Plate: rigid for plate bending in a plane
– Rigid Rod: rigid for extension along an axis
– Rigid Beam: rigid for beam bending on an axis
• Equal-displacement behavior, in which the translations and rotations are equal
at the constrained joints
• Symmetry and anti-symmetry conditions
The use of constraints reduces the number of equations in the system to be solved
and will usually result in increased computational efficiency.
Most constraint types must be defined with respect to some fixed coordinate system. The coordinate system may be the global coordinate system or an alternate coordinate system, or it may be automatically determined from the locations of the
constrained joints. The Local Constraint does not use a fixed coordinate system, but
references each joint using its own joint local coordinate system.
Welds are used to connect together different parts of the model that were defined
separately. Each Weld consists of a set of joints that may be joined. The program
searches for joints in each Weld that share the same location in space and constrains
them to act as a single joint.

Overview

Chapter V

Constraints and Welds

Body Constraint
A Body Constraint causes all of its constrained joints to move together as a
three-dimensional rigid body. By default, all degrees of freedom at each connected
joint participate. However, you can select a subset of the degrees of freedom to be
constrained.
This Constraint can be used to:
• Model rigid connections, such as where several beams and/or columns frame
together
• Connect together different parts of the structural model that were defined using
separate meshes
• Connect Frame elements that are acting as eccentric stiffeners to Shell elements
Welds can be used to automatically generate Body Constraints for the purpose of
connecting coincident joints.
See Topic “Welds” (page 64) in this Chapter for more information.

Joint Connectivity
Each Body Constraint connects a set of two or more joints together. The joints may
have any arbitrary location in space.

Local Coordinate System
Each Body Constraint has its own local coordinate system, the axes of which are
denoted 1, 2, and 3. These correspond to the X, Y, and Z axes of a fixed coordinate
system that you choose.

Constraint Equations
The constraint equations relate the displacements at any two constrained joints
(subscripts I and j) in a Body Constraint. These equations are expressed in terms of
the translations (u1, u2, and u3), the rotations (r1, r2, and r3), and the coordinates (x1,
x2, and x3), all taken in the Constraint local coordinate system:
u1j = u1i + r2i Dx3 – r3i Dx2
u2j = u2i + r3i Dx1 - r1i Dx3

Body Constraint

CSI Analysis Reference Manual
u3j = u3i + r1i Dx2 - r2i Dx1
r1i = r1j
r2i = r2j
r3i = r3j
where Dx1 = x1j - x1i, Dx2 = x2j - x2i, and Dx3 = x3j - x3i.
If you omit any particular degree of freedom, the corresponding constraint equation
is not enforced. If you omit a rotational degree of freedom, the corresponding terms
are removed from the equations for the translational degrees of freedom.

Plane Definition
The constraint equations for each Diaphragm or Plate Constraint are written with
respect to a particular plane. The location of the plane is not important, only its
orientation.
By default, the plane is determined automatically by the program from the spatial
distribution of the constrained joints as follows:
• The centroid of the constrained joints is determined
• The second moments of the locations of all of the constrained joints about the
centroid are determined
• The principal values and directions of these second moments are found
• The direction of the smallest principal second moment is taken as the normal to
the constraint plane; if all constrained joints lie in a unique plane, this smallest
principal moment will be zero
• If no unique direction can be found, a horizontal (X-Y) plane is assumed in coordinate system csys; this situation can occur if the joints are coincident or collinear, or if the spatial distribution is more nearly three-dimensional than
planar.
You may override automatic plane selection by specifying the following:
• csys: A fixed coordinate system (the default is zero, indicating the global coordinate system)
• axis: The axis (X, Y, or Z) normal to the plane of the constraint, taken in coordinate system csys.

Plane Definition

Chapter V

Constraints and Welds

This may be useful, for example, to specify a horizontal plane for a floor with a
small step in it.

Diaphragm Constraint
A Diaphragm Constraint causes all of its constrained joints to move together as a
planar diaphragm that is rigid against membrane deformation. Effectively, all constrained joints are connected to each other by links that are rigid in the plane, but do
not affect out-of-plane (plate) deformation.
This Constraint can be used to:
• Model concrete floors (or concrete-filled decks) in building structures, which
typically have very high in-plane stiffness
• Model diaphragms in bridge superstructures
The use of the Diaphragm Constraint for building structures eliminates the numerical-accuracy problems created when the large in-plane stiffness of a floor diaphragm is modeled with membrane elements. It is also very useful in the lateral
(horizontal) dynamic analysis of buildings, as it results in a significant reduction in
the size of the eigenvalue problem to be solved. See Figure 10 (page 54) for an
illustration of a floor diaphragm.

Joint Connectivity
Each Diaphragm Constraint connects a set of two or more joints together. The
joints may have any arbitrary location in space, but for best results all joints should
lie in the plane of the constraint. Otherwise, bending moments may be generated
that are restrained by the Constraint, which unrealistically stiffens the structure. If
this happens, the constraint forces reported in the analysis results may not be in
equilibrium.

Local Coordinate System
Each Diaphragm Constraint has its own local coordinate system, the axes of which
are denoted 1, 2, and 3. Local axis 3 is always normal to the plane of the constraint.
The program arbitrarily chooses the orientation of axes 1 and 2 in the plane. The
actual orientation of the planar axes is not important since only the normal direction
affects the constraint equations. For more information, see Topic “Plane Definition” (page 52) in this Chapter.

Diaphragm Constraint

CSI Analysis Reference Manual

Rigid Floor Slab

Constrained
Joint

Beam

Constrained
Joint

Automatic
Master Joint

Effective
Rigid Links

Constrained
Joint

Column

Constrained
Joint
Global

Figure 10
Use of the Diaphragm Constraint to Model a Rigid Floor Slab

Constraint Equations
The constraint equations relate the displacements at any two constrained joints
(subscripts I and j) in a Diaphragm Constraint. These equations are expressed in
terms of in-plane translations (u1 and u2), the rotation (r3) about the normal, and the
in-plane coordinates (x1 and x2), all taken in the Constraint local coordinate system:
u1j = u1i – r3i Dx2
u2j = u2i + r3i Dx1
r3i = r3j
where Dx1 = x1j - x1i and Dx2 = x2j - x2i.

Diaphragm Constraint

Chapter V

Constraints and Welds

Plate Constraint
A Plate Constraint causes all of its constrained joints to move together as a flat plate
that is rigid against bending deformation. Effectively, all constrained joints are
connected to each other by links that are rigid for out-of-plane bending, but do not
affect in-plane (membrane) deformation.
This Constraint can be used to:
• Connect structural-type elements (Frame and Shell) to solid-type elements
(Plane and Solid); the rotation in the structural element can be converted to a
pair of equal and opposite translations in the solid element by the Constraint
• Enforce the assumption that “plane sections remain plane” in detailed models
of beam bending

Joint Connectivity
Each Plate Constraint connects a set of two or more joints together. The joints may
have any arbitrary location in space. Unlike the Diaphragm Constraint, equilibrium
is not affected by whether or not all joints lie in the plane of the Plate Constraint.

Local Coordinate System
Each Plate Constraint has its own local coordinate system, the axes of which are denoted 1, 2, and 3. Local axis 3 is always normal to the plane of the constraint. The
program arbitrarily chooses the orientation of axes 1 and 2 in the plane. The actual
orientation of the planar axes is not important since only the normal direction affects the constraint equations.
For more information, see Topic “Plane Definition” (page 52) in this Chapter.

Constraint Equations
The constraint equations relate the displacements at any two constrained joints
(subscripts I and j) in a Plate Constraint. These equations are expressed in terms of
the out-of-plane translation (u3), the bending rotations (r1 and r2), and the in-plane
coordinates (x1 and x2), all taken in the Constraint local coordinate system:
u3j = u3i + r1i Dx2 - r2i Dx1
r1i = r1j

Plate Constraint

CSI Analysis Reference Manual
r2i = r2j
where Dx1 = x1j - x1i and Dx2 = x2j - x2i.

Axis Definition
The constraint equations for each Rod or Beam Constraint are written with respect
to a particular axis. The location of the axis is not important, only its orientation.
By default, the axis is determined automatically by the program from the spatial
distribution of the constrained joints as follows:
• The centroid of the constrained joints is determined
• The second moments of the locations of all of the constrained joints about the
centroid are determined
• The principal values and directions of these second moments are found
• The direction of the largest principal second moment is taken as the axis of the
constraint; if all constrained joints lie on a unique axis, the two smallest principal moments will be zero
• If no unique direction can be found, a vertical (Z) axis is assumed in coordinate
system csys; this situation can occur if the joints are coincident, or if the spatial
distribution is more nearly planar or three-dimensional than linear.
You may override automatic axis selection by specifying the following:
• csys: A fixed coordinate system (the default is zero, indicating the global coordinate system)
• axis: The axis (X, Y, or Z) of the constraint, taken in coordinate system csys.
This may be useful, for example, to specify a vertical axis for a column with a small
offset in it.

Rod Constraint
A Rod Constraint causes all of its constrained joints to move together as a straight
rod that is rigid against axial deformation. Effectively, all constrained joints maintain a fixed distance from each other in the direction parallel to the axis of the rod,
but translations normal to the axis and all rotations are unaffected.
This Constraint can be used to:

Axis Definition

Chapter V

Constraints and Welds

• Prevent axial deformation in Frame elements
• Model rigid truss-like links
An example of the use of the Rod Constraint is in the analysis of the two-dimensional frame shown in Figure 11 (page 58). If the axial deformations in the beams
are negligible, a single Rod Constraint could be defined containing the five joints.
Instead of five equations, the program would use a single equation to define the
X-displacement of the whole floor. However, it should be noted that this will result
in the axial forces of the beams being output as zero, as the Constraint will cause the
ends of the beams to translate together in the X-direction. Interpretations of such results associated with the use of Constraints should be clearly understood.

Joint Connectivity
Each Rod Constraint connects a set of two or more joints together. The joints may
have any arbitrary location in space, but for best results all joints should lie on the
axis of the constraint. Otherwise, bending moments may be generated that are restrained by the Constraint, which unrealistically stiffens the structure. If this happens, the constraint forces reported in the analysis results may not be in
equilibrium.

Local Coordinate System
Each Rod Constraint has its own local coordinate system, the axes of which are denoted 1, 2, and 3. Local axis 1 is always the axis of the constraint. The program arbitrarily chooses the orientation of the transverse axes 2 and 3. The actual orientation
of the transverse axes is not important since only the axial direction affects the
constraint equations.
For more information, see Topic “Axis Definition” (page 56) in this Chapter.

Constraint Equations
The constraint equations relate the displacements at any two constrained joints
(subscripts I and j) in a Rod Constraint. These equations are expressed only in terms
of the axial translation (u1):
u1j = u1i

Rod Constraint

CSI Analysis Reference Manual

Figure 11
Use of the Rod Constraint to Model Axially Rigid Beams

Beam Constraint
A Beam Constraint causes all of its constrained joints to move together as a straight
beam that is rigid against bending deformation. Effectively, all constrained joints
are connected to each other by links that are rigid for off-axis bending, but do not
affect translation along or rotation about the axis.
This Constraint can be used to:
• Connect structural-type elements (Frame and Shell) to solid-type elements
(Plane and Solid); the rotation in the structural element can be converted to a
pair of equal and opposite translations in the solid element by the Constraint
• Prevent bending deformation in Frame elements

Joint Connectivity
Each Beam Constraint connects a set of two or more joints together. The joints may
have any arbitrary location in space, but for best results all joints should lie on the
axis of the constraint. Otherwise, torsional moments may be generated that are restrained by the Constraint, which unrealistically stiffens the structure. If this hap-

Beam Constraint

Chapter V

Constraints and Welds

pens, the constraint forces reported in the analysis results may not be in
equilibrium.

Local Coordinate System
Each Beam Constraint has its own local coordinate system, the axes of which are
denoted 1, 2, and 3. Local axis 1 is always the axis of the constraint. The program
arbitrarily chooses the orientation of the transverse axes 2 and 3. The actual orientation of the transverse axes is not important since only the axial direction affects the
constraint equations.
For more information, see Topic “Axis Definition” (page 56) in this Chapter.

Constraint Equations
The constraint equations relate the displacements at any two constrained joints
(subscripts I and j) in a Beam Constraint. These equations are expressed in terms of
the transverse translations (u2 and u3), the transverse rotations (r2 and r3), and the axial coordinate (x1), all taken in the Constraint local coordinate system:
u2j = u2i + r3i Dx1
u3j = u3i - r2i Dx1
r2i = r2j
r3i = r3j
where Dx1 = x1j - x1i.

Equal Constraint
An Equal Constraint causes all of its constrained joints to move together with the
same displacements for each selected degree of freedom, taken in the constraint local coordinate system. The other degrees of freedom are unaffected.
The Equal Constraint differs from the rigid-body types of Constraints in that there
is no coupling between the rotations and the translations.
This Constraint can be used to partially connect together different parts of the structural model, such as at expansion joints and hinges

Equal Constraint

CSI Analysis Reference Manual
For fully connecting meshes, it is better to use the Body Constraint when the constrained joints are not in exactly the same location.

Joint Connectivity
Each Equal Constraint connects a set of two or more joints together. The joints may
have any arbitrary location in space, but for best results all joints should share the
same location in space if used for connecting meshes. Otherwise, moments may be
generated that are restrained by the Constraint, which unrealistically stiffens the
structure. If this happens, the constraint forces reported in the analysis results may
not be in equilibrium.

Local Coordinate System
Each Equal Constraint uses a fixed coordinate system, csys, that you specify. The
default for csys is zero, indicating the global coordinate system. The axes of the
fixed coordinate system are denoted X, Y, and Z.

Selected Degrees of Freedom
For each Equal Constraint you may specify a list, cdofs, of up to six degrees of freedom in coordinate system csys that are to be constrained. The degrees of freedom
are indicated as UX, UY, UZ, RX, RY, and RZ.

Constraint Equations
The constraint equations relate the displacements at any two constrained joints
(subscripts I and j) in an Equal Constraint. These equations are expressed in terms
of the translations (ux, uy, and uz) and the rotations (rx, ry, and rz), all taken in fixed
coordinate system csys:
uxj = uxi
uyj = uyi
uzj = uzi
r1i = r1j
r2i = r2j
r3i = r3j

Equal Constraint

Chapter V

Constraints and Welds

If you omit any of the six degrees of freedom from the constraint definition, the corresponding constraint equation is not enforced.

Local Constraint
A Local Constraint causes all of its constrained joints to move together with the
same displacements for each selected degree of freedom, taken in the separate joint
local coordinate systems. The other degrees of freedom are unaffected.
The Local Constraint differs from the rigid-body types of Constraints in that there
is no coupling between the rotations and the translations. The Local Constraint is
the same as the Equal Constraint if all constrained joints have the same local coordinate system.
This Constraint can be used to:
• Model symmetry conditions with respect to a line or a point
• Model displacements constrained by mechanisms
The behavior of this Constraint is dependent upon the choice of the local coordinate
systems of the constrained joints.

Joint Connectivity
Each Local Constraint connects a set of two or more joints together. The joints may
have any arbitrary location in space. If the joints do not share the same location in
space, moments may be generated that are restrained by the Constraint. If this happens, the constraint forces reported in the analysis results may not be in equilibrium. These moments are necessary to enforce the desired symmetry of the displacements when the applied loads are not symmetric, or may represent the
constraining action of a mechanism.
For more information, see:
• Topic “Force Output” (page 48) in Chapter “Joints and Degrees of Freedom.”
• Topic “Global Force Balance Output” (page 45) in Chapter “Joints and Degrees of Freedom.”

Local Constraint

CSI Analysis Reference Manual

No Local Coordinate System
A Local Constraint does not have its own local coordinate system. The constraint
equations are written in terms of constrained joint local coordinate systems, which
may differ. The axes of these coordinate systems are denoted 1, 2, and 3.

Selected Degrees of Freedom
For each Local Constraint you may specify a list, ldofs, of up to six degrees of freedom in the joint local coordinate systems that are to be constrained. The degrees of
freedom are indicated as U1, U2, U3, R1, R2, and R3.

Constraint Equations
The constraint equations relate the displacements at any two constrained joints
(subscripts I and j) in a Local Constraint. These equations are expressed in terms of
the translations (u1, u2, and u3) and the rotations (r1, r2, and r3), all taken in joint local
coordinate systems. The equations used depend upon the selected degrees of freedom and their signs. Some important cases are described next.
Axisymmetry
Axisymmetry is a type of symmetry about a line. It is best described in terms of a
cylindrical coordinate system having its Z axis on the line of symmetry. The structure, loading, and displacements are each said to be axisymmetric about a line if
they do not vary with angular position around the line, i.e., they are independent of
the angular coordinate CA.
To enforce axisymmetry using the Local Constraint:
• Model any cylindrical sector of the structure using any axisymmetric mesh of
joints and elements
• Assign each joint a local coordinate system such that local axes 1, 2, and 3 correspond to the coordinate directions +CR, +CA, and +CZ, respectively
• For each axisymmetric set of joints (i.e., having the same coordinates CR and
CZ, but different CA), define a Local Constraint using all six degrees of freedom: U1, U2, U3, R1, R2, and R3
• Restrain joints that lie on the line of symmetry so that, at most, only axial translations (U3) and rotations (R3) are permitted
The corresponding constraint equations are:

Local Constraint

Chapter V

Constraints and Welds

u1j = u1i
u2j = u2i
u3j = u3i
r1i = r1j
r2i = r2j
r3i = r3j
The numeric subscripts refer to the corresponding joint local coordinate systems.
Cyclic symmetry
Cyclic symmetry is another type of symmetry about a line. It is best described in
terms of a cylindrical coordinate system having its Z axis on the line of symmetry.
The structure, loading, and displacements are each said to be cyclically symmetric
about a line if they vary with angular position in a repeated (periodic) fashion.
To enforce cyclic symmetry using the Local Constraint:
• Model any number of adjacent, representative, cylindrical sectors of the structure; denote the size of a single sector by the angle q
• Assign each joint a local coordinate system such that local axes 1, 2, and 3 correspond to the coordinate directions +CR, +CA, and +CZ, respectively
• For each cyclically symmetric set of joints (i.e., having the same coordinates
CR and CZ, but with coordinate CA differing by multiples of q), define a Local
Constraint using all six degrees of freedom: U1, U2, U3, R1, R2, and R3.
• Restrain joints that lie on the line of symmetry so that, at most, only axial translations (U3) and rotations (R3) are permitted
The corresponding constraint equations are:
u1j = u1i
u2j = u2i
u3j = u3i
r1i = r1j
r2i = r2j
r3i = r3j
Local Constraint

CSI Analysis Reference Manual
The numeric subscripts refer to the corresponding joint local coordinate systems.
For example, suppose a structure is composed of six identical 60° sectors, identically loaded. If two adjacent sectors were modeled, each Local Constraint would
apply to a set of two joints, except that three joints would be constrained on the
symmetry planes at 0°, 60°, and 120°.
If a single sector is modeled, only joints on the symmetry planes need to be constrained.
Symmetry About a Point
Symmetry about a point is best described in terms of a spherical coordinate system
having its Z axis on the line of symmetry. The structure, loading, and displacements
are each said to be symmetric about a point if they do not vary with angular position
about the point, i.e., they are independent of the angular coordinates SB and SA.
Radial translation is the only displacement component that is permissible.
To enforce symmetry about a point using the Local Constraint:
• Model any spherical sector of the structure using any symmetric mesh of joints
and elements
• Assign each joint a local coordinate system such that local axes 1, 2, and 3 correspond to the coordinate directions +SB, +SA, and +SR, respectively
• For each symmetric set of joints (i.e., having the same coordinate SR, but different coordinates SB and SA), define a Local Constraint using only degree of
freedom U3
• For all joints, restrain the degrees of freedom U1, U2, R1, R2, and R3
• Fully restrain any joints that lie at the point of symmetry
The corresponding constraint equations are:
u3j = u3i
The numeric subscripts refer to the corresponding joint local coordinate systems.
It is also possible to define a case for symmetry about a point that is similar to cyclic
symmetry around a line, e.g., where each octant of the structure is identical.

Local Constraint

Chapter V

Constraints and Welds

221

121

Mesh B
222

122
123

124

125
223

224

225

Mesh A

Figure 12
Use of a Weld to Connect Separate Meshes at Coincident Joints

Welds
A Weld can be used to connect together different parts of the structural model that
were defined using separate meshes. A Weld is not a single Constraint, but rather is
a set of joints from which the program will automatically generate multiple Body
Constraints to connect together coincident joints.
Joints are considered to be coincident if the distance between them is less than or
equal to a tolerance, tol, that you specify. Setting the tolerance to zero is permissible but is not recommended.
One or more Welds may be defined, each with its own tolerance. Only the joints
within each Weld will be checked for coincidence with each other. In the most
common case, a single Weld is defined that contains all joints in the model; all coincident groups of joints will be welded. However, in situations where structural discontinuity is desired, it may be necessary to prevent the welding of some coincident
joints. This may be facilitated by the use of multiple Welds.
Figure 12 (page 65) shows a model developed as two separate meshes, A and B.
Joints 121 through 125 are associated with mesh A, and Joints 221 through 225 are
associated with mesh B. Joints 121 through 125 share the same location in space as
Joints 221 through 225, respectively. These are the interfacing joints between the
two meshes. To connect these two meshes, a single Weld can be defined containing
all joints, or just joints 121 through 125 and 221 through 225. The program would

Welds

CSI Analysis Reference Manual
generate five Body Constraints, each containing two joints, resulting in an
integrated model.
It is permissible to include the same joint in more than one Weld. This could result
in the joints in different Welds being constrained together if they are coincident
with the common joint. For example, suppose that Weld 1 contained joints 1,2, and
3, Weld 2 contained joints 3, 4, and 5. If joints 1, 3, and 5 were coincident, joints 1
and 3 would be constrained by Weld 1, and joints 3 and 5 would be constrained by
Weld 2. The program would create a single Body Constraint containing joints 1, 3,
and 5. One the other hand, if Weld 2 did not contain joint 3, the program would only
generate a Body Constraint containing joint 1 and 3 from Weld 1; joint 5 would not
be constrained.
For more information, see Topic “Body Constraint” (page 51) in this Chapter.

Automatic Master Joints
The program automatically creates an internal master joint for each explicit Constraint, and a master joint for each internal Body Constraint that is generated by a
Weld. Each master joint governs the behavior of the corresponding constrained
joints. The displacement at a constrained degree of freedom is computed as a linear
combination of the displacements of the master joint.
See Topic “Degrees of Freedom” (page 30) in Chapter “Joints and Degrees of Freedom” for more information.

Stiffness, Mass, and Loads
Joint local coordinate systems, springs, masses, and loads may all be applied to
constrained joints. Elements may also be connected to constrained joints. The joint
and element stiffnesses, masses and loads from the constrained degrees of freedom
are be automatically transferred to the master joint in a consistent fashion.
The translational stiffness at the master joint is the sum of the translational
stiffnesses at the constrained joints. The same is true for translational masses and
loads.
The rotational stiffness at a master joint is the sum of the rotational stiffnesses at the
constrained degrees of freedom, plus the second moment of the translational
stiffnesses at the constrained joints for the Body, Diaphragm, Plate, and Beam Constraints. The same is true for rotational masses and loads, except that only the first
moment of the translational loads is used. The moments of the translational

Automatic Master Joints

Chapter V

Constraints and Welds

stiffnesses, masses, and loads are taken about the center of mass of the constrained
joints. If the joints have no mass, the centroid is used.

Local Coordinate Systems
Each master joint has two local coordinate systems: one for the translational degrees of freedom, and one for the rotational degrees of freedom. The axes of each
local system are denoted 1, 2, and 3. For the Local Constraint, these axes correspond to the local axes of the constrained joints. For other types of Constraints,
these axes are chosen to be the principal directions of the translational and rotational masses of the master joint. Using the principal directions eliminates coupling
between the mass components in the master-joint local coordinate system.
For a Diaphragm or Plate Constraint, the local 3 axes of the master joint are always
normal to the plane of the Constraint. For a Beam or Rod Constraint, the local 1
axes of the master joint are always parallel to the axis of the Constraint.

Constraint Output
For each Body, Diaphragm, Plate, Rod, and Beam Constraint having more than two
constrained joints, the following information about the Constraint and its master
joint is printed in the output file:
• The translational and rotational local coordinate systems for the master joint
• The total mass and mass moments of inertia for the Constraint that have been
applied to the master joint
• The center of mass for each of the three translational masses
The degrees of freedom are indicated as U1, U2, U3, R1, R2, and R3. These are referred to the two local coordinate systems of the master joint.

Constraint Output

CSI Analysis Reference Manual

Constraint Output

C h a p t e r VI

Material Properties
The Materials are used to define the mechanical, thermal, and density properties
used by the Frame, Cable, Tendon, Shell, Plane, Asolid, and Solid elements.
Basic Topics for All Users
• Overview
• Local Coordinate System
• Stresses and Strains
• Isotropic Materials
• Uniaxial Materials
• Mass Density
• Weight Density
• Design-Type Indicator
Advanced Topics
• Orthotropic Materials
• Anisotropic Materials
• Temperature-Dependent Materials

CSI Analysis Reference Manual
• Element Material Temperature
• Material Damping
• Nonlinear Material Behavior
• Hysteresis Models
• Modified Darwin-Pecknold Concrete Model
• Time-dependent Properties

Overview
The Material properties may be defined as isotropic, orthotropic or anisotropic.
How the properties are actually utilized depends on the element type. Each Material
that you define may be used by more than one element or element type. For each element type, the Materials are referenced indirectly through the Section properties
appropriate for that element type.
All elastic material properties may be temperature dependent. Properties are given
at a series of specified temperatures. Properties at other temperatures are obtained
by linear interpolation.
For a given execution of the program, the properties used by an element are assumed to be constant regardless of any temperature changes experienced by the
structure. Each element may be assigned a material temperature that determines
the material properties used for the analysis.
Time-dependent properties include creep, shrinkage, and age-dependent elasticity.
These properties can be activated during a staged-construction analysis, and form
the basis for subsequent analyses.
Nonlinear stress-strain curves may be defined for use with fiber hinges in frame elements or nonlinear layers in shell elements.

Local Coordinate System
Each Material has its own Material local coordinate system used to define the
elastic and thermal properties. This system is significant only for orthotropic and
anisotropic materials. Isotropic materials are independent of any particular
coordinate system.

Overview

Chapter VI

Material Properties

s 33

s 23

s 13
s 13

s 22
s 12
2

Material Local
Coordinate System

s 12

s 11

Stress Components

Figure 13
Definition of Stress Components in the Material Local Coordinate System

The axes of the Material local coordinate system are denoted 1, 2, and 3. By default,
the Material coordinate system is aligned with the local coordinate system for each
element. However, you may specify a set of one or more material angles that rotate
the Material coordinate system with respect to the element system for those elements that permit orthotropic or anisotropic properties.
For more information:
• See Topic “Material Angle” (page 193) in Chapter “The Shell Element.”
• See Topic “Material Angle” (page 219) in Chapter “The Plane Element.”
• See Topic “Material Angle” (page 229) in Chapter “The Asolid Element.”
• See Topic “Material Angles” (page 246) in Chapter “The Solid Element.”

Stresses and Strains
The elastic mechanical properties relate the behavior of the stresses and strains
within the Material. The stresses are defined as forces per unit area acting on an elemental cube aligned with the material axes as shown in Figure 13 (page 71). The
stresses s 11 , s 22 , and s 33 are called the direct stresses and tend to cause length

Stresses and Strains

CSI Analysis Reference Manual
change, while s 12 , s 13 , and s 23 are called the shear stresses and tend to cause angle
change.
Not all stress components exist in every element type. For example, the stresses
s 22 , s 33 , and s 23 are assumed to be zero in the Frame element, and stress s 33 is
taken to be zero in the Shell element.
The direct strains e 11 , e 22 , and e 33 measure the change in length along the Material
local 1, 2, and 3 axes, respectively, and are defined as:
e 11 =

du1
dx 1

e 22 =

du 2
dx 2

e 33 =

du 3
dx 3

where u1, u2, and u3 are the displacements and x1, x2, and x3 are the coordinates in the
Material 1, 2, and 3 directions, respectively.
The engineering shear strains g 12 , g 13 , and g 23 , measure the change in angle in the
Material local 1-2, 1-3, and 2-3 planes, respectively, and are defined as:
g 12 =

du1 du 2
+
dx 2 dx 1

g 13 =

du1 du 3
+
dx 3 dx 1

g 23 =

du 2 du 3
+
dx 3 dx 2

Note that the engineering shear strains are equal to twice the tensorial shear strains
e 12 , e 13 , and e 23 , respectively.
Strains can also be caused by a temperature change, DT, that can be specified as a
load on an element. No stresses are caused by a temperature change unless the induced thermal strains are restrained.
See Cook, Malkus, and Plesha (1989), or any textbook on elementary mechanics.

Stresses and Strains

Chapter VI

Material Properties

Isotropic Materials
The behavior of an isotropic material is independent of the direction of loading or
the orientation of the material. In addition, shearing behavior is uncoupled from
extensional behavior and is not affected by temperature change. Isotropic behavior
is usually assumed for steel and concrete, although this is not always the case.
The isotropic mechanical and thermal properties relate strain to stress and temperature change as follows:
é1
ê e1
ê
ì e 11 ü ê
ïe ï ê
ï 22 ï ê
ïe 33 ï ê
í
ý=ê
ï g 12 ï ê
ï g 13 ï ê
ïg ï ê
î 23 þ
ê
ê
êë

-u12
e1
1
e1

sym.

-u12
e1
-u12
e1
1
e1

1
g12

0
1
g12

0 ù
ú
ú
0 ú ì s 11 ü ì a1 ü
ú ïs 22 ï ï a1 ï
ï ï ï
0 úï
ú ïs 33 ï + ï a1 ï DT
í
ý í ý
0 ú ïs 12 ï ï 0 ï
ú
ú ïs 13 ï ï 0 ï
0 ú ïs ï ï 0 ï
î 23 þ î þ
ú
1 ú
g12 úû

(Eqn. 1)

where e1 is Young’s modulus of elasticity, u12 is Poisson’s ratio, g12 is the shear
modulus, and a1 is the coefficient of thermal expansion. This relationship holds regardless of the orientation of the Material local 1, 2, and 3 axes.
The shear modulus is not directly specified, but instead is defined in terms of
Young’s modulus and Poisson’s ratio as:
g12 =

e1
2 (1 + u12 )

Note that Young’s modulus must be positive, and Poisson’s ratio must satisfy the
condition:
-1< u12 <

1
2

Isotropic Materials

CSI Analysis Reference Manual

Uniaxial Materials
Uniaxial materials are used for modeling rebar, cable, and tendon behavior. These
types of objects primarily carry axial tension and have a preferred direction of action. Shearing behavior may be considered in certain applications, such as for rebar
when used in layered shell sections.
Uniaxial behavior can be considered as an isotropic material with stresses
s 22 = s 33 = s 23 = 0, regardless of the strains. This relationship is directional and is
always aligned with the Material local 1 axis.
The uniaxial mechanical and thermal properties relate strain to stress and temperature change as follows:
é1
ê e1
ê
ì e 11 ü ê
ïe ï ê
ï 22 ï ê
ïe 33 ï ê
í
ý=ê
ï g 12 ï ê
ï g 13 ï ê
ïg ï ê
î 23 þ
ê
ê
êë

-u12
e1
1
e1

sym.

-u12
e1
-u12
e1
1
e1

1
g12

0
1
g12

0 ù
ú
ú
0 ú ìs 11 ü ì a1 ü
úï 0 ï ï0ï
ï ï ï
0 úï
ú ï 0 ï + ï 0 ï DT
í
ý í ý
0 ú ïs 12 ï ï 0 ï
ú
ú ïs 13 ï ï 0 ï
0 úï 0 ï ï0ï
î
þ î þ
ú
1 ú
g12 úû

(Eqn. 2)

where e1 is Young’s modulus of elasticity, u12 is Poisson’s ratio, g12 is the shear
modulus, and a1 is the coefficient of thermal expansion.
When used, the shear modulus is not directly specified, but instead is defined in
terms of Young’s modulus and Poisson’s ratio as:
g12 =

e1
2 (1 + u12 )

Note that Young’s modulus must be positive, and Poisson’s ratio must satisfy the
condition:
-1< u12 <

Uniaxial Materials

1
2

Chapter VI

Material Properties

Orthotropic Materials
The behavior of an orthotropic material can be different in each of the three local
coordinate directions. However, like an isotropic material, shearing behavior is uncoupled from extensional behavior and is not affected by temperature change.
The orthotropic mechanical and thermal properties relate strain to stress and temperature change as follows:
é1
ê e1
ê
ì e 11 ü ê
ïe ï ê
ï 22 ï ê
ïe 33 ï ê
í
ý=ê
g
12
ï
ï ê
ï g 13 ï ê
ïg ï ê
î 23 þ
ê
ê
êë

-u12
e2
1
e2

sym.

-u13
e3
-u23
e3
1
e3

1
g12

0
1
g13

0 ù
ú
ú
0 ú ì s 11 ü ì a1 ü
ú ïs 22 ï ï a2 ï
ï ï ï
0 úï
ú ïs 33 ï + ï a3 ï DT
í
ý í ý
0 ú ïs 12 ï ï 0 ï
ú
ú ïs 13 ï ï 0 ï
0 ú ïs ï ï 0 ï
î 23 þ î þ
ú
1 ú
g23 úû

(Eqn. 3)

where e1, e2, and e3 are the moduli of elasticity; u12, u13, and u23 are the Poisson’s ratios; g12, g13, and g23 are the shear moduli; and a1, a2, and a3 are the coefficients of thermal expansion.
Note that the elastic moduli and the shear moduli must be positive. The Poisson’s
ratios may take on any values provided that the upper-left 3x3 portion of the stressstrain matrix is positive-definite (i.e., has a positive determinant.)

Anisotropic Materials
The behavior of an anisotropic material can be different in each of the three local
coordinate directions. In addition, shearing behavior can be fully coupled with extensional behavior and can be affected by temperature change.
The anisotropic mechanical and thermal properties relate strain to stress and temperature change as follows:

Orthotropic Materials

CSI Analysis Reference Manual
é1
ê e1
ê
e
ì 11 ü ê
ïe ï ê
ï 22 ï ê
ïe 33 ï ê
í
ý=ê
g
12
ï
ï ê
ï g 13 ï ê
ïg ï ê
î 23 þ ê
ê
ê
ë

-u12
e2
1
e2

-u13
e3
-u23
e3
1
e3

sym.

-u14
g12
-u24
g12
-u34
g12
1
g12

-u15
g13
-u25
g13
-u35
g13
-u45
g13
1
g13

-u16 ù
(Eqn. 4)
ú
g23
-u26 ú
ú ì s ü ì a1 ü
g23 ú ï 11 ï ï
ï
-u36 ú ïs 22 ï ï a2 ï
g23 ú ïs 33 ï + ï a3 ï DT
-u46 ú ís 12 ý í a12 ý
ï ï
ï
úï
g23 ú ïs 13 ï ï a13 ï
-u56 ú ï
ï ï
ï
îs 23 þ î a23 þ
g23 ú
1 ú
ú
g23 û

where e1, e2, and e3 are the moduli of elasticity; u12, u13, and u23 are the standard
Poisson’s ratios; u14, u24..., u56 are the shear and coupling Poisson’s ratios; g12,
g13, and g23 are the shear moduli; a1, a2, and a3 are the coefficients of thermal expansion; and a12, a13, and a23 are the coefficients of thermal shear.
Note that the elastic moduli and the shear moduli must be positive. The Poisson’s
ratios must be chosen so that the 6x6 stress-strain matrix is positive definite. This
means that the determinant of the matrix must be positive.
These material properties can be evaluated directly from laboratory experiments.
Each column of the elasticity matrix represents the six measured strains due to the
application of the appropriate unit stress. The six thermal coefficients are the measured strains due to a unit temperature change.

Temperature-Dependent Properties
All of the mechanical and thermal properties given in Equations (1) to (4) may depend upon temperature. These properties are given at a series of specified material
temperatures t. Properties at other temperatures are obtained by linear interpolation
between the two nearest specified temperatures. Properties at temperatures outside
the specified range use the properties at the nearest specified temperature. See
Figure 14 (page 77) for examples.
If the Material properties are independent of temperature, you need only specify
them at a single, arbitrary temperature.

Temperature-Dependent Properties

Chapter VI

Material Properties

E
indicates specified value e
at temperature t

Ematt
Ematt

Tmatt

Interpolated Value

Tmatt

Extrapolated Value

Figure 14
Determination of Property Ematt at Temperature Tmatt from Function E(T)

Element Material Temperature
You can assign each element an element material temperature. This is the temperature at which temperature-dependent material properties are evaluated for the
element. The properties at this fixed temperature are used for all analyses regardless of any temperature changes experienced by the element during loading.
The element material temperature may be uniform over an element or interpolated
from values given at the joints. In the latter case, a uniform material temperature is
used that is the average of the joint values. The default material temperature for any
element is zero.
The properties for a temperature-independent material are constant regardless of
the element material temperatures specified.

Mass Density
For each Material you may specify a mass density, m, that is used for calculating
the mass of the element. The total mass of the element is the product of the mass
density (mass per unit volume) and the volume of the element. This mass is apportioned to each joint of the element. The same mass is applied along of the three
translational degrees of freedom. No rotational mass moments of inertia are computed.

Element Material Temperature

CSI Analysis Reference Manual
Consistent mass units must be used. Typically the mass density is equal to the
weight density of the material divided by the acceleration due to gravity, but this is
not required.
The mass density property is independent of temperature.
For more information:
• See Topic “Mass” (page 134) in Chapter “The Frame Element.”
• See Topic “Mass” (page 172) in Chapter “The Cable Element.”
• See Topic “Mass” (page 206) in Chapter “The Shell Element.”
• See Topic “Mass” (page 220) in Chapter “The Plane Element.”
• See Topic “Mass” (page 232) in Chapter “The Asolid Element.”
• See Topic “Mass” (page 248) in Chapter “The Solid Element.”
• See Topic “Mass Source” (page 334) in Chapter “Load Patterns”.

Weight Density
For each Material you may specify a weight density, w, that is used for calculating
the self-weight of the element. The total weight of the element is the product of the
weight density (weight per unit volume) and the volume of the element. This
weight is apportioned to each joint of the element. Self-weight is activated using
Self-weight Load and Gravity Load.
The weight density property is independent of temperature.
For more information:
• See Topic “Self-Weight Load” (page 325) in Chapter “Load Patterns.”
• See Topic “Gravity Load” (page 326) in Chapter “Load Patterns.”

Material Damping
You may specify material damping to be used in dynamic analyses. Different types
of damping are available for different types of Load Cases. Material damping is a
property of the material and affects all Load Cases of a given type in the same way.
You may specify additional damping in each Load Case.

Weight Density

Chapter VI

Material Properties

Because damping has such a significant affect upon dynamic response, you should
use care in defining your damping parameters.
The material used for calculating damping is determined for the different types of
elements as follows:
• For frame elements, if a material overwrite is specified, that material is used.
Otherwise the material for the current frame section is used, with non-prismatic
sections using a simple average of the damping coefficients over all materials
along the full length of the section.
• For shell elements, if a material overwrite is specified, that material is used.
Otherwise the material for the current shell section is used, with layered sections using a thickness-weighted average of the damping coefficients over all
material layers in the section.
• For cable, tendon, plane, asolid, and solid elements, the material for the current
section is used.
Material-based damping does not apply to link elements.

Modal Damping
The material modal damping available in SAP2000 is stiffness weighted, and is
also known as composite modal damping. It is used for all response-spectrum and
modal time-history analyses. For each material you may specify a material modal
damping ratio, r, where 0 £ r < 1. The damping ratio, rij , contributed to mode I by element j of this material is given by
T

rij =

rf i K j f i
Ki

where f i is mode shape for mode I, K j is the stiffness matrix for element j, and K i
is the modal stiffness for mode I given by
K i = å f Ti K j f i
j

summed over all elements, j, in the model.

Material Damping

CSI Analysis Reference Manual

Viscous Proportional Damping
Viscous proportional damping is used for direct-integration time-history analyses.
For each material, you may specify a mass coefficient, c M , and a stiffness coefficient, c K . You may specify these two coefficients directly, or they may be computed by specifying equivalent fractions of critical modal damping at two different
periods or frequencies.
The damping matrix for element j of the material is computed as:
C j = c M M j + cK K

0
j

where M j is the mass of the element, and K 0j is the stiffness of the element. The superscript “0” indicates that for nonlinear elements, the initial stiffness is used. This
is the stiffness of the element at zero initial conditions, regardless of the current
nonlinear state of the element. The exception to this rule is that if the current nonlinear state has zero stiffness and zero force or stress (such as for cracked concrete material), then zero damping is assumed. In the case where the initial stiffness is different in the negative and positive direction of loading, the larger stiffness is used.

Hysteretic Proportional Damping
Hysteretic proportional damping is used for steady-state and power-spectral-density analyses. For each material, you may specify a mass coefficient, d M , and a
stiffness coefficient, d M . The hysteretic damping matrix for element j of the material is computed as:
D j = d MM j + dKK

0
j

where M j is the mass of the element, and K 0j is the stiffness of the element. See the
subtopic “Viscous Proportional Damping” above for how the material stiffness is
determined for nonlinear elements.

Nonlinear Material Behavior
Nonlinear material behavior is available in certain elements using a directional material model, in which uncoupled stress-strain behavior is modeled for one or more
stress-strain components. This is a simple and practical engineering model suitable
for many applications such as beams and columns, shear walls, bridge decks, tunnels, retaining walls, and others. You should carefully examine the applicability of

Nonlinear Material Behavior

Chapter VI

Material Properties

this model before using it in a general continuum model where the governing
stresses change direction substantially from place to place.
In addition, a two-dimensional concrete model is available for use in the layered
shell. This model is discussed in topic “Modified Darwin-Pecknold Concrete
Model” later in this chapter. The remainder of this present topic concerns the directional material model.
Nonlinear material behavior is currently not temperature-dependent. The behavior
specified at the initial (most negative) temperature is used for all material temperatures.

Tension and Compression
For each material you may specify an axial stress-strain curve that is used to represent the direct (tension-compression) stress-strain behavior of the material along
any material axis. For Uniaxial materials, this represents the relationship between
s 11 and e 11 . For Isotropic, Orthotropic, and Anisotropic materials, this curve represents the behavior along each of the three material axes, s 11 -e 11 , s 22 -e 22 , and
s 33 -e 33 . The nonlinear stress-strain behavior is the same in each direction, even
for Orthotropic, and Anisotropic materials.
Tension is always positive, regardless of the type of material (steel, concrete, etc.)
The tensile and compressive sides of the stress-strain behavior may be different
from each other. For what follows, the direct stress-strain curve may be written as
follows:
ìs (e ), e ii ³ 0
s ii (e ii ) = í T ii
îs C (e ii ), e ii £ 0

(Eqn. 5a)

where s T (e ) represents tensile behavior, and s C (e ) represents compressive behavior, subject to the restrictions:
s T (e ) ³ 0, s T (0) = 0
s C (e ) £ 0, s C (0) = 0

(Eqn. 5b)

Shear
A shear stress-strain curve is computed internally from the direct stress-strain
curve. The assumption is made that shearing behavior can be computed from tensile and compressive behavior acting at 45° to the material axes using Mohr's circle
Nonlinear Material Behavior

CSI Analysis Reference Manual
in the plane. For an Isotropic, Orthotropic, or Anisotropic material, this results in
the following symmetrical relationship for shear:
ì s S (e ij ), e ij ³ 0
s ij (e ij ) = í
î -s S ( -e ij ), e ij £ 0

(Eqn. 6a)

where
s S (e ij ) = 14 (s T (e ij ) - s C ( -e ij )), e ij = 12 g ij ³ 0, i ¹ j

(Eqn. 6b)

For the case where the direct stress-strain curve is symmetrical, such as for steel, we
have s T (e ) = -s C ( -e ), and therefore:
ìs T (e ij ), e ij ³ 0
s ij (e ij ) = 12 í
îs C (e ij ), e ij £ 0
To create a material where the shearing relationship, s S (e ), is primary and known,
you can define a symmetrical direct stress-strain relationship such that:
s T (e ) = -s C ( -e ) = 2s S (e )
When shear stress is considered for a Uniaxial material, the stress is half that for an
Isotropic material. In this way, if you have two uniaxial materials at 90° to each
other, the shear behavior matches that of an Isotropic material. Thus for Uniaxial
materials:
ì s S (e ij ), e ij ³ 0
s ij (e ij ) = 12 í
(for Uniaxial material)
î -s S ( -e ij ), e ij £ 0

(Eqn. 6c)

Hysteresis
Several hysteresis models are available to define the nonlinear stress-strain behavior when load is reversed or cycled. For the most part, these models differ in the
amount of energy they dissipate in a given cycle of deformation, and how the energy dissipation behavior changes with an increasing amount of deformation.
Details are provided in Topic “Hysteresis Models" (page 85) in this chapter.

Nonlinear Material Behavior

Chapter VI

Material Properties

Application
Nonlinear stress-strain curves are currently used in the two applications described
in the following.
Fiber Hinges
Fiber hinges are used to define the coupled axial force and bi-axial bending behavior at locations along the length of a frame element. The hinges can be defined manually, or created automatically for certain types of frame sections, including Section-Designer sections.
For each fiber in the cross section at a fiber hinge, the material direct nonlinear
stress-strain curve is used to define the axial s 11 - e 11 relationship. Summing up the
behavior of all the fibers at a cross section and multiplying by the hinge length
gives the axial force-deformation and biaxial moment-rotation relationships.
The s 11 - e 11 is the same whether the material is Uniaxial, Isotropic, Orthotropic, or
Anisotropic. Shear behavior is not considered in the fibers. Instead, shear behavior
is computed for the frame section as usual using the linear shear modulus g12.
For more information:
• See Topic “Section Designer Sections” (page 134) in Chapter “The Frame Element.”
• See Chapter “Frame Hinge Properties” (page 147).
Layered Shell Element
The Shell element with the layered section property may consider linear, nonlinear,
or mixed material behavior. For each layer, you select a material, a material angle,
and whether each of the in-plane stress-strain relationships are linear, nonlinear, or
inactive (zero stress). These relationships include s 11 - e 11 , s 22 -e 22 , and s 12 -e 12 .
For Uniaxial materials, the stress s 22 = 0 always. However, shear stiffness is assumed to be present, but may be set to zero by setting the shear relationship to be inactive.
For all materials, the transverse normal stress s 33 = 0. The transverse shear behavior is always linear, using the appropriate shear moduli g13 and g23 from the material matrix (Eqns. 1–4 above.)

Nonlinear Material Behavior

CSI Analysis Reference Manual
If all three in-plane relationships for a given layer are linear, the corresponding linear matrix is used (Eqns. 1–4 above), adjusted for the plane-stress condition
s 33 = 0. Poisson effects are included, which may couple the two direct stresses.
If any of the in-plane relationships for a given layer are nonlinear or inactive, then
all three relationships become uncoupled according to these rules:
• Poisson’s ratio is taken to be zero.
• Linear direct stress-strain relationships use stiffness e1 from the material matrix (Eqns. 1-4).
• Linear shear stress-strain relationships use shear modulus g12 (Eqns. 1-4).
• Nonlinear direct stress-strain relationships use Eqns. 5 above.
• Nonlinear shear stress-strain relationships use Eqns. 6 above.
• Inactive stress-strain relationships assume that the corresponding stress is zero.
The stress-strain behavior for a given layer is always defined in the material coordinate system specified by the material angle for that layer. It is particularly important to keep this in mind when using Uniaxial materials, for which s 22 = 0.
The above description is for the directional material. In addition, a two-dimensional concrete model is available for use in the layered shell. This model is discussed in topic “Modified Darwin-Pecknold Concrete Model” later in this chapter.
For more information, see Subtopic “Layered Section Property” (page 193) in
Chapter “The Shell Element.”

Friction and Dilitational Angles
For concrete materials, you can specify a friction angle and a dilitational angle.
These should normally be set to zero. The friction angle is an experimental parameter, and is not recommended for normal use. The dilitational angle is a future parameter, and has no effect on the model.
The friction angle, f, takes values 0 £ f < 90°. For the recommended value of f = 0,
shear behavior is as described above. For experimental use with f > 0, the shear
stress is computed primarily using a frictional model having linear stiffness g12 up
to a limiting stress given by:
ì 0, s ³ 0
s 12 £ tan f í
î -s , s < 0

Nonlinear Material Behavior

(Eqn. 7a)

Chapter VI

Material Properties

where s = 12 (s 11 + s 22 ). Compression is required in order to develop any shear
strength by this equation. In addition, cohesion is added using (Eqn. 6a) above, but
considering only the contribution to shear due to tension:
s S (e 12 ) = 14 s T (e 12 ), e 12 = 12 g 12 ³ 0

(Eqn. 7b)

This behavior, while interesting, can present computational challenges unless the
model is well defined and reasonably loaded, with sufficient ductility provided using reinforcing steel. To repeat: This is an experimental behavior and is not recommended for normal use.

Hysteresis Models
Hysteresis is the process of energy dissipation through deformation (displacement), as opposed to viscosity which is energy dissipation through deformation
rate (velocity). Hysteresis is typical of solids, whereas viscosity is typical of fluids,
although this distinction is not rigid.
Hysteretic behavior may affect nonlinear static and nonlinear time-history load
cases that exhibit load reversals and cyclic loading. Monotonic loading is not affected.
Several different hysteresis models are available to describe the behavior of different types of materials. For the most part, these differ in the amount of energy they
dissipate in a given cycle of deformation, and how the energy dissipation behavior
changes with an increasing amount of deformation.
Each hysteresis model may be used for the following purposes:
• Material stress-strain behavior, affecting frame fiber hinges and layered shells
that use the material
• Single degree-of-freedom frame hinges, such as M3 or P hinges. Interacting
hinges, such as P-M3 or P-M2-M3, currently use the isotropic model
• Link/support elements of type multi-linear plasticity.
Although the present chapter concerns material properties, this discussion pertains
equally to all three of these applications.

Hysteresis Models

CSI Analysis Reference Manual

Backbone Curve (Action vs. Deformation)
For each material, hinge, or link degree of freedom, a unaxial action vs. deformation curve defines the nonlinear behavior under monotonic loading in the positive
and negative directions.
Here action and deformation are an energy conjugate pair as follows:
• For materials, stress vs. strain
• For hinges and multi-linear links, force vs. deformation or moment vs. rotation,
depending upon the degree of freedom to which it is applied
For each model, the uniaxial action-deformation curve is given by a set of points
that you define. This curve is called the backbone curve, and it can take on almost
any shape, with the following restrictions:
• One point must be the origin, (0,0)
• At least one point with positive deformation, and one point with negative deformation, must be defined
• The deformations of the specified points must increase monotonically, with no
two values being equal
• The action at each point must have the same sign as the deformation (they can
be zero)
• The slope given by the last two points specified on the positive deformation
axis is extrapolated to infinite positive deformation, or until it reaches zero
value. Similarly, the slope given by the last two points specified on the negative
deformation axis is extrapolated to infinite negative deformation, or until it
reaches zero value.
The given curve defines the action-deformation relationship under monotonic
loading. The first slope on either side of the origin is elastic; the remaining segments define plastic deformation. If the deformation reverses, it typically follows
the two elastic segments before beginning plastic deformation in the reverse direction, except as described below.

Cyclic Behavior
Several hysteresis models are available in SAP2000, ETABS, and CSiBridge. The
available models may vary from product to product, and may include any or all of
the models described below.

Hysteresis Models

Chapter VI

Material Properties

Figure 15
Elastic Hysteresis Model under Increasing Cyclic Load - No Energy Dissipation
Showing the Backbone Curve Used for All Hysteresis Figures
Typical for all models, cyclic loading behaves as follows:
• Initial loading in the positive or negative direction follows the backbone curve
• Upon reversal of deformation, unloading occurs along a different path, usually
steeper than the loading path. This is often parallel or nearly parallel to the initial elastic slope.
• After the load level is reduced to zero, continued reversal of deformation
causes reverse loading along a path that eventually joins the backbone curve on
the opposite side, usually at a deformation equal to the maximum previous deformation in that direction or the opposite direction.
In the descriptions below of cyclic deformation, “loading” refers to increasing the
magnitude of deformation in a given positive or negative direction, and “unloading” refers to subsequent reduction of the deformation until the force level reaches
zero. Continued reduction of the deformation is “reverse loading” until the deformation reaches zero, after which the deformation increases again with the same
sign as the load and is “loading” again. Loading and unloading occur in the positive
(first and third) quadrants of the action-deformation plot, and reverse loading occurs in the negative (second and fourth) quadrants.
Hysteresis Models

CSI Analysis Reference Manual

Figure 16
Kinematic Hysteresis Model under Increasing Cyclic Load

Elastic Hysteresis Model
The behavior is nonlinear but it is elastic. This means that the material always loads
and unloads along the backbone curve, and no energy is dissipated. This behavior is
illustrated in Figure 15 (page 87). This same backbone curve is used in the figures
for all subsequent models, except that the concrete model uses only the positive
portion of the curve, with the negative portion being defined separately.

Kinematic Hysteresis Model
This model is based upon kinematic hardening behavior that is commonly observed
in metals, and it is the default hysteresis model for all metal materials in the program. This model dissipates a significant amount of energy, and is appropriate for
ductile materials.
Under the rules of kinematic hardening, plastic deformation in one direction
“pulls” the curve for the other direction along with it. Matching pairs of points are
linked. No additional parameters are required for this model.

Hysteresis Models

Chapter VI

Material Properties

Upon unloading and reverse loading, the curve follows a path made of segments
parallel to and of the same length as the previously loaded segments and their opposite-direction counterparts until it rejoins the backbone curve when loading in the
opposite direction. This behavior is shown in Figure 16 (page 88) for cycles of increasing deformation.
When you define the points on the multi-linear curve, you should be aware that
symmetrical pairs of points will be linked, even if the curve is not symmetrical.
This gives you some control over the shape of the hysteretic loop.
The kinematic model forms the basis for several of the other model described below, including Takeda, degrading, and BRB hardening.

Degrading Hysteresis Model
This model is very similar to the Kinematic model, but uses a degrading hysteretic
loop that accounts for decreasing energy dissipation and unloading stiffness with
increasing plastic deformation.
Two measures are used for plastic deformation:
• Maximum plastic deformation in each the positive and negative directions
• Accumulated plastic deformation, which is the absolute sum of each increment
of positive or negative plastic deformation. Plastic deformation is that which
does not occur on the two elastic segments of the action-deformation curve
Accumulated plastic deformation can occur under cyclic loading of constant amplitude, and can be used to represent fatigue.
For this model, the following parameters are required:
• Separately for positive and negative deformations
– Initial energy factor at yield, f0, usually 1.0
– Energy factor at moderate deformation, f1
– Energy factor at maximum deformation, f2
– Moderate deformation level, x1, as a multiple of the yield deformation
– Maximum deformation level, x2, as a multiple of the yield deformation
– Accumulated deformation weighting factor, a
• Stiffness degradation weighting factor, s
• Larger-smaller weighting factor, w, usually 0.0

Hysteresis Models

CSI Analysis Reference Manual

Figure 17
Degrading Hysteresis Model under Increasing Cyclic Load
Exhibiting Elastic Degradation (s = 0.0)
The energy factors represent the area of a degraded hysteresis loop divided by the
energy of the non-degraded loop, such as for the kinematic model. For example, an
energy factor of 0.3 means that a full cycle of deformation would only dissipate
30% of the energy that the non-degraded material would. The energy factors must
satisfy 1.0 ³ f0 ³ f1 ³ f2 > 0.0. The deformation levels must satisfy 1.0 < x1 < x2.
All weighting factors may take any value from 0.0 to 1.0, inclusive. Because the accumulated plastic deformation is constantly increasing, it is recommended that the
weighting factor a generally be small or zero.
For each increment of deformation:
• The absolute maximum positive and negative plastic deformations that have
occurred up to this point in the analysis are determined, d max pos and d max neg ,
as well as the accumulated plastic deformation, d acc .
• A positive plastic deformation level is calculated as
d pos = ad acc + (1 - a )d max pos
where a is the accumulated weighting factor for positive deformation.

Hysteresis Models

Chapter VI

Material Properties

Figure 18
Degrading Hysteresis Model under Increasing Cyclic Load
Exhibiting Stiffness Degradation (s = 1.0)
• Comparing d pos with the positive deformation levels d1 and d2, obtained by
multiplying x1 and x2 with the positive yield deformation, an energy factor
f pos can be determined by interpolation. If d pos > d2, then f pos = f2.
• Following the same approach, the energy factor for negative deformation,
f neg , is computed using the corresponding parameters for negative deformation.
• The larger of these two energy factor is called f max , and the smaller is f min .
The final energy factor is computed as
f = wf max + (1 - w) f min
In the most common case, w = 0 and f = f min .
Degradation does not occur during monotonic loading. However, upon load reversal, the curve for unloading and reverse loading is modified according to the energy
factor computed for the last deformation increment. This is done by squeezing, or
flattening, the curve toward the diagonal line that connects the two points of maximum positive and negative deformation.

Hysteresis Models

CSI Analysis Reference Manual

Figure 19
Degrading Hysteresis Model under Increasing Cyclic Load
Exhibiting Combined Degradation (s = 0.5)
This squeezing is scaled to achieve the desired decrease in energy dissipation. The
scaling can occur in two directions:
• Parallel to the elastic unloading line, called elastic degradation
• Parallel to the horizontal axis, called stiffness degradation
The amount of scaling in each direction is controlled by the stiffness degradation
weighting parameter, s. For s = 0.0, all degradation is of elastic type. For s = 1.0, all
degradation is of stiffness type. For intermediate values, the degradation is apportioned accordingly.
While the deformation and individual energy levels are computed separately for the
positive and negative directions, the final energy level is a single parameter that affects the shape of the hysteresis loop in both directions.
Note that if all the energy factors are equal to 1.0, this model degenerates to the kinematic hysteresis model.
Figures 17, 18, and 19 (pages 90-92) show the shape of the hysteresis loop for elastic degradation, stiffness degradation, and a mixture with a stiffness degradation

Hysteresis Models

Chapter VI

Material Properties

Figure 20
Takeda Hysteresis Model under Increasing Cyclic Load
factor of s = 0.5. Each of these three cases dissipates the same amount of energy for
a given cycle of loading, and less than the energy dissipated for the equivalent kinematic model shown in Figure 16 (page 88).

Takeda Hysteresis Model
This model is very similar to the kinematic model, but uses a degrading hysteretic
loop based on the Takeda model, as described in Takeda, Sozen, and Nielsen
(1970). This simple model requires no additional parameters, and is more appropriate for reinforced concrete than for metals. Less energy is dissipated than for the kinematic model.
Unloading is along the elastic segments similar to the kinematic model. When reloading, the curve follows a secant line to the backbone curve for loading in the opposite direction. The target point for this secant is at the maximum deformation that
occurred in that direction under previous load cycles. This results in a decreasing
amount of energy dissipation with larger deformations. Unloading is along the
elastic segments.
This behavior is illustrated in Figure 20 (page 93).
Hysteresis Models

CSI Analysis Reference Manual

Figure 21
Pivot Hysteresis Model under Increasing Cyclic Load

Pivot Hysteresis Model
This model is similar to the Takeda model, but has additional parameters to control
the degrading hysteretic loop. It is particularly well suited for reinforced concrete
members, and is based on the observation that unloading and reverse loading tend
to be directed toward specific points, called pivots points, in the action-deformation
plane. The most common use of this model is for moment-rotation. This model is
fully described in Dowell, Seible, and Wilson (1998). This model is not intended
for unreinforced concrete. See the separate concrete model below.
The following additional parameters are specified for the Pivot model:
• a 1 , which locates the pivot point for unloading to zero from positive force. Unloading occurs toward a point on the extension of the positive elastic line, but at
a negative force value of a 1 times the positive yield force.
• a 2 , which locates the pivot point for unloading to zero from negative force.
Unloading occurs toward a point on the extension of the negative elastic line,
but at a positive force value of a 2 times the negative yield force.
• b1 , which locates the pivot point for reverse loading from zero toward positive
force. Reloading occurs toward a point on the positive elastic line at a force

Hysteresis Models

Chapter VI

Material Properties

Figure 22
Pivot Hysteresis Model Parameters

value of b1 times the positive yield force, where 0.0 < b1 £ 1.0. Beyond that
point, loading occurs along the secant to the point of maximum previous positive deformation on the backbone curve.
• b 2 , which locates the pivot point for reverse loading from zero toward negative
force. Reloading occurs toward a point on the negative elastic line at a force
value of b 2 times the negative yield force, where 0.0 < b 2 £ 1.0. Beyond that
point, loading occurs along the secant to the point of maximum previous negative deformation on the backbone curve.
• h, which determines the amount of degradation of the elastic slopes after plastic
deformation, where 0.0 < h £ 1.0
These parameters and the behavior are illustrated in Figures 21 and 22 (pages 94
and 95).

Concrete Hysteresis Model
This model is intended for unreinforced concrete and similar materials, and is the
default model for concrete and masonry materials in the program. Tension and

Hysteresis Models

CSI Analysis Reference Manual

Figure 23
Concrete Hysteresis Model under Increasing Cyclic Load
with Compression as Positive and Energy Factor f = 0.7
compression behavior are independent and behave differently. The force-deformation (stress-strain) curve is used to determine the sign of compression, which can be
positive or negative. The point having the largest absolute value of stress or force is
considered to be in compression, so that the sign of compression can be either positive or negative. Likewise, the concrete model can also be used to represent a tension-only material whose behavior is similar to concrete in compression.
This model is primarily intended for axial behavior, but can be applied to any degree of freedom. Reinforced concrete is better modeled using the pivot, degrading,
or Takeda models.
A non-zero force-deformation curve should always be defined for compression.
The force-deformation curve for tension may be all zero, or it may be non-zero provided that the maximum force value is of smaller magnitude than that for the compression side.
A single parameter, the energy degradation factor f, is specified for this model. This
value should satisfy 0.0 £ f £ 1.0. A value of f = 0.0 is equivalent to a clean gap
when unloading from compression and dissipates the least amount of energy. A

Hysteresis Models

Chapter VI

Material Properties

value of f = 1.0 is dissipates the most energy and could be caused by rubble filling
the gap when unloading from compression.
Compression behavior is modeled as follows:
• Initial loading is along the backbone curve
• Unloading to zero occurs along a line nearly parallel to the compression elastic
line. The line is actually directed to a pivot point on the extension of the compressive elastic line, located so that the unloading slope at maximum compressive force has half the stiffness of the elastic loading line.
• At zero force, reverse loading toward tension occurs at zero force.
• Subsequent loading in compression occurs along the previous unloading line if
the energy factor f = 0.0, and along the secant from the origin to the point of
maximum previous compressive deformation if the energy factor is 1.0. An intermediate secant from the horizontal axis is used for other values of f.
Tension behavior, if non-zero, is modeled as follows:
• Initial loading is along the backbone curve
• Unloading occurs along a secant line to the origin.
• Subsequent loading occurs along the unloading secant from the origin to the
point of maximum previous tensile deformation.
See Figure 23 (page 96) for an example of this behavior for an energy degradation
factor of f = 0.7.

BRB Hardening Hysteresis Model
This model is similar to the kinematic model, but accounts for the increasing
strength with plastic deformation that is typical of bucking-restrained braces, causing the backbone curve, and hence the hysteresis loop, to progressively grow in
size. It is intended primarily for use with axial behavior, but can be applied to any
degree of freedom.
Two measures are used for plastic deformation:
• Maximum plastic deformation in each the positive and negative directions
• Accumulated plastic deformation, which is the absolute sum of each increment
of positive or negative plastic deformation. Plastic deformation is that which
does not occur on the two elastic segment of the force-deformation curve

Hysteresis Models

CSI Analysis Reference Manual

Figure 24
BRB Hardening Hysteresis Model under Increasing Cyclic Load
with Hardening Factor h = 1.5
Accumulated plastic deformation can occur under cyclic loading of constant amplitude.
For this model, the following parameters are required:
• Separately for tension (positive) and compression (negative) deformations
– Hardening factor at maximum deformation, h, where h ³ 1.0.
– Maximum plastic deformation level at full hardening, x2, as a multiple of
yield deformation, where x2 > 1.0
– Maximum accumulated plastic deformation level at full hardening, x4, as a
multiple of yield deformation, where x4 > 1.0
– Accumulated deformation weighting factor, a, where 0.0 £ a £ 1.0.
The hardening factors scale the size of the backbone curve and hysteresis loop in
the action (stress/force/moment) direction. Because the accumulated plastic deformation is constantly increasing, it is recommended that the weighting factor a generally be small or zero.
For each increment of deformation:

Hysteresis Models

Chapter VI

Material Properties

• The absolute maximum positive and negative plastic deformations that have
occurred up to this point in the analysis are determined, d max pos and d max neg ,
as well as the accumulated plastic deformation, d acc .
• Comparing d max pos with the positive deformation level d2, obtained by multiplying x2 by the positive yield deformation, a hardening factor h max pos can be
determined by interpolation. If d max pos > d2, then h max pos = h.
• Comparing d acc with the positive deformation level d4, obtained by multiplying x4 by the positive yield deformation, a hardening factor h acc pos can be determined by interpolation. If d acc > d4, then h acc pos = h
• The net hardening factor due to positive deformation, h pos , is computed as
h pos = ah acc pos + (1 - a )h max pos
• Following the same approach, the hardening factor due to negative deformation, h neg , is computed using the corresponding parameters for negative deformation.
Degradation does not occur during monotonic loading. However, upon load reversal, the curve for unloading and reverse loading in the opposite direction is modified according to the hardening factor computed for the last deformation increment.
This is done by scaling the action values in that direction, including the backbone
curve for further loading.
Important! Positive deformation and the corresponding hardening parameters only
affect the negative strength, and vice versa.
Note that if the hardening factor is equal to 1.0, this model degenerates to the kinematic hysteresis model.
This behavior is illustrated in Figure 24 (page 98).

Isotropic Hysteresis Model
This model is, in a sense, the opposite of the kinematic model. Plastic deformation
in one direction “pushes” the curve for the other direction away from it, so that both
directions increase in strength simultaneously. Unlike the BRB hardening model,
the backbone curve itself does not increase in strength, only the unloading and reverse loading behavior. Matching pairs of points are linked. No additional parameters are required for this model.
Unloading and reverse loading occur along a path parallel to the elastic line until
the magnitude of the action in the reverse direction equals that of backbone curve at

Hysteresis Models

CSI Analysis Reference Manual

Figure 25
Isotropic Hysteresis Model under Increasing Cyclic Load

the same amount of deformation in the reverse direction, and then continues along a
horizontal secant to the backbone curve.
When you define the points on the multi-linear curve, you should be aware that
symmetrical pairs of points will be linked, even if the curve is not symmetrical.
This gives you some control over the shape of the hysteretic loop.
This model dissipates the most energy of all the models. This behavior is illustrated
in Figure 25 (page 100).

Modified Darwin-Pecknold Concrete Model
A two-dimensional nonlinear concrete material model is available for use in the
layered shell. This model is based on the Darwin-Pecknold model, with consideration of Vecchio-Collins behavior. This model represents the concrete compression, cracking, and shear behavior under both monotonic and cyclic loading, and
considers the stress-strain components s 11 -e 11 , s 22 -e 22 , and s 33 -e 33 . A state of
plane stress is assumed.

100

Modified Darwin-Pecknold Concrete Model

Chapter VI

Material Properties

The direction of cracking can change during the loading history, and the shear
strength is affected by the tension strain in the material. The axial stress-strain
stress-strain curve specified for the material is simplified to account for initial stiffness, yielding, ultimate plateau, and strength loss due to crushing. Zero tensile
strength is assumed.
Hysteresis is governed by the concrete hysteresis model described in the previous
topic, with the energy dissipation factor f = 0.
The layered shell allows this material to be used for membrane and/or flexural behavior and to be combined with steel reinforcement placed in arbitrary directions
and locations. Transverse (out-of-plane) shear is assumed to be elastic and isotropic
using the shear stiffness G13 for both s 13 -g 13 and s 23 -g 23 behavior.
See separate Technical Note “Modified Darwin-Pecknold 2-D Reinforced Concrete Material Model” for more information, available using the command Help >
Documentation.

Time-dependent Properties
For any material having a design type of concrete or tendon, you may specify time
dependent material properties that are used for creep, shrinkage, and aging effects
during a staged-construction analysis.
For more information, see Topic “Staged Construction” (page 439) in Chapter
“Nonlinear Static Analysis.”

Properties
For concrete-type materials, you may specify:
• Aging parameters that determine the change in modulus of elasticity with age
• Shrinkage parameters that determine the decrease in direct strains with time
• Creep parameters that determine the change in strain with time under the action
of stress
For tendon-type materials, relaxation behavior may be specified that determines
the change in strain with time under the action of stress, similar to creep.
Currently these behaviors can be specified for the CEB-FIP 1990 code (Comite
Euro-International Du Beton, 1993) for concrete and tendon materials, and for con-

Time-dependent Properties

101

CSI Analysis Reference Manual
crete materials using the following codes: CEB-FIP 2010, ACI 290R-92, and
user-specified curves.

Time-Integration Control
For each material, you have the option to model the creep behavior by full integration or by using a Dirichlet series approximation.
With full integration, each increment of stress during the analysis becomes part of
the memory of the material. This leads to accurate results, but for long analyses
with many stress increments, this requires computer storage and execution time
that both increase as the square of the number of increments. For larger problems,
this can make solution impractical.
Using the Dirichlet series approximation (Ketchum, 1986), you can choose a fixed
number of series terms that are to be stored. Each term is modified by the stress increments, but the number of terms does not change during the analysis. This means
the storage and execution time increase linearly with the number of stress increments. Each term in the Dirichlet series can be thought of as a spring and dashpot
system with a characteristic relaxation time. The program automatically chooses
these spring-dashpot systems based on the number of terms you request. You
should try different numbers of terms and check the analysis results to make sure
that your choice is adequate.
It is recommended that you work with a smaller problem that is representative of
your larger model, and compare various numbers of series terms with the full integration solution to determine the appropriate series approximation to use.

Design-Type
You may specify a design-type for each Material that indicates how it is to be
treated for design by the SAP2000, ETABS, SAFE, or CSiBridge graphical user interface. The available design types are:
• Steel: Frame elements made of this material will be designed according to steel
design codes
• Concrete: Frame elements made of this material will be designed according to
concrete design codes
• Aluminum: Frame elements made of this material will be designed according
to aluminum design codes

102

Design-Type

Chapter VI

Material Properties

• Cold-formed: Frame elements made of this material will be designed according
to cold-formed steel design codes
• None: Frame elements made of this material will not be designed
When you choose a design type, additional material properties may be specified
that are used only for design; they do not affect the analysis. Consult the on-line
help and design documentation for further information on these design properties.

Design-Type

103

CSI Analysis Reference Manual

104

Design-Type

C h a p t e r VII

The Frame Element
The Frame element is a very powerful element that can be used to model beams,
columns, braces, and trusses in planar and three-dimensional structures. Nonlinear
material behavior is available through the use of Frame Hinges.
Basic Topics for All Users
• Overview
• Joint Connectivity
• Degrees of Freedom
• Local Coordinate System
• Section Properties
• Insertion Point
• End Offsets
• End Releases
• Mass
• Self-Weight Load
• Concentrated Span Load
• Distributed Span Load

105

CSI Analysis Reference Manual
• Internal Force Output
• Stress Output
Advanced Topics
• Advanced Local Coordinate System
• Property Modifiers
• Nonlinear Properties
• Gravity Load
• Temperature Load
• Strain and Deformation Load
• Target-Force Load

Overview
The Frame element uses a general, three-dimensional, beam-column formulation
which includes the effects of biaxial bending, torsion, axial deformation, and biaxial shear deformations. See Bathe and Wilson (1976).
Structures that can be modeled with this element include:
• Three-dimensional frames
• Three-dimensional trusses
• Planar frames
• Planar grillages
• Planar trusses
• Cables
A Frame element is modeled as a straight line connecting two points. In the graphical user interface, you can divide curved objects into multiple straight objects, subject to your specification.
Each element has its own local coordinate system for defining section properties
and loads, and for interpreting output.
The element may be prismatic or non-prismatic. The non-prismatic formulation allows the element length to be divided into any number of segments over which
properties may vary. The variation of the bending stiffness may be linear, para-

106

Overview

Chapter VII

The Frame Element

bolic, or cubic over each segment of length. The axial, shear, torsional, mass, and
weight properties all vary linearly over each segment.
Insertion points and end offsets are available to account for the finite size of beam
and column intersections. The end offsets may be made partially or fully rigid to
model the stiffening effect that can occur when the ends of an element are embedded in beam and column intersections. End releases are also available to model different fixity conditions at the ends of the element.
Each Frame element may be loaded by gravity (in any direction), multiple concentrated loads, multiple distributed loads, strain and deformation loads, and loads due
to temperature change.
Target-force loading is available that iteratively applies deformation load to the element to achieve a desired axial force.
Element internal forces are produced at the ends of each element and at a userspecified number of equally-spaced output stations along the length of the element.
Cable behavior is usually best modeled using the catenary Cable element (page
165). However, there are certain cases where using Frame elements is necessary.
This can be achieved by adding appropriate features to a Frame element. You can
release the moments at the ends of the elements, although we recommend that you
retain small, realistic bending stiffness instead. You can also add nonlinear behavior as needed, such as the no-compression property, tension stiffening (p-delta effects), and large deflections. These features require nonlinear analysis.

Joint Connectivity
A Frame element is represented by a straight line connecting two joints, I and j, unless modified by insertion points as described below. The two joints must not share
the same location in space. The two ends of the element are denoted End I and End
J, respectively.

Insertion Points
Sometimes the neutral axis of the element cannot be conveniently located by joints
that connect to other elements in the structure. You have the option to specify insertion points that locate the element with respect to the joints. The insertion
points consists of a cardinal point specified for the section, plus independent joint
offsets specified at each end of the element. By default the cardinal point is the centroid of the section and the joints offsets are zero.
Joint Connectivity

107

CSI Analysis Reference Manual
The two ends of the neutral axis, considering the coordinates of joints I and j plus
the insertion points, must not be coincident. It is generally recommended that the
offsets due to the insertion points be perpendicular to the axis of the element, although this is not required.
For more information on the insertion points, including how they affect the local
coordinate system of the element, see Topic “Insertion Points” (page 125).

Degrees of Freedom
The Frame element activates all six degrees of freedom at both of its connected
joints. If you want to model truss or cable elements that do not transmit moments at
the ends, you may either:
• Set the geometric Section properties j, i33, and i22 all to zero (a is non-zero;
as2 and as3 are arbitrary), or
• Release both bending rotations, R2 and R3, at both ends and release the torsional rotation, R1, at either end
In either case, the joint offsets and the end offsets must both be zero to avoid moments at the ends.
For more information:
• See Topic “Degrees of Freedom” (page 30) in Chapter “Joints and Degrees of
Freedom.”
• See Topic “Section Properties” (page 114) in this Chapter.
• See Topic “End Offsets” (page 127) in this Chapter.
• See Topic “End Releases” (page 131) in this Chapter.

Local Coordinate System
Each Frame element has its own element local coordinate system used to define
section properties, loads and output. The axes of this local system are denoted 1, 2
and 3. The first axis is directed along the length of the element at its centroid; the remaining two axes lie in the plane perpendicular to the element with an orientation
that you specify.
It is important that you clearly understand the definition of the element local 1-2-3
coordinate system and its relationship to the global X-Y-Z coordinate system. Both

108

Degrees of Freedom

Chapter VII

The Frame Element

systems are right-handed coordinate systems. It is up to you to define local systems
which simplify data input and interpretation of results.
In most structures the definition of the element local coordinate system is extremely simple. The methods provided, however, provide sufficient power and
flexibility to describe the orientation of Frame elements in the most complicated
situations.
Local axes are first computed for the element without considering the insertion
points, i.e., as if the neutral axis connects the two joints. These are called the nominal local axes. If the insertion points shift the neutral axis by a different amount at
the two ends, the local axes are then transformed by projecting them onto the neutral axis to determine the actual local coordinate system used for analysis.
The discussion below considers the calculation of the nominal local axes using the
joints. The transformation for the insertion points, if needed, is discussed later in
Topic “Insertion Points”.
The simplest method for computing the element local coordinate system, using the
default orientation and the Frame element coordinate angle, is described in this
topic. Additional methods for defining the Frame element local coordinate system
are described in the next topic.
For more information:
• See Chapter “Coordinate Systems” (page 11) for a description of the concepts
and terminology used in this topic.
• See Topic “Advanced Local Coordinate System” (page 110) in this Chapter.
• See Topic “Insertion Points” (page 125) in this Chapter.

Longitudinal Axis 1
The local axis 1 is always the longitudinal axis of the element, the positive direction
being directed from End I to End J. This axis is always located at the centroid of the
cross section, and connects joint I to joint j.

Default Orientation
The default orientation of the local 2 and 3 axes is determined by the relationship
between the local 1 axis and the global Z axis. The local 1 axis is directed along the
line between the joints I and j without considering any offsets:
• The local 1-2 plane is taken to be vertical, i.e., parallel to the Z axis
Local Coordinate System

109

CSI Analysis Reference Manual
• The local 2 axis is taken to have an upward (+Z) sense unless the element is vertical, in which case the local 2 axis is taken to be horizontal along the global +X
direction
• The local 3 axis is horizontal, i.e., it lies in the X-Y plane
An element is considered to be vertical if the sine of the angle between the local 1
axis and the Z axis is less than 10-3.
The local 2 axis makes the same angle with the vertical axis as the local 1 axis
makes with the horizontal plane. This means that the local 2 axis points vertically
upward for horizontal elements.

Coordinate Angle
The Frame element coordinate angle, ang, is used to define element orientations
that are different from the default orientation. It is the angle through which the local
2 and 3 axes are rotated about the positive local 1 axis from the default orientation.
The rotation for a positive value of ang appears counterclockwise when the local
+1 axis is pointing toward you.
For vertical elements, ang is the angle between the local 2 axis and the horizontal
+X axis. Otherwise, ang is the angle between the local 2 axis and the vertical plane
containing the local 1 axis. See Figure 26 (page 111) for examples.

Advanced Local Coordinate System
By default, the element local coordinate system is defined using the element coordinate angle measured with respect to the global +Z and +X directions, as described
in the previous topic. In certain modeling situations it may be useful to have more
control over the specification of the local coordinate system.
This topic describes how to define the orientation of the transverse local 2 and 3
axes with respect to an arbitrary reference vector when the element coordinate angle, ang, is zero. If ang is different from zero, it is the angle through which the local
2 and 3 axes are rotated about the positive local 1 axis from the orientation determined by the reference vector. The local 1 axis is always directed from end I to end
J of the element.
The discussion below considers the calculation of the nominal local axes using the
joints. The transformation for the insertion points, if needed, is discussed later in
Topic “Insertion Points”.

110

Advanced Local Coordinate System

Chapter VII
Z

The Frame Element
Z
1

ang=90°

j
ang=30° 2

i
1

3
Y

Local 1 Axis is Parallel to +Y Axis
Local 2 Axis is Rotated 90° from Z-1 Plane

X
Local 1 Axis is Not Parallel to X, Y, or Z Axes
Local 2 Axis is Rotated 30° from Z-1 Plane

Z
3

1
j

ang=30°

2
ang=90°
Local 1 Axis is Parallel to +Z Axis
Local 2 Axis is Rotated 90° from X-1 Plane

1
Local 1 Axis is Parallel to –Z Axis
Local 2 Axis is Rotated 30° from X-1 Plane

Figure 26
The Frame Element Coordinate Angle with Respect to the Default Orientation

For more information:
• See Chapter “Coordinate Systems” (page 11) for a description of the concepts
and terminology used in this topic.

Advanced Local Coordinate System

111

CSI Analysis Reference Manual
• See Topic “Local Coordinate System” (page 108) in this Chapter.
• See Topic “Insertion Points” (page 125) in this Chapter.

Reference Vector
To define the transverse local axes 2 and 3, you specify a reference vector that is
parallel to the desired 1-2 or 1-3 plane. The reference vector must have a positive
projection upon the corresponding transverse local axis (2 or 3, respectively). This
means that the positive direction of the reference vector must make an angle of less
than 90° with the positive direction of the desired transverse axis.
To define the reference vector, you must first specify or use the default values for:
• A primary coordinate direction pldirp (the default is +Z)
• A secondary coordinate direction pldirs (the default is +X). Directions pldirs
and pldirp should not be parallel to each other unless you are sure that they are
not parallel to local axis 1
• A fixed coordinate system csys (the default is zero, indicating the global coordinate system)
• The local plane, local, to be determined by the reference vector (the default is
12, indicating plane 1-2)
You may optionally specify:
• A pair of joints, plveca and plvecb (the default for each is zero, indicating the
center of the element). If both are zero, this option is not used
For each element, the reference vector is determined as follows:
1. A vector is found from joint plveca to joint plvecb. If this vector is of finite
length and is not parallel to local axis 1, it is used as the reference vector V p
2. Otherwise, the primary coordinate direction pldirp is evaluated at the center of
the element in fixed coordinate system csys. If this direction is not parallel to
local axis 1, it is used as the reference vector V p
3. Otherwise, the secondary coordinate direction pldirs is evaluated at the center
of the element in fixed coordinate system csys. If this direction is not parallel to
local axis 1, it is used as the reference vector V p
4. Otherwise, the method fails and the analysis terminates. This will never happen
if pldirp is not parallel to pldirs

112

Advanced Local Coordinate System

Chapter VII

ang=90°

The Frame Element

Y
pldirp = +Y
pldirs = –X
local = 12

1
j

1
Z

ang=90°

X
3

2
Local 1 Axis is Not Parallel to pldirp (+Y)
Local 2 Axis is Rotated 90° from Y-1 Plane

Local 1 Axis is Parallel to pldirp (+Y)
Local 2 Axis is Rotated 90° from X-1 Plane

Figure 27
The Frame Element Coordinate Angle with Respect to Coordinate Directions

A vector is considered to be parallel to local axis 1 if the sine of the angle between
them is less than 10-3.
The use of the Frame element coordinate angle in conjunction with coordinate directions that define the reference vector is illustrated in Figure 27 (page 113). The
use of joints to define the reference vector is shown in Figure 28 (page 114).

