Datum planes are used as sketching surfaces and references for creating and construction features.  In this section, you will learn to use datum planes to create a rib.  You will learn how to create several basic features. 

1. Start Pro/E Wildfire.
2. Select [File] -> [New], and type the part name [Example3] in Text Box.
3. Click [OK] Button.
4. Select the Extrude Tool icon from the tool bar at the right of the screen.
5. Select the Sketcher icon from the dashboard, and click the reference plane marked as FRONT.
6. Click the Sketch button from the Section menu.  Pro/E will switch to Sketch Mode.
7. Close the References dialog box.
8. Select [Sketch] -> [Options] from menu bar.  Turn ON the [Grid] and [Snap To Grid], and click the green check button.
9. Select [Sketch] -> [Intent Manager] from the menu bar.
10. Use pan and zoom operations to change the viewing so that you see the coordinates as shown in Figure 3.1.
11. Now sketch the shape of the cross-section shown in Figure 3.1.  Select [Line] from the Menu Manager GEOMETRY menu.  Click points A, B, C, D, A with the left mouse button, and then press the middle mouse button.

    
    [Figure 3.1]

     

12. Select [Regenerate] from SKETCHER menu.
13. Now set dimensions as shown in Figure 3.2. Follow the steps below.
    • Click Edge1 and Edge3 with the left mouse button, and click point A with the middle mouse button.
    • Click Edge2 and Edge4 with the left mouse button, and click point B with the middle mouse button.
    • Select [Regenerate].
    • Modify dimensions to match those shown in Figure 3.2 if necessary, and Select [Regenerate].

    
    [Figure 3.2]

     

14. Select [Done] from Menu Manager.
15. Enter extrusion depth as 150, and click check button.
16. Select [View] -> [Orientation] -> [Default Orientation] from menu bar. You will see the image shown in Figure 3.3.

    
    [Figure 3.3]

     

1. Select Shell Tool icon from the tool bar at the right of the screen, as shown in Figure 3.4.

   
   [Figure 3.4]

    

2. Input 10 in Thickness textbox on the shell tool bar on the dashboard.
3. Use the left mouse button to select the front plane.  It should become highlighted in pink as shown in Figure 3.5.

   
   [Figure 3.5]

    

4. Click the check button.  You should see the shelled part shown in Figure 3.6.

    

   
   [Figure 3.6]

    

5. Select the Extrude Tool icon from the tool bar at the right of the screen.
6. Select the Sketcher icon from the dashboard.
7. Select the inside bottom of the shape near point A in Figure 3.6.
8. Click the Sketch button from the Section menu.  Pro/E will switch to Sketch Mode.
9. Select [Sketch] -> [Intent Manager] from the menu bar.
10. Select [Circle] from the GEOMETRY menu.
11. Click point A and point B shown in Figure 3.7.

    
    [Figure 3.7]

     

12. Select [Regenerate] from SKETCHER menu.

13. Now set dimensions as shown in Figure 3.8. Follow the steps below.
    • Click point A and Edge1 with the left mouse button, and click point B with the middle mouse button.
    • Click point A and Edge2 with the left mouse button, and click point C with the middle mouse button.
    • Click Circle with the left mouse button, and click point D with the middle mouse button.
    • Select [Regenerate].
    • Modify dimensions to match those shown in Figure 3.8 if necessary, and Select [Regenerate].

      
      [Figure 3.8]

14. Select [Done] from Menu Manager.
15. Enter extrusion depth as 90, and click check button.
16. Select [View] -> [Orientation] -> [Default Orientation] from menu bar. You will see the image shown in Figure 3.9.

1. Select Datum Plane Tool icon from the tool bar at the right of the screen, as shown in Figure 3.10.

   
   [Figure 3.10]

    

2. Select the center axis of the circular protrusion.  Hold CTRL and select Edge1 shown in Figure 3.11.  This will define references for the datum plane so that the plane passes through the axis and is normal to the edge.

    

   
   [Figure 3.11]

    

3. Select OK on the Datum Plane pop-up window.
4. Select Datum Plane Tool icon again.
5. Select the center axis of the circular protrusion.  Hold CTRL and select Edge2 shown in Figure 3.11. 
6. Select OK on the Datum Plane pop-up window.  You should see the two perpendicular planes shown in Figure 3.12.

    

   
   [Figure 3.12]

    

7. Select Rib Tool icon from the tool bar at the right of the screen, as shown in Figure 3.13.

   
   [Figure 3.13]

    

8. Select the Sketcher icon from the dashboard.
9. Select the second datum plane (the longer one) to define the sketch plane.
10. Select the first datum plane (the shorter one) to define the reference.
11. Make sure the Orientation in the Section menu is set to Right.  The Section menu should look like Figure 3.14.

     
    [Figure 3.14]

     

12. Select the Sketch button from the Section menu.
13. Do not close the References window once Pro/E enters Sketch Mode.
14. Select the Wireframe icon to change the view of the image to wireframe, as shown in Figure 3.15.

    
    [Figure 3.15]

     

15. Click on Edge1, Edge2, Edge3, and Edge4 shown in Figure 3.16 to define these edges as references.

    
    [Figure 3.16]

     

16. Select [Sketch] -> [Intent Manager] from the menu bar.
17. Draw a line from point A to point B as shown in Figure 3.16.
18. Select [Regenerate].
19. Dimension the distance from point B to Edge4 as shown in Figure 3.17.  Modify this distance if necessary.

    
    [Figure 3.17]

     

20. Select Regenerate, and then select Done.
21. Enter 5 into the Thickness textbox in the rib tool bar on the dashboard.
22. If the yellow rib direction arrow is not facing towards the inside of the part, select it with the left mouse button.  An outline of a rib should be shown, as in Figure 3.18.

    
    [Figure 3.18]

     

23. Click the check button.
24. Select the Shading icon on the tool bar at the top of the screen, as shown in Figure 3.19. 

    
    [Figure 3.19]

     

25. Rotate the part to see it from different views.  You should see the image shown in Figure 3.20.

    
    [Figure 3.20]

     

26. Select [File] -> [Save] from the menu bar to save the part.
27. Test the information you have learned in this tutorial by completing Problem 3.