SolidWorks 2011 Assemblies Bible - Matt Lombard [100]
SolidWorks allows only certain types of features to be used as assembly cuts:
• Extruded cuts
• Revolved cuts
• Hole features
For example, you cannot use a lofted cut as an assembly feature, but you can use a lofted solid in a cavity feature (which is an in-context feature, not an assembly feature). You could also do a lofted cut of a combined solid in a single part, then split the part into multiple bodies, and then into multiple parts (using master model techniques discussed in Chapter 19). SolidWorks provides many ways to do almost anything you can imagine. Your job is to determine which methods give you the most flexibility, cost you the least time, and give the most accurate results.
When you set up an assembly cut, you do it in the same way that you would set up a cut in the part environment, but with a couple of exceptions.
First, it is best to sketch on an assembly plane rather than a part face or plane that belongs to a part. This is not a requirement; it is just a best-practice suggestion.
Second, you have to use the Feature Scope to tell SolidWorks if you want to cut through all possible components, or just selected components. Further, you can have SolidWorks automatically select parts for you. For the most stable results, it is probably best to select the parts manually you want to cut. This avoids automating mistakes and additional rebuild time that might be caused by giving the software too much control over your design.
Sometimes assembly cuts are created for documentation purposes rather than design purposes. For example, if you want to cut a model section and display it in an isometric view, or an exploded section view, you have to do that using an assembly cut, probably in conjunction with a configuration so that you can also show the assembly without the section. For example, Figure 11.1 shows an isometric cutaway view created by an assembly feature, Cut Extrude.
FIGURE 11.1
Using an assembly feature to cut away a model for illustration purposes
When you place a feature in the assembly like this, the cut only exists in the assembly. If you open up any individual part in its own window, the part is not cut. If you open the part in another assembly, the part is not cut there either. The cut only exists within the assembly in which it was made.
Figure 11.2 shows the PropertyManager of the cut. The Cut-Extrude1 feature is displayed in the FeatureManager of the assembly, after the Mate folder, local patterns, and even after an assembly sketch.
FIGURE 11.2
The assembly cut is created and then displayed in the FeatureManager of the assembly.
Using the Feature Scope
You can access the Feature Scope in the PropertyManager. In this example, all of the parts were cut because the cut went through the entire assembly. In reality, some of the parts may not have needed to be cut, but in this case, it would have taken longer to find them than it did to just cut all the parts. You can partially cut the assembly in a couple of different ways. One way is to orient the feature such that you can control the depth of the cut by the sketch, and then sketch to suit your needs. Another way is to use the blind cut depth to control the depth. Finally, of course, you can use the Feature Scope to avoid cutting certain parts.
Propagating features to parts
One of the common mistakes SolidWorks users make is sketching in the assembly when they mean to sketch in a part in order to create a feature in the part. For example, you may not be paying attention to what you are doing, and forget to click that “Edit Part” button before starting a sketch.
In addition to that common mistake, sometimes features are simply easier to draw at the assembly level, and, especially if they affect multiple parts, you may want to find an easy fix. Well, there is one. The Feature Scope panel of the assembly feature Cut-Extrude PropertyManager contains an option called Propagate Feature to Parts.