usyd_abaqus_2006

ABAQUS: Selected Topics L3.19

Yield Functions

( )– The yield function of the metal plasticity models, f σ ,σ 0 , defines when

the metal begins to deform inelastically.

• When f = 0, the metal is yielding.
• σ is the true stress in the metal (it is a tensor quantity).
• σ 0 is the yield stress (usually a scalar quantity).

– The yield function is often written in terms of stress invariants. The
commonly used stress invariants are

equivalent pressure stress, p = − 1 trace(σ ),

3

Mises equivalent stress, q = 3 ( S : S ),

2

where S is the deviatoric stress, defined as σ = S − pI.
• Note that for uniaxial loading, q = σuniaxial.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.20

Yield Functions

– There are two yield functions available for the classical metal plasticity
models in ABAQUS:
• The Mises yield function,

f = q −σ 0.

• Hill’s anisotropic yield function,

2 + G (σ zz − σ xx )2 + H 2
( ) ( )f = 2 2 2 −σ 0.
F σ yy − σ zz σ xx − σ yy + 2Lσ yz + 2M σ zx + 2Nσ xy

F, G, H, L, M, and N are

material constants

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.21

Yield Functions

– The Mises yield function is suitable when:
• The metal is subjected to monotonic loads, such as crash analyses
and forming simulations.
• The material has isotropic yielding.

– Hill’s yield function is intended for metals that have initial anisotropy in their
yield behavior.
• The anisotropy does not evolve with plastic deformation of the
material.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.22

Yield Functions

– Defining Mises plasticity in ABAQUS

*Material, name=steel

*Elastic Linear elasticity

2.e11, 0.3

*Plastic Plastic strain at
4.e8, 0.0 initial yield = 0.0
4.2e8, 0.02

5.e8, 0.2

6.e8, 0.5

True stress and log plastic strain

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.23

Yield Functions

– Defining Hill’s plasticity in ABAQUS

*Material, name=steel
*Elastic
2.e11, 0.3
*Plastic
4.e8, 0.0
4.2e8, 0.02
5.e8, 0.2
6.e8, 0.5
*Potential
1.5, 1., 1., 1., 1., 1.

Stress ratios; can
be functions of
temperature and
field variables.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.24

Yield Functions

– ABAQUS calculates the values of the constants F, G, H, L, M, and N of

Hill’s yield function from stress ratios:

R11 = σ11 σ 0, R22 = σ 22 σ 0, R33 = σ 33 σ 0

R12 = σ12 τ 0, R13 = σ13 τ 0, R23 = σ 23 τ 0

where σ11, σ 22, K are the yield stress values when σ ij is the only
nonzero component of stress, σ 0 is the reference yield stress value and
τ0 =σ 0 3.

σ 0 is given on the *PLASTIC option or in the Plastic definition area of

the material editor; it is usually chosen as one of the three direct yield
stress magnitudes.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.25

Yield Functions

• Example: cylindrical cup deep drawing with transverse anisotropy

– We examine two cases: one in which the material is considered isotropic,
another in which transverse anisotropy is assumed. This example is
modeled using the ∗POTENTIAL option within the material block:

∗POTENTIAL
1., 1., 1.1511, 1., 1. , 1.

– Plots of blank thickness in the final formed configuration for both cases are
shown in the figures on the next page.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.26

Yield Functions

– The effect of the anisotropy on the thickness is readily apparent, as the
increased strength in the thickness direction results in less thinning of the
blank.

isotropic anisotropic

Effect of transverse anisotropy on blank thickness

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Hardening

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.28

Hardening

• Yield surface must be coupled to a hardening relationship
– The yield surface may change as a result of plastic deformation. The
change in the yield surface is defined by the hardening law.
– The following hardening laws are available in ABAQUS:

• Perfect plasticity Intended for applications such as
• Isotropic hardening crash analyses, metal forming,
and general collapse studies.
• Kinematic hardening
• Combined isotropic/kinematic hardening Intended for applications
involving cyclic loading.
• Johnson-Cook plasticity
Well suited to model high-strain-
rate deformation of metals; only
available in ABAQUS/Explicit.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.29

Hardening

• Perfect plasticity (no hardening)
– Simplest definition of plasticity

– In perfect plasticity the metal’s yield function, f, does not evolve as the

metal accumulates plastic strains.
– Perfect plasticity can be used with either the Mises or the Hill yield

function.
– Perfect plasticity is defined by providing only one value for the yield stress

of the metal, σ 0.

