ME-546 Computer Aided Manufacturing

Lesson 5 -- Shaft Tray

 

Pro/ENGINEER Functions

Cut
Blend

 

Design Objective

In this lesson you will be adding to the part created in Lesson 4. After these changes are complete, the part should resemble the one shown in Figure II.5-1.

 

Modeling Strategy

I. Use Cut to create an inclined plane on the part's top face.

II. Use Blend to cut out the slots for the shaft.

 

Detailed Construction

I. Use Cut to create an inclined plane on the part's top face.

1. Retrieve the tray:
1. MODE - Part - Retrieve
2. Enter part name: [tray]
2. Set up cut feature:
1. PART - Feature - Create - Cut - Extrude - Solid- Done - Both Sides - Done - Setup New - Plane - Pick
2. Select the plane labeled DTM 1 (refer to Figure II.5-2 ) as the sketching plane. A red arrow, pointing inward, indicates the direction of the cut to be made.
3. - Okay
4. - Top
5. - Select Plane DTM3 as shown in Figure II.5-2. This rotates the tray so that Plane DTM3 is now the top surface of the sketch (as if it were coming straight out of the screen toward you.)
3. Sketch the cut cross section:
1. Sketch line 1 as shown in Figure II.5-3.
2. Dimension the angle as shown in Figure II.5-3.
3. Align Points A and B to the part
4. Modify angle to 6.0.
5. - Regenerate - Done
   The red arrow points inward, indicating that the material in the direction of the arrow is to be cut. Since we don't want to cut away the material indicated, we need to flip the arrow.
6. - Flip - Okay
7. Thru all - Done
4. Return to the default view:
   MAIN - View - Orientation - Default - Done/Return

II. Use Blend to cut out the slots for the shaft.

A blended feature consists of a set of planar sections which are connected by transition surfaces to form a solid. These planes must be parallel to each other.

1. Create a new Datum Plane through Plane B
2. Create a cut using Blend:
1. FEAT - Create - Cut - Blend - Solid - Done - Parallel - Reg Section - Sketch sec- Done - Straight - Done
   Select Plane DTM4.
   This will be your sketching plane. Again, the red arrow indicates the direction of the cut to be made. Read the message window.
3. SKET VIEW - Bottom
1. Select Plane DTM 1.
2. Use the Sketcher to draw the first sub-section as shown in Figure II.5-4. (HINT: Use Align to align the centers of the circles to the horizontal line.)
3. - Sec Tools - Toggle
   Doing this toggles you to another sketching section. Watch how the circle changes color when you toggle.
4. Rechoose the Sketch option to create the second subsection as shown in Figure II.5-4.
5. Dimension the sketch, modify the dimensions, and regenerate.
6. - Done
   The red arrow indicates the direction of the cut to be made.
7. - Depth - From to
8. Pick the first and last surfaces to be cut.
9. Done
4. MAIN - View - Default

Your part should now look like the one referenced at the beginning of this lesson, Figure II.5-1. Don't forget to save the file.

Create an eliptical hole of aspect 2:1, minor diameter of 0.5 in the flange of the tray.