Material Data Definition

In the simplest case of a constant property, only the constant value is entered. When the material data are functions of only one variable, the data must be given in order of increasing values of the independent variable. Abaqus then interpolates linearly for values between those given. Thus, you can give as many or as few input values as are necessary for the material model. If the material data depend on the independent variable in a strongly nonlinear manner, you must specify enough data points so that a linear interpolation captures the nonlinear behavior accurately.

When material properties depend on several variables, the variation of the properties with respect to the first variable must be given at fixed values of the other variables, in ascending values of the second variable, then of the third variable, and so on. The data must always be ordered so that the independent variables are given increasing values. This process ensures that the value of the material property is completely and uniquely defined at any values of the independent variables upon which the property depends. See Input Syntax Rules for further explanation and an example.

Example: Temperature-Dependent Linear Isotropic Elasticity

Figure 1 shows a simple, isotropic, linear elastic material, giving the Young's modulus and the Poisson's ratio as functions of temperature.

Example of material definition.

In this case six sets of values are used to specify the material description, as shown in the following table:

Elastic Modulus	Poisson's Ratio	Temperature
$E_1$	${\nu }_1$	${\theta }_1$
$E_2$	${\nu }_2$	${\theta }_2$
$E_3$	${\nu }_3$	${\theta }_3$
$E_4$	${\nu }_4$	${\theta }_4$
$E_5$	${\nu }_5$	${\theta }_5$
$E_6$	${\nu }_6$	${\theta }_6$

For temperatures that are outside the range defined by ${\theta }_1$ and ${\theta }_6$, Abaqus assumes constant values for E and $\nu$. The dotted lines on the graph represent the straight-line approximations that will be used for this model. In this example only one value of the thermal expansion coefficient is given, ${\alpha }_1$, and it is independent of temperature.

Example: Elastic-Plastic Material

Figure 2 shows an elastic-plastic material for which the yield stress is dependent on the equivalent plastic strain and temperature.

Example of material definition with two independent variables.

In this case the second independent variable (temperature) must be held constant, while the yield stress is described as a function of the first independent variable (equivalent plastic strain). Then, a higher value of temperature is chosen and the dependence on equivalent plastic strain is given at this temperature. This process, as shown in the following table, is repeated as often as necessary to describe the property variations in as much detail as required:

Yield Stress	Equivalent Plastic Strain	Temperature
${\sigma }_{01}$	${\epsilon }_{01}$	${\theta }_1$
${\sigma }_{11}$	${\epsilon }_{11}$	${\theta }_1$
${\sigma }_{21}$	${\epsilon }_{21}$	${\theta }_1$
${\sigma }_{31}$	${\epsilon }_{31}$	${\theta }_1$
${\sigma }_{02}$	${\epsilon }_{02}$	${\theta }_2$
${\sigma }_{12}$	${\epsilon }_{12}$	${\theta }_2$
${\sigma }_{22}$	${\epsilon }_{22}$	${\theta }_2$
${\sigma }_{32}$	${\epsilon }_{32}$	${\theta }_2$

By default, the property is assumed to be constant outside the range of independent variables given (except for fabric materials, where the property is extrapolated linearly outside the specified range). For some properties, Abaqus allows you to choose the extrapolation method outside the specified range. In these cases, you can specify if the value of the property is constant or is extrapolated linearly outside the range. If the latter method is selected, Abaqus extrapolates the property linearly using the slope at the last specified data point.

Example: Extrapolation for Elastic-Plastic Material with Isotropic Hardening

In Table 1 the Mises isotropic yield surface is defined by providing three data points.

Table 1. Isotropic hardening data.

Yield Stress	Equivalent Plastic Strain
${\sigma }_0^Y$	$0$
${\sigma }_1^Y$	${\overline{\epsilon }}_1^{pl}$
${\sigma }_2^Y$	${\overline{\epsilon }}_2^{pl}$

The response of the material outside the range of equivalent plastic strain ( ${\overline{\epsilon }}^{pl}>{\overline{\epsilon }}_2^{pl}$ ) depends on the extrapolation method specified, as shown in Figure 3.

Material response for constant and linear extrapolations.

You can specify the number of user-defined field variable dependencies required for many material behaviors (see Predefined Fields). If you do not specify a number of field variable dependencies for a material behavior with which field variable dependence is available, the material data are assumed not to depend on field variables.

User subroutines USDFLD in Abaqus/Standard and VUSDFLD in Abaqus/Explicit allow you to define field variables at a material point as functions of time, material directions, and any of the available material point quantities. These quantities are listed in Abaqus/Standard Output Variable Identifiers for USDFLD and in Available Output Variable Keys for VUSDFLD. Material properties defined as functions of these field variables, therefore, can be dependent on the solution.

User subroutines USDFLD and VUSDFLD are called at each material point for which the material definition includes a reference to the user subroutine.

For general analysis steps the values of variables provided in user subroutines USDFLD and VUSDFLD are those corresponding to the start of the increment. Hence, the solution dependence introduced in this way is explicit; the material properties for a given increment are not influenced by the results obtained during the increment. Consequently, the accuracy of the results generally depends on the time increment size. This is not typically a concern in Abaqus/Explicit because the stable time increment is usually sufficiently small to ensure good accuracy. In Abaqus/Standard you can control the time increment from inside user subroutine USDFLD. For linear perturbation steps the solution variables in the base state are available. For a discussion of general and linear perturbation steps, see General and Perturbation Procedures.