Copyright 2005 ABAQUS, Inc. L3.30

ABAQUS: Selected Topics

Hardening

– Defining perfect plasticity in ABAQUS

*Material, name=steel
*Elastic
2.e11, 0.3
*Plastic
4.e8, 0.0

One value of the yield

stress of the metal, σ 0,

is provided.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.31

Hardening

• Isotropic hardening (default)

– Isotropic hardening is used to model gross plastic straining or when
straining at a point is essentially in the same direction in strain space.

– The yield stress increases (or decreases) uniformly in all stress directions
as plastic straining occurs

– With isotropic hardening the metal’s yield stress evolves as the metal

( )accumulates plastic strains, σ 0 ε pl .

ε pl is the equivalent plastic strain, defined as

∫ε pl = t 2 ε& pl : ε& pl 
 dt.
0 3 

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.32

Hardening

• ε pl is obtained through the variable PEEQ in ABAQUS.

– It is obtained by integrating the equivalent plastic strain rate over
the history of the deformation.

– Thus, it always grows with any plastic deformation.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.33

Hardening

– Define isotropic hardening by

providing tabular data of σ 0 and ε pl .

– Isotropic hardening can be used
with either Mises or Hill’s yield
function.

*Material, name=steel
*Elastic
2.e11, 0.3
*Plastic
4.e8, 0.0
4.2e8, 0.02
5.e8, 0.2
6.e8, 0.5

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.34

Hardening

• Linear kinematic hardening
– Linear kinematic hardening is used to model the behavior of metals
subjected to cyclic loading.
– The linear kinematic model defines the yield function as

f = q(σ −α ) −σ 0 = 0.

α is the backstress tensor that describes how the center of the yield

surface moves in stress space as plastic strains accumulate.

• q (σ −α ) can be either Mises or Hill’s yield potential (function).

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.35

Hardening

– Define linear kinematic hardening ( )σ 0 , ε pl
by providing the initial yield
1.0 (σ , 0)
stress, σ 0, and the yield stress, 0
σ 0(ε pl), at some finite plastic [×103]
Stress—S11
strain. 0.5
−5. 0. 5. 10.
• Pick the second data point 0.0
from stabilized cyclic test
data. −0.5

• The linear kinematic −1.0
hardening data can be a −10.

function of θ only. Strain—E11 [×10−3]

• No field variable ( fi ) or rate

dependence is allowed

Calibrating the linear kinematic
hardening model

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.36

Hardening

– Sample usage:

*Material, name=steel
*Elastic
200.E3,.3
*Plastic, hardening=kinematic
200., 0.0
220., 0.0009

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.37

Hardening

– The linear kinematic model can provide a first-order approximation of the
anisotropic hardening that occurs in metals when they are loaded
cyclically.

• The model accounts for the translation of the yield surface with plastic
deformation but does not consider any change in the size of the yield
surface.

• The linear kinematic model is valid only for relatively small strains

(ε < 0.05).

• Approximates the Bauschinger stress A
effect seen in cyclic loading.
Y

B

O strain

C
Y

−

The Bauschinger
effect

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Input of Material Data for Plasticity

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L3.39

Input of Material Data for Plasticity

– Experimental measurements are often reported in terms of nominal
(engineering) stress versus nominal strain. For approximately
incompressible material behavior, a simple conversion to true stress and
logarithmic strain can be carried out:

( )σ true = σ nom 1+ εnom ,

εln = ln (1+ εnom ).

– These expressions relate true stress versus logarithmic total strain.

ABAQUS requires true stress versus logarithmic plastic strain to be

defined with the plasticity model options. Logarithmic plastic strain can be

obtained from logarithmic total strain using

ε lpnl = εln − σ true .
E

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Workshop 3a: Plasticity and Hardening
Workshop 3b: Skew Plate with
Plasticity

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Lecture 4 L4.2

Materials - Concrete

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Overview

• Introduction
• Mechanical Behavior of Plain Concrete
• ABAQUS Constitutive Models for Concrete
• Concrete Smeared Cracking
• Usage
• Calibration
• Modeling Aspects
• Reinforcement Modeling
• Workshop 4: Collapse of a Concrete Slab

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Introduction

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.4

Introduction

• ABAQUS offers a variety of constitutive material models suited for the
analysis of concrete structures.

