SolidWorks 2011 Parts Bible - Matt Lombard [249]
FIGURE 19.8
Splitting a part to perform a local operation
Using the Shell feature
The Shell feature hollows out one solid body at a time. If there are multiple solid bodies, then you must select one to be shelled. Any face of the solid that you select will be removed during the shelling. You can select a body without selecting a face by using the small Solid Body selection box under the larger Faces to Remove selection box in the PropertyManager. If you do not select any faces to be removed, then the body will be hollowed out with no external indication that the part is hollow unless you view it in section view, transparency view, or wireframe view. Single or multiple faces can be removed. This feature works by offsetting the faces of the outside of the model, and the feature may fail if this causes problems with the internal geometry.
The Multi-thickness Shell option enables you to select faces that will have a different thickness from the overall shell thickness. This is one method that you can sometimes use to limit the scope of the Shell feature to a certain area of a body, but it is somewhat limited. Faces with different thicknesses cannot be tangent to one another.
Because the Shell feature only works on one body at a time, splitting a part into multiple bodies can be an effective way to limit the scope of the feature. The part shown in Figure 19.9 has been split in half, and one-half has been made transparent for visualization purposes; as a result, you can see that the part is shelled on the bottom on one end and on the top on the other end. The Shell feature has no option for doing this with existing geometry. The only ways that you can do this are either through feature order or by using multi-bodies. You can find the part shown in Figure 19.9 on the DVD with the name Chapter 19 – LocalOps Shell.sldprt.
FIGURE 19.9
Shelling locally
To shell the part this way with feature order, you create one block and shell it, and then create the other block and shell that. In order for this technique to work, the second shell needs to be as big as, or bigger than, the first shell. If it is smaller, then it will (or may) hollow out areas that are not intended to be hollow.
To shell the part with multi-bodies, you can use two methods. One method is to build the first block, and then build the second block but turn off the Merge option. This creates bodies that are side by side. You then shell one block on the bottom and the other on the top. To avoid a double-thickness wall between them, the end face can be removed along with either the top or bottom face. If you edit the part, then you may notice that one of the Shell features has two faces removed.
The second method is to build a single block, then split it using a sketch line, a plane, or a surface, and then proceed in the same way as the first method.
Patterning
Patterns of bodies are fast, powerful, and commonly used alternatives to patterning features. Chapter 8 discusses feature patterns and mirroring, and examines, at least in part, how different types of patterns affect model rebuild speeds. When appropriate, patterning bodies can also be a big rebuild time-saver. When patterning a body, none of the parametrics or intelligence is patterned with it, but you must pattern the entire body. Another odd thing about patterning bodies in SolidWorks is that there is no option to join the bodies either to one another or to a main body. This requires an extra step that involves adding a Combine feature. Mirroring is the same, except that it has an option