The capability described in this section can be used to model a bonded
interface, with or without the possibility of damage and failure of the bond,
and to model regular contact behavior where the interface is not bonded. This
capability has similarities to other features that could be considered for a
bonded interface, including cohesive elements (see
About Cohesive Elements).
Cohesive contact behavior is typically easier to define than modeling the
interface using cohesive elements and allows simulation of a wider range of
cohesive interactions, such as two sticky surfaces coming into
contact during an analysis.
Contact cohesive behavior is primarily intended for situations in which
the interface thickness is negligibly small. If the interface adhesive layer
has a finite thickness and macroscopic properties (such as stiffness and
strength) of the adhesive material are available, it may be more appropriate to
model the response using conventional cohesive elements (see
Defining the Constitutive Response of Cohesive Elements Using a Continuum Approach).
In
Abaqus/Explicit
the surface-based cohesive behavior framework can also be used to model crack
propagation in initially partially bonded surfaces via linear elastic fracture
mechanics principles (LEFM) as implemented
using the Virtual Crack Closure Technique
(VCCT).
Contact cohesive behavior:
is defined as a surface interaction property;
can be used to model the delamination at interfaces directly in terms
of traction versus separation;
can be used to model “sticky” contact (i.e., surfaces or parts of
surfaces that are not initially in contact may bond on coming into contact;
subsequently the bond may damage and fail);
can be restricted to surface regions that are initially in contact;
allows specification of cohesive data such as the fracture energy as a
function of the ratio of normal to shear displacements (mode mix) at the
interface;
assumes a linear elastic traction-separation law prior to damage;
assumes that failure of the cohesive bond is characterized by
progressive degradation of the cohesive stiffness, which is driven by a damage
process (in
Abaqus/Explicit
brittle fracture can also be modeled using a
VCCT fracture crierion);
allows specification of postfailure cohesive behavior if failed nodes
re-enter contact;
is implemented within the general contact algorithmic framework in
Abaqus/Standard
and
Abaqus/Explicit
and within the contact pair framework in
Abaqus/Standard;
is enforced with the surface-to-surface, edge-to-surface,
edge-to-edge, and vertex-to-surface contact formulations for general contact in
Abaqus/Standard;
is enforced only for node-to-face contact interactions in
Abaqus/Explicit
and is not available for edge-to-edge and node-to-analytical rigid surface
contact interactions;
is enforced for the node-to-surface contact formulation for contact pairs in Abaqus/Standard and is not available for the finite-sliding, surface-to-surface contact formulation for
contact pairs in Abaqus/Standard;
can be used as an alternative to rough friction surface
interactions, the no separation contact relationship, or a
combined no separation and rough friction behavior within the
general contact framework;
is an alternative way to tie surfaces; and
cannot be used in a coupled Eulerian-Lagrangian analysis in
Abaqus/Explicit.
Cohesive contact can be used in a variety of workflows. Cohesive contact
behavior often is one of many possible approaches to modeling interface
behavior. Common usages of cohesive contact include:
Modeling a permanently bonded
interface.
Modeling a bonded interface in
which the bond may damage and fail.
Approximating interface behavior
in a simplified form while a model is being built (and other aspects of the
model are being refined).
These usages are discuss in more detail below.
Modeling a Permanently Bonded Interface
In it simplest form, cohesive contact can be used as an alternative to
surface-based tie constraints (which are discussed in
Mesh Tie Constraints) or
other modeling methods. There is no need to specify stiffness or damage
properties of the contact cohesive behavior in this case; you can allow
Abaqus
to assign default interfacial stiffness components. Bonded regions remain
bonded throughout a simulation if cohesive damage characteristics are not
specified. Unlike surface-based tie constraints, cohesive contact will not
constrain rotational degrees of freedom.
Modeling a permanently bonded interface as a type of contact behavior rather
than as a surface-based tie constraint has the following advantages:
Enables contact output variables
to be used to evaluate interface stresses and other quantities.
Enables numerical softening to
be introduced in the constraint enforcement, which avoids the potential for
numerical issues associated with overconstraints where different types of
strictly enforced "hard" constraints overlap.
Optionally, allows a specific
interface stiffness representative of physical behavior to be specified.
Permanent cohesive bonds with default cohesive stiffness or user-specified
cohesive stiffness at least as stiff as the default cohesive stiffness have the
following characteristics for general contact in
Abaqus/Standard:
No regular contact constraints
act in parallel to cohesive contact constraints: Conditions for regular contact
constraints acting in parallel to cohesive contact constraints are discussed in
Interaction between Cohesive Properties and Regular Contact Properties.
