Starting a new Component in the context of an Assembly
Most of the documentation and training material for SolidWorks focuses on creating new component parts in an assembly by using the menus: Insert - Component - New Part. You then have to select a face or plane to align the Front plane of the new component, and this creates an InPlace mate. Some users have noted a few apparent limitations imposed by this method. For example, what if the new component really needs to be affixed first via the Top or Right planes; or, what if it should be located via a vertex or an edge (for hinge or ball-joint action)?
In fact, the Insert - Component - New Part sequence is a convenience feature to save the user several steps. A more general, unconstrained method to add a new part in-context is as follows:
1) Use the New icon to create a new, empty part.
2) Save the new part with some appropriate file name.
3) Add the part to the assembly. You could do this via the menus (Insert - Component - Existing Part) or you click on the top-level icon in the part's FeatureManager, and drag it into the assembly window.
4) Create whatever Mate relationships are desired, using the origin or any of the default planes of the empty part.
5) Right-mouse click on the icon in the assembly's FeatureManager that represents the empty part. Choose the function Edit Part.
6) Pick a plane or face and insert a sketch to serve as the base feature of the new component.
7) Now go to town, sketching and building features just as you would have before.
You have just duplicated the functionality of the Insert - Component - New Part function, with the important difference that you have not created any InPlace mates and have instead located the new part using one or more mates of your own choosing.
