Mechanical APDL Structural Analysis Guide

15.7.11. Solve the Nonlinear Buckling Analysis

1. Introduce model imperfections calculated by the previous analysis. Choose menu path Main Menu>
   Preprocessor> Modeling> Update Geom. In the Update nodes using results file displacements dialog,
   enter 0.002 in the “Scaling factor” field, 1 in the “Load step” field, 1 in the “Substep” field, and file.rst
   in the “Selection” field. Click OK.


2. Choose menu path Main Menu> Solution> Analysis Type> New Analysis.


3. Select the "Static" option, then click OK.


4. Choose menu path Main Menu> Solution> Load Step Opts> Output Ctrls> DB/Results File and be
   sure the drop down lists display All Items and All entities respectively. Choose the Every substep for the
   File write frequency radio button and click OK.


5. Choose menu path Main Menu> Solution> Analysis Type> Analysis Options. Select the radio button
   beside Large deform effects, then click OK.


6. Set the arc-length method, and set parameters for the termination of the solution. Choose menu path
   Main Menu> Solution> Load Step Opts> Nonlinear> Arc-Length Opts. Select the Arc-length method
   on/off radio button and set it to On. Choose the pull down menu next to the Lab label and select Dis-
   placement lim. Enter 1.0 in the “Max desired U” field. Enter 2 in the “Node number for VAL” field. From
   the pull-down menu (next to the “Degree of freedom” label), select “UZ.” Click OK.


7. Define the number of substeps to be run during this load step. Choose menu path Main Menu> Solution>
   Load Step Opts> Time/Frequenc> Time and Substps. Enter 10000 in the “Number of substeps” field
   and click OK.


8. Solve the current model. Choose menu path Main Menu> Solution> Solve> Current LS. Review the
   summary information in the /STATUS command window, then select Close from its menu bar. Click OK
   in the Solve Current Load Step window to begin the solution. A Nonlinear Solution window with a Stop
   button appears. A convergence graph is built, and can take several minutes to complete.


9. You may receive a warning message. You should review the information in the message but you do not
   need to close it. Continue waiting for the solution to complete. When the Solution is Done! window ap-
   pears, click Close to close it.


10. Choose menu path Main Menu> Finish.

15.7.12. Plot and Review the Results

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


2. Define the load point deflection 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 Nodal DOF result option is selected.
   Click OK.


4. The Define Nodal Data picker appears. In the Graphics window, pick node 2 (the end node on the right
   side of the beam) and click OK.

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

Beam Analysis and Cross Sections