General and Perturbation Procedures

General Analysis Steps

A general analysis step is one in which the effects of any nonlinearities present in the model can be included. The starting condition for each general step is the ending condition from the last general step, with the state of the model evolving throughout the history of general analysis steps as it responds to the history of loading. If the first step of the analysis is a general step, the initial conditions for the step can be specified directly (Initial Conditions).

Abaqus always considers total time to increase throughout a general analysis. Each step also has its own step time, which begins at zero in each step. If the analysis procedure for the step has a physical time scale, as in a dynamic analysis, step time must correspond to that physical time. Otherwise, step time is any convenient time scale—for example, 0.0 to 1.0—for the step. The step times of all general analysis steps accumulate into total time. Therefore, if an option such as creep (available only in Abaqus/Standard) whose formulation depends on total time is used in a multistep analysis, any steps that do not have a physical time scale should have a negligibly small step time compared to the steps in which a physical time scale does exist.

Sources of Nonlinearity

Nonlinear stress analysis problems can contain up to three sources of nonlinearity: material nonlinearity, geometric nonlinearity, and boundary nonlinearity.

Material Nonlinearity

Abaqus offers models for a wide range of nonlinear material behaviors (see Combining Material Behaviors). 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.

Geometric Nonlinearity

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 Formulations in Abaqus/Standard and Contact Formulations for Contact Pairs in Abaqus/Explicit). 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). 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 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, pipe, 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) 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.

Boundary Nonlinearity

Contact problems are a common source of nonlinearity in stress analysis—see About Contact Interactions. Other sources of boundary nonlinearity are nonlinear elastic springs, films, radiation, multi-point constraints, etc.

Loading

In a general analysis step the loads must be defined as total values. The rules for applying loads in a general, multistep analysis are defined in About Loads.

Incrementation

The general analysis procedures in Abaqus offer two approaches for controlling incrementation. Automatic control is one choice: you define the step and, in some procedures, specify certain tolerances or error measures. Abaqus then automatically selects the increment size as it develops the response in the step. Direct user control of increment size is the alternative approach, whereby you specify the incrementation scheme. The direct approach is sometimes useful in repetitive analyses with Abaqus/Standard, where you have a good “feel” for the convergence behavior of the problem. The methods for selecting automatic or direct incrementation are discussed in the individual procedure sections.

In nonlinear problems in Abaqus/Standard the challenge is always to obtain a convergent solution in the least possible computational time. In these cases automatic control of the time increment is usually more efficient because Abaqus/Standard can react to nonlinear response that you cannot predict ahead of time. Automatic control is particularly valuable in cases where the response or load varies widely through the step, as is often the case in diffusion-type problems such as creep, heat transfer, and consolidation. Ultimately, automatic control allows nonlinear problems to be run with confidence in Abaqus/Standard without extensive experience with the problem.

Strong nonlinearities typically do not present difficulties in Abaqus/Explicit because of the small time increments that are characteristic of an explicit dynamic analysis product.

Stabilization of Unstable Problems in Abaqus/Standard

Some static problems can be naturally unstable, for a variety of reasons.

Unconstrained Rigid Body Motions

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 Adjusting Contact Controls in Abaqus/Standard) when rigid body motions exist during the approach of two bodies that will eventually come into contact.

Localized Buckling Behavior or Material Instability

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, Quasi-Static Analysis, Steady-State Transport Analysis, Fully Coupled Thermal-Stress Analysis, Fully Coupled Thermal-Electrical-Structural Analysis, or Coupled Pore Fluid Diffusion and Stress Analysis).

Linear Perturbation Analysis Steps

Linear perturbation analysis steps are available only in Abaqus/Standard (Abaqus/Foundation is essentially the linear perturbation functionality in Abaqus/Standard). The response in a linear analysis step is the linear perturbation response about the base state. The base state is the current state of the model at the end of the last general analysis step prior to the linear perturbation step. If the first step of an analysis is a perturbation step, the base state is determined from the initial conditions (Initial Conditions). In Abaqus/Foundation the base state is always determined from the initial state of the model.

Linear perturbation analyses can be performed from time to time during a fully nonlinear analysis by including the linear perturbation steps between the general response steps. The linear perturbation response has no effect as the general analysis is continued. The step time of linear perturbation steps, which is taken arbitrarily to be a very small number, is never accumulated into the total time. A simple example of this method is the determination of the natural frequencies of a violin string under increasing tension (see Vibration of a cable under tension). The tension of the string is increased in several geometrically nonlinear analysis steps. After each of these steps, the frequencies can be extracted in a linear perturbation analysis step.

If geometric nonlinearity is included in the general analysis upon which a linear perturbation study is based, stress stiffening or softening effects and load stiffness effects (from pressure and other follower forces) are included in the linear perturbation analysis.

