SolidWorks 2011 Parts Bible - Matt Lombard [252]
FIGURE 19.14
A towel rack, modeled as a single part and broken into individual parts in an assembly
It is worth mentioning two potential difficulties that you may run into with methods like this. The first is that if you have people making drawings from parts that have been derived from bodies in a single part, then they are forced into the Reference Dimension scheme of dimensioning parts because the feature dimensions do not survive being moved from the multi-body part. This may or may not be an issue, depending on how the people doing the drawings are accustomed to working.
The second potential issue is what you do in situations where there are multiple instances of a part that has been modeled this way. Notice in the towel rack in Figure 19.14 that there are several finials, spacers, rails, and other parts that are duplicated. This requires some manual assembly modeling. You can make the assembly directly from the multi-body part, but if you need to make multiple instances of particular parts, you need to do this manually rather than automatically.
Creating Multi-Bodies
In the first section in this chapter, I raised the questions of if or when multi-bodies should be used, and in the second section, I raised the question of why multi-bodies should be used. In this section, I simply ask, or rather answer, how they should be used.
Using disjoint sketches
The easiest way to create multiple bodies is to simply create what SolidWorks classifies as multiple disjoint closed contours. What that means is simply two circles or rectangles that do not touch or overlap. If these are created in the same sketch, then when extruded, they will create as many bodies as there are closed loops in the sketch.
If the part has an existing solid, then creating a sketch that does not touch the solid can also create a separate body. You cannot make Multiple Thin features in a single sketch. This is presumably because the interface has no way to identify different thickness directions for different open profiles. This holds true whether or not the Multiple Thin features create multiple bodies.
If a solid feature other than a mirror or pattern touches a solid body, then the new and the old bodies will be merged into a single body.
Turning off the Merge Result option
You can prevent a feature from automatically combining with other bodies by deselecting the Merge Result option. This holds true between features, but not across all bodies in a part. For example, if an extrude feature uses the Merge result option, all the bodies that it touches become merged together, but if the original extrude feature does not touch a body, it will not be merged. This option is shown in Figure 19.15 and is found on all features that create new solid bodies except for the Patterns, Rib, and Move/Copy Bodies features.
FIGURE 19.15
The Merge result option
Applying the Feature Scope to bodies
The Feature Scope used for multi-bodies is not the same as the Feature Scope used for assembly features, but it does function in a similar way. In assemblies, the Feature Scope identifies which parts are affected by the current assembly feature. In parts, it only applies to bodies and can be used for features that add material as well as features that remove material (assembly features can only remove material).
The Feature Scope is a way to make the Merge result option more selective. The Merge result option by default does not discriminate; it causes the feature to merge with any other solid body that it touches. However, the Feature Scope enables the user to select which bodies to merge with or otherwise affect. Feature Scope also applies to additional feature types such as cuts. The Feature Scope becomes