usyd_abaqus_2006

ABAQUS: Selected Topics L5.13

Eigenvalue Problem Formulation

– Values λcr, which provide nontrivial solutions to this problem, define the

critical buckling load as P0 + λ ∆P with corresponding buckling mode
cr

shapes V .

– Buckling mode shapes V are normalized vectors, just as modes of free

vibration are, and do not represent actual magnitudes of deformation at the
critical load.

• They are often the most useful outcome of the eigenvalue analysis
since they predict the likely failure mode of the structure.

– The mode shapes are also often used to generate perturbations in
geometry for collapse analysis.

• They are typically scaled to a fraction of a relevant structural
dimension (such as a beam cross-section or a shell thickness) before
they are used to perturb the geometry.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.14

Eigenvalue Problem Formulation

– Estimating the maximum load level
• Nonlinear pre-buckling makes the method approximate.
• The estimate is more accurate if the structure is preloaded to a level
close to the pre-buckling load capacity.
• Generally alternative solution techniques (e.g., Riks) are required for
accurate prediction.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

ABAQUS Usage L5.16

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

ABAQUS Usage

– ABAQUS will calculate the initial stress and
load stiffness matrix corresponding to the live
load directly.
• The ∗BUCKLE step is a linear
perturbation step, and the magnitude of
the live load is not important.
• The live load is specified in the
∗BUCKLE step.

– The ∗BUCKLE step may be preceded by a
∗STATIC step in which the dead load is
applied.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.17
L5.18
ABAQUS Usage

– The buckling mode shapes of
symmetric structures are either
symmetric or antisymmetric.
• For such structures it is more
efficient to model only part of the
structure and to perform the
buckling analysis twice: once with
symmetric boundary conditions
and once with antisymmetric
boundary conditions.

– The live load pattern is usually
symmetric, so symmetric boundary
conditions are needed for the
calculation of the perturbation
stresses used in the formation of the
initial stress stiffness matrix.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

ABAQUS Usage

– The boundary conditions must be
switched to antisymmetric in the
∗BUCKLE step to obtain the
antisymmetric modes.
• This is done by giving the
antisymmetric boundary
conditions with LOAD CASE=2 on
the ∗BOUNDARY option in the
∗BUCKLE step.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.19

ABAQUS Usage

• Example 1: Antisymmetric buckling of a symmetric structure

Finite element model Boundary conditions Boundary conditions
for load case 1 for load case 2

• B21 elements

• Rectangular cross-section (1 in × 1in)

• Linear elastic material:

E = 30E6 psi
ν=0

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.20

ABAQUS Usage

• Partial input for antisymmetric buckling of a symmetric structure

*heading
antisymmetric ring buckling
eigenvalue estimate
:
:
*nset, nset=left
4
*transform, nset=left
1., 1., 0., -1., 1., 0.
*boundary
right, 2
right, 6
left, 2
left, 6
*step, name=Step-1
*buckle
3,
*boundary, load case = 2, op=new
right, 2
right, 6
left, 1
*dsload
ring, p, 1.
*end step

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.21

ABAQUS Usage

– The dead and live loads can be point loads, distributed loads, or thermal
loads; dead loads can also include nonzero prescribed boundary
conditions.

• If the live loads include uniform motion of a boundary, use multi-point
constraints to constrain these nodes to a single point and load that
point.

– The dead load, P0, and the live load, ∆P, can be entirely different in

magnitude and in nature.

– Multiple buckling modes and associated critical load values can be
obtained in a single eigenvalue buckling step.

• Obtaining multiple buckling modes is often useful since many common
systems (such as short cylindrical shells) have several closely spaced
critical modes.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.22

ABAQUS Usage

– Negative eigenvalues are sometimes obtained.
• These values can indicate that there is a buckling mode
corresponding to the load applied in the opposite direction.
– For example, a pressure vessel under internal pressure might
buckle under external pressure.
• However, they can also point to spurious modes if nonlinearities occur
before buckling.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.23

ABAQUS Usage

– The load stiffness can have a significant effect on the critical buckling load.

• ABAQUS will use the symmetric form of load stiffness in eigenvalue
calculations.

– Follower force effects are associated with pressure, hydrostatic pressure,
buoyancy effects, centrifugal loading, and Coriolis loading and also with
concentrated loads with the FOLLOWER option.

– Eigenvalue buckling analysis with concentrated FOLLOWER loads will not
yield the correct results since the follower force effects are not taken into
account (the load stiffness is generally not symmetric).

