Additive Loft¶

In one sentence: Blend a solid smoothly through two or more cross-section sketches to create a shape that transitions from one profile to the next.

Overview¶

Workbench: Part Design · Menu: Part Design → Additive Features → Additive Loft
Toolbar: Part Design Modeling Features · Shortcut: none

Additive Loft takes a profile sketch and one or more section sketches and constructs a solid that smoothly interpolates between them in order. The result is fused into the active Body, adding material. Unlike Additive Pipe, which requires a spine to define the path, Additive Loft connects the sections directly, inferring the transition shape between them. Use it whenever you need a solid that changes cross-sectional shape from one plane to another.

Intuition¶

Imagine a soft lump of clay connecting two wire frames: a circle at the bottom and a square at the top. The clay bulges out to fill both shapes at each end and creates a smooth transition in between. That transition is the loft.

The key insight is that Additive Loft does not need a path sketch — it finds its own route between the sections by interpolating through space. The order in which you add the sections determines the sequence of the transition; the loft always travels from the profile to the first section, then to the second, and so on.

A practical consequence: the spatial positioning of each section sketch matters enormously. Each section must be placed on a different plane (datum plane or face) so the loft has somewhere to go. Sections on the same plane, or very close together, produce extremely thin geometry that often fails.

When to use it¶

You need a solid that transitions between two different cross-sections — for example, a nozzle that is circular at the inlet and rectangular at the outlet.
You are modelling an ergonomic shape like a handle or grip that is wider at one end than the other.
You want to blend through several intermediate cross-sections with full control over the shape at each station.
The profile and sections are all closed wires (the loft produces a closed solid rather than an open shell).
You need to close a shape back to its starting profile — use the Closed option to create a torus-like body that loops from the last section back to the first.

When NOT to use it¶

The cross-section is constant along the path — use Pad for straight paths or Additive Pipe for curved paths; they are simpler and more robust.
The shape follows a specific curved spine — use Additive Pipe, which gives you explicit control over the path the profile travels.
The shape revolves around an axis — use Revolution, which is simpler and more predictable for axisymmetric solids.
You want to remove material — use Subtractive Loft, which has identical parameters but cuts instead of adds.

Step-by-step walkthrough¶

Prerequisites: An active Body with at least two fully-constrained sketches placed on different planes. The profile is the starting cross-section; the sections are the subsequent cross-sections in order.

Create the profile sketch. Draw and fully constrain the starting cross-section. This sketch will be the "first" shape in the loft sequence. Close the Sketcher task panel.
Create section sketches. For each additional cross-section, add a datum plane at the desired position along the loft, then create and constrain a sketch on that plane. Each section must have the same number of closed wires as the profile (or exactly one point as the final section to close to a tip). Close each Sketcher task panel after completing it.
Activate Part Design → Additive Features → Additive Loft. The task panel opens with two checkboxes (Ruled surface, Closed), a Profile group, and Add Section / Remove Section buttons.
Set the Profile. In the Profile group, click Object and then click the starting profile sketch in the model tree or viewport. The sketch name appears in the text field.
Add sections. Click Add Section, then click the first section sketch. Click Add Section again for each additional section, selecting them in the order you want the loft to travel through them. The section names appear in the list widget.
Reorder sections if needed. The list widget supports drag-and-drop reordering. The loft always travels from the profile through the list in top-to-bottom order.
Enable Ruled surface or Closed if required (see Parameters).
Click OK. FreeCAD blends through all the sections and fuses the result into the Body.

Tip

You can remove a section from the loft by selecting it in the list and clicking Remove Section. The profile itself cannot be removed via the sections list — edit the Profile property directly if you need to change the starting sketch.

Parameters¶

Parameter	Type	Default	Description
Ruled surface	Checkbox	Off	When on, each span between adjacent sections is a ruled surface (straight lines connecting corresponding points on adjacent profiles). Produces a faceted, prismatic appearance instead of a smooth blend.
Closed	Checkbox	Off	When on, the loft adds a final span connecting the last section back to the profile, forming a closed loop. Requires at least three sections (profile plus two more); automatically disabled with fewer sections.
Profile	Object link	—	The first cross-section sketch. Sets the starting shape of the loft.
Add Section / Remove Section	Buttons	—	Toggle selection mode to add or remove section sketches from the ordered list.
Sections list	Ordered list	—	The section sketches in loft order. Drag and drop to reorder. All sections must have the same number of closed wires as the profile; only the last section may be a single point (to taper to a tip).

