PartDesign InvoluteGear

Description
This tool allows you to create a 2D profile of an involute gear or spline. 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



Create the profile

 * 1) Optionally activate the correct body.
 * 2) Go to the menu.
 * 3) Set the Involute parameters.
 * 4) Click.
 * 5) If there was no active body: drag and drop the gear into a body for the application of further features like padding.

Create a spur gear

 * 1) Select the gear profile in the Tree view.
 * 2) Press the  button.
 * 3) Set the pad's  to the desired face width of the gear.
 * 4) Click.

Create a helical gear

 * 1) Select the gear profile in the Tree view.
 * 2) Press the  button.
 * 3) Choose as Axis the normal of the gear profile, that is  . (In earlier versions the  can be used as long as the profile's plane has not been altered.)
 * 4) Choose a  mode.
 * 5) Set the  to the desired face width of the gear.
 * 6) To set the desired helical angle an Expression for the  is required.
 * 7) Click the blue [[Image:Bound-expression.svg|16px]] icon at the right of the input field.
 * 8) Enter the following formula:, where  is an example for the desired helical angle (also known as beta-value) and  is the   of the profile.
 * 9) Click  to close the formula editor.
 * 10) Click  to close the task panel.

Hint: To make the helical angle an accessible parameter, use a dynamic property:
 * 1) Select the profile.
 * 2) In the Property editor activate the  option in the context menu.
 * 3) Again in the context menu, select . Note: this entry is only available when  is active.
 * 4) In the  dialog:
 * 5) Choose  as Type.
 * 6) Set  as Group.
 * 7) Set  as Name (without a space).
 * 8) Click.
 * 9) Now a new property  (space added automatically), with an initial value of, becomes available.
 * 10) Assign the desired helical angle to the new property.
 * 11) In the formula of the  property of the AdditiveHelix, you can now reference  instead of the hard coded value of e.g. ; again assuming  is the  of the profile.

Cut a hub for an involute splined shaft

 * 1) Activate the correct body.
 * 2) Create an internal involute gear profile with the required number of grooves and adapt the values of pressure angle, addendum-, dedendum- and root fillet coefficient. See also the table in Notes below for feasible values. For example:
 * : False
 * : 12
 * : 37.5°
 * : 0.45
 * : 0.7
 * : 0.3
 * 1) Select the gear profile in the Tree view.
 * 2) Press the  button.
 * 3) Set the pocket's  to Through All.
 * 4) Check the pocket's  option.
 * 5) Click.

Properties

 * : True or false.


 * : True or false.


 * : Pitch diameter divided by the number of teeth.


 * : Sets the number of teeth.


 * : Acute angle between the line of action and a normal to the line connecting the gear centers. Default is 20 °. See Involute gear.


 * : The height of the tooth from the pitch circle up to its tip, normalized by the module. Default is 1.0 for the standard full-depth system.


 * : The height of the tooth from the pitch circle down to its root, normalized by the module. Default is 1.25 for the standard full-depth system.


 * : The radius of the fillet at the root of the tooth, normalized by the module. Default is 0.38 as defined by the ISO rack.

Limitations

 * It is currently not possible to adjust the tooth thickness. Tooth and tooth space are distributed equally on the pitch circle. Thus the only way to control backlash is to adjust the center distance in a gear paring.
 * There is currently no undercut in the generated gear profile. That means gears with a low number of teeth can interfere with the teeth of the mating gear. The lower limit depends on the and is around 17 teeth for 20° and 32 for 14.5°. Most practical applications tolerate a missing undercut for gears a little smaller than this theoretical limit though.

Tutorials
Video: How to make gears in FreeCAD

Related

 * FCGear Workbench