ABAQUS offers models for a wide range of nonlinear material behaviors (see “Combining material behaviors,” Section 9.1.3). Many of the materials are history dependent: the material's response at any time depends on what has happened to it at previous times. Thus, the solution must be obtained by following the actual loading sequence. The general analysis procedures are designed with this in view.

It is possible in ABAQUS to define a problem as a “small-displacement” analysis, which means that geometric nonlinearity is ignored in the element calculations—the kinematic relationships are linearized. By default, large displacements and rotations are accounted for in contact constraints even if the small-displacement element formulations are used for the analysis; i.e., a large-sliding contact tracking algorithm is used (see “Contact formulation for ABAQUS/Standard contact pairs,” Section 21.2.2, and “Contact formulation for ABAQUS/Explicit contact pairs,” Section 21.4.4). The elements in a small-displacement analysis are formulated in the reference (original) configuration, using original nodal coordinates. The errors in such an approximation are of the order of the strains and rotations compared to unity. The approximation also eliminates any possibility of capturing bifurcation buckling, which is sometimes a critical aspect of a structure's response (see “Unstable collapse and postbuckling analysis,” Section 6.2.4). You must consider these issues when interpreting the results of such an analysis.

The alternative to a “small-displacement” analysis in ABAQUS is to include large-displacement effects. In this case most elements are formulated in the current configuration using current nodal positions. Elements therefore distort from their original shapes as the deformation increases. With sufficiently large deformations, the elements may become so distorted that they are no longer suitable for use; for example, the volume of the element at an integration point may become negative. In this situation ABAQUS will issue a warning message indicating the problem. In addition, ABAQUS/Standard will cut back the time increment before making further attempts to continue the solution. ABAQUS/Explicit also offers element failure models to allow elements that reach high strains to be removed from a model; see “Dynamic failure models,” Section 11.2.8, for details.

For each step of an analysis you specify whether a small- or large-displacement formulation should be used (i.e., whether geometric nonlinearity should be ignored or included). By default, ABAQUS/Standard uses a small-displacement formulation and ABAQUS/Explicit uses a large-displacement formulation. The default value for the formulation in an import analysis is the same as the value at the time of import. If a large-displacement formulation is used during any step of an analysis, it will be used in all following steps in the analysis; there is no way to turn it off.

Almost all of the elements in ABAQUS use a fully nonlinear formulation. The exceptions are the cubic beam elements in ABAQUS/Standard and the small-strain shell elements (those shell elements other than S3/S3R, S4, S4R, and the axisymmetric shells) in which the cross-sectional thickness change is ignored so that these elements are appropriate only for large rotations and small strains. Except for these elements, the strains and rotations can be arbitrarily large.

The calculated stress is the “true” (Cauchy) stress. For beam and shell elements the stress components are given in local directions that rotate with the material. For all other elements the stress components are given in the global directions unless a local orientation (“Orientations,” Section 2.2.5) is used at a point. For small-displacement analysis the infinitesimal strain measure is used, which is output with the strain output variable E; strain output specified with output variables LE and NE is the same as with E.

*STEP, NLGEOM=YES (default in ABAQUS/Explicit)

*STEP, NLGEOM=NO (default in ABAQUS/Standard)

Contact problems are a common source of nonlinearity in stress analysis—see “Contact interaction analysis: overview,” Section 21.1.1. Other sources of boundary nonlinearity are nonlinear elastic springs, films, radiation, multi-point constraints, etc.

Instability may occur because unconstrained rigid body motions exist. ABAQUS/Standard may be able to handle this type of problem with automatic viscous damping (see “Common difficulties associated with contact modeling in ABAQUS/Standard,” Section 21.2.9) when rigid body motions exist during the approach of two bodies that will eventually come into contact.

*CONTACT CONTROLS, APPROACH
*CONTACT CONTROLS, STABILIZE

Instability may also be caused by localized buckling behavior or by material instability; such instabilities are especially significant when no time-dependent behavior exists in the material modeling. The static, general analysis procedures in ABAQUS/Standard can stabilize this type of problem if you request it (see “Static stress analysis,” Section 6.2.2; “Quasi-static analysis,” Section 6.2.5; “Fully coupled thermal-stress analysis,” Section 6.5.4; or “Coupled pore fluid diffusion and stress analysis,” Section 6.7.1).

*STATIC, STABILIZE
*VISCO, STABILIZE
*COUPLED TEMPERATURE-DISPLACEMENT, STABILIZE
*SOILS, CONSOLIDATION, STABILIZE

Multiple load cases can be analyzed simultaneously for static and direct-solution steady-state dynamic linear perturbation steps. See “Multiple load case analysis,” Section 6.1.3, for a description of this capability.