However, those conditions are not relevant to stiff, permanent cohesive
constraints, and regular contact constraints are avoided in these cases to
improve convergence behavior and performance.
Details of the cohesive contact
formulation are enhanced for stiff, permanent cohesive bonds. Results for stiff
cohesive bonds may differ, even prior to cohesive damage, depending on whether
or not a cohesive damage evolution model is specified.
Modeling a Bonded Interface That May Fail
Specifying a damage model for the contact cohesive behavior allows for
modeling of a bonded interface that may fail as a result of the loading. This
modeling approach is an alternative to using cohesive elements or other element
types that directly discretize the cohesive material for the simulation.
Comparisons of cohesive-contact versus cohesive-element approaches are
discussed below in
High-Level Comparison of Cohesive-Element and Cohesive-Contact Approaches.
Approximating and Modifying Interface Behavior While a Finite Element Model Is Built
Using different interface modeling strategies across different stages of
building and refining a finite element model is sometimes a good strategy for
improving your efficiency. For example, during an initial stage of a model
build, you may choose to model interfaces as permanently bonded to enable more
focus on noninterface modeling details. You can switch to more physically
representative interface behavior (such as regular contact or bonded contact
with the possibility of damage and failure) in later stages of the model build.
The later stages often require more care to avoid unconstrained rigid body
modes and other types of static instabilities.
Analysts sometimes use surface-based tie constraints (Mesh Tie Constraints) in
early stages of building a model and then switch to contact specifications as
the model becomes more mature. An alternative is to specify cohesive contact
behavior with a permanently bonded interface and default stiffness in the early
stages, and then reassign a more realistic contact behavior as the model
becomes more mature. This alternative of reassigning the contact behavior as
the model matures, rather than switching from a constraint option to a contact
option during the model evolution, may result in greater consistency across
different stages of the model build.
High-Level Comparison of Cohesive-Element and Cohesive-Contact Approaches
Figure 1
provides a high-level comparison of the cohesive-element and cohesive-contact
modeling approaches. Both of these approaches are viable for many modeling
situations.
The formulae and laws that govern cohesive constitutive behavior are very
similar for cohesive contact and cohesive elements. The similarities extend to
the linear elastic traction-separation model, damage initiation criteria, and
damage evolution laws. Constitutive behavior details for contact cohesive
behavior are discussed later in this section, starting with
Linear Elastic Traction-Separation Behavior.
Constitutive behavior details for cohesive element are discussed in
Defining the Constitutive Response of Cohesive Elements Using a Traction-Separation Description.
It is important to recognize differences between the cohesive-contact and
cohesive-element approaches, including the aspects discussed below.
No Cohesive Contact Thickness
Cohesive material thickness cannot be introduced as a characteristic for
cohesive contact but can be for cohesive elements. Surface thickness can be
modified (Assigning Surface Properties)
to account for cohesive material thickness. Since thickness effects are not
considered for a cohesive property, material definitions used to describe
traction-separation response for cohesive elements with thickness effects may
not be directly reusable for cohesive contact.
Tangential Refinement of the Interface
Constitutive calculations are evaluated for cohesive contact and cohesive
elements at the following locations:
For cohesive elements,
constitutive calculations are calculated at the material points of the
elements.
For cohesive contact, constitutive calculations are
calculated for individual contact constraints. The number of potential contact
constraints is approximately equal to the number of nodes acting as secondary nodes.
Modeling with cohesive elements allows the possibility of different
tangential mesh refinement for cohesive elements as compared to the mesh
refinement of the adjacent bodies. Use of a more refined mesh for the cohesive
elements may improve the resolution of spatial variations in the cohesive
response, independent, to a degree, of the mesh refinement of the adjacent
bodies. The cohesive element example in
Figure 1
shows a slightly more refined mesh for the cohesive elements than the adjacent
bodies.
For the cohesive contact modeling approach, cohesive calculations are computed at contact
constraint locations, which are primarily associated with secondary nodes. The more
refined surface of an interaction typically acts as the secondary surface. Therefore, the
resolution of spatial variations in the cohesive response is usually primarily associated
with whichever adjacent body has the more refined surface.
Interaction between Cohesive Properties and Regular Contact Properties
"Regular" contact behavior is automatically in effect if the cohesive
contact bond becomes fully damaged. Cohesive elements do not have an analogous
behavior in this regard unless contact is defined between surfaces of the
adhered parts in addition to having cohesive elements defined between the
adhered parts. A surface interaction property definition containing cohesive
specifications will also include noncohesive, mechanical contact
specifications, such as discussed in
Contact Pressure-Overclosure Relationships
and
Frictional Behavior.
