SolidWorks 2011 Parts Bible - Matt Lombard [68]
Tip
You can view individual sketches and reference geometry entities such as planes from the RMB menu. The global settings for the visibility of these items are found in the View menu. You can access these items faster by using the View toolbar, or by linking the commands to hotkeys.
2. Right-click the sketch in the graphics window and click Select Chain. This selects any non-construction, end-to-end sketch entities. Click Offset Entities on the Sketch toolbar. Offset to the inside by .400 inches. Apply .500-inch sketch fillets to each of the corners.
3. Click Extruded Cut on the Feature toolbar. By default, the extruded cut will cut away everything inside the closed profile of the sketch. Look down the FeatureManager window and select the check box on the top bar of the Thin Feature panel. Make the cut Blind, .100 inch. The Thin Feature type should be set to Mid Plane with a width of .400 inches. The PropertyManager and graphics window should look like Figure 4.9.
Figure 4.9
Creating the groove with a thin feature cut
Using sketch techniques
Although you could create the next two features more easily and efficiently using a cut, I will show you how to create them as two extrudes. The intent here is to show some useful sketch techniques rather than optimum efficiency. Begin with the part from the previous section and follow these steps:
1. Open a new sketch on the large face opposite from the groove. Draw a corner rectangle picking up the automatic coincident relation to one corner and then dragging across the part and picking up another coincident to the edge on the opposite side. Figure 4.10 shows the rectangle before and after this edit.
Tip
If you want to continue using the recommended best practice mentioned earlier of making relations to sketches rather than model edges, here are a few tips. In some situations (such as the current one), the sketch plane is offset from the sketch that you want to make relations to, and the best bet is to use the Normal To view. The next obstacle is making sure that automatic relations pick up the sketch rather than the edge, and so you can use the Selection Filter to select sketch entities only.
2. Delete the Horizontal relation on the line that is not lined up with an edge. This enables you to drag it to an angle or apply the dimensions shown in Figure 4.10.
3. Extrude sketch to a depth of 0.25 inch.
You can delete the Horizontal relation by selecting the icon on the screen and pressing Delete on the keyboard. As a reminder, you can show and hide the sketch relation icons from the View menu. You can check to ensure that the relations were created to the sketch rather than the model edges by clicking the Display/Delete Relations button on the Sketch toolbar, clicking the relation icon to check, and expanding the Entities panel in the PropertyManager. The Entities box shows where the relation is attached to, as shown in Figure 4.11. In this case, it is a point in Sketch1. Without custom programming, there is no way to identify items in a sketch by name, but you already know which point it is; you just needed to know whether it was in the sketch or on the model. The second sketch trick involves the use of a setting.
Figure 4.10
Edits to a rectangle
Figure 4.11
The Display/Delete Relations dialog box
4. Choose Tools⇒Options⇒Sketch and ensure that Prompt to Close Sketch is turned on; then click OK to close the dialog box.
5. Open another new sketch on the same face that was used by the last extrusion. Draw an angled line across the left and bottom sides of the box with the dimensions shown in Figure 4.12. In this case, for this technique to work, the endpoints of the line have to be coincident with the model edges rather than the sketch entities.
This line by itself constitutes an open sketch profile, meaning that it does not enclose an area and has unshared endpoints.