Determining Transverse Axes 2 and 3
The program uses vector cross products to determine the transverse axes 2 and 3
once the reference vector has been specified. The three axes are represented by the
three unit vectors V1 , V2 and V3 , respectively. The vectors satisfy the cross-product
relationship:
V1 = V2 ´ V3
The transverse axes 2 and 3 are defined as follows:
• If the reference vector is parallel to the 1-2 plane, then:
V3 = V1 ´ V p and
V2 = V3 ´ V1
Advanced Local Coordinate System

113

CSI Analysis Reference Manual
The following two specifications are equivalent:
(a) local=12, plveca=0, plvecb=100
(b) local=13, plveca=101, plvecb=102

Plane 1-2

Vp (a)
Axis 1

100

Axis 2
Joint j
Z
Vp (b)
102

Joint i
101

Plane 1-3
Axis 3

Figure 28
Using Joints to Define the Frame Element Local Coordinate System

• If the reference vector is parallel to the 1-3 plane, then:
V2 = V p ´ V1 and
V3 = V1 ´ V2
In the common case where the reference vector is perpendicular to axis V1 , the
transverse axis in the selected plane will be equal to V p .

Section Properties
A Frame Section is a set of material and geometric properties that describe the
cross-section of one or more Frame elements. Sections are defined independently
of the Frame elements, and are assigned to the elements.
Section properties are of two basic types:
• Prismatic — all properties are constant along the full element length
• Non-prismatic — the properties may vary along the element length

114

Section Properties

Chapter VII

The Frame Element

Non-prismatic Sections are defined by referring to two or more previously defined
prismatic Sections.
All of the following subtopics, except the last, describe the definition of prismatic
Sections. The last subtopic, “Non-prismatic Sections”, describes how prismatic
Sections are used to define non-prismatic Sections.

Local Coordinate System
Section properties are defined with respect to the local coordinate system of a
Frame element as follows:
• The 1 direction is along the axis of the element. It is normal to the Section and
goes through the intersection of the two neutral axes of the Section.
• The 2 and 3 directions are parallel to the neutral axes of the Section. Usually the
2 direction is taken along the major dimension (depth) of the Section, and the 3
direction along its minor dimension (width), but this is not required.
See Topic “Local Coordinate System” (page 108) in this Chapter for more information.

Material Properties
The material properties for the Section are specified by reference to a previouslydefined Material. Isotropic material properties are used, even if the Material selected was defined as orthotropic or anisotropic. The material properties used by
the Section are:
• The modulus of elasticity, e1, for axial stiffness and bending stiffness
• The shear modulus, g12, for torsional stiffness and transverse shear stiffness
• The coefficient of thermal expansion, a1, for axial expansion and thermal
bending strain
• The mass density, m, for computing element mass
• The weight density, w, for computing Self-Weight and Gravity Loads
The material properties e1, g12, and a1 are all obtained at the material temperature
of each individual Frame element, and hence may not be unique for a given Section.
See Chapter “Material Properties” (page 69) for more information.

Section Properties

115

CSI Analysis Reference Manual

Geometric Properties and Section Stiffnesses
Six basic geometric properties are used, together with the material properties, to
generate the stiffnesses of the Section. These are:
• The cross-sectional area, a. The axial stiffness of the Section is given by a × e1;
• The moment of inertia, i33, about the 3 axis for bending in the 1-2 plane, and
the moment of inertia, i22, about the 2 axis for bending in the 1-3 plane. The
corresponding bending stiffnesses of the Section are given by i33 × e1 and
i22 × e1;
• The torsional constant, j. The torsional stiffness of the Section is given by
j × g12. Note that the torsional constant is not the same as the polar moment of
inertia, except for circular shapes. See Roark and Young (1975) or Cook and
Young (1985) for more information.
• The shear areas, as2 and as3, for transverse shear in the 1-2 and 1-3 planes, respectively. The corresponding transverse shear stiffnesses of the Section are
given by as2 × g12 and as3 × g12. Formulae for calculating the shear areas of
typical sections are given in Figure 29 (page 117).
Setting a, j, i33, or i22 to zero causes the corresponding section stiffness to be zero.
For example, a truss member can be modeled by setting j = i33 = i22 = 0, and a planar frame member in the 1-2 plane can be modeled by setting j = i22 = 0.
Setting as2 or as3 to zero causes the corresponding transverse shear deformation to
be zero. In effect, a zero shear area is interpreted as being infinite. The transverse
shear stiffness is ignored if the corresponding bending stiffness is zero.

Shape Type
For each Section, the six geometric properties (a, j, i33, i22, as2 and as3) may be
specified directly, computed from specified Section dimensions, or read from a
specified property database file. This is determined by the shape type, shape, specified by the user:
• If shape=GENERAL (general section), the six geometric properties must be
explicitly specified
• If shape=RECTANGLE, PIPE, BOX/TUBE, I/WIDE FLANGE, or one of
several others offered by the program, the six geometric properties are automatically calculated from specified Section dimensions as described in “Automatic Section Property Calculation” below, or obtained from a specified property database file. See “Section Property Database Files” below.

116

Section Properties

Chapter VII

Section

Description

Effective
Shear Area

Rectangular Section
Shear Forces parallel to the b or d
directions

The Frame Element

5/ bd
6

b
bf
tf

Wide Flange Section
Shear Forces parallel to flange

5/ t b
3 f f

Wide Flange Section
Shear Forces parallel to web

Thin Walled
Circular Tube Section
Shear Forces from any direction

r
t

yt
n
b(y)

X
n.a.

2td

General Section
Shear Forces parallel to
Y-direction
I x= moment of inertia of
section about X-X

Q(Y) =
y

n b(n) dn

0.9

Thin Walled
Rectangular Tube Section
Shear Forces parallel to
d-direction

y
b

(0.9 - 0.4 s) A
where
s = (r - t) / r
A = (2r - t) t

Solid Circular Section
Shear Forces from any direction

tw d

Ix
yt

2
Q (y)

y
b

b(y)

Figure 29
Shear Area Formulae

• If shape=SD SECTION (Section Designer Section), you can create your own
arbitrary Sections using the Section Designer utility within the program, and
Section Properties

117

CSI Analysis Reference Manual
the six geometric properties are automatically calculated. See “Section Designer Sections” below.
• If shape=NONPRISMATIC, the Section is interpolated along the length of the
element from previously defined Sections as described in “Nonprismatic Section” below.

Automatic Section Property Calculation
The six geometric Section properties can be automatically calculated from specified dimensions for the simple shapes shown in Figure 30 (page 119), and for others
offered by the program. The required dimensions for each shape are shown in the
figure.
Note that the dimension t3 is the depth of the Section in the 2 direction and contributes primarily to i33.

Section Property Database Files
Geometric Section properties may be obtained from one or more Section property
database files. Several database files are currently supplied with SAP2000,
ETABS, or CSiBridge that provide properties for different regions, codes, and
manufacturers. Their format and content may be different for each product. Additional property database files may created by the user or may be available from
other sources.
The geometric properties are stored in the length units specified when the database
file was created. These are automatically converted to the appropriate units when
used in a model. Different frame sections can be obtained from different database
files for the same model.

Section-Designer Sections
Section Designer is a separate utility built into SAP2000, ETABS, and CSiBridge
that can be used to create your own frame section properties. You can build sections
of arbitrary geometry and combinations of materials. The basic analysis geometric
properties (areas, moments of inertia, and torsional constant) are computed and
used for analysis. In addition, Section Designer can compute nonlinear frame hinge
properties.
For more information, see the on-line help within Section Designer.

118

Section Properties

Chapter VII

The Frame Element
t2

tf
2

t3
tw

tw
tw

SH = R

SH = P

SH = B

t2t

tft
2

tw
tw
tfb

t2b

SH = I

SH = T

SH = C

t2
tf
2

2
3

tw
tf
t2

SH = L

dis

SH = 2L

Figure 30
Automatic Section Property Calculation

Section Properties

119

CSI Analysis Reference Manual

Additional Mass and Weight
You may specify mass and/or weight for a Section that acts in addition to the mass
and weight of the material. The additional mass and weight are specified per unit of
length using the parameters mpl and wpl, respectively. They could be used, for example, to represent the effects of nonstructural material that is attached to a Frame
element.
The additional mass and weight act regardless of the cross-sectional area of the
Section. The default values for mpl and wpl are zero for all shape types.

Non-prismatic Sections
Non-prismatic Sections may be defined for which the properties vary along the element length. You may specify that the element length be divided into any number
of segments; these do not need to be of equal length. Most common situations can
be modeled using from one to five segments.
The variation of the bending stiffnesses may be linear, parabolic, or cubic over each
segment of length. The axial, shear, torsional, mass, and weight properties all vary
linearly over each segment. Section properties may change discontinuously from
one segment to the next.
See Figure 31 (page 122) for examples of non-prismatic Sections.
Segment Lengths
The length of a non-prismatic segment may be specified as either a variable length,
vl, or an absolute length, l. The default is vl = 1.
When a non-prismatic Section is assigned to an element, the actual lengths of each
segment for that element are determined as follows:
• The clear length of the element, Lc , is first calculated as the total length minus
the end offsets:
Lc = L - ( ioff + joff )
See Topic “End Offsets” (page 127) in this Chapter for more information.
• If the sum of the absolute lengths of the segments exceeds the clear length, they
are scaled down proportionately so that the sum equals the clear length. Otherwise the absolute lengths are used as specified.
• The remaining length (the clear length minus the sum of the absolute lengths) is
divided among the segments having variable lengths in the same proportion as

120

Section Properties

Chapter VII

The Frame Element

the specified lengths. For example, for two segments with vl = 1 and vl = 2, one
third of the remaining length would go to the first segment, and two thirds to
the second segment.
Starting and Ending Sections
The properties for a segment are defined by specifying:
• The label, seci, of a previously defined prismatic Section that defines the properties at the start of the segment, i.e., at the end closest to joint I.
• The label, secj, of a previously defined prismatic Section that defines the properties at the end of the segment, i.e., at the end closest to joint j. The starting and
ending Sections may be the same if the properties are constant over the length
of the segment.
The Material would normally be the same for both the starting and ending Sections
and only the geometric properties would differ, but this is not required.
Variation of Properties
Non-prismatic Section properties are interpolated along the length of each segment
from the values at the two ends.
The variation of the bending stiffnesses, i33×e1 and i22×e1, are defined by specifying the parameters eivar33 and eivar22, respectively. Assign values of 1, 2, or 3 to
these parameters to indicate variation along the length that is linear, parabolic, or
cubic, respectively.
Specifically, the eivar33-th root of the bending stiffness in the 1-2 plane:
eivar33

i33 × e1

varies linearly along the length. This usually corresponds to a linear variation in
one of the Section dimensions. For example, referring to Figure 30 (page 119): a
linear variation in t2 for the rectangular shape would require eivar33=1, a linear
variation in t3 for the rectangular shape would require eivar33=3, and a linear
variation in t3 for the I-shape would require eivar33=2.
The interpolation of the bending stiffness in the 1-2 plane, i22 × e1, is defined in the
same manner by the parameter eivar22.
The remaining properties are assumed to vary linearly between the ends of each
segment:

Section Properties

121

CSI Analysis Reference Manual

Section B

Section A

Axis 2

End J

End I

l=24

vl=1

l=30

seci=B
secj=B

seci=A
secj=A

seci=B
secj=B

Steel Beam with Cover Plates at Ends
End J

l=50

seci=A
secj=B
eivar33=3

Section B

Section A

vl=1

End I

seci=A
secj=A

Axis 2

Concrete Column with Flare at Top

Figure 31
Examples of Non-prismatic Sections

• Stiffnesses: a × e1, j × g12, as2 × g12, and as3 × g12
• Mass: a×m + mpl

122

Section Properties

Chapter VII

The Frame Element

• Weight: a×w + wpl
If a shear area is zero at either end, it is taken to be zero along the full segment, thus
eliminating all shear deformation in the corresponding bending plane for that segment.
Advanced Location Parameters
Normally the full variation of a non-prismatic section occurs over the length of a
single frame object. When the object is auto-meshed into multiple frame elements,
each element will represent a portion of the full non-prismatic length.
Similarly, if you explicitly divide a non-prismatic frame object into multiple frame
objects, it is necessary to specify for each frame object what portion of the total
nonprismatic variation applies to each object. This is done by assigning to each object:
• The length of the total non-prismatic section. This will be the same for each object derived from a single parent frame object, and will be longer than each derived object.
• The relative location
For example, consider a single non-prismatic frame object of length 8 meters, divided into four equal-length objects. For each derived object, the assigned
non-prismatic length should be 8 meters and the relative starting locations should
be 0.0, 0.25, 0.5, and 0.75, respectively.
Effect upon End Offsets
Properties vary only along the clear length of the element. Section properties within
end offset ioff are constant using the starting Section of the first segment. Section
properties within end offset joff are constant using the ending Section of the last
segment.
See Topic “End Offsets” (page 127) in this Chapter for more information.

Property Modifiers
You may specify scale factors to modify the computed section properties. These
may be used, for example, to account for cracking of concrete or for other factors
not easily described in the geometry and material property values. Individual
modifiers are available for the following eight terms:
Property Modifiers

123

CSI Analysis Reference Manual
• The axial stiffness a × e1
• The shear stiffnesses as2 × g12 and as3 × g12
• The torsional stiffness j × g12
• The bending stiffnesses i33 × e1 and i22 × e1
• The section mass a×m + mpl
• The section weight a×w + wpl
You may specify multiplicative factors in two places:
• As part of the definition of the section property
• As an assignment to individual elements.
If modifiers are assigned to an element and also to the section property used by that
element, then both sets of factors multiply the section properties. Modifiers cannot
be assigned directly to a nonprismatic section property, but any modifiers applied
to the sections contributing to the nonprismatic section are used.
When performing steel frame design using the Direct Analysis Method of design
code AISC 360-05/IBC2006, further property modifiers may be computed by the
design algorithm for the axial and bending stiffnesses. In this case, the computed
modifiers are multiplied by those assigned to the element and those specified in the
section property used by that element, so that all three sets of factors apply.

Named Property Sets
In addition to directly assigning property modifiers to frame elements, you can apply them to a frame element in a staged-construction Load Case using a Named
Property Set of Frame Property Modifiers. A Named Property Set includes the
same eight factors above that can be assigned to an element.
When a Named Property Set is applied to an element in a particular stage of a Load
Case, it replaces only the values that are assigned to the element or that had been applied in a previous stage; values computed by the Direct Analysis Method of design
are also replaced. However, property modifiers specified with the section property
remain in force and are not affected by the application of a Named Property Set.
The net effect is to use the factors specified in the Named Property Set multiplied
by the factors specified in the section property.
When property modifiers are changed in a staged construction Load Case, they do
not change the response of the structure up to that stage, but only affect subsequent
response. In other words, the effect is incremental. For example, consider a cantile-

124

Property Modifiers

Chapter VII

The Frame Element

ver with only default (unity) property modifiers, and a staged construction case as
follows:
• Stage 1: Self-weight load is applied, resulting in a tip deflection of 1.0 and
a support moment of 1000.
• Stage 2: Named Property Set “A” is applied that multiplies all stiffnesses
by 2.0, and the mass and weight by 1.0. The tip deflection and support moment do not change.
• Stage 3: Self-weight load is applied again (incrementally). The resulting
tip deflection is 1.5 and the support moment is 2000. Compared to Stage 1,
the same incremental load is applied, but the structure is twice as stiff.
• Stage 4: Named Property Set “B” is applied that multiplies all stiffnesses,
as well as the mass and weight, by 2.0. The tip deflection and support moment do not change.
• Stage 5: Self-weight load is applied again (incrementally). The resulting
tip deflection is 2.5 and the support moment is 4000. Compared to Stage 1,
twice the incremental load is applied, and the structure is twice as stiff

Insertion Points
The local 1 axis of the element runs along the neutral axis of the section, i.e., at the
centroid of the section. By default this connects to the joints I and j at the ends of
the element. However, it is often convenient to specify another location on the section, such as the top of a beam or an outside corner of a column, to connect to the
joints.
There is a set of pre-defined locations within the section, called cardinal points,
that can be used for this purpose. The available choices are shown in Figure 32
(page 126). The default location is point 10, the centroid.
You can further offset the cardinal point from the joint by specifying joint offsets.
The joint offsets together with the cardinal point make up the insertion point assignment. The total offset from the joint to the centroid is given as the sum of the
joint offset plus the distance from the cardinal point to the centroid.
This feature is useful, as an example, for modeling beams and columns when the
beams do not frame into the center of the column. Figure 33 (page 128) shows an elevation and plan view of a common framing arrangement where the exterior beams
are offset from the column center lines to be flush with the exterior of the building.

Insertion Points

125

CSI Analysis Reference Manual
2 axis
7

5
10
11

1. Bottom left
2. Bottom center
3. Bottom right
4. Middle left
3 axis
5. Middle center
6. Middle right
7. Top left
8. Top center
9. Top right
10. Centroid
11. Shear center

Note: For doubly symmetric members such as
this one, cardinal points 5, 10, and 11 are
the same.

Figure 32
Frame Cardinal Points

Also shown in this figure are the cardinal points for each member and the joint offset dimensions.
Offsets along the neutral axis of the element are usually specified using end offsets
rather than insertion points. See topic “End Offsets” (page 127). End offsets are
treated as part of the length of the element, have element properties and loads, and
may or may not be rigid.
Offsets due to insertion points are external to the element and do not have any mass
or loads. Internally the analysis represents the insertion point by a fully rigid constraint that connects the neutral axis to the joints.

Local Axes
The insertion points can interact significantly with the element local coordinate
system. As described previously, the nominal local axes are computed for the default insertion points, such that the local 1 axis connects joints I and j.
The centroids of the section are then located using both the cardinal point and joint
offsets. Joint offsets may be specified using the global coordinate system or the element local system. In the latter case, the nominal local axes are used for this purpose.

126

Insertion Points

Chapter VII

The Frame Element

If the neutral axis of the frame section remains parallel to the nominal local 1 axis
(the line connecting the two joints), then no further transformation is needed. The
element local axes are the same as the nominal axes.
If the neutral axis has changed direction, then the element local coordinate system
is computed as follows:
~
~
V3 = V1 ´ V2 and
~
~
~
V2 = V3 ´ V1
where V1 , V2 , and V3 and the nominal local axes computed previously based on the
~ ~
~
joints; and V1 , V2 , and V3 are the transformed local axes used for analysis. If V2 is
~
vertical, then V3 will always be horizontal. Note that the two systems are identical
~
if V1 = V1 , the usual case.
The nominal axes are used only for determining the direction of joint offsets. The
transformed axes are used for all analysis and design purposes, including loading
and results output.
For non-prismatic elements with non-centroidal cardinal points, the local 1 axis
may not be straight, and as a consequence the local 2 and 3 axes may change orientation between segments. This can be expected to cause jumps in the axial force,
shear, and moments. However, the change will be a small deviation from the axes
that would have been calculated for an element with no insertion points.

End Offsets
Frame elements are modeled as line elements connected at points (joints). However, actual structural members have finite cross-sectional dimensions. When two
elements, such as a beam and column, are connected at a joint there is some overlap
of the cross sections. In many structures the dimensions of the members are large
and the length of the overlap can be a significant fraction of the total length of a
connecting element.
You may specify two end offsets for each element using parameters ioff and joff
corresponding to ends I and J, respectively. End offset ioff is the length of overlap
for a given element with other connecting elements at joint I. It is the distance from
the joint to the face of the connection for the given element. A similar definition applies to end offset joff at joint j. See Figure 34 (page 129).

End Offsets

127

CSI Analysis Reference Manual

Cardinal
Point C1

Cardinal
Point B1

B1
Cardinal
Point B2

Elevation
B2
2"

Y
B1
X
2"

Plan
Figure 33
Example Showing Joint Offsets and Cardinal Points

End offsets are automatically calculated by the SAP2000 graphical interface for
each element based on the maximum Section dimensions of all other elements that
connect to that element at a common joint.

128

End Offsets

Chapter VII

The Frame Element

Total Length L
Clear Length L c
I

Horizontal
Member

ioff

End Offsets

J
CL

joff

Support Face

Figure 34
Frame Element End Offsets

Clear Length
The clear length, denoted Lc , is defined to be the length between the end offsets
(support faces) as:
Lc = L - ( ioff + joff )
where L is the total element length. See Figure 34 (page 129).
If end offsets are specified such that the clear length is less than 1% of the total element length, the program will issue a warning and reduce the end offsets proportionately so that the clear length is equal to 1% of the total length. Normally the end
offsets should be a much smaller proportion of the total length.

Rigid-end Factor
An analysis based upon the centerline-to-centerline (joint-to-joint) geometry of
Frame elements may overestimate deflections in some structures. This is due to the
stiffening effect caused by overlapping cross sections at a connection. It is more
likely to be significant in concrete than in steel structures.

End Offsets

129

CSI Analysis Reference Manual
You may specify a rigid-end factor for each element using parameter rigid, which
gives the fraction of each end offset that is assumed to be rigid for bending and
shear deformation. The length rigid×ioff, starting from joint I, is assumed to be
rigid. Similarly, the length rigid×joff is rigid at joint j. The flexible length L f of the
element is given by:
L f = L - rigid ( ioff + joff )
The rigid-zone offsets never affect axial and torsional deformation. The full element length is assumed to be flexible for these deformations.
The default value for rigid is zero. The maximum value of unity would indicate that
the end offsets are fully rigid. You must use engineering judgment to select the appropriate value for this parameter. It will depend upon the geometry of the connection, and may be different for the different elements that frame into the connection.
Typically the value for rigid would not exceed about 0.5.

Effect upon Non-prismatic Elements
At each end of a non-prismatic element, the Section properties are assumed to be
constant within the length of the end offset. Section properties vary only along the
clear length of the element between support faces. This is not affected by the value
of the rigid-end factor, rigid.
See Subtopic “Non-prismatic Sections” (page 120) in this Chapter for more information.

Effect upon Internal Force Output
All internal forces and moments are output at the faces of the supports and at other
equally-spaced points within the clear length of the element. No output is produced
within the end offset, which includes the joint. This is not affected by the value of
the rigid-end factor, rigid.
See Topic “Internal Force Output” (page 144) in this Chapter for more information.

Effect upon End Releases
End releases are always assumed to be at the support faces, i.e., at the ends of the
clear length of the element. If a moment or shear release is specified in either bending plane at either end of the element, the end offset is assumed to be rigid for bend-

130

End Offsets

Chapter VII

The Frame Element

Continous
Joint

Axis 1

Pin Joint
J
Axis 2

Continous
Joint

Axis 3

I
Global

For diagonal element: R3 is released at end J

Figure 35
Frame Element End Releases

ing and shear in that plane at that end (i.e., it acts as if rigid = 1). This does not affect the values of the rigid-end factor at the other end or in the other bending plane.
See Topic “End Releases” (page 131) in this Chapter for more information.

End Releases
Normally, the three translational and three rotational degrees of freedom at each
end of the Frame element are continuous with those of the joint, and hence with
those of all other elements connected to that joint. However, it is possible to release
(disconnect) one or more of the element degrees of freedom from the joint when it
is known that the corresponding element force or moment is zero. The releases are
always specified in the element local coordinate system, and do not affect any other
element connected to the joint.
In the example shown in Figure 35 (page 131), the diagonal element has a moment
connection at End I and a pin connection at End J. The other two elements connecting to the joint at End J are continuous. Therefore, in order to model the pin condition the rotation R3 at End J of the diagonal element should be released. This assures that the moment is zero at the pin in the diagonal element.
End Releases

131

CSI Analysis Reference Manual

Unstable End Releases
Any combination of end releases may be specified for a Frame element provided
that the element remains stable; this assures that all load applied to the element is
transferred to the rest of the structure. The following sets of releases are unstable,
either alone or in combination, and are not permitted.
• Releasing U1 at both ends;
• Releasing U2 at both ends;
• Releasing U3 at both ends;
• Releasing R1 at both ends;
• Releasing R2 at both ends and U3 at either end;
• Releasing R3 at both ends and U2 at either end.

Effect of End Offsets
End releases are always applied at the support faces, i.e., at the ends of the element
clear length. The presence of a moment or shear release will cause the end offset to
be rigid in the corresponding bending plane at the corresponding end of the element.
See Topic “End Offsets” (page 127) in this Chapter for more information.

Named Property Sets
In addition to directly assigning end releases to frame elements, you can apply them
to a frame element in a staged-construction Load Case using a Named Property Set
of Frame Releases. A Named Property Set includes the same options that can be assigned to an element.
When property modifiers are changed in a staged construction Load Case, they do
not change the response of the structure up to that stage, but only affect subsequent
response. In other words, the effect is incremental. For example, consider a beam
with assigned moment releases that is added between two columns in a staged construction case as follows:
• Stage 1: The beam is added to an existing structure and self-weight is
applied. Because the element has moment releases assigned to it, the beam
is added as simply-supported and has no fixed-end moments. The
mid-span moment is 1000.

132

End Releases

Chapter VII

The Frame Element

• Stage 2: Named Property Set “A” is applied that has no end releases. The
mid-span moment does not change.
• Stage 3: Self-weight load is applied again (incrementally). The resulting
mid-span moment increases to 1333, and the end span moments are -667
each.
This example illustrates the common case where beams are initially added as simply-supported, then connected to provide fully moment continuity. In another common situation, two independent staged construction cases can be considered: One
for gravity load where certain members have moment releases, and the other for lateral load where the same members have moment continuity. Each of these cases
can be used as the basis for further linear or nonlinear Load Cases, and the results
considered together for design.

Nonlinear Properties
Two types of nonlinear properties are available for the Frame/Cable element: tension/compression limits and plastic hinges.
When nonlinear properties are present in the element, they only affect nonlinear
analyses. Linear analyses starting from zero conditions (the unstressed state) behave as if the nonlinear properties were not present. Linear analyses using the stiffness from the end of a previous nonlinear analysis use the stiffness of the nonlinear
property as it existed at the end of the nonlinear case.

Tension/Compression Limits
You may specify a maximum tension and/or a maximum compression that a
frame/cable element may take. In the most common case, you can define a no-compression cable or brace by specifying the compression limit to be zero.
If you specify a tension limit, it must be zero or a positive value. If you specify a
compression limit, it must be zero or a negative value. If you specify a tension and
compression limit of zero, the element will carry no axial force.
The tension/compression limit behavior is elastic. Any axial extension beyond the
tension limit and axial shortening beyond the compression limit will occur with
zero axial stiffness. These deformations are recovered elastically at zero stiffness.
Bending, shear, and torsional behavior are not affected by the axial nonlinearity.

Nonlinear Properties

133

CSI Analysis Reference Manual

Plastic Hinge
You may insert plastic hinges at any number of locations along the clear length of
the element. Detailed description of the behavior and use of plastic hinges is presented in Chapter “Frame Hinge Properties” (page 147).

Mass
In a dynamic analysis, the mass of the structure is used to compute inertial forces.
The mass contributed by the Frame element is lumped at the joints I and j. No inertial effects are considered within the element itself.
The total mass of the element is equal to the integral along the length of the mass
density, m, multiplied by the cross-sectional area, a, plus the additional mass per
unit length, mpl.
For non-prismatic elements, the mass varies linearly over each non-prismatic segment of the element, and is constant within the end offsets.
The total mass is apportioned to the two joints in the same way a similarly-distributed transverse load would cause reactions at the ends of a simply-supported beam.
The effects of end releases are ignored when apportioning mass. The total mass is
applied to each of the three translational degrees of freedom: UX, UY, and UZ. No
mass moments of inertia are computed for the rotational degrees of freedom.
For more information:
• See Topic “Mass Density” (page 77) in Chapter “Material Properties.”
• See Topic “Section Properties” (page 114) in this Chapter for the definition of
a and mpl.
• See Subtopic “Non-prismatic Sections” (page 120) in this Chapter.
• See Topic “End Offsets” (page 127) in this Chapter.
• See Topic “Mass Source” (page 334) in Chapter “Load Patterns”.
• See Chapter “Static and Dynamic Analysis” (page 341).

Self-Weight Load
Self-Weight Load activates the self-weight of all elements in the model. For a
Frame element, the self-weight is a force that is distributed along the length of the

134

Mass

Chapter VII

The Frame Element

element. The magnitude of the self-weight is equal to the weight density, w, multiplied by the cross-sectional area, a, plus the additional weight per unit length, wpl.
For non-prismatic elements, the self-weight varies linearly over each non-prismatic
segment of the element, and is constant within the end offsets.
Self-Weight Load always acts downward, in the global –Z direction. You may
scale the self-weight by a single scale factor that applies equally to all elements in
the structure.
For more information:
• See Topic “Weight Density” (page 78) in Chapter “Material Properties” for the
definition of w.
• See Topic “Section Properties” (page 114) in this Chapter for the definition of
a and wpl..
• See Subtopic “Non-prismatic Sections” (page 120) in this Chapter.
• See Topic “End Offsets” (page 127) in this Chapter.
• See Topic “Self-Weight Load” (page 325) in Chapter “Load Patterns.”

Gravity Load
Gravity Load can be applied to each Frame element to activate the self-weight of
the element. Using Gravity Load, the self-weight can be scaled and applied in any
direction. Different scale factors and directions can be applied to each element.
If all elements are to be loaded equally and in the downward direction, it is more
convenient to use Self-Weight Load.
For more information:
• See Topic “Self-Weight Load” (page 134) in this Chapter for the definition of
self-weight for the Frame element.
• See Topic “Gravity Load” (page 326) in Chapter “Load Patterns.”

Concentrated Span Load
The Concentrated Span Load is used to apply concentrated forces and moments at
arbitrary locations on Frame elements. The direction of loading may be specified in

Gravity Load

135

CSI Analysis Reference Manual
uz

2
Global Z Force

Global Z Moment

3
All loads applied
at rd=0.5
1

2
Local 2 Force

Local 2 Moment
Z

Global

Figure 36
Examples of the Definition of Concentrated Span Loads

a fixed coordinate system (global or alternate coordinates) or in the element local
coordinate system.
The location of the load may be specified in one of the following ways:
• Specifying a relative distance, rd, measured from joint I. This must satisfy
0 £ rd £ 1. The relative distance is the fraction of element length;
• Specifying an absolute distance, d, measured from joint I. This must satisfy
0 £ d £ L, where L is the element length.
Any number of concentrated loads may be applied to each element. Loads given in
fixed coordinates are transformed to the element local coordinate system. See
Figure 36 (page 136). Multiple loads that are applied at the same location are added
together.
See Chapter “Load Patterns” (page 321) for more information.

136

Concentrated Span Load

Chapter VII

The Frame Element

Distributed Span Load
The Distributed Span Load is used to apply distributed forces and moments on
Frame elements. The load intensity may be uniform or trapezoidal. The direction of
loading may be specified in a fixed coordinate system (global or alternate coordinates) or in the element local coordinate system.
See Chapter “Load Patterns” (page 321) for more information.

Loaded Length
Loads may apply to full or partial element lengths. Multiple loads may be applied to
a single element. The loaded lengths may overlap, in which case the applied loads
are additive.
A loaded length may be specified in one of the following ways:
• Specifying two relative distances, rda and rdb, measured from joint I. They
must satisfy 0 £ rda < rdb £ 1. The relative distance is the fraction of element
length;
• Specifying two absolute distances, da and db, measured from joint I. They
must satisfy 0 £ da < db £ L, where L is the element length;
• Specifying no distances, which indicates the full length of the element.

Load Intensity
The load intensity is a force or moment per unit of length. Except for the case of
projected loads described below, the intensity is measured per unit of element
length.
For each force or moment component to be applied, a single load value may be
given if the load is uniformly distributed. Two load values are needed if the load intensity varies linearly over its range of application (a trapezoidal load).
See Figure 37 (page 138) and Figure 38 (page 139).

Projected Loads
A distributed snow or wind load produces a load intensity (force per unit of element
length) that is proportional to the sine of the angle between the element and the direction of loading. This is equivalent to using a fixed load intensity that is measured

Distributed Span Load

137

CSI Analysis Reference Manual
uz

Global Z Force

Global Z Moment

uzp

rzp

1
q

Global Z Force on
Projected Length
(To be Scaled by sinq)

Global Z Moment on
Projected Length
(To be Scaled by cosq)

Local 2 Force

Local 2 Moment

Z
Global
Y

All loads applied from rda=0.25 to rdb=0.75

Figure 37
Examples of the Definition of Distributed Span Loads

per unit of projected element length. The fixed intensity would be based upon the

138

Distributed Span Load

Chapter VII
AXIS 2

The Frame Element

rda=0.0
rdb=0.5
u2a=–5
u2b=–5
5
AXIS 1

AXIS 3
da=0
db=4
u3a=0
u3b=5

da=4
db=16
u3a=5
u3b=5

da=16
db=20
u3a=5
u3b=0

AXIS 1

16
20

da=10
db=16
u2a=10
u2b=10

AXIS 2

da=4
db=10
u2a=5
u2b=5
10
5
AXIS 1

4
10
16
20

Figure 38
Examples of Distributed Span Loads

depth of snow or the wind speed; the projected element length is measured in a
plane perpendicular to the direction of loading.
Distributed Span Load

139

CSI Analysis Reference Manual
Distributed Span Loads may be specified as acting upon the projected length. The
program handles this by reducing the load intensity according to the angle, q, between the element local 1 axis and the direction of loading. Projected force loads
are scaled by sin q, and projected moment loads are scaled by cosq. The reduced
load intensities are then applied per unit of element length.
The scaling of the moment loads is based upon the assumption that the moment is
caused by a force acting upon the projected element length. The resulting moment
is always perpendicular to the force, thus accounting for the use of the cosine instead of the sine of the angle. The specified intensity of the moment should be computed as the product of the force intensity and the perpendicular distance from the
element to the force. The appropriate sign of the moment must be given.

Temperature Load
Temperature Load creates thermal strain in the Frame element. This strain is given
by the product of the Material coefficient of thermal expansion and the temperature
change of the element. All specified Temperature Loads represent a change in temperature from the unstressed state for a linear analysis, or from the previous temperature in a nonlinear analysis.
Three independent Load Temperature fields may be specified:
• Temperature, t, which is constant over the cross section and produces axial
strains
• Temperature gradient, t2, which is linear in the local 2 direction and produces
bending strains in the 1-2 plane
• Temperature gradient, t3, which is linear in the local 3 direction and produces
bending strains in the 1-3 plane
Temperature gradients are specified as the change in temperature per unit length.
The temperature gradients are positive if the temperature increases (linearly) in the
positive direction of the element local axis. The gradient temperatures are zero at
the neutral axes, hence no axial strain is induced.
Each of the three Load Temperature fields may be constant along the element
length or linearly interpolated from values given at the joints by a Joint Pattern.
See Chapter “Load Patterns” (page 321) for more information.

140

Temperature Load

Chapter VII

The Frame Element

Strain Load
Six types of strain load are available, one corresponding to each of the internal
forces and moments in a frame element. These are:
• Axial strain, e 11 , representing change in length per unit length. Positive strain
increases the length of an unrestrained element, or causes compression in a restrained element.
• Shear strains, g 12 and g 13 , representing change in angle per unit length. The angle change is measured between the cross section and the neutral axis. Positive
shear strain causes shear deformation in the same direction as would positive
shear forces V2 and V3, respectively.
• Torsional curvature, y 1 , representing change in torsional angle per unit length.
Positive curvature causes deformation in the same direction as would positive
torque T.
• Bending curvatures, y 2 and y 3 , representing change in angle per unit length.
The angle is measured between adjacent sections that remain normal to the
neutral axis. Positive curvature causes bending deformation in the same direction as would positive moments M2 and M3, respectively.
Each of the Strain Loads may be constant along the element length or linearly interpolated from values given at the joints by a Joint Pattern.
In an unrestrained element, strain loads cause deformation between the two ends of
the element, but induce no internal forces. This unrestrained deformation has the
same sign as would deformation caused by the corresponding (conjugate) forces
and moments acting on the element. On the other hand, strain loading in a restrained element causes corresponding internal forces that have the opposite sign as
the applied strain. Most elements in a real structure are connected to finite stiffness,
and so strain loading would cause both deformation and internal forces. Note that
the effects of shear and bending strain loading are coupled.
For more information, see Topic “Internal Force Output” (page 144) in this chapter,
and also Chapter “Load Patterns” (page 321.)

Strain Load

141

CSI Analysis Reference Manual
choose whichever type of loading is most conveniently specified for your particular
application.
Currently only axial Deformation Load is available. The specified axial deformation is converted to axial Strain Load by simply dividing by the element length. The
computed strain loads are assumed to be constant along the length of the element.
See Chapter “Load Patterns” (page 321) for more information.

Target-Force Load
Target-Force Load is a special type of loading where you specify a desired axial
force, and deformation load is iteratively applied to achieve the target force. Since
the axial force may vary along the length of the element, you must also specify the
relative location where the desired force is to occur. Target-Force loading is only
used for nonlinear static and staged-construction analysis. If applied in any other
type of Load Case, it has no effect.
Unlike all other types of loading, target-force loading is not incremental. Rather,
you are specifying the total force that you want to be present in the frame element at
the end of the Load Case or construction stage. The applied deformation that is calculated to achieve that force may be positive, negative, or zero, depending on the
force present in the element at the beginning of the analysis. When a scale factor is
applied to a Load Pattern that contains Target-Force loads, the total target force is
scaled. The increment of applied deformation that is required may change by a different scale factor.
See Topic “Target-Force Load” (page 331) in Chapter “Load Patterns” and Topic
“Target-Force Iteration” (page 444) in Chapter “Nonlinear Static Analysis” for
more information.

Internal Force Output
The Frame element internal forces are the forces and moments that result from integrating the stresses over an element cross section. These internal forces are:
• P, the axial force
• V2, the shear force in the 1-2 plane
• V3, the shear force in the 1-3 plane
• T, the axial torque

142

Target-Force Load

Chapter VII

The Frame Element

Axis 2

Axis 1

Positive Axial Force and Torque

Axis 3

V2
Compression Face
Axis 2
Axis 1

Positive Moment and Shear
in the 1-2 Plane
M3

Axis 3

Positive Moment and Shear
in the 1-3 Plane

Tension Face

Axis 2

Axis 1

Tension Face

V3
V3

Compression Face
Axis 3

Figure 39
Frame Element Internal Forces and Moments

• M2, the bending moment in the 1-3 plane (about the 2 axis)
• M3, the bending moment in the 1-2 plane (about the 3 axis)
Internal Force Output

143

CSI Analysis Reference Manual
These internal forces and moments are present at every cross section along the
length of the element, and may be requested as part of the analysis results.
The sign convention is illustrated in Figure 39 (page 143). Positive internal forces
and axial torque acting on a positive 1 face are oriented in the positive direction of
the element local coordinate axes. Positive internal forces and axial torque acting
on a negative face are oriented in the negative direction of the element local coordinate axes. A positive 1 face is one whose outward normal (pointing away from element) is in the positive local 1 direction.
Positive bending moments cause compression at the positive 2 and 3 faces and tension at the negative 2 and 3 faces. The positive 2 and 3 faces are those faces in the
positive local 2 and 3 directions, respectively, from the neutral axis.

Effect of End Offsets
When end offsets are present, internal forces and moments are output at the faces of
the supports and at points within the clear length of the element. No output is produced within the length of the end offset, which includes the joint. Output will only
be produced at joints I or j when the corresponding end offset is zero.
See Topic “End Offsets” (page 127) in this Chapter for more information.

Stress Output
Axial stress results are available for graphical display and tabular output along with
the internal forces described above. The axial stress is denoted S11 and is computed
at any point in the frame cross section as:
S 11 =

P
M3
M2
- x2
- x3
a
i33
i22

where
• P is the axial force, and M2 and M3 are the bending moments, as defined in
Topic “Internal Force Output” (page 144)
• a is the cross-sectional area, and i22 and i33 are the section moments of inertia, as defined in Topic “Section Properties” (page 114)
• x2 and x3 are the coordinates of the point where the stress is calculated, measured from the centroid of the section along the local 2 and 3 axes, respectively.

144

Stress Output

Chapter VII

The Frame Element

Based on this definition, tensile stresses are always positive, and compressive
stresses are always negative, regardless of the material.
Stresses are computed at the same axial stations as are the internal forces. At each
station, stresses are computed at selected stress points over the cross section, with
locations that depend upon the shape of the section:
• I-sections, T-sections, rectangles, boxes, channels, and angles - at all corners
where the maximum stresses could occur
• Cover-plated I sections - at the same locations as for an I-section, plus the extreme corners of the cover plates, if present
• Circles and pipes - at eight points on the circumference
• Section Designer sections - at the stress points defined when the section was
drawn; if no stress points have been defined, stress points are assumed at the
four corners of the rectangular bounding box for the section; this box has dimensions t3 x t2
• General sections and all other shapes - at the four corners of the rectangular
bounding box for the section; this box has dimensions t3 x t2
• Nonprismatic sections - computed as above from the interpolated shape, if the
shape type is the same at both ends of the frame segment; if the shape type is not
the same at both ends, then zero stress is reported.
• For all shapes except the box and pipe, stresses are also computed at the centroid of the section
In addition to the value of S11 at each stress point, two extreme stress values are reported at each station:
• S11Max – the maximum value over all stress points at that station
• S11Min – the minimum value over all stress points at that station
Stresses are computed for all load cases except for moving-load cases, for which
zero values will be reported.
The following assumptions pertain to the stresses reported for frame elements:
• Stresses are computed for the base material of the section. No account is made
for the modular ratio. This usually has no effect on stresses for any section
types except for some Section Designer shapes.
• Stresses are computed based on the properties of the section assigned to the
frame element. If the section property is changed during a staged-construction

Stress Output

145

CSI Analysis Reference Manual
load case, the calculated stress values may not be appropriate. However, the internal forces and moments are still correct.
• If any of the properties a, i22, or i33 is zero, the stress S11 will be reported as
zero. It is recommended to use end releases rather than setting the section properties to zero.
• Property modifiers that are applied to a, i22, or i33 do not change these property values when used for stress calculation. In some cases property modifiers
may have an indirect effect upon the stresses if they affect the corresponding
axial force or bending moments.
The description in this topic pertains only to the stress values reported as analysis
results. Stresses used for frame design and bridge design are computed separately,
as appropriate for the applicable material and design procedure.

146

Stress Output

C h a p t e r VIII

Hinge Properties
You may insert plastic hinges at any number of locations along the clear length of
any Frame element or Tendon object. ETABS also admits hinges in vertical
shear-wall elements. Each hinge represents concentrated post-yield behavior in one
or more degrees of freedom. Hinges only affect the behavior of the structure in nonlinear static and nonlinear time-history analyses.
Advanced Topics
• Overview
• Hinge Properties
• Automatic, User-Defined, and Generated Properties
• Automatic Hinge Properties
• Analysis Modeling
• Analysis Results

Overview
Yielding and post-yielding behavior can be modeled using discrete user-defined
hinges. Hinges can be assigned to a frame element at any location along the clear

Overview

147

CSI Analysis Reference Manual
length of the element. Uncoupled moment, torsion, axial force and shear hinges are
available. There are also coupled P-M2-M3 hinges which yield based on the interaction of axial force and bi-axial bending moments at the hinge location. Subsets of
these hinges may include P-M2, P-M3, and M2-M3 behavior.
Fiber hinges P-M2-M3 can be defined, which are a collection of material points
over the cross section. Each point represents a tributary area and has its own
stress-strain curve. Plane sections are assumed to remain planar for the section,
which ties together the behavior of the material points. Fiber hinges are often more
realistic than force-moment hinges, but are more computationally intensive.
More than one type of frame hinge can exist at the same location, for example, you
might assign both an M3 (moment) and a V2 (shear) hinge to the same end of a
frame element. Hinge properties can be computed automatically from the element
material and section properties according to FEMA-356 (FEMA, 2000) or ACSE
41-13 criteria.
For ETABS, hinges can also be assigned to vertical shear walls. These hinges are of
type fiber P-M3, and always act at the center of the shell element. When hinges are
present in a shear wall shell element, the vertical membrane stress behavior is governed by hinge, while horizontal and shear membrane stress, as well as out-of-plane
bending behavior, are governed by the properties of the shell element.
Hinges only affect the behavior of the structure in nonlinear static and nonlinear
time-history analyses. Hinge behavior does not affect nonlinear modal time-history
(FNA) analyses unless the hinges are modeled as links, as described later in this
chapter.
Strength loss is permitted in the hinge properties, and in fact the FEMA and ASCE
hinges assume a sudden loss of strength. However, you should use this feature judiciously. Sudden strength loss is often unrealistic and can be very difficult to analyze, especially when elastic snap-back occurs. We encourage you to consider
strength loss only when necessary, to use realistic negative slopes, and to carefully
evaluate the results.
To help with convergence, the program automatically limits the negative slope of a
hinge to be no stiffer than 10% of the elastic stiffness of the Frame element containing the hinge. If you need steeper slopes, you can assign a hinge overwrite that automatically meshes the frame element around the hinge. By reducing the size of the
meshed element, you can increase the steepness of the drop-off.
Everything in this Chapter applies to Tendon objects as well as to Frame elements,
although only the use of axial hinges makes sense for Tendons.

148

Overview

Chapter VIII

Hinge Properties

Force

B
IO

CP
D

Displacement
Figure 40
The A-B-C-D-E curve for Force vs. Displacement
The same type of curve is used for Moment vs. Rotation

Hinge Properties
A hinge property is a named set of nonlinear properties that can be assigned to
points along the length of one or more Frame elements. You may define as many
hinge properties as you need.
Force- and moment-type hinges are rigid-plastic. For each force degree of freedom
(axial and shear), you may specify the plastic force-displacement behavior. For
each moment degree of freedom (bending and torsion) you may specify the plastic
moment-rotation behavior. Each hinge property may have plastic properties specified for any number of the six degrees of freedom. The axial force and the two
bending moments may be coupled through an interaction surface. Degrees of freedom that are not specified remain elastic.
Fiber hinges are elastic-plastic and consist of a set of material points, each representing a portion of the frame cross-section having the same material. Force-deflection and moment-rotation curves are not specified, but rather are computed during
the analysis from the stress-strain curves of the material points.
Hinge Properties

149

CSI Analysis Reference Manual

Hinge Length
Each plastic hinge is modeled as a discrete point hinge. All plastic deformation,
whether it be displacement or rotation, occurs within the point hinge. This means
you must assume a length for the hinge over which the plastic strain or plastic curvature is integrated.
There is no easy way to choose this length, although guidelines are given in
FEMA-356 and ASCE 41-13. Typically it is a fraction of the element length, and is
often on the order of the depth of the section, particularly for moment-rotation
hinges.
You can approximate plasticity that is distributed over the length of the element by
inserting many hinges. For example, you could insert ten hinges at relative locations within the element of 0.05, 0.15, 0.25, ..., 0.95, each with deformation properties based on an assumed hinge length of one-tenth the element length. Of course,
adding more hinges will add more computational cost, so this should only be done
where needed.
For force/moment-type hinges, elastic deformation occurs along the entire length
of the Frame element and is not affected by the presence of the hinges. For fiber
hinges, elastic behavior along the hinge length is determined from the hinge material stress-strain curves, and the elastic properties of the frame element are ignored
within the hinge length. For this reason, the hinge length should not exceed the
length of frame element.

Plastic Deformation Curve
For each force or moment degree of freedom, you define a force-displacement (moment-rotation) curve that gives the yield value and the plastic deformation following yield. This is done in terms of a curve with values at five points, A-B-C-D-E, as
shown in Figure 40 (page 149). You may specify a symmetric curve, or one that differs in the positive and negative direction.
The shape of this curve as shown is intended for pushover analysis. You can use
any shape you want. The following points should be noted:
• Point A is always the origin.
• Point B represents yielding. No deformation occurs in the hinge up to point B,
regardless of the deformation value specified for point B. The displacement
(rotation) at point B will be subtracted from the deformations at points C, D,
and E. Only the plastic deformation beyond point B will be exhibited by the
hinge.

150

Hinge Properties

Chapter VIII

Hinge Properties

• Point C represents the ultimate capacity for pushover analysis. However, you
may specify a positive slope from C to D for other purposes.
• Point D represents a residual strength for pushover analysis. However, you
may specify a positive slope from C to D or D to E for other purposes.
• Point E represent total failure. Beyond point E the hinge will drop load down to
point F (not shown) directly below point E on the horizontal axis. If you do not
want your hinge to fail this way, be sure to specify a large value for the deformation at point E.
You may specify additional deformation measures at points IO (immediate occupancy), LS (life safety), and CP (collapse prevention). These are informational
measures that are reported in the analysis results and used for performance-based
design. They do not have any effect on the behavior of the structure.
Prior to reaching point B, all deformation is linear and occurs in the Frame element
itself, not the hinge. Plastic deformation beyond point B occurs in the hinge in addition to any elastic deformation that may occur in the element.
When the hinge unloads elastically, it does so without any plastic deformation, i.e.,
parallel to slope A-B.

Scaling the Curve
When defining the hinge force-deformation (or moment-rotation) curve, you may
enter the force and deformation values directly, or you may enter normalized values
and specify the scale factors that you used to normalized the curve.
In the most common case, the curve would be normalized by the yield force (moment) and yield displacement (rotation), so that the normalized values entered for
point B would be (1,1). However, you can use any scale factors you want. They do
not have to be yield values.
Remember that any deformation given from A to B is not used. This means that the
scale factor on deformation is actually used to scale the plastic deformation from B
to C, C to D, and D to E. However, it may still be convenient to use the yield deformation for scaling.
When automatic hinge properties are used, the program automatically uses the
yield values for scaling. These values are calculated from the Frame section properties. See the next topic for more discussion of automatic hinge properties.

Hinge Properties

151

CSI Analysis Reference Manual

Strength Loss
Strength loss is permitted in the hinge properties, and in fact the FEMA hinges assume a sudden loss of strength. However, you should use this feature judiciously.
Any loss of strength in one hinge causes load redistribution within the structure,
possibly leading to failure of another hinge, and ultimately causing progressive collapse. This kind of analysis can be difficult and time consuming. Furthermore, any
time negative stiffnesses are present in the model, the solution may not be mathematically unique, and so may be of questionable value.
Sudden strength loss (steep negative stiffness) is often unrealistic and can be even
more difficult to analyze. When an unloading plastic hinge is part of a long beam or
column, or is in series with any flexible elastic subsytem, “elastic snap-back” can
occur. Here the elastic unloading deflection is larger than, and of opposite sign to,
the plastic deformation. This results in the structure deflecting in the direction opposite the applied load. SAP2000, ETABS, and CSiBridge have a built-in mechanism to deal with snap-back for certain hinges, but this may not always be enough
to handle several simultaneous snap-back hinge failures.
Consider carefully what you are trying to accomplish with your analysis. A well designed structure, whether new or retrofitted, should probably not have strength loss
in any primary members. If an analysis shows strength loss in a primary member,
you may want to modify the design and then re-analyze, rather than trying to push
the analysis past the first failure of the primary members. Since you need to re-design anyway, what happens after the first failure is not relevant, since the behavior
will become changed.
To help with convergence, the program automatically limits the negative slope of a
hinge to be no stiffer than 10% of the elastic stiffness of the Frame element containing the hinge. By doing this, snap-back is prevented within the element, although it
may still occur in the larger structure.
If you need steeper slopes, you can assign a Frame Hinge Overwrite that automatically meshes the Frame object around the hinge. When you assign this overwrite,
you can specify what fraction of the Frame object length should be used for the element that contains the hinge. For example, consider a Frame object containing one
hinge at each end, and one in the middle. If you assign a Frame Hinge Overwrite
with a relative length of 0.1, the object will be meshed into five elements of relative
lengths 0.05, 0.4, 0.1, 0.4, and 0.05. Each hinge is located at the center of an element with 0.1 relative length, but because two of the hinges fall at the ends of the
object, half of their element lengths are not used. Because these elements are
shorter than the object, their elastic stiffnesses are larger, and the program will permit larger negative stiffnesses in the hinges.

152

Hinge Properties

Chapter VIII

Hinge Properties

By reducing the size of the meshed element, you can increase the steepness of the
drop-off, although the slope will never be steeper than you originally specified for
the hinge. Again, we recommend gradual, realistic slopes whenever possible, unless you truly need to model brittle behavior.

Types of P-M2-M3 Hinges
Normally the hinge properties for each of the six degrees of freedom are uncoupled
from each other. However, you have the option to specify coupled axial-force/biaxial-moment behavior. This is called a P-M2-M3 or PMM hinge. Three types are
available. In summary:
• Isotropic P-M2-M3 hinge: This hinge can handle complex and unsymmetrical
PMM surfaces and can interpolate between multiple moment-rotation curves.
Two-dimensional subsets of the hinge are available. It is limited to isotropic
hysteresis, which may not be suitable for some structures.
• Parametric P-M2-M3 hinge: This hinge is limited to doubly symmetric section
properties and uses a simple parametric definition of the PMM surface.
Hysteretic energy degradation can be specified, making it more suitable than
the isotropic hinge for extensive cyclic loading.
• Fiber P-M2-M3 hinge. This is the most realistic hinge, but may require the
most computational resources in terms of analysis time and memory usage.
Various hysteresis models are available and they can be different for each material in the hinge.
These hinges are described in more detail in the following topics.

Isotropic P-M2-M3 Hinge
This hinge can handle complex and unsymmetrical PMM surfaces and can interpolate between multiple moment-rotation curves. It is limited to isotropic hysteresis,
which may not be suitable for some structures.
Three additional coupled hinges are available as subsets of the PMM hinge: P-M2,
P-M3, and M2-M3 hinges.
Tension is Always Positive!
It is important to note that SAP2000 uses the sign convention where tension is always positive and compression is always negative, regardless of the material being
used. This means that for some materials (e.g., concrete) the interaction surface
may appear to be upside down.
Hinge Properties

153

CSI Analysis Reference Manual
Interaction (Yield) Surface
For the PMM hinge, you specify an interaction (yield) surface in three-dimensional
P-M2-M3 space that represents where yielding first occurs for different combinations of axial force P, minor moment M2, and major moment M3.
The surface is specified as a set of P-M2-M3 curves, where P is the axial force (tension is positive), and M2 and M3 are the moments. For a given curve, these moments may have a fixed ratio, but this is not necessary. The following rules apply:
• All curves must have the same number of points.
• For each curve, the points are ordered from most negative (compressive) value
of P to the most positive (tensile).
• The three values P, M2 and M3 for the first point of all curves must be identical,
and the same is true for the last point of all curves
• When the M2-M3 plane is viewed from above (looking toward compression),
the curves should be defined in a counter-clockwise direction
• The surface must be convex. This means that the plane tangent to the surface at
any point must be wholly outside the surface. If you define a surface that is not
convex, the program will automatically increase the radius of any points which
are “pushed in” so that their tangent planes are outside the surface. A warning
will be issued during analysis that this has been done.
You can explicitly define the interaction surface, or let the program calculate it using one of the following formulas:
• Steel, AISC-LRFD Equations H1-1a and H1-1b with phi = 1
• Steel, FEMA-356 Equation 5-4
• Concrete, ACI 318-02 with phi = 1
You may look at the hinge properties for the generated hinge to see the specific surface that was calculated by the program.
Moment-Rotation Curves
For PMM hinges you specify one or more moment/plastic-rotation curves corresponding to different values of P and moment angle q. The moment angle is measured in the M2-M3 plane, where 0° is the positive M2 axis, and 90° is the positive
M3 axis.

154

Hinge Properties

Chapter VIII

Hinge Properties

You may specify one or more axial loads P and one or more moment angles q. For
each pair (P,q), the moment-rotation curve should represent the results of the following experiment:
• Apply the fixed axial load P.
• Increase the moments M2 and M3 in a fixed ratio (cos q, sin q) corresponding
to the moment angle q.
• Measure the plastic rotations Rp2 and Rp3 that occur after yield.
• Calculate the resultant moment M = M2*cos q + M3*sin q, and the projected
plastic rotation Rp = Rp2*cos q + Rp3*sin q at each measurement increment
• Plot M vs. Rp, and supply this data to SAP2000
Note that the measured direction of plastic strain may not be the same as the direction of moment, but the projected value is taken along the direction of the moment.
In addition, there may be measured axial plastic strain that is not part of the projection. However, during analysis the program will recalculate the total plastic strain
based on the direction of the normal to the interaction (yield) surface.
During analysis, once the hinge yields for the first time, i.e., once the values of P,
M2 and M3 first reach the interaction surface, a net moment-rotation curve is interpolated to the yield point from the given curves. This curve is used for the rest of the
analysis for that hinge.
If the values of P, M2, and M3 change from the values used to interpolate the curve,
the curve is adjusted to provide an energy equivalent moment-rotation curve. This
means that the area under the moment-rotation curve is held fixed, so that if the resultant moment is smaller, the ductility is larger. This is consistent with the underlying stress strain curves of axial “fibers” in the cross section.
As plastic deformation occurs, the yield surface changes size according to the shape
of the M-Rp curve, depending upon the amount of plastic work that is done. You
have the option to specify whether the surface should change in size equally in the
P, M2, and M3 directions, or only in the M2 and M3 directions. In the latter case,
axial deformation behaves as if it is perfectly plastic with no hardening or collapse.
Axial collapse may be more realistic in some hinges, but it is computationally difficult and may require nonlinear direct-integration time-history analysis if the structure is not stable enough the redistribute any dropped gravity load.

Hinge Properties

155

CSI Analysis Reference Manual

Parametric P-M2-M3 Hinge
This hinge is limited to doubly symmetric section properties and uses a simple
parametric definition of the PMM surface. Hysteretic energy degradation can be
specified, making it more suitable than the isotropic hinge for extensive cyclic
loading.
Two versions of the hinge are available, one for steel frame sections, and one for reinforced-concrete frame sections. Currently this hinge is only available in ETABS,
and will be added to SAP2000 and CSiBridge in subsequent versions.
The description and theory for this hinge formulation are presented in the Technical
Note “Parametric P-M2-M3 Hinge Model”. This document can be found in the
Manuals subfolder where the software is installed on your computer. It can be accessed from inside the software using the menu command Help > Documentation >
Technical Notes.
Detailed descriptions of the input values needed to define the properties for either
the steel or concrete hinge are available from the Help facility within the software.
This can be accessed using the menu command Help > Product Help, or pressing
the F1 key at any time.

Fiber P-M2-M3 Hinge
The Fiber P-M2-M3 (Fiber PMM) hinge models the axial behavior of a number of
representative axial “fibers” distributed across the cross section of the frame element. Each fiber has a location, a tributary area, and a stress-strain curve. The axial
stresses are integrated over the section to compute the values of P, M2 and M3.
Likewise, the axial deformation U1 and the rotations R2 and R3 are used to compute the axial strains in each fiber. Plane sections are assumed to remain planar.
You can define you own fiber hinge, explicitly specifying the location, area, material and its stress-strain curve for each fiber, or you can let the program automatically create fiber hinges for circular and rectangular frame sections.
The Fiber PMM hinge is more “natural” than the Isotropic or Parametric PMM
hinges described above, since it automatically accounts for interaction, changing
moment-rotation curve, and plastic axial strain. However, it is also more
computationally intensive, requiring more computer storage and execution time.
You may have to experiment with the number of fibers needed to get an optimum
balance between accuracy and computational efficiency.

156

Hinge Properties

Chapter VIII

Hinge Properties

Strength loss in a fiber hinge is determined by the strength loss in the underlying
stress-strain curves. Because all the fibers in a cross section do not usually fail at the
same time, the overall hinges tend to exhibit more gradual strength loss than hinges
with directly specified moment-rotation curves. This is especially true if reasonable
hinge lengths are used. For this reason, the program does not automatically restrict
the negative drop-off slopes of fiber hinges. However, we still recommend that you
pay close attention to the modeling of strength loss, and modify the stress-strain
curves if necessary.
For more information:
• See Topic “Stress-Strain Curves” (page 80) in Chapter “Material Properties.”
• See Topic “Section-Designer Sections” (page 118) Chapter “The Frame Element.”

Hysteresis Models
The plastic force-deformation or moment-rotation curve defines the nonlinear behavior under monotonic loading. This curve, combined with the elastic behavior of
the hinge length in the parent frame element, is also known as the backbone curve
for the hinge.
Under load reversal or cyclic loading, the behavior will deviate from the backbone
curve. Several different hysteresis models are available to describe this behavior
for different types of materials. For the most part, these differ in the amount of energy they dissipate in a given cycle of deformation, and how the energy dissipation
behavior changes with an increasing amount of deformation.
Hysteresis models are described in Topic “Hysteresis Models” (page 85) of Chapter “Material Properties.”
Hysteresis models are applicable to the different types of hinges as follows:
• Single degree of freedom hinges: All inelastic models (kinematic, degrading,
Takeda, pivot, concrete, BRB hardening, and isotopic)
• Coupled P-M2-M3, P-M2, P-M3, and M2-M3 hinges: Isotropic model only
• Fiber P-M2-M3 hinges: For each material fiber, all models (elastic, kinematic,
degrading, Takeda, pivot, concrete, BRB hardening, and isotopic)
Note that all of these models are available in the current version of ETABS. Some
of the models are not yet available in SAP2000 and CSiBridge but will be added in
subsequent versions.

Hinge Properties

157

CSI Analysis Reference Manual
Hysteretic behavior may affect nonlinear static and nonlinear time-history load
cases that exhibit load reversals and cyclic loading. Monotonic loading is not affected. Note, however, that even static pushover load cases can produce load reversal in some hinges caused by strength loss in other hinges.

Automatic, User-Defined, and Generated Properties
There are three types of hinge properties in SAP2000:
• Automatic hinge properties
• User-defined hinge properties
• Generated hinge properties
Only automatic hinge properties and user-defined hinge properties can be assigned
to frame elements. When automatic or user-defined hinge properties are assigned to
a frame element, the program automatically creates a generated hinge property for
each and every hinge.
The built-in automatic hinge properties for steel members are based on Table 5-6 in
FEMA-356. The built-in automatic hinge properties for concrete members are
based on Tables 6-7 and 6-8 in FEMA-356, or on Caltrans specifications for concrete columns. After assigning automatic hinge properties to a frame element, the
program generates a hinge property that includes specific information from the
frame section geometry, the material, and the length of the element. You should review the generated properties for their applicability to your specific project.
User-defined hinge properties can either be based on a hinge property generated
from automatic property, or they can be fully user-defined.
A generated property can be converted to user-defined, and then modified and
re-assigned to one or more frame elements. This way you can let the program do
much of the work for you using automatic properties, but you can still customize
the hinges to suit your needs. However, once you convert a generated hinge to
user-defined, it will no longer change if you modify the element, its section or material.
It is the generated hinge properties that are actually used in the analysis. They can
be viewed, but they can not be modified. Generated hinge properties have an automatic naming convention of LabelH#, where Label is the frame element label, H
stands for hinge, and # represents the hinge number. The program starts with hinge
number 1 and increments the hinge number by one for each consecutive hinge applied to the frame element. For example if a frame element label is F23, the gener-

158

Automatic, User-Defined, and Generated Properties

Chapter VIII

Hinge Properties

ated hinge property name for the second hinge assigned to the frame element is
F23H2.
The main reason for the differentiation between defined properties (in this context,
defined means both automatic and user-defined) and generated properties is that
typically the hinge properties are section dependent. Thus it would be necessary to
define a different set of hinge properties for each different frame section type in the
model. This could potentially mean that you would need to define a very large number of hinge properties. To simplify this process, the concept of automatic properties is used in SAP2000. When automatic properties are used, the program combines its built-in default criteria with the defined section properties for each element to generate the final hinge properties. The net effect of this is that you do significantly less work defining the hinge properties because you don’t have to define
each and every hinge.

Automatic Hinge Properties
Automatic hinge properties are based upon a simplified set of assumptions that may
not be appropriate for all structures. You may want to use automatic properties as a
starting point, and then convert the corresponding generated hinges to user-defined
and explicitly overwrite calculated values as needed.
Automatic properties require that the program have detailed knowledge of the
Frame Section property used by the element that contains the hinge. For this reason,
only the following types of automatic hinges are available:
Concrete Beams in Flexure
M2 or M3 hinges can be generated using FEMA Table 6-7 (I) for the following
shapes:
• Rectangle
• Tee
• Angle
• Section Designer
Concrete Columns in Flexure
M2, M3, M2-M3, P-M2, P-M3, or P-M2-M3 hinges can be generated using
FEMA Table 6-8 (I), for the following shapes:

Automatic Hinge Properties

159

CSI Analysis Reference Manual
• Rectangle
• Circle
• Section Designer
or using Caltrans specifications, for the following shapes:
• Section Designer only
Steel Beams in Flexure
M2 or M3 hinges can be generated using FEMA Table 5-6, for the following
shapes:
– I/Wide-flange only
Steel Columns in Flexure
M2, M3, M2-M3, P-M2, P-M3, or P-M2-M3 hinges can be generated using
FEMA Table 5-6, for the following shapes:
• I/Wide-flange
• Box
Steel Braces in Tension/Compression
P (axial) hinges can be generated using FEMA Table 5-6, for the following
shapes:
• I/Wide-flange
• Box
• Pipe
• Double channel
• Double angle
Fiber Hinge
P-M2-M3 hinges can be generated for steel or reinforced concrete members using the underlying stress-strain behavior of the material for the following
shapes:
• Rectangle
• Circle

160

Automatic Hinge Properties

Chapter VIII

Hinge Properties

Additional Considerations
You must make sure that all required design information is available to the Frame
section as follows:
• For concrete Sections, the reinforcing steel must be explicitly defined, or else
the section must have already been designed by the program before nonlinear
analysis is performed
• For steel Sections, Auto-select Sections can only be used if they have already
been designed so that a specific section has been chosen before nonlinear analysis is performed
For more information, see the on-line help that is available while assigning automatic hinges to Frame elements in the Graphical User Interface.

Analysis Modeling
Hinges are assigned to a Frame or Shell (shear wall) element to represent the nonlinear behavior of their parent element. When the analysis model is created, there
are two ways the hinge can be represented:
• Hinge embedded in the element
• Hinge as a separate link element
The latter method is currently only available in the ETABS Ultimate level, and enables hinge behavior to be considered in nonlinear model time-history (FNA) load
cases. As a rule, FNA analysis runs significantly faster than nonlinear direct-integration time-history analysis. Nonlinear static analysis and nonlinear direct-integration time history analysis are available for both types of analysis modeling.
When the hinge is modeled as a link element, the parent Frame element is divided at
the hinge location into separate subelements, and a zero-length link element is created that contains the hinge property and connects the frame subelements. A very
small amount of axial mass and rotational inertia are added at the two connecting
joints to improve FNA iteration. A similar internal modeling is employed for shear
wall elements when the hinge is modeled as a link element.
A second, independent modeling option is available to assign automatic subdivision of Frame elements at hinge locations. Using this assignment, you specify a relative length that is used when creating the analysis model of the hinges for the selected elements. The effect of this depends upon how the hinge is modeled:

Analysis Modeling

161

CSI Analysis Reference Manual
• For the hinge embedded in the element: The Frame object is subdivided into
separate frame elements, with one element containing the hinge that is equal in
length to that specified in the assignment.
This has the advantage of introducing more degrees of freedom into the model
that may improve convergence when multiple hinges are failing at the same
time, with a possible increase in computation time. In addition, steeper
drop-offs are permitted when the hinge curve exhibits strength loss because the
element containing the hinge is shorter, and hence stiffer.
On the other hand, not subdividing the frame element leads to a smaller analysis model, typically requiring less computation time and storage. In addition,
stiffness proportional damping for nonlinear direct-integration time-history
analysis is better modeled in longer elements.
• For the hinge as a separate link element: The subdivision into two frame elements and a zero-length link is not changed. However, the elastic flexibility of
the link is changed to be equal to the length of the frame element specified in
the assignment, and the corresponding length of the adjacent frame sub-elements are made rigid.
This has the advantage of improving stiffness-proportional damping in nonlinear direct-integration time-history analysis, and can be recommend for this reason. On the other hand, this is not necessary for FNA analysis.
The default relative length for automatic subdivision is 0.02. Recommended values
typically range from 0.02 to 0.25.

Computational Considerations
The most important advice is to only add hinges to the model where nonlinear behavior is expected to have a significant effect on the analysis and design. Adding
extra hinges increases the time and effort it takes to create the model, to run the
analyses, and to interpret the results.
Start with the simplest model possible so that you can make many analysis runs
quickly. This helps to better understand the behavior of your structure early in the
design process and to correct modeling errors. Add hinges and complexity gradually as you determine where nonlinearity is expected and/or desired.
Adding hinges everywhere to find the nonlinearity is tempting, but this approach
usually wastes much more time than incrementally growing the model.

162

Computational Considerations

Chapter VIII

Hinge Properties

Most models with hinges benefit from using event-to-event stepping for nonlinear
static and nonlinear direct-integration time-history load cases. This is particularly
true for the parametric P-M2-M3 hinge. However, it may be necessary to turn off
event-to-event stepping if the model has a very large number of hinges, or if there is
a significant amount of other types of nonlinearity in the structure. This is best determined by running analyses both with and without events to see which is most efficient.
Most nonlinear time-history analysis benefits from the presence of mass at the nonlinear degrees-of-freedom. Inertia tends to stabilize iteration when the nonlinear
behavior is changing rapidly. This is particularly true for FNA analysis. For
ETABS, it is usually best to define the mass source to include vertical mass and to
not lump the mass at the story levels for models that have hinges.
For FNA analysis, it is usually most efficient to damp out the very high modes.
Some of the Ritz modes needed for FNA analysis can be expected to be of high frequency. An example of how to do this would be to define the load-case damping to
be of type “Interpolated by Frequency”. Then specify your desired structure damping ratio (say 0.025) for frequencies up to 999 Hz, and a damping ratio of 0.99 for
frequencies above 1000 Hz. You can experiment with this cutoff value to see the effect on runtime and results.

Analysis Results
For each output step in a nonlinear static or nonlinear direct-integration time-history Load Case, you may request analysis results for the hinges. These results include:
• The forces and/or moments carried by the hinge. Degrees of freedom not defined for the hinge will report zero values, even though non-zero values are carried rigidly through the hinge.
• The plastic displacements and/or rotations.
• The most extreme state experienced by the hinge in any degree of freedom.
This state does not indicate whether it occurred for positive or negative deformation:
– A to B
– B to C
– C to D
– D to E

Analysis Results

163

CSI Analysis Reference Manual
– >E
• The most extreme performance status experienced by the hinge in any degree
of freedom. This status does not indicate whether it occurred for positive or
negative deformation:
– A to B
– B to IO
– IO to LS
– LS to CP
– > CP
When you display the deflected shape in the graphical user interface for a nonlinear
static or nonlinear direct-integration time-history Load Case, the hinges are plotted
as colored dots indicating their most extreme state or status:
• B to IO
• IO to LS
• LS to CP
• CP to C
• C to D
• D to E
• >E
The colors used for the different states are indicated on the plot. Hinges that have
not experienced any plastic deformation (A to B) are not shown.

164

Analysis Results

Chapter IX

The Cable Element
The Cable element is a highly nonlinear element used to model the catenary behavior of slender cables under their own self-weight. Tension-stiffening and large-deflections nonlinearity are inherently included in the formulation. Nonlinear analysis is required to make use of the Cable element. Linear analyses can be performed
that use the stiffness from the end of nonlinear Load Cases.
Advanced Topics
• Overview
• Joint Connectivity
• Undeformed Length
• Shape Calculator
• Degrees of Freedom
• Local Coordinate System
• Section Properties
• Property Modifiers
• Mass
• Self-Weight Load

165

CSI Analysis Reference Manual
• Gravity Load
• Distributed Span Load
• Temperature Load
• Strain and Deformation Load
• Target-Force Load
• Nonlinear Analysis
• Element Output

Overview
The Cable element uses an elastic catenary formulation to represent the behavior of
a slender cable under its own self-weight, temperature, and strain loading. This behavior is highly nonlinear, and inherently includes tension-stiffening (P-delta) and
large-deflection effects. Slack and taut behavior is automatically considered.
In the graphical user interface, you can draw a cable object connecting any two
points. A shape calculator is available to help you determine the undeformed length
of the cable. The undeformed length is extremely critical in determining the behavior of the cable.
An unloaded, slack cable is not stable and has no unique position. Therefore linear
Load Cases that start from zero initial conditions may be meaningless. Instead, all
linear Load Cases should use the stiffness from the end of a nonlinear static Load
Case in which all cables are loaded by their self-weight or other transverse load. For
cases where no transverse load is present on a slack Cable element, the program
will internally assume a very small self-weight load in order to obtain a unique
shape. However, it is better if you apply a realistic load for this purpose.
Each Cable element may be loaded by gravity (in any direction), distributed forces,
strain and deformation loads, and loads due to temperature change. To apply concentrated loads, a cable should be divided at the point of loading, and the force applied to the connecting joint.
Target-force loading is available that iteratively applies deformation load to the cable to achieve a desired tension.
Element output includes the axial force and deflected shape at a user-specified
number of equally-spaced output stations along the length of the element.

166

Overview

Chapter IX

The Cable Element

You have the option when drawing a cable object in the model to use the catenary
element of this chapter, or to model the cable as a series of straight frame elements.
Using frame elements allows you to consider material nonlinearity and complicated loading, but the catenary formulation is better suited to most applications.

Joint Connectivity
A Cable element is represented by a curve connecting two joints, I and j. The two
joints must not share the same location in space. The two ends of the element are
denoted end I and end J, respectively.
The shape of the cable is defined by undeformed length of the cable and the load
acting on it, unless it is taut with no transverse load, in which case it is a straight
line.

Undeformed Length
In the graphical user interface, you can draw a cable object connecting any two
points. A shape calculator is available to help you determine the undeformed length
of the cable. The relationship between the undeformed length and the chord length
(the distance between the two end joints) is extremely critical in determining the
behavior of the cable.
In simple terms, when the undeformed length is longer that the chord length, the cable is slack and has significant sag. When the undeformed length is shorter than the
chord length, the cable is taut and carries significant tension with little sag.
When transverse load acts on the cable, there is a transition range where the
undeformed length is close to the chord length. In this regime, the tension and sag
interact in a highly nonlinear way with the transverse load.
Temperature, strain, and distortion loads can change the length of the cable. The effect of these changes is similar to changing the undeformed length, except that they
do not change the weight of the cable. Strain in the cable due to any source is calculated as the difference between the total length and the undeformed length, divided
by the undeformed length (engineering strain).
If the undeformed length of a cable is shorter than the chord length at the beginning
of a nonlinear analysis, or when the cable is added to the structure during staged
construction, tension will immediately exist in the cable and iteration may be required to bring the structure into equilibrium before any load is applied.
Joint Connectivity

167

CSI Analysis Reference Manual

Shape Calculator
The ultimate purpose of the shape calculator (also called Cable Layout form) in the
graphical user interface is to help you calculate the undeformed length of a cable
object. By default, the undeformed length is assumed to be equal to the chord
length between the undeformed positions of the two end joints.
You may specify a vertical load acting on the cable consisting of:
• Self-weight (always included in the shape calculator)
• Additional weight per unit of undeformed length of the cable
• Addition load per unit horizontal length between the two joints
Note that these loads are only used in the shape calculator. They are not applied to
the element during analysis. Loads to be used for analysis must be assigned to the
elements in Load Patterns.
You may choose one of the following ways to calculate the undeformed length:
• Specifying the undeformed length, either absolute or relative to the chord
length
• Specifying the maximum vertical sag, measured from the chord to the cable
• Specifying the maximum low-point sag, measured from the joint with the
lowest Z elevation to the lowest point on the cable
• Specifying the constant horizontal component of tension in the cable
• Specifying the tension at either end of the cable
• Requesting the shape which gives the minimum tension at either end of the
cable
See Figure 41 (page 169) for a description of the cable geometry.
Note that there does exist an undeformed length that yields a minimum tension at
either end of the cable. Longer cables carry more self weight, increasing the tension. Shorter cables are tauter, also increasing the tension. If you intend to specify
the tension at either end, it is a good idea first to determine what is the minimum
tension, since attempts to specify a lower tension will fail. When a larger value of
tension is specified, the shorter solution will be returned.
It is important to note that the shape calculated here may not actually occur during
any Load Case, nor are the tensions calculated here directly imposed upon the cable. Only the cable length is determined. The deformed shape of the cable and the

168

Shape Calculator

Chapter IX

I, J = Joints
L0 = Undeformed length
LC = Chord length

The Cable Element

H = Horizontal force
TI = Tension at Joint I
TJ = Tension at Joint J

LC
EA,w
EA = Stiffness
w = Weight per length

uMAX
L0

uLOW

uMAX = Maximum vertical sag
uLOW = Low-point sag

Figure 41
Cable Element, showing connectivity, local axes, dimensions, properties, and
shape parameters

tensions it carries will depend upon the loads applied and the behavior of the structure during analysis. For example, the shape calculator assumes that the two end
joints remain fixed. However, if the cable is connected to a deforming structure, the
chord length and its orientation may change, yielding a different solution.

Cable vs. Frame Elements
In the shape calculator, you may specify whether the cable is to be modeled with the
catenary element of this chapter, or using straight frame elements.
If you are interested in highly variable loading or material nonlinearity, using frame
elements may be appropriate. Large-deflection geometrically nonlinear analysis of
the entire structure will be needed to capture full cable behavior. P-delta analysis

Shape Calculator

169

CSI Analysis Reference Manual
with compression limits may be sufficient for some applications. For more information, see Chapter “The Frame Element” (page 105).
For most cable applications, however, the catenary cable element is a better choice,
especially if the cable is very slender, or significant support movement is expected.
Nonlinear analysis is still required, but the geometric nonlinearity (P-delta and/or
large-deflection behavior) of the catenary element will be considered internally regardless of how the rest of the structure is treated.

Number of Segments
In the shape calculator, you may specify the number of segments into which the cable object should be broken. Each segment will be modeled as a single catenary cable or single frame element.
For the catenary element, a single segment is usually the best choice unless you are
considering concentrated loads or intermediate masses for cable vibration.
For the frame element, multiple segments (usually at least eight, and sometimes
many more) are required to capture the shape variation, unless you are modeling a
straight stay or brace, in which case a single segment may suffice.
For more information, see Chapter “Objects and Elements” (page 7)

Degrees of Freedom
The Cable element activates the three translational degrees of freedom at each of its
connected joints. Rotational degrees of freedom are not activated. This element
contributes stiffness to all of these translational degrees of freedom.
For more information, see Topic “Degrees of Freedom” (page 30) in Chapter
“Joints and Degrees of Freedom.”

Local Coordinate System
Each Cable element has its own element local coordinate system which can be
used to define loads acting on the element. The axes of this local system are denoted
1, 2 and 3. The first axis is directed along the chord connecting the two joints of the
element; the remaining two axes lie in the plane perpendicular to the chord with an
orientation that you specify. This coordinate system does not necessarily corre-

170

Degrees of Freedom

Chapter IX

The Cable Element

spond to the direction of sag of the cable, and does not change as the direction of
sag changes during loading.
The definition of the cable element local coordinate system is not usually important
unless you want to apply concentrated or distributed span loads in the element local
system.
The definition of the Cable local coordinate system is exactly the same as for the
Frame element. For more information, see Topics “Local Coordinate System”
(page 108) and “Advanced Local Coordinate System” (page 110) in Chapter “The
Frame Element.”

Section Properties
A Cable Section is a set of material and geometric properties that describe the
cross-section of one or more Cable elements. Sections are defined independently of
the Cable elements, and are assigned to the elements.
Cable Sections are always assumed to be circular. You may specify either the diameter or the cross-sectional area, from which the other value is computed. Bending
moments of inertia, the torsional constant, and shear areas are also computed by the
program for a circular shape.

Material Properties
The material properties for the Section are specified by reference to a previously-defined Material. Isotropic material properties are used, even if the Material
selected was defined as orthotropic or anisotropic. The material properties used by
the Section are:
• The modulus of elasticity, e1, for axial stiffness
• The coefficient of thermal expansion, a1, for temperature loading
• The mass density, m, for computing element mass
• The weight density, w, for computing Self-Weight and Gravity Loads
The material properties e1 and a1 are obtained at the material temperature of each
individual Cable element, and hence may not be unique for a given Section. See
Chapter “Material Properties” (page 69) for more information.

Section Properties

171

CSI Analysis Reference Manual

Geometric Properties and Section Stiffnesses
For the catenary formulation, the section has only axial stiffness, given by a × e1,
where a is the cross-sectional area and e1 is the modulus of elasticity.

Mass
In a dynamic analysis, the mass of the structure is used to compute inertial forces.
The mass contributed by the Cable element is lumped at the joints I and j. No inertial effects are considered within the element itself.
The total mass of the element is equal to the undeformed length of the element multiplied by the mass density, m, and by the cross-sectional area, a. It is apportioned
equally to the two joints. The mass is applied to each of the three translational degrees of freedom: UX, UY, and UZ.
To capture dynamics of a cable itself, it is necessary to divide the cable object into
multiple segments. A minimum of four segments is recommended for this purpose.
For many structures, cable vibration is not important, and no subdivision is necessary.
For more information:
• See Topic “Mass Density” (page 77) in Chapter “Material Properties.”
• See Topic “Section Properties” (page 171) in this Chapter for the definition of
a.
• See Topic “Mass Source” (page 334) in Chapter “Load Patterns”.
• See Chapter “Static and Dynamic Analysis” (page 341).

Self-Weight Load
Self-Weight Load activates the self-weight of all elements in the model. For a Cable element, the self-weight is a force that is distributed along the arc length of the
element. The magnitude of the self-weight is equal to the weight density, w, multiplied by the cross-sectional area, a. As the cable stretches, the magnitude is correspondingly reduced, so that the total load does not change.
Self-Weight Load always acts downward, in the global –Z direction. You may
scale the self-weight by a single scale factor that applies equally to all elements in
the structure.

172

Mass

Chapter IX

The Cable Element

For more information:
• See Topic “Weight Density” (page 78) in Chapter “Material Properties” for the
definition of w.
• See Topic “Section Properties” (page 171) in this Chapter for the definition of
a.
• See Topic “Self-Weight Load” (page 325) in Chapter “Load Patterns.”

Gravity Load
Gravity Load can be applied to each Cable element to activate the self-weight of the
element. Using Gravity Load, the self-weight can be scaled and applied in any direction. Different scale factors and directions can be applied to each element. The
magnitude of a unit gravity load is equal to the weight density, w, multiplied by the
cross-sectional area, a. As the cable stretches, the magnitude is correspondingly reduced, so that the total load does not change.
If all elements are to be loaded equally and in the downward direction, it is more
convenient to use Self-Weight Load.
For more information:
• See Topic “Self-Weight Load” (page 134) in this Chapter for the definition of
self-weight for the Frame element.
• See Topic “Gravity Load” (page 326) in Chapter “Load Patterns.”

Distributed Span Load
The Distributed Span Load is used to apply distributed forces on Cable elements.
The load intensity may be specified as uniform or trapezoidal. However, the load is
actually applied as a uniform load per unit of undeformed length of the cable.
The total load is calculated and divided by the undeformed length to determine the
magnitude of load to apply. As the cable stretches, the magnitude is correspondingly reduced, so that the total load does not change.
The direction of loading may be specified in a fixed coordinate system (global or
alternate coordinates) or in the element local coordinate system.