• This lecture is intended as an introduction to the Smeared Cracking
Model in ABAQUS/Standard.
– Suitable for modeling reinforced concrete under low confining pressures
and monotonic loading.
– Other models are available, but are beyond the scope of this course.

• This lecture also provides an overview of modeling reinforcement.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.5

Introduction

• Typical applications
– Collapse load calculations of structural components, such as reinforced
beams, columns, shear walls, etc.
– Nuclear reactor engineering: Failure analysis of reinforced concrete
containment by overpressurization
– Road and bridge engineering

Copyright 2005 ABAQUS, Inc.
ABAQUS: Selected Topics

Mechanical Behavior of Plain Concrete

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.7

Mechanical Behavior of Plain Concrete

• Concrete behaves as a quasi-brittle material except under high triaxial
compression.

• Unlike classically brittle solids, concrete can undergo inelastic
deformation that may be significantly larger than the elastic strains.

• What follows are general observations about the macroscopic behavior of
typical plain concrete.

– These observations are useful for constructing and understanding
constitutive models

– No attempt is made to discuss the highly complex microscopic behaviour
of concrete

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.8

Mechanical Behavior of Plain Concrete

• Uniaxial behavior
– Beyond some stress threshold, concrete behaves nonlinearly, exhibiting
progressive and irreversible damage until complete collapse occurs.
– Strain softening results from the formation of micro-cracks.

Uniaxial compression behavior Uniaxial tension behavior

Karsan and Jirsa (1969) Mazars and Pijaudier-Cabot (1989)

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.9

Mechanical Behavior of Plain Concrete

• Dilatancy: Volume increase that results from the formation and growth of
cracks parallel to the direction of the greatest compressive
stress.

Typical plot of compressive stress vs. axial, lateral, and volumetric strain

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.10

Mechanical Behavior of Plain Concrete

• Biaxial loading
– Under biaxial compressive loading, concrete strength is greater than the
one observed in uniaxial tests.

Compressive stress vs. strain components and volumetric strain under biaxial-compressive loading

Kupfer et al. (1969)

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.11

Mechanical Behavior of Plain Concrete

• Biaxial strength envelope

Biaxial strength envelope of concrete Failure modes of biaxially loaded concrete

Kupfer et al. (1969)

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.12

Mechanical Behavior of Plain Concrete

• Triaxial loading
– Under high confining pressure, crack propagation is prevented. The brittle
behavior disappears and is replaced by ductility with work hardening.

Triaxial concrete behavior

Chen (1982)

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.13

Mechanical Behavior of Plain Concrete

• Cyclic behavior
– Plasticity and stiffness degradation
– Stiffness recovery upon load reversal (unilateral effect)

Stress-deformation curve under cyclic Stress-deformation curve under cyclic
loading (small compressive stress) loading (large compressive stress)

Reinhardt and Cornelissen (1984) Reinhardt and Cornelissen (1984)

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

ABAQUS Constitutive Models for
Concrete

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.15

ABAQUS Constitutive Models for Concrete

• ABAQUS uses a continuum description of the concrete material response
instead of tracking discrete “macro” cracks. Constitutive calculations are
performed independently at each integration point.

• Models for concrete at low pressure stress
– Smeared cracking model (ABAQUS/Standard)
– Brittle cracking model (ABAQUS/Explicit)
– Concrete damaged plasticity model

• Models for concrete under high compression
– Cap model

• This lecture will only cover the smeared cracking model

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.16

ABAQUS Constitutive Models for Concrete

• Modeling reinforcement – “Tension Stiffening”

– In ABAQUS reinforcement in concrete structures is typically provided by
means of rebar and/or embedded elements.

– With this modeling approach, the concrete behavior is considered
independently of the rebar.

