SolidWorks 2011 Parts Bible - Matt Lombard [71]
Best Practice
Do not dimension sketches to model edges that are created by fillets. While the previous best practice about relations to sketch entities instead of model edges was a mild warning, you must heed this one more carefully.
To add fillets and chamfers to your part, follow these steps:
1. Initiate a Fillet feature, and select the four short edges on the part. Set the radius value to .600 inches. Click OK to accept the Fillet feature.
Tip
When selecting edges around a four-sided part, the first three edges are usually visible and the fourth edge is not. You can select invisible edges by expanding the Fillet Options panel of the Fillet PropertyManager, and selecting the Select through faces option. When you have a complex part with many hidden edges, this setting can be bothersome, but in simple cases like this, it is useful. Figure 4.17 shows this option in action.
Figure 4.17
Selecting an edge through model faces
2. Apply chamfers to the edges of the angled slot through the part, as indicated in Figure 4.18. Make the chamfers .050 inches by 45 degrees.
Chamfers observe many of the same best practices as fillets.
Tip
Feature order is important with features like chamfers and fillets because of how they both tend to propagate around tangent edges. Although you can turn this setting off for both types of feature, it is best to get the correct geometry by applying the features in order.
Cross-Reference
The Fillet Xpert, which helps you to manage large numbers of overlapping fillets by automatically sorting through feature order issues, is discussed in detail in Chapter 20.
3. Select the four edges that are indicated for fillets in Figure 4.18. Apply .050-inch-radius fillets.
4. Apply a last set of .050-inch chamfers to the backside of the counterbores and slot.
Figure 4.18
Edges for fillet and chamfer features
The finished part is simple, but you have learned many useful techniques along the way.
On the DVD
You will find two video tutorials on the DVD for this chapter. One of them deals with the concept of feature-based modeling, and the other is a demonstration of creating a simple part and drawing.
Tutorial: Making a Simple Drawing
In SolidWorks, drawing views are created from the 3D model. Even the most complex section views are almost free, because they are simply projected from the 3D model. When you make changes to the 3D model, all 2D views update automatically. You can handle dimensions in a couple of ways, either using the dimensions that you used to create the model or placing new dimensions on the drawing (best practice for modeling is not necessarily the same as best practice for manufacturing drawings). To make a simple drawing of a SolidWorks native part, follow these steps:
1. Click the New button from the Standard toolbar or choose File⇒New. From the New SolidWorks Document window, select the Drawing template. The template contains all the document-specific settings.
2. After selecting the drawing template, the Sheet Format/Size dialog box appears, as shown in Figure 4.19. Select the D-Landscape sheet size, as well as the format that automatically associates with that sheet size, and click OK. If the Model View PropertyManager appears, click the red X icon to exit.
Figure 4.19
The Sheet Format/Size dialog box
3. Before creating any views on the drawing, set up some fields in the format to be filled out automatically when you bring the part into the drawing. Right-click anywhere on the drawing sheet (on the paper) and select Edit Sheet Format.
4. Zoom in to the lower-right corner of the drawing. Notice that there are several variables with the format $PRPSHEET:{Description}. These annotations