Datasheet

Chapter 1: Introducing SolidWorks

removing the sleeve inside instead of the hole on top. You can try this for yourself by opening the part

indicated previously, dragging the Shell1 feature in the FeatureManager, and dropping it just above

the Cut-Extrude1 feature.

Note

You can only drag one item at a time in the FeatureManager. Therefore, you may drag the shell, and then drag

each of two fillets, or you could just drag the cut feature down the tree. Alternatively, you can put the shell and

fillets in a folder and drag the folder to a new location. Reordering is limited by parent-child relationships between

dependent features.

Cross-Reference

You can read more about reordering folders in Chapter 12.

In some cases, reordering the features in the FeatureManager may result in geometry that might not

make any sense; for example, if the fillets are applied after the shell, they might break through to the

inside of the part. In these cases, SolidWorks gives an error that helps you to fix the problem.

In 2D CAD programs where you are just drawing lines, the order in which you draw the lines does not

matter. This is one of the fundamental differences between history-based modeling and drawing.

Features are really just like steps in building a part; the steps can either add material or remove it.

However, when you make a part on a mill or lathe, you are only removing material. Some people

choose to model following manufacturing methods, so they start from a piece of stock and apply fea-

tures that remove material. This approach works best for machining, but doesn’t work well for mold-

ing, casting, sheet metal, or progressive dies. The FeatureManager is like an instruction sheet to build

the part. When you reorder and revise history, you change the order of operations and thus the final

result.

Sketching with Parametrics

Sketching is the foundation that underlies the most common feature types. You will find that sketch-

ing in parametric software is vastly different from drawing lines in 2D CAD.

Dictionary.com defines the word parameter as “one of a set of measurable factors . . . that define a sys-

tem and determine its behavior and [that] are varied in an experiment.” SolidWorks sketches are

parametric. What this means is that you can create sketches that change according to certain rules,

and maintain relationships through those changes. This is the basis of parametric design. It extends

beyond sketching to all the types of geometry you can create in SolidWorks. Creating sketches and

features with intelligence is the basis of the concept of Design Intent, which I cover in more detail

later in this chapter.

In addition to 2D sketching, SolidWorks also makes 3D sketching possible. Of the two methods, 2D

sketches are by far more widely used. You create 2D sketches on a selected plane, planar solid, or sur-

face face and then use them to establish shapes for features such as Extrude, Revolve, and others.

Relations in 2D sketches are often created between sketch entities and other model edges that may or

may not be in the sketch plane. In situations where other entities are not in the sketch plane, the out-

of-plane entity is projected into the sketch plane in a direction that is normal to the sketch plane. This

does not happen for 3D sketches.

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