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The error caused by a Shape feature being forced to update in SolidWorks 2010 or later is shown in Figure 8.11.

FIGURE 8.11

Shape features may fail in SolidWorks 2010 and later

The Dome feature has two notable settings: the Elliptical Dome and Continuous Dome.

The Elliptical Dome is available only on flat faces where the boundary is either a complete circle or an ellipse. The cross-section of the dome is elliptical and does not account for draft, which means that it is always tangent to the perpendicular from the selected flat face.

The Continuous Dome is a setting for any noncircular or elliptical face, including polygons and closed-loop splines. The setting results in a single unbroken face. If you deselect the Continuous Dome setting, it functions like the Elliptical Dome setting. Figure 8.12 shows the most useful settings for the Dome feature.

The workflow for the Dome feature is as follows:

1. Select an area to be domed, or use a split line to create an area to be domed on an existing face.

2. Initiate the Dome feature, set a height, tell it to add or remove material, and set the other settings including the constraint sketch.

3. Accept the feature with the green check mark.

FIGURE 8.12

Examples of various types of domes

Using the Wrap feature

The Wrap feature enables you to wrap 2D sketches around cylindrical and conical faces. However, trying to wrap around 360 degrees can cause some difficulties, although all the available documentation from SolidWorks on the Wrap feature says that you can wrap onto a conical surface.

The Wrap feature works by flattening the face, relating the sketch to the flat pattern of the face, and then mapping the face boundaries and sketch back onto the 3D face. The reason why it is limited to cylindrical and conical faces is that these types of geometry are developable. This means that the faces can be mapped to the flat pattern through some relatively simple techniques that happen behind the scenes. Developable geometry can be flattened without stretching. You will see in a later chapter that sheet metal functions are limited in the same way and for the same reasons.

SolidWorks does not wrap onto other types of surfaces, such as spherical, toroidal, or general NURBS surfaces, because you cannot flatten these shapes without distorting or stretching the material. The distinguishing characteristic is that Wrap works on faces with curvature in only one direction and will not work with compound curvature. There is software that can flatten these shapes, but it is typically done for sheet metal deep-drawing applications, which highly deform the metal. Figure 8.13 shows the Wrap PropertyManager interface.

The Wrap feature has three main options:

• Emboss

• Deboss

• Scribe

Using Scribe

Scribe is the simplest of the options to explain, and understanding it can help you understand the other options. Scribe creates a split line–like edge on the face.

FIGURE 8.13

The Wrap PropertyManager interface

Several requirements must be met in order to make a wrap feature work:

• The face must be a cylindrical or conical face.

• The loop must be a closed loop or nested closed loop 2D sketch.

• The sketch must be on a plane that is either tangent to or parallel to another plane that is tangent to the face.

• Wrap supports multiple closed loops within a single feature.

• Wrap supports wrapping onto multiple faces.

• The wrap should not be self-intersecting when it wraps around the part. (Self-intersection will not cause the feature to fail, but on the other types, Emboss and Deboss, it may produce unexpected results.)

Scribes can be created on solid or surface faces. Scribed surfaces are frequently thickened to create a boss or a cut. Figure 8.13 shows a scribed wrap.

Using Emboss

The Wrap Emboss option works much like the scribe, but it adds material inside the closed loop sketch, at the thickness that you specify in the Emboss PropertyManager. Embossing can only be done on solid geometry. If the feature