Gravity Load

173

CSI Analysis Reference Manual
To model the effect of a non-uniform distributed load on a catenary cable object,
specify multiple segments for the single cable object. The distributed load on the
object will be applied as piecewise uniform loads over the segments.
For more information:
• See Topic “Distributed Span Load” (page 137) in Chapter “The Frame Element.”
• See Chapter “Objects and Elements” (page 7) for how a single cable object is
meshed into elements (segments) at analysis time.
• See Chapter “Load Patterns” (page 321).

Temperature Load
Temperature Load creates axial thermal strain in the Cable element. This strain is
given by the product of the Material coefficient of thermal expansion and the temperature change of the element. All specified Temperature Loads represent a
change in temperature from the unstressed state for a linear analysis, or from the
previous temperature in a nonlinear analysis.
The Load Temperature may be constant along the element length or interpolated
from values given at the joints.
See Chapter “Load Patterns” (page 321) for more information.

Strain and Deformation Load
Axial Strain and Deformation Load change the length of the cable element. Deformation Load is the total change in length, whereas Strain Load is the change in
length per unit of undeformed length. Positive values of these loads increase sag
and tend to reduce tension in the cable, while negative values tighten up the cable
and tend to increase tension.
See Chapter “Load Patterns” (page 321) for more information.

Target-Force Load
Target-Force Load is a special type of loading where you specify a desired cable
tension, and deformation load is iteratively applied to achieve the target tension.

174

Temperature Load

Chapter IX

The Cable Element

Since the tension may vary along the length of the cable, you must also specify the
relative location where the desired tension is to occur. Target-Force loading is only
used for nonlinear static and staged-construction analysis. If applied in any other
type of Load Case, it has no effect.
Unlike all other types of loading, target-force loading is not incremental. Rather,
you are specifying the total force that you want to be present in the cable element at
the end of the Load Case or construction stage. The applied deformation that is calculated to achieve that force may be positive, negative, or zero, depending on the
force present in the element at the beginning of the analysis. When a scale factor is
applied to a Load Pattern that contains Target-Force loads, the total target force is
scaled. The increment of applied deformation that is required may change by a different scale factor.
See Topic “Target-Force Load” (page 331) in Chapter “Load Patterns” and Topic
“Target-Force Iteration” (page 444) in Chapter “Nonlinear Static Analysis” for
more information.

Nonlinear Analysis
Nonlinear analysis is required to get meaningful results with the Cable element.
Linear analyses can be performed, but they should always use the stiffness from the
end of a nonlinear static Load Case in which all cables are loaded by their
self-weight or other transverse load. For cases where no transverse load is present
on a slack Cable element, the program will internally assume a very small
self-weight load in order to obtain a unique shape. However, it is better if you apply
a realistic load for this purpose.
Models with Cable elements will usually converge better if you allow a large number of Newton-Raphson iterations in the Load Case, say 25 or more. Convergence
behavior is generally improved by using fewer segments in the cable object, and by
applying larger load increments. Note that this is the opposite behavior than can be
expected for cables modeled as frames, where using more segments and smaller
load increments is usually advantageous.

Element Output
The catenary Cable element produces axial force (tension only) and displacement
output along its length.

Nonlinear Analysis

175

CSI Analysis Reference Manual

176

Element Output

Chapter X

The Shell Element
The Shell element is a type of area object that is used to model membrane, plate,
and shell behavior in planar and three-dimensional structures. The shell material
may be homogeneous or layered through the thickness. Material nonlinearity can
be considered when using the layered shell.
Basic Topics for All Users
• Overview
• Joint Connectivity
• Edge Constraints
• Degrees of Freedom
• Local Coordinate System
• Section Properties
• Mass
• Self-Weight Load
• Uniform Load
• Surface Pressure Load
• Internal Force and Stress Output

177

CSI Analysis Reference Manual
Advanced Topics
• Advanced Local Coordinate System
• Property Modifiers
• Joint Offsets and Thickness Overwrites
• Gravity Load
• Temperature Load

Overview
The Shell element is a three- or four-node formulation that combines membrane
and plate-bending behavior. The four-joint element does not have to be planar.
Each Shell element has its own local coordinate system for defining Material properties and loads, and for interpreting output. Temperature-dependent, orthotropic
material properties are allowed. Each element may be loaded by gravity and uniform loads in any direction; surface pressure on the top, bottom, and side faces; and
loads due to strain and temperature change.
A four-point numerical integration formulation is used for the Shell stiffness.
Stresses and internal forces and moments, in the element local coordinate system,
are evaluated at the 2-by-2 Gauss integration points and extrapolated to the joints of
the element. An approximate error in the element stresses or internal forces can be
estimated from the difference in values calculated from different elements attached
to a common joint. This will give an indication of the accuracy of a given finite-element approximation and can then be used as the basis for the selection of a new and
more accurate finite element mesh.
Structures that can be modeled with this element include:
• Floor systems
• Wall systems
• Bridge decks
• Three-dimensional curved shells, such as tanks and domes
• Detailed models of beams, columns, pipes, and other structural members
Two distinct formulations are available: homogenous and layered.

178

Overview

Chapter X

The Shell Element

Homogeneous
The homogeneous shell combines independent membrane and plate behavior.
These behaviors become coupled if the element is warped (non-planar.) The membrane behavior uses an isoparametric formulation that includes translational inplane stiffness components and a “drilling” rotational stiffness component in the
direction normal to the plane of the element. See Taylor and Simo (1985) and Ibrahimbegovic and Wilson (1991). In-plane displacements are quadratic.
Plate-bending behavior includes two-way, out-of-plane, plate rotational stiffness
components and a translational stiffness component in the direction normal to the
plane of the element. You may choose a thin-plate (Kirchhoff) formulation that neglects transverse shearing deformation, or a thick-plate (Mindlin/Reissner) formulation which includes the effects of transverse shearing deformation. Out-of-plane
displacements are cubic.
For each homogeneous Shell element in the structure, you can choose to model
pure-membrane, pure-plate, or full-shell behavior. It is generally recommended
that you use the full shell behavior unless the entire structure is planar and is adequately restrained.

Layered
The layered shell allows any number of layers to be defined in the thickness direction, each with an independent location, thickness, behavior, and material. Material
behavior may be nonlinear.
Membrane deformation within each layer uses a strain-projection method (Hughes,
2000.) In-plane displacements are quadratic. Unlike for the homogeneous shell, the
“drilling” degrees of freedom are not used, and they should not be loaded. These rotations normal to the plane of the element are only loosely tied to the rigid-body rotation of the element to prevent instability.
For bending, a Mindlin/Reissner formulation is used which always includes transverse shear deformations. Out-of-plane displacements are quadratic and are consistent with the in-plane displacements.
The layered Shell usually represents full-shell behavior, although you can control
this on a layer-by-layer basis. Unless the layering is fully symmetrical in the thickness direction, membrane and plate behavior will be coupled.

Overview

179

CSI Analysis Reference Manual

Joint Connectivity
Each Shell element (and other types of area objects/elements) may have either of
the following shapes, as shown in Figure 42 (page 181):
• Quadrilateral, defined by the four joints j1, j2, j3, and j4.
• Triangular, defined by the three joints j1, j2, and j3.
The quadrilateral formulation is the more accurate of the two. The triangular element is only recommended for locations where the stresses do not change rapidly.
The use of large triangular elements is not recommended where in-plane
(membrane) bending is significant. The use of the quadrilateral element for meshing various geometries and transitions is illustrated in Figure 43 (page 182), so that
triangular elements can be avoided altogether.
Edge constraints are also available to create transitions between mis-matched
meshes without using distorted elements. See Subtopic “Edge Constraints” (page
183) for more information.
The joints j1 to j4 define the corners of the reference surface of the shell element.
For the homogeneous shell this is the mid-surface of the element; for the layered
shell you choose the location of this surface relative to the material layers.
You may optionally assign joint offsets to the element that shift the reference surface away from the joints. See Topic “Joint Offsets and Thickness Overwrites”
(page 203) for more information.

Shape Guidelines
The locations of the joints should be chosen to meet the following geometric conditions:
• The inside angle at each corner must be less than 180°. Best results for the
quadrilateral will be obtained when these angles are near 90°, or at least in the
range of 45° to 135°.
• The aspect ratio of an element should not be too large. For the triangle, this is
the ratio of the longest side to the shortest side. For the quadrilateral, this is the
ratio of the longer distance between the midpoints of opposite sides to the
shorter such distance. Best results are obtained for aspect ratios near unity, or at
least less than four. The aspect ratio should not exceed ten.

180

Joint Connectivity

Chapter X

The Shell Element

Axis 3

Face 3

Face 2
Axis 1

Axis 2

j2
j4

Face 6: Top (+3 face)
Face 5: Bottom (–3 face)

Face 1
Face 4
j1

Four-node Quadrilateral Shell Element

Axis 3

Face 2

Axis 2

Axis 1

j3
j2
Face 6: Top (+3 face)
Face 5: Bottom (–3 face)

Face 1

Face 3
j1
Three-node Triangular Shell Element

Figure 42
Area Element Joint Connectivity and Face Definitions

• For the quadrilateral, the four joints need not be coplanar. A small amount of
twist in the element is accounted for by the program. The angle between the
normals at the corners gives a measure of the degree of twist. The normal at a
Joint Connectivity

181

CSI Analysis Reference Manual

Triangular Region

Infinite Region

Circular Region

Mesh Transition

Figure 43
Mesh Examples Using the Quadrilateral Area Element

corner is perpendicular to the two sides that meet at the corner. Best results are
obtained if the largest angle between any pair of corners is less than 30°. This
angle should not exceed 45°.
These conditions can usually be met with adequate mesh refinement. The accuracy
of the thick-plate and layered formulations is more sensitive to large aspect ratios
and mesh distortion than is the thin-plate formulation.

182

Joint Connectivity

Chapter X

The Shell Element

Figure 44
Connecting Meshes with the Edge Constraints: Left Model – No Edge
Constraints; Right Model – Edge Constraints Assigned to All Elements

Edge Constraints
You can assign automatic edge constraints to any shell element (or any area objects.) When edge con straints are as signed to an element, the pro gram
automatically connects all joints that are on the edge of the element to the adjacent
corner joints of the element. Joints are considered to be on the edge of the element if
they fall within the auto-merge tolerance set by you in the Graphical User Interface.
Edge constraints can be used to connect together mis-matched shell meshes, but
will also connect any element that has a joint on the edge of the shell to that shell.
This include beams, columns, restrained joints, link supports, etc.
These joints are connected by flexible interpolation constraints. This means that the
displacements at the intermediate joints on the edge are interpolated from the displacements of the corner joints of the shell. No overall stiffness is added to the
model; the effect is entirely local to the edge of the element.

Edge Constraints

183

CSI Analysis Reference Manual
Figure 44 (page 183) shows an example of two mis-matched meshes, one connected with edge constraints, and one not. In the connected mesh on the right, edge
constraints were assigned to all elements, although it was really only necessary to
do so for the elements at the transition. Assigning edge constraints to elements that
do not need them has little effect on performance and no effect on results.
The advantage of using edge constraints instead of the mesh transitions shown in
Figure 43 (page 182) is that edge constraints do not require you to create distorted
elements. This can increase the accuracy of the results.
It is important to understand that near any transition, whether using edge constraints or not, the accuracy of stress results is controlled by the largest element
size. Furthermore, the effect of the coarser mesh propagates into the finer mesh for
a distance that is on the order of the size of the larger elements, as governed by St.
Venant’s effect. For this reason, be sure to create your mesh transitions far enough
away from the areas where you need detailed stress results.
Important Note: Edge constraints transfer load from intermediate joints to corner
joints along the edge of a shell. Applying an edge constraint along an edge that is
co-linear with a frame, cable, tendon or link object can result in load being transferred by the edge constraint instead of by that object. Using edge constraints in
these locations should be avoided if detailed results in the frame/cable/tendon/link
are of interest. In particular, frame design results could be affected, and may be
unconservative. Frame/cable/tendon/link objects with only one joint connected to
the edge are not affected, and in fact one of the advantages of using edge constraints
is to connect such elements to a coarse shell mesh, provided that detailed local
stresses in the shells are not needed. When frame/cable/tendon/link objects are
co-linear with an edge constraint, the overall effect of the object on the model is
captured, but local response may not be accurate.

Degrees of Freedom
The Shell element always activates all six degrees of freedom at each of its connected joints. When the element is used as a pure membrane, you must ensure that
restraints or other supports are provided to the degrees of freedom for normal translation and bending rotations. When the element is used as a pure plate, you must ensure that restraints or other supports are provided to the degrees of freedom for inplane translations and the rotation about the normal.
The use of the full shell behavior (membrane plus plate) is recommended for all
three-dimensional structures.

184

Degrees of Freedom

Chapter X

The Shell Element

Note that the “drilling” degree of freedom (rotation about the normal) is not used
for the layered shell and should not be loaded.
See Topic “Degrees of Freedom” (page 30) in Chapter “Joints and Degrees of Freedom” for more information.

Local Coordinate System
Each Shell element (and other types of area objects/elements) has its own element
local coordinate system used to define Material properties, loads and output. The
axes of this local system are denoted 1, 2 and 3. The first two axes lie in the plane of
the element with an orientation that you specify; the third axis is normal.
It is important that you clearly understand the definition of the element local 1-2-3
coordinate system and its relationship to the global X-Y-Z coordinate system. Both
systems are right-handed coordinate systems. It is up to you to define local systems
which simplify data input and interpretation of results.
In most structures the definition of the element local coordinate system is extremely simple. The methods provided, however, provide sufficient power and
flexibility to describe the orientation of Shell elements in the most complicated
situations.
Local axes are first computed for the element without considering joint offsets.
These are called the nominal local axes. If the joint offsets shift the reference surface by a different amount at each joint, the local axes are then transformed by projecting them onto the new normal to determine the actual local coordinate system
used for analysis.
The discussion below considers the calculation of the nominal local axes using the
joints. The transformation for the joint offsets, if needed, is discussed later in Topic
“Joint Offsets and Thickness Overwrites” (page 203).
The simplest method, using the default orientation and the Shell element coordinate angle, is described in this topic. Additional methods for defining the Shell element local coordinate system are described in the next topic.
For more information:
• See Chapter “Coordinate Systems” (page 11) for a description of the concepts
and terminology used in this topic.
• See Topic “Advanced Local Coordinate System” (page 186) in this Chapter.

Local Coordinate System

185

CSI Analysis Reference Manual

Normal Axis 3
Local axis 3 is always normal to the plane of the Shell element. This axis is directed
toward you when the path j1-j2-j3 appears counterclockwise. For quadrilateral elements, the element plane is defined by the vectors that connect the midpoints of the
two pairs of opposite sides.

Default Orientation
The default orientation of the local 1 and 2 axes is determined by the relationship
between the local 3 axis and the global Z axis:
• The local 3-2 plane is taken to be vertical, i.e., parallel to the Z axis
• The local 2 axis is taken to have an upward (+Z) sense unless the element is
horizontal, in which case the local 2 axis is taken along the global +Y direction
• The local 1 axis is horizontal, i.e., it lies in the X-Y plane
The element is considered to be horizontal if the sine of the angle between the local
-3
3 axis and the Z axis is less than 10 .
The local 2 axis makes the same angle with the vertical axis as the local 3 axis
makes with the horizontal plane. This means that the local 2 axis points vertically
upward for vertical elements.

Element Coordinate Angle
The Shell element coordinate angle, ang, is used to define element orientations that
are different from the default orientation. It is the angle through which the local 1
and 2 axes are rotated about the positive local 3 axis from the default orientation.
The rotation for a positive value of ang appears counterclockwise when the local
+3 axis is pointing toward you.
For horizontal elements, ang is the angle between the local 2 axis and the horizontal
+Y axis. Otherwise, ang is the angle between the local 2 axis and the vertical plane
containing the local 3 axis. See Figure 45 (page 187) for examples.

Advanced Local Coordinate System
By default, the element local coordinate system is defined using the element coordinate angle measured with respect to the global +Z and +Y directions, as described

186

Advanced Local Coordinate System

Chapter X

The Shell Element

Z
Top row:
2nd row:
3rd row:
4th row:

ang = 45°
ang = 90°
ang = 0°
ang = –90°

45°
2
1
3

90°

1
2
3
2
–90°
1

Y
2
3

1
For all elements,
Axis 3 points outward,
toward viewer

Figure 45
The Area Element Coordinate Angle with Respect to the Default Orientation

in the previous topic. In certain modeling situations it may be useful to have more
control over the specification of the local coordinate system.
This topic describes how to define the orientation of the tangential local 1 and 2
axes, with respect to an arbitrary reference vector when the element coordinate angle, ang, is zero. If ang is different from zero, it is the angle through which the local
1 and 2 axes are rotated about the positive local 3 axis from the orientation determined by the reference vector. The local 3 axis is always normal to the plane of the
element.
Advanced Local Coordinate System

187

CSI Analysis Reference Manual
For more information:
• See Chapter “Coordinate Systems” (page 11) for a description of the concepts
and terminology used in this topic.
• See Topic “Local Coordinate System” (page 185) in this Chapter.

Reference Vector
To define the tangential local axes, you specify a reference vector that is parallel to
the desired 3-1 or 3-2 plane. The reference vector must have a positive projection
upon the corresponding tangential local axis (1 or 2, respectively). This means that
the positive direction of the reference vector must make an angle of less than 90°
with the positive direction of the desired tangential axis.
To define the reference vector, you must first specify or use the default values for:
• A primary coordinate direction pldirp (the default is +Z)
• A secondary coordinate direction pldirs (the default is +Y). Directions pldirs
and pldirp should not be parallel to each other unless you are sure that they are
not parallel to local axis 3
• A fixed coordinate system csys (the default is zero, indicating the global coordinate system)
• The local plane, local, to be determined by the reference vector (the default is
32, indicating plane 3-2)
You may optionally specify:
• A pair of joints, plveca and plvecb (the default for each is zero, indicating the
center of the element). If both are zero, this option is not used
For each element, the reference vector is determined as follows:
1. A vector is found from joint plveca to joint plvecb. If this vector is of finite
length and is not parallel to local axis 3, it is used as the reference vector V p
2. Otherwise, the primary coordinate direction pldirp is evaluated at the center of
the element in fixed coordinate system csys. If this direction is not parallel to
local axis 3, it is used as the reference vector V p
3. Otherwise, the secondary coordinate direction pldirs is evaluated at the center
of the element in fixed coordinate system csys. If this direction is not parallel to
local axis 3, it is used as the reference vector V p

188

Advanced Local Coordinate System

Chapter X
Z

Intersection of Element
Plane & Global Y-Z Plane

Intersection of Element
Plane & Global Z-X Plane

V1
j3

pldirp = –Y

The Shell Element

pldirp = +X

V3
V1

pldirp = –X

j4
For all cases: local = 32

pldirp = +Y

pldirp = +Z

pldirp = –Z

Intersection of Element
Plane & Global X-Y Plane

Figure 46
Area Element Local Coordinate System Using Coordinate Directions

4. Otherwise, the method fails and the analysis terminates. This will never happen
if pldirp is not parallel to pldirs
A vector is considered to be parallel to local axis 3 if the sine of the angle between
them is less than 10-3.
The use of the coordinate direction method is illustrated in Figure 46 (page 189) for
the case where local = 32.

Determining Tangential Axes 1 and 2
The program uses vector cross products to determine the tangential axes 1 and 2
once the reference vector has been specified. The three axes are represented by the
three unit vectors V1 , V2 and V3 , respectively. The vectors satisfy the cross-product
relationship:
V1 = V2 ´ V3
The tangential axes 1 and 2 are defined as follows:

Advanced Local Coordinate System

189

CSI Analysis Reference Manual
• If the reference vector is parallel to the 3-1 plane, then:
V2 = V3 ´ V p and
V1 = V2 ´ V3
• If the reference vector is parallel to the 3-2 plane, then:
V1 = V p ´ V3 and
V2 = V3 ´ V1
In the common case where the reference vector is parallel to the plane of the element, the tangential axis in the selected local plane will be equal to V p .

Section Properties
A Shell Section is a set of material and geometric properties that describe the
cross-section of one or more Shell objects (elements.) A Shell Section property is a
type of Area Section property. Sections are defined independently of the objects,
and are assigned to the area objects.

Area Section Type
When defining an area section, you have a choice of three basic element types:
• Shell – the subject of this Chapter, with translational and rotational degrees of
freedom, capable of supporting forces and moments
• Plane (stress or strain) – a two-dimensional solid, with translational degrees of
freedom, capable of supporting forces but not moments. This element is covered in Chapter “The Plane Element” (page 215).
• Asolid – axisymmetric solid, with translational degrees of freedom, capable of
supporting forces but not moments. This element is covered in Chapter “The
Asolid Element” (page 225).

Shell Section Type
For Shell sections, you may choose one of the following types of behavior:
• Membrane
– Pure membrane behavior
– Supports only the in-plane forces and the normal (drilling) moment
– Linear, homogeneous material.

190

Section Properties

Chapter X

The Shell Element

• Plate
– Pure plate behavior
– Supports only the bending moments and the transverse force
– Thick- or thin-plate formulation
– Linear, homogeneous material.
• Shell
– Full shell behavior, a combination of membrane and plate behavior
– Supports all forces and moments
– Thick- or thin-plate formulation
– Linear, homogeneous material.
• Layered
– Multiple layers, each with a different material, thickness, behavior, and location
– Provides full-shell behavior unless all layers have only membrane or only
plate behavior
– With full-shell behavior, supports all forces and moments except the “drilling” moment
– Thick-plate formulation; may be nonlinear.
It is generally recommended that you use the full-shell behavior unless the entire
structure is planar and is adequately restrained.

Homogeneous Section Properties
Homogeneous material properties are used for the non-layered Membrane, Plate,
and Shell section types. The following data needs to be specified.
Section Thickness
Each homogeneous Section has a constant membrane thickness and a constant
bending thickness. The membrane thickness, th, is used for calculating:
• The membrane stiffness for full-shell and pure-membrane Sections
• The element volume for the element self-weight and mass calculations
The bending thickness, thb, is use for calculating:

Section Properties

191

CSI Analysis Reference Manual
• The plate-bending and transverse-shearing stiffnesses for full-shell and
pure-plate Sections
Normally these two thicknesses are the same and you only need to specify th. However, for some applications, you may wish to artificially change the membrane or
plate stiffness. For this purpose, you may specify a value of thb that is different
from th. For more detailed control, such as representing corrugated or orthotropic
construction, the use of property modifiers is better. See Topic “Property
Modifiers” (page 201.)
Thickness Formulation
Two thickness formulations are available, which determine whether or not transverse shearing deformations are included in the plate-bending behavior of a plate or
shell element:
• The thick-plate (Mindlin/Reissner) formulation, which includes the effects of
transverse shear deformation
• The thin-plate (Kirchhoff) formulation, which neglects transverse shearing deformation
Shearing deformations tend to be important when the thickness is greater than
about one-tenth to one-fifth of the span. They can also be quite significant in the vicinity of bending-stress concentrations, such as near sudden changes in thickness
or support conditions, and near holes or re-entrant corners.
Even for thin-plate bending problems where shearing deformations are truly negligible, the thick-plate formulation tends to be more accurate, although somewhat
stiffer, than the thin-plate formulation. However, the accuracy of the thick-plate
formulation is more sensitive to large aspect ratios and mesh distortion than is the
thin-plate formulation.
It is generally recommended that you use the thick-plate formulation unless you are
using a distorted mesh and you know that shearing deformations will be small, or
unless you are trying to match a theoretical thin-plate solution.
The thickness formulation has no effect upon membrane behavior, only upon
plate-bending behavior.
Section Material
The material properties for each Section are specified by reference to a previously-defined Material. The material may be isotropic, uniaxial, or orthotropic. If

192

Section Properties

Chapter X

The Shell Element

an anisotropic material is chosen, orthotropic properties will be used. The material
properties used by the Shell Section are:
• The moduli of elasticity, e1, e2, and e3
• The shear modulus, g12, g13, and g23
• The Poisson’s ratios, u12, u13, and u23
• The coefficients of thermal expansion, a1 and a2
• The mass density, m, for computing element mass
• The weight density, w, for computing Self-Weight and Gravity Loads
The properties e3, u13, and u23 are condensed out of the material matrix by assuming a state of plane stress in the element. The resulting, modified values of e1, e2,
g12, and u12 are used to compute the membrane and plate-bending stiffnesses.
The shear moduli, g13 and g23, are used to compute the transverse shearing stiffness if the thick-plate formulation is used. The coefficients of thermal expansion,
a1 and a2, are used for membrane expansion and thermal bending strain.
All material properties (except the densities) are obtained at the material temperature of each individual element.
See Chapter “Material Properties” (page 69) for more information.
Section Material Angle
The material local coordinate system and the element (Shell Section) local coordinate system need not be the same. The local 3 directions always coincide for the
two systems, but the material 1 axis and the element 1 axis may differ by the angle a
as shown in Figure 47 (page 194). This angle has no effect for isotropic material
properties since they are independent of orientation.
See Topic “Local Coordinate System” (page 70) in Chapter “Material Properties”
for more information.

Layered Section Property
For the layered Section property, you define how the section is built-up in the thickness direction. Any number of layers is allowed, even a single layer. Layers are located with respect to a reference surface. This reference surface may be the middle
surface, the neutral surface, the top, the bottom, or any other location you choose.
By default, the reference surface contains the element nodes, although this can be
changed using joint offsets.
Section Properties

193

CSI Analysis Reference Manual
2 (Element)

2 (Material)
1 (Material)

a
1 (Element)

3 (Element, Material)

Figure 47
Shell Section Material Angle

The thick-plate (Mindlin/Reissner) formulation, which includes the effects of
transverse shear deformation, is always used for bending behavior the layered
shell.
The following eight parameters are specified to define each layer, as illustrated in
Figure 48 (page 195.)
(1) Layer Name
The layer name is arbitrary, but must be unique within a single Section. However,
the same layer name can be used in different Sections. This can be useful because
results for a given layer name can be plotted simultaneously for elements having
different Sections.
(2) Layer Distance
Each layer is located by specifying the distance from the reference surface to the
center of the layer, measured in the positive local-3 direction of the element. This
value is called d in the examples below.

194

Section Properties

Chapter X

The Shell Element

Axis 3

Layer “D”

Thickness

Layer “C”

Distance

Layer “B”

Reference
Surface

Layer “A”

Axis 1

Figure 48
Four-Layer Shell, Showing the Reference Surface, the Names of the Layers,
and the Distance and Thickness for Layer “C”
(3) Layer Thickness
Each layer has a single thickness, measured in the local-3 direction of the element.
For modeling rebar or material fibers, you can specify a very thin “smeared” layer
that has an equivalent cross-sectional area. This value is called th in the examples
below.
(4) Layer Type
You can choose between:
• Membrane: Strains in the layer (e 11 , e 22 , g 12 ) are computed only from in-plane
membrane displacements, and stresses in the layer (s 11 , s 22 , s 12 ) contribute
only to in-plane membrane forces ( F11 , F22 , F12 ).
• Plate: Strains in the layer (e 11 , e 22 , g 12 , g 13 , g 23 ) are computed only from
plate-bending rotations and transverse displacements, and stresses in the layer
(s 11 , s 22 , s 12 , s 13 , s 23 ) contribute only to plate-bending moments and transverse shearing forces ( M 11 , M 22 , M 12 ,V13 ,V 23 ).
• Shell, which combines membrane and plate behavior: Strains in the layer
(e 11 , e 22 , g 12 , g 13 , g 23 ) are computed from all displacements and plate-bending rotations, and stresses in the layer (s 11 , s 22 , s 12 , s 13 , s 23 ) contribute to

Section Properties

195

CSI Analysis Reference Manual
all
fo r c es
and
p la t e- b e n d i n g
(F11 , F22 , F12 , M 11 , M 22 , M 12 ,V13 ,V 23 ).

mo me n t s

In most applications, layers should use shell behavior. See shear-wall modeling below for an example of where you might want to separate membrane and plate behavior.
Important Note: Mass and weight are computed only for membrane and shell layers, not for plate layers. This prevents double-counting when independent membrane and plate layers are used for the same material.
(5) Layer Number of Thickness Integration Points
Material behavior is integrated (sampled) at a finite number of points in the thickness direction of each layer. You may choose one to five points for each layer. The
location of these points follows standard Guass integration procedures. This value
is called n in the examples below.
For a single layer of linear material, one point in the thickness direction is adequate
to represent membrane behavior, and two points will capture both membrane and
plate behavior. If you have multiple layers, you may be able to use a single point for
thinner layers.
Nonlinear behavior may require more integration points or more layers in order to
capture yielding near the top and bottom surfaces. Using an excessive number of
integration points can increase analysis time. You may need to experiment to find a
balance between accuracy and computational efficiency.
(6) Layer Material
The material properties for each layer are specified by reference to a previously-defined Material. The material may be isotropic, uniaxial, or orthotropic. If an
anisotropic material is chosen, orthotropic properties will be used. The behavior of
the material depends on the material component behavior chosen for the layer, as
described below.
(7) Layer Material Angle
For orthotropic and uniaxial materials, the material axes may be rotated with respect to the element axes. Each layer may have a different material angle. For example, you can model rebar in two orthogonal directions as two layers of uniaxial
material with material angles 90° apart. This value is called ang in the examples below. For further information, see topic “Section Material Angle” above (page 193.)

196

Section Properties

Chapter X

The Shell Element

(8) Layer Material Behavior
Choose between “Directional” and “Coupled”. Directional behavior can be applied
to all materials and is described in the remainder of this topic. Coupled behavior is
available for concrete materials only, and uses the modified Darwin-Pecknold behavior as described in Chapter “Material Properties”, Topic “Modified Darwin-Pecknold Concrete Model” (page 100).
(9) Layer Material Components
This option applies only to “Directional” material behavior. For each of the three
membrane stress components (s 11 , s 22 , s 12 ), you can choose whether the behavior is linear, nonlinear, or inactive. For a uniaxial material, only the two components (s 11 , s 12 ) are significant, since s 22 = 0 always. Material components are defined in the material local coordinate system, which depends on the material angle
and may not be the same for every layer.
If all three components are linear (two for the uniaxial material), then the linear material matrix is used for the layer, according to Equations (1) to (4) in Chapter “Material Properties” (page 69). Note that for anisotropic materials, the shear coupling
terms in Equation (4) are neglected so that the behavior is the same as given by
Equation (3).
If one or more of the three components is nonlinear or inactive, then all linear components use an uncoupled isotropic linear stress-strain law, all nonlinear components use the nonlinear stress-strain relationship, and all inactive components assume zero stress. The components become uncoupled, and behave as if Poisson’s
ratio is zero. The behavior is summarized in the following table:
Component

Linear

Nonlinear

Inactive

s 11

s 11 = e1 × e 11

Eqns. (5)

s 11 = 0

s 22

s 22 = e1 × e 22

Eqns. (5)

s 22 = 0

s 12

s 12 = e1 × e 12

Eqns. (6)

s 12 = 0

Note that the linear equation for s 12 is for an isotropic material with zero Poisson’s
ratio. See Chapter “Material Properties” (page 69) for Equations (5) and (6).
For a uniaxial material, s 22 = 0 and s 12 is half the value given in the table above.

Section Properties

197

CSI Analysis Reference Manual
Transverse shear behavior is always linear, and is controlled by the corresponding
moment components. For a layer of type Membrane, the transverse shear stresses
(s 13 , s 23 ) are both zero. For a layer of type Plate or Shell:
• s 13 = 0 if s 11 is inactive, else s 13 = g13 × g 13
• s 23 = 0 if s 22 is inactive, else s 23 = g23 × g 23
Interaction Between Layers
Layers are defined independently, and it is permissible for layers to overlap, or for
gaps to exist between the layers. It is up to you to decide what is appropriate.
For example, when modeling a concrete slab, you can choose a single layer to represent the full thickness of concrete, and four layers to represent rebar (two near the
top at a 90° angle to each other, and two similar layers at the bottom.) These rebar
layers would be very thin, using an equivalent thickness to represent the cross-sectional area of the steel. Because the layers are so thin, there is no need to worry
about the fact that the rebar layers overlap the concrete. The amount of excess concrete that is contained in the overlapped region is very small.
Layers are kinematically connected by the Mindlin/Reissner assumption that normals to the reference surface remain straight after deformation. This is the shell
equivalent to the beam assumption that plane sections remain plane.
Integration in the Plane
Force-deflection behavior is computed by integrating the stress-strain behavior
through the thickness and over the 1-2 plane of the element. You can specify the
number of integration points in the thickness direction of each layer as described
above.
For each of these thickness locations, integration in the plane is performed at the
standard 2 x 2 Gauss points (coordinates ±0.577 on a square of size ±1.0). Nonlinear behavior is sampled only at these points. This is equivalent to having two fibers,
located approximately at the ¼ and ¾ points, in each of the local 1 and 2 directions.
Plotted or tabulated stresses at locations other than the four Gauss points are interpolated or extrapolated, and do not necessarily represent the sampled nonlinear
stresses. For this reason, stresses at the joints may sometimes appear to exceed failure stresses.

198

Section Properties

Chapter X

The Shell Element

Example: Nonlinear Shear-Wall, “Realistic” Modeling
An important application for the layered shell element is nonlinear shear-wall modeling, and it will serve as an example for other applications. Let's consider an 18
inch (457 mm) thick vertical wall, with two vertical and two horizontal layers of
rebar having 3 inch (76 mm) cover from both faces. The two horizontal layers together provide a 1% rebar area ratio, and the two vertical layers together provide an
area ratio of 2%.
When modeling linear behavior, it is not usually necessary to include the rebar, but
it is essential for nonlinear behavior. In the simplest case, the entire wall section
will be considered as nonlinear for both membrane and bending behavior, leading
to the most “realistic”, if not the most practical model. The requires a layered section with five layers:
“Realistic” Shear-Wall Model
n

s 11

s 22

s 12

0°

+6.

0°

0.09

-6.

0°

Rebar

0.18

+6.

90°

Rebar

0.18

-6.

90°

Layer

Type

Material

ang

Shell

Conc

18.00

Shell

Rebar

0.09

Shell

Rebar

Shell

For the stress components, “N” indicates nonlinear, “L” indicates linear, and “-”
indicates inactive. The concrete material behavior may be “Directional” or “Coupled”.
Note that for the rebar, s 11 is always nonlinear. Vertical rebar is defined by setting
the material angle to 90°, which aligns it with the shell local-2 axis. Hence the vertical rebar stress s 11 corresponds to shell s 22 .
Also note that for the rebar, s 12 is set to be nonlinear. This allows the rebar to carry
shear when the concrete cracks. This can taken to represent dowel action, although
no information on actual dowel behavior is present in the model, so it is only an approximation. You must use your engineering judgement to determine if this approach is suitable to your needs. The most conservative approach is to set the rebar
stress component s 12 to be inactive.

Section Properties

199

CSI Analysis Reference Manual
Example: Nonlinear Shear-Wall, “Practical” Modeling
The five-layer model above seems realistic, but presents many failure mechanisms
that may cloud the engineering information required for performance-based design. Whenever possible, the simplest model should be used to meet the engineering goals. Doing this will make the analysis run faster and make the interpretation
of results easier.
With this in mind, a more practical model is presented below, with only the vertical
membrane stresses taken to be nonlinear. Such a model may be suitable for taller
shear walls where column-like behavior governs:
“Practical” Shear-Wall Model
n

s 11

s 22

s 12

0°

+6.

90°

0.18

-6.

90°

16.00

0°

Layer

Type

Material

ang

Membr

Conc

18.00

Membr

Rebar

0.18

Membr

Rebar

Plate

Conc

In this model, only membrane behavior is nonlinear, and only for the vertical stress
component s 22 . This corresponds to rebar stress component s 11 when the material
angle is 90°. Concrete material behavior is “Directional”.
It is generally not necessary to include rebar for linear behavior, so the horizontal
rebar is omitted, and the rebar shear stress component s 12 is set to be inactive.
Out-of-plane behavior is assumed to be linear, so a single concrete plate layer is
used. The thickness has been reduced to account for cracking without explicit nonlinear modeling. Plate bending stiffness is proportional to the cube of the thickness.
Example: In-fill Panel
There are many ways to model an infill panel. Two approaches will be presented
here, both intended to represent membrane shear resistance only. The simplest is a
single layer of concrete material carrying only membrane shear stress, as shown in
the following model:

200

Section Properties

Chapter X

The Shell Element

Infill Wall - Simple Shear Model
Layer

Type

Material

Membr

Conc

18.00

ang
0.

0°

s 11

s 22

s 12

In the second model, the concrete is assumed to act as compression struts along the
two diagonals. For a square panel, these two struts would act at material angles of
±45°, as shown in the following model:
Infill Wall - Compression Strut Model
Layer

Type

Material

Membr

Conc

18.00

Membr

Conc

18.00

s 11

s 22

s 12

45°

-45°

ang

Other possibilities exist. For both models, there is no vertical or horizontal membrane stiffness, and no plate-bending stiffness. Therefore, these models should only
be used when the element is completely surrounded by frame or other supporting
elements, and the elements should not be meshed.
Summary
As these examples show, you have considerable flexibility to create layered shell
sections to represent a variety of linear and nonlinear behavior. The simplest model
that accomplishes the engineering goals should be used. Even when more complicated models may be warranted, it is recommended to start with simple, mostly linear models, and increase the level of complexity and nonlinearity as you gain experience with your model and its behavior.
To assure a stable model, be sure to include layers that, when combined, provide
both membrane and plate contributions to each of the three stress components.

Property Modifiers
You may specify scale factors to modify the computed section properties. These
may be used, for example, to account for cracking of concrete, corrugated or
orthotropic fabrication, or for other factors not easily described in the geometry and

Property Modifiers

201

CSI Analysis Reference Manual
material property values. Individual modifiers are available for the following ten
terms:
• Membrane stiffness corresponding to force F11
• Membrane stiffness corresponding to force F22
• Membrane stiffness corresponding to force F12
• Plate bending stiffness corresponding to moment M11
• Plate bending stiffness corresponding to moment M22
• Plate bending stiffness corresponding to moment M12
• Plate shear stiffness corresponding to force V12
• Plate shear stiffness corresponding to force V13
• Mass
• Weight
The stiffness modifiers affect only homogenous elements, not layered elements.
The mass and weight modifiers affect all elements.
See Topic “Internal Force and Stress Output” (page 210) for the definition of the
force and moment components above.
You may specify multiplicative factors in two places:
• As part of the definition of the section property
• As an assignment to individual elements.
If modifiers are assigned to an element and also to the section property used by that
element, then both sets of factors multiply the section properties.

Named Property Sets
In addition to directly assigning property modifiers to shell elements, you can apply
them to a shell element in a staged-construction Load Case using a Named Property
Set of Shell Property Modifiers. A Named Property Set includes the same ten factors above that can be assigned to an element.
When a Named Property Set is applied to an element in a particular stage of a Load
Case, it replaces only the values that are assigned to the element or that had been applied in a previous stage; values computed by the Direct Analysis Method of design
are also replaced. However, property modifiers specified with the section property
remain in force and are not affected by the application of a Named Property Set.

202

Property Modifiers

Chapter X

The Shell Element

The net effect is to use the factors specified in the Named Property Set multiplied
by the factors specified in the section property.
When property modifiers are changed in a staged construction Load Case, they do
not change the response of the structure up to that stage, but only affect subsequent
response. In other words, the effect is incremental. For example, consider a cantilever with only default (unity) property modifiers, and a staged construction case as
follows:
• Stage 1: Self-weight load is applied, resulting in a tip deflection of 1.0 and
a support moment of 1000.
• Stage 2: Named Property Set “A” is applied that multiplies all stiffnesses
by 2.0, and the mass and weight by 1.0. The tip deflection and support moment do not change.
• Stage 3: Self-weight load is applied again (incrementally). The resulting
tip deflection is 1.5 and the support moment is 2000. Compared to Stage 1,
the same incremental load is applied, but the structure is twice as stiff.
• Stage 4: Named Property Set “B” is applied that multiplies all stiffnesses,
as well as the mass and weight, by 2.0. The tip deflection and support moment do not change.
• Stage 5: Self-weight load is applied again (incrementally). The resulting
tip deflection is 2.5 and the support moment is 4000. Compared to Stage 1,
twice the incremental load is applied, and the structure is twice as stiff

Joint Offsets and Thickness Overwrites
You may optionally assign joint offset and thickness overwrites to any element.
These are often used together to align the top or bottom of the shell element with a
given surface. See Figure 49 (page 204.)

Joint Offsets
Joint offsets are measured from the joint to the reference surface of the element in
the direction normal to the plane of the joints. If the joints define a warped surface,
the plane is determine by the two lines connecting opposite mid-sides (i.e., the middle of j1-j2 to the middle of j3-j4, and the middle of j1-j3 to the middle of j2-j4.) A
positive offset is in the same direction as the positive local-3 axis of the element.
Joint offsets locate the reference plane of the element. For homogeneous shells, this
is the mid-surface of the element. For layered shells, the reference surface is the
Joint Offsets and Thickness Overwrites

203

CSI Analysis Reference Manual

Axis 3

Thickness 2
ce
Reference Surfa

Thickness 1

Axis 1

Offset 2

Offset 1
Joint Plane
Joint 1

Joint 2

Figure 49
Joint Offsets and Thickness Overwrites for a Homogeneous Shell
Edge View shown Along One Side
surface you used to locate the layers in the section. By changing the reference surface in a layered section, you can accomplish the same effect as using joint offsets
that are equal at the joints. See Topic “Layered Section Property” (page 193) for
more information.
When you assign joint offsets to a shell element, you can explicitly specify the offsets at the element joints, or you can reference a Joint Pattern. Using a Joint Pattern
makes it easy to specify consistently varying offsets over many elements. See
Topic “Joint Patterns” (page 332) in Chapter “Load Patterns” for more information.
Note that when the neutral surface of the element, after applying joint offsets, is no
longer in the plane of the joints, membrane and plate-bending behavior become
coupled. If you apply a diaphragm constraint to the joints, this will also constrain
bending. Likewise, a plate constraint will constrain membrane action.

Effect of Joint Offsets on the Local Axes
The insertion points can interact significantly with the element local coordinate
system. As described previously, the nominal local axes are computed for zero joint
offsets, such the reference surface connects to the joints.
If there are no joint offsets, or the joint offsets are equal at the joints, the offset reference plane is parallel to the original reference plane of the joints. In this case no

204

Joint Offsets and Thickness Overwrites

Chapter X

The Shell Element

further transformation is necessary, and the element local axes are the same as the
nominal local axes.
~
If the joint offsets are not equal, a new local 3 axis (V3 ) is computed as the normal
to the plane determined from the two lines connecting the midsides of the reference
surface after applying the offsets to the joints.
If the normal has changed direction, then the element local coordinate system is
computed as follows:
~
~
V1 = V2 ´ V3 and
~
~
~
V2 = V3 ´ V1
where V1 , V2 , and V3 and the nominal local axes computed previously based on the
~ ~
~
joints; and V1 , V2 , and V3 are the transformed local axes used for analysis. If V2 is
~
vertical, then V1 will always be horizontal. Note that the two systems are identical if
~
V3 = V3 , the usual case.
The nominal axes are used only for determining the direction of joint offsets. The
transformed axes are used for all analysis purposes, including loading and results
output.

Thickness Overwrites
Normally the thickness of the shell element is defined by the Section Property assigned to the element. You have the option to overwrite this thickness, including
the ability to specify a thickness that varies over the element.
Currently this option only affects homogeneous shells. The thickness of layered
shells is not changed. When thickness overwrites are assigned to a homogeneous
shell, both the membrane thickness, th, and the bending thickness, thb, take the
overwritten value.
When you assign thickness overwrites to a shell element, you can explicitly specify
the thicknesses at the element joints, or you can reference a Joint Pattern. Using a
Joint Pattern makes it easy to specify consistently varying thickness over many elements. See Topic “Joint Patterns” (page 332) in Chapter “Load Patterns” for more
information.
As an example, suppose you have a variable thickness slab, and you want the top
surface to lie in a single flat plane. Define a Joint Pattern that defines the thickness
over the slab. Draw the elements so that the joints lie in the top plane. Assign thickJoint Offsets and Thickness Overwrites

205

CSI Analysis Reference Manual
ness overwrites to all the elements using the Joint Pattern with a scale factor of one,
and assign the joint offsets using the same Joint Pattern, but with a scale factor of
one-half (positive or negative, as needed).

Mass
In a dynamic analysis, the mass of the structure is used to compute inertial forces.
The mass contributed by the Shell element is lumped at the element joints. No inertial effects are considered within the element itself.
The total mass of the element is equal to the integral over the plane of the element of
the mass density, m, multiplied by the membrane thickness, th, for homogeneous
sections, and the sum of the masses of the individual layers for layered sections.
Note that for layered shells, mass is computed only for membrane and shell layers,
not for plate layers. The total mass may be scaled by the mass property modifier.
The total mass is apportioned to the joints in a manner that is proportional to the diagonal terms of the consistent mass matrix. See Cook, Malkus, and Plesha (1989)
for more information. The total mass is applied to each of the three translational degrees of freedom: UX, UY, and UZ. No mass moments of inertia are computed for
the rotational degrees of freedom.
For more information:
• See Topic “Mass Density” (page 77) in Chapter “Material Properties”.
• See Topic “Property Modifiers” (page 201) in this chapter.
• See Topic “Mass Source” (page 334) in Chapter “Load Patterns”.
• See Chapter “Static and Dynamic Analysis” (page 341).

Self-Weight Load
Self-Weight Load activates the self-weight of all elements in the model. For a Shell
element, the self-weight is a force that is uniformly distributed over the plane of the
element. The magnitude of the self-weight is equal to the weight density, w, multiplied by the membrane thickness, th, for homogeneous sections, and the sum of the
weights of the individual layers for layered sections. Note that for layered shells,
weight is computed only for membrane and shell layers, not for plate layers. The total weight may be scaled by the weight property modifier.

206

Mass

Chapter X

The Shell Element

Self-Weight Load always acts downward, in the global –Z direction. You may
scale the self-weight by a single scale factor that applies equally to all elements in
the structure.
For more information:
• See Topic “Weight Density” (page 78) in Chapter “Material Properties” for the
definition of w.
• See Topic “Property Modifiers” (page 201) in this chapter.
• See Topic “Self-Weight Load” (page 325) in Chapter “Load Patterns.”

Gravity Load
Gravity Load can be applied to each Shell element to activate the self-weight of the
element. Using Gravity Load, the self-weight can be scaled and applied in any direction. Different scale factors and directions can be applied to each element.
If all elements are to be loaded equally and in the downward direction, it is more
convenient to use Self-Weight Load.
For more information:
• See Topic “Self-Weight Load” (page 191) in this Chapter for the definition of
self-weight for the Shell element.
• See Topic “Gravity Load” (page 326) in Chapter “Load Patterns.”

Uniform Load
Uniform Load is used to apply uniformly distributed forces to the midsurfaces of
the Shell elements. The direction of the loading may be specified in a fixed coordinate system (global or Alternate Coordinates) or in the element local coordinate
system.
Load intensities are given as forces per unit area. Load intensities specified in different coordinate systems are converted to the element local coordinate system and
added together. The total force acting on the element in each local direction is given
by the total load intensity in that direction multiplied by the area of the mid-surface.
This force is apportioned to the joints of the element.
Forces given in fixed coordinates can optionally be specified to act on the projected
area of the mid-surface, i.e., the area that can be seen along the direction of loading.
Gravity Load

207

CSI Analysis Reference Manual
Uniformly distributed force uzp acts on
the projected area of the midsurface.
This is equivalent to force uzp cosq
acting on the full midsurface area.

uzp

3
q

Global
Y

Edge View of Shell Element

Figure 50
Example of Uniform Load Acting on the Projected Area of the Mid-surface

The specified load intensity is automatically multiplied by the cosine of the angle
between the direction of loading and the normal to the element (the local 3 direction). This can be used, for example, to apply distributed snow or wind loads. See
Figure 50 (page 208).
See Chapter “Load Patterns” (page 321) for more information.

Surface Pressure Load
The Surface Pressure Load is used to apply external pressure loads upon any of the
six faces of the Shell element. The definition of these faces is shown in Figure 42
(page 181). Surface pressure always acts normal to the face. Positive pressures are
directed toward the interior of the element.
The pressure may be constant over a face or interpolated from values given at the
joints. The values given at the joints are obtained from Joint Patterns, and need not
be the same for the different faces. Joint Patterns can be used to easily apply hydrostatic pressures.
The bottom and top faces are denoted Faces 5 and 6, respectively. The top face is
the one visible when the +3 axis is directed toward you and the path j1-j2-j3 ap-

208

Surface Pressure Load

Chapter X

The Shell Element

pears counterclockwise. The pressure acting on the bottom or top face is integrated
over the plane of the element and apportioned to the corner joints..
The sides of the element are denoted Faces 1 to 4 (1 to 3 for the triangle), counting
counterclockwise from side j1-j2 when viewed from the top. The pressure acting
on a side is multiplied by the thickness, th, integrated along the length of the side,
and apportioned to the two joints on that side. the bending thickness, thb, is not
used.
For layered shells, the thickness used for edge loads is measured from the bottom of
the bottom-most membrane or shell layer to the top of the top-most membrane or
shell layer. Gaps between layers and overlapping layers do not change the thickness used. Plate layers are not considered when computing the loaded thickness.
For more information:
• See Topic “Thickness” (page 193) in this Chapter for the definition of th.
• See Chapter “Load Patterns” (page 321).

Temperature Load
Temperature Load creates thermal strain in the Shell element. This strain is given
by the product of the Material coefficient of thermal expansion and the temperature
change of the element. All specified Temperature Loads represent a change in temperature from the unstressed state for a linear analysis, or from the previous temperature in a nonlinear analysis.
Two independent Load Temperature fields may be specified:
• Temperature, t, which is constant through the thickness and produces membrane strains
• Temperature gradient, t3, which is linear in the thickness direction and produces bending strains
The temperature gradient is specified as the change in temperature per unit length.
The temperature gradient is positive if the temperature increases (linearly) in the
positive direction of the element local 3 axis. The gradient temperature is zero at the
mid-surface, hence no membrane strain is induced.
Each of the two Load Temperature fields may be constant over the plane of the element or interpolated from values given at the joints.
See Chapter “Load Patterns” (page 321) for more information.
Temperature Load

209

CSI Analysis Reference Manual

Strain Load
Eight types of strain load are available, one corresponding to each of the internal
forces and moments in a shell element. These are:
• Membrane strain loads, e 11 , e 22 , and e 12 , representing change in the size and
shape of the element that is uniform through the thickness. Positive membrane
strain causes negative corresponding membrane forces in a restrained element.
• Bending strain loads, k11 , k 22 , and k12 , representing change in the size and
shape of the element that varies linearly through the thickness. Positive bending strain causes negative corresponding bending moments in a restrained element.
• Shear strain loads, g 13 and g 23 , representing the change in angle between the
midsurface normal and the midsurface. Positive shear strain causes negative
corresponding shear forces in a restrained element. Shear strain load has no effect on a thin shell or thin plate element, for which shear strain is assumed to be
zero.
Any of the strain load fields may be constant over the plane of the element or interpolated from values given at the joints.
In an unrestrained element, strain loads cause deformation but induce no internal
forces. This unrestrained deformation has the same sign as would deformation
caused by the corresponding (conjugate) forces and moments acting on the element. On the other hand, strain loading in a restrained element causes corresponding internal forces that have the opposite sign as the applied strain. Most elements
in a real structure are connected to finite stiffness, and so strain loading would
cause both deformation and internal forces. Note that the effects of shear and bending strain loading are coupled.
For more information, see Topic “Internal Force and Stress Output” below, and
also Chapter “Load Patterns” (page 321.)

Internal Force and Stress Output
The Shell element internal forces (also called stress resultants) are the forces and
moments that result from integrating the stresses over the element thickness. For a
homogeneous shell, these internal forces are:
• Membrane direct forces:

210

Strain Load

Chapter X
F11 = ò

+ th / 2

- th / 2

F22 = ò

+ th / 2

- th / 2

s 11 dx 3

The Shell Element
(Eqns. 1)

s 22 dx 3

• Membrane shear force:
F12 = ò

+ th / 2

- th / 2

s 12 dx 3

• Plate bending moments:
M 11 = - ò

+ thb/ 2

- thb/ 2

M 22 = - ò

+ thb/ 2

- thb/ 2

x 3 s 11 dx 3
x 3 s 22 dx 3

• Plate twisting moment:
M 12 = - ò

+ thb/ 2

- thb/ 2

x 3 s 12 dx 3

• Plate transverse shear forces:
V13 = ò

+ thb/ 2

- thb/ 2

V 23 = ò

+ thb/ 2

- thb/ 2

s 13 dx 3
s 23 dx 3

where x 3 represents the thickness coordinate measured from the mid-surface of the
element, th is the membrane thickness, and thb is the plate-bending thickness.
For a layered shell, the definitions are the same, except that the integrals of the
stresses are now summed over all layers, and x 3 is always measured from the reference surface.
It is very important to note that these stress resultants are forces and moments per
unit of in-plane length. They are present at every point on the mid-surface of the element.
For the thick-plate (Mindlin/Reissner) formulation of the homogeneous shell, and
for the layered shell, the shear stresses are computed directly from the shearing deformation. For the thin-plate homogeneous shell, shearing deformation is assumed
to be zero, so the transverse shear forces are computed instead from the moments
using the equilibrium equations:
V13 = -

dM 11 dM 12
dx 1
dx 2

Internal Force and Stress Output

211

CSI Analysis Reference Manual
V 23 = -

dM 12 dM 22
dx 1
dx 2

Where x 1 and x 2 are in-plane coordinates parallel to the local 1 and 2 axes.
The sign conventions for the stresses and internal forces are illustrated in Figure 51
(page 213). Stresses acting on a positive face are oriented in the positive direction
of the element local coordinate axes. Stresses acting on a negative face are oriented
in the negative direction of the element local coordinate axes.
A positive face is one whose outward normal (pointing away from element) is in the
positive local 1 or 2 direction.
Positive internal forces correspond to a state of positive stress that is constant
through the thickness. Positive internal moments correspond to a state of stress that
varies linearly through the thickness and is positive at the bottom. Thus for a homogeneous shell:
F11 12 M 11
x3
3
th
thb
12 M 22
F
= 22 x3
3
th
thb

s 11 =
s 22

(Eqns. 2)

F12 12 M 12
x3
3
th
thb
V
= 13
thb
V
= 23
thb

s 12 =
s 13
s 23

s 33 = 0
The transverse shear stresses given here are average values. The actual shear stress
distribution is parabolic, being zero at the top and bottom surfaces and taking a
maximum or minimum value at the mid-surface of the element.
The force and moment resultants are reported identically for homogeneous and layered shells. Stresses are reported for homogeneous shells at the top and bottom surfaces, and are linear in between. For the layered shell, stresses are reported in each
layer at the integration points, and at the top, bottom, and center of the layer.
The stresses and internal forces are evaluated at the standard 2-by-2 Gauss integration points of the element and extrapolated to the joints. Although they are reported

212

Internal Force and Stress Output

Chapter X

The Shell Element

F-MIN
Axis 2

F-MAX
j3

Forces are per unit
of in-plane length

Axis 1

ANGLE
F22
F12

j4
F11

Transverse Shear (not shown)
Positive transverse shear forces and
stresses acting on positive faces
point toward the viewer

j1
STRESSES AND MEMBRANE FORCES
Stress Sij Has Same Definition as Force Fij

Axis 2
M-MIN

M-MAX

Moments are per unit
of in-plane length

ANGLE
M12

M22

Axis 1

M12
M11

PLATE BENDING AND TWISTING MOMENTS

Figure 51
Shell Element Stresses and Internal Resultant Forces and Moments

at the joints, the stresses and internal forces exist over the whole element. See
Cook, Malkus, and Plesha (1989) for more information.

Internal Force and Stress Output

213

CSI Analysis Reference Manual
Principal values and the associated principal directions are available for Load
Cases and Load Combinations that are single valued. The angle given is measured
counterclockwise (when viewed from the top) from the local 1 axis to the direction
of the maximum principal value.
For more information, see Topic “Stresses and Strains” (page 71) in Chapter “Material Properties”.

214

Internal Force and Stress Output

C h a p t e r XI

The Plane Element
The Plane element is used to model plane-stress and plane-strain behavior in
two-dimensional solids. The Plane element/object is one type of area object. Depending on the type of section properties you assign to an area, the object could also
be used to model shell and axisymmetric solid behavior. These types of elements
are discussed in the previous and following Chapters.
Advanced Topics
• Overview
• Joint Connectivity
• Degrees of Freedom
• Local Coordinate System
• Stresses and Strains
• Section Properties
• Mass
• Self-Weight Load
• Gravity Load
• Surface Pressure Load
• Pore Pressure Load

215

CSI Analysis Reference Manual
• Temperature Load
• Stress Output

Overview
The Plane element is a three- or four-node element for modeling two-dimensional
solids of uniform thickness. It is based upon an isoparametric formulation that includes four optional incompatible bending modes. The element should be planar; if
it is not, it is formulated for the projection of the element upon an average plane
calculated for the element.
The incompatible bending modes significantly improve the bending behavior of
the element if the element geometry is of a rectangular form. Improved behavior is
exhibited even with non-rectangular geometry.
Structures that can be modeled with this element include:
• Thin, planar structures in a state of plane stress
• Long, prismatic structures in a state of plane strain
The stresses and strains are assumed not to vary in the thickness direction.
For plane-stress, the element has no out-of-plane stiffness. For plane-strain, the element can support loads with anti-plane shear stiffness.
Each Plane element has its own local coordinate system for defining Material properties and loads, and for interpreting output. Temperature-dependent, orthotropic
material properties are allowed. Each element may be loaded by gravity (in any direction); surface pressure on the side faces; pore pressure within the element; and
loads due to temperature change.
An 2 x 2 numerical integration scheme is used for the Plane. Stresses in the element
local coordinate system are evaluated at the integration points and extrapolated to
the joints of the element. An approximate error in the stresses can be estimated from
the difference in values calculated from different elements attached to a common
joint. This will give an indication of the accuracy of the finite element approximation and can then be used as the basis for the selection of a new and more accurate
finite element mesh.

216

Overview

Chapter XI

The Plane Element

Joint Connectivity
The joint connectivity and face definition is identical for all area objects, i.e., the
Shell, Plane, and Asolid elements. See Topic “Joint Connectivity” (page 180) in
Chapter “The Shell Element” for more information.
The Plane element is intended to be planar. If you define a four-node element that is
not planar, an average plane will be fit through the four joints, and the projection of
the element onto this plane will be used.

Degrees of Freedom
The Plane element activates the three translational degrees of freedom at each of its
connected joints. Rotational degrees of freedom are not activated.
The plane-stress element contributes stiffness only to the degrees of freedom in the
plane of the element. It is necessary to provide restraints or other supports for the
translational degrees of freedom that are normal to this plane; otherwise, the structure will be unstable.
The plane-strain element models anti-plane shear, i.e., shear that is normal to the
plane of the element, in addition to the in-plane behavior. Thus stiffness is created
for all three translational degrees of freedom.
See Topic “Degrees of Freedom” (page 30) in Chapter “Joints and Degrees of Freedom” for more information.

Stresses and Strains
The Plane element models the mid-plane of a structure having uniform thickness,
and whose stresses and strains do not vary in the thickness direction.

Joint Connectivity

217

CSI Analysis Reference Manual
Plane-stress is appropriate for structures that are thin compared to their planar dimensions. The thickness normal stress (s 33 ) is assumed to be zero. The thickness
normal strain (e 33 ) may not be zero due to Poisson effects. Transverse shear
stresses (s 12 , s 13 ) and shear strains (g 12 , g 13 ) are assumed to be zero. Displacements in the thickness (local 3) direction have no effect on the element.
Plane-strain is appropriate for structures that are thick compared to their planar dimensions. The thickness normal strain (e 33 ) is assumed to be zero. The thickness
normal stress (s 33 ) may not be zero due to Poisson effects. Transverse shear
stresses (s 12 , s 13 ) and shear strains (g 12 , g 13 ) are dependent upon displacements in
the thickness (local 3) direction.
See Topic “Stresses and Strains” (page 71) in Chapter “Material Properties” for
more information.

Section Properties
A Plane Section is a set of material and geometric properties that describe the
cross-section of one or more Plane elements. Sections are defined independently of
the Plane elements, and are assigned to the area objects.

Section Type
When defining an area section, you have a choice of three basic element types:
• Plane (stress or strain) – the subject of this Chapter, a two-dimensional solid,
with translational degrees of freedom, capable of supporting forces but not moments.
• Shell – shell, plate, or membrane, with translational and rotational degrees of
freedom, capable of supporting forces and moments. This element is covered in
Chapter “The Shell Element” (page 177).
• Asolid – axisymmetric solid, with translational degrees of freedom, capable of
supporting forces but not moments. This element is covered in Chapter “The
Asolid Element” (page 225).
For Plane sections, you may choose one of the following sub-types of behavior:
• Plane stress
• Plane strain, including anti-plane shear

218

Section Properties

Chapter XI

The Plane Element

Material Properties
The material properties for each Plane element are specified by reference to a previously-defined Material. Orthotropic properties are used, even if the Material selected was defined as anisotropic. The material properties used by the Plane element are:
• The moduli of elasticity, e1, e2, and e3
• The shear modulus, g12
• For plane-strain only, the shear moduli, g13 and g23
• The Poisson’s ratios, u12, u13 and u23
• The coefficients of thermal expansion, a1, a2, and a3
• The mass density, m, for computing element mass
• The weight density, w, for computing Self-Weight and Gravity Loads
The properties e3, u13, u23, and a3 are not used for plane stress. They are used to
compute the thickness-normal stress (s 33 ) in plane strain.
All material properties (except the densities) are obtained at the material temperature of each individual element.
See Chapter “Material Properties” (page 69) for more information.

Material Angle
The material local coordinate system and the element (Plane Section) local coordinate system need not be the same. The local 3 directions always coincide for the
two systems, but the material 1 axis and the element 1 axis may differ by the angle a
as shown in Figure 52 (page 220). This angle has no effect for isotropic material
properties since they are independent of orientation.
See Topic “Local Coordinate System” (page 70) in Chapter “Material Properties”
for more information.

Thickness
Each Plane Section has a uniform thickness, th. This may be the actual thickness,
particularly for plane-stress elements; or it may be a representative portion, such as
a unit thickness of an infinitely-thick plane-strain element.

Section Properties

219

CSI Analysis Reference Manual
2 (Element)

2 (Material)
1 (Material)

a
1 (Element)

3 (Element, Material)

Figure 52
Plane Element Material Angle

The element thickness is used for calculating the element stiffness, mass, and loads.
Hence, joint forces computed from the element are proportional to this thickness.

Incompatible Bending Modes
By default each Plane element includes four incompatible bending modes in its
stiffness formulation. These incompatible bending modes significantly improve
the bending behavior in the plane of the element if the element geometry is of a rectangular form. Improved behavior is exhibited even with non-rectangular geometry.
If an element is severely distorted, the inclusion of the incompatible modes should
be suppressed. The element then uses the standard isoparametric formulation. Incompatible bending modes may also be suppressed in cases where bending is not
important, such as in typical geotechnical problems.

Mass
In a dynamic analysis, the mass of the structure is used to compute inertial forces.
The mass contributed by the Plane element is lumped at the element joints. No inertial effects are considered within the element itself.

220

Mass

Chapter XI

The Plane Element

The total mass of the element is equal to the integral over the plane of the element of
the mass density, m, multiplied by the thickness, th. The total mass is apportioned
to the joints in a manner that is proportional to the diagonal terms of the consistent
mass matrix. See Cook, Malkus, and Plesha (1989) for more information. The total
mass is applied to each of the three translational degrees of freedom (UX, UY, and
UZ) even when the element contributes stiffness to only two of these degrees of
freedom.
For more information:
• See Topic “Mass Density” (page 77) in Chapter “Material Properties.”
• See Topic “Mass Source” (page 334) in Chapter “Load Patterns”.
• See Chapter “Load Cases” (page 341).

Self-Weight Load
Self-Weight Load activates the self-weight of all elements in the model. For a Plane
element, the self-weight is a force that is uniformly distributed over the plane of the
element. The magnitude of the self-weight is equal to the weight density, w, multiplied by the thickness, th.
Self-Weight Load always acts downward, in the global –Z direction. You may
scale the self-weight by a single scale factor that applies equally to all elements in
the structure.
For more information:
• See Topic “Weight Density” (page 78) in Chapter “Material Properties” for the
definition of w.
• See Topic “Thickness” (page 219) in this Chapter for the definition of th.
• See Topic “Self-Weight Load” (page 325) in Chapter “Load Patterns.”

Gravity Load
Gravity Load can be applied to each Plane element to activate the self-weight of the
element. Using Gravity Load, the self-weight can be scaled and applied in any direction. Different scale factors and directions can be applied to each element.
If all elements are to be loaded equally and in the downward direction, it is more
convenient to use Self-Weight Load.
Self-Weight Load

221

CSI Analysis Reference Manual
For more information:
• See Topic “Self-Weight Load” (page 221) in this Chapter for the definition of
self-weight for the Plane element.
• See Topic “Gravity Load” (page 326) in Chapter “Load Patterns.”

Surface Pressure Load
The Surface Pressure Load is used to apply external pressure loads upon any of the
three or four side faces of the Plane element. The definition of these faces is shown
in Figure 42 (page 181). Surface pressure always acts normal to the face. Positive
pressures are directed toward the interior of the element.
The pressure may be constant over a face or interpolated from values given at the
joints. The values given at the joints are obtained from Joint Patterns, and need not
be the same for the different faces. Joint Patterns can be used to easily apply hydrostatic pressures.
The pressure acting on a side is multiplied by the thickness, th, integrated along the
length of the side, and apportioned to the two or three joints on that side.
See Chapter “Load Patterns” (page 321) for more information.

Pore Pressure Load
The Pore Pressure Load is used to model the drag and buoyancy effects of a fluid
within a solid medium, such as the effect of water upon the solid skeleton of a soil.
Scalar fluid-pressure values are given at the element joints by Joint Patterns, and interpolated over the element. The total force acting on the element is the integral of
the gradient of this pressure field over the plane of the element, multiplied by the
thickness, th. This force is apportioned to each of the joints of the element. The
forces are typically directed from regions of high pressure toward regions of low
pressure.
See Chapter “Load Patterns” (page 321) for more information.

222

Surface Pressure Load

Chapter XI

The Plane Element

Temperature Load
The Temperature Load creates thermal strain in the Plane element. This strain is
given by the product of the Material coefficient of thermal expansion and the temperature change of the element. The temperature change is measured from the element Reference Temperature to the element Load Temperature. Temperature
changes are assumed to be constant through the element thickness.
See Chapter “Load Patterns” (page 321) for more information.

Stress Output
The Plane element stresses are evaluated at the standard 2-by-2 Gauss integration
points of the element and extrapolated to the joints. See Cook, Malkus, and Plesha
(1989) for more information.
Principal values and their associated principal directions in the element local 1-2
plane are also computed for single-valued Load Cases. The angle given is measured
counterclockwise (when viewed from the +3 direction) from the local 1 axis to the
direction of the maximum principal value.
For more information:
• See Chapter “Load Patterns” (page 321).
• See Chapter “Load Cases” (page 341).

Temperature Load

223

CSI Analysis Reference Manual

224

Stress Output

C h a p t e r XII

The Asolid Element
The Asolid element is used to model axisymmetric solids under axisymmetric loading.
Advanced Topics
• Overview
• Joint Connectivity
• Degrees of Freedom
• Local Coordinate System
• Stresses and Strains
• Section Properties
• Mass
• Self-Weight Load
• Gravity Load
• Surface Pressure Load
• Pore Pressure Load
• Temperature Load
• Rotate Load

225

CSI Analysis Reference Manual
• Stress Output

Overview
The Asolid element is a three- or four-node element for modeling axisymmetric
structures under axisymmetric loading. It is based upon an isoparametric formulation that includes four optional incompatible bending modes.
The element models a representative two-dimensional cross section of the three-dimensional axisymmetric solid. The axis of symmetry may be located arbitrarily in
the model. Each element should lie fully in a plane containing the axis of symmetry.
If it does not, it is formulated for the projection of the element upon the plane containing the axis of symmetry and the center of the element.
The geometry, loading, displacements, stresses, and strains are assumed not to vary
in the circumferential direction. Any displacements that occur in the circumferential direction are treated as axisymmetric torsion.
The use of incompatible bending modes significantly improves the in-plane bending behavior of the element if the element geometry is of a rectangular form. Improved behavior is exhibited even with non-rectangular geometry.
Each Asolid element has its own local coordinate system for defining Material
properties and loads, and for interpreting output. Temperature-dependent,
orthotropic material properties are allowed. Each element may be loaded by gravity
(in any direction); centrifugal force; surface pressure on the side faces; pore pressure within the element; and loads due to temperature change.
An 2 x 2 numerical integration scheme is used for the Asolid. Stresses in the element local coordinate system are evaluated at the integration points and extrapolated to the joints of the element. An approximate error in the stresses can be estimated from the difference in values calculated from different elements attached to a
common joint. This will give an indication of the accuracy of the finite element approximation and can then be used as the basis for the selection of a new and more
accurate finite element mesh.

226

Overview

Chapter XII

The Asolid Element

The Asolid element is intended to be planar and to lie in a plane that contains the
axis of symmetry. If not, a plane is found that contains the axis of symmetry and the
center of the element, and the projection of the element onto this plane will be used.
Joints for a given element may not lie on opposite sides of the axis of symmetry.
They may lie on the axis of symmetry and/or to one side of it.

Degrees of Freedom
The Asolid element activates the three translational degrees of freedom at each of
its connected joints. Rotational degrees of freedom are not activated.
Stiffness is created for all three degrees of freedom. Degrees of freedom in the
plane represent the radial and axial behavior. The normal translation represents
circumferential torsion.
See Topic “Degrees of Freedom” (page 30) in Chapter “Joints and Degrees of Freedom” for more information.

Local Coordinate System
The element local coordinate system is identical for all area objects, i.e., the Shell,
Plane, and Asolid elements. See Topics “Local Coordinate System” (page 185) and
“Advanced Local Coordinate System” (page 186) in Chapter “The Shell Element”
for more information.
The local 3 axis is normal to the plane of the element, and is the negative of the circumferential direction. The 1-2 plane is the same as the radial-axial plane, although
the orientation of the local axes is not restricted to be parallel to the radial and axial
axes.
The radial direction runs perpendicularly from the axis of symmetry to the center of
the element. The axial direction is parallel to the axis of symmetry, with the positive
sense being upward when looking along the circumferential (–3) direction with the
radial direction pointing to the right.

Degrees of Freedom

227

CSI Analysis Reference Manual

Stresses and Strains
The Asolid element models the mid-plane of a representative sector of an axisymmetric structure whose stresses and strains do not vary in the circumferential direction.
Displacements in the local 1-2 plane cause in-plane strains (g 11 , g 22 , g 12 ) and
stresses (s 11 , s 22 , s 12 ).
Displacements in the radial direction also cause circumferential normal strains:
e 33 =

ur
r

where u r is the radial displacement, and r is the radius at the point in question. The
circumferential normal stress (s 33 ) is computed as usual from the three normal
strains.
Displacements in the circumferential (local 3) direction cause only torsion, resulting in circumferential shear strains (g 12 , g 13 ) and stresses (s 12 , s 13 ).
See Topic “Stresses and Strains” (page 71) in Chapter “Material Properties” for
more information.

Section Properties
An Asolid Section is a set of material and geometric properties that describe the
cross-section of one or more Asolid elements. Sections are defined independently
of the Asolid elements, and are assigned to the area objects.

Section Type
When defining an area section, you have a choice of three basic element types:
• Asolid – the subject of this Chapter, an axisymmetric solid, with translational
degrees of freedom, capable of supporting forces but not moments.
• Plane (stress or strain) – a two-dimensional solid, with translational degrees of
freedom, capable of supporting forces but not moments. This element is covered in Chapter “The Plane Element” (page 215).

228

Stresses and Strains

Chapter XII

The Asolid Element

• Shell – shell, plate, or membrane, with translational and rotational degrees of
freedom, capable of supporting forces and moments. This element is covered in
Chapter “The Shell Element” (page 177).
After selecting an Asolid type of section, you must supply the rest of the data described below.

Material Properties
The material properties for each Asolid element are specified by reference to a previously-defined Material. Orthotropic properties are used, even if the Material selected was defined as anisotropic. The material properties used by the Asolid element are:
• The moduli of elasticity, e1, e2, and e3
• The shear moduli, g12, g13, and g23
• The Poisson’s ratios, u12, u13 and u23
• The coefficients of thermal expansion, a1, a2, and a3
• The mass density, m, for computing element mass
• The weight density, w, for computing Self-Weight and Gravity Loads
All material properties (except the densities) are obtained at the material temperature of each individual element.
See Chapter “Material Properties” (page 69) for more information.

Material Angle
The material local coordinate system and the element (Asolid Section) local coordinate system need not be the same. The local 3 directions always coincide for the
two systems, but the material 1 axis and the element 1 axis may differ by the angle a
as shown in Figure 53 (page 230). This angle has no effect for isotropic material
properties since they are independent of orientation.
See Topic “Local Coordinate System” (page 70) in Chapter “Material Properties”
for more information.

Section Properties

229

CSI Analysis Reference Manual
2 (Element)

2 (Material)
1 (Material)

a
1 (Element)

3 (Element, Material)

Figure 53
Asolid Element Material Angle

Axis of Symmetry
For each Asolid Section, you may select an axis of symmetry. This axis is specified
as the Z axis of an alternate coordinate system that you have defined. All Asolid elements that use a given Asolid Section will have the same axis of symmetry.
For most modeling cases, you will only need a single axis of symmetry. However,
if you want to have multiple axes of symmetry in your model, just set up as many alternate coordinate systems as needed for this purpose and define corresponding
Asolid Section properties.
You should be aware that it is almost impossible to make a sensible model that connects Asolid elements with other element types, or that connects together Asolid elements using different axes of symmetry. The practical application of having multiple axes of symmetry is to have multiple independent axisymmetric structures in
the same model.
See Topic “Alternate Coordinate Systems” (page 16) in Chapter “Coordinate Systems” for more information.

230

Section Properties

Chapter XII

The Asolid Element

Z, 2

arc

j9
X, 3

Y, 1

j1
j3

Figure 54
Asolid Element Local Coordinate System and Arc Definition

Arc and Thickness
The Asolid element represents a solid that is created by rotating the element’s planar shape through 360° about the axis of symmetry. However, the analysis considers only a representative sector of the solid. You can specify the size of the sector,
in degrees, using the parameter arc. For example, arc=360 models the full structure, and arc=90 models one quarter of it. See Figure 54 (page 231). Setting arc=0,
the default, models a one-radian sector. One radian is the same as 180°/p, or approximately 57.3°.
The element “thickness” (circumferential extent), h, increases with the radial distance, r, from the axis of symmetry:
h=

p × arc
r
180

Clearly the thickness varies over the plane of the element.
The element thickness is used for calculating the element stiffness, mass, and loads.
Hence, joint forces computed from the element are proportional to arc.
Section Properties

231

CSI Analysis Reference Manual

Incompatible Bending Modes
By default each Asolid element includes four incompatible bending modes in its
stiffness formulation. These incompatible bending modes significantly improve
the bending behavior in the plane of the element if the element geometry is of a rectangular form. Improved behavior is exhibited even with non-rectangular geometry.
If an element is severely distorted, the inclusion of the incompatible modes should
be suppressed. The element then uses the standard isoparametric formulation. Incompatible bending modes may also be suppressed in cases where bending is not
important, such as in typical geotechnical problems.

Mass
In a dynamic analysis, the mass of the structure is used to compute inertial forces.
The mass contributed by the Asolid element is lumped at the element joints. No inertial effects are considered within the element itself.
The total mass of the element is equal to the integral over the plane of the element of
the product of the mass density, m, multiplied by the thickness, h. The total mass is
apportioned to the joints in a manner that is proportional to the diagonal terms of
the consistent mass matrix. See Cook, Malkus, and Plesha (1989) for more information. The total mass is applied to each of the three translational degrees of freedom (UX, UY, and UZ).
For more information:
• See Topic “Mass Density” (page 77) in Chapter “Material Properties.”
• See Topic “Mass Source” (page 334) in Chapter “Load Patterns”.
• See Chapter “Load Cases” (page 341).

Self-Weight Load
Self-Weight Load activates the self-weight of all elements in the model. For an
Asolid element, the self-weight is a force that is distributed over the plane of the
element. The magnitude of the self-weight is equal to the weight density, w, multiplied by the thickness, h.
Self-Weight Load always acts downward, in the global –Z direction. If the downward direction corresponds to the radial or circumferential direction of an Asolid

232

Mass

Chapter XII

The Asolid Element

element, the Self-Weight Load for that element will be zero, since self-weight acting in these directions is not axisymmetric. Non-zero Self-Weight Load will only
exist for elements whose axial direction is vertical.
You may scale the self-weight by a single scale factor that applies equally to all elements in the structure.
For more information:
• See Topic “Weight Density” (page 78) in Chapter “Material Properties” for the
definition of w.
• See Subtopic “Arc and Thickness” (page 231) in this Chapter for the definition
of h.
• See Topic “Self-Weight Load” (page 325) in Chapter “Load Patterns.”

Gravity Load
Gravity Load can be applied to each Asolid element to activate the self-weight of
the element. Using Gravity Load, the self-weight can be scaled and applied in any
direction. Different scale factors and directions can be applied to each element.
However, only the components of Gravity load acting in the axial direction of an
Asolid element will be non-zero. Components in the radial or circumferential direction will be set to zero, since gravity acting in these directions is not axisymmetric.
If all elements are to be loaded equally and in the downward direction, it is more
convenient to use Self-Weight Load.
For more information:
• See Topic “Self-Weight Load” (page 232) in this Chapter for the definition of
self-weight for the Asolid element.
• See Topic “Gravity Load” (page 326) in Chapter “Load Patterns.”

Surface Pressure Load
The Surface Pressure Load is used to apply external pressure loads upon any of the
three or four side faces of the Asolid element. The definition of these faces is shown
in Figure 42 (page 181). Surface pressure always acts normal to the face. Positive
pressures are directed toward the interior of the element.

Gravity Load

233

CSI Analysis Reference Manual
The pressure may be constant over a face or interpolated from values given at the
joints. The values given at the joints are obtained from Joint Patterns, and need not
be the same for the different faces. Joint Patterns can be used to easily apply hydrostatic pressures.
The pressure acting on a side is multiplied by the thickness, h, integrated along the
length of the side, and apportioned to the two or three joints on that side.
See Chapter “Load Patterns” (page 321) for more information.

Pore Pressure Load
The Pore Pressure Load is used to model the drag and buoyancy effects of a fluid
within a solid medium, such as the effect of water upon the solid skeleton of a soil.
Scalar fluid-pressure values are given at the element joints by Joint Patterns, and interpolated over the element. The total force acting on the element is the integral of
the gradient of this pressure field, multiplied by the thickness h, over the plane of
the element. This force is apportioned to each of the joints of the element. The
forces are typically directed from regions of high pressure toward regions of low
pressure.
See Chapter “Load Patterns” (page 321) for more information.

Temperature Load
The Temperature Load creates thermal strain in the Asolid element. This strain is
given by the product of the Material coefficient of thermal expansion and the temperature change of the element. All specified Temperature Loads represent a
change in temperature from the unstressed state for a linear analysis, or from the
previous temperature in a nonlinear analysis. Temperature changes are assumed to
be constant through the element thickness.
See Chapter “Load Patterns” (page 321) for more information.

Rotate Load
Rotate Load is used to apply centrifugal force to Asolid elements. Each element is
assumed to rotate about its own axis of symmetry at a constant angular velocity.

234

Pore Pressure Load

Chapter XII

The Asolid Element

The angular velocity creates a load on the element that is proportional to its mass,
its distance from the axis of rotation, and the square of the angular velocity. This
load acts in the positive radial direction, and is apportioned to each joint of the element. No Rotate Load will be produced by an element with zero mass density.
Since Rotate Loads assume a constant rate of rotation, it does not make sense to use
a Load Pattern that contains Rotate Load in a time-history analysis unless that Load
Pattern is applied quasi-statically (i.e., with a very slow time variation).
For more information:
• See Topic “Mass Density” (page 77) in Chapter “Material Properties.”
• See Chapter “Load Patterns” (page 321).

Stress Output
The Asolid element stresses are evaluated at the standard 2-by-2 Gauss integration
points of the element and extrapolated to the joints. See Cook, Malkus, and Plesha
(1989) for more information.
Principal values and their associated principal directions in the element local 1-2
plane are also computed for single-valued Load Cases. The angle given is measured
counterclockwise (when viewed from the +3 direction) from the local 1 axis to the
direction of the maximum principal value.
For more information:
• See Chapter “Load Patterns” (page 321).
• See Chapter “Load Cases” (page 341).

Stress Output

235

CSI Analysis Reference Manual

236

Stress Output

C h a p t e r XIII

The Solid Element
The Solid element is used to model three-dimensional solid structures.
Advanced Topics
• Overview
• Joint Connectivity
• Degrees of Freedom
• Local Coordinate System
• Advanced Local Coordinate System
• Stresses and Strains
• Solid Properties
• Mass
• Self-Weight Load
• Gravity Load
• Surface Pressure Load
• Pore Pressure Load
• Temperature Load
• Stress Output

237

CSI Analysis Reference Manual

Overview
The Solid element is an eight-node element for modeling three-dimensional structures and solids. It is based upon an isoparametric formulation that includes nine
optional incompatible bending modes.
The incompatible bending modes significantly improve the bending behavior of
the element if the element geometry is of a rectangular form. Improved behavior is
exhibited even with non-rectangular geometry.
Each Solid element has its own local coordinate system for defining Material properties and loads, and for interpreting output. Temperature-dependent, anisotropic
material properties are allowed. Each element may be loaded by gravity (in any direction); surface pressure on the faces; pore pressure within the element; and loads
due to temperature change.
An 2 x 2 x 2 numerical integration scheme is used for the Solid. Stresses in the element local coordinate system are evaluated at the integration points and extrapolated to the joints of the element. An approximate error in the stresses can be estimated from the difference in values calculated from different elements attached to a
common joint. This will give an indication of the accuracy of the finite element approximation and can then be used as the basis for the selection of a new and more
accurate finite element mesh.

Joint Connectivity
Each Solid element has six quadrilateral faces, with a joint located at each of the
eight corners as shown in Figure 55 (page 239). It is important to note the relative
position of the eight joints: the paths j1-j2-j3 and j5-j6-j7 should appear counterclockwise when viewed along the direction from j5 to j1. Mathematically stated,
the three vectors:
• V12 , from joints j1 to j2,
• V13 , from joints j1 to j3,
• V15 , from joints j1 to j5,
must form a positive triple product, that is:
( V12 ´ V13 ) × V15 > 0

238

Overview

Chapter XIII

The Solid Element

j8
Face 2
Face 3
j6
j7

j4
Face 6

Face 4

Face 1
j2

j3
Face 5
j1

Figure 55
Solid Element Joint Connectivity and Face Definitions

The locations of the joints should be chosen to meet the following geometric conditions:
• The inside angle at each corner of the faces must be less than 180°. Best results
will be obtained when these angles are near 90°, or at least in the range of 45° to
135°.
• The aspect ratio of an element should not be too large. This is the ratio of the
longest dimension of the element to its shortest dimension. Best results are obtained for aspect ratios near unity, or at least less than four. The aspect ratio
should not exceed ten.
These conditions can usually be met with adequate mesh refinement.

