Fusion 360 Lesson 4

Introduction to CAD for Engineers

Step by Step Guide
Lesson 4: Model

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About This Lesson

In this lesson, you model many of the parts required for the kick scooter. You start the part
design by creating a parametric sketch, then use constraints and dimensions to capture the
design intent.

The model is typically built using the Press Pull functionality and further refined using one of the
many modify tools such as Fillet, Chamfer, and Hole.

Note: The My Scooter Design project and datasets are required for this project. If you have not
created the project or uploaded the files, refer to the Getting Started section.

Objectives:

In this lesson, you:

• Model scooter parts using parametric modeling techniques
• Use top-down modeling techniques

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Exercise: Model the Bearing Ring
In this exercise, you model the bearing ring. Two of these parts are
used in the kick scooter and assembled onto the front fork as part of
the steering column.
Objectives:

• Create the body
• Add fillets and chamfers
• Save the file
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 Circle > Center Diameter Circle.

4. Click the origin to locate the center, then drag the cursor to preview the circle.
5. For diameter, enter 46, then press Enter.

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6. In the graphics window, right-click, then select Repeat Center Diameter Circle.
7. Create a 25 mm diameter circle as shown.

8. In the graphics window, right-click, then select Press Pull.
9. Drag the area between the two circles, then enter 6.

10. Click OK.

11. On the Sketch panel, click Create Sketch.

12. Select the top face of the part.
13. On the Sketch panel, click Circle > Center Diameter Circle.

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14. Create a 34 mm diameter circle as shown.

15. In the graphics window, right-click, then select Press Pull.
16. Drag the area between the two circles, then enter 4.

17. Click OK. 6|Page

Step 2: Add Fillets and Chamfers
1. On the Modify panel, click Fillet.

2. Select the edge as shown.

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3. For radius, enter 4, then click OK.
4. On the Modify panel, click Chamfer.

5. Select the two edges edge as shown. Hold down the CTRL key to select the second
edge.

6. For Radius, enter 1, then click OK. 7|Page

Step 3: Save the File
1. Click Save.

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2. For Name, enter Brake Spring.

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3. The project is My Scooter Project.

4. Click Save.
Exercise: Model the Front Wheel Carrier
In this exercise, you model the front wheel carrier that is a component in the front
fork assembly.
Objectives:

• Create the body
• Add a thread
• Add a chamfer
• Save the file
Step 1: Create the Body
1. On the Sketch panel, click Create Sketch.

2. Select the plane as shown.

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3. On the Sketch panel, click Circle > Center Diameter Circle.
4. Click on the origin, then create a 25 mm diameter circle as shown.

5. In the graphics window, right-click, then select Press Pull.
6. Drag the circle upwards, then enter 130.
7. On the ViewCube, click Home.

8. On the Sketch panel, click Create Sketch. 10 | P a g e

9. Select the top face of the part as shown.

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

11. Click the origin, then create a 34 mm diameter circle as shown.

12. In the graphics window, right-click, then select Press Pull.
13. Select the two circles, then drag the circle upwards. Enter 5.
14. Click OK.

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Step 2: Add a Thread
1. On the Create panel, click Thread.

2. Select the lower face of the part.

3. In the Thread dialog box, uncheck Full Length.
4. For Length, enter 70, then click OK.

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Step 3: Add a Chamfer
1. On the Modify panel, click Chamfer.

2. Select the edge as shown.

3. For Distance, enter 2, then click OK.

4. In the graphics window, right-click, then click Repeat Chamfer.
5. Select the edge as shown.

6. For Distance, enter 1, then click OK. 14 | P a g e

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7. On the ViewCube, click OK.

Step 4: Save the File
1. Click Save.
2. For Name, enter Front Wheel Carrier.
3. The project is My Scooter Project.

4. Click Save.

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Green Material Selection

Now that you have modeled two parts for the kick scooter, you need to consider what material
to select for these parts and for the remaining parts of the scooter. Let’s look at the front wheel
carrier as an example. By default, Autodesk Fusion 360 uses steel for the part material.

Introduction to Green Materials Selection

Thanks to advances in material science, today’s engineers and designers have more options for
choosing greener materials. Choosing more sustainable materials often means making informed
tradeoffs. To make an informed choice, you need good data on a material’s environmental
impacts, and you need to consider that data alongside other design requirements.

See more at: Green Materials Selection

Environmental Properties

When considering the environmental properties of materials, look for materials that are
abundant, non-toxic, have low embodied energy, and meet or exceed regulations.

