Create new components

Create new components in an Assembly or Hybrid Design in Fusion.

Create a new external component

Open or create an Assembly or Hybrid Design.
In the Design toolbar, click Assemble > New Component .

The New Component dialog displays.
Select the Design Type and associated settings:
- Part : Creates a new Part Design and inserts it as an external component.
  - Standard : Creates a new Standard Part Design and inserts it as an external component.
  - Sheet Metal : Creates a new Sheet Metal Part Design and inserts it as an external component.
- Assembly : Creates a new Assembly Design and inserts it as an external component.
- Hybrid: Creates a new Hybrid Design and inserts it as an external component.
- Linked PCB: Creates a new PCB in an Electronics Design and inserts it as an external component.
Enter a unique Design Name for the new component.
Specify where to create the new component, relative to the design:
- Parent: The new component is created within the parent component. The active component is automatically selected as the parent.
- Location: The new design that will contain the new component is saved here. The project folder where the current design is saved is automatically selected. Fusion automatically saves it in the same location as its parent. To change the location:
  1. Click the folder name or the X.
    
    The Select Folder dialog displays.
  2. In the Select Folder dialog, navigate to the new location where you want to save the design.
  3. Click Select.
For a Sheet Metal component, select a Sheet Metal Rule.
(Optional) Check Activate to activate the new component once it is created and enter Edit In Place.
Click OK.

Fusion automatically saves the new design in the same location as its parent.

If the parent component is not selected, the default location matches the active project and folder in the Data Panel.
If the parent component has not been saved yet, the default location matches the active project and folder in the Data Panel.

The new component is referenced into the current design and displays in the browser beneath the parent component you selected. If Activate was checked, the component is automatically activated, and an Edit In Place session begins so that you can start working in the new component in the context of the active design.

Create internal components

In Hybrid Designs, you can create both external and internal components. Note: By default, Assembly designs can only contain external components. To create internal components in an Assembly Design, enable modeling tools.

Create a new internal component

Open or create a Hybrid Design.
In the Design toolbar, click Assemble > New Component .

The New Component dialog displays.
Uncheck External.

Design Type is disabled. The Part Type and Design Name fields are replaced by Component Type, Component Name, and From Bodies.
Select the Component Type:
- Standard : Creates a standard internal component.
- Sheet Metal : Creates a Sheet Metal internal component.
Enter a unique Component Name.
(Optional) Check From Bodies to convert existing bodies in the active design to individual components instead of creating an empty component.
- If checked, you can no longer select the parent component. See Create components from existing bodies below.
To change the parent component:
1. Click the X next to the Parent field to clear the selection.
2. In the browser, click to select the new parent component.
For a Sheet Metal component, select a Sheet Metal Rule.
(Optional) Check Activate to activate the new component once it is created.
Click OK.

The new component displays in the browser beneath the specified parent component. If the Activate setting was checked, the component is automatically activated, so that you can start working in the new component.

Create components from existing bodies

Open or create a Hybrid Design.
In the browser, expand the Bodies folder.
Select the bodies you want to convert to components.
Right-click, then select Create Components from Bodies .

Note: You can also right-click the Bodies folder to select and convert all of the bodies within it.

For each selected body, a new component displays in the browser beneath the component where the body originated. The body is moved from the Bodies folder in the original component to the Bodies folder in the new component.

Note: Although the body moves into the new component, any sketches you used to create it, and any modifications you applied to it, remain in the original component. This can make the timeline difficult to understand and interact with, so it is typically best to create empty components first, and then create the geometry of that component entirely within it.

Create a component during an active command

Open or create a Hybrid Design.
In the toolbar, activate a command from the Create panel, such as Extrude, Revolve, Box, or Cylinder.
In the dialog, expand the Operation dropdown menu.
Select New Component from the list.
Adjust any additional settings for the command.
Click OK.

The new component displays in the browser. The bodies you created during the command display in the canvas and in the Bodies folder of the new component.

Important: If you intend to make copies of a component, avoid using the New Component operation within command dialogs. This option works well for a closed design that requires motion, but the sketch and body remain with the default component, which impacts the Save Copy As command.

bracket components example

Tips

To ensure the parametric history of a component is stored entirely inside the component, create a new component before you start creating any geometry for the component. This ensures any copy of the component will be parametrically complete, excluding references to other components.
Name each component as you create it, so that you and anyone you collaborate with can easily understand the assembly structure.
Before you convert bodies to components, rename each body. The name of the new component will match descriptive name you gave the body, and it will be easier to find in the assembly.
In the browser, click the radio button next to a component to activate it. Always make a component active before you add geometry to it.