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Slice to Compound

In one sentence: Cut a Base shape using a Tool shape and keep all resulting fragments in a single compound object, leaving both originals intact.

Overview

Workbench: Part
Menu: Part → Split → Slice to Compound
Shortcut: none

Cuts a Base shape using a Tool shape and bundles all resulting fragments into a single compound Part::Feature. The operation is non-destructive — the original Base and Tool remain as separate objects in the model tree.

Intuition

Like Slice Apart, but the sliced pieces stay bundled together in one container. The original shapes are still there, and the compound holds the result.

Use Slice to Compound when you want to keep the fragments linked together for further operations — export, assembly, or FEA — without separating them into independent tree objects.

When to use it

  • Slicing geometry for export: you want one file containing all slices as a compound.
  • Slicing a solid along a datum plane to apply boundary conditions in FEA.
  • Analysing a cross-section: slice the part and inspect the resulting faces.
  • Non-destructive splitting where you may want to undo or adjust the cut.

When NOT to use it

  • Don't use it if you need independent objects after slicing — use Slice Apart to get separate tree entries per fragment.
  • Don't use it as a replacement for Boolean Cut — if you want to remove one piece and keep the other, use Boolean Cut instead.

Step-by-step

  1. Select the Base shape (the shape to cut).
  2. Ctrl+click the Tool shape (the cutting surface or solid).
  3. Choose Part → Split → Slice to Compound.
  4. A compound containing all fragments appears in the tree. The Base and Tool remain unchanged.
  5. Use Part → Explode Compound to separate fragments into individual objects later if needed.

Parameters

Parameter Description
Base The shape to cut (kept in tree; result compound is separate)
Tool The cutting shape (kept in tree; defines the cut boundary)

Common mistakes and pitfalls

Tool must intersect the Base

If the Tool does not cross the Base, no slice is performed and the compound contains only the unmodified Base.

Result is a compound — explode to access individual fragments

The output is a single compound object. To work with individual fragments separately, use Part → Explode Compound or Part → Convert → Explode Compound.

Faces at the cut boundary are shared

The cut boundary faces appear in both fragments of the compound. This is intentional for FEA conforming meshes but may be unexpected in other contexts.

Python API

import FreeCAD as App
import BOPTools.SplitFeatures as SF

doc = App.newDocument()

box = doc.addObject("Part::Box", "Box")
box.Length = 40; box.Width = 20; box.Height = 20

# Cutting plane as a thin slab
plane = doc.addObject("Part::Box", "CutPlane")
plane.Length = 50; plane.Width = 50; plane.Height = 0.001
plane.Placement = App.Placement(App.Vector(-5, -15, 10), App.Rotation())
doc.recompute()

sliced = SF.makeSlice(name="SlicedCompound")
sliced.Objects = [box, plane]
sliced.Proxy.execute(sliced)
doc.recompute()

print(f"Fragments in compound: {len(sliced.Shape.Solids)}")

See also