This chapter contains a few general recommendations regarding material models for implicit analyses inLS-DYNA. For a detailed description of the available material models, see Keyword Manual Vol. II. Not all material models are supported for implicit analysis. If unsupported materials are used, LS-DYNA prints an error message in the d3hsp file and terminates.

The material model *MAT_PIECEWISE_LINEAR_PLASTICITY (or *MAT_24) is commonly used in explicit analyses to characterize metallic materials with plasticity. It also performs well for implicit analyses. (This applies from R9 if IACC = 1 on *CONTROL_ACCURACY, which is active in the attached include files.)

If anisotropy or kinematic hardening is of interest, use *MAT_103 as an alternative to *MAT_24. A template for basic use of *MAT_103 (with isotropic hardening and no strain rate effects) follows:

*MAT_ANISOTROPIC_VISCOPLASTIC_TITLE
Define material title
MID, RO, E, PR, 0., 2, LCSS, 1.
Insert 5 blank lines here

The parameter LCSS is the load curve ID of the hardening curve. After the line defining material ID, density, and so forth, 5 blank rows must follow. For mixed or kinematic hardening with a nonlinear hardening curve, *MAT_225 could be of interest. *MAT_DAMAGE_3 (MAT_153) is a Chaboche-type material model for nonlinear mixed or kinematic hardening. You can use it to specify temperature-dependent material parameters.

If a material model with linear isotropic hardening using a tangent modulus is required, Ansys recommends you use *MAT_24. Specify the yield stress (SIGY), the tangent modulus (ETAN), and the elastic parameters on card 1 and leave the other cards blank. For this case, it is not recommended to use *MAT_3 (*MAT_PLASTIC_KINEMATIC) with the parameter BETA = 1.

For linear implicit analyses, the material response is linearized. Stresses are computed from the strains obtained via the displacement solution to the linear problem. Since no equilibrium iterations are performed in a linear analysis, the obtained stresses can be nonsensical. If consistent estimates of stresses are of interest in a linear analysis, Ansys recommends *MAT_ELASTIC, which is an elastic material model. (From R15 of LS-DYNA, material models are automatically linearized in linear analyses.)

However, Ansys does not recommend using *MAT_ELASTIC to model rubber-like behavior in a nonlinear analysis. Rubber is a hypoelastic material model, which may cause instabilities at large strains. Use *MAT_HYPERELASTIC_RUBBER (*MAT_77) to model rubber materials. An alternative material model for rubber materials is *MAT_SIMPLIFIED_RUBBER_FOAM (*MAT_181), which allows for direct input of results from materials testing. The material model *MAT_MOONEY-RIVLIN_RUBBER (*MAT_27) is generally not recommended for modeling rubber or rubber-like materials. If an elastic response is desired, *MAT_ORTHOTROPIC_ELASTIC (*MAT_2) can be used, since it is a hyperelastic material model which works also for large elastic deformations. For a more detailed discussion of how to model rubber, see Rubber Modeling for Implicit Analysis

LS-DYNA offers many possibilities for modeling creep effects [37]. For example, *MAT_THERMO_ELASTO_VISCOPLASTIC_CREEP (*MAT_188) may be useful.

For modeling fabrics, *MAT_FABRIC can be used. Ansys recommends using the option FORM = -14. This allows you to apply an elastic coating (thickness TCOAT and Young's modulus ECOAT) to the fabric, which can improve convergence of implicit analyses. For the mesh of the fabric part, shell elform 9 is recommended.

You can improve convergence when using the foam materials *MAT_LOW_DENSITY_FOAM and *MAT_FU_CHANG_FOAM, by setting one or both of the following variables:

For these materials, Ansys also recommends that you check that the Youngs modulus (variable E) is consistent with the initial slope of the stress-strain curve.