Fusion 360 Lesson 4

5. On the Sketch panel, click Circle > Center Diameter Circle.

6. Create a 24 mm diameter circle as shown.
7. On the Sketch panel, click Line.
8. Click the left side of the circle to start the line, then drag the line upwards.

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9. For length, enter 62. Note that the line is vertical as shown by the 180.0 deg angle.

10. Click to place the endpoint of the line.
11. Drag the line to the right, then for the length enter 42.

12. Click to place the endpoint of the line. 52 | P a g e

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13. Drag the line down, then for the length, enter 25.

14. Drag the line down and hover the cursor over the circle to display the tangency symbol.
15. Click to place the endpoint of the line.

16. On the Sketch Palette, click Horizontal/Vertical, then select the two vertical lines and the
horizontal line. Constraint symbols are displayed on the lines.

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17. On the Sketch Palette, click Tangent, then select the vertical line on the left and the
circle. A constraint symbol is displayed.

18. On the ViewCube, click Home.
19. Right-click in the graphics window, then click Press Pull.
20. Select the two sections of the profile, then drag the profile upwards. For distance, enter

40.
21. Click OK.

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Step 2: Create the Side Cut-Outs
1. Rotate the part as shown.

2. On the ViewCube, click the front corner as shown.
3. Right-click the ViewCube, then select Set Current View as Home > Fit to View.

4. On the Sketch panel, click Create Sketch.
5. Select the face as shown.

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6. On the ViewCube, click Front.

7. On the Sketch panel, click Line.

8. Create a sketch as shown. Review the sketch and make sure that the lines are
constrained as shown. The line on the left is collinear with left edge of the part.

9. On the Sketch panel, click Sketch Dimension. 56 | P a g e

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10. Add a 45 mm dimension as shown.

11. Add a 5 mm dimension as shown.
12. Add a 5 mm dimension as shown.

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13. Drag the bottom edge of the sketch close to the bottom of the part.

14. On the ViewCube, click Home.
15. Right-click in the graphics window, then click Press Pull.
16. Select both sections of the profile, then drag the profile back through the part.

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17. In the Extrude dialog, from the Extents list select All. Note that the Operation is Cut
because you dragged the profile through the part.

Step 3: Add Fillets and a Hole
1. On the ViewCube, click the top-left corner.
2. On the Modify panel, click Fillet.

3. Select the edge as shown.

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4. For radius, enter 6, then click OK.

5. Right-click in the graphics window, then click Repeat Fillet.
6. Add a 3 mm fillet to the edge as shown.

9. Rotate the part as shown.

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10. On the Create panel, click Hole.

11. Select the face as shown, then drag the center point of the hole preview to the origin.

12. From the Hole Type list, select Counterbore.
• For Diameter, enter 8.25.
• For Counterbore Depth, enter 1.
• For Counterbore Diameter, enter 15.
• From the Extents list, select All.

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13. Click OK.

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Step 4: Mirror the Features 64 | P a g e
1. View the part as shown.

2. On the Construct panel, click Midplane.

3. Select the front and back faces as shown.

4. On the Create panel, click Mirror.

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5. Rotate the part then select the faces as shown. There are six faces to select.

6. In the Mirror dialog box, click Mirror plane > Select, then select the plane.
7. Click OK.
8. On the ViewCube, click Home.

9. In the browser, expand the Construction folder, then click the light bulb to turn off the
visibility of the plane.

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Step 5: Save the File 66 | P a g e
1. Click Save.
2. For Name, enter Front Fork.
3. The project is My Scooter Project.

4. Click Save.
Step 6: Model the Profile

1. On the Sketch panel, click Create Sketch.

2. Select the face of the part as shown.

3. On the ViewCube, click Front.
4. On the Sketch panel, click Offset.

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5. Select the top edge of the part, then drag the offset profile down. The profile should be
on the inside of the part as shown.

6. For Offset position, enter -3, then click OK.
7. On the Sketch panel, click Rectangle > 2-Point Rectangle.

8. Click to place the first corner as shown.

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9. Drag the preview to the corner as shown (do not click), then drag downwards below the
part. Click to place the other corner of the rectangle.

10. Rotate the part as shown.

11. In the graphics window, right-click, then select Press Pull.
12. Select the three profiles as shown.

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13. Drag the profiles back through the part, then drag the profile back through the part.

14. In the Extrude dialog box, from the Extents list, select All. Note that the Operation is Cut
because you dragged the profile through the part.

