Basic Modeling Techniques: Revolves, Patterns, And Copies

Creating a Revolved Part

1. Start Pro/E Wildfire.
2. Choose [File] -> [New] and name the new part [Example5].
3. Select the Revolve Tool icon from the tool bar at the right of the screen, as shown in Figure 5.1.

   
   [Figure 5.1]

4. Select the Sketcher icon from the revolve tool bar on the dashboard.
5. Select the plane labeled FRONT and select the Sketch button in the Section menu.
6. Select [Sketch] -> [Intent Manager] from the menu bar.
7. Zoom in so that you see the coordinates shown in Figure 5.2.
8. Select [Line] from the GEOMETRY menu, and select [Centerline] from the LINE TYPE menu.
9. Click point A and point B shown in Figure 5.2 to create a centerline.
10. Select [Geometry] from the LINE TYPE menu.
11. Draw the section shown in Figure 5.2 by clicking the endpoints with the left mouse button, and then clicking the middle mouse button.

    
    [Figure 5.2]

12. Select [Regenerate] from the SKETCHER menu.
13. Add the dimension shown at point A in Figure 5.3 by performing the following steps:
    • Click Edge1 with the left mouse button.
    • Click Centerline with the left mouse button.
    • Click Edge1 again with the left mouse button.
    • Click point A with the middle mouse button.
14. Follow the same procedure to add the dimensions at points B and C.
15. Follow the normal procedure for dimensioning to add the dimensions at points D, E, F, G, and H.
16. Select [Regenerate]. You should now be able to see dimensions similar to those shown in Figure 5.3.

    
    [Figure 5.3]

17. Select [Scale] from the MOD SKETCH menu.
18. Select the dimension at point A.
19. Type 50 into the textbox and click the check mark.
20. Select [Regenerate]. All of the dimensions should scale.
21. Select [Mod Entity] from the MOD SKETCH menu.
22. Change the dimension of B to 100, C to 200, D to 12.5, E to 25, F to 50, G to 62.5, and H to 75.
23. Select [Regenerate]. You should see the image shown in Figure 5.4.

    
    [Figure 5.4]

24. Choose [Done] from Menu Manager.
25. Click the check button in the revolve tool bar.
26. Rotate the part to examine the modifications. You should see the image shown in Figure 5.5.

    
    [Figure 5.5]

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Creating a Sketched Hole by Revolving Section

1. Select the Hole Tool icon from the tool bar at the right of the screen.
2. Select [Sketched] for the shape of the hole in the hole tool bar on the dashboard.
3. Select the Sketcher icon, as shown in Figure 5.6.

   
   [Figure 5.6]

4. Select [Sketch] -> [Intent Manager] from the menu bar.
5. Select [Line] from the GEOMETRY menu and [Centerline] from the LINE TYPE menu.
6. Click points A and B to draw a centerline as shown in Figure 5.7.
7. Select [Geometry] from the LINE TYPE menu and click points C, D, E, F, G, H, C to draw the section shown in Figure 5.7.

   
   [Figure 5.7]

8. Select [Regenerate] from the SKETCHER menu.
9. Dimension the section as shown in Figure 5.8.
   • Using the left mouse button, click Edge1, Centerline, and Edge1 again. Click point A with the middle mouse button.
   • Using the left mouse button, click Edge2, Centerline, and Edge2 again. Click point B with the middle mouse button.
   • Add the dimensions at points C and D using the normal method.
10. Select [Regenerate] from the SKETCHER menu.
11. Modify the dimensions to match those shown in Figure 5.8.

    
    [Figure 5.8]

12. Select [Regenerate] and then [Done] from the SKETCHER menu.
13. Select the top surface of the pulley. An outline of a hole should be shown as in Figure 5.9.

    
    [Figure 5.9]

14. Click on the Placement menu on the dashboard and select [Radial] for the hole placement dimensions, as shown in Figure 5.10.
15. Click and drag one handle on the hole to the center axis of the hole in the pulley. Drag the other handle to the plane labeled FRONT (do not select the handle that changes the diameter of the hole). You should see the image shown in Figure 5.10.

    
    [Figure 5.10]

16. Double click on the dimension at point A in Figure 5.10 and change it to 70.
17. Double click on the dimension at point B and change it to 0 degrees.
18. Click the check button and rotate the pulley to examine the hole. You should see the image shown in Figure 5.11.

    
    [Figure 5.11]

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    Creating Patterns and Copies

1. Select the hole that was just created and select the Pattern Tool icon from the tool bar at the right of the screen.

   
   [Figure 5.12]

2. Double click on the dimension that was shown at point B in Figure 5.10. Change the value from 0 to 60, as shown in Figure 5.13.
3. Change the number of features to 6, as in Figure 5.13. This will make a pattern of 6 holes located 60 degrees apart.

   
   [Figure 5.13]

4. Click the check button. You should see the image shown in Figure 5.14.

   
   [Figure 5.14]

5. To create a plane to mirror the holes, select the Datum Plane icon from the tool bar at the right of the screen.
6. To define references, select the plane labeled TOP.
7. From the DATUM PLANE menu, enter 37.5 into the Offset Translation textbox, and click the OK button. This will put a datum plane in the center of the pulley, as shown in Figure 5.15.

   
   [Figure 5.15]

8. Select [Edit] -> [Feature Operations] from the menu bar. Menu Manager will pop up.
9. Select [Copy] from the FEAT menu.
10. Select [Mirror] from the COPY FEAT menu.
11. Select [Done] from the COPY FEAT menu.
12. Select the Pattern (Hole) branch of the model tree at the left of the screen, and select [Done] from the SELECT FEAT menu.
13. Select the datum plane that was just created, and select [Done] from the COPY menu. There should now be holes on both side of the pulley, as shown in Figure 5.16.

    
    [Figure 5.16]

14. Select [File] -> [Save] from menu bar to save the part.
15. Test the information you have learned in this tutorial by completing Problem