SolidWorks 2010 Bible

Chapter 16: Modeling in Context

The in-context process

You can perform in-context modeling using one of two basic schemes. You can build parts from

the very beginning in the context of the assembly (using the Insert ➪ Component ➪ New Part menu

option) or you can start them using bottom-up techniques, creating the parts in a separate part

window, adding them to the assembly, and then adding additional in-context features later.

Starting out in-context

To start a new part in the context of an assembly, you will first assume that the assembly contains
another part. Creating a new part in a blank assembly is not very interesting. In this case, I am
using the assembly shown in Figure 16.1. To create the new part, choose Insert ➪ Component ➪
New Part. This command is also available through a toolbar button (shown to the left) that you can
place on the Assembly toolbar. At this point, SolidWorks prompts you to select a face or plane on
which to locate the new part. When you select the face or plane to place, SolidWorks places the
Front plane of the new part on it, opens a new sketch and adds an InPlace mate to the assembly.
In-context parts start as virtual parts, saved inside the assembly; you can choose to save it as an
external or internal part the next time you save the assembly. I discuss virtual part functionality
later in this chapter.

The InPlace mate

The mate that SolidWorks adds automatically when a part is created in-context is called an InPlace
mate. It works like the Fixed option, but is actually a mate that is listed with the other mates and
that may be deleted but not edited.

The InPlace mate clamps the part down to any face or plane where it is applied. It is meant to pre-

vent the in-context part from moving. I will explain later in this chapter why it is so important for

in-context parts not to move.

Alternative technique

Instead of using the Insert ➪ Component ➪ New Part command, you can simply create a blank part

in its own window and save it to the desired location. Then insert the blank part into the assembly

and mate the origins coincident. You can then edit the part in-context, the same as if you had cre-

ated it in-context from the beginning. The only difference between parts developed this way and

parts created in-context is the InPlace mate. The InPlace mate cannot be edited and does not have

relations to other geometry in the usual sense. Many users feel more secure with real mates to real

geometry, which they can identify and change if necessary.

Valid relations

Sketches, vertices, edges, and faces from the other parts in the assembly can be referenced from the

in-context part as if they were in the same part as the sketch. Most common relations are concen-

tric for holes, and coincident for hole centers. Converted entities (On-Edge relations) make a line-

on-edge relation between the parts, and Offset sketch relations are also often used.