– Effects associated with the rebar/concrete interface, such as bond slip and
dowel action, are modeled approximately

– This is done by introducing some “tension stiffening” into the post-
cracking concrete response to simulate load transfer across cracks
through the rebar.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.17

ABAQUS Constitutive Models for Concrete

• Brittle cracking model
– Intended for applications in which the concrete behavior is dominated by
tensile cracking and compressive failure is not important.
– Includes consideration of the anisotropy induced by cracking.
– The compressive behavior is assumed to be always linear elastic.
– A brittle failure criteria allows the removal of elements from a mesh.
– This material model is not discussed further in this class.
• For more information see “Cracking model for concrete,” section
11.5.2 of the ABAQUS Analysis User's Manual.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.18

ABAQUS Constitutive Models for Concrete

• Concrete Damaged Plasticity Model
– Intended as a general capability for the analysis of concrete structures
under monotonic, cyclic, and/or dynamic loading
– Scalar (isotropic) damage model, with tensile cracking and compressive
crushing modes
– Degradation of elastic stiffness in both tension and compression
– Takes into account stiffness recovery effects in cyclic loading
– This material model is not discussed further in this class.
• For more information see “Concrete damaged plasticity,” section
11.5.3 of the ABAQUS Analysis User's Manual.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Smeared Cracking Model

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.20

Smeared Cracking Model

– Intended for applications in which concrete is subjected to essentially
monotonic straining and a material point exhibits either tensile cracking or
compressive crushing.

– Plastic straining in compression is controlled by a “compression yield”
surface.

– Tensile cracking occurs when the stress reaches the “crack detection”
surface.

– Cracking is assumed to be the most important aspect of the behavior, and
the representation of cracking and post-cracking anisotropic behavior
dominates the modeling.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.21

Smeared Cracking Model

• Features of smeared cracking model

• Compressive response
– Elastic-plastic with
hardening/softening
– Undamaged elastic
stiffness

• Tensile response

– Elastic with failure

– Post-failure softening and
damaged elasticity

Unixaxial behaviour of plain concrete

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.22

Smeared Cracking Model

• Multiaxial response
– Yield and failure surfaces are
fitted to experimental data

Yield and failure surfaces in the (p–q) plane Yield and failure surfaces in plane stress

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.23

Smeared Cracking Model

• Tensile Crack Detection
– Cracking is assumed to occur when the stress reaches “crack detection
surface.”
– Cracks are irrecoverable: they remain for the rest of the calculation (but
may open and close).
– No more than three orthogonal cracks can occur at any point (in 3D).
– Following crack detection, the crack affects the calculations because a
damaged elasticity model is used.
– Stiffness degradation affects the normal stiffness and optionally the
shear stiffness as well (using the Shear Retention option).

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.24

Smeared Cracking Model Post-failure response in tension

• Post-cracking Response
– Defined by “tension
stiffening” curve input
by user
– This is the
mechanism by which
the rebar/concrete
interaction is modeled
– Also includes
damaged elasticity
normal to crack
– Optionally, can
include degradation
of shear stiffness

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Usage L4.26

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Usage

• Isotropic Linear Elasticity for
undamaged elastic response

***
** MATERIALS
**
*Material, name=concrete
*Elastic
29000., 0.18

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.27

Usage

• Defining the plastic response in compression
– User enters the uniaxial stress-strain response
– Give tabular data defining yield stress as a function of plastic strain
– Data is usually readily available from a uniaxial compression test

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.28

Usage

• Plastic response in compression

***

** MATERIALS

**

*Material, name=concrete

*Elastic

29000., 0.18

*Concrete

18.4, 0.

32., 0.0013

Yield stress as function of
plastic strain

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.29

Usage

• Post-cracking tensile response – “tension stiffening”
– The post-crack response is defined by a tension stiffening curve
– Two possible ways of specifying tension stiffening:
• Postfailure stress-strain relation
• Fracture energy cracking criterion (stress-displacement relation)
– The default is to define a Postfailure stress-strain relation (Type=Strain)
• Give tabular data defining fraction of stress remaining versus post-
cracking strain

Ratio of stress to
failure stress 1.0

Crack opening strain

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.30

Usage

• Tension stiffening – continued…

– When there is no reinforcement in the concrete, the stress-strain softening
approach introduces unreasonable mesh sensitivity.

