SolidWorks 2011 Parts Bible - Matt Lombard [127]
FIGURE 8.9
A part created from a composite curve
Using Split lines
Split lines are not exactly curves; they are just edges that split faces into multiple faces. Split lines are used for several purposes, but are primarily intended to split faces so that draft can be added. They are also used for creating a broken-out face for a color break or to create an edge for a hold line fillet, discussed in Chapter 7.
There are some limitations to using split lines. First, they must split a face into at least two fully enclosed areas. You cannot have a split line with an open loop sketch where the ends of the loop are on the face that is to be split; they must either hang off the face to be split or be coincident with the edges. If you think you need a split line from an open loop, try using a projected curve instead.
The SolidWorks 2010 version removed some other long-standing limitations, such as splitting on multiple bodies, using multiple closed loops, and using nested loops. These much-needed improvements will help users avoid workarounds.
Caution
A word of caution is needed when using split lines, especially if you plan to add or remove split lines from an existing model. The split lines should go as far down the tree as possible. Split lines change the face IDs of the faces that they split, and often the edges as well. If you roll back and apply a split line before existing features, you may have a significant amount of cleanup to do. Similarly, if you remove a split line that already has several dependent features, many other features may also be deleted or simply lose their references.
Using the equation driven curve
The equation driven curve is not really a curve feature; it is a sketch entity. It specifies a spline inside a 2D sketch with an actual equation. Even though this is a spline-based sketch entity, it can only be controlled through the equation, and not by using spline controls. This feature is covered in more detail in Chapter 3, with other sketch entities.
Selecting a Specialty Feature
SolidWorks contains several specialty features that perform tasks that you will use less often than some of the standard features mentioned in Chapter 7. Although you will not use these features as frequently as others, you should still be aware of them and what they do, because you never know when you will need them.
These features include:
• Scale
• Dome
• Wrap
• Flex
• Deform
• Indent
Other types of less commonly used features fall into specialty categories such as sheet metal, multi-bodies, surfacing, plastics, or mold design. This includes features such as Freeform, Combine, Cavity, Scale, and several others. I placed the discussion about these features in chapters devoted to those specialized topics. The features treated in this chapter are more general use features.
Using Scale
The Scale feature, found at Insert⇒Feature⇒Scale, is mainly used for preparing models of plastic parts to make mold cavity geometry; however, it can be used for any purpose on solid or surface geometry. Scale does not act by scaling up dimensions for individual sketches and features; rather, it scales the entire part at the point in the FeatureManager history at which it is applied. The Scale PropertyManager is shown in Figure 8.10.
FIGURE 8.10
Applying the Scale feature
The Scale feature only becomes available when the part contains at least one solid or surface body. You can scale multiple bodies at once and can select from one of three options for the “Scale About” or fixed reference: the part origin, the geometry centroid, or a custom coordinate system. Of these, it is generally preferable to select the part origin because it is most often the case that you would want the standard planes moving with respect to the rest of the part as little as possible. If you needed to scale about a specific point on the geometry, you would need to create