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.24

ABAQUS Usage

– If temperature-dependent elastic properties are used, the elastic stiffness
will be based on the temperatures prior to the eigenvalue buckling step.

• Modifying temperatures in an eigenvalue buckling step will not change
the elastic stiffness matrix.

– When nonlinear material properties such as hyperelasticity are present in a
model, ABAQUS/Standard ignores the nonlinear effects during the
eigenvalue buckling analysis.

• The material response during the buckling analysis is based on the
linear elastic stiffness in the (potentially nonlinear) base state at the
end of the previous step.

– Inelastic behavior such as plasticity can be used if the eigenvalue buckling
step is applied before the stress at any point has reached yield.

• ABAQUS will use the elastic stiffness, defined with linear elasticity, in

the eigenvalue buckling procedure to calculate ∆K, not the tangent

stiffness from the hardening curve.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.25

ABAQUS Usage

• Choice of eigenvalue extraction method
– In ABAQUS/Standard you have the choice of using either the subspace
iteration or the Lanczos method to extract the eigenvalues.
– The Lanczos method is generally faster when a large number of
eigenmodes are required for a system with many degrees of freedom.
• The subspace iteration method may be faster when only a few (less
than 20) eigenmodes are needed.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.26

ABAQUS Usage

– By default, the subspace iteration method is used when extracting the
buckling modes.
• To use the Lanczos solver, include the EIGENSOLVER=LANCZOS
parameter on the ∗BUCKLE option.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.27

ABAQUS Usage

– When the Lanczos eigensolver is requested, you can also specify the
minimum and/or maximum eigenvalues of interest on the data line.
• ABAQUS extracts eigenvalues until either the requested number of
eigenvalues has been extracted in the given range or all the
eigenvalues in the given range have been extracted.

– The Lanczos eigensolver has the following restrictions for buckling
simulations; it cannot be used with:
• A model containing hybrid elements
• A model containing distributing coupling elements
• A model containing contact pairs or contact elements
• A model that has been preloaded above the bifurcation (buckling) load

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Closely Spaced Eigenvalues

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.29

Closely Spaced Eigenvalues

– Certain buckling problems may have many buckling modes with very
closely spaced critical loads.
• The eigenvalue algorithm may converge slowly in such a case.

– Cylindrical shells with axial compressive loads are a good example of this
case.

Radius = 100
Length = 800
Thickness = 0.25
Young’s modulus = 30 × 106
Poisson’s ratio = 0.3

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.30

Closely Spaced Eigenvalues bottom

• Example 2: Buckling of a thin cylinder

– S9R5 elements

– Linear elastic material

– Lanczos eigensolver

– Symmetry (only half the cylinder length is modeled)

*heading

cylinder buckling

:

:

:

*step

*buckle, eigensolver=lanczos

5,

*cload Midside nodes
bot1, 3, 65450.0

bot2, 3, 32725.0 Corner nodes top

*boundary

bottom, 1, 2

top, zsymm

*node file

u

*end step

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.31

Closely Spaced Eigenvalues

– Critical stress as a function of mode shape (analytical results)

Axial modes Circum. modes Critical stress

1 4 40718.09
2 5 43291.86
6 9 44283.65
5 8 44292.48
8 10 44662.13
4 7 44711.87
9 11 44751.29
10 11 44867.94
3 6 44874.56
7 10 44909.49
3 7 45608.18
7 9 45718.54
10 12 45792.77
4 8 45827.96
… …
…

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.32

Closely Spaced Eigenvalues

– Critical buckling mode of axially compressed cylinder

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.33

Closely Spaced Eigenvalues

– Closely spaced eigenvalues are usually an indication that a structure is
imperfection sensitive.

• The imperfections cause the buckling modes to interact and will trigger
collapse at a much lower level than predicted by the eigenvalue
buckling analysis.

• Hence, the actual buckling mode shape is usually not the same as the
lowest buckling mode in the eigenvalue analysis.

– Convergence can be improved substantially by applying part of the critical
live load as a dead load, loading the structure to just below the buckling
load.

• This provides a larger separation of the eigenvalues and much
improved convergence.