– To deal with this, we assume that the fracture energy to open a unit area of

crack, Gf , is a material property.

– With this approach the concrete’s brittle behavior is characterized by a
stress-displacement response rather than a stress-strain response.

– Use Type=Disp to activate this approach

• Specify the displacement, u0, at which linear loss of strength gives

zero stress

Ratio of stress to 1.0 u0
failure stress

Crack opening
displacement

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.31

Usage

Mesh sensitivity for unreinforced concrete:

P
u

Constant softening slope Constant fracture energy

P (σ−ε) P (σ−u)

1 element 1, 2, 4, and 8 elements

84 2 elements u

u *Tension Stiffening, Type=Disp

*Tension Stiffening, Type=Strain

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.32

Usage

• Tension stiffening – continued…
– The user must specify the tension stiffening behaviour; it cannot be
omitted.
– However, this data is not easily specified since the tension stiffening
behaviour depends on the amount an orientation of reinforcement
– But it is very important to the behaviour of the model
– See later comments on Calibration and Modelling Aspects

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.33

Usage

• Tension stiffening

***

** MATERIALS

**

*Material, name=concrete

*Elastic

29000., 0.18

*Concrete

18.4, 0.

32., 0.0013

*Tension Stiffening

1., 0.

0., 0.0008

Fraction of Post-
remaining cracking
stress strain

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.34

Usage

• Defining the yield/failure surfaces

– The user can enter four ratios to define the yield and failure surfaces

• Ratio of ultimate biaxial compressive stress to ultimate uniaxial
compressive stress

• Ratio of uniaxial tensile stress at failure to ultimate uniaxial
compressive stress

• Ratio of magnitude of principal plastic strain at ultimate stress in
biaxial compression to plastic strain at ultimate stress in uniaxial
compression

• Ratio of tensile principal stress at cracking in plane stress (when the
other principal stress is at the ultimate compressive value) to the
tensile cracking stress in uniaxial tension

– If this data is not specified, default values are used

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.35

Usage

• Failure ratios

***

** MATERIALS

**

*Material, name=concrete

*Elastic

29000., 0.18

*Concrete

18.4, 0.

32., 0.0013

*Tension Stiffening

1., 0.

0., 0.0008

*Failure Ratios

1.16, 0.0625, 1.28, 0.3333

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.36

Usage

• Shear retention
– The user can specify data to define how the shear modulus degrades in
the presence of cracking.
– The data required is
• Fraction of shear modulus applicable to a closed crack
• Crack opening strain at which the shear modulus is zero
– If this option is omitted, the default is for full shear retention (i.e. the
shear modulus is unaffected by cracking)

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.37

Usage

• Shear retention

***

** MATERIALS

**

*Material, name=concrete

*Elastic

29000., 0.18

*Concrete

18.4, 0.

32., 0.0013

*Tension Stiffening

1., 0.

0., 0.0008

*Failure Ratios

1.16, 0.0625, 1.28, 0.3333

*Shear Retention

0.9, 0.002

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Calibration

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.39

Calibration

• Minimum of two experiments are required to calibrate the simplest
version of the concrete model (using all possible defaults)
– Uniaxial compression test
– Uniaxial tension test

• Uniaxial compression
– This test gives the compressive stress-strain curve

• Uniaxial tensile test
– This test is difficult to perform, and data is often not available
– Assumption required for tensile failure strength (usually about 7-10% of
compressive strength)
– Calibration of post-failure response depends on nature of reinforcing

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.40

Calibration

• Shear Retention
– Combined tension and shear experiments are required to calibrate the
post-cracking shear behaviour
– Tests are difficult so default (full shear retention) is often used

• Failure Ratios
– Biaxial experiments are required to calibrate the Failure Ratios
– Tests are difficult so default values are generally used

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Modeling Aspects

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.42

Modeling Aspects

• Choice of material properties

– The user’s success in analyzing concrete problems depends significantly
on making sensible choices regarding the concrete material parameters.

– The values chosen for tension stiffening are the most important item when
analyzing problems that involve cracking failure of the concrete. Generally,
the more tension stiffening is included, the easier it is to obtain numerical
solutions.