"Regular" contact-behavior aspects are sometimes partially in effect even
before the cohesive has failed, as described below:
Normal-direction behavior: The
noncohesive contact pressure-overclosure relationship (see
Contact Pressure-Overclosure Relationships)
is in effect while the contact pressure is positive, regardless of whether
cohesive behavior is specified and the amount of cohesive damage accumulated
except for stiff, permanent cohesive cohesive behavior. No regular contact
constraints act in parallel to cohesive contact constraints for stiff,
permanent cohesive behavior.
Tangential behavior: If cohesive
bonding at a particular interface location is active and undamaged, the
resistance to tangential motion is governed by the cohesive behavior only. Once
cohesive damage starts to accumulate at a particular location of the interface,
the interface shear stress has contributions from the cohesive model and the
friction model. The contribution from the friction model is weighted by the
scalar damage variable of the cohesive behavior (see
Damage Evolution). When
the cohesive bond is fully damaged (failed), the only contribution to the
interface shear stress is from the friction model.
Nonmechanical interactions are ignored when surface-based cohesive behavior
is defined.
Interface Versus Element Quantities
The table below compares how various simulation operations associated with
cohesive modeling can be performed with the cohesive contact and cohesive
element modeling approaches.
Simulation operation
Cohesive contact
Cohesive elements
Defining where a cohesive region is located
Interaction property assignment (based on surface
pairings)
Including cohesive elements (and nodes) in the
model
Defining cohesive damage model and other aspects
of cohesive constitutive behavior
Interaction property specification
Material property specification
Studying results for stretching and shearing of a
cohesive material
Contact opening and sliding distance output
Element strain output
Studying results for stresses within a cohesive
material
Contact stresses output for normal and tangent
directions
Element stress output
Specifying Cohesive Interface "Material" Behavior within a Surface Interaction Property Definition
Cohesive interface "material" behavior is defined as part of a surface
interaction property. Surface interaction properties are assigned to contact
interactions as discussed in
Defining the Contact Property Model.
Cohesive interface behavior includes stiffness characteristics associated with
the bonded interface and characteristics governing any cohesive damage.
Bonded-interface stiffness characteristics are assigned by default if these
stiffness characteristics are not specified explicitly. The magnitudes of these
default stiffness characteristics are similar to the magnitude of the default
contact penalty stiffness. A damage model is not included in the cohesive
material behavior unless damage characteristics are specified explicitly as
part of the damage behavior definition.
Initial Cohesive Contact State
The initial contact status as a function of position along a cohesive
contact interface can fundamentally affect simulation results. Consider the
example shown in
Figure 2.
The intent for this example is that the block is initially touching the wall
with the cohesive status initialized to bonded. However, a small, unintended
initial gap exists between the block and the wall in the initial configuration,
so the contact status is initialized to "opened" or "inactive," and the
cohesive status is initialized to unbonded by default. If there is no initial
cohesive bonding in this example, the applied force will push the block away
from the wall or perhaps, in a static analysis, a numerical issue will be
reported by
Abaqus/Standard
due to unconstrained rigid-body motion of the block. User controls associated
with the initial contact status (see
Contact Initialization for General Contact in Abaqus/Standard,
Contact Initialization for Contact Pairs in Abaqus/Standard,
and
Contact Initialization for General Contact in Abaqus/Explicit)
can be used to ensure that the contact status will be properly initialized over
various regions of an interface, such that interface stresses associated with
cohesive contact will counter the applied force. Most user controls associated
with the initial contact status are not specific to cohesive contact behavior.
Consider the example shown in
Figure 3,
in which the cohesive status is intended to be initialized to bonded over much
of the interface but should be initialized to unbonded over a specific portion
of the interface. The desired initialization can be achieved by assigning zero
initial clearance to the portion of the interface that should be initially
bonded and very small positive initial clearance to the portion of the
interface that should not be initially bonded, such as shown in the
Abaqus/Standard
input file example below.
Limiting Cohesive Bonding to Original Contact Constraints
The most common usage of cohesive contact is for situations in which
cohesive bonds exist at the beginning of a simulation. By default,
Abaqus
limits cohesive bonds to those that exist at the beginning of a simulation.
Limiting Cohesive Bonding to Subset of Original Contact Constraints
For contact pairs in Abaqus/Standard you can specify as part of the cohesive behavior definition that only a subset of
initially active contact constraints should have cohesive bonds. Initial strain-free
adjustments to positions of secondary nodes will be made, if necessary, to ensure they are
initially in contact with the main surface. Similar behavior can be achieved with general
contact by selectively assigning initialization controls to control which regions of the
interface are initially in contact and limiting cohesive behavior to initially active
contact constraints (see Initial Cohesive Contact State).
