Mechanical APDL Structural Analysis Guide

3. Click on Def + undef edge for items to be plotted. Click OK.The deformed mesh appears in the Graphics
   window.


4. Choose menu path Main Menu> General Postproc> Plot Results> Contour Plot> Element Solu. The
   Contour Element Solution Data dialog box appears.


5. In the selection box on the left, choose Strain-plastic. In the selection box on the right, choose Eqv plastic
   EPEQ. Click OK.The contour plot appears in the Graphics window.


6. Choose Utility Menu> Plot> Elements.

8.13.3.16. Define Variables for Time-History Postprocessing

1. Choose menu path Utility Menu> Select> Entities. The Select Entities dialog box appears.


2. Verify that Nodes and By Num/Pick are selected in the first two boxes. Click OK.The Select nodes picking
   menu appears.


3. Type "ntop" in the picker and press RETURN. Click OK.


4. Choose menu path Utility Menu> Select> Entities. The Select Entities dialog box appears. Choose Ele-
   ments in the first drop-down selection box. Choose Attached to in the second drop-down selection box.
   Verify that Nodes is selected. Click OK.


5. Choose Utility Menu> Select> Everything.


6. Choose Main Menu> TimeHist Postpro> Define Variables. The Defined Time-History Variables dialog
   box appears. Click on Add. The Add Time-History Variable dialog box appears.


7. Click on Element results. Click OK.The Define Elemental Data picking menu appears.


8. Click on the top left element in the Graphics window. Click OK on the picking menu. The Define Nodal
   Data picking menu appears.


9. Click on the top left node of the top left element. Click OK on the picking menu. The Define Element
   Results Variable dialog box appears.


10. Verify that the reference number of the variable is 2.


11. Choose Stress in the selection list on the left. Choose Y-direction SY in the selection list on the right.
    Click OK.The Defined Time-History Variables dialog box reappears, with a second variable listed (ESOL).
    The dialog box should show element number 281, node number 50, item S, component Y, and name
    SY.


12. Click on Add. Repeat steps 7-10, with variable reference number 3.

13.In the Define Element Results Variable dialog box, choose Strain-elastic in the selection list on the left.
Choose Y-dir'n EPEL Y in the selection list on the right. Click OK.

14. Click on Add. Repeat steps 7-10, with variable reference number 4.

15.In the Define Element Results Variable dialog box, choose Strain-plastic in the selection list on the left.
Choose Y-dir'n EPPL Y in the selection list on the right. Click OK.

16. Click on Close on the Defined Time-History Variables dialog box.

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

Nonlinear Structural Analysis