Assignment 2

  • Click New from the main toolbar and select Part as the Type. Type INDEX_SLIDE as the Name and press ENTER.
  • Click Datum Axes , Datum Points , and Coordinate Systems from the main toolbar (top of the screen) to disable their display.
  • To setup units, select from the pull down menu EDIT SETUP  UNITS millimeter Kilogram second (mmKs)  Set Convert dimensions (for example 1” becomes 25.4mm) OK  CLOSE.

Task 3-1. Create shape for main body

1)Start the Sketch Tool from the feature toolbar (right of the screen).

2)Select datum plane FRONT from the model, and click Sketch from the Sketch dialog box.

3)By default F1 (Right) and F2 (Top) are being selected as the dimension reference. Click CLOSE from the References dialog box.

4)Begin sketching the shape of the main body. Make a rectangle shape first, then make lines and connect them to make the shape.


Create basic rectangular shape /
Make a long vertical line of reference 11 mm from rectangles side

Make the 2 slanted lines of 30º (Refer Assg1) by:
1)Starting from top corner of rectangle to vertical line
2)Modify angle value accordingly
3)Starting from bottom corner of rectangle to vertical line
4)Modify angle value accordingly /
Delete the long vertical line, and connect the 2 ends of the slanted lines

Make sure you DELETE the vertical line! So the result will look like this
  • Click Complete Sketch from the sketcher toolbar (right of the screen).
  • Click Saved View List from the main toolbar and select Standard Orientation.
  • Click Datum Planes from the main toolbar to enable their display
  • Start the Extrude Tool from the feature toolbar (right of the screen).
  • Click theblack arrow on the Depth Options Flyout in the dashboard (bottom of the screen) and select Both Sides .
  • Type 28 (length) in the dashboard and for the depth and press ENTER.
  • Click Refit from the main toolbar (top of the screen).
  • Click Complete Feature from the dashboard (bottom of the screen). SAVE NOW!!

Task 3-2. Removing Materials from the top

1)Set the view to FRONT.

2)Start the Sketch Tool from the feature toolbar (right of the screen).

3)For datum plane, manually select the Top Surface from the model (see example below), make sure orientation is RIGHT and click Sketch from the Sketch dialog box.

4)By default F1 (Right) and F2 (Top) are being selected as the dimension reference. Add reference, by clicking top ledge, bottom ledge and left ledge. Click CLOSE from the References dialog box.

5)Begin sketching. Make a vertical reference line 11 mm from the left ledge. (shown below)

6)Create arc by picking its center and endpoints. Use this icon



= CLICK HERE
First pick the center of the arc. Make sure its center is on the centerline… click anywhere on the centerline (modify later) /
Then click at the intersection between the vertical line created and top ledge… then click at the intersection between vertical line created and bottom ledge.

7)Modify the radius to be = 95 mm

8)Create the other arc by using the same arc-center. Set its radius to be 70 mm.

9)Create 2 horizontal line to complete the shape


DO NOT delete the vertical line YET !!!!! /
Create a rectangular box as shown.
Modify the dimension where is to be 1 mm
(Refer to drawing as to why)
NOW delete the first vertical line created
  • Click Complete Sketch from the sketcher toolbar (right of the screen).
  • Click Saved View List from the main toolbar and select Standard Orientation.
  • Click Datum Planes from the main toolbar to enable their display
  • Start the Extrude Tool from the feature toolbar (right of the screen).
  • Click on . Set extrusion length to 6mm. Make sure direction is correct by rotating an inspecting. If wrong direction, change it by using .
  • Direction is into the solid (we want to remove material)
  • Click Remove Material from the dashboard, and then clickComplete Feature
  • Don’t use this method if for example…both extrusion are of different depth

Task 3-3. Holes

1)Set the view to FRONT.

2)Start the Sketch Tool from the feature toolbar (right of the screen).

3)For datum plane, select FRONT, make sure orientation is RIGHT and click Sketch from the Sketch dialog box.

4)By default F1 (Right) and F2 (Top) are being selected as the dimension reference. Add reference, by clicking top ledge, bottom ledge and left ledge. Click CLOSE from the References dialog box.

BIG HOLE


For big hole, create a vertical line (just temporary for reference). This vertical line and the horizontal centerline should intersect where the center of the circle should be.
Determine the length of x.xx mm.
x.xx mm is the horizontal length from centerline to circle center
(Refer to assignment) /
Create circle of diameter 28.6mm
Delete the vertical line

SMALL HOLES


Create a horizontal line starting from where the is.
Length of line = 95 mm. The other end will be the arc’s center. /
Using the arc’s center, create the middle arc line with
Radius = 82 mm
Delete the horizontal line.

Create 2 horizontal line (for reference where the circle’s center should be)
Both lines are 16 mm from centerline /
After determining the circle’s center, create circles.
Diameter = 10 mm

Delete all the unnecessary lines, resulting sketch should look like picture above
  • Click Complete Sketch from the sketcher toolbar (right of the screen).
  • Using extrusion (material removal), create these holes

Task 3-4. Removing Materials from the top (Groove)

1)Set the view to STANDARD.

2)Start the Sketch Tool from the feature toolbar (right of the screen).

3)For datum plane, select EDGE’s surface (refer to picture) , make sure orientation is BOTTOM and click Sketch from the Sketch dialog box.

4)By default F1 (Right) and F2 (Top) are being selected as the dimension reference. Add reference you desire. Click CLOSE from the References dialog box.

5)Sketch the shape that we want to remove

6)Remove by extrusion…

Print according to the instructions on the white board.

Congratulations, you have finished yet another 6% of your grade