Now that you have created your part, you can define your analysis steps. For the cantilever beam tutorial the analysis will consist of two steps:
An initial step, in which you will apply a boundary condition that constrains one end of the cantilever beam.
A general, static analysis step, in which you will apply a pressure load to the top face of the beam.
Create a general, static step that follows the initial step of the analysis.
To create a general, static analysis step:
In the Model Tree, double-click the Steps container to create a step.
ABAQUS/CAE switches to the Step module. The Create Step dialog box appears with a list of all the general procedures and a default step name of Step-1. General procedures are those that can be used to analyze linear or nonlinear response.
Name the step BeamLoad.
From the list of available general procedures in the Create Step dialog box, select Static, General if it is not already selected and click Continue.
The Edit Step dialog box appears with the default settings for a general, static step.
The Basic tab is selected by default. In the Description field, type Load the top of the beam.
Click the Incrementation tab, and accept the default time incrementation settings.
Click the Other tab to see its contents; you can accept the default values provided for the step.
Click OK to create the step and to exit the Edit Step dialog box.
When you submit your job for analysis, ABAQUS/Standard or ABAQUS/Explicit writes the results of the analysis to the output database. For each step you create, you can use the Field Output Requests Manager and the History Output Requests Manager to do the following:
Select the region of the model for which ABAQUS will generate data.
Select the variables that ABAQUS will write to the output database.
Select the section points of beams or shells for which ABAQUS will generate data.
Change the frequency at which ABAQUS will write data to the output database.
For the cantilever beam tutorial, you will simply examine the output requests and accept the default configuration.
To examine your output requests:
In the Model Tree, click mouse button 3 on the Field Output Requests container and select Manager from the menu that appears.
ABAQUS/CAE displays the Field Output Requests Manager. This manager displays an alphabetical list of existing output requests along the left side of the dialog box. The names of all the steps in the analysis appear along the top of the dialog box in the order of execution. The table formed by these two lists displays the status of each output request in each step.
Review the default output request that ABAQUS/CAE generates for the Static, General step you created and named BeamLoad.
Click the cell in the table labeled Created; that cell becomes highlighted, and the following information related to the cell appears in the legend at the bottom of the manager:
The type of analysis procedure carried out in the step in that column.
The list of output request variables.
The output request status.
On the right side of the Field Output Requests Manager, click Edit to view more detailed information about the output request.
The field output editor appears. In the Output Variables region of the dialog box, a text box lists all the variables that will be output. If you change an output request, you can always return to the default settings by clicking Preselected defaults above the text box.
Click the arrows next to each output variable category to see exactly which variables will be output. The check boxes next to each category title allow you to see at a glance whether all variables in that category will be output. A black check mark on a white background indicates that all variables will be output, while a dark gray check mark on a light gray background indicates that only some variables will be output.
Based on the selections shown at the bottom of the dialog box, data will be generated at every default section point in the model and will be written to the output database after every increment during the analysis.
Click Cancel to close the field output editor, since you do not wish to make any changes to the default choice.
Click Dismiss to close the Field Output Requests Manager.
Note: What is the difference between the Dismiss and Cancel buttons? Dismiss buttons appear in dialog boxes that contain data that you cannot modify. For example, the Field Output Requests Manager allows you to view output requests, but you must use the field output editor to modify those requests. Clicking the Dismiss button simply closes the Field Output Requests Manager. Conversely, Cancel buttons appear in dialog boxes that allow you to make changes. Clicking Cancel closes the dialog box without saving your changes.
Review the history output requests in a similar manner by clicking mouse button 3 on the History Output Requests container in the Model Tree and then opening the history output editor.