Degenerate Solids
Degenerate solids, such as wedges and tetrahedra, can be created by collapsing various sides of the element. This is done by specifying the same joint number for two
or more of the eight corner nodes, so long as the ordering of the nodes remains the
same. Examples include:

Joint Connectivity

239

CSI Analysis Reference Manual
• Wedge (triangular bottom, triangular top): j1, j2, j3 = j4, j5, j6, j7 = j8
• Tetrahedron (triangular bottom, point top): j1, j2, j3 = j4, j5 = j6 = j7 = j8
• 7-node (rectangular bottom, triangular top): j1, j2, j3, j4, j5, j6, j7 = j8
• Pyramid (rectangular bottom, point top): j1, j2, j3, j4, j5 = j6 = j7 = j8
Other examples are possible, but these are the recommended configurations.

Degrees of Freedom
The Solid element activates the three translational degrees of freedom at each of its
connected joints. Rotational degrees of freedom are not activated. This element
contributes stiffness to all of these translational degrees of freedom.
See Topic “Degrees of Freedom” (page 30) in Chapter “Joints and Degrees of Freedom” for more information.

Local Coordinate System
Each Solid element has its own element local coordinate system used to define
Material properties, loads and output. The axes of this local system are denoted 1, 2
and 3. By default these axes are identical to the global X, Y, and Z axes, respectively. Both systems are right-handed coordinate systems.
The default local coordinate system is adequate for most situations. However, for
certain modeling purposes it may be useful to use element local coordinate systems
that follow the geometry of the structure.
For more information:
• See Topic “Upward and Horizontal Directions” (page 13) in Chapter “Coordinate Systems.”
• See Topic “Advanced Local Coordinate System” (page 240) in this Chapter.

Advanced Local Coordinate System
By default, the element local 1-2-3 coordinate system is identical to the global
X-Y-Z coordinate system, as described in the previous topic. In certain modeling
situations it may be useful to have more control over the specification of the local
coordinate system.

240

Degrees of Freedom

Chapter XIII

The Solid Element

A variety of methods are available to define a solid-element local coordinate system. These may be used separately or together. Local coordinate axes may be defined to be parallel to arbitrary coordinate directions in an arbitrary coordinate system or to vectors between pairs of joints. In addition, the local coordinate system
may be specified by a set of three element coordinate angles. These methods are described in the subtopics that follow.
For more information:
• See Chapter “Coordinate Systems” (page 11).
• See Topic “Local Coordinate System” (page 240) in this Chapter.

Reference Vectors
To define a solid-element local coordinate system you must specify two reference
vectors that are parallel to one of the local coordinate planes. The axis reference
vector, Va , must be parallel to one of the local axes (I = 1, 2, or 3) in this plane and
have a positive projection upon that axis. The plane reference vector, V p , must
have a positive projection upon the other local axis (j = 1, 2, or 3, but I ¹ j) in this
plane, but need not be parallel to that axis. Having a positive projection means that
the positive direction of the reference vector must make an angle of less than 90°
with the positive direction of the local axis.
Together, the two reference vectors define a local axis, I, and a local plane, i-j.
From this, the program can determine the third local axis, k, using vector algebra.
For example, you could choose the axis reference vector parallel to local axis 1 and
the plane reference vector parallel to the local 1-2 plane (I = 1, j = 2). Alternatively,
you could choose the axis reference vector parallel to local axis 3 and the plane reference vector parallel to the local 3-2 plane (I = 3, j = 2). You may choose the plane
that is most convenient to define using the parameter local, which may take on the
values 12, 13, 21, 23, 31, or 32. The two digits correspond to I and j, respectively.
The default is value is 31.

Defining the Axis Reference Vector
To define the axis reference vector, you must first specify or use the default values
for:
• A coordinate direction axdir (the default is +Z)

Advanced Local Coordinate System

241

CSI Analysis Reference Manual
• A fixed coordinate system csys (the default is zero, indicating the global coordinate system)
You may optionally specify:
• A pair of joints, axveca and axvecb (the default for each is zero, indicating the
center of the element). If both are zero, this option is not used.
For each element, the axis reference vector is determined as follows:
1. A vector is found from joint axveca to joint axvecb. If this vector is of finite
length, it is used as the reference vector Va
2. Otherwise, the coordinate direction axdir is evaluated at the center of the element in fixed coordinate system csys, and is used as the reference vector Va

Defining the Plane Reference Vector
To define the plane reference vector, you must first specify or use the default values
for:
• A primary coordinate direction pldirp (the default is +X)
• A secondary coordinate direction pldirs (the default is +Y). Directions pldirs
and pldirp should not be parallel to each other unless you are sure that they are
not parallel to local axis 1
• A fixed coordinate system csys (the default is zero, indicating the global coordinate system). This will be the same coordinate system that was used to define
the axis reference vector, as described above
You may optionally specify:
• A pair of joints, plveca and plvecb (the default for each is zero, indicating the
center of the element). If both are zero, this option is not used.
For each element, the plane reference vector is determined as follows:
1. A vector is found from joint plveca to joint plvecb. If this vector is of finite
length and is not parallel to local axis I, it is used as the reference vector V p
2. Otherwise, the primary coordinate direction pldirp is evaluated at the center of
the element in fixed coordinate system csys. If this direction is not parallel to
local axis I, it is used as the reference vector V p

242

Advanced Local Coordinate System

Chapter XIII

The Solid Element

3. Otherwise, the secondary coordinate direction pldirs is evaluated at the center
of the element in fixed coordinate system csys. If this direction is not parallel to
local axis I, it is used as the reference vector V p
4. Otherwise, the method fails and the analysis terminates. This will never happen
if pldirp is not parallel to pldirs
A vector is considered to be parallel to local axis I if the sine of the angle between
-3
them is less than 10 .

Determining the Local Axes from the Reference Vectors
The program uses vector cross products to determine the local axes from the reference vectors. The three axes are represented by the three unit vectors V1 , V2 and
V3 , respectively. The vectors satisfy the cross-product relationship:
V1 = V2 ´ V3
The local axis Vi is given by the vector Va after it has been normalized to unit
length.
The remaining two axes, V j and Vk , are defined as follows:
• If I and j permute in a positive sense, i.e., local = 12, 23, or 31, then:
Vk = Vi ´ V p and
V j = Vk ´ Vi
• If I and j permute in a negative sense, i.e., local = 21, 32, or 13, then:
Vk = V p ´ Vi and
V j = Vi ´ Vk
An example showing the determination of the element local coordinate system using reference vectors is given in Figure 56 (page 244).

Element Coordinate Angles
The solid-element local coordinate axes determined from the reference vectors may
be further modified by the use of three element coordinate angles, denoted a, b,
and c. In the case where the default reference vectors are used, the coordinate angles define the orientation of the element local coordinate system with respect to
the global axes.

Advanced Local Coordinate System

243

CSI Analysis Reference Manual
Va is parallel to axveca-axvecb
Vp is parallel to plveca-plvecb
V3 = V a
V2 = V3 x Vp
V1 = V 2 x V3

All vectors normalized to unit length.

Z
plvecb

plveca

Plane 3-1
V3

axveca

Va
Global
axvecb
X

Figure 56
Example of the Determination of the Solid Element Local Coordinate System
Using Reference Vectors for local=31. Point j is the Center of the Element.

The element coordinate angles specify rotations of the local coordinate system
about its own current axes. The resulting orientation of the local coordinate system
is obtained according to the following procedure:
1. The local system is first rotated about its +3 axis by angle a
2. The local system is next rotated about its resulting +2 axis by angle b
3. The local system is lastly rotated about its resulting +1 axis by angle c
The order in which the rotations are performed is important. The use of coordinate
angles to orient the element local coordinate system with respect to the global system is shown in Figure 4 (page 29).

244

Advanced Local Coordinate System

Chapter XIII

The Solid Element

Z, 3

a
Step 1: Rotation about
local 3 axis by angle a
2

a
a

1
Z

3
b

Step 2: Rotation about new
local 2 axis by angle b

2
Y

X
b

1
Z
3

Step 3: Rotation about new
local 1 axis by angle c

2
c

Figure 57
Use of Element Coordinate Angles to Orient the
Solid Element Local Coordinate System

Advanced Local Coordinate System

245

CSI Analysis Reference Manual

Stresses and Strains
The Solid element models a general state of stress and strain in a three-dimensional
solid. All six stress and strain components are active for this element.
See Topic “Stresses and Strains” (page 71) in Chapter “Material Properties” for
more information.

Solid Properties
A Solid Property is a set of material and geometric properties to be used by one or
more Solid elements. Solid Properties are defined independently of the Solid elements/objects, and are assigned to the elements.

Material Properties
The material properties for each Solid Property are specified by reference to a previously-defined Material. Fully anisotropic material properties are used. The material properties used by the Solid element are:
• The moduli of elasticity, e1, e2, and e3
• The shear moduli, g12, g13, and g23
• All of the Poisson’s ratios, u12, u13, u23, ..., u56
• The coefficients of thermal expansion, a1, a2, a3, a12, a13, and a23
• The mass density, m, used for computing element mass
• The weight density, w, used for computing Self-Weight and Gravity Loads
All material properties (except the densities) are obtained at the material temperature of each individual element.
See Chapter “Material Properties” (page 69) for more information.

Material Angles
The material local coordinate system and the element (Property) local coordinate
system need not be the same. The material coordinate system is oriented with respect to the element coordinate system using the three angles a, b, and c according
to the following procedure:
• The material system is first aligned with the element system;

246

Stresses and Strains

Chapter XIII

The Solid Element

3 (Element)
3 (Material)
a
b
c

2 (Material)
c
a
a
b

1 (Element)

b
2 (Element)

c
1 (Material)

Rotations are performed in the order
a-b-c about the axes shown.

Figure 58
Solid Element Material Angles

• The material system is then rotated about its +3 axis by angle a;
• The material system is next rotated about the resulting +2 axis by angle b;
• The material system is lastly rotated about the resulting +1 axis by angle c;
This is shown in Figure 58 (page 247). These angles have no effect for isotropic
material properties since they are independent of orientation.
See Topic “Local Coordinate System” (page 70) in Chapter “Material Properties”
for more information.

Incompatible Bending Modes
By default each Solid element includes nine incompatible bending modes in its
stiffness formulation. These incompatible bending modes significantly improve
the bending behavior of the element if the element geometry is of a rectangular
form. Improved behavior is exhibited even with non-rectangular geometry.
If an element is severely distorted, the inclusion of the incompatible modes should
be suppressed. The element then uses the standard isoparametric formulation. InSolid Properties

247

CSI Analysis Reference Manual
compatible bending modes may also be suppressed in cases where bending is not
important, such as in typical geotechnical problems.

Mass
In a dynamic analysis, the mass of the structure is used to compute inertial forces.
The mass contributed by the Solid element is lumped at the element joints. No inertial effects are considered within the element itself.
The total mass of the element is equal to the integral of the mass density, m, over the
volume of the element. The total mass is apportioned to the joints in a manner that is
proportional to the diagonal terms of the consistent mass matrix. See Cook,
Malkus, and Plesha (1989) for more information. The total mass is applied to each
of the three translational degrees of freedom (UX, UY, and UZ).
For more information:
• See Topic “Mass Density” (page 77) in Chapter “Material Properties.”
• See Topic “Mass Source” (page 334) in Chapter “Load Patterns”.
• See Chapter “Load Cases” (page 341).

Self-Weight Load
Self-Weight Load activates the self-weight of all elements in the model. For a Solid
element, the self-weight is a force that is uniformly distributed over the volume of
the element. The magnitude of the self-weight is equal to the weight density, w.
Self-Weight Load always acts downward, in the global –Z direction. You may
scale the self-weight by a single scale factor that applies equally to all elements in
the structure.
For more information:
• See Topic “Weight Density” (page 78) in Chapter “Material Properties” for the
definition of w.
• See Topic “Self-Weight Load” (page 325) in Chapter “Load Patterns.”

248

Mass

Chapter XIII

The Solid Element

Gravity Load
Gravity Load can be applied to each Solid element to activate the self-weight of the
element. Using Gravity Load, the self-weight can be scaled and applied in any direction. Different scale factors and directions can be applied to each element.
If all elements are to be loaded equally and in the downward direction, it is more
convenient to use Self-Weight Load.
For more information:
• See Topic “Self-Weight Load” (page 248) in this Chapter for the definition of
self-weight for the Solid element.
• See Topic “Gravity Load” (page 326) in Chapter “Load Patterns.”

Surface Pressure Load
The Surface Pressure Load is used to apply external pressure loads upon any of the
six faces of the Solid element. The definition of these faces is shown in Figure 55
(page 239). Surface pressure always acts normal to the face. Positive pressures are
directed toward the interior of the element.
The pressure may be constant over a face or interpolated from values given at the
joints. The values given at the joints are obtained from Joint Patterns, and need not
be the same for the different faces. Joint Patterns can be used to easily apply hydrostatic pressures.
The pressure acting on a given face is integrated over the area of that face, and the
resulting force is apportioned to the four corner joints of the face.
See Chapter “Load Patterns” (page 321) for more information.

Gravity Load

249

CSI Analysis Reference Manual
portioned to each of the joints of the element. The forces are typically directed from
regions of high pressure toward regions of low pressure.
See Chapter “Load Patterns” (page 321) for more information.

Temperature Load
The Temperature Load creates thermal strain in the Solid element. This strain is
given by the product of the Material coefficient of thermal expansion and the temperature change of the element. All specified Temperature Loads represent a
change in temperature from the unstressed state for a linear analysis, or from the
previous temperature in a nonlinear analysis.
See Chapter “Load Patterns” (page 321) for more information.

Stress Output
The Solid element stresses are evaluated at the standard 2 x 2 x 2 Gauss integration
points of the element and extrapolated to the joints. See Cook, Malkus, and Plesha
(1989) for more information.
Principal values and their associated principal directions in the element local coordinate system are also computed for single-valued Load Cases and Load Combinations. Three direction cosines each are given for the directions of the maximum and
minimum principal stresses. The direction of the middle principal stress is perpendicular to the maximum and minimum principal directions.
For more information:
• See Chapter “Load Patterns” (page 321).
• See Chapter “Load Cases” (page 341).

250

Temperature Load

C h a p t e r XIV

The Link/Support Element—Basic
The Link element is used to connect two joints together. The Support element is
used to connect one joint to ground. Both element types use the same types of properties. Each Link or Support element may exhibit up to three different types of behavior: linear, nonlinear, and frequency-dependent, according to the types of properties assigned to that element and the type of analysis being performed.
This Chapter describes the basic and general features of the Link and Support elements and their linear behavior. The next Chapter describes advanced behavior,
which can be nonlinear or frequency-dependent.
Advanced Topics
• Overview
• Joint Connectivity
• Zero-Length Elements
• Degrees of Freedom
• Local Coordinate System
• Advanced Local Coordinate System
• Internal Deformations
• Link/Support Properties

251

CSI Analysis Reference Manual
• Coupled Linear Property
• Mass
• Self-Weight Load
• Gravity Load
• Internal Force and Deformation Output

Overview
A Link element is a two-joint connecting link. A Support element is a one-joint
grounded spring. Properties for both types of element are defined in the same way.
Each element is assumed to be composed of six separate “springs,” one for each of
six deformational degrees-of freedom (axial, shear, torsion, and pure bending).
There are two categories of Link/Support properties that can be defined: Linear/Nonlinear, and Frequency-Dependent. A Linear/Nonlinear property set must
be assigned to each Link or Support element. The assignment of a Frequency-Dependent property set to a Link or Support element is optional.
All Linear/Nonlinear property sets contain linear properties that are used by the element for linear analyses, and for other types of analyses if no other properties are
defined. Linear/Nonlinear property sets may have nonlinear properties that will be
used for all nonlinear analyses, and for linear analyses that continue from nonlinear
analyses.
Frequency-dependent property sets contain impedance (stiffness and damping)
properties that will be used for all frequency-dependent analyses. If a Frequency-Dependent property has not been assigned to a Link/Support element, the
linear properties for that element will be used for frequency-dependent analyses.
The types of nonlinear behavior that can be modeled with this element include:
• Viscoelastic damping
• Gap (compression only) and hook (tension only)
• Multi-linear uniaxial elasticity
• Uniaxial plasticity (Wen model)
• Multi-linear uniaxial plasticity with several types of hysteretic behavior: kinematic, Takeda, and pivot
• Biaxial-plasticity base isolator

252

Overview

Chapter XIV

The Link/Support Element—Basic

• Friction-pendulum base isolator, with or without uplift prevention. This can
also be used for modeling gap-friction contact behavior
Each element has its own local coordinate system for defining the forcedeformation properties and for interpreting output.
Each Link/Support element may be loaded by gravity (in any direction).
Available output includes the deformation across the element, and the internal
forces at the joints of the element.

Joint Connectivity
Each Link/Support element may take one of the following two configurations:
• A Link connecting two joints, I and j; it is permissible for the two joints to
share the same location in space creating a zero-length element
• A Support connecting a single joint, j, to ground

Conversion from One-Joint Objects to Two-Joint Elements
During analysis, all one-joint Link/Support objects used for modeling are actually
converted to two-joint Link/Support elements of zero length. The original joint, j,
remains connected to the structure. A new joint , I, is generated at the same location
and is fully restrained. Reactions are calculated at generated joint I but are reported
at the original joint j. Conversely, ground displacement loads applied at joint j are
transferred to joint I.
For the remainder of this chapter and the next, we will continue to refer to one-joint
elements for convenience, and to clarify how the one-joint modeling objects behave.

Zero-Length Elements
The following types of Link/Support elements are considered to be of zero length:
• Single-joint Support elements
• Two-joint Link elements with the distance from joint I to joint j being less than
or equal to the zero-length tolerance that you specify.

Joint Connectivity

253

CSI Analysis Reference Manual
The length tolerance is set using the Auto Merge Tolerance in the graphical user interface. Two-joint elements having a length greater than the Auto Merge Tolerance
are considered to be of finite length. Whether an element is of zero length or finite
length affects the definition of the element local coordinate system, and the internal
moments due to shear forces.

Degrees of Freedom
The Link/Support element always activates all six degrees of freedom at each of its
one or two connected joints. To which joint degrees of freedom the element contributes stiffness depends upon the properties you assign to the element. You must
ensure that restraints or other supports are provided to those joint degrees of freedom that receive no stiffness.
For more information:
• See Topic “Degrees of Freedom” (page 30) in Chapter “Joints and Degrees of
Freedom.”
• See Topic “Link/Support Properties” (page 263) in this Chapter.

Local Coordinate System
Each Link/Support element has its own element local coordinate system used to
define force-deformation properties and output. The axes of this local system are
denoted 1, 2 and 3. The first axis is directed along the length of the element and corresponds to extensional deformation. The remaining two axes lie in the plane perpendicular to the element and have an orientation that you specify; these directions
correspond to shear deformation.
It is important that you clearly understand the definition of the element local 1-2-3
coordinate system and its relationship to the global X-Y-Z coordinate system. Both
systems are right-handed coordinate systems. It is up to you to define local systems
which simplify data input and interpretation of results.
In most structures the definition of the element local coordinate system is extremely simple. The methods provided, however, provide sufficient power and
flexibility to describe the orientation of Link/Support elements in the most complicated situations.

254

Degrees of Freedom

Chapter XIV

The Link/Support Element—Basic

The simplest method, using the default orientation and the Link/Support element coordinate angle, is described in this topic. Additional methods for defining
the Link/Support element local coordinate system are described in the next topic.
For more information:
• See Chapter “Coordinate Systems” (page 11) for a description of the concepts
and terminology used in this topic.
• See Topic “Advanced Local Coordinate System” (page 256) in this Chapter.

Longitudinal Axis 1
Local axis 1 is the longitudinal axis of the element, corresponding to extensional
deformation. This axis is determined as follows:
• For elements of finite length this axis is automatically defined as the direction
from joint I to joint j
• For zero-length elements the local 1 axis defaults to the +Z global coordinate
direction (upward)
For the definition of zero-length elements, see Topic “Zero-Length Elements”
(page 253) in this Chapter.

Default Orientation
The default orientation of the local 2 and 3 axes is determined by the relationship
between the local 1 axis and the global Z axis. The procedure used here is identical
to that for the Frame element:
• The local 1-2 plane is taken to be vertical, i.e., parallel to the Z axis
• The local 2 axis is taken to have an upward (+Z) sense unless the element is vertical, in which case the local 2 axis is taken to be horizontal along the global +X
direction
• The local 3 axis is always horizontal, i.e., it lies in the X-Y plane
An element is considered to be vertical if the sine of the angle between the local 1
axis and the Z axis is less than 10-3.
The local 2 axis makes the same angle with the vertical axis as the local 1 axis
makes with the horizontal plane. This means that the local 2 axis points vertically
upward for horizontal elements.

Local Coordinate System

255

CSI Analysis Reference Manual

Coordinate Angle
The Link/Support element coordinate angle, ang, is used to define element orientations that are different from the default orientation. It is the angle through which the
local 2 and 3 axes are rotated about the positive local 1 axis from the default orientation. The rotation for a positive value of ang appears counterclockwise when the
local +1 axis is pointing toward you. The procedure used here is identical to that for
the Frame element.
For vertical elements, ang is the angle between the local 2 axis and the horizontal
+X axis. Otherwise, ang is the angle between the local 2 axis and the vertical plane
containing the local 1 axis. See Figure 59 (page 257) for examples.

Advanced Local Coordinate System
By default, the element local coordinate system is defined using the element coordinate angle measured with respect to the global +Z and +X directions, as described
in the previous topic. In certain modeling situations it may be useful to have more
control over the specification of the local coordinate system.
This topic describes how to define the orientation of the transverse local 2 and 3
axes with respect to an arbitrary reference vector when the element coordinate angle, ang, is zero. If ang is different from zero, it is the angle through which the local
2 and 3 axes are rotated about the positive local 1 axis from the orientation determined by the reference vector.
This topic also describes how to change the orientation of the local 1 axis from the
default global +Z direction for zero-length elements. The local 1 axis is always directed from joint I to joint j for elements of finite length.
For more information:
• See Chapter “Coordinate Systems” (page 11) for a description of the concepts
and terminology used in this topic.
• See Topic “Local Coordinate System” (page 253) in this Chapter.

256

Advanced Local Coordinate System

Chapter XIV

The Link/Support Element—Basic

Z
1

ang=90°

j
ang=30° 2

i
1

3
Y

Local 1 Axis is Parallel to +Y Axis
Local 2 Axis is Rotated 90° from Z-1 Plane

X
Local 1 Axis is Not Parallel to X, Y, or Z Axes
Local 2 Axis is Rotated 30° from Z-1 Plane

Z
3

1
j

ang=30°

2
ang=90°
Local 1 Axis is Parallel to +Z Axis
Local 2 Axis is Rotated 90° from X-1 Plane

1
Local 1 Axis is Parallel to –Z Axis
Local 2 Axis is Rotated 30° from X-1 Plane

Figure 59
The Link/Support Element Coordinate Angle with Respect to the Default
Orientation

Axis Reference Vector
To define the local 1 axis for zero-length elements, you specify an axis reference
vector that is parallel to and has the same positive sense as the desired local 1 axis.
The axis reference vector has no effect upon finite-length elements.
Advanced Local Coordinate System

257

CSI Analysis Reference Manual
To define the axis reference vector, you must first specify or use the default values
for:
• A coordinate direction axdir (the default is +Z)
• A fixed coordinate system csys (the default is zero, indicating the global coordinate system). This will be the same coordinate system that is used to define
the plane reference vector, as described below
You may optionally specify:
• A pair of joints, axveca and axvecb (the default for each is zero, indicating the
center of the element). If both are zero, this option is not used
For each element, the axis reference vector is determined as follows:
1. A vector is found from joint axveca to joint axvecb. If this vector is of finite
length, it is used as the reference vector Va
2. Otherwise, the coordinate direction axdir is evaluated at the center of the element in fixed coordinate system csys, and is used as the reference vector Va
The center of a zero-length element is taken to be at joint j.
The local 1 axis is given by the vector Va after it has been normalized to unit length.

Plane Reference Vector
To define the transverse local axes 2 and 3, you specify a plane reference vector
that is parallel to the desired 1-2 or 1-3 plane. The procedure used here is identical
to that for the Frame element.
The reference vector must have a positive projection upon the corresponding transverse local axis (2 or 3, respectively). This means that the positive direction of the
reference vector must make an angle of less than 90° with the positive direction of
the desired transverse axis.
To define the reference vector, you must first specify or use the default values for:
• A primary coordinate direction pldirp (the default is +Z)
• A secondary coordinate direction pldirs (the default is +X). Directions pldirs
and pldirp should not be parallel to each other unless you are sure that they are
not parallel to local axis 1

258

Advanced Local Coordinate System

Chapter XIV

The Link/Support Element—Basic

• A fixed coordinate system csys (the default is zero, indicating the global coordinate system). This will be the same coordinate system that was used to define
the axis reference vector, as described above
• The local plane, local, to be determined by the reference vector (the default is
12, indicating plane 1-2)
You may optionally specify:
• A pair of joints, plveca and plvecb (the default for each is zero, indicating the
center of the element). If both are zero, this option is not used
For each element, the reference vector is determined as follows:
1. A vector is found from joint plveca to joint plvecb. If this vector is of finite
length and is not parallel to local axis 1, it is used as the reference vector Vp.
2. Otherwise, the primary coordinate direction pldirp is evaluated at the center of
the element in fixed coordinate system csys. If this direction is not parallel to
local axis 1, it is used as the reference vector Vp.
3. Otherwise, the secondary coordinate direction pldirs is evaluated at the center
of the element in fixed coordinate system csys. If this direction is not parallel to
local axis 1, it is used as the reference vector Vp.
4. Otherwise, the method fails and the analysis terminates. This will never happen
if pldirp is not parallel to pldirs
A vector is considered to be parallel to local axis 1 if the sine of the angle between
-3
them is less than 10 .
The use of the Link/Support element coordinate angle in conjunction with coordinate directions that define the reference vector is illustrated in Figure 60 (page
260). The use of joints to define the reference vector is shown in Figure 61 (page
261).

Advanced Local Coordinate System

259

CSI Analysis Reference Manual
Y

ang=90°

Y
pldirp = +Y
pldirs = –X
local = 12

1
j

1
Z

ang=90°

X
3

2
Local 1 Axis is Not Parallel to pldirp (+Y)
Local 2 Axis is Rotated 90° from Y-1 Plane

Local 1 Axis is Parallel to pldirp (+Y)
Local 2 Axis is Rotated 90° from X-1 Plane

Figure 60
The Link/Support Element Coordinate Angle with Respect to Coordinate
Directions
The transverse axes 2 and 3 are defined as follows:
• If the reference vector is parallel to the 1-2 plane, then:
V3 = V1 ´ V p and
V2 = V3 ´ V1
• If the reference vector is parallel to the 1-3 plane, then:
V2 = V p ´ V1 and
V3 = V1 ´ V2
In the common case where the reference vector is perpendicular to axis V1 , the
transverse axis in the selected plane will be equal to Vp.

Internal Deformations
Six independent internal deformations are defined for the Link/Support element.
These are calculated from the relative displacements of joint j with respect to:
• Joint I for a two-joint element
• The ground for a single-joint element

260

Internal Deformations

Chapter XIV
The following two specifications are equivalent:
(a) local=12, plveca=0, plvecb=100
(b) local=13, plveca=101, plvecb=102

The Link/Support Element—Basic

Plane 1-2

Vp (a)
Axis 1

100

Axis 2
Joint j
Z
Vp (b)
102

Joint i
101

Plane 1-3
Axis 3

Figure 61
Using Joints to Define the Link/Support Element Local Coordinate System

For two-joint Link/Support elements the internal deformations are defined as:
• Axial:

du1 = u1j – u1i

• Shear in the 1-2 plane:

du2 = u2j – u2i – dj2 r3j – (L – dj2) r3i

• Shear in the 1-3 plane:

du3 = u3j – u3i + dj3 r2j + (L – dj3) r2i

• Torsion:

dr1 = r1j – r1i

• Pure bending in the 1-3 plane: dr2 = r2i – r2j
• Pure bending in the 1-2 plane: dr3 = r3j – r3i
where:
• u1i, u2i, u3i, r1i, r2i, and r3i are the translations and rotations at joint I
• u1j, u2j, u3j, r1j, r2j, and r3j are the translations and rotations at joint j
• dj2 is the distance you specify from joint j to the location where the shear deformation du2 is measured (the default is zero, meaning at joint j)
• dj3 is the distance you specify from joint j to the location where the shear deformation du3 is measured (the default is zero, meaning at joint j)
• L is the length of the element
Internal Deformations

261

CSI Analysis Reference Manual

du1

u1j

u2j
dr3
dj2

r3j

r3j
r3i
du2

r3i

1
u1i

2
u2i

Axial Deformation

Shear Deformation

Bending Deformation

Figure 62
Internal Deformations for a Two-Joint Link Element

All translations, rotations, and deformations are expressed in terms of the element
local coordinate system.
Note that shear deformation can be caused by rotations as well as translations.
These definitions ensure that all deformations will be zero under rigid-body motions of the element.
Important! Note that dj2 is the location where pure bending behavior is measured
in the 1-2 plane, in other words, it is where the moment due to shear is taken to be
zero. Likewise, dj3 is the location where pure bending behavior is measured in the
1-3 plane.
It is important to note that the negatives of the rotations r2i and r2j have been used for
the definition of shear and bending deformations in the 1-3 plane. This provides
consistent definitions for shear and moment in both the Link/Support and Frame elements.
Three of these internal deformations are illustrated in Figure 62 (page 262).
For one-joint grounded-spring elements the internal deformations are the same as
above, except that the translations and rotations at joint I are taken to be zero:

262

Internal Deformations

Chapter XIV

The Link/Support Element—Basic

• Axial:

du1 = u1j

• Shear in the 1-2 plane:

du2 = u2j – dj2 r3j

• Shear in the 1-3 plane:

du3 = u3j + dj3 r2j

• Torsion:

dr1 = r1j

• Pure bending in the 1-3 plane: dr2 = – r2j
• Pure bending in the 1-2 plane: dr3 = r3j

Link/Support Properties
A Link/Support Property is a set of structural properties that can be used to define
the behavior of one or more Link or Support elements. Each Link/Support Property
specifies the force-deformation relationships for the six internal deformations.
Mass and weight properties may also be specified.
Link/Support Properties are defined independently of the Link and Support elements and are referenced during the definition of the elements.
There are two categories of Link/Support properties that can be defined:
• Linear/Nonlinear. A Linear/Nonlinear property set must be assigned to each
Link or Support element.
• Frequency-Dependent. The assignment of a Frequency-Dependent property
set to a Link or Support element is optional.
All Linear/Nonlinear property sets contain linear properties that are used by the element for linear analyses, and for other types of analyses if no other properties are
defined. Linear/Nonlinear property sets may also have nonlinear properties that
will be used for all nonlinear analyses, and for linear analyses that continue from
nonlinear analyses.
Frequency-dependent property sets contain impedance (stiffness and damping)
properties that will be used for all frequency-dependent analyses. If a Frequency-Dependent property has not been assigned to a Link/Support element, the
linear properties for that element will be used for frequency-dependent analyses.
This is summarized in the table of Figure 63 (page 264).

Link/Support Properties

263

CSI Analysis Reference Manual

Load Case
Type

Linear

Nonlinear

Load Case
Initial
Conditions

Element has
Nonlinear
Properties?

Element has
Freq. Dep.
Properties?

Actual
Property
Used

Zero

Yes or No

Linear

Yes or No

Linear

Yes

Yes or No

Nonlinear

Yes or No

Linear

Yes

Yes or No

Nonlinear

Linear

Yes

Freq. Dep.

Linear

Yes

Nonlinear

Yes or No

Yes

Freq. Dep.

Nonlinear
Case

Any

Zero
Frequency
Dependent
Nonlinear
Case

Yes or No

Figure 63
Link/Support Stiffness Properties Actually Used for Different Types of Analysis

Local Coordinate System
Link/Support Properties are defined with respect to the local coordinate system of
the Link or Support element. The local 1 axis is the longitudinal direction of the element and corresponds to extensional and torsional deformations. The local 2 and 3
directions correspond to shear and bending deformations.
See Topic “Local Coordinate System” (page 253) in this Chapter.

Internal Spring Hinges
Each Link/Support Property is assumed to be composed of six internal “springs” or
“Hinges,” one for each of six internal deformations. Each “spring” may actually

264

Link/Support Properties

Chapter XIV

The Link/Support Element—Basic

Joint j

dj2

Axial

Shear

Pure
Bending

2
Joint i
or ground

Figure 64
Three of the Six Independent Spring Hinges in a Link/Support Element

consist of several components, including springs and dashpots. The forcedeformation relationships of these springs may be coupled or independent of each
other.
Figure 64 (page 265) shows the springs for three of the deformations: axial, shear in
the 1-2 plane, and pure-bending in the 1-2 plane. It is important to note that the
shear spring is located a distance dj2 from joint j. All shear deformation is assumed
to occur in this spring; the links connecting this spring to the joints (or ground) are
rigid in shear. Deformation of the shear spring can be caused by rotations as well as
translations at the joints. The force in this spring will produce a linearly-varying
moment along the length. This moment is taken to be zero at the shear spring, which
acts as a moment hinge. The moment due to shear is independent of, and additive
to, the constant moment in the element due to the pure-bending spring.
The other three springs that are not shown are for torsion, shear in the 1-3 plane, and
pure-bending in the 1-3 plane. The shear spring is located a distance dj3 from joint
j.
The values of dj2 and dj3 may be different, although normally they would be the
same for most elements.

Link/Support Properties

265

CSI Analysis Reference Manual
P

M2
j

j
V3

2
3

M3
i

i
V2

Figure 65
Link/Support Element Internal Forces and Moments, Shown Acting at the Joints

Spring Force-Deformation Relationships
There are six force-deformation relationships that govern the behavior of the element, one for each of the internal springs:
• Axial:

fu1 vs. du1

• Shear:

fu2 vs. du2 , fu3 vs. du3

• Torsional:

fr1 vs. dr1

• Pure bending: fr2 vs. dr2 , fr3 vs. dr3
where fu1, fu2, and fu3 are the internal-spring forces; and fr1, fr2, and fr3 are the internalspring moments.
Each of these relationships may be zero, linear only, or linear/nonlinear for a given
Link/Support Property. These relationships may be independent or coupled. The

266

Link/Support Properties

Chapter XIV

The Link/Support Element—Basic

forces and moments may be related to the deformation rates (velocities) as well as
to the deformations.

Element Internal Forces
The Link/Support element internal forces, P, V 2, V 3, and the internal moments, T,
M 2, M 3, have the same meaning as for the Frame element. These are illustrated in
Figure 65 (page 266). These can be defined in terms of the spring forces and moments as:
• Axial:

P = fu1

• Shear in the 1-2 plane:

V2 = fu2 ,

M3s = (d – dj2) fu2

• Shear in the 1-3 plane:

V3 = fu3 ,

M2s = (d – dj3) fu3

• Torsion:

T = fr1

• Pure bending in the 1-3 plane: M2b = fr2
• Pure bending in the 1-2 plane: M3b = fr3
where d is the distance from joint j. The total bending-moment resultants M 2 and
M 3 composed of shear and pure-bending parts:
M 2 = M 2s + M 2b
M 3 = M 3s + M 3b
These internal forces and moments are present at every cross section along the
length of the element.
See Topic “Internal Force Output” (page 144) in Chapter “The Frame Element.”

Uncoupled Linear Force-Deformation Relationships
If each of the internal springs are linear and uncoupled, the spring forcedeformation relationships can be expressed in matrix form as:
ì f u1 ü é k u1
ïf ï ê
ï u2 ï ê
ï f u3 ï ê
í
ý=ê
ï f r1 ï ê
ï f r2 ï ê
ïf ï ê
î r3 þ ë

0
k u2

sym.

0
0

k u3

0
k r1

0
0
k r2

0 ù ì d u1 ü
0 ú ï d u2 ï
úï
ï
0 ú ï d u3 ï
í
ý
0 ú ï d r1 ï
ú
0 ú ï d r2 ï
k r 3 úû ïî d r 3 ïþ

Link/Support Properties

(Eqn. 1)

267

CSI Analysis Reference Manual
where ku1, ku2, ku3, kr1, kr2, and kr3 are the linear stiffness coefficients of the internal
springs.
This can be recast in terms of the element internal forces and displacements at joint
j for a one-joint element as:
(Eqn. 2)
ì P ü
é k u1
ïV2 ï
ê
ï
ï
ê
ïV3 ï
ê
í
ý =ê
ï T ï
ê
ï M 2ï
ê
ï M 3ï
ê
î
þj ë

0
k u2

0
0

k u3

0
k r1

-dj3 k u 3
0
k r 2 + dj3 2 k u 3

sym.

ù ì u1 ü
úï u ï
ú ï 2ï
0
ú ï u3 ï
úí r ý
0
ú ï 1ï
0
ú ï -r2 ï
2
+ dj2 k u 2 úû ïî r3 ïþ j

0
-dj2 k u 2

k r3

This relationship also holds for a two-joint element if all displacements at joint I are
zero.
Similar relationships hold for linear damping behavior, except that the stiffness
terms are replaced with damping coefficients, and the displacements are replaced
with the corresponding velocities.
Consider an example where the equivalent shear and bending springs are to be
computed for a prismatic beam with a section bending stiffness of EI in the 1-2
plane. The stiffness matrix at joint j for the 1-2 bending plane is:
ìV2 ü
EI
í
ý = 3
î M 3þ j L

é 12 -6Lù ì u 2 ü
ê -6L 4L2 ú í r ý
ë
û î 3 þj

From this it can be determined that the equivalent shear spring has a stiffness of
EI
L
located at dj2 = , and the equivalent pure-bending spring has a stiffk u2 = 12
3
2
L
EI
ness of k r3 = .
L
For an element that possesses a true moment hinge in the 1-2 bending plane, the
pure-bending stiffness is zero, and dj2 is the distance to the hinge. See Figure 66
(page 269).

268

Link/Support Properties

Chapter XIV
u2j

The Link/Support Element—Basic
u2j

u2j
j

dj2=0
dj2
dj2
1

2
i

i
Hinge at Joint j

Hinge near Joint i

i
No hinge

Figure 66
Location of Shear Spring at a Moment Hinge or Point of Inflection

Types of Linear/Nonlinear Properties
The primary Linear/Nonlinear Link/Support Properties may be of the following
types:
• Coupled Linear
• Damper
• Gap
• Hook
• Multi-linear Elastic
• Multi-linear Plastic
• Plastic (Wen)
• Hysteretic (Rubber) Isolator
• Friction-Pendulum Isolator
• Tension/Compression Friction Pendulum Isolator
The first type, Coupled Linear, may have fully coupled linear stiffness and damping coefficients. This property type is described in Topic “Coupled Linear Property” (page 269) in this Chapter.
All other property types are considered nonlinear. However, for each nonlinear
property type you also specify a set of uncoupled linear stiffness and damping coefLink/Support Properties

269

CSI Analysis Reference Manual
ficients that are used instead of the nonlinear properties for linear analyses. These
substitute linear properties are called “linear effective stiffness” and “linear effective damping” properties.
For more information:
• See Topic “Coupled Linear Property” (page 269) in this Chapter.
• See Chapter “The Link/Support Element—Advanced” (page 275).

Coupled Linear Property
The Coupled Linear Link/Support Property is fully linear. It has no nonlinear behavior. The linear behavior is used for all linear and nonlinear analyses. It is also
used for frequency-dependent analyses unless frequency-dependent properties
have been assigned to the Link/Support element.
The stiffness matrix of Eqn. (1) (page 267) may now be fully populated:
ì f u1 ü é k u1
ïf ï ê
ï u2 ï ê
ï f u3 ï ê
í
ý=ê
ï f r1 ï ê
ï f r2 ï ê
ïf ï ê
î r3 þ ë

k u1u 2
k u2

k u1u 3
k u2u3

k u1r1
k u 2 r1

k u1r 2
k u2r 2

k u3

k u 3 r1
k r1

k u3r 2
k r1r 2
k r2

sym.

k u1r 3 ù ì d u1 ü
k u2r 3 ú ï d u2 ï
úï
ï
k u3r 3 ú ï d u3 ï
í
ý
k r1r 3 ú ï d r1 ï
ú
k r 2r 3 ú ï d r 2 ï
k r 3 úû ïî d r 3 ïþ

(Eqn. 3)

where ku1, ku1u2, ku2, ku1u3, ku2u3, ku3, ..., kr3 are the linear stiffness coefficients of the internal springs.
The corresponding matrix of Eqn. (2) (page 268) can be developed from the relationships that give the element internal forces in terms of the spring forces and moments. See Topic “Element Internal Forces” (page 267) in this Chapter.
Similarly, the damping matrix is fully populated and has the same form as the stiffness matrix. Note that the damping behavior is active for all dynamic analyses. This
is in contrast to linear effective damping, which is not active for nonlinear analyses.

Fixed Degrees of Freedom
It is possible to select any number or all of the element deformation degrees of freedom (DOF) to be fixed, i.e., that their deformation is zero. For a two-joint link, this

270

Coupled Linear Property

Chapter XIV

The Link/Support Element—Basic

is equivalent to specifying a joint constraint. For a one-joint link, this is equivalent
to specifying a restraint.
While this feature is convenient, it should be used with care. There are several important considerations that should be kept in mind.
• Link elements with fixed DOF should not be connected to other fixed link elements or connected to constrained joints. Otherwise, this will result in joints
that are multiply-constrained, which may be inaccurate for dynamics.
• For link elements with non-zero length, fixing fewer than all six DOF can lead
to loss of mass coupling between rotational and translational DOF, which can
affect the dynamics of the structure if large masses or rotational inertias are
present at the connected joints.
• When all six DOF are fixed, a full rigid-body constraint is used so that the
translational and rotational inertia will be accurately handled, with no loss of
coupling, provided that the link elements is not connected to other constrained
joints or fixed links.
• Link forces are not reported for fixed DOF.
If forces are needed at fixed DOF, if fixed links are connected to constrained joints,
or if inertial coupling will be lost for non-zero length elements, it is recommended
that large stiffnesses be used rather than fixed DOF to represent rigid conditions. It
is important to use stiffness values that are large enough to prevent significant deformation, but not so large as to cause numerical sensitivity in the equation solution, particularly near nonlinearities in the model. Choose stiffness values that are
about 100 to 10000 times larger than those in connected elements that are expected
to undergo deformation.

Mass
In a dynamic analysis, the mass of the structure is used to compute inertial forces.
The mass contributed by the Link or Support element is lumped at the joints I and j.
No inertial effects are considered within the element itself.
For each Link/Support Property, you may specify a total translational mass, m.
Half of the mass is assigned to the three translational degrees of freedom at each of
the element’s one or two joints. For single-joint elements, half of the mass is assumed to be grounded.
You may additionally specify total rotational mass moments of inertia, mr1, mr2,
and mr3, about the three local axes of each element. Half of each mass moment of
Mass

271

CSI Analysis Reference Manual
inertia is assigned to each of the element’s one or two joints. For single-joint elements, half of each mass moment of inertia is assumed to be grounded.
The rotational inertias are defined in the element local coordinate system, but will
be transformed by the program to the local coordinate systems for joint I and j. If
the three inertias are not equal and element local axes are not parallel to the joint local axes, then cross-coupling inertia terms will be generated during this transformation. These will be discarded by the program, resulting in some error.
It is strongly recommended that there be mass corresponding to each nonlinear deformation load in order to generate appropriate Ritz vectors for nonlinear modal
time-history analysis. Note that rotational inertia is needed as well as translational
mass for nonlinear shear deformations if either the element length or dj is non-zero.
For more information:
• See Topic “Mass Source” (page 334) in Chapter “Load Patterns”.
• See Chapter “Static and Dynamic Analysis” (page 341).
• See Topic “Nonlinear Deformation Loads” (page 271) in this Chapter.

Self-Weight Load
Self-Weight Load activates the self-weight of all elements in the model. For each
Link/Support Property, a total self-weight, w, may be defined. Half of this weight is
assigned to each joint of each Link/Support element using that Link/Support Property. For single-joint elements, half of the weight is assumed to be grounded.
Self-Weight Load always acts downward, in the global –Z direction. You may
scale the self-weight by a single scale factor that applies equally to all elements in
the structure.
See Topic “Self-Weight Load” (page 325) in Chapter “Load Patterns” for more information.

Gravity Load
Gravity Load can be applied to each Link/Support element to activate the selfweight of the element. Using Gravity Load, the self-weight can be scaled and applied in any direction. Different scale factors and directions can be applied to each
element.

272

Self-Weight Load

Chapter XIV

The Link/Support Element—Basic

If all elements are to be loaded equally and in the downward direction, it is more
convenient to use Self-Weight Load.
For more information:
• See Topic “Self-Weight Load” (page 272) in this Chapter for the definition of
self-weight for the Link/Support element.
• See Topic “Gravity Load” (page 326) in Chapter “Load Patterns.”

Internal Force and Deformation Output
Link/Support element internal forces and deformations can be requested for Load
Cases and Load Combinations.
Results for linear analyses are based upon the linear effective-stiffness and
effective-damping properties and do not include any nonlinear effects. Only the results for nonlinear Load Cases include nonlinear behavior.
The element internal forces were defined in Subtopic “Element Internal Forces”
(page 267) of this Chapter. The internal deformations were defined in Topic “Internal Deformations” (page 260) of this Chapter.
The element internal forces are labeled P, V2, V3, T, M2, and M3 in the output. The
internal deformations are labeled U1, U2, U3, R1, R2, and R3 in the output, corresponding to the values of du1, du2, du3, dr1, dr2, and dr3.
For more information:
• See Chapter “Load Patterns” (page 321).
• See Chapter “Load Cases” (page 341).

Internal Force and Deformation Output

273

CSI Analysis Reference Manual

274

Internal Force and Deformation Output

C h a p t e r XV

The Link/Support Element—Advanced
The basic, linear behavior of the Link and Support elements was described in the
previous Chapter. The present Chapter describes the use of the Link and Support elements to model nonlinear behavior and frequency-dependent behavior.
Advanced Topics
• Overview
• Nonlinear Link/Support Properties
• Linear Effective Stiffness
• Linear Effective Damping
• Exponential Maxwell Damper Property
• Bilinear Maxwell Damper Property
• Friction-Spring Damper Property
• Gap Property
• Hook Property
• Wen Plasticity Property
• Multi-Linear Elastic Property
• Multi-Linear Plastic Property

275

CSI Analysis Reference Manual
• Hysteretic (Rubber) Isolator Property
• Friction-Pendulum Isolator Property
• Double-Acting Friction-Pendulum Isolator Property
• Triple-Pendulum Isolator Property
• Nonlinear Deformation Loads
• Frequency-Dependent Properties

Overview
The basic features of the Link and Support elements were described in the previous
Chapter, “The Link/Support Element—Basic” (page 251).
This Chapter describes the various type of nonlinear properties that are available,
the concepts of linear effective stiffness and damping, the use of nonlinear deformation loads for Ritz-vector analysis, and frequency-dependent properties.

Nonlinear Link/Support Properties
The nonlinear properties for each Link/Support Property must be of one of the
various types described below. The type determines which degrees of freedom may
be nonlinear and the kinds of nonlinear force-deformation relationships available
for those degrees of freedom.
Every degree of freedom may have linear effective-stiffness and effective-damping
properties specified, as described below in Subtopics “Linear Effective Stiffness”
and “Linear Effective Damping.”
During nonlinear analysis, the nonlinear force-deformation relationships are used
at all degrees of freedom for which nonlinear properties were specified. For all
other degrees of freedom, the linear effective stiffnesses are used during a nonlinear
analysis.
Linear analyses that start from zero initial conditions will use the linear effective
stiffness regardless of whether nonlinear properties were specified or not. Linear
analyses that use the stiffness from the end of a previous nonlinear analysis will use
the nonlinear properties. Linear effective damping is used for all linear analyses,
but it is not used for any nonlinear analysis.

276

Overview

Chapter XV

The Link/Support Element—Advanced

Each nonlinear force-deformation relationship includes a stiffness coefficient, k.
This represents the linear stiffness when the nonlinear effect is negligible, e.g., for
rapid loading of the Damper; for a closed Gap or Hook; or in the absence of yielding or slipping for the Plastic1, Isolator1, or Isolator2 properties. If k is zero, no
nonlinear force can be generated for that degree of freedom, with the exception of
the pendulum force in the Isolator2 property.
IMPORTANT! You may sometimes be tempted to specify very large values for k,
particularly for Maxwell Dampers, Gap, and Hook properties. Resist this temptation! If you want to limit elastic deformations in a particular internal spring, it is
2
4
usually sufficient to use a value of k that is from 10 to 10 times as large as the corresponding stiffness in any connected elements. Larger values of k may cause numerical difficulties during solution. See the additional discussion for the Maxwell
Damper properties below.

Linear Effective Stiffness
For each nonlinear type of Link/Support Property, you may specify six uncoupled
linear effective-stiffness coefficients, ke, one for each of the internal springs.
The linear effective stiffness represents the total elastic stiffness for the Link/Support element that is used for all linear analyses that start from zero initial conditions. The actual nonlinear properties are ignored for these types of analysis.
If you do not specify nonlinear properties for a particular degree of freedom, then
the linear effective stiffness is used for that degree of freedom for all linear and nonlinear analyses.
The effective force-deformation relationships for the Link/Support Properties are
given by Equation 1 above with the appropriate values of ke substituted for ku1, ku2,
ku3, kr1, kr2, and kr3.

Special Considerations for Modal Analyses
The effective stiffness properties are not used for nonlinear degrees of freedom during nonlinear time-history analysis. However, nonlinear modal time-history (FNA)
analyses do make use of the vibration modes that are computed based on the effective stiffness if the modal analysis itself uses the stiffness from zero initial conditions. During time integration the behavior of these modes is modified so that the
structural response reflects the actual stiffness and other nonlinear parameters spec-

Linear Effective Stiffness

277

CSI Analysis Reference Manual
ified. The rate of convergence of the nonlinear iteration may be improved by
changing the effective stiffness.
Following are some guidelines for selecting the linear effective stiffness. You
should deviate from these as necessary to achieve your modeling and analysis
goals. In particular, you should consider whether you are more interested in the results to be obtained from linear analyses, or in obtaining modes that are used as the
basis for nonlinear modal time-history analyses.
• When carrying out analyses based on the UBC ‘94 code or similar, the effective
stiffness should usually be the code-defined maximum effective stiffness
• For Gap and Hook elements the effective stiffness should usually be zero or k,
depending on whether the element is likely to be open or closed, respectively,
in normal service
• For Damper elements, the effective stiffness should usually be zero
• For other elements, the stiffness should be between zero and k
• If you have chosen an artificially large value for k, be sure to use a much
smaller value for ke to help avoid numerical problems in nonlinear modal
time-history analyses
In the above, k is the nonlinear stiffness property for a given degree of freedom. See
Chapter “The Link/Support Element—Basic” (page 251).
Remember that the above considerations do not apply for modes calculated using
the stiffness from the end of a nonlinear static or nonlinear direct-integration
time-history load case. In this case, the actual nonlinear stiffness of the links at the
end of the nonlinear stiffness load case is used, and the effective stiffness is disregarded for nonlinear degrees of freedom.
For more information, see Topic “Nonlinear Modal Time-History Analysis
(FNA)” (page 349) in Chapter “Nonlinear Time-History Analysis.”

Linear Effective Damping
For each nonlinear-type of Link/Support Property, you may specify six uncoupled
linear effective-damping coefficients, ce, one for each of the internal springs. By
default, each coefficient ce is equal to zero.
The linear effective damping represents the total viscous damping for the
Link/Support element that is used for response-spectrum analyses, for linear and
periodic time-history analyses, and for frequency-dependent analyses if fre-

278

Linear Effective Damping

Chapter XV

The Link/Support Element—Advanced

quency-dependent properties have not been assigned to a given Link or Support element. The actual nonlinear properties are ignored for these types of analysis. Effective damping can be used to represent energy dissipation due to nonlinear damping, plasticity, or friction.
The effective force/deformation-rate relationships for the Link/Support Properties
are given by Equation 1 above with the appropriate values of ce substituted for ku1,
ku2, ku3, kr1, kr2, and kr3, and deformation rates substituted for the corresponding deformations.
For response-spectrum and linear modal time-history analysis, the effective damping values are converted to modal damping ratios assuming proportional damping,
i.e., the modal cross-coupling damping terms are ignored. These effective
modal-damping values are added to any other modal damping that you specify directly. The program will not permit the total damping ratio for any mode to exceed
99.995%.
Important Note: Modal cross-coupling damping terms can be very significant for
some structures. A linear analysis based on effective-damping properties may
grossly overestimate or underestimate the amount of damping present in the structure.
Nonlinear time-history analysis is strongly recommended to determine the effect of
added energy dissipation devices. Nonlinear time-history analysis does not use the
effective damping values since it accounts for energy dissipation in the elements directly, and correctly accounts for the effects of modal cross-coupling.

Exponential Maxwell Damper Property
This element is very well suited for modeling viscous dampers that have a nonlinear force-velocity relationship. For simple linear damping, you may instead want to
use the coupled linear Link Support Property. The linear property does not require
the series spring used by the exponential Maxwell damper, and it does allow you to
consider a parallel spring. See Topic “Coupled Linear Property” (page 270) for
more information
For the exponential damper, you can specify independent damping properties for
each deformational degree of freedom. The damping properties are based on the
Maxwell model of viscoelasticity (Malvern, 1969) having a exponential viscous
damper in series with a linear spring. See Figure 67 (page 280). If you do not specify nonlinear properties for a degree of freedom, that degree of freedom is linear using the effective stiffness, which may be zero.
Exponential Maxwell Damper Property

279

CSI Analysis Reference Manual
j

Gap

Damper

Hook

open

Figure 67
Maxwell Dampers, Gap, and Hook Property Types,
Shown for Axial Deformations

The nonlinear force-deformation relationship is given by:
cexp
f = k d k = c d& c

where k is the spring constant, c is the damping coefficient, cexp is the damping exponent, d k is the deformation across the spring, and d& c is the deformation rate
across the damper. The damping exponent must be positive; the practical range is
between 0.2 and 2.0.
The spring and damping deformations sum to the total internal deformation:
d = dk + dc
The series spring is very important for capturing realistic behavior of nonlinear
dampers, especially those with fractional exponents. It represents the elastic flexibility of the damping device, including the fluid column and the connecting mechanisms. It prevents the damping term from producing unrealistically large viscous
forces at small velocities, which can have a very significant impact on overall structural behavior.
You may be tempted to introduce a large stiffness value, k, to represent “pure”
damping, but this may result in unconservative and unrealistic behavior. It would
be better to get a realistic value of the elastic flexibility from the manufacturer of

280

Exponential Maxwell Damper Property

Chapter XV

The Link/Support Element—Advanced

the device and the details of the connections, or make an engineering estimate of
the value. For more information about the importance of the spring constant, see the
Software Verification Manual, where SAP2000 results are compared with experiment.

Bilinear Maxwell Damper Property
This element is well suited for modeling viscous dampers, including oil dampers,
that have a bilinear force-velocity relationship. Such dampers typically have a relief valve that reduces the damping coefficient when a certain relief (or “yield”)
force level is reached. See Kasai (2004) for more information.
For the bilinear damper, you can specify independent damping properties for each
deformational degree of freedom. The damping properties are based on the
Maxwell model of viscoelasticity (Malvern, 1969) having a bilinear viscous
damper in series with a linear spring. See Figure 67 (page 280). If you do not specify nonlinear properties for a degree of freedom, that degree of freedom is linear using the effective stiffness, which may be zero.
The nonlinear force-deformation relationship is given by:
ìï
c1 d& c
c1| d& c | £ f1
f = k dk = í
ïî f1 + c2 ( d& c - d& c1 ) c1| d& c | ³ f1
where k is the spring constant, c1 is the damping coefficient for force levels below
the relief force, c2 is the damping coefficient for force levels above the relief force,
f1 is the relief force, d k is the deformation across the spring, d& c is the deformation
rate across the damper, and d& = f1 / c1. The damping coefficients must satisfy the
c1

relationship c1 > c2 ³ 0.
The spring and damping deformations sum to the total internal deformation:
d = dk + dc
The series spring is very important for capturing realistic behavior of nonlinear
dampers. It represents the elastic flexibility of the damping device, including the
fluid column and the connecting mechanisms, which can have a very significant
impact on overall structural behavior.
You may be tempted to introduce a large stiffness value, k, to represent “pure”
damping, but this may result in unconservative and unrealistic behavior. It would

Bilinear Maxwell Damper Property

281

CSI Analysis Reference Manual
be better to get a realistic value of the elastic flexibility from the manufacturer of
the device and the details of the connections, or make an engineering estimate of
the value. Expected values for oil dampers may be on the order of c1 / k = 0.1 second.
The formulation used for this element works best if the time-step size is small compared to the period of excitation. This is usually not a problem for nonlinear modal
(FNA) time-history analysis, which tends to automatically use very small time
sub-steps. For nonlinear direct-integration time-history analysis, you should try
different time-step sizes until consistent results are obtained. You can either change
the size of the output time steps or change the maximum sub-step size (one of the
nonlinear load-case parameters).

Friction-Spring Damper Property
This element represents a hysteretic damping system consisting of a stack of alternating inner and outer metallic rings that exhibit internal friction when the stack is
loaded in compression and again when the stack unloads. Each cycle of loading and
unloading dissipates energy hysteretically, meaning that it is based on displacement and is independent of velocity.
Although the fundamental mechanism is compression of the ring stack, manufactured devices may exhibit external damping behavior in compression, tension, or
both. In addition, kinematic mechanisms may be devised so that the frictional behavior can be applied to shear or moment degrees of freedom. For this reason, friction-spring behavior may be defined independently for any of the six degrees of
freedom of a link element.
A friction-spring system under loading-slipping exhibits a linear stiffness k1 that is
a combination of the elastic stiffness to compress the inner rings and expand the
outer rings, plus the frictional resistance. When unloading-slipping, the system exhibits a smaller linear stiffness k2 that is a combination of the same elastic stiffness
due to ring compression and expansion, but this time with the frictional resistance
acting in the opposite direction. The elastic transition between loading and unloading stiffness is along a much larger elastic stiffness k0.
This behavior is shown in Figure 68 (page 283). The stiffness values should satisfy
the following relationship:
k0 >> k1 > k2 > 0

282

Friction-Spring Damper Property

Chapter XV

The Link/Support Element—Advanced

k0
k2

Figure 68
Force-Deformation Behavior of a Friction-Spring Damper in Tension
with Stop Displacement but No Precompression
There is usually a limiting stop displacement ds > 0 beyond which the rings can no
longer slip. All deformation beyond the stop displacement loads and unloads along
the elastic stiffness of k0. If you set ds = 0 then no stop displacement is applied.
A precompression displacement dc < 0 may also be specified. This has the effect of
increasing the initial force at which slipping begins when loading to approximately
-k1 × dc, and at which slipping ends when unloading to approximately -k2 × dc, as
shown in Figure 69 (page 284). Loading and unloading from zero to these values
Friction-Spring Damper Property

283

CSI Analysis Reference Manual

k0
k2
k0
dc

Figure 69
Force-Deformation Behavior of a Friction-Spring Damper in Tension
with Stop Displacement and Precompression Displacement
occurs along the elastic stiffness of k0. If you set dc = 0 then no precompression
displacement is applied, and slipping begins and ends at zero force.
The force-deformation relationships shown in Figure 68 and Figure 69 are for tension (or any positive force or moment). Similar behavior could be specified in compression as well. If tension and compression behavior are both requested, the behavior is symmetrical about the origin as shown in Figure 70 (page 285). If unsym-

284

Friction-Spring Damper Property

Chapter XV

The Link/Support Element—Advanced

-ds

-dc

ds d

Figure 70
Force-Deformation Behavior of a Friction-Spring Damper in Symmetrical
Tension and Compression
metrical behavior is desired, you can use two elements in parallel, one for the tension behavior and one for the compression behavior.
Loading and unloading can occur along the solid lines, but only in the direction of
the arrows. The dotted lines in Figure 69 and Figure 70 are shown for reference to
the precompression displacement dc. However loading and unloading cannot occur
along the dotted lines.
The nonlinear force-deformation relationship when slipping is given by:
Friction-Spring Damper Property

285

CSI Analysis Reference Manual
f = k1 ( d - dc ) when loading-slipping, dd& > 0
f = k2 ( d - dc ) when unloading-slipping, dd& < 0
The force-displacement relationship is elastic along a line with stiffness k0 in the
transitions: (1) between sliding while loading and unloading, (2) from zero when
dc < 0, and (3) after the stop displacement ds > 0.
The values of k0, k1, k2, ds, and dc should be obtained from the manufacturer of
the device. The value of k0 should be large compared to k1 and k2, but not so large
as to cause numerical sensitivity, which in turn may produce inaccurate results or
nonlinear convergence problems. A realistic value is best, but it should probably be
no more than about 10,000 times larger than k1.

Gap Property
For each deformational degree of freedom you may specify independent gap
(“compression-only”) properties. See Figure 67 (page 280).
All internal deformations are independent. The opening or closing of a gap for one
deformation does not affect the behavior of the other deformations.
If you do not specify nonlinear properties for a degree of freedom, that degree of
freedom is linear using the effective stiffness, which may be zero.
The nonlinear force-deformation relationship is given by:
ì k ( d + open ) if d + open < 0
f =í
otherwise
î0
where k is the spring constant, and open is the initial gap opening, which must be
zero or positive.

Hook Property
For each deformational degree of freedom you may specify independent hook
(“tension-only”) properties. See Figure 67 (page 280).
All internal deformations are independent. The opening or closing of a hook for one
deformation does not affect the behavior of the other deformations.

286

Gap Property

Chapter XV

The Link/Support Element—Advanced

k,
yield,
ratio,
exp

Figure 71
Wen Plasticity Property Type for Uniaxial Deformation

If you do not specify nonlinear properties for a degree of freedom, that degree of
freedom is linear using the effective stiffness, which may be zero.
The nonlinear force-deformation relationship is given by:
ì k ( d - open ) if d - open > 0
f =í
otherwise
î0
where k is the spring constant, and open is the initial hook opening, which must be
zero or positive.

Wen Plasticity Property
For each deformational degree of freedom you may specify independent uniaxialplasticity properties. The plasticity model is based on the hysteretic behavior proposed by Wen (1976). See Figure 71 (page 287).
All internal deformations are independent. The yielding at one degree of freedom
does not affect the behavior of the other deformations.
If you do not specify nonlinear properties for a degree of freedom, that degree of
freedom is linear using the effective stiffness, which may be zero.
Wen Plasticity Property

287

CSI Analysis Reference Manual
f
exp ® ¥

ratio·k

yield
exp = 1
exp = 2

Figure 72
Definition of Parameters for the Wen Plasticity Property

The nonlinear force-deformation relationship is given by:
f = ratio k d + (1 - ratio ) yield z
where k is the elastic spring constant, yield is the yield force, ratio is the specified
ratio of post-yield stiffness to elastic stiffness (k), and z is an internal hysteretic
variable. This variable has a range of | z | £ 1, with the yield surface represented by
| z | =1. The initial value of z is zero, and it evolves according to the differential
equation:
z& =

k
yield

ì d& (1 - | z | exp ) if d& z > 0
í&
otherwise
îd

where exp is an exponent greater than or equal to unity. Larger values of this exponent increases the sharpness of yielding as shown in Figure 72 (page 288). The
practical limit for exp is about 20. The equation for z& is equivalent to Wen’s model
with A =1 and a = b = 05
..

288

Wen Plasticity Property

Chapter XV

The Link/Support Element—Advanced

Multi-Linear Elastic Property
For each deformational degree of freedom you may specify multi-linear elastic
properties.
All internal deformations are independent. The deformation in one degree of freedom does not affect the behavior of any other. If you do not specify nonlinear properties for a degree of freedom, that degree of freedom is linear using the effective
stiffness, which may be zero.
The nonlinear force-deformation relationship is given by a multi-linear curve that
you define by a set of points. The curve can take on almost any shape, with the following restrictions:
• One point must be the origin, (0,0)
• At least one point with positive deformation, and one point with negative deformation, must be defined
• The deformations of the specified points must increase monotonically, with no
two values being equal
• The forces (moments) can take on any value
The slope given by the last two specified points on the positive deformation axis is
extrapolated to infinite positive deformation. Similarly, the slope given by the last
two specified points on the negative deformation axis is extrapolated to infinite
negative deformation.
The behavior is nonlinear but it is elastic. This means that the element loads and unloads along the same curve, and no energy is dissipated. On the other hand, the
Multi-Linear Plastic Property defined next does exhibit hysteresis and dissipates
energy under reverse and cyclic loading.
See also Topic “Hysteresis Models” (page 85) in Chapter “Material Properties.”

Multi-Linear Plastic Property
This model is similar to the Multi-Linear Elastic Property defined above, but the
Plastic property exhibits different loading and unloading behavior, and thus dissipates energy according to various hysteresis models that are available. For each
deformational degree of freedom you may specify independent multi-linear plasticity properties.

Multi-Linear Elastic Property

289

CSI Analysis Reference Manual
All internal deformations are independent. The deformation in one degree of freedom does not affect the behavior of any other. If you do not specify nonlinear properties for a degree of freedom, that degree of freedom is linear using the effective
stiffness, which may be zero.
The nonlinear force-deformation relationship is given by a multi-linear curve that
you define by a set of points. The curve can take on almost any shape, with the following restrictions:
• One point must be the origin, (0,0)
• At least one point with positive deformation, and one point with negative deformation, must be defined
• The deformations of the specified points must increase monotonically, with no
two values being equal
• The forces (moments) at a point must have the same sign as the deformation
(they can be zero)
• The slope given by the last two points specified on the positive deformation
axis is extrapolated to infinite positive deformation, or until it reaches zero
value. Similarly, the slope given by the last two points specified on the negative
deformation axis is extrapolated to infinite negative deformation, or until it
reaches zero value.
The given curve defines the force-deformation (moment-rotation) relationship under monotonic loading. The first slope on either side of the origin is elastic; the remaining segments define plastic deformation. If the deformation reverses after
plastic deformation, unloading occurs along a different, steeper curve before beginning plastic deformation in the reverse direction.
This process of loading and unloading along different curves dissipates energy and
is called hysteresis. Several different hysteresis models are available to describe the
behavior of different types of materials. For the most part, these differ in the
amount of energy they dissipate in a given cycle of deformation, and how the energy dissipation behavior changes with an increasing amount of deformation.
The available hysteresis models for the Multi-Linear Plastic Property are described
in Topic “Hysteresis Models” (page 85) in Chapter “Material Properties”. These include kinematic, degrading, Takeda, pivot, concrete, BRB hardening, and isotropic.

290

Multi-Linear Plastic Property

Chapter XV

The Link/Support Element—Advanced

Hysteretic (Rubber) Isolator Property
This is a biaxial hysteretic isolator that has coupled plasticity properties for the two
shear deformations, and linear effective-stiffness properties for the remaining four
deformations. The plasticity model is based on the hysteretic behavior proposed by
Wen (1976), and Park, Wen and Ang (1986), and recommended for base-isolation
analysis by Nagarajaiah, Reinhorn and Constantinou (1991). See Figure 73 (page
292).
For each shear deformation degree of freedom you may independently specify either linear or nonlinear behavior:
• If both shear degrees of freedom are nonlinear, the coupled force-deformation
relationship is given by:
f u 2 = ratio2 k2 d u 2 + (1 - ratio2 ) yield2 z 2
f u 3 = ratio3 k3 d u 3 + (1 - ratio3 ) yield3 z 3
where k2 and k3 are the elastic spring constants, yield2 and yield3 are the yield
forces, ratio2 and ratio3 are the ratios of post-yield stiffnesses to elastic stiffnesses (k2 and k3), and z 2 and z 3 are internal hysteretic variables. These variz 2 2 + z 3 2 £ 1, with the yield surface represented by

ables have a range of

z 2 2 + z 3 2 = 1. The initial values of z 2 and z 3 are zero, and they evolve according to the differential equations:
2

ì z& 2 ü é1 - a 2 z 2
í& ý=ê
î z 3 þ ë -a 2 z 2 z 3

ì k2
-a 3 z 2 z 3 ù ïï yield2
úí
1 - a 3 z 3 2 û ï k3
ïî yield3

d& u 2 ü
ïï
ý
d& u 3 ï
ïþ

Where:
ì1 if d& u 2 z 2 > 0
a2 = í
î0 otherwise
ì1 if d& u 3 z 3 > 0
a3 = í
î0 otherwise
These equations are equivalent to those of Park, Wen and Ang (1986) with A =1
and b = g = 05
..

Hysteretic (Rubber) Isolator Property

291

CSI Analysis Reference Manual
j

fu
d

fu2

du2

1
3

2
i

Figure 73
Hysteretic Isolator Property for Biaxial Shear Deformation

• If only one shear degree of freedom is nonlinear, the above equations reduce to
the uniaxial plasticity behavior of the Plastic1 property with exp = 2 for that degree of freedom.
A linear spring relationship applies to the axial deformation, the three moment deformations, and to any shear deformation without nonlinear properties. All linear
degrees of freedom use the corresponding effective stiffness, which may be zero.

Friction-Pendulum Isolator Property
This is a biaxial friction-pendulum isolator that has coupled friction properties for
the two shear deformations, post-slip stiffness in the shear directions due the pendulum radii of the slipping surfaces, gap behavior in the axial direction, and linear
effective-stiffness properties for the three moment deformations. See Figure 74
(page 293).

292

Friction-Pendulum Isolator Property

Chapter XV

The Link/Support Element—Advanced
P
j

1
3

2
i
P

Figure 74
Friction-Pendulum Isolator Property for Biaxial Shear Behavior
This element can be used for gap-friction contact problems
This element can also be used to model gap and friction behavior between contacting surfaces by setting the radii to zero, indicating a flat surface.
The friction model is based on the hysteretic behavior proposed by Wen (1976),
and Park, Wen and Ang (1986), and recommended for base-isolation analysis by
Nagarajaiah, Reinhorn and Constantinou (1991). The pendulum behavior is as recommended by Zayas and Low (1990).
The friction forces and pendulum forces are directly proportional to the compressive axial force in the element. The element cannot carry axial tension.

Axial Behavior
The axial force, f u1 , is always nonlinear, and is given by:
Friction-Pendulum Isolator Property

293

CSI Analysis Reference Manual
ì k1 d u1 if d u1 < 0
f u1 = P = í
otherwise
î0
In order to generate nonlinear shear force in the element, the stiffness k1 must be
positive, and hence force P must be negative (compressive). A reasonable value for
the stiffness k1 can be obtained as the AE/L of the device, and should include the
flexibility of the connections or supports that is not otherwise included in the
model.
You may additionally specify a damping coefficient, c1, for the axial degree of
freedom, in which case the axial force becomes:
ìc1 d& u1 if d u1 < 0
f u1 = P + í
otherwise
î0
The damping force only exists when the isolator is in compression, regardless of
the sign of the velocity.
Force f u1 is the total axial force exerted by the element on the connected joints.
However, only the stiffness force P is assumed to act on the bearing surface, causing shear resistance. The damping force is external.
The purpose of the damping coefficient is to reduce the numerical chatter (oscillation) that can be present in some analyses. You can estimate the damping coefficient needed to achieve a certain ratio, r, of critical damping (e.g., r = 0.05) from the
formula
r=

c1
2 k1 m

where m is the tributary mass for the isolator, which could be estimated from the
self-weight axial force divided by the acceleration due to gravity. It is up to you to
verify the applicability of this approach for your particular application. See the
Software Verification Manual for a discussion on the use of this damping coefficient.

Shear Behavior
For each shear deformation degree of freedom you may independently specify either linear or nonlinear behavior:

294

Friction-Pendulum Isolator Property

Chapter XV

The Link/Support Element—Advanced

• If both shear degrees of freedom are nonlinear, the friction and pendulum effects for each shear deformation act in parallel:
f u2 = f u2 f + f u2 p
f u3 = f u3 f + f u3 p
The frictional force-deformation relationships are given by:
f u2 f = - P m u2 z 2
f u3 f = - P m u3 z 3
where m 2 and m 3 are friction coefficients, and z 2 and z 3 are internal hysteretic
variables. The friction coefficients are velocity-dependent according to:
m u 2 = fast2 - ( fast2 - slow2 ) e - r v

(Eqn. 1a)

m u 3 = fast3 - ( fast3 - slow3 ) e - r v
where slow2 and slow3 are the friction coefficients at zero velocity, fast2 and
fast3 are the friction coefficients at fast velocities, v is the resultant velocity of
sliding:
v = d& u 2 2 + d& u 3 2

(Eqn. 1b)

r is an effective inverse velocity given by:
r=

rate2 d& u 2 2 + rate3 d& u 3 2

(Eqn. 1c)

and rate2 and rate3 are the inverses of characteristic sliding velocities. For a
Teflon-steel interface the coefficient of friction normally increases with sliding
velocity (Nagarajaiah, Reinhorn, and Constantinou, 1991).
The internal hysteretic variables have a range of z 2 2 + z 3 2 £ 1, with the yield
surface represented by z 2 2 + z 3 2 = 1. The initial values of z 2 and z 3 are zero,
and they evolve according to the differential equations:
ì k2
2
a
z
z
&
é
ù
3 2 3 ï
ì z 2 ü 1 - a2 z 2
ï P m u2
í& ý=ê
úí
2
î z 3 þ ë -a 2 z 2 z 3 1 - a 3 z 3 û ï k3
îï P m u 3

d& u 2 ü
ïï
ý
d& u 3 ï
ïþ

Friction-Pendulum Isolator Property

295

CSI Analysis Reference Manual
where k2 and k3 are the elastic shear stiffnesses of the slider in the absence of
sliding, and
ì1
a2 = í
î0
ì1
a3 = í
î0

if d& u 2 z 2 > 0
otherwise
if d& u 3 z 3 > 0
otherwise

These equations are equivalent to those of Park, Wen and Ang (1986) with A =1
and b = g = 05
..
This friction model permits some sliding at all non-zero levels of shear force;
the amount of sliding becomes much larger as the shear force approaches the
“yield” value of P m. Sliding at lower values of shear force can be minimized by
using larger values of the elastic shear stiffnesses. However, realistic values of
the shear stiffness are recommended, and can be estimated as AG/L of the
locked-up device. This should also include the flexibility of the connections or
supports that is not otherwise included in the model.
The pendulum force-deformation relationships are given by:
d u2
radius2
d u3
=-P
radius3

f u2 p = - P
f u3 p

The specified radius should actually be the effective pendulum length, which is
the radius of the sliding surface minus the distance from the surface to the point
of articulation of the device. This information should be obtained from the
manufacturer of the device.
Normally the radii in the two shear directions will be equal (spherical surface),
or one radius will be zero (cylindrical surface). However, it is permitted to
specify unequal non-zero radii.
A zero radius indicates a flat surface, and the corresponding perpendicular
shear force is zero. This can be used to model general gap-friction behavior .
• If only one shear degree of freedom is nonlinear, the above frictional equations
reduce to:
f

296

=-Pm z

Friction-Pendulum Isolator Property

Chapter XV
m = fast - ( fast - slow ) e
z& =

k
Pm

The Link/Support Element—Advanced

- rate d&

ì d& (1 - z 2 ) if d& z > 0
í&
otherwise
îd

The above pendulum equation is unchanged for the nonlinear degree of freedom.

Linear Behavior
A linear spring relationship applies to the three moment deformations, and to any
shear deformation without nonlinear properties. All linear degrees of freedom use
the corresponding effective stiffness, which may be zero. The axial degree of freedom is always nonlinear for nonlinear analyses.

Double-Acting Friction-Pendulum Isolator Property
This is a biaxial friction-pendulum isolator that supports tension as well as compression, and has uncoupled behavior in the two shear directions. The frictional resistance can be different depending on whether then isolator is in tension or compression. This device consists of two orthogonal, curved rails that are interlocked
together. It is intended to provide seismic isolation with uplift prevention, and is
described in detail by Roussis and Constantinou [2005].

Axial Behavior
Independent stiffnesses and gap openings may be specified for tension and compression. The axial force, f u1 , is always nonlinear, and is given by:
f u1

ì k1c ( d u1 + openc ) if ( d u1 + openc ) < 0
ï
= P = í k1t ( d u1 - opent ) if ( d u1 - opent ) > 0
ï0
otherwise
î

where k1c is the compressive stiffness, k1t is the tensile stiffness, openc is the gap
opening in compression, and opent is the gap opening in tension. Each of the four
values may be zero or positive.
You may additionally specify a damping coefficient, c1, for the axial degree of
freedom, in which case the axial force becomes:

Double-Acting Friction-Pendulum Isolator Property

297

CSI Analysis Reference Manual
f u1 = P + c1 d& u1
The damping force exists whether the isolator is in tension, compression, or is gapping.
Force f u1 is the total axial force exerted by the element on the connected joints.
However, only the stiffness force P is assumed to act on the bearing surface, causing shear resistance. The damping force is external. See Topic “Friction-Pendulum
Isolator Property” (page 292) for a discussion on the use of this damping.

Shear Behavior
For each shear deformation degree of freedom you may independently specify either linear or nonlinear behavior. The behavior in the two shear directions is uncoupled, although they both depend on the same axial force P.
For each nonlinear shear degree of freedom u2 or u3, you independently specify the
following parameters:
• Stiffness k, representing the elastic behavior before sliding begins. This value
is the same for positive or negative P.
• Friction coefficients slowc and fastc for friction under compression at different
velocities, and coefficients slowt and fastt for friction under tension at different velocities.
• Rate parameters ratec and ratet for friction under compression and tension, respectively. These are the inverses of characteristic sliding velocities. For a Teflon-steel interface the coefficient of friction normally increases with sliding velocity (Nagarajaiah, Reinhorn, and Constantinou, 1991).
• Radius radius, which is the same for tension and compression.
Looking at one shear direction, and considering either tension or compression using the appropriate friction parameters, the shear force f is given by:
f =f
f

+fp

=-Pm z

m = fast - ( fast - slow ) e
z& =

298

k
Pm

- rate d&

ì d& (1 - z 2 ) if d& z > 0
í&
otherwise
îd

Double-Acting Friction-Pendulum Isolator Property

Chapter XV
f p =-P

The Link/Support Element—Advanced

d
radius

where d is the shear deformation and z is an internal hysteretic variable. In the
above, the indicators for shear degree of freedom u2 or u3, as well as for tension or
compression, have been dropped.

Triple-Pendulum Isolator Property
This is a biaxial friction-pendulum isolator (or bearing) that has four spherical sliding surfaces, two outer and two inner, as shown in Figure 75 (page 301). Kinematic
considerations couple the motion of the two inner sliders, resulting in behavior that
can be modeled as three friction-pendulum isolators in series. By choosing different friction coefficients and radii for the various sliding surfaces, the transverse
(shear) force-deflection curve can be tailored to provide different response for different levels of excitation. The properties of the two inner sliders are assumed to be
identical. The characteristics and performance of this type of isolator are described
in Morgan and Mahin (2008).
Each of the three pendula that act series for the triple pendulum uses the same mathematical model as described in the topic “Friction-Pendulum Isolator Property”
(page 292), with differences as described below. The axial and moment behavior
are for the isolator as a whole. The shear forces are equal in the three pendula, while
the shear deformations and velocities are additive.
The friction forces and pendulum forces are directly proportional to the compressive axial force in the element. The element cannot carry axial tension.

Axial Behavior
The axial force, f u1 , is always nonlinear, and is given by:
ì k1 d u1 if d u1 < 0
f u1 = P = í
otherwise
î0
Triple-Pendulum Isolator Property

299

CSI Analysis Reference Manual
In order to generate nonlinear shear force in the element, the stiffness k1 must be
positive, and hence force P must be negative (compressive).
You may additionally specify a damping coefficient, c1, for the axial degree of
freedom, in which case the axial force becomes:
ìc1 d& u1 if d u1 < 0
f u1 = P + í
otherwise
î0
The damping force only exists when the isolator is in compression.
Force f u1 is the total axial force exerted by the element on the connected joints.
However, only the stiffness force P is assumed to act on the sliding surfaces, causing shear resistance. The damping force is external.
The purpose of the damping coefficient is to reduce the numerical chatter (oscillation) that can be present in some analyses. You can estimate the damping coefficient needed to achieve a certain ratio, r, of critical damping (e.g., r = 0.05) from the
formula
r=

c1
2 k1 m

Shear Behavior
For each shear deformation degree of freedom you may independently specify either linear or nonlinear behavior. In the usual case where both the u2 and u3 degrees
of freedom are nonlinear, the behavior is isotropic and the properties are identical
in both directions. In other words, the sliding surfaces are spherical.
The four sliding surfaces are identified as:
• Inner Bottom (index 1)
• Inner Top, identical to Inner Bottom (index 1)
• Outer Bottom (index 2)
• Outer Top (index 3)

300

Triple-Pendulum Isolator Property

Chapter XV

The Link/Support Element—Advanced

Figure 75
Triple-Pendulum Isolator with Four Sliding Surfaces
The two inner surfaces are always symmetrical
These are shown in Figure 75 (page 301). In the discussion below, the indices
shown above will be used to identify the three pendulum mechanisms.
For each sliding surface, the following isotropic properties are specified:
• stiff, shear stiffness before sliding, and stiffness at the stop
• slow, friction coefficient at zero velocity
• fast, friction coefficient at fast velocity
• rate, inverse of the characteristic velocity for friction
• radius, actual spherical radius of the surface
• stop, transverse displacement permitted before encountering a stiff stop
In addition, two heights are specified giving the distances between the sliding surfaces:
• heightin, maximum distance between the two inner surfaces at zero displacement
• heightout, maximum distance between the two outer surfaces at zero displacement

Triple-Pendulum Isolator Property

301

CSI Analysis Reference Manual
The isolator stiffness at each stage of sliding is dependent upon the effective
pendulum lengths. For each surface, the pendulum length is given by the radius minus the distance to the point of articulation, a fraction of the distance between the
surfaces. Thus:
L1 = radius 1 - 05
. heightin
L2 = radius 2 - a heightout
L3 = radius 3 - (1 - a ) heightout
where
a=

radius 2
radius 2 + radius 3

During sliding, the net friction coefficient for each surface is dependent upon the
velocity of sliding on that surface according to the rate-dependent friction equations (Eqns. 1, page 293) given for the friction-pendulum isolator.
The monotonic, radial force-deflection behavior of a typical triple-pendulum isolator is shown in Figure 76 (page 303). The isolator is assumed to be in compression,
~
~
and the plotted shear force, V , is normalized by the compression load: V = V P ,
P < 0.
The actual behavior will depend on the relative pendulum lengths, friction coefficients, and stop distances. For the purpose of the following discussion, we will assume that the net coefficients for the three surfaces are constant and ordered such
that m 1 £ m 2 £ m 3 , and that the stop distances are large enough as described. The
following behavior is observed:
• 0 £ u £ u a : The initial resistance is given by the elastic stiffness until first sliding begins. This occurs at a normalized shear force equal to the lowest friction
coefficient, m 1 , for the inner sliding surfaces.
• u a £ u £ u b : The shear stiffness is now governed by the pendulum lengths of
the two inner surfaces, both of which are sliding. This stiffness is 1 (2L1 ).
• u b £ u £ u c : When the shear force increases to the second friction coefficient,
m 2 , sliding shifts from the inner-bottom surface to the outer-bottom surface,
and the stiffness becomes 1 ( L1 + L2 ).
• u c £ u £ u d : Similarly, at the level of the third friction coefficient, m 3 , sliding
shifts from the inner-top surface to the outer-top surface, and the stiffness becomes 1 ( L2 + L3 ).