• The process is equivalent to a dynamic eigenfrequency extraction with
shift.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.34

Closely Spaced Eigenvalues

– If you exceed the critical (lowest) buckling load of the structure when
applying the dead load, the analysis may terminate prematurely because
ABAQUS will not be able to find the lowest buckling loads.
• In addition, the Lanczos method will fail in that case.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.35

Closely Spaced Eigenvalues

– Buckling of axially loaded cylinder without imperfections

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.36

Closely Spaced Eigenvalues

– Buckling of axially loaded cylinder with imperfections

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.37

Closely Spaced Eigenvalues

• Example 3: Buckling of a thin cylinder with preload

*heading

cylinder buckling with preload

:

:

:

*step, nlgeom

*static

*cload

bot2, 3, 130900.0 preload
bot1, 3, 261800.0

*endstep

*step

*buckle, eigensolver=lanczos

5,

*cload

bot2, 3, 32725.0

bot1, 3, 65450.0

*node file

u

*end step

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.38

Closely Spaced Eigenvalues

– The analysis with the preload converges much faster.

• The analysis without the dead load has 5 converged eigenvalues after
60 iterations.

• The analysis with the dead load obtains 5 converged eigenvalues after
only 19 iterations.

– Buckling of thin-walled cylinders often involves high numbers of waves in
both axial and circumferential directions.

• For accurate results very refined meshes are needed.

– If reduced-integration elements are used, pseudobuckling modes involving
extensive hourglassing may be found.

• These modes do not affect physical buckling modes and can be
suppressed by increasing the hourglass control with the
∗HOURGLASS STIFFNESS option.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Concluding Remarks

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.40

Concluding Remarks

– Eigenvalue buckling analysis yields a reliable estimate for the buckling
load only if the assumptions of small geometric changes and linear elastic
material response before buckling are realistic for the structure being
modeled and if the collapse is not imperfection sensitive.

– If in doubt, introduce an imperfection (in the shape of the lowest buckling
modes) into the structure and use ∗STEP, NLGEOM with the ∗STATIC,
RIKS procedure to obtain the complete pre- and postbuckling history.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.41

Concluding Remarks

• For more examples of buckling and collapse analysis with ABAQUS see:
– ABAQUS Benchmarks Manual:
• 1.2.1 Buckling analysis of beams
• 1.2.2 Buckling of a ring in a plane under external pressure
• 1.2.3 Buckling of a cylindrical shell under uniform axial pressure
– ABAQUS Example Problems Manual:
• 1.2.2 Laminated composite shells: buckling of a cylindrical panel with
a circular hole
• 1.2.6 Buckling of an imperfection sensitive cylindrical shell

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Workshop 5a: Cargo Crane Buckling
Workshop 5b: Square Tube Buckling

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Lecture 6

Static Postbuckling and
Snap-Through Analysis

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.2

Overview

• Introduction
• ABAQUS Implementation
• ABAQUS Usage
• Snap-Through Problems
• Postbuckling Problems
• Introducing Imperfections for Postbuckling Simulations
• Postbuckling Examples
• Usage Hints
• Limitations
• Summary
• Workshop 6a: Cargo Crane – Riks Analysis
• Workshop 6b: Square Tube with Imperfections

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Introduction

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.4

Introduction

– Eigenvalue buckling analysis is useful for the analysis of “stiff” structures.

• The method is not suitable if large geometry changes occur prior to
buckling and can provide very misleading results if the structure is
imperfection sensitive.

– In cases where the eigenvalue buckling procedure is not applicable or its
results are questionable, a fully nonlinear transient analysis is required.

• A transient analysis can be done dynamically or by addition of viscous
forces to the static problem.

• The disadvantage of such analyses is that it is hard to understand the
characteristics of the structure after the load maximum is reached.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.5

Introduction

– To avoid any of the effects of the stabilizing forces,
we would like to obtain a solution to the static
equilibrium equation without adding such forces.

– An algorithm is needed in which the applied loads
are adapted automatically.
• The solution algorithm must solve
simultaneously for loads and displacements.

– As a consequence another quantity must be selected
to measure the progress of the solution.

• For this we choose the “arc length,” l, which is

the length along the static equilibrium path in
load-displacement space.
– A form of this method is activated in ABAQUS by
adding the RIKS parameter on the ∗STATIC option.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.6

Introduction

– Static analysis of snap-through and postbuckling problems with the arc-
length method provides valuable information about the characteristics of
structures in the unstable regime.

– The method works well if the equilibrium path in the load-displacement
space is smooth and does not branch.

• Otherwise, convergence and incrementation problems may occur.

• Generally, this means that the method should always be applied to
imperfect geometries—the “perfect” structure’s initial coordinates
should be perturbed to create a suitable imperfection.

