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1. Start Pro/E Wildfire.
2. Select [File] -> [New], and type the part name as [Benchvise100_part7].
3. Select the Extrude tool icon followed by the sketcher icon at the bottom
of the screen.
4. Click on the reference plane labeled FRONT to select it as the sketch
plane.
5. Click on the sketch button, and switch to sketch mode.
6. Draw a circle with a diameter of 1.00 as shown in Figure 1.1.
[Fig 1.1]
7. Select the Continue icon from the tool bar
to exit the Sketcher Mode.
8. Type 5.375 into the Extrusion Depth textbox on
the dashboard.
9. Click the green check button on the
dashboard.
10. Select [View] -> [Orientation] ->
[Default Orientation] from the menu bar. You should see the part as shown
in Figure 1.2.
[Fig 1.2]
11. Select the Revolve tool icon, followed by the Sketch icon.
12. Select RIGHT to be the sketch plane.
13.Draw the profile shown in Figure 1.3.
- Select the horizontal line running through the middle to be the centerline
by selecting it and then choosing centerline from the right menu.
[Fig 1.3]
14. Select the Continue icon from the tool bar
to exit the Sketcher Mode.
16. Select the Remove Material Icon, and make sure that the yellow arrow points in the right
direction. Also, as shown in Figure 1.4.
- Select the Revolve from Sketch Plane icon and specify the angle to be 360.
[Fig 1.4]
17. Select the green check button on the bottom right of the screen to
complete the revolved cut; the part should resemble Figure 1.5.
[Fig 1.5]
18.Draw the profile shown in Figure 1.3.
- Select the horizontal line running through the middle to be the centerline
by selecting it and then choosing centerline from the right menu.
[Fig 1.6]
19. Select the Continue icon from the tool bar
to exit the Sketcher Mode.
20. Select the Remove Material Icon, and make sure that the yellow arrow points in the right
direction (away from the model)
- Select the Revolve from Sketch Plane icon and specify the angle to be 360.
21. Select the green check button on the bottom right of the screen to
complete the revolved cut; the part should look like Figure 1.7.
[Fig 1.7]
22. Select the Hole Tool icon from the toolbar on the right, and as shown in
Figure 1.10:
- Select the RIGHT plane to place the hole.
- Place it 0.50 units from the FRONT plane, and 0.00 units from the TOP
plane.
- Input 0.3750 in the Diameter textbox.
- Select the Drill on Both Sides icon in the Depth pull down menu, and type
1.00 in the Depth box.
[Fig 1.8]
23. Click on the green check button to complete the hole.
24. The completed model should look like Figure 1.9 below.
[Fig 1.9]
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