Cohesive Rebonding upon Repeated Contact
In some situations it is desirable to allow cohesive rebonding each time contact is established,
even for secondary nodes previously involved in cohesive contact that have fully damaged and
debonded. For such situations, you can indicate that cohesive rebonding can repeatedly occur
at the same interface location.
Cohesive Rebonding upon Repeated Contact Limited to Locations of Initial Cohesive Bonds
General contact in Abaqus/Explicit and contact pairs in Abaqus/Standard allow cohesive bonding to be limited to originally active contact constraints with only
these secondary nodes to be eligible to rebond upon subsequent contact, and contact pairs
in Abaqus/Standard allow this behavior for a subset of initially active contact constraints.
Limiting Cohesive Bonding to First Contact Constraints
It is sometimes desirable to establish cohesive bonds for initial contact constraints plus the
first time an initially not-in-contact region comes into contact during a simulation.
General contact in Abaqus/Explicit and contact pairs in Abaqus/Standard optionally support each secondary node associated with interactions that are assigned a
cohesive property to become bonded once (either initially or during a simulation).
Simulation results with this option can be highly sensitive to the assignment of secondary
and main roles since the check for prior cohesive bonds at a location is done only for nodes
acting as secondary nodes. General contact in Abaqus/Standard allows cohesive behavior to be limited to initial contact constraints (see Limiting Cohesive Bonding to Original Contact Constraints) and allows cohesive behavior for all new contact
constraints (see Cohesive Rebonding upon Repeated Contact) but does not support limiting cohesive behavior to first contact
constraints.
When cohesive contact behavior applies to contact that develops after the
start of the simulation, cohesive effects are activated one increment after the
contact constraint becomes active.
Main and Secondary Roles and Contact Formulations Associated with Cohesive Interactions
Interactions assigned a cohesive surface interaction property are modeled with pure
main-secondary roles in the contact formulation. The main and secondary roles are
established as follows:
General contact in Abaqus/Standard: main and secondary roles for interactions associated with cohesive behavior are the
same as for other types of contact behavior (see Main and Secondary Surface Roles of a Contact Formulation).
General contact in Abaqus/Explicit: main and secondary roles for interactions associated with cohesive behavior follow
the convention that the first surface specified in a contact property assignment
involving cohesive behavior is treated as a secondary surface and the second surface is
treated as its corresponding main surface.
Contact pairs in Abaqus/Standard: main and secondary roles are defined by the usual conventions associated with
defining a contact pair.
Linear Elastic Traction-Separation Behavior
The available traction-separation model in
Abaqus
assumes initially linear elastic behavior (see
Defining Elasticity in Terms of Tractions and Separations for Cohesive Elements)
followed by the initiation and evolution of damage. The elastic behavior is
written in terms of an elastic constitutive matrix that relates the normal and
shear stresses to the normal and shear separations across the interface.
The nominal traction stress vector, , consists of three
components (two components in two-dimensional problems):
,
,
and (in three-dimensional problems) ,
which represent the normal (along the local 3-direction in three dimensions and
along the local 2-direction in two dimensions) and the two shear tractions
(along the local 1- and 2-directions in three dimensions and along the local
1-direction in two dimensions), respectively. The corresponding separations are
denoted by ,
,
and .
The elastic behavior can then be written as
Uncoupled Traction-Separation Behavior
The simplest specification of cohesive behavior generates contact penalties
that enforce the cohesive constraint in both normal and tangential directions.
By default, the normal and tangential stiffness components will not be coupled:
pure normal separation by itself does not give rise to cohesive forces in the
shear directions, and pure shear slip with zero normal separation does not give
rise to any cohesive forces in the normal direction.
For uncoupled traction-separation behavior, the terms
,
,
and
must be defined, as well as any dependencies on temperature or field variables.
If these terms are not defined,
Abaqus
uses default contact penalties to model the traction-separation behavior.
Coupled Traction-Separation Behavior
In its full generality, the elasticity matrix provides fully coupled
behavior between all components of the traction vector and separation vector
and can depend on temperature and/or field variables. All terms in the matrix
must be defined for coupled traction-separation behavior.
Cohesive Behavior in the Normal or Shear Direction Only
To restrict the cohesive constraint to act along the contact normal
direction only, define uncoupled cohesive behavior and specify zero values for
the shear stiffness components,
and .
Alternatively, if only tangential cohesive constraints are to be enforced, the
normal stiffness term, ,
can be set to zero, in which case the normal “separations” will not be
constrained. Normal compressive forces are resisted as per the usual contact
behavior.