• This converts a pure bifurcation behavior into a snap-through problem.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

ABAQUS Implementation

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.8

ABAQUS Implementation

• Riks method for globally Load
unstable problems P2

– Consider this load-
displacement curve:

P1 Converged solution for increment 1

Displacement

Unstable force-displacement curve

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.9

ABAQUS Implementation

– At the top of the curve the gradient equals zero and the stiffness is
singular. This can occur when structures “snap-through,” buckle, or
collapse.

• The structure’s instability may be the result of geometric or material
effects.

– In an unstable problem the structure must release energy to remain in
equilibrium. In reality, this energy is converted to kinetic energy.

– A way of studying a buckling problem is to use displacement control rather
than force control; i.e., you prescribe the motion of a particular part of the
model and look at the reaction forces to understand the load-displacement
behavior.

• Even with displacement control the structure may buckle dynamically.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.10

ABAQUS Implementation

– An alternative is to use the “modified Riks method.”

• The basic solution method is still the Newton-Raphson method, so the
usual convergence rules apply.

• It is the method by which the analysis progresses along the solution
path that is changed.

– The Riks method solves for both the displacements and the applied loads
to find the equilibrium path.

• The method can calculate solutions even when the slope of the force-
deflection curve is negative.

• The magnitude of the load must be expressed in terms of a load

proportionality factor, λ.

• The method uses the concept of “arc length” (l) to track the size of the

increment and how “far” the analysis has progressed.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.11

ABAQUS Implementation

• RIKS is an arc-length control procedure
– The solution is advanced along the load-deflection curve by
solving for the equilibrium position a particular arc-length away
from the last position.
Load

l
∆l

Displacement

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.12

ABAQUS Implementation

– In the Riks method we always deal with proportional loading within an
analysis step. The load is assumed to consist of:

• An initial load vector, P0, which has already been applied at the start

of the step and remains constant throughout the step.

• A load, λP, where P is a nominal load vector and λ is the “load

proportionality factor” that ABAQUS will find as part of the solution.

– In the simplest case P0 will be zero and P will be the result of distributing,

for example, a uniform pressure of unit magnitude onto the structure.

– In general, P is obtained as the difference between the reference load Pref
specified in the Riks step and the dead load, P0 :

P = Pref − P0 .

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

ABAQUS Usage

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.14

ABAQUS Usage

– The Riks procedure is invoked by including the Riks parameter on the
∗STATIC option.

• Since the method is generally used with geometrically nonlinear
cases, the NLGEOM parameter is usually included on the ∗STEP
option.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.15

ABAQUS Usage

– A typical input sequence for a postbuckling analysis is

*STEP, NLGEOM (apply optional dead load)
*STATIC…
(define the dead load and specify output requests)
*END STEP
*STEP, NLGEOM, INC=… (postbuckling Riks step)
*STATIC, RIKS
∆linit, lperiod, ∆ lmin, ∆ lmax, λend, node, dof, umax
(define the reference load and specify output requests)
*END STEP

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.16

ABAQUS Usage

– The first two entries on the ∗STATIC, RIKS data line define the initial and
estimated total arc lengths associated with the step.

*STATIC, RIKS
∆linit, lperiod, ∆ lmin, ∆ lmax, λend, node, dof, umax

∆linit
lperiod

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.17

ABAQUS Usage

– The second two entries are optional and form bounds for the arc length

increment, ∆l.

*STATIC, RIKS
∆linit, lperiod, ∆ lmin, ∆ lmax, λend, node, dof, umax

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.18

ABAQUS Usage

– The last four optional entries serve as alternate termination criteria.

*STATIC, RIKS
∆linit, lperiod, ∆ lmin, ∆ lmax, λend, node, dof, umax

• λ is provided to terminate the
end
step when the load exceeds a

certain magnitude.

• node, dof, umax are provided to

terminate the step when a
particular displacement
component exceeds a given
value.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.19

ABAQUS Usage

– ABAQUS will not stop exactly at these values but will stop when the values
are exceeded.

– If none of the above termination criteria is included, ABAQUS will stop
when the maximum number of increments is reached or when the solution
fails (for example, because of excessive distortion).

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.20

ABAQUS Usage

– Any amplitude references are ignored in the Riks procedure.

• All loads are ramped from the initial (dead load) value to the reference
value specified.

• If the reference load is equal to the dead load, the Riks procedure will
fail.

• The load magnitudes are available as output.

– The status (.sta) file shows clearly that a step uses the Riks procedure.

