Features and Macros in SolidWorks
In this sample chapter from Mastering SolidWorks, 3rd Edition, learn mechanical design basics using SolidWorks, from feature-based modeling to macros that aid in design automation. Step-by-step projects teach you how to construct a spur gear, create a compression spring, and more.
This chapter is from the book
This chapter is from the book
This chapter is from the book
4.1 Introduction
We have been using a limited set of features thus far in the book. We have used extrusions and revolves. We have used the SolidWorks features Extruded Boss/Base and Revolved Boss/Base and their subtracting counterparts, Extruded Cut and Revolved Cut. These four features create one class of parts: those with constant cross sections. We use the extruded boss or cut to create uniform thickness parts. We use the revolved boss or cut to create axisymmetric parts. Amazingly, these four features can create 80% or more of the mechanical parts you are likely to need.
These four features cannot create some classes of parts: They cannot create parts whose cross sections are variable or parts that have nonplanar faces or other geometric shapes. The features that allow us to create these types of parts are Lofted Boss/Base, Swept Boss/Base, Lofted Cut, Swept Cut, Hole Wizard, Rib, Draft, Shell, and Dome, as shown in Figure 4.1. We cover all these features in this chapter. You can also access more features by clicking this sequence: Insert (menu) > Features.
)
Figure 4.1 Available features
A feature is defined as a solid that, when combined with other features (solids), creates parts. A CAD part consists of a set of features created in a certain sequence stored in its feature tree. Some features, such as bosses and cuts, originate as sketches, while others, such as shells and fillets, modify other features. Features are always listed in the feature tree (which SolidWorks calls the FeatureManager Design Tree) of the part.
Today’s modeling is referred to as feature-based modeling, and the resulting models are known as feature-based models. The first feature you create in a part is known as the base feature. You use the base feature as the basis to create other features. A base feature obviously cannot be negative (i.e., a cut), and SolidWorks does not allow it. When you begin creating a feature, Extruded Boss/Base and Revolved Boss/Base are the only selectable feature types. You might also expect Swept Boss/Base and Lofted Boss/Base to be selectable when you begin creating a feature, but they are not. Lofted Boss/Base becomes selectable only after you create a sketch (profile), and Swept Boss/Base becomes selectable after you create a cross section and a path (sweep direction).