Hertz Contact

1. Hertz Contact MSC.Marc 2005r2 MSC.Patran 2005r2 Estimated Time for Completion: 30 minutes Experience Level: Lower

2. Topics Covered • Creating deformable contact boundary conditions of two bodies • Controlling solutions for nonlinear geometric effects • Reviewing the results and comparing to a theoretical value • Using local adaptive meshing

3. Problem Description • In this example problem, a steel cylinder with a radius of 5” is pressed against a 2” deep aluminum base. The problem is linear except the contact condition at the base which is modeled using the contact pair approach. • We will use Patran to complete the problem description from a given 2D meshed model and analyze it by using Marc.

4. Summary of Model 10,000 psi pressure Steel E = 30E6 v = 0.30 Constrain 2 nodes along the vertical center line <0,,> Aluminum E = 10E6 v = 0.33 Constrain any node along the vertical center line <0,,> 5” radius 2” 16” Constrain all bottom nodes <,0,>

5. Goal • In this example, we will determine the maximum compressive stresses in a cylinder and a flat plate being compressed against each other. • The results from Marc will be compared to a theoretical value. • We will also demonstrate how the results can be improved through the use of adaptive meshing.

6. Expected Results Maximum compressive stress is 2.12E5 psi. Y-Component stresses Results WITHOUT the use of adaptive meshing

7. Expected Results Maximum compressive stress is 2.38E5 psi. Y-Component stresses Y-Component stresses Results WITH the use of adaptive meshing

8. Create Database Create Database a b c d e • Click File menu / Select New • In File Name, enter hertz.db • Click OK • Select Analysis Code to be MSC. Marc • Click OK

9. Import Model a b c d • Click File menu / Select Import • Select Source to be MSC. Patran DB • Locate and select file hertz_model.db • Click Apply

10. Create Fixed Displacements n e a b c d f g h i j k l m • Click Loads/BCs icon • Select Action to be Create • Select Object to be Displacement • Select Type to be Nodal • In New Set Name, enter fixed_base_x • Click Input Data • In Translations, enter <0, ,> • Click OK • Click Select Application Region • Select Geometry Filter to be FEM • In Select Nodes, select any node along vertical line of the base from screen or enter Node 1167 • Click Add • Click OK • Click Apply Repeat (e) – (m) for the following new sets of BCs

11. Create Deformable Contacts a b c d e f g h i • Select Object to be Contact • In New Set Name, enter base_contact • Select Target Element Type to be 2D • Click Select Application Region • Select Geometry Filter to be Geometry • In Select Surfaces, select base on screen or enter Surface 3 • Click Add • Click OK • Click Apply Repeat (b) – (i) for the following new set of BCs

12. Create Pressure a b c d e f g h i j • Select Object to be Pressure • In New Set Name, enter pressure • Select Target Element Type to be 2D • Click Input Data • In Edge Pressure, enter 10000 • Click OK • Click Select Application Region • In Select Surfaces or Edges, select edges on top of cylinder and click Add to add the selected edge to Application Region one by one or enter Surface 1.4 2.2 • Click OK • Click Apply

13. Define Material a b c d e f g • Click Materials icon • In Material Name,enter steel • Click Input Properties • In Elastic Modulus, enter 30e6 • In Poisson Ratio, enter 0.3 • Click OK • Click Apply Repeat (b) – (g) for the following new material

14. Define Element Properties a b c d e f g h i j • Click Properties icon • Select Type to be 2D Solid • In Property Set Name, enter cylinder_prop • Click Input Properties • Click Mat Prop Name icon and select steel • In Thickness, enter 1 • Click OK • In Select Members, select surfaces of cylinder on screen or enter Surface 1 2 • Click Add • Click Apply Repeat (c) – (j) for the following new property

15. Modify Solution Control and Run Analysis a b c d e f g • Click Analysis icon • Click Load Step Creation • Click Solution Parameters • Select Nonlinear Geometric Effects to be None • Click OK • Click Apply (answer Yes to modify the Default Static Step) • Click Apply ** Wait until analysis is completed **

16. Read Results File a b c d e • Select Action to be Read Results • Click Select Results File • Locate file hertz.t16 • Click OK • Click Apply

17. Plot Results a b c d e f • Click Results icon • In Select Result Cases, select the last increment • In Select Fringe Result, select Stress, Global System • Select Quantity to be Y Component • In Select Deformation Result, select Displacement, Translation • Click Apply Maximum compressive stress is 2.12E5

18. Theoretical Comparison

19. Theoretical Comparison Maximum compressive stress

20. Turn On Adaptive Meshing and Run Analysis a b c d e f g h i j k • Click Analysis icon • In Job Name, enter hertz_amesh • Click Job Parameters • Click Adaptive Meshing • Select Adaptivity Type to be Local • In Zone Name, enter contact_zone • In Select a Group, select all • Click Apply • Click OK • Click OK • Click Apply ** Wait until analysis is completed **

21. Read Results File a b c d e • Select Action to be Read Results • Click Select Results File • Locate file hertz_amesh.t16 • Click OK • Click Apply

22. Plot Results a b c d e f • Click Results icon • In Select Result Cases, select the last increment • In Select Fringe Result, select Stress, Global System • Select Quantity to be Y Component • In Select Deformation Result, select Displacement, Translation • Click Apply Maximum compressive stress is 2.38E5

23. Investigate Modified Meshes Meshes have been refined automatically where the contact occurred, giving more accurate results.

24. Theoretical Comparison • Investigate the improvement in the results when using adaptive meshing Maximum compressive stress Use of adaptive meshing, which refines meshes in the contact zone, can improve the accuracy of the results without having to refine meshes of the entire model.