ME-546 Computer Aided Manufacturing

Lesson 4 -- Shaft Tray

 

Pro/ENGINEER Functions

Sweep           Hole
Round           Pattern

 

Design Objective

In this lesson you will create a shaft tray like the one shown in Figure II 4-1that results from sweeping a cross section along a trajectory section.

 

Modeling Strategy

I. Use Sweep to create a trajectory and a cross-section.

II. Use Round to add curvature to the lower vertical edges of the part.

III. Use Hole and Pattern to create the four identical holes on the base.

 

Detailed Construction

I. Use a cross-section along a trajectory to sweep a 3D solid object.

1. Begin a new part:
1. MAIN - Mode - Part - Create
2. Enter Part name: [tray]
2. Define the solid feature:
1. PART - Feature - Create - Solid - Protrusion - Sweep - Solid - Done
3. Create the Sweep trajectory:
1. Use the sketcher to draw the trajectory displayed in Figure II.4-2 .
2. Refer to Figure II.4-3 to dimension the sketch, modify the dimensions, and regenerate.
3. - Done
4. - No Inn Fcs - Done
   The No Inn Fcs option specifies that no top or bottom faces will be added to the part. It also means that a closed cross-section is required, but any trajectory can be used. Also note the warning which appe ars in the message window, stating that you must sketch the trajectory first. Look carefully for the arrow indicating the plane and direction Pro/E expects the soon to be created section to appear in.
4. Create the cross-section:
   Two dotted crossing lines or "crosshairs" should appear. These are really hard to see because they tend to get lost among the grid lines!!
1. Use the sketcher to draw the cross-section displayed in Figure II.4-4.
   Be sure that the lower left-hand corner of the cross-section is aligned with the center of the crosshairs. The regenerated object appears, in a much smaller scale, on the screen.
2. Dimension the sketch, modify the dimensions, and regenerate.
3. - Done
4. MAIN - View - Orientation - Default - Done/Return

II. Use Round to add curvature to the lower vertical edges of the part.

1. Round all the corners:
1. FEAT - Create - Solid - Round - Simple - Done - Query Sel
2. Select the four short edges to be rounded.
   Query Sel enables you to select hidden geometry, and, in complicated models, entities that are difficult to select using the default option. It will highlight the entity closest to that which you select. If you want the entity that is currently highlighted, choose Accept from CONFIRM. If the highlighted entity is not the one you intended, choose Next from CONFIRM, and Pro/ENGINEER will highlight the next closest entity. Continue using Next until the entity you want is highlighted.
3. - Done Sel - Done - Enter
4. - Enter Radius [ 0.25 ]
5. -OK
   The four rounded corners should appear on the tray.

III. Use Hole and Pattern to create the four identical holes on the base.

1. First, you may wish to remove the hidden lines from the display:
   MAIN - Environment - No hidden - Done/Return
2. Create the first hole:
1. FEAT - Create - Solid - Hole - Straight - Done - Linear - Done
2. Create a DTM corresponding to Plane A in Figure II.4-5.
   This is the surface where the holes will be placed.
3. Pick location on screen where hole will go
4. Select first DTM to dimension from as shown in Figure II.4-5.
5. Enter distance from reference [ 5]
6. Select second DTM to dimension from as shown in Figure II.4-5.
7. Enter distance from reference [ 8]
8. Enter diameter [ 0.35 ]
   The first hole is created; it will appear in the corner of the tray.
3. Zoom in on the hole and the area around it:
1. MAIN - View - Pan/Zoom
   - Indicate two locations to define a box for the Zoom area (use the left mouse button).
2. - Done/Return
4. Create the four-hole pattern:
1. FEAT - Pattern - Query Sel
2. Select the existing hole.
3. - Accept or Next
4. - Identical - Done
5. Select "5.0", the dimension parallel to Edge A.
6. Enter dimension increment: [ -10]
7. EXIT - Done
8. Enter total number of holes ( including original) : [ 2 ]
9. Select "8", the dimension parallel to Edge B.
10. Enter dimension increment: [ -16 ]
11. - Done
12. Enter total number of holes (including the original one) : [ 2 ]

If the pattern fails, try 10 and/or 16 for the increments; your choices for DTM were different.

5. Return to the default view:
   MAIN - View - Orientation - Default - Done/Return
6. Save the file:
   MAIN - Dbms - Save - Press RETURN

Your part should now look like the one referred to back at the beginning of this lesson, Figure II.4-1.

Insert a shaded rendering of your part into an MSWord document and submit with your part file.