Involute Gear¶

In one sentence: Generate a fully constrained 2-D sketch profile of an involute gear tooth form, ready to be extruded into a solid gear.

Overview¶

Workbench: Part Design · Menu: Part Design → Involute Gear
Toolbar: none (menu only) · Shortcut: none

Involute Gear creates a Part::Part2DObjectPython feature — a parametric 2-D wire — in the shape of a complete involute gear outline. The result is a closed sketch-like profile placed inside the active Body (or Part). It is not a solid by itself; you must follow it with a Pad or Revolution to obtain a 3-D gear. All tooth geometry is driven by a small set of standard gear parameters, so changing the module or tooth count immediately regenerates the correct profile.

Intuition¶

An involute gear tooth has a specific curved flank shape — the involute — that guarantees smooth rolling contact between meshing gears regardless of small centre-distance errors. Drawing that curve by hand with splines would be tedious and nearly impossible to get right. This tool calculates the exact involute curve from the engineering parameters you already know (module, number of teeth, pressure angle) and hands you a finished, dimensionally correct profile.

Think of it as a gear calculator that outputs geometry rather than numbers. You specify the gear's standard parameters, and the tool fills in every curve — the involute flanks, the root fillets, and the tip arc — then assembles them into one closed wire that is ready to extrude.

The profile lives in the XY plane by default. Once you Pad it, you have a spur gear body. If you want a helical gear, apply a Draft angle or use an Additive Helix as the sweep path.

When to use it¶

You need a standard spur gear profile and do not want to draw involute curves manually.
You are building a parametric gear train and want the tooth geometry to update automatically when you change the module or tooth count.
You need either an external (conventional, outward-pointing teeth) or internal (ring gear, inward-pointing teeth) gear profile.
You want to use profile-shift (rack offset) to correct for undercut on low-tooth-count gears or to adjust the meshing centre distance.

When NOT to use it¶

You need a 3-D bevel, helical, or worm gear — this tool only produces a 2-D spur-gear cross-section. Create the profile here and then use an Additive Pipe with a helical spine for helical gears, or look for dedicated add-ons (e.g. the FCGear workbench) for more gear types.
You need a sprocket for a roller chain — use Sprocket, which uses chain-standard tooth geometry rather than involute curves.
You need to mesh two gears with animated motion — this tool produces geometry only; simulation and animation require the Assembly workbench or an external tool.

Step-by-step walkthrough¶

Prerequisites: An active document. If you want the gear inside a Body for later Part Design operations, activate or create a Body first.

Open Involute Gear via Part Design → Involute Gear.
The Involute Parameter task panel opens and a gear profile appears immediately in the viewport using the default parameters.
Set Number of teeth. Enter the integer tooth count in the Number of teeth spin box. The default is 26. Typical spur gears range from 12 to 200 teeth.

Low tooth counts cause undercut

Gears with fewer than roughly 17 teeth (at the standard 20° pressure angle and zero profile shift) will have undercut at the root, weakening the tooth. Either increase the number of teeth, increase the pressure angle, or apply a positive Profile shift coefficient to eliminate the undercut.
Set Module. Enter the gear module (tooth size) in the Module field. The default is 2.5 mm. The module equals the pitch diameter divided by the tooth count; all meshing gears in a train must share the same module.
Set Pressure angle. Enter the standard pressure angle. The default is 20°, which is the ISO and AGMA standard for most spur gears. Older designs sometimes use 14.5° or 25°.
Choose gear type. Set External gear to True for a conventional gear with outward-pointing teeth (default), or False for a ring gear (internal gear) with inward-pointing teeth.
Adjust advanced coefficients if needed:
Addendum coefficient — tooth height above the pitch circle, normalised by the module. Default 1.0 (external) or 0.6 (internal).
Dedendum coefficient — tooth depth below the pitch circle, normalised by the module. Default 1.25.
Root fillet coefficient — fillet radius at the tooth root, normalised by the module. Default 0.38.
Profile shift coefficient — outward shift of the reference profile, normalised by the module. Default 0.0 (no shift).
Set High precision to True (default) to use two 3-control-point Bézier curves per involute flank (more accurate). Set to False to use a single 4-control-point curve (faster for large assemblies).
Click OK. The gear wire is created and added to the Body (or the active Part if no Body is active).
Pad or revolve the wire. Select the gear feature, then apply Pad with the desired gear face width to produce a solid spur gear.

Tip

To edit the gear after creation, double-click the gear object in the model tree. The task panel reopens with the current values, and any changes immediately update the profile in the viewport.

