Additive Cone¶

In one sentence: Insert a parametric cone or frustum (truncated cone) directly into a Part Design Body without needing a sketch.

Overview¶

Workbench: Part Design · Menu: Part Design → Additive Primitives → Additive Cone
Toolbar: Part Design Modeling Primitives (CompPrimitiveAdditive) · Shortcut: none

Additive Cone creates a solid cone or frustum defined by two radii (one per end face), a height, and an optional sweep angle, then fuses it into the active Body. No sketch is required. Setting the top radius to zero gives a true cone with a sharp apex; setting both radii to the same non-zero value gives a cylinder; any other combination gives a frustum (truncated cone). A sweep angle less than 360° cuts the shape into a sector.

Intuition¶

Think of an ice-cream cone or a bucket. A cone narrows from a wide base to a point; a frustum (bucket shape) narrows from a wide base to a smaller flat top. The Additive Cone captures both shapes through two radius parameters:

Radius1 is the radius of the bottom face (at Z = 0).
Radius2 is the radius of the top face (at Z = Height).

When Radius2 = 0, the top collapses to a single point: a sharp apex. When Radius2 > 0, the top is a flat circular face: a frustum. Either radius can be larger than the other — you can have a cone that widens toward the top by making Radius2 > Radius1.

Note

When Radius1 == Radius2 (within floating-point precision), FreeCAD internally builds the shape as a cylinder rather than a degenerate cone. The resulting solid is identical in shape to Additive Cylinder with the same radius and height.

The sweep angle (Angle) works the same as in Additive Cylinder: at 360° you get the full rotational solid; at less than 360° you get a sector wedge.

When to use it¶

You need a conical boss, taper, or spigot without drawing a trapezoidal sketch to revolve.
You need a frustum (truncated cone) for a tapered fitting, plug, or transition between two circular sizes.
You want a sharp-pointed cone for a tip, spike, or reference geometry.
You are scripting or generating parametric models and want a single API call to produce a cone feature.
You need a conical sector (partial cone) by setting the sweep angle to less than 360°.

When NOT to use it¶

The taper profile is non-linear (curved side wall) — draw a curve profile as a sketch and use Revolution. Additive Cone only produces straight-sided tapers.
You need a hollow cone or thin-walled conical shell — a Pad of a ring sketch combined with a Shell operation is more appropriate.
You want to cut a conical pocket or tapered hole into existing material — use Subtractive Cone, which has identical parameters but cuts instead of adds.
The cone cross-section should be elliptical rather than circular — use Revolution with an appropriate sketch, or Additive Ellipsoid if a partial ellipsoid is sufficient.

Step-by-step walkthrough¶

Prerequisite: An active Part Design document. An active Body is required; FreeCAD will offer to create one if none exists.

Invoke the tool. Go to Part Design → Additive Primitives → Additive Cone, or click the Additive Cone icon in the CompPrimitiveAdditive toolbar drop-down.
If no Body exists, FreeCAD creates one automatically. If multiple Bodies exist, choose the target Body in the dialog.
The task panel opens with four fields: Radius1, Radius2, Height, and Angle.
Set Radius1 — the base (bottom) radius. Default is 2 mm.
Set Radius2 — the top radius. Default is 4 mm. Set to 0 for a sharp apex; set equal to Radius1 for a cylinder; set larger than Radius1 for an upward-flaring frustum.
Set Height. Default is 10 mm. Must be greater than zero.
Set Angle. Default is 360° (full rotational solid). Reduce to create a sector.
Optionally configure Attachment in the lower task panel section to position the cone relative to a face, edge, or datum.
Click OK. The cone is fused into the Body and appears in the model tree.

Tip

To produce a standard sharp cone pointing upward, set Radius1 to your desired base radius, Radius2 to 0, and Height to the desired length. The apex will be at the top of the Z-axis.

Parameters¶

Parameter	Type	Default	Description
Radius1	Length (mm)	2.0 mm	Radius of the bottom face (at Z = 0). Range: 0 mm to max float. May be 0 only if Radius2 > 0.
Radius2	Length (mm)	4.0 mm	Radius of the top face (at Z = Height). Range: 0 mm to max float. Set to 0 for a sharp apex.
Height	Length (mm)	10.0 mm	Distance between the two circular faces along the local Z-axis. Must be greater than zero.
Angle	Angle (°)	360.0°	Sweep angle of the cross-section around the central axis. Range: 0° (exclusive) to 360°. Values less than 360° produce a sector with two planar lateral faces.

