# 5. Material Models

This chapter describes material models that can be used in conjunction with the elements in Sierra/SM. Most of the material models can be used in either implicit or explicit analyses. Even though a material model can be used by both implicit and explicit, usage of the model may be better suited for the type of problems solved implicit versus explicit. For example, a material model that was built to characterize behavior over a long time would be better suited for use in Adagio/Implicit than in Presto/Explicit.

The material models described in this chapter are, in general, applicable to solid elements. Structural elements, such as shells and beams, have a more limited set of material models. Section 6 describes the element library, including which material models are available for the various elements. The introduction to Section 6 summarizes all the element types available in Sierra/SM. For each element type, a list of available material models is provided.

State variable output is available for many materials. See Section 9.12.2 to learn how to output the state variables for materials or to the specific material model sections for the list of computed state variables for that material model.

Most material models used by Sierra/SM are defined by the LAMÉ material library [[1]].

`MATERIAL` command blocks appear in the SIERRA scope in the general form shown below.

    BEGIN MATERIAL <string>mat_name
      #
      # Command lines and command blocks for material
      # models appear in this scope.
      #
    END [MATERIAL <string>mat_name]

`MATERIAL` command blocks are physics independent in the sense that the information in them can be shared by more than one application. The command block begins with the line:

    BEGIN MATERIAL <string>mat_name

and terminates with the line:

    END [MATERIAL <string>mat_name]

Here, the string `mat_name` is a user-specified name for the command block. This name is typically descriptive of the material being modeled, e.g., `aluminum_t6061`.

Within a `MATERIAL` command block, there will usually be at least one `BEGIN PARAMETERS FOR MODEL` command block as well as other general material command lines used to describe particular material models. The general material command lines, if present, are listed first, followed by one or more material-model command blocks. The general material command lines may be used to specify the density of the material, the Biot’s coefficient, and the application of temperatures and thermal strains. Each material-model command block follows the naming convention of `PARAMETERS FOR MODEL model_name`, where `model_name` identifies a particular material model, such as elastic, elastic-plastic, or orthotropic crush. Each such command block contains all the parameters needed to describe a particular material model.

As noted above, more than one material-model command block can appear within a `MATERIAL` command block. For example, a `MATERIAL` command block called `steel` could have two nested material-model command blocks. One of the material-model command blocks would provide an elastic model for `steel` and the other an elastic-plastic model for `steel`. The general form of a `MATERIAL` command block would be as follows:

    BEGIN MATERIAL <string>mat_name
      #
      # General material command lines
      DENSITY = <real>density_value
      BIOTS COEFFICIENT = <real>biots_coefficient_value
      #
      THERMAL \{LOG|ENGINEERING\} STRAIN FUNCTION =
        <string>thermal_strain_function
      # or all three of the following
      THERMAL \{LOG|ENGINEERING\} STRAIN X FUNCTION =
        <string>thermal_strain_x_function
      THERMAL \{LOG|ENGINEERING\} STRAIN Y FUNCTION =
        <string>thermal_strain_y_function
      THERMAL \{LOG|ENGINEERING\} STRAIN Z FUNCTION =
        <string>thermal_strain_z_function
      THERMAL \{LOG|ENGINEERING\} STRAIN DIRECTION
        <string>dir_name FUNCTION = <string>funcName
      #
      ARTIFICIAL ENGINEERING STRAIN FUNCTION =
        <string>artificial_strain_function
      # or all three of the following
      ARTIFICIAL ENGINEERING STRAIN X FUNCTION =
        <string>artificial_strain_x_function
      ARTIFICIAL ENGINEERING STRAIN Y FUNCTION =
        <string>artificial_strain_y_function
      ARTIFICIAL ENGINEERING STRAIN Z FUNCTION =
        <string>artificial_strain_z_function
      ARTIFICIAL ENGINEERING STRAIN DIRECTION
        <string>dir_name FUNCTION = <string>funcName
      #
      BEGIN PARAMETERS FOR MODEL <string>model_name1
        #
        # Parameters for material model model_name1
      END PARAMETERS FOR MODEL <string>model_name1
      #
      BEGIN PARAMETERS FOR MODEL <string> model_name2
        #
        # Parameters for material model model_name2
      END PARAMETERS FOR MODEL <string> model_name2
      #
      # Additional model command blocks if required
      #
    END [MATERIAL <string>mat_name]

In the above general form for a `MATERIAL` command block, the string `model_name1` could be `ELASTIC` and the string `model_name2` could be `ORTHOTROPIC CRUSH`. Typically, however, only one material model would be desired for a given block, and the `MATERIAL` command block would have only one `PARAMETERS FOR MODEL` command block. A particular material model may only appear once within a given `MATERIAL` command block.

Although multiple material models can be defined for one material within a `MATERIAL` command block, only one material model is actually used for a given element block during an analysis. The ability to define multiple constitutive models for one material is provided as a convenience to enable easily switching between models. The material name and the model name are both referenced when material models are assigned to element blocks within the `FINITE ELEMENT MODEL` command block, which is described in Section 6.1.

This chapter is organized according to the general form for the `MATERIAL` command block. Section 5.1 discusses the `DENSITY` command line, the `BIOTS COEFFICIENT` command line, and the command lines used for thermal strains, and also explains how temperatures and thermal strains are applied. Section 5.2 describes each of the material models that are used by Sierra/SM. References applicable to Sierra/SM are listed at the end of the chapter.

As indicated in the introductory material, not all the material models are applicable to all element types. As one example, there are the material models available for use with cohesive zone elements or with Dash contact, as detailed in Section 5.3. As another example, there is a one-dimensional elastic material model that is used for a truss element but is not applicable to solid elements such as hexahedra or tetrahedra. For this particular example, the specific material-model usage is hidden from the user. If the user specifies a linear elastic material model for a truss, the one-dimensional elastic material model is used. If the user specifies a linear elastic material model for a hexahedron, a full three-dimensional elastic material model is used. As another example, the energy-dependent material models in Presto can only be used for solid elements such as hexahedra and tetrahedra. (Section 6 indicates what material models are available for which element formulations.)

Nonlinear material models have state variables. See Section 9.12.2 for more information on how to output the state variables for the nonlinear material models.

Brief descriptions of the material models are presented in this chapter. More detailed descriptions can be found in the references for most material models.

[1]

W.M. Scherzinger and D.C. Hammerand. Constitutive models in LAMÉ. Technical Report SAND2007-5873, Sandia National Laboratories, Albuquerque, NM, September 2007. URL: http://infoserve.sandia.gov/sand_doc/2007/075873.pdf.