Parameters¶

Parameter	Type	Default	Description
Number of teeth	Integer	`26`	Total number of gear teeth. Minimum is 3 (UI enforces this).
Module	Length	`2.5 mm`	Tooth size parameter. Equals pitch diameter ÷ number of teeth. All gears in a mesh must share the same module.
Pressure angle	Angle	`20°`	Angle between the tooth flank normal and the pitch-circle tangent. Standard values are 14.5°, 20°, or 25°.
High precision	Dropdown (`True`/`False`)	`True`	`True`: each involute flank is approximated by two 3-control-point Bézier curves (more accurate). `False`: one 4-control-point curve (faster).
External gear	Dropdown (`True`/`False`)	`True`	`True`: external gear (teeth point outwards). `False`: internal/ring gear (teeth point inwards).
Addendum coefficient	Float	`1.0` (external), `0.6` (internal)	Tooth height above the pitch circle, divided by the module. Standard value is 1.0.
Dedendum coefficient	Float	`1.25`	Tooth depth below the pitch circle, divided by the module. Standard value is 1.25 (includes clearance).
Root fillet coefficient	Float	`0.38`	Radius of the fillet at the tooth root, divided by the module.
Profile shift coefficient	Float	`0.0`	Outward displacement of the reference profile from the gear centre, divided by the module. Positive values reduce undercut and increase tooth thickness.

Advanced usage¶

Profile shift to eliminate undercut¶

For gears with fewer than about 17 teeth at a 20° pressure angle, the tooth root may be undercut, weakening the base of the tooth. A positive profile shift moves the cutter outward, effectively thickening the root. A shift coefficient of x = 1 - z / 17 (where z is the tooth count) is a common starting point. The meshing gear should receive an equal-and-opposite shift to maintain the correct centre distance.

Meshing a pair of gears¶

Two gears mesh correctly when they share the same module and pressure angle. For zero-shift gears the centre distance is (z1 + z2) * m / 2. When using profile shift, the operating centre distance changes; consult a gear design reference for the corrected formula.

Internal gear (ring gear)¶

Setting External gear to False generates a ring gear profile. The default addendum coefficient changes to 0.6, which is typical for internal gears. The resulting wire represents the inner bore profile with inward-facing teeth. Pad this wire to produce a ring gear body, then use Boolean Cut to create a housing or planet-carrier clearance if needed.

Common mistakes and pitfalls¶

Profile is an open wire or wire builder error

Cause: Extreme combinations of parameters (very few teeth with large addendum or large profile shift) can push the tip circle inside the base circle, making a valid involute impossible.
Fix: Reduce the addendum coefficient, add a positive profile shift, or increase the tooth count.

Pad fails on the gear profile

Cause: The gear wire is a Part::Part2DObjectPython, not a Sketcher::SketchObject. Some Part Design operations require a Sketcher-based profile.
Fix: If Pad reports an error, try using Part → Extrude instead, or convert the wire to a sketch by mapping it to a face.

Two gears do not mesh smoothly

Cause: The gears have different modules or different pressure angles.
Fix: Ensure both gears use identical Module and Pressure angle values. Pitch diameter = Module × NumberOfTeeth; verify that the sum of pitch radii equals the actual centre distance in the assembly.

Python API¶

Minimal example¶

import FreeCAD as App
import FreeCADGui as Gui

doc = App.newDocument()

# Load the InvoluteGear module and create a gear feature
Gui.activateWorkbench("PartDesignWorkbench")
import InvoluteGearFeature
gear = InvoluteGearFeature.makeInvoluteGear("InvoluteGear")

# Adjust parameters
gear.NumberOfTeeth = 20
gear.Modules = "3 mm"
gear.PressureAngle = "20 deg"
gear.ExternalGear = True
gear.HighPrecision = True
gear.AddendumCoefficient = 1.0
gear.DedendumCoefficient = 1.25
gear.RootFilletCoefficient = 0.38
gear.ProfileShiftCoefficient = 0.0

doc.recompute()
print(f"Gear wire created: {gear.Shape.Length:.2f} mm perimeter")

Resulting feature properties¶

Property	Type	Description
`NumberOfTeeth`	`App::PropertyInteger`	Number of gear teeth.
`Modules`	`App::PropertyLength`	Gear module (tooth size).
`PressureAngle`	`App::PropertyAngle`	Pressure angle of the tooth flank.
`HighPrecision`	`App::PropertyBool`	Use two 3-CP Béziers per flank (`True`) or one 4-CP Bézier (`False`).
`ExternalGear`	`App::PropertyBool`	`True` for external gear, `False` for internal/ring gear.
`AddendumCoefficient`	`App::PropertyFloat`	Addendum height divided by module.
`DedendumCoefficient`	`App::PropertyFloat`	Dedendum depth divided by module.
`RootFilletCoefficient`	`App::PropertyFloat`	Root fillet radius divided by module.
`ProfileShiftCoefficient`	`App::PropertyFloat`	Reference profile shift divided by module.