usyd_abaqus_2006

ABAQUS: Selected Topics

ABAQUS: Selected Topics

University of Sydney
28 Feb 2006 – 02 Mar 2006

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics 2

Day 1

• Lecture 1 Overview of ABAQUS

– Workshop 1 Linear Static Analysis of Cantilever Beam

• Lecture 2 Introduction to Non-linear Analysis

– Workshop 2 Non-linear Analysis of Skew Plate

• Lecture 3 Materials – Metal

– Workshop 3a Plasticity and Hardening – 2D Cantilever Beam

– Workshop 3b Skew Plate with Plasticity

• Lecture 4 Materials – Concrete

– Workshop 4 Collapse of a Concrete Slab

Copyright 2006 ABAQUS, Inc.

ABAQUS: Selected Topics 3

Day 2

• Lecture 5 Eigenvalue Buckling Analysis

– Workshop 5a Cargo Crane – Critical Load Estimation

– Workshop 5b Eigenvalue Buckling of a Square Tube

• Lecture 6 Static Post-buckling Analysis

– Workshop 6a Cargo Crane – Riks Analysis

– Workshop 6b Buckling of a Square Tube with Imperfections

• Lecture 7 Damped Static Post-buckling Analysis

– Workshop 7a Cargo Crane – Stabilized Static Analysis

– Workshop 7b Cargo Crane – Dynamic Analysis

Copyright 2006 ABAQUS, Inc.

ABAQUS: Selected Topics 4

Day 3

• Lecture 8 Introduction to Contact Modeling

– Workshop 8a Hinge Model

– Workshop 8b Clip and Plate Model

• Lecture 9 Bolted Connection Modeling

– Workshop 9a Pump Model – Bolt Loading

– Workshop 9b Beam-Column Connection with Fasteners

• Lecture 10 Including Initial Stresses (Optional)

• Question Session

Copyright 2006 ABAQUS, Inc.

ABAQUS: Selected Topics 5

Legal Notices

The information in this document is subject to change without notice and should not be construed as
a commitment by ABAQUS, Inc.
ABAQUS, Inc., assumes no responsibility for any errors that may appear in this document.
The software described in this document is furnished under license and may be used or copied only
in accordance with the terms of such license.
No part of this document may be reproduced in any form or distributed in any way without prior
written agreement with ABAQUS, Inc.

Copyright © ABAQUS, Inc., 2005.
Printed in U.S.A.
All Rights Reserved.
ABAQUS is a registered trademark of ABAQUS, Inc.
The following are trademarks of ABAQUS, Inc.:
ABAQUS/Aqua; ABAQUS/CAE; ABAQUS/Design; ABAQUS/Explicit; ABAQUS/Foundation;
ABAQUS/Standard; ABAQUS/Viewer; ABAQUS Interface for MOLDFLOW; ABAQUS Interface for
MSC.ADAMS; and the ABAQUS, Inc., logo.
All other brand or product names are trademarks or registered trademarks of their respective
companies or organizations.

Copyright 2006 ABAQUS, Inc.

ABAQUS: Selected Topics

Lecture 1

Overview of ABAQUS

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.2

Overview

• Introduction
• Components of an ABAQUS Model
• Structure of an ABAQUS Input File
• ABAQUS Conventions
• Workshop 1: Linear Static Analysis of a Cantilever Beam

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

What is ABAQUS?

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.4

Introduction

ABAQUS is a suite of finite element analysis modules

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.5

Introduction

• The heart of ABAQUS are the analysis modules, ABAQUS/Standard and
ABAQUS/Explicit, which are complementary and integrated analysis
tools.

– ABAQUS/Standard is a general-purpose, finite element module.

• It provides a large number of capabilities for analyzing many different
types of problems, including many nonstructural applications.

– ABAQUS/Explicit is an explicit dynamics finite element module.