Advanced usage¶

Tapering to a point¶

The last section in the list may be a single vertex (a point sketch) rather than a closed wire. This causes the loft to taper to a sharp tip at that end, producing cone-like or pyramid-like shapes. The profile and all intermediate sections must still be closed wires.

Closed lofts¶

When Closed is enabled the loft adds a span from the last section back to the profile, creating a continuous closed solid. This is useful for torus-like shapes or solid blobs that must loop around. At least three profiles (profile + two sections) are required; with only two sections FreeCAD silently ignores the flag.

Matching wire count¶

Each section must have exactly the same number of closed wires as the profile. A single-loop circle and a single-loop square can loft together (both have one wire). A circle and a figure-eight (two loops) cannot — FreeCAD will report a shape error. If you need to loft between profiles with different topology, break the operation into separate Additive Loft features and join them.

Common mistakes and pitfalls¶

At least one section is needed

Cause: Clicking OK without adding any sections. The profile alone is not enough to define a loft — there is nothing to loft to.
Fix: Add at least one section sketch using the Add Section button.

Sections have different wire counts

Cause: The profile has (for example) two closed wires (a ring with an inner and outer boundary) but a section has only one. The loft engine cannot match them.
Fix: Ensure every section sketch has the same number of closed loops as the profile, or adjust the profile.

Failed to create shell / Resulting shape is not a solid

Cause: Two sections are on the same plane or very close together, the sections cross each other in 3-D space, or a section is not closed.
Fix: Confirm that each section is on a distinctly different plane. Check that all sections are fully closed. Check that the section outlines do not visually overlap when viewed from the side.

Section sketches placed in the wrong order

Cause: The loft travels through sections in list order. If sections are listed out of spatial order the solid twists or self-intersects.
Fix: Drag the entries in the sections list to match the physical order from the profile outward.

Python API¶

Minimal example¶

import FreeCAD as App
import Part
import Sketcher

doc = App.newDocument()

# Create the body
body = doc.addObject("PartDesign::Body", "Body")

# Profile sketch: circle of radius 10 mm on the XY plane (Z=0)
profile = doc.addObject("Sketcher::SketchObject", "Profile")
body.addObject(profile)
profile.addGeometry(Part.Circle(App.Vector(0, 0, 0), App.Vector(0, 0, 1), 10), False)
profile.addConstraint(Sketcher.Constraint("Coincident", 0, 3, -1, 1))
doc.recompute()

# Datum plane at Z=40
plane = doc.addObject("PartDesign::Plane", "DatumPlane")
body.addObject(plane)
plane.MapMode = "FlatFace"
plane.AttachmentSupport = (doc.XY_Plane, [""])
plane.MapPathParameter = 0.0
plane.AttachmentOffset.Base.z = 40.0
doc.recompute()

# Section sketch: square 15×15 mm on the datum plane at Z=40
section = doc.addObject("Sketcher::SketchObject", "Section")
body.addObject(section)
section.MapMode = "FlatFace"
section.AttachmentSupport = (plane, [""])
doc.recompute()
# (add geometry + constraints for a 15x15 square centred at origin)  # TODO: verify

# Create the Additive Loft
loft = doc.addObject("PartDesign::AdditiveLoft", "AdditiveLoft")
body.addObject(loft)
loft.Profile = profile
loft.Sections = [(section, [])]
loft.Ruled = False
loft.Closed = False
doc.recompute()

print(f"Volume: {loft.Shape.Volume:.4f} mm³")

Key properties¶

Property	Type	Default	Description
`Profile`	`App::PropertyLinkSub`	—	The first (starting) cross-section sketch. Inherited from `ProfileBased`.
`Sections`	`App::PropertyLinkSubList`	`[]`	The ordered list of section sketches (everything after the profile).
`Ruled`	`App::PropertyBool`	`False`	Generate ruled (straight-line) spans between sections instead of smooth curves.
`Closed`	`App::PropertyBool`	`False`	Close the loft by adding a final span from the last section back to the profile. Silently ignored if fewer than three profiles total are provided.