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Boolean Fuse (Union)

In one sentence: Merge two shapes into a single solid by taking their union — the resulting solid contains all material from both inputs.

Overview

Workbench: Part · Menu: Part → Boolean → Fuse
Toolbar: Part Boolean · Shortcut: none

Boolean Fuse (also called "union" in set theory) produces a solid that encompasses all the volume of both operands. Internal coincident faces where the two shapes were touching are removed, leaving a clean watertight solid.

Intuition

Think of gluing two metal bars together: the result is one continuous piece with no internal boundary. The Fuse operation is mathematically equivalent — it takes the union of the two volumes and produces a single manifold solid.

Common uses:

  • Adding a boss to a base plate (fuse a cylinder onto a box).
  • Building an L-bracket by fusing two rectangular blocks.
  • Merging several bodies that came in as separate STEP parts.

When to use it

  • Combining two touching or overlapping solids into one.
  • Building complex geometry from simple primitives (constructive solid geometry).
  • Unifying separate imported STEP bodies that should be a single piece.

When NOT to use it

  • Shapes that do not touch or overlap — Fuse succeeds but produces a compound with two separate shells, not one solid. Use Make Compound to group non-touching shapes.
  • Inside a Part Design Body — use Body Boolean (Fuse) or simply place additive features next to each other.
  • More than two shapes — apply successive Fuses, or use Boolean Fragments.

Step-by-step walkthrough

  1. Select the first shape (Base).
  2. Ctrl+click the second shape (Tool).
  3. Part → Boolean → Fuse.
  4. A Part::Fuse object appears.
  5. Optionally run Refine Shape to merge redundant co-planar faces.

Parameters

Parameter Description
Base First operand
Tool Second operand
Refine Remove redundant edges from the result (toggle in Data panel)

Common mistakes and pitfalls

Non-touching shapes produce a compound, not a solid

If Base and Tool do not share any volume, Fuse returns a compound of two separate solids. Move one shape to overlap the other before fusing.

Redundant faces after fusing co-planar shapes

When you fuse two boxes that share a flat face, the shared face becomes an internal seam in the result. Use Refine Shape to remove it. This is important before running Fillet or Chamfer.

Python API

import FreeCAD as App

doc = App.newDocument()

# Two overlapping boxes: form an L-shape
box1 = doc.addObject("Part::Box", "Horizontal")
box1.Length = 60; box1.Width = 10; box1.Height = 10

box2 = doc.addObject("Part::Box", "Vertical")
box2.Length = 10; box2.Width = 10; box2.Height = 50
# They share the first 10×10×10 corner
doc.recompute()

fuse = doc.addObject("Part::Fuse", "LBracket")
fuse.Base = box1
fuse.Tool = box2
doc.recompute()

# Refine to remove the internal seam
import Part
refined = fuse.Shape.removeSplitter()
feat = doc.addObject("Part::Feature", "LBracketRefined")
feat.Shape = refined
doc.recompute()

print(f"Volume: {feat.Shape.Volume:.2f} mm³")

See also