1. Comparing 2D and 3D Structural Analysis Winter Semester 2009-2010

2. 2 Goals  This workshop consists of a 2 parts assembly representing a pressure cap and retaining flange (full model shown below).  We will solve the model in 2 ways, as a 90 degree symmetry sector and as a 2D axisymmetric model (shown on next page).  Our goal is to compare the 2 methods both for consistency and for economy. Pressure Cap Retaining Ring Full Model

3. 3 Geometry  Shown here are the 3D sector model and the 2D axisymmetry model. Pressure Cap Retaining Ring

4. 4 Assumptions  Assumptions: The retaining ring is fixed at its mounting holes. The contact region between the parts is frictionless. The base of the pressure cap is constrained using a compression only support. Note: due to the presence of the bolt holes the structure is not truly axisymmetric. Part of our goal is to determine the validity of the axisymmetric assumption in this case.

5. 5 2D Model

6. 6 Start Page  From the launcher start Simulation.

7. 7 Geometry Setup  Important: Before importing the geometry highlight the “ Geometry ” branch and change the “ Analysis Type ” preference to “ 2D ” in the details.  Choose “ Geometry > From File... “ and browse to the file “ Axisym_pressure_2D.x_t ”.  Choose “ Static Structural ” under “ New analysis ” menu

8. 8 Preprocessing 1.Set the working unit system to the metric mm system. “ Units > Metric (mm, Kg, N, C, s) ”. 2.Highlight Parts 1 and 2 in the tree and rename them to be: “ Retaining Ring ” and “ Pressure Cap ”. 3.High light the “ Geometry ”,in the details, change the “ 2D Behavior ” to “ Axisymmetric ”.

9. 9 Preprocessing 4.Materials: highlight the “ Pressure Cap ” branch, in the details window, change the material to be “ Stainless Steel ”. Details-> Material -> Import -> Stainless Steel

10. 10 Contact  Highlight the “ Contact Region ” ; notice the target contains a single edge. We will add a second edge to insure all possible contact is detected. Additional target edge to be added (shown dashed)

11. 11 Contact 5.Click in the “ Target ” field then select the 2 edges of the pressure cap shown here. 6.“ Apply ” the new selection. Note: if you have difficulty selecting the edges of the Pressure Cap, use the “hide” feature to hide the retaining ring during selection. Select Edges

12. 12 Contact 7.In the Contact Region details, change the “ Type ” to “ Bonded ”. 8.Highlight the “ Mesh ” branch, RMB and “ Generate Mesh ” (note the speed with which the 2D mesh is generated as well as the density).

13. 13 Environment 9.Select the 3 inside edges of the Pressure Cap. 10.Insert “ Pressure ” under the “ Loads ” menu (or by RMB  insert  pressure). 11.Set the pressure magnitude = 0.1MPa.

14. 14 Environment 12. Highlight the bottom edge of the pressure cap. “ RMB > Insert > Compression Only Support ”.

15. 15 Environment 14. Select the top of the retaining ring. “ RMB > Insert > Fixed Support ”. Remember, the axisymmetric assumption here is that the retaining ring is a continuous solid. Actually there are bolt holes around its circumference. For this reason, when the model was created in DesignModeler this separate line was intentionally created to provide a location to add our support.

16. 16 Solution  Highlight the Solution branch, RMB and insert: 16. Stress > Equivalent (von-Mises) 17. Deformation > Total 18. Switch to body select mode, select the pressure cap and repeat steps 16 and 17. Note, the last two results are now scoped to the retaining ring. This will allow us to isolate its response.

17. 17 Solution Solve the analysis Notes on axisymmetry: 1.Notice that the model lies completely in +X space with the Y axis as the axis of revolution. This is required for axisymmetry. 2.Axisymmetry assumes that the model is a complete 360 degree model. For this reason no constraints in the X direction are required. The portion of the pressure load acting in the +X direction is assumed to be offset by an equal portion in the –X direction.

