OS-SL-T: 1000 Nonlinear Analysis of Rubber Ring

This tutorial demonstrates the creation of finite elements on a given CAD geometry of a rubber ring.

Before you begin, copy the file(s) used in this tutorial to your working directory.

Application of boundary conditions and a finite element analysis of the problem are explained. Post-processing tools are used to determine stress developed during crushing and sliding of a rubber ring.

The following exercises are included:
  • Set up the problem in SimLab
  • Apply Loads and Boundary Conditions
  • Solve the job
  • View the results

Launch SimLab

Launch SimLab.

Import the Model

  1. From the menu bar, click File > Import > Database.
    An Import File dialog opens.
  2. Select the Rubber_Ring.gda file you saved to your working directory from the Rubber_Ring.zip file.
  3. Click Open.
    The Rubber_Ring.gda database is loaded into SimLab. The .gda file only contains geometric data.

Create Solution

  1. From the Solutions ribbon, Physics group, click the Structural tool.
    A Create Solution dialog opens.
  2. In the Create Solution dialog, define the following options:
    1. For Name, enter Rubber_Ring
    2. For Solver, select OptiStruct.
    3. For Solution type, select Non Linear Static.
    4. For Select bodies, select all the bodies from the Model Browser and click OK.
      Figure 1. Solution Creation


In the Solutions tab of the Model Browser, an OptiStruct – Non Linear Static solution with the selected bodies is created.
Figure 2. Solution defined in Solutions Browser


Set up the Model

Import Material

  1. In the Property tab of the Model Browser, right-click on Materials and select Import from the context menu.
  2. In the Open dialog, select the Rubber_Material.xml file and click Open.
    The Rubber_Material and respective data tables is added to the current materials list.
  3. From the Analysis ribbon, Property group, click the Material tool.
    A Material dialog opens.
  4. Enter the values, as shown below and click OK.
    Figure 3. Creating Rigid Material


Create Properties

  1. From the Analysis ribbon, Property group, click the Property tool.
    A Analysis Property dialog opens.
  2. In the Analysis Property dialog, enter the values shown below.
    Figure 4. Create Rubber_Ring Property


  3. Assign property to Ring.
    1. In the Assembly tab of the Model Browser, select Ring.
    2. In the Analysis Property dialog, click Apply.
    Figure 5. Assign Property to Ring


  4. Create a property for Top and Bottom Ends.
    1. Enter the values in the Analysis Property dialog, as shown below.
    2. In the Assembly tab of the Model Browser, select Top & Bottom Ends.
    3. In the Analysis Property dialog, click Apply.
    Figure 6. Assign Property to Top & Bottom End


  5. Create property for RBEs.
    1. Enter the values in the Analysis Property dialog, as shown below.
    2. In the Assembly tab of the Model Browser, select Top RBE and End RBE.
    3. In the Analysis Property dialog, click Apply.
    Figure 7. Assign Property to RBEs


The created Materials and Properties are listed in the Property tab of the Model Browser.

Set Up Loads and Constraints

Create Contacts

Contacts are created between the Ring and End Faces to simulate the Compressing and Sliding action of the ring against the Top and Bottom Ends.

  1. From the Analysis ribbon, Loads and Constraints group, click the Contact tool.
    A Define Contact dialog opens.
  2. In the Define Contact dialog, set the parameters as shown below.
    Figure 8. Contact Creation between Top End and Ring


  3. In the Define Contact dialog, select the line edit field for Main faces.
    The line edit field is highlighted.
  4. In the modeling window, select the Top End faces.
    Figure 9. Main Face Inputs for Contact Creation


  5. In the Define Contact dialog, select the line edit field for Secondary faces.
    The line edit field is highlighted.
  6. In the modeling window, select the Outer Ring faces.
    Figure 10. Secondary Face Inputs for Contact Creation


  7. In the Define Contact dialog, click Apply.
    The contact will be created and added to the Solution tab in the Model Browser.
  8. Create a contact between Bottom End & Ring.
    1. Set the following parameters in the Define Contact dialog, as shown below.
      Figure 11. Contact Creation between Bottom End and Ring


