Advanced 3D Drawing

Fusion 360 contains many modelling tools beyond basic sketches and extrusions. This chapter introduces several of the most useful ones.

• 1. Planes and Axes
  • Exercise 1
  • Exercise 2
• 2. Mirror and Pattern
  • Exercise 1
• 3. Shell
  • Exercise 1
• 4. Loft
  • Exercise 1
  • Exercise 2
  • Exercise 3
• 5. Revolve
  • Exercise 1: Printed Bearing
  • Exercise 2
• 6. Sweep
  • Exercise 1
  • Exercise 2
• 7. Combined Exercise
  • Exercise 1

1. Planes and Axes

Construction planes are frequently used to place sketches away from existing faces.

1. Offset Plane: creates a plane parallel to a selected face at a specified distance.
2. Midplane: creates a plane halfway between two faces, particularly useful for mirroring.
3. Plane Through Two Edges / Plane Through Three Points: defines a plane from existing geometry, often for splitting a solid.

Exercise 1

1. Sketch the base in Front view.
2. Extrude it symmetrically by 65 mm.
3. Use Plane at Angle to create a plane at 30°.
4. Sketch on the angled plane and extrude the feature.
5. Show Sketch2 again and cut the hole down to the bottom as specified.

Exercise 2

Each grid square represents 10 × 10 mm.

1. On the front plane, sketch the rectangle and define the first sloping face.
2. Extrude the full profile by 40 mm.
3. Sketch the second slope on the side face.
4. Show both sketches and create Plane Through Three Points.
5. Use Split Body, then hide the plane and unwanted corner.

2. Mirror and Pattern

Mirror and Pattern reproduce repeated features accurately and efficiently.

Exercise 1

1. Sketch a 130 × 80 mm centre rectangle on XY and extrude it 50 mm.

   

2. On top, sketch a 30 × 25 mm rectangle and cut it 30 mm deep.

   

3. Run Mirror, choose Feature, select the cut and use the YZ plane.

4. Mirror again, selecting both the original cut and first Mirror feature, across XZ.

5. Press H, place a hole 15 and 12 mm from the two edges, set Extent to All, Hole Type to Counterbore, Tap Type to Simple, and use any drill point because it is through-all.
6. 4 HOLES Ø8 THRU ALL ⌴Ø18 ↧3 means four 8 mm through-holes with an 18 mm counterbore 3 mm deep.

7. Use Rectangular Pattern with type Feature, select the Hole feature, choose the two directions and set spacing to 100 mm and 56 mm.

8. Create the central circular opening either by sketching the semicircles and cutting them, or with Hole.

9. Create the final threaded hole 15 and 40 mm from the edges. Choose Simple hole, Tapped, the pointed drill tip, M12 × 1.5 and Modeled threads.

10. Mirror the threaded hole across YZ; use Optimized as the Compute Option so the complete threaded feature is mirrored.

11. Sketch on the front and remove the specified region with Extrude.

12. Apply 2 mm fillets to the specified edges.

3. Shell

Shell removes selected opening faces and gives the remaining solid a specified wall thickness, avoiding a separate offset body and Boolean subtraction.

Exercise 1

Hints

Create and extrude the base.

Create one cylinder and use Rectangular Pattern to make eight.

Sketch the three lower cylinders from underneath. They stop 1.2 mm above the very bottom of the LEGO-style part.

4. Loft

Loft joins profiles of different shapes and sizes. It is useful for transitions such as round-to-square ducts. Profiles can be connected directly or guided by rails/centre lines.

Exercise 1

1. On XY, draw a circle of radius 170 mm and extrude it 40 mm.

2. Offset a plane 315 mm from the cylinder top.
3. On it, draw a 170 mm-diameter circle whose centre is 225 mm from the origin.

4. Loft between the upper circle and cylinder top, with no Rails.

5. Extrude the upper circle 40 mm, then mirror the last two features.

6. Shell the model inward by 2 mm, selecting both upper circular faces and the bottom circle as openings.

Exercise 2

Hints

Exercise 3

📝NOTE

The drawing is dimensioned in inches. Search for Change Active Units and switch the design to inches.

Hints

5. Revolve

Revolve is the CAD equivalent of turning on a lathe: a profile rotates around an axis to form a solid.

Exercise 1: Printed Bearing

Bearings are standard-sized components and often determine a design's dimensions. Large commercial bearings become expensive quickly. For low-speed, low-precision applications, a printed bearing can use readily available Ø4.5 mm stainless-steel balls.

1. On XZ, create a 6 × 6 mm centre rectangle with its edge 20 mm from the origin. The 20 mm radius gives a 40 mm bore. Add a Ø4.8 mm circle, a centreline and the two symmetric lines with a 0.5 mm gap.
2. Revolve the solid profile 360° about Z.

⚠️WARNING

If two Revolve commands appear, choose the blue solid command. The orange command creates only a surface.

3. Sketch on XY. Press P to project two edges as points, add a centreline and draw a Ø4.8 mm circle.
4. Cut the ball channel with Extrude.

5. Chamfer the four circular edges by 0.5 mm.

6. Use Sphere to create a Ø4.5 mm ball at the origin.
7. Move it 23 mm along X.

8. Use Circular Pattern to make 30 balls around the axis.

Exercise 2

Model this common 8 mm linear bearing used in 3D printers.

6. Sweep

Sweep moves a profile along a path.

Exercise 1

1. On XZ, sketch the pipe centreline to the drawing dimensions.

2. On YZ, sketch the Ø25 mm outside profile.

3. Sweep the circle as Profile along the centreline Path.

4. Shell through both ends with 2.5 mm wall thickness.

5. On one end, sketch the Ø45 mm flange and extrude it 7.5 mm.

6. Sketch the six mounting holes on the flange.
7. Cut them with Extrude set to To Object, selecting the rear flange face.

8. Repeat on the other end.

Exercise 2

💡TIP

This exercise requires Plane Along Path.

7. Combined Exercise

This final problem combines several modelling tools.

Exercise 1

Hints

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