15. Click OK.

16. Save the file. Add a version number. 69 | P a g e
Step 7: Add Fillets

1. On the Modify panel, click Fillet.

2. Select the two edges as shown.

3. For radius, enter 6, then click OK.

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4. In the graphics window, right-click, then click Repeat Fillet.
5. Add 3 mm fillets to the inside edges as shown.

Step 8: Add a Hole
1. On the Create panel, click Hole.

2. Select the top surface of the part, then drag the center point of the hole preview to the
center of the part.

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3. From the Hole Type list, select Simple.
4. For Diameter, enter 25.
5. From the Extents list, select Distance.

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6. Rotate the part, then drag the hole preview through the top of the part.
7. Select the face as shown, then click OK.
8. On the ViewCube, click Home.

9. Save the file. 72 | P a g e

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Exercise: Model the Steering Clamp
In this exercise, you model the steering clamp. The clamp assembly
will be modeled using top-down assembly. That means the other
parts of the assembly, including shaft, nut, pin and arm, will be
modeled in the same file as the clamp. Each of these parts is a
body, which is then converted to a component and assembled
according to its function in the assembly.
Objectives:

• Create the body
• Create the slot in the body
• Create the outside body profile
• Create the hole
• Add fillets and chamfers
• Add a cutout for the screw
Step 1: Create the Body
1. On the Sketch panel, click Create Sketch.

2. Select the plane as shown.

3. On the Sketch panel, click Line.

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4. Click the origin, then drag the cursor to the right. Enter 35, then click to create the line as
shown. Make sure the line is at 90.0 deg as shown.

5. Drag the cursor upwards, then enter 30. Press Enter to create the line as shown.

6. Right-click in the graphics window, then click Repeat Line.
7. Create a 30 mm line as shown.

8. On the ViewCube, click Top. 74 | P a g e

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9. If required, on the ViewCube click the arrow to rotate the sketch to the position as
shown.

10. On the Sketch panel, click Arc > 3-Point Arc.

11. Click the top end of the line on the right, then click the top end of the line on the left.
12. Drag the arc upwards to create the semicircle as shown. The cursor will snap into

position when the semicircle is created.

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13. On the Sketch panel, click Circle > Center Diameter Circle.
14. Create a 25 mm diameter circle centered on the semicircle as shown.

15. On the ViewCube, click Home. 76 | P a g e

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16. In the graphics window, right-click, then click Press Pull.
17. Select the profile outside the circle, then drag the profile upwards.

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18. For Distance, enter 20, then click OK.

Step 2: Create the Slot in the Body
1. On the Sketch panel, click Create Sketch.

2. Select the top face of the part.
3. On the ViewCube, click Top.
4. If required, on the ViewCube click the arrow to rotate the view to the position as shown.

5. On the Sketch panel, click Rectangle > 2-Point Rectangle.

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6. Create a rectangle as shown.

7. On the Sketch panel, click Sketch Dimension.
8. Add a 6 mm dimension as shown.

9. On the Sketch Palette, click Midpoint.
10. Select the midpoint on the lower edge of the part. The midpoint icon is displayed when

you hover over the midpoint.

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11. Select the bottom edge of the sketch. The sketch is now located at the midpoint of the
part.

Note: The top edge of the rectangle must extend into the hole area. If it does not, drag
the top edge into the hole area.

12. On the ViewCube, click Home.
13. In the graphics window, right-click, then click Press Pull.
14. Select the profile, then drag the profile downwards through the part.

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15. In the Press Pull dialog, from the Extents list, select All.
16. Click OK.

Step 3: Create the Outside Body Profile
1. On the Sketch panel, click Create Sketch.

2. Select the top face of the part.
3. On the ViewCube, click Top.

4. If required, on the ViewCube click the arrow to rotate the view to the position as shown.

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5. On the Sketch panel, click Circle > Center Diameter Circle.

6. Create a circle as shown. It is centered on the hole.

7. On the Sketch Palette, click Equal.
8. Select the circle and the outside edge of the arc.

9. On the Sketch panel, click Line. 83 | P a g e

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10. Draw a line from the bottom edge to the edge of the hole. Make sure you do not select
the midpoint of the bottom edge. The coincident and perpendicular constraint icons
should be displayed.

11. On the Sketch Panel, click Point.
12. Place the point on the right edge of the part.
13. On the Sketch panel, click Sketch Dimension.

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14. Add a 9 mm dimension between the bottom edge and the point.