See more at: Environmental Properties of Materials

Physical Properties

You also need to ensure that the material has the right physical properties to get the job done
and that it won’t drive up costs.

See more at: Physical Properties of Materials

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Exercise: Model the Headstock Nut Lower
In this exercise, you model the headstock nut for the lower part
of the kick scooter. The nut is used to hold the bearings rings
onto the front fork assembly.
Objectives:

• Create the polygon feature
• Create the main body
• Add a chamfer and fillets
• Add a beveled edge using a sketch
• Add a threaded hole
Step 1: Create the Polygon Feature
1. On the Sketch panel, click Create Sketch.

2. Select the plane as shown.

3. On the ViewCube, click Top.

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4. If required, click the arrow to rotate the axes as shown.

5. On the Sketch panel, click Polygon > Circumscribed Polygon.

6. Click the origin to locate the center, then drag the cursor vertically upwards to preview
the polygon.

7. For diameter, enter 18, then press the TAB key. Enter 8 for the number of sides.

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8. Click in the graphics window to place the polygon.

9. On the Sketch Palette, click Horizontal / Vertical.
10. Select the top edge of the polygon. A constraint symbol is added to the line.

11. On the ViewCube, click Home.
12. In the graphics window, right-click, then select Press Pull.
13. Drag the polygon, then enter 5.
14. Click OK.

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

2. Rotate the part, then select the bottom face.

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

4. Create a 48 mm diameter circle as shown.

5. In the graphics window, right-click, then select Press Pull.
6. Select both profiles then drag down.
7. Enter 7, then click OK.

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Step 3: Add a Chamfer and Fillets
1. On the ViewCube, click Home.
2. On the Modify panel, click Chamfer.

3. Select the edge as shown.

4. In the Chamfer dialog, box, from the Chamfer Type list, select Two Distances.

5. For distance 1 enter 1.25, and for distance 2 enter 4.25. Click OK.

7. On the Modify panel, click Fillet.

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8. Select the 8 edges as shown.

9. For radius, enter 0.25, then click OK.

Step 4: Add a Beveled Edge
1. On the Construct panel, click Plane Through Two Edges.

2. Select the edge as shown. 22 | P a g e

3. Select the second edge as shown.

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4. On the Sketch panel, click Create Sketch.
5. Select the plane.
6. In the browser, expand the Sketches folder.
7. Right-click the last plane, then click Slice Sketch.

8. On the ViewCube, click Right.

9. On the Sketch panel, click Project / Include > Project.

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10. Select the two edges as shown, then click OK.

11. Zoom into the projected lines.
12. On the Sketch panel, click Line.
13. Draw a line close to the right corner as shown.

14. On the Sketch panel, click Sketch Dimension.
15. Add 1.25 mm dimensions as shown.

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16. On the ViewCube, click Home.
17. Zoom into the sketch profile.

18. On the Create panel, click Revolve.

19. Select the profile.

20. In the Revolve dialog box, click Axis > Select.
21. In the browser, expand the Origin folder then select Y.

22. Click OK. 26 | P a g e

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23. On the ViewCube, click Home.

Step 5: Add a Chamfer
1. On the Modify panel, click Chamfer.

2. In the Chamfer dialog box, from the Chamfer Type list, select Equal Distance.
3. Select the top and bottom edges as shown.

4. For Distance, enter 0.5.
5. Click OK.

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Step 6: Add a Threaded Hole
1. On the Create panel, click Hole.

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

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

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6. Click OK.
7. On the Create panel, click Thread.

8. Select the face of the hole, then click OK. 29 | P a g e

Step 7: Save the File
1. Click Save.
2. For Name, enter Headstock Nut Lower.

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3. The project is My Scooter Project.
4. Click Save.

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Exercise: Model the Brake Spring

In this exercise, you model the brake spring using the coil command.
The spring is used in the brake assembly to return the rear mud guard
back to its starting position after the rider has pressed on the mud
guard, which acts as the brake.

Objectives:

• Create a coil
• Modify the coil
• Save the file

Step 1: Create a Coil

1. On the Create panel, click Coil.

2. Select the plane as shown.
3. Click the origin, then drag to create a circle. For the circle diameter, enter 8. Press Enter.

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4. In the Coil dialog, enter the following values:
• For Type, select Revolution and Pitch from the list
• For Revolutions, enter 4.
• For Pitch, enter 2.25.
• For Section Size, enter 2.

5. Click OK. 32 | P a g e

Step 2: Modify the Coil
1. On the ViewCube, click Home.
2. On the Sketch panel, click Create Sketch.

