Pro/E's assembly module allows parts to be grouped into assemblies or subassemblies to model a complete part or mechanism.  In this tutorial, you will learn how to create assemblies, apply constraints between parts, change view properties of parts, and create exploded views.  These techniques will be applied to a pulley mechanism.

1. For this tutorial, you will need the parts you created in Problem 2 and Tutorial 5.  You will also need to download the parts below.  Make sure all parts are stored in the same folder.

                    shaft.prt

                    bearing.prt

    

2. Start Pro/E Wildfire.
3. Select [File] -> [New] and choose Assembly under the Type category.  Name the assembly [Example8].
4. You will now begin to add parts to the assembly.  Select the Add Component icon from the tool bar at the right of the screen, as shown in Figure 8.1.

   
   [Figure 8.1]

    

5. Select the part you made in Problem 2.  This part will be used as a support for the pulley mechanism.
6. The Component Placement window will pop up as shown in Figure 8.2.  This window will be used to constrain the part.
7. Select [Coord Sys] from the pull down menu under the Type category, as shown in Figure 8.2.

   
   [Figure 8.2]

    

8. Select the part's coordinate system and then the assembly's coordinate system, as shown in Figure 8.3.  This will align the part and fully constrain it.

   
   [Figure 8.3]

    

9. If you have trouble locating the coordinate systems, or if you have trouble locating a datum at any point during this tutorial, you can use the icons at the tool bar at the top of the screen to select what to display.  These icons can be used to hide datum planes, axes, points, and coordinate systems.  The icons are shown in Figure 8.4.

   
   [Figure 8.4]

    

10. Select Okay from the Component Placement window.
11. Now you will add the other support.  Select the Add Component icon again, and select the part from Problem 2 again.
12. Select [Align] from the Type category in the Component Placement window.  Click near points A and B in Figure 8.5 to select the bottom surfaces of each support.

    
    [Figure 8.5]

     

13. Make sure the offset of the constraint in the Component Placement window is set to [Coincident], as shown in Figure 8.6.  If it is not set to [Coincident], double click on it and use the pull-down menu to select [Coincident].

    
    [Figure 8.6]

     

14. Now select [Mate] from the second pull-down menu in the Type category.  Click near points C and D in Figure 8.7 to select the front faces of the supports.  The second support that you just added should rotate so that the two sides face each other.

    
    [Figure 8.7]

     

15. If the offset of the constraint is set to [Coincident] or [Oriented], double click on it and change it to [0.0] as shown in Figure 8.8.

    
    [Figure 8.8]

     

16. Type [340] into the textbox, as shown in Figure 8.9, and hit the Enter key.  This will specify the distance between the two supports.  You should see the parts as shown in Figure 8.10.

    
    [Figure 8.9]

     

17. Click the plus sign icon in the Components Placement window to add a new constraint. 
18. Select [Align] from the Type menu, and select the axes of the holes of each part, as shown in Figure 8.10.

    
    [Figure 8.10]

     

19. Make sure the offset is set to [Coincident].  You should see the parts as shown in Figure 8.11.

    
    [Figure 8.11]

     

20. The Placement Status section in the Component Placement window should now say Fully Constrained.  Hit the OK button.
21. Now you will add the bearings.  Select the Add Component icon again, and select the part called bearing.prt.
22. Set the first constraint to be [Insert].  Select the outer surface of the bearing and the inner surface of the hole in one of the supports, as shown in Figure 8.12.

    
    [Figure 8.12]

     

23. Set the second constraint to be [Align].  Select the front surface of the bearing and the back surface of the support, as shown in Figure 8.13.

    
    [Figure 8.13]

     

24. Set the offset to [-7.5].  This should place the bearing inside the hole, as shown in Figure 8.14.

    
    [Figure 8.14]

     

25. The Placement Status section in the Component Placement window should now say Fully Constrained.  Hit the OK button.
26. Repeat steps 21-25 to add a bearing inside the other support.
27. Now you will add the pulley.  Select the Add Component icon again, and select the pulley you made in Tutorial 5.
28. Set the first constraint to be [Align].  Select the central axis of the pulley and the axis through the hole in one of the supports.  You may have a hard time locating the axis of the hole in the support since the bearing has many axes.  Run the cursor over the location you think it should be until you see a description of an axis that mentions Problem2, such as what is shown in Figure 8.15.

