The progressive damage and failure models described in
About Damage and Failure for Ductile Metals
are the recommended method for modeling material damage and failure in
Abaqus;
these models are suitable for both quasi-static and dynamic situations.
Abaqus/Explicit
offers two additional element failure models suitable only for high-strain-rate
dynamic problems. The shear failure model is driven by plastic yielding. The
tensile failure model is driven by tensile loading. These failure models can be
used to limit subsequent load-carrying capacity of an element (up to the point
of removing the element) once a stress limit is reached. Both models can be
used for the same material.
The shear failure model:
is designed for high-strain-rate deformation of many materials,
including most metals;
uses the equivalent plastic strain as a failure measure;
offers two choices for what occurs upon failure, including the removal
of elements from the mesh;
can be used in conjunction with either the Mises or the Johnson-Cook
plasticity models; and
can be used in conjunction with the tensile failure model.
The tensile failure model:
is designed for high-strain-rate deformation of many materials,
including most metals;
uses the hydrostatic pressure stress as a failure measure to model
dynamic spall or a pressure cutoff;
offers a number of choices for what occurs upon failure, including the
removal of elements from the mesh;
can be used in conjunction with either the Mises or the Johnson-Cook
plasticity models or the equation of state material model; and
can be used in conjunction with the shear failure model.
The shear failure model can be used in conjunction with the Mises or the
Johnson-Cook plasticity models in
Abaqus/Explicit
to define shear failure of the material.
Shear Failure Criterion
The shear failure model is based on the value of the equivalent plastic
strain at element integration points; failure is assumed to occur when the
damage parameter exceeds 1. The damage parameter, ,
is defined as
where
is any initial value of the equivalent plastic strain,
is an increment of the equivalent plastic strain,
is the strain at failure, and the summation is performed over all increments in
the analysis.
The strain at failure, ,
is assumed to depend on the plastic strain rate, ;
a dimensionless pressure-deviatoric stress ratio,
(where p is the pressure stress and q
is the Mises stress); temperature; and predefined field variables. There are
two ways to define the strain at failure, .
One is to use direct tabular data, where the dependencies are given in a
tabular form. Alternatively, the analytical form proposed by Johnson and Cook
can be invoked (see
Johnson-Cook Plasticity
for more details).
When direct tabular data are used to define the shear failure model, the
strain at failure, ,
must be given as a tabular function of the equivalent plastic strain rate, the
pressure-deviatoric stress ratio, temperature, and predefined field variables.
This method requires the use of the Mises plasticity model.
For the Johnson-Cook shear failure model, you must specify the failure
parameters, –
(see
Johnson-Cook Plasticity
for more details on these parameters). The shear failure data must be
calibrated at or below the transition temperature, ,
defined in
Johnson-Cook Plasticity.
This method requires the use of the Johnson-Cook plasticity model.
Element Removal
When the shear failure criterion is met at an integration point, all the
stress components are set to zero and that material point fails. An element is
deleted (or removed) from a mesh upon material failure. Details for element
deletion driven by material failure are described in
Material Failure and Element Deletion.
The status of a material point and an element can be determined by requesting
output variables STATUSMP and STATUS, respectively. Element deletion is the default failure choice.
An alternative failure choice, where the element is not deleted, is to
specify that when the shear failure criterion is met at a material point, the
deviatoric stress components are set to zero for that point and remain zero for
the rest of the calculation. The pressure stress is then required to remain
compressive; that is, if a negative pressure stress is computed in a failed
material point in an increment, it is reset to zero. This failure choice is not
allowed when using plane stress, shell, membrane, beam, pipe, and truss
elements because the structural constraints may be violated.
Determining When to Use the Shear Failure Model
The shear failure model in
Abaqus/Explicit
is suitable for high-strain-rate dynamic problems where inertia is important.
Improper use of the shear failure model may result in an incorrect simulation.
For quasi-static problems that may require element removal, the progressive damage and failure
models or the Gurson porous metal plasticity model (Porous Metal Plasticity) are recommended.
Tensile Failure Model
The tensile failure model can be used in conjunction with either the Mises
or the Johnson-Cook plasticity models or the equation of state material model
in
Abaqus/Explicit
to define tensile failure of the material.
