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AbhayAradhya1-Visitor
1-Visitor
November 3, 2012
Question

Help! Gear mechanism selection in application menu not working.

  • November 3, 2012
  • 1 reply
  • 3401 views

I'm relatively new to Creo Parametric 2.0. I have two gears mounted on a beam with axles. I tried creating datum axes out of the axles and then selecting them through the gears menu. The datum axes worked. However, when I go to select the gears, nothing highlights and I can't select anything. Any help?


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    1 reply

    T
    twinwood-21-Visitor
    1-Visitor
    November 6, 2012

    Hello Abhay,

    You need to apply a pin connection between each axle and an axis or hole within the assembly. (it cannot be in the gear or shaft component, must be something fixed in the assembly, another component or an assembly axis).

    To do this you will need to select the axle component within the assembly, Right-Click and Edit definition. Go to the constraints tab in the ribbon and delete any constraints that you may have already applied.

    In the ribbon you will see two drop-down menu's the one on the left is the connections drop-down. From here you need to select the 'pin' connection and apply this between 2 cylindrical surfaces or axes in the axle and the assembly. This will define the axis of rotation.

    However this axis of rotation in infinitely long, therefore the axle could sit anywhere along the axis; so you need to define the translation, this could be between 2 planes or 2 planar surfaces of the component and the assembly. In the ribbon it should say 'connection definition complete' once you have succesfully completed the connection.

    To test that this works you can use the drag components tool (looks like a hand) to drag the axle and spin it on the axis in the assembly.

    Once you have done this to both axles and they are spinning as desired you need to define the relationship between the gears. Go to applications> mechanism. You should not see an spiral arrow symbol representing the two pin connections. Go to the Gears tool, select one arrow as the first gear and define its diameter, change to the gear 2 tab, select the second arrow symbol and define its diameter.

    Now use the Drag components tool to rotate one gear and the second should move with it.

    I hope this helps! A little easier to explain with a video but I have nothing to record with at the minute!

    Cheers,

    Tim

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