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Features · Lesson 14

SOLIDWORKS Sweep

Sweep moves a profile along a path, like squeezing toothpaste along a curve. It makes pipes, handles, springs, wires and O-rings. You need two sketches: a closed profile and a path that crosses the profile's plane. For round sections you can skip the profile sketch entirely — since SOLIDWORKS 2016 a circular profile just needs a diameter.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Circular profile swept along a bent path into a curved rod with the path shown

Where to find it

Features tab → Swept Boss/Base; Swept Cut

Sweep options

Option What it does
Sketch Profile / Circular Profile Sketched shape, or just a diameter (since 2016)
Solid Profile (Swept Cut only) Sweeps a tool body — e.g. a cutter — along a path
Profile orientation Follow Path (default) or Keep Normal Constant
Profile Twist Twist along the path in degrees or revolutions
Guide Curves Extra curves that change the profile's size or shape along the path
Thin Feature Hollow sweep, e.g. a tube

Tips

  • Draw the path first, then put the profile on a plane at its start.
  • Multiple guide curves can live in one sketch.
  • For coiled springs, sweep along a helix; for threads, see Thread.
  • Paths that bend in space come from a 3D sketch.

Practise it: the compression spring and swept handle exercises.

Practise it: the compression spring, the helical gear and the thread of the bottle.

When it fails: sweep and loft errors covers Pierce relations, self-intersection and guide curves.

Step by step

  1. 1

    Sketch the path

    On the Front Plane, starting at the origin, draw a horizontal line of 50 mm, a tangent arc of R20 turning 90° upward, and a vertical line of 50 mm. Fully define it and exit the sketch.

    Sweep path sketch with a 50 mm line, an R20 tangent arc and a 50 mm line
    A path of two lines joined by a tangent arc.
  2. 2

    Start the sweep with a circular profile

    Features → Swept Boss/Base. Choose Circular Profile, select the path and type a diameter of 10 mm. No profile sketch is needed.

  3. 3

    Or use a sketched profile

    For other shapes, sketch the profile on a plane normal to the start of the path (select the path's end point and the plane, or select the edge near its end and click Sketch), and add a Pierce relation between the profile centre and the path.

  4. 4

    Confirm

    Leave Profile orientation at Follow Path and click the tick. You get a bent rod.

Common mistakes

  • The path does not cross the profile's plane. Add a Pierce relation from the profile to the path.
  • A path with sharp corners and a profile too large for the bend radius — the sweep self-intersects and fails. Use tangent arcs larger than the profile radius.
  • Self-intersecting profiles or paths are not allowed.
  • Using Sweep for a straight section — Extrude is simpler.

Lesson 14 of 18 in the features course.

Practice

Sweep a Ø10 circular profile along the path above (50 mm line, R20 90° tangent arc, 50 mm line). Check: volume 10,321.38 mm³ — the circle's area times the path length (131.42 mm).

Sources

Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.

Frequently asked questions

What do I need for a sweep in SOLIDWORKS?

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A closed profile and a path. The path can be open or closed and must cross the profile's plane. For round sections, Circular Profile needs only the path and a diameter.

What is the Pierce relation for?

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It ties a point of the profile sketch to where the path passes through the profile's plane, so the profile always sits on the path.

What is the difference between Follow Path and Keep Normal Constant?

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Follow Path keeps the profile at the same angle to the path as it bends. Keep Normal Constant keeps the profile parallel to its starting position.

Can I twist a sweep?

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Yes. Profile Twist can specify a twist value in degrees or revolutions along the path, without needing a helix.