A sweep creates a base, boss, cut, or surface by moving a profile along a path, or by specifying a path and a diameter.
There are three types of profiles:
- A sketch profile creates a sweep by moving a 2D profile along a 2D or 3D sketch path.
- A circular profile creates a solid rod or hollow tube along a sketch line, edge, or curve directly on a model, without having to sketch.
- A solid profile creates a cut sweep using a tool body and path, for example to create a cut around a cylindrical body.
If you use a sketch profile, you must follow these rules:
- The profile must be closed for a base or boss sweep feature; the profile may be open or closed for a surface sweep feature.
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The path may be open or closed.
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The path may be a set of sketched curves contained in one sketch, a curve, or a set of model edges.
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The path must intersect the plane of the profile.
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Neither the section, the path, nor the resulting solid can be self-intersecting.
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The guide curve must be coincident with the profile or with a point in the profile sketch.
For a circular profile, you only need to select an existing path and specify a diameter. You do not need to sketch the profile.
For cut sweeps only, you create a solid sweep by moving a tool body along a path. The path must be tangent within itself (no sharp corners) and begin at a point on or within the tool body profile.
You can view the sweep using zebra stripes as you create the sweep. Place the pointer on the sweep, open the shortcut menu, and select Zebra Stripes Preview. If you apply zebra stripes, when you create another sweep, or loft, or add a loft section, the zebra stripes appear. Use the shortcut menu to clear Zebra Stripes Preview.