Damage Modeling
Damage modeling allows you to simulate the degradation and eventual failure
of the bond between two cohesive surfaces. The failure mechanism consists of
two ingredients: a damage initiation criterion and a damage evolution law. The
initial response is assumed to be linear as discussed above. However, once a
damage initiation criterion is met, damage can occur according to a
user-defined damage evolution law.
Figure 4
shows a typical traction-separation response with a failure mechanism. If the
damage initiation criterion is specified without a corresponding damage
evolution model,
Abaqus
evaluates the damage initiation criterion for output purposes only; there is no
effect on the response of the cohesive surfaces (i.e., no damage will occur).
Cohesive surfaces do not undergo damage under pure compression.
Damage of the traction-separation response for cohesive surfaces is defined
within the same general framework used for conventional materials (see
About Progressive Damage and Failure),
except the damage behavior is specified as part of the interaction properties
for the surfaces. Multiple damage response mechanisms are not available for
cohesive surfaces: cohesive surfaces can have only one damage initiation
criterion and only one damage evolution law.
Damage Initiation
Damage initiation refers to the beginning of degradation of the cohesive
response at a contact point. The process of degradation begins when the contact
stresses and/or contact separations satisfy certain damage initiation criteria
that you specify. Several damage initiation criteria are available and are
discussed below.
Each damage initiation criterion also has an output variable associated with
it to indicate whether the criterion is met. A value of 1 or higher indicates
that the initiation criterion has been met. Damage initiation criteria that do
not have an associated evolution law affect only output. Thus, you can use
these criteria to evaluate the propensity of the material to undergo damage
without actually modeling the damage process (i.e., without actually specifying
damage evolution).
In the discussion below, ,
,
and
represent the peak values of the contact stress when the separation is either
purely normal to the interface or purely in the first or the second shear
direction, respectively. Likewise, ,
,
and
represent the peak values of the contact separation, when the separation is
either purely along the contact normal or purely in the first or the second
shear direction, respectively. The symbol
used in the discussion below represents the Macaulay bracket with the usual
interpretation. The Macaulay brackets are used to signify that a purely
compressive displacement (i.e., a contact penetration) or a purely compressive
stress state does not initiate damage.
Maximum Stress Criterion
Damage is assumed to initiate when the maximum contact stress ratio (as
defined in the expression below) reaches a value of one. This criterion can be
represented as
Maximum Separation Criterion
Damage is assumed to initiate when the maximum separation ratio (as defined
in the expression below) reaches a value of one. This criterion can be
represented as
Quadratic Stress Criterion
Damage is assumed to initiate when a quadratic interaction function
involving the contact stress ratios (as defined in the expression below)
reaches a value of one. This criterion can be represented as
Quadratic Separation Criterion
Damage is assumed to initiate when a quadratic interaction function
involving the separation ratios (as defined in the expression below) reaches a
value of one. This criterion can be represented as
Rate Dependency
The damage initiation criterion can be defined as a tabular function of the
effective rate of separation.
Damage Evolution
The damage evolution law describes the rate at which the cohesive stiffness
is degraded once the corresponding initiation criterion is reached. The general
framework for describing the evolution of damage in bulk materials (as opposed
to interfaces modeled using cohesive surfaces) is described in
Damage Evolution and Element Removal for Ductile Metals.
Conceptually, similar ideas apply for describing damage evolution in cohesive
surfaces.
A scalar damage variable, D, represents the overall
damage at the contact point. It initially has a value of 0. If damage evolution
is modeled, D monotonically evolves from 0 to 1 upon
further loading after the initiation of damage. The contact stress components
are affected by the damage according to
where ,
,
and
are the contact stress components predicted by the elastic traction-separation
behavior for the current separations without damage.
To describe the evolution of damage under a combination of normal and shear
separations across the interface, it is useful to introduce an effective
separation (Camanho and Davila, 2002) defined as
The relative proportions of normal and shear separations at a contact point
define the mode mix at the point.
Abaqus
uses three measures of mode mix, two that are based on energies and one that is
based on tractions. You can choose one of these measures when you specify the
mode dependence of the damage evolution process. Denoting by
,
,
and
the work done by the tractions and their conjugate separations in the normal,
first, and second shear directions, respectively, and defining
,
the mode-mix definitions based on energies are as follows:
Clearly, only two of the three quantities defined above are independent. It
is also useful to define the quantity
to denote the portion of the total work done by the shear traction and the
corresponding separation components. As discussed later,
Abaqus
requires that you specify material properties related to damage evolution as
functions of
(or, equivalently, )
and .
