There is some terminology that you need to come to grips with before we dive into building models with SolidWorks. Notice that I talk about "modeling" rather than "drawing." This is because SolidWorks is really virtual prototyping software. Whether you are building an assembly line for automotive parts or designing decorative perfume bottles, SolidWorks can help you visualize your product in the most realistic way possible without actually having it in your hand. This is more akin to making a physical model in the shop than drawing on paper.

"Feature-based" modeling means that you build the model by incrementally identifying functional shapes, and applying processes to create the shapes. For example, you can create a simple box by using the Extrude process, and you can create a sphere by using the Revolve process. However, you can make a cylinder by using either process, by revolving a rectangle or extruding a circle. You start by visualizing the 3D shape, and then apply a process to a 2D sketch to create that shape. This concept on its own is half of what you need to know to create models with SolidWorks.

Figure 1.1 shows images of simple feature types with the 2D sketches from which they were created.

Many different feature types in SolidWorks enable you to create everything from the simplest geometry shown above to free-form shapes. In general, when I talk about modeling, I am talking about solid modeling, although SolidWorks also has a complete complement of surfacing tools. I will discuss the distinction between solid and surface modeling in a later chapter.

Table 1.1 lists some of the most common features that are found in SolidWorks, and classifies them according to whether they always require a sketch, a sketch is optional, or they never require a sketch.

Figure 1.1. Simple extruded and revolved features

While the bulk of this book focuses on the use of solid features, I believe that no set of modeling tools is complete without surface-modeling functions. Hybrid features combine the use of solids and surfaces in some way, and are discussed in more detail in Chapter 27. The surfacing and hybrid features available in SolidWorks are:

In addition to these features, there are many other types that create reference geometry (such as curves, planes, and axes), or perform some operation on existing geometry.

In addition to being feature-based, SolidWorks is also history-based. To indicate process history, there is a panel to the left side of the SolidWorks window called the FeatureManager design tree. The FeatureManager keeps a list of the features in the order in which you have added them. It also enables you to reorder items in the tree (in effect, to change history). As a result, the order in which you perform operations is important. For example, consider Figure 1.2. This model was created by the following process:

If the order of operations used in the above part were slightly reordered, the resulting part would also look slightly different, as shown in Figure 1.3.

Figure 1.4 shows a comparison of the FeatureManager design trees for the two different feature orders. You can reorder features by dragging them up or down the tree. Relationships between features can prevent reordering; for example, the fillets are dependent on the second extruded feature, and cannot be reordered before it. This is referred to as a Parent/Child relationship.

Figure 1.2. Features that are used to create a simple part

Figure 1.3. Using a different order of features for the same part

Figure 1.4. Compare the FeatureManager design trees for the parts from Figure 1.2 and Figure 1.3.

The order of operations, or history, is important to the final state of the part. For example, if you change the order so that the shell comes before the extruded cut, the geometry of the model changes, creating a sleeve inside instead of just a hole on top. You can try this for yourself by opening the part indicated above, dragging the Shell1 feature in the FeatureManager, and dropping it just above the Cut-Extrude1 feature.

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, because the results are the same. This is one of the fundamental differences between history-based modeling and non-history-based 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. The FeatureManager is like an instruction sheet to build the part. When you reorder and revise history, you change the final result.

You have already seen that sketching is the foundation that underlies the most common feature types. We will now find that sketching 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 system and determine its behavior and [that] are varied in an experiment." What this means to us as SolidWorks users in a practical sense is that we 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 curve elements, surface features, and solid features.

SolidWorks makes 2D and 3D sketching possible. Of the two methods, 2D sketches are by far the more widely used. You create 2D sketches on a selected plane, planar solid or surface face, and 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 entities 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.

You use 3D sketches for the Hole Wizard, piping, wiring, and weldments, among other applications such as complex shape creation.

Both 2D and 3D sketches share some relation types, although some of these relations work differently in the two types of sketches. Some relations that are unique to each type of sketch. The available sketch relations are:

For a simple example of working with sketch relations in a 2D sketch, consider the sketch that is shown in Figure 1.5. The only relationships between the four lines are that they form a closed loop that is touching end to end, and one of the corners is coincident to the part origin. The small square icon near the origin is the symbol for a coincident sketch relation. The setting to enable or disable these sketch relation symbols is found at View

Figure 1.5. A sketch of four lines

If you drag any of the unconstrained corners (except for the corner that is coincident to the origin), the two neighboring lines will follow the dragged endpoint, as shown in Figure 1.6. Notice the ghosted image left by the original position of the sketch. This is helpful when experimenting with changes to the sketch because you can see both the new and the old states of the sketch. The setting to enable or disable this ghosted position is found at Tools

Figure 1.6. Dragging an endpoint

If you add a parallel relation between opposing lines, they now act differently, as shown in Figure 1.7.

