Creating and Modifying History Output Requests

History output is the output of variables that are written relatively frequently to the output database—as often as every increment. Typically, you request history output for a small area of your model, such as a single integration point or a small region; however, some history output in a Nonlinear Structural case such as total mass, total volume, and center of gravity requires selection of the whole model. You can use the tool to create new history output requests; and you can use the history output editor to modify new or existing history output requests, either in the step in which they were created or in a step to which they were propagated.

Note:  Abaqus for CATIA V5 automatically creates a default history output request in the specification tree when you create a new Explicit Dynamics step in the Nonlinear Structural Analysis workbench. This history request has every energy-related variable toggled on by default. For more information, see Inserting a New Explicit Dynamics Step.

If you modify a propagated history output request, you can modify only the output variables and the output frequency. You cannot request history output from a frequency step.

History output requests are contained in a History Output Request object under the History Output Requests objects set for the step.

To create or modify a history output request:

  1. To create a new history output request, click .

    To edit an existing history output request, double-click on the History Output Request object under the History Output Requests objects set for the analysis step.

    The History Output Request dialog box is displayed.

  2. If you edit the output request in the step in which it was created, you can change the name of the output request.

  3. If you edit the output request in the step in which it was created, you can change the region for which variables will be output.

    • To request that Abaqus write history data to the output database for the entire model, toggle on Whole model from the Support section at the top of the dialog box.

    • To select a smaller region, toggle off Whole model and select a new model region from the viewport or from the specification tree. You can select point, line, vertex, or edge groups; you cannot select surfaces.

    Note:  Unless the analysis model is relatively small, writing history data for the whole model at a high frequency will produce a very large amount of data for analyses with many increments. Use of a small region of interest is recommended.

  4. In the Output Variables section of the editor, choose one of the following variable selection methods:

    Preselected defaults

    Choose this method to allow Abaqus to select a preselected (default) set of output variables appropriate for the step type.

    All

    Choose this method to automatically select all of the allowable output variables within each variable category in the list.

    Select from list below

    Choose this method to select the output variables of interest from the list of variable categories. Use the following techniques to select particular variables:

    • From the list of variables, select the variables of your choice.

    • For categories with multiple selections, you can select individual variables or toggle the desired variable category to select or deselect all variables within that category.

    Additional variables

    When you use Select from list below, you can type a comma-separated list of variables to be appended to the current list.

  5. Click More to edit the section points and frequency of history output or to view the propagation and activation status for the output request.

  6. If you edit the output request in the step in which it was created, you can change the section points from which variables will be output for shells and beams. The section points that you select can significantly affect the results, for example, a shell with an applied bending load is under tension on one side, compression on the other, and neutral at the center. Choose one of the following:

    Use defaults

    Choose Use defaults to request that Abaqus write history data to the output database from the default section points. (The default section points are usually the outer fibers of the section.)

    All

    Choose All to request that Abaqus write history data for all shell and beam section points to the output database.

    Specify

    Choose Specify to manually type the section points for which Abaqus will write history data to the output database.

  7. Specify the desired output frequency in the Save Output At area.

    For a Nonlinear Structural or Thermal case you can request output Every __ increments (the default) and select the number of increments, or you can request output for only the last increment. If you specify the frequency in increments, Abaqus also writes output for the last increment of the step.

    For an Explicit Dynamics case, you can specify the output frequency in Equally spaced intervals (the default), Every __ units of time, or Every __ increments; and enter the desired number of intervals, time units, or increments.

    For more information, see Output to the output database in the Abaqus Output Guide.

  8. The propagation and activation status are provided for information only; you cannot edit them from the History Output Request dialog box. You can edit the activation status from the specification tree.

    See Status Terms for information on the terms used to describe the propagation and activation status and for instructions on changing the activation status.

  9. When you have finished defining the output request, click OK to save your changes.