SUMMARY OF JOB INFORMATION:

MONITOR NODE: 1 DOF: 2

STEP INC ATT SEVERE EQUIL TOTAL TOTAL STEP INC OF DOF IF
TIME/ TIME/LPF TIME/LPF MONITOR RIKS
DISCON ITERS ITERS FREQ

ITERS

1 11 0 3 3 0.0471 0.04713 -0.195 R
0.0882 0.04110 -0.397 R
1 21 0 2 2 0.138 0.04958 -0.714 R
0.184 0.04638 -1.22 R
1 31 0 3 3 0.200 0.01590 -2.00 R
0.177 -0.02278 -2.93 R
1 41 0 3 3
λ ∆λ
1 51 0 3 3

1 61 0 3 3

flag indicating that this
is a Riks analysis

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Snap-Through Problems

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.22

Snap-Through Problems

– The Riks method works very well for snap-through problems.

• Classical snap-through problems are characterized by a smooth load-
displacement curve and do not exhibit branching (bifurcation).

• As a result, the Riks procedure can solve this kind of problem with
ease.

• Generally, you do not need to take any special precautions to ensure
a successful analysis.

– An example of a problem with a smooth load-displacement curve (taken
from the ABAQUS Example Problems Manual) is the shallow-arch problem
shown on the following pages.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.23

Snap-Through Problems

Example 1: Shallow circular arch under pressure

Copyright 2004 ABAQUS, Inc. L6.24

ABAQUS: Selected Topics

Snap-Through Problems

• History input for shallow circular arch

*step, nlgeom
loading
*static, riks
0.05, 1.0, , 0.2, 0.4
*dsload
arch, p, 5000.
.
.
.
*end step

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.25

Snap-Through Problems

• Load-displacement curve of shallow arch

Copyright 2004 ABAQUS, Inc.
ABAQUS: Selected Topics

Postbuckling Problems

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.27

Postbuckling Problems

– The Riks method can also be used to solve postbuckling problems, both
with stable and unstable postbuckling behavior.

– The exact postbuckling problem cannot be analyzed directly because of
the discontinuous response at the point of (bifurcation) buckling.

– To analyze the problem, you must turn it into a problem with continuous
response instead of bifurcation.

• The problem can be converted by introducing an initial imperfection in
the model so that there is some response in the buckling mode before
the critical load is reached.

– If the imperfection is small, the deformation will be quite small (relative to
the imperfection) below the critical load.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.28

Postbuckling Problems

– The response will grow quickly near the critical load, introducing a rapid
change in behavior.

• Such a rapid transition is difficult to analyze.

– If the imperfection is large, the postbuckling response will grow steadily
before the critical load is reached.

• The transition into postbuckled behavior will be smooth and relatively
easy to analyze.

– Imperfections are usually introduced as perturbations in the initial
geometry of the model.

– Imperfections can also be introduced by perturbations in the loads or the
boundary conditions.

– Moreover, imperfections based on linear buckling modes can be useful for
analyzing structures that behave inelastically prior to reaching peak load.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Introducing Imperfections for
Postbuckling Simulations

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.30

Introducing Imperfections for Postbuckling Simulations

– Imperfections in otherwise “perfect” models are necessary to develop
models that are suitable for use in postbuckling analyses.

– Two methods are used to introduce imperfections into a model:
1. Geometric imperfections are the most commonly used method.
Perturbations in the model’s initial geometry cause the structure
to buckle in the appropriate manner.
2. Loading imperfections may also be used to ensure that the structure
buckles in the appropriate manner.
Small fictitious “trigger loads” are used to deform the model so
that it buckles correctly.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.31

Introducing Imperfections for Postbuckling Simulations

• Geometric imperfections:
– They are typically based on previous eigenvalue buckling analyses.
– A few of the buckling modes are used typically to perturb the geometry.
• However, the lowest buckling modes are assumed to provide the most
critical imperfections, so usually the lower modes are scaled and
added to the perfect geometry to create the perturbed mesh.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.32

Introducing Imperfections for Postbuckling Simulations

– The magnitude of the imperfection should be chosen realistically.

• For example, the size of the imperfections may be determined by
manufacturing tolerances.

• Often the magnitude is chosen as a few percent of a relevant
structural dimension such as a beam cross-section or a shell
thickness.

– In shells the imperfection magnitude is typically chosen to be
1%–100% of the thickness.

