Modifying field output requests

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.

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.

• 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 select the substructure sets for which you want to write field data. Select multiple sets by using the Ctrl or Shift keys while clicking on set names. You can use the name filter to show only substructure sets that match a specified pattern, such as belonging to a particular substructure part instance.

• 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.

• 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 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, 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.

• Select Integration points to request field output at the integration points where they are calculated (this is the default).

• Select Centroidal to request field output at the centroid of each element.

• Select Nodes to request field output at the node of each element.

• Select Averaged at nodes to request field output extrapolated to the nodes of each element and then averaged with the values from surrounding elements that have the same type of properties.

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.

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 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.

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.

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 The Filter toolset.