– ABAQUS/CAE incorporates the analysis modules into a Complete
ABAQUS Environment for modeling, managing, and monitoring ABAQUS
analyses and visualizing results.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.6

Introduction ABAQUS/CAE main user interface

• ABAQUS/CAE
– Complete ABAQUS Environment for
modeling, managing, and monitoring
ABAQUS analyses, as well as
visualizing results.
– Intuitive and consistent user
interface throughout the system.
– Based on the concepts of parts and
assemblies of part instances, which
are common to many CAD systems.
– Parts can be created within
ABAQUS/CAE or imported from
other systems as geometry (to be
meshed in ABAQUS/CAE) or as
meshes.
– Built-in feature-based parametric
modeling system for creating parts.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.7

Introduction

• Solver modules
– ABAQUS/Standard and ABAQUS/Explicit provide the user with two
complementary analysis tools.
ABAQUS/Standard’s capabilities:
– General analyses
• Static stress/displacement analysis:
– Rate-independent response
– Rate-dependent (viscoelastic/creep/viscoplastic) response
• Transient dynamic stress/displacement analysis
• Transient or steady-state heat transfer analysis
• Transient or steady-state mass diffusion analysis

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.8

Introduction

• Steady-state transport analysis
• Coupled problems:

– Thermo-mechanical (sequentially or fully coupled)
– Thermo-electrical
– Pore fluid flow-mechanical
– Stress-mass diffusion (sequentially coupled)
– Piezoelectric (linear only)
– Acoustic-mechanical

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.9

Introduction

– Linear perturbation analyses
• Static stress/displacement analysis:
– Linear static stress/displacement analysis
– Eigenvalue buckling load prediction
• Dynamic stress/displacement analysis:
– Determination of natural modes and frequencies
– Transient response via modal superposition
– Steady-state response resulting from harmonic loading
• Includes alternative “subspace projection” method for
efficient analysis of large models with frequency-dependent
properties (like damping)
– Response spectrum analysis
– Dynamic response resulting from random loading

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.10

Introduction

ABAQUS/Explicit’s capabilities:
– Explicit dynamic response with or without adiabatic heating effects
– Fully coupled thermo-mechanical analysis
– Structural-acoustic analysis
– Annealing for multistep forming simulations
– Automatic adaptive meshing allows the robust solution of highly nonlinear

problems

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.11

Introduction

Comparing ABAQUS/Standard and ABAQUS/Explicit
– ABAQUS/Standard

• A general-purpose finite element program.
• Can solve for true static equilibrium in structural simulations.
• Provides a large number of capabilities for analyzing many different

types of problems, including many nonstructural applications.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.12

Introduction

– ABAQUS/Explicit
• Solution procedure does not require iteration.
• Solves highly discontinuous high-speed dynamic problems efficiently.
• Does not require as much disk space as ABAQUS/Standard for larger
problems.
• Contact calculations are easier with ABAQUS/Explicit. Applications
such as quasi-static metal forming simulations are easier.
• Provides an adaptive meshing capability.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.13

Introduction

– Documentation
• Unless otherwise indicated, all documentation is available both online
and in print.
• ABAQUS Analysis User’s Manual
• ABAQUS/CAE User’s Manual
• ABAQUS Example Problems Manual
• ABAQUS Benchmarks Manual (online only)
• ABAQUS Verification Manual (online only)
• ABAQUS Theory Manual (online only)

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.14

Introduction

– Additional reference materials
• Installation and Licensing Guide
– (Installation instructions)
• Release Notes
– (Explains changes since previous release)
• Advanced lecture notes on various topics (print only)
• Tutorials
– Getting Started with ABAQUS
– Getting Started with ABAQUS/Standard: Keywords Version
(online only)
– Getting Started with ABAQUS/Explicit: Keywords Version
(online only)
• ABAQUS Home Page

www.abaqus.com

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Components of an ABAQUS Model

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.16

Components of an ABAQUS Model

– The ABAQUS analysis modules run as batch programs. The primary input
to the analysis modules is an input file
• A text file which contains options from element, material, procedure,
and loading libraries.

– When working in ABAQUS/CAE, this input file is created “behind the
scenes” when an analysis job is submitted

• For many analyses, the user need never see the input file

• In some cases, the user may need to manually edit the input file
before submitting the analysis

– A basic understanding of the ABAQUS input file format and contents is
beneficial

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.17

Components of an ABAQUS Model

– The input file is divided into two parts: model data and history data.

