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Belt/Chain PropertyManager

The Belt/Chain PropertyManager appears when you create or edit a belt/chain assembly feature.

Belt Members

PM_pulley_components_belt_chain.gif Pulley components In the graphics area, select axes or cylindrical faces of components you want to include in the belt and pulleys system. You can click:
  • Move Up or Move Down to change the order of pulleys.
  • Flip belt side to flip the belt to the other side of the selected pulley.
You can also click the feature handle on a pulley to flip the belt to the other side. Video: Belt Flip Direction
Diameter of selected pulley This value is used in calculating the belt length and determining the amount of relative rotation between adjacent pulleys. By default, the measured diameter of the selected pulley is displayed. If you override the measured value, the value you enter appears in bold type. To revert to the measured value, enter 0.

Belt Location Plane

Belt sketch plane position You can select a vertex, plane, or planar face to change the position of the belt sketch plane.
All pulleys in the feature must be parallel. The belt sketch plane is normal to the axes of the pulleys.

Properties

  Belt Length Displays the length of the belt. The software calculates the length of the belt based on the positions and diameters of the pulleys. Optionally, click Driving to specify the length of the belt and have the pulley positions adjust (at least one pulley must have an appropriate degree of freedom).
  Use belt thickness Select to specify a thickness for the belt. The belt curve is offset from the cylindrical faces of the pulleys by one half the specified belt thickness.
  Engage belt

Select to cause rotation of the pulleys relative to each other. Video: Assembly Belt Engaged

Clear to suppress the belt mates, which enables you to reposition a pulley without causing the other pulleys to rotate. Video: Assembly Belt Disengaged
  Create belt part Select to automatically create a new part containing the belt sketch and add the part to the assembly. In the part file, use the sketch as a sweep path to create a solid belt. If you change the pulley positions in the assembly, the sketch updates in the belt part.


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