Inserting a New Riks Step

Inserting a Riks step within the Simulation History indicates that the Riks method should be used to simultaneously solve for loads and displacements. The Riks method is typically used to analyze model response where material nonlinearity, geometric nonlinearity, or unstable response are likely, such as under buckling, collapse, or snap-through conditions. The Riks step is available only in a Nonlinear Structural case, and it must be defined as the last step in the case. A Riks step can be defined in new analysis cases or in analysis cases that contain general static or static linear perturbation steps; it cannot be defined in analysis cases that contain heat transfer steps. However, analysis documents can contain additional cases with heat transfer steps. Sequentially coupled thermal-stress analyses, in which the stress/displacement solution is dependent on a temperature field but there is no inverse dependency, can be performed by reading the temperature solution from a heat transfer analysis case into a stress analysis case as a predefined field. See Step Sequence Restrictions for more information.

Abaqus treats any preexisting loads at the start of the Riks step as having a constant magnitude. Loads defined during the Riks step are ramped from zero to the defined value during the step. Abaqus uses the arc length along the static equilibrium path in load-displacement space to determine the progress of the analysis. The load proportionality factor is used to determine the incrementation. The load proportionality factor is the ratio of the current arc length increment to the estimated total arc length scale factor. The Initial arc length increment is used as the current arc length increment for the first increment. For subsequent increments Abaqus calculates the arc length increment as part of the analysis. See Unstable collapse and postbuckling analysis in the Abaqus Analysis Guide for more information on the Riks method.

This task shows you how to insert a new Riks step in a Nonlinear Structural case.

  1. Select Start>Analysis & Simulation>Nonlinear Structural Analysis from the menu bar to enter the Nonlinear Structural Analysis workbench.

  2. From the New Analysis Case dialog box, select Nonlinear Structural Case.

  3. Click the Riks Step icon .

    Tip:  Alternatively, you can select Insert>Riks Step from the menu bar, or you can right-click the last step in the simulation history and select Insert Step Below>Riks Step from the menu that appears.

    The Riks Step dialog box appears, and a Riks Step objects set appears in the specification tree under the Simulation History objects set for the current Nonlinear Structural case.

  4. You can change the step identifier by editing the Step name field. This name will be used in the specification tree.

  5. Enter a description for the step in the Step description field.

  6. If necessary, do the following to modify the Basic Step Data:

    1. Specify whether Abaqus should account for nonlinear geometric effects in the step by selecting Off or On for Nonlinear geometry. (The default value is Off unless hyperelastic materials are included in the model.) See Accounting for Nonlinear Geometric Effects for more information.

    2. Edit the Stopping Criteria to specify a maximum load proportionality factor and/or maximum displacement that will stop the analysis.

      Since the load and the displacement are being calculated simultaneously, the stopping criteria provide methods to end the analysis before the maximum number of increments is reached.

  7. If necessary, do the following to modify the Incrementation Controls:

    1. Select the Incrementation type: Automatic or Fixed. Automatic incrementation means that Abaqus will select increment sizes based on computational efficiency. Fixed incrementation means that you specify a fixed increment size; this option is not recommended for Riks steps since it prevents Abaqus from reducing the arc length if a severe nonlinearity occurs.

    2. Enter a value for the Maximum number of increments. The default number of increments for a step is 100; if significant nonlinearity is present in the simulation, the analysis may require many more increments. If Abaqus needs more increments than the specified upper limit to complete the step, it will terminate the analysis with an error message.

    3. Enter a value for the Initial arc length increment. The ratio of the initial arc length increment to the estimated total arc length scale factor specifies the proportion of load applied in the first increment. The default initial increment length is the same as the estimated total arc length for the step. As a result, Abaqus applies all of the loads defined in the step in the first increment. Since nonlinearity is expected, a converged solution is not likely with application of the full load. However, Abaqus uses the initial increment to calculate a new increment size and continue the analysis.

    4. Enter a value for the Minimum arc length increment. This parameter is used only for automatic incrementation. Abaqus will terminate an analysis if excessive cutbacks caused by convergence problems reduce the increment size below the minimum value.

    5. Enter a value for the Maximum arc length increment. This parameter is used only for automatic incrementation. Effectively, there is no upper limit for the arc length—by default it is 1e+36. Depending on your simulation, you may want to specify a different maximum arc length.

    6. Enter a value for the Total arc length scale factor. This value is used with the initial arc length increment to determine the load proportionality factor for the initial step. The default value is 1.

  8. Click OK when you have finished defining the step.

    The Riks Step objects set contains a default Field Output Request object in a Field Output Requests objects set. See Requesting Results for more information.