First Part Outline





Start the Part

Run Pro/Engineer
Select File>New


Select Part>Enter First_Part>OK

Select inlbs_part_solid>OK


You'll see this screen



Create the Extrude Feature

Select Extrude  

Select Placement>Define

Select the Front Datum Plane>Sketch


You should see the Sketcher Mode ready to select the references


Select the edges of the TOP and RIGHT Datums Planes as your Sketcher References
Select Close on the References Dialogue Box


You are ready to Sketch


Turn off the Datum Display by cliking on the Datum  Plane Display Icon

Create the Sketch below:  (Use the Dimensioning and Modify Dimension tools as needed)



Select Done from Sketcher

Enter a depth of 10.00

Preview >OK to complete the feature

Return to the Default View to see


Create the Cut Feature

Select Extrude


Select Placement>Define

Select the top surface of the top as the sketch plane>Sketch

Select the Edges Indicated as the Sketcher References > Close


Create the Sketch below



Select Done from Sketcher

Select Remove Material  and the Through All  Depth

Select Preview >OK to complete the feature



Create the Round Features

Select the Round Feature

Enter a Radius Value of .250

Select the four Edges as shown (Hold down the Control Key)


Select Preview > OK



Select the Round Feature again

Enter a Radius Value of .250

Select the two Edges as shown (Hold down the Control Key)


Select Preview > OK


Create the Chamfer Feature

Select the Chamfer Tool

Select 45 X D for the type of Chamfer and enter a value of .125 for the Chamfer Depth

Select the two top edges of the previous cut feature as shown (Hold down the Control Key)


Select Preview>OK


Create the Shell Feature

Select the Shell Tool

Enter a Thickness Value of .250

Rotate the Part and select the bottom face to be removed


Select Preview>OK


Reorder the Shell Feature

On the Model Tree, Select the Shell Feature and drag it to just after the first Extrude Feature



To produce



Return to the Default View
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Save the Part