    2. In the Define Contact dialog, select the line edit field for Main faces.
      The line edit field is highlighted.
    3. In the modeling window, select the Bottom End faces.
      Figure 12. Main Face Inputs for Contact Creation


    4. In the Define Contact dialog, select the line edit field for Secondary faces.
      The line edit field is highlighted.
    5. In the modeling window, select the outer Ring faces.
      Figure 13. Secondary Face Inputs for Contact Creation


    6. In the Define Contact dialog, click Apply.
    The created contact is listed in the Solution tab of the Model Browser.
  9. Ceate a contact for the inner faces of the Ring.
    1. Set the following parameters in the Define Contact dialog, as shown below.
      Figure 14. Contact Creation within Ring


    2. In the Define Contact dialog, select the line edit field for Main faces.
      The line edit field is highlighted.
    3. In the modeling window, select the top semi-circular inner face of the ring.
      Figure 15. Top Semi-Circular Inner Face for Contact Creation


    4. In the Define Contact dialog, select the line edit field for Secondary faces.
      The line edit field is highlighted.
    5. In the modeling window, select the bottom semi-circular inner face of the ring.
      Figure 16. Bottom Semi-Circular Inner Face for Contact Creation


    6. In the Define Contact dialog, click OK.
    The contact will be created and added to the Solution tab in the Model Browser.

Create Loadcases

  1. In the Model Browser, click the Solutions tab.
  2. In the Solutions tab, right-click Rubber Ring and select Define using Load case from the context menu.
    A Non Linear Static loadcase type is created.
  3. Right-click on the created loadcase (Loadcase1), select Rename from the context menu, and enter Ring_Compression.
    The Loads and Constraints pertaining to simulate the Compressing action on the Ring will be added in the Ring_Compression loadcase.
  4. Create an additional loadcase.
    1. Right-click on LoadCase, and select Create Loadcase from the context menu.
    2. Right-click on LoadCase2, select Rename from the context menu, and enter Ring_Sliding.
    3. Verify Type is set to Non Linear Static.

Define Constraints

  1. From the Solutions tab of the Model Browser, right-click on the Ring_Compression loadcase and select Set Current from the context menu.
    The Ring_Compression loadcase becomes current and all the loads and constraints created will be added to the current load case only.
  2. From the Assembly tab of the Model Browser, select Ring.
    The Ring body is highlighted in the modeling window.
  3. Right-click in the modeling window and select Isolate from the context menu.
    The Ring body is isolated in the modeling window.
  4. Right-click in the modeling window and change the selection filter to Face.
    Figure 17. Face Selection Filter


  5. From the Analysis ribbon, Loads and Constraints group, click the Constraints tool.
  6. From the secondary tool set, select the Fixed tool.
    The Fixed Constraint dialog opens.
  7. In the Fixed Constraint dialog, set the Axes as shown below.
    Figure 18. Constraint for the Ring Body Along Z Axis


  8. In the modeling window, select all four faces of the Ring body and click Apply in the Fixed Constraint dialog.
    The constraint is added to Ring_Compression loadcase.
  9. Right-click in the modeling window and change the selection filter to Node.
    Figure 19. Node Selection Filter


  10. In the modeling window, select the Nodes on the front and back sides of the Ring body, as shown below.
    Figure 20. Node Selection for “Ring_X” Constraint


  11. In the Fixed Constraint dialog, set the Axes as shown below and click Apply.
    Figure 21. Constraint for the Ring Body Along X Axis


  12. Right-click in the modeling window and select Redisplay Model from the context menu.
    All bodies display in the modeling window.
  13. Right-click in the modeling window and change the selection filter to RBE Node.
    Figure 22. RBE Node Selection Filter


  14. In the modeling window, select the RBE Main Node of the End RBE, as shown below.
    Figure 23. End RBE Main Node


  15. In the Fixed Constraint dialog, set the Axes as shown below and click OK.
    Figure 24. Constraint for the Bottom End Body


The created constraints are added to the Ring_Compression loadcase.
Figure 25. Constraints are added to the Ring_Compression LoadcaseA