Tensile Failure Criterion
The
Abaqus/Explicit
tensile failure model uses the hydrostatic pressure stress as a failure measure
to model dynamic spall or a pressure cutoff. The tensile failure criterion
assumes that failure occurs when the pressure stress, p,
becomes more tensile than the user-specified hydrostatic cutoff stress,
.
The hydrostatic cutoff stress may be a function of temperature and predefined
field variables. There is no default value for this stress.
The tensile failure model can be used with either the Mises or the
Johnson-Cook plasticity models or the equation of state material model.
Failure Choices
When the tensile failure criterion is met at an element integration point, the material
point fails. Five failure choices are offered for the failed material points: the default
choice, which includes element removal, and four different spall models. These failure
choices are described below.
Element Removal
When the tensile failure criterion is met at an integration point, all the stress
components are set to zero and that material point fails. By default, an element is
deleted (or removed) from a mesh upon material failure. Details for element deletion
driven by material failure are described in Material Failure and Element Deletion. The status of a material point and an element can be determined by
requesting output variables STATUSMP
and STATUS, respectively.
Spall Models
An alternative failure choice that is based on spall (the crumbling of a material),
rather than element removal, is also available. Four failure combinations are available
in this category. When the tensile failure criterion is met at a material point, the
deviatoric stress components may be unaffected or may be required to be zero, and the
pressure stress may be limited by the hydrostatic cutoff stress or may be required to be
compressive. Therefore, there are four possible failure combinations (see Figure 1, where “O” is the stress that would exist if the tensile failure model were not
used).
These failure combinations are as follows:
Ductile shear and ductile pressure: this choice corresponds to point 1 in Figure 1 and models the case in which the deviatoric stress components are unaffected and
the pressure stress is limited by the hydrostatic cutoff stress; that is, .
Brittle shear and ductile pressure: this choice corresponds to point 2 in Figure 1 and models the case in which the deviatoric stress components are set to zero and
remain zero for the rest of the calculation, and the pressure stress is limited by
the hydrostatic cutoff stress; that is, .
Brittle shear and brittle pressure: this choice corresponds to point 3 in Figure 1 and models the case in which the deviatoric stress components are set to zero and
remain zero for the rest of the calculation, and the pressure stress is required to
be compressive; that is, .
Ductile shear and brittle pressure: this choice corresponds to point 4 in Figure 1 and models the case in which the deviatoric stress components are unaffected and
the pressure stress is required to be compressive; that is, .
There is no default failure combination for the spall models. If you choose not to use
the element deletion model, you must specify the failure combination explicitly. If the
material's deviatoric behavior is not defined (for example, the equation of state model
without deviatoric behavior is used), the deviatoric part of the combination is
meaningless and will be ignored. The spall models are not allowed when using plane
stress, shell, membrane, beam, pipe, and truss elements.
Determining When to Use the Tensile Failure Model
The tensile failure model in
Abaqus/Explicit
is suitable for high-strain-rate dynamic problems in which inertia effects are
important. Improper use of the tensile failure model may result in an incorrect
simulation.
Using the Failure Models with Rebar
It is possible to use the shear failure and/or the tensile failure models in
elements for which rebars are also defined. When such elements fail according
to the failure criterion, the base material contribution to the element
stress-carrying capacity is removed or adjusted depending on the type of
failure chosen, but the rebar contribution to the element stress-carrying
capacity is not removed. However, if you also include failure in the rebar
material definition, the rebar contribution to the element stress-carrying
capacity will also be removed or adjusted if the failure criterion specified
for the rebar is met.
Elements
The shear and tensile failure models with element deletion can be used with
any elements in
Abaqus/Explicit
that include mechanical behavior (elements that have displacement degrees of
freedom). The shear and tensile failure models without element deletion can be
used only with plane strain, axisymmetric, and three-dimensional solid
(continuum) elements in
Abaqus/Explicit.
Output
In addition to the standard output identifiers available in
Abaqus/Explicit
(Abaqus/Explicit Output Variable Identifiers),
the following variable has special meaning for the shear and tensile failure
models:
STATUS
Status of element (1.0 if the element is active, 0.0 if it is not).
STATUSMP
Status of each material point in the element (1.0 if a material point is
active, 0.0 if it is not).