Ruled Surface¶

In one sentence: Create a surface by linearly blending between two parallel edges or wires — every point on the surface lies on a straight line connecting corresponding points on the two rails.

Overview¶

Workbench: Part · Menu: Part → Ruled Surface
Toolbar: Part Modeling · Shortcut: none

A ruled surface is a special case of a surface where every generating line is straight. Select two edges or wires (the "rails") and FreeCAD creates a surface by linearly interpolating between them.

Intuition¶

Imagine stretching a sheet of rubber between two parallel wires of different shapes — the rubber takes the form of a ruled surface. The surface is not curved in the mathematical sense (no curvature in one direction), but the two edges can be any shape.

Classic ruled surfaces: - Cylinder — two identical parallel circles. - Cone — a circle and a point (degenerate case). - Hyperbolic paraboloid (saddle) — two non-parallel straight lines. - Helicoid — a line sweeping around an axis (if the line is the generator).

In FreeCAD, Ruled Surface is useful for: - Connecting two different cross-sections with a smooth (but ruled) transition. - Creating mould split-line surfaces. - Approximating developable surfaces (sails, sheet metal).

When to use it¶

You need a transition surface between two rails and a straight-line cross-section is acceptable (no curvature).
Sheet metal design: ruled surfaces are developable and can be unrolled flat.

When NOT to use it¶

Smooth curved blend — use Loft which uses curve-smoothing algorithms.
Profile along a path — use Sweep.

Step-by-step walkthrough¶

Create two edges or wires (the rails). They should be oriented in the same direction for a predictable result.
Select the first edge/wire.
Ctrl+click the second edge/wire.
Part → Ruled Surface.
A surface (shell) appears connecting the two rails.

Parameters¶

The tool has no dialog parameters — it operates on the two pre-selected edges/wires directly. The orientation and direction of the resulting surface depend on the direction in which each wire is traversed.

Common mistakes and pitfalls¶

Twisted surface — wire orientations are opposite

If the two rails are traversed in opposite directions (one clockwise, one counter-clockwise), the ruled surface will twist. Reverse one wire's direction by selecting it and using Part → Reverse Shapes, or rearrange the wire edges.

Result is a shell (surface), not a solid

Ruled Surface produces an open shell. To get a solid, cap the open ends with Face from Wires and use Shape Builder or Convert to Solid.

Python API¶

import FreeCAD as App
import Part

doc = App.newDocument()

# Two rails: a circle at Z=0 and a circle at Z=20
circle1 = Part.makeCircle(10.0, App.Vector(0, 0, 0), App.Vector(0, 0, 1))
circle2 = Part.makeCircle(15.0, App.Vector(0, 0, 20), App.Vector(0, 0, 1))

wire1 = Part.Wire([circle1])
wire2 = Part.Wire([circle2])

# Create ruled surface
surface = Part.makeRuledSurface(wire1, wire2)
feat = doc.addObject("Part::Feature", "RuledSurface")
feat.Shape = surface
doc.recompute()