1. 9.0 New Features Metal Shaft with Rubber Boot Workshop 7 Load Steps in Workbench

2. 9.0 New Features Workshop ANSYS v9.0 October 1, 2004 Inventory #002157 WS7-2 © 2004 ANSYS, Inc. Workbench Load Steps Problem Description A rubber boot surrounding a metal shaft is used to demonstrate the load step new feature available in the Workbench GUI at ANSYS version 9.0. Load Steps will be used to push the shaft down, then to the side. – In previous versions of Workbench, the user would have to insert commands to perform load step application. Now, the Workbench GUI supports load step definition and the viewing of results at each load step. The entire analysis will be shown: – Starting an empty project – Linking to the DesignModeler geometry file – Meshing – Contact – Hyperelastic and isotropic material properties – Solution options – Load Step Definition *** 9.0 NEW FEATURE *** – Inserting and viewing results

3. 9.0 New Features Workshop ANSYS v9.0 October 1, 2004 Inventory #002157 WS7-3 © 2004 ANSYS, Inc. Workbench Load Steps START > Programs > ANSYS 9.0 > ANSYS Workbench. Click on Empty Project Link to Geometry File > Browse to find DesignModeler file: BootwithShaft.agdb

4. 9.0 New Features Workshop ANSYS v9.0 October 1, 2004 Inventory #002157 WS7-4 © 2004 ANSYS, Inc. Workbench Load Steps Click on the link for New simulation Close the Simulation Wizard Set the units to be metric (mm, kg, N)

5. 9.0 New Features Workshop ANSYS v9.0 October 1, 2004 Inventory #002157 WS7-5 © 2004 ANSYS, Inc. Workbench Load Steps Mesh – Click on Mesh and look in the Details Change the Global Control from Basic to Advanced Slide the Curve/Proximity from 0 to 100 – Right Click on Mesh > Insert > Sizing Pick the Shaft body Enter an Element Size of 6mm – Right Click on Mesh > Preview Mesh.

6. 9.0 New Features Workshop ANSYS v9.0 October 1, 2004 Inventory #002157 WS7-6 © 2004 ANSYS, Inc. Workbench Load Steps Contact Creation – Rename contact Contact > Rename Based on Geometry You will now see the Contact Region renamed as “Boot to Shaft” – Automatic contact detection Automatic contact detection has found the contact between the shaft and the rubber boot. Some settings in the Details of “Boot to Shaft” need to be changed: –The automatic contact detection found two contact surfaces, deselect the conical surface –Definition > Behavior > Asymmetric –Advanced > Formulation > MPC – Manual contact creation When the boot is subjected to loading, two ribs of the boot come into contact with each other. Fortunately, we already know which ones will come into contact. Contact > Insert > Manual Contact Region –Definition > Type > Rough –Scope > Contact Bodies > Select the two contact faces shown in red (on middle rib) –Scope > Target Bodies > two target faces shown in blue (on bottom rib) –Definition > Behavior > Auto Asymmetric –Advanced > Update Stiffness > Each Equilibrium Iteration –Rename based on geometry > Contact region is named “Boot to Boot”

7. 9.0 New Features Workshop ANSYS v9.0 October 1, 2004 Inventory #002157 WS7-7 © 2004 ANSYS, Inc. Workbench Load Steps Material Properties – The Boot is to be modeled with hyperelastic material properties. Hyperelasticity can be used to analyze rubber-like materials (elastomers) that undergo large strains and displacements with small volume changes (nearly incompressible materials). This is done in Workbench by inserting the appropriate ANSYS commands. Here we will specify Mooney-Rivlin hyperelastic material properties: Right click on Boot > Insert Commands Enter the following commands: TB,HYPE,matid,1,2,mooney !Mooney-Rivlin Properties TBTEMP,0 !Temperature TBDATA,,1,0.1,1e-4 !Mooney-Rivlin Constants keyo,matid,6,1 !U-P Formulation for SOLID186 – Click on Boot and look in the details The material shown is Structural Steel, however this material definition will be deleted by the inserted commands. To help prevent volumetric mesh locking, change the Definition of the Brick Integration Scheme to Reduced. – The Shaft is aluminum In the details of Shaft, click on Structural Steel, then Import Aluminum Alloy.

8. 9.0 New Features Workshop ANSYS v9.0 October 1, 2004 Inventory #002157 WS7-8 © 2004 ANSYS, Inc. Workbench Load Steps The Boot is to be fixed at the bottom and constraints need to be applied on the plane of symmetry. Assign boundary conditions – Environment > Insert > Fixed Support Select the bottom surface of the Boot, shown in green in the plot – Environment > Insert > Frictionless Support Select the two surfaces of the Boot shown in purple in the plot.

