Generating tabular data reports

In addition to the graphical capabilities described above, Abaqus/CAE allows you to write data to a text file in a tabular format. This feature is a convenient alternative to writing tabular output to the data (.dat) file. Output generated this way has many uses; for example, it can be used in written reports. In this problem you will generate a report containing the element stresses, nodal displacements, and reaction forces.

  1. From the main menu bar, select ReportField Output.
  2. In the Variable tabbed page of the Report Field Output dialog box, accept the default position labeled Integration Point. Click the triangle next to S: Stress components to expand the list of available variables. From this list, toggle on S11.
  3. In the Setup tabbed page, name the report Frame.rpt. In the Data region at the bottom of the page, toggle off Column totals.
  4. Click Apply.

    The element stresses are written to the report file.

  5. In the Variable tabbed page of the Report Field Output dialog box, change the position to Unique Nodal. Toggle off S: Stress components, and select U1 and U2 from the list of available U: Spatial displacement variables.
  6. Click Apply.

    The nodal displacements are appended to the report file.

  7. In the Variable tabbed page of the Report Field Output dialog box, toggle off U: Spatial displacement, and select RF1 and RF2 from the list of available RF: Reaction force variables.
  8. In the Data region at the bottom of the Setup tabbed page, toggle on Column totals.
  9. Click OK.

    The reaction forces are appended to the report file, and the Report Field Output dialog box closes.