Modifying history output requests

From the main menu bar, select OutputHistory Output RequestManager.

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

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

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

Abaqus/CAE displays the Edit History 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.

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 history data to the output database for the entire model.
Select Set to request that Abaqus write history 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 history 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 history 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 Contour integral to request that Abaqus write history data to the output database for only the contour integral that you specify. Click the arrow, and select the name from the list of contour integrals that appears.

When you request output from a contour integral, the History Output Request editor allows you to select only the frequency of output, the number of contour integrals, and the type of contour integral calculation. For more information, see Requesting contour integral output.
Select Fastener to request that Abaqus write history 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 General contact surface to request that Abaqus write history data to the output database for only the general contact surface that you specify (this option is available only for Abaqus/Explicit analyses). Click the arrow, and select the surface from the list of surfaces that appears. History output will be written only for surfaces within the general contact domain.
Select Integrated output section to request that Abaqus write history data to the output database for only the integrated output section that you specify. Click the arrow, and select the name from the list of sections that appears. See Defining integrated output sections, for information on creating an integrated output section.
Select Interaction to request that Abaqus write history 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 history 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 Spring/Dashpot to request that Abaqus write history data to the output database for only the springs/dashpots that you specify. Click the arrow, and select the name from the list of springs/dashpots that appears.
Select Stringer to request that Abaqus write history 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.

Specify the desired output frequency:

Select Last increment to request history 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 history 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 n time increments to request that Abaqus write history data to the output database in time increments. You can then specify the number of time increments in the n field that appears. This output frequency is available only when you choose an Abaqus/Explicit analysis procedure.
Select Evenly spaced time intervals to request that Abaqus write history 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 history 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 history 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 only when you choose an Abaqus/Standard analysis procedure.

If you selected an Abaqus/Standard analysis procedure and 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.

From the Output Variables field, choose the variables and variable components to output:

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:

In the top half of the editor, click the arrow next to the desired variable category. From the list of variables that appears, select the variables of your choice. If a variable of interest has components, click the arrow next to the variable and select the components of interest. To select or deselect all components of a variable, toggle the variable itself.
Toggle the desired variable category to select or deselect all variables and variable components within that category.

The check box next to a variable category name becomes completely filled when all variables within that category are selected as well as all of the components of those variables. The box becomes half filled if only some of the variables or variable components within that category are selected. Likewise, the check box next to a variable name becomes completely filled when all components of that variable are selected. The box becomes half filled if only some of the components of that variable are selected.

Preselected defaults

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

All

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

Edit variables

Choose this method to enter or delete output variables and components 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 an 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.

If you want to include sensor output, toggle on Include sensor when available. This option is available when the domain Set is selected.

Toggle Use global directions for vector-valued output. This option is available when the domain Set is selected.

When Use global directions for vector-valued output is on, nodal history output is requested in the global directions.

When Use global directions for vector-valued output is off, nodal history output is requested in the local directions defined by nodal transformations.

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

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.
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.

If your domain is set to Composite layup, specify the section points from which variables will be output.

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.
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.
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. For example, if you have three plies, each with three section points, and you want output from the middle section point of each ply, you would enter 2,5,8. The specified section points are used only during the selected output request; Abaqus reverts to the default section points for subsequent output requests.

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 history 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 The Filter toolset.

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