302

Triple-Pendulum Isolator Property

Chapter XV

The Link/Support Element—Advanced

Figure 76
Normalized Force-Deflection Curve for the Triple-Pendulum Isolator
Typical behavior for monotonic radial loading at slow speed
• u d £ u £ u e : With increased sliding, one of the stops is hit, say for the
outer-bottom surface. Sliding shifts back to the adjacent inner surface, and the
stiffness becomes 1 ( L1 + L3 ).
• u e £ u £ u f : When the outer-top stop is hit, sliding shifts back to the adjacent
inner surface and the stiffness becomes 1 (2L1 ) again.
• u > u f : After both inner stops are hit, the initial elastic stiffness is engaged.
The actual behavior will depend on the relative values of the parameters used for
the actual isolator, the velocities of sliding as they affect the friction coefficients,
and the history and direction of the motion.
The transition to sliding is not abrupt, but rather occurs gradually as the normalized
shear force approaches each friction coefficient. This friction model permits some
sliding at all non-zero levels of shear force; the amount of sliding becomes much
larger as the shear force approaches the “yield” value of P m. Sliding at lower values
of shear force can be minimized by using larger values of the elastic shear
stiffnesses, stiff. However, realistic values of the shear stiffness are recommended,
and can be estimated as AG/L of the locked-up device. This should also include the
flexibility of the connections or supports that is not otherwise included in the
Triple-Pendulum Isolator Property

303

CSI Analysis Reference Manual
model. In no case should the stiffness values be more than about 100 to 10000 times
larger than |P/L|, where P is a typical axial compression value for the isolator, and L
is the pendulum length. Larger values serve no practical purpose and make nonlinear convergence more difficult.

Nonlinear Deformation Loads
A nonlinear deformation load is a set of forces and/or moments on the structure
that activates a nonlinear internal deformation of an Link/Support element. A nonlinear internal deformation is an Link/Support internal deformation for which nonlinear properties have been specified.
Nonlinear deformation loads are used as starting load vectors for Ritz-vector analysis. Their purpose is to generate Modes that can adequately represent nonlinear behavior when performing nonlinear modal time-history analyses. A separate nonlinear deformation load should be used for each nonlinear internal deformation of
each Link/Support element.
When requesting a Ritz-vector analysis, you may specify that the program use
built-in nonlinear deformation loads, or you may define your own Load Patterns for
this purpose. In the latter case you may need up to six of these Load Patterns per
Link/Support element in the model.
The built-in nonlinear deformation loads for a single two-joint Link element are
shown in Figure 77 (page 305). Each set of forces and/or mo ments is
self-equilibrating. This tends to localize the effect of the load, usually resulting in a
better set of Ritz-vectors. For a single-joint element, only the forces and/or moments acting on joint j are needed.
It is strongly recommended that mass or mass moment of inertia be present at each
degree of freedom that is acted upon by a force or moment from a nonlinear deformation load. This is needed to generate the appropriate Ritz vectors.

304

Nonlinear Deformation Loads

Chapter XV

The Link/Support Element—Advanced

L = Element Length
dj2

dj3

j
1

L–dj2

1
i

Load for
Deformation
du1

Load for
Deformation
du2

L–dj3
Load for
Deformation
du3

j
1

2
3

3
1

1
Load for
Deformation
dr1

Load for
Deformation
dr2

Load for
Deformation
dr3

Figure 77
Built-in Nonlinear Deformation Loads for a Two-joint Link Element

Nonlinear Deformation Loads

305

CSI Analysis Reference Manual
For more information:
• See Topic “Internal Deformations” (page 260) in this Chapter.
• See Topic “Link/Support Properties” (page 263) in this Chapter.
• See Topic “Mass” (page 271) in this Chapter.
• See Topic “Ritz-Vector Analysis” (page 349) in Chapter “Load Cases.”
• See Topic “Nonlinear Modal Time-History Analysis (FNA)” (page 349) in
Chapter “Load Cases.”

Frequency-Dependent Link/Support Properties
Each Link or Support element can have an optional set of frequency-dependent
properties assigned to it in addition to the linear/nonlinear property set that must always be assigned. Frequency-dependent properties are only used for frequency-domain types of analyses, such as Steady-State or Power-Spectral-Density analyses.
Frequency-dependent properties represent the complex impedance of the element.
There is a real part that represents the stiffness and inertial effects, and an imaginary
part that represents the hysteretic damping effects. Frequency-dependent properties for the six degrees of freedom of the element may be may be coupled or uncoupled coupled, as given by:
ì f u1 ü é z u1
ïf ï ê
ï u2 ï ê
ï f u3 ï ê
í
ý=ê
f
r
1
ï
ï ê
ï f r2 ï ê
ïf ï ê
î r3 þ ë

z u1u 2
z u2

sym.

z u1u 3
z u2u3

z u1r1
z u 2 r1

z u1r 2
z u2r 2

z u3

z u 3 r1
z r1

z u3r 2
z r1r 2
z r2

z u1r 3 ù ì d u1 ü
z u2r 3 ú ï d u2 ï
úï
ï
z u3r 3 ú ï d u3 ï
í
ý
z r1r 3 ú ï d r1 ï
ú
z r 2r 3 ú ï d r 2 ï
z r 3 úû ïî d r 3 ïþ

(Eqn. 2)

where z u1 = k u1 + ic u1 is the impedance term in the u1 degree of freedom, and
where k u1 is the stiffness/inertial component, c u1 is the damping component, and i
is the square root of –1. The other impedance terms are similar.
In Eqn. (2), the force terms on the left-hand side of the equation and the displacement terms on the right-hand side of the equations are also complex. The real parts
of these terms represent the behavior at a phase angle of zero, with time variation
given by the cosine function, and the imaginary parts represent behavior at a phase
angle of 90°, with time variation given by the sine function.

306

Frequency-Dependent Link/Support Properties

Chapter XV

The Link/Support Element—Advanced

Each of the 21 impedance terms may vary with frequency. You define the variation
for each term as a set of points giving stiffness vs. frequency and damping vs. frequency. It is not unusual for the stiffness term to be negative over part of the range.
A common use for frequency-dependent properties would be in Support elements
that represent the far-field radiation-damping effect of the soil region under a rigid
foundation.

Frequency-Dependent Link/Support Properties

307

CSI Analysis Reference Manual

308

Frequency-Dependent Link/Support Properties

C h a p t e r XVI

The Tendon Object
Tendons are a special type of object that can be embedded inside other objects
(frames, shells, planes, asolids, and solids) to represent the effect of prestressing
and post-tensioning. These tendons attach to the other objects and impose load
upon them.
Advanced Topics
• Overview
• Geometry
• Discretization
• Tendons Modeled as Loads or Elements
• Connectivity
• Degrees of Freedom
• Local Coordinate Systems
• Section Properties
• Nonlinear Properties
• Mass
• Prestress Load

309

CSI Analysis Reference Manual
• Self-Weight Load
• Gravity Load
• Temperature Load
• Strain Load
• Deformation Load
• Target-Force Load
• Internal Force Output

Overview
Tendons are a special type of object that can be embedded inside other objects
(frames, shells, planes, asolids, and solids) to represent the effect of prestressing
and post-tensioning. These tendons attach to the other objects through which they
pass and impose load upon them.
You may specify whether the tendons are to be modeled as independent elements in
the analysis, or just to act upon the rest of the structure as loads. Modeling as loads
is adequate for linear analyses when you know the losses that will be caused by
elastic shortening and time-dependent effects.
Tendons should be modeled as elements if you want the program to calculate the
losses due to elastic shortening and time-dependent effects, if you want to consider
nonlinearity in the Tendons, or if you want to know the forces acting in the Tendons
due to other loading on the structure.
Tendon objects share some features with Frame elements, which will be cross-referenced in this Chapter.

Geometry
Any number of tendons may be defined. Each tendon is drawn or defined as a type
of line object between two joints, I and j. The two joints must not share the same location in space. The two ends of the Tendon are denoted end I and end J, respectively.
The Tendon may have an arbitrary curved or segmented shape in three dimensions
between those points, and may be offset at the ends from these joints.

310

Overview

Chapter XVI

The Tendon Object

Discretization
A Tendon may be a long object with complicated geometry, but it will be automatically discretized into shorter segments for purposes of analysis. You must specify
the maximum length of these discretization segments during the definition of the
Tendon. These lengths can affect how the Tendon loads the structure and the accuracy of the analysis results. You should choose shorter lengths for Tendons with
highly curved geometry, or Tendons that pass through parts of the structure with
complicated geometry or changes in properties. If you are not sure what value to
use, try several different values to see how they affect the results.

Tendons Modeled as Loads or Elements
You have a choice for each Tendon how it is to be modeled for analysis:
• As equivalent loads that act upon the structure
• As independent elements with stiffness, mass and loading
Modeling as loads is adequate for linear analyses when you know in advance the
losses that will be caused by elastic shortening and time-dependent effects.
Tendons should be modeled as elements if you want the program to calculate the
losses due to elastic shortening and time-dependent effects, if you want to consider
nonlinearity in the Tendons, or if you want to know the forces acting in the Tendons
due to other loading on the structure. The discretized Tendon is internally analyzed
as a series of equivalent short, straight Frame elements.

Connectivity
The Tendon is connected to Frame, Shell, Plane, Asolid, and Solid elements
through which it passes along its length. This connection is made automatically by
the program. See additional description below for parts of the tendon which do not
fall inside another element.
To determine the elements through which the Tendon passes, the program uses the
concept of a bounding box:
• For Frame elements, the bounding box is a rectangular prism bounded by the
length of the element and its maximum cross-sectional dimensions in the local
2 and 3 directions.

Discretization

311

CSI Analysis Reference Manual
• For Shell, Plane, and Asolid elements, it is the hexahedron bounded by the four
sides of the element and the upper and lower surfaces in the local 3 direction,
with thickness being considered.
• For Solid elements, it is the volume bounded by the six faces.
By default, the Tendon will be checked for connection against all elements in the
model. You may restrict this by specifying a group of objects to which the Tendon
may connect. The Tendon will not connect to any objects that are not in that group.
See Topic “Groups” (page 9) in Chapter “Objects and Elements” for more information. Only elements from objects in this group are considered in the discussion below, where they are called “bounding elements.”
For Tendons modeled as loads, if any portion of the Tendon passes through a
bounding element, load from that portion of the tendon within the bounding element is transferred to the joints of that element in a statically equivalent fashion.
The load on any portion of a Tendon that does not fall within a bounding element is
transferred to the nearest joint that is connected to a bounding element.
For Tendons modeled as elements, if any discretization point (i.e., either end of a
discretization segment) falls within a bounding element, that point is connected by
an interpolation constraint to all joints of that element. This means that for large
discretizations, the tendon may not actually be connected to every element through
which it passes. If the end of the entire Tendon object does not fall within a bounding element, it is connected by constraint to the nearest joint that is connected to a
bounding element. However, internal discretization points that do not fall within a
bounding element will not be connected to any element (except to adjacent tendon
elements themselves), so that the tendon will be external to the structure at those locations.

Degrees of Freedom
The Tendon object has six degrees of freedom along its length. However, its effect
upon the structure depends upon the elements to which it connects. When connecting to Frame and Shell elements, it may transmit forces and moments to the joints in
those elements. When connecting to Planes, Asolids, and Solids, it only transmits
forces to the joints.
Even when modeled as elements, a Tendon adds no additional degrees of freedom
to a structure, since it is always constrained to act with the elements that contain it.
The exception would be if there is a portion of the Tendon which is not embedded
in any other element and acts as a external length of tendon.

312

Degrees of Freedom

Chapter XVI

The Tendon Object

For more information, please see Topic “Degrees of Freedom” (page 30) in Chapter
“Joints and Degrees of Freedom.”

Local Coordinate Systems
Each Tendon object has two local coordinate systems:
• Base-line local coordinate system, which is fixed for the whole object
• Natural local coordinate system, which varies along the length of the Tendon
These are described in the following.

Base-line Local Coordinate System
The Tendon base-line local coordinate system is used only to define the Tendon
natural local coordinate system.
The axes of base-line system are denoted 1, 2 and 3. The first axis is directed along
the straight line connecting the joints I and j that were used to define the Tendon.
The remaining two axes lie in the plane perpendicular to this axis with an orientation that you specify. The base-line local coordinate system is fixed for the length
of the Tendon, regardless of the Tendon’s trajectory in space.
Base-line local axes are defined exactly the same as for a Frame element connected
to joints I and j, except the Tendon has zero joint offsets. Please see Topics “Local
Coordinate System” (page 108) and “Advanced Local Coordinate System” (page
110) in Chapter “The Frame Element”.

Natural Local Coordinate System
The Tendon natural local coordinate system is used to define section properties,
loads, and internal force output. This coordinate system is defined with respect to
the base-line local coordinate system as follows:
• The 1 direction is directed along the tangent to the Tendon, in the direction
from end I to end J.
• The 2 direction is parallel to the 1-2 plane of the base-line local coordinate system.
• The 3 direction is computed as the cross product of the natural local 1 and 2 directions.

Local Coordinate Systems

313

CSI Analysis Reference Manual
See Topic “Local Coordinate Systems” (page 312) in this Chapter for more information.

Section Properties
A Tendon Section is a set of material and geometric properties that describe the
cross-section of one or more Tendon objects. Sections are defined independently of
the Tendons, and are assigned to the Tendon objects.
The cross section shape is always circular. The Section has axial, shear, bending
and torsional properties, although we are primarily interested in only the axial behavior.

Material Properties
The material properties for the Section are specified by reference to a previously-defined Material. Uniaxial or isotropic material properties are used, even if
the Material selected was defined as orthotropic or anisotropic. The material properties used by the Section are:
• The modulus of elasticity, e1, for axial stiffness and bending stiffness
• The shear modulus, g12, for torsional stiffness and transverse shear stiffness
• The coefficient of thermal expansion, a1, for axial expansion and thermal
bending strain
• The mass density, m, for computing element mass
• The weight density, w, for computing Self-Weight Loads
The material properties e1, g12, and a1 are all obtained at the material temperature
of each individual Tendon object, and hence may not be unique for a given Section.
See Chapter “Material Properties” (page 69) for more information.

Geometric Properties and Section Stiffnesses
The cross section shape is always circular. You may specify either the diameter or
the area, a. The axial stiffness of the Section is given by a × e1.
The remaining section properties are automatically calculated for the circular
shape. These, along with their corresponding Section stiffnesses, are given by:

314

Section Properties

Chapter XVI

The Tendon Object

• The moment of inertia, i33, about the 3 axis for bending in the 1-2 plane, and
the moment of inertia, i22, about the 2 axis for bending in the 1-3 plane. The
corresponding bending stiffnesses of the Section are given by i33 × e1 and
i22 × e1;
• The torsional constant, j. The torsional stiffness of the Section is given by
j × g12. For a circular section, the torsional constant is the same as the polar moment of inertia.
• The shear areas, as2 and as3, for transverse shear in the 1-2 and 1-3 planes, respectively. The corresponding transverse shear stiffnesses of the Section are
given by as2 × g12 and as3 × g12.
Note that although six stiffness values are computed, only the axial stiffness is of
significance in a practical model. The other terms provide stability but have little
influence on the behavior of the model.

Tension/Compression Limits
You may specify a maximum tension and/or a maximum compression that a Tendon may take. In the most common case, you would define no-compression behavior by specifying the compression limit to be zero. Even this may not be needed for
bonded tendons, which can take some compression.
If you specify a tension limit, it must be zero or a positive value. If you specify a
compression limit, it must be zero or a negative value. If you specify a tension and
compression limit of zero, the Tendon will carry no axial force.
The tension/compression limit behavior is elastic. Any axial extension beyond the
tension limit or axial shortening beyond the compression limit will occur with zero
axial stiffness. These deformations are recovered elastically at zero stiffness.
Important! Tension/compression limits are nonlinear, and only affect Tendons
that are modeled as elements, not Tendons modeled as loads. Furthermore, they are
only effective in a nonlinear analysis.
Linear analyses starting from zero conditions (the unstressed state) behave as if
there were no tension/compression limits. Linear analyses that use the stiffness
from the end of a previous nonlinear analysis will have a constant stiffness: zero if a
tension or compression limit was exceeded at the end of the nonlinear case, otherwise the elastic material stiffness of the tendon.

Tension/Compression Limits

315

CSI Analysis Reference Manual

Mass
In a dynamic analysis, the mass of the structure is used to compute inertial forces.
When modeled as elements, the mass contributed by the Tendon is lumped at each
discretization point along the length of the Tendon. When modeled as loads, no
mass is contributed to the model. This is not usually of any significance since the
mass of a Tendon is generally small.
The total mass of the Tendon is equal to the integral along the length of the mass
density, m, multiplied by the cross-sectional area, a.
For more information, see Topic “Mass Source” (page 334) in Chapter “Load Patterns”.

Prestress Load
Each Tendon produces a set of self-equilibrating forces and moments that act on the
rest of the structure. You may assign different Prestress loading in different Load
Patterns.
In a given Load Pattern, the Prestress Load for any Tendon is defined by the following parameters:
• Tension in the Tendon, before losses.
• Jacking location, either end I or end J, where the tensioning of the Tendon will
occur
• Curvature coefficient. This specifies the fraction of tension loss (due to friction) per unit of angle change (in radians) along the length of the Tendon,
measured from the jacking end.
• Wobble coefficient. This specifies the fraction of tension loss (due to friction)
per unit of Tendon length, measured from the jacking end, due to imperfect
straightness of the tendon.
• Anchorage set slip. This specifies the length of slippage at the jacking end of
the Tendon due to the release of the jacking mechanism.
The following additional load parameters may be specified that only apply when
the Tendon is modeled as loads:
• Elastic shortening stress, due to compressive shortening in the elements that
are loaded by the Tendon. This may be due to loads from the Tendon itself or
from other loads acting on the structure.

316

Mass

Chapter XVI

The Tendon Object

• Creep stress, due to compressive creep strains in the elements that are loaded
by the Tendon.
• Shrinkage stress, due to compressive shrinkage strains in the elements that are
loaded by the Tendon.
• Steel relaxation stress, due to tensile relaxation strains in the Tendon itself.
For Tendons modeled as elements, the elastic shortening stress is automatically accounted for in all analyses; the time-dependent creep, shrinkage, and relaxation
stresses can be accounted for by performing a time-dependent staged-construction
analysis. See Topic “Staged Construction” (page 439) in Chapter “Nonlinear Static
Analysis” for more information.
The tension and all of the loss effects are converted to an equivalent set of distributed and concentrated forces acting along the length of the Tendon. These can be
displayed and tabulated in the graphical user interface. They are applied to the
model as follows:
• For Tendons modeled as loads, these forces are transferred to the joints of the
bounding elements as described earlier in this chapter under Topic “Connectivity”
• For Tendons modeled as elements, the tension at each end of a discretized tendon element is converted to an equivalent strain load, -P/(a × e1), where P is the
local tension after losses, and may vary along the length.
To account for complicated jacking procedures, you can specify different prestress
loads in different Load Patterns and apply them as appropriate.

Self-Weight Load
Self-Weight Load activates the self-weight of all elements in the model. For a
Tendon object, the self-weight is a force that is distributed along the length of the
element. The magnitude of the self-weight is equal to the weight density, w, multiplied by the cross-sectional area, a.
Self-Weight Load always acts downward, in the global –Z direction. You may
scale the self-weight by a single scale factor that applies equally to all elements in
the structure.
For more information:
• See Topic “Weight Density” (page 78) in Chapter “Material Properties” for the
definition of w.
Self-Weight Load

317

CSI Analysis Reference Manual
• See Topic “Section Properties” (page 314) in this Chapter for the definition of
a.
• See Topic “Self-Weight Load” (page 325) in Chapter “Load Patterns.”

Gravity Load
Gravity Load can be applied to each Tendon to activate the self-weight of the
object. Using Gravity Load, the self-weight can be scaled and applied in any direction. Different scale factors and directions can be applied to each element.
If all elements are to be loaded equally and in the downward direction, it is more
convenient to use Self-Weight Load.
For more information:
• See Topic “Self-Weight Load” (page 134) in this Chapter for the definition of
self-weight for the Frame element.
• See Topic “Gravity Load” (page 326) in Chapter “Load Patterns.”

Temperature Load
Temperature Load creates thermal strain in the Tendon object. This strain is given
by the product of the Material coefficient of thermal expansion and the temperature
change of the object. All specified Temperature Loads represent a change in temperature from the unstressed state for a linear analysis, or from the previous temperature in a nonlinear analysis.
For any Load Pattern, you may specify a Load Temperature field that is constant
over the cross section and produces axial strains. This temperature field may be
constant along the element length or interpolated from values given at the joints.
See Chapter “Load Patterns” (page 321) for more information.

Strain Load
Axial strain load represents a change in length per unit length. Positive strain increases the length of an unrestrained element, or causes compression in a restrained
element. Strain and temperature load act similarly, differing only by a scale factor,
namely the coefficient of thermal expansion.

318

Gravity Load

Chapter XVI

The Tendon Object

Strain loads may be constant along the element length or linearly interpolated from
values given at the joints by a Joint Pattern.
For more information, see Topic “Internal Force Output” (page 144) in this chapter,
and also Chapter “Load Patterns” (page 321.)

Deformation Load
While Strain Load specifies a change in deformation per unit length, Deformation
Load specifies the total deformation between the two ends of an unrestrained element. Deformation Load is internally converted to Strain Load, so you should
choose whichever type of loading is most conveniently specified for your particular
application. The specified axial deformation is converted to axial Strain Load by
simply dividing by the element length. The computed strain loads are assumed to
be constant along the length of the element.
See Chapter “Load Patterns” (page 321) for more information.

Deformation Load

319

CSI Analysis Reference Manual

Internal Force Output
The Tendon internal forces are the axial forces, P, that result from integrating the
axial stresses over the object cross section. These internal forces are present at every cross section along the length of the Tendon, and may be plotted or tabulated as
part of the analysis results. As is always true in SAP2000, tension is positive.
Important! Internal force output is only available for Tendons that are modeled as
elements.

320

Internal Force Output

C h a p t e r XVII

Load Patterns
A Load Pattern is a specified spatial distribution of forces, displacements, temperatures, and other effects that act upon the structure. A Load Pattern by itself does
not cause any response of the structure. Load Patterns must be applied in Load
Cases in order to produce results.
Basic Topics for All Users
• Overview
• Load Patterns, Load Cases, and Load Combinations
• Defining Load Patterns
• Coordinate Systems and Load Components
• Force Load
• Restraint Displacement Load
• Spring Displacement Load
• Self-Weight Load
• Concentrated Span Load
• Distributed Span Load
• Tendon Prestress Load

321

CSI Analysis Reference Manual
• Uniform Load
• Mass Source
• Acceleration Loads
Advanced Topics
• Gravity Load
• Surface Pressure Load
• Pore Pressure Load
• Temperature Load
• Strain and Deformation Load
• Rotate Load
• Joint Patterns

Overview
Each Load Pattern may consist of an arbitrary combination of the available load
types:
• Concentrated forces and moments acting at the joints
• Displacements at the grounded ends of joint restraints, joint springs, and
one-joint Link/Support elements
• Self-weight and/or gravity acting on all element types
• Concentrated or distributed forces and moments acting on the Frame elements
• Distributed forces acting on the Shell elements
• Surface pressure acting on the Shell, Plane, Asolid, and Solid elements
• Pore pressure acting on the Plane, Asolid, and Solid elements
• Thermal expansion acting on the Frame, Shell, Plane, Asolid, and Solid elements
• Prestress load due to Tendons acting in Frame, Shell, Plane, Asolid, and Solid
elements
• Centrifugal forces acting on Asolid elements
For practical purposes, it is usually most convenient to restrict each Load Pattern to
a single type of load, using Load Cases and Load Combinations to create more
complicated combinations.

322

Overview

Chapter XVII

Load Patterns

Load Patterns, Load Cases, and Load Combinations
A Load Pattern is a specified spatial distribution of forces, displacements, temperatures, and other effects that act upon the structure. A Load Pattern by itself does
not cause any response of the structure.
Load Patterns must be applied in Load Cases in order to produce results. A Load
Case defines how the Load Patterns are to be applied (e.g., statically or dynamically), how the structure responds (e.g., linearly or nonlinearly), and how the analysis is to be performed (e.g., modally or by direct-integration.) A Load Case may apply a single Load Pattern or a combination of Load Patterns.
The results of Load Cases can be combined after analysis by defining Load Combinations, also called Combos. A Load Combination is a sum or envelope of the
results from different Load Cases. For linear problems, algebraic-sum types of
Load Combinations make sense. For nonlinear problems, it is usually best to combine Load Patterns in the Load Cases, and use Load Combinations only for computing envelopes.
When printing, plotting, or displaying the response of the structure to loads, you
may request results for Load Cases and Load Combinations, but not directly for
Load Patterns.
When performing design, only the results from Load Combinations are used. Load
Combinations can be automatically created by the design algorithms, or you can
create your own. If necessary, you can define Load Combinations that contain only
a single Load Case.
• See Chapter “Load Cases” (page 341).
• See Topic “Load Combinations (Combos)” (page 351) in Chapter “Load
Cases”.

Defining Load Patterns
You can define as many Load Patterns as you want, each with a unique name that
you specify. Within each Load Pattern, any number of joints or elements may be
loaded by any number of different load types.
Each Load Pattern has a design type, such as DEAD, WIND, or QUAKE. This
identifies the type of load applied so that the design algorithms know how to treat
the load when it is applied in a Load Case.

Load Patterns, Load Cases, and Load Combinations

323

CSI Analysis Reference Manual

Coordinate Systems and Load Components
Certain types of loads, such as temperature and pressure, are scalars that are independent of any coordinate system. Forces and displacements, however, are vectors
whose components depend upon the coordinate system in which they are specified.
Vector loads may be specified with respect to any fixed coordinate system. The
fixed coordinate system to be used is specified as csys. If csys is zero (the default),
the global system is used. Otherwise csys refers to an Alternate Coordinate System.
The X, Y, and Z components of a force or translation in a fixed coordinate system
are specified as ux, uy, and uz, respectively. The X, Y, and Z components of a moment or rotation are specified as rx, ry, and rz, respectively.
Most vector loads may also be specified with respect to joint and element local coordinate systems. Unlike fixed coordinate systems, the local coordinate systems
may vary from joint to joint and element to element.
The 1, 2, and 3 components of a force or translation in a local coordinate system are
specified as u1, u2, and u3, respectively. The 1, 2, and 3 components of a moment
or rotation are specified as r1, r2, and r3, respectively.
You may use a different coordinate system, as convenient, for each application of a
given type of load to a particular joint or element. The program will convert all
these loads to a single coordinate system and add them together to get the total load.
See Chapter “Coordinate Systems” (page 11) for more information.

Effect upon Large-Displacements Analysis
In a large-displacements analysis, all loads specified in a joint or element local coordinate system will rotate with that joint or element. All loads specified in a fixed
coordinate system will not change direction during the analysis.
For linear analyses, and analyses considering only P-delta geometric nonlinearity,
the direction of loading does not change during the analysis.
See Chapter “Geometric Nonlinearity” (page 409) for more information.

324

Coordinate Systems and Load Components

Chapter XVII

Load Patterns

Force Load
Force Load applies concentrated forces and moments to the joints. You may specify components ux, uy, uz, rx, ry, and rz in any fixed coordinate system csys, and
components u1, u2, u3, r1, r2, and r3 in the joint local coordinate system. Force
values are additive after being converted to the joint local coordinate system.
See Topic “Force Load” (page 42) in Chapter “Joints and Degrees of Freedom” for
more information.

Ground Displacement Load
Ground Displacement Load applies specified ground displacements (translations
and rotations) along the supported degrees of freedom at the joints. Supports include joint restraints, joint springs, and one-joint Link/Support elements. You may
specify components ux, uy, uz, rx, ry, and rz in any fixed coordinate system csys,
and components u1, u2, u3, r1, r2, and r3 in the joint local coordinate system. Displacement values are additive after being converted to the joint local coordinate
system.
See Topic “Ground Displacement Load” (page 42) in Chapter “Joints and Degrees
of Freedom” for more information.

Self-Weight Load
Self-Weight Load activates the self-weight of all elements in the model. Selfweight always acts downward, in the global –Z direction. You may scale the selfweight by a single scale factor that applies to the whole structure. No Self-Weight
Load can be produced by an element with zero weight.
For more information:
• See Topic “Upward and Horizontal Directions” (page 13) in Chapter “Coordinate Systems.”
• See Topic “Self-Weight Load” (page 134) in Chapter “The Frame Element.”
• See Topic “Self-Weight Load” (page 172) in Chapter “The Cable Element.”
• See Topic “Self-Weight Load” (page 191) in Chapter “The Shell Element.”
• See Topic “Self-Weight Load” (page 221) in Chapter “The Plane Element.”
• See Topic “Self-Weight Load” (page 232) in Chapter “The Asolid Element.”
Force Load

325

CSI Analysis Reference Manual
• See Topic “Self-Weight Load” (page 248) in Chapter “The Solid Element.”
• See Topic “Self-Weight Load” (page 272) in Chapter “The Link/Support Element—Basic.”
• See Topic “Self-Weight Load” (page 317) in Chapter “The Tendon Object.”

Gravity Load
Gravity Load activates the self-weight of the Frame, Cable, Shell, Plane, Asolid,
Solid, and Link/Support elements. For each element to be loaded, you may specify
the gravitational multipliers ux, uy, and uz in any fixed coordinate system csys.
Multiplier values are additive after being converted to the global coordinate system.
Each element produces a Gravity Load, having three components in system csys,
equal to its self-weight multiplied by the factors ux, uy, and uz. This load is apportioned to each joint of the element. For example, if uz = –2, twice the self-weight is
applied to the structure acting in the negative Z direction of system csys. No Gravity Load can be produced by an element with zero weight.
The difference between Self-Weight Load and Gravity Load is:
• Self-Weight Load acts equally on all elements of the structure and always in
the global –Z direction
• Gravity Load may have a different magnitude and direction for each element in
the structure
Both loads are proportional to the self-weight of the individual elements.
For more information:
• See Topic “Gravity Load” (page 135) in Chapter “The Frame Element.”
• See Topic “Gravity Load” (page 173) in Chapter “The Cable Element.”
• See Topic “Gravity Load” (page 207) in Chapter “The Shell Element.”
• See Topic “Gravity Load” (page 221) in Chapter “The Plane Element.”
• See Topic “Gravity Load” (page 233) in Chapter “The Asolid Element.”
• See Topic “Gravity Load” (page 249) in Chapter “The Solid Element.”
• See Topic “Gravity Load” (page 272) in Chapter “The Link/Support Element—Basic.”
• See Topic “Gravity Load” (page 318) in Chapter “The Tendon Object.”

326

Gravity Load

Chapter XVII

Load Patterns

Concentrated Span Load
Concentrated Span Load applies concentrated forces and moments at arbitrary locations on Frame elements. You may specify components ux, uy, uz, rx, ry, and rz
in any fixed coordinate system csys, and components u1, u2, u3, r1, r2, and r3 in
the Frame element local coordinate system. Force values are additive after being
converted to the Frame element local coordinate system.
See Topic “Concentrated Span Load” (page 135) in Chapter “The Frame Element”
for more information.

Distributed Span Load
Distributed Span Load applies distributed forces and moments at arbitrary locations on Frame and Cable elements. You may specify components ux, uy, uz, rx,
ry, and rz in any fixed coordinate system csys, and components u1, u2, u3, r1, r2,
and r3 in the Frame element local coordinate system. Force values are additive after
being converted to the Frame element local coordinate system.
For more information, See Topic “Distributed Span Load” (page 137) in Chapter
“The Frame Element”, and Topic “Distributed Span Load” (page 173) in Chapter
“The Cable Element”

Tendon Prestress Load
Tendons are a special type of object that can be embedded inside other objects
(frames, shells, planes, asolids, and solids) to represent the effect of prestressing
and post-tensioning. These tendons attach to the other objects and impose load
upon them.
You may specify whether the tendons are to be modeled as independent elements in
the analysis, or just to act upon the rest of the structure as loads. This affects the
types of loads that are directly imposed upon the structure.
See Topic “Prestress Load” (page 316) in Chapter “The Tendon Object” for more
information.

Concentrated Span Load

327

CSI Analysis Reference Manual

Uniform Load
Uniform Load applies uniformly distributed forces to the mid-surface of Shell elements. You may specify components ux, uy, and uz in any fixed coordinate system
csys, and components u1, u2, and u3 in the element local coordinate system. Force
values are additive after being converted to the element local coordinate system.
See Topic “Uniform Load” (page 207) in Chapter “The Shell Element” for more information.

Surface Pressure Load
Surface Pressure Load applies an external pressure to any of the outer faces of the
Shell, Plane, Asolid, and Solid elements. The load on each face of an element is
specified independently.
You may specify pressures, p, that are uniform over an element face or interpolated
from pressure values given by Joint Patterns. Hydrostatic pressure fields may easily
be specified using Joint Patterns. Pressure values are additive.
For more information:
• See Topic “Surface Pressure Load” (page 208) in Chapter “The Shell Element.”
• See Topic “Surface Pressure Load” (page 222) in Chapter “The Plane Element.”
• See Topic “Surface Pressure Load” (page 233) in Chapter “The Asolid Element.”
• See Topic “Surface Pressure Load” (page 249) in Chapter “The Solid Element.”
• See Topic “Joint Patterns” (page 332) in this Chapter.

Pore Pressure Load
Pore Pressure Load models the drag and buoyancy effects of a fluid within a solid
medium, such as the effect of water upon the solid skeleton of a soil. Pore Pressure
Load may be used with Shell, Asolid, and Solid elements.

328

Uniform Load

Chapter XVII

Water Surface

Earth Dam

Load Patterns

Flow Lines
Equipotential
Lines (Constant
Pore Pressure)

Bedrock

Figure 78
Flow-net Analysis of an Earth Dam to Obtain Pore Pressures

Scalar fluid-pressure values are given at the element joints by Joint Patterns, and interpolated over the element. These pressure values may typically be obtained by
flow-net analysis, such as illustrated in Figure 78 (page 329). Hydrostatic pressure
fields may easily be specified using Joint Patterns. Pressure values are additive.
The total force acting on the element is the integral of the gradient of this pressure
field over the volume of the element. This force is apportioned to each of the joints
of the element. The forces are typically directed from regions of high pressure toward regions of low pressure.
Note that although pressures are specified, it is the pressure gradient over an element that causes the load. Thus a uniform pressure field over an element will cause
no load. Pressure differences between elements also cause no load. For this reason,
it is important that the pore-pressure field be continuous over the structure.
The displacements, stresses, and reactions due to Pore Pressure Load represent the
response of the solid medium, not that of the combined fluid and solid structure. In
the case of soil, the stresses obtained are the usual “effective stresses” of soil mechanics (Terzaghi and Peck, 1967). Note, however, that the total soil weight and
mass density should be used for the material properties.
For more information:
• See Topic “Pore Pressure Load” (page 222) in Chapter “The Plane Element.”

Pore Pressure Load

329

CSI Analysis Reference Manual
• See Topic “Pore Pressure Load” (page 234) in Chapter “The Asolid Element.”
• See Topic “Pore Pressure Load” (page 249) in Chapter “The Solid Element.”
• See Topic “Joint Patterns” (page 332) in this Chapter.

Temperature Load
Temperature Load creates thermal strains in the Frame, Cable, Shell, Plane, Asolid,
and Solid elements. These strains are given by the product of the Material coefficients of thermal expansion and the temperature change of the element. All specified Temperature Loads represent a change in temperature from the unstressed state
for a linear analysis, or from the previous temperature in a nonlinear analysis.
Load Temperature gradients may also be specified in the two transverse directions
of the Frame element, and in the thickness direction of the Shell element. These
gradients induce bending strains in the elements. Temperature gradients are specified as the linear change in temperature per unit length. Thus to specify a given difference in temperature across the depth of a Frame or Shell element, divide the temperature difference by the corresponding depth, and assign this value as the temperature gradient load.
The Load Temperatures and gradients may be different for each Load Pattern. You
may specify temperatures and/or gradients that are uniform over an element or that
are interpolated from values given by Joint Patterns.
For more information:
• See Topic “Temperature Load” (page 140) in Chapter “The Frame Element.”
• See Topic “Temperature Load” (page 174) in Chapter “The Cable Element.”
• See Topic “Temperature Load” (page 209) in Chapter “The Shell Element.”
• See Topic “Temperature Load” (page 223) in Chapter “The Plane Element.”
• See Topic “Temperature Load” (page 234) in Chapter “The Asolid Element.”
• See Topic “Temperature Load” (page 250) in Chapter “The Solid Element.”
• See Topic “Temperature Load” (page 318) in Chapter “The Tendon Object.”
• See Topic “Joint Patterns” (page 332) in this Chapter.

330

Temperature Load

Chapter XVII

Load Patterns

Strain Load
Strain Load induces distributed strains in the Frame, Cable, and Shell elements.
The imposed strains tend to cause deformation in unrestrained elements, or create
internal forces and stresses in restrained elements. The types of strains that are
available is different for each type of element.
You may specify strains that are uniform over an element or that are interpolated
from values given by Joint Patterns.
For more information:
• See Topic “Strain Load” (page 141) in Chapter “The Frame Element.”
• See Topic “Strain and Deformation Load” (page 174) in Chapter “The Cable
Element.”
• See Topic “Strain Load” (page 210) in Chapter “The Frame Element.”
• See Topic “Joint Patterns” (page 332) in this Chapter.

Deformation Load
Deformation Load is an alternative form of Strain Load where the applied deformation is specified over the whole element rather than on a per-unit-length basis. Deformation Load is only available for Frame and Cable elements. The assumed distribution of strain over the element is fixed as described in the topics referenced below. Joint Patterns are not used.
For more information:
• See Topic “Deformation Load” (page 141) in Chapter “The Frame Element.”
• See Topic “Strain and Deformation Load” (page 174) in Chapter “The Cable
Element.”

Strain Load

331

CSI Analysis Reference Manual
used for nonlinear static and staged-construction analysis. If applied in any other
type of Load Case, it has no effect.
Unlike all other types of loading, target-force loading is not incremental. Rather,
you are specifying the total force that you want to be present in the frame element at
the end of the Load Case or construction stage. The applied deformation that is calculated to achieve that force may be positive, negative, or zero, depending on the
force present in the element at the beginning of the analysis. When a scale factor is
applied to a Load Pattern that contains Target-Force loads, the total target force is
scaled. The increment of applied deformation that is required may change by a different scale factor.
For more information:
• See Topic “Target-Force Load” (page 142) in Chapter “The Frame Element.”
• See Topic “Target-Force Load” (page 174) in Chapter “The Cable Element.”
• See Topic “Target-Force Iteration” (page 444) in Chapter “Nonlinear Static
Analysis” for more information.

Rotate Load
Rotate Load applies centrifugal force to Asolid elements. You may specify an angular velocity, r, for each element. The centrifugal force is proportional to the
square of the angular velocity. The angular velocities are additive. The load on the
element is computed from the total angular velocity.
See Topic “Rotate Load” (page 234) in Chapter “The Asolid Element.”

Joint Patterns
A Joint Pattern is a named entity that consists of a set of scalar numeric values, one
value for each joint of the structure. A Joint Pattern can be used to describe how
pressures or temperatures vary over the structure. Joint Patterns may also be used to
specify joint offsets and thickness overwrite for Shell elements.
Patterns are most effective for describing complicated spatial distributions of numeric values. Their use is optional and is not required for simple problems.
Since Pattern values are scalar quantities, they are independent of any coordinate
system. The definition of a Joint Pattern by itself causes no effect on the structure.

Chapter XVII

Load Patterns

Zero Datum = Fluid Surface
z
Fluid weight density = g
Joint j
Z

Pressure gradient vz = – g
zj

Pressure value vj = – g (zj – z)

Global
X

Figure 79
Example of a Hydrostatic Pressure Pattern

The pattern must be used in a pressure, temperature, or other assignment that is applied to the model.
For complicated Patterns, values could be generated in a spreadsheet program or by
some other means, and brought into the model by importing tables or by using interactive table editing.
In the graphical user interface, Pattern values can be assigned to selected joints.
They are specified as a linear variation in a given gradient direction from zero at a
given datum point. An option is available to permit only positive or only negative
values to be defined. This is useful for defining hydrostatic pressure distributions.
Multiple linear variations may be assigned to the same or different joints in the
structure.
The following parameters are needed for a pattern assignment:
• The components of the gradient, A, B, and C, in the global coordinate system
• The value D of the pattern at the global origin
• The choice between:
– Setting negative values to zero
– Setting positive values to zero
– Allow all positive and negative values (this is the default)

Joint Patterns

333

CSI Analysis Reference Manual
The component A indicates, for example, how much the Pattern value changes per
unit of distance parallel to the global X axis.
The Pattern value, vj, defined for a joint j that has coordinates (xj, yj, zj) is given by:
vj = A xj + B yj + C zj + D

(Eqn. 1)

If you know the coordinates of the datum point, x, y, and z, in global coordinate system at which the pattern value should be zero (say the free surface of water), then:
vj = A (xj – x) + B (yj – y) + C (zj – z)

(Eqn. 2)

from which we can calculate that:
D=–(Ax+By+Cz)

(Eqn. 3)

In most cases, the gradient will be parallel to one of the coordinate axes, and only
one term in Eqn. 2 is needed.
For example, consider a hydrostatic pressure distribution caused by water impounded behind a dam as shown in Figure 79 (page 333). The Z direction is up in
the global coordinate system. The pressure gradient is simply given by the fluid
weight density acting in the downward direction. Therefore, A = 0, B = 0 , and C =
–62.4 lb/ft3 or –9810 N/m3.
The zero-pressure datum can be any point on the free surface of the water. Thus z
should be set to the elevation of the free surface in feet or meters, as appropriate,
and D = – C z. For hydrostatic pressure, you would specify that negative values be
ignored, so that any joints above the free surface will be assigned a zero value for
pressure.

Mass Source
The mass used as inertia in dynamic analyses or to calculate certain types of loads
can be controlled by specifying the Mass Source. Multiple Mass Sources can be defined so that different load cases can use a different mass distributions for loading
and inertia. Examples could include modeling a structure supporting different configurations of equipment, or explicitly considering the effect of different eccentricities of the story mass on the mode shapes. However, for most models only a single
Mass Source is needed, and this is the default.
There are three possible contributions to a Mass Source:

334

Mass Source

Chapter XVII

Load Patterns

• Element Self Mass — This includes the mass from the section properties used
by the elements. For the Link/Support elements, this mass is explicitly defined
in the section property. For all other elements the mass comes from the material
property referenced by the section property.
• Additional Mass — This includes mass assigned to the joints and any additional mass assigned to the frame or shell elements.
• Specified Load Patterns — Mass is computed from the gravity load as computed from a specified linear combination of load patterns.
For each defined Mass Source you may specify which of the above contributions
are to be considered. By default, there is only a single Mass Source, and this includes the Element Self Mass and the Additional Mass, with no contribution from
Specified Load Patterns.

Mass from Specified Load Patterns
When defining a Mass Source, you may include the mass from a linear combination
of Load Patterns. For each Load Pattern in this combination you specify a scale factor that multiplies the loads. The mass is calculated as follows:
• For each individual joint or element, joint loads are calculated based on the
specified linear combination of load patterns.
• For each joint of this element, the combined load acting in the gravity direction
(negative global Z) is divided by the gravitational constant, and then assigned
equally to the translational degrees of freedom at that joint.
• Downward loads (–Z) create positive mass, and upward loads (+Z) create negative mass.
Important notes:
• Loads are calculated for each element in its original configuration, independent
of any large-deflection analysis.
• The mass calculated from loads acts in all three translational directions even
though the load creating the mass acts vertically.
• Self-equilibrating loads, such as temperature, strain, and prestressing, should
not be used for Mass Source.
• Be careful not to double-count the self-mass by specifying both Element Self
mass and a load pattern that contains self-weight.

Mass Source

335

CSI Analysis Reference Manual

Negative Mass
All mass values used for analysis must be positive or zero. Negative mass is not realistic and is not allowed. However, you can use negative mass in the mass source if
your intention is to subtract it from other positive mass.
The contributions due to Element Self Mass and Additional Mass come from materials, link properties, joint mass, line mass, and area mass. Except for joint mass,
these contributions are always positive and are equal for the three translational degrees of freedom at each joint. Joint mass can be positive or negative and may be
different at each of the six joint degrees of freedom.
The contributions from Specified Load Patterns are equal for the three translational
degrees of freedom at each joint. Downward loads generate positive mass and upward loads generate negative mass.
The net result after combining all these contributions for any joint degree of freedom may be positive or negative and will be reported as such in the “Assembled
Joint Mass” table. During equation solution, any negative mass values that remain
after combining the mass for constraints are set to zero and a warning issued in the
analysis log file.

Multiple Mass Sources
For most models, a single Mass Source is sufficient and is defined as described
above. This will apply to all loads calculated from mass and to all dynamic load
cases.
However, you have the option (when available) to specify multiple Mass Sources
for use with different load cases. Each Mass Source is defined as described above
by specifying the three contributions to the mass. One Mass Source is selected as
the default and this will be used for all Load Cases unless specified otherwise.
A specified Mass Source can selected for the following types of load cases:
• Nonlinear static
• Nonlinear staged-construction
• Nonlinear direct-integration time-history
If you do not select a specified Mass Source for these types of load cases, the Mass
source used will be the default Mass Source if the load case starts from zero initial
conditions, or the Mass Source used in the previous load case if continuing from another one of these same three types of load cases.

336

Mass Source

Chapter XVII

Load Patterns

For all other load cases, a similar rule applies. The default Mass Source will be used
if the load case uses the stiffness from zero load conditions. Otherwise, the Mass
Source used will be the same as for the nonlinear static, staged-construction, or direct-in te gra tion time-his tory load case used to cal cu late the stiff ness.
Response-spectrum and modal time-history load cases use the Mass Source of their
corresponding modal load case. See Chapter “Load Cases” (page 341) for more information, especially Topic “Sequence of Analysis” (page 344).
For example, consider the case where a response-spectrum analysis is to be carried
out for a tower both with and without a significant equipment load. You could do
the following:
• Define two load patterns
– DEAD, which includes the self-weight of the tower structure
– LIVE, which includes only the weight of the equipment
• Define two mass sources
– MASSDEAD, which includes only the load pattern DEAD with a scale
factor of 1.0, and no Element Self Mass or Additional Mass
– MASSDEADLIVE, which includes both load patterns DEAD and LIVE,
each with a scale factor of 1.0, and no Element Self Mass or Additional
Mass
• Define two nonlinear static load cases
– DEAD, which specifies mass source MASSDEAD
– DEADLIVE, which specifies mass source MASSDEADLIVE
• Define two modal load cases
– MODALDEAD, which uses the stiffness of load case DEAD
– MODALDEADLIVE, which uses the stiffness of load case DEADLIVE
• Define two response-spectrum load cases
– SPECDEAD, which uses the modes of load case MODALDEAD
– DEADLIVE, which uses the modes of load case MODALDEADLIVE
Note that in the above example the nonlinear static load cases were used only to
specify the Mass Source. However, in most practical cases you would also want to
apply the corresponding load patterns as loads and consider P-delta effects, as these
would likely also have an effect on the modes.
Note that the response-spectrum cases, in addition to considering the inertial effect
of the different masses on the modes, also apply acceleration loads that are based on
Mass Source

337

CSI Analysis Reference Manual
mass. These loads will automatically be based on the mass from the same Mass
Source used to calculate the modes. See topic “Acceleration Load” (page 338).

Automated Lateral Loads
Automated lateral loads are available as specified in the separate “Automated
Lateral Loads Manual” provided with the software. Most of the seismic loads, and
some wind loads, are calculated based on mass, which in turn is calculated by analysis from the Mass Source.
When multiple Mass Sources are used, the mass could be different between load
cases. For this reason, any given load pattern that contains an automated lateral load
based on mass can only be applied in load cases that use the same mass source. If
the same load pattern is applied in multiple load cases using different mass sources,
a warning will be issued when the analysis is run and only those load cases using
one of the mass sources will be run. In this case, you can define duplicate load patterns as needed for use with load cases using different mass sources.
Some automated lateral loads use a modal period that can be specified by the user or
determined from analysis. By default, this period will be determined from the first
modal load case that is run, whether or not it uses the same Mass Source as other
load cases that apply the load pattern. For this reason, when using multiple Mass
Sources, it is strongly recommended that you review the modal period used for automated lateral loads and specify your own value to be used if the calculated value
does not apply.

Acceleration Loads
In addition to the Load Patterns that you define, the program automatically computes three Acceleration Loads that act on the structure due to unit translational accelerations in each of the global directions, and three unit rotational accelerations
about the global axes at the global origin. Acceleration Loads can be applied in a
Load Case just like Load Patterns.
Acceleration Loads are determined by d’Alembert’s principal, and are denoted m x ,
m y , m z , m rx , m ry , and m rz . These loads are used for applying ground accelerations in response-spectrum (translation only) and time-history analyses, and can be
used as starting load vectors for Ritz-vector analysis.
These loads are computed for each joint and element and summed over the whole
structure. The translational Acceleration Loads for the joints are simply equal to the

338

Acceleration Loads

Chapter XVII

Load Patterns

negative of the joint translational masses in the joint local coordinate system. These
loads are transformed to the global coordinate system.
The translational Acceleration Loads for all elements except for the Asolid are the
same in each direction and are equal to the negative of the element mass. No coordinate transformations are necessary. Rotational acceleration will generally differ
about each axis.
For the Asolid element, the Acceleration Load in the global direction corresponding to the axial direction is equal to the negative of the element mass. The Acceleration Loads in the radial and circumferential directions are zero, since translations in
the corresponding global directions are not axisymmetric. Similar considerations
apply to the rotational accelerations.
The Acceleration Loads can be transformed into any coordinate system. In a fixed
coordinate system (global or Alternate), the translational Acceleration Loads along
the positive X, Y, and Z axes are denoted UX, UY, and UZ, respectively; the rotational Acceleration Loads about the X, Y, and Z axes are similarly denoted RX,
RY, and RZ.
In a local coordinate system defined for a response-spectrum or time-history analysis, the Acceleration Loads along or about the positive local 1, 2, and 3 axes are denoted U1, U2, U3, R1, R2, and R3 respectively. Rotational accelerations will be applied about the origin of the coordinate system specified with the Acceleration
Load in the Load Case. Each Acceleration Load applied in a given Load Case can
use a separate coordinate system.
Although the rotational accelerations are applied in load cases about the origins of
the specified coordinate systems, the modal participation factors and the various
modal participation ratios for the accelerations RX, RY, and RZ are reported about
the center of mass for the structure:
• For the RX load, this location is the y centroid of the UZ load and the z centroid
of the UY load.
• For the RY load, this location is the z centroid of the UX load and the x centroid
of the UZ load.
• For the RZ load, this location is the z centroid of the UY load and the y centroid
of the UX load.
This makes the rotational participation factors and ratios are more meaningful because they do not include any contribution from the translational accelerations.

Acceleration Loads

339

CSI Analysis Reference Manual

340

Acceleration Loads

C h a p t e r XVIII

Load Cases
A Load Case defines how the loads are to be applied to the structure (e.g., statically
or dynamically), how the structure responds (e.g., linearly or nonlinearly), and how
the analysis is to be performed (e.g., modally or by direct-integration.)
Basic Topics for All Users
• Overview
• Load Cases
• Types of Analysis
• Sequence of Analysis
• Running Load Cases
• Linear and Nonlinear Load Cases
• Linear Static Analysis
• Functions
• Load Combinations (Combos)
• Global Energy Response
Advanced Topics
• Multi-Step Static Analysis

341

CSI Analysis Reference Manual
• Linear Buckling Analysis
• Equation Solvers
• Environment Variables to Control Analysis
• Accessing the Assembled Stiffness and Mass Matrices

Overview
A Load Case defines how loads are to be applied to the structure, and how the structural response is to be calculated. You may define as many named Load Cases of
any type that you wish. When you analyze the model, you may select which cases
are to be run. You may also selectively delete results for any Load Case.
Note: Load Patterns by themselves do not create any response (deflections,
stresses, etc.) You must define a Load Case to apply the load.
There are many different types of Load Cases. Most broadly, analyses are classified
as linear or nonlinear, depending upon how the structure responds to the loading.
The results of linear analyses may be superposed, i.e., added together after analysis.
The available types of linear analysis are:
• Static analysis
• Modal analysis for vibration modes, using eigenvectors or Ritz vectors
• Response-spectrum analysis for seismic response
• Time-history dynamic response analysis
• Buckling-mode analysis
• Moving-load analysis for bridge and other vehicle live loads
• Steady-state analysis
• Power-spectral-density analysis
The results of nonlinear analyses should not normally be superposed. Instead, all
loads acting together on the structure should be combined directly within the Load
Cases. Nonlinear Load Cases may be chained together to represent complex loading sequences. The available types of nonlinear analyses are:
• Nonlinear static analysis
• Nonlinear time-history analysis

342

Overview

Chapter XVIII

Load Cases

Named Load Combinations can also be defined to combine the results of Load
Cases. Results can be combined additively or by enveloping. Additive Load Combinations of nonlinear Load Cases is not usually justified.

Load Cases
Each different analysis performed is called a Load Case. For each Load Case you
define, you need to supply the following type of information:
• Case name: This name must be unique across all Load Cases of all types. The
case name is used to request analysis results (displacements, stresses, etc.), for
creating Load Combinations, and sometimes for use by other dependent Load
Cases.
• Analysis type: This indicate the type of analysis (static, response-spectrum,
buckling, etc.), as well as available options for that type (linear, nonlinear,
etc.).
• Prerequisite load cases: Some load cases may continue from a previous load
case, use the stiffness from a previous load case, and/or use the modes from a
previous load case.
• Loads applied: For most types of analysis, you specify the Load Patterns that
are to be applied to the structure.
Additional data may be required, depending upon the type of analysis being defined.

Types of Analysis
There are many different types of Load Cases. Most broadly, analyses are classified
as linear or nonlinear, depending upon how the structure responds to the loading.
See Topic “Linear and Nonlinear Load Cases” (page 346) in this Chapter.
The results of linear analyses may be superposed, i.e., added together after analysis.
The available types of linear analysis are:
• Static analysis
• Modal analysis
• Response-spectrum analysis
• Time-history analysis, by modal superposition or direct integration

Load Cases

343

CSI Analysis Reference Manual
• Buckling analysis
• Moving-load analysis
• Steady-state analysis
• Power-spectral-density analysis
The results of nonlinear analyses should not normally be superposed. Instead, all
loads acting together on the structure should be combined directly within the Load
Cases. Nonlinear Load Cases may be chained together to represent complex loading sequences. The available types of nonlinear analyses are:
• Nonlinear static analysis
• Nonlinear time-history analysis, by modal superposition or direct integration
After you have defined a Load Case, you may change its type at any time. When
you do, the program will try to carry over as many parameters as possible from the
old type to the new type. Parameters that cannot be carried over will be set to default values, which you can change.
For more information:
• See Topic “Linear Static Analysis” (page 348) in this Chapter
• See Topic “Buckling Analysis” (page 349) in this Chapter
• See Chapter “Modal Analysis” (page 365)
• See Chapter “Response-Spectrum Analysis” (page 383)
• See Chapter “Linear Time-History Analysis” (page 397)
• See Chapter “Nonlinear Static Analysis” (page 425)
• See Chapter “Nonlinear Time-History Analysis” (page 447)
• See Chapter “Frequency-Domain Analysis” (page 465)
• See Chapter “Moving-Load Analysis” (page 477)

Sequence of Analysis
A Load Case may be dependent upon other Load Cases in the following situations:
• A modal-superposition type of Load Case (response-spectrum or modal
time-history) uses the modes calculated in a modal Load Case
• A nonlinear Load Case may continue from the state at the end of another nonlinear case

344

Sequence of Analysis

Chapter XVIII

Load Cases

• A linear Load Cases may use the stiffness of the structure as computed at the
end of a nonlinear case
A Load Case which depends upon another case is called dependent. The case upon
which it depends is called a prerequisite case.
When the program performs analysis, it will always run the cases in the proper order so that dependent cases are run after any of their prerequisite cases.
You can build up one or more sequences of Load Cases that can be as simple or as
complicated as you need. However, each sequence must ultimately start with a
Load Case that itself starts from zero and does not have any prerequisite cases.
Example
A common example would be to define a nonlinear static Load Case with the following main features:
• The name is, say, “PDELTA”
• The type is nonlinear static
• The loads applied are Load Pattern “DEAD” scaled by 1.0 plus Load Pattern
“LIVE” scaled by 0.25. These represent a typical amount of gravity load on the
structure
• The only nonlinearity considered is the P-delta effect of the loading
We are not necessarily interested in the response of Load Case PDELTA, but rather
we will use the stiffness at the end this case for a series of linear Load Cases that we
are interested in. These may include linear static cases for all loads of interest (dead,
live, wind, snow, etc.), a modal Load Case, and a response-spectrum Load Case.
Because these cases have all been computed using the same stiffness, their results
are superposable, making it very simple to create any number of Load Combinations for design purposes.

Running Load Cases
After you have defined a structural model and one or more Load Cases, you must
explicitly run the Load Cases to get results for display, output, and design purposes.
When an analysis is run, the program converts the object-based model to finite elements, and performs all calculations necessary to determine the response of the
Running Load Cases

345

CSI Analysis Reference Manual
structure to the loads applied in the Load Cases. The analysis results are saved for
each case for subsequent use.
By default, all Load Cases defined in the model are run each time you perform an
analysis. However, you can change this behavior. For each Load Case, you can set
a flag that indicates whether or not it will be run the next time you perform an analysis. This enables you to define as many different cases as you need without having
to run all of them every time. This is particularly useful if you have nonlinear cases
that may take a long time to run.
If you select a case to be run, the program will also run all prerequisite cases that
have not yet been run, whether you select them or not.
You can create new Load Cases without deleting the results of other cases that have
already been run. You can also modify existing Load Cases. However, the results
for the modified case and all cases that depend upon it will be deleted.
When an analysis is performed, the cases will be run in an order that is automatically determined by the program in order to make sure all prerequisite cases are run
before their dependent cases. If any prerequisite cases fail to complete, their dependent cases will not be run. However, the program will continue to run other
cases that are not dependent upon the failed cases.
You should always check the analysis log (.LOG) file to see statistics, warnings,
and error messages that were reported during the analysis. You can also see a summary of the cases that have been run, and whether or not they completed successfully, using the Analysis commands in the graphical user interface.
Whenever possible, the program will re-use the previously solved stiffness matrix
while running Load Cases. Because of this, the order in which the cases are run may
not be the same each time you perform an analysis.
See Topic “Sequence of Analysis” (page 467) in this Chapter for more information.

Linear and Nonlinear Load Cases
Every Load Case is considered to be either linear or nonlinear. The difference between these two options is very significant in SAP2000, as described below.
All Load Case types may be linear. Only static analysis and time-history analysis
may be nonlinear.

346

Linear and Nonlinear Load Cases

Chapter XVIII

Load Cases

Structural properties
Linear: Structural properties (stiffness, damping, etc.) are constant during the
analysis.
Nonlinear: Structural properties may vary with time, deformation, and loading. How much nonlinearity actually occurs depends upon the properties you
have defined, the magnitude of the loading, and the parameters you have specified for the analysis.
Initial conditions
Linear: The analysis starts with zero stress. It does not contain loads from any
previous analysis, even if it uses the stiffness from a previous nonlinear analysis.
Nonlinear: The analysis may continue from a previous nonlinear analysis, in
which case it contains all loads, deformations, stresses, etc., from that previous
case.
Structural response and superposition
Linear: All displacements, stresses, reactions, etc., are directly proportional to
the magnitude of the applied loads. The results of different linear analyses may
be superposed.
Nonlinear: Because the structural properties may vary, and because of the possibility of non-zero initial conditions, the response may not be proportional to
the loading. Therefore, the results of different nonlinear analyses should not
usually be superposed.

Linear Static Analysis
The linear static analysis of a structure involves the solution of the system of linear
equations represented by:
K u =r
where K is the stiffness matrix, r is the vector of applied loads, and u is the vector of
resulting displacements. See Bathe and Wilson (1976).
You may create any number of linear static Load Cases. For each case you may
specify a combination of one or more Load Patterns and/or Acceleration Loads that
Linear Static Analysis

347

CSI Analysis Reference Manual
make up the load vector r. Normally, you would specify a single Load Pattern with
a scale factor of one.
Every time you define a new Load Pattern, the program automatically creates a corresponding linear static Load Case of the same name. This Load Case applies the
Load Case with a unit scale factor. If you delete or modify the Load Case, the analysis results will not be available, even though the Load Case may still exist.
For a new model, the program creates a default Load Pattern call DEAD which applies the self weight of the structure. The corresponding linear static Load Case is
also called DEAD.
For each linear static Load Case, you may specify that the program use the stiffness
matrix of the full structure in its unstressed state (the default), or the stiffness of the
structure at the end of a nonlinear Load Case. The most common reasons for using
the stiffness at the end of a nonlinear case are:
• To include P-delta effects from an initial P-delta analysis
• To include tension-stiffening effects in a cable structure
• To consider a partial model that results from staged construction
See Chapter “Nonlinear Static Analysis” (page 425) for more information.

Multi-Step Static Analysis
Certain types of Load Patterns are multi-stepped, meaning that they actually represent many separate spatial loading patterns applied in sequence. These include the
Vehicle-Live and Wave types of Load Patterns.
You can apply multi-stepped Load Patterns in a Multi-Step Static Load Case. This
type of Load Case will perform a series of independent linear analyses, one for each
step of the Load Pattern:
K u i = ri
where ri is the load at step I, and u i is the resulting solution.
You can apply any linear combination of Load Patterns in the same Load Case,
each with an independent scale factor. These will be summed together as follows:
all multi-stepped Load Patterns will be synchronized, applying the load for the
same step number at the same time, and all single-stepped Load Patterns (e.g., dead
load) will be applied in every step.

348

Multi-Step Static Analysis

Chapter XVIII

Load Cases

The number of solution steps for the Load Case will be equal to the largest number
of load steps of any of the applied multi-stepped Load Patterns.
Although the multi-stepped Load Patterns represent a time series of loads,
Multi-Step Static Analysis does not include any dynamical effects. You can consider dynamics by converting the Multi-Step Static Load Case to a Time-History
Load Case, which can be linear or nonlinear.

Linear Buckling Analysis
Linear buckling analysis seeks the instability modes of a structure due to the P-delta
effect under a specified set of loads. Buckling analysis involves the solution of the
generalized eigenvalue problem:
[ K - l G(r) ] Y = 0
where K is the stiffness matrix, G(r) is the geometric (P-delta) stiffness due to the
load vector r, l is the diagonal matrix of eigenvalues, and Y is the matrix of corresponding eigenvectors (mode shapes).
Each eigenvalue-eigenvector pair is called a buckling mode of the structure. The
modes are identified by numbers from 1 to n in the order in which the modes are
found by the program.
The eigenvalue l is called the buckling factor. It is the scale factor that must multiply the loads in r to cause buckling in the given mode. It can also be viewed as a
safety factor: if the buckling factor is greater than one, the given loads must be increased to cause buckling; if it is less than one, the loads must be decreased to prevent buckling. The buckling factor can also be negative. This indicates that buckling will occur if the loads are reversed.
You may create any number of linear buckling Load Cases. For each case you specify a combination of one or more Load Patterns and/or Acceleration Loads that
make up the load vector r. You may also specify the number of modes to be found
and a convergence tolerance. It is strongly recommended that you seek more than
one buckling mode, since often the first few buckling modes may have very similar
buckling factors. A minimum of six modes is recommended.
It is important to understand that buckling modes depend upon the load. There is
not one set of buckling modes for the structure in the same way that there is for natural vibration modes. You must explicitly evaluate buckling for each set of loads of
concern.

Linear Buckling Analysis

349

CSI Analysis Reference Manual
For each linear buckling Load Case, you may specify that the program use the stiffness matrix of the full structure in its unstressed state (the default), or the stiffness
of the structure at the end of a nonlinear Load Case. The most common reasons for
using the stiffness at the end of a nonlinear case are:
• To include P-delta effects from an initial P-delta analysis
• To include tension-stiffening effects in a cable structure
• To consider a partial model that results from staged construction
See Chapter “Nonlinear Static Analysis” (page 425) for more information.

Functions
A Function is a series of digitized abscissa-ordinate pairs that may represent:
• Pseudo-spectral acceleration vs. period for response-spectrum analysis, or
• Load vs. time for time-history analysis
• Load vs. frequency for steady-state analysis
• Power density (load squared per frequency) vs. frequency for power-spectral-density analysis
You may define any number of Functions, assigning each one a unique label. You
may scale the abscissa and/or ordinate values whenever the Function is used.
The abscissa of a Function is always time, period, or frequency. The abscissaordinate pairs must be specified in order of increasing abscissa value.
If the increment between abscissa values is constant and the Function starts at abscissa zero, you need only specify the abscissa increment, dt, and the successive
function values (ordinates) starting at abscissa zero. The function values are specified as:
f0, f1, f2, ..., fn
corresponding to abscissas:
0, dt, 2 dt, ..., n dt
where n + 1 is the number of values given.
If the abscissa increment is not constant or the Function does not start at abscissa
zero, you must specify the pairs of abscissa and function value as:

350

Functions

Chapter XVIII

Load Cases

t0, f0, t1, f1, t2, f2, ..., tn, fn
where n + 1 is the number of pairs of values given.

Load Combinations (Combos)
A Load Combination (Combo) is a named combination of the results from Load
Cases or other Load Combinations. Combo results include all displacements and
forces at the joints and internal forces or stresses in the elements.
You may define any number of Combos. To each one of these you assign a unique
name, that also should not be the same as any Load Case. Combos can combine the
results of Load Cases and also those of other Combos, provided a circular dependency is not created.
By default, each Combo produces a pair of values for each response quantity: a
maximum and a minimum. These two values may be equal for certain type of Combos, as discussed below.
Alternatively, correspondence may be requested for tabular output, in which case
multiple pairs of maximum and minimum values may be produced at each output
location for each Combo. This is discussed in more detail in the subtopic “Correspondence” below. The discussion that immediately follows next considers the default case where a single maximum and minimum value is produced for each response quantity.

Contributing Cases
Each contributing Load Case or Combo supplies one or two values to the Combo
for each response quantity:
• Linear static cases, individual modes from Modal or Buckling cases, individual
steps from multi-stepped Load Cases, and additive Combos of these types of
results provide a single value. For the purposes of defining the Combos below,
this single value can be considered to be two equal values
• Response-spectrum cases provide two values: the maximum value used is the
positive computed value, and the minimum value is just the negative of the
maximum.
• Envelopes of results from multi-stepped Load Cases provide two values: a
maximum and minimum.

Load Combinations (Combos)

351

CSI Analysis Reference Manual
• For Moving-Load Load Cases, the values used are the maximum and minimum
values obtained for any vehicle loading of the lanes permitted by the parameters of the analysis.
For some types of Combos, both values are used. For other types of Combos, only
the value with the larger absolute value is used.
Each contributing case is multiplied by a scale factor, sf, before being included in a
Combo.

Types of Combos
Five types of Combos are available. For each individual response quantity (force,
stress, or displacement component) the two Combo values are calculated as follows:
• Additive type: The Combo maximum is an algebraic linear combination of the
maximum values for each of the contributing cases. Similarly, Combo minimum is an algebraic linear combination of the minimum values for each of the
contributing cases.
• Absolute type: The Combo maximum is the sum of the larger absolute values
for each of the contributing cases. The Combo minimum is the negative of the
Combo maximum.
• SRSS type: The Combo maximum is the square root of the sum of the squares
of the larger absolute values for each of the contributing cases. The Combo
minimum is the negative of the Combo maximum.
• Range type: The Combo maximum is the sum of the positive maximum values
for each of the contributing cases (a case with a negative maximum does not
contribute.) Similarly, the Combo minimum is the sum of the negative minimum values for each of the contributing cases (a case with a positive minimum
does not contribute.)
• Envelope type: The Combo maximum is the maximum of all of the maximum
values for each of the contributing cases. Similarly, Combo minimum is the
minimum of all of the minimum values for each of the contributing cases.
Only additive Combos of single-valued Load Cases produce a single-valued result,
i.e., the maximum and minimum values are equal. All other Combos will generally
have different maximum and minimum values.

352

Load Combinations (Combos)

Chapter XVIII

Load Cases

Examples
For example, suppose that the values, after scaling, for the displacement at a particular joint are 3.5 for Linear Static Load Case LL and are 2.0 for Response-spectrum
case QUAKE. Suppose that these two cases have been included in an additive-type
Combo called COMB1 and an envelope-type Combo called COMB2. The results
for the displacement at the joint are computed as follows:
• COMB1: The maximum is 3.5 + 2.0 = 5.5, and the minimum is 3.5 – 2.0 = 1.5
• COMB2: The maximum is max (3.5, 2.0) = 3.5, and the minimum is min (3.5, –
2.0) = –2.0
As another example, suppose that Linear Static Cases GRAV, WINDX and
WINDY are gravity load and two perpendicular, transverse wind loads, respectively; and that a response-spectrum case named EQ has been performed. The following four Combos could be defined:
• WIND: An SRSS-type Combo of the two wind loads, WINDX and WINDY.
The maximum and minimum results produced for each response quantity are
equal and opposite
• GRAVEQ: An additive-type Combo of the gravity load, GRAV, and the
response-spectrum results, EQ. The Combo automatically accounts for the
positive and negative senses of the earthquake load
• GRAVWIN: An additive-type Combo of the gravity load, GRAV, and the
wind load given by Combo WIND, which already accounts for the positive and
negative senses of the load
• SEVERE: An envelope-type Combo that produces the worst case of the two
additive Combos, GRAVEQ and GRAVWIN
Suppose that the values of axial force in a frame element, after scaling, are 10, 5, 3,
and 7 for cases GRAV, WINDX, WINDY, and EQ, respectively. The following results for axial force are obtained for the Combos above:
• WIND: maximum = 5 2 + 3 2 = 58
. , minimum = -58
.
• GRAVEQ: maximum = 10 + 7 = 17 , minimum = 10 - 7 = 3
• GRAVWIN: maximum = 10 + 58
. = 158
. , minimum = 10 - 58
. = 42
.
• SEVERE: maximum = max(17 ,158
. ) = 17 , minimum = min(3,42
. ) =3
Range-type Combos enable you to perform skip-pattern loading very efficiently.
For example, suppose you have a four-span continuous beam, and you want to

Load Combinations (Combos)

353

CSI Analysis Reference Manual
know what pattern of uniform loading on the various spans creates the maximum
response:
• Create four Load Patterns, each with uniform loading on a single span
• Create four corresponding Linear Static Load Cases, each applying a single
Load Pattern.
• Create a single range Combo, combining the results of the four Load Cases
The effect of this Combo is the same as enveloping all additive combinations of any
single span loaded, any two spans loaded, any three spans loaded, and all four spans
loaded. This range Combo could be added or enveloped with other Load Cases and
Combos.
As you can see, using Combos of Combos gives you considerable power and flexibility in how you can combine the results of the various Load Cases.

Correspondence
When correspondence is requested for tabular output, the maximum and minimum
value is produced for each response quantity as described above, but these are presented with the values of other related response quantities at the same location that
occur at the same time the given maximum or minimum is achieved.
For example, when considering Frame-element forces, the maximum value of axial
force P at a given output station is presented with the corresponding values of V2,
V3, T, M2, and M3 at the same output station. Six corresponding values are also
presented for the minimum value of P, and so on for the maximum and minimum
values of V2, V3, T, M2, and M3.
Without correspondence, the following tabular results would be presented for a
given output station in a given Combo:
Type

Max

100

-6

1245

Min

-50

-5

-9

-123

-333

With correspondence, the tabular results for the same output station location would
be presented as:

354

Load Combinations (Combos)

Chapter XVIII

Load Cases

Type

PMax

100

-4

-6

-123

-111

PMin

-50

-6

999

V2Max

-7

-65

328

V2Min

-30

-5

-6

-44

172

V3Max

-7

-65

328

V3Min

-30

-5

-6

-44

172

TMax

-6

-69

1033

TMin

-4

-9

-77

-197

M2Max

-20

-8

1158

M2Min

-4

-7

-123

890

M3Max

-6

1245

M3Min

-38

-5

-9

-123

-333

In this example, row PMax presents the maximum value of axial force P and the
corresponding values of the other frame forces and moments that occur at the same
time as maximum P. For a Combo that is the envelope of several linear static load
cases, this would be the frame forces and moments from the contributing load case
that had the maximum value of P. For an additive Combo of a dead load case plus a
time-history load case, this would be the summed frame forces and moments from
that time step in the time-history case that, when combined with dead load, produces that maximum value of P. Similarly, row PMin is the minimum value of P
and its corresponding forces and moments, and so on for V2Max through M3Min.
The shaded values in the table above indicate the maximum and minimum values
that would be presented in the table without correspondence. All other values in a
given column will be within the range of these two values.
It is possible, in some cases, that the maximum or minimum value of a response
quantity could occur at more than one instance in a Combo, in which case the corre-

Load Combinations (Combos)

355

CSI Analysis Reference Manual
sponding values will be presented for the first instance encountered. In this case,
the corresponding results may not be unique.
Correspondence is available for tabular output of the following quantities in software products that offer this option:
• Joint displacements
• Joint reactions
• Frame forces, Shell forces
• Shell stresses, Plane stresses, Asolid stresses, Solid stresses
• Link/Support forces and deformations
• Element joint forces
• Section Cuts
• Base reactions
• Bridge object section forces, Bridge object girder forces (CSiBridge only)
For each of the above, the correspondence is presented between the various components of the same type (e.g., 6 displacements, 6 forces, or 6 stresses) at a given location (joint or output station). Correspondence is not presented between components
at different locations or between components of different types (e.g., displacement
and force). The only exception to this is the Link/Support element, where correspondence is presented between the 6 deformation and 12 force components of a
given element. If you want to see the full corresponding state of the structure, you
must use step-by-step analysis.
Correspondence is available for Combos of types Additive, Envelope, and Range,
provided that the contributing load cases and Combos also support correspondence.
Correspondence is not available for Combos of types Absolute and SRSS, nor for
Combos that contain any of the following types of contributing load cases and/or
Combos:
• Response-spectrum load case
• Steady-state load case
• PSD load case
• Moving-load case without correspondence
• Absolute Combo
• SRSS Combo

356

Load Combinations (Combos)

Chapter XVIII

Load Cases

• A Combo that contains any of the above
• In addition, correspondence is not available for base reactions or element joint
forces for any Combo that contains a moving-load case.
Requesting correspondence for tabular output does not affect any other type of display, design, or the Open API functions. Correspondence for design purposes is
controlled by the Design Preferences. See the various design manuals that are included with the software for more information

Additional Considerations
Moving-Load Load Cases should not normally be added together, in order to avoid
multiple loading of the lanes. Additive combinations of Moving Loads should only
be defined within the Moving-Load Load Case itself. Therefore, it is recommended
that only a single Moving Load be included in any additive-, absolute-, SRSS-, or
range-type Combo, whether referenced directly as a Moving Load or indirectly
through another Combo. Multiple Moving Loads may be included in any
envelope-type Combo, since they are not added.
Nonlinear Load Cases should not normally be added together, since nonlinear results are not usually superposable. Instead, you should combine the applied loads
within a nonlinear Load Case so that their combined effect can be properly analyzed. This may require defining many different Load Cases instead of many different Combos. Nonlinear Load Cases may be included in an envelope-type
Combo, since they are not added.

Global Energy Response
Energy response is provided for the entire structure for certain types of load cases,
including linear and nonlinear modal time-history, nonlinear static and staged construction, and nonlinear direct-integration time history (but see Limitations below).
Energy response can be plotted and produced in output tables.
Three basic types of energy are considered: the work done by external agents that
put energy into the structure, conservative energy in the structure that can be recovered, and unconservative energy that is dissipated by the structure. Looking at the
energy response can tell you a lot about the behavior of the structure, but it is most
useful for determining the effectiveness of energy-dissipating mechanisms that are
intentionally provided as part of the design. This can include dampers, isolators,
and plastic hinging in structural members.

Global Energy Response

357

CSI Analysis Reference Manual
Global Energy Response Components
The following types of energy are reported for each considred load case:
• Input. This is the work done by external agents that put energy into the structure. This includes:
– Forces, moments, pressures, self-weight, and similar loads
– Ground acceleration
– Ground displacement
– Element strains and displacements, including thermal and time-dependent
strains (but see Limitations below).
– P-delta effects, such as the work done by vertical forces through lateral displacements when P-delta nonlinearity is considered
• Potential. This is a conservative type of energy in the structure due to elastic
strain that can be recovered when the loading is removed. It is often desirable to
limit potential energy to the reasonable extent possible, since it represents
forces and stresses to be designed against.
• Kinetic. This is a conservative type of energy due to the motion of the structure. It is often desirable to limit kinetic energy since this can represent the potential for damage to structural and non-structural items. Kinetic energy is always zero in a static analysis.
• Nonlinear Viscous Damping. This represents the viscous energy dissipated
by the velocity-based damper elements. Nonlinear viscous damping does not
change during nonlinear static and staged construction load cases. The following types of link elements can generate this energy component during time-history load cases:
– Linear damping properties
– Damper – Exponential
– Damper – Bilinear
– The three Friction-Pendulum Isolators (axial degree of freedom only)
• Nonlinear Hysteretic Damping. This represents the hysteretic energy dissipated by the displacement-based damper elements and the plastic deformation
of materials (including hinges). Nonlinear hysteretic damping can be generated
by the following elements during nonlinear static, staged-construction, and
time-history load cases:
– Link elements having the following types of properties:
* Damper – Friction Spring

358

Global Energy Response

Chapter XVIII

Load Cases

* Multilinear Plastic
* Plastic (Wen)
* Rubber Isolator
* The three Friction-Pendulum Isolators (shear degrees of freedom)
– Frame nonlinear hinges of all types
– Layered shell elements with nonlinear material properties
• Global Damping. This represents the energy dissipated by the structure as a
whole. For modal time-history load cases, this includes the modal damping
specified for the load case as well as modal damping specified for the materials,
if any. For nonlinear direct-integration time-history load cases, this includes
stiffness- and mass-proportional damping specified for the load case as well as
such damping specified for the materials, if any. Global damping is viscous
(velocity-based) and does not change during nonlinear static and staged-construction load cases.
• Error. It is expected that the sum of the potential, kinetic, and three damping
energies be equal to the input energy. The energy error is calculated as the difference between the input energy and this sum. There are several reasons why
this error may not be zero, such as:
– Discretization error due to larger steps sizes for P-delta or large-displacement geometric nonlinearity. This can be checked by re-running the load
case with a smaller step size.
– Round-off error in numerically sensitive or ill-conditioned systems.
– Energy that is excluded due to the Limitations listed below, such as for certain types of strain loading.
Remarks
Following are some general remarks considering the nature and use of these global
energy response components:
• The input energy can increase or decrease as the sum of the conservative energy increases or decreases. However, the three damping energies represent
work done that is not recoverable, and these can only increase the input energy.
• For purposes of design, it is generally preferable that the primary energy dissipation be in the form of nonlinear viscous and hysteretic damping, meaning
that it comes from devices (dampers, isolators, etc.) and hinging mechanisms.
Global damping represents other effects that are not explicitly modeled, such
as from non-structural elements and the intrinsic nature of the materials. If this
Global Energy Response

359

CSI Analysis Reference Manual
is too large, then it is difficult to know whether or not the design intent is being
met.
• When an object is removed during staged construction, its potential energy is
removed and is also deducted from the input energy. Any damping energy produced by that object is not removed, as that is already assumed to have been
dissipated as waste heat.
• If a nonlinear static or staged-construction load case continues from a direct-integration time-history load case, the velocity-based viscous damping energies
are held constant during the static analysis. However, kinetic energy is set to
zero during the static analysis and the input energy is correspondingly reduced.
If a nonlinear direct-integration time-history load case then continues from the
nonlinear static or staged-construction load case, the velocity continues from
the end of the most recent time-history load case in the sequence and the kinetic
energy is recomputed from those velocities. In effect, the nonlinear static or
staged-construction load cases are assumed to have occurred instantaneously
from the dynamics point of view. If this is not desired, the previous time-history load cases should be run long enough to damp out the velocities.
• The presence of energy error does not invalidate the analysis results, but can be
an indication that further investigation is warranted. See Limitations below for
some of the possible reasons. Note that the energy response is calculated from
the basic analysis results (displacements, forces, stresses) and does not affect
these results.
Limitations
Following are some limitations of the current implmentation of the global energy
response:
• For SAP2000 and CSiBridge, energy response is currently limited to linear and
nonlinear modal time-history load cases. Nonlinear static, staged-construction,
and direct-integration time-history load cases are available only for ETABS at
the present time.
• Nonlinear modal time-history (FNA) load cases only support nonlinearity in
link elements, hence nonlinear hysteretic damping energy from frame hinges
and shear walls is only produced if the “Model Hinges as Separate Link Elements” option is used (see Topic “Analysis Modeling” in Chapter “Hinge
Properties”). When using the “Model Hinges within Elements” option,
hysteretic damping energy from frame hinges and shear walls is not considered. Hysteretic behavior for layered shells is not considered for FNA load
cases either way.

