A variety of geometric shapes and constructions can be designed automatically with Pro/E, including holes, rounds, and chamfers. The Hole option creates many types of holes, including straight holes, sketched holes, and holes for standard fasteners. The Round option creates a fillet or a round on an edge that is a smooth transition with a circular profile between two adjacent surfaces.  The Chamfer option creates a beveled surface at the intersection of edges.

1. Start Pro/E Wildfire.
2. Select [File] -> [New], and type the part name [Example2] 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. In this section, you will sketch the cross-section of the part using the same method as in Tutorial 1.  Start by closing 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 2.1.

    
    [Figure 2.1]

     

11. Now sketch the shape of the cross-section shown in Figure 2.2. Follow the steps below:
    • Select [Line] from the Menu Manager GEOMETRY menu.
    • Click points A and B with the left mouse button, and then press the middle mouse button.
    • Select [Arc] from GEOMETRY menu.
    • Click points B and C with the left mouse button.
    • Select [Line] from GEOMETRY menu.
    • Click points C, D, E and A with the left mouse button, and then press the middle mouse button.  Try to draw all points at the exact locations shown.

    
    [Figure 2.2]

     

12. Select [Regenerate] from SKETCHER menu.
13. Now set dimensions as shown in Figure 2.3. Follow the steps below.
    • Click Edge1 and Edge3 with the left mouse button, and click point A with the middle mouse button.
    • Click point B and Edge2 with the left mouse button, and click point C with the middle mouse button.
    • Click Arc with the left mouse button, and click point D with the middle mouse button.
    • Select [Regenerate].
    • Modify dimensions to match those shown in Figure 2.3 if necessary, and Select [Regenerate].

    
    [Figure 2.3]

     

14. Select [Done] from Menu Manager.
15. Enter extrusion depth as 100, and click check button.
16. Select [View] -> [Orientation] -> [Default Orientation] from menu bar. You will see the image shown in Figure 2.4.

    
    [Figure 2.4]

1. Select Hole Tool icon from the tool bar at the right of the screen, as shown in Figure 2.5.
   

   
   [Figure 2.5]

    

2. Input 50 in Diameter textbox on the hole tool bar on the dashboard.
3. Select the Through All icon from the depth menu, as shown in Figure 2.6.
4. Click point A shown in Figure 2.6 with the left mouse button to select the right plane.

   
   [Figure 2.6]

    

5. Select the bottom reference handle on the hole and drag it to Edge 1 shown in Figure 2.7.  Select the other reference handle and drag it to Edge 2.  Dimensions will be displayed as in the figure.  The other handles change the diameter of the hole and the position of the hole.  Do not modify these.

   
   [Figure 2.7]

    

6. Double click on the dimension near Edge1, change the value to 120, and hit Enter.
7. Double click on the dimension near Edge2, change the value to 100, and hit Enter.
8. Click check button. The hole will be created as shown in Figure 2.8.

   
   [Figure 2.8]

1. Select Round Tool icon from the tool bar at the right of the screen, as shown in Figure 2.9.

   
   [Figure 2.9]

    

2. Enter 10 into the textbox in the round tool bar on the dashboard.
3. Click Edge1, Edge2 and Edge3 from Figure 2.10 with the left mouse button.

   
   [Figure 2.10]

    

4. Click the check button, and you should see Figure 2.11.

   
   [Figure 2.11]

    

5. Select Chamfer Tool icon from the tool bar at the right of the screen, as shown in Figure 2.12.

    
   [Figure 2.12]

    

6. Enter 10 into the textbox in the chamfer tool bar on the dashboard.

7. Select the edge around the hole in the part, and click the check button.  If you followed the directions correctly, you should see Figure 2.13.

   
   [Figure 2.13]

    

8. Select [File] -> [Save] from menu bar to save the part.

In this section, you will use Intent Manager to create the same part that was created in the previous section.  Many people find this method easier to use - you have less work to do since Pro/E is making assumptions about the geometry you are drawing.  In future tutorials and problems, you can use either sketching method.  However, the tutorials will demonstrate the use the first method, without Intent Manager. 

1. Select [File] -> [New], and type the part name [Example2B] in Text Box.
2. Click [OK] Button.
3. Select the Extrude Tool icon from the tool bar at the right of the screen.
4. Select the Sketcher icon from the dashboard, and click the reference plane marked as FRONT.
5. Click the Sketch button from the Section menu.  Pro/E will switch to Sketch Mode.
6. Use pan and zoom operations to change the viewing so that you see the coordinates as shown in Figure 2.14.
7. Now sketch the shape of the cross-section shown in Figure 2.14. Follow the steps below:
   • Select the Line icon from the tool bar at the right of the screen.
   • Click points A and B with the left mouse button, and then press the middle mouse button.
   • Select the Arc icon from the tool bar at the right of the screen.
   • Click points B and C with the left mouse button, and then press the middle mouse button.  The letter "T" should appear near point B.  This indicates that the arc is tangent to the line.
   • Select the Line icon again.
   • Click points C, D, E, and A with the left mouse button, and then press the middle mouse button. 

     
     [Figure 2.14]

      

8. You should see dimensions drawn very faintly on the sketch.  These indicate weak dimensions, meaning they can be overridden by manually dimensioning the drawing.  You can change these dimensions by performing the steps below:
   • Select the Modify Dimension icon from the tool bar at the right of the screen.
   • Click on the dimension at point A in Figure 2.15, and change the value to 240.  You may need to pan and zoom to see the image.
   • Select the Modify Dimension icon again.
   • Click on the dimension at point B, and change the value to 65.
   • Change the value of the dimension at C to be 180 if necessary.
   • You should notice that the dimensions you changed are now shown in yellow.
   • If you wish to add dimensions in locations where there are no weak dimensions, use the Add Dimension Icon.  Manually entered dimensions will override weak dimensions.

     
     [Figure 2.15]

      

9. Click on the check button icon at the right of the screen to exit Sketcher.
10. Enter extrusion depth as 100, and click the check button.
11. Select [View] -> [Orientation] -> [Default Orientation] from menu bar. You will see the image shown in Figure 2.16.  This should be the the same part as the one created in the first section.

    
    [Figure 2.16]

     

12. Select [File] -> [Save] from menu bar to save the part.
13. Test the information you have learned in this tutorial by completing Problem 2.