Fusion 360 Components & Bodies for New Designers

Aaron.Magnin August 28, 2018 9 min read

Use a CAD tool like Inventor or SolidWorks, and you’ll start to notice a difference in how assemblies are organized. Take, for example, a simple design like an adjustable wrench.

To design this in a tool like SolidWorks, you would need to draw up each part and save it in a separate file. That would be 5 files in total for the handle, jaw, spring, pin, and knurl. You would then need to make a primary assembly and insert each of those files to make the complete wrench. Are you starting to see the problem with this workflow?

This might be a straightforward example, but imagine designs with hundreds of parts. Keeping track and managing every file would be a total pain for experienced and new designers alike.

And what happens if one of those files gets moved around by accident? Suddenly a link is severed, and the assembly drawing doesn’t know how to display a critical part.

Fusion 360 solves both of these problems with a structure of bodies and components. Within a single Fusion 360 file, you can have a collection of parts that are all connected to an assembly.

Regardless of how complex your design grows, you’ll always have one file and one design environment for your entire workflow.

Sketch to Bodies Explained

Let’s start with the most simple of the two – bodies. In Fusion 360, a body is any continuous 3D shape. That might be a sphere, cube, cone, etc. Whenever you create a 2D sketch in Fusion 360 and then extrude it into a 3D shape, you automatically create a body.

The keyword about a body is that it has to be continuous. Take a cube and cut it in half, and you now have two bodies.

Bodies are great when you want to model an object that won’t require any associated motion. Maybe you decide to model a cup. This is a static object that won’t move and will likely consist of a collection of bodies, including a mug and handle.

There are several specific constraints you’ll want to know about bodies. Remember these:

What happens when you make a body but realize you wanted it to be a component? This is a simple fix. Right-click the body in your Browser, and select Create Components from Bodies.

Fusion 360 Components Explained

In Fusion 360, a component is a part that is capable of motion and has its own unique origin. A component can also serve as a container for a variety of design objects, including:

For example, in the image below, we’re working on designing a tensioner and pulley system. If you look at the browser on the left, you can see that Pulley 1:1 is a component designated by its block icon.

If we expand Pulley 1:1, this reveals several other objects nested within the component, including a set of origins, a body, and two sketches.

Components are great not just for the organization but also for design reuse. Say you want to reuse one of the pulleys in another design. If your pulley were just a random collection of sketches and bodies, you wouldn’t have any way to bring it into your new design. However, by housing all of these individual objects inside a component, you can quickly export just that one component into your new design.

Let’s try this out so you can see what we mean. We’re going to right-click on the Pulley 1:1 component and select Export.

We’ll give it a name and save it to our Fusion 360 cloud storage. In our Data panel, we can then right-click the exported file and Insert into Current Design.

If we insert this pulley into another design, you’ll see the same component from our original design, with all of its associated objects, including an origin, body, and two sketches.

Like bodies, there are several constraints that you’ll want to know about when using components. Remember these:

Overall, anytime you plan to design an assembly or subassembly with parts that will have motion, you will need to create those parts as components.

Other Ways to Understand Bodies & Components

It might be easier to understand the relationship between bodies and components by viewing them in a tree-like structure, as shown below:

Here we can see a clear parent-child relationship unfolding. The assembly sits at the top of our design hierarchy and can contain one or multiple components. Components can contain one or multiple bodies, including other design objects like sketches, construction geometry, etc.

Prefer a table to compare these two concepts side by side?

 BodyComponent
What it isAny continuous 3D shape, e.g. cylinder, sphere, etc.Acts as a part within an assembly and/or a container for other design objects
When to use itFor static modelsFor assemblies that require movement between parts
Origin/CoordinatesSame as assemblyEach component has unique origin/coordinates
MotionNoYes, with joints
ManufacturingWill not show up in parts list or drawingShows up in part list/drawing, each component has a unique part name, number, description
Copy/paste behaviorChanges to a copied body do not affect the original bodyChanges to a copied component can affect the original component

Bodies and Components In Action

Hopefully, these concepts are all making sense by now. When in doubt, the best way to understand is by jumping into Fusion. We’ll be walking through an example design that contains both bodies and components.

