Learn how to copy and paste bodies and components between Fusion designs. This tutorial covers important workflows for transferring geometry, retaining feature history, and solving common copy-paste challenges in your CAD projects.

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Copy & paste in Fusion

Copying a body or part of your design from one Fusion file to another can sometimes feel frustratingly complicated, especially when you want to preserve as much design intelligence and history as possible. However, understanding the differences between bodies and components in Fusion and matching your workflow accordingly, allows for more streamlined, flexible cross-file collaboration. Here’s an in-depth look at the essential techniques to move your designs and unlock greater productivity in Fusion.​

Why copying bodies trips up users

Here’s a scenario that’s familiar to almost every Fusion user at some point: after building geometry in one file, you want to reuse that shape in a new project. Searching for a simple solution often leads to dated or tangential forum threads, because—unlike in some CAD tools—Fusion distinguishes sharply between a “body” and a “component.”

• A body is fundamentally a fixed piece of geometry within a component and doesn’t retain independent feature history. Think of it as a “dumb” shape—the final geometry, separated from the procedural details that created it.
• A component is more flexible, acting as a design container that maintains its own timeline and feature tree. Components can be moved, edited, and reused more intelligently across designs.​

This distinction is foundational to every copy-paste strategy, so understanding the basics is critical before choosing the best method for your needs.

Method 1: Copying a body as a base feature

The quickest route to bring a body into a new Fusion file is using base features:

1. Copy the body from your original design (Ctrl+C or Command+C).
2. Open a new file and select “Paste” (Ctrl+V or Command+V) to drop it in.
3. Fusion will prompt you to make a “Base Feature.” Complete the operation and finish the base feature in your timeline.

This approach is fast and works well if you just need end geometry—not the history of how it was made. It’s essentially a “dumb” transfer: fast, but you lose parametric and feature intelligence. For non-history driven tasks or quick transfer of reference shapes, it’s a solid solution.​

What about timeline access?

If you attempt to paste with design history enabled, Fusion blocks the operation to avoid confusion. As a workaround, you can turn off design history temporarily (right-click the root and choose “Do Not Capture Design History”), paste your body, and then decide whether to re-enable the timeline. Remember: turning design history back on does NOT make the pasted body parametric—it stays a base feature.​

Method 2: Derive for dynamic linking

If you want to maintain a live reference to the original body (so updates propagate), Fusion’s Derive command is your friend. Here’s how:

1. In your target design, use Insert → Derive and navigate to the source file.
2. Select the desired body or component.
3. The derived object now appears in your new design. Any changes in the original file update here too.

This is powerful for modular workflows or master-model approaches, ensuring your new file always mirrors the source.​

Method 3: Copying components to retain feature history

Often, you aren’t just moving a shape—you want the full power of timeline edits, feature rolls, and parameter tweaking in the new context. That means working with components rather than bodies.

1. Organize your geometry as a component before you copy—don’t wait until after!
2. Copy the component and use “Paste New” in your new Fusion file.
3. The component, along with its full timeline and feature tree, is pasted as a new instance.

This method is powerful but requires that your new design also contains any references or linked features used in the original. If not, Fusion will throw warnings or errors, requiring you to resolve missing geometry or references.​

Method 4: Insert with break link for editable history

Fusion’s Insert into Current Design enables referencing another file—maintaining a link so changes reflect across files. Sometimes, you want both the original’s intelligence and local edit freedom. After inserting, right-click the inserted item and choose “Break Link.”

• Now, the inserted geometry is native to your file.
• You retain the full timeline and history for detailed modifications.

This is especially useful for developing variations on a master part, or integrating externally designed features into your new product’s assembly.​

Choose your workflow wisely

Which copy & paste method is best? It all depends on your goal:

• Use Base Feature for basic geometry transfers.
• Use Derive if you want a live update link.
• Use Paste New Component to keep editing features and design intent.
• Insert & Break Link blends referencing with editable history.

Fusion’s powerful but nuanced copy & paste tools let you collaborate efficiently, reuse valuable designs, and maintain the smart CAD models your workflow demands—once you know which workflow fits your need.