Requesting Results

You can request two kinds of results from a nonlinear or thermal analysis: field output and history output.

  • Field output is the output of variables that are written relatively infrequently to the output database file. Typically, you request field output for your entire model or for a large region. When you create the first step in a nonlinear or thermal analysis case, Nonlinear Structural Analysis or Thermal Analysis creates a default field output request that is propagated to subsequent steps. Field output requests generate the data used to produce results images.

  • 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. History output is not requested by default.

You can modify both types of output requests in each step to change the output variables or the output frequency. You can deactivate an output request for a step and activate it in a later step. You can delete an output request in the step in which it was created.

The output requested in a general step is independent of the output requested in a frequency step. Otherwise, the propagation behavior for output requests is the same as the propagation behavior for prescribed conditions described in Propagation.

Nonlinear Structural Analysis or Thermal Analysis creates a default field output request for the first step of each type (general or heat transfer) in your model. You can modify or delete the default request, create additional field output requests, or create history output requests. Nonlinear Structural Analysis and Thermal Analysis propagate the output requests created in a step to all subsequent steps of the same type. For example, if you add a history output request to a general step, Nonlinear Structural Analysis propagates your request to all subsequent general steps but not to any frequency steps. Likewise, if you modify an output request, your change is propagated to all subsequent steps of the same type.

The following sections discuss the use of output requests in Nonlinear Structural Analysis and Thermal Analysis:

Creating and Modifying Field Output Requests: Creates or modifies a field output request in the current analysis step.

Creating and Modifying History Output Requests: Creates or modifies a history output request in the current analysis step.

Creating and Modifying Field Output Requests

Field output is the output of variables that are written relatively infrequently to the output database. Typically, you request field output for your entire model or for a large region. Each Nonlinear Structural Analysis and Thermal Analysis analysis case contains a default field output request for each type of step in the analysis. The default request is created in the first step of each step type and writes output to the output database (.odb) file when you run the analysis. The field output requests created in a step are propagated to all subsequent steps of the same step type. Field output requests generate the data used to produce results images (see Visualizing Results).

By default, output is requested from every node or integration point and from the default section points for the entire model. The default set of output variables corresponds to the step type (see Table 4–2); these variables are written by default at every increment.

Table 4–2 Default output variables.

Step Type Default Output
General Static Stresses, strains, plastic strains, equivalent plastic strains, plastic strain magnitudes, displacements, reaction forces, point loads and concentrated moments, contact pressures and frictional shear stresses, and contact openings and relative tangential motions
Frequency Displacements, stresses, and strains
Heat Transfer Heat flux per unit area, nodal temperatures, and reaction flux values

You can use the tool to create new field output requests; and you can use the field output editor to modify new or existing field output requests—including the default requests—either in the step in which they were created or a step to which they were propagated. If you modify a propagated field output request, you can modify only the output variables and the output frequency.

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

To create or modify a field output request:

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

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

    The Edit Field 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 the solver write field 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 also select surface groups.

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

    Preselected defaults

    Choose this method to allow the solver 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 field 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 the solver write field 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 the solver write field data for all section points to the output database.

    Specify

    Choose Specify to manually type the section points for which the solver will write field 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, the solver also writes output for the last increment of the step.

    • For a frequency step in a Nonlinear Structural case, you can request output of All modes (the default), or you can Specify individual modes and enter the desired modes.

  8. The propagation and activation status are provided for information only; you cannot edit them from the Field 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.

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. 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 the solver 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 the solver 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 the solver 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 the solver 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 the solver 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, the solver also writes output for the last increment of the step.

  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.