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Cover Sheet for Exemplary Lessons/Units Project

Faculty Member Name: David Lee Date: 8/13/07

Organization: Bristol Central High School

Title of Lesson/Unit: Unit: Reverse Engineering a 3 ½” Hinge

Lesson: Creating Hinge Parts Using Solidworks

Applicable for: Technology Education Students

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Science, Technology, Engineering and Math) STEM Concepts Addressed:

This lesson is the first part of a 3 part unit involving the reverse engineering of a 3 ½” brass hinge. In this lesson the students are challenged to disassemble a typical 3 ½” hinge, apply measuring tools and skills to determine the part sizes, create a dimensioned and annotated freehand sketch of each part, then create the parts using Solidworks.

As the students examine, measure, sketch and create parts the ITEA Standards that are addressed are:

· Students will develop an understanding of the attributes of design.

· Students will develop an understanding of engineering design.

· Students will develop the abilities to use and maintain technological products and systems.

· Students will develop and understanding of and be able to select and use information and communication technologies.

Length of instruction period: 84 minutes

How many periods needed to implement lesson unit: 3

Grade Level(s) for use: 9-12

Objectives:

1. Create neat, proportional freehand sketches of each part (left leaf, right leaf and pin).

2. Select appropriate tools to obtain accurate measurements.

3. Determine where measurements should be taken to accurately describe the part.

4. Dimension and annotate the sketch.

5. Apply appropriate drawing commands to create and save the parts using Solidworks.

Materials: 3 ½” brass hinge, blank 8 ½ x 11 paper, pencil, eraser, Vernier calipers, computer with Solidworks installed.

Procedures:

Creating the sketches

· Make an isometric sketch of the assembled hinge in the full open position with the 3 ½” dimension vertical, and the countersunk holes oriented towards the front plane.

· Disassemble the hinge.

· Draw the front and top view of each component in their proper orientation. Be sure to include hidden lines and centerlines.

· Measure each component to an accuracy of 1/32” using the Vernier calipers.

· Dimension the sketch using the measurements that you have obtained.

· Annotate the sketch as follows:

o Title: 3 ½” HINGE

o Component names: LEFT LEAF, RIGHT LEAF, PIN

o Material: BRASS

o Your initials and the date.

Creating the Solidworks parts

· Select Part.

· Select Tools – Options – Document Properties

· Select Detailing – Dim Std – ANSI

· Select – Units – Inch

· Select OK

· Select Feature – Revolve Boss/Base

· Select the Front Plane

· Using the Line command draw a half profile with the vertical line on the left as a centerline and the flange on top pointing to the right.

· Smart Dimension the sketch.

· Click OK.

· In Revolve Boss/Base select the vertical line on the left as the centerline and 360 degrees for the revolution.

· Click OK.

· Under Feature Manager double click Material and change the material to Brass.

· Save the part as PIN.

In order to create the left and right leaf it becomes obvious that a single extrusion is not possible and that we will need to develop five separate sketch-extrusion elements to complete the leaf blank.

LEFT LEAF

· Select Part.

· Select Tools – Options – Document Properties

· Select Detailing – Dim Std – ANSI

· Select – Units – Inch

· Select OK.

· Select Extrude Boss/Base.

· Select the Top Plane.

· Select Rectangle and sketch a rectangle with the lower right corner at the Origin.

· Smart Dimension the rectangle to 1 15/32” wide by 3/32” high.

· Click OK.

· Extrude up a distance of 9/16”.

· Place a sketch on the top surface.

· Use the Convert command to draw the top rectangle.

· Draw a circle to the right of the rectangle with the center collinear with the bottom line of the rectangle.

· Smart Dimension the center of the circle to be 1 23/32” from the lower left corner and 3/32” down from the upper right corner. Dimension the circle to 7/16”.

· Create a concentric circle and dimension it to ¼”.

· Add a tangent line from the upper right corner to the 7/16” circle.

· Offset this line a distance of 3/32” toward the ¼” circle.

· Use Trim to extend this line and the bottom line of the rectangle so that they intersect.

· Select Line to create a line parallel to the bottom of the rectangle and passing through the concentric circles.

· Smart Dimension this line to be 1/64” below the rectangle.

· Use Trim to delete unnecessary lines to achieve the profile.

· Click OK.

· Select Extrude Boss/Base and extrude the profile up 13/16”.

· Click OK.

· Place a sketch on the top surface.

· Select Rectangle and recreate the 1 15/32” x 3/32” profile.

· Click OK.

· Select Extrude Boss/Base and extrude up a distance of ¾”.

· Click OK.

· Place a sketch on the top surface.

· Use the Convert command to draw the top rectangle.

· Use the Convert command to draw the tangent and circular entities.

· Delete the vertical line on the right of the rectangle.

· Click OK.

· Select Extrude Boss/Base and extrude the profile up 13/16”.

· Click OK.

· Place a sketch on the top surface.

· Select Rectangle and recreate the 1 15/32” x 3/32” profile.

· Click OK.

· Select Extrude Boss/Base and extrude up a distance of 9/16”.

· Click OK.

· On the Features Toolbar use Hole Wizard to create the countersunk holes.

· Under Custom set the hole diameter to 9/32”, the countersink diameter to 3/8” and the countersink angle to 90 degrees.

· Place the holes on the hinge face and Smart Dimension them as per your sketch.

· Click OK.

· On the Features Toolbar select Fillet and set the radius to ¼”.

· Select the edge of the two outside corners and click OK.

· Save the part as LEFT LEAF.

RIGHT LEAF

Use the same process as shown in the LEFT LEAF, however, start with a full profile then the 1 15/32” x 3/32” profile alternating as you build the extrusion. Use your sketch for proper orientation and dimensions.

Assessment: Students will independently measure and sketch the hinge components. A rubric will be used to assess the sketch for general presentation, accuracy, line quality and lettering. The Solidworks parts will be reviewed for compliance with the sketch.

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Resources Used: Solidworks Tutorials

Copyrighted Materials:

· None