This chapter is from the book
This chapter is from the book
This chapter is from the book
4.2 Features
To master feature-based modeling, you should be able to answer three fundamental questions:
What are the available features that a CAD/CAM system offers for modeling parts?
What is the input required to create each feature?
Which feature should you use for a given modeling problem?
Section 4.1 and Figure 4.1 provide the answer to the first question. Table 4.1 answers the other two questions. It shows a simple basic example of each feature. Keep in mind that the third question may have multiple answers; one of them is always the best answer. For example, you may use a loft or a sweep. However, if a part has a constant cross section along a curve, sweep is better to use because it requires fewer steps to create the part. If the part has a variable cross section, a loft is better to use. The tutorials in this chapter provide some modeling examples.
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The other features shown in Figure 4.1 and not covered in Table 4.1 are covered in the tutorials in this chapter.
Example 4.1
Create the free-form torus shown in Figure 4.2.
Solution The torus shown in Figure 4.2 is a variation of the torus (donut shape) feature (No. 2) shown in Table 4.1. While that feature of Table 4.1 is a revolve, the free-form torus shown in Figure 4.2 can only be created as a sweep. The key modeling concept here is to use pierce relations to force the torus cross section (small circle) to conform to the sweep path (large circle) and the guide curve (closed spline), as shown in Figure 4.2. You pierce the small circle to the spline and pierce the center of the small circle to the large circle. These two pierce conditions force the small circle to become “elastic”; that is, it expands and shrinks, as it must always touch the spline and the big circle. Pierce condition is only available to pierce a point to a curve. You cannot pierce two curves. SolidWorks enables the pierce condition in the right context.
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Figure 4.2 Free-form torus
Step 1: Create Sketch1-Path (sweep path): File > New > Part > OK > Top Plane > Sketch tab > Circle on Sketch tab > click origin to sketch and dimension as shown > exit sketch > File > Save As > example4.1 > Save.
Step 2. Create Sketch2-Guide (sweep guide curve): Top Plane > Sketch tab > Spline on Sketch tab > sketch free spline as shown > exit sketch.
Note: Sketch1-Path and Sketch2-Guide are two separate sketches, and they both use Top Plane.
Step 3. Create Sketch3-Profile (sweep profile): Front Plane > Sketch tab > Circle on Sketch tab > sketch a circle anywhere > Point on Sketch tab > click circle anywhere.
Note: Do not dimension the circle as doing so over-constrains it when you apply the pierce relation.
Step 4. Create pierce relations: While Sketch3-Profile is still open from Step 3, click small circle center + Ctrl + select large circle > Pierce relation > ✓ > select point created on circle + Ctrl + spline > Pierce relation > ✓ > exit sketch.
Step 5. Create Sweep-Torus feature: Features tab > Swept Boss/Base > select Sketch3-Profile as Profile > select Sketch1-Path as Path > select Sketch2-Guide as Guide Curve > ✓.
