Mechanical APDL Structural Analysis Guide

9. In the scroll box for Variable to redefine, scroll to "Variable 2" and select it. In the scroll box for
   Quantity to be monitored, scroll to "FY" and select it. Click OK.

8.13.3.11. Apply Constraints

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


2. Select Nodes and By Location in the first two selection boxes. Verify that X coordinates are selected, and
   enter "radius" in the Min, Max field. Click OK.


3. Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On
   Nodes. The Apply U,ROT on Nodes picking menu appears.


4. Click Pick All. The Apply U,ROT on Nodes dialog box appears.


5. Click on "All DOF" for DOFs to be constrained. Click OK.


6. Choose menu path Utility Menu> Select> Entities. The Select Entities dialog box appears. Verify that
   Nodes, By Location, and X coordinates are selected. Enter "0" in the Min, Max field and click OK.This action
   selects the nodes at the X=0 position.


7. Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Displacement> On
   Nodes. The Apply U,ROT on Nodes picking menu appears.


8. Click Pick All. The Apply U,ROT on Nodes dialog box appears.


9. Click on "UX" for DOFs to be constrained. Click on All DOF to deselect it.


10. Enter "0.0" as the Displacement value. Click OK.


11. Choose menu path Utility Menu> Select> Entities. The Select Entities dialog box appears. Verify that
    Nodes and By Location are selected.


12. Click on Y coordinates and enter "thick" in the Min, Max field. Click OK.


13. Choose menu path Main Menu> Solution> Define Loads> Apply> Structural> Pressure> On Nodes.
    The Apply PRES on Nodes picking menu appears.


14. Click on Pick All. The Apply PRES on nodes dialog box appears.


15. Enter "0.125" in the Load PRES value field and click OK.


16. Choose menu path Utility Menu> Select> Everything.


17. Click on SAVE_DB on the Toolbar.

8.13.3.12. Solve the First Load Step

1. Choose menu path Main Menu> Solution> Load Step Opts> Time/Frequenc> Time and Substps. The
   Time and Substep Options dialog appears.


2. Enter 10 as the number of substeps, enter 50 as the maximum number of substeps, and enter 5 as the
   minimum number of substeps. Click OK.


3. Choose menu path Main Menu> Solution> Solve> Current LS. Review the information in the /STAT
   window, and click on Close.

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

Nonlinear Structural Analysis