Swept Boss/Base and Swept Cut¶
Sweeps a closed profile along a path to add material (Swept Boss/Base) or remove it (Swept Cut).
Features tab > Swept Boss/Base or Swept Cut, or Insert > Boss/Base > Swept… or Insert > Cut > Swept….

Creating a Sweep¶
- Sketch the profile, closed, on a plane perpendicular to the path where the path starts.
- Sketch the path in another sketch, starting on the profile's plane.
- Select the profile sketch, then the path sketch.
- Click Swept Boss/Base or Swept Cut.
- Click OK or press Enter.
Of the sketches selected, the first is the profile and the second the path. You can also select them after the page opens. With no sketch selected, a sketch that is the last feature in the design tree and is not used by a feature is taken as the profile.
Creating a Tube¶
- Draw the path in a 3D sketch, or in a 2D sketch.
- Select the path sketch alone. With a 3D sketch, click Swept Boss/Base and the page opens with Profile type set to Tube; with a 2D sketch, set Profile type to Tube on the page.
- Set Diameter and Wall thickness.
- Click OK or press Enter.
Profile and Path¶
- Profile type
- Sketch: the profile is a sketch. Tube: a round tube or rod, square to the path where the path starts, with no profile sketch.
- Profile
- The profile sketch. It must hold at least one closed profile, and its plane must be perpendicular to the path where the path starts.
- Diameter
- With Tube: the tube's outer diameter.
- Wall thickness
- With Tube: the tube's wall. Leave it blank for a solid rod.
- Path
-
The path: a sketch or a 3D sketch of one chain of lines, arcs and splines, or one circle; or model edges end to end. Construction geometry is left out. A 3D sketch's corners between lines are bent to its Bend radius. A tube starts at a free end of the path.
- An open chain must start on the profile's plane, at one of its ends.
- A closed chain must have a vertex on the profile's plane.
- A circle's center must lie on the profile's plane, and the plane must cross the circle.
The path must be tangent-continuous. Round sharp corners with sketch fillets. The profile and the path must be different sketches.

The profile keeps its orientation to the path as it sweeps.
End¶
Where the sweep ends. Path End: at the end of the path. Up To Surface: where it first reaches the face or plane in Up to, the path running on past it. Offset From Surface: as Up To Surface, stopped the Offset short of it (or past it, with the arrow button beside it). Up To Body: where it first reaches the body in Up to. The path must be open, and the whole profile must reach the surface or body.
Output¶
- Operation
- Join adds the sweep to the bodies it touches. Cut removes it from every body it passes through. Intersect keeps only what each body it overlaps has in common with it. New body makes it a separate body. A feature that still has its automatic name is renamed to match, for example Boss-Extrude1 to Cut-Extrude1. An Intersect feature cannot be patterned or mirrored.
When a Sweep Fails¶
The page shows the reason. Common causes:
- The profile's sketch is not perpendicular to the path where the path starts.
- The path turns sharply between two segments.
- The path branches or is in pieces.
- A path arc's radius is smaller than the profile, so the profile crosses the arc's axis.
A Swept Cut that misses the model still builds, with a warning that it does not intersect the model.