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3. Select the face of the coil as shown.

4. In the graphics window, right-click, and then select Press Pull.
5. Drag the face, then enter 15.

6. Click OK. 33 | P a g e
7. Rotate the model to view the second face.

8. On the Sketch panel, click Create Sketch.

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9. Select the face of the coil as shown.
10. In the graphics window, right-click, then select Press Pull.
11. Drag the face, then enter 15.

12. Click OK. 34 | P a g e
13. On the ViewCube, click Home.

Step 3: Save the File
1. Click Save.
2. For Name, enter Brake Spring.
3. The project is My Scooter Project.

4. Click Save.

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Exercise: Model the Lower Steering Clamp
In this exercise, you model the clamp that is used to connect
the steering column to the front fork assembly.
Objectives:

• Create the body
• Create a slot in the body
• Create the outside profile of the body
• Add chamfers and fillets
• Add a counterbore hole
• Add a threaded hole
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.

4. Click the origin, then drag the line to the right.
5. Enter 42, then click to place the endpoint.
6. Drag the line vertically upwards, then enter 31.

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7. Press Enter.

8. In the graphics window, right-click, then click Repeat Line.
9. Draw a 31 mm line at the left side of the sketch.

10. View the sketch as shown.

11. On the Sketch panel, click Arc > 3-Point Arc. 36 | P a g e

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

position when the semicircle is created.

14. On the Sketch panel, click Circle > Center Diameter Circle.
15. Create a 28 mm diameter circle as shown.

16. On the ViewCube, click Home. 37 | P a g e

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17. In the graphics window, right-click, then select Press Pull.
18. Select the profile outside the circle.

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19. Drag the profile upwards, then enter 16.

20. Click OK.
Step 2: Create a Slot in the Body

1. On the Sketch panel, click Create Sketch.

2. Select the top face of the body.
3. View the body as shown.

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

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5. Create a rectangle as shown.

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

8. On the Sketch Palette, click Midpoint.
9. 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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10. 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.

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

14. In the Press Pull dialog, from the Extents dialog, select All. 41 | P a g e

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15. Click OK.

Step 3: Create the Outside Profile of the Body
1. On the Sketch panel, click Create Sketch.
2. Select the top face of the body.
3. View the body as shown.

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

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5. Draw a 20 mm diameter circle in the slot as shown. Make sure the center is above the
bottom edge.

6. On the Sketch panel, click Sketch Dimension.
7. Add a 1 mm dimension between the bottom edge and the center of the circle as shown.

8. On the Sketch Palette, click Horizontal/Vertical.
9. Select the center of the circle and the center of the large circle above.

10. On the ViewCube, click Home. 43 | P a g e

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11. Select the two profiles, then drag the profile downwards through the part.

12. In the Press Pull dialog, from the Extents list, select All.
13. Click OK.

Step 4: Add Fillets and Chamfers
1. On the Modify panel, click Fillet.
2. Select the four edges as shown.

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3. For radius, enter 8, then click OK.
4. On the Modify panel, click Chamfer.
5. Select the outside edge.
6. Enter 0.75, then click OK.

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7. Add 0.75 mm chamfers to the top and bottom edges of the hole as shown.
8. Add 0.5 mm fillets to the edges as shown.

9. Save the drawing as Lower Steering Clamp.
Step 5: Add a Counterbore Hole

1. On the Create panel, click Hole.

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2. Select the front face of the part, then drag the center point of the hole preview to the
center of the arc.

3. In the Hole dialog box:
• From the Type list, select Counterbore.
• For Diameter, enter 6.
• For Counterbore Depth, enter 6.5
• For Counterbore Diameter, enter 10.
• From the Extents list, select All.

4. Click OK. 47 | P a g e

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5. Add a 0.75 mm chamfer to the edge of the hole as shown.

Step 6: Add a Threaded Hole
1. On the Create panel, click Thread.
2. Select the hole on the right side of the body.

3. Click OK.

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4. On the ViewCube, click Home.
5. Save the file.

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Exercise: Model the Front Fork
In this exercise, you model the front fork. This component is assembled to
the steering column and then has the wheel assembly inserted.
Objectives:

• Create the body
• Create the side cut-outs
• Add fillets and a hole
• Mirror the features
• Save the file
• Model the profile
• Add fillets
• Add a hole
Step 1: Create the Body
1. On the Sketch panel, click Create Sketch.

2. Select the plane as shown.

3. On the ViewCube, click Top.

4. If required, click the arrow to rotate the axes as shown.

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