Viewing the analysis of a meshed beam cross-section

This example illustrates how you can view the results of a meshed beam cross-section analysis that was generated using Timoshenko beams, as described in Meshed beam cross-sections. Before you execute the example script, you must run two analyses that create the following output database files:

  • An output database generated by the two-dimensional cross-section analysis. The script reads cross-section data, including the out-of-plane warping function, from this output database.

  • An output database generated by the beam analysis. The script reads generalized section strains (SE) from this output database.

Use the following command to retrieve the example script:

abaqus fetch job=compositeBeam

You must run the script from Abaqus/CAE by selecting FileRun Script from the main menu bar. The script uses getInputs to display a dialog box that prompts you for the name of the output databases generated by the two-dimensional cross-section analysis and by the beam analysis. The names are case-insensitive, and you can omit the .odb file suffix. The files must be in the local directory. The dialog box also prompts you for the following:

  • The name of the step

  • The increment or mode number (for a frequency analysis)

  • The name of the load case (if any)

  • The name of the part instance

  • The element number

  • The integration point number

If you do not enter a value in a field, the script looks in the beam analysis output database for possible values. The script then enters a default value in the dialog box and displays information about the range of possible values in the Abaqus/CAE message area. You can leave the load case field blank if the analysis did not include load cases. The script does not continue until all the values in the dialog box are acceptable. The same values are written to a file called compositeBeam_values.dat in the local directory, and these values appear as defaults in the dialog box the next time you run the example script.

After the getInputs method returns acceptable values, the script reads the two output databases and writes the generated data back to the output database created by the two-dimensional cross-section analysis. The script then displays an undeformed contour plot of S11 and uses the getInputs method again to display a dialog box with a list of the available stress and strain components (S11, S22, S33, E11, E22, and E33). Click OK in this dialog box to cycle through the available components. Click Cancel to end the script. You can also select the component to display by starting the Visualization module and selecting ResultField Output from the main menu bar.

The example script writes new stress and strain fields. The script must provide a unique name for the generated field output because each of these fields is generated for a specific beam analysis output database and for a specific part instance, step, frame, element, and integration point. The script constructs this unique name as follows:

  • All contour stress and strain fields for a specific beam analysis output database are written to a new frame, where the description of the frame is the name of the output database. For example, for a beam analysis output database called beam_run17.odb, the frame description is Beam ODB: beam_run17.

  • The field name is assembled from a concatenation of the step name, frame index, instance name, element, and integration point, followed by E or S. For example, Step-1_4_LINEARMESHED_12_1_E. Any spaces in a step or instance name are replaced by underscores.

You can run the script many times; for example, to create contour data for a particular step, increment, and integration point along each element of the beam. In this case you would also use ResultField Output to select which element to display.

The contour data generated by the example script are written back to the output database that was originally created by the two-dimensional, cross-section analysis. If you want to preserve this database in its original form, you must save a copy before you run the example script.