– The tensile postfailure behavior is not easily specified: the loss of strength
depends on such factors as the density of reinforcement and the quality of
the bond between the rebar and the concrete.

– Some trial and error may be required to calibrate the tension stiffening in
each particular case

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.43

Modeling Aspects

– A reasonable starting point for reinforced concrete is to assume that the
strain softening after failure reduces the stress linearly to zero at a total
strain about 10 times the strain at failure.

σt
σ t0

ε t0 ∼10×ε t0

– The strain at failure is typically 10-4, so a total strain of 10-3 is reasonable

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.44

Modeling Aspects

• Elements

– ABAQUS offers a variety of elements for use with the concrete cracking
model including beam, shell, plane stress, plane strain, axisymmetric, and
three-dimensional continuum elements.

– For general shell analysis more than the default number of 5 integration
points through the thickness of the shell should be used; 9 thickness
integration points are commonly used to model progressive failure of the
concrete through the thickness with acceptable accuracy.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.45

Modeling Aspects

• Output

– In addition to the standard output identifiers available in ABAQUS, the
following variables relate specifically to material points in the smeared
crack concrete model:

CRACK Unit normal to cracks in concrete
CONF
Number of cracks at a concrete
material point

– These variables are only available in the printed results file (*.dat)
– Not currently supported through ABAQUS/CAE

• Must be manually requested

*El Print, Elset=concrete_elems
CONF, CRACK

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.46

Modeling Aspects

• Other considerations

– Considerable nonlinearity is expected in the response of concrete
structures, including the possibility of unstable regimes as the concrete
cracks. The following is recommended to alleviate possible convergence
difficulties:

• Use automatic stabilization in static steps, ∗STATIC, STABILIZE. In
problems with global instabilities, use the modified Riks method,
∗RIKS.

• Since the overall convergence of the solution is expected to be non-
monotonic, use ∗CONTROLS, ANALYSIS=DISCONTINUOUS to
prevent premature termination of the equilibrium iteration process
because the solution may appear to be diverging.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Reinforcement Modeling

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.48

Reinforcement Modeling

• Reinforcement in ABAQUS
– In ABAQUS, concrete reinforcement is modeled using REBAR LAYERS
– Shell, membrane, and surface elements are reinforced by directly
specifying a rebar layer in the element.
• Surface elements do not have any element properties other than the
rebar layer and are used primarily as place-holders for rebar layers.
– Solid elements are reinforced using the embedded element constraint.
• In this technique, either surface or membrane elements reinforced
with rebar layers are embedded in the solid host elements.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.49

Reinforcement Modeling

Reinforcement

Solid elements Structural elements

Embedded Rebar layers in Rebar layers
element membranes in shells
constraint

Rebar layers in Rebar layers in
membranes surface elements

Rebar layers in various element types in ABAQUS

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.50

Reinforcement Modeling

– Rebars layers are used for modeling uniaxial reinforcement in shell,
membrane and surface elements.

– Rebars layers have the following properties:

• Their material properties are independent of those of the underlying
elements.

• As many different combinations and orientations of rebar layers as are
needed can be defined within a single element.

• The rebar layer volume is not subtracted from the volume of the
element to which the rebar layer is added.

– Thus, rebar layers should be used only when the volume fraction
of reinforcement is small (such as with reinforced concrete where
the volume fraction of the rebar is between 1% and 4%).

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.51

Reinforcement Modeling

• Specification of rebar layers
– The ∗REBAR LAYER option is used in conjunction with the

∗SHELL SECTION,
∗MEBRANE SECTION, or
∗SURFACE SECTION

options to specify reinforcement layers in shell, membranes, and surface
elements, respectively.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.52

Reinforcement Modeling

– Sample usage:

*SHELL SECTION, ELSET=...
*REBAR LAYER, ORIENTATION=ORI1

name, a, s, f, mat, alpha, 1

name mat a s alpha f

*SHELL SECTION, ELSET=...
*REBAR LAYER, ORIENTATION=ORI1

name, a, s, f, mat, alpha, 1

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.53

Reinforcement Modeling

– For each rebar layer, specify
• rebar layer name (used to identify the layer in the list of section points
when postprocessing with ABAQUS/Viewer);
• the rebar material name;
• cross-sectional area a of each rebar;
• the rebar spacing s in the plane of the membrane, shell, or surface
element;
• the angular orientation alpha, in degrees, measured relative to the
local 1-direction, positive in the direction of the element normal; and
• the position of the rebars in the thickness direction f (for shell
elements only), measured from the midsurface of the shell (positive in
the direction of the positive normal to the shell).

