Draft¶

In one sentence: Taper selected faces of a solid by rotating them about a neutral plane, producing angled walls that allow a moulded part to release from its mould.

Overview¶

Workbench: Part Design · Menu: Part Design → Dress-Up Features → Draft
Toolbar: Part Design Dress-Up Features · Shortcut: none

Draft takes one or more faces on the current solid and tilts each of them by a specified angle relative to a neutral plane — the plane that stays fixed while the face rotates. The result is a tapered wall rather than a vertical one. This is essential for plastic injection moulding and die casting, where vertical walls would lock the part inside the mould; adding a small draft angle (typically 1°–5°) allows the part to release cleanly.

Intuition¶

Picture a sand castle bucket: the walls are not vertical — they slope slightly outward from bottom to top. When you turn the bucket upside down to release the castle, the angle allows the sand to slide out. Without the slope the sand would grip the walls and the castle would break.

The neutral plane is the cross-section of the solid that does not move during drafting — it is the "hinge" about which the face rotates. Everything on one side of the neutral plane moves inward; everything on the other side moves outward (or vice versa, depending on pull direction and angle sign).

The pull direction is the axis along which the mould is pulled — the direction of opening. By default, FreeCAD derives the pull direction automatically from the neutral plane's normal. You can override it with a datum line or a straight edge if the mould opens at an angle to the part's main axes.

When to use it¶

You are finalising a plastic or die-cast part and every vertical wall needs a draft angle for mould release.
You want the walls of a boss, rib, or housing to be slightly tapered rather than perfectly vertical.
You need to apply a consistent taper angle (e.g. 1.5°) across multiple faces that share the same pull direction and neutral plane.
You need to reverse the draft direction on one side of a parting line.

When NOT to use it¶

You want a flat angled cut along an edge — use Chamfer instead; Draft operates on full faces, not edges.
You need to taper a sketch profile before padding it — taper the sketch geometry or use an angled attachment plane instead.
The part is being machined rather than moulded — draft angles are rarely needed for machined parts; use Chamfer or Fillet for edge treatment.
You are working on a Part workbench solid outside a Body — Draft is a PartDesign dress-up feature and requires an active Body.

Step-by-step walkthrough¶

Prerequisite: An active Body with at least one solid feature containing planar or curved faces that can be drafted.

Select the faces to draft. Click one or more faces in the 3-D viewport. Hold Ctrl to add more faces. The faces must not be the neutral plane itself — they are the walls that will be tilted.
Open Draft. Go to Part Design → Dress-Up Features → Draft, or click the Draft button in the Part Design Dress-Up Features toolbar.
Set the draft angle. Enter a value in the Draft angle field. The default is 1.5°. Valid range: -90° to just below 90°. A positive angle typically means the face tilts outward (adding material at the base); a negative angle tilts inward.
Set the neutral plane. Click the Neutral Plane button and then click a flat face or a datum plane in the viewport. The neutral plane is the cross-section that remains stationary — it is usually the parting plane of the mould.

Neutral plane is required

If no neutral plane is set, FreeCAD attempts to guess one from the geometry of the first selected face. If it cannot, the operation fails with "No neutral plane specified and none can be guessed." Always set the neutral plane explicitly for reliable results.
Optionally set a pull direction. Click the Pull Direction button and select a straight edge or a datum line to override the default pull direction. Leave blank to use the neutral plane normal (the most common case).
Optionally tick Reversed to flip the direction of taper (equivalent to negating the angle sign).
Click OK. The Draft feature is added to the model tree.

Tip

To check that your draft angles are correct, use Part Design → Analyse → Draft Analysis (if available) after applying the feature. Correct draft angles will show uniform colour across each face.

Parameters¶

Parameter	Type	Default	Description
Draft angle	Angle	`1.5°`	The tilt angle applied to each selected face. Valid range: `-90°` to just under `90°`. Positive values tilt the face in the direction of the pull direction; negative values tilt it opposite.
Neutral Plane	Object/sub-element link	—	The plane that stays fixed during drafting. Can be a datum plane, an `App::Plane` origin plane, a flat face of an existing feature, or a linear edge (if a pull direction is also set). If omitted, FreeCAD guesses from the selected face geometry.
Pull Direction	Object/sub-element link	—	The axis along which the mould is opened. Can be a datum line, an `App::Line` origin axis, or a straight edge of an existing feature. If omitted, the normal of the neutral plane is used.
Reversed	Toggle	off	When enabled, negates the draft angle — equivalent to multiplying the angle by −1. Useful for drafting faces on the opposite side of the neutral plane without changing the angle value.
References (face list)	Sub-element links	—	The faces that will be drafted. At least one face must be selected.

