can be used in conjunction with the models of progressive damage and failure in Abaqus/Explicit (About Damage and Failure for Ductile Metals) to specify different damage initiation
criteria and damage evolution laws that allow for the progressive degradation of the
material stiffness and the removal of elements from the mesh.
Anisotropic yield or creep behavior using quadratic Hill's potential is modeled through the
use of yield or creep stress ratios, . In the case of anisotropic yield the yield ratios are defined with
respect to a reference yield stress, (given for the metal plasticity definition), such that if is applied as the only nonzero stress, the corresponding yield stress is . The plastic flow rule is defined below.
In the case of anisotropic creep the are creep ratios used to scale the stress value when the creep strain rate
is calculated. Thus, if is the only nonzero stress, the equivalent stress, , used in the user-defined creep law is .
Yield and creep stress ratios can be defined as constants or as tabular functions of
temperature and predefined field variables. A local orientation must be used to define the
direction of anisotropy (see Orientations).
Input File Usage
Use the following option to define anisotropic yield or creep:
This option must appear immediately after the PLASTIC or the CREEP material option data to
which it applies. Thus, if anisotropic metal plasticity and anisotropic creep behavior are
both required, the POTENTIAL option must appear twice
in the material definition, once after the metal plasticity data and again after the creep
data.
Abaqus/CAE Usage
Use one of the following models:
Property module: material editor:
MechanicalPlasticityPlastic: SuboptionsPotentialMechanicalPlasticityCreep: SuboptionsPotential
Anisotropic Yield
Hill's potential function is a simple extension of the Mises function, which can be
expressed in terms of rectangular Cartesian stress components as
where and N are constants obtained by tests of the material
in different orientations. They are defined as
where each is the measured yield stress value when is applied as the only nonzero stress component; is the user-defined reference yield stress specified for the metal
plasticity definition; , , , , , and are anisotropic yield stress ratios; and . Therefore, the six yield stress ratios are defined as follows (in the
order in which you must provide them):
Because of the form of the yield function, all of these ratios must be positive. If the
constants F, G, and H are
positive, the yield function is always well defined. However, if one or more of these
constants is negative, the yield function might be undefined for some stress states because
the quantity under the square root is negative.
Property module: material editor: MechanicalPlasticityPlastic: SuboptionsPotential
Anisotropic Creep
For anisotropic creep in Abaqus/Standard Hill's function can be expressed as
where is the equivalent stress and F,
G, H, L,
M, and N are constants obtained by tests of the
material in different orientations. The constants are defined with the same general
relations as those used for anisotropic yield (above); however, the reference yield stress, , is replaced by the uniaxial equivalent deviatoric stress, (found in the creep law), and , , , , , and are referred to as “anisotropic creep stress ratios.” The six creep stress
ratios are, therefore, defined as follows (in the order in which they must be provided):
You must define the ratios in each direction that will be used to scale the stress value when the
creep strain rate is calculated. If all six values are set to unity, isotropic creep is obtained.
Property module: material editor: MechanicalPlasticityCreep: SuboptionsPotential
Defining Anisotropic Yield Behavior on the Basis of Strain Ratios (Lankford's
r-Values)
As discussed above, Hill's anisotropic plasticity potential is defined in Abaqus from user input consisting of ratios of yield stress in different directions with respect
to a reference stress. However, in some cases, such as sheet metal forming applications, it
is common to find the anisotropic material data given in terms of ratios of width strain to
thickness strain. Mathematical relationships are then necessary to convert the strain ratios
to stress ratios that can be input into Abaqus.
In sheet metal forming applications, we are generally concerned with plane stress
conditions. Consider to be the “rolling” and “cross” directions in the plane of the sheet;
z is the thickness direction. From a design viewpoint, the type of
anisotropy usually desired is that in which the sheet is isotropic in the plane and has an
increased strength in the thickness direction, which is normally referred to as transverse
anisotropy. Another type of anisotropy is characterized by different strengths in different
directions in the plane of the sheet, which is called planar anisotropy.
In a simple tension test performed in the x-direction in the plane of
the sheet, the flow rule for this potential (given above) defines the incremental strain
ratios (assuming small elastic strains) as
Therefore, the ratio of width to thickness strain, often referred to as Lankford's
r-value, is
Similarly, for a simple tension test performed in the y-direction in
the plane of the sheet, the incremental strain ratios are
and
Transverse Anisotropy
A transversely anisotropic material is one where . If we define in the metal plasticity model to be equal to ,
and, using the relationships above,
If (isotropic material), and the Mises isotropic plasticity model is recovered.
Planar Anisotropy
In the case of planar anisotropy and are different and will all be different. If we define in the metal plasticity model to be equal to ,
and, using the relationships above, we obtain
Again, if , and the Mises isotropic plasticity model is recovered.
General Anisotropy
Thus far, we have only considered loading applied along the axes of anisotropy. To derive
a more general anisotropic model in plane stress, the sheet must be loaded in one other
direction in its plane. Suppose we perform a simple tension test at an angle to the x-direction; then, from equilibrium
considerations we can write the nonzero stress components as
where is the applied tensile stress. Substituting these values in the flow
equations and assuming small elastic strains yields
Assuming small geometrical changes, the width strain increment (the increment of strain
at right angles to the direction of loading, ) is written as
and Lankford's r-value for loading at an angle is
One of the more commonly performed tests is that in which the loading direction is at
45°. In this case
If is equal to in the metal plasticity model, . are as defined before for transverse or planar anisotropy and, using the
relationships above,
Progressive Damage and Failure
In Abaqus/Explicit Hill anisotropic yield can be used in conjunction with the models of progressive damage
and failure discussed in About Damage and Failure for Ductile Metals. The capability allows
for the specification of one or more damage initiation criteria, including ductile, shear,
forming limit diagram (FLD), forming limit stress diagram
(FLSD), and Müschenborn-Sonne forming limit diagram
(MSFLD) criteria. After damage initiation, the material
stiffness is degraded progressively according to the specified damage evolution response.
The model offers two failure choices, including the removal of elements from the mesh as a
result of tearing or ripping of the structure. The progressive damage models allow for a
smooth degradation of the material stiffness, making them suitable for both quasi-static and
dynamic situations.
Property module: material editor: MechanicalDamage for Ductile Metalsdamage initiation type: specify the damage initiation criterion: SuboptionsDamage Evolution: specify the damage evolution parameters
Initial Conditions
When we need to study the behavior of a material that has already been subjected to some
work hardening, Abaqus allows you to prescribe initial conditions for the equivalent plastic strain, , by specifying the conditions directly (Initial Conditions).
Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step; Definition: User-defined
Elements
You can define Hill anisotropic yield for any element that can be used with the following models:
You cannot define Hill anisotropic yield for one-dimensional elements in Abaqus/Explicit (beams and trusses). In Abaqus/Standard it can also be defined for any element that can be used with the linear kinematic
hardening plasticity model (Models for Metals Subjected to Cyclic Loading) but not with the
nonlinear isotropic/kinematic hardening model. Likewise, anisotropic creep with Hill's
function can be defined for any element that can be used with the classical metal creep
model in Abaqus/Standard (Rate-Dependent Plasticity: Creep and Swelling).