– Repeat the data to define each rebar layer
– Similar method is used to define rebar in membrane and surface element

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.54

Reinforcement Modeling

• Prestresses in rebar layers

– Prestress can be defined in the rebars using the *INITIAL CONDITIONS,
TYPE=STRESS, REBAR option, with or without using the *PRESTRESS
HOLD option.

• With the *PRESTRESS HOLD option the initial stress defined in the
rebar is held constant.

– While equilibrium iterations are performed to obtain the
corresponding (self-equilibrating) stresses in the matrix material,
the rebar layer will strain, but this strain is not allowed to cause
changes in the stress in the rebar layer.

• Without the *PRESTRESS HOLD option, the initial stresses are
allowed to change during an equilibrating static analysis step as both
the matrix and the rebar stresses adjust to the equilibrium
configuration.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.55

Reinforcement Modeling

• For example, in reinforced concrete:

– The rebar are initially stretched to a desired tension before being
covered by concrete.

– After the concrete cures and bonds to the rebar, release of the
initial rebar tension transfers load to the concrete, introducing
compressive stresses in the concrete.

– The resulting deformation in the concrete reduces the stress in
the rebar.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.56

Reinforcement Modeling

• Output
– ABAQUS/CAE supports visualization of rebar layer orientations and results
in rebar layers.
– Output of variables such as stresses and strains at the rebar integration
points is available
• Results can be viewed on a layer-by-layer basis.
• To display results for a given rebar layer, select the named rebar layer
from the list of available section points.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.57
L4.58
Reinforcement Modeling

– The force in the rebar is available at
the layer integration points as
RBFOR, which is the rebar stress
times the current cross-sectional area
(see the figure on the following page).

– RBANG and RBROT identify the
current orientation of rebar within the
element and the relative rotation of
the rebar layer as a result of finite
deformation.

– Sample output request:

*Element output, rebar
S, E, RBANG, RBROT, RBFOR

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Reinforcement Modeling

• Rebar force output

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.59

Reinforcement Modeling

• Embedding Rebar Layers
– Membrane and surface elements reinforced with rebar layers can be
embedded in continuum (solid) elements in an arbitrary manner such that
the two meshes need not match.
• This is accomplished using an EMBEDDED REGION constraint.

Copyright 2005 ABAQUS, Inc. L4.60

ABAQUS: Selected Topics

Reinforcement Modeling

• Usage:

*EMBEDDED ELEMENT, HOST ELSET=tread,
ROUNDOFF TOLERANCE=1.e-6
belt1, belt2

– The ROUNDOFF TOLERANCE
parameter is used to adjust the
position of embedded nodes such that
they lie exactly on a host element face
or edge.

– This reduces the number of constraint
equations required, allowing for a
more economical solution.

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.61

Reinforcement Modeling rebar orientation

embedded membrane element

host solid element

Reinforced solid element using the embedded element technique

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Workshop 4: Concrete Slab Analysis

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.63

Workshop 4: Collapse of a Concrete Slab

– This workshop illustrates reinforced concrete modeling of typical slab-type
structures.

– The square slab is supported at its four corners and loaded by a point load
at its center.

– The slab is reinforced in two directions at 75% of its depth.
– Noteworthy features:

• Reinforced concrete shell modeling using rebar layer
• Tension stiffening is modeled assuming a linear loss of strength

beyond the cracking failure of concrete
• Use of the Riks solution algorithm for globally unstable response

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.64

Workshop 4: Collapse of a Concrete Slab

Geometry of the square slab and reinforcement

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics L4.65

Workshop 4: Collapse of a Concrete Slab

• Load-deflection response:

ABAQUS/Standard

Load-deflection response for three different values of tension stiffening

Copyright 2005 ABAQUS, Inc.

