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Figure 8.22

The sketch for Step 5

8. Draw a two-point spline to join the ends of the 3D sketch entities that are closest to one another. Assign tangent relations to the ends to make the transition smooth. Figure 8.23 illustrates what the model should look like at this point.

Figure 8.23

The results up to Step 8

Tip

You may have to adjust the length of one of the spline tangency length arrows to keep the spline from remaining inside the cylinder of the helix.

9. Open a sketch on the Right plane, and draw an arc that is centered on the Origin and coincident with the end of the 3D sketch helix. The 185-degree angle is created by activating the dimension tool and clicking first the center of the arc and then the two endpoints of the arc. Now place the dimension. This type of dimensioning allows you to get an angle dimension without dimensioning to angled lines. Exit the sketch.

10. Create a composite curve (Insert⇒Curve⇒Composite) consisting of the 3D sketch and the new 2D sketch.

11. Create a new plane using the Normal to Curve option, selecting one end of the composite curve.

12. On the new plane, draw a circle that is centered on the end of the curve with a diameter of .120 inches. You need to create a Pierce relation between the center of the circle and the composite curve.

13. Create a sweep feature using the circle as the profile and the composite curve as the path. To create the sweep, you must first exit the sketch.

14. Hide any curves that still display.

15. Choose Insert⇒Cut⇒With Surface. From the Flyout FeatureManager, select the Right plane. Make sure that the arrow is pointing to the side of the plane with the least amount of material. Click OK to accept the cut. The finished part is shown in Figure 8.24.

Figure 8.24

The finished part

Summary

SolidWorks has a wide range of features beyond the basic extrudes and revolves. You saw the depth of the standard features in Chapter 7, and now in Chapter 8 you have seen the breadth of some of the less-used, but still useful operations. Not all of these secondary features measure up in terms of value for general modeling, but it is nice to know that if you need to show a model in a flexed in-use state, you at least don't have to directly model the deformed part manually.

Chapter 9: Patterning and Mirroring

In This Chapter

Using the Pattern function in sketch mode

Using the Mirror function in sketch mode

Using geometry pattern

Patterning or mirroring as bodies

Understanding Pattern faces

Patterning fillets with their parent geometry

Introducing pattern types

Creating the appearance of geometry with Cosmetic Patterns

Discover 3D mirroring techniques

Creating a circular pattern tutorial

Mirroring features tutorial

Applying a Cosmetic Pattern tutorial

Patterning and mirroring in SolidWorks are great tools to help you improve your efficiency. SolidWorks software provides many powerful pattern types that also help you accomplish design tasks. In addition to the different types of patterns, there are options that enable functionality that you may not have considered. A solid understanding of patterning and mirroring tools is necessary to be able to build the maximum amount of parametric intelligence into your models, and to open up the possibilities of your design objectives.

Patterning in a Sketch

You can use both pattern and mirror functions in sketch mode, although sketch patterns are not a preferred choice. The distinction between patterning and mirroring in sketch mode is important when it comes to sketch performance.

Performance

Although there are many metrics for how software performs, in SolidWorks, the word performance means the same thing as speed. Sketch patterns have a very adverse effect on speed and do not offer the same level of control as feature patterns.

You might hear a lot of conflicting information about which features are better to use in different situations.