Engineering drawings are critical for communicating design ideas.  Pro/E's drawing mode allows a user to create detailed drawings of previously created parts and assemblies.  In this tutorial, you will learn the fundamentals of drawing mode while creating an annotated multiview drawing of a part.

1. Start Pro/E Wildfire.
2. Select [File] -> [New].  Select [Drawing] from the Type category of the pop-up window, name the drawing Example7, and click OK.

   
   [Figure 7.1]

    

3. A New Drawing window will pop up, as shown in Figure 7.2.  Use the Browse button set the Default Model to the part [example1.prt] that you created in the first tutorial.
4. Select [Empty with format] from the Specify Template category.
5. Select the Browse button from the Format category.  A Systems Formats folder should open.  Select a.frm from the list of formats.  This will give you a size A paper (standard 8 1/2 x 11) with a standard title block.

    
   [Figure 7.2]

    

6. Click the OK button on the New Drawing window.  You should see the view shown in Figure 7.3.

   
   [Figure 7.3]

    

7. Select [Insert] -> [Drawing View] from the menu bar.
8. Select [Done] from the Menu Manager.  This will allow you to create a typical view of the part.
9. Left click on the screen near point A shown in Figure 7.3 to locate the center of the view.  You should see the outline of the part as shown in Figure 7.4.
10. You will now be prompted to select the front view of the part.  Select plane A shown in Figure 7.4.
11. You will now be prompted to select the top view of the part.  Select plane B shown in Figure 7.4.

    
    [Figure 7.4]

     

12. Select the OK button from the Orientation window.  You should see the front of the part as shown in Figure 7.5.

    
    [Figure 7.5]

     

13. Select [Insert] -> [Drawing View] from the menu bar again.
14. Select [Done] from the Menu Manager and click near point B shown in Figure 7.5.  This will place a side view of the part to the right of the front view.  Other views could also be added to the drawing (top view, section view, orthogonal view, etc.), but the front and side views are all that is necessary to show all the features for this part.
15. Right click on the Layers branch of the Layer Tree at the left of the screen, and select [Blank Layer].  This will remove the coordinate axis and view plane data from the drawing, and you should see the view shown in Figure 7.6.

    
    [Figure 7.6]

1. Double click on SCALE at the bottom of the screen, and change it to 0.01.  This will make the views of the part slightly larger.

   
   [Figure 7.7]

    

2. Select [View] -> [Show and Erase] from the menu bar.
3. Select the Dimension Icon from the Type category in Show/Erase window, as shown in Figure 7.8.
4. Select Part and View from the Show By category.
5. Make sure Erase and Never Shown are checked in the Options category.  This will allow all dimensions which are not currently shown to be displayed.

   
   [Figure 7.8]

    

6. Select the Show All button from the Show By category.  Select Yes when prompted to confirm.  Select the Accept All button from the Preview category of the Show/Erase window.
7. Select the Close button to close the Show/Erase window.  You should see all the dimensions of the part as shown in Figure 7.9.

   
   [Figure 7.9]

    

8. Click somewhere on the screen to deselect all the dimensions.
9. Now move the dimensions so that they are easier to read.  Use the mouse to select a dimension in the front view, and then use the mouse to drag it.  Do this for all dimensions, so that you see the view shown in Figure 7.10.
10. Repeat this process for the dimensions on the side view of the part.

    
    [Figure 7.10]

     

11. Since the front view of the part is somewhat cluttered, you can move the some dimensions to the side view.  Left click on the dimension which labels the height of the cut as 100.
12. Select [Edit] -> [Move Item to View] from the menu bar.
13. Click somewhere inside the side view of the part.  The dimension should now be shown in that view, as shown in Figure 7.11.

    
    [Figure 7.11]

     

14. Use the mouse to draw a selection box around both of the views to select all the dimensions.  The dimensions should be shown in red.
15. Select [Edit] -> [Cleanup] -> [Dimensions] from the menu bar.
16. Select the Apply button from the Clean Dimensions window.  This will set the location of the dimensions to be a consistent distance from the part.
17. Select the Close button from the Clean Dimensions window.  You should see the dimensions as shown in Figure 7.12.

    
    [Figure 7.12]

     

18. To reposition the views so that they better fill the page, select [Tools] -> [Environment] from the menu bar.
19. Uncheck the box that says Lock View Movement and click the OK button.
20. You can now click on a view and drag it to a new location.  Notice that the side view always stays aligned with the front view.
21. To add tolerances to the dimensions, select [File] -> [Properties] from the menu bar.  Select [Drawing Options] from the Menu Manager.
22. An Options window will appear.  This window is useful for changing many properties of the drawing including text, view, and dimension properties.
23. Type [tol_display] into the Options text box and hit Enter.  Use the pull-down menu next to the text box to change the value to [Yes]. 
24. Click the Add/Change button, and then click the OK button.

    
    [Figure 7.13]

     

25. Select [Done/Return] from the Menu Manager.
26. Select [Edit] -> [Regenerate] -> [Model] from the menu bar.  You should see tolerances as shown in Figure 7.14.

    
    [Figure 7.14]

     

27. To change the type of tolerancing, left click on a dimension to select it.  Select [Edit] -> [Properties] from the menu bar.
28. Change the Tolerance Mode to [+- Symmetric] and click the OK button. The dimension will be shown as in Figure 7.15.

    
    [Figure 7.15]

     

1. In this section you will fill in the title block of the drawing.  Select [Insert] -> [Note] from the menu bar.
2. Select [Make Note] from the Menu Manager and click near point A shown in Figure 7.16.  Type [Carnegie Mellon University] into the text box at the bottom of the screen and click the check button twice.

   
   [Figure 7.16]

    

3. Select [Make Note] again and click near point B.  Type the part name [Part 1] into the text box, and click the check button twice.
4. Repeat this process to add [Drawing No. 001] at point C, [SCALE 0.01] at point D, and your name at point E. 
5. Select [Done/Return] from the Menu Manager.
6. Use the mouse to click and drag the notes to position them at the center of the boxes so that they look like those shown in Figure 1.17.

   
   [Figure 7.17]

    

7. Now change the size of the text.  Select the Scale note and select [Format] -> [Text Style] from the menu bar.
8. In the Text Style window, uncheck the box labeled Default for the height of the text.  Change the value to 0.09, as shown in Figure 7.18.  Click the OK button.

    
   [Figure 7.18]

    

9. Click the OK button on the Text Style window.  The note should now fit in the box as shown in Figure 7.19.

    
   [Figure 7.19]

    

10. Select [File] -> [Save] from the menu bar to save the drawing.
11. Test the information you have learned in this tutorial by completing Problem 7.