Model data Geometric options—nodes, elements
Material options
Other model options

History data Procedure options
Loading options
Output options

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.18

Components of an ABAQUS Model

• History subdivided into analysis steps
– Steps are convenient subdivisions in an analysis history.
– Different steps can contain different analysis procedures—for example,
static followed by dynamic.
– Distinction between general and linear perturbation steps:
• General steps define a sequence of events that follow one another.
– The state of the model at the end of the previous general step
provides the initial conditions for the start of the next step. This is
needed for any history-dependent analysis.
• Linear perturbation steps provide the linear response about the base
state, which is the state at the end of the most recent general step.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.19

Components of an ABAQUS Model

• Example: bow and arrow
simulation

Step 3 = natural
frequency extraction

Step 1 = pretension Step 2 = pull back Step 4 = dynamic release

Step 1: String the bow
Step 2: Pull back on the bow string
Step 3: Linear perturbation step to extract the natural frequencies of the system—

has no effect on subsequent steps
Step 4: Release the arrow

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Structure of an ABAQUS Input File

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.21

Structure of an ABAQUS Input File

• Option blocks
– All data are defined in “option blocks” that describe specific aspects of the
problem definition, such as an element definition, etc. Together the option
blocks build the model.

Node option Property reference
block option block

Model Material option Element option Boundary conditions
data block block option block

History Contact option Initial conditions
data block option block

Analysis procedure Loading option block Output request
option block option block

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.22

Structure of an ABAQUS Input File

– Each option block begins with a keyword line (first character is *).
– Data lines, if needed, follow the keyword line.
– Comment lines, starting with **, can be included anywhere.

• Keyword lines *MATERIAL, NAME=material name

– Begin with a single * followed keyword parameter parameter value
directly by the name of the
option. The first line in a material option block

– May include a combination of
required and optional
parameters, along with their
values, separated by commas.

• Example: A material
option block defines a set
of material properties.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.23

Structure of an ABAQUS Input File

• Data lines *ELEMENT, TYPE=B21 keyword line

– Define the bulk data for a given 560, 101, 102 data lines
option; for example, element 564, 102, 103
definitions.
572, 103, 104
– A keyword line may have many
data lines associated with it. ⋅

• Example: An element ⋅ node numbers (as required
option block defines for beam B21 elements)
elements by specifying the
element type, the element element numbers
numbers, and the nodal
connectivity.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

ABAQUS Conventions

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.25

ABAQUS Conventions

• Units
– ABAQUS uses no inherent set of units.
– It is the user’s responsibility to use consistent units.

Common systems of consistent units

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.26

ABAQUS Conventions

• Time measures

– ABAQUS keeps track of both total time in an analysis and step time for
each analysis step.

– Time is physically meaningful for some analysis procedures, such as
transient dynamics.

– Time is not physically meaningful for some procedures. In rate-
independent, static procedures “time” is just a convenient, monotonically
increasing measure for incrementing loads.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.27

ABAQUS Conventions local rectangular
coordinate system
• Coordinate systems with YSYMM
boundary conditions
– For boundary conditions and
point loads, the default Boundary conditions on a skew edge
coordinate system is the
rectangular Cartesian system.
• Alternative local
rectangular, cylindrical, and
spherical systems can be
defined.
• These local directions do
not rotate with the material
in large-displacement
analyses.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.28

ABAQUS Conventions Default material directions for solid elements

– For material directions (i.e., directions
associated with each element’s material or
integration points) the default coordinate
system depends on the element type:

• Solid elements use global rectangular
Cartesian system.

• Shell and membrane elements use a
projection of the global Cartesian
system onto the surface.

Default material directions for shell and
membrane elements

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.29

ABAQUS Conventions

– Alternative rectangular, cylindrical,
and spherical coordinate systems
may be defined.
• Affects input: anisotropic
material directions.
• Affects output: stress/strain
output directions.
• Local material directions
rotate with the material in
large-displacement analyses.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.30

ABAQUS Conventions

• Degrees of freedom
– Primary solution variables at the nodes.
– Available nodal degrees of freedom depend on the element type.
– Each degree of freedom is labeled with a number: 1=x-displacement,
2=y-displacement, 11=temperature, etc.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Workshop 1: Linear Static Analysis of
a Cantilever Beam

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L1.32

Workshop 1: Linear Static Analysis of a Cantilever Beam

• Workshop tasks
1. Follow detailed instructions
to create a simple cantilever
beam model using the
ABAQUS/CAE modules.
2. Submit a job for analysis.
3. View the analysis results.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Lecture 2

Nonlinear Analysis in
ABAQUS/Standard

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.2

Overview

• Equilibrium Equations
• Linear Analysis
• Nonlinearity in Structural Mechanics
• Solving Nonlinear Equilibrium Equations
• Including Nonlinear Effects in an ABAQUS Simulation
• Convergence Issues
• Diagnostics
• Workshop 2: Nonlinear Analysis of a Skew Plate

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Equilibrium Equations

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.4

Equilibrium Equations

• The finite element method seeks to find the displacements of a structure,

u, such that:

– The solution is continuous across element boundaries.

