Access
Ribbon:
3D Model tab
Create panel
Sweep
- Profile
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Specifies one or more profiles of a sketch to sweep along the selected path. Use closed profiles to create either solid or surface sweep features. Use open profiles to create only surface sweep features. Hold down Ctrl to cancel the selection of profiles.
- Path
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Specifies the trajectory or path for the profile sweep. The path can be an open or closed loop, but must pierce the profile plane.
- Solids
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In a multi-body part file, specifies the participating solid bodies. Not available in a part file with only one solid body.
Type
The selected sweep type determines displayed options.
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Path
Orientation:
Path -
Holds the swept profile constant to the sweep path. All sweep sections maintain the original profile relationship to the path.
Parallel -
Holds the swept profile parallel to the original profile.
- Taper
-
Sets taper angle for sweeps normal to the sketch plane (not available for Parallel). The taper is shown in the solid sweep preview. Not available for closed paths.
Positive Angle taper angle increases the section area as the sweep moves away from the start point.
Negative Angle taper angle decreases the section area as the sweep moves away from the start point.
Nested Profiles the sign (positive or negative) of the taper angle is applied to the outer loop of nested profiles; inner loops have the opposite sign.
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Path & Guide Rail
- Guide Rail
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Selects a guide curve or rail that controls the scaling and twist of the swept profile. The guide rail must pierce the profile plane.
- Profile Scaling
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Specifies how the swept section scales to meet the guide rail.
- X & Y
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Scales the profile in both the X and Y directions as the sweep progresses.
- X
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Scales the profile in the X direction as the sweep progresses.
- None
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Keeps the profile at a constant shape and size as the sweep progresses. Using this option, the rail controls only profile twist.
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Path & Guide Surface
- Guide Surface
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Specifies a surface whose normal controls the twist of the swept profile about the path. For best results, the path should be on or near the guide surface.
Output
Solid -
Creates a solid feature from an open or closed profile. Open profile is not available for base features.
Surface -
Creates a surface feature from an open or closed profile. Can be used as a construction surface on which other features terminate, or as a split tool to create a split part.
Not available in the assembly environment.
Operation
Specifies whether the sweep joins, cuts, or intersects with another feature, or creates a new solid body. Not available for base features, but is required for all other sweep features.
Join -
Adds the volume created by the sweep feature to another feature or body.
Not available in the assembly environment.
Cut -
Removes the volume created by the sweep feature from another feature or body.
Intersect -
Creates a new feature from the shared volume of the sweep feature and another feature or body. Material not included in the shared volume is deleted.
Not available in the assembly environment.
New solid -
Creates a new solid body. If the sweep is the first solid feature in a part file, this selection is the default. Select to create a new body in a part file with existing solid bodies. Each body is an independent collection of features separate from other bodies. A body can share features with other bodies.
- Optimize for Single Selection
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Automatically advances to the next selector if you make a single selection. To make multiple selections, clear the check box.
- Preview
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Provides a solid preview of the sweep based on the current selections. If Preview is enabled, and no preview appears in the graphics window, it usually means the sweep feature was not created.
Tip: To save computation time for complex sweeps, clear the Preview check box, provide the necessary input in the dialog box, and then enable the Preview again.