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Tip

You can either hide or show different types of entities in groups by using the View menu. Hide All Types hides everything, and disables the options for individual entity types to be used.

11. Open a sketch on the Right plane. Sketch an ellipse such that the center is oriented 1.750 inches vertically from the Origin, and the ellipse measures .750 inches horizontally and 1.500 inches vertically.

12. Extrude this ellipse using the Up To Next end condition. If Up To Next does not appear in the list, then change the direction of the extrude and try it again.

13. Show the sketch of the Bosses feature by expanding the feature (click the “+” next to it), right- or left-clicking the sketch icon, and clicking the Hide/Show icon (eyeglasses). Next, open a sketch on the Right plane. Sketch two circles that are concentric with the original circles, with the dimensions of .875 inches and 1.250 inches. Exit the sketch.

14. Use Instant 3D to create an extruded cut that goes through the large circular bosses. This feature will look like a boss extrusion at first, so when you have finished dragging its depth, a small toolbar with two icons appears. One of the icons enables you to add draft; the other enables you to turn the boss into a cut. Figure 7.55 shows the state of the model up to this step.

Figure 7.55

The results up to Step 14

15. Start a fillet feature, and select the face of the Loft feature. Assign a radius of .200 inches.

Note

Although this fillet is created by selecting a face, it is not a face fillet. Selecting a face for a regular constant radius fillet simply fillets any edge that is on the face.

16. Create a mirror feature, using the Right plane as the mirror plane. In the Mirror PropertyManager, expand the Bodies To Mirror panel, and select anywhere on the part. Make sure that the Merge Solids option is selected. Click OK to accept the mirror.

17. Orient the view to the Front view, and then turn the view on its side (hold down Alt and press the left- or right-arrow key six times).

18. Open a new sketch on the Front plane. From the View menu, make sure that Hide All Types is not selected, and show Temporary Axes. Draw and dimension a horizontal construction line, as shown in Figure 7.56.

Figure 7.56

The results up to Step 18

19. With the construction line selected, start the Sketch Text command (Tools⇒Sketch Entities⇒Text). Make sure that the line appears in the Curves selection box.

20. Click in the text box, and type Made in USA (or your name or company name). Select the text and click the Bold button. Deselect the Use Document Font option, change the font to use units, and set the height to .175 inches.

21. Click OK to exit the Sketch Text PropertyManager, and click OK again to exit the sketch. You can turn off the Temporary Axis display.

22. Choose Insert⇒Features⇒Wrap. You should be prompted to select a plane or a sketch. Use the Flyout FeatureManager to select the sketch that you just created with the sketch text in it. Next, select the cylindrical face of the boss to see a preview of the text wrapped onto the face. If the text appears backward, then select the Reverse Direction option in the Wrap PropertyManager.

23. Select the Emboss option, and assign a thickness of .025 inches. Click in the Pull Direction selection box and select the Front plane. Click OK to accept the feature.

24. Save the part and close it. If you would like to examine the reference part, you can find it on the DVD with the filename Chapter 7 Tutorial Bracket Casting.sldprt. The finished part is shown in Figure 7.57.

Figure 7.57

The finished part

Summary

SolidWorks has a wide selection of feature types to choose from, ranging from simple extrudes and revolves to more complex lofts and sweeps. Some features have so many options that it may be difficult to take them all in at once. You should browse through the models on the DVD for this chapter and use the Rollback