– Equilibrium is achieved, and the prescribed boundary conditions are
satisfied.

• Static equilibrium

– The basic statement of static equilibrium is that the internal forces exerted

on the nodes, I, resulting from the element stresses and external forces, P,

acting at every node must balance:

P(u) − I (u) = 0 (Eq. 2.1)

– Equation 2.1 is general, and makes no assumptions about the forms of

P(u) and I(u).

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.5

Equilibrium Equations

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.6

Linear Analysis

• Linear assumptions
– If we assume
• the deflections, rotations and strains are small
• the material behaves linearly, and
• the loads and boundary conditions do not change as the
structure deforms

then P is constant and I = Ku where K is constant
– The equilibrium equation is then linear in u and the solution can be

found directly:

u = K-1P

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.7

Linear Analysis

• Characteristics of a linear analysis
– Results (stress, strain, displacement) vary in proportion to the
applied loads.
• Eg twice the load gives twice the displacement
• If the problem is solved once, the results can be scaled
– For a given set of boundary conditions, the results from distinct
loads can be superimposed to find the combined effect

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.8

Linear Analysis

• Linear analysis has historically been widely used
– Linear methods are easy and fast to solve
– ABAQUS can solve linear problems

• But…
– Real world problems are only approximately linear
– Linear analysis is often inappropriate:
• Non-linear material response
• Large deformations
• Loads or boundary conditions dependent on solution

• In these cases, a nonlinear analysis is required to correctly model the
structural response.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Nonlinearity in Structural Mechanics

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.10

Nonlinearity in Structural Mechanics

• Sources of nonlinearity Some examples of material nonlinearity

– Material nonlinearities:

• Nonlinear elasticity

• Plasticity

• Material damage

• Failure mechanisms

• Etc.

– Note: material dependencies on
temperature or field variables do
not introduce nonlinearity if the
temperature or field variables
are predefined.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.11
L2.12
Nonlinearity in Structural Mechanics

– Boundary nonlinearities:
• Contact problems
– Boundary conditions change
during the analysis.
– Extremely discontinuous form
of nonlinearity.

An example of self-contact: “Compression of
a jounce bumper,” Example Problem 1.1.16
in the ABAQUS Example Problems Manual

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Nonlinearity in Structural Mechanics

– Geometric nonlinearities:
• Large deflections and deformations
• Large rotations
• Structural instabilities (buckling)
• Preloading effects

An example of a load-displacement curve
from a buckling analysis

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.13

Nonlinearity in Structural Mechanics

– Typical nonlinear problems have all three forms of nonlinearity.
• Must include the nonlinear terms in the equations.

An example of with nonlinearity— Video Clip
elastomeric keyboard dome

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Solving Nonlinear Equilibrium Equations

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.15

Solving Nonlinear Equilibrium Equations

• Static equilibrium
– As before, we have

P = Ku

– However, now P and K can depend on u :

P = P(u) and K = K(u)

• It is no longer possible to solve for u directly

– Nonlinear problems are generally solved using an incremental and iterative
numerical technique

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.16

Solving Nonlinear Equilibrium Equations

• Incremental solution scheme
– For a static problem a fraction of the total load is applied to the structure
and the equilibrium solution corresponding to the current load level is
obtained.
• The load level is then increased (i.e., incremented) and the process is
repeated until the full load level is applied.
P

Increments Final equilibrium
in applied solution at total load
load
u
Copyright 2004 ABAQUS, Inc.
Intermediate
equilibrium solutions

ABAQUS: Selected Topics L2.17

Solving Nonlinear Equilibrium Equations

– To solve for equilibrium in nonlinear problems, ABAQUS/Standard uses an
incremental-iterative solution, based on the Newton-Raphson technique.

– Assume that the solution to the previous load increment, u0, is known.

