Loft¶

In one sentence: Blend smoothly through a series of 2-D cross-section profiles to create a solid or shell whose shape transitions from one cross-section to the next.

Overview¶

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

Loft creates a solid or surface by connecting a sequence of closed (or open) profile wires. Unlike Ruled Surface (which connects only two rails with straight generators), Loft can connect any number of profiles and uses smooth (B-spline) blending.

Intuition¶

An aircraft fuselage transitions from a circular nose cross-section through various oval sections to a different tail cross-section. A Loft operation models exactly this: you provide the cross-sections at key stations and FreeCAD blends smoothly between them.

Unlike Sweep — which takes a constant cross-section and moves it along a path — Loft takes changing cross-sections and threads them together. You can combine both by providing cross-sections at different Z heights and letting Loft figure out the spine.

When to use it¶

Aerodynamic or ergonomic shapes that transition between cross-sections.
Bottle or vase profiles that change shape from base to neck to rim.
Blending a round tube into a rectangular duct.

When NOT to use it¶

Constant cross-section along a path — use Sweep.
Two rails only, straight lines — use Ruled Surface for a simpler, potentially more stable result.

Step-by-step walkthrough¶

Create the cross-section profiles. Each must be a closed wire or sketch lying in a plane roughly perpendicular to the loft direction.
Open the Loft dialog: Part → Loft.
In the dialog, add profiles in order (first to last) using the Add button.
Set options:
Ruled — straight (ruled) transitions between profiles (= Ruled Surface generalised to N sections).
Closed — connect the last profile back to the first.
Create Solid — closed ends produce a solid; open ends produce a shell.
Click OK.

Parameters¶

Parameter	Type	Default	Description
Profiles	List of wires	—	Cross-section profiles in order
Ruled	Bool	No	Straight (ruled) vs smooth (B-spline) blending
Closed	Bool	No	Connect last profile back to first
Create Solid	Bool	Yes	Solid vs open shell

Deep dive: Ruled vs smooth blending¶

Ruled mode¶

Intuition: Straight-line generators connect corresponding points on successive profiles. Computationally cheaper and guaranteed to stay between the profiles. Produces faceted (polyhedral) surfaces when profiles differ significantly.

Use ruled mode when: - The shape must be developable (unfoldable) for sheet metal. - You want maximum control with no unexpected curvature. - Speed matters and the approximation is acceptable.

Smooth mode (default)¶

Intuition: OCCT fits B-spline surfaces through the profiles, honouring tangency at each end profile if the profile has an adjacent face to be tangent to. Produces continuously curved surfaces.

Use smooth mode (default) when: - The lofted shape must look organic, aerodynamic, or fully smooth. - You plan to use the result in CFD, rendering, or Class-A surface work.

Common mistakes and pitfalls¶

Profile order determines shape

Profiles are blended in the order you add them. Adding them out of order produces a self-intersecting loft. Always add profiles from one end to the other.

Profiles must have compatible topology

Blending a circle (1 edge) with a square (4 edges) requires OCCT to map one circular arc to each of the four square sides. The mapping may produce unexpected transitions. Use a profile with the same number of edges as the target, or use a smooth round-rectangle ("squircle") intermediate profile.

Closed loft requires at least 3 profiles

Closing a loft with only 2 profiles produces a degenerate result. Add a third intermediate profile.

Python API¶

import FreeCAD as App
import Part

doc = App.newDocument()

# Three profiles at different Z heights
circle_bottom = Part.Wire([Part.makeCircle(10, App.Vector(0, 0, 0), App.Vector(0, 0, 1))])
circle_mid    = Part.Wire([Part.makeCircle(15, App.Vector(0, 0, 15), App.Vector(0, 0, 1))])
circle_top    = Part.Wire([Part.makeCircle(5,  App.Vector(0, 0, 30), App.Vector(0, 0, 1))])

loft = Part.makeLoft([circle_bottom, circle_mid, circle_top],
                     solid=True, ruled=False, closed=False)

feat = doc.addObject("Part::Feature", "LoftedSolid")
feat.Shape = loft
doc.recompute()
print(f"Volume: {feat.Shape.Volume:.2f} mm³")

Parametric Loft object¶

import FreeCAD as App

doc = App.newDocument()
# Create sketch profiles in the document...
# sketch1 = ... sketch2 = ... sketch3 = ...

loft_obj = doc.addObject("Part::Loft", "Loft")
loft_obj.Sections = [sketch1, sketch2, sketch3]
loft_obj.Solid    = True
loft_obj.Ruled    = False
loft_obj.Closed   = False
doc.recompute()