Swept Cut
Swept Cut takes material away along a path. A closed profile, drawn in one sketch, travels along a path of lines and arcs drawn in another, and everything it passes through is cut out of the part. Up to two guide curves, each in a sketch of its own, can make the profile grow, shrink, stretch or turn as it goes, so the groove or hole changes size along its length. It is the cut side of Sweep: the same panel, set to Cut material.
When to Use It
- Cut a groove, a channel or a slot that follows a bent path, such as an O-ring groove or a cable channel
- Cut a hole whose size changes along its length, such as a tapered bore, with a guide curve
- Cut a groove that turns as it goes (Scale and twist) or widens one way only (Stretch with two guides)
- Cut a round channel of a set size along a path with Circular profile, with no profile sketch
Step by Step
- Start with a part to cut. Swept Cut needs a solid already there.
- Draw the profile: a closed shape in a sketch on the plane where the cut starts, often a face of the part. Click Exit Sketch so it waits in the Model tree (see Exit Sketch).
- Draw the path: lines and arcs joined end to end, in a sketch on a plane that crosses the profile, starting on the profile's plane. Click Exit Sketch.
- For a cut that changes size, draw one or two guide curves (optional, see Guide Curves below), each in a sketch of its own, and click Exit Sketch after each.
- Click Advanced on the Features tab, then Swept Cut. The panel opens as Swept Cut with Cut material lit.
- Pick the Profile, or click Circular profile and type a Diameter.
- Pick the Path: a path sketch, or Model edges to follow edges of the part.
- To guide the cut, pick a sketch under Guide curve 1 (and Guide curve 2 if you want), then choose Follow guides.
- On a part with more than one body, choose which bodies to cut under Bodies to cut in the Cut panel (see Extrude and Cut).
- Watch the red preview, then click Swept Cut.
Guide Curves
A guide curve for a swept cut is the same as for a sweep: an open run of lines and arcs in a sketch of its own that starts on the edge of the profile (on a side or a corner) and runs beside the path the whole way. As the profile travels, it changes so its edge stays on the guide, and the cut follows.
- Scale (one guide): the profile grows or shrinks evenly about the path.
- Scale and twist (one guide): the same, and the profile also turns to keep facing the guide.
- Stretch (two guides): the profile stretches along the line between the guides so it spans them; across that line it keeps its size.
- Scale (two guides): the profile grows or shrinks evenly so it spans the two guides.
The path must be one smooth open run that starts on the profile's plane. Twist Along Path is off while a guide is picked. The Sweep page has every rule for guide curves; they are the same for the cut.
Options
- Add material or Cut material: the panel heading reads Swept Boss/Base or Swept Cut. The Swept Cut button opens it as a cut, and after it the Sweep button opens as an added solid again. The two buttons in the panel switch it either way, and a choice made there stays; the lit button on the toolbar follows.
- Sketch profile or Circular profile with its Diameter.
- Path: a sketch, or Model edges of the part.
- Guide curve 1 and Guide curve 2: None, or a guide sketch. None on a list takes only that guide away.
- Follow guides: Scale or Scale and twist with one guide, Stretch or Scale with two.
- Orientation (no guides): Follow Path or Twist Along Path with a twist angle.
- Thin Feature: a wall of the profile's outline instead of the whole shape, as on the Sweep page. It does not work with guide curves yet.
- Bodies to cut: set in the Cut panel when the part has more than one body.
Edit It Later
Right-click the step in the Model tree and choose Edit Feature. A guided swept cut lists its Guide curves, each with a × that removes it, and Follow guides. Follow guides shows the choices for the guides left: with one left, a two guide Stretch becomes Scale and Scale and twist can be picked; with none left the list goes and the step is the plain swept cut. Click Apply to rebuild. To change the profile, the path or a guide, right-click its sketch under the step and choose Edit Sketch. To add a guide, delete the step and cut again. Undo puts a removed guide back.
Tips and What to Expect
- The cut is exact. A 20 mm cube cut by a 2 x 2 mm square swept 10 mm straight down from its top face, with one guide running from 1 mm to 2 mm out from the path, removes a tapered hole 2 x 2 at the top and 4 x 4 at the bottom: 10/3 x (4 + 16 + 8) = 93.333 mm3.
- With Circular profile and a guide, the round hole stays round as it grows.
- The red preview shows the shape that will be cut away, before you click.
- After the cut is made, the profile, path and guide sketches are taken into the step and show under it in the Model tree.
Common Problems
- "The cut removed no material." followed by "The swept shape does not pass through the part." The profile, the path or a guide put the shape off the part. Move them so the sweep runs into the part.
- "There is nothing to cut yet." Make a solid first, for example with Extrude.
- "That cut would remove every body, leaving nothing." Make the profile smaller or the path shorter.
- "Tick at least one body under Bodies to cut (Cut panel), or tick Cut every body it touches."
- "A sweep takes at most two guide curves. Remove one."
- "Guide curve 1 does not start on the edge of the profile: it starts 8.500 mm away from it." Snap the start of the guide onto a side or a corner of the profile.
- "Guide curve 1 does not reach the profile 80 percent of the way along the path." Make the guide run beside the path to its end.
- "Thin Feature does not work with guide curves yet." Set the guide curves to None, or untick Thin Feature.