– Assume that after an iteration, i, an approximation, ui, to the solution has
been obtained. Let ci+1 be the difference between this solution and the

exact solution to the discrete equilibrium equation, Equation 2.1, so that

P(ui + ci+1) − I (ui + ci+1) = 0. (Eq. 2.2)

– Expanding the left-hand side of Equation 2.2 in a Taylor series about the

approximate solution, ui, then gives

P(ui ) − I (ui ) +  ∂P(ui ) − ∂I (ui )  ci+1 + .... = 0. (Eq. 2.3)
 ∂u ∂u 

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.18

Solving Nonlinear Equilibrium Equations

– By ignoring higher-order terms, the equation can be written as

Kici+1 = P(ui ) − I (ui ),

where Ki = ∂I (ui ) − ∂P(ui ) is the tangent stiffness.
∂u ∂u

– The next approximation to the solution is

ui+1 = ui + ci+1.

– Note that if the load depends on displacement (e.g., pressure on a surface
that rotates), the stiffness matrix includes a load stiffness contribution.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.19

Solving Nonlinear Equilibrium Equations

– ABAQUS then forms Ki+1 and calculates Ii+1 based on the updated state
of the model, ui+1.

– The difference between the total applied force, PTOTAL, and the internal
force, Ii+1, is called the force residual, Ri+1: Ri+1= PTOTAL− Ii+1.

– If R1 is very small (within the tolerance limit) at every degree of freedom in

the model, the structure is in equilibrium.

• The default tolerance is that R1 must be less than 0.5% of the time

averaged force in the structure.

• ABAQUS automatically calculates the time averaged force.

– If the iteration does not produce a converged solution, ABAQUS will
perform another iteration in an attempt to find a converged solution.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.20

Solving Nonlinear Equilibrium Equations

– This procedure is repeated until force residuals are within the tolerance

limits. Each iteration, i, requires:

1. Formulation of tangent stiffness, Ki.
2. Solution of simultaneous system of equations for ci+1.

• Update the estimate of the solution: ui+1 = ui + ci+1.
3. Calculation of internal force vector Ii+1 based on ui+1.

4. Judgment of equilibrium convergence:

• Is Ri+1 within the “tolerance”?

∑#iter

• Is ci+1 << c j?

j=1

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.21

Solving Nonlinear Equilibrium Equations

– The method can be understood quite easily (in one dimension) from a
load-displacement diagram:

Residual Two convergence criteria:
Internal force Small residuals
Small corrections

12
Correction

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.22

Solving Nonlinear Equilibrium Equations

• Steps, increments, and iterations
– Analysis steps
• The load history for a simulation consists of one or more steps.
– Increments
• An increment is part of a step.
– In static problems the total load applied in a step is broken into
smaller increments so that the nonlinear solution path may be
followed.
– In dynamic problems the total time period is broken into smaller
increments to integrate the equations of motion.
– Iterations
• An iteration is an attempt at finding the equilibrium solution in an
increment.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.23

Solving Nonlinear Equilibrium Equations

• Automatic time incrementation
– ABAQUS automatically adjusts the size of the increments so that nonlinear
problems are solved easily and efficiently.
• Heuristic algorithm (based on many years of experience).
– In static problems it is based on number of iterations required to converge.
• Convergence is easily achieved:
⇒increase increment size
• Convergence difficult or divergence occurs:
⇒cut back increment size
• Otherwise:
⇒maintain same increment size
– Tip: For highly nonlinear problems, it is recommended that the initial time
increment be chosen as a small fraction (e.g., 10%) of the total step time.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.24

Solving Nonlinear Equilibrium Equations

• Incrementation data: Suggested initial Automatic time
ABAQUS/Standard increment size. incrementation chosen by
default.
– Specify the initial increment Default is the time
size and the number of period. Default maximum
increments allowed. number of increments
allowed for the step.
– ABAQUS will stop if:
Minimum and
• The maximum number of maximum increment
increments is reached sizes.
before the total load is Defaults based on time
applied period for step.

or

• If increment sizes smaller
than the minimum are
required.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Including Nonlinear Effects in an
ABAQUS Simulation

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.26

Including Nonlinear Effects in an ABAQUS Simulation

• Material nonlinearity
– Define a nonlinear material model (e.g., plasticity, hyperelasticity, etc).
– Examples are discussed in Lectures 3 and 4

• Boundary nonlinearity
– Define contact interactions between bodies.
– Discussed further in Lecture 8.