15. On the Sketch Panel, click Arc > Center Point Arc.

16. For the arc center, click on the point, then click on the lower edge about 10 mm from the
right edge. Make sure you do not click on the midpoint of the bottom edge.

17. Drag the arc close to the circle, then click to complete the arc.

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18. On the Sketch Palette, click Tangent.
19. Select the arc and the circle.

20. On the Sketch panel, click Extend.
21. Select the arc. It extends to the circle.

22. On the ViewCube, click Home.
23. In the graphics window, right-click, then select Press Pull.
24. Select the two outside profiles, then drag the profiles downwards through the part.

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25. In the Extrude dialog box, from the Extents list, select All.
26. Click OK.

27. On the ViewCube, click Home. 87 | P a g e
28. Save the file as Steering Clamp.

Step 4: Create the Hole
1. On the Sketch panel, click Create Sketch.

2. Select the side face of the part.

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3. On the ViewCube, click Front.
4. On the Sketch panel, click Circle > Center Diameter Circle.
5. Create a 5.2 mm diameter circle as shown.

6. On the Sketch Palette, click Horizontal/Vertical.

7. Select the center point of the circle and the midpoint of the vertical edge. 88 | P a g e

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8. On the Sketch panel, click Sketch Dimension.
9. Add a 9 mm dimension as shown.

10. On the ViewCube, click Home.
11. In the graphics window, right-click, then select Press Pull.

12. Select the circle, then drag the profile backwards through the part.

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13. In the Extrude dialog box, from the Extents list, select All.
14. Click OK.

15. Save the file.

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Step 5: Add Fillets and Chamfers
1. On the Modify panel, click Fillet.

2. Select the edge, then enter 3.

3. Click OK.
4. In the graphics window, click Repeat Fillet.

5. Select the edge, then enter 1.

6. In the graphics window, click Repeat Fillet.
7. Click below and to the left of the part, then drag up and to the right to create a window

around the part. All the edges without fillets are selected.

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8. For Radius, enter 0.3, then click OK. 92 | P a g e

9. Save the file.
Step 6: Add a Cutout for the Screw
1. On the Sketch panel, click Create Sketch.

2. Select the face as shown.

3. On the ViewCube, click Front.

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4. On the Sketch panel, click Circle > Center Diameter Circle.
5. Create a 17 mm diameter circle as shown.

6. On the ViewCube, click Home.
7. In the graphics window, right-click, then select Press Pull.
8. Select the circle (two profiles), then drag the profile away from the part.

9. For Distance, enter 10. 93 | P a g e

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10. Click OK.
11. Save the file.

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Exercise: Model the Clamp Screw
The first part of the steering clamp assembly is modeled, and you will use
top-down modeling to model the remaining four parts in the steering
clamp assembly. The first part is the clamp screw.
In this example, the appearance of the clamp was changed to a custom
color. Your clamp model may appear differently.
Objectives:

• Create the body
• Add chamfers and threads
Step 1: Create the Body
1. The Steering Clamp file should be open.

2. On the Construct panel, click Midplane.

3. Select the first face as shown.

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4. Rotate the part, then select the second face.

5. On the ViewCube, click Home.

6. On the Sketch panel, click Create Sketch.
7. Select the plane.
8. On the Sketch panel, click Project / Include > Project.
9. Select the inside diameter of the hole as shown.

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10. Click OK.

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11. On the Sketch panel, click Circle > Center Diameter Circle.
12. Click in the center of the projected circle, then drag to preview the circle.

13. Enter 5, then press Enter.

14. In the graphics window, right-click, then click Press Pull.
15. Zoom and rotate to view the circle as shown.

16. Select the circle. 98 | P a g e

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17. In the Extrude dialog box:
• From the Direction list, select Two Side.
• From the Operation list, select New Body.
• For Distance 1, enter 27.
• For Distance 2, enter 21.
• Click OK.

18. On the ViewCube, click Home.

Step 2: Add Chamfers and Threads 99 | P a g e
1. On the Modify panel, click Chamfer.

2. Select the edges on both ends of the clamp screw.

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3. For radius, enter 0.5, then click OK.

4. On the Create panel, click Thread.

5. Select the clamp screw on the left end.
6. In the Thread dialog box, uncheck Full Length.
7. For Length, enter 24.
8. Click OK.

9. In the graphics window, right-click, then click Repeat Thread.
10. On the ViewCube, click the top right corner as shown.

11. Select the other end of the clamp screw.
12. For Length, enter 8.

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