Figure 1.7. Dragging an endpoint where lines have relations

Next, a second parallel and a horizontal relation are added, as shown in Figure 1.8. If you are following along by recreating the sketch on your computer, you will notice that one line has turned from blue to black.

Figure 1.8. Horizontal and parallel relations are added.

The colors represent sketch states. Sketch states include Underdefined, Overdefined, Fully Defined, Unsolvable, Zero Length, and Dangling. There can be entities with different states within a single sketch. Also, endpoints of lines can have a different state than the rest of the sketched entity. For example, a line that is sketched horizontally from the origin has a coincident at one endpoint to the origin, and the line itself is horizontal. As a result, the line and first endpoint are black, but the other endpoint is underdefined because the length of the line is not defined. Sketch states are indicated in the lower-right corner of the graphics window and also in the status bar.

Now you can see that dragging one corner only allows the lines to move in certain ways, as shown in Figure 1.9.

Figure 1.9. Sketch motion is becoming more constrained.

Dimensions are also part of the parametric scheme. If you apply an angle dimension about the origin and try dragging again, as shown in Figure 1.10, you see that the only aspect that is not locked down is the length of the sides. Notice also that when the angle dimension is added, another line turns black.

Figure 1.10. Open degrees of freedom can be dragged.

Finally, adding length dimensions for the unequal sides completes the definition of the sketch, as shown in Figure 1.11. At this point, all lines have turned black. This is the state that we call "fully defined." Between the dimensions and sketch relations, there is enough information to recreate this sketch exactly.

Figure 1.11. The fully defined sketch cannot be dragged, and there are no degrees of freedom.

It is the idea of reacting to change that most concerns us regarding parametric design. There are other factors that can also drive the sketch, such as equations, other model geometry that is external to the sketch, and even geometry from another part in an assembly, as you shall see later.

"Design Intent" is a phrase that you will hear SolidWorks users say a lot. I like to think of it as "design for change." Design Intent means that when you put the parametric sketch relations together with the feature intelligence, you can build models that react to change in predictable ways.

An example of Design Intent could be a statement in words that describes general aspects that help define the design of a part, such as "This part is symmetrical, with holes that line up with Part A, and thick enough to be flush with Part B." From this description, and the surrounding parts, it is possible to recreate the part in such a way that if Part A or Part B changes, the part being described updates to match.

There are some types of changes that cause features to fail or sketch relations to conflict. In most situations, SolidWorks has ample tools for troubleshooting and editing that allow you to either repair or change the model. In these situations, it is often the Design Intent itself that is changing.

Design Intent is generally thought of as a static concept that controls changing geometry. However, this is not always the way things are. Design Intent often changes, thus requiring the way in which the model reacts to geometric changes to also change. Fortunately, SolidWorks has many tools to help you deal with situations like this.

Associativity in SolidWorks refers to links between documents, such as a part that has an associative link to a drawing. If the part changes, the drawing updates as well. Bi-directional associativity means that the part can actually be changed from the drawing. One of the implications of this is that you do not edit a SolidWorks drawing by simply moving lines on the drawing; you must change the model, which causes all views of the part or assembly to update correctly.

Other associative links include using base parts, where one part is inserted as the first feature in another part. This might be the case when you build a casting. If the part is designed in its "as cast" state, it is then inserted into another part where machining operations are performed by cut features and the part is transformed into its "as machined" state. This technique is also used for plastic parts where a single shape spans multiple plastic pieces. A "master part" is created and split into multiple parts that could, for example, become a mouse cover and buttons.

One of the most important aspects of associativity is file management. Associated files are kept connected by filenames. If a document name is changed, and one of the associated files does not know about the change, then the association between the files can become broken. For this reason, you should use SolidWorks Explorer to change names of associated files. There are other techniques that work, as well as some techniques that you should avoid.

Product development is about design, but it is even more about change. You actually design something once, but you may modify it endlessly (or it may seem that way sometimes). Similarly, SolidWorks is about design, but it really enables change. Think of SolidWorks as virtual prototyping software that allows you to change your prototype rather than having to make a new one. Virtual prototypes will never completely replace physical models, but they may reduce your dependence on them to some extent.

SolidWorks is also about reusing data. Associativity allows you to model a part once and use it for Finite Element Analysis, or FEA, creating 2D drawings, building assemblies, creating photorealistic renderings, and so on. When you make changes to the model, your drawing is already updated, and you don't have to reapply FEA materials and conditions or redo the rendering setup. Associativity saves you time by reusing your data. Associativity and change driven by feature-based and history-based modeling can take some getting used to if you have had limited exposure to it, but with some practice it becomes intuitive and you will see the many benefits for enabling change. Parametric sketching and feature creation help you to maintain Design Intent and also adjust it as necessary.