Load stiffness contributions are also generated for centrifugal and Coriolis loading. In direct steady-state dynamic analysis Coriolis loading generates an imaginary antisymmetric matrix. This contribution is accounted for currently in solid and truss elements only and is activated by using the unsymmetric matrix storage and solution scheme in the step.

Linear Perturbation Procedures

The following purely linear perturbation procedures are available in Abaqus/Standard:

In addition, the following analysis techniques are treated as linear perturbation steps in an analysis:

Except for these procedures and the static procedure (explained below), all other procedures can be used only in general analysis steps (in other words, they are not available with Abaqus/Foundation). All linear perturbation procedures except for the complex eigenvalue extraction procedure are available with Abaqus/Foundation.

Static Perturbation Analysis

A static perturbation stress analysis (Static Stress Analysis) can be conducted in Abaqus/Standard.

Contact within Static Perturbation Analysis

Two approaches are available for handling contact in a static perturbation analysis.

In the static linear perturbation procedure, which is the default, the open/closed status of each contact constraint is assumed to remain as it is in the base state. Further, points in contact (i.e., with a “closed” status) are also assumed to be sticking if friction is present except when a velocity differential is imposed by the motion of the reference frame or the transport velocity. In the latter case, slipping conditions are assumed regardless of the friction coefficient. Thus, by freezing contact status, the contact contributions and thereby the overall governing equations are imposed to be linear in the solution variables and result in a purely linear static perturbation analysis.

In the special case where all contact constraints in an analysis are modeled with the small sliding formulation and friction is absent, the non-default LCP solution technique (see Linear Complementarity Problem (LCP) Solution Technique for Solving Contact Problems) can be activated. The static LCP perturbation procedure treats contact in a nonlinear manner by allowing for contact status changes due to applied perturbation loads and boundary conditions. As a result, the actual set of points in contact (that can be different from base state) and their normal contact pressure values are computed as a part of the solution process during the perturbation analysis. The static LCP perturbation procedure, with the exception of nonlinearities from contact, shares its behavior with the static linear perturbation procedure in most respects. For example, the solution from the perturbation analysis including the (possibly) modified contact status is not carried over to subsequent steps.

Loading and Output

Load magnitudes (including the magnitudes of prescribed boundary conditions and predefined temperatures and fields) during a linear perturbation analysis step are defined as the magnitudes of the load perturbations only. Likewise, the value of any solution variable is output as the perturbation value only—the value of the variable in the base state is not included.

Multiple Load Case Analysis

Multiple load cases can be analyzed simultaneously for static, direct-solution steady-state dynamic and SIM-based steady-state dynamic (including subspace projection) linear perturbation steps. See Multiple Load Case Analysis for a description of this capability.

Restrictions

A linear perturbation analysis is subject to the following restrictions:

In a linear perturbation analysis, amplitude references (Amplitude Curves) can be used to specify loads and boundary conditions as functions of frequency (in a direct steady-state dynamic analysis) or to define loads and base motion as functions of frequency (in frequency-domain mode-based dynamic procedures) or as functions of time (in a transient modal dynamic analysis). If loads or boundary conditions are specified as functions of time in a linear perturbation analysis that has no time period (for example, in a static perturbation analysis), the amplitude value corresponding to time=0 will be used.
A general implicit dynamic analysis (Implicit Dynamic Analysis Using Direct Integration) cannot be interrupted to perform perturbation analyses: before performing the perturbation analysis, Abaqus/Standard requires that the structure be brought into static equilibrium.
During a linear perturbation analysis step, the model's response is defined by its linear elastic stiffness at the base state. For viscoelastic materials the elastic moduli at the base state is evaluated as described in Material Options for static procedures and in Evaluating Frequency-Dependent Material Properties for frequency-based procedures. Plasticity and other inelastic effects are ignored during a linear perturbation analysis step. For hyperelasticity (Hyperelastic Behavior of Rubberlike Materials) or hypoelasticity (Hypoelastic Behavior), the tangent elastic moduli in the base state are used. If cracking has occurred—for example, in the concrete model (Concrete Smeared Cracking)—the damaged elastic (secant) moduli are used.
The default behavior where the contact state is not allowed to change applies to any linear perturbation step and not just to static linear perturbation steps (see Contact within Static Perturbation Analysis). This restriction does not apply to the LCP solution technique, which can be activated only within a static perturbation step.
The effects of temperature and field variable perturbations are ignored for materials that are dependent on temperature and field variables. However, temperature perturbations will produce perturbations of thermal and field expansion strains (see Computing Thermal Strains in Linear Perturbation Steps and Computing Field Expansion Strains in Linear Perturbation Steps).