You can create a part or assembly while working in an existing assembly. Creating an in-place part has the same result as inserting a previously created part file. You can sketch on the face of an assembly component (or an assembly work plane) and include geometry from other assembly components in your feature sketches. When you click Create and select a plane on which to sketch, the part environment is activated. Enter a meaningful name for the new part file. In the browser, the top-level assembly is unavailable, and the new part is active.
Parts created in place (in an assembly context) can be:
You select the default BOM Structure for the in-place component. The BOM Structure property defines the status of the component in the BOM. BOM Structure has five basic options: Normal, Phantom, Reference, Purchased, and Inseparable. At the component instance level, you can override the structure to be Reference.
You can choose to create a virtual component. The virtual component is a component that requires no modeling of geometry and no file. It is the equivalent to a custom part in a parts list.
Virtual components are considered and treated as real components for all practical purposes. They have a browser representation, have properties such as quantity, BOM Structure, Part Number, and so on.
New parts can be sketched on the faces of other components that have edges or features needed for the new part. A geometric constraint is applied (by default) between the selected face and the face created from the new sketch. If you must relocate the part later, you can delete the constraint.
If you prefer, you can make the constraint adaptive by setting an option on the Assembly tab of the Application Options dialog box. This option allows the part to resize or change position if the constraining parameters or components change.
When creating a part, you can project geometry from the face of another part. You can make the new part associative to the parent part. Before you create the part, in the Application Options dialog, Assembly tab, select the check box for Enable Associative Edge/Loop Geometry Projection During In-Place Modeling. Usually, you set this option once as a workflow preference.
Parts can terminate on the face of another component. Use the From To or To extents options for Extruded features. Extruded features with From To or To extents to other assembly components are adaptive by default. They can resize or reposition relative to other components as necessary.