Creating and Modifying Field Output Requests
Field output is the output of variables that are written relatively infrequently to the output database. Typically, you request field output for your entire model or for a large region. Each Abaqus for CATIA V5 analysis case contains a default field output request for each type of step in the analysis. The default request is created in the first step of each step type and writes output to the output database (.odb) file when you run the analysis. The field output requests created in a step are propagated to all subsequent steps of the same step type. Field output requests generate the data used to produce Abaqus results images (see Visualizing Results).
By default, output is requested from every node or integration point and from the default section points for the entire model. The default set of output variables corresponds to the step type (see Table 4–2); these variables are written by default at every increment.
Table 4–2 Default output variables.
| Step Type | Default Output |
|---|---|
| General Static | Stresses, strains, plastic strains, equivalent plastic strains, plastic strain magnitudes, displacements, reaction forces, point loads and concentrated moments, contact pressures and frictional shear stresses, contact openings and relative tangential motions, and the element energy density error |
| Static Linear Perturbation | Stresses, strains, displacements, reaction forces, point loads, concentrated moments, and the element energy density error |
| Frequency | Displacements |
| Riks | Stresses, strains, plastic strains, equivalent plastic strains, plastic strain magnitudes, displacements, reaction forces, point loads and concentrated moments, contact pressures and frictional shear stresses, contact openings and relative tangential motions, and the element energy density error |
| Heat Transfer | Heat flux per unit area, nodal temperatures, and reaction flux values |
| Explicit Dynamics | Stresses, strains, plastic strains, equivalent plastic strains, displacements, reaction forces, contact stresses, velocities, and accelerations |
You can use the 
tool to create new field output requests, and you can use the field output editor to modify new or existing field output requests—including the default requests—either in the step in which they were created or a step to which they were propagated. If you modify a propagated field output request, you can modify only the output variables and the output frequency.
Field output requests are contained in a Field Output Request object under the Field Output Requests objects set for the step.
To create or modify a field output request:
To create a new field output request, click
.To edit an existing field output request, double-click on the Field Output object under the Field Output Requests objects set for the analysis step.
The Edit Field Output Request dialog box is displayed.
If you edit the output request in the step in which it was created, you can change the name of the output request.
If you edit the output request in the step in which it was created, you can change the region for which variables will be output.
To request that Abaqus write field data to the output database for the entire model, toggle on Whole model from the Support section at the top of the dialog box.
To select a smaller region, toggle off Whole model and select a new model region from the viewport or from the specification tree. You can also select surface groups.
In the Output Variables section of the editor, choose one of the following variable selection methods:
Preselected defaults
Choose this method to allow Abaqus to select a preselected (default) set of output variables appropriate for the step type.
All
Choose this method to automatically select all of the allowable output variables within each variable category in the list.
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:
From the list of variables, select the variables of your choice.
For categories with multiple selections, you can select individual variables or toggle the desired variable category to select or deselect all variables within that category.
Additional variables
When you use Select from list below, you can type a comma-separated list of variables to be appended to the selection list.
Click More to edit the section points and frequency of field output or to view the propagation and activation status for the output request.
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 for shells and beams. The section points that you select can significantly affect the results, for example, a shell with an applied bending load is under tension on one side, compression on the other, and neutral at the center. 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. (The default section points are usually the outer fibers of the section.)
All
Choose All to request that Abaqus write field data for all section points to the output database.
Specify
Choose Specify to manually type the section points for which Abaqus will write field data to the output database.
Specify the desired output frequency in the Save Output At area.
For a Nonlinear Structural or Thermal case, you can request output Every __ increments (the default) and select the number of increments, or you can request output for only the last increment. If you specify the frequency in increments, Abaqus also writes output for the last increment of the step.
For a frequency step in a Nonlinear Structural case, you can request output of All modes (the default), or you can Specify individual modes and enter the desired modes.
For an Explicit Dynamics case, you can specify the output frequency in Equally spaced intervals (the default), Every __ units of time, or Every __ increments; and enter the desired number of intervals, time units, or increments.
For more information, see Output to the output database in the Abaqus Output Guide.
If you chose equally spaced intervals or units of time for the output frequency in an Explicit Dynamics case, you can specify whether output is saved approximately or exactly at the specified times or intervals.
The propagation and activation status are provided for information only; you cannot edit them from the Field Output Request dialog box. You can edit the activation status from the specification tree.
See Status Terms for information on the terms used to describe the propagation and activation status and for instructions on changing the activation status.
When you have finished defining the output request, click OK to save your changes.