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New Part

In one sentence: Create a new empty Part Design body inside the active assembly so you can model the part in-context, with all surrounding assembly parts visible as references.

Overview

Workbench: Assembly
Menu: Assembly → Insert Component → New Part
Shortcut: none

New Part creates a new PartDesign::Body inside the assembly's Parts container and activates it for editing. You can then use Part Design tools normally while seeing all other assembly parts in the 3-D view — allowing geometry to be modelled with reference to adjacent parts.

Intuition

Sometimes a part's geometry is fundamentally defined by the assembly context around it. A custom bracket that must span between two specific faces, a spacer whose length equals the gap between two components, a cover plate whose outline exactly follows the assembly footprint — these parts can only be designed meaningfully when you can see the assembly.

New Part gives you exactly this: a blank Body inside the assembly, ready to model, with every other inserted part visible and available as external geometry references in your sketches.

When to use it

  • The part's geometry depends on the exact positions or shapes of neighbouring parts.
  • You are designing a custom interface component (bracket, adapter, spacer) that fits a specific assembly configuration.
  • You want to model a part and immediately see how it fits without switching documents.

When NOT to use it

  • Don't use this for standalone, reusable parts — model those independently in their own document and use Insert Component. Parts created with New Part live inside the assembly document and cannot easily be referenced by other assemblies.
  • Don't use this to import existing parts — use Insert Component for parts that already exist.

Step-by-step

  1. Make sure the assembly is active.
  2. Choose Assembly → Insert Component → New Part.
  3. A new Body appears in the model tree under Parts and is immediately activated (shown in bold).
  4. Switch to the Sketcher or Part Design workbench.
  5. Model the part normally — sketches, pads, pockets, etc.
  6. Other assembly parts are visible in the 3-D view. Use Sketcher → External Geometry to reference their edges and faces.
  7. When finished, double-click the Assembly object in the model tree to re-activate the assembly.
  8. Add joints to position the new part relative to the others.

Tip

If you need the new part to sit flush against another part's face, place your first sketch directly on that face — the sketch will be attached to the face and update if the face moves.

Parameters

The Body created by New Part has the same parameters as any Part Design Body — no special assembly-specific parameters.

Common mistakes and pitfalls

Forgetting to re-activate the assembly

After modelling the new part, the Body remains active. If you then try to Insert Component or add joints, they will be applied to the Body rather than the assembly. Always double-click the Assembly object to return to assembly context.

In-context parts are not reusable

The Body created by New Part lives inside the assembly document. To use it in another assembly, you must save it as a separate file. Consider whether the part should be standalone before choosing this approach.

External geometry references can break

If you reference a face of another assembly part via External Geometry and then change that part significantly (removing or reordering features), the reference may break. Check External Geometry links when updating referenced parts.

Python API

import FreeCAD as App

doc = App.newDocument("Assembly")

# Create assembly
asm = doc.addObject("Assembly::AssemblyObject", "Assembly")
doc.recompute()

# Create a new body inside the assembly
body = doc.addObject("PartDesign::Body", "NewPart")
asm.getObject("Parts").addObject(body)
doc.recompute()

# The body is now inside the assembly and ready for Part Design features

See also