Abaqus
computes the energy quantities described above either based on the current
state of deformation (nonaccumulative measure of energy) or based on the
deformation history (accumulative measure of energy) at an integration point.
The former approach, available only in
Abaqus/Standard,
is useful in mixed-mode simulations where the primary energy dissipation
mechanism is associated with the creation of new surfaces due to failure in the
cohesive zone. Such problems are typically adequately described utilizing the
methods of linear elastic fracture mechanics. The latter approach provides an
alternate way of defining the mode-mix and may be useful in situations where
other significant dissipation mechanisms also govern the overall structural
response.
The corresponding definitions of the mode mix based on traction components
are given by
where
is a measure of the effective shear traction. The angular measures used in the
above definition (before they are normalized by the factor
)
are illustrated in
Figure 5.
Comparison of Mixed-Mode Definitions
The mode-mix ratios defined in terms of energies and tractions can be
quite different in general. The following example illustrates this point. In
terms of energies a separation in the purely normal direction is one for which
and ,
irrespective of the values of the normal and the shear tractions. In
particular, for coupled traction-separation behavior both the normal and shear
tractions may be nonzero for a purely normal separation. For this case the
definition of mode mix based on energies would indicate a purely normal
separation, while the definition based on tractions would suggest a mix of both
normal and shear separation.
When the mode mix is defined based on accumulated energies, an artificial
path-dependence may be introduced in the mixed-mode behavior that may not be
consistent, for example, with predictions that are based on linear elastic
fracture mechanics. Therefore, if an interface is first loaded purely in the
normal deformation mode, unloaded, and subsequently loaded in a purely shear
deformation mode, the mode-mix ratios based on accumulated energies at the end
of the above deformation path evaluate to (assuming the shear deformation to be
in the local-1 direction only)
and .
On the other hand, the mode-mix ratios based on nonaccumulated energies
evaluate to
and
at the end of the above deformation path.
Damage Evolution Definition
There are two components to the definition of damage evolution. The first
component involves specifying either the effective separation at complete
failure, ,
relative to the effective separation at the initiation of damage,
;
or the energy dissipated due to failure,
(see
Figure 6).
The second component to the definition of damage evolution is the specification
of the nature of the evolution of the damage variable, D,
between initiation of damage and final failure. This can be done by either
defining linear or exponential softening laws or specifying
D directly as a tabular function of the effective
separation relative to the effective separation at damage initiation. The data
described above will in general be functions of the mode mix, temperature,
and/or field variables.
Figure 7
is a schematic representation of the dependence of damage initiation and
evolution on the mode mix for a traction-separation response with isotropic
shear behavior. The figure shows the traction on the vertical axis and the
magnitudes of the normal and the shear separations along the two horizontal
axes. The unshaded triangles in the two vertical coordinate planes represent
the response under pure normal and pure shear separation, respectively. All
intermediate vertical planes (that contain the vertical axis) represent the
damage response under mixed-mode conditions with different mode mixes. The
dependence of the damage evolution data on the mode mix can be defined either
in tabular form or, in the case of an energy-based definition, analytically.
The manner in which the damage evolution data are specified as a function of
the mode mix is discussed later in this section.
Unloading subsequent to damage initiation is always assumed to occur
linearly toward the origin of the traction-separation plane, as shown in
Figure 6.
Reloading subsequent to unloading also occurs along the same linear path until
the softening envelope (line AB) is reached.
Once the softening envelope is reached, further reloading follows this envelope
as indicated by the arrow in
Figure 6.
Evolution Based on Effective Separation
You specify the quantity
(i.e., the effective separation at complete failure,
, relative to the effective separation at damage initiation,
,
as shown in
Figure 6)
as a tabular function of the mode mix, temperature, and/or field variables. In
addition, you also choose either a linear or an exponential softening law that
defines the detailed evolution (between initiation and complete failure) of the
damage variable, D, as a function of the effective
separation beyond damage initiation. Alternatively, instead of using linear or
exponential softening, you can specify the damage variable,
D, directly as a tabular function of the effective
separation after the initiation of damage, ;
mode mix; temperature; and/or field variables.
Linear Damage Evolution
For linear softening (see
Figure 6)
Abaqus
uses an evolution of the damage variable, D, that reduces
(in the case of damage evolution under a constant mode mix, temperature, and
field variables) to the following expression:
In the preceding expression and in all later references,
refers to the maximum value of the effective separation attained during the
loading history. The assumption of a constant mode mix at a contact point
between initiation of damage and final failure is customary for problems
involving monotonic damage (or monotonic fracture).