– Only the coordinates of the nodes are affected; the nodal normals are not
modified.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.33

Introducing Imperfections for Postbuckling Simulations

• Loading imperfections:
– The “trigger loads” should perturb the structure in the expected buckling
modes.
– Typically, these loads are applied as “dead” loads prior to the Riks step so
that they have a fixed magnitude.
– The magnitude must be sufficiently small so that the trigger loads do not
affect the overall postbuckling solution.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.34

Introducing Imperfections for Postbuckling Simulations

• Introducing geometric imperfections

– Use the ∗IMPERFECTION option to introduce geometric imperfections for
postbuckling and collapse simulations.

– The geometric imperfection can be based on nodal displacements written
to the results (.fil) file during a previous simulation.

• The FILE parameter is used to identify the name of the results file
from the previous simulation.

• The STEP parameter must be used to identify the step from the
previous analysis containing the results that will define the geometric
imperfection.

• An imperfection that uses only a subset of the model’s nodes can be
created by using the optional NSET parameter to identify the subset.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.35

Introducing Imperfections for Postbuckling Simulations

– Imperfections can be formed by the superposition of weighted eigenmodes
from a previous eigenvalue buckling or frequency extraction analysis.

– Any number of eigenmodes can be specified and scaled with this option.
– The syntax for this case is:

*IMPERFECTION, FILE=file_name, STEP=n [, NSET=name]
mode_number, scale_factor

– Eigenmodes are stored such that the largest component of displacement
has a magnitude of 1.0.
• Therefore, they must be scaled to give an appropriate imperfection.

This option is not currently supported by ABAQUS/CAE. You
may use the Keywords Editor to add it to your model, however.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.36

Introducing Imperfections for Postbuckling Simulations

– Geometric imperfections can also be based on the scaled displacements
from a previous static simulation.

• Only the displacements from a single increment can be used to form
the imperfection.

– Use the INC parameter to identify the specific increment containing the
results that will define the geometric imperfection. The syntax for this case
is

*IMPERFECTION, FILE=file_name, STEP=n, INC=m
1, scale_factor

First data line entry must
be set to 1 in this case.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.37

Introducing Imperfections for Postbuckling Simulations

– You can also define geometric imperfections directly with the
∗IMPERFECTION option.

• By default, such imperfections are given in the global Cartesian
coordinate system.

• The SYSTEM parameter may be used if the imperfections are defined
in an alternative coordinate system (either cylindrical or spherical).

• The data for this format of the ∗IMPERFECTION option can be read
from a separate file. The INPUT parameter identifies the additional file
containing the imperfection data.

– The syntax for this format is:

*IMPERFECTION [, SYSTEM=C or S, INPUT=file_name]
node_number, U1, U2, U3

where U1, U2, and U3 are the components of the imperfection that will be

added to the node’s initial position.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.38

Introducing Imperfections for Postbuckling Simulations

– For accurate postbuckling analysis of such structures, it is important that
the imperfections be chosen correctly.
• The magnitudes of the imperfections should be chosen appropriately.
• It is safest to introduce an imperfection of the proper magnitude
consisting of several superimposed buckling modes.
• The weight of the various modes must be chosen by the user; usually
the lowest buckling mode should have the largest weight.

• Imperfections consisting of a single buckling mode tend to yield
nonconservative results.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.39

Introducing Imperfections for Postbuckling Simulations

– No default protections are provided to check whether or not the resulting
perturbed geometry is reasonable.

• It is the user’s responsibility to ensure that the geometry of the model
to be analyzed is representative of the problem being considered.

• ABAQUS/Viewer can be used to visualize the imperfections to the
model.

– Likewise, no default protections are provided to check whether or not any
of the applied trigger loads are reasonable.

• It is the user’s responsibility to choose appropriate magnitudes and
locations for such fictitious loads.

– Most often, a number of analyses are carried out to investigate the
sensitivity of the results to the types of imperfections used in a
postbuckling calculation.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.40

Introducing Imperfections for Postbuckling Simulations

– Certain structures (in particular thin shells) can be very imperfection
sensitive.

• Imperfection sensitivity means that the load-carrying capacity
decreases rapidly with increased imperfection size.

• The actual load-carrying capacity of such structures is usually much
less than that predicted by eigenvalue buckling analysis.

– Often these structures are characterized by closely spaced eigenvalues in
an eigenvalue buckling analysis.

• The interaction of the buckling modes causes the rapid degradation in
load-carrying capacity.