    
    [Figure 8.15]

     

29. Set the second constraint to be [Align].  Select one face of the pulley and one face of the left support, as shown in Figure 8.16.
30. Change the Offset to be [207.5].  This should place the pulley in the center of the two supports.

    
    [Figure 8.16]

     

31. The Placement Status section in the Component Placement window should now say Fully Constrained.  Hit the OK button.
32. Now you will add the shaft.  Select the Add Component icon again, and select the part called shaft.prt.
33. Set the first constraint to be [Insert].  Select the surface of the shaft and the inner surface of a bearing, as shown in Figure 8.17.

    
    [Figure 8.17]

     

34. Set the second constraint to be [Align].  Select the end face of the shaft and the back face of the support, as shown in Figure 8.18.
35. Change the offset to be [0.0]. 

    
    [Figure 8.18]

     

36. The Placement Status section in the Component Placement window should now say Fully Constrained.  Hit the OK button.  You should see the assembly as shown in Figure 8.19.

1. In this section you will modify the appearance of the parts.  Select [View] -> [Color and Appearance] from the menu bar.
2. There is currently only one appearance available - the grey shaded coloring of the parts in the assembly.  To add more colors and textures, select the plus sign arrow in the Appearance Editor window as shown in Figure 8.20.
3. Select the Color icon to alter the color of the new appearance.

   
   [Figure 8.20]

    

4. A Color Editor window will pop up, as shown in Figure 8.21.  Use the R, G, and B slide bars to change the amounts of red, green, and blue to define a new color.  Alternatively, you can select a color from the color wheel.

   
   [Figure 8.21]

    

5. Select the Close button from the Color Editor window when you are satisfied with the new color.  You can use the other slide bars in the Appearance Editor window to adjust other properties of the new appearance.
6. To set a part to this appearance, select [Components] from the Assignment category.
7. Select a part from the assembly with the left mouse button, and then click the middle mouse button somewhere on the screen.
8. Select the Apply button from the Appearance Editor window.  The part should change color, as shown in Figure 8.22.

   
   [Figure 8.22]

    

9. You can repeat this process to allow different parts to have different appearances.  An example of this is shown in Figure 8.23.

   
   [Figure 8.23]

1. In this section you will create an exploded view of the assembly.  Select [View] -> [View Manager] from the menu bar.
2. Select the Explode tab in the View Manager window.
3. Right click on the Default view and select [Explode] from the menu, as shown in Figure 8.24.

    
   [Figure 8.24]

    

4. You will see an exploded view of the assembly.  However, this view is not very good (some of the parts overlap, it is not clear where the bearings belong, etc), so you will now define your own exploded view.
5. Right click on the Default view and select [Unexplode]. 
6. Select the New button under the Explode tab, type [Exploded1], and hit Enter.
7. Right click on the Exploded1 view and select [Redefine].  This will bring up the Menu Manager.
8. Select [Position] on the Menu Manager.
9. Select [Plane Normal] as the Motion Reference in the Explode Position window.  Select a plane parallel to the support, such as the one shown in Figure 8.25.

   
   [Figure 8.25]

    

10. Click on the right support.  You can now move the mouse back and forth to move the part.  Click again farther to the right to set the new location for the support, as shown in Figure 8.26.

    
    [Figure 8.26]

     

11. Now click on the bearing and move it to the right.
12. Repeat this process for all of the parts so that they are all separated, as shown in Figure 8.27.

    
    [Figure 8.27]

     

13. Select the OK button from the Explode Position window, and select [Done/Return] from the Menu Manager.
14. You can unexplode and explode the view by right clicking on the Exploded1 view and selecting the appropriate command.
15. Select [File] -> [Save] from menu bar to save the assembly.
16. Test the information you have learned in this tutorial by completing Problem 8.