Advanced usage¶

Neutral plane versus pull direction¶

These two inputs are related but distinct. The neutral plane defines where the face is hinged; the pull direction defines which way the mould moves. In the simplest case (a vertical mould opening along the Z axis) the neutral plane is horizontal (the XY plane) and the pull direction is Z — and FreeCAD can derive Z from the horizontal plane automatically.

When the mould opens at an angle to the part's main axes (a side-action or angled-pull mould), you must set both the neutral plane and the pull direction explicitly. The pull direction must be perpendicular to the neutral plane edge you specify as the hinge reference.

Drafting convex versus concave faces¶

A positive angle on a convex face (an external wall) adds material toward the base. The same positive angle on a concave face (an internal cavity wall) removes material. If you need external walls to draft outward and internal walls to draft inward for mould release, you may need to apply two separate Draft features with opposite signs or use Reversed.

Multiple Draft features¶

If different groups of faces need different draft angles or different neutral planes, apply multiple Draft features in sequence, each targeting a different set of faces.

Common mistakes and pitfalls¶

No neutral plane specified and none can be guessed

Cause: The Neutral Plane field is empty and FreeCAD could not automatically determine a hinge plane from the selected face's geometry.
Fix: Click the Neutral Plane button and explicitly select a datum plane or a flat face of the solid that should remain fixed during drafting.

Resulting shape is null

Cause: The draft angle or geometry produced an invalid solid — often because the angle is too large and the drafted face intersects another face.
Fix: Reduce the angle, or draft fewer faces at once. Also check that the neutral plane is on the correct side of the selected faces.

Pull direction reference edge must be linear

Cause: A curved edge was selected as the pull direction reference.
Fix: Select a straight edge or a datum line as the pull direction reference.

Draft looks correct but the angle is in the wrong direction

Cause: The pull direction is opposite to what you expected, or the selected faces are on the wrong side of the neutral plane.
Fix: Tick Reversed to flip the draft, or move the neutral plane to the other side of the faces.

Python API¶

Minimal example¶

import FreeCAD as App
import PartDesign
import Sketcher
import Part

doc = App.newDocument()

body = doc.addObject("PartDesign::Body", "Body")

sketch = doc.addObject("Sketcher::SketchObject", "Sketch")
body.addObject(sketch)
sketch.addGeometry(Part.LineSegment(App.Vector(0,0,0), App.Vector(30,0,0)), False)
sketch.addGeometry(Part.LineSegment(App.Vector(30,0,0), App.Vector(30,30,0)), False)
sketch.addGeometry(Part.LineSegment(App.Vector(30,30,0), App.Vector(0,30,0)), False)
sketch.addGeometry(Part.LineSegment(App.Vector(0,30,0), App.Vector(0,0,0)), False)
sketch.addConstraint(Sketcher.Constraint("Coincident", 0,2, 1,1))
sketch.addConstraint(Sketcher.Constraint("Coincident", 1,2, 2,1))
sketch.addConstraint(Sketcher.Constraint("Coincident", 2,2, 3,1))
sketch.addConstraint(Sketcher.Constraint("Coincident", 3,2, 0,1))
doc.recompute()

pad = doc.addObject("PartDesign::Pad", "Pad")
body.addObject(pad)
pad.Profile = sketch
pad.Length = 20.0
doc.recompute()

# Apply a 2° draft to the four side faces, using the XY origin plane as neutral plane
draft = doc.addObject("PartDesign::Draft", "Draft")
body.addObject(draft)
# Reference the four side faces of the pad  # TODO: verify face sub-element name syntax
draft.Base = (pad, ["Face1", "Face2", "Face3", "Face4"])
draft.Angle = 2.0                            # 2 degrees
draft.NeutralPlane = (doc.XY_Plane, [""])    # XY plane as neutral plane
draft.PullDirection = None                   # derived from neutral plane normal (Z axis)
draft.Reversed = False
doc.recompute()

Resulting feature properties¶

Property	Type	Description
`Angle`	`App::PropertyAngle`	The draft taper angle in degrees. Valid range: −90° to just under 90°. Default: `1.5°`.
`NeutralPlane`	`App::PropertyLinkSub`	The plane that stays fixed. Accepts datum planes, `App::Plane` origin planes, flat faces, or linear edges (if `PullDirection` is also set).
`PullDirection`	`App::PropertyLinkSub`	The mould opening direction. Accepts datum lines, `App::Line` origin axes, or straight edges. If unset, derived from `NeutralPlane` normal.
`Reversed`	`App::PropertyBool`	Negates the angle direction. Default: `False`.
`Base`	`App::PropertyLinkSub`	Link to the base feature and the selected sub-faces. Inherited from `DressUp`.