• Geometric nonlinearity
– Set the Nlgeom option when defining the analysis step.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.27

Including Nonlinear Effects in an ABAQUS Simulation

• Geometric nonlinearity Specify time period
of the step.
– Include all nonlinear geometric
effects due to: Set Nlgeom to On to include include all
nonlinear geometric effects.
• Large deflections,
rotations, deformation. Edit Step dialog box

• Preloading (initial
stresses).

• Load stiffness.

– If the above are not important,
the answer will be the same as
with Nlgeom set to Off but the
analysis will be more
expensive.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Convergence Issues

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.29

Convergence Issues (Noncontact Related)

• What does convergence mean?
– For an implicit solver such as ABAQUS/Standard:
• Equilibrium state has been obtained based on predefined criteria
(small residuals, small solution corrections, etc.).

• Non-convergence
– If ABAQUS is unable to converge to the equilibrium state in an acceptable
number of iterations, the analysis will terminate at that point
– Information is available to help diagnose convergence problems
• Error and warning messages
• Detailed information about the solution progress
– Available in
• Message file (*.msg)
• Job Monitor and Job Diagnostics in ABAQUS/CAE

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.30

Convergence Issues (Noncontact Related)

• Some common warning messages ABAQUS/Standard

Numerical singularities These indicate that so many digits are
lost during linear equation solution that
the results are not reliable. The most
common cause is an unconstrained rigid
body mode in a static stress analysis.

Zero pivots These occur during linear equation
solution when there is a force term but no
corresponding stiffness. Common causes
are unconstrained rigid body modes and
overconstrained degrees of freedom.

Negative eigenvalues Negative eigenvalues indicate that the
stiffness matrix is not positive definite. For
example, a buckling load may have been
exceeded.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Diagnostics

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.32

Diagnostics

– Job Monitor
• Summarizes the solution progress.
• The same information is also printed to the status (.sta) file.

– Job Diagnostics
• Provides details of each iteration for an ABAQUS/Standard analysis.
• The same information is also printed to the message (.msg) file.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.33

Diagnostics

• Understanding the Job Monitor
– Summarizes how analysis
proceeds—shows automatic time
incrementation at work.
– You can check the status file
while the job is running.
– One line written after each
successful increment.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.34

Diagnostics

• Understanding Job Diagnostics in ABAQUS/Standard
– Includes:
• All iteration details.
• Solver messages.
• Useful troubleshooting information:
– Locations of highest residuals.
– Locations of excessive deformation.
– Locations of contact changes.
– The locations can be highlighted in the model.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.35

Diagnostics Initial time increment

Tools Job Diagnostics

Copyright 2004 ABAQUS, Inc. L2.36
ABAQUS: Selected Topics
A similar display is given for
Diagnostics rotational degrees of freedom

Copyright 2004 ABAQUS, Inc. Toggle on to see the locations in
the model where the largest
residuals and displacement
increments and corrections occur.

ABAQUS: Selected Topics L2.37

Diagnostics × 0.005
0.012
Copyright 2004 ABAQUS, Inc.
ABAQUS: Selected Topics L2.38

Diagnostics × 0.005
0.012
Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.39

Diagnostics

4 or fewer
iterations (do
this again and
∆t can increase)

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.40

Diagnostics

no increase

Two consecutive ∆t = 1.5∆told
increments with 4 or
fewer iterations: ∆t =
1.5∆ told

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.41

Diagnostics

Copyright 2004 ABAQUS, Inc.
ABAQUS: Selected Topics

Workshop 2: Nonlinear Analysis of a
Skew Plate

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L2.43

Workshop 2: Nonlinear Analysis of a Skew Plate

• Workshop tasks
1. Create model.
a. Local material directions.
b. Local boundary
condition directions.
2. Run static analysis:
a. Linear
b. Geometric nonlinearity
3. Postprocess the results.

