Part II: Building Intelligence into Your Parts
As an exercise, I often try to see how many different ways a particular shape might be modeled,
and how each modeling method relates to manufacturing methods, costs, editability, efficiency,
and so on. You may also want to try this approach for fun or for education.As SolidWorks grows more and more complex, and the feature count increases with every release,
understanding how the features work and how to select the best tool for the job becomes ever
more important. If you are only familiar with the standard half-dozen or so features that most users
use, your options are limited. Sometimes simple features truly are the correct ones to use, but
using them because they are the only things you know is not always the best choice.Using the Extrude feature
Extruded features can be grouped into several categories, with extruded Boss and Cut features at
the highest level. When you use Instant3D, extruded bosses can be transformed into cuts by sim-
ply dragging them the other direction. It is unclear what advantage this has in real-world model-
ing, but it is an available option. As a result, the names of newly created extrude features are
simply Extrude1 where they used to be Extrude-Boss1 or Extrude-Cut1.
The “Base” part of the Extruded Boss/Base is a holdover from when SolidWorks did not allow
multi-body parts, and the first feature in a part had special significance that it no longer has. This
is also seen in the menus at Insert ➪ Boss/Base. The Base feature was the first solid feature in the
FeatureManager, and you could not change it without deleting the rest of the features. The intro-
duction of multi-body support in SolidWorks has removed this limitation.Cross-Reference
Multi-body parts are covered in detail in Chapter 26. n
Solid feature ..................................................................................................
In this case, the term solid feature is used as an opposite of thin feature. This is the simple type of
feature that you create by default when you extrude a closed loop sketch. A closed loop sketch
fully encloses an area without gaps or overlaps at the sketch entity endpoints. Figure 7.1 shows a
closed loop sketch creating an extruded solid feature. This is the default type of geometry for
closed loop sketches.Thin feature ...................................................................................................
The Thin Feature option is available in several features, but is most commonly used with Extruded
Boss features. Thin features are created by default when you use open loop sketches, but you can
also select the Thin Feature option for closed loop sketches. Thin features are commonly used for
ribs, thin walls, hollow bosses, and many other types of features that are common to plastic parts,
castings, or sheet metal.Even experienced users tend to forget that thin features are not just for bosses, but that they can
also be used for cuts. For example, you can easily create grooves and slots with thin feature cuts.