Exponential Damage Evolution
For exponential softening (see
Figure 8)
Abaqus
uses an evolution of the damage variable, D, that reduces
(in the case of damage evolution under a constant mode mix, temperature, and
field variables) to
In the expression above
is a nondimensional parameter that defines the rate of damage evolution and
is the exponential function.
Tabular Damage Evolution
For tabular softening you define the evolution of D
directly in tabular form. D must be specified as a
function of the effective separation relative to the effective separation at
initiation, mode mix, temperature, and/or field variables.
Evolution Based on Energy
Damage evolution can be defined based on the energy that is dissipated as a
result of the damage process, also called the fracture energy. The fracture
energy is equal to the area under the traction-separation curve (see
Figure 6).
You specify the fracture energy as a property of the cohesive interaction and
choose either a linear or an exponential softening behavior.
Abaqus
ensures that the area under the linear or the exponential damaged response is
equal to the fracture energy.
The dependence of the fracture energy on the mode mix can be specified
either directly in tabular form or by using analytical forms as described
below. When the analytical forms are used, the mode-mix ratio is assumed to be
defined in terms of energies.
Tabular Form
The simplest way to define the dependence of the fracture energy is to
specify it directly as a function of the mode mix in tabular form.
Power Law Form
The dependence of the fracture energy on the mode mix can be defined based
on a power law fracture criterion. The power law criterion states that failure
under mixed-mode conditions is governed by a power law interaction of the
energies required to cause failure in the individual (normal and two shear)
modes. It is given by
The mixed-mode fracture energy
when the above condition is satisfied. In other words,
You specify the quantities ,
,
and ,
which refer to the critical fracture energies required to cause failure in the
normal, the first, and the second shear directions, respectively.
Benzeggagh-Kenane (BK) Form
The Benzeggagh-Kenane fracture criterion (Benzeggagh and Kenane, 1996) is
particularly useful when the critical fracture energies during separation
purely along the first and the second shear directions are the same; i.e.,
.
It is given by
where ,
,
and
is a cohesive property parameter. You specify ,
,
and .
Linear Damage Evolution
For linear softening (see
Figure 6)
Abaqus
uses an evolution of the damage variable, D, that reduces
to
where
with
as the effective traction at damage initiation.
refers to the maximum value of the effective separation attained during the
loading history.
Exponential Damage Evolution
For exponential softening
Abaqus
uses an evolution of the damage variable, D, that reduces
to
In the expression above
and
are the effective traction and separation, respectively.
is the elastic energy at damage initiation. In this case the traction might not
drop immediately after damage initiation, which is different from what is seen
in
Figure 8.
Defining Damage Evolution Data as a Tabular Function of Mode Mix
As discussed earlier, the data defining the evolution of damage at the
cohesive interface can be tabular functions of the mode mix. The manner in
which this dependence must be defined in
Abaqus
is outlined below for mode-mix definitions based on energy and traction,
respectively. In the following discussion it is assumed that the evolution is
defined in terms of energy. Similar observations can also be made for evolution
definitions based on effective separation.
Mode Mix Based on Energy
For an energy-based definition of mode mix, in the most general case of a
three-dimensional state of separation with anisotropic shear behavior the
fracture energy, ,
must be defined as a function of
and .
The quantity
is a measure of the fraction of the total separation that is shear, while
is a measure of the fraction of the total shear separation that is in the
second shear direction.
Figure 9
shows a schematic of the fracture energy versus mode-mix behavior.
The limiting cases of pure normal and pure shear separations in the first
and second shear directions are denoted in
Figure 9
by ,
,
and ,
respectively. The lines labeled “Modes n-s,” “Modes n-t,” and “Modes s-t” show
the transition in behavior between the pure normal and the pure shear in the
first direction, pure normal and pure shear in the second direction, and pure
shears in the first and second directions, respectively. In general,
must be specified as a function of
at various fixed values of .
In the discussion that follows we refer to a data set of
versus
corresponding to a fixed
as a “data block.” The following guidelines are useful in defining the fracture
energy as a function of the mode mix:
For a two-dimensional problem
needs to be defined as a function of
(
in this case) only. The data column corresponding to
must be left blank. Hence, essentially only one “data block” is needed.
For a three-dimensional problem with isotropic shear response, the
shear behavior is defined by the sum
and not by the individual values of
and .
Therefore, in this case a single “data block” (the “data block” for
)
also suffices to define the fracture energy as a function of the mode mix.
In the most general case of three-dimensional problems with
anisotropic shear behavior, several “data blocks” would be needed. As discussed
earlier, each “data block” would contain
versus
at a fixed value of .
