Extrusions are one of the most basic ways to design a part in Pro/E, and sketching is an important part of the design process.  In this section, you will learn basic operations by creating a simple part using an extruded protrusion. You will then modify the part using a cutting operation.

1. Start Pro/E Wildfire.
2. Select [File] -> [New] from the menu bar. The dialog shown in Figure 1.1 will pop up.

   
   [Figure 1.1]

    

3. Type the part name [Example1] in Text Box.
4. Click [OK] button (or press Enter Key). You will see the screen shown in Figure 1.2.

1. Select the Extrude Tool icon from the tool bar at the right of the screen, as shown in Figure 1.2.
2. Select the Sketcher icon from the extrusion tool bar on the dashboard at the bottom of the screen. 
3. Select the plane labeled FRONT.  This will allow you to sketch in the xy plane and extrude in the z direction.

   
   [Figure 1.3]

    

4. Click the Sketch button from the Section pop-up menu.  Pro/E will switch to Sketch Mode, and you will see the screen as shown in Figure 1.4.

    
   [Figure 1.4]

    

5. Close the References Dialog.
6. Select [Sketch] -> [Options] from menu bar. The dialog shown in Figure 1.5 will pop up.  Turn ON the [Grid] and [Snap To Grid], and click the green check button.

   
   [Figure 1.5]

    

7. Select [Sketch] -> [Intent Manager] from the menu bar.  This will bring up the Menu Manager shown in Figure 1.6. 

   
   [Figure 1.6]

    

8. Now sketch the shape shown in Figure 1.7. Select [Line] from GEOMETRY menu of the Menu Manager.
9. Use the left mouse button to click points A, B, C, D, E, F and A shown in Figure 1.7. After clicking these points, press the mouse middle button.

    
   [Figure 1.7]

    

10. Select [Regenerate] from SKETCHER menu of the Menu Manager.
11. Zoom in using the wheel on the mouse or by moving the mouse up and down while holding CTRL and middle mouse button.
12. Move the sketch to the center of the screen by moving the mouse while holding the middle mouse button and the Shift key.
13. Now set the size of the shape. Follow the steps below:
    • Select [Dimension] from SKETCHER menu.
    • Click Edge2 and Edge6 with the left mouse button, and then click point A with the middle mouse button.
    • Click Edge1 and Edge5 with the left mouse button, and then click point B with the middle mouse button.
    • Click Edge2 and Edge4 with the left mouse button, and then click point c with the middle mouse button.
    • Click Edge3 and Edge5 with the left mouse button, and then click point D with the middle mouse button.

      
      [Figure 1.8]

       

14. Select [Regenerate] from SKETCHER menu.  The dimensions of the part will be shown as in Figure 1.9.

    
    [Figure 1.9]

     

15. Select [Modify] from SKETCHER menu.
16. Click the number that is circled by A shown in Figure 1.9. Then type the correct dimension underneath the toolbar. In this case, type 200 in the text box, and click the check button.
17. Similarly, change the number that is circled by B to 200, by C to 50, and by D to 50.
18. Select [Regenerate], and then Select [Done] from SKETCHER menu.  Pro/E will exit Sketcher Mode.
19. Type in 100 into the extrusion depth box on the dashboard and click check button.

     
    [Figure 1.10]

     

20. Select [View] -> [Orientation] -> [Default Orientation] from menu bar. If you followed the instructions correctly, you will see the three-dimensional image shown in Figure 1.11.

    
    [Figure 1.11]

     

21. While there is no real undo option in Pro/E, the model tree can be used to modify features you have already created.  Right click on the part you wish to alter, and select [Edit Definition] from the list of options.  You can then alter the part.  This topic will be explored further in Tutorial 4.

22. Select [File] -> [Save] from menu bar and click the check button at the bottom of the screen to save the part.

     

1. Select the Extrude Tool icon from the tool bar on the right of the screen, as in Step 1 of the previous section.
2. Select the Remove Material icon from the extrusion tool bar on the dashboard, as shown in Figure 1.12. 
3. Select the Sketcher icon.

   
   [Figure 1.12]

    

4. Locate the bottom face of the part by using View Manager as described in Step 21 of the previous section.  Select [View] -> [View Manager] from the menu bar, and then double click [Bottom] from the pop-up window.  You should see the view shown in Figure 1.13.
5. Click on the bottom face of the part near point A in Figure 1.13 to select it as the sketching plane.
6. Change the orientation to [Bottom] on the Section menu.

1. Click the Sketch button from the Section menu.  Pro/E will switch to Sketch Mode.
2. Select [Sketch] -> [Intent Manager] from the menu bar.
3. Select [Line] from GEOMETRY menu.
4. Click points A, B and C shown in Figure 1.14 with the mouse left button, and then click the middle mouse button.

   
   [Figure 1.14]

    

5. Select [Regenerate] from SKETCHER menu.
6. To dimension the cut, click E2 and E4 shown in Figure 1.15 with the left mouse button, and then click near A with the middle mouse button. Similarly, click E1, E3, and B.  Zoom and pan if necessary.

   
   [Figure 1.15]

    

7. Select [Regenerate] from SKETCHER menu.
8. Click the dimensions at points A and B, and then change them to 25. You should see the image shown in Figure 1.16.

    
   [Figure 1.16]

    

9. Select [Regenerate] and then Select [Done] from the SKETCHER menu. You will see the screen shown in Figure 1.17.

    
   [Figure 1.17]

    

10. Rotate the part until you see an outline of what the cut will look like.  If the cut is outside the part as shown in Figure 1.8, click on the yellow cutting direction arrow as shown.  The outline should now be inside the part.

    
    [Figure 1.18]

     

11. Type 100 into the Extrusion Depth box and click the check button.
12.  Use the mouse to zoom and rotate the part to see it from different angles.  You should see the image shown in Figure 1.18.

    
    [Figure 1.18]

     

13. Select [File] -> [Save] from menu bar to save the part.
14. Test the information you have learned in this tutorial by completing Problem 1.