Note

Both Radius1 and Radius2 may be zero, but not simultaneously — that would produce a degenerate shape with no volume. The source (quantityRangeZero) allows zero for both radii individually, but OCCT will reject a cone with both radii at zero.

The task panel also exposes an Attachment section (inherited from Part::AttachExtension) for positioning the cone relative to faces, edges, vertices, or datum objects.

Advanced usage¶

Inverted frustums¶

If Radius2 > Radius1, the cone flares outward toward the top — an inverted frustum. This is useful for draft-angle modelling, nozzle interiors, or funnel shapes.

Zero top radius — sharp apex¶

Setting Radius2 = 0.0 in the Python API produces a cone with a geometric point at the apex. Note that this creates a degenerate (non-manifold) vertex in the OCCT topology; downstream operations like Fillet on the apex edge may fail or behave unexpectedly. For most downstream purposes a very small Radius2 (e.g. 0.01 mm) is safer than exactly zero.

Using the cone as a construction aid¶

Cones placed with Additive Cone can be used as reference geometry for positioning other features. For example, place a cone at the centre of a circular boss to visualise draft angles, then delete or suppress the cone feature when it is no longer needed.

Cone sector for angular geometry¶

Set Angle to 90° to create a quarter-cone sector. Combined with a polar pattern, this can tile into a full cone while retaining the sector as a discrete reusable feature.

Common mistakes and pitfalls¶

Both Radius1 and Radius2 are zero — feature fails

Cause: If both radii are set to zero there is no volume to build. FreeCAD will report a geometry failure from OCCT.
Fix: Set at least one radius to a value greater than zero.

Expected a cone but got a cylinder

Cause: Radius1 and Radius2 are equal (or differ by less than OCCT's precision threshold). When the two radii are the same, FreeCAD internally uses BRepPrimAPI_MakeCylinder and produces a cylinder.
Fix: If you intended a frustum, adjust Radius1 and Radius2 to different values. This is intentional behaviour, not a bug.

Cone appears as a sector instead of a full solid

Cause: The Angle property is less than 360°.
Fix: Open the feature for editing and reset Angle to 360°.

Height too small — feature fails to compute

Cause: Height must be greater than approximately 2 × 10⁻⁷ mm. Setting it to zero triggers an error.
Fix: Use a positive Height value.

Python API¶

Minimal example¶

import FreeCAD as App
import PartDesign  # noqa: F401 — registers PartDesign object types
import math

doc = App.newDocument()

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

# Create an Additive Cone (frustum: bottom radius 6, top radius 3, height 15)
cone = doc.addObject("PartDesign::AdditiveCone", "Cone")
body.addObject(cone)

cone.Radius1 = 6.0   # mm — bottom radius
cone.Radius2 = 3.0   # mm — top radius
cone.Height  = 15.0  # mm
cone.Angle   = 360.0 # full solid (degrees)

doc.recompute()

# Volume of a frustum: (π/3) × H × (R1² + R1·R2 + R2²)
expected = (math.pi / 3.0) * 15.0 * (6.0**2 + 6.0 * 3.0 + 3.0**2)
print(f"Volume: {cone.Shape.Volume:.4f} mm³")
# Expected: (π/3) × 15 × (36 + 18 + 9) ≈ 989.6018 mm³

# Sharp apex cone: Radius2 = 0
apex_cone = doc.addObject("PartDesign::AdditiveCone", "ApexCone")
body.addObject(apex_cone)
apex_cone.Radius1 = 5.0
apex_cone.Radius2 = 0.0
apex_cone.Height  = 12.0
apex_cone.Angle   = 360.0
doc.recompute()

Resulting feature properties¶

Property	Type	Default	Description
`Radius1`	`App::PropertyLength`	`2.0 mm`	Bottom face radius. Range: [0, ∞). At least one radius must be > 0.
`Radius2`	`App::PropertyLength`	`4.0 mm`	Top face radius. Range: [0, ∞). Set to 0 for a sharp apex.
`Height`	`App::PropertyLength`	`10.0 mm`	Axial length. Must be > 0.
`Angle`	`App::PropertyAngle`	`360.0°`	Sweep angle around the central axis. Range: (0°, 360°].