There are applications where it is desirable to redefine a field variable to be equal to the value of a scalar output variable. In such cases, you can avoid the overhead of writing and maintaining a user subroutine and, instead, introduce solution dependence directly by associating a field variable with an existing scalar output variable in Abaqus. For scalar output variables, you only need to specify the output variable identifier to build this association. However, for a vector or a tensor output variable, you must specify the appropriate component of the variable (for example, specify PE11 instead of PE to associate a field variable with the -11- component of the plastic strain tensor).

Any output variable that is available with the GETVRM or the VGETVRM utility routine, used to access material point information in Abaqus/Standard and Abaqus/Explicit, respectively, can be associated with a field variable.

For general analysis steps the values of the output variables are those corresponding to the start of the increment. Hence, the solution dependence introduced in this way is explicit; the material properties for a given increment are not influenced by the results obtained during the increment. Consequently, the accuracy of the results typically depends on the time increment size. This is usually not a concern in Abaqus/Explicit because the stable time increment is usually sufficiently small to ensure good accuracy. For linear perturbation steps the output variables in the base state are used. For a discussion of general and linear perturbation steps, see General and Perturbation Procedures.

In Abaqus/Standard an element is removed from the mesh if the material fails at all of the section points at all the integration locations of the element. In addition, for cohesive elements with traction-separation response, elements are deleted only if none of the integration points are in compression.

In Abaqus/Explicit a general rule for element deletion from the mesh is that the material fails at all of the section points at any one integration location of an element. It is not necessary for all material points in the element to fail. The following examples describe default behavior that results in element removal:

• Solid elements: material failure at any one integration point.
• Second-order reduced-integration beam elements: material failure at all section points through the thickness at either of the two element integration locations along the beam axis.
• Modified triangular and tetrahedral solid elements and fully integrated membrane elements: material failure at any one integration point.

The general rule has two exceptions. First, the criterion for element deletion for cohesive elements is that the material fails at all integration points. In addition, for cohesive elements with traction-separation response, elements are deleted only if none of the integration points are in compression.

Second, a shell element is removed from the mesh by default when all of the active section points (that is, section points where the material has not failed) at any one integration location share the same through-the-thickness z-location. In this condition, the shell element cannot sustain any bending moment. Specifically, a shell element is deleted when any one integration location has at most one active section point or at least two active section points and all of them share the same z-location. For example, in the case of a two-layer composite with three section points per layer, the third section point of the first layer and the first point of the second layer share the same z-location (on the interface between the two layers). The element deletion criterion is triggered if only one of the six section points is left active or if only the two points mentioned above (that share the same z-location) remain active.

When elements are removed from the model, their nodes still remain in the model even if they are not attached to any active elements. When the solution progresses, these nodes can undergo nonphysical displacements due to the extrapolation scheme used in Abaqus/Standard to speed up the solution (see Convergence Criteria for Nonlinear Problems). You can prevent these nonphysical displacements by turning off the extrapolation. In addition, applying a point load to a node that is not attached to an active element causes convergence difficulties since there is no stiffness to resist the load. You should take precautions to avoid these situations.

It is not always desirable to regularize the input data so that they are reproduced exactly in a piecewise linear manner. Suppose the yield stress is defined as a function of plastic strain in Abaqus/Explicit as follows:

It is possible to regularize the data exactly but it is not very economical, since it requires the subdivision of the data into 1000 regular intervals. Regularization is more difficult if the smallest interval you defined is small compared to the range of the independent variable.

Abaqus/Explicit uses an error tolerance to regularize the input data. The number of intervals in the range of each independent variable is chosen such that the error between the piecewise linear regularized data and each of your defined points is less than the tolerance times the range of the dependent variable. In some cases the number of intervals becomes excessive and Abaqus/Explicit cannot regularize the data using a reasonable number of intervals. The number of intervals considered reasonable depends on the number of intervals you define. If you defined 50 or less intervals, the maximum number of intervals used by Abaqus/Explicit for regularization is equal to 100 times the number of user-defined intervals. If you defined more than 50 intervals, the maximum number of intervals used for regularization is equal to 5000 plus 10 times the number of user-defined intervals above 50. If the number of intervals becomes excessive, the program stops during the data checking phase and issues an error message. You can either redefine the material data or change the tolerance value. The default tolerance is 0.03.

The yield stress data in the example above are a typical case where such an error message might be issued. In this case you can simply remove the last data point since it produces only a small difference in the ultimate yield value.

Since strain rate dependence of data is usually measured at logarithmic intervals, Abaqus/Explicit regularizes strain rate data using logarithmic intervals rather than uniformly spaced intervals by default. This generally provides a better match to typical strain-rate-dependent curves. You can specify linear strain rate regularization to use uniform intervals for regularization of strain rate data. The use of linear strain rate regularization affects only the regularization of strain rate as an independent variable and is relevant only if one of the following behaviors is used to define the material data:

• low-density foams (Low-Density Foams)

• rate-dependent metal plasticity (Classical Metal Plasticity)

• rate-dependent viscoplasticity defined by yield stress ratios (Rate-Dependent Yield)

• shear failure defined using direct tabular data (Dynamic Failure Models)

• rate-dependent Drucker-Prager hardening (Extended Drucker-Prager Models)

• rate-dependent concrete damaged plasticity (Concrete Damaged Plasticity)

• rate-dependent damage initiation criterion (Damage Initiation for Ductile Metals)