Chapter 3: Working with Sketches
Working with Reference Geometry
Reference geometry in SolidWorks is used to help establish locations for geometry that you can’t
physically touch, such as planes, axes, coordinate systems, and points. You often use reference
geometry to establish a characteristic of the finished solid model before the model is created or to
include an item that you may want to mate another part to in an assembly later. Mate References
are also classified as Reference Geometry, although I do not cover them until Chapter 19, in the
course of discussing library parts.The importance of working with reference geometry becomes obvious in situations where you
need to create geometry that doesn’t line up with the standard planes. You might use planes to rep-
resent faces and axes to represent the centers of holes. Axes are often used to establish a direction,
such as in plastic parts where, because of draft, you never truly have any vertical edges; an axis is
frequently used to establish the direction of pull for the mold.Coordinate systems come in handy, especially when translating a part from one system to another
for the purpose of machining or some type of analysis. SolidWorks users usually model in such a
way that the modeling work is made simpler by the choice of how the part origin is positioned rel-
ative to features of the part, but rapid prototyping, machining, mold building, and sheet metal
manufacturing applications may have different requirements. As a part modeler, you cannot
account for the needs of all downstream applications with your initial choice of origin placement,
but you can always create a reference coordinate system for those downstream applications to use.Creating planes
Planes are the most commonly used type of reference geometry because they are used for sketching,
cutting, as extrude end conditions, and more. The Plane feature PropertyManager and functionality
has changed significantly in SolidWorks 2010. With the new interface, shown in Figure 3.35, you
start by selecting model items (faces, edges, points, vertices, or other sketch or reference geometry)
that you want to use to create the plane. The new plane uses constraints like sketch relations from
the selected references. For example, in Figure 3.35, the new plane is tangent to the selected First
Reference cylindrical face and at an angle to the selected Second Reference of a plane.
The good news about this method is that there are far more options for creating planes than in the
previous method, but the bad news is that going into the feature, you may not know all the avail-
able options. You have to make a selection before it shows you the available constraints. The older
interface presented the available options right up front, but there were fewer to choose from.
Hopefully this interface matures in the future. Meanwhile, you may need to experiment to see what
works best for the type of modeling you do.