In each “data block”
can vary between 0 and 1.0. The case
(the first data point in any “data block”), which corresponds to a purely
normal mode, can never be achieved when
(i.e., the only valid point on line OB in
Figure 9
is the point O, which corresponds to a purely
normal separation). However, in the tabular definition of the fracture energy
as a function of mode mix, this point simply serves to set a limit that ensures
a continuous change in fracture energy as a purely normal state is approached
from various combinations of normal and shear separations. Hence, the fracture
energy of the first data point in each “data block” must always be set equal to
the fracture energy in a purely normal separation ().
As an example of the anisotropic shear case, consider that you want to
input three “data blocks” corresponding to fixed values of
0., 0.2, and 1.0, respectively. For each of the three “data blocks,” the first
data point must be
for the reasons discussed above. The rest of the data points in each “data
block” define the variation of the fracture energy with increasing proportions
of shear separation.
Mode Mix Based on Traction
The fracture energy needs to be specified in tabular form of
versus
and .
Thus,
needs to be specified as a function of
at various fixed values of .
A “data block” in this case corresponds to a set of data for
versus ,
at a fixed value of .
In each “data block”
may vary from 0 (purely normal separation) to 1 (purely shear separation). An
important restriction is that each data block must specify the same value of
the fracture energy for .
This restriction ensures that the energy required for fracture as the traction
vector approaches the normal direction does not depend on the orientation of
the projection of the traction vector on the shear plane (see
Figure 5).
Rate Dependency
The damage evolution criterion can be defined as a tabular function of the
effective rate of separation.
Viscous Regularization in Abaqus/Standard
Models exhibiting various forms of softening behavior and stiffness
degradation often lead to severe convergence difficulties in
Abaqus/Standard.
Viscous regularization of the constitutive equations defining surface-based
cohesive behavior can be used to overcome some of these convergence
difficulties. This technique is also applicable to cohesive elements, fastener
damage, and the concrete material model in
Abaqus/Standard.
Viscous regularization damping causes the tangent stiffness matrix that defines
the contact stresses to be positive for sufficiently small time increments.
The approximate amount of energy associated with viscous regularization over
the whole model is included in the output variable ALLCD.
Virtual Crack Closure Technique in Abaqus/Explicit
In
Abaqus/Explicit,
the surface-based cohesive behavior framework can be used to model brittle
crack propagation problems based on linear elastic fracture mechanics
principles. The Virtual Crack Closure Technique
(VCCT) fracture criterion can be used to model
crack propagation in initially partially bonded surfaces. A detailed discussion
of this topic can be found in
Crack Propagation Analysis.
The VCCT fracture criterion cannot be
combined with a damage-based surface behavior of the traction-separation
response. However, you can use a surface-based
VCCT fracture criterion in conjunction with
cohesive elements. VCCT could model brittle
failure/crack propagation while the cohesive elements could model other aspects
of the bonded interface such as stitches.
This variable indicates whether the maximum contact stress damage initiation
criterion has been satisfied at a contact point up to the current increment. It
is evaluated as ,
where
is the current increment number.
CSMAXUCRT
This variable indicates whether the maximum separation damage initiation
criterion has been satisfied at a contact point up to the current increment. It
is evaluated as ,
where
is the current increment number.
CSQUADSCRT
This variable indicates whether the quadratic contact stress damage
initiation criterion has been satisfied at a contact point up to the current
increment. It is evaluated as ,
where
is the current increment number.
CSQUADUCRT
This variable indicates whether the quadratic separation damage initiation
criterion has been satisfied at a contact point up to the current increment. It
is evaluated as ,
where
is the current increment number.
For the variables above that indicate whether a certain damage initiation
criterion has been satisfied or not, a value that is less than 1.0 indicates
that the criterion has not been satisfied, while a value of 1.0 indicates that
the criterion has been satisfied. Each damage initiation output variable
indicates the maximum value of the initiation criteria up to the current
increment. For example, if a loading spike causes a peak value in a damage
initiation criterion between output frames, the value of the corresponding
output variable will reflect the peak value at subsequent output frames. If
damage evolution is specified for this criterion, the maximum value of this
variable does not exceed 1.0.
References
Benzeggagh, M.L., and M. Kenane, “Measurement
of Mixed-Mode Delamination Fracture Toughness of Unidirectional Glass/Epoxy
Composites with Mixed-Mode Bending
Apparatus,” Composites Science and
Technology, vol. 56, pp. 439–449, 1996.
Camanho, P.P., and C. G. Davila, “Mixed-Mode
Decohesion Finite Elements for the Simulation of Delamination in Composite
Materials,” NASA/TM-2002–211737, pp. 1–37, 2002.