ABAQUS: Selected Topics

Lecture 5

Eigenvalue Buckling Analysis

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.2

Overview

• Introduction
• Eigenvalue Problem Formulation
• ABAQUS Usage
• Closely Spaced Eigenvalues
• Concluding Remarks
• Workshop 5a: Cargo Crane – Critical Load Estimation
• Workshop 5b: Eigenvalue Buckling of a Square Tube

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Introduction

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.4

Introduction

– The stability of structures is a problem that analysts face frequently.

• These problems predominantly occur in beam and shell structures.

– Such stability studies usually require two types of analyses:

• Eigenvalue buckling analysis

• Postbuckling or collapse analysis

– We focus on eigenvalue buckling analysis, which very often is a required
step for the more general collapse or load-displacement response
analysis.

– Eigenvalue buckling analysis is used to obtain estimates of the critical load
at which the response of a structure will bifurcate, assuming that the
response prior to bifurcation is essentially linear.

• The simplest example is the Euler column, which responds very stiffly
to a compressive axial load until a critical load is reached, at which
point it bends suddenly and exhibits much lower stiffness.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.5

Introduction

– Load-displacement response of an Euler column

Copyright 2004 ABAQUS, Inc. L5.6

ABAQUS: Selected Topics

Introduction

– Deformed configurations of an Euler column

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.7

Introduction

– The purpose of eigenvalue buckling analysis is to investigate singularities
in a linear perturbation of the structure’s stiffness matrix.

• The resulting estimates will be of value in design only if the linear
perturbation is a realistic reflection of the structure’s response before it
buckles.

• Therefore, eigenvalue buckling is useful for “stiff” structures
(structures that exhibit only small, elastic deformations prior to
buckling).

– In most cases of stiff structures, even when inelastic response may occur
before collapse, eigenvalue buckling analysis provides a useful estimate of
the collapse mode shape.

– Only in quite restricted cases (linear elastic, stiff response; no imperfection
sensitivity) is it the only analysis needed to understand the structure’s
collapse limit.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.8

Introduction

– In many cases the post-buckled response is unstable; the collapse load
will then depend strongly on imperfections in the original geometry.

• This is known as “imperfection sensitivity.”

• In this case the actual collapse load may be significantly lower than
the bifurcation load predicted by eigenvalue buckling analysis.

– Thus, eigenvalue buckling analysis provides a nonconservative
estimate of the structure’s load carrying capacity.

– Even if the pre-buckling response is stiff and linear elastic, nonlinear load-
displacement response analysis (of the imperfect structure) is generally
recommended to augment the eigenvalue buckling analysis.

• This is essential if the structure is imperfection sensitive.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics

Eigenvalue Problem Formulation

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.10

Eigenvalue Problem Formulation

– The objective of an eigenvalue buckling analysis is to
• find the load level at which the equilibrium becomes unstable

or
• estimate the maximum load level which the structure can sustain.

– The critical load level depends on the structure’s stiffness
– The stiffness is dependent on the internal stress and, if the load follows the

structure, on the applied load.
• It will be assumed that the loading is conservative, so the stiffness
matrix is symmetric.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.11

Eigenvalue Problem Formulation

– First apply a “dead” load, P0.

• This defines the stiffness of the base state K0 which includes preload

effects (even if NLGEOM is not used).

– Now add a “live” load, λ∆P, where λ is the magnitude of the live load being
added and ∆P is the pattern of the live load.

– As noted earlier, the method works best if the response is linear prior to

bifurcation. Thus, as long as the response is stiff and linear elastic, the

stress and, hence, the structural stiffness will change proportionally with λ,

as K0 + λ∆K, Stiffness change is proportional to λ.

and

∆K = K∆σ + K∆P. Due to incremental loading pattern; made up
of two parts: the internal stress and the
applied load.

Copyright 2004 ABAQUS, Inc.

ABAQUS: Selected Topics L5.12

Eigenvalue Problem Formulation

– We need to find values of λ, which provide singularities in this tangent

stiffness; this poses the eigenproblem.
• In other words, a loss of stability occurs when the total stiffness matrix
is singular:

( K0 + λ∆K )V = 0.

Copyright 2004 ABAQUS, Inc.