Shelling a Solid Body

1. What is the Shell Command?

The Shell command takes a solid body and carves out its interior, leaving behind a "shell" with walls of a uniform thickness that you define. You can either create a completely hollow, closed object or remove one or more faces to create an open container.

The tool is located in the Modify dropdown menu in the Solid workspace toolbar.

2. Basic Application: Open vs. Closed Shells

There are two fundamental ways to apply the Shell command, and the result depends entirely on what you select.

1. Shelling a Closed Body: If you select the entire body from the Browser tree on the left, Fusion 360 will hollow out the inside, leaving no opening. This is useful for creating parts that are lightweight but appear solid from the outside.
2. Shelling an Open Body: If you select one or more faces on the model itself, Fusion 360 will remove those faces and then hollow out the interior from that opening. This is the standard method for creating boxes, cases, and containers.

This video provides an excellent demonstration of these two approaches.

Practice: Your First Shell

Let's try this yourself.

1. Create a new design.
2. Create a basic solid body: sketch a 50mm x 50mm square and Extrude it up by 50mm to form a cube.
3. Closed Shell:
   • Activate the Shell tool (Modify > Shell).
   • In the Browser, click on the Body1 icon to select the entire cube.
   • Enter a thickness of 3mm. Click OK.
   • The cube looks unchanged. To see the result, go to the Inspect menu and select Section Analysis. Choose one of the flat side faces as the plane to see the hollow interior. You can turn off the analysis by clicking the eye icon next to it in the Browser.
4. Open Shell:
   • Undo the Shell operation (Ctrl+Z or Cmd+Z).
   • Activate the Shell tool again.
   • This time, click directly on the top face of the cube in the viewport.
   • Enter a thickness of 3mm. Click OK.
   • Now you have an open-topped box.

3. Controlling Wall Position: The Direction Setting

When you create a shell, you have precise control over where the wall thickness is applied relative to the original surfaces of your model. This is controlled by the Direction setting in the Shell dialog box.

• Inside: This is the default. The new wall is created inside the original boundaries of your model. The exterior dimensions of your part remain unchanged. This is what you'll use most often, especially when a part needs to fit into a specific, pre-defined space.
• Outside: The wall thickness is added to the outside of your model. This increases the overall dimensions of your part. This is useful for creating a case or housing that needs to fit around another object.
• Both: The thickness is applied in both directions from the original surface, centered on it. If you specify a 4mm thickness, it will add 2mm to the inside and 2mm to the outside.

Let's return to the video to see a clear explanation of these options.

Experiment with these settings on the open box you created. Try each of the three Direction options with a 5mm thickness and use the Inspect > Measure tool to check the final outside dimensions of your box after each operation. You will see how Inside preserves the 50x50mm footprint, while Outside and Both expand it.

4. Practical Application: Creating Custom Enclosures

The real power of the Shell command becomes apparent when you use it to create parts designed to interact with other objects. A perfect example, relevant to your interest in gaming accessories, is creating a custom holder or enclosure.

Often, the workflow involves modeling the object you want to encase first, then using a copy of that object's geometry as the starting point for its holder.

The final part of this video demonstrates a practical workflow for creating a custom camera holder. This is a slightly more advanced technique that combines multiple tools, but it's a great example of what's possible.

This example of creating a holder for a camera is directly analogous to how you might design a custom charging dock for a game controller or a protective case for a portable hard drive.

5. Final Practice: Design a Component Tray

Let's consolidate what you've learned by building a simple but practical object: a small tray for holding screws, game pieces, or other small items. This exercise will also use the Fillet tool from our previous lesson.

1. Create the Base Solid:

   • Start a new design.
   • Sketch a rectangle 120mm by 90mm on the ground plane.
   • Extrude the rectangle up by 25mm.

2. Add Internal Fillets:

   • Activate the Fillet tool (F key).
   • Select the four vertical corner edges of the box.
   • Give these edges a large radius, for example, 15mm.
   • This creates a smooth, rounded interior shape, which is good for a tray.

3. Shell the Body:

   • Activate the Shell tool.
   • Select the top face of the model to remove it.
   • Set the Thickness to 2mm. The standard Inside direction is fine.
   • Click OK.

You now have a tray with a uniform 2mm wall thickness. Notice how the Shell command correctly followed the rounded corners you created with the Fillet tool. This is a great example of how features in the timeline build upon one another.

Conclusion

You have now mastered the Shell command, a fundamental tool for any designer focused on 3D printing and product design. You can now create hollow objects efficiently, which is key to saving material, reducing print time, and designing enclosures.

Key Takeaways:

• The Shell command hollows out solid bodies to a specified, uniform wall thickness.
• Selecting the body in the browser creates a closed, hollow part. Selecting faces on the model removes them to create an open shell.
• The Direction setting (Inside, Outside, Both) is critical for controlling the final dimensions of your part and ensuring it fits with other components.
• Shell is the go-to tool for creating cases, containers, and lightweight parts.

In our next lesson, we will dive deeper into how different bodies interact. We'll formally cover the Join, Cut, and New Body operations within tools like Extrude. Understanding these boolean operations is the next crucial step to building complex models composed of multiple distinct parts.