Components vs Bodies

Overview#

The single most important habit for building assemblies in Fusion is understanding the difference between a body and a component. Beginners often model an entire product as a set of bodies inside one component, then discover that joints, motion, bills of materials, and external references simply do not work. Almost every assembly feature in Fusion operates on components, not bodies.

• A body is, in Autodesk's words, a single container for a contiguous 3D shape (solid, surface, sheet metal, T-Spline or mesh). Each component can contain multiple bodies, but you cannot create joints or motion between bodies; bodies that need relative motion must reside in separate components.
• A component is a container for design elements: its own origin, coordinate system and timeline, and a name, number and description that display in a parts list. It can contain an origin, construction geometry, sketches, bodies, joint origins and other components, and it can be moved, jointed, pinned and referenced from another design.

Think of a component as a "part" or "sub-assembly" and a body as "a lump of material inside that part". A single machined part with several disjoint solids (say a bracket and its pressed-in bushing modeled as one part) might legitimately hold multiple bodies. Two parts that move relative to each other must be separate components.

Every Fusion design has a Default Component, the top node in the Browser. Everything else lives under it. Document settings, named views, analyses, joints, contact sets and motion studies are always located in the Default Component. A design with only bodies is really "one component containing bodies".

A component can be internal (contained in the current design) or external (an xref to a separate design; see External References). Hybrid designs can contain both; by default Assembly designs contain only external components. Components are required if you plan to use the tools in the Manufacture and Drawing workspaces.

Where to find it#

Tip: Press S to open Command Search and type "component" if you cannot find a command.

Step by step#

Creating a component before you model (the recommended way)#

1. Start a new design and save it so it has a name (it becomes the top-level component).
2. Choose Assemble > New Component in a Hybrid design. Uncheck External to create an internal component, then set Component Type (Standard or Sheet Metal), Component Name (for example "Base Plate"), Parent (the active component is selected automatically) and optionally From Bodies (a separate component for each selected body). With External checked, you instead choose a Design Type, Design Name and Location.
3. Check Activate if you want the component activated on creation (for an external component this starts an Edit In Place session). Click OK.
4. Confirm the new component is the active one (its Activate Component radio button is filled). Parent and sibling components become translucent, and the timeline shows only features of the active component.
5. Create a sketch and extrude. New sketches, bodies and construction geometry are contained in the active component.
6. When finished, activate the Default Component (which shows the entire assembly history) or another component before creating the next one. This avoids accidentally modeling a second part inside the first.

Converting bodies to components#

1. Model several bodies in one component. (This is common when you start in "bodies mode".)
2. In the Browser, expand Bodies. Right-click one body and choose Create Components from Bodies. You can also select several bodies first.
3. Fusion creates one new component per selected body and moves each body into it. Components appear under the parent. Note that the history of features that created the bodies stays in the Default Component and remains associated with the full assembly timeline.
4. Rename each component immediately (general guidance).

Moving an existing body into an existing component#

Autodesk documents Create Components from Bodies for this, not drag-and-drop. If you drag a body to another component in the Browser, check afterward that sketches it depends on are still where you expect. Moving a body does not move the sketches or features that built it (general guidance).

Options reference#

New Component dialog#

Component properties (right-click > Properties)#

Note: not confirmed in Autodesk's documentation: an "Exclude from BOM" property. Earlier text listed one.

Why components matter#

Joints and motion#

A joint connects two components. Autodesk is explicit that you cannot create joints or motion between bodies; bodies that need relative motion must live in separate components.

Each component has its own origin#

Each component carries its own origin point and planes. When you activate a component and create a sketch on its Front plane, you are sketching on that component's Front plane, which moves when the component moves. This is what makes parts "portable": you can rotate a component 90 degrees in the assembly and its internal sketches follow.

By contrast, bodies in one component all share that component's origin. Moving one body relative to the others using Move/Copy with Bodies selected is a modeling operation recorded in the timeline, not an assembly constraint.

Bill of materials#

The BOM lists components with quantities. A parts list or BOM is built from the component structure, so a bodies-only design gives you almost nothing to list (general reasoning).

Reuse and copying#

Autodesk has three commands for reusing components: Paste, Paste New and Insert into Current Design. Paste creates an identical copy that stays linked with the others: change one and all update, and each copy can be positioned independently (names get :1, :2 suffixes). Paste New creates an independent copy; changing one does not update the others (in a collaborative editing hub the pasted component gets a new, unique part number). Use Paste to place eight identical bolts and Paste New for a variant, such as a longer bolt. After pasting you position the copy with the manipulator or Move/Copy dialog.

Naming rules#

Fusion shows copy suffixes as :1, :2. If you need a different part from a linked copy, use Paste New or a new component rather than editing a shared one (general guidance).

Active component and why things end up in the wrong place#

Fusion places new geometry in whichever component is active. Most "my part is in the wrong component" problems come from forgetting to activate before sketching. Symptoms:

• A new sketch appears under the wrong component in the Browser.
• Extrude creates a body in the base plate instead of the lid.
• Joint Origins land in the wrong component, causing joint errors.

Always check the Activate Component radio button. Joints, contact sets and motion studies are an exception: they are always stored in the Default Component because they affect the whole assembly.

Tips and pitfalls#

Tip: Create components first and model inside them. Retrofitting is possible with Create Components from Bodies, but sketches, features, and references that were built across bodies may not split cleanly.

Tip: Use short, meaningful names and consistent prefixes (for example "01-Base", "02-Jaw"). Sorted names make large assemblies navigable. Avoid special characters that may break CSV exports.

Warning: Bodies inside a single component cannot be jointed to one another. If a joint command will not accept your selection, check whether both objects belong to the same component.

Warning: Create Components from Bodies leaves the feature history in the Default Component, tied to the full assembly timeline, which Autodesk says makes the timeline hard to follow. Autodesk's best practice is to create a new component first, name it, activate it, then design.

Tip: A pure-bodies workflow is fine for a single 3D-printed part. The moment you need two parts that move, mate, or appear on a BOM, switch to components.

Practice exercise#

1. Create a new design and save it as "Hinge Practice".
2. Create two components: "Leaf A" and "Leaf B". Activate each in turn and extrude a 50 x 30 x 3 mm plate in each.
3. Right-click Leaf A and choose Pin.
4. Now try Assemble > Joint and select the two plates. The Joint command should accept the selection. Confirm the Browser shows two components with two bodies.
5. Undo, then repeat the exercise by modeling both plates as bodies in one component. Try to create a joint. Observe that joints cannot be created between bodies, and note the difference.
6. Finally, select both bodies, right-click, and choose Create Components from Bodies. Verify that the Joint command now works.

Expected result: a design with two components where the joint command accepts the plates, and where converting bodies to components fixes the earlier limitation.

Related#

• Top-Down vs Bottom-Up Design
• Joint Origins
• Joints
• BOM and Parts Lists
• External References