Extruding Sketches into Solids

1. From 2D Profile to 3D Solid: The Extrude Command

At its core, the Extrude command takes a closed 2D sketch profile and pulls it along a straight path to create a 3D shape. If you've ever seen how aluminum profiles are manufactured by pushing a billet through a die, the concept is very similar—you're extending a 2D shape into a 3D form.

Let's start by watching a quick demonstration of a basic extrusion.

As you saw, the process is straightforward:

1. Finish your 2D sketch.
2. Activate the Extrude tool from the Solid tab or by pressing the E key.
3. Select the closed profile(s) you want to extrude.
4. Define the distance by dragging the arrow or typing a value.
5. Click OK.

2. Practice: Giving Your VESA Plate Thickness

Let's apply this to a design you've already made.

1. Open the VESA adapter plate design you created in the last lesson's practice exercise.
2. Ensure you have exited the sketch environment by clicking "Finish Sketch" in the toolbar.
3. Press the E key to activate the Extrude command.
4. Fusion 360 will likely pre-select the main plate profile. If not, click on the area of the large square, but not inside the small circles for the holes.
5. In the Extrude dialog box, enter a distance of 3mm.
6. Click OK.

You've just created your first 3D object! Notice that because you selected the profile around the hole sketches, Fusion 360 automatically created cutouts. This is a common and efficient workflow for creating parts with holes.

3. Mastering the Extrude Options

The Extrude command is much more than a simple pull. The dialog box contains powerful options that give you precise control over your design. A deep understanding of these options is crucial for efficient modeling.

To explore these, we'll watch a detailed guide that breaks down the most important settings.

Directional Control

• One Side: The default; extrudes in one direction from the sketch plane.
• Two Sides: Allows you to specify different extrusion distances for each direction from the sketch plane.
• Symmetric: Extrudes an equal distance in both directions, keeping your sketch plane perfectly in the middle. This is extremely useful for mirrored parts or when you plan to assemble components around a central plane.

Next, let's look at how Extrude can be used to add or remove material.

Key Operations and Extent Types

• Operations:
  • Join: Adds the new extrusion to an existing solid body, merging them into one.
  • Cut: Removes the volume of the extrusion from an existing body.
  • New Body: Creates a new, separate solid body within the same component. This is useful when designing parts that are close together but are not physically one piece.
  • Intersect: Creates a solid from the shared volume of the extrusion and an existing body.
• Extent Types:
  • Distance: The standard method where you specify a numeric value.
  • To Object: Extrudes up to a selected face, surface, or point. This creates a robust relationship in your design.
  • All: Extrudes through all geometry in a given direction. Ideal for through-cuts.

Finally, let's look at two more useful features: taper angles and thin extrudes.

4. Practice: Modeling a Simple Organizer Box

Let's combine these concepts to model a simple box, a common starting point for many custom organizer projects.

1. Start a new design.
2. Create a New Component: Go to Assemble > New Component. Name it Organizer Box and click OK. Working in components is a crucial organizational habit.
3. Sketch the Base:
   • Create a sketch on the bottom (XY) plane.
   • Use the Center Rectangle tool and start from the origin.
   • Dimension the rectangle to be 80mm wide and 60mm long.
   • Click Finish Sketch.
4. Extrude the Solid Body:
   • Press E for Extrude.
   • Select the rectangle profile.
   • Set the Distance to 40mm.
   • The Operation should be New Body. Click OK.
5. Sketch the Pocket:
   • Create a new sketch, but this time, select the top face of the box you just created.
   • Use the Offset tool (O key).
   • Select the outer edge of the face.
   • Enter an offset distance of -3mm. This will create a smaller, concentric rectangle inside the first one. A 3mm wall thickness is a sturdy choice for 3D printing.
   • Click Finish Sketch.
6. Extrude the Cut:
   • Press E for Extrude.
   • Select the inner rectangle profile you just created with the offset tool.
   • Drag the arrow down into the box. Notice the operation automatically switches to Cut and the preview turns red.
   • For the Distance, enter -37mm. (This is 40mm total height minus a 3mm floor thickness).
   • Click OK.

You should now have a hollow box with 3mm walls and a 3mm floor. You created this using only two sketches and two extrude operations. This fundamental workflow is one you'll use constantly.

Conclusion

Today you've made the transition from 2D to 3D. You learned that the Extrude command is the primary tool for turning a flat sketch into a solid object.

Key Takeaways:

• Extrude (E) creates 3D geometry by adding depth to a 2D profile.
• The Operation setting determines whether you Join, Cut, or create a New Body.
• The Direction setting (One Side, Two Sides, Symmetric) provides control over how the extrusion is positioned relative to your sketch plane. Using Symmetric is a powerful technique for maintaining central datums.
• Extent Types like To Object and All create intelligent, parametric relationships that make your models more robust to changes.

In our next lesson, we will explore the second core 3D modeling tool: Revolve. While Extrude is perfect for linear or prismatic shapes, Revolve is used to create parts with rotational symmetry, like wheels, knobs, or vases, by spinning a sketch profile around a central axis.