To modify a field output request:

1. From the main menu bar, select OutputField Output RequestManager.

   Abaqus/CAE displays the Field Output Requests Manager. The manager indicates in which step the output request was created and into which steps it was propagated.

2. From the list of field output requests in the manager, select the step in which you want to modify the request.

3. From the buttons on the right side of the Field Output Requests Manager, click Edit.

   Abaqus/CAE displays the Edit Field Output Request editor. Information at the top of the editor indicates the following:

   • The name of the output request.

   • The name of the step in which you are editing the output request.

   • The analysis procedure associated with the step.

4. If you edit the output request in the step in which it was created, you can change the region from which variables will be output. From the top of the editor, click the arrow next to the Domain text field and select one of the following:

   • Select Whole model to request that Abaqus write field data to the output database for the entire model. Toggle on Exterior only to request output only on the exterior nodes and elements; this option is applicable only for three-dimensional models in an Abaqus/Standard or Abaqus/Explicit analysis.

   • Select Set to request that Abaqus write field data to the output database for only the named region that you specify. Click the arrow, and select the name from the list of sets that appears.

   • Select Bolt load to request that Abaqus write field data to the output database for only the bolt load that you specify. Click the arrow, and select the name from the list of bolt loads that appears.

   • Select Composite layup to request that Abaqus write field data to the output database for only the plies in the composite layup that you specify. Click the arrow, and select the name from the list of composite layups that appears.

   • Select Fastener to request that Abaqus write field data to the output database for only the fastener that you specify. Click the arrow, and select the name from the list of fasteners that appears.

   • Select Substructure to request that Abaqus write field data to the output database for only the substructure sets that you specify. Click to open the Select Substructure Sets dialog box, then toggle on the substructure sets in each substructure part instance for which you want to write field data. If you want to write field data for all of the sets in a particular substructure part instance, toggle on its Entire Substructure option.

   • Select Interaction to request that Abaqus write field data to the output database for only the interaction that you specify. Click the arrow, and select the name from the list of surface-to-surface contact and self-contact interactions that appears.

   • Select Skin to request that Abaqus write field data to the output database for only the skin reinforcement that you specify. Click the arrow, and select the name from the list of skins that appears.

   • Select Stringer to request that Abaqus write field data to the output database for only the stringer reinforcements that you specify. Click the arrow, and select the name from the list of stringers that appears.

5. Specify the desired output frequency:

   • Select Last increment to request field output for the last increment only. This output frequency is available only when you choose an Abaqus/Standard analysis procedure.

   • Select Every n increments to request that Abaqus write field data to the output database in increments. You can then specify the number of increments in the n field that appears. If you specify the frequency in increments, Abaqus also writes output after the last increment of the step. This output frequency is available when you choose an Abaqus/Standard or Abaqus/CFD analysis procedure.

   • Select Every time increment to request that Abaqus write field data to the output database at every time increment. This output frequency is available only when you choose an Abaqus/Explicit analysis procedure.

   • Select Evenly spaced time intervals to request that Abaqus write field data to the output database at a number of evenly spaced time intervals. You can then specify the number of intervals in the Intervals field that appears.

   • Select Every x units of time to request that Abaqus write field data to the output database every time a particular length of time elapses. You can then specify the length of time in the x field that appears.

   • Select From time points to request that Abaqus write field data to the output database according to a set of time points. You can then select a set of time points from the Time Points list that appears or click to create a new set of time points. See “Defining time points,” Section 14.13.5, for more information about creating a set of time points. This output frequency is available when you choose an Abaqus/Standard or Abaqus/Explicit analysis procedure.

6. If you requested output at Evenly spaced time intervals, Every x units of time, or From time points, you can also select Output at exact times from the Timing field to alter the time incrementation size to match the time intervals exactly.

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

   Select from list below

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

   • Click the arrow next to the desired variable category. From the list of variables that appears, select the variables of your choice.

   • Toggle the desired variable category. This action selects or deselects all variables within that category.

   The check box next to a variable category becomes completely filled when all variables within that category are selected. The box becomes half filled if only some of the variables within that category are selected.

   Preselected defaults

   Choose this method to allow Abaqus/CAE to select a preselected (default) set of output variables appropriate for the step's analysis procedure.

   All

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

   Edit variables

   Choose this method to enter or delete output variables in the text field located above the list of variable categories.

   Note:  In addition to the current analysis procedure, other aspects of the model may affect the preselected default output variables. For example, if a selected output variable is valid for the analysis procedure but is not valid for the element type used in the mesh, Abaqus will remove that variable during the analysis.

8. If your domain is set to Whole model, Set, Skin, or Stringer, do the following:

   1. If your model contains rebar and you edit the output request in the step in which it was created, you can include output for rebar in the field data that Abaqus writes to the output database. From the bottom of the editor, toggle on Output for rebar and choose one of the following options that appears:

      Include

      Choose Include to request that Abaqus write output for rebar in addition to output for the underlying material to the output database.

      Only

      Choose Only to request that Abaqus write only output for rebar to the output database.

      If you want to view rebar orientations in the Visualization module, you must toggle on Output for rebar.

   2. 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. From the bottom of the editor, choose one of the following:

      Use defaults

      Choose Use defaults to request that Abaqus write field data to the output database from the default section points. Abaqus chooses the default section points based on the section selected in the Property module. (The default section points are usually the outer fibers of the section.) For more information see Chapter 12, “The Property module.”

      Specify

      Choose Specify to enter the section points for which Abaqus will write field data to the output database. The specified section points are used only during the selected output request; Abaqus reverts to the default section points for subsequent output requests.

   3. Toggle off Include local coordinate directions when available to reduce the size of the output database by excluding material orientations from the saved data.

9. If your domain is set to Bolt load or Interaction, toggle off Include local coordinate directions when available to reduce the size of the output database by excluding material orientations from the saved data.

   Note:  If you exclude local coordinate directions from the output database, Abaqus/CAE displays all analysis results from the output database in the default coordinate system.

10. If your domain is set to Composite layup, specify the section points from which variables will be output. For more information, see “Requesting output from a composite layup,” Section 23.5.

    Note:  By default, Abaqus/CAE writes field output data from only the top and bottom of a composite layup, and no data from the plies are generated. Therefore, if your model contains a composite layup and you want data from individual plies, you must create a new output request or edit the default output request and specify the section points from which variables will be output.

    From the bottom of the editor, choose one of the following:

    Selected

    Choose Selected points for each ply to request that Abaqus write field data to the output database from the top, middle, and/or bottom section point of each ply in the selected composite layup.

    All

    Choose All section points in all plies to request that Abaqus write field data to the output database from all of the section points of all of the plies in the selected composite layup.

    Specify

    Choose Specify to enter the section points for which Abaqus will write field data to the output database. Section points are numbered sequentially from the top of the first ply to the bottom of the last ply. The specified section points are used only during the selected output request; Abaqus reverts to the default section points for subsequent output requests.

11. If you edit the output request for an Abaqus/Explicit analysis procedure in the step in which it was created, you can apply a filter to remove high frequency data from the field output.

    From the bottom of the editor, toggle on Apply filter and choose the default Antialiasing filter or select a named filter that was created using the Filter toolset. For more information, see Chapter 66, “The Filter toolset.”

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