Once you create your belt sketch and calculate the length in SolidWorks, then you have to develop the belt as a part in the assembly. Save your assembly. From within the Assembly,
1. Click Insert Component, New Part.
2.Select a plane (usually the plane of your belt sketch). The FeatureManager inserts a new part and is displayed in blue.
3. Hold the Ctrl key down and select the belt sketch (or right click select chain)
4. Click Convert Entities. Click Extrude Base. Enter your belt depth and direction.
If you need cuts in your belt:
1. Click the face of the belt. Click Sketch. Click the inside belt tangent edges. Click Convert Entities. Exit the Sketch you will need this for your pattern.
2. Create an Extruded Cut.
3. Click Pattern, Curve Driven Pattern, Select the belt and select convented sketch. Enter number of cuts. The pattern will follow the tangent curve.
The same procedure is for a chain. You need the sketch of the belt from the assembly. Copy this to a new part and create one individual link. Pattern and Mirror save rebuild time.
See
http://www.3dcontentcentral.com/secu...d=171&id=10717 Marie