SolidWorks 2011 Parts Bible - Matt Lombard [286]
Lofted Bends is not part of the Base Flange method, but it is part of the newer set of sheet metal tools available in SolidWorks. Figure 21.35 shows what is probably the most common application of this feature. The bend lines shown must be established in the PropertyManager when you create or edit the feature. Bend Lines are only an option if both profiles have the same number of straight lines. For example, if one of the profiles is a circle instead of a rectangle with very large fillets, then the Bend Lines options are not available in the PropertyManager.
FIGURE 21.35
The Lofted Bends PropertyManager, a sample, and a Flat Pattern with bend lines
Like the forming tools, you can also use Lofted Bends in situations for which they were probably not intended. Figure 21.36 shows how lofting between 3D curves can also create shapes that can be flattened in SolidWorks. In this case, a couple of intermediate steps were required to get to the 3D curves, which involve surface features.
Note
This part is included on the DVD with the name Chapter 21– wrap.sldprt.
FIGURE 21.36
Using 3D curves with Lofted Bends to create flatten complex shapes
Using the Unfold and Fold features
Unfold is a feature that unfolds selected bends temporarily. It is typically used in conjunction with a Fold feature to refold the bends. This combination is used to apply a feature that must be applied to the Flat Pattern; for example, a hole that spans across a bend.
Figure 21.37 shows the FeatureManager of a part where this combination has been applied, as well as the part itself, showing the bend across a hole, and the PropertyManager, which is the same for both features.
FIGURE 21.37
Applying the Unfold and Fold features
Both the Unfold and Fold features make it easy to select the bends without zooming in, even for small bends. A filter is placed on the cursor when the command is active, which allows only bends to be selected. The Collect All Bends option also becomes available. This feature also requires that you select a stationary face to hold still while the rest of the model moves during the unfolding and folding process.
Making Sheet Metal Parts from Generic Models
SolidWorks can also convert generic constant thickness models into sheet metal parts that flatten, and on which any of the dedicated sheet metal features can be used. You can make models from thin feature extrudes or regular extrudes with Shell features, and then use the Insert Bends feature to make them sheet metal parts. The structure of parts created with the Insert Bends feature is somewhat different. Figure 21.38 shows a comparison of the two methods' FeatureManagers for simple parts.
FIGURE 21.38
A comparison between default features for Base Flange and Insert Bends
The most notable difference is that the Insert Bends part starts off with non–sheet metal features. The Rip feature also stands out, but the Rip feature is not exclusive to sheet metal. Although you can use Rip on any model, it is found only on the Sheet Metal toolbar.
The Sheet Metal feature is found in both the Base Flange and Insert Bends methods and has the same PropertyManager function in both methods.
The new features in the Insert Bends method are the Flatten Bends and Process Bends features. The way the Insert Bends method works is that the model that is built with the sharp-cornered non–sheet metal feature is flattened by the Flatten Bends feature. The model is then reconstructed with bends by the Process Bends feature.
The main rule that SolidWorks enforces on sheet metal models regardless of how they came to be sheet metal is that the parts should have a consistent wall thickness. When all the geometry is made from the beginning as a sheet metal part (using the Base Flange method), there is never a problem with this. However, when the part is modeled from thin features, cuts, shells, and so on, there