You can create a new part within an assembly using the Create Part In-Place command. If you are working in a newly created assembly document, you must save that document before you can create a part in place.
Choose the Create Part In-Place command 
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In the Create New Part In-Place dialog box, do all of the following:
Choose a document template matching the part, sheet metal, or subassembly that you want to create.
Specify a name and location for the new document.
Select By Graphic Input.
Tip:
You also can create new parts and subassemblies relative to the assembly origin using the Create New Part In-Place dialog box. To do this, choose either the Coincident With Assembly Origin or Offset From Assembly Origin options instead of the By Graphic Input option.
(Optional) Select Ground Parts And Assemblies.
To create the part and begin editing it, click the Create Part And Edit button.
Tip:
To only create the part document, click the Create Part button.
Select a part in the assembly. This part is used to position the new part you are creating.
On the selected part, click a planar face or reference plane.
Define the base orientation of the new part by clicking a part face, a part edge, or another plane.
Define the x-axis origin of the new part by clicking near one end of the displayed reference axis.
Define the origin of the reference planes for the new part.
Use the feature construction commands to construct the new part.
Save the changes you made to the new document.
To return to the assembly document, choose Home tab→Close group→Close And Return.
Tip:
You can control whether the part is displayed in another assembly, a drawing of the assembly, or included in a parts list with the Reference options on the Properties dialog box. See the Help topic, Reference parts.
You cannot create new parts in an assembly until the assembly has been saved.
Sometimes user may want to combine (unite/subtract/intersect) multiple parts to make a single part.