360

Global Energy Response

Chapter XVIII

Load Cases

• The input energy and potential energy due to span loads within a frame element
may be under- or over-estimated if the internal deflection of the beam is significant compared to the displacements of the two ends. In such cases, subdividing
or meshing the frame element may result in a different and often more accurate
input and potential energy due to span loads. This effect may be especially pronounced when nonlinear hinges without hinge overwrites are present in a frame
element with large span loads. Using shorter hinge overwrites or the “Model
Hinges as Separate Link Elements” analysis option can be used to resolve this
issue. This is a limitation on the reported energy response and does not affect
any force, stress, displacement, or deformation response.
• Temperature and strain loading create self-equilibrating forces acting at the
joints of the element. The input energy for this type of loading is calculated as
the work done by these forces acting through the joint displacements. For a
fully restrained element, no input energy would be computed, and correspondingly the potential energy will also be reported as zero. On the other hand, an
unrestrained element will report non-zero work and potential energy due to
temperature loading. Note that the layered shell and frame hinges behave oppositely in this regard. Their energy is computed based on the internal stress state,
and thus they report nonzero input and potential energy due to restrained temperature loading, and zero energy for unrestrained loading.
• Hysteretic materials may sometimes underestimate the amount of potential energy present because they assume that unloading will occur along the original
elastic stiffness, when it may actually occur along a reduced stiffness. As a result, hysteretic energy may show a slight decrease when an element unloads
since some additional potential energy is recovered. This effect is generally insignificant for practical models.

Equation Solvers
You can choose from three solvers available for solving the stiffness equations:
• Standard Solver. This is the slowest of the solvers for larger problems and uses
the most disk space. However, it provides detailed warning messages about instabilities and sensitivity of the stiffness matrix.
• Advanced Solver. This is the default solver. It may be one or two orders of
magnitude faster than the Standard solver for larger problems, and it also uses
much less disk space. It provides limited information about instabilities.
• Multi-threaded Solver. This is the faster solver on machines with multiple
cores or processors. It runs in memory and does not use any disk space. It pro-

Equation Solvers

361

CSI Analysis Reference Manual
vides no information on instabilities. Depending on the amount of memory
available, you may need to use the Advanced solver for the largest problems.
Because the solvers perform numerical operations in a different order, it is possible
that sensitive problems may yield slightly different results with the different solvers due to numerical roundoff. Parallel processing can increase this effect. In extremely sensitive, nonlinear, history-dependent problems, the differences may be
more pronounced.
All verification examples have been run and checked using all three solvers. The results using the advanced solver are reported for comparison in the verification manuals.
The advanced solver is based on proprietary CSI technology. It uses, in part, code
derived from TAUCS family of solvers. Please see the copyright notice at the end
of Chapter “References” (page 533) for more information.

Environment Variables to Control Analysis
Several environment variables are available to control the solution process. These
are rarely needed. If you do use them, they can be set in the Windows Control Panel
or by using the SET command in a command prompt window. In general we recommend not changing these.
Using Windows Control Panel, you can add, remove, or change the environment
variables. By default they do not exist. Setting the value to zero or deleting the environment variable will result in default behavior. Changes made in the Control Panel
only affect instances of SAP2000 or other CSI products that are started after the
change is made. You cannot change the behavior of an instance that is already
started.
Using the command prompt, changes made to an environment variable only affect
instances of SAP2000 or other CSI products that are started from within that same
command prompt.

SAPFIRE_NUM_THREADS
Certain parts of the analysis process are parallelized, most notably moving-load
analysis and the calculation of certain element events, states, and stiffness matrices.
More parallelism will be implemented over time in future versions. By default the
analysis uses all the available physical cores, which may be half of the hyper-threaded cores.

362

Environment Variables to Control Analysis

Chapter XVIII

Load Cases

You can set SAPFIRE_NUM_THREADS to a positive number to reduce the number of threads if you plan to run multiple instances of the analysis, or want to
change the settings to obtain optimum performance from your machine.
The Multi-threaded solver uses its own logic to obtain optimum performance.
However, SAPFIRE_NUM_THREADS does set the maximum number of threads
to be used. You can override this value with the separate environment variable
SAPFIRE_NUM_THREADS_SOLVE. This is rarely needed but could be used to
achieve reproducible results in very sensitive models where the numerical calculations may be affected by the order of parallelized operations.
For the most complete control of the Multi-threaded solver, set the environment
variable MKL_DYNAMIC to value FALSE, which forces the solver to use the
specified number of threads. By default this value is TRUE. We do not generally
recommend changing the default behavior, since it may affect the efficiency of the
solver and other parallelized calculations. It could also affect other software products performing scientific and engineering computation if set in Windows Control
Panel.

SAPFIRE_FILESIZE_MB
By default the file-size limit for internal files used during analysis is 100 GB, but
this can be changed using the environment variable SAPFIRE_FILESIZE_MB to
specify an integer number of megabytes (MB). The value can represent 1 TB or
more, although the default value will rarely need to be increased. For most practical
problems, the amount of disk space and other system resources will control the size
of the model and associated analysis files that can be handled.
On the other hand, you will need to decrease this limit for Windows FAT32 file systems that are limited to 2 GB. In this case, set SAPFIRE_FILESIZE_MB to 2048 or
less. Most Windows machines use NTFS file systems and are not affected by this
limit. This value may also be needed for files that are intended to be zipped-up
(compressed) for storage or shipping.

Accessing the Assembled Stiffness and Mass Matrices
When using the advanced equation solver, you may request that the program produce the assembled stiffness and mass matrices in the form of text files. This can be
done for a single linear static, modal, or buckling Load Case. To get the stiffness
and mass matrices for a nonlinear case, define a linear case that uses the stiffness
from the final state of the desired nonlinear case.
Accessing the Assembled Stiffness and Mass Matrices

363

CSI Analysis Reference Manual
The assembled matrices are provided in five text files that have the same name as
the model file, but with the following extensions and contents:
• Extension .TXA: This file includes the counts of the number of joints and
equations in the model, and also describes the format and contents of the other
four files.
• Extension .TXE: This file gives the equation numbers for each degree of freedom (DOF) at each joint. Equation numbers are positive for active DOF that
are present in the stiffness and mass matrices, negative for constrained DOF
that are computed as linear combinations of active DOF, and zero for restrained
or null DOF.
• Extension .TXC: This file defines the constraint equations, and is only present
if there are constraints in the model.
• Extension .TXK: This file gives the lower half of the symmetric stiffness matrix.
• Extension .TXM: This file gives the lower half of the symmetric mass matrix.
Each of the latter four files contains a single header line that begins with “Note:”
and defines the data columns. All subsequent lines provide Tab-delimited data for
easy import into text editors or spreadsheet programs.

364

Accessing the Assembled Stiffness and Mass Matrices

C h a p t e r XIX

Modal Analysis
Modal analysis is used to determine the vibration modes of a structure. These
modes are useful to understand the behavior of the structure. They can also be used
as the basis for modal superposition in response-spectrum and modal time-history
Load Cases.
Basic Topics for All Users
• Overview
• Eigenvector Analysis
• Ritz-Vector Analysis
• Modal Analysis Output

Overview
A modal analysis is defined by creating a Load Case and setting its type to
“Modal”. You can define multiple modal Load Cases, resulting in multiple sets of
modes.
There are two types of modal analysis to choose from when defining a modal Load
Case:

Overview

365

CSI Analysis Reference Manual
• Eigenvector analysis determines the undamped free-vibration mode shapes
and frequencies of the system. These natural modes provide an excellent insight into the behavior of the structure.
• Ritz-vector analysis seeks to find modes that are excited by a particular loading. Ritz vectors can provide a better basis than do eigenvectors when used for
response-spectrum or time-history analyses that are based on modal superposition
You can request that static correction modes be calculated along with eigenvectors.
They are automatically included with Ritz vectors. Static correction-modes can be
very important for getting accurate response at stiff supports. Their use is generally recommended.
Modal analysis is always linear. A modal Load Case may be based on the stiffness
of the full unstressed structure, or upon the stiffness at the end of a nonlinear Load
Case (nonlinear static or nonlinear direct-integration time-history).
By using the stiffness at the end of a nonlinear case, you can evaluate the modes under P-delta or geometric stiffening conditions, at different stages of construction, or
following a significant nonlinear excursion in a large earthquake.
In addition, the mass used for a modal analysis can be changed if multiple Mass
Sources have been defined. The Mass Source to be used for a given modal load case
can be specified in the same types of nonlinear Load Cases that can be used to calculate the stiffness.
For more information:
• See Topic “Mass Source” (page 334) in Chapter “Load Patterns”.
• See Chapter “Load Cases” (page 341).

Eigenvector Analysis
Eigenvector analysis determines the undamped free-vibration mode shapes and frequencies of the system. These natural Modes provide an excellent insight into the
behavior of the structure. They can also be used as the basis for response-spectrum
or time-history analyses, although Ritz vectors are recommended for this purpose.
Eigenvector analysis involves the solution of the generalized eigenvalue problem:
[ K - W 2 M ]F = 0

366

Eigenvector Analysis

Chapter XIX

Modal Analysis

where K is the stiffness matrix, M is the diagonal mass matrix, W 2 is the diagonal
matrix of eigenvalues, and F is the matrix of corresponding eigenvectors (mode
shapes).
Each eigenvalue-eigenvector pair is called a natural Vibration Mode of the structure. The Modes are identified by numbers from 1 to n in the order in which the
modes are found by the program.
The eigenvalue is the square of the circular frequency, w, for that Mode (unless a
frequency shift is used, see below). The cyclic frequency, f, and period, T, of the
Mode are related to w by:
T=

1
f

and

f =

w
2p

You may specify the number of modes to be found, a convergence tolerance, and
the frequency range of interest. These parameters are described in the following
subtopics.

Number of Modes
You may specify the maximum and minimum number of modes to be found.
The program will not calculate more than the specified maximum number of
modes. This number includes any static correction modes requested. The program
may compute fewer modes if there are fewer mass degrees of freedom, all dynamic
participation targets have been met, or all modes within the cutoff frequency range
have been found.
The program will not calculate fewer than the specified minimum number of
modes, unless there are fewer mass degrees of freedom in the model.
A mass degree of freedom is any active degree of freedom that possesses translational mass or rotational mass moment of inertia. The mass may have been assigned
directly to the joint or may come from connected elements.
Only the modes that are actually found will be available for use by any subsequent
response-spectrum or modal time-history Load Cases.
See Topic “Degrees of Freedom” (page 30) in Chapter “Joints and Degrees of Freedom.”

Eigenvector Analysis

367

CSI Analysis Reference Manual

Frequency Range
You may specify a restricted frequency range in which to seek the Vibration Modes
by using the parameters:
• shift: The center of the cyclic frequency range, known as the shift frequency
• cut: The radius of the cyclic frequency range, known as the cutoff frequency
The program will only seek Modes with frequencies f that satisfy:
| f - shift | £ cut
The default value of cut = 0 does not restrict the frequency range of the Modes.
Modes are found in order of increasing distance of frequency from the shift. This
continues until the cutoff is reached, the requested number of Modes is found, or
the number of mass degrees of freedom is reached.
A stable structure will possess all positive natural frequencies. When performing a
seismic analysis and most other dynamic analyses, the lower-frequency modes are
usually of most interest. It is then appropriate to the default shift of zero, resulting
in the lowest-frequency modes of the structure being calculated. If the shift is not
zero, response-spectrum and time-history analyses may be performed; however,
static, moving-load, and p-delta analyses are not allowed.
If the dynamic loading is known to be of high frequency, such as that caused by vibrating machinery, it may be most efficient to use a positive shift near the center of
the frequency range of the loading.
A structure that is unstable when unloaded will have some modes with zero frequency. These modes may correspond to rigid-body motion of an inadequately
supported structure, or to mechanisms that may be present within the structure. It is
not possible to compute the static response of such a structure. However, by using a
small negative shift, the lowest-frequency vibration modes of the structure, including the zero-frequency instability modes, can be found. This does require some
mass to be present that is activated by each instability mode.
A structure that has buckled under P-delta load will have some modes with zero or
negative frequency. During equation solution, the number of frequencies less than
the shift is determined and printed in the log file. If you are using a zero or negative
shift and the program detects a negative-frequency mode, it will stop the analysis
since the results will be meaningless. If you use a positive shift, the program will
permit negative frequencies to be found; however, subsequent static and dynamic
results are still meaningless.

368

Eigenvector Analysis

Chapter XIX

Modal Analysis

When using a frequency shift, the stiffness matrix is modified by subtracting from
it the mass matrix multiplied by w0 2 , where w0 = 2 p shift. If the shift is very near a
natural frequency of the structure, the solution becomes unstable and will complain
during equation solution. Run the analysis again using a slightly different shift
frequency.
The circular frequency, w, of a Vibration Mode is determined from the shifted eigenvalue, m, as:
w=

m + w0 2

Automatic Shifting
As an option, you may request that the eigen-solver use automatic shifting to speed
up the solution and improve the accuracy of the results. This is particularly helpful
when seeking a large number of modes, for very large structures, or when there are
a lot of closely spaced modes to be found.
The solver will start with the requested shift frequency, shift (default zero), and
then successively then shift to the right (in the positive direction) as needed to improve the rate of convergence.
If no cutoff frequency has been specified (cut = 0), automatic shifting will only be
to the right, which means that eigenvalues to the left of the initial shift may be
missed. This is not usually a problem for stable structures starting with an initial
shift of zero.
If a cutoff frequency has been specified (cut > 0), automatic shifting will be to the
right until all eigenvalues between shift and shift + cut have been found, then the
automatic shifting will return to the initial shift and proceed to the left from there.
In either case, automatic shifting may not find eigenvalues in the usual order of increasing distance from the initial shift.

Convergence Tolerance
SAP2000 solves for the eigenvalue-eigenvectors pairs using an accelerated subspace iteration algorithm. During the solution phase, the program prints the approximate eigenvalues after each iteration. As the eigenvectors converge they are
removed from the subspace and new approximate vectors are introduced. For details of the algorithm, see Wilson and Tetsuji (1983).

Eigenvector Analysis

369

CSI Analysis Reference Manual
You may specify the relative convergence tolerance, tol, to control the solution; the
default value is tol = 10-9. The iteration for a particular Mode will continue until the
relative change in the eigenvalue between successive iterations is less than 2 × tol,
that is until:
m
-mi ½
1½
½ i+1
½£ tol
2½ m i + 1 ½
where m is the eigenvalue relative to the frequency shift, and i and i +1 denote successive iteration numbers.
In the usual case where the frequency shift is zero, the test for convergence becomes approximately the same as:
T - Ti ½
½
½ i+1
½£ tol
½ Ti + 1 ½

f
- fi ½
½
½ i+1
½£ tol
fi
½
½

provided that the difference between the two iterations is small.
Note that the error in the eigenvectors will generally be larger than the error in the
eigenvalues. The relative error in the global force balance for a given Mode gives a
measure of the error in the eigenvector. This error can usually be reduced by using a
smaller value of tol, at the expense of more computation time.

Static-Correction Modes
Static correction-modes can be very important for getting accurate response at stiff
supports. Their use is generally recommended.
You may request that the program compute the static-correction modes for any Acceleration Load or Load Pattern. A static-correction mode is the static solution to
that portion of the specified load that is not represented by the found eigenvectors.
When applied to acceleration loads, static-correction modes are also known as
missing-mass modes or residual-mass modes.
Static-correction modes are of little interest in their own right. They are intended to
be used as part of a modal basis for response-spectrum or modal time-history analysis for high frequency loading to which the structure responds statically. Although
a static-correction mode will have a mode shape and frequency (period) like the
eigenvectors do, it is not a true eigenvector.

370

Eigenvector Analysis

Chapter XIX

Modal Analysis

You can specify for which Load Patterns and/or Acceleration Loads you want static
correction modes calculated, if any. One static-correction mode will be computed
for each specified Load unless all eigenvectors that can be excited by that Load
have been found. Static-correction modes count against the maximum number of
modes requested for the Load Case.
As an example, consider the translational acceleration load in the UX direction, mx.
Define the participation factor for mode n as:
f xn = j n T m x
The static-correction load for UX translational acceleration is then:
n-M

m x0 = m x -

å f xnj n
n =1

The static-correction mode-shape vector, j x0 , is the solution to:
K j x0 = m x0
If m x0 is found to be zero, all of the modes necessary to represent UX acceleration
have been found, and no residual-mass mode is needed or will be calculated.
The static-correction modes for any other acceleration load or Load Pattern are defined similarly.
Each static-correction mode is assigned a frequency that is calculated using the
standard Rayleigh quotient method. When static-correction modes are calculated,
they are used for Response-spectrum and Time-history analysis just as the
eigenvectors are.
The use of static-correction modes assures that the static-load participation ratio
will be 100% for the selected acceleration loads. However, static-correction modes
do not generally result in mass-participation ratios or dynamic-load participation
ratios of 100%. Only true dynamic modes (eigen or Ritz vectors) can increase these
ratios to 100%.
See Topic “Modal Analysis Output” (page 349) in this Chapter for more information on modal participation ratios.
Note that Ritz vectors, described next, always include the residual-mass effect for
all starting load vectors.

Eigenvector Analysis

371

CSI Analysis Reference Manual

Ritz-Vector Analysis
Research has indicated that the natural free-vibration mode shapes are not the best
basis for a mode-superposition analysis of structures subjected to dynamic loads. It
has been demonstrated (Wilson, Yuan, and Dickens, 1982) that dynamic analyses
based on a special set of load-dependent Ritz vectors yield more accurate results
than the use of the same number of natural mode shapes. The algorithm is detailed
in Wilson (1985).
The reason the Ritz vectors yield excellent results is that they are generated by taking into account the spatial distribution of the dynamic loading, whereas the direct
use of the natural mode shapes neglects this very important information.
In addition, the Ritz-vector algorithm automatically includes the advantages of the
proven numerical techniques of static condensation, Guyan reduction, and static
correction due to higher-mode truncation.
The spatial distribution of the dynamic load vector serves as a starting load vector
to initiate the procedure. The first Ritz vector is the static displacement vector corresponding to the starting load vector. The remaining vectors are generated from a
recurrence relationship in which the mass matrix is multiplied by the previously obtained Ritz vector and used as the load vector for the next static solution. Each static
solution is called a generation cycle.
When the dynamic load is made up of several independent spatial distributions,
each of these may serve as a starting load vector to generate a set of Ritz vectors.
Each generation cycle creates as many Ritz vectors as there are starting load vectors. If a generated Ritz vector is redundant or does not excite any mass degrees of
freedom, it is discarded and the corresponding starting load vector is removed from
all subsequent generation cycles.
Standard eigen-solution techniques are used to orthogonalize the set of generated
Ritz vectors, resulting in a final set of Ritz-vector Modes. Each Ritz-vector Mode
consists of a mode shape and frequency. The full set of Ritz-vector Modes can be
used as a basis to represent the dynamic displacement of the structure.
When a sufficient number of Ritz-vector Modes have been found, some of them
may closely approximate natural mode shapes and frequencies. In general, however, Ritz-vector Modes do not represent the intrinsic characteristics of the structure in the same way the natural Modes do. The Ritz-vector modes are biased by the
starting load vectors.

372

Ritz-Vector Analysis

Chapter XIX

Modal Analysis

You may specify the number of Modes to be found, the starting load vectors to be
used, and the number of generation cycles to be performed for each starting load
vector. These parameters are described in the following subtopics.

Number of Modes
You may specify the maximum and minimum number of modes to be found.
The program will not calculate more than the specified maximum number of
modes. The program may compute fewer modes if there are fewer mass degrees of
freedom, all dynamic participation targets have been met, or the maximum number
of cycles has been reached for all loads.
The program will not calculate fewer than the specified minimum number of
modes, unless there are fewer mass degrees of freedom in the model.
A mass degree of freedom is any active degree of freedom that possesses
translational mass or rotational mass moment of inertia. The mass may have been
assigned directly to the joint or may come from connected elements.
Only the modes that are actually found will be available for use by any subsequent
response-spectrum or modal time-history Load Cases.
See Topic “Degrees of Freedom” (page 30) in Chapter “Joints and Degrees of Freedom.”

Starting Load Vectors
You may specify any number of starting load vectors. Each starting load vector
may be one of the following:
• An Acceleration Load in the global X, Y, or Z direction
• A Load Pattern
• A built-in nonlinear deformation load, as described below
For response-spectrum analysis, only the Acceleration Loads are needed. For
modal time-history analysis, one starting load vector is needed for each Load Pattern or Acceleration Load that is used in any modal time-history.
If nonlinear modal time-history analysis is to be performed, an additional starting
load vector is needed for each independent nonlinear deformation. You may specify that the program use the built-in nonlinear deformation loads, or you may define
your own Load Patterns for this purpose. See Topic “Nonlinear Deformation
Ritz-Vector Analysis

373

CSI Analysis Reference Manual
Loads” (page 271) in Chapter “The Link/Support Element—Basic” for more information.
If you define your own starting load vectors, do the following for each nonlinear
deformation:
• Explicitly define a Load Pattern that consists of a set of self-equilibrating
forces that activates the desired nonlinear deformation
• Specify that Load Pattern as a starting load vector
The number of such Load Patterns required is equal to the number of independent
nonlinear deformations in the model.
If several Link/Support elements act together, you may be able to use fewer starting
load vectors. For example, suppose the horizontal motion of several base isolators
are coupled with a diaphragm. Only three starting load vectors acting on the diaphragm are required: two perpendicular horizontal loads and one moment about the
vertical axis. Independent Load Cases may still be required to represent any vertical
motions or rotations about the horizontal axes for these isolators.
It is strongly recommended that mass (or mass moment of inertia) be present at
every degree of freedom that is loaded by a starting load vector. This is automatic
for Acceleration Loads, since the load is caused by mass. If a Load Pattern or nonlinear deformation load acts on a non-mass degree of freedom, the program issues a
warning. Such starting load vectors may generate inaccurate Ritz vectors, or even
no Ritz vectors at all.
Generally, the more starting load vectors used, the more Ritz vectors must be requested to cover the same frequency range. Thus including unnecessary starting
load vectors is not recommended.
In each generation cycle, Ritz vectors are found in the order in which the starting
load vectors are specified. In the last generation cycle, only as many Ritz vectors
will be found as required to reach the total number of Modes, n. For this reason, the
most important starting load vectors should be specified first, especially if the
number of starting load vectors is not much smaller than the total number of Modes.
For more information:
• See Topic “Nonlinear Modal Time-History Analysis (FNA)” (page 149) in
Chapter “Nonlinear Time-History Analysis”.
• See Chapter “Load Patterns” (page 321).

374

Ritz-Vector Analysis

Chapter XIX

Modal Analysis

Number of Generation Cycles
You may specify the maximum number of generation cycles, ncyc, to be performed
for each starting load vector. This enables you to obtain more Ritz vectors for some
starting load vectors than others. By default, the number of generation cycles performed for each starting load vector is unlimited, i.e., until the total number, n, of
requested Ritz vectors have been found.
As an example, suppose that two linear time-history analyses are to be performed:
(1) Gravity load is applied quasi-statically to the structure using Load Patterns DL
and LL
(2) Seismic load is applied in all three global directions
The starting load vectors required are the three Acceleration Loads and Load Patterns DL and LL. The first generation cycle creates the static solution for each starting load vector. This is all that is required for Load Patterns DL and LL in the first
History, hence for these starting load vectors ncyc = 1 should be specified. Additional Modes may be required to represent the dynamic response to the seismic
loading, hence an unlimited number of cycles should be specified for these starting
load vectors. If 12 Modes are requested (n = 12), there will be one each for DL and
LL, three each for two of the Acceleration Loads, and four for the Acceleration
Load that was specified first as a starting load vector.
Starting load vectors corresponding to nonlinear deformation loads may often need
only a limited number of generation cycles. Many of these loads affect only a small
local region and excite only high-frequency natural modes that may respond
quasi-statically to typical seismic excitation. If this is the case, you may be able to
specify ncyc = 1 or 2 for these starting load vectors. More cycles may be required if
you are particularly interested in the dynamic behavior in the local region.
You must use your own engineering judgment to determine the number of Ritz vectors to be generated for each starting load vector. No simple rule can apply to all
cases.

Modal Analysis Output
Various properties of the Vibration Modes are available as analysis results. This information is the same regardless of whether you use eigenvector or Ritz-vector
analysis, and is described in the following subtopics.

Modal Analysis Output

375

CSI Analysis Reference Manual

Periods and Frequencies
The following time-properties are printed for each Mode:
• Period, T, in units of time
• Cyclic frequency, f, in units of cycles per time; this is the inverse of T
• Circular frequency, w, in units of radians per time; w = 2 p f
• Eigenvalue, w2, in units of radians-per-time squared

Participation Factors
The modal participation factors are the dot products of the six Acceleration Loads
with the modes shapes. The participation factors for Mode n corresponding to
translational Acceleration Loads in the global X, Y, and Z directions are given by:
f xn = j n T m x
f

=j nT m y

f zn = j n T m z
where j n is the mode shape and mx, my, and, mz are the unit translational Acceleration Loads.
Similarly, the participation factors corresponding to rotational Acceleration Loads
about the centroidal axes parallel to the global X, Y, and Z axes are given by:
f rxn = j n T m rx
f ryn = j n T m ry
f rzn = j n T m rz
Here mrx, mry, and, mrz are the unit rotational Acceleration Loads.
These factors are the generalized loads acting on the Mode due to each of the Acceleration Loads. These values are called “factors” because they are related to the
mode shape and to a unit acceleration. The modes shapes are each normalized, or
scaled, with respect to the mass matrix such that:
j n T M j n =1

376

Modal Analysis Output

Chapter XIX

Modal Analysis

The actual magnitudes and signs of the participation factors are not important.
What is important is the relative values of the six factors for a given Mode.
Important: Although the rotational accelerations are applied in load cases about
the origins of the specified coordinate systems, the modal participation factors and
the various modal participation ratios described below for the rotational accelerations are reported about the center of mass for the structure. This makes the rotational participation factors and ratios are more meaningful because they do not include any contribution from the translational accelerations
For more information, See Topic “Acceleration Loads” (page 338) in Chapter
“Load Patterns.”

Participating Mass Ratios
The participating mass ratio for a Mode provides a measure of how important the
Mode is for computing the response to the six Acceleration Loads in the global coordinate system. Thus it is useful for determining the accuracy of responsespectrum analyses and seismic time-history analyses. The participating mass ratio
provides no information about the accuracy of time-history analyses subjected to
other loads.
The participating mass ratios for Mode n corresponding to translational Acceleration Loads in the global X, Y, and Z directions are given by:
rxn =

r yn =

r zn

( f xn ) 2
Mx
(f

yn )

( f zn ) 2
=
Mz

where fxn, fyn, and fzn are the participation factors defined in the previous subtopic;
and Mx, My, and Mz are the total unrestrained masses acting in the global X, Y, and Z
directions.
The participating mass ratios corresponding to rotational Acceleration Loads about
centroidal axes parallel to the global X, Y, and Z directions are given by:

Modal Analysis Output

377

CSI Analysis Reference Manual

rrxn =

rryn =

rrzn =

( f rxn ) 2
M rx
( f ryn )

M ry
( f rzn ) 2
M rz

where frxn, fryn, and frzn are the participation factors defined in the previous subtopic;
and Mrx, Mry, and Mrz are the total rotational inertias of the unrestrained masses acting about the centroidal axes parallel to the global X, Y, and Z directions.
The cumulative sums of the participating mass ratios for all Modes up to Mode n
are printed with the individual values for Mode n. This provides a simple measure
of how many Modes are required to achieve a given level of accuracy for
ground-acceleration loading.
If all eigen Modes of the structure are present, the participating mass ratio for each
of the Acceleration Loads should generally be unity (100%). However, this may
not be the case in the presence of Asolid elements or certain types of Constraints
where symmetry conditions prevent some of the mass from responding to translational accelerations.

Static and Dynamic Load Participation Ratios
The static and dynamic load participation ratios provide a measure of how adequate
the calculated modes are for representing the response to time-history analyses.
These two measures are printed in the output file for each of the following spatial
load vectors:
• The three unit Acceleration Loads
• Three rotational Acceleration loads
• All Load Patterns specified in the definition of the modal Load Case
• All nonlinear deformation loads, if they are specified in the definition of the
modal Load Case
The Load Patterns and Acceleration Loads represent spatial loads that you can explicitly specify in a modal time-history analysis, whereas the last represents loads
that can act implicitly in a nonlinear modal time-history analysis.

378

Modal Analysis Output

Chapter XIX

Modal Analysis

For more information:
• See Topic “Nonlinear Deformation Loads” (page 271) in Chapter “The
Link/Support Element—Basic.”
• See Chapter “Load Patterns” (page 321).
• See Topic “Acceleration Loads” (page 338) in Chapter “Load Patterns.”
• See Topic “Linear Modal Time-History Analysis” (page 403) in Chapter “Linear Time-History Analysis” .
• See Topic “Nonlinear Modal Time-History Analysis” (page 149) in Chapter
“Nonlinear Time-History Analysis”.
Static Load Participation Ratio
The static load participation ratio measures how well the calculated modes can represent the response to a given static load. This measure was first presented by Wilson (1997). For a given spatial load vector p, the participation factor for Mode n is
given by
f n =j nT p
where j n is the mode shape (vector) of Mode n. This factor is the generalized load
acting on the Mode due to load p. Note that f n is just the usual participation factor
when p is one of the six unit Acceleration Loads.
The static participation ratio for this mode is given by
2

æ fn ö
çç
÷
wn ÷ø
è
=
T
u p

where u is the static solution given by Ku = p. This ratio gives the fraction of the total strain energy in the exact static solution that is contained in Mode n. Note that
the denominator can also be represented as u T Ku.
Finally, the cumulative sum of the static participation ratios for all the calculated
modes is printed in the output file:
æ j nT p ö
÷
å çç
÷
n =1è wn ø
=
uT p
N

R S = å rnS
n =1

Modal Analysis Output

379

CSI Analysis Reference Manual
where N is the number of modes found. This value gives the fraction of the total
strain energy in the exact static solution that is captured by the N modes.
When solving for static solutions using quasi-static time-history analysis, the value
of R S should be close to 100% for any applied static Loads, and also for all nonlinear deformation loads if the analysis is nonlinear.
Note that when Ritz-vectors are used, the value of R S will always be 100% for all
starting load vectors. This may not be true when eigenvectors are used without
static correction modes. In fact, even using all possible eigenvectors will not give
100% static participation if load p acts on any massless degrees-of-freedom, or if
the system is sensitive or ill-conditioned. Static-correction or Ritz modes are highly
recommended in these cases.
Dynamic Load Participation Ratio
The dynamic load participation ratio measures how well the calculated modes can
represent the response to a given dynamic load. This measure was developed for
SAP2000, and it is an extension of the concept of participating mass ratios. It is assumed that the load acts only on degrees of freedom with mass. Any portion of load
vector p that acts on massless degrees of freedom cannot be represented by this
measure and is ignored in the following discussion.
For a given spatial load vector p, the participation factor for Mode n is given by
f n =j nT p
where j n is the mode shape for Mode n. Note that f n is just the usual participation
factor when p is one of the six unit Acceleration Loads.
The dynamic participation ratio for this mode is given by
D

rn =

( f n )2
T

a p

where a is the acceleration given by Ma = p. The acceleration a is easy to calculate
since M is diagonal. The values of a and p are taken to be zero at all massless degrees of freedom. Note that the denominator can also be represented as a T Ma .
Finally, the cumulative sum of the dynamic participation ratios for all the calculated modes is printed in the output file:

380

Modal Analysis Output

Chapter XIX
N

å (j n T p)

R D = å rnD = n =1
n =1

Modal Analysis

aT p

where N is the number of modes found. When p is one of the unit acceleration
loads, r D is the usual mass participation ratio, and R D is the usual cumulative mass
participation ratio.
When R D is 100%, the calculated modes should be capable of exactly representing
the solution to any time-varying application of spatial load p. If R D is less than
100%, the accuracy of the solution will depend upon the frequency content of the
time-function multiplying load p. Normally it is the high frequency response that is
not captured when R D is less than 100%.
The dynamic load participation ratio only measures how the modes capture the spatial characteristics of p, not its temporal characteristics. For this reason, R D serves
only as a qualitative guide as to whether enough modes have been computed. You
must still examine the response to each different dynamic loading with varying
number of modes to see if enough modes have been used.

Modal Analysis Output

381

CSI Analysis Reference Manual

382

Modal Analysis Output

C h a p t e r XX

Response-Spectrum Analysis
Response-spectrum analysis is a statistical type of analysis for the determination of
the likely response of a structure to seismic loading.
Basic Topics for All Users
• Overview
• Local Coordinate System
• Response-Spectrum Function
• Modal Damping
• Modal Combination
• Directional Combination
• Response-Spectrum Analysis Output

Overview
The dynamic equilibrium equations associated with the response of a structure to
ground motion are given by:
K u( t ) + C u&( t ) + M u&&( t ) = m x u&&gx ( t ) + m y u&&gy ( t ) + m z u&&gz ( t )
Overview

383

CSI Analysis Reference Manual
where K is the stiffness matrix; C is the proportional damping matrix; M is the di& and u&& are the relative displacements, velocities, and accelagonal mass matrix; u, u,
erations with respect to the ground; mx, my, and mz are the unit Acceleration Loads;
and u&&gx , u&&gy , and u&&gz are the components of uniform ground acceleration.
Response-spectrum analysis seeks the likely maximum response to these equations
rather than the full time history. The earthquake ground acceleration in each direction is given as a digitized response-spectrum curve of pseudo-spectral acceleration
response versus period of the structure.
Even though accelerations may be specified in three directions, only a single, positive result is produced for each response quantity. The response quantities include
displacements, forces, and stresses. Each computed result represents a statistical
measure of the likely maximum magnitude for that response quantity. The actual
response can be expected to vary within a range from this positive value to its negative.
No correspondence between two different response quantities is available. No information is available as to when this extreme value occurs during the seismic loading, or as to what the values of other response quantities are at that time.
Response-spectrum analysis is performed using mode superposition (Wilson and
Button, 1982). Modes may have been computed using eigenvector analysis or
Ritz-vector analysis. Ritz vectors are recommended since they give more accurate
results for the same number of Modes. You must define a Modal Load Case that
computes the modes, and then refer to that Modal Load Case in the definition of the
Response-Spectrum Case.
Response-spectrum can consider high-frequency rigid response if requested and if
appropriate modes have been computed. When eigen modes are used, you should
request that static correction vectors be computed. This information is automatically available in Ritz modes generated for ground acceleration. In either case, you
must be sure to have sufficient dynamical modes below the rigid frequency of the
ground motion.
Any number of response-spectrum Load Cases can be defined. Each case can differ
in the acceleration spectra applied and in the way that results are combined. Different cases can also be based upon different sets of modes computed in different
Modal Load Cases. For example, this would enable you to consider the response at
different stages of construction, or to compare the results using eigenvectors and
Ritz vectors.

384

Overview

Chapter XX

Response-Spectrum Analysis
Z, 3

ang

Global

csys

ang
Y

ang
X
1

Figure 80
Definition of Response Spectrum Local Coordinate System

Local Coordinate System
Each Spec has its own response-spectrum local coordinate system used to define
the directions of ground acceleration loading. The axes of this local system are denoted 1, 2, and 3. By default these correspond to the global X, Y, and Z directions,
respectively.
You may change the orientation of the local coordinate system by specifying:
• A fixed coordinate system csys (the default is zero, indicating the global coordinate system)
• A coordinate angle, ang (the default is zero)
The local 3 axis is always the same as the Z axis of coordinate system csys. The local 1 and 2 axes coincide with the X and Y axes of csys if angle ang is zero. Otherwise, ang is the angle from the X axis to the local 1 axis, measured counterclockwise when the +Z axis is pointing toward you. This is illustrated in Figure 80 (page
385).

Response-Spectrum Function
The response-spectrum curve for a given direction is defined by digitized points of
pseudo-spectral acceleration response versus period of the structure. The shape of

Local Coordinate System

385

CSI Analysis Reference Manual
40

PseudoSpectral
Acceleration
Response

Period (time)

Figure 81
Digitized Response-Spectrum Curve

the curve is given by specifying the name of a Function. All values for the abscissa
and ordinate of this Function must be zero or positive. See (page 381).
The function is assumed to be normalized with respect to gravity. You may specify
a scale factor sf to multiply the ordinate (pseudo-spectral acceleration response) of
the function. This should be used to convert the normalized acceleration to units
consistent with the rest of the model. The scale factor itself has acceleration units
and will be automatically converted if you change length units.
If the response-spectrum curve is not defined over a period range large enough to
cover the Vibration Modes of the structure, the curve is extended to larger and
smaller periods using a constant acceleration equal to the value at the nearest defined period.
See Topic “Functions” (page 350) in this Chapter for more information.

Damping
The response-spectrum curve chosen should reflect the damping that is present in
the structure being modeled. Note that the damping is inherent in the shape of the

386

Response-Spectrum Function

Chapter XX

Response-Spectrum Analysis

response-spectrum curve itself. As part of the response-spectrum function definition, you must specify the damping value that was used to generate the response-spectrum curve. During the analysis, the response-spectrum curve will automatically be adjusted from this damping value to the actual damping present in
the model.
If zero damping is specified for either the response-spectrum function or the response-spectrum load case, no scaling will be performed.

Modal Damping
Damping in the structure has two effects on response-spectrum analysis:
• It modifies the shape of the response-spectrum input curve
• It affects the amount of statistical coupling between the modes for certain
methods of response-spectrum modal combination (e.g., CQC and GMC)
The damping in the structure is modeled using uncoupled modal damping. Each
mode has a damping ratio, damp, which is measured as a fraction of critical damping and must satisfy:
0 £ damp < 1
Modal damping has three different sources, which are described in the following.
Damping from these sources are added together. The program automatically makes
sure that the total is less than one.
Modal Damping from the Load Case
For each response-spectrum Load Case, you may specify modal damping ratios
that are:
• Constant for all modes
• Linearly interpolated by period or frequency. You specify the damping ratio at
a series of frequency or period points. Between specified points the damping is
linearly interpolated. Outside the specified range, the damping ratio is constant
at the value given for the closest specified point.
• Mass and stiffness proportional. This mimics the proportional damping used
for direct-integration, except that the damping value is never allowed to exceed
unity.

Modal Damping

387

CSI Analysis Reference Manual
In addition, you may optionally specify damping overwrites. These are specific
values of damping to be used for specific modes that replace the damping obtained
by one of the methods above. The use of damping overwrites is rarely necessary.
Composite Modal Damping from the Materials
Modal damping ratios, if any, that have been specified for the Materials are converted automatically to composite modal damping. Any cross coupling between the
modes is ignored. These modal-damping values will generally be different for each
mode, depending upon how much deformation each mode causes in the elements
composed of the different Materials.
Effective Damping from the Link/Support Elements
Linear effective-damping coefficients, if any, that have been specified for
Link/Support elements in the model are automatically converted to modal damping. Any cross coupling between the modes is ignored. These effective
modal-damping values will generally be different for each mode, depending upon
how much deformation each mode causes in the Link/Support elements.

Modal Combination
For a given direction of acceleration, the maximum displacements, forces, and
stresses are computed throughout the structure for each of the Vibration Modes.
These modal values for a given response quantity are combined to produce a single,
positive result for the given direction of acceleration. The response has two parts:
periodic and rigid. You can control the contribution of these two parts by specifying controlling frequencies that are properties of the seismic loading.
In addition, you can choose the statistical method used to compute the periodic response. Modal damping, as described in the previous topic, may affect the coupling
between the modes, depending upon the method chosen for periodic modal combination.

Periodic and Rigid Response
For all modal combination methods except Absolute Sum, there are two parts to the
modal response for a given direction of loading: periodic and rigid. The distinction
here is a property of the loading, not of the structure. Two frequencies are defined,
f1 and f2, which define the rigid-response content of the ground motion, where f1 £
f2.

388

Modal Combination

Chapter XX

Response-Spectrum Analysis

For structural modes with frequencies less than f1 (longer periods), the response is
fully periodic. For structural modes with frequencies above f2 (shorter periods), the
response is fully rigid. Between frequencies f1 and f2, the amount of periodic and
rigid response is interpolated, as described by Gupta (1990).
Frequencies f1 and f2 are properties of the seismic input, not of the structure. Gupta
defines f1 as:
f1 =

S Amax
2p S Vmax

where S Amax is the maximum spectral acceleration and S Vmax is the maximum
spectral velocity for the ground motion considered. The default value for f1 is
unity.
Gupta defines f2 as:
1
2
f2 = f1 + f r
3
3
where f r is the rigid frequency of the seismic input, i.e., that frequency above
which the spectral acceleration is essentially constant and equal to the value at zero
period (infinite frequency). Others have defined f2 as:
f2 = f r
The following rules apply when specifying f1 and f2:
• If f2 = 0, no rigid response is calculated and all response is periodic, regardless
of the value specified for f1.
• Otherwise, the following condition must be satisfied: 0 £ f1 £ f2.
• Specifying f1 = 0 is the same as specifying f1 = f2.
For any given response quantity (displacement, stress, force, etc.), the periodic response, R p , is computed by one of the modal combination methods described below. The rigid response, R r , is always computed as an algebraic (fully correlated)
sum of the response from each mode having frequency above f2, and an interpolated portion of the response from each mode between f1 and f2. The total response,
R, is computed by one of the following two methods:
• SRSS, as recommended by Gupta (1990) and NRC (2006), which assumes that
these two parts are statistically independent:

Modal Combination

389

CSI Analysis Reference Manual
2

R = R p + Rr

• Absolute Sum, for compatibility with older methods:
R = R p + Rr
Please note that the choice of using the SRSS or Absolute Sum for combining periodic and rigid response is independent of the periodic modal combination or the directional combination methods described below.

CQC Method
The Complete Quadratic Combination technique for calculating the periodic response is described by Wilson, Der Kiureghian, and Bayo (1981). This is the default method of modal combination.
The CQC method takes into account the statistical coupling between closelyspaced Modes caused by modal damping. Increasing the modal damping increases
the coupling between closely-spaced modes. If the damping is zero for all Modes,
this method degenerates to the SRSS method.

GMC Method
The General Modal Combination technique for calculating the periodic response is
the complete modal combination procedure described by Equation 3.31 in Gupta
(1990). The GMC method takes into account the statistical coupling between
closely-spaced Modes similarly to the CQC method, but uses the Rosenblueth correlation coefficient with the time duration of the strong earthquake motion set to infinity. The result is essentially identical to the CQC method.
Increasing the modal damping increases the coupling between closely-spaced
modes. If the damping is zero for all Modes, this method degenerates to the SRSS
method.

SRSS Method
This method for calculating the periodic response combines the modal results by
taking the square root of the sum of their squares. This method does not take into
account any coupling of the modes, but rather assumes that the response of the
modes are all statistically independent. Modal damping does not affect the results.

390

Modal Combination

Chapter XX

Response-Spectrum Analysis

Absolute Sum Method
This method combines the modal results by taking the sum of their absolute values.
Essentially all modes are assumed to be fully correlated. This method is usually
over-conservative. The distinction between periodic and rigid response is not considered for this method. All modes are treated equally. Modal damping does not affect the results.

NRC Ten-Percent Method
This technique for calculating the periodic response is the Ten-Percent method of
the U.S. Nuclear Regulatory Commission Regulatory Guide 1.92 (NRC, 2006).
The Ten-Percent method assumes full, positive coupling between all modes whose
frequencies differ from each other by 10% or less of the smaller of the two frequencies. Modal damping does not affect the coupling.

NRC Double-Sum Method
This technique for calculating the periodic response is the Double-Sum method of
the U.S. Nuclear Regulatory Commission Regulatory Guide 1.92. (NRC, 2006).
The Double-Sum method assumes a positive coupling between all modes, with correlation coefficients that depend upon damping in a fashion similar to the CQC and
GMC methods, and that also depend upon the duration of the earthquake. You
specify this duration as parameter td as part of the Load Cases definition.

Directional Combination
For each displacement, force, or stress quantity in the structure, the modal combination produces a single, positive result for each direction of acceleration. These directional values for a given response quantity are combined to produce a single,
positive result. Three methods are available for combining the directional response,
SRSS, CQC3, and Absolute Sum.

SRSS Method
This method combines the response for different directions of loading by taking the
square root of the sum of their squares:

Directional Combination

391

CSI Analysis Reference Manual
2

R = R1 + R 2 + R 3

where R1 , R 2 , and R 3 are the modal-combination values for each direction. This
method is invariant with respect to coordinate system, i.e., the results do not depend
upon your choice of coordinate system when the given response-spectrum curves
are the same in each direction. This is the default method for directional combination, and is closely related to the CQC3 method described next.

CQC3 Method
The CQC3 method (Menun and Der Kiureghian, 1998) is an extension of the SRSS
method of directional combination. It is applicable when the two horizontal spectra
are identical in shape but have different scale factors, as is often assumed. When the
direction of loading for the two spectra is not known, it is necessary to consider the
envelope of loading at all possible angles.
The CQC3 method does this automatically by calculating the critical loading angle
for each response quantity, and reporting the maximum response at that angle. All
that is required is to specify the same response-spectrum function for directions U1
and U2, but with two different scale factors, and to select the CQC3 method for directional combination. The same response will be obtained no matter what value
you specify for the loading angle, ang, in a given coordinate system, csys, since all
angles are enveloped.
The response to vertical loading in direction U3, if present, is combined with the
maximum horizontal response using the SRSS rule. No variation of the vertical direction is considered.
If the horizontal spectra and their scale factors are both identical, the CQC3 method
degenerates to the SRSS method.
If different spectra are specified for the two horizontal directions, the CQC3
method may still be selected and the same calculations will be performed. However, the results are no longer completely independent of loading angle, and they
must be reviewed by an engineer for their significance.
The CQC3 method was originally defined for periodic response and for the CQC
method of modal combination. It has been extended in SAP2000 to apply to all
types of modal combination, and also to include the rigid response, if any. When
the absolute modal combination is used, the CQC3 results are not completely independent of loading angle, but for all quadratic types of modal combination, angular
independence is obtained. CQC3 can be recommended over the SRSS method un-

392

Directional Combination

Chapter XX

Response-Spectrum Analysis

less the direction of loading is known. Both methods are independent of the choice
of global coordinate system.

Absolute Sum Method
This method combines the response for different directions of loading by taking the
sum of their absolute values. A scale factor, dirf, is available for reducing the interaction between the different directions.
Specify dirf = 1 for a simple absolute sum:
R = R1 + R 2 + R 3
This method is usually over-conservative.
Specify 0 < dirf < 1 to combine the directional results by the scaled absolute sum
method. Here, the directional results are combined by taking the maximum, over all
directions, of the sum of the absolute values of the response in one direction plus
dirf times the response in the other directions.
For example, if dirf = 0.3, the spectral response, R, for a given displacement, force,
or stress would be:
R = max ( R1 , R 2 , R 3 )
where:
R1 = R1 + 03
. (R2 + R3 )
R 2 = R 2 + 03
. ( R1 + R 3 )
R 3 = R 3 + 03
. ( R1 + R 2 )
and R1 , R 2 , and R 3 are the modal-combination values for each direction.
Unlike the SRSS and CQC3 methods, the absolute sum method can give different
results depending upon your arbitrary choice of coordinate system, even when the
angle between the direction of loading and the principal axes of the structure is
fixed, and even when the magnitude of loading is the same in two or three directions.
Results obtained using dirf = 0.3 are comparable to the SRSS method (for equal input spectra in each direction), but may be as much as 8% unconservative or 4%
over-conservative, depending upon the coordinate system. Larger values of dirf
tend to produce more conservative results.
Directional Combination

393

CSI Analysis Reference Manual

Response-Spectrum Analysis Output
Information about each response-spectrum Load Case is available for display,
printing, and export using the SAP2000 database tables. This information is described in the following subtopics.

Damping and Accelerations
The modal damping and the ground accelerations acting in each direction are given
for every Mode.
The damping value printed for each Mode is the sum of the specified damping for
the Load Case, plus the modal damping contributed by effective damping in the
Link/Support elements, if any, and the composite modal damping specified in the
Material Properties, if any.
The accelerations printed for each Mode are the actual values as interpolated at the
modal period from the response-spectrum curves after scaling by the specified
value of sf and modification for damping. The accelerations are always referred to
the local axes of the response-spectrum analysis. They are identified in the output
as U1, U2, and U3.

Modal Amplitudes
The response-spectrum modal amplitudes give the multipliers of the mode shapes
that contribute to the displaced shape of the structure for each direction of Acceleration. For a given Mode and a given direction of acceleration, this is the product
of the modal participation factor and the response-spectrum acceleration, divided
by the eigenvalue, w2, of the Mode.
This amplitude, multiplied by any modal response quantity (displacement, force,
stress, etc.), gives the contribution of that mode to the value of the same response
quantity reported for the response-spectrum load case.
The acceleration directions are always referred to the local axes of the responsespectrum analysis. They are identified in the output as U1, U2, and U3.
For more information:
• See the previous Topic “Damping and Acceleration” for the definition of the
response-spectrum accelerations.

394

Response-Spectrum Analysis Output

Chapter XX

Response-Spectrum Analysis

• See Topic “Modal Analysis Output” (page 349) in Chapter “Modal Analysis”
for the definition of the modal participation factors and the eigenvalues.

Base Reactions
The base reactions are the total forces and moments about the global origin required
of the supports (Restraints, Springs, and one-joint Link/Support elements) to resist
the inertia forces due to response-spectrum loading.
These are reported separately for each individual Mode and each direction of loading without any combination. The total response-spectrum reactions are then reported after performing modal combination and directional combination.
The reaction forces and moments are always referred to the local axes of the
response-spectrum analysis. They are identified in the output as F1, F2, F3, M1,
M2, and M3.
Important Note: Accurate base reactions are best obtained when static-correction
modes are included in an eigen analysis, or when Ritz vectors are used. This is particularly true when large stiffnesses are used at the supports and the model is sensitive or ill-conditioned.

Response-Spectrum Analysis Output

395

CSI Analysis Reference Manual

396

Response-Spectrum Analysis Output

C h a p t e r XXI

Linear Time-History Analysis
Time-history analysis is a step-by-step analysis of the dynamical response of a
structure to a specified loading that may vary with time. The analysis may be linear
or nonlinear. This Chapter describes time-history analysis in general, and linear
time-history analysis in particular. See Chapter “Nonlinear Time-History Analysis” (page 447) for additional information that applies only to nonlinear time-history analysis.
Basic Topics for All Users
• Overview
Advanced Topics
• Loading
• Initial Conditions
• Time Steps
• Modal Time-History Analysis
• Direct-Integration Time-History Analysis

397

CSI Analysis Reference Manual

Overview
Time-history analysis is used to determine the dynamic response of a structure to
arbitrary loading. The dynamic equilibrium equations to be solved are given by:
K u( t ) + C u&( t ) + M u&&( t ) = r ( t )
where K is the stiffness matrix; C is the damping matrix; M is the diagonal mass
& and u&& are the displacements, velocities, and accelerations of the strucmatrix; u, u,
ture; and r is the applied load. If the load includes ground acceleration, the
displacements, velocities, and accelerations are relative to this ground motion.
Any number of time-history Load Cases can be defined. Each time-history case can
differ in the load applied and in the type of analysis to be performed.
There are several options that determine the type of time-history analysis to be performed:
• Linear vs. Nonlinear.
• Modal vs. Direct-integration: These are two different solution methods, each
with advantages and disadvantages. Under ideal circumstances, both methods
should yield the same results to a given problem.
• Transient vs. Periodic: Transient analysis considers the applied load as a
one-time event, with a beginning and end. Periodic analysis considers the load
to repeat indefinitely, with all transient response damped out.
Periodic analysis is only available for linear modal time-history analysis.
This Chapter describes linear analysis; nonlinear analysis is described in Chapter
“Nonlinear Time-History Analysis” (page 447). However, you should read the
present Chapter first.

Loading
The load, r(t), applied in a given time-history case may be an arbitrary function of
space and time. It can be written as a finite sum of spatial load vectors, p i , multiplied by time functions, f i ( t ), as:
r ( t ) = å f i ( t ) pi
i

398

Overview

(Eqn. 1)

Chapter XXI

Linear Time-History Analysis

The program uses Load Patterns and/or Acceleration Loads to represent the spatial
load vectors. The time functions can be arbitrary functions of time or periodic functions such as those produced by wind or sea wave loading.
If Acceleration Loads are used, the displacements, velocities, and accelerations are
all measured relative to the ground. The time functions associated with the Acceleration Loads mx, my, and mz are the corresponding components of uniform ground
acceleration, u&&gx , u&&gy , and u&&gz .

Defining the Spatial Load Vectors
To define the spatial load vector, pi, for a single term of the loading sum of Equation
1, you may specify either:
• The label of a Load Pattern using the parameter load, or
• An Acceleration Load using the parameters csys, ang, and acc, where:
– csys is a fixed coordinate system (the default is zero, indicating the global
coordinate system)
– ang is a coordinate angle (the default is zero)
– acc is the Acceleration Load (U1, U2, or U3) in the acceleration local coordinate system as defined below
Each Acceleration Load in the loading sum may have its own acceleration local coordinate system with local axes denoted 1, 2, and 3. The local 3 axis is always the
same as the Z axis of coordinate system csys. The local 1 and 2 axes coincide with
the X and Y axes of csys if angle ang is zero. Otherwise, ang is the angle from the X
axis to the local 1 axis, measured counterclockwise when the +Z axis is pointing toward you. This is illustrated in Figure 82 (page 400).
The response-spectrum local axes are always referred to as 1, 2, and 3. The global
Acceleration Loads mx, my, and mz are transformed to the local coordinate system
for loading.
It is generally recommended, but not required, that the same coordinate system be
used for all Acceleration Loads applied in a given time-history case.
Load Patterns and Acceleration Loads may be mixed in the loading sum.
For more information:
• See Chapter “Load Patterns” (page 321).
• See Topic “Acceleration Loads” (page 338) in Chapter “Load Patterns”.
Loading

399

CSI Analysis Reference Manual
Z, 3

ang

Global

csys

ang
Y

ang
X
1

Figure 82
Definition of History Acceleration Local Coordinate System

Defining the Time Functions
To define the time function, fi(t), for a single term of the loading sum of Equation 1,
you may specify:
• The label of a Function, using the parameter func, that defines the shape of the
time variation (the default is zero, indicating the built-in ramp function defined
below)
• A scale factor, sf, that multiplies the ordinate values of the Function (the default is unity)
• A time-scale factor, tf, that multiplies the time (abscissa) values of the Function
(the default is unity)
• An arrival time, at, when the Function begins to act on the structure (the default
is zero)
The time function, fi(t), is related to the specified Function, func(t), by:
fi(t) = sf · func(t)
The analysis time, t, is related to the time scale, t, of the specified Function by:
t = at + tf · t

400

Chapter XXI

Linear Time-History Analysis

fi(t)
Ramp function after scaling

Built-in ramp function

Figure 83
Built-in Ramp Function before and after Scaling

If the arrival time is positive, the application of Function func is delayed until after
the start of the analysis. If the arrival time is negative, that portion of Function func
occurring before t = – at / tf is ignored.
For a Function func defined from initial time t0 to final time tn, the value of the
Function for all time t < t0 is taken as zero, and the value of the Function for all time
t > tn is held constant at fn, the value at tn.
If no Function is specified, or func = 0, the built-in ramp function is used. This
function increases linearly from zero at t = 0 to unity at t =1 and for all time thereafter. When combined with the scaling parameters, this defines a function that increases linearly from zero at t = at to a value of sf at t = at + tf and for all time thereafter, as illustrated in Figure 83 (page 401). This function is most commonly used
to gradually apply static loads, but can also be used to build up triangular pulses and
more complicated functions.
See Topic “Functions” (page 350) in Chapter “Load Cases” for more information.

401

CSI Analysis Reference Manual

Initial Conditions
The initial conditions describe the state of the structure at the beginning of a
time-history case. These include:
• Displacements and velocities
• Internal forces and stresses
• Internal state variables for nonlinear elements
• Energy values for the structure
• External loads
The accelerations are not considered initial conditions, but are computed from the
equilibrium equation.
For linear transient analyses, zero initial conditions are always assumed.
For periodic analyses, the program automatically adjusts the initial conditions at
the start of the analysis to be equal to the conditions at the end of the analysis
If you are using the stiffness from the end of a nonlinear analysis, nonlinear elements (if any) are locked into the state that existed at the end of the nonlinear analysis. For example, suppose you performed a nonlinear analysis of a model containing tension-only frame elements (compression limit set to zero), and used the stiffness from this case for a linear time-history analysis. Elements that were in tension
at the end of the nonlinear analysis would have full axial stiffness in the linear
time-history analysis, and elements that were in compression at the end of the nonlinear analysis would have zero stiffness. These stiffnesses would be fixed for the
duration of the linear time-history analysis, regardless of the direction of loading.
See also Topic “Mass Source” (page 334) in Chapter “Load Patterns” for additional
information.

Time Steps
Time-history analysis is performed at discrete time steps. You may specify the
number of output time steps with parameter nstep and the size of the time steps
with parameter dt.
The time span over which the analysis is carried out is given by nstep·dt. For periodic analysis, the period of the cyclic loading function is assumed to be equal to this
time span.

402

Initial Conditions

Chapter XXI

Linear Time-History Analysis

Responses are calculated at the end of each dt time increment, resulting in nstep+1
values for each output response quantity.
Response is also calculated, but not saved, at every time step of the input time functions in order to accurately capture the full effect of the loading. These time steps
are call load steps. For modal time-history analysis, this has little effect on efficiency.
For direct-integration time-history analysis, this may cause the stiffness matrix to
be re-solved if the load step size keeps changing. For example, if the output time
step is 0.01 and the input time step is 0.005, the program will use a constant internal
time-step of 0.005. However, if the input time step is 0.075, then the input and output steps are out of synchrony, and the loads steps will be: 0.075, 0.025, 0.05, 0.05,
0.025, 0.075, and so on. For this reason, it is usually advisable to choose an output
time step that evenly divides, or is evenly divided by, the input time steps.

Modal Time-History Analysis
Modal superposition provides a highly efficient and accurate procedure for performing time-history analysis. Closed-form integration of the modal equations is
used to compute the response, assuming linear variation of the time functions,
f i ( t ), between the input data time points. Therefore, numerical instability problems
are never encountered, and the time increment may be any sampling value that is
deemed fine enough to capture the maximum response values. One-tenth of the
time period of the highest mode is usually recommended; however, a larger value
may give an equally accurate sampling if the contribution of the higher modes is
small.
The modes used are computed in a Modal Load Case that you define. They can be
the undamped free-vibration Modes (eigenvectors) or the load-dependent Ritz-vector Modes.
If all of the spatial load vectors, p i , are used as starting load vectors for Ritz-vector
analysis, then the Ritz vectors will always produce more accurate results than if the
same number of eigenvectors is used. Since the Ritz-vector algorithm is faster than
the eigenvector algorithm, the former is recommended for time-history analyses.
It is up to you to determine if the Modes calculated by the program are adequate to
represent the time-history response to the applied load. You should check:
• That enough Modes have been computed
• That the Modes cover an adequate frequency range
Modal Time-History Analysis

403

CSI Analysis Reference Manual
• That the dynamic load (mass) participation mass ratios are adequate for the
Load Patterns and/or Acceleration Loads being applied
• That the modes shapes adequately represent all desired deformations
Important Note: Accurate base reactions are best obtained when static-correction
modes are included in an eigen analysis, or when Ritz vectors are used. This is particularly true when large stiffnesses are used at the supports and the model is sensitive or ill-conditioned. The use of static-correction modes or Ritz vectors is generally recommended for all modal time-history analyses.
See Chapter “Modal Analysis” (page 365) for more information.

Modal Damping
The damping in the structure is modeled using uncoupled modal damping. Each
mode has a damping ratio, damp, which is measured as a fraction of critical damping and must satisfy:
0 £ damp < 1
Modal damping has three different sources, which are described in the following.
Damping from these sources is added together. The program automatically makes
sure that the total is less than one.
Modal Damping from the Load Case
For each linear modal time-history Load Case, you may specify modal damping ratios that are:
• Constant for all modes
• Linearly interpolated by period or frequency. You specify the damping ratio at
a series of frequency or period points. Between specified points the damping is
linearly interpolated. Outside the specified range, the damping ratio is constant
at the value given for the closest specified point.
• Mass and stiffness proportional. This mimics the proportional damping used
for direct-integration, except that the damping value is never allowed to exceed
unity.
In addition, you may optionally specify damping overwrites. These are specific
values of damping to be used for specific modes that replace the damping obtained
by one of the methods above. The use of damping overwrites is rarely necessary.

404

Modal Time-History Analysis

Chapter XXI

Linear Time-History Analysis

Composite Modal Damping from the Materials
Modal damping ratios, if any, that have been specified for the Materials are converted automatically to composite modal damping. Any cross coupling between the
modes is ignored. These modal-damping values will generally be different for each
mode, depending upon how much deformation each mode causes in the elements
composed of the different Materials.
Effective Damping from the Link/Support Elements
Linear effective-damping coefficients, if any, that have been specified for
Link/Support elements in the model are automatically converted to modal damping. Any cross coupling between the modes is ignored. These effective
modal-damping values will generally be different for each mode, depending upon
how much deformation each mode causes in the Link/Support elements.

Direct-Integration Time-History Analysis
Direct integration of the full equations of motion without the use of modal superposition is available in SAP2000. While modal superposition is usually more accurate
and efficient, direct-integration does offer the following advantages for linear problems:
• Full damping that couples the modes can be considered
• Impact and wave propagation problems that might excite a large number of
modes may be more efficiently solved by direct integration
For nonlinear problems, direct integration also allows consideration of more types
of nonlinearity that does modal superposition.
Direct integration results are extremely sensitive to time-step size in a way that is
not true for modal superposition. You should always run your direct-integration
analyses with decreasing time-step sizes until the step size is small enough that results are no longer affected by it.
In particular, you should check stiff and localized response quantities. For example, a much smaller time step may be required to get accurate results for the axial
force in a stiff member than for the lateral displacement at the top of a structure.

Direct-Integration Time-History Analysis

405

CSI Analysis Reference Manual

Time Integration Parameters
A variety of common methods are available for performing direct-integration
time-history analysis. Since these are well documented in standard textbooks, we
will not describe them further here, except to suggest that you use the default
“Hilber-Hughes-Taylor alpha” (HHT) method, unless you have a specific preference for a different method.
The HHT method uses a single parameter called alpha. This parameter may take
values between 0 and -1/3.
For alpha = 0, the method is equivalent to the Newmark method with gamma = 0.5
and beta = 0.25, which is the same as the average acceleration method (also called
the trapezoidal rule.) Using alpha = 0 offers the highest accuracy of the available
methods, but may permit excessive vibrations in the higher frequency modes, i.e.,
those modes with periods of the same order as or less than the time-step size.
For more negative values of alpha, the higher frequency modes are more severely
damped. This is not physical damping, since it decreases as smaller time-steps are
used. However, it is often necessary to use a negative value of alpha to encourage a
nonlinear solution to converge.
For best results, use the smallest time step practical, and select alpha as close to zero
as possible. Try different values of alpha and time-step size to be sure that the solution is not too dependent upon these parameters.

Damping
In direct-integration time-history analysis, the damping in the structure is modeled
using a full damping matrix. Unlike modal damping, this allows coupling between
the modes to be considered.
Direct-integration damping has three different sources, which are described in the
following. Damping from these sources is added together.
Proportional Damping from the Load Case
For each direct-integration time-history Load Case, you may specify proportional
damping coefficients that apply to the structure as a whole. The damping matrix is
calculated as a linear combination of the stiffness matrix scaled by a coefficient,
c K , and the mass matrix scaled by a second coefficient, c M .

406

Direct-Integration Time-History Analysis

Chapter XXI

Linear Time-History Analysis

You may specify these two coefficients directly, or they may be computed by specifying equivalent fractions of critical modal damping at two different periods or frequencies.
For each nonlinear element in the structure, the coefficient c K multiplies the initial
stiffness matrix, i.e., the stiffness of the element at zero initial conditions, regardless of the nonlinear state used to start this analysis. The exception to this rule is that
if the starting nonlinear state has zero stiffness and zero force or stress (such as an
open gap or a cracked concrete material), then zero damping is assumed. In the case
where the initial stiffness is different in the negative and positive direction of loading, the larger stiffness is used.
For cable elements, the damping matrix is proportional to the stiffness matrix for an
equivalent truss element along the current chord having the same axial stiffness
(AE/L), where L is the undeformed length.
The resulting stiffness-proportional damping is linearly proportional to frequency.
It is related to the deformations within the structure. Stiffness proportional damping
may excessively damp out high frequency components.
The resulting mass-proportional damping is linearly proportional to period. It is related to the motion of the structure, as if the structure is moving through a viscous
fluid. Mass proportional damping may excessively damp out long period components.
Proportional Damping from the Materials
You may specify stiffness and mass proportional damping coefficients for individual materials. For example, you may want to use larger coefficients for soil materials than for steel or concrete. The same interpretation of these coefficients applies
as described above for the Load Case damping. Be sure not to double-count the
damping by including the same amount in both the Load Case and the materials.
Effective Damping from the Link/Support Elements
Linear effective-damping coefficients, if any, that have been specified for
Link/Support elements are directly included in the damping matrix.

Direct-Integration Time-History Analysis

407

CSI Analysis Reference Manual

408

Direct-Integration Time-History Analysis

C h a p t e r XXII

Geometric Nonlinearity
SAP2000 is capable of considering geometric nonlinearity in the form of either
P-delta effects or large-displacement/rotation effects. Strains within the elements
are assumed to be small. Geometric nonlinearity can be considered on a
step-by-step basis in nonlinear static and direct-integration time-history analysis,
and incorporated in the stiffness matrix for linear analyses.
Advanced Topics
• Overview
• Nonlinear Load Cases
• The P-Delta Effect
• Initial P-Delta Analysis
• Large Displacements

Overview
When the load acting on a structure and the resulting deflections are small enough,
the load-deflection relationship for the structure is linear. For the most part,
SAP2000 analyses assume such linear behavior. This permits the program to form
the equilibrium equations using the original (undeformed) geometry of the strucOverview

409

CSI Analysis Reference Manual
ture. Strictly speaking, the equilibrium equations should actually refer to the geometry of the structure after deformation.
The linear equilibrium equations are independent of the applied load and the resulting deflection. Thus the results of different static and/or dynamic loads can be
superposed (scaled and added), resulting in great computational efficiency.
If the load on the structure and/or the resulting deflections are large, then the
load-deflection behavior may become nonlinear. Several causes of this nonlinear
behavior can be identified:
• P-delta (large-stress) effect: when large stresses (or forces and moments) are
present within a structure, equilibrium equations written for the original and
the deformed geometries may differ significantly, even if the deformations are
very small.
• Large-displacement effect: when a structure undergoes large deformation (in
particular, large strains and rotations), the usual engineering stress and strain
measures no longer apply, and the equilibrium equations must be written for
the deformed geometry. This is true even if the stresses are small.
• Material nonlinearity: when a material is strained beyond its proportional
limit, the stress-strain relationship is no longer linear. Plastic materials strained
beyond the yield point may exhibit history-dependent behavior. Material
nonlinearity may affect the load-deflection behavior of a structure even when
the equilibrium equations for the original geometry are still valid.
• Other effects: Other sources of nonlinearity are also possible, including nonlinear loads, boundary conditions and constraints.
The large-stress and large-displacement effects are both termed geometric (or kinematic) nonlinearity, as distinguished from material nonlinearity. Kinematic
nonlinearity may also be referred to as second-order geometric effects.
This Chapter deals with the geometric nonlinearity effects that can be analyzed using SAP2000. For each nonlinear static and nonlinear direct-integration time-history analysis, you may choose to consider:
• No geometric nonlinearity
• P-delta effects only
• Large displacement and P-delta effects
The large displacement effect in SAP2000 includes only the effects of large translations and rotations. The strains are assumed to be small in all elements.

410

Overview

Chapter XXII

Geometric Nonlinearity

Material nonlinearity is discussed in Chapters “The Frame Element” (page 105),
“Frame Hinge Properties” (page 147), and “The Link/Support Element—Basic”
(page 251). Since small strains are assumed, material nonlinearity and geometric
nonlinearity effects are independent.
Once a nonlinear analysis has been performed, its final stiffness matrix can be used
for subsequent linear analyses. Any geometric nonlinearity considered in the nonlinear analysis will affect the linear results. In particular, this can be used to include
relatively constant P-delta effects in buildings or the tension-stiffening effects in
cable structures into a series of superposable linear analyses.
For more information:
• See Chapter “Load Cases” (page 341)
• See Chapter “Nonlinear Static Analysis” (page 425)
• See Chapter “Nonlinear Time-History Analysis” (page 447)

Nonlinear Load Cases
For nonlinear static and nonlinear direct-integration time-history analysis, you may
choose the type of geometric nonlinearity to consider:
• None: All equilibrium equations are considered in the undeformed configuration of the structure
• P-delta only: The equilibrium equations take into partial account the deformed
configuration of the structure. Tensile forces tend to resist the rotation of elements and stiffen the structure, and compressive forces tend to enhance the rotation of elements and destabilize the structure. This may require a moderate
amount of iteration.
• Large displacements: All equilibrium equations are written in the deformed
configuration of the structure. This may require a large amount of iteration;
Newton-Raphson iterations are usually most effective. Although large displacement and large rotation effects are modeled, all strains are assumed to be
small. P-delta effects are included.
When continuing one nonlinear Load Case from another, it is recommended that
they both have the same geometric-nonlinearity settings.
The large displacement option should be used for any structures undergoing significant deformation; and for buckling analysis, particularly for snap-through buckling and post-buckling behavior. Cables (modeled by frame elements) and other elNonlinear Load Cases

411

CSI Analysis Reference Manual
F

Original Configuration

F
P

Deformed Configuration
D

Figure 84
Geometry for Cantilever Beam Example

ements that undergo significant relative rotations within the element should be divided into smaller elements to satisfy the requirement that the strains and relative
rotations within an element are small.
For most other structures, the P-delta option is adequate, particularly when material
nonlinearity dominates.
If reasonable, it is recommended that the analysis be performed first without geometric nonlinearity, adding P-delta, and possibly large-displacement effects later.
Geometric nonlinearity is not available for nonlinear modal time-history (FNA)
analyses, except for the fixed effects that may have been included in the stiffness
matrix used to generate the modes.
Note that the catenary Cable element does not require P-delta or Large Displacements to exhibit its internal geometric nonlinearity. The choice should be determined by the rest of the structure.

412

Nonlinear Load Cases

Chapter XXII

Geometric Nonlinearity

The P-Delta Effect
The P-Delta effect refers specifically to the nonlinear geometric effect of a large
tensile or compressive direct stress upon transverse bending and shear behavior. A
compressive stress tends to make a structural member more flexible in transverse
bending and shear, whereas a tensile stress tends to stiffen the member against
transverse deformation.
This option is particularly useful for considering the effect of gravity loads upon
the lateral stiffness of building structures, as required by certain design codes (ACI
2002; AISC 2003). It can also be used for the analysis of some cable structures,
such as suspension bridges, cable-stayed bridges, and guyed towers. Other applications are possible.
The basic concepts behind the P-Delta effect are illustrated in the following example. Consider a cantilever beam subject to an axial load P and a transverse tip load F
as shown in Figure 84 (page 412). The internal axial force throughout the member
is also equal to P.
If equilibrium is examined in the original configuration (using the undeformed geometry), the moment at the base is M = FL, and decreases linearly to zero at the
loaded end. If, instead, equilibrium is considered in the deformed configuration,
there is an additional moment caused by the axial force P acting on the transverse
tip displacement, D. The moment no longer varies linearly along the length; the
variation depends instead upon the deflected shape. The moment at the base is now
M = FL - PD. The moment diagrams for various cases are shown in Figure
85 (page 414).
Note that only the transverse deflection is considered in the deformed configuration. Any change in moment due to a change in length of the member is neglected
here.
If the beam is in tension, the moment at the base and throughout the member is reduced, hence the transverse bending deflection, D, is also reduced. Thus the member is effectively stiffer against the transverse load F.
Conversely, if the beam is in compression, the moment throughout the member,
and hence the transverse bending deflection, D, are now increased. The member is
effectively more flexible against the load F.
If the compressive force is large enough, the transverse stiffness goes to zero and
hence the deflection D tends to infinity; the structure is said to have buckled. The

The P-Delta Effect

413

CSI Analysis Reference Manual

Moment in Original Configuration without P-Delta

PD
FL

Moment for Tensile Load P with P-Delta

Moment for Compressive Load P with P-Delta

Figure 85
Moment Diagrams for Cantilever Beam Examples

theoretical value of P at which this occurs is called the Euler buckling load for the
beam; it is denoted by Pcr and is given by the formula
Pcr = -

414

p 2 EI
4 L2

The P-Delta Effect

Chapter XXII

Geometric Nonlinearity

where EI is the bending stiffness of the beam section.
The exact P-Delta effect of the axial load upon the transverse deflection and stiffness is a rather complicated function of the ratio of the force P to the buckling load
Pcr . The true deflected shape of the beam, and hence the effect upon the moment
diagram, is described by cubic functions under zero axial load, hyperbolic functions under tension, and trigonometric functions under compression.
The P-Delta effect can be present in any other beam configuration, such as simplysupported, fixed-fixed, etc. The P-Delta effect may apply locally to individual
members, or globally to the structural system as a whole.
The key feature is that a large axial force, acting upon a small transverse deflection,
produces a significant moment that affects the behavior of the member or structure.
If the deflection is small, then the moment produced is proportional to the deflection.

P-Delta Forces in the Frame Element
The implementation of the P-Delta effect in the Frame element is described in the
following subtopics.
Cubic Deflected Shape
The P-Delta effect is integrated along the length of each Frame element, taking into
account the deflection within the element. For this purpose the transverse deflected
shape is assumed to be cubic for bending and linear for shear between the rigid ends
of the element. The length of the rigid ends is the product of the rigid-end factor and
the end offsets, and is usually zero. See Topic “End Offsets” (page 127) in Chapter
“The Frame Element” for more information.
The true deflected shape may differ somewhat from this assumed cubic/linear deflection in the following situations:
• The element has non-prismatic Section properties. In this case the P-Delta deflected shape is computed as if the element were prismatic using the average of
the properties over the length of the element
• Loads are acting along the length of the element. In this case the P-Delta deflected shape is computed using the equivalent fixed-end forces applied to the
ends of the element.

The P-Delta Effect

415

CSI Analysis Reference Manual
• A large P-force is acting on the element. The true deflected shape is actually described by trigonometric functions under large compression, and by hyperbolic
functions under large tension.
The assumed cubic shape is usually a good approximation to these shapes except
under a compressive P-force near the buckling load with certain end restraints. Excellent results, however, can be obtained by dividing any structural member into
two or more Frame elements. See the Software Verification Manual for more detail.
Computed P-Delta Axial Forces
The P-Delta axial force in each Frame element is determined from the axial displacements computed in the element. For meaningful results, it is important to use
realistic values for the axial stiffness of these elements. The axial stiffness is determined from the Section properties that define the cross-sectional area and the
modulus of elasticity. Using values that are too small may underestimate the
P-Delta effect. Using values that are too large may make the P-Delta force in the element very sensitive to the iteration process.
Elements that have an axial force release, or that are constrained against axial deformation by a Constraint, will have a zero P-Delta axial force and hence no
P-Delta effect.
The P-Delta axial force also includes loads that act within the element itself. These
may include Self-Weight and Gravity Loads, Concentrated and Distributed Span
Loads, Prestress Load, and Temperature Load.
The P-Delta axial force is assumed to be constant over the length of each Frame element. If the P-Delta load combination includes loads that cause the axial force to
vary, then the average axial force is used for computing the P-Delta effect. If the
difference in axial force between the two ends of an element is small compared to
the average axial force, then this approximation is usually reasonable. This would
normally be the case for the columns in a building structure. If the difference is
large, then the element should be divided into many smaller Frame elements wherever the P-Delta effect is important. An example of the latter case could be a flagpole under self-weight.
For more information:
• See Topic “Section Properties” (page 114) in Chapter “The Frame Element.”
• See Topic “End Releases” (page 131) in Chapter “The Frame Element.”
• See Chapter “Constraints and Welds” (page 49).

416

The P-Delta Effect

Chapter XXII

Geometric Nonlinearity

Prestress
When Prestress Load is included in the P-Delta load combination, the combined
tension in the prestressing cables tends to stiffen the Frame elements against transverse deflections. This is true regardless of any axial end releases. Axial compression of the Frame element due to Prestress Load may reduce this stiffening effect,
perhaps to zero.
See Topic “Prestress Load” (page 138) in Chapter “The Frame Element” for more
information.
Directly Specified P-delta Axial Forces
You may directly specify P-delta forces known to be acting on Frame elements.
This is an old-fashioned feature that can be used to model cable structures where
the tensions are large and well-known. No iterative analysis is required to include
the effect of directly specified P-Delta axial forces.
Use of this feature is not usually recommended! The program does not check if the
forces you specify are in equilibrium with any other part of the structure. The directly specified forces apply in all analyses and are in addition to any P-delta affects calculated in a nonlinear analysis.
We recommend instead that you perform a nonlinear analysis including P-delta or
large-displacement effects.
If you use directly specified P-delta forces, you should treat them as if they were a
section property that always affects the behavior of the element.
You can assign directly specified P-Delta force to any Frame element using the following parameters:
• The P-Delta axial force, p
• A fixed coordinate system, csys (the default is zero, indicating the global coordinate system)
• The projection, px, of the P-Delta axial force upon the X axis of csys
• The projection, py, of the P-Delta axial force upon the Y axis of csys
• The projection, pz, of the P-Delta axial force upon the Z axis of csys
Normally only one of the parameters p, px, py, or pz should be given for each
Frame element. If you do choose to specify more than one value, they are additive:

The P-Delta Effect

417

CSI Analysis Reference Manual
P0 = p +

px py pz
+
+
cx c y c z

where P0 is the P-Delta axial force, and cx, cy, and cz are the cosines of the angles between the local 1 axis of the Frame element and the X, Y, and Z axes of coordinate
system csys, respectively. To avoid division by zero, you may not specify the projection upon any axis of csys that is perpendicular to the local 1 axis of the element.
The use of the P-delta axial force projections is convenient, for example, when
specifying the tension in the main cable of a suspension bridge, since the horizontal
component of the tension is usually the same for all elements.
It is important when directly specifying P-Delta axial forces that you include all
significant forces in the structure. The program does not check for equilibrium of
the specified P-Delta axial forces. In a suspension bridge, for example, the cable
tension is supported at the anchorages, and it is usually sufficient to consider the
P-Delta effect only in the main cable (and possibly the towers). On the other hand,
the cable tension in a cable-stayed bridge is taken up by the deck and tower, and it is
usually necessary to consider the P-Delta effect in all three components.

P-Delta Forces in the Link/Support Element
P-delta effects can only be considered in a Link/Support element if there is stiffness
in the axial (U1) degree of freedom to generate an axial force. A transverse displacement in the U2 or U3 direction creates a moment equal to the axial force (P)
times the amount of the deflection (delta).
The total P-delta moment is distributed to the joints as the sum of:
• A pair of equal and opposite shear forces at the two ends that cause a moment
due to the length of the element
• A moment at End I
• A moment at End J
The shear forces act in the same direction as the shear displacement (delta), and the
moments act about the respectively perpendicular bending axes.
For each direction of shear displacement, you can specify three corresponding
fractions that indicate how the total P-delta moment is to be distributed between the
three moments above. These fractions must sum to one.

418

The P-Delta Effect

Chapter XXII

Geometric Nonlinearity

For any element that has zero length, the fraction specified for the shear forces will
be ignored, and the remaining two fractions scaled up so that they sum to one. If
both of these fractions are zero, they will be set to 0.5.
You must consider the physical characteristics of the device being modeled by a
Link/Support element in order to determine what fractions to specify. Long brace
or link objects would normally use the shear force. Short stubby isolators would
normally use moments only. A friction-pendulum isolator would normally take all
the moment on the dish side rather than on the slider side.

Other Elements
For element types other than the Frame and Link/Support, the stresses in the each
element are first determined from the displacements computed in the previous iteration. These stresses are then integrated over the element, with respect to the derivatives of the isoparametric shape functions for that element, to compute a standard
geometric stiffness matrix that represents the P-delta effect. This is added to the
original elastic stiffness matrix of the element. This formulation produces only
forces, no moments, at each joint in the element.
Shell elements that are modeling only plate bending will not produce any P-delta
effects, since no in-plane stresses will be developed.

Initial P-Delta Analysis
For many applications, it is adequate to consider the P-delta effect on the structure
under one set of loads (usually gravity), and to consider all other analyses as linear
using the stiffness matrix developed for this one set of P-delta loads. This enables
all analysis results to be superposed for the purposes of design.
To do this, define a nonlinear static Load Case that has, at least, the following features:
• Set the name to, say, “PDELTA”
• Start from zero initial conditions
• Apply the Load Patterns that will cause the P-delta effect; often this will be
dead load and a fraction of live load
• For geometric nonlinearity, choose P-delta effects
Other parameters include the number of saved steps, the number of iterations allowed per step, and the convergence tolerance. If the P-delta effect is reasonably
Initial P-Delta Analysis

419

CSI Analysis Reference Manual
small, the default values are adequate. We are not considering staged construction
here, although that could be added.
We will refer to this nonlinear static case as the initial P-delta case. You can then
define or modify other linear Load Cases so that they use the stiffness from case
PDELTA:
• Linear static cases
• A modal Load Cases, say called “PDMODES”
• Linear direct-integration time-history cases
• Moving-Load Load Cases
Other linear Load Cases can be defined that are based on the modes from case
PDMODES:
• Response-spectrum cases
• Modal time-history cases
Results from all of these cases are superposable, since they are linear and are based
upon the same stiffness matrix.
You may also want to define a buckling Load Case that applies the same loads as
does case PDELTA, and that starts from zero conditions (not from case PDELTA).
The resulting buckling factors will give you an indication of how far from buckling
are the loads that cause the P-delta effect.
Below are some additional guidelines regarding practical use of the P-Delta analysis option. See also the Software Verification Manual for example problems.

