1. Advanced Results Processing Winter Semester 2009-2010

2. 2 Goals  In this workshop a high pressure vent assembly is been analyzed for stress and deflection.  Some of the results from the analysis will be difficult to interpret if all bodies are active during postprocessing.  Our goal is to isolate parts of the model and use some of the advanced features for postprocessing.

3. 3 Assumptions  We will assume that gas is been vented through the inlet pipe into the expansion chamber. Inside the chamber the pressure drops to 20% of the inlet pressure.  The expansion chamber is rigidly mounted to the inlet thus we will leave this contact region defined as ‘ bonded ’.  The support bracket allows limited movement to the pipe so ‘ no separation ’ contact will be used here. [See the contact description on the next page].  The inlet pipe and bracket are modeled using structural steel while the expansion chamber is made of polyethylene.

4. 4 Part/Contact Description Bonded Contact No Separation Contact Support Bracket Inlet Pipe Expansion Chamber

5. 5 Start Page  From the launcher start Simulation.  Choose “ Geometry > From File... “ and browse to the file “ Pressure_System.x_t ”.

6. 6 Preprocessing  Set the working units to Metric (mm). 1.“ Units > Metric (mm, kg, N, C, s) ”.  Change the bracket/pipe contact type to no separation: 2.Highlight the “ Contact Region 2 ” branch. 3.In the detail window change the contact “ type ” to “ No Separation ”.

7. 7 Preprocessing  Change the material for the expansion chamber to polyethylene. 4.Highlight the part in the tree. 5.In the detail window click in the material field and “ Import... > Polyethylene ”.

8. 8 Environment  Apply pressure to the inside surfaces of the pipe: 6.Highlight the “ Static structural ” branch. 7.Select the 5 interior surfaces of the pipe (use Extend to limits). 8.“ RMB > Insert > Pressure ”.

9. 9 Environment 9.In the detail window for the pressure enter 1 in the magnitude field (1MPa). 9

10. 10 Environment 10.Select the 3 interior surfaces of the expansion chamber.  Note, using the selection planes, the status bar and the CTRL key will simplify this selection.  Alternately use “ RMB > Hide All Other Bodies ” Selection planes Status Bar “RMB > Insert > Pressure”. In the detail window change the magnitude to 0.2MPa.

11. 11 Environment 11.Select the end surface of the pipe. 12.“ RMB > Insert > Fixed Support ”.

12. 12 Environment 15.Select the surface of the cylinder in the bracket. 16.“ RMB > Insert > Cylindrical Support ” (leave default fixed,fixed,fixed).

13. 13 Environment 17.Select the back face of the bracket. 18.“ RMB > Insert > Frictionless Support ”.

14. 14 Solution 19.Highlight the solution branch. 20.RMB > Insert > Stress > Equivalent (von Mises) 21.RMB > Insert > Deformation > Total  Solve

15. 15 Results  When the solution is complete, highlight the 2 result objects and view them. Notice the total deformation plot contains very little details for the inlet pipe and support bracket parts of the assembly.

16. 16 Results  Scope a new total deformation to the expansion chamber 22. Highlight the solution branch. 23. Switch to body select mode and highlight the expansion chamber in the graphics window. 24. “ RMB > Insert > Deformation > Total ”.

17. 17 Results for each part  Repeat the procedure on the previous page but choose “ Equivalent stress ” as the result.  Repeat the procedure on the previous page and above for the remaining parts.  Solve again to update the new result objects.  Compare the overall result to the individual ones (as shown below). Note the increased detail shown in the individual plots.

18. 18 Results – slice plane  Add a slice plane. Plot the stress scoped to the expansion chamber then reorient the model to look into the Z axis as shown below.  Note the triad at the bottom of the screen can be convenient to reorient the model. 25. Click on the “ New selection plane ” icon. 26.A “ selection planes ” details window will appear at the bottom.

19. 19 Results – slice plane Hold down the left mouse button and draw a line down the center of the plot (see figure on the next slide). In order to see the sliced plane you will need highlight the specific solution branch (in this case the equivalent stress branch) and change into “ slice planes ”

20. 20 Results – slice plane  By clicking on one of the dashed lines on either end of the handle you can activate the result plot on one side of the slice plane. Note the dashed line then becomes solid. This is a toggle control.

21. 21 Slice Plane Notes  You may create as many slice planes as desired and each can be edited individually. This can be useful for things like plotting a quarter section of a result.  To hide the slice plane(s) use the drop down geometry type icon and return to an “ exterior ” plot. The slice plane(s) remains in its current location and can be reactivated whenever desired.  Figures which contain slice planes will display slice planes regardless of the setting of the geometry icon.  In order to activate the desire planes, you should mark there name in the details window Geometry Icon

22. 22 Results  Change the plot type from slice planes to “ Exterior ” and plot the result for the support bracket.  Change to the “ IsoSurfaces ” display type.

23. 23 Results  Change to the “ capped isosurface ” display type.  By clicking in the legend and dragging the slider the capping point can be modified. Drag

24. 24 Results  Reactivate the exterior plot for the complete assembly stresses.  From the “ Edges ” icon choose to “ Show Elements ”. Edges Icon

25. 25 Results  Finally add some annotations to pin point results.  Plot the exterior stress plot for the assembly.  Activate the “ Probe ” and click several locations on the model to add annotations.  Note to remove annotations activate the “ Label ” icon and highlight the specific annotation. Use the keyboard “ delete ” key to remove the annotation.