9. 9.0 New Features Workshop ANSYS v9.0 October 1, 2004 Inventory #002157 WS7-9 © 2004 ANSYS, Inc. Workbench Load Steps Load Steps – The shaft is displaced downward, then to the side. This will be accomplished by using a Remote Displacement with two load steps. – Click on Environment In the toolbar, change the loading from Static to Sequence. In the Details of Environment, change the sequence steps from 1 to 2. – Insert remote displacement Select the bottom surface of the Shaft The graph at the bottom left of the screen shows what load step you are defining loads for, select load step 1. Load Step 1 –Push the Shaft down by setting the Y component to a value of –5mm. –Set the X and Z components to a value of zero mm. –Set the Rotation X, Y, and Z components to a value of 0 degrees. –Change the Behavior to Rigid Load Step 2 application on the next slide

10. 9.0 New Features Workshop ANSYS v9.0 October 1, 2004 Inventory #002157 WS7-10 © 2004 ANSYS, Inc. Workbench Load Steps – Remote displacement, cont’d Load Step 2 –Click on the “2” on the graph at the lower left of the screen. –Enter a value of –5 for Y displacement and a value of 25 degrees for rotation about Z. All other values continue to be set to zero. – Load steps can also be defined by clicking on the Worksheet tab and entering the data for each load step.

11. 9.0 New Features Workshop ANSYS v9.0 October 1, 2004 Inventory #002157 WS7-11 © 2004 ANSYS, Inc. Workbench Load Steps Set the solution options – Look in the details of Solution Change the Solver Type from Program Controlled to Direct Change Weak Springs from Program Controlled to Off Change Large Deflection from Off to On For Load Step 1, leave Auto Time Stepping as Program Controlled For Load Step 2, change Auto Time Stepping from Program Controlled to On –Set the Initial Substeps to 100 –Set the Minimum Substeps to 5 –Set the Maximum Substeps to 1000

12. 9.0 New Features Workshop ANSYS v9.0 October 1, 2004 Inventory #002157 WS7-12 © 2004 ANSYS, Inc. Workbench Load Steps Insert Results – Insert Solution Information Right Click on Solution > Insert > Solution Information – Show results for both load steps Right Click on Solution and insert Equivalent Stress –On the graph in the lower left portion of the screen, click on the “1” (for the first load step) –Scope the Results to the Boot body only –Rename this result as “Equivalent Stress Load Step 1” Right Click on Solution and insert Equivalent Stress –On the graph in the lower left portion of the screen, click on the “2” (for the second load step) –Scope the Results to the Boot body only –Rename this result as “Equivalent Stress Load Step 2” Repeat for Total Deformation –Name these results “Total Deformation Load Step 1” and “Total Deformation Load Step 2” –These results can be shown for both the Boot and the Shaft together

13. 9.0 New Features Workshop ANSYS v9.0 October 1, 2004 Inventory #002157 WS7-13 © 2004 ANSYS, Inc. Workbench Load Steps Insert Results, cont’d – Right Click on Solution > Insert > Contact Tool > Contact Tool – In the details of Contact Tool, pick the 4 rib faces that were selected for “Boot to Boot” contact Below Contact Tool, select Status, define and name it for Load Step 1 Repeat for Load Step 2 Also, insert Contact Pressure for Load Steps 1 and 2

14. 9.0 New Features Workshop ANSYS v9.0 October 1, 2004 Inventory #002157 WS7-14 © 2004 ANSYS, Inc. Workbench Load Steps The analysis is ready to be solved. However, this takes some time, so if you want to skip to the results then open the BootwithShaft_Solved.dsdb file. If you choose to solve the analysis, while it is solving view the Solution Information > Solver Output in the Worksheet tab.

15. 9.0 New Features Workshop ANSYS v9.0 October 1, 2004 Inventory #002157 WS7-15 © 2004 ANSYS, Inc. Workbench Load Steps View the Equivalent Stress Results for each load step

16. 9.0 New Features Workshop ANSYS v9.0 October 1, 2004 Inventory #002157 WS7-16 © 2004 ANSYS, Inc. Workbench Load Steps View the Total Deformation Results for each load step

17. 9.0 New Features Workshop ANSYS v9.0 October 1, 2004 Inventory #002157 WS7-17 © 2004 ANSYS, Inc. Workbench Load Steps View the contact status and pressure for load step 2