• Use all (or many) of the eigenmodes associated with closely spaced
eigenvalues to seed the imperfection.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Postbuckling Examples

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.42

Postbuckling Examples

• Example 2: Rectangular frame with point load at corner
– The (lowest) critical load and buckling mode are easily obtained with the
eigenvalue buckling procedure.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.43

Postbuckling Examples

– We use the buckling mode to introduce an imperfection with an amplitude
of −0.1% of the frame height and analyze the resulting structure with the
Riks method.

name of previous analysis
scale factor

eigenmode

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.44

Postbuckling Examples

– The load-displacement curve is shown below:

– Since this is a nonsymmetric structure, different behavior is obtained if the
sign of the imperfection is reversed.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.45

Postbuckling Examples Perturbed geometry of the cylindrical
shell (imperfection factor = 5 × thickness
• Example 3: Buckling of an imperfection- for illustration only; actual imperfection
sensitive cylindrical shell factor used = .5 × thickness).

– Problem 1.2.6 in the ABAQUS Example
Problems Manual.

– Simply supported cylinder loaded by
uniform, compressive axial load.

– Internal pressure also applied
(increases imperfection sensitivity of the
cylindrical shell).

– Very thin shell (t/r = 1/500).

– Refined mesh: Full length model
accounts for both symmetric and anti-
symmetric buckling modes.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.46

Postbuckling Examples

– Solution procedure:
1. Perform linear eigenvalue buckling analysis.
2. Introduce imperfections using different combinations of modes.
– Fix imperfection size by prescribing the maximum “out-of-
roundness.”
3. Postbuckling analysis using the Riks method.

– Repeated eigenvalues:
• The presence of repeated eigenvalues implies there is no preferred
direction.
• The mode shapes associated with repeated eigenvalues are always
the same; their phases, however, may vary between analyses (and
computer platforms).

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.47

Postbuckling Examples

• As the relative phase between repeated modes changes, the
imperfection and therefore the postbuckling response changes.

• To overcome these problems, the phase is fixed before the
postbuckling analysis is performed.

• In this example, the eigenvectors associated with repeated
eigenmodes are scaled such that their linear combination generates a

maximum displacement of 1 on the X-axis.

– A FORTRAN program is run to read the results file from the linear
eigenvalue analysis to generate the imperfection:

• The scale factors are computed for linear combinations of repeated
eigenmodes.

• The maximum “out-of-roundness” is enforced.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.48

Postbuckling Examples

– Results: First 19 eigenvalues of the cylindrical shell.

Eigenvalues of the cylindrical shell

Mode number Eigenvalue

1 11721
2, 3 11722
4, 5 11726
6, 7 11733
8, 9 11744
10, 11 11758
12, 13 11777
14, 15 11802
16, 17 11833
18, 19 11872

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.49

Postbuckling Examples

– The buckling load is normalized with respect to the linear eigenvalue
buckling load. The results when different modes are used to seed the
imperfection are shown below.

Normalized buckling loads

Mode used to seed Normalized
the imperfection buckling load

1 0.902
2, 3 0.707
4, 5 0.480
6, 7 0.355
8, 9 0.351
10, 11 0.340
12, 13 0.306
14, 15 0.323
16, 17 0.411
18, 19 0.422
All modes (1–19) 0.352

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.50

Postbuckling Examples

• Load-displacement curve

Load displacement curve when first 19 modes
are used to seed the imperfection

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Usage Hints

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.52

Usage Hints

– The Riks procedure works very well for problems exhibiting global snap-
through behavior.

– Since the solution may pass unstable points, it is important that the
residuals at the beginning of a new increment be small.

• The default tolerances in ABAQUS are sufficiently tight in most cases;
however, for very unstable postbuckling problems, tighter tolerances
may need to be specified with the ∗CONTROLS option—particularly if
the prebuckling behavior is nearly linear and very rapid stiffness
changes occur near the instability point.

– Even with tight controls, the procedure may fail if such a point is
approached with large load increments.

• Under such circumstances the load and the solution may track back to
the starting point, as shown in the following figure.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.53

Usage Hints

– Backtracking near a sharp transition:

Copyright 2004 ABAQUS, Inc. L6.54

ABAQUS: Selected Topics

Usage Hints

– You can make the problem easier by
introducing a larger imperfection into
the initial model so that the
nonlinearity in the overall response is
less severe.

– You can avoid the problem by limiting

the arc length increment with ∆lmax.