Building Structures
For most building structures, especially tall buildings, the P-Delta effect of most
concern occurs in the columns due to gravity load, including dead and live load.
The column axial forces are compressive, making the structure more flexible
against lateral loads.
Building codes (ACI 2002; AISC 2003) normally recognize two types of P-Delta
effects: the first due to the overall sway of the structure and the second due to the
deformation of the member between its ends. The former effect is often significant;
it can be accounted for fairly accurately by considering the total vertical load at a
story level, which is due to gravity loads and is unaffected by any lateral loads. The
latter effect is significant only in very slender columns or columns bent in single

420

Initial P-Delta Analysis

Chapter XXII

Geometric Nonlinearity

curvature (not the usual case); this requires consideration of axial forces in the
members due to both gravity and lateral loads.
SAP2000 can analyze both of these P-Delta effects. However, it is recommended
that the former effect be accounted for in the SAP2000 analysis, and the latter effect
be accounted for in design by using the applicable building-code moment-magnification factors (White and Hajjar 1991). This is how the SAP2000 design processors
for steel frames and concrete frames are set up.
The P-Delta effect due to the sway of the structure can be accounted for accurately
and efficiently, even if each column is modeled by a single Frame element, by using
the factored dead and live loads in the initial P-delta Load Case. The iterative
P-Delta analysis should converge rapidly, usually requiring few iterations.
As an example, suppose that the building code requires the following load combinations to be considered for design:
(1) 1.4 dead load
(2) 1.2 dead load + 1.6 live load
(3) 1.2 dead load + 0.5 live load + 1.3 wind load
(4) 1.2 dead load + 0.5 live load – 1.3 wind load
(5) 0.9 dead load + 1.3 wind load
(6) 0.9 dead load + 1.3 wind load
For this case, the P-Delta effect due to overall sway of the structure can usually be
accounted for, conservatively, by specifying the load combination in the initial
P-delta Load Case to be 1.2 times the dead load plus 0.5 times the live load. This
will accurately account for this effect in load combinations 3 and 4 above, and will
conservatively account for this effect in load combinations 5 and 6. This P-delta effect is not generally important in load combinations 1 and 2 since there is no lateral
load.
The P-Delta effect due to the deformation of the member between its ends can be
accurately analyzed only when separate nonlinear Load Cases are run for each load
combination above. Six cases would be needed for the example above. Also, at
least two Frame elements per column should be used. Again, it is recommended
that this effect be accounted for instead by using the SAP2000 design features.

Initial P-Delta Analysis

421

CSI Analysis Reference Manual

Cable Structures
The P-Delta effect can be a very important contributor to the stiffness of suspension
bridges, cable-stayed bridges, and other cable structures. The lateral stiffness of cables is due almost entirely to tension, since they are very flexible when unstressed.
In many cable structures, the tension in the cables is due primarily to gravity load,
and it is relatively unaffected by other loads. If this is the case, it is appropriate to
define an initial P-delta Load Case that applies a realistic combination of the dead
load and live load. It is important to use realistic values for the P-delta load combination, since the lateral stiffness of the cables is approximately proportional to the
P-delta axial forces.
P-delta effects are inherent in any nonlinear analysis of Cable elements. P-delta
analysis of the whole structure should be considered if you are concerned about
compression in the tower, or in the deck of a cable-stayed bridge.
Because convergence tends to be slower for stiffening than softening structures, the
nonlinear P-delta analysis may require many iterations. Twenty or more iterations
would not be unusual.

Guyed Towers
In guyed towers and similar structures, the cables are under a large tension produced by mechanical methods that shorten the length of the cables. These structures
can be analyzed by the same methods discussed above for cabled bridges.
A Strain or Deformation load can be used to produce the requisite shortening. The
P-delta load combination should include this load, and may also include other loads
that cause significant axial force in the cables, such as gravity and wind loads. Several analyses may be required to determine the magnitude of the length change
needed to produce the desired amount of cable tension.

Large Displacements
Large-displacements analysis considers the equilibrium equations in the deformed
configuration of the structure. Large displacements and rotations are accounted for,
but strains are assumed to be small. This means that if the position or orientation of
an element changes, its effect upon the structure is accounted for. However, if the
element changes significantly in shape or size, this effect is ignored.

422

Large Displacements

Chapter XXII

Geometric Nonlinearity

The program tracks the position of the element using an updated Lagrangian formulation. For Frame, Shell, and Link/Support elements, rotational degrees of freedom are updated assuming that the change in rotational displacements between
steps is small. This requires that the analysis use smaller steps than might be required for a P-delta analysis. The accuracy of the results of a large-displacement
analysis should be checked by re-running the analysis using a smaller step size and
comparing the results.
Large displacement analysis is also more sensitive to convergence tolerance than is
P-delta analysis. You should always check your results by re-running the analysis
using a smaller convergence tolerance and comparing the results.

Applications
Large-displacement analysis is well suited for the analysis of some cable or membrane structures. Cable structures can be modeled with Frame elements, and membrane structures with full Shell elements (you could also use Plane stress elements).
Be sure to divide the cable or membrane into sufficiently small elements so that the
relative rotations within each element are small.
The catenary Cable element does not require large-displacements analysis. For
most structures with cables, P-delta analysis is sufficient unless you expect significant deflection or rotation of the structure supporting or supported by the cables.
Snap-through buckling problems can be considered using large-displacement analysis. For nonlinear static analysis, this usually requires using displacement control
of the load application. More realistic solutions can be obtained using nonlinear direct-integration time-history analysis.

Initial Large-Displacement Analysis
The discussion in Topic “Initial P-Delta Analysis” (page 419) in this Chapter applies equally well for an initial large-displacement analysis. Define the initial nonlinear static Load Case in the same way, select large-displacement effects instead of
P-delta effects, and make sure the convergence tolerance is small enough. This case
can be used as the basis for all subsequent linear analyses.

Large Displacements

423

CSI Analysis Reference Manual

424

Large Displacements

C h a p t e r XXIII

Nonlinear Static Analysis
Nonlinear static analysis is can be used for a wide variety of purposes, including: to
analyze a structure for material and geometric nonlinearity; to form the P-delta
stiffness for subsequent linear analyses; to investigate staged (incremental) construction with time-dependent material behavior; to perform cable analysis; to perform static pushover analysis; and more.
Although much of this Chapter is advanced, basic knowledge of nonlinear static
analysis is essential for P-delta analysis and modeling of tension-only braces and
cables.
Basic Topics for All Users
• Overview
• Nonlinearity
• Important Considerations
• Loading
• Initial Conditions
• Output Steps

425

CSI Analysis Reference Manual
Advanced Topics
• Load Application Control
• Staged Construction
• Nonlinear Solution Control
• Static Pushover Analysis

Overview
Nonlinear static analysis can be used for many purposes:
• To perform an initial P-delta or large-displacement analysis to get the stiffness
used for subsequent superposable linear analyses
• To perform staged (incremental, segmental) construction analysis, including
material time-dependent effects like aging, creep and shrinkage
• To change the Mass Source to be used for subsequent analyses
• To analyze structures with tension-only bracing
• To analyze cable structures
• To perform static pushover analysis
• To perform snap-through buckling analyses
• To establish the initial conditions for nonlinear direct-integration time-history
analyses
• For any other static analysis that considers the effect of material or geometric
nonlinear behavior
Any number of nonlinear Static Load Cases can be defined. Each case can include
one or more of the features above. In a nonlinear analysis, the stiffness and load
may all depend upon the displacements. This requires an iterative solution to the
equations of equilibrium.

Nonlinearity
The following types of nonlinearity are available in SAP2000:
• Material nonlinearity
– Various type of nonlinear properties in Link/Support elements
– Tension and/or compression limits in Frame elements

426

Overview

Chapter XXIII

Nonlinear Static Analysis

– Plastic hinges in Frame elements
– Nonlinear material behavior in layered Shell elements
• Geometric nonlinearity
– P-delta effects
– Large displacement effects
• Staged construction
– Changes in the structure
– Aging, creep, and shrinkage
All material nonlinearity that has been defined in the model will be considered in a
nonlinear static Load Case.
You have a choice of the type of geometric nonlinearity to be considered:
• None
• P-delta effects
• Large displacement effects
If you are continuing from a previous nonlinear analysis, it is strongly recommended that you select the same geometric nonlinearity parameters for the current
case as for the previous case. See Chapter “Geometric Nonlinearity” (page 409) for
more information.
Staged construction is available as an option. Even if the individual stages are linear, the fact that the structure changes from one stage to the next is considered to be
a type of nonlinearity.

Important Considerations
Nonlinear analysis takes time and patience. Each nonlinear problem is different.
You can expect to need a certain amount of time to learn the best way to approach
each new problem.
Start with a simple model and build up gradually. Make sure the model performs as
expected under linear static loads and modal analysis. Rather than starting with
nonlinear properties everywhere, add them in increments beginning with the areas
where you expect the most nonlinearity.
If you are using frame hinges, start with models that do not lose strength for primary members; you can modify the hinge models later or redesign the structure.
Important Considerations

427

CSI Analysis Reference Manual
When possible, perform your initial analyses without geometric nonlinearity. Add
P-delta effects, and possibly large deformations, much later. Start with modest target displacements and a limited number of steps. In the beginning, the goal should
be to perform the analyses quickly so that you can gain experience with your
model. As your confidence grows with a particular model you can push it further
and consider more extreme nonlinear behavior.
Mathematically, nonlinear static analysis does not always guarantee a unique solution. Inertial effects in dynamic analysis and in the real world limit the path a structure can follow. But this is not true for static analysis, particularly in unstable cases
where strength is lost due to material or geometric nonlinearity. If a nonlinear static
analysis continues to cause difficulties, change it to a direct-integration time-history analysis and apply the load quasi-statically (very slowly.)
Small changes in properties or loading can cause large changes in nonlinear response. For this reason, it is extremely important that you consider many different
loading cases, and that you perform sensitivity studies on the effect of varying the
properties of the structure.

Loading
You may apply any combination of Load Patterns, Acceleration Loads, and modal
loads.
A modal load is a specialized type of loading used for pushover analysis. It is a pattern of forces on the joints that is proportional to the product of a specified mode
shape times its circular frequency squared (w2 ) times the mass tributary to the joint.
The specified combination of loads is applied simultaneously. Normally the loads
are applied incrementally from zero to the full specified magnitude. For specialized
purposes (e.g., pushover or snap-though buckling), you have the option to control
the loading by monitoring a resulting displacement in the structure. See Topic
“Load Application Control” (page 428) in this Chapter for more information.

Load Application Control
You may choose between a load-controlled or displacement-controlled nonlinear
static analysis. For both options, the pattern of loads acting on the structure is determined by the specified combination of loads. Only the scaling is different.

428

Chapter XXIII

Nonlinear Static Analysis

Normally you would choose load control. It is the most common, physical situation.
Displacement control is an advanced feature for specialized purposes.

Load Control
Select load control when you know the magnitude of load that will be applied and
you expect the structure to be able to support that load. An example would be when
applying gravity load, since it is governed by nature.
Under load control, all loads are applied incrementally from zero to the full specified magnitude.

Displacement Control
Select displacement control when you know how far you want the structure to
move, but you don’t know how much load is required. This is most useful for structures that become unstable and may lose load-carrying capacity during the course
of the analysis. Typical applications include static pushover analysis and
snap-through buckling analysis.
To use displacement control, you must select a displacement component to monitor. This may be a single degree of freedom at a joint, or a generalized displacement
that you have previously defined. See Topic “Generalized Displacement” (page 45)
in Chapter “Joints and Degrees of Freedom” for more information.
You must also give the magnitude of the displacement that is your target for the
analysis. The program will attempt to apply the load to reach that displacement.
The load magnitude may be increased and decreased during the analysis.
Be sure to choose a displacement component that monotonically increases during
loading. If this is not possible, you may need to divide the analysis into two or more
sequential cases, changing the monitored displacement in the different cases. The
use of the conjugate displacement control, described below, may help solve this
problem for you.
Important note: Using displacement control is NOT the same thing as applying
displacement loading on the structure! Displacement control is simply used to
MEASURE the displacement at one point that results from the applied loads, and to
adjust the magnitude of the loading in an attempt to reach a certain measured displacement value. The overall displaced shape of the structure will be different for
different patterns of loading, even if the same displacement is controlled.
Load Application Control

429

CSI Analysis Reference Manual
Conjugate Displacement Control
If analysis is having trouble reaching the desired displacement target, you can try
the option for the load case to use the conjugate displacement for control. The
conjugate displacement is a weighted average of all displacements in the structure,
each displacement degree of freedom being weighted by the load acting on that degree of freedom. In other words, it is a measure of the work done by the applied
load.
This option is particularly useful for unsymmetrical buildings where the top story
level may rotate about the vertical axis while being pushed under lateral load. The
rotation could cause the monitored displacement to move backward even while the
weighted average displacement is moving forward.
If you choose to use the conjugate displacement control, it will be used to determine
whether the load should be increased or decreased. The specified monitored displacement will still be used to set the target displacement, i.e., how far the structure
should move. However, this target may not be matched exactly.

Initial Conditions
The initial conditions describe the state of the structure at the beginning of a Load
Case. These include:
• Displacements and velocities
• Internal forces and stresses
• Internal state variables for nonlinear elements
• Energy values for the structure
• External loads
For a static analysis, the velocities are always taken to be zero.
For nonlinear analyses, you may specify the initial conditions at the start of the
analysis. You have two choices:
• Zero initial conditions: the structure has zero displacement and velocity, all elements are unstressed, and there is no history of nonlinear deformation.
• Continue from a previous nonlinear analysis: the displacements, velocities,
stresses, loads, energies, and nonlinear state histories from the end of a previous analysis are carried forward.

430

Initial Conditions

Chapter XXIII

Nonlinear Static Analysis

Nonlinear static and nonlinear direct-integration time-history cases may be chained
together in any combination, i.e., both types of analysis are compatible with each
other. It is strongly recommended that you select the same geometric nonlinearity
parameters for the current case as for the previous case.
When continuing from a previous case, all applied loads specified for the present
Load Case are incremental, i.e., they are added to the loads already acting at the end
of the previous case.
When multiple Mass Sources have been defined, you can specify which Mass
Source to use for a nonlinear static or nonlinear direct-integration time-history load
case. However, the default is to use the same Mass Source as the previous load
case, or the default Mass Source if starting from zero initial conditions. See Topic
“Mass Source” (page 334) in Chapter “Load Patterns” for more information.
Nonlinear static cases cannot be chained together with nonlinear modal time-history (FNA) cases.

Output Steps
Normally, only the final state is saved for a nonlinear static analysis. This is the result after the full load has been applied.
You can choose instead to save intermediate results to see how the structure responded during loading. This is particularly important for static pushover analysis,
where you need to develop the capacity curve.
If you are only interested in the saving the final result, you can skip the rest of this
topic.

Saving Multiple Steps
If you choose to save multiple states, the state at the beginning of the analysis (step
0) will be saved, as well as a number of intermediate states. From a terminology
point of view, saving five steps means the same thing as saving six states (steps 0 to
5): the step is the increment, and the state is the result.
The number of saved steps is determined by the parameters:
• Minimum number of saved steps
• Maximum number of saved steps
• Option to save positive increments only
Output Steps

431

CSI Analysis Reference Manual
These are described in the following.
Minimum and Maximum Saved Steps
The Minimum Number of Saved Steps and Maximum Number of Saved Steps provide control over the number of points actually saved in the analysis. If the minimum number of steps saved is too small, you may not have enough points to adequately represent a pushover curve. If the minimum and maximum number of
saved steps is too large, then the analysis may consume a considerable amount of
disk space, and it may take an excessive amount of time to display results.
The program automatically determines the spacing of steps to be saved as follows.
The maximum step length is equal to total force goal or total displacement goal divided by the specified Minimum Number of Saved Steps. The program starts by
saving steps at this increment. If a significant event occurs at a step length less than
this increment, then the program will save that step too and continue with the maximum increment from there. For example, suppose the Minimum Number of Saved
Steps and Maximum Number of Saved Steps are set at 20 and 30 respectively, and
the target is to be to a displacement of 10 inches. The maximum increment of saved
steps will be 10 / 20 = 0.5 inches. Thus, data is saved at 0.5, 1, 1.5, 2, 2.5 inches.
Suppose that a significant event occurs at 2.7 inches. Then data is also saved at 2.7
inches, and continues on from there being saved at 3.2, 3.7, 4.2, 4.7, 5.2, 5.7, 6.2,
6.7, 7.2, 7.7, 8.2, 8.7, 9.2, 9.7 and 10.0 inches.
The Maximum Number of Saved Steps controls the number of significant events
for which data will be saved. The program will always reach the force or displacement goal within the specified number of maximum saved steps, however, in doing
so it could have to skip saving steps at later events. For example, suppose the Minimum Saved Steps is set to 20, the Maximum Number of Saved Steps is set to 21,
and the pushover is to be to a displacement of 10 inches. The maximum increment
of saved steps will be 10 / 20 = 0.5 inches. Thus, data is saved at 0.5, 1, 1.5, 2, 2.5
inches. Suppose that a significant event occurs at 2.7 inches. Then data is also saved
at 2.7 inches, and continues on from there being saved at 3.2 and 3.7 inches. Suppose another significant event occurs at 3.9 inches. The program will not save the
data at 3.9 inches because if it did it would not be able to limit the maximum increment to 0.5 inches and still get through the full pushover in no more than 21 steps.
Note that if a second significant event occurred at 4.1 inches rather than 3.9 inches,
then the program would be able to save the step and still meet the specified criteria
for maximum increment and maximum number of steps.

432

Output Steps

Chapter XXIII

Nonlinear Static Analysis

Save Positive Increments Only
This option is primarily of interest for pushover analysis under displacement control. In the case of extreme nonlinearity, particularly when a frame hinge sheds
load, the pushover curve may show negative increments in the monitored displacement while the structure is trying to redistribute the force from a failing component.
You may choose whether or not you want to save only the steps having positive increments. The negative increments often make the pushover curve look confusing.
However, seeing them can provide insight into the performance of the analysis and
the structure.
You may want to choose to Save Positive Increments Only in most cases except
when the analysis is having trouble converging.

Nonlinear Solution Control
The specified combination of applied loads is applied incrementally, using as many
steps as necessary to satisfy equilibrium and to produce the requested number of
saved output steps.
The nonlinear equations are solved iteratively in each load step. This may require
re-forming and re-solving the stiffness matrix. The iterations are carried out until
the solution converges. If convergence cannot be achieved, the program divides the
step into smaller substeps and tries again.
Several parameters are available for you to control the iteration and substepping
process. These are described in the following. We recommend that you use the default values of these parameters to start, except that you may often need to increase
the maximum number of total steps and null steps for more complex models.
If you are having convergence difficulties, you may try varying the iteration control
parameters below. However, you should also consider that the model itself may
need improvement. Look for instabilities due to inadequate support, buckling, and
excessively large stiffnesses. If you have hinges or materials that lose strength,
make sure that this behavior is really necessary and that the negative slopes are not
unrealistically too steep.

Nonlinear Solution Control

433

CSI Analysis Reference Manual

Maximum Total Steps
This is the maximum number of steps allowed in the analysis. It may include saved
steps as well as intermediate substeps whose results are not saved. The purpose of
setting this value is to give you control over how long the analysis will run.
Start with a smaller value to get a feel for the time the analysis will take. If an analysis does not reach its target load or displacement before reaching the maximum
number of steps, you can re-run the analysis after increasing this maximum number
of saved steps. The length of time it takes to run a nonlinear static analysis is approximately proportional to the total number of steps.

Maximum Null (Zero) Steps
Null (zero) steps may occur during the nonlinear solution procedure when:
• Iteration does not converge and a smaller step size is attempted
• Snap-back is detected due to strength loss in a frame hinge
An excessive number of null steps may indicate that the solution is stalled due to instability or numerical sensitivity.
You can set the Maximum Null (Zero) Steps so that the solution will terminate
early if it is having trouble converging. Set this value equal to the Maximum Total
Steps if you do not want the analysis to terminate due to null steps.

Event-to-Event Stepping Control
Event-to-event stepping is available as an option for nonlinear static analysis. Using this strategy, an increment of load is applied until one of the nonlinear elements
experiences an “event” that causes a significant change in the stiffness of the structure. Iteration is performed for this load increment to ensure that equilibrium is
achieved to within a specified convergence tolerance. The stiffness matrix is then
reformed, and another load increment is applied to reach the next event. This continues in a series of event steps until the entire load has been applied.
Events are implemented for the following nonlinear models: all frame hinges; layered shells with directional or coupled nonlinear behavior; and links with multi-linear plasticity, gap, hook, friction-pendulum, and triple-pendulum behavior. Events
typically include first yield, unloading, strength loss, increasing stiffness, and other
significant changes in behavior that depend on the type of element or material.

434

Nonlinear Solution Control

Chapter XXIII

Nonlinear Static Analysis

You can specify whether or not to use event-to-event stepping. When events are
used, each load increment tends to be more linear, thus reducing equilibrium unbalance and lessening the need for iteration. On the other hand, models with a large
number of nonlinear elements and/or hinges may generate a large number of
events, which can significantly increase the analysis time.
When using event stepping, you can specify a relative event-lumping tolerance that
will group multiple events together. Effectively, the load increment calculated to
reach the first event is increased by the tolerance to include other events that would
occur soon afterward. Larger event tolerances reduce the number of event steps
taken, but may increase the amount of iteration required.
Note that for isotropic frame hinges the event lumping tolerance may also allow the
force or deformation response to deviate from the backbone curve. The relative
magnitude of the deviations is on the order of the relative lumping tolerance.
Whether or not to use event stepping is a problem-dependent decision. Normally
using events will improve convergence behavior. However, if a large number of
event steps are generated that make the analysis run slowly, try turning event-stepping off for that model or load case. Either way, results for a stable model should be
consistent to within the convergence tolerance.
Nonlinear iteration is always used for nonlinear static analysis, whether or not
event-stepping is used. This is different from nonlinear direct-integration time-history analysis where events can be used with or without iteration. Note that the
line-search iteration option is not available when event stepping is used for
nonlinear static analysis.

Nonlinear Iteration
Iteration is used to ensure that equilibrium is achieved at each step and substep of
the analysis to within a specified convergence tolerance. You can specify the relative convergence tolerance used to compare the magnitude of force error with the
magnitude of the force acting on the structure.
You may need to use significantly smaller values of convergence tolerance to get
good results for large-displacements problems than for other types of nonlinearity.
Try decreasing this value until you get consistent results.
For each step, constant-stiffness iteration is tried first. If convergence is not
achieved, Newton-Raphson (tangent-stiffness) iteration is tried next. If both fail,
the step size is reduced, and the process is repeated.

Nonlinear Solution Control

435

CSI Analysis Reference Manual
You can separately control the number of constant-stiffness and Newton-Raphson
iterations allowed in each step. Setting either parameter to zero prevents that type
of iteration. Setting both to zero causes the analysis to use the default number of iterations. Constant-stiffness iterations are faster than Newton-Raphson iterations,
but the latter are usually more effective, especially for cables and geometric
nonlinearity. The default values work well in many situations.

Line Search Option
Line search is an iteration option that can increase the efficiency of equilibrium iterations by scaling the solution increment in a trial-and-error fashion to find the
smallest unbalance. This increases the computation time for each iteration, but often results in fewer iterations and better convergence behavior, with a net gain in efficiency. Line search is particularly effective for stiffening systems, such as tightening cables, closing gaps, unloading from plastic yielding, and sticking after
frictional sliding.
You can choose whether or not to use line search, except that line search is not
available when using event-to-event stepping. Line search is also not used for displacement-controlled load cases.
When using line search, specify the following parameters:
• Maximum number of line searches per Iteration. Use this parameter to limit
the number of line searches allowed per iteration, usually in the range of 5
to 40.
• Line-Search Acceptance Tolerance (Relative). The solution increment is
successively reduced or increased until the minimum error is found, the
maximum number of line searches is reached, or the relative change in error from the previous trial is less than the acceptance tolerance set here.
The practical range is about 0.02 to 0.50. This value should not be too
small, since the goal is only to improve the next iteration.
• Line-Search Step Factor. For each line-search trial, the solution increment
is successively reduced by the step factor specified here until the minimum
error is found, the maximum number of line searches is reached, or the acceptance tolerance is satisfied. If reducing the increment does not decrease
the error, the increment is instead increased by the step factor following the
same procedure. This factor must be greater than 1.0, and should usually be
no more than 2.0.

436

Nonlinear Solution Control

Chapter XXIII

Nonlinear Static Analysis

The default values are recommended as starting point. For stiffening systems that
are slow to converge, try increasing the maximum number of line searches per iteration, decreasing the acceptance tolerance, and reducing the step factor.

Static Pushover Analysis
Nonlinear static pushover analysis is a specialized procedure used in performance-based design for seismic loading. SAP2000 provides the following tools
needed for pushover analysis:
• Material nonlinearity at discrete, user-defined hinges in Frame elements. The
hinge properties were created with pushover analysis in mind. Default hinge
properties are provided based on ASCE 41and other code-based criteria. See
Chapter “Frame Hinge Properties” (page 147). In ETABS, discrete fiber P-M3
hinges can be assigned to wall elements.
• Nonlinear static analysis procedures specially designed to handle the sharp
drop-off in load carrying capacity typical of frame hinges used in pushover
analysis.
• Nonlinear static analysis procedures that allow displacement control, so that
unstable structures can be pushed to desired displacement targets. See Topic
“Load Application Control” (page 428) in this Chapter.
• Display capabilities in the graphical user interface to generate and plot pushover curves, including demand and capacity curves in spectral ordinates. See
the online Help facility in the graphical user interface for more information.
• Capabilities in the graphical user interface to plot and output the state of every
hinge at each step in the pushover analysis. See Chapter “Frame Hinge Properties” (page 147) and the online Help facility in the graphical user interface for
more information.
In addition to these specialized features, the full nonlinearity of the program can be
used, in clud ing non lin ear Shell and Link/Sup port be hav ior, geo met ric
nonlinearity, and staged construction. In addition, you are not restricted to static
pushover analysis: you can also perform full nonlinear time-history analysis.
The following general sequence of steps is involved in performing nonlinear static
pushover analysis using SAP2000:
1. Create a model just like you would for any other analysis.
2. Define frame hinge properties and assign them to the frame elements.

Static Pushover Analysis

437

CSI Analysis Reference Manual
3. Define any Load Patterns and static and dynamic Load Cases that may be
needed for steel or concrete design of the frame elements, particularly if default
hinges are used.
4. Run the Load Cases needed for design.
5. If any concrete hinge properties are based on default values to be computed by
the program, you must perform concrete design so that reinforcing steel is determined.
6. If any steel hinge properties are based on default values to be computed by the
program for Auto-Select frame section properties, you must perform steel design and accept the sections chosen by the program.
7. Define the Load Patterns that are needed for use in the pushover analysis,
including:
• Gravity loads and other loads that may be acting on the structure before the
lateral seismic loads are applied. You may have already defined these Load
Patterns above for design.
• Lateral loads that will be used to push the structure. If you are going to use
Acceleration Loads or modal loads, you don’t need any new Load Patterns,
although modal loads require you to define a Modal Load Case.
8. Define the nonlinear static Load Cases to be used for pushover analysis, including:
• A sequence of one or more cases that start from zero and apply gravity and
other fixed loads using load control. These cases can include staged construction and geometric nonlinearity.
• One or more pushover cases that start from this sequence and apply lateral
pushover loads. These loads should be applied under displacement control.
The monitored displacement is usually at the top of the structure and will
be used to plot the pushover curve.
9. Run the pushover Load Cases.
10. Review the pushover results: Plot the pushover curve, the deflected shape
showing the hinge states, force and moment plots, and print or display any
other results you need.
11. Revise the model as necessary and repeat.

438

Static Pushover Analysis

Chapter XXIII

Nonlinear Static Analysis

It is important that you consider several different lateral pushover cases to represent
different sequences of response that could occur during dynamic loading. In particular, you should push the structure in both the X and Y directions, and possibly at
angles in between. For non-symmetrical structures, pushing in the positive and
negative direction may yield different results. When pushing in a given direction,
you may want to consider different vertical distributions of the lateral load, such as
the first and second mode in that direction.

Staged Construction
Staged construction is a special type of nonlinear static analysis that requires a separate add-on module for this feature to become available in the program.
Staged construction allows you to define a sequence of stages wherein you can add
or remove portions of the structure, selectively apply load to portions of the structure, and to consider time-dependent material behavior such as aging, creep, and
shrinkage. Staged construction is variously known as incremental construction, sequential construction, or segmental construction.
Normally the program analyzes the whole structure in all Load Cases. If you do not
want to perform staged-construction analysis, you can skip the rest of this topic.
Staged construction is considered a type of nonlinear static analysis because the
structure may change during the course of the analysis. However, consideration of
material and geometric nonlinearity is optional. Because staged construction is a
type of nonlinear static analysis, it may be part of a sequence of other nonlinear
static and direct-integration time-history Load Cases, and it may also be used as a
stiffness basis for linear Load Cases.
If you continue any nonlinear analysis from a staged construction analysis, or perform a linear analysis using its stiffness, only the structure as built at the end of the
staged construction will be used.

Stages
For each nonlinear staged-construction Load Case, you define a sequence of stages.
These are analyzed in the order defined. You can specify as many stages as you
want in a single Load Case. Staged construction can also continue from one Load
Case to another.
For each stage you specify the following:

Staged Construction

439

CSI Analysis Reference Manual
• A duration, in days. This is used for time-dependent effects. If you do not want
to consider time-dependent effects in a given stage, set the duration to zero.
• Any number of objects to be added to the structure, or none. The age of the objects at the time they are added can be specified, if time-dependent effects are to
be considered.
• Any number of objects to be removed from the structure, or none
• Any number of objects to be loaded by specified Load Patterns, or none. You
may specify that all objects in the group are to be loaded, or only those objects
in the group that are being added to the structure in this stage.
• Property-Modifier Named Sets may be assigned to any number of frame or
shell objects. See Chapters “The Frame Element” and “The Shell Element” for
more information.
• End-Release Named Sets may be assigned to any number of frame objects. See
Chapter “The Frame Element” for more information.
• Section properties may be changed for any number of frame, shell, tendon, and
link/support objects.
• Bridge superstructure girders may be flagged as composite or non-composite
for design purposes. By default, they are non-composite. This option is available only in CSiBridge, and only for bridge groups that contain top-slab
components. This flag in only used in bridge superstructure design checks for
constructability. It has absolutely no effect upon analysis.
Objects may be specified individually or by using groups, including specialized
groups such as ETABS building stories or CSiBridge superstructure segments. In
most cases, the use of groups is convenient, so the first step to setting up
staged-construction analysis is to define groups for that purpose. See Topic
“Groups” (page 9) in Chapter “Objects and Elements” for more information. Note
that there is always a built-in group called "ALL" that includes the whole structure.
When an operation only pertains to some object types, only objects of those types
in a group will be affected.
When you specify staged construction, the analysis starts with the structure as built
from the previous Load Case. If you are starting from zero, then the structure starts
with no objects.
Each stage is analyzed separately in the order the stages are defined. The analysis of
a stage has two parts:

440

Staged Construction

Chapter XXIII

Nonlinear Static Analysis

(1) Changes to the structure and application of loads are analyzed. These occur instantaneously in time, i.e., the analysis may be incremental, but no time elapses
from the point-of-view of the material
(2) If non-zero duration has been specified, time-dependent material effects are
then analyzed. During this time, the structure does not change and applied
loads are held constant. However, internal stress redistribution may occur.
The instantaneous part (1) of the stage is analyzed as follows (reference to groups
includes individual objects as well):
• The objects to be added, if any, are processed. Only new objects in the specified
groups (not already present in the structure) are added. For each non-joint object added, all joints connected to that object are also added, even if they are not
explicitly included in the group.
• The groups to be removed, if any, are processed. Only objects actually present
in the structure are removed. When objects are removed, their stiffness, mass,
loads, and internal forces are removed from the structure and replaced with
equivalent forces. These forces are linearly reduced to zero during the course of
the analysis. Joints that were automatically added will be removed when all
connected objects are removed.
• Section properties changes, if any, are processed as described below.
• Named set assignments, if any, are processed.
• All specified loads will be increased linearly during the course of the analysis.
Loads specified on all objects in a group will only be applied to objects that are
actually present in the structure or are being added in this stage. Loads specified on added objects in a group will only be applied to objects that are being
added in this stage.
If an object is included in more than one group that is being added or removed, the
object will only be added or removed once. Whether it is added or removed depends on which operation occurs last in the order you have specified them. For example, if an object is included in three groups that are being added and one group
that is being removed, the object will be removed if that was the last operation specified for that stage. Changing section properties acts as a removal and addition, and
it will occur in sequence with explicit addition and removal depending on the order
of operations you specify. See below for more information.
If an object is included in more than one group that is being loaded, the object will
be multiply loaded.
Load application must be by load control. Displacement control is not allowed.
Staged Construction

441

CSI Analysis Reference Manual

Changing Section Properties
The main purpose for changing section properties is to be able to model multiple
configurations of the same structure. This can be accomplished changing the properties of newly added, unstressed objects. You may, however, change section properties for stressed objects, and it is important that you understand exactly what the
analysis is doing so that you can achieve the results you want.
Section property changes on each object are processed as follows:
• If the object is present, it is removed and replaced with equivalent forces so that
the structure does not deflect.
• The object is added again, this time with the new section property, but unstressed and without any loading that may have been acting on the object when
it was removed. The object will be added even if it was not previously present
in the structure.
• The equivalent forces, if any, are then reversed. This will usually deform the
object and cause the structure will deflect.
You would normally want to reapply self-weight to any object whose section properties are changed, since previous loading is discarded.
This operation is essentially removing a stressed object and replacing it with an unstressed object. You can apply forces to unload the object before changing its section if you want to simulate removing an unstressed object.
Changing section properties is useful for analysis purposes. However, the object
will be treated as if it has its original section property for all display, output, and design purposes.

Output Steps
The specification of output steps is similar to that described earlier in this Chapter
in Topic “Output Steps” (page 431), except that you can individually control the
number of steps to be saved for the two parts of each stage:
(1) How many steps to save during changes to the structure and instantaneous application of load
(2) How many steps to save during the time-dependent analysis for aging, creep
and shrinkage.

442

Staged Construction

Chapter XXIII

Nonlinear Static Analysis

The number of steps requested for these two parts of each stage applies equally to
all stages in the Load Case.
Important! The time step used for the time-dependent analysis is based on the
number of steps saved. For statically indeterminate structures where significant
stress redistribution may occur due to creep and shrinkage, it is important to use
small-enough time steps, especially during the youth of the structure where large
changes may be occurring. You may want to re-run the analysis with increasing
numbers of steps saved until you are satisfied that the results have converged.

Example
Let’s build a simple bridge. Define four groups: “BENTS,” “DECK1,” “DECK2,”
“SHORING,” and “APPURTS.” The structure can be linear or nonlinear. Time-dependent properties are assumed for the concrete material.
Also define three Load Patterns:
• “GRAVITY”, to apply dead load
• “TENSION”, to apply post-tensioning cable loads
• “EQUIPMENT”, to apply the weight of temporary construction equipment on
the deck
Define a staged-construction Load Case called “BUILD” that starts from zero, and
contains the following stages:
1. a) Add group “BENTS” with an age of 10 days.
b) Apply load “GRAVITY” to added elements in group “ALL”.
c) No time-dependent effects need to be considered—we can assume these already happened in the first 10 days.
2. a) Add group “SHORING” with an age of 10 days.
b) Apply load “GRAVITY” to added elements in group “ALL”.
c) No time-dependent effects need to be considered for the shoring.
3. a) Add group “DECK1” with an age of 0 days (wet concrete).
b) Apply load “GRAVITY” to added elements in group “ALL”.
c) Apply load “EQUIPMENT” to all elements in group “DECK1”.
d) Allow 3 days duration for aging, creep, and shrinkage.
4. a) Add group “DECK2” with an age of 0 days (wet concrete).
b) Apply load “GRAVITY” to added elements in group “ALL”.
c) Remove load “EQUIPMENT” from all elements in group “DECK1” (apply
Staged Construction

443

CSI Analysis Reference Manual
with a scale factor of -1.0).
d) Apply load “EQUIPMENT” to all elements in group “DECK2”.
e) Allow 3 days duration for aging, creep, and shrinkage.
5. a) Remove load “EQUIPMENT” from all elements in group “DECK2” (apply
with a scale factor of -1.0).
b) Apply load “TENSION” to all elements in group “ALL”.
4. a) Remove group “SHORING”.
b) Allow 3 days duration for aging, creep, and shrinkage.
5. a) Add group “APPURTS” with an age of 10 days.
b) Allow 30 days duration for aging, creep, and shrinkage.
6. a) Allow 300 days duration for aging, creep, and shrinkage.
7. a) Allow 3000 days duration for aging, creep, and shrinkage.
The reason for adding several stages with increasing length of time at the end is to
get long term effects at increasing time-step size, since the number of output steps is
the same for all stages.
Case BUILD can now be used to define the stiffness matrix for any number of linear analyses, including modal, response-spectrum, moving-load, and other types.
You can also continue case BUILD with a nonlinear direct-integration time-history
analysis for seismic load, or even more nonlinear static cases that may include
pushover analysis or more staged construction for the purposes of retrofit.

Target-Force Iteration
When any Load Pattern containing target-force loads is applied in a nonlinear static
Load Case, internal deformation load is iteratively applied to achieve the target
force. In a staged-construction analysis, the iteration occurs individually over any
stage for which target-force loads are applied. Otherwise, the iteration is for the
whole nonlinear static Load Case.
Trial deformation loads are applied to those elements for which target forces have
been assigned, and a complete nonlinear analysis (or stage thereof) is performed.
At the end of the analysis, and assuming that convergence for equilibrium has been
achieved, forces in the targeted elements are compared with their desired targets. A
relative error is computed that is the root-mean-square over all the elements of the
difference between the target and the actual force, divided by the larger of the two
values. If this error is greater than the relative convergence tolerance that you speci-

444

Target-Force Iteration

Chapter XXIII

Nonlinear Static Analysis

fied, a revised deformation load is computed and the complete nonlinear analysis
(or stage thereof) is performed again. This process is repeated until the error is less
than the tolerance, or the specified maximum number of iterations is reached.
As part of the definition of the nonlinear static Load Case, you may specify the following parameters to control target-force iteration:
• Relative convergence tolerance: This is the error you are willing to accept in
the target forces. Since target forces represent your desire, and not a natural requirement like equilibrium, a large value such as 0.01 to 0.10 is recommended.
• Maximum number of iterations: Many iterations may be required for some
structures, and each iteration may take some time. Start with a moderate value,
such as 5 to 10, and increase it as necessary.
• Acceleration factor: The difference between the target force and the force actually achieved is converted to deformation load and applied in the next iteration.
You can increase or decrease this load by the acceleration factor. Use a value
greater than one if conference is slow, such as when pulling or pushing against
a flexible structure. Use a value less than one if the solution is diverging, i.e.,
the unbalance is growing or oscillating between iterations.
• Whether to continue the analysis if convergence is not achieved: Since achieving the target forces is not a natural requirement, and may not even be possible,
you may want to continue the analysis even if the target is not reached.
You should be realistic in your expectations for target-force iteration. You cannot
arbitrarily specify the forces in a statically determinate structure, such as a truss.
Convergence will be slow when target forces are specified in elements connected to
very flexible supports, or that act against other target-force elements. Best results
will be obtained in stiff, redundant structures.
Target-force loads can be applied at the same time as other loads. However, better
convergence behavior may be obtained by applying target-force loads in a separate
stage or Load Case when this is possible.
For more information:
• See Topic “Target-Force Load” (page 142) in Chapter “The Frame Element.”
• See Topic “Target-Force Load” (page 174) in Chapter “The Cable Element.”
• See Topic “Target-Force Load” (page 331) in Chapter “Load Patterns.”

Target-Force Iteration

445

CSI Analysis Reference Manual

446

Target-Force Iteration

C h a p t e r XXIV

Nonlinear Time-History Analysis
Time-history analysis is a step-by-step analysis of the dynamical response of a
structure to a specified loading that may vary with time. The analysis may be linear
or nonlinear. The Chapter describes concepts that apply only to nonlinear time-history analysis. You should first read Chapter “Linear Time-History Analysis” (page
397) which describes concepts that apply to all time-history analyses.
Advanced Topics
• Overview
• Nonlinearity
• Loading
• Initial Conditions
• Time Steps
• Nonlinear Modal Time-History Analysis (FNA)
• Nonlinear Direct-Integration Time-History Analysis

447

CSI Analysis Reference Manual

Overview
Time-history analysis is used to determine the dynamic response of a structure to
arbitrary loading. The dynamic equilibrium equations to be solved are given by:
K u( t ) + C u&( t ) + M u&&( t ) = r ( t )
where K is the stiffness matrix; C is the damping matrix; M is the diagonal mass
& and u&& are the displacements, velocities, and accelerations of the strucmatrix; u, u,
ture; and r is the applied load. If the load includes ground acceleration, the
displacements, velocities, and accelerations are relative to this ground motion.
Any number of time-history Load Cases can be defined. Each time-history case can
differ in the load applied and in the type of analysis to be performed.
There are several options that determine the type of time-history analysis to be performed:
• Linear vs. Nonlinear.
• Modal vs. Direct-integration: These are two different solution methods, each
with advantages and disadvantages. Under ideal circumstances, both methods
should yield the same results to a given problem.
• Transient vs. Periodic: Transient analysis considers the applied load as a
one-time event, with a beginning and end. Periodic analysis considers the load
to repeat indefinitely, with all transient response damped out.
In a nonlinear analysis, the stiffness, damping, and load may all depend upon the
displacements, velocities, and time. This requires an iterative solution to the equations of motion.
Before reading this Chapter on nonlinear analysis, you should first read Chapter
“Linear Time-History Analysis” (page 397) which describes concepts that apply to
all time-history analyses

448

Overview

Chapter XXIV

Nonlinear Time-History Analysis

– Hinges in Frame elements
– Geometric nonlinearity in Cable elements
– Material nonlinearity in layered Shell elements
• Geometric nonlinearity
– P-delta effects
– Large displacement effects
For nonlinear direct-integration time-history analysis, all of the available
nonlinearities may be considered.
For nonlinear modal time-history analysis, only the nonlinear behavior of the
Link/Support elements is included. If the modes used for this analysis were computed using the stiffness from the end of a nonlinear load case, all other types of
nonlinearities are locked into the state that existed at the end of that nonlinear load
case.

Loading
The application of load for nonlinear time-history analysis is identical to that used
for linear time-history analysis. Please see Topic “Loading” (page 398) in Chapter
“Linear Time-History Analysis” for more information.

449

CSI Analysis Reference Manual
• Zero initial conditions: the structure has zero displacement and velocity, all elements are unstressed, and there is no history of nonlinear deformation.
• Continue from a previous nonlinear analysis: the displacements, velocities,
stresses, loads, energies, and nonlinear state histories from the end of a previous analysis are carried forward.
There are some restrictions when continuing from a previous nonlinear case:
• Nonlinear static and nonlinear direct-integration time-history cases may be
chained together in any combination, i.e., both types of analysis are compatible
with each other.
• Nonlinear modal time-history (FNA) cases can only continue from other FNA
cases that use modes from the same modal Load Case.
When continuing from a previous case, all applied loads specified for the present
Load Case are incremental, i.e., they are added to the loads already acting at the end
of the previous case.
When performing a nonlinear time-history analysis, such as for earthquake loading, it is often necessary to start from a nonlinear static state, such as due to gravity
loading. For nonlinear direct-integration analysis, you can continue from a nonlinear static Load Case. But since FNA analyses can only continue from other FNA
cases, special consideration must be given to how to model static loading using
FNA. See Topic “Nonlinear Modal Time-History Analysis (FNA)” (page 149) for
more information.
Note that, by contrast, linear time-history analyses always start from zero initial
conditions.

Time Steps
The choice of output time steps is the same for linear and nonlinear time-history
analysis. Please see Topic “Time Steps” (page 402) in Chapter “Linear Time-History Analysis” for more information.
The nonlinear analysis will internally solve the equations of motion at each output
time step and at each load function time step, just as for linear analysis. In addition,
you may specify a maximum substep size that is smaller than the output time step in
order to reduce the amount of nonlinear iteration, and also to increase the accuracy
of direct-integration analysis. The program may also choose smaller substeps sizes
automatically when it detects slow convergence.

450

Time Steps

Chapter XXIV

Nonlinear Time-History Analysis

Nonlinear Modal Time-History Analysis (FNA)
The method of nonlinear time-history analysis used in SAP2000 is an extension of
the Fast Nonlinear Analysis (FNA) method developed by Wilson (Ibrahimbegovic
and Wilson, 1989; Wilson, 1993). The method is extremely efficient, particularly
for structural systems which are primarily linear elastic but which have a limited
number of predefined nonlinear elements. However, there is no limit on the number
of nonlinear elements that can be considered, provided that adequate modes are obtained. This is best done using a sufficient number of Ritz vectors.
For the FNA method, all nonlinearity is restricted to the Link/Support elements.
This includes hinges that are modeled as Links, as described in Topic “Analysis
Modeling” (page 161) of Chapter “Hinge Properties”.
A short description of the method follows. The dynamic equilibrium equations of a
linear elastic structure with predefined nonlinear Link/Support elements subjected
to an arbitrary load can be written as:
K L u( t ) + C u&( t ) + M u&&( t ) + r N ( t ) = r ( t )
where K L is the stiffness matrix for the linear elastic elements (all elements except
the Links/Supports); C is the proportional damping matrix; M is the diagonal mass
matrix; r N is the vector of forces from the nonlinear degrees of freedom in the
& and u&& are the relative displacements, velocities, and
Link/Support elements; u, u,
accelerations with respect to the ground; and r is the vector of applied loads. See
Topic “Loading” (page 398) in Chapter “Linear Time-History Analysis” for the
definition of r.

Initial Conditions
See Topic “Initial Conditions” (page 149) in this Chapter for a general discussion
of initial conditions.
Because FNA analyses can only continue from other FNA analyses, special consideration must be given to how you can model static loads that may act on the structure prior to a dynamic analysis.
It is actually very simple to perform static analysis using FNA. The load is applied
quasi-statically (very slowly) with high damping. To define a quasi-static FNA
analysis:
• Define a ramp-type time-history function that increases linearly from zero to
one over a length of time that is long (say ten times) compared to the first period
Nonlinear Modal Time-History Analysis (FNA)

451

CSI Analysis Reference Manual
of the structure, and then holds constant for an equal length of time. Call this
function “RAMPQS”
• Define a nonlinear modal time-history (FNA) case:
– Call this case “HISTQS”
– Start from zero or another FNA case
– Apply the desired Load Pattern(s) using function “RAMPQS”
– Use as few or as many time steps as you wish, but make sure the total time
is at least twice the ramp-up time of function “RAMPQS”
– Use high modal damping, say 0.99
You can use case “HISTQS” as the initial conditions for other FNA cases.
This approach is particularly useful for nonlinear analysis where the behavior of
certain Link/Support elements, especially the Gap, Hook and Friction types, is
strongly dependent on the total force or displacement acting on the elements.

Link/Support Effective Stiffness
For the purposes of analysis, a linear effective stiffness is defined for each degree
of freedom of the nonlinear elements. The effective stiffness at nonlinear degrees of
freedom is arbitrary, but generally varies between zero and the maximum nonlinear
stiffness of that degree of freedom.
The equilibrium equation can then be rewritten as:
K u( t ) + C u&( t ) + M u&&( t ) = r ( t ) - [ r N ( t ) - K N u( t ) ]
where K = K L + K N , with K L being the stiffness of all the linear elements and for
the linear degrees of freedom of the Link/Support elements, and K N being the linear effective-stiffness matrix for all of the nonlinear degrees of freedom.
See Chapter “The Link/Support Element—Basic” (page 251) for more information.

Mode Superposition
Modal analysis is performed using the full stiffness matrix, K, and the mass matrix,
M. It is strongly recommended that the Ritz-vector method be used to perform the
modal analysis.

452

Nonlinear Modal Time-History Analysis (FNA)

Chapter XXIV

Nonlinear Time-History Analysis

Using standard techniques, the equilibrium equation can be written in modal form
as:
W 2 a ( t ) + L a&( t ) + I a&&( t ) = q ( t ) - q N ( t )
where W 2 is the diagonal matrix of squared structural frequencies given by:
W2 =F T K F
L is the modal damping matrix which is assumed to be diagonal:
L =F T C F
I is the identity matrix which satisfies:
I =F

q( t ) is the vector of modal applied loads:
q( t ) = F

r (t)

q N ( t ) is the vector of modal forces from the nonlinear elements:
q N (t) = F

[ r N ( t ) - K N u( t ) ]

a( t ) is the vector of modal displacement amplitudes such that:
u( t ) = F a ( t )
and F is the matrix of mode shapes.
It should be noted that, unlike linear dynamic analysis, the above modal equations
are coupled. In general the nonlinear forces, q N ( t ), will couple the modes since
they are functions of the modal displacements, a( t ).
It is important to recognize that the solution to these modal equations is dependent
on being able to adequately represent the nonlinear forces by the modal forces,
q N ( t ). This is not automatic, but requires the following special considerations:
• Mass and/or mass moments of inertia should be present at all nonlinear degrees
of freedom.
• The Ritz-vector method should be used to determine the Modes, unless all possible structural Modes are found using eigenvector analysis

Nonlinear Modal Time-History Analysis (FNA)

453

CSI Analysis Reference Manual
• The Ritz starting load vectors should include a nonlinear deformation load for
each independent nonlinear degree of freedom
• A sufficient number of Ritz-vectors should be sought to capture the deformation in the nonlinear elements completely
For more information:
• See Topic “Ritz-Vector Analysis” (page 349) in Chapter “Modal Analysis”.
• See Chapter “The Link/Support Element—Basic” (page 251).

Modal Damping
As for linear modal time-history analysis, the damping in the structure is modeled
using uncoupled modal damping. Each mode has a damping ratio, damp, which is
measured as a fraction of critical damping and must satisfy:
0 £ damp < 1
Modal damping has two different sources, which are described in the following.
Damping from these sources is added together. The program automatically makes
sure that the total is less than one.
Important note: For linear modal time-history analysis, the linear effective damping for the Link/Support elements is also used. However, it is not used for nonlinear
modal time-history analysis.
Modal Damping from the Load Case
For each nonlinear modal time-history Load Case, you may specify modal damping
ratios that are:
• Constant for all modes
• Linearly interpolated by period or frequency. You specify the damping ratio at
a series of frequency or period points. Between specified points the damping is
linearly interpolated. Outside the specified range, the damping ratio is constant
at the value given for the closest specified point.
• Mass and stiffness proportional. This mimics the proportional damping used
for direct-integration, except that the damping value is never allowed to exceed
unity.

454

Nonlinear Modal Time-History Analysis (FNA)

Chapter XXIV

Nonlinear Time-History Analysis

In addition, you may optionally specify damping overwrites. These are specific
values of damping to be used for specific modes that replace the damping obtained
by one of the methods above. The use of damping overwrites is rarely necessary.
It is also important to note that the assumption of modal damping is being made
with respect to the total stiffness matrix, K, which includes the effective stiffness
from the nonlinear elements. If non-zero modal damping is to be used, then the effective stiffness specified for these elements is important. The effective stiffness
should be selected such that the modes for which these damping values are specified are realistic.
In general it is recommended that either the initial stiffness of the element be used
as the effective stiffness or the secant stiffness obtained from tests at the expected
value of the maximum displacement be used. Initially-open gap and hook elements
and all damper elements should generally be specified with zero effective stiffness.
Composite Modal Damping from the Materials
Modal damping ratios, if any, that have been specified for the Materials are converted automatically to composite modal damping. Any cross coupling between the
modes is ignored. These modal-damping values will generally be different for each
mode, depending upon how much deformation each mode causes in the elements
composed of the different Materials.

Iterative Solution
The nonlinear modal equations are solved iteratively in each time step. The program assumes that the right-hand sides of the equations vary linearly during a time
step, and uses exact, closed-form integration to solve these equations in each iteration. The iterations are carried out until the solution converges. If convergence cannot be achieved, the program divides the time step into smaller substeps and tries
again.
Several parameters are available for you to control the iteration process. In general,
the use of the default values is recommended since this will solve most problems. If
convergence cannot be achieved, inaccurate results are obtained, or the solution
takes too long, changing these control parameters may help. However, you should
first check that reasonable loads and properties have been specified, and that appropriate Modes have been obtained, preferably using the Ritz vector method.
The parameters that are available to control iteration and substepping are:
• The relative force convergence tolerance, ftol
Nonlinear Modal Time-History Analysis (FNA)

455

CSI Analysis Reference Manual
• The relative energy convergence tolerance, etol
• The maximum allowed substep size, dtmax
• The minimum allowed substep size, dtmin
• The maximum number of force iterations permitted for small substeps, itmax
• The maximum number of force iterations permitted for large substeps, itmin
• The convergence factor, cf
These parameters are used in the iteration and substepping algorithm as described
in the following.
Force Convergence Check
Each time step of length dt is divided into substeps as needed to achieve convergence. In each substep, the solution is iterated until the change in the right-hand
side of the modal equations, expressed as a fraction of the right-hand side, becomes
less than the force tolerance, ftol. If this does not occur within the permitted number
of iterations, the substep size is halved and the iteration is tried again.
-5

The default value for ftol is 10 . It must satisfy ftol > 0.
Energy Convergence Check
If force convergence occurs within the permitted number of iterations, the work
done by the nonlinear forces is compared with the work done by all the other force
terms in the modal equilibrium equations. If the difference, expressed as a fraction
of the total work done, is greater than the energy tolerance, etol, the substep size is
halved and the iteration is tried again.
This energy check essentially measures how close to linear is the variation of the
nonlinear force over the time step. It is particularly useful for detecting sudden
changes in nonlinear behavior, such as the opening and closing of gaps or the onset
of yielding and slipping. Setting etol greater than unity turns off this energy check.
The default value for etol is 10-5. It must satisfy etol > 0.
Maximum and Minimum Substep Sizes
If the substep meets both the force and energy convergence criteria, the results of
the substep are accepted, and the next substep is attempted using twice the previous
substep length. The substep size is never increased beyond dtmax.

456

Nonlinear Modal Time-History Analysis (FNA)

Chapter XXIV

Nonlinear Time-History Analysis

When the substep size is halved because of failure to meet either the force or energy
convergence criteria, the resulting substep size will never be set less than dtmin. If
the failed substep size is already dtmin, the results for the remaining time steps in
the current History are set to zero and a warning message is issued.
The default value for dtmax is dt. The default value for dtmin is dtmax·10-9. They
must satisfy 0 < dtmin £ dtmax £ dt.
Maximum Number of Iterations
The maximum number of iterations permitted for force iteration varies between
itmin and itmax. The actual number permitted for a given substep is chosen automatically by the program to achieve a balance between iteration and substepping.
The number of iterations permitted tends to be larger for smaller substeps.
The default values for itmin and itmax are 2 and 100, respectively. They must satisfy 2 £ itmin £ itmax.
Convergence Factor
Under-relaxation of the force iteration may be used by setting the convergence factor, cf, to a value less than unity. Smaller values increase the stability of the iteration, but require more iterations to achieve convergence. This is generally only
needed when Damper-type elements are present with nonlinear damping exponents. Specifying cf to be greater than unity may reduce the number of iterations required for certain types of problems, but may cause instability in the iteration and is
not recommended.
The default value for cf is 1. It must satisfy cf > 0.

Static Period
Normally all modes are treated as being dynamic. In each time step, the response of
a dynamic mode has two parts:
• Forced response, which is directly proportional to the modal load
• Transient response, which is oscillatory, and which depends on the displacements and velocities of the structure at the beginning of the time step
You may optionally specify that high-frequency (short period) modes be treated as
static, so that they follow the load without any transient response. This is done by
specifying a static period, tstat, such that all modes with periods less than tstat are

Nonlinear Modal Time-History Analysis (FNA)

457

CSI Analysis Reference Manual
considered to be static modes. The default for tstat is zero, meaning that all modes
are considered to be dynamic.
Although tstat can be used for any nonlinear time-history analysis, it is of most use
for quasi-static analyses. If the default iteration parameters do not work for such an
analysis, you may try using the following parameters as a starting point:
• tstat greater than the longest period of the structure
• itmax = itmin ³ 1000
• dtmax = dtmin = dt
• ftol £ 10-6
• cf = 0.1
This causes all modes to be treated as static, and uses iteration rather than
substepping to find a solution. The choice of parameters to achieve convergence is
very problem dependent, and you should experiment to find the best values to use
for each different model.

Nonlinear Direct-Integration Time-History Analysis
Direct integration of the full equations of motion without the use of modal superposition is available in SAP2000. While modal superposition is usually more accurate
and efficient, direct-integration does offer the following advantages:
• Full damping that couples the modes can be considered
• Impact and wave propagation problems that might excite a large number of
modes may be more efficiently solved by direct integration
• All types of nonlinearity available in SAP2000 may be included in a nonlinear
direct integration analysis.
Direct integration results are extremely sensitive to time-step size in a way that is
not true for modal superposition. You should always run your direct-integration
analyses with decreasing time-step sizes until the step size is small enough that results are no longer affected by it.

Time Integration Parameters
See Topic “Linear Direct-Integration Time-History Analysis” (page 149) for information about time-integration parameters. The same considerations apply here as
for linear analysis.

458

Nonlinear Direct-Integration Time-History Analysis

Chapter XXIV

Nonlinear Time-History Analysis

If your nonlinear analysis is having trouble converging, you may want to use the
HHT method with alpha = -1/3 to get an initial solution, then re-run the analysis
with decreasing time step sizes and alpha values to get more accurate results.

Nonlinearity
All material nonlinearity that has been defined in the model will be considered in a
nonlinear direct-integration time-history analysis.
You have a choice of the type of geometric nonlinearity to be considered:
• None
• P-delta effects
• Large displacement effects
If you are continuing from a previous nonlinear analysis, it is strongly recommended that you select the same geometric nonlinearity parameters for the current
case as for the previous case. See Chapter “Geometric Nonlinearity” (page 409) for
more information.

Initial Conditions
See Topic “Initial Conditions” (page 149) in this Chapter for a general discussion
of initial conditions.
You may continue a nonlinear direct-integration time-history analysis from a nonlinear static analysis or another direct-integration time-history nonlinear analysis.
It is strongly recommended that you select the same geometric nonlinearity parameters for the current case as for the previous case.
When multiple Mass Sources have been defined, you can specify which Mass
Source to use for a nonlinear static or nonlinear direct-integration time-history load
case. However, the default is to use the same Mass Source as the previous load
case, or the default Mass Source if starting from zero initial conditions. See Topic
“Mass Source” (page 334) in Chapter “Load Patterns” for more information.

Nonlinear Direct-Integration Time-History Analysis

459

CSI Analysis Reference Manual
Direct-integration damping has two different sources, which are described in the
following. Damping from these sources is added together.
Important note: For linear direct-integration time-history analysis, the linear effective damping for the nonlinear Link/Support elements is also used. However, it is
not used for nonlinear direct-integration time-history analysis.
Proportional Damping from the Load Case
For each direct-integration time-history Load Case, you may specify proportional
damping coefficients that apply to the structure as a whole. The damping matrix is
calculated as a linear combination of the stiffness matrix scaled by a coefficient,
c K , and the mass matrix scaled by a second coefficient, c M .
You may specify these two coefficients directly, or they may be computed by specifying equivalent fractions of critical modal damping at two different periods or frequencies.
For each nonlinear element in the structure, the coefficient c K multiplies the initial
stiffness matrix, i.e., the stiffness of the element at zero initial conditions, regardless of the current nonlinear state of the element. The exception to this rule is that if
the current nonlinear state has zero stiffness and zero force or stress (such as an
open gap or a cracked concrete material), then zero damping is assumed. In the case
where the initial stiffness is different in the negative and positive direction of loading, the larger stiffness is used.
For cable elements, the damping matrix is proportional to the stiffness matrix for an
equivalent truss element along the current chord having the same axial stiffness
(AE/L), where L is the undeformed length.
Mass proportional damping is linearly proportional to period. It is related to the
motion of the structure, as if the structure is moving through a viscous fluid. Mass
proportional damping may excessively damp out long period components.
Proportional Damping from the Materials
You may specify stiffness and mass proportional damping coefficients for individual materials. For example, you may want to use larger coefficients for soil materials than for steel or concrete. The same interpretation of these coefficients applies
as described above for the Load Case damping. Be sure not to double-count the
damping by including the same amount in both the Load Case and the materials.

460

Nonlinear Direct-Integration Time-History Analysis

Chapter XXIV

Nonlinear Time-History Analysis

Nonlinear Solution Control
The nonlinear equations are solved using event-to-event stepping and/or equilibrium iteration in each time step. This may require re-forming and re-solving the
stiffness and damping matrices at each step or iteration.
Several parameters are available for you to control the stepping and iteration process. These are described in the following. We recommend that you start with the
default values of these parameters, except that you may want to vary the maximum
substep size for reasons of accuracy.
If you are having convergence difficulties, you can try varying the solution control
parameters below. However, you should also consider that the model itself may
need improvement. Look for instabilities due to inadequate support, buckling, and
excessively large stiffnesses. If you have hinges or materials that lose strength,
make sure that this behavior is really necessary and that the negative slopes are not
unrealistically too steep.
Maximum Substep Size
The analysis will always stop at every output time step, and at every time step
where one of the input time-history functions is defined. You may, in addition, set
an upper limit on the step size used for integration. For example, suppose your output time step size was 0.005, and your input functions were also defined at 0.005
seconds. If you set the Maximum Substep Size to 0.001, the program will internally
take five integration substeps for every saved output time step. The program may
automatically use even smaller substeps if necessary to achieve convergence when
iterating.
The accuracy of direct-integration methods is very sensitive to integration time
step, especially for stiff (high-frequency) response. You should try decreasing the
maximum substep size until you get consistent results. You can keep your output
time step size fixed to prevent storing excessive amounts of data.
Minimum Substep Size
When using iteration and the solution cannot converge within the specified maximum number of iterations, the program automatically reduces the current step size
and tries again. You can limit the smallest substep size the program will use. If the
program tries to reduce the step size below this limit, it will stop the analysis and indicate that convergence had failed. The minimum substep size has no effect when
using event-to-event stepping without iteration.

Nonlinear Direct-Integration Time-History Analysis

461

CSI Analysis Reference Manual
Event-to-Event Stepping Control
Event-to-event stepping is available as an option for nonlinear direct-integration
time-history analysis. Using this strategy, an increment of load is applied in each
time step until one of the nonlinear elements experiences an “event” that causes a
significant change in the stiffness of the structure. The stiffness matrix is then reformed, and another load increment is applied to reach the next event. This continues in a series of event steps until the entire load for that time step has been applied.
If no event occurs within a time step, the full load for that time step is applied all at
once.
Events are implemented for the following nonlinear models: all frame hinges; layered shells with directional or coupled nonlinear behavior; and links with multi-linear plasticity, gap, hook, friction-pendulum, and triple-pendulum behavior. Events
typically include first yield, unloading, strength loss, increasing stiffness, and other
significant changes in behavior that depend on the type of element or material.
When event-to-event stepping is used, you may specify whether or not to perform
iteration to reduce any equilibrium error to within a specified convergence tolerance (see next subtopic). If iteration is requested, this will be performed at the end
of each time step, not at the end of each event.
If iteration is not requested, the relative equilibrium error will be reported in the
analysis log file (.LOG) and the unbalanced load will be applied in the next time
step. Although the structure may be slightly out of equilibrium at each time step,
the unbalance does not accumulate over time. This method can be quite effective
because the deviation from linearity is usually small between events. However, iteration for equilibrium is recommended for models having significant geometric
nonlinearity, including models with cable elements.
When iteration is not performed, there can be no convergence failure. For this reason, event-to-event stepping without iteration may help with certain load cases that
otherwise fail to complete, although the results should be reviewed carefully for acceptable equilibrium error.
You can specify whether or not to use event-to-event stepping. When events are
used, each load increment tends to be more linear, thus reducing equilibrium unbalance and lessening the need for iteration. On the other hand, models with a large
number of nonlinear elements and/or hinges may generate a large number of
events, which can significantly increase the analysis time.
When using event stepping, you can specify a relative event-lumping tolerance that
will group multiple events together. Effectively, the load increment calculated to
reach the first event is increased by the tolerance to include other events that would

462

Nonlinear Direct-Integration Time-History Analysis

Chapter XXIV

Nonlinear Time-History Analysis

occur soon afterward. Larger event tolerances reduce the number of event steps
taken, but may increase the equilibrium unbalance or amount of iteration required.
Note that for isotropic frame hinges the event lumping tolerance may also allow the
force or deformation response to deviate from the backbone curve. The relative
magnitude of the deviations is on the order of the relative lumping tolerance.
You can also specify the maximum number of events to allow per time step. Increasing this number may increase the accuracy of the analysis when iteration is not
used, or lessen the need for iteration when used. On the other hand, allowing fewer
events per time step may increase the speed of the analysis at the expense of more
equilibrium error or iteration.
Whether or not to use event stepping is a problem-dependent decision. Normally
using events will improve convergence behavior. However, if a large number of
event steps are generated that make the analysis run slowly, try turning event-stepping off for that model or load case. Either way, results for a stable model should be
consistent to within the convergence tolerance when iteration is used.
Nonlinear Iteration
Iteration may be used to ensure that equilibrium is achieved at each step of the analysis to within a specified convergence tolerance. You may specify whether or not to
use iteration when using event-to-event stepping, as described in the preceding
subtopic. Iteration is always used when event stepping is not used.
When using iteration, you can specify the relative convergence tolerance used to
compare the magnitude of force error with the magnitude of the force acting on the
structure. You may need to use significantly smaller values of convergence tolerance to get good results for large-displacements problems than for other types of
nonlinearity. Try decreasing this value until you get consistent results.
For each time step, constant-stiffness iteration is tried first. If convergence is not
achieved, Newton-Raphson (tangent-stiffness) iteration is tried next. If both fail,
the step size is reduced, and the process is repeated.
You can separately control the number of constant-stiffness and Newton-Raphson
iterations allowed in each step. Setting either parameter to zero prevents that type
of iteration. Setting both to zero causes the analysis to use the default number of iterations. Constant-stiffness iterations are faster than Newton-Raphson iterations,
but the latter are usually more effective, especially for cables and geometric
nonlinearity. The default values work well in many situations.

Nonlinear Direct-Integration Time-History Analysis

463

CSI Analysis Reference Manual
Line Search Option
Line search is an iteration option that can increase the efficiency of equilibrium iterations by scaling the solution increment in a trial-and-error fashion to find the
smallest unbalance. This increases the computation time for each iteration, but often results in fewer iterations and better convergence behavior, with a net gain in efficiency. Line search is particularly effective for stiffening systems, such as tightening cables, closing gaps, unloading from plastic yielding, and sticking after
frictional sliding.
You can choose whether or not to use line search, provided that iteration is being
used. Unlike nonlinear static analysis, line search for time-history analysis can be
used in conjunction with event-to-event stepping.
When using line search, specify the following parameters:
• Maximum number of line searches per Iteration. Use this parameter to limit
the number of line searches allowed per iteration, usually in the range of 5
to 40.
• Line-Search Acceptance Tolerance (Relative). The solution increment is
successively reduced or increased until the minimum error is found, the
maximum number of line searches is reached, or the relative change in error from the previous trial is less than the acceptance tolerance set here.
The practical range is about 0.02 to 0.50. This value should not be too
small, since the goal is only to improve the next iteration.
• Line-Search Step Factor. For each line-search trial, the solution increment
is successively reduced by the step factor specified here until the minimum
error is found, the maximum number of line searches is reached, or the acceptance tolerance is satisfied. If reducing the increment does not decrease
the error, the increment is instead increased by the step factor following the
same procedure. This factor must be greater than 1.0, and should usually be
no more than 2.0.
The default values are recommended as starting point. For stiffening systems that
are slow to converge, try increasing the maximum number of line searches per iteration, decreasing the acceptance tolerance, and reducing the step factor.

464

Nonlinear Direct-Integration Time-History Analysis

C h a p t e r XXV

Frequency-Domain Analyses
Frequency-domain analysis is based upon the dynamical response of the structure
to harmonically varying load. Two types of frequency-domain Load Cases are currently available: deterministic Steady-State analysis and probabilistic Power-Spectral-Density analysis.
Advanced Topics
• Overview
• Harmonic Motion
• Frequency Domain
• Damping
• Loading
• Frequency Steps
• Steady-State Analysis
• Power-Spectral-Density Analysis

465

CSI Analysis Reference Manual

Overview
Frequency-domain analysis is based upon the dynamical response of the structure
to harmonically varying load. The analysis is performed at one or more frequencies
of vibration. At each frequency, the loading varies with time as sine and cosine
functions. Two types of frequency-domain Load Cases are currently available:
steady-state analysis and power-spectral-density analysis.
Steady-state analysis computes the deterministic response at each requested frequency. The loading may have components at acting different phase angles. The
phase angles of the response are computed and may be displayed.
Power-spectral-density analysis is based on a probabilistic spectrum of loading.
The analysis computes a probabilistic spectrum for each response component. In
addition, a single probabilistic expected value for each response component is presented that is the root-mean-square (RMS) of the probabilistic spectrum. The loading may have components at acting different phase angles, but the phase information is not preserved for the probabilistic response.
Hysteretic and viscous damping may be specified. Frequency-dependent properties
for Link and Support elements, if defined, are considered in the analyses. All analyses are performed in the complex domain.

Harmonic Motion
Harmonic loading is of the form r ( t ) = p0 cos(wt ) + p90 sin(wt ), where w is the circular frequency of the excitation. This loading is assumed to exist for all time, so
that transient components of the response have vanished. In other words,
steady-state conditions have been achieved.
The spatial loading consists of two parts: the in-phase component p0, and the 90°
out-of-phase component p90. The spatial distributions do not vary as a function of
time.
The equilibrium equations for the structural system are of the following form:
K u( t ) + C u&( t ) + M u&&( t ) = r ( t ) = p0 cos(wt ) + p90 sin(wt )
where K is the stiffness matrix, C is the viscous damping matrix, M is the diagonal
& and u&& are the joint displacements, velocities, and acceleramass matrix, and u, u,
tions, respectively.

466

Overview

Chapter XXV

Frequency-Domain Analyses

Frequency Domain
It is more convenient to re-write the equations in complex form. The loading is then
given by
r ( t ) = p exp( iwt ) = p (cos(wt ) + i sin(wt ))
where the overbar indicates a complex quantity. The real cosine term represents the
in-phase component, and the imaginary sine term represents the 90° out-of-phase
component.
The steady-state solution of this equation requires that the joint displacements be of
the same form:
u ( t ) = a exp( iwt ) = a (cos(wt ) + i sin(wt ))
Substituting these into the equation of motion yields:
2

[ K + iwC - w M ] a = p
We can define a complex impedance matrix
2

K = K - w M + i wC
where the real part represents stiffness and inertial effects, and the imaginary part
represents damping effects. Note that the real part may be zero or negative. The
equations of motion can be written:
(Eqn. 1)

K (w) a (w) = p(w)

where here we emphasize that the impedance matrix, the loading, and the displacements are all functions of frequency.
The impedance matrix is a function of frequency not only because of the inertial
and damping terms, but also because frequency-dependent Link and Support element properties are permitted. Thus
2

K (w) = K(w) - w M + iwC(w)
Please see Topic “Frequency-Dependent Link/Support Properties” (page 306) in
Chapter “The Link/Support Element—Advanced” for more information.

Frequency Domain

467

CSI Analysis Reference Manual

Damping
It is common for frequency-domain problems to specify a hysteretic (displacement-based) damping matrix D rather than a viscous (velocity-based) damping matrix C. These are related as:
D = wC
[As an aside, note that from this definition a nonzero value of hysteretic damping D
at w = 0 (static conditions) results in an undefined value for viscous damping C. This
leads to considerations of the noncausality of hysteretic damping, as discussed in
Makris and Zhang (2000). However, this is usually ignored.]
Hysteretic damping may be specified as a function of frequency, i.e., D = D(w), and
there is no restriction imposed on the value at w = 0.
Using hysteretic damping, the complex impedance matrix becomes
2

K (w) = K(w) - w M + iD(w)

Sources of Damping
In frequency-domain analysis, the damping matrix D(w) has four different sources
as described in the following. Damping from these sources is added together.
Hysteretic Damping from the Load Case
For each Steady-state or Power-spectral-density Load Case, you may specify proportional damping coefficients that apply to the structure as a whole. The damping
matrix is calculated as a linear combination of the stiffness matrix scaled by a coefficient, d K , and the mass matrix scaled by a second coefficient, d M . For most practical cases, d M = 0 and only d K is used.
You may specify that these coefficients are constant for all frequencies, or they
may be linearly interpolated between values that you specify at different frequencies. Thus the damping matrix becomes:
D(w) =d K (w)K + d M (w)M
The stiffness matrix used here includes all elements in the structure except for any
Link or Support elements that have frequency-dependent properties.
If you specify d M = 0 and d K (w) to linearly increase with frequency, this is equivalent to viscous damping.

468

Damping

Chapter XXV

Frequency-Domain Analyses

You can approximate modal damping by setting d M = 0 and d K (w) = 2d(w), where
d(w) is the modal damping ratio. For example, if you typically use a constant 5%
modal damping for all modes, the equivalent hysteretic damping value is a constant
d K (w) = 010
. . For each mode, this leads to approximately the same level of response
at resonance.
Hysteretic Damping from the Materials
You may specify stiffness and mass proportional damping coefficients for individual materials. For example, you may want to use larger coefficients for soil materials than for steel or concrete. The same interpretation of these coefficients applies
as described above for the Load Case damping. Be sure not to double-count the
damping by including the same amount in both the Load Case and the materials.
Hysteretic Damping from Frequency-Dependent Link/Support Elements
For any Link or Support elements that have frequency-dependent properties assigned to them, the frequency-dependent hysteretic damping values are added to
the damping matrix used.
Viscous Damping from the Link/Support Elements
For any Link or Support elements that do not have frequency-dependent properties
assigned to them, the linear effective-damping coefficients are multiplied by frequency w and added to the damping matrix. The linear effective-damping values are
used regardless of whether or not nonlinear damping coefficients have been specified.

Loading
The load, p(w), applied in a given Steady-state or Power-spectral-density case may
be an arbitrary function of space and frequency. It can be written as a finite sum of
spatial load vectors, p i , multiplied by frequency functions, f i (w), as:
p(w) = å s j f j (w) p j e
j

iq j

= å s j f j (w) p j (cos q j + i sin q j )

(Eqn. 2)

Here s j is a scale factor and q j is the phase angle at which load p j is applied.
The program uses Load Patterns and/or Acceleration Loads to represent the spatial
load vectors, p j , as described below.

469

CSI Analysis Reference Manual
The frequency functions used here depend on the type of analysis. See Topics
“Steady-State Analysis” (page 471) and “Power-Spectral-Density Analysis” (page
473) in this Chapter for more information.
If Acceleration Loads are used, the displacements, velocities, and accelerations are
all measured relative to the ground. The frequency functions associated with the
Acceleration Loads mx, my, and mz are the corresponding components of uniform
ground acceleration, u&&gx , u&&gy , and u&&gz .
See Topic “Functions” (page 350) in Chapter “Load Cases” for more information.

Defining the Spatial Load Vectors
To define the spatial load vector, p j , for a single term of the loading sum of Equation 2, you may specify either:
• The label of a Load Pattern using the parameter load, or
• An Acceleration Load using the parameters csys, ang, and acc, where:
– csys is a fixed coordinate system (the default is zero, indicating the global
coordinate system)
– ang is a coordinate angle (the default is zero)
– acc is the Acceleration Load (U1, U2, or U3) in the acceleration local coordinate system as defined below
Each Acceleration Load in the loading sum may have its own acceleration local coordinate system with local axes denoted 1, 2, and 3. The local 3 axis is always the
same as the Z axis of coordinate system csys. The local 1 and 2 axes coincide with
the X and Y axes of csys if angle ang is zero. Otherwise, ang is the angle from the X
axis to the local 1 axis, measured counterclockwise when the +Z axis is pointing toward you. This is illustrated in Figure 82 (page 400).
The acceleration local axes are always referred to as 1, 2, and 3. The global Acceleration Loads mx, my, and mz are transformed to the local coordinate system for
loading.
It is generally recommended, but not required, that the same coordinate system be
used for all Acceleration Loads applied in a given Load Case.
Load Patterns and Acceleration Loads may be mixed in the loading sum.
For more information:
• See Chapter “Load Patterns” (page 321).

470

Chapter XXV

Frequency-Domain Analyses

• See Topic “Acceleration Loads” (page 338) in Chapter “Load Patterns”.

Frequency Steps
Frequency-domain analyses are performed at discrete frequency steps. For a
Steady-state or Power-spectral-density Load Case, you may request the response at
the following frequencies:
• A required range of equally spaced frequencies. This is defined by specifying
the first frequency, f 1 ³ 0; the last frequency, f 2 ³ f 1 ; and the number of increments, n > 0. This results in the following set of frequencies:
f 1 , f 1 + Df , f 1 + 2Df ,K , f 2 ,
where Df = ( f 2 - f 1 ) / n.
• Optionally, at all frequencies calculated in a specified Modal Load Case. Only
frequencies that fall within the frequency range f 1 to f 2 will be used. See
Chapter “Modal Analysis” (page 365) for more information.
• Optionally, at specified fractional deviations from all frequencies calculated in
a specified Modal Load Case. For example, suppose you specify fractional deviations of 0.01 and -0.02. For each frequency f found by the Modal Load
Case, the frequency-domain analysis will be performed at 101
. f and 098
. f.
Only frequencies that fall within the frequency range f 1 to f 2 will be used.
• Optionally, at any number of directly specified frequencies f . Only frequencies that fall within the frequency range f 1 to f 2 will be used.
Frequencies may be specified in Hz (cycles/second) or RPM (cycles/minute).
These will be converted to circular frequencies, w, by the program.
The use of modal frequencies and their fractional deviations can be very important
to capture resonant behavior in the structure. Any set of equally-spaced frequencies
could easily skip over the most significant response in a given frequency range. The
use of directly specified frequencies can be important when you are concerned
about sensitive equipment that may respond strongly at certain frequencies.

Steady-State Analysis
Steady-state analysis seeks the response of the structure at one or more frequencies
to loading of the form:

Frequency Steps

471

CSI Analysis Reference Manual
p(w) = å s j f j (w) p j e
j

iq j

= å s j f j (w) p j (cos q j + i sin q j )
j

See Topic “Loading” (page 469) in this Chapter for more information about this
type of loading.
The frequency function, f j (w), is given directly by a steady-state function that you
define. It represents the magnitude of the load before scaling by s j . See Topic
“Functions” (page 350) in Chapter “Load Cases” for more information.
If you are interested in the response characteristics of the structure itself, a constant
function could be used, i.e., f j (w) =1. For loading that is caused by rotating machinery, f j (w) = w2 might be used.

Example
Suppose we have a machine with a spinning flywheel that has an eccentric mass.
The mass is m and the center of mass is eccentric by an amount e. The flywheel
spins about an axis parallel to the global Y axis. This machine is mounted on a
structure, and we are interested in the steady-state response of the structure to the
machine running at any speed in the range from 0 to 30Hz (1800 RPM).
The magnitude of the force from the eccentric mass that acts on the center of rotation is given by emw2 . This force rotates in the X-Z plane. To define the loading, we
need the following:
• A Load Pattern, say “ECCX”, in which a unit load in the +X direction is assigned to the joint that represents the center of the flywheel.
• Another Load Pattern, say “ECCZ”, in which a unit load in the +Z direction is
assigned to the same joint.
• A Steady-state Function, say “FSQUARED”, which varies as f j (w) = w2
• A Modal Load Case, say “MODAL”, which calculates all natural frequencies
in the range from 0 to 30Hz. This can be for eigen or Ritz vectors; if Ritz, use
the two Load Patterns “ECCX” and “ECCZ” as the starting load vectors.
We then define a Steady-state Load Case with the following features:
• The loads applied include the following two contributions:
– Load Pattern “ECCX”, Function “FSQUARED”, a scale factor equal to
em, and a phase angle of 0°

472

Steady-State Analysis

Chapter XXV

Frequency-Domain Analyses

– Load Pattern “ECCZ”, Function “FSQUARED”, a scale factor equal to
em, and a phase angle of 90°
• Frequency range from 0 to 30Hz, with 15 increments (every 2Hz)
• Additional frequencies at the modal frequencies of Load Case “MODAL”
• Additional frequencies at the following fractional deviations from the modal
frequencies of Load Case “MODAL”: +0.01, -0.01, +0.02, -0.02, +0.03,
-0.03, +0.05, -0.05
• Stiffness-proportional hysteretic damping with a coefficient of d k = 004
. , corresponding to modal damping of 2%, which may be appropriate for small vibrations
After analysis, we can plot the deflected shape or force/stress response at any of the
requested frequencies and at any phase angle. For example, the response at phase
angle 0° primarily represents the behavior due to horizontal loading, plus a damping component due to vertical loading. We can instead plot the magnitude of the response at any requested frequency, where the magnitude is given by the square-root
of the sum of the squares of the real (0°) and imaginary (90°) response components.
It is also possible to display plots of any response quantity as a function of frequency, yielding a frequency spectrum. This can be done for the component at any
phase angle, or for the magnitude of the response.

Power-Spectral-Density Analysis
Power-spectral-density (PSD) analysis is similar to Steady-state analysis in that it
considers the harmonic behavior of the structure over a range of frequencies. However, the loading is considered to be probabilistic over the frequency range of the
analysis, and so too is the response. This probabilistic response can be integrated
over the frequency range to determine a single expected value. This can be useful,
for example, for fatigue design.
A PSD Load Case considers correlated loading of the form:
p(w) = å s j f j (w) p j e
j

iq j

= å s j f j (w) p j (cos q j + i sin q j )
j

See Topic “Loading” (page 469) in this Chapter for more information about this
type of loading.

Power-Spectral-Density Analysis

473

CSI Analysis Reference Manual
The frequency function, f j (w), used in this sum is taken as the square root of a
Power-spectral-density function that you define.
To explain this further, PSD functions are specified as load-squared per unit of frequency. In order to combine correlated loading algebraically, the square-root of
these functions are used. Normally one would expect that the same PSD function
would be used for all correlated loading terms, but this is not required. Note that using a scale factor s j = 2 in the sum here is the same as multiplying the PSD function
itself by a factor of four. See Topic “Functions” (page 350) in Chapter “Load
Cases” for more information.
The PSD curve for any response quantity (displacement, force, stress, etc.) is given
by the square of the magnitude of that calculated response, plotted at every requested frequency step. The square-root of the integral under the PSD curve for a
given response quantity gives the probabilistic expected value for that quantity,
i.e., the root-mean-square (RMS) value. This will always be a positive number.
Because the PSD curves represent the square of the response, most of the integrated
area will be near resonant frequencies of the structure. For accuracy, it is very important to capture the response at frequency steps at and around the natural modes
of the structure.
Uncorrelated loading should be defined in separate PSD Load Cases, and then
combined using SRSS-types of Load Combinations. See Topic “Load Combinations (Combos)” (page 351) in Chapter “Load Cases.”

Example
Consider the same example used in Topic “Steady-State Analysis” (page 471) of
this Chapter. Suppose that the machine is expected to operate 95% of the time in the
range of 20 to 25Hz, and 5% of the time at other frequencies from 0 to 30Hz.
The only difference between the definition of the two types of Load Cases for this
problem is in the functions. Now we will use a PSD Function, say “FPOWER”, defined as follows:
. / 25Hz , 0 £ w< 20Hz
ì005
F j (w) = w í095
. / 5Hz , 20 £ w< 25Hz
ï005
î . / 25Hz , 25 £ w £ 30Hz
4ï

474

Power-Spectral-Density Analysis

Chapter XXV

Frequency-Domain Analyses

Note that the w2 term is squared again. However, in the definition of the PSD Load
Case, the scale factor will still be em (not squared), since it was not included in the
PSD function itself.
The two loads, “ECCX” and “ECCZ”, must be combined in the same Load Case
because they are clearly correlated. However, if a second machine with its own independent functioning was mounted to the same structure, this should be analyzed
in a separate PSD Load Case and the two cases combined in an SRSS Load Combination.

Power-Spectral-Density Analysis

475

CSI Analysis Reference Manual

476

Power-Spectral-Density Analysis

C h a p t e r XXVI

Moving-Load Analysis
Moving-load analysis is available in CSiBridge to compute influence lines and surfaces for traffic lanes on bridge structures and to analyze these structures for the response due to vehicle live loads. A simplified version of moving-load analysis is
available in SAP2000 for moving vehicles, such as cranes, on rails or other one-dimensional paths.
Advanced Topics
• Overview for CSiBridge
• Moving-Load Analysis in SAP2000
• Bridge Modeler
• Bridge Analysis Procedure
• Lanes
• Influence Lines and Surfaces
• Vehicle Live Loads
• General Vehicle
• Vehicle Response Components
• Standard Vehicles
• Vehicle Classes

477

CSI Analysis Reference Manual
• Moving Load Load Cases
• Moving Load Response Control
• Step-by-Step Analysis
• Computational Considerations

Overview for CSiBridge
For CSiBridge, moving-load analysis can be used to determine the response of
bridge structures due to the weight of Vehicle live loads. Considerable power and
flexibility is provided for determining the maximum and minimum displacements,
forces, and stresses due to multiple-lane loads on complex structures, such as highway interchanges. The effects of Vehicle live loads can be combined with static and
dynamic loads, and envelopes of the response can be computed.
The bridge to be analyzed can be created using the parametric Bridge Modeler in
CSiBridge; built manually using Frame, Shell, Solid, and/or Link elements; or by
combining these two approaches. The superstructure can be represented by a simple “spine” (or “spline”) model using Frame elements, or it can be modeled in full
3-dimensional detail using Shell or Solid elements.
Lanes are defined that represent where the live loads can act on the superstructure.
Lanes may have width and can follow any straight or curved path. Multiple Lanes
need not be parallel nor of the same length, so that complex traffic patterns may be
considered. The program automatically determines how the Lanes load the superstructure, even if they are eccentric to a spine model. Conventional influence lines
and surfaces due to the loading of each Lane can be displayed for any response
quantity.
You may select Vehicle live loads from a set of standard highway and railway Vehicles, or you may create your own Vehicle live loads. Vehicles are grouped in Vehicle Classes, such that the most severe loading of each Class governs.
Each vehicle may generate vertical and/or horizontal forces, representing the effects of gravity, braking and acceleration, and centrifugal forces. Overturning moments due to super-elevation and centrifugal load may also be included.
Two types of live-load analysis can be performed:
• Influence-based enveloping analysis: Vehicles move in both directions along
each Lane of the bridge. Using the influence surface, Vehicles are automatically located at such positions along the length and width of the Lanes to pro-

478

Overview for CSiBridge

Chapter XXVI

Moving-Load Analysis

duce the maximum and minimum response quantities throughout the structure.
Each Vehicle may be allowed to act on every lane or be restricted to certain
lanes. The program can automatically find the maximum and minimum response quantities throughout the structure due to placement of different Vehicles in different Lanes. For each maximum or minimum extreme response
quantity, the corresponding values for the other components of response can
also be computed. Vertical and/or horizontal loading may be considered in any
combination.
• Step-by-step analysis: Any number of Vehicles can be run simultaneously on
the Lanes, each with its own starting time, position, direction and speed.
Step-by-step static or time-history analysis can be performed, with nonlinear
effects included if desired. Currently only vertical loading may be considered
in step-by-step analysis.
For most design purposes the enveloping-type analysis using Moving-Load Load
Cases is most appropriate. For special studies and unusual permit vehicles, the
step-by-step approach can be valuable.
The moving-load features in SAP2000 are a subset of those available in CSiBridge,
as described in the next topic.

Moving-Load Analysis in SAP2000
This chapter is primarily written to describe the full moving-load capabilities for
bridge design as available in CSiBridge. Moving-load analysis is also available in
SAP2000, but is intended for a different class of problems, primarily for cranes riding on rails and similar one-dimensional applications.
For SAP2000, the following differences apply:
• Lanes are called “Paths” in SAP2000.
• Paths are defined by reference to a sequence (line or curve) of Frame elements,
and the vehicle loads will be applied to these elements.
• Paths may be defined that are eccentric to the specified frame elements.
• Width effects for Paths and Vehicles are not included.
• Influence lines, but not surfaces, are available.
• Only the general vehicle is available, with the following features:
– Any number of concentrated axle and uniform inter-axle loads
– One inter-axle distance may be variable
Moving-Load Analysis in SAP2000

479

CSI Analysis Reference Manual
– No floating axle loads
– No loaded-length effects
– Vertical loading only
– No limitations on the type of response calculated for the vehicle
– The vehicle may be restricted to the length of the lane.

Bridge Modeler
The Bridge Modeler in CSiBridge provides a powerful way to create and manage
simple or complex bridge models. The bridge is represented parametrically with a
set of high-level objects: layout (alignment) lines, bents (pier supports), abutments
(end supports), deck cross sections, prestress tendons, etc.
These objects are combined into a super object called a Bridge Object. Typically a
single Bridge Object represents the entire structure, although you may need multiple Bridge Objects if you have parallel structures, or want to consider merges or
splits.
A Bridge Wizard is available within the Bridge Modeler to guide you through the
process of creating a bridge model, and help is available within the wizard itself.
The important thing to understand here is that this parametric model of the bridge
exists independently from the discretization of the model into elements. You may
choose to discretize the Bridge Object as Frames (spine model), Shells, or Solids,
and you may choose the size of the elements to be used. You can change the
discretization at any time without affecting your parameterized bridge model.
When you do this, the previously generated elements are automatically deleted, and
new elements created.
You can add additional elements to the model to represent features of the bridge
that may not be provided by the Bridge Modeler. These elements will not be affected by changes to the Bridge Object or its discretization, although it may be necessary to move or modify them if you change the geometry of the bridge.
You can make changes to the elements generated from a Bridge Object, such as assigning different properties or additional loads. These changes will survive regeneration of the model if a new element is generated in exactly the same location.
However, this may not occur if there are changes in bridge geometry or
discretization, so it is best to check a regenerated model and make your changes
again if necessary.

480

Bridge Modeler

Chapter XXVI

Moving-Load Analysis

Moving-Load Analysis Procedure
There are two types of vehicle live-load analysis that can be performed: influence-base enveloping analysis, and step-by-step analysis with full correspondence.
The basic steps required for these two types of analysis are as follows.
For both types of analysis:
(1) Create a structural model using the Bridge Modeler and/or standard structural
model-building techniques.
(2) Define Lanes that specify the location where vehicles can travel.
(3) Define Vehicles that represent the live load acting in the Lanes.
For Influence-Based Analysis:
(4) Define Vehicle Classes that group together one or more Vehicles that should be
enveloped.
(5) Define Moving-Load Load Cases that specify which Vehicle Classes should be
moved on which Lanes to produce the enveloped response, and what combination of vertical and horizontal loads are to be considered.
(6) Specify Bridge Response parameters that determine for which elements moving-load response should be calculated, and set other parameters that control
the influence-based analysis.
(7) After running the analysis, you may view influence lines for any element response quantity in the structure, and envelopes of response for those elements
requested under Bridge Response.
For Step-by-Step Analysis:
(8) Define Load Patterns of type “Vehicle Live” that specify which Vehicles move
on which Lanes, at what speed, and from what starting positions.
(9) Apply the Vehicle-Live Load Patterns in Multi-Step Static Load Cases, or in
Time-History Load Cases if you are interested in dynamical effects.
(10) After running the analysis, you may view step-by-step response or envelopes
of response for any element in the structure. You may create a video showing
the step-by-step static or dynamic results. Influence lines are not available.

Moving-Load Analysis Procedure

481

CSI Analysis Reference Manual
Both types of bridge analysis may exist in the same model. You may create additional Load Patterns and Load Cases, and combine the results of these with the results for either type of bridge analysis.

Lanes
The Vehicle live loads are considered to act in traffic Lanes transversely spaced
across the bridge roadway. The number of Lanes and their transverse spacing can
be chosen to satisfy the appropriate design-code requirements. For simple bridges
with a single roadway, the Lanes will usually be parallel and evenly spaced, and
will run the full length of the bridge structure.
For complex structures, such as interchanges, multiple roadways may be considered; these roadways can merge and split. Lanes need not be parallel nor be of the
same length. The number of Lanes across the roadway may vary along the length to
accommodate merges. Multiple patterns of Lanes on the same roadway may be created to examine the effect of different lateral placement of the Vehicles.
Lanes in SAP2000 are called Paths, and they have no width effects.

Centerline and Direction
A traffic Lane is defined with respect to a reference line, which can be either a
bridge layout line or a line (path) of Frame elements. The transverse position of the
Lane centerline is specified by its eccentricity relative to the reference line. Lanes
are said to “run” in a particular direction, namely from the first location on the reference line used to define the Lane to the last.

Eccentricity
Each Lane across the roadway width will usually refer to the same reference line,
but will typically have a different eccentricity. The eccentricity for a given Lane
may also vary along the length.
The sign of a Lane eccentricity is defined as follows: in an elevation view of the
bridge where the Lane runs from left to right, Lanes located in front of the roadway
elements have positive eccentricity. Alternatively, to a driver traveling on the roadway in the direction that the Lane runs, a Lane to the right of the reference line has a
positive eccentricity. The best way to check eccentricities is to view them graphically in the graphical user interface.

482

Lanes

Chapter XXVI

Moving-Load Analysis

In a spine model, the use of eccentricities is primarily important for the determination of torsion in the bridge deck and transverse bending in the substructure. In
Shell and Solid models of the superstructure, the eccentricity determines where the
load is applied on the deck.

Centrifugal Radius
The radius is used to compute centrifugal loads, and is only available for lanes defined from a bridge layout line, not for those defined from a line (path) of frame elements. The centrifugal radius is specified independently of the actual geometry of
the lane in order to give more control over the loading.
A positive radius curves to the right when traveling in the direction that the Lane
runs, generating centrifugal forces that act to the left. Conversely, a negative radius
curves to the left, generating forces that act to the right. A zero radius actually indicates infinite radius, or zero curvature, representing a straight Lane that generates
no centrifugal forces. The radius may be constant or variable along the length of the
Lane. When variable, the curvature (inverse of the radius) is interpolated linearly
between specified values.
For the Eurocode and similar prescriptive codes, you should set any radii that are
larger than the prescribed upper limit to zero so as to generate no centrifugal forces,
and set radii that are smaller than the prescribed lower limit to the value of that
lower limit.

Width
You may specify a width for each Lane, which may be constant or variable along
the length of the Lane. When a Lane is wider than a Vehicle, each axle or distributed load of the Vehicle will be moved transversely in the Lane to maximum effect.
If the Lane is narrower than the Vehicle, the Vehicle is centered on the Lane and the
Vehicle width is reduced to the width of the Lane.

Interior and Exterior Edges
Certain AASHTO vehicles require that the wheel loads maintain a specified minimum distance from the edge of the lane. This distance may be different depending
on whether the edge of the lane is at the edge of the roadway or is interior to the
roadway. For each lane, you may specify for the left and right edges whether they
are interior or exterior, with interior being the default. This only affects vehicles
which specify minimum distances for the wheel loads. By default, vehicle loads

Lanes

483

CSI Analysis Reference Manual
may be placed transversely anywhere in the lane, i.e., the minimum distance is zero.
Left and right edges are as they would be viewed by a driver traveling in the direction the lane runs.

Discretization
A influence surface will be constructed for each Lane for the purpose of placing the
vehicles to maximum effect. This surface is interpolated from unit point loads,
called influence loads, placed along the width and length of the Lane. Using more
influence loads increases the accuracy of the analysis at the expense of more
computational time, memory, and disk storage.
You can control the number of influence loads by independently specifying the
discretization to be used along the length and across the width of each Lane.
Discretization is given as the maximum distance allowed between load points.
Transversely, it is usually sufficient to use half the lane width, resulting in load
points at the left, right, and center of the Lane. Along the length of the Lane, using
eight to sixteen points per span is often adequate.
For Lanes applied to a general structure, the distance between the load points along
the length is chosen as the largest value that provides uniform spacing but does not
exceed the specified discretization length.
For Lanes applied to a bridge object created by the Bridge Modeler, the load points
are created as follows:
• Along the Lane centerline, load points are placed at each discretization line.
Discretization lines include the beginning and end of each span, in-span
hinges, full-width dia phragms, user-spec i fied span points, and other
discretization lines that created so as not to exceed the bridge-object
discretization length or angle.
• Between these load points, additional points are added at equal spaces that do
not exceed the minimum value of:
– The discretization length specified along-the-length for the Lane
– The fraction of the lane length specified for the Lane, if any
– The fraction of the span length specified for the Lane, if any, using the
shortest span in the bridge object
– The submesh size specified when updating the bridge object.

484

Lanes

Chapter XXVI

Moving-Load Analysis

• For each load point located on the lane centerline, transverse load points are
placed along the discretization line at equal distances not to exceed the
discretization length specified across-the-width for the Lane.
As with analyses of any type, it is strongly recommended that you start with models
that run quickly, using coarser discretization, so that you can gain experience with
your model and perform reality checks. Later, you can increase the refinement until
you achieve the desired level of accuracy and obtain the detailed results that you
need.

Influence Lines and Surfaces
CSiBridge uses influence lines and surfaces to compute the response to vehicle live
loads. Influence lines and surfaces are also of interest in their own right for understanding the sensitivity of various response quantities to traffic loads.
Influence lines are computed for Lanes of zero width, while influence surfaces are
computed for Lanes having finite width. Only influence lines are available in
SAP2000.
An influence line can be viewed as a curve of influence values plotted at the load
points along a traffic Lane. For a given response quantity (force, displacement, or
stress) at a given location in the structure, the influence value plotted at a load point
is the value of that response quantity due to a unit concentrated downward force
acting at that load point. The influence line thus shows the influence upon the given
response quantity of a unit force moving along the traffic lane. Figure 86 (page 486)
shows some simple examples of influence lines. An influence surface is the extension of this concept into two dimensions across the width of the lane.
Influence lines and surfaces may exhibit discontinuities (jumps) at the location of
the response quantity when it is located at a load point on the traffic lane. Discontinuities may also occur where the structure itself is not continuous (e.g., expansion
joints).
Influence lines and surfaces may be displayed in the graphical user interface for the
displacement, force, or stress response of any element in the structure. They are
plotted on the Lanes with the influence values plotted in the vertical direction. A
positive influence value due to gravity load is plotted upward. Influence values are
linearly interpolated between the known values at the load points.

Influence Lines and Surfaces

485

CSI Analysis Reference Manual

(a) Influence Line for Vertical Shear at Center
of a Simple Span

(b) Influence Line for Moment at Center of Left Span
of Two Continuous Spans

Figure 86
Examples of Influence Lines for One-Span and Two-Span Beams

486

Influence Lines and Surfaces

Chapter XXVI

Moving-Load Analysis

Vehicle Live Loads
Any number of Vehicle live loads, or simply Vehicles, may be defined to act on the
traffic Lanes. You may use standard types of Vehicles known to the program, or design your own using the general Vehicle specification.

Distribution of Loads
Longitudinally, each Vehicle consists of one or more axle loads and/or one or more
uniform loads. Axle loads act at a single longitudinal location in the vehicle. Uniform loads may act between pairs of axles, or extend infinitely before the first axle
or after the last axle. The width of each axle load and each uniform load is independently specified. These widths may be fixed or equal to the width of the Lane.
For Moving-Load Load Cases using the influence surface, both axle loads and uniform loads are used to maximum effect. For step-by-step analysis, only the axle
loads are used.

Axle Loads
Longitudinally, axle loads look like a point load. Transversely, axle loads may be
represented as one or more point (wheel) loads or as distributed (knife-edge) loads.
Knife-edge loads may be distributed across a fixed width or the full width of the
lane. Axle loads may be zero, which can be used to separate uniform loads of different magnitude.

Uniform Loads
Longitudinally, the uniform loads are constant between axles. Leading and trailing
loads may be specified that extend to infinity. Transversely, these loads may be distributed uniformly across the width of the lane, over a fixed width, or they may be
concentrated at the center line of the lane.

Minimum Edge Distances
Certain AASHTO vehicles require that the wheel loads maintain a specified minimum distance from the edge of the lane. For any vehicle, you may specify a minimum distance for interior edges of lanes, and another distance for exterior edges.
By default, these distances are zero. The specified distances apply equally to all
axle loads, but do not affect longitudinally-uniform loads. The definition of interior
and exterior edges is given in Subtopic “Lanes” (page 482).
Vehicle Live Loads

487

CSI Analysis Reference Manual

Directions of Loading
All vehicle live loads are specified as weight and are assumed, by default, to act
downward in the –Z global coordinate direction. However, horizontal loads representing braking, acceleration, and centrifugal forces may also be specified as part
of the vehicle definition.
See “Upward and Horizontal Directions” (page 13) in Chapter “Coordinate Systems.”
All vertical and horizontal loads are generated from the same distribution of
weights, i.e., the axle and uniform loads as described above. The various directions
of load are additive, depending upon scale factors defined in the moving load cases,
and are computed simultaneously for each vehicle position.
In the discussion that follows, W is the total weight of an axle load or weight per
length of a uniform load at a given longitudinal position within a vehicle. All generated vertical or horizontal loads have the same distribution across the width of the
vehicle, except as described for overturning moments below.
Vertical Loads
By default the specified axle and uniform loads act in the gravity direction. You
may optionally specify that vertical loads are to be excluded if you want to define a
special vehicle that represents horizontal loading only. Accordingly, the vertical
force FV is either
FV = W or FV = 0
where W is the axle or uniform weight of the vehicle at a given location.
Note that vertical load is required to generate both super-elevation and centrifugal
overturning moments, as discussed below.
Braking and Acceleration Loads
Braking and acceleration loads may be considered by specifying one or two sets of
coefficients multiplying the axle and uniform loads. For example, the first set could
specify a coefficient of 0.25 on the axle loads and 0.0 on the uniform loads. The second set, if requested, could specify a coefficient of 0.05 on both the axle and the
uniform loads. If two sets are requested, the envelope of the two sets will be determined and reported.

488

Vehicle Live Loads

Chapter XXVI

Moving-Load Analysis

The specified values effectively act as coefficients of friction, and the longitudinal
force FB is computed as
FB = ±bW
where b is the specified braking coefficient for axle or uniform loads, and W is the
axle or uniform weight of the vehicle at a given location.
Braking and acceleration loads act longitudinally, parallel to the centerline of the
Lane, and along the grade of the layout line used to define the Lane. These forces
will be assumed to act both forward and backward, so that the maximum and minimum response reported will be equal and opposite to each other. They will be based
on either the maximum or minimum response computed, whichever has the larger
absolute value.
Optionally, skew braking and acceleration loads can be considered by specifying
skew coefficients for axle and uniform loads. The coefficients multiply the longitudinal braking and acceleration forces, and are applied transversely, perpendicular
to the Lane centerline. If the Lane is acting on a bridge object, the skew forces will
act along the super-elevation slope of the bridge. Otherwise, skew braking forces
act in the horizontal plane. Skew forces acting to the left and right, simultaneously
with the longitudinal forces, will both be considered and the envelope reported. The
skew coefficient is effectively the tangent of the angle between the direction of
braking or acceleration and the centerline of the Lane, and the skew braking/acceleration force FK is computed as
FK = ±kFB
where k is the skew coefficient.
Centrifugal Loads
Centrifugal loads may be considered by specifying a velocity and a set of coefficients multiplying the axle and uniform loads. The centrifugal force FC is
computed as
FC = -c

VC2 W
g R

where c is the specified centrifugal coefficient for axle or uniform loads, VC is the
specified velocity, g is the acceleration due to gravity, W is the axle or uniform
weight of the vehicle at a given location, and R is the centrifugal radius specified as
part of the Lane definition. When R = 0, the radius is taken as infinity (straight) and
the force FC = 0.
Vehicle Live Loads

489

CSI Analysis Reference Manual
For the Eurocode and other prescriptive codes, a reference length (typically one
meter) may be specified instead of a velocity. In this case the centrifugal force is
computed as
FC = -cLC

W
R

where LC is the reference length.
Centrifugal forces are applied transversely, perpendicular to the centerline of the
Lane, and always act in the horizontal plane regardless of any super-elevation. Note
that the force acts to the left (negative) when the radius curves to the right (positive), and vice-versa.
Overturning Moments
Two types of overturning moments may be considered, centrifugal and super-elevation. Both are proportional to the height of the centroid of vehicle weight above
the surface of the bridge deck. Separate heights are specified for axle and uniform
loads, but the same heights apply to both types of overturning moment.
For centrifugal loads, the overturning moment (torque) TC is given by
TC = FC h
where FC is the centrifugal force as defined above, and h is the height to the centroid of the vehicle weight causing this force. This generates a vertical force couple
±FTC acting over a moment arm equal to the wheel spacing s, computed as
FTC =

TC
h
= FC
s
s

For vertical loads, the overturning moment TV is given by
TV = FV h sin q
where FV is the vertical force as defined above, h is the height to the centroid of the
vehicle weight causing the force, q = tan -1 e is the angle of super-elevation, and e is
the super-elevation defined as a ratio. This generates a vertical force couple ±FTV
acting over a moment arm equal to the horizontal wheel spacing scosq, computed
as
FTV =

490

TV
h
= TV e
s cosq
s

Vehicle Live Loads

Chapter XXVI

Moving-Load Analysis

The total overturning vertical force couple ±FT is given by
FT = FTC + FTV = ( FC + FV e )

h
s

Note that the overturning moment due to super-elevation tends to counteract the
centrifugal overturning effects on a curve, but may itself cause overturning when
acting alone for vehicles that are stationary. Both cases must be considered in an
enveloping analysis or design.
For a vehicle load of width w, the spacing s and the application of the vertical force
FT couple depend on the transverse distribution of the load as follows:
• For a single point load, or for a zero-width lane, s = 0 and no overturning moments are considered.
• For two point loads, s = w, and the overturning load FT is added to the two vertical loads as an equal-but-opposite pair at the two wheel locations.
• For four equally-spaced point loads, s = 2 3 w, and overturning loads FT /2 are
added to the two vertical loads on one side of the vehicle width and subtracted
from the loads on the other side.
• For a uniform transverse distribution of load, s = 1 2 w, and a uniform overturning load FT /(w/2) is added to the vertical load on one half of the vehicle width
and subtracted from the other half.
• Note that the width of the vehicle will be reduced, if necessary, to fit within the
width of the lane.
Important Note! The overturning load is restricted so as not to cause uplift on the
inner or upward side of the vehicle. This restriction is enforced during analysis, and
can be stated as
FT =

FV
2

regardless of the width distribution of loads.
In particular, no overturning moments will be considered for a load case where the
vertical load is zero. When defining moving load cases, be sure to combine vertical
load with centrifugal load if overturning moments are important. A centrifugal load
case by itself will exclude overturning moments, even if later included in a load
combination with vertical load cases. See Topic “Moving-Load Load Cases” (page
509) for more information.

Vehicle Live Loads

491

CSI Analysis Reference Manual
Elevation of Horizontal Loads
Horizontal loads generated for influence surfaces or individual vehicles are applied
at vertical elevations intended to represent the top surface of the bridge deck.
Specifically:
• For spine and solid models of a bridge object, horizontal loads act at the elevation of the top surface, after taking into account the grade and super-elevation
of the bridge object.
• For area (shell) models of a bridge object, the loads act at the joints of the area
objects representing the top slab. This is typically at the mid-surface of the top
slab, and hence the loads act at a half slab-thickness below the top surface.
Grade and super-elevation are included in the location of these joints.
• For models not created with the Bridge Modeler, horizontal loads on frame objects act at the elevation of the layout line. Horizontal loads on area objects act
at their joints (typically at the mid-surface), and they act at the top-surface
joints of solid objects.
For this reason, torsional moments created by transverse loads and vertical moments (M3) caused by longitudinal loads may be slightly different according to the
type of model generated to represent the bridge object. The difference is generally
small but should be recognized.

Restricting a Vehicle to the Lane Length
When moving a vehicle along the length of the lane, the front of the vehicle starts at
one end of the lane, and the vehicle travels forward until the back of the vehicle exits the other end of the lane. This means that all locations of the vehicle are considered, whether fully or partially on the lane
You have the option to specify that a vehicle must remain fully on the lane. This is
useful for cranes and similar vehicles that have stops at the end of their rails that
prevent them from leaving the lane. This setting only affects influence-surface
analysis, not step-by-step analysis where you can explicitly control where the
vehicle runs.

Application of Loads to the Influence Surface
The maximum and minimum values of a response quantity are computed using the
corresponding influence line or surface. Concentrated loads are multiplied by the
influence value at the point of application to obtain the corresponding response;

492

Vehicle Live Loads

Chapter XXVI

Moving-Load Analysis

distributed loads are multiplied by the influence values and integrated over the
length and width of application.
By default, each concentrated or distributed load is considered to represent a range
of values from zero up to a specified maximum. When computing a response quantity (force or displacement) the maximum value of load is used where it increases
the severity of the response, and zero is used where the load would have a relieving
effect. Thus the specified load values for a given Vehicle may not always be applied proportionally. This is a conservative approach that accounts for Vehicles
that are not fully loaded. Thus the maximum response is always positive (or zero);
the minimum response is always negative (or zero).
You may override this conservative behavior as discussed in the next Subtopic,
“Option to Allow Reduced Response Severity”.
By way of example, consider the influence line for the moment at the center of the
left span shown in Figure 86(b) (page 486). Any axle load or portion of a distributed load that acts on the left span would contribute only to the positive maximum
value of the moment response. Loads acting on the right span would not decrease
this maximum, but would contribute to the negative minimum value of this moment
response.
Option to Allow Reduced Response Severity
You have the option to allow loads to reduce the severity of the response. If you
choose this option, all concentrated and uniform loads will be applied at full value
on the entire influence surface, regardless of whether or not that load reduces the
severity of the response. This is less conservative than the default method of load
application. The use of this option may be useful for routing special vehicles whose
loads are well known. However, for notional loads that represent a distribution or
envelope of unknown vehicle loadings, the default method may be more appropriate.
Width Effects
Fixed-width loads will be moved transversely across the width of a Lane for maximum effect if the Lane is wider than the load. If the Lane is narrower than the load,
the load will be centered on the Lane and its width reduced to be equal to that of the
Lane, keeping the total magnitude of the load unchanged.
The load at each longitudinal location in the vehicle is independently moved across
the width of the Lane. This means that the front, back, and middle of the vehicle

Vehicle Live Loads

493

CSI Analysis Reference Manual
may not occupy the same transverse location in the lane when placed for maximum
effect.

Length Effects
You may specify that the magnitude of the loading depends on lane length using
built-in or user-defined length functions. One function may be used to affect the
concentrated (axle) loads, and another function may be used for the distributed
loads. These functions act as scale factors on the specified load values.
Concentrated (Axle) Loads
If you specify a length-effect function for the axle loads, all axle loads will be
scaled equally by the function, including floating axle loads. Built-in length-effect
functions include the AASHTO Standard Impact function and the JTG-D60 Lane
load function. You may define your own function.
The intent of this function is to scale the load according to span length. In a given
structure, there may not be a constant span length, so the program uses the influence
line to determine what span length to use. This may differ for each computed response quantity, and may not always correspond to the obvious span length in the
global structure.
For a given response quantity, the maximum point on the influence line is found,
and the distance between the zero-crossings on either side of this maximum is taken
to be the span length. For the three influence lines of Figure 86 (page 486), this
would result in a span length of half the distance between the supports for the shear
in (a), and the full distance between the supports for the moments in (b) and ©). For
shear near the support, the span length would be essentially the same as the distance
between the support.
This approach generally works well for moments and for shear near the supports. A
shorter span length is computed for shear near midspan, but here the shear is
smaller anyway, so it is not usually of concern.
Distributed Loads
If you specify a length-effect function for the distributed loads, all distributed loads
will be scaled equally by the function. Built-in length-effect functions include the
AASHTO Standard Impact function and the British HA function. You may define
your own function.

494

Vehicle Live Loads

Chapter XXVI

Moving-Load Analysis

The intent of this function is to scale the load according to the loaded length, but not
unconservatively. The influence line is used to determine the loaded length for each
individual response quantity. Only loaded lengths that increase the severity of the
response are considered.
To prevent long lengths of small influence from unconservatively reducing the response, an iterative approach is used where the length considered is progressively
increased until the maximum response is computed. Any further increases in length
that reduce the response due to decreasing function value are ignored.
On the other hand, the loaded length used for scaling is never reduced below the
length of a single span, which is determined separately for each influence line as the
distance between zero crossings on either side of the point of maximum influence.

Application of Loads in Multi-Step Analysis
Vehicles can be moved in a multi-step analysis. This can use either Multi-Step
Static Load Cases or Time-History Load Cases, the latter of which can be linear or
nonlinear. Currently only vertical loading is considered for multi-step analysis.
Influence surfaces are not used for this type of analysis. Rather, CSiBridge creates
many internal Load Patterns representing different positions of the vehicles along
the length of the lanes.
Only axle loads are considered; the uniform loads are not applied. In the case of a
variable axle spacing, the minimum distance is used. The transverse distribution of
the axle loads is considered. The vehicle is moved longitudinally along the centerline of the lane; it is not moved transversely within the lane. To consider different
transverse positions, you can define additional lanes.
The full magnitude of the loads are applied, regardless of whether they increase or
decrease the severity of the response. Each step in the analysis corresponds to a specific position of each vehicle acting in its lane. All response at that step is fully correlated.

General Vehicle
The general Vehicle may represent an actual vehicle or a notional vehicle used by a
design code. Most trucks and trains can be modeled by the general Vehicle in
CSiBridge.

General Vehicle

495

CSI Analysis Reference Manual
pm

pxm

pn-1

Leading
w1

Trailing
wn+1

Notes:
(1) All loads are point loads or uniform line loads acting on the Lane center line
(2) Any of the point loads or uniform line loads may be zero
(3) The number of axles, n, may be zero or more
(4) One of the inter-axle spacings, d2 through dn, may vary over a specified range
(5) The locations of loads pm and pxm are arbitrary

Figure 87
General Vehicle Definition

The general Vehicle consists of n axles with specified distances between them.
Concentrated loads may exist at the axles. Uniform loads may exist between pairs
of axles, in front of the first axle, and behind the last axle. The distance between any
one pair of axles may vary over a specified range; the other distances are fixed. The
leading and trailing uniform loads are of infinite extent. Additional “floating” concentrated loads may be specified that are independent of the position of the axles.
By default for influence surface analysis, applied loads never decrease the severity
of the computed response, so the effect of a shorter Vehicle is captured by a longer

496

General Vehicle

Chapter XXVI

Moving-Load Analysis

Vehicle that includes the same loads and spacings as the shorter Vehicle. Only the
longer Vehicle need be considered in such cases.
If you choose the option to allow loads to reduce the severity of response, then you
must consider the shorter and longer vehicles, if they both apply. This is also true
for step-by-step analysis.

Specification
To define a Vehicle, you may specify:
• n–1 positive distances, d, between the pairs of axles; one inter-axle distance
may be specified as a range from dmin to dmax, where 0 < dmin £ dmax, and
dmax = 0 can be used to represent a maximum distance of infinity
• n concentrated loads, p, at the axles, including the transverse load distribution
for each
• n+1 uniform loads, w: the leading load, the inter-axle loads, and the trailing
load, including the transverse load distribution for each
• Floating axle loads:
– Load pm for superstructure moments, including its transverse distribution.
You may specify whether or not to double this load for negative superstructure moments over the supports, as described below
– Load pxm for all response quantities except superstructure moments, including its transverse distribution
• Whether or not this Vehicle is to be used for calculating:
– “Negative” superstructure moments over the supports
– Reaction forces at interior supports
– Response quantities other than the two types above
• Minimum distances between the axle loads and the edges of the lane; by default
these distances are zero
• Whether or not the vehicle must remain fully within the length of lane
• Whether or not to automatically scale the magnitude of the axle loads based on
the loaded length of the lane according to the Chinese JTG or other codes
• Whether or not to automatically scale the magnitude of the uniform loads based
on the loaded length of the lane according to the British or other codes
• Whether or not to consider vertical loading, and whether or not to include the
corresponding overturning moments due to super-elevation
General Vehicle

497

CSI Analysis Reference Manual
• Whether or not to consider braking and acceleration loading, and the scale factors defining these loads
• Whether or not to consider centrifugal loading, the scale factors defining these
loads, and whether or not to include the corresponding overturning moments
The number of axles, n, may be zero, in which case only a single uniform load and
the floating concentrated loads can be specified.
These parameters are illustrated in Figure 87 (page 496). Some specific examples
are given in Topic “Standard Vehicles” (page 500). Additional detail is provided in
the following.

Moving the Vehicle
When a Vehicle is applied to a traffic Lane, the axles are moved along the length of
the lane to where the maximum and minimum values are produced for every response quantity in every element. Usually this location will be different for each response quantity. For asymmetric (front to back) Vehicles, both directions of travel
are considered.

Vehicle Response Components
Certain features of the AASHTO H, HS, and HL vehicular live loads (AASHTO,
2004) apply only to certain types of bridge response, such as negative moment in
the superstructure or the reactions at interior supports. CSiBridge uses the concept
of vehicle response components to identify these response quantities. You select
the objects that need special treatment, and assign the appropriate vehicle response
components to them.
The different types of available vehicle response components are described in the
following subtopics.
Vehicle response components do not apply to SAP2000.

Superstructure (Span) Moment
For AASHTO H and HS “Lane” loads, the floating axle load pm is used for calculating the superstructure moment. How this moment is represented depends on the
type of model used. For all other types of response, the floating axle load pxm is
used.

498

Vehicle Response Components

Chapter XXVI

Moving-Load Analysis

The general procedure is to select the elements representing the superstructure and
assign vehicle response components “H and HS Lane Loads – Superstructure Moment” to the desired response quantities, as described next.
For a spine (spline) model where the superstructure is modeled as a line of frame elements, superstructure moment corresponds to frame moment M3 for elements
where the local-2 axis is in the vertical plane (the default.) Thus you would select
all frame elements representing the superstructure and assign the vehicle response
components to M3, indicating to “Use All Values” (i.e., positive and negative.)
Load pm will be used for computing M3 of these elements.
For a full-shell model of the superstructure, superstructure moment corresponds to
longitudinal stresses or membrane forces in the shell elements. Assuming the local-1 axes of the shell elements are oriented along the longitudinal direction of the
bridge, you would select all shell elements representing the superstructure and assign the vehicle response components to S11 and/or F11, indicating to “Use All
Values” (i.e., positive and negative.) You could also make this same assignment to
shell moments M11. Load pm will be used for computing any components you
have so assigned.

Negative Superstructure (Span) Moment
For AASHTO H and HS “Lane” loads, the floating axle load pm is applied in two
adjacent spans for calculating the negative superstructure moment over the
supports. Similarly, for AASHTO HL loads, a special double-truck vehicle is used
for calculating negative superstructure moment over interior supports. Negative
moment here means a moment that causes tension in the top of the superstructure,
even if the sign of the CSiBridge response is positive due to a particular choice of
local axes.
The procedure for different types of structures is very similar to that described
above for superstructure moment: select the elements representing the superstructure, but now assign vehicle response components “H, HS and HL Lane Loads –
Superstructure Negative Moment over Supports” to the desired response quantities. However, we have to decide how to handle the sign.
There are two general approaches. Let's consider the case of the spine model with
frame moment M3 representing superstructure moment:
(1) You can select the entire superstructure, and assign the vehicle response components to M3, indicating to “Use Negative Values”. Only negative values of
M3 will be computed using the double pm or double-truck load.

Vehicle Response Components

499

CSI Analysis Reference Manual
(2) You can select only that part of the superstructure within a pre-determined negative-moment region, such as between the inflection points under dead load.
Assign the vehicle response components to M3, indicating to “Use Negative
Values” or “Use All Values.”
The first approach may be slightly more conservative, giving negative moments
over a larger region. However, it does not require you to determine a negative-moment region.
The situation with the shell model is more complicated, since negative moments
correspond to positive membrane forces and stresses at the top of the superstructure, negative values at the bottom of the superstructure, and changing sign in between. For this reason, approach (2) above may be better: determine a negative-moment region, then assign the vehicle response components to the desired shell
stresses, membrane forces, and/or moments, indicating to “Use All Values.” This
avoids the problem of sign where it changes through the depth.

Reactions at Interior Supports
For AASHTO HL loads, a special double-truck vehicle is used for calculating the
reactions at interior supports. It is up to you to determine what response components you want to be computed for this purpose. Choices could include:
• Vertical upward reactions, or all reactions, for springs and restraints at the base
of the columns
• Compressive axial force, or all forces and moments, in the columns
• Compressive axial force, or all forces and moments, in link elements representing bearings
• Bending moments in outriggers at the columns
The procedure is as above for superstructure moment. Select the elements representing the interior supports and assign the vehicle response components “HL – Reactions at Interior Supports” to the desired response quantities. Carefully decide
whether you want to use all values, or only negative or positive values. You will
have to repeat this process for each type of element that is part of the interior supports: joints, frames, links, shells, and/or solids.

Standard Vehicles
There are many standard vehicles available in CSiBridge to represent vehicular live
loads specified in various design codes. More are being added all the time. A few

500

Standard Vehicles

Chapter XXVI

Moving-Load Analysis

examples are provided here for illustrative purposes. Only the longitudinal distribution of loading is shown in the figures. Please see the graphical user interface for
all available types and further information.
Hn-44 and HSn-44
Vehicles specified with type = Hn-44 and type = HSn-44 represent the AASHTO
standard H and HS Truck Loads, respectively. The n in the type is an integer scale
factor that specifies the nominal weight of the Vehicle in tons. Thus H15-44 is a
nominal 15 ton H Truck Load, and HS20-44 is a nominal 20 ton HS Truck Load.
These Vehicles are illustrated in Figure 88 (page 503).
The effect of an H Vehicle is included in an HS Vehicle of the same nominal
weight. If you are designing for both H and HS Vehicles, only the HS Vehicle is
needed.
Hn-44L and HSn-44L
Vehicles specified with type = Hn-44L and type = HSn-44L represent the
AASHTO standard H and HS Lane Loads, respectively. The n in the type is an integer scale factor that specifies the nominal weight of the Vehicle in tons. Thus
H15-44 is a nominal 15 ton H Lane Load, and HS20-44 is a nominal 20 ton HS
Lane Load. These Vehicles are illustrated in Figure 88 (page 503). The Hn-44L and
HSn-44L Vehicles are identical.
AML
Vehicles specified with type = AML represent the AASHTO standard Alternate
Military Load. This Vehicle consists of two 24 kip axles spaced 4 ft apart.
HL-93K, HL-93M and HL-93S
Vehicles specified with type = HL-93K represent the AASHTO standard HL-93
Load consisting of the code-specified design truck and the design lane load.
Vehicles specified with type = HL-93M represent the AASHTO standard HL-93
Load consisting of the code-specified design tandem and the design lane load.
Vehicles specified with type = HL-93S represent the AASHTO standard HL-93
Load consisting of two code-specified design trucks and the design lane load, all
scaled by 90%. The axle spacing for each truck is fixed at 14 ft. The spacing between the rear axle of the lead truck and the lead axle of the rear truck varies from
50 ft to the length of the Lane. This vehicle is only used for negative superstructure

Standard Vehicles

501

CSI Analysis Reference Manual
moment over supports and reactions at interior supports. The response will be zero
for all response quantities that do not have the appropriately assigned vehicle response components.
A dynamic load allowance may be specified for each Vehicle using the parameter
im. This is the additive percentage by which the concentrated truck or tandem axle
loads will be increased. The uniform lane load is not affected. Thus if im = 33, all
concentrated axle loads for the vehicle will be multiplied by the factor 1.33.
These Vehicles are illustrated in Figure 89 (page 504) for im = 0.
P5, P7, P9, P11, and P13
Vehicles specified with type = P5, type = P7, type = P9, type = P11, and type =
P13 represent the Caltrans standard Permit Loads. These Vehicles are illustrated in
Figure 90 (page 505).
The effect of a shorter Caltrans Permit Load is included in any of the longer Permit
Loads. If you are designing for all of these permit loads, only the P13 Vehicle is
needed.
Cooper E 80
Vehicles specified with type = COOPERE80 represent the AREA standard Cooper
E 80 train load. This Vehicle is illustrated in Figure 91 (page 506).
UICn
Vehicles specified with type = UICn represent the European UIC (or British RU)
train load. The n in the type is an integer scale factor that specifies magnitude of the
uniform load in KN/m. Thus UIC80 is the full UIC load with an 80 kn/m uniform
load, and UIC60 is the UIC load with an 60 kn/m uniform load. The concentrated
loads are not affected by n.
This Vehicle is illustrated in Figure 91 (page 506).
RL
Vehicles specified with type = RL represent the British RL train load. This Vehicle
is illustrated in Figure 91 (page 506).

502

Standard Vehicles

Chapter XXVI

Moving-Load Analysis

32 k

14'
H20-44 Truck Load

32 k

14'

14' to 30'

HS20-44 Truck Load

26 k
pxm

18 k
pm

0.640 k/ft
¥
H20-44L and HS20-44L Lane Loads

Figure 88
AASHTO Standard H and HS Vehicles

Standard Vehicles

503

CSI Analysis Reference Manual
25 k 25 k

Note: All point loads will be increased
by the dynamic load allowance,
im, expressed as a percentage
0.640 k/ft
¥

HL-93M Tandem and Lane Load

32 k

0.640 k/ft
¥

14'

14' to 30'

HL-93K Truck and Lane Load

28.8 k

7.2 k

28.8 k

7.2 k

0.576 k/ft
¥

14'

50' to ¥

14'

HL-93S Truck and Lane Load for Negative Moment and Reactions at Interior Piers

Figure 89
AASHTO Standard HL Vehicles

504

Standard Vehicles

Chapter XXVI
48 k

Moving-Load Analysis

48 k

26 k

P5 Permit Load

18'

48 k

26 k

P7 Permit Load

18'

48 k

18'

48 k

26 k

P9 Permit Load

18'

48 k

18'

48 k

18'

48 k

26 k

P11 Permit
Load

18'

48 k

18'

48 k

18'

48 k

18'

P13 Permit
Load

48 k

26 k

18'

Figure 90
Caltrans Standard Permit Vehicles

Standard Vehicles

505

CSI Analysis Reference Manual
4 @ 80 k

4 @ 80 k
4 @ 52 k

40 k

4 @ 52 k
40 k

8 k/ft
8'

5' 5' 5'

5' 6' 5'

5' 5' 5'

5' 6' 5' 5'

Cooper E 80 Train Load

250 kN

80 kN/m
¥

80 kN/m
0.8 m

1.6 m

0.8 m

UIC80 Train Load
200 kN
px

50 kN/m
25 kN/m
¥

25 kN/m
100 m

RL Train Load

Figure 91
Standard Train Vehicles

506

Standard Vehicles

Chapter XXVI

Moving-Load Analysis

Eurocode Vehicles
Vehicles are available for the four Load Models of the European Standard EN
1991-2:2003.
There are eight vehicles in total that represent Load Model 1. Each vehicle combines the tandem system TS (concentrated load) with the UDL system (uniform
load), but with different scale factors.
For use as a characteristic load, there are separate vehicles for loading the first, second, third, and subsequent lanes. These are given in the table below:
Vehicle

Location

TS, Axle Load
Qik (KN)

UDL Load
qik (KN/m2)

Euro_LM1_Lane1_Char

Lane Number 1

300

Euro_LM1_Lane2_Char

Lane Number 2

200

2.5

Euro_LM1_Lane3_Char

Lane Number 3

100

2.5

Euro_LM1_Other_Char

Other lanes

2.5

A moving-load case defined for use as a characteristic load, and having four or
more lanes, should apply a single instance each of the first three vehicles to all the
lanes and apply multiple instances of the last vehicle to all lanes. The automatic
permutations in the moving load case will consider the most severe combination of
the vehicles loading the various lanes. If there are fewer than four lanes, the latter
vehicles are not needed, respectively.
For use as a frequent load, there are separate vehicles for loading the first, second,
third, and subsequent lanes. These are given in the table below:
Vehicle

Location

TS, Axle Load
Qik (KN)

UDL Load
qik (KN/m2)

Euro_LM1_Lane1_Freq

Lane Number 1

225

3.6

Euro_LM1_Lane2_Freq

Lane Number 2

150

1.0

Euro_LM1_Lane3_Freq

Lane Number 3

1.0

Euro_LM1_Other_Freq

Other lanes

1.0

Because of the different ratios of TS and UDL load, separate moving-load cases
need to be defined for characteristic and frequent loading.
Standard Vehicles

507

CSI Analysis Reference Manual
A moving-load case defined for use as a frequent load, and having four or more
lanes, should apply a single instance each of the first three vehicles to all the lanes
and apply multiple instances of the last vehicle to all lanes. The automatic permutations in the moving load case will consider the most severe combination of the vehicles loading the various lanes. If there are fewer than four lanes, the latter vehicles
are not needed, respectively.
A single vehicle is available for Load Model 2, Euro_LM2, that applies a single
axle load. This should be applied in a moving-load case that loads all the lanes, but
only a single lane at a time.
There are multiple vehicles available to represent the various types defined for
Load Model 3. For vehicles with 100 to 200 kn axle-lines, the axle loads are applied
as a knife-edge load distributed over a 2.7 m width. For vehicles with 240 kn
axle-lines, the axle loads are applied as a knife-edge load distributed over a 4.2 m
width. These can be combined with the Load Model 1 vehicles in a moving-load
case, loading separate lanes. The 240 kn axle-lines are not automatically applied to
two adjacent lanes. Instead, you will need to define a new lane that is double-wide
and use that lane in the moving-load case in place of the two adjacent lanes.
A single vehicle is available for Load Model 4, Euro_LM4, that applies a uniform
load. This should be applied in a moving-load case that loads all lanes simultaneously. Additional lanes may need to be defined to represent areas that may be
loaded by pedestrians but are not otherwise used for traffic.

Vehicle Classes
The designer is often interested in the maximum and minimum response of the
bridge to the most extreme of several types of Vehicles rather than the effect of the
individual Vehicles. For this purpose, Vehicle Classes are defined that may include
any number of individual Vehicles. The maximum and minimum force and displacement response quantities for a Vehicle Class will be the maximum and minimum values obtained for any individual Vehicle in that Class. Only one Vehicle
ever acts at a time.
For influence-based analyses, all Vehicle loads are applied to the traffic Lanes
through the use of Vehicle Classes. If it is desired to apply an individual Vehicle
load, you must use a Vehicle Class that contains only that single Vehicle. Such single-vehicle Classes are automatically created for each Vehicle, and cannot be
changed. You need to define your own Vehicle Classes only if you want to envelope multiple Vehicles or change the scale factor on a single Vehicle.

508

Vehicle Classes

Chapter XXVI

Moving-Load Analysis

For example, the you may need to consider the most severe of a Truck Load and the
corresponding Lane Load, say the HS20-44 and HS20-44L loads. A Vehicle Class
can be defined to contain these two Vehicles. Additional Vehicles, such as the Alternate Military Load type AML, could be included in the Class as appropriate. Different members of the Class may cause the most severe response at different locations in the structure.
For HL-93 loading, you would first define three Vehicles, one each of the standard
types HL-93K, HL-93M, and HL-93S. You then could define a single Vehicle
Class containing all three Vehicles.
For step-by-step analysis, Vehicle loads are applied directly without the use of
Classes, since no enveloping is performed.

Moving-Load Load Cases
The final step in the definition of the influence-based vehicle live loading is the application of the Vehicle Classes to the traffic Lanes. This is done by creating independent Moving-Load Load Cases.
A Moving-Load Load Case is a type of Load Case. Unlike most other Load Cases,
you cannot apply Load Patterns in a Moving-Load Load Case. Instead, each Moving-Load Load Case consists of a set of assignments that specify how the Classes
are assigned to the Lanes.
Each assignment in a Moving-Load Load Case requires the following data:
• A Vehicle Class, class
• A scale factor, sf, multiplying the effect of class (the default is unity)
• A list, lanes, of one or more Lanes in which class may act (the default is all
Lanes)
• The minimum number, lmin, of Lanes lanes in which class must act (the default is zero)
• The maximum number, lmax, of Lanes lanes in which class may act (the default is all of lanes)
The program looks at all of the assignments in a Moving-Load Load Case, and tries
every possible permutation of loading the traffic Lanes with Vehicle Classes that is
permitted by the assignments. No Lane is ever loaded by more than one Class at a
time.

Moving-Load Load Cases

509

CSI Analysis Reference Manual
You may specify multiple-lane scale factors, rf1, rf2, rf3, ..., for each Moving-Load Load Case that multiply the effect of each permutation depending upon
the number of loaded Lanes. For example, the effect of a permutation that loads two
Lanes is multiplied by rf2.
The maximum and minimum response quantities for a Moving-Load Load Case
will be the maximum and minimum values obtained for any permutation permitted
by the assignments. Usually the permutation producing the most severe response
will be different for different response quantities.
The concepts of assignment can be clarified with the help of the following examples.

Directions of Loading
For each moving-load load case, three scale factors are specified to multiply and
combine the vertical load (cfv), braking/acceleration load (cfb), and centrifugal
load (cfc) for all vehicles acting in this load case. By default, cfv = 1 and cfb = cfc =
0. When two or more factors are non-zero, the effects of the different directions of
loading for a given vehicle are considered simultaneously for each position of the
vehicle in the lane. This is more accurate and less over-conservative than considering the three directions of loading separately and then adding them together later in
a load combination.
Important Note! The overturning load due to centrifugal load is restricted so as not
to cause uplift on the inner or upward side of the vehicle. In particular, no overturning moments will be considered for a load case where the vertical load is zero. For
this reason, it is recommended to combine full vertical load with centrifugal load if
overturning moments are important. A centrifugal load case by itself will exclude
overturning moments, even if later included in a load combination with vertical
load cases. See topic “Vehicle Live Loads” (page 487) for more information.
When multiple directions of loading are considered in a moving-load load case, the
following permutations are automatically considered during analysis depending
upon the type of combination requested by the choice of scale factors:

510

Combination

Vertical (V)

Braking (B)

Centrif. ©)

V only

cfv

B only

cfb

C only

cfc

Moving-Load Load Cases

Double

Chapter XXVI

Combination

Moving-Load Analysis

Vertical (V)

Braking (B)

Centrif. ©)

Double

cfv

cfb

cfv

-cfb

cfv

cfc

cfv

cfb

cfc

cfb

-cfb

cfc

-cfb

cfv

cfb

cfc

cfv

cfb

cfv

-cfb

cfc

cfv

-cfb

V+B

V+C

B+C

V+B+C

For vehicles with a non-zero skew factor specified for braking and acceleration
loads, the permutations indicated with (*) in the Double column will be doubled to
consider both signs of the transverse load due to skew braking/acceleration.
Note that for the “B only” case, the results are automatically enveloped in both directions without any additional computational effort.
Comparing the computational effort to consider all three directions of loading in a
single load case versus running them in separate load cases and then adding them
together later in load combinations: A single load case requires four permutations,
whereas the three individual load cases only require three permutations. However,
running all three in a single load case generally provides better results and allows
consideration of overturning moments. If the three directions of loading are to be
combined with various different sets of scale factors, doing so with load combinations is clearly more efficient than running multiple load cases, although again less
accurate.
In general, it is recommended to combine the various directions of loading in the
load cases rather than load combinations.

Moving-Load Load Cases

511

CSI Analysis Reference Manual

Example 1 — AASHTO HS Loading
Consider a four-lane bridge designed to carry AASHTO HS20-44 Truck and Lane
Loads, and the Alternate Military Load (AASHTO, 1996). Suppose that it is required that the number of Lanes loaded be that which produces the most severe response in every member. Only one of the three Vehicle loads is allowed per lane.
Load intensities may be reduced by 10% and 25% when three or four Lanes are
loaded, respectively.
Generally, loading all of the Lanes will produce the most severe moments and
shears along the span and axial forces in the piers. However, the most severe torsion
of the bridge deck and transverse bending of the piers will usually be produced by
loading only those Lanes possessing eccentricities of the same sign.
Assume that the bridge structure and traffic Lanes have been defined. Three Vehicles are defined:
• name = HSK, type = HS20-44
• name = HSL, type = HS20-44L
• name = AML, type = AML
where name is an arbitrary label assigned to each Vehicle. The three Vehicles are
assigned to a single Vehicle Class, with an arbitrary label of name = HS, so that the
most severe of these three Vehicle loads will be used for every situation.
A single Moving-Load Load Case is then defined that seeks the maximum and
minimum responses throughout the structure for the most severe of loading all four
Lanes, any three Lanes, any two Lanes or any single Lane. This can be accomplished using a single assignment. The parameters for the assignment are:
• class = HS
• sf = 1
• lanes = 1, 2, 3, 4
• lmin = 1
• lmax = 4
The scale factors for the loading of multiple Lanes in the set of assignments are rf1
= 1, rf2 = 1, rf3 = 0.9, and rf4 = 0.75.
There are fifteen possible permutations assigning the single Vehicle Class HS to
any one, two, three, or four Lanes. These are presented in the following table:

512

Moving-Load Load Cases

Chapter XXVI

Permutation

Lane 1

Lane 2

Lane 3

HS
HS

1.00
HS

HS
HS

7
HS

HS
HS

14
HS

1.00
HS

1.00

1.00
1.00

Scale Factor

1.00

Lane 4

1.00

Moving-Load Analysis

1.00
HS

1.00
0.90

0.90

0.75

An “HS” in a Lane column of this table indicates application of Class HS; a blank
indicates that the Lane is unloaded. The scale factor for each permutation is determined by the number of Lanes loaded.

Example 2 — AASHTO HL Loading
Con sider a four- lane bridge designed to carry AASHTO HL- 93 loading
(AASHTO, 2004). The approach is the same as used for AASHTO HS loading in
the previous example. Only the multiple-lane scale factors and the Vehicles differ.
Three Vehicles are defined:
• name = HLK, type = HL-93K
• name = HLM, type = HL-93M
• name = HLS, type = HL-93S
Moving-Load Load Cases

513

CSI Analysis Reference Manual
where name is an arbitrary label assigned to each Vehicle.
The three Vehicles are assigned to a single Vehicle Class, with an arbitrary label of
name = HL, so that the most severe of these three Vehicle loads will be used for
every situation. By definition of the standard Vehicle type HL-93S, Vehicle HLS
will only be used when computing negative moments over supports or the reaction
at interior piers. The other two Vehicles will be considered for all response quantities.
A single Moving-Load Load Case is then defined that is identical to that of the previous example, except that class = HL, and the scale factors for multiple Lanes are
rf1 = 1.2, rf2 = 1, rf3 = 0.85, and rf4 = 0.65.
There are again fifteen possible permutations assigning the single Vehicle Class
HL to any one, two, three, or four Lanes. These are similar to the permutations of
the previous example, with the scale factors changed as appropriate.

Example 3 — Caltrans Permit Loading
Consider the four-lane bridge of the previous examples now subject to Caltrans
Combination Group I PW (Caltrans, 1995). Here the permit load(s) are to be used
alone in a single traffic Lane, or in combination with one HS or Alternate Military
Load in a separate traffic lane, depending upon which is more severe.
Four Vehicles are defined:
• name = HSK, type = HS20-44
• name = HSL, type = HS20-44L
• name = AML, type = AML
• name = P13, type = P13
where name is an arbitrary label assigned to each Vehicle.
The first three Vehicles are assigned to a Vehicle Class that is given the label name
= HS, as in Example 1. The last Vehicle is assigned as the only member of a Vehicle
Class that is given the label name = P13. Note that the effects of CSiBridge Vehicle
types P5, P7, P9, and P11 are captured by Vehicle type P13.
Combination Group I PW is then represented as a single Moving-Load Load Case
consisting of the assignment of Class P13 to any single Lane with or without Class
HS being assigned to any other single Lane. This can be accomplished using two
assignments. A scale factor of unity is used regardless of the number of loaded
Lanes.

514

Moving-Load Load Cases

Chapter XXVI

Moving-Load Analysis

The first assignment assigns Class P13 to any single Lane:
• class = P13
• sf = 1
• lanes = 1, 2, 3, 4
• lmin = 1
• lmax = 1
The second assignment assigns Class HS to any single Lane, or to no Lane at all:
• class = HS
• sf = 1
• lanes = 1, 2, 3, 4
• lmin = 0
• lmax = 1
There are sixteen possible permutations for these two assignments such that no
Lane is loaded by more than one Class at a time. These are presented in the following table:
Permutation

Lane 1

Lane 2

Lane 3

Lane 4

Scale Factor
1.00

1.00
HS

1.00

9
10
11

HS
HS

1.00
HS

1.00

Moving-Load Load Cases

515

CSI Analysis Reference Manual

Permutation

Lane 1

Lane 2

12
13

Lane 3

Lane 4

Scale Factor

1.00

14
15

HS
HS

Example 4 — Restricted Caltrans Permit Loading
Consider the four-Lane bridge and the Caltrans permit loading of Example 3, but
subject to the following restrictions:
• The permit Vehicle is only allowed in Lane 1 or Lane 4
• The Lane adjacent to the Lane occupied by the permit Vehicle must be empty
Two Moving-Load Load Cases are required, each containing two assignments. A
scale factor of unity is used regardless of the number of loaded Lanes.
The first Moving-Load Load Case considers the case where the permit Vehicle occupies Lane 1. The first assignment assigns Class P13 to Lane 1
• class = P13
• sf = 1
• lanes = 1
• lmin = 1
• lmax = 1
The second assignment assigns Class HS to either Lane 3 or 4, or to no Lane at all:
• class = HS
• sf = 1
• lanes = 3, 4
• lmin = 0
• lmax = 1
These assignments permits the following three permutations:

516

Moving-Load Load Cases

Chapter XXVI

Permutation

Lane 1

Lane 2

Lane 3

Moving-Load Analysis

Lane 4

Scale Factor
1.00

1.00
HS

1.00

Similarly, the second Moving-Load Load Case considers the case where the permit
Vehicle occupies Lane 4. The first assignment assigns Class P13 to Lane 4
• class = P13
• sf = 1
• lanes = 4
• lmin = 1
• lmax = 1
The second assignment assigns Class HS to either Lane 1 or 2, or to no Lane at all:
• class = HS
• sf = 1
• lanes = 1, 2
• lmin = 0
• lmax = 1
These assignments permits the following three permutations:
Permutation

Lane 1

Lane 2

1
2
3

HS
HS

Lane 3

Lane 4

Scale Factor

1.00

An envelope-type Combo that includes only these two Moving-Load Load Cases
would produce the most severe response for the six permutations above.
See Topic “Load Combinations (Combos)” (page 351) in Chapter “Load Cases”
for more information.

Moving-Load Load Cases

517

CSI Analysis Reference Manual

Example 5 — Eurocode Characteristic Load Model 1
Consider a five-lane bridge Eurocode Load Model 1 for use as a characteristic load.
There are separate vehicles for each of the first three lanes, and a fourth vehicle for
the remaining lanes. All permutations of vehicles loading the lanes need to be considered.
Four Vehicles are defined:
• name = Load1, type = Euro_LM1_Lane1_Char
• name = Load2, type = Euro_LM1_Lane2_Char
• name = Load3, type = Euro_LM1_Lane3_Char
• name = LoadX, type = Euro_LM1_Other_Char
where name is an arbitrary label assigned to each Vehicle.
Each vehicle is assigned automatically to a Vehicle Class of the same name.
The characteristic load is then represented as a single Moving-Load Load Case
consisting of the assignment of each of the first three vehicles to a single lane, and
the fourth vehicle to the remaining lanes. This can be accomplished using four assignments. A scale factor of unity is used regardless of the number of loaded Lanes.
The first assignment assigns Class Load 1 to any single Lane:
• class = Load1
• sf = 1
• lanes = 1, 2, 3, 4, 5
• lmin = 1
• lmax = 1
A similar assignment is made for the second and third vehicles.
The fourth assignment assigns Class LoadX to the remaining lanes:
• class = LoadX
• sf = 1
• lanes = 1, 2, 3, 4, 5
• lmin = 2
• lmax = 2

518

Moving-Load Load Cases

Chapter XXVI

Moving-Load Analysis

There are 60 possible permutations for these four assignments such that every Lane
is loaded by a single Class at a time. These permutations will be automatically created. Some of these are presented in the following table:
Permutation

Lane 1

Lane 2

Lane 3

Lane 4

Lane 5

Load1

Load2

Load3

LoadX

Load1

Load2

LoadX

Load3

LoadX

Load1

Load2

LoadX

Load3

Load1

Load3

Load2

LoadX

Load1

Load3

LoadX

Load2

LoadX

…

LoadX

Load3

Load2

Load1

Considering the possibility that the lanes loaded by LoadX are not loaded at all increases the number of permutations from 60 to 240. However, this is not necessary,
since the loading will not be applied in the case that it decreases the severity of the
response.
A similar moving-load case can be defined for applying the frequent Load Model 1
vehicles to the Lanes.

Moving Load Response Control
Several parameters are available for controlling influence-based Moving-Load
Load Cases. These have no effect on step-by-step analysis.

Bridge Response Groups
By default, moving-load response is calculated for all joints and elements. Because
this calculation is computationally intensive, you have the option to restrict this calculation to a portion of the structure.
For each of the following types of response, you may request a Group of elements
for which the response should be calculated:
• Joint displacements
• Joint reactions
Moving Load Response Control

519

CSI Analysis Reference Manual
• Frame forces and moments
• Shell stresses
• Shell resultant forces and moments
• Plane stresses
• Solid stresses
• Link/support forces and deformations
If the displacements, reactions, spring forces, or internal forces are not calculated
for a given joint or Frame element, no Moving Load response can be printed or
plotted for that joint or element. Likewise, no response can be printed or plotted for
any Combo that contains a Moving-Load Load Case.
Additional control is available as described in the following subtopics.

Correspondence
For each maximum or minimum Frame-element response quantity computed, the
corresponding values for the other five internal force and moment components may
be determined. For example, the shear, moment, and torque that occur at the same
time as the maximum axial force in a Frame element may be computed.
Similarly, corresponding displacements, stresses, forces and moments can be computed for any response quantity of any element type. Only the corresponding values
for each joint or element are computed at each output location. If you want to see
the full corresponding state of the structure, you must use step-by-step analysis.
By default, no corresponding quantities are computed since this significantly increases the computation time for moving-load response.

Influence Line Tolerance
CSiBridge simplifies the influence lines used for response calculation in order to
increase efficiency. A relative tolerance is used to reduce the number of load points
by removing those that are approximately duplicated or that can be approximately
linearly-interpolated. The default value of this tolerance permits response errors on
the order of 0.01%. Setting the tolerance to zero will provide exact results to within
the resolution of the analysis.

520

Moving Load Response Control

Chapter XXVI

Moving-Load Analysis

Exact and Quick Response Calculation
For the purpose of moving a Vehicle along a lane, each axle is placed on every load
point in turn. When another axle falls between two load points, the effect of that
axle is determined by linear interpolation of the influence values. The effect of uniform loads is computed by integrating the linearly-interpolated segments of the influence line. This method is exact to within the resolution of the analysis, but is
computationally intensive if there are many load points.
A “Quick” method is available which may be much faster than the usual “Exact”
method, but it may also be less accurate. The Quick method approximates the influence line by using a limited number of load points in each “span.” For purposes of
this discussion, a span is considered to be a region where the influence line is all
positive or all negative.
The degree of approximation to be used is specified by the parameter quick, which
may be any non-negative integer. The default value is quick = 0, which indicates to
use the full influence line, i.e., the Exact method.
Positive values indicate increasing degrees of refinement for the Quick method. For
quick = 1, the influence line is simplified by using only the maximum or minimum
value in each span, plus the zero points at each end of the span. For quick = 2, an
additional load point is used on either side of the maximum/minimum. Higher degrees of refinement use additional load points. The number of points used in a span
quick
can be as many as 2 +1, but not more than the number of load points available in
the span for the Exact method.
It is strongly recommended that quick = 0 be used for all final analyses. For preliminary analyses, quick = 1, 2, or 3 is usually adequate, with quick = 2 often providing a good balance between speed and accuracy. The effect of parameter quick
upon speed and accuracy is problem-dependent, and you should experiment to determine the best value to use for each different model.

Step-By-Step Analysis
Step-by-step analysis can consider any combination of Vehicles operating on the
Lanes. Multiple Vehicles can operate simultaneously, even in the same Lane if desired. You define a Load Pattern of type “Vehicle Live,” in which you specify one
or more sets of the following:
• Vehicle type
• Lane in which it is traveling
Step-By-Step Analysis

521

CSI Analysis Reference Manual
• Starting position in the Lane
• Starting time
• Vehicle speed
• Direction (forward or backward, relative to the Lane direction)
You also specify a time-step size and the total number of time steps to be considered. The total duration of loading is the product of these two. To get a finer spatial
discretization of loading, use smaller time steps, or reduce the speed of the vehicles.

Loading
This type of Load Pattern is multi-stepped. It automatically creates a different pattern of loading for each time step. At each step, the load applied to the structure is
determined as follows:
• The longitudinal position of each Vehicle in its Lane at the current time is determined from its starting position, speed and direction.
• The Vehicle is centered transversely in the Lane.
• Axle loads are applied to the bridge deck. Concentrated axles loads are applied
as specified. Distributed axle loads are converted to four equivalent concentrated loads.
• For each individual concentrated load, consistent joint loads are calculated at
the corners of any loaded shell or solid element on the deck. In a spine model, a
concentrated force and eccentric moment is applied to the closest frame element representing the superstructure.
• Variable axle spacing, if present, is fixed at the minimum distance.
• Longitudinally-uniform loads are not considered.
• Floating axle loads are not considered.
If you wish to consider different axle spacing, define additional Vehicles. If you
wish to consider different transverse placement of the Vehicles, define additional
Lanes.

Static Analysis
When a Load Pattern of type “Vehicle Live” is applied in a Multi-Step Static Load
Case, it results in a separate linear static solution step for each time step, starting at
time zero. Each solution is independent, representing the displacement and stress
state in the structure for the current position of the vehicles. You can plot these re-

522

Step-By-Step Analysis

Chapter XXVI

Moving-Load Analysis

sults in sequence, create a video showing the movement of the vehicles across the
structure along with the resulting displacements and/or stresses, or envelope the results for the Load Case.
Since the analysis is static, the speed of the Vehicles has no effect on the results,
other than determining the change in position from one load step to the next.
If any additional loads are assigned to structural objects in Load Pattern of type
“Vehicle Live”, these loads are applied equally to the structure in every load step of
a multi-step static load case, and act in addition to the vehicle loads.

Time-History Analysis
When a Load Pattern of type “Vehicle Live” is applied in a Time-History Load
Case, a separate time function is automatically created for each load pattern that
was generated for the vehicle. Each time function ramps the load up from zero to
one over one time step, and back down to zero in the succeeding time step. This is
done regardless of what time function you may specify with the load pattern in the
load case. Thus at any given time within a time step, the applied load due to a Vehicle is a linear interpolation of the load pattern for the vehicle at the beginning and
the end of the time step.
If any additional loads are assigned to structural objects in a Load Pattern of type
“Vehicle Live”, these loads are applied using the time-function specified with the
load pattern, and act in addition to the vehicle loads.
Direct integration is recommended. Modal superposition would require a very
large number of modes since the spatial distribution of the load is constantly changing.
Dynamical effects are important in a time-history analysis, and different results
may be expected depending upon the speed of the vehicle.
The Time-History Load Case may be linear or nonlinear. If you wish to consider
static nonlinearity, you should perform a quasi-static nonlinear time-history analysis, i.e., at very slow speed with long time steps. The speed should be slow enough
so that the time it takes to cross a span is significantly longer than the first period of
the structure.

Step-By-Step Analysis

523

CSI Analysis Reference Manual

Enveloping and Load Combinations
Results for each step-by-step Load Case may be displayed or printed for individual
steps, or as an envelope giving the maximum and minimum response. When included in Load Combinations, envelope results will be used.
You can approximate an influence-based analysis by the following technique:
• Define one or more Load Patterns of type Vehicle Live, each of which moves a
single Vehicle in a single Lane in a single direction
• For each Load Pattern, create a corresponding Multi-Step Static Load Case that
applies only that Load Pattern
• For each Lane, define an envelope-type Load Combination of all Load Cases
defined for that Lane
• Define a single range-type Combo that includes all of the Lane envelope-type
Load Combinations
You can modify this procedure as needed for your particular application. The important thing is to be sure that in the final Load Combination, no Lane is ever
loaded by more than one Vehicle at a time, unless that is your intention.
Influence-based analysis is still more comprehensive, since it includes distributed
loads, transverse placement of the Vehicles in the Lanes, variable axle spacing, and
more accurate placement of the Vehicles for maximum effect.
See Topic “Load Combinations (Combos)” (page 351) in Chapter “Load Cases”
for more information.

Computational Considerations
The computation of influence lines requires a moderate amount of computer time
and a large amount of disk storage compared with the execution of other typical
CSiBridge analyses. The amount of computer time is approximately proportional
to N2L, where N is the number of structure degrees-of-freedom, and L is the number
of load points. The amount of disk storage required is approximately proportional
to NL.
The computation of Moving Load response may require a large amount of computer time compared with the execution of other typical CSiBridge analyses. The
amount of disk storage needed (beyond the influence lines) is small.

524

Computational Considerations

Chapter XXVI

Moving-Load Analysis

The computation time for Moving Load response is proportional to the number of
response quantities requested. The computation time for Moving Load response is
also directly proportional to the number of Lanes.
For each Vehicle load, the computation time is approximately proportional to the
square of the number of axles. It is also proportional to L¢, the effective number of
load points. Larger values of the truck influence tolerance tend to produce smaller
values of L¢ compared to L. The value of L¢ will be different for each response quantity; it tends to be smaller for structures with simple spans than with continuous
spans.
For step-by-step analysis, computational time is primarily affected by the number
of time steps used. Discretization of the Lanes, and the number and type of Vehicles
used has a secondary effect.

Computational Considerations

525

CSI Analysis Reference Manual

526

Computational Considerations

C h a p t e r XXVII

References
AASHTO, 2002
Standard Specifications for Highways Bridges, 17th Edition, The American
Association of State Highway and Transportation Officials, Inc., Washington,
D.C.
AASHTO, 2008
AASHTO LRFD Bridge Design Specifications, 4th Edition 2007, with 2008 Interim Revisions, The American Association of State Highway and Transportation Officials, Inc., Washington, D.C.
ACI, 2005
Building Code Requirements for Structural Concrete (ACI 318-05) and Commentary (ACI 318R-05), American Concrete Institute, Farmington Hills, Mich.
AISC, 2005
ANSI/AISC 360-05: An American National Standard ¾ Specification for
Structural Steel Buildings, American Institute of Steel Construction, Chicago,
Ill.

527

CSI Analysis Reference Manual
K. J. Bathe, 1982
Finite Element Procedures in Engineering Analysis, Prentice-Hall, Englewood
Cliffs, N.J.
K. J. Bathe and E. L. Wilson, 1976
Numerical Methods in Finite Element Analysis, Prentice-Hall, Englewood
Cliffs, N.J.
K. J. Bathe, E. L. Wilson, and F. E. Peterson, 1974
SAP IV — A Structural Analysis Program for Static and Dynamic Response of
Linear Systems, Report No. EERC 73-11, Earthquake Engineering Research
Center, University of California, Berkeley.
J. L. Batoz and M. B. Tahar, 1982
“Evaluation of a New Quadrilateral Thin Plate Bending Element,” International Jour nal for Nu meri cal Meth ods in En gi neer ing, Vol. 18, pp.
1655–1677.
Caltrans, 1995
Bridge Design Specifications Manual, as amended to December 31, 1995,
State of California, Department of Transportation, Sacramento, Calif.
Comite Euro-International Du Beton, 1993
CEB-FIP Modal Code, Thomas Telford, London
P. C. Roussis and M. C. Constantinou, 2005
Experimental and Analytical Studies of Structures Seismically Isolated with
and Uplift-Restraint Isolation System, Report No. MCEER-05-0001, MCEER,
State University of New York, Buffalo
R. D. Cook, D. S. Malkus, and M. E. Plesha, 1989
Concepts and Applications of Finite Element Analysis, 3rd Edition, John Wiley
& Sons, New York, N.Y.
R. D. Cook and W. C. Young, 1985
Advanced Mechanics of Materials, Macmillan, New York, N.Y.

528

Chapter XXVII

References

R. K. Dowell, F. S. Seible, and E. L. Wilson, 1998
“Pivot Hysteretic Model for Reinforced Concrete Members,” ACI Structural
Journal, Vol. 95, pp. 607–617.
FEMA, 2000
Prestandard and Commentary for Seismic Rehabilitation of Buildings, Prepared by the American Society of Civil Engineers for the Federal Emergency
Management Agency (Report No. FEMA-356), Washington, D.C.
A. K. Gupta, 1990
Response Spectrum Method in Seismic Analysis and Design of Structures,
Blackwell Scientific Publications, Cambridge, Mass.
J. P. Hollings and E. L. Wilson, 1977
3–9 Node Isoparametric Planar or Axisymmetric Finite Element, Report No.
UC SESM 78-3, Division of Structural Engineering and Structural Mechanics,
University of California, Berkeley.
T. J. R. Hughes, 2000
The Finite Element Method: Linear Static and Dynamic Finite Element Analysis, Dover.
A. Ibrahimbegovic and E. L. Wilson, 1989
“Simple Numerical Algorithms for the Mode Superposition Analysis of Linear
Structural Systems with Non-proportional Damping,” Computers and Structures, Vol. 33, No. 2, pp. 523–531.
A. Ibrahimbegovic and E. L. Wilson, 1991
“A Unified Formulation for Triangular and Quadrilateral Flat Shell Finite Elements with Six Nodal Degrees of Freedom,” Communications in Applied Numerical Methods, Vol. 7, pp. 1–9.
K. Kasai, O. Takahashi, and Y. Sekiguchi, 2004
“JSSI Manual for Building Passive Control Technology, Part-10 Time-History
Analysis Model for Nonlinear Oil Dampers,” Paper 1283, Proceedings of The
13th World Conference on Earthquake Engineering, Vancouver, Canada.

529

CSI Analysis Reference Manual
M. A. Ketchum, 1986
Redistribution of Stresses in Segmentally Erected Prestressed Concrete
Bridges, Report No. UCB/SESM-86/07, Department of Civil Engineering,
University of California, Berkeley.
N. Makris and J. Zhang, 2000
“Time-domain Viscoelastic Analysis of Earth Structures,” Earthquake Engineering and Structural Dynamics, Vol. 29, pp. 745–768.
L. E. Malvern, 1969
Introduction to the Mechanics of a Continuous Medium, Prentice-Hall, Englewood Cliffs, N.J.
C. Menun and A. Der Kiureghian, 1998
“A Replacement for the 30%, 40%, and SRSS Rules for Multicomponent Seismic Analysis,” Earthquake Spectra, Vol. 14, No. 1, pp. 153-163.
T. A. Morgan and S. A. Mahin, 2008
“The Optimization of Multi-Stage Friction Pendulum Isolators for Loss Mitigation Considering a Range of Seismic Hazard,” Proceedings of The 14th
World Conference on Earthquake Engineering, Beijing, China
S. Nagarajaiah, A. M. Reinhorn, and M. C. Constantinou, 1991
3D-Basis: Nonlinear Dynamic Analysis of Three-Dimensional Base Isolated
Structures: Part II, Technical Report NCEER-91-0005, National Center for
Earthquake Engineering Research, State University of New York at Buffalo,
Buffalo, N. Y.
NRC, 2006
“Combining Modal Responses and Spatial Components in Seismic Response
Analysis,” Regulatory Guide 1.92, Revision 2, U.S. Nuclear Regulatory
Commission.
Y. J. Park, Y. K. Wen, and A. H-S. Ang, 1986
“Random Vibration of Hysteretic Systems under Bi-Directional Ground Motions,” Earthquake Engineering and Structural Dynamics, Vol. 14.
R. J. Roark and W. C. Young, 1975

530

Chapter XXVII

References

Formulas for Stress and Strain. 5th Edition, McGraw-Hill, New York, N.Y.
T. Takeda, M. A. Sozen, and N. N. Nielsen, 1970
“Reinforced Concrete Response to Simulated Earthquakes,” J. Struct. Engrg.
Div., ASCE, Vol. 96, No. 12, pp. 2257–2273.
R. L. Taylor and J. C. Simo, 1985
“Bending and Membrane Elements for Analysis of Thick and Thin Shells,”
Proceedings of the NUMEETA 1985 Conference, Swansea, Wales.
K. Terzaghi and R. B. Peck, 1967
Soil Mechanics in Engineering Practice, 2nd Edition, John Wiley & Sons,
New York, N.Y.
S. Timoshenko and S. Woinowsky-Krieger, 1959
Theory of Plates and Shells, 2nd Edition, McGraw-Hill, New York, N.Y.
Y. K. Wen, 1976
“Method for Random Vibration of Hysteretic Systems,” Journal of the Engineering Mechanics Division, ASCE, Vol. 102, No. EM2.
D. W. White and J. F. Hajjar, 1991
“Application of Second-Order Elastic Analysis in LRFD: Research to Practice,” Engineering Journal, AISC, Vol. 28, No. 4, pp. 133–148.
E. L. Wilson, 1970
SAP — A General Structural Analysis Program, Report No. UC SESM 70-20,
Structural Engineering Laboratory, University of California, Berkeley.
E. L. Wilson, 1972
SOLID SAP — A Static Analysis Program for Three Dimensional Solid Structures, Report No. UC SESM 71-19, Structural Engineering Laboratory, University of California, Berkeley.
E. L. Wilson, 1985
“A New Method of Dynamic Analysis for Linear and Non-Linear Systems,”
Finite Elements in Analysis and Design, Vol. 1, pp. 21–23.
E. L. Wilson, 1993

531

CSI Analysis Reference Manual
“An Efficient Computational Method for the Base Isolation and Energy Dissipation Analysis of Structural Systems,” ATC17-1, Proceedings of the Seminar
on Seismic Isolation, Passive Energy Dissipation, and Active Control, Applied
Technology Council, Redwood City, Calif.
E. L. Wilson, 1997
Three Dimensional Dynamic Analysis of Structures with Emphasis on Earthquake Engineering, Computers and Structures, Inc., Berkeley, Calif.
E. L. Wilson and M. R. Button, 1982
“Three Dimensional Dynamic Analysis for Multicomponent Earthquake Spectra,” Earthquake Engineering and Structural Dynamics, Vol. 10.
E. L. Wilson, A. Der Kiureghian, and E. P. Bayo, 1981
“A Replacement for the SRSS Method in Seismic Analysis,” Earthquake Engineering and Structural Dynamics, Vol. 9.
E. L. Wilson and I. J. Tetsuji, 1983
“An Eigensolution Strategy for Large Systems,” Computers and Structures,
Vol. 16.
E. L. Wilson, M. W. Yuan, and J. M. Dickens, 1982
“Dynamic Analysis by Direct Superposition of Ritz Vectors,” Earthquake Engineering and Structural Dynamics, Vol. 10, pp. 813–823.
V. Zayas and S. Low, 1990
“A Simple Pendulum Technique for Achieving Seismic Isolation,” Earthquake
Spectra, Vol. 6, No. 2.
O. C. Zienkiewicz and R. L. Taylor, 1989
The Finite Element Method, 4th Edition, Vol. 1, McGraw-Hill, London.
O. C. Zienkiewicz and R. L. Taylor, 1991
The Finite Element Method, 4th Edition, Vol. 2, McGraw-Hill, London.

532

Chapter XXVII

References

Copyright Notice for TAUCS:
TAUCS Version 2.0, November 29, 2001. Copyright ©) 2001, 2002, 2003 by
Sivan Toledo, Tel-Aviv Univesity, stoledo@tau.ac.il. All Rights Reserved.
TAUCS License:
Your use or distribution of TAUCS or any derivative code implies that you
agree to this License.
THIS MATERIAL IS PROVIDED AS IS, WITH ABSOLUTELY NO WARRANTY EXPRESSED OR IMPLIED. ANY USE IS AT YOUR OWN RISK.
Permission is hereby granted to use or copy this program, provided that the
Copyright, this License, and the Availability of the original version is retained
on all copies. User documentation of any code that uses this code or any derivative code must cite the Copyright, this License, the Availability note, and
“Used by permission.” If this code or any derivative code is accessible from
within MATLAB, then typing “help taucs” must cite the Copyright, and “type
taucs” must also cite this License and the Availability note. Permission to modify the code and to distribute modified code is granted, provided the Copyright,
this License, and the Availability note are retained, and a notice that the code
was modified is included. This software is provided to you free of charge.
Availability:
As of version 2.1, we distribute the code in 4 formats: zip and tarred-gzipped
(tgz), with or without binaries for external libraries. The bundled external libraries should allow you to build the test programs on Linux, Windows, and
MacOS X without installing additional software. We recommend that you
download the full distributions, and then perhaps replace the bundled libraries
by higher performance ones (e.g., with a BLAS library that is specifically optimized for your machine). If you want to conserve bandwidth and you want to
install the required libraries yourself, download the lean distributions. The zip
and tgz files are identical, except that on Linux, Unix, and MacOS, unpacking
the tgz file ensures that the configure script is marked as executable (unpack
with tar zxvpf), otherwise you will have to change its permissions manually.
Used by permission.

533

CSI Analysis Reference Manual

534

Source Exif Data:

File Type                       : PDF
File Type Extension             : pdf
MIME Type                       : application/pdf
PDF Version                     : 1.6
Linearized                      : No
Author                          : Computers and Structures, Inc.
Create Date                     : 2016:08:14 12:12:04Z
Modify Date                     : 2016:10:26 09:54:27-07:00
Has XFA                         : No
XMP Toolkit                     : Adobe XMP Core 4.2.1-c043 52.372728, 2009/01/18-15:08:04
Format                          : application/pdf
Creator                         : Computers and Structures, Inc.
Title                           : SapRefer3.vp
Creator Tool                    : Corel Ventura 10.0
Metadata Date                   : 2016:10:26 09:54:27-07:00
Producer                        : Corel PDF Engine Version 10.397
Document ID                     : uuid:b9e26f7c-6ec6-4c01-9175-e9c539868f61
Instance ID                     : uuid:40d4eda4-6b51-4762-9c9d-daa35fb6c319
Page Layout                     : SinglePage
Page Count                      : 556

EXIF Metadata provided by EXIF.tools

SapRefer3.vp CSi Refer

Navigation menu

Versions of this User Manual:

Views

Navigation