Sweep¶

In one sentence: Move a cross-section profile along a spine path to create a solid or surface — the profile's shape stays constant while its position and orientation follow the path.

Overview¶

Workbench: Part · Menu: Part → Sweep
Toolbar: Part Modeling · Shortcut: none

Sweep creates a solid or shell by moving one or more closed profiles along a 3-D spine path. The profiles are placed perpendicular to the spine at each point, creating the swept volume.

Intuition¶

Think of squeezing toothpaste: the nozzle (profile) is constant; the tube of toothpaste (spine) determines where the material goes. The bead of toothpaste is the Sweep result.

Common swept shapes: - Pipes and tubing — circle profile along a 3-D spline spine. - Springs — circle profile along a Helix spine. - Channels and extrusions — custom cross-section along a straight or curved path. - Wiring looms — oval profile following cable routing paths.

When to use it¶

Any profile you want to route through 3-D space along a defined path.
Springs: circle profile along a Part Helix.
Pipe bends: circle profile along a 3-D arc or spline.

When NOT to use it¶

Changing cross-section — use Loft instead.
Linear extrusion — use Extrude (simpler and more stable).

Step-by-step walkthrough¶

Create the spine path — a wire, edge, or sketch that defines the path. It can be 3-D (a spline, helix, arc sequence).
Create the profile — a closed wire or sketch perpendicular to the start of the spine.
Open Part → Sweep.
In the dialog:
Add the profile (click the profile, then Add).
Set the spine (click the spine object, then the Spine button).
Configure Frenet mode and Transition options.
Click OK.

Parameters¶

Parameter	Type	Default	Description
Sections	List of wires	—	Cross-section profiles to sweep
Spine Path	Wire	—	The path to sweep along
Create Solid	Bool	Yes	Solid vs open shell
Frenet	Bool	No	Use Frenet frame to orient the profile along the path
Transition	Enum	Right Corner	How profile handles sharp corners in the spine: Right Corner / Round Corner / Transformed

Deep dive: Frenet mode and Transition options¶

Frenet mode¶

Intuition: Without Frenet, the profile orientation is determined by the minimum rotation frame, which can produce twisting for certain paths. With Frenet on, the profile is oriented by the path's tangent and normal vectors (the Frenet–Serret frame), which avoids twist for planar paths but may introduce twist for highly 3-D paths.

Use Frenet for: - Paths that lie in a single plane (2-D arcs, circles). - Situations where the "up" direction of the profile should follow the path curvature naturally.

Transition: Right Corner¶

Intuition: At sharp corners in the spine, the profile is simply moved/rotated to the new direction — a miter joint. Produces sharp corners in the swept solid.

Transition: Round Corner¶

Intuition: At sharp corners, FreeCAD inserts an arc to smooth the transition, producing a rounded corner in the swept solid.

Transition: Transformed¶

Intuition: The profile is scaled or sheared at corners to fit the transition. Less commonly needed.

Common mistakes and pitfalls¶

Profile must be at the start of the spine

Place the profile's plane at the starting point of the spine. If the profile is far from the spine start, the sweep result will be offset or misaligned.

Spine must be a connected wire, not separate edges

If the spine consists of several disconnected edges, assemble them into a wire using Shape Builder first.

Self-intersecting sweep when spine curves too sharply

If the spine has a curve with a radius smaller than the profile's extent, the swept solid self-intersects. Increase the spine radius or reduce the profile size.

Python API¶

import FreeCAD as App
import Part

doc = App.newDocument()

# Profile: small circle at the origin (XY plane)
circle_edge = Part.makeCircle(3.0, App.Vector(0, 0, 0), App.Vector(0, 0, 1))
profile = Part.Wire([circle_edge])

# Spine: a helix
helix = doc.addObject("Part::Helix", "Helix")
helix.Pitch  = 8.0    # mm
helix.Height = 40.0   # mm
helix.Radius = 12.0   # mm
doc.recompute()

# Sweep via Part object
sweep = doc.addObject("Part::Sweep", "Spring")
sweep.Sections  = [doc.addObject("Part::Feature", "Profile")]
doc.getObject("Profile").Shape = profile

sweep.Spine     = (helix, ["Edge1"])   # spine from helix
sweep.Solid     = True
sweep.Frenet    = True
doc.recompute()

Practical note: For a spring sweep, create the helix with the Primitives dialog, create a small circle Sketcher sketch on the XY plane, then run Sweep interactively — it is easier than the scripted approach.