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This chapter is from the book

This chapter is from the book

Mastering SolidWorks, 3rd EditionMastering SolidWorks, 3rd Edition

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This chapter is from the book

This chapter is from the book

Mastering SolidWorks, 3rd EditionMastering SolidWorks, 3rd Edition

Learn More Buy

4.2 Features

To master feature-based modeling, you should be able to answer three fundamental questions:

  1. What are the available features that a CAD/CAM system offers for modeling parts?

  2. What is the input required to create each feature?

  3. 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.

Table 4.1 Available Features

No.

Feature

Input (sketch)

Resulting Feature

When to Use in Modeling?

1

Extrusion

Cross section and a thickness

  • Use for parts with constant cross section (CS) and uniform thickness (UT).

  • If needed, break part into subparts, each with a constant CS and UT.

2

Revolve

Cross section, an axis of revolution, and an angle of revolution

  • Use for parts that are axisymmetric.

  • If needed, break part into subparts, each of which is axisymmetric.

3

Sweep

Linear sweep: cross section and a line as a path

  • Use for parts with constant cross section (CS) along a linear direction (path) that may or may not be perpendicular to the cross section.

  • If the path is perpendicular to the cross section, the linear sweep becomes an extrusion.

Nonlinear sweep: cross section and a curve as a path

  • Use for parts with constant cross section (CS) along a nonlinear direction that may or may not be perpendicular to the cross section.

4

Loft

Linear loft: at least two cross sections (profiles)

  • Use for parts with variable cross section along a given direction.

  • The cross sections are blended linearly from one section to the other.

Nonlinear loft: at least two cross sections (profiles), and a curve as a guide curve

  • Use for parts with variable cross section along a given direction.

  • The cross sections are blended nonlinearly from one section to the other, along the guide curve.

5

Rib

Rib profile (e.g., line or stepwise line)

  • Use when a stiffener between angled walls (faces) of a part is required to increase part structural strength.

6

Shell

Shell face and shell wall thickness

  • Use when you need to remove material from an existing part.

  • The material removal (shelling) occurs in a direction perpendicular to the selected shelling face.

  • While you can achieve the same result using an extrude cut for simple shells, a shell operation is faster to use.

7

Draft

Direction of pull, parting lines, and a draft angle. The direction of pull must be perpendicular to the parting lines.

  • Use when you need to draft faces at an angle; usually used for injection molding to allow pulling the molded part from the mold cavity.

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.

Figure 4.2

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 > ✓.

Hands-on for Example 4.1

Re-create the free-form torus by replacing the spline by a circle that is not centric with the large circle.

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