Material data definition

Any number of materials can be defined in an analysis. Each material definition can contain any number of material behaviors, as required, to specify the complete material behavior. For example, in a linear static stress analysis only elastic material behavior may be needed, while in a more complicated analysis several material behaviors may be required.

A name must be assigned to each material definition. This name allows the material to be referenced from the section definitions used to assign this material to regions in the model.

MATERIAL, NAME=name

Property module: material editor: Name
Use the menu bar under the Material Options list to add behaviors to 
a material.

When giving material properties for finite-strain calculations, “stress” means “true” (Cauchy) stress (force per current area) and “strain” means logarithmic strain. For example, unless otherwise indicated, for uniaxial behavior

Material data are often specified as functions of independent variables such as temperature. Material properties are made temperature dependent by specifying them at several different temperatures.

In some cases a material property can be defined as a function of variables calculated by Abaqus; for example, to define a work-hardening curve, stress must be given as a function of equivalent plastic strain.

Material properties can also be dependent on “field variables” (user-defined variables that can represent any independent quantity and are defined at the nodes, as functions of time). For example, material moduli can be functions of weave density in a composite or of phase fraction in an alloy. See Specifying field variable dependence for details. The initial values of field variables are given as initial conditions (see Initial conditions in Abaqus/Standard and Abaqus/Explicit) and can be modified as functions of time during an analysis (see Predefined Fields). This capability is useful if, for example, material properties change with time because of irradiation or some other precalculated environmental effect.

Any material behaviors defined using a distribution in Abaqus/Standard (mass density, linear elastic behavior, and/or thermal expansion) cannot be defined with temperature and/or field dependence. However, material behaviors defined with distributions can be included in a material definition with other material behaviors that have temperature and/or field dependence. See Density, Linear elastic behavior, and Thermal expansion.

In Abaqus you can introduce dependence on solution variables with a user subroutine. 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, of material directions, and of any of the available material point quantities: those listed in Abaqus/Standard output variable identifiers for the case of USDFLD and those listed in Available output variable keys for the case of VUSDFLD. Material properties defined as functions of these field variables may, thus, 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 will generally depend 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. In Abaqus/Standard you can control the time increment from inside subroutine USDFLD. For linear perturbation steps the solution variables in the base state are available. (See General and perturbation procedures for a discussion of general and linear perturbation steps.)

USER DEFINED FIELD

The characteristic element length is used by Abaqus for the regularization of models that exhibit strain softening or is passed to user subroutines that are called at a material point. By default, Abaqus computes the characteristic element length using the geometric mean–based definition.

The default value for a first-order element is the typical length of a line across an element, and the default value for a second-order element is half of the same typical length. For trusses the default value is a characteristic length along the element axis. For membranes and shells the default value is a characteristic length in the reference surface. For axisymmetric elements the default value is a characteristic length in the r–z plane only.

In Abaqus/Explicit you can redefine the value of the characteristic element length based on the element topology and geometry in user subroutine VUCHARLENGTH.

CHARACTERISTIC LENGTH, DEFINITION=GEOMETRIC MEAN

CHARACTERISTIC LENGTH, DEFINITION=USER, COMPONENTS=n, PROPERTIES=n

Interpolating material data as functions of independent variables requires table lookups of the material data values during the analysis. The table lookups occur frequently in Abaqus/Explicit and are most economical if the interpolation is from regular intervals of the independent variables. For example, the data shown in Figure 1 are not regular because the intervals in temperature (the independent variable) between adjacent data points vary. You are not required to specify regular material data. Abaqus/Explicit will automatically regularize user-defined data. For example, the temperature values in Figure 1 may be defined at 10°, 20°, 25°, 28°, 30°, and 35° C. In this case Abaqus/Explicit can regularize the data by defining the data over 25 increments of 1° C and your piecewise linear data will be reproduced exactly. This regularization requires the expansion of your data from values at 6 temperature points to values at 26 temperature points. This example is a case where a simple regularization can reproduce your data exactly.

If there are multiple independent variables, the concept of regular data also requires that the minimum and maximum values (the range) be constant for each independent variable while specifying the other independent variables. The material definition in Figure 2 illustrates a case where the material data are not regular since ${ϵ}_{11}\ne {ϵ}_{12}$, ${ϵ}_{21}\ne {ϵ}_{22}$, and ${ϵ}_{31}\ne {ϵ}_{32}$. Abaqus/Explicit will also regularize data involving multiple independent variables, although the data provided must satisfy the rules specified in Input Syntax Rules.

Rate-sensitive material constitutive behavior may introduce nonphysical high-frequency oscillations in an explicit dynamic analysis. To overcome this problem, Abaqus/Explicit computes the equivalent plastic strain rate used for the evaluation of strain-rate-dependent data as

Here $\mathrm{\Delta }{\overline{\epsilon }}^{pl}$ is the incremental change in equivalent plastic strain during the time increment $\mathrm{\Delta }t$, and ${{\dot{\overline{\epsilon }}}^{pl}❘}_t$ and ${{\dot{\overline{\epsilon }}}^{pl}|}_{t+\mathrm{\Delta }t}$ are the strain rates at the beginning and end of the increment, respectively. The factor $\omega$ ($0<\omega \le 1$) facilitates filtering high-frequency oscillations associated with strain-rate-dependent material behavior. You can specify the value of the strain rate factor, $\omega$, directly. The default value is 0.9. A value of $\omega =1$ does not provide the desired filtering effect and should be avoided.

MATERIAL, SRATE FACTOR=$\omega$