• If the problem has already
occurred, you can correct it by
using the ∗RESTART, READ,
END STEP option just before the
instability point to make sure that
the point is approached with
small arc length increments.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.55

Usage Hints

– The analysis of problems involving local instabilities sometimes leads to
difficulties.

• Such instabilities cause local growth of the solution, which may be
insufficiently constrained by the algorithm.

• In addition, local instabilities can be “fueled” by release of elastic
energy from other parts of the structure, which makes it difficult to
control the solution by changing the applied load.

– Nevertheless, with careful control of the increment size, it is often possible
to complete such analyses successfully.

Copyright 2004 ABAQUS, Inc.
ABAQUS: Selected Topics

Limitations

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.57

Limitations

– The Riks postbuckling procedure requires that the equilibrium path be
continuous.
• Such continuity is not present in instability problems involving loss of
contact constraints, as shown below:

Snap-through of shallow, cylindrical roof under a point load applied to A

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.58

Limitations

– Loss of contact occurs as the roof snaps through.
• When the contact force is zero, the roof and Point A have separated.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.59

Limitations

– Problems with discontinuities typically occur when the load on a structure
is applied by motion of a rigid surface and the structure buckles under the
applied load.

• Once the structure buckles away from the constraints, the solution can
no longer be controlled by the applied loads and the Riks algorithm no
longer has any beneficial effect.

– In such cases a successful solution will be obtained only if the regular
Newton algorithm is able to bridge the gap in the equilibrium path at this
point.

• If the jump cannot be made, the analysis may fail or backtrack.

• In some cases the contact surface moves back but the structure
freezes in a load-free, unstable equilibrium configuration.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Summary

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L6.61

Summary

– The static Riks procedure in ABAQUS is a useful tool for the analysis of
snap-through and postbuckling problems.

– Snap-through problems are handled with relative ease.
– For postbuckling problems you must ensure that:

• Suitable imperfections are introduced.
• Sufficiently small load increments are chosen.
– Extra tight controls may be required for very unstable postbuckling and
localization problems.
– For postbuckling problems involving loss of contact, the Riks method will
usually not work and inertia or viscous damping forces must be introduced
to stabilize the solution.
• Such procedures are discussed in Lecture 7.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Workshop 6a: Cargo Crane – Riks
Workshop 6b: Square Tube with
Imperfections

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Lecture 7

Damped Static Postbuckling Analysis

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.2

Overview

• Motivation
• Automatic Stabilization and Dashpots
• Postbuckling and Loss of Contact
• Example
• Summary
• Workshop 7a: Cargo Crane – Damped Static Analysis
• Workshop 7b: Cargo Crane – Dynamic Analysis

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Motivation

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.4

Motivation

– To obtain an accurate assessment of the postbuckling behavior of
structures, static analysis methods are preferred because they provide
insight into the postbuckling characteristics of the structure.

– However, it is not always possible to carry out such an analysis: in
situations where loss of contact occurs or where the deformation localizes,
the static postbuckling method may fail to yield a solution.

• In such cases a transient analysis can be done, either dynamically or
statically with viscous forces.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.5

Motivation

– The addition of inertial forces provides a solution to the physical
postbuckling behavior.

– However, it is not always required or even desired that the actual dynamic
solution be obtained.

• In many cases the objective of the analysis is not to simulate the
actual dynamic response but to obtain the static equilibrium state after
buckling.

– In some cases, such as in automotive roof crush or side intrusion
calculations, elastic buckling is only an initial effect that is followed by
extensive bending and plastic deformation.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.6

Motivation

– In such cases a more effective and less “noisy” solution may be obtained
through the addition of suitable “damping” forces in a static analysis.

– There are two ways in which damping can be introduced in a static analysis:
• Damping can be introduced using automatic viscous damping with the
ABAQUS static procedure options.
• Alternatively, discrete dashpots can be added to the model.
– Element type DASHPOT1 can be used to damp absolute motions.
– Element type DASHPOT2 can be used to damp relative motions.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L7.7

Motivation

– If damping is used in static analysis, the velocity is assumed to be equal to
the displacement increment divided by the time increment.

– Assume that the cumulative effect of all damping added to the static model

is described by the damping matrix C.

– The equilibrium equations can then be written in the form

Cu& + I = C∆u / ∆t + I = P.

– In linearized form this becomes

 1
K + ∆t C  cu = P − I − C∆u / ∆t.

– It is clear that the damping matrix becomes more important when the time
increment decreases.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Automatic Stabilization and Dashpots

Copyright 2004 ABAQUS, Inc.