Identifying Bodies and Components

First, you’ll need an example design to play with. Download our pulley and tensioner sample file here.

Once downloaded, swing open the Data panel in Fusion 360, navigate to a project, and select the Upload button.

Open your uploaded design, and let’s focus on the Browser for a bit. Bodies and components each have their own unique icons to make them easily identifiable.

Look for the cylinder icon, which identifies a single body.

Look for the block icon, which identifies a single component.

Lastly, look for the multi-block icon, which identifies a component that contains multiple components and other design objects.

For example, Tensioner:1 has a multi-block icon and contains three subcomponents, Tension Arm:1, Pulley:1, and Bolt:1.

How Components are Named

Another thing to make a note of is how components are named in the Browser. When you copy and paste a component with the standard Paste command, these two components are linked together. Make a change to one, and it will change the other.

The number/semicolon structure can identify these connected components after their name. For example, Pulley 1:2 is the 2nd instance of the 1st pulley, which is Pulley 1:1.

If you copy and paste a component with the Paste New command, then your new component will not be linked with the original.

This newly pasted component will have a naming convention that looks like this:

Components and the Timeline

One important feature that components have is their own unique timeline. Hover over a component in your browser and select the radial button to activate it.

Now take a look at your Timeline at the bottom of the canvas and notice that the history is different. The history that you see here is specific to the component that you just activated. Activate your top-level assembly, and your Timeline will switch to its default view.

This is an important distinction to make. When building out the features for a specific component, it’s common for designers to activate the component first and then start working on it. This helps to keep component-specific changes nested within their own timeline.

Extruding to Create a Body or Component

Now that we understand how to identify bodies and components let’s walk through how to create them. In this example, we want to extrude a sketch to create a pulley belt.

First, we’ll activate the Extrude command by pressing E or selecting the Extrude feature in the Model workspace.

Then select the side of the belt sketch. If you did it right, it should look like the image below.

This will open the Extrude dialog. We already have our profile selected, so we can enter a Distance of 4mm to extrude.

The chamfers on this pulley system are a little out of alignment, so we need to add a small offset to the pulley belt. Change the Start option to Offset Plane and enter 1mm for the Offset. This will ensure that the belt doesn’t overlap any of the pulley geometry.

The most important part of this dialog is the Operation dropdown. Expand this, and we have several choices, the two most important being to create a New Body or New Component.

Let’s do both to see the difference. If you select New Body and press OK, then you’ll have a new pulley body created in the main Bodies folder in your browser.

Undo what you just did and extrude the sketch again. This time select New Component for the operation and select OK. If it worked as planned, you should have a new Component 2:1 listed at the bottom of your browser.

Note: If you don’t see this new component created in your browser, take a look at what component you currently have activated. We goofed and originally had our Tensioner:1 component activated on the first extrude. This created the component within the Tension:1 component instead of our main assembly.

One last thing to note. If you left-click and hold to select the tensioner then move it left or right, the belt doesn’t move with it. Why’s that?

This is because we created the belt based on a sketch created outside of the tensioner component. If we wanted the belt to interact with the tensioner, the original sketch would need to be created inside the tensioner component.

Now You Know

There you have it, everything you need to know about the basics of bodies and components in Fusion 360. Components are an extremely versatile tool that can keep even the most complex projects organized by housing-related sketches, joints, components, and other objects in one convenient location. Plus, using components allows you to easily reuse individual parts of your design in other projects without reinventing the wheel.

If there’s only one thing you remember about bodies and components, it’s this – components have motion, bodies do not. Just making a static object? Bodies will do. Planning to make an assembly with moving parts? Start with components first. The rest of the details can be learned as you go.

Keep this knowledge fresh. Practice your body and component fundamentals now! Try Fusion 360 for free today.

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