SolidWorks 2011 Parts Bible - Matt Lombard [254]
FIGURE 19.17
The Bodies to Keep dialog box
Notice that the Bodies to Keep settings are also configurable; therefore, different bodies can be kept in different configurations, which is very useful.
Managing bodies with the Split feature
The Split feature has essentially three functions:
• To split a single solid body into multiple solid bodies using planes, sketches, or surface bodies
• To save individual solid bodies out to individual part files
• To reassemble individual part files that are saved out into an assembly where the parts are all positioned in the same relative position as their corresponding bodies
The part of the Split feature that concerns this chapter is the first function mentioned, which is splitting a single solid body into multiple bodies using a sketch, a plane, or a surface body.
The Split feature cannot be used to split surface bodies. In fact, nothing in SolidWorks can split surface bodies. Only solid bodies can be split. Surface bodies can only be trimmed, so the effective workaround for not being able to split surface bodies is to copy the body, then trim and keep one side of the copy and the other side of the original. This seems like a functionality oversight, and would make a great enhancement request if you have ever come across the need for this functionality.
Splitting with a sketch
When you are using a sketch to split a single solid body into multiple bodies, the Split process works like this:
1. Create a sketch with an open or closed loop; even a mixture of open and closed profiles will work. If it is open, then the endpoints have to either be on an exterior edge or hanging off into space; they cannot actually be inside the boundaries of the solid.
2. Initiate the Split feature from the Features toolbar or from the menus by choosing Insert⇒Features⇒Split. You can do this with the sketch active, with the sketch inactive but selected, or with nothing selected at all.
3. Click the Cut Part button. This does not actually cut anything; it only previews the split. When this is done, the resulting bodies appear in the window below and callout flags are placed on the part in the graphics window. These flags are often useless because they tend to point to the borders between two different bodies in such a way that it is completely ambiguous as to which body they are indicating. However, in the example shown in Figure 19.18, the result is very clear.
Check marks next to the body in the list indicate that the body will be split out. The lack of a check mark does not necessarily mean anything. For example, in Figure 19.18, notice that two boxes are checked, but this will result in a total of four bodies. If only Body 1 were selected, then the result would be only two bodies.
Clicking the Save All Bodies button simply puts check marks in all the boxes. If the Resulting Bodies box contains more than ten bodies, then the interface changes slightly, as shown in the image to the right in Figure 19.18. The Consume cut bodies option removes, or consumes, any of the bodies that have a check mark.
Figure 19.18
Using the Split feature
Splitting with a plane
Splitting with a plane provides the same type of results, and uses the same options, as splitting with a sketch. However, you never have to worry about the plane being extended far enough, because the cut is made from the infinite extension of the plane. The only thing you have to worry about with a plane is whether it intersects the part.
Splitting with a surface body
Surface bodies are used to split solid bodies for a couple of reasons. In the part shown in Figure 19.10, a surface body was used to make the split instead of a sketch or a plane, because both of those entities split everything in an infinite distance either normal to the sketch plane or in the selected plane. A surface body only splits to the extents of the splitting surface body. If you look closely at the part, you