18. 18 Postprocessing  Highlight each of the result objects to inspect the response. Note: due to meshing and machine variations, results may not match exactly those shown here.  For future reference, highlight the “ Equivalent Stress 2 ” result (scoped) and note the maximum value here:________________

19. 19 Postprocessing  Open the “ Solution Information ” file, under Solution branch. The graphics window will change to the Worksheet view. Scroll to the bottom of the solution information and note the Elapsed Time (this will vary by machine). Elapsed Time = ___________________________ Note, CP time represents the sum for all processors used. In multiprocessor machines it will generally exceed elapsed time.

20. 20 3D Model

21. 21 3D Symmetry Model  We ’ ll now set up and solve the 3D symmetry model using the same boundary conditions.  Save the current 2D project  Highlight the “ Project ” and start new model be choosing “ New Model ”

22. 22 Geometry Setup  Choose “ Geometry > From File... “ and browse to the file “ Axisym_pressure_3D.x_t ”.  In the details window, make sure that the model type is set to be 3-D.

23. 23 Preprocessing 1.The working unit system should still be set to the metric mm system. “ Units > Metric (mm, Kg, MPa, C, s) ”.  Note, once again rename the 2 parts in the model to be: “ Retaining Ring ” and “ Pressure Cap ”

24. 24 Preprocessing 2.From details for the “ Pressure Cap ” and import the material “ Stainless Steel ”.

25. 25 Contact 3.Highlight the “ Contact Region ” branch and change the “ Type ” to “ Bonded ”. 4.Highlight the “ Mesh ” branch, RMB and “ Preview Mesh ”. Refer to slide number 12 to compare the 2D mesh.

26. 26 Environment 5.From the Environment branch highlight the 6 faces representing the planes of symmetry (cut planes). 6.RMB > Insert > Frictionless Support. 6 Note, frictionless supports provide constraints in the normal direction. This is used to model the symmetry condition. Note: there are six (6) faces to select.

27. 27 Environment 7.Highlight the bottom face of the pressure cap, “ RMB > Insert > Compression Only Support ”.

28. 28 Environment 8.Highlight the 3 inside faces on the pressure cap, “ RMB > Insert > Pressure ”. 9. Change the Magnitude to “0.1” in the detail window.

29. 29 Environment 10.Highlight the 3 cylindrical faces of the bolt holes, “ RMB > Insert > Fixed Support ”.

30. 30 Solution  Highlight the Solution branch, RMB and insert: 11.Stress > Equivalent (von-Mises) 12.Deformation > Total 13.Switch to body select mode, select the pressure cap and repeat steps 16 and 17. –Solve As before, the last two results are scoped to the pressure cap.

31. 31 Postprocessing  As before highlight each of the result objects and inspect the response.  For reference, highlight the “ Equivalent Stress 2 ” result (scoped) and note the maximum value here:________________

32. 32 Postprocessing The graphics window will change to the Worksheet view. Scroll to the bottom of the solution information and note the Elapsed Time (this will vary by machine). Elapsed Time = ___________________________  Open the “ Solution Information ” file, under Solution branch.

33. 33 Comparison Between the Models

34. 34 Comparison  Using the example shown in the exercise we now compare analyses (note, your actual results may vary from those shown here. Also, your solution times will almost certainly differ from those shown here.  Maximum von-Mises Stress Results: Axisymmetric = 0.829 MPa 3D Symmetry = 0.749 MPa Note, meshing differences account for the results difference (see next page). Recall that the 2D model resulted in a more refined mesh than the 3D. The next page shows the results from a more refined 3D model.  Elapsed Time: Axisymmetric = 8.0 seconds 3D Symmetry = 40.0 seconds

35. 35 Comparison  Maximum von-Mises Stress Results: 3D Symmetry (refined) = 0.852 MPa  Elapsed Time: 3D Symmetry (refined) = 578.0 seconds Results using a more refined mesh with the 3D symmetry model