Apply Enforced Displacement

  1. From the Analysis ribbon, Loads and Constraints group, click the Constraints tool.
  2. From the secondary tool set, select the Enforced tool.
    The Enforced Constraint dialog opens.
  3. Right-click in the modeling window and change the selection filter to RBE Node.
    Figure 26. RBE Node Selection Filter


  4. In the modeling window, select the RBE Main Node of the Top RBE, as shown below.
    Figure 27. Top RBE Main Node


  5. In the Enforced Constraint dialog, define the parameters as shown below and click OK.
    Figure 28. Enforced Displacement for Ring_Compression


    The Enforced Displacement is added to the Ring_Compression loadcase.
    Figure 29. Enforced Displacement Added to Ring_Compression Loadcase


  6. Add constraints to the Ring_Sliding loadcase.
    1. In the Solutions tab of the Model Browser, right-click on the Ring_Sliding loadcase and select Set Current from the context menu.
    2. Right-click the Ring_Z constraint under Ring_Compression, and select Add to current Loadcase from the context menu.
    3. Right-click the Bottom_End constraint under Ring_Compression, and select Add to current Loadcase from the context menu.
    The Ring_Z and Bottom_End constraints are added to the current Loadcase.
    Figure 30. Ring_Z and Bottom_End Constraints Added to Ring_Sliding Loadcase


  7. Repeat steps 1 through 3.
  8. In the Enforced Constraint dialog, define the parameters as shown below.
    Figure 31. Enforced Displacement for Ring_Sliding


  9. In the modeling window, select the RBE Main Node of the Top RBE, as shown below.
    Figure 32. Top RBE Main Node


  10. In the Enforced Constraint dialog, click OK.
    The Enforced Displacement for generating the sliding force is added to the current loadcase.
    Figure 33. Enforced Displacement Added to Ring_Sliding Loadcase


Define Loadcase Parameters

  1. In the Solutions tab of the Model Browser, right-click the Ring_Compression loadcase and select Loadcase Parameters from the context menu.
    The Loadcase Parameters dialog opens.
  2. In the Loadcase Parameters dialog, set the values as shown below and click OK.
    Figure 34. Set the Values for Loadcase Parameters for Ring_Compression Loadcase


  3. Create Loadcase parameters for the Ring_Sliding loadcase.
    1. In the Solutions tab of the Model Browser, right-click the Ring_Sliding loadcase and select Loadcase Parameters from the context menu.
    2. In the Loadcase Parameters dialog, set the values as shown below and click OK.
      Figure 35. Create Loadcase Parameters for Ring_Sliding loadcase


The Loadcase Parameters are added in the Solutions tab of the Model Browser.

Create Solution Parameters and Output Requests

  1. In the Solutions tab of the Model Browser, right-click on the Rubber_Ring solution and select Solution Parameters from the context menu.
    The Solution Parameters dialog opens.
  2. In the Solution Parameters dialog, set the values as shown below and click OK.
    Figure 36. Set Values for Solution Parameters


  3. In the Solutions tab of the Model Browser, right-click on the Rubber_Ring solution and select Result Request from the context menu.
    The Result Request dialog opens.
  4. In the Result Request dialog, set the values as shown below and click OK.
    Figure 37. Set Values for Output Request


The Solution Parameters and Output Requests are added to the Rubber_Ring solution.

Solve and View Results

Solve the Solution

  1. In the Solutions tab of the Model Browser, right-click on Results and click Update.
    The solution begins to solve. After solving, the results are automatically loaded back into the database. After the solving is completed, the results are loaded into SimLab and the results for the final loadcase are displayed by default.
  2. In the Solutions tab of the Model Browser, right-click on Results under the Ring_Compression loadcase and click Display.
    The results for the Ring_Compression loadcase are displayed.
  3. Optional: Change the Results components using the Results panel at the top of the modeling window and animate the results using the Animation panel at the bottom of the modeling window.
    Figure 38. Results of Ring_Compression Loadcase


  4. In the Solutions tab of the Model Browser, right-click on Results under the Ring_Sliding loadcase and click Display.
    The results for the Ring_Sliding loadcase are displayed.