Defining steps and specifying output requests

You will now define the analysis steps. Since interactions, loads, and boundary conditions can be step dependent, analysis steps must be defined before these can be specified. For this simulation you will define a single static, general step. In addition, you will specify output requests for your analysis. These requests will include output to the output database (.odb) file.

This task shows you how to:

Define a step

  1. In the Model Tree, double-click the Steps container to create an analysis step. In the Create Step dialog box that appears, name the step LugLoad and accept the General procedure type. From the list of available procedure options, accept Static, General. Click Continue.

  2. In the Edit Step dialog box that appears, enter the following step description: Apply uniform pressure to the hole. Accept the default settings, and click OK.

Specify output requests to the .odb file

Context:

Since you will use the Visualization module to postprocess the results, you must specify the output data you wish to have written to the output database file. Default history and field output requests are selected automatically by Abaqus/CAE for each procedure type. Edit these requests so that only the displacements, stresses, and reaction forces are written as field data to the output database file.

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

  2. In the Field Output Requests Manager that appears, select the cell labeled Created in the column labeled LugLoad if it is not already selected. The information at the bottom of the dialog box indicates that preselected default field output requests have been made for this step.

  3. On the right side of the dialog box, click Edit to change the field output requests. In the Edit Field Output Request dialog box that appears:

    1. Click the arrow next to Stresses to show the list of available stress output. Accept the default selection of stress components and invariants.
    2. Under Forces/Reactions, make the following changes:

      1. Toggle off concentrated force and moment output (CF).

      2. Toggle on nodal forces due to element stresses (NFORC).

    3. Toggle off Strains and Contact.
    4. Accept the default Displacement/Velocity/Acceleration output.
    5. Click OK, and click Dismiss to close the Field Output Requests Manager.

    Note: The option Exterior only in the Edit Field Output Request dialog box can be used to restrict field output to nodes and elements that belong to the exterior of three-dimensional elements in a model; this option reduces the size of the output database file.

  4. Delete all history output requests. In the Model Tree, click mouse button 3 on the History Output Requests container and select Manager to open the History Output Requests Manager. In the History Output Requests Manager, select the cell labeled Created in the column labeled LugLoad if it is not already selected. At the bottom of the dialog box, click Delete and click Yes in the warning dialog box that appears. Click Dismiss to close the History Output Requests Manager.