1. Start Pro/E Wildfire.

2. Select [File] -> [New], and type the part name as [Benchvise100_part8].

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 0.375 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 5.0 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 Extrude tool icon, followed by the Sketch icon.

12. Select the FRONT plane as the sketch plane, and the RIGHT plane as the reference plane.

13. Draw a circle with a diameter of 0.25 as shown in Figure 1.3.

                                                                                                                        [Fig 1.3]

14. Select the Continue icon from the tool bar to exit the Sketcher Mode.

15. Select the Remove Material Icon, and make sure that the yellow arrow points in the right direction. Also,  as shown in Figure 1.4.

• Specify the Extrusion Depth to be 0.750 units.

                                                                                                                        [Fig 1.4]

16. Click on the green check button to complete the extrusion; the part should look like Figure 1.5 below.

                                                                                                                        [Fig 1.5]

17. Select the Make Datum icon from the right toolbar. For its references, click on the FRONT plane, and enter an offset distance of 1.25 units; see Figure 1.6. 

                                                                                                                        [Fig 1.6]

18. Select [OK] on the Datum Plane Menu to complete modeling of the new datum, DTM1 (your names could differ)..

20. Select [Edit] -> [Feature Operations]. From the Menu Manager:

Select [Copy] -> [Mirror] -> [Select] -> [Dependent] -> [Done]

• Select the cut (second protrusion) that got completed in last few steps, and click on [Done]; see Figure 1.7.
• Select [Setup Plane] -> [Plane], and choose the plane DTM1 (just created) on the model. Select [Done] from the menu manager.

                                                                                                                        [Fig 1.7]

21. The completed model should look like Figure 1.8.

                                                                                                                        [Fig 1.8]