PartDesign InvoluteGear

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Revision as of 19:38, 26 December 2021 by Jonasb (talk | contribs) (Extend the "Usage" section with instructions for spur and helical gears)
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PartDesign InvoluteGear.svg PartDesign InvoluteGear

Menu location
Part Design → Involute gear...
Workbenches
PartDesign
Default shortcut
None
Introduced in version
-
See also
FCGear Workbench

Description

This tool allows you to create a 2D profile of an involute gear. This 2D profile is fully parametric, and can be padded with the PartDesign Pad or PartDesign AdditiveHelix feature.

For more detailed information see Wikipedia's entries for: Gear and Involute Gear

PartDesign Involute Gear 01.png

Usage

Create the Profile

  1. Go to the menu Part Design → PartDesign InternalExternalGear.svg Involute gear....
  2. Set the Involute parameters.
  3. Click OK
  4. The involute gear is created outside of the active body. Drag and drop it into a body for the application of further features like padding.

Create a Spur Gear

  1. Select the gear profile in the tree.
  2. Press the PartDesign Pad.svg Pad button.
  3. Set the pad's DataLength to the desired face width of the gear.
  4. Click OK

Create a Helical Gear introduced in version 0.19

  1. Select the gear profile in the tree.
  2. Press the PartDesign AdditiveHelix.svg PartDesign AdditiveHelix button.
  3. Choose as Axis the normal of the gear profile, that is Normal sketch axis introduced in version 0.20. (In earlier versions the Base Z axis can be used as long as the profile's plane has not been altered.)
  4. Choose a Height-Turns mode.
  5. Set the DataHeight to the desired face width of the gear.
  6. To set the desired helical angle an Expressions for the DataTurns is required.
    1. Click the blue 16px icon at reh right of the turns' input filed
    2. Enter the following formula: Height * tan(25°) / (InvoluteGear.NumberOfTeeth * InvoluteGear.Modules * pi), where 25° is the desired helical angle (aka beta-value) and InvoluteGear is the Name of the profile.

Parameters

  • Number of teeth: Sets the number of teeth.
  • Modules: Pitch diameter divided by the number of teeth.
  • Pressure angle: Acute angle between the line of action and a normal to the line connecting the gear centers. Default is 20 degrees. (More info)
  • High precision: True or false
  • External gear: True or false

Tutorials

How to make gears in FreeCAD

Related