Requesting data output

Finite element analyses can create very large amounts of output. Abaqus allows you to control and manage this output so that only data required to interpret the results of your simulation are produced. Four types of output are available from an Abaqus analysis:

  • Results stored in a neutral binary file used by Abaqus/CAE for postprocessing. This file is called the Abaqus output database file and has the extension .odb.

  • Printed tables of results, written to the Abaqus data (.dat) file. Output to the data file is available only in Abaqus/Standard.

  • Restart data used to continue the analysis, written to the Abaqus restart (.res) file.

  • Results stored in binary files for subsequent postprocessing with third-party software, written to the Abaqus results (.fil) file.

You will use only the first of these in the overhead hoist simulation.

Context:

By default, Abaqus/CAE writes the results of the analysis to the output database (.odb) file. When you create a step, Abaqus/CAE generates a default output request for the step. A list of the preselected variables written by default to the output database is given in the Abaqus Output Guide. You do not need to do anything to accept these defaults. You use the Field Output Requests Manager to request output of variables that should be written at relatively low frequencies to the output database from the entire model or from a large portion of the model. You use the History Output Requests Manager to request output of variables that should be written to the output database at a high frequency from a small portion of the model; for example, the displacement of a single node.

For this example you will examine the output requests to the .odb file and accept the default configuration.

  1. In the Model Tree, click mouse button 3 on the Field Output Requests container and select Manager from the menu that appears.

    Abaqus/CAE displays the Field Output Requests Manager. This manager displays the status of field output requests in a table format. The left side of the table has an alphabetical list of existing output requests. The top of the table lists the names of all the steps in the analysis in the order of execution. Each cell of the table displays the status of each output request in each step.

    You can use the Field Output Requests Manager to do the following:

    • Select the variables that Abaqus will write to the output database.

    • Select the section points for which Abaqus will generate output data.

    • Select the region of the model for which Abaqus will generate output data.

    • Change the frequency at which Abaqus will write data to the output database.

  2. Review the default output request that Abaqus/CAE generates for the Static, Linear perturbation step you created and named Apply load.

    Select the cell in the table labeled Created if it is not already selected. The following information related to the cell is shown in the legend at the bottom of the manager:

    • The type of analysis procedure carried out in the step in that column.

    • The list of output request variables.

    • The output request status.

  3. On the right side of the Field Output Requests Manager, click Edit to view more detailed information about the output request.

    The field output editor appears. In the Output Variables region of this dialog box, there is a text box that lists all variables that will be output. If you change an output request, you can always return to the default settings by choosing Preselected defaults above the text box.

  4. Click the arrows next to each output variable category to see exactly which variables will be output. The boxes next to each category title allow you to see at a glance whether all variables in that category will be output. A black check mark indicates that all variables are output, while a gray check mark indicates that only some variables will be output.

    Based on the selections shown at the bottom of the dialog box, data will be generated at every default section point in the model and will be written to the output database after every increment during the analysis.

  5. Click Cancel to close the field output editor, since you do not wish to make any changes to the default output requests.

  6. Click Dismiss to close the Field Output Requests Manager.

    Note:

    What is the difference between the Dismiss and Cancel buttons? Dismiss buttons appear in dialog boxes that contain data that you cannot modify. For example, the Field Output Requests Manager allows you to view output requests, but you must use the field output editor to modify those requests. Clicking the Dismiss button simply closes the Field Output Requests Manager. Conversely, Cancel buttons appear in dialog boxes that allow you to make changes. Clicking Cancel closes the dialog box without saving your changes.

  7. Review the history output requests in a similar manner by right-clicking the History Output Requests container in the Model Tree and opening the history output editor.