Mechanical APDL Structural Analysis Guide

5. The Define Nodal Data dialog appears. Be sure the Ref number of variable and Node number are both
   set to 2. Enter TIPLATDI in the “User-specified label” field. Select Translation UZ from the menu and click
   OK.


6. Define the total reaction force to be read from the results file. Select Add from the Defined Time-History
   Variables dialog.


7. When the Add Time-History Variable dialog appears, choose the Reaction forces radio button and then
   click OK.


8. The Define Reaction Force picker appears. Pick the end node on the left side of the beam and click OK.


9. The Define Reaction Force Variable dialog appears. Be sure the “Ref number of variable” is set to 3 and
   “Node number” is set to 1. Select “Struct Force FY” from the menu and click OK. Click Close to close the
   Defined Time-History Variables dialog.


10. Choose menu path Main Menu> TimeHist Postpro> Math Operations> Multiply. In the Multiply Time-
    History Variables dialog, enter 4 in the “Reference number for result” field, -1.0 in the “1st Factor” field,
    and 3 in the “1st Variable” field. Click OK.


11. Display the X variable. Choose menu path Main Menu> TimeHist Postpro> Settings> Graph. Choose
    the single variable button, enter 2 in the “Single variable no.” field, and click OK.


12. Plot the load versus deflection curve to confirm the critical load calculated by the eigenvalue method.
    Choose menu path Main Menu> TimeHist PostPro> Graph Variables. Enter 4 in the “1st variable to
    graph” field. Click OK.

13.List the variables versus time. Choose menu path Main Menu> TimeHist PostPro> List Variables. Enter
2 in the “1st variable to list” field and 4 in the “2nd variable” field and click OK.

14. Check the values in the PRVAR Command window to see how they compare against the values generated
    by the eigenvalue buckling analysis. Expected results are: Critical buckling load, Pcr = 0.01892. Close the
    PRVAR Command window.

15.7.13. Plot and Review the Section Results

1. Replot the beam. Choose menu path Utility Menu> Plot> Elements.


2. Define the compression stress at the base to be read from the results file. Choose menu path Main
   Menu> TimeHist PostPro> Define Variables. When the Defined Time-History Variables dialog appears,
   select Add.


3. When the Add Time-History Variable dialog appears, be sure the “...by seq no.” option is selected. Click
   OK.


4. The Define Element Results picker appears. In the Graphics window, pick element 1 (the end element
   on the left side of the beam) and click OK.


5. The Define Element Results by Seq No. dialog appears. Be sure the Ref number of variable is set to 5 and
   Element number is set to 1. Enter BASESX in the “User-specified label” field. Select “LS” from the menu.


6. To retrieve the X component of Stress from the bottom middle of the section (this is node 3, or the 2nd
   node where stress is stored), type 4 for the Comp Sequence number and click OK.

Release 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information

Example Lateral Torsional Buckling Analysis