Analysis StepsA nonlinear or thermal analysis is based on the concept of steps, which define the history of the analysis. Multiple steps can be defined in an analysis. Steps can be introduced simply to change the output requests or to change the loads, boundary conditions, analysis procedure, etc. There is no limit on the number of steps in an analysis. The state of the model at the end of a general step provides the initial conditions for the next step, making it easy to simulate consecutive loadings of a model, such as a dynamic response following a static preload or the loading of a product during its usage following a simulation of the manufacturing process. The following are described in this section: What is a Step?A nonlinear or thermal model uses the following two types of steps to describe the environmental actions on a system: The initial step Nonlinear Structural Analysis or Thermal Analysis creates a special initial step at the beginning of the Simulation History and names it Initialization. Only one initial step is created for each model. You can rename the initial step, but you cannot edit, replace, copy, or delete it. The initial step allows you to define interactions that are applicable at the very beginning of the analysis. For example, if a connection or field is applied throughout the analysis, it is usually convenient to apply such conditions in the initial step. Likewise, when the first analysis step is a frequency step, conditions applied in the initial step form part of the base state for the procedure. Analysis steps The initialization step is followed by one or more analysis steps. Each analysis step represents a period of time in the simulation history and is associated with a specific analysis procedure, such as a static stress analysis or a transient heat transfer analysis. You can change the analysis procedure from step to step. Since the state of the model (stresses, strains, temperatures, etc.) is updated throughout all general analysis steps, the effects of previous history are always included in the response for each new analysis step. There is no limit to the number of analysis steps you can define, but there are restrictions on the step sequence. (For more information, see Step Sequence Restrictions.) For example, consider the following structural analysis of a section of a piping system: Initialization Step: No changes are needed in the default initial step. Step 1: Compress Apply boundary conditions to fix the left end of the pipe and to allow only axial movement at the right end. Apply a compressive force to the right end of the pipe. This step is a general static step. When you create or edit an analysis step (as discussed in Structural Analysis Steps or Thermal Analysis Steps), it becomes the current step. All analysis step operations you perform, such as defining loads or boundary conditions, act on the current step. To set a different analysis step to be current, right-click on the step in the specification tree and select Set As Current Step from the menu that appears. Linear Perturbation StepsThe response in a linear perturbation 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 case is a perturbation step, the base state is determined from the Initialization step. Nonlinear geometric effects are not considered during a linear perturbation step. You can add linear perturbation steps only in structural analysis cases. You can include linear perturbation steps between general static analysis steps; the linear perturbation response has no effect as the general static 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 analysis time (the total accumulated time over all general analysis steps within a particular nonlinear structural analysis case). During a linear perturbation analysis step, the model's response is defined by its linear elastic stiffness at the base state. Plasticity and other inelastic effects are ignored. A Frequency linear perturbation step is available in the Nonlinear Structural Analysis workbench. Accounting for Nonlinear Geometric EffectsFor each step in the analysis you can choose whether the solver will account for nonlinear effects from large displacements and deformations. If the displacements in a model due to loading are relatively small during a step, the effects may be small enough to be ignored. By default, these geometrically nonlinear effects are considered for General Static steps, and these effects are not considered for all other types of steps. However, in cases where the loads on a model result in large displacements, nonlinear geometric effects can become important. The Nonlinear geometry setting for a step determines whether the solver will account for geometric nonlinearity in that step. The sequence of steps and the current setting determine whether you can change the setting in a particular step. For example, if the solver is already accounting for geometric nonlinearity, it continues to do so in all subsequent steps and you cannot change the setting. The Nonlinear geometry setting is turned on by default for General Static steps, and turned off by default for all other types of steps. However, if hyperelastic materials are included in the model, the Nonlinear geometry setting is also turned on by default for other step types in a Nonlinear Structural case. The sequence of steps and the current Nonlinear geometry setting determine whether you can change the Nonlinear geometry setting in a particular step. For example, if the solver is already accounting for geometric nonlinearity, the Nonlinear geometry setting is toggled on for all subsequent steps, and you cannot toggle it off. Step Sequence RestrictionsThe analysis step can be either a static or heat transfer consideration of the system response, depending on the workbench you are using and the case you selected, as shown in Table 4–1. There is no limit to the number of analysis steps you can define. However, once you define a step within an Analysis Case, only compatible steps can be added to that analysis case. For example, if you create a general static step in a structural case, you can add only general static or frequency steps to that analysis case. A thermal analysis can contain only thermal analysis cases, and the cases can contain only heat transfer steps. |