SolidWorks 2011 Parts Bible - Matt Lombard [278]
Auto reliefs were formerly called Bend reliefs. You can specify three different Auto relief options to be applied automatically to bends that end in the middle of material. These options are illustrated in Figure 21.9.
FIGURE 21.9
The three Auto relief configurations: Rectangular, Tear, and Obround
For the Rectangular and Obround types, you can control the width and the distance past the tangent line of the bend through the Relief Ratio selection box, which is immediately below the type selection box in the Sheet Metal PropertyManager. This ratio is the width of the relief divided by the part thickness. For the Rectangular relief, a ratio of .5 and a thickness of .050 inches means that the relief is .025 inches wide and that it goes .025 inches deeper into the part beyond the tangent line of the bend. The Obround relief goes slightly deeper because it has a full radius after the distance past the tangent line of the bend, and so it essentially goes a total of one full material thickness past the tangent line.
The Tear relief is simply a face-to-face shear of the material with no gap.
Using the Flat Pattern feature
The Flat Pattern feature is added automatically to the end of the tree when the Base Flange feature is added. This feature is used to flatten the sheet metal part when the feature is unsuppressed. The Flatten toolbar button acts as a toggle to unsuppress or suppress the Flat Pattern feature in the tree. It may be a little confusing, but the Flatten toolbar button and the flat-pattern feature in the FeatureManager refer to the same functionality. As mentioned earlier, the Flat Pattern has a couple of special properties that are not seen in other features. The first is that it remains at the bottom of the FeatureManager when other Sheet Metal features are added.
The second property of the Flat Pattern feature is that it is added in the suppressed state. When it is unsuppressed, it flattens out the sheet metal bends.
Notice also that the Flat Pattern PropertyManager allows you to select an edge, axis, or sketch line to denote the grain of the material.
By editing the Flat Pattern feature, you can set a few options. The Flat Pattern PropertyManager is shown in Figure 21.10.
FIGURE 21.10
The Flat Pattern PropertyManager
The Fixed face parameter determines which face remains stationary when the part is flattened out. Generally, the largest face available is selected automatically, but if you want to specify a different face to remain stationary, you can do that here.
When the Merge faces option is selected, it causes the Flat Pattern to form a single face rather than being broken up by the tangent lines around the bends. This does a few things. First, selecting the face of the flattened part and clicking Convert Entities (found on the Sketch toolbar) makes an outline of the entire flattened part, which is easier to use for certain programming applications. Second, the edges around the outside are not broken up. Third, the tangent edges around the bends are not shown. The differences between Flat Patterns with this option selected and unselected are shown in Figure 21.11.
Bend lines are shown in both examples in Figure 21.11.
When you turn on the Simplify Bends option, it simplifies curved edges that are caused by flattening bends to straight lines from arcs or splines. When the option is off, the complex edges remain complex. Simple edges can be cut by standard punches and do not require Computer Numerical Control (CNC) controlled lasers or abrasive water jets.
The Corner Treatment option controls whether or not a corner treatment is applied to the Flat Pattern of a part. The corner treatment is illustrated in Figure 21.12. The model used to create this corner used a Miter Flange around the edges of a rectangular sheet.
FIGURE 21.11
The Merge Faces option showing on and off
FIGURE 21.12
Using the Corner Treatment setting in the Flat Pattern PropertyManager
Note
You can export a *.dxf file of the Flat