PartDesign InvoluteGear/de

Beschreibung
Dieses Werkzeug erlaubt es ein 2D-Profil eines Evolventenrades oder einer Evolventenverzahnung zu erstellen. Dieses 2D-Profil ist vollständig parametrisch und kann mit den Formelementen PartDesign Aufpolsterung oder PartDesign Wendel extrudiert werden.

Für detailliertere Informationen siehe Wikipedia: Gear und Involute Gear (engl.).



Anwendung


Profil erstellen

 * 1) Wahlweise den richtigen Körper aktivieren.
 * 2) Zum Menü  wechseln.
 * 3) Die Evolventenparameter anpassen.
 * 4)  klicken.
 * 5) Wurde noch kein Körper aktiviert: Das Zahnrad auf einen Körper ziehen und ablegen, um es mit weiteren Formelementen zu verwenden.



Ein geradverzahntes Stirnrad erstellen

 * 1) Das Zahnradprofil in der Baumansicht Auswählen.
 * 2) Die Schaltfläche  drücken.
 * 3) Die  des Blocks auf die gewünschte Zahnradbreite einstellen.
 * 4)  klicken.



Ein schrägverzahntes Stirnrad erstellen

 * 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.

Eigenschaften

 * : 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.


 * (Stirnrad): Wahr oder Falsch


 * (Hohe Präzision): Wahr oder Falsch


 * (der Modul): Teilkreisdurchmesser geteilt durch die Anzahl der Zähne.


 * : Legt die Anzahl der Zähne fest.


 * (Eingriffswinkel): Winkel zwischen der Wirkungslinie und einer Normalen zu der Linie, die die Zahnradmitten verbindet. Standard ist 20°. Siehe (Evolventenverzahnung)


 * : The distance by which the reference profile is shifted outwards, normalized by the module. Default is zero. Profile shift may be positive or negative.


 * : 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.

Tutorien
Video: How to make gears in FreeCAD

Verwandt

 * Arbeitsbereich FCGear