Video Clip

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Lecture 3 L3.2

Materials - Metal

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Overview

• Introduction
• Typical Metal Behaviour
• Linear Elasticity
• Metal Plasticity
• Yield Functions
• Hardening
• Input of Material Data for Plasticity
• Workshop 3a: Plasticity and Hardening
• Workshop 3b: Skew Plate with Plasticity

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Introduction

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.4

Introduction

• ABAQUS has a wide variety of built-in material models designed to be
used to model

– Metals, ceramics, rubbers, foams, plastics, soils, concrete and other
geotechnical materials

• Phenomenological Approach

– Most material models (for metal and concrete) are based upon
experimental observations.

– Capture critical material behaviour within a usable and stable continuum
description

• Material Input

– Key material parameters (eg Youngs Modulus) must be entered by the
user

– ABAQUS has no inbuilt library of material parameters

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.5

Introduction

• This course provides general information about modeling two particular
materials in ABAQUS
– Metals
– Concrete

• The focus of this lecture is on modeling Metals
– Conrete is discussed in the next lecture

Copyright 2005 ABAQUS, Inc.
ABAQUS: Selected Topics

Typical Metal Behaviour

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.7

Typical Metal Behaviour

– Consider a uniaxial tension test performed on a metal specimen at
relatively low temperature.

stress B

A

E
1

C strain
Uniaxial stress-strain data for a metal

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.8

Typical Metal Behaviour

– The material initially exhibits stiff linear response to the applied load:

• Young’s modulus E quantifies the material stiffness.

• The deformation is fully recoverable—if the load is released, the
specimen will return to its original configuration.

– At point A the material yields, and the deformation beyond this point is not

fully recoverable—it is no longer purely elastic.
– Yield is usually accompanied by a drastic reduction in the stiffness of the

material:
• Response to further loading follows a much lower work hardening
modulus.
• In extreme cases the material exhibits no stiffness beyond the initial
yield point and is considered perfectly plastic.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.9

Typical Metal Behaviour

– If the strain is reversed at point B, the material immediately recovers its

elastic stiffness.

– If the specimen is completely unloaded, the strain at point C represents the

permanent deformation in the material.

– If the unloading does not continue beyond the elastic range and the
specimen is again loaded in the original direction, the material yields at, or

very close to, point B.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.10

Typical Metal Behaviour

– If the unloading is continued so that yield occurs in the opposite direction,
the yield stress is reduced compared to that of the original specimen. This
is known as the Bauschinger effect.

stress B
A

C
strain

D
A−

The Bauschinger effect

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.11

Typical Metal Behaviour

– Discussion thus far has been limited to uniaxial stress-strain
measurements at one temperature and one strain rate. For most metals:

• As the material temperature increases, the yield stress decreases.

• As the strain rate increases, the yield stress increases.

– Varying the temperature and strain rate provides results similar to those
shown in the figure below.

stress stress

temperature strain rate
increasing increasing

strain strain

Effect of temperature and strain rate on stress-strain data

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Linear Elasticity

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.13

Linear Elasticity

– Most metals have some range of deformation in which their behavior
remains elastic and linear

– The linear elastic material model:
• Is valid for small elastic strains (normally less than 5%);
• Can be isotropic, orthotropic, or fully anisotropic; and
• Can have properties that depend on temperature and/or other field
variables.

– Orthotropic and anisotropic material definitions require the use of local
material directions.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.14

Linear Elasticity

– For a linear elastic material, Hooke's law states:
stress ∝ strain.

– The generalized form of the law is written as

σ = Del : ε el
– where σ is the Cauchy (or “true”) stress, Del is the fourth-order elasticity

tensor, and ε el is the elastic log strain.

1

Uniaxial stress-strain curve
for a linear elastic material

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.15

Linear Elasticity

• Defining linear elasticity in ABAQUS

*Material, name=steel
*Elastic
2.e11, 0.3

Temperature-
dependence

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Metal Plasticity

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.17

Metal Plasticity

– When inelastic material models are used in ABAQUS, the total strain in the
model, ε, is decomposed into elastic, plastic, and creep strains:

ε = ε el + ε pl + ε cr .

– ABAQUS plasticity models are usually formulated in terms of a yield
surface, a flow rule, and hardening.
• A yield surface is a test function that determines if the material
responds purely elastically at a particular stress state.
• A flow rule defines the plastic deformation that occurs if the material is
no longer responding purely elastically.
• Hardening defines the way in which the yield and/or flow definitions
change as inelastic deformation occurs.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Yield Functions

Copyright 2005 ABAQUS, Inc.