You can use the Create Part In-Place command 
to do either of the following:
Construct a new part or subassembly within the context of an existing assembly.
Create and name a series of empty part documents that are ready for someone else to use to create assembly parts.
You use the Create New Part In-Place dialog box to define the following:
Document template
Document name
Storage location
Placement option
Whether to apply a ground relationship
Whether to create the new document and continue editing the part, or simply to create the new file.
Note:
The document name and storage location are disabled when you work in the Solid Edge Embedded Client environment. You use the New Document dialog box to create the file properties in Teamcenter.
There are three placement options for creating a part in-place:
The Coincident With Assembly Origin option places the reference planes of the new part directly on top of the assembly origin, oriented exactly as the assembly.
The By Graphic Input option positions the new part relative to an existing part. You need to select an existing planar face or reference plane where the new part will be placed. You then select the origin location of the base reference planes for the new part.
The Offset From Assembly Origin option offsets the reference planes of the new part from the assembly reference planes by a specified keypoint or value. Select a keypoint on any part already placed in the assembly, or type an x, y, and z offset distance applied relative to the assembly origin. The reference planes of the new part will be oriented the same as the assembly reference planes.
In the Create New Part In-Place dialog box, you can choose whether to apply a ground relationship to the new part. The default is no.
Constraints—If you leave the part ungrounded, you are free to modify its position with respect to the assembly. You can always add constraints later with the options in the Relate group on the ribbon.
Exploding Assemblies—If you use a ground relationship, you will not be able to use the Automatic Explode command in the Explode-Render-Animate environment to explode the part later. Instead, you can use the Explode command to explode the part manually.
After choosing the placement method for the new part or subassembly, you then choose whether to simply create the new file, or whether to create the new file and open it in the appropriate Solid Edge environment for editing. Use the buttons on the Create New Part In-Place dialog box to identify which you want to do.
If you choose to continue working in the new document, you can create new features as you normally would when working in a part or assembly.
Upon completion, save the new part document, and then choose Close And Return, which is located in the Close group on the ribbon, to return to the original assembly file.