Body¶

In one sentence: Create an independent solid container that holds all Part Design features and owns the Origin geometry they attach to.

Overview¶

Workbench: Part Design · Menu: Part Design → New Body
Toolbar: Part Design Helper Features · Shortcut: none

A Body is the root container for a single solid in the Part Design workflow. Every sketch, datum, and shaping feature (Pad, Pocket, Fillet, …) must live inside a Body. When you create a Body, FreeCAD immediately activates it so that subsequent operations are placed inside it, and automatically creates an Origin — three reference planes (XY, XZ, YZ), three reference axes (X, Y, Z), and an origin point — that everything else can attach to.

Intuition¶

Think of a Body as an individual machined part sitting on a workbench. The workbench itself has built-in reference lines and a flat top surface (the Origin). Everything you make — sketches, extrusions, holes, fillets — goes on or into that one part. When you are done, the part is a single solid, and that is what you hand to someone.

The "feature tree" inside the Body records every operation you applied, in order, like a machinist's job sheet. You can rewind to any step (by moving the Tip), change a dimension, and FreeCAD re-applies every subsequent operation automatically. The Body is what makes that history possible: it owns the sequence and produces the final shape as the cumulative result.

A document can contain multiple Bodies — one for each independent solid in the assembly. Bodies do not automatically interact with each other; joining them requires a Boolean operation or a Part container.

When to use it¶

You are starting a new Part Design model and need a container for the first sketch and feature.
You are designing a document that contains several independent solid components (e.g. a bolt and a nut in the same file) — create one Body per component.
You want to import an existing Part solid (a box, a sphere, a body from another workbench) and continue adding Part Design features on top of it — select the solid before creating the Body to use it as a Base Feature.
You need the clean Origin reference geometry (datum planes and axes) that a Body provides to anchor your first sketch.

When NOT to use it¶

You already have an active Body and just want to add another feature to it — do not create a new Body; instead use New Sketch or any additive/subtractive feature directly. Creating a second Body produces a completely independent solid.
You want to combine two existing Bodies into one solid — use Boolean to merge, cut, or intersect them; a Body alone does not perform that combination.
You are working in the Part workbench — that workbench does not use Bodies. Bodies are exclusive to the Part Design workflow.

Step-by-step walkthrough¶

Prerequisites: An open FreeCAD document. No other precondition is required; a Body can be the very first object in a new document.

Optionally select a base solid. If you want the Body to start from an existing Part solid (e.g. a box from the Part workbench), click it in the model tree before activating the command. The solid becomes the Body's Base Feature — the first solid in its feature chain.

Base Feature restrictions

The selected solid must not already belong to another Body and must not itself be a Body. Selecting multiple solids will prevent the command from running — only one base feature is permitted. If the selected feature has multiple solids or shells, a warning dialog appears.
Activate the command via one of:
- Menu: Part Design → New Body
- Toolbar: click the Body button in the Part Design Helper Features toolbar
Observe what appears in the model tree. FreeCAD:
- Creates a PartDesign::Body object labelled Body (or Body001, etc. if names are already taken).
- Creates an Origin object inside it containing the XY, XZ, and YZ reference planes, the X, Y, and Z axes, and the origin point.
- If a base feature was selected, adds a BaseFeature proxy inside the Body that wraps the selected solid.
- Makes the new Body the active body for the current view.
Begin building the model. With the Body active, create a sketch (Part Design → New Sketch or the toolbar button). The Sketcher opens and you select one of the Body's Origin planes as the attachment plane. Close the sketch, then apply an additive feature such as Pad.
Keep adding features. Each subsequent sketch and feature is automatically placed inside the active Body and appended to its feature tree. The Tip (the last solid feature) updates each time.

Tip

If you accidentally create a Body when you meant to add to an existing one, undo the action (Ctrl+Z), then double-click the intended Body in the tree to re-activate it before continuing.

Parameters¶

A Body has no task-panel dialog. Its parameters appear in the Property editor (bottom-left panel in the default layout) when the Body is selected.

Parameter	Type	Default	Description
`Label`	String	`Body`	Human-readable name shown in the model tree. Editable; auto-incremented to avoid duplicates.
`Tip`	Link	`None`	The feature that provides the Body's current shape. Defaults to the last solid feature added. Move the tip to "rewind" the history.
`BaseFeature`	Link	`None`	An external Part solid that acts as the starting shape for the first feature inside the Body. Set at creation time if a solid was selected; not normally changed later.
`Group`	LinkList	`[]`	The ordered list of all objects inside the Body (sketches, datums, solid features, binders). Managed automatically; edit with caution.
`AllowCompound`	Bool	`True`	When `True`, features that produce multiple disconnected solids are allowed (the Body's shape becomes a compound). When `False`, the first feature that would create multiple solids causes a recompute error. The default at creation time follows the preference `BaseApp/Preferences/Mod/PartDesign/AllowCompoundDefault`.
`Placement`	Placement	identity	Position and orientation of the entire Body in world space. Rarely needed — moving individual features is preferred.
`ShapeMaterial`	Material	—	Appearance material applied to the Body's shape and propagated to all contained features.

Advanced usage¶

Multiple Bodies in one document¶

Each Body produces one independent solid. A document can contain as many Bodies as needed. To work on a specific Body, double-click it in the model tree to make it active; its label turns bold. Features created while a Body is active are added to that Body.

To combine two Body solids (e.g. subtract one from the other), use Boolean. To reference geometry from one Body inside another, use Sub-Shape Binder.

Using an existing solid as a Base Feature¶

Any Part::Feature-derived solid (a box from the Part workbench, an imported STEP shape, a FreeCAD Mesh converted to a solid) can serve as the starting point for a Body. Select the solid before creating the Body; FreeCAD wraps it in an internal FeatureBase proxy and presents it as the first step in the feature chain. All subsequent Part Design features add to or subtract from that base.

If the selected object is a Sketcher sketch rather than a solid, FreeCAD adds the sketch to the Body's group and prompts you to choose which Origin plane to attach it to.

Moving the Tip to inspect intermediate states¶

Right-click any feature in the Body's model tree and choose Set Tip (or use Part Design → Set Tip) to rewind the history to that feature. The viewport shows the shape as it was at that point, and new features are inserted after the Tip rather than at the end of the tree. Move the Tip back to the last feature to resume normal editing.

AllowCompound and multi-solid models¶

With AllowCompound = True (the default), operations that accidentally disconnect the solid — such as a pattern that places copies apart from the main body — produce a compound result without error. Set AllowCompound = False to enforce single-solid discipline; FreeCAD will then report an error on the feature that first creates multiple disconnected solids, making the problem visible immediately.

Common mistakes and pitfalls¶

Feature created outside the active Body

Cause: No Body was active when a sketch or feature was created, or the wrong Body was active. The feature appears as a top-level document object rather than inside the intended Body.
Fix: Use Part Design → Move Object To… to reassign the feature to the correct Body, or undo and re-activate the intended Body before recreating the feature.

Two Bodies instead of one solid

Cause: A second Body was created instead of continuing to add features to the first one. The model tree shows two separate Body objects.
Fix: Either delete the second Body and re-activate the first, or — if both Bodies contain useful geometry — combine them with Boolean.

Tip not at the end of the tree

Cause: The Tip was moved to an intermediate feature (e.g. to inspect a step) and not moved back. Subsequent features are inserted after the current Tip, not at the end, which can produce unexpected geometry.
Fix: Right-click the last feature in the tree and choose Set Tip (or Part Design → Set Tip) to restore normal behaviour.

Base feature already belongs to another Body

Cause: The solid selected before running New Body is already inside a Body (or is itself a Body). FreeCAD refuses this to prevent circular dependencies.
Fix: Choose a solid that is not yet inside any Body, or use Sub-Shape Binder to reference the existing Body's shape from the new Body.

Python API¶

Minimal example¶

import FreeCAD as App

doc = App.newDocument()

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

print(body.Label)         # "Body"
print(body.Tip)           # None — no features yet
print(body.AllowCompound) # True

Creating a Body with a base feature¶

import FreeCAD as App
import Part

doc = App.newDocument()

# Create a Part box to use as the base solid
box = doc.addObject("Part::Box", "Box")
box.Length = 50
box.Width  = 30
box.Height = 20
doc.recompute()

# Create the Body and attach the box as its Base Feature
body = doc.addObject("PartDesign::Body", "Body")
body.BaseFeature = box
doc.recompute()

print(body.Tip.Label)  # "BaseFeature" proxy created automatically

Key methods¶

# Add an already-created feature (sketch, datum, solid feature) to the Body.
# The feature is inserted at the current insert point (just after the Tip).
body.addObject(feature)

# Insert a feature at a specific position relative to an existing feature.
# target: the reference feature (must already be in the Body); None → end/start
# after: if True, insert after target; if False (default), insert before target
body.insertObject(feature, target, after=False)

# Remove a feature from the Body without deleting it from the document.
body.removeObject(feature)

# Return the currently visible PartDesign feature inside the Body (Python property).
visible = body.VisibleFeature  # TODO: verify attribute name; source: BodyPyImp.cpp::getVisibleFeature

Body properties reference¶

Property	Type	Description
`Label`	`App::PropertyString`	Human-readable name of the Body.
`Tip`	`App::PropertyLink`	Link to the feature that determines the Body's current output shape.
`BaseFeature`	`App::PropertyLink`	Optional external solid that the first PartDesign feature builds upon.
`Group`	`App::PropertyLinkList`	Ordered list of all objects inside the Body.
`AllowCompound`	`App::PropertyBool`	`True` allows multiple disconnected solids in the result. Default: `True`.
`Placement`	`App::PropertyPlacement`	Position and orientation of the Body in world space.
`ShapeMaterial`	`App::PropertyMaterial`	Appearance material propagated to all contained features.
`Shape`	`Part::PropertyPartShape`	The output shape — a copy of the Tip feature's shape. Read-only; recomputed automatically.