Body, Origin, and the Feature Tree¶

In one sentence: The Part Design Body is the container that holds all features of a single solid; the Origin provides its built-in reference planes and axes; and the Tip marks where in the feature sequence FreeCAD stops evaluating — making it the "current shape" of the Body.

The Body¶

A Body (PartDesign::Body) is the fundamental container for one solid part in the Part Design workflow. Every Pad, Pocket, Fillet, and other feature must live inside a Body. You cannot have free-floating Part Design features outside a Body.

What a Body contains¶

When you create a new Body, FreeCAD automatically places the following objects inside it:

Object	Type	Purpose
Origin	`App::Origin`	Built-in reference geometry: three planes (XY, XZ, YZ) and three axes (X, Y, Z)
(your features)	Various `PartDesign::*`	Pad, Pocket, Fillet, etc., added by you

Each feature is ordered in the Body's feature tree. The Body evaluates the features from top to bottom, chaining the shape of each feature into the next. Reordering features (with Move Feature in Tree) changes the final shape.

One Body = one solid¶

A Body represents one contiguous solid body — one connected piece of material. A FreeCAD document can contain multiple Bodies (for multi-part assemblies), but each Body is independent. To combine two Bodies into a single solid, use Boolean.

Active Body¶

Only one Body is active at a time. New features are automatically placed into the active Body. To activate a Body, double-click it in the model tree. The active Body is highlighted in the tree and its features appear in the 3-D view.

The Origin¶

Every Body automatically contains an Origin object. The Origin provides built-in reference geometry anchored to the Body's local coordinate system:

Origin contents¶

Reference	Type	Axis / Normal
XY Plane	Reference plane	Normal along Z
XZ Plane	Reference plane	Normal along Y
YZ Plane	Reference plane	Normal along X
X Axis	Reference axis	Points in +X
Y Axis	Reference axis	Points in +Y
Z Axis	Reference axis	Points in +Z

All six are always available. Show or hide the Origin in the 3-D view by pressing Space while the Origin is selected, or toggle its visibility from the Model tree.

Using the Origin for sketches¶

The most common use of the Origin is as the plane for the very first sketch. Before any external geometry exists, the Body's Origin planes are the only reference available:

Select XY_Plane (or XZ_Plane or YZ_Plane) inside the Body's Origin.
Create a new sketch — it is mapped to that plane.
Draw and constrain the profile.
Apply a Pad or Revolution.

The Origin is always at the Body's local (0, 0, 0). Moving the Body's Placement moves the entire solid — including the Origin — while keeping all internal feature geometry intact.

Origin vs Datum Planes¶

	Origin plane	Datum Plane
Created automatically	Yes	No — you add them
Count	Three fixed (XY, XZ, YZ)	As many as you need
Position	Fixed at Body origin	Anywhere you attach them
Editable	No	Yes
Use	First sketch reference; axis references	Additional planes for later features

Origin planes are sufficient for simple parts. For complex parts requiring angled sketch planes or planes offset from the body centre, create Datum Planes.

The Feature Tree¶

The feature tree is the ordered list of features inside the Body. It is the core of Part Design's parametric history model.

How the feature tree works¶

Body
├── Origin
│     ├── XY_Plane
│     ├── XZ_Plane
│     ├── YZ_Plane
│     ├── X_Axis
│     ├── Y_Axis
│     └── Z_Axis
├── Sketch           ← profile for the first Pad
├── Pad              ← first additive feature
├── Sketch001        ← profile for the Pocket
├── Pocket           ← subtractive feature
├── Fillet           ← dress-up
└── LinearPattern    ← transformation   (← Tip is here)

FreeCAD evaluates the tree top to bottom, computing a cumulative shape at each step. The result at the bottom of the tree is the Body's current shape — visible in the 3-D view.

Why order matters¶

Because each feature adds to or modifies the shape produced by all preceding features:

A Fillet applied to an edge that is later removed by a Pocket will fail — the edge it referenced no longer exists.
A LinearPattern below a Pocket repeats only the patterned feature(s), not the whole body from before the Pocket (unless Transform Body mode is used).
Reordering features can fix dependency errors, allow new features to reference edges that didn't exist earlier, or change the final shape.

The Tip¶

The Tip is a marker in the Body that indicates which feature is currently the "end" of the evaluation sequence. FreeCAD computes the solid only up to and including the Tip; features below the Tip in the tree are not included in the body's displayed shape.

Why Tip matters¶

Adding features: When you add a new feature, it is inserted just below the current Tip. Moving the Tip lets you insert features at any point in the history — not just at the end.
Inspecting history: Moving the Tip backwards lets you see what the part looked like at any earlier stage of the design.
Recovering from errors: If a later feature fails, moving the Tip to the last valid feature lets you work on the part before re-fixing the failing feature.

Moving the Tip¶

Use Move Tip (right-click → Set Tip) on any feature in the Body. The Tip jumps to that feature, and all features after it are temporarily excluded from the shape evaluation.

The Tip is shown in the model tree with a small green marker on the feature's icon.

Tip and new features¶

When you add a new Pad, Pocket, or other feature, FreeCAD places it immediately after the current Tip and advances the Tip to the new feature. This is the expected behaviour: new features build on top of the current shape.

If you need to insert a feature in the middle of the history: 1. Move the Tip to the feature just above where you want to insert. 2. Add the new feature (it goes after the current Tip). 3. Move the Tip back to the end (or to the final feature).

Practical tips¶

Always start with a sketch on the XY plane

For most parts, the first sketch belongs on the Body's XY plane (Z-up convention). This ensures that View → Standard Views → Top shows the part plan view, and Front shows the elevation — matching engineering drawing conventions.

One part = one Body

Resist the temptation to put multiple independent parts in the same Body using Boolean. Use one Body per physical component and combine them in the Assembly workbench or with Part Design Boolean at the top level.

Multi-Body booleans require explicit Boolean feature

Two separate Bodies do not automatically interact. Even if they visually overlap in the 3-D view, each Body's solid is independent. Use Boolean to fuse, cut, or intersect two Bodies into a single solid.

Features after the Tip are invisible but not deleted

Moving the Tip hides features below it